Con Cmas
Uploaded by
kleidi85Con Cmas
Uploaded by
kleidi85DIANA
Finite Element Analysis
User’s Manual
Concrete and Masonry
Analysis
Release 9.4.3
TNO DIANA BV
ii
DIANA – Finite Element Analysis
User’s Manual release 9.4.3
Concrete and Masonry Analysis
Edited by: Jonna Manie
Published by:
TNO DIANA bv
Delftechpark 19a, 2628 XJ Delft, The Netherlands.
Phone: +31 88 34262 00
Fax: +31 88 34262 99
E-mail: info@tnodiana.com
Web page: tnodiana.com
Trademarks.
Diana is a registered trademark of TNO DIANA bv. FemGV, FemGen, FemView
are trademarks of Femsys Ltd. CADfix is a registered trademark of Transcen-
Data Europe Limited. Windows is a registered trademark of Microsoft Corporation.
PostScript, Acrobat and Acrobat Reader are registered trademarks of Adobe Sys-
tems, Inc. AutoCAD is a registered trademark of Autodesk Inc. DXF is a trademark
of Autodesk Inc. ACIS is a registered trademark of Spatial Technology Inc. CADDS
and Pro/ENGINEER are registered trademarks of Parametric Technology Corpora-
tion. CATIA is a registered trademark of Dassault Systemes S.A. IGES is a trademark
of IGES Data Analysis, Inc. Parasolid is a registerd trademark of UGS Corporation.
PATRAN is a registered trademark of MSC Software Corporation. The X Window
System is a trademark of M.I.T. unix is a registered trademark of UNIX Systems Lab-
oratories, Inc. Intel is a registered trademark of Intel Corporation. SUN and Solaris
are trademarks or registered trademarks of Sun Microsystems, Inc. HP is a registered
trademark of Hewlett-Packard Company. All other brand names, product names or
trademarks belong to their respective holders.
First edition, November 8, 2010.
Copyright © 2010 by TNO DIANA bv, all rights reserved. No part of this publication
may be reproduced in any form by print, photoprint, microfilm or any other means,
without the prior written permission of the publisher.
The information in this document is subjected to change without notice and should
not be construed as a commitment by TNO DIANA bv. TNO DIANA bv assumes
no responsibility for any errors that may appear in this document.
The Diana system is the sole property of TNO DIANA bv. Software materials made
available are solely for use at a single site; they are not to be distributed to others
without prior written permission of TNO DIANA bv.
This document was prepared with the LATEX Document Preparation System.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis
Contents at a Glance
Preface xv
Glossary of Symbols xvii
I General Introduction 1
1 Basic Principles 3
II Structural Design 5
2 Reinforcement Forces and Moments for a Bridge 7
3 Fire under Concrete Slab 43
III Cracking and Failure 63
4 Smeared Cracking in a Notched Beam 65
5 Discrete Cracking in a Notched Beam 79
6 Shear Failure in Reinforced Concrete Beam 95
7 Shear Wall Panel 109
8 Column–Beam Joint in a Portal Frame 129
9 Reinforced Concrete Slab 145
10 Fire near Concrete Safety Tank 159
11 Gas Explosion in Tunnel 209
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis November 8, 2010 – First ed.
iv
IV Creep and Shrinkage 241
12 Post-tensioned Concrete Beam 243
13 Long Term Behavior of RC Beam 269
14 Concrete Viaduct 287
15 Stress Ribbon Bridge 313
V Young Hardening Concrete 331
16 Hydration of Concrete Column 333
17 Thermal and Flow–Stress Analysis of a Box Girder 347
18 Wall with Cooling Pipes 371
19 Cooling Pipes in a Tunnel 389
20 Early Age Behavior of a Purification Wall 415
21 Adiabatic Hydration of Concrete 441
VI Masonry Modeling 447
22 Interfaces in Masonry Wall 449
23 Discrete Modeling of Masonry 463
24 Composite Modeling of Masonry 489
Bibliography 507
Index 509
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis
Contents
Preface xv
Glossary of Symbols xvii
I General Introduction 1
1 Basic Principles 3
II Structural Design 5
2 Reinforcement Forces and Moments for a Bridge 7
2.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 8
2.1.1 Geometry Definition . . . . . . . . . . . . . . . . . . . . 8
2.1.2 Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . . 12
2.1.3 Axes Consistency . . . . . . . . . . . . . . . . . . . . . 15
2.1.4 Material and Physical Properties . . . . . . . . . . . . . 16
2.1.5 Boundary Constraints . . . . . . . . . . . . . . . . . . . 16
2.1.6 Loads . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18
2.2 Linear Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . 18
2.2.1 Displacements . . . . . . . . . . . . . . . . . . . . . . . 20
2.2.2 Stresses . . . . . . . . . . . . . . . . . . . . . . . . . . . 21
2.2.3 Local Element Axes . . . . . . . . . . . . . . . . . . . . 22
2.2.4 Distributed Bending Moments . . . . . . . . . . . . . . 23
2.2.5 Distributed Forces . . . . . . . . . . . . . . . . . . . . . 24
2.2.6 Reinforcement Moments . . . . . . . . . . . . . . . . . . 25
2.2.7 Reinforcement Forces . . . . . . . . . . . . . . . . . . . 26
2.2.8 Combined Moments and Forces . . . . . . . . . . . . . 26
2.2.9 Shear Reinforcement . . . . . . . . . . . . . . . . . . . . 28
2.3 Prestress . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28
2.3.1 Applying Prestress . . . . . . . . . . . . . . . . . . . . . 29
2.3.2 Linear Analysis . . . . . . . . . . . . . . . . . . . . . . 30
2.3.3 Normal Forces and Stresses . . . . . . . . . . . . . . . . 31
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis November 8, 2010 – First ed.
vi CONTENTS
2.3.4 Reinforcement Forces . . . . . . . . . . . . . . . . . . . 32
2.3.5 Reinforcement Moments . . . . . . . . . . . . . . . . . . 32
2.4 Asymmetric Loading . . . . . . . . . . . . . . . . . . . . . . . . 33
2.4.1 Applying Load According to Eurocode . . . . . . . . . 33
2.4.2 Linear Analysis . . . . . . . . . . . . . . . . . . . . . . 36
2.4.3 Displacements . . . . . . . . . . . . . . . . . . . . . . . 37
2.4.4 Combined Moments and Forces . . . . . . . . . . . . . 37
2.4.5 Shear Reinforcement . . . . . . . . . . . . . . . . . . . . 39
3 Fire under Concrete Slab 43
3.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 44
3.1.1 Geometry Definition . . . . . . . . . . . . . . . . . . . . 45
3.1.2 Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . . 46
3.1.3 Boundary Elements . . . . . . . . . . . . . . . . . . . . 46
3.1.4 Reinforcements . . . . . . . . . . . . . . . . . . . . . . . 48
3.1.5 Material and Physical Properties . . . . . . . . . . . . . 49
3.1.6 Mechanical Loading . . . . . . . . . . . . . . . . . . . . 51
3.1.7 Boundary Constraints . . . . . . . . . . . . . . . . . . . 52
3.1.8 Temperature . . . . . . . . . . . . . . . . . . . . . . . . 53
3.2 Staggered Flow–Stress Analysis . . . . . . . . . . . . . . . . . . 54
3.2.1 Transient Heat Flow Analysis . . . . . . . . . . . . . . 54
3.2.2 Temperature Distribution and Development . . . . . . 55
3.2.3 Structural Analysis . . . . . . . . . . . . . . . . . . . . 58
3.2.4 Stresses in the Concrete Slab . . . . . . . . . . . . . . . 59
3.2.5 Stresses in the Reinforcement Grid . . . . . . . . . . . . 61
III Cracking and Failure 63
4 Smeared Cracking in a Notched Beam 65
4.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 65
4.1.1 Geometry Definition . . . . . . . . . . . . . . . . . . . . 66
4.1.2 Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . . 67
4.1.3 Mirror to Full Model . . . . . . . . . . . . . . . . . . . 68
4.1.4 Material and Physical Properties . . . . . . . . . . . . . 68
4.1.5 Supports and Loading . . . . . . . . . . . . . . . . . . . 70
4.2 Preliminary Linear Analysis . . . . . . . . . . . . . . . . . . . . 70
4.2.1 Deformation . . . . . . . . . . . . . . . . . . . . . . . . 71
4.2.2 Principal Cauchy Stresses . . . . . . . . . . . . . . . . . 72
4.3 Nonlinear Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . 72
4.3.1 Load–Displacement Diagram . . . . . . . . . . . . . . . 74
4.3.2 Principal Cauchy Stresses . . . . . . . . . . . . . . . . . 75
4.3.3 Crack Pattern . . . . . . . . . . . . . . . . . . . . . . . 76
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis
CONTENTS vii
5 Discrete Cracking in a Notched Beam 79
5.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 80
5.1.1 Geometry Definition . . . . . . . . . . . . . . . . . . . . 80
5.1.2 Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . . 81
5.1.3 Expansion to Full Model . . . . . . . . . . . . . . . . . 82
5.1.4 Material and Physical Properties . . . . . . . . . . . . . 83
5.1.5 Boundary Conditions . . . . . . . . . . . . . . . . . . . 84
5.1.6 Moving Parts Together . . . . . . . . . . . . . . . . . . 85
5.2 Preliminary Linear Analysis . . . . . . . . . . . . . . . . . . . . 86
5.2.1 Deformation . . . . . . . . . . . . . . . . . . . . . . . . 87
5.2.2 Principal Cauchy Stresses . . . . . . . . . . . . . . . . . 87
5.2.3 Interface Normal Tractions . . . . . . . . . . . . . . . . 88
5.3 Nonlinear Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . 88
5.3.1 Load–Displacement Diagram . . . . . . . . . . . . . . . 90
5.3.2 Interface Normal Tractions . . . . . . . . . . . . . . . . 91
5.3.3 Von Mises Stresses . . . . . . . . . . . . . . . . . . . . . 91
6 Shear Failure in Reinforced Concrete Beam 95
6.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 96
6.1.1 Geometry Definition . . . . . . . . . . . . . . . . . . . . 96
6.1.2 Reinforcement . . . . . . . . . . . . . . . . . . . . . . . 97
6.1.3 Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . . 97
6.1.4 Material and Physical Properties . . . . . . . . . . . . . 98
6.1.5 Boundary Conditions . . . . . . . . . . . . . . . . . . . 99
6.2 Nonlinear Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . 100
6.2.1 Load–Displacement Diagram . . . . . . . . . . . . . . . 101
6.2.2 Reinforcement Stresses . . . . . . . . . . . . . . . . . . 102
6.2.3 Crack Development . . . . . . . . . . . . . . . . . . . . 104
6.3 Force-Controlled Analysis . . . . . . . . . . . . . . . . . . . . . . 105
6.3.1 Creating a Force Load . . . . . . . . . . . . . . . . . . . 105
6.3.2 Nonlinear Analysis . . . . . . . . . . . . . . . . . . . . . 106
6.3.3 Load–Displacement Diagram . . . . . . . . . . . . . . . 107
6.3.4 Ultimate Limit State . . . . . . . . . . . . . . . . . . . 107
7 Shear Wall Panel 109
7.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 109
7.1.1 Geometry Definition . . . . . . . . . . . . . . . . . . . . 110
7.1.2 Reinforcement . . . . . . . . . . . . . . . . . . . . . . . 113
7.1.3 Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . . 114
7.1.4 Material and Physical Properties . . . . . . . . . . . . . 114
7.1.5 Boundary Conditions . . . . . . . . . . . . . . . . . . . 117
7.2 Preliminary Linear Analysis . . . . . . . . . . . . . . . . . . . . 118
7.2.1 Stresses . . . . . . . . . . . . . . . . . . . . . . . . . . . 119
7.2.2 Displacements . . . . . . . . . . . . . . . . . . . . . . . 119
7.3 Nonlinear Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . 121
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis November 8, 2010 – First ed.
viii CONTENTS
7.4 Load–Displacement Diagram . . . . . . . . . . . . . . . . . . . . 122
7.4.1 Principal Stress . . . . . . . . . . . . . . . . . . . . . . 124
7.4.2 Plastic Strains in Reinforcements . . . . . . . . . . . . . 124
7.4.3 Cracking . . . . . . . . . . . . . . . . . . . . . . . . . . 125
7.5 Cyclic Loading . . . . . . . . . . . . . . . . . . . . . . . . . . . . 127
8 Column–Beam Joint in a Portal Frame 129
8.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 130
8.1.1 Geometry Definition . . . . . . . . . . . . . . . . . . . . 131
8.1.2 Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . . 131
8.1.3 Reinforcement . . . . . . . . . . . . . . . . . . . . . . . 132
8.1.4 Material and Physical Properties . . . . . . . . . . . . . 133
8.1.5 Boundary Conditions . . . . . . . . . . . . . . . . . . . 134
8.2 Nonlinear Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . 134
8.2.1 Load–Displacement Diagram . . . . . . . . . . . . . . . 136
8.2.2 Crack Development . . . . . . . . . . . . . . . . . . . . 137
8.2.3 Principal Stress . . . . . . . . . . . . . . . . . . . . . . 139
8.2.4 Concrete Crushing via Plastic Strain . . . . . . . . . . 139
8.2.5 Yielding in Reinforcement . . . . . . . . . . . . . . . . . 141
9 Reinforced Concrete Slab 145
9.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 146
9.1.1 Slab Geometry . . . . . . . . . . . . . . . . . . . . . . . 146
9.1.2 Concrete Properties and Thickness . . . . . . . . . . . . 147
9.1.3 Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . . 148
9.1.4 Reinforcement Grids . . . . . . . . . . . . . . . . . . . . 148
9.1.5 Steel Amount and Properties . . . . . . . . . . . . . . . 149
9.1.6 Boundary Constraints . . . . . . . . . . . . . . . . . . . 150
9.2 Nonlinear Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . 151
9.2.1 Results for Step 11 . . . . . . . . . . . . . . . . . . . . 154
9.2.2 Results for Step 21 . . . . . . . . . . . . . . . . . . . . 155
9.2.3 Results for Step 31 . . . . . . . . . . . . . . . . . . . . 156
9.2.4 Results for Step 81 . . . . . . . . . . . . . . . . . . . . 156
9.2.5 Deformation . . . . . . . . . . . . . . . . . . . . . . . . 157
9.2.6 Load–Displacement Diagram . . . . . . . . . . . . . . . 157
9.3 Concluding Remarks . . . . . . . . . . . . . . . . . . . . . . . . . 158
10 Fire near Concrete Safety Tank 159
10.1 Model for Linear Structural Analysis . . . . . . . . . . . . . . . 160
10.1.1 Floor . . . . . . . . . . . . . . . . . . . . . . . . . . . . 161
10.1.2 Wall . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 163
10.1.3 Beam . . . . . . . . . . . . . . . . . . . . . . . . . . . . 164
10.1.4 Dome . . . . . . . . . . . . . . . . . . . . . . . . . . . . 166
10.1.5 Foundation Interface . . . . . . . . . . . . . . . . . . . . 166
10.1.6 Reinforcement . . . . . . . . . . . . . . . . . . . . . . . 168
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis
CONTENTS ix
10.1.7 Supports . . . . . . . . . . . . . . . . . . . . . . . . . . 171
10.1.8 Loading . . . . . . . . . . . . . . . . . . . . . . . . . . . 173
10.1.9 Properties . . . . . . . . . . . . . . . . . . . . . . . . . 175
10.2 Linear Structural Analysis . . . . . . . . . . . . . . . . . . . . . 177
10.2.1 Deformation for Load Cases . . . . . . . . . . . . . . . 179
10.2.2 Combining Load Cases . . . . . . . . . . . . . . . . . . 179
10.2.3 Empty Tank . . . . . . . . . . . . . . . . . . . . . . . . 181
10.2.4 Fully Filled Tank . . . . . . . . . . . . . . . . . . . . . 182
10.2.5 Calamity Situation . . . . . . . . . . . . . . . . . . . . 184
10.3 Model for Flow–Stress Analysis . . . . . . . . . . . . . . . . . . 185
10.3.1 Model for Heat Flow Analysis . . . . . . . . . . . . . . 187
10.3.2 Model for Nonlinear Structural Analysis . . . . . . . . . 194
10.4 Staggered Flow–Stress Analysis . . . . . . . . . . . . . . . . . . 198
10.4.1 Transient Nonlinear Heat Flow Analysis . . . . . . . . . 199
10.4.2 Transient Nonlinear Structural Analysis . . . . . . . . . 202
11 Gas Explosion in Tunnel 209
11.1 Description . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 209
11.1.1 Loading . . . . . . . . . . . . . . . . . . . . . . . . . . . 209
11.1.2 Explosion . . . . . . . . . . . . . . . . . . . . . . . . . . 210
11.1.3 Material Properties . . . . . . . . . . . . . . . . . . . . 210
11.1.4 Finite Element Idealization . . . . . . . . . . . . . . . . 212
11.2 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 212
11.2.1 Geometry Definition . . . . . . . . . . . . . . . . . . . . 213
11.2.2 Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . . 214
11.2.3 Reinforcements . . . . . . . . . . . . . . . . . . . . . . . 215
11.2.4 Boundary Constraints . . . . . . . . . . . . . . . . . . . 216
11.2.5 Loading . . . . . . . . . . . . . . . . . . . . . . . . . . . 217
11.2.6 Material and Physical Properties . . . . . . . . . . . . . 219
11.3 Linear Static Analysis . . . . . . . . . . . . . . . . . . . . . . . . 221
11.3.1 Dead Weight . . . . . . . . . . . . . . . . . . . . . . . . 222
11.3.2 Sand and Water Pressure . . . . . . . . . . . . . . . . . 222
11.3.3 Initial Explosion . . . . . . . . . . . . . . . . . . . . . . 222
11.4 Eigenvalue Analysis . . . . . . . . . . . . . . . . . . . . . . . . . 224
11.4.1 Eigenfrequencies . . . . . . . . . . . . . . . . . . . . . . 225
11.4.2 Eigenmodes . . . . . . . . . . . . . . . . . . . . . . . . . 225
11.5 Initial Static Nonlinear Analysis . . . . . . . . . . . . . . . . . . 226
11.5.1 Deformation . . . . . . . . . . . . . . . . . . . . . . . . 228
11.5.2 Crack Formation . . . . . . . . . . . . . . . . . . . . . . 229
11.5.3 Stresses . . . . . . . . . . . . . . . . . . . . . . . . . . . 231
11.5.4 Plasticity in Reinforcements . . . . . . . . . . . . . . . 232
11.6 Transient Nonlinear Dynamic Analysis . . . . . . . . . . . . . . 233
11.6.1 Consideration of Options . . . . . . . . . . . . . . . . . 233
11.6.2 Performing Time Steps . . . . . . . . . . . . . . . . . . 234
11.6.3 Results after Start of Explosion . . . . . . . . . . . . . 236
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis November 8, 2010 – First ed.
x CONTENTS
11.6.4 Results at End of Explosion . . . . . . . . . . . . . . . 237
11.6.5 Results at End of Analysis . . . . . . . . . . . . . . . . 237
11.6.6 History Diagrams . . . . . . . . . . . . . . . . . . . . . 238
IV Creep and Shrinkage 241
12 Post-tensioned Concrete Beam 243
12.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 244
12.1.1 Beam . . . . . . . . . . . . . . . . . . . . . . . . . . . . 245
12.1.2 Reinforcement . . . . . . . . . . . . . . . . . . . . . . . 246
12.1.3 Material and Physical Properties . . . . . . . . . . . . . 247
12.1.4 Checking the Mesh and the Reinforcement . . . . . . . 249
12.1.5 Boundary Conditions and Loading . . . . . . . . . . . . 249
12.1.6 Specifying the Reinforcement Shape . . . . . . . . . . . 250
12.2 Preliminary Linear Analysis . . . . . . . . . . . . . . . . . . . . 251
12.2.1 Reinforcement Stress . . . . . . . . . . . . . . . . . . . 253
12.2.2 Bending Moments in the Beam . . . . . . . . . . . . . . 254
12.2.3 Forces in the Beam . . . . . . . . . . . . . . . . . . . . 255
12.3 Serviceability Limit State Analysis . . . . . . . . . . . . . . . . . 256
12.3.1 Adapting the Element Integration Scheme . . . . . . . 256
12.3.2 Running the Analysis . . . . . . . . . . . . . . . . . . . 256
12.3.3 Prestress Relaxation in the Tendon . . . . . . . . . . . 258
12.3.4 Stress Relaxation in the Beam . . . . . . . . . . . . . . 259
12.4 Ultimate Limit State Analysis . . . . . . . . . . . . . . . . . . . 260
12.4.1 Plastic Yield in the Tendon . . . . . . . . . . . . . . . . 263
12.4.2 Stress in the Tendon . . . . . . . . . . . . . . . . . . . . 264
12.4.3 Crack Development in the Beam . . . . . . . . . . . . . 265
13 Long Term Behavior of RC Beam 269
13.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 270
13.2 Preliminary Linear Analysis . . . . . . . . . . . . . . . . . . . . 272
13.2.1 Displacements . . . . . . . . . . . . . . . . . . . . . . . 273
13.2.2 Shear Force and Bending Moment . . . . . . . . . . . . 274
13.3 Material Parameters . . . . . . . . . . . . . . . . . . . . . . . . . 275
13.4 Nonlinear Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . 277
13.4.1 Experiment C11 . . . . . . . . . . . . . . . . . . . . . . 278
13.4.2 Experiment C15 . . . . . . . . . . . . . . . . . . . . . . 281
14 Concrete Viaduct 287
14.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 288
14.1.1 Element Mesh and Reinforcement . . . . . . . . . . . . 290
14.1.2 Material Definition . . . . . . . . . . . . . . . . . . . . 294
14.1.3 Boundary Conditions . . . . . . . . . . . . . . . . . . . 297
14.2 Phased Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . 297
14.2.1 Phase One . . . . . . . . . . . . . . . . . . . . . . . . . 297
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis
CONTENTS xi
14.2.2 Phase Two . . . . . . . . . . . . . . . . . . . . . . . . . 299
14.2.3 Analysis and Results . . . . . . . . . . . . . . . . . . . 301
14.3 Appendix: Aging Study . . . . . . . . . . . . . . . . . . . . . . . 308
14.3.1 Loading Age One Day . . . . . . . . . . . . . . . . . . . 308
14.3.2 Loading Age 89 Days . . . . . . . . . . . . . . . . . . . 310
15 Stress Ribbon Bridge 313
15.1 Phase 1 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 314
15.1.1 Finite Element Model . . . . . . . . . . . . . . . . . . . 315
15.1.2 Initialization and Nonlinear Analysis . . . . . . . . . . 316
15.2 Phase 2 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 319
15.2.1 Material Models . . . . . . . . . . . . . . . . . . . . . . 319
15.2.2 Finite Element Model . . . . . . . . . . . . . . . . . . . 321
15.2.3 Thermal Contraction . . . . . . . . . . . . . . . . . . . 324
15.2.4 Nonlinear Analysis . . . . . . . . . . . . . . . . . . . . . 324
V Young Hardening Concrete 331
16 Hydration of Concrete Column 333
16.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 334
16.1.1 Geometry Definition . . . . . . . . . . . . . . . . . . . . 334
16.1.2 Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . . 335
16.1.3 Material Properties . . . . . . . . . . . . . . . . . . . . 336
16.1.4 Boundary and Initial Conditions . . . . . . . . . . . . . 338
16.2 Nonlinear Transient Heat Flow Analysis . . . . . . . . . . . . . . 339
16.2.1 Temperatures . . . . . . . . . . . . . . . . . . . . . . . 341
16.2.2 Degree of Reaction . . . . . . . . . . . . . . . . . . . . . 342
16.3 Nonlinear Structural Analysis . . . . . . . . . . . . . . . . . . . 342
16.3.1 Stresses . . . . . . . . . . . . . . . . . . . . . . . . . . . 344
17 Thermal and Flow–Stress Analysis of a Box Girder 347
17.1 Model for Thermal Analysis . . . . . . . . . . . . . . . . . . . . 348
17.1.1 Geometry Definition . . . . . . . . . . . . . . . . . . . . 348
17.1.2 Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . . 350
17.1.3 Material Properties . . . . . . . . . . . . . . . . . . . . 352
17.1.4 Boundary and Initial Conditions . . . . . . . . . . . . . 354
17.2 Transient Nonlinear Heat Flow Analysis . . . . . . . . . . . . . . 355
17.2.1 Temperature Within the Concrete . . . . . . . . . . . . 356
17.2.2 Degree of Reaction . . . . . . . . . . . . . . . . . . . . . 359
17.3 Model for Flow–Stress Analysis . . . . . . . . . . . . . . . . . . 360
17.3.1 Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . . 360
17.3.2 Material Properties . . . . . . . . . . . . . . . . . . . . 362
17.3.3 Flow Boundary and Initial Conditions . . . . . . . . . . 364
17.3.4 Mechanical Loading and Boundary Constraints . . . . . 365
17.4 Staggered Flow–Stress Analysis . . . . . . . . . . . . . . . . . . 366
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis November 8, 2010 – First ed.
xii CONTENTS
17.4.1 Thermal Strain . . . . . . . . . . . . . . . . . . . . . . . 368
17.4.2 Principal Stress . . . . . . . . . . . . . . . . . . . . . . 368
17.4.3 Longitudinal Stress . . . . . . . . . . . . . . . . . . . . 370
18 Wall with Cooling Pipes 371
18.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 371
18.1.1 Geometry Definition . . . . . . . . . . . . . . . . . . . . 372
18.1.2 Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . . 376
18.1.3 Materials and Physical Properties . . . . . . . . . . . . 377
18.1.4 Boundary and Initial Conditions . . . . . . . . . . . . . 380
18.2 Transient Nonlinear Heat Flow Analysis . . . . . . . . . . . . . . 382
18.2.1 Temperature within the Concrete . . . . . . . . . . . . 383
18.2.2 Degree of Reaction and Equivalent Age . . . . . . . . . 386
18.2.3 Temperature of Coolant . . . . . . . . . . . . . . . . . . 387
19 Cooling Pipes in a Tunnel 389
19.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 391
19.1.1 Geometry Definition . . . . . . . . . . . . . . . . . . . . 391
19.1.2 Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . . 400
19.1.3 Boundary Elements . . . . . . . . . . . . . . . . . . . . 401
19.1.4 Material and Physical Properties . . . . . . . . . . . . . 403
19.1.5 Boundary and Initial Conditions . . . . . . . . . . . . . 405
19.2 Transient Nonlinear Heat Flow Analysis . . . . . . . . . . . . . . 406
19.2.1 Temperature within Concrete . . . . . . . . . . . . . . . 408
19.2.2 Degree of Reaction . . . . . . . . . . . . . . . . . . . . . 411
19.2.3 Internal Temperature of Cooling Pipe . . . . . . . . . . 412
20 Early Age Behavior of a Purification Wall 415
20.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 416
20.1.1 Geometry Definition . . . . . . . . . . . . . . . . . . . . 416
20.1.2 Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . . 418
20.1.3 Modeling the Boundary . . . . . . . . . . . . . . . . . . 420
20.1.4 Material Properties . . . . . . . . . . . . . . . . . . . . 421
20.1.5 Boundary Conditions and Loading . . . . . . . . . . . . 425
20.1.6 Boundary Constraints . . . . . . . . . . . . . . . . . . . 426
20.1.7 Initial Temperature Field . . . . . . . . . . . . . . . . . 427
20.2 First Stage – Casting the Base Slab . . . . . . . . . . . . . . . . 428
20.2.1 Heat Flow Analysis Results . . . . . . . . . . . . . . . . 429
20.2.2 Structural Analysis Results . . . . . . . . . . . . . . . . 430
20.3 Second Stage – Casting the Wall . . . . . . . . . . . . . . . . . . 433
20.3.1 Heat Flow Analysis Results . . . . . . . . . . . . . . . . 435
20.3.2 Structural Analysis Results . . . . . . . . . . . . . . . . 436
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis
CONTENTS xiii
21 Adiabatic Hydration of Concrete 441
21.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 442
21.2 Nonlinear Transient Analysis . . . . . . . . . . . . . . . . . . . . 443
21.2.1 Temperature and Degree of Reaction . . . . . . . . . . 445
21.2.2 Time Response . . . . . . . . . . . . . . . . . . . . . . . 446
VI Masonry Modeling 447
22 Interfaces in Masonry Wall 449
22.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 450
22.1.1 Geometry Definition . . . . . . . . . . . . . . . . . . . . 450
22.1.2 Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . . 452
22.1.3 Supports . . . . . . . . . . . . . . . . . . . . . . . . . . 453
22.1.4 Material and Physical Properties . . . . . . . . . . . . . 454
22.1.5 Loading . . . . . . . . . . . . . . . . . . . . . . . . . . . 456
22.1.6 Gluing the Surfaces Together . . . . . . . . . . . . . . . 456
22.1.7 Temperature in Time . . . . . . . . . . . . . . . . . . . 458
22.2 Transient Nonlinear Analysis . . . . . . . . . . . . . . . . . . . . 458
22.2.1 Deformation and Horizontal Stress . . . . . . . . . . . . 460
23 Discrete Modeling of Masonry 463
23.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 464
23.1.1 Modeling Half a Brick . . . . . . . . . . . . . . . . . . . 465
23.1.2 Material and Physical Properties . . . . . . . . . . . . . 466
23.1.3 Creating the Two-brick Model . . . . . . . . . . . . . . 468
23.1.4 Expansion to the Complete Model . . . . . . . . . . . . 469
23.1.5 Cutting the Hole . . . . . . . . . . . . . . . . . . . . . . 472
23.1.6 Boundary Constraints and Loading . . . . . . . . . . . 472
23.1.7 Generating the Final Mesh . . . . . . . . . . . . . . . . 473
23.2 Linear Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . 475
23.2.1 Displacements . . . . . . . . . . . . . . . . . . . . . . . 476
23.2.2 Strains . . . . . . . . . . . . . . . . . . . . . . . . . . . 476
23.3 Nonlinear Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . 477
23.3.1 Displacements . . . . . . . . . . . . . . . . . . . . . . . 479
23.3.2 Stresses in the Bricks . . . . . . . . . . . . . . . . . . . 480
23.3.3 Crack Strain . . . . . . . . . . . . . . . . . . . . . . . . 480
23.4 Additional Exercise . . . . . . . . . . . . . . . . . . . . . . . . . 482
23.4.1 Nonlinear Analysis . . . . . . . . . . . . . . . . . . . . . 483
23.4.2 Displacements . . . . . . . . . . . . . . . . . . . . . . . 484
23.4.3 Stresses in the Bricks . . . . . . . . . . . . . . . . . . . 485
23.4.4 Crack Strain . . . . . . . . . . . . . . . . . . . . . . . . 485
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis November 8, 2010 – First ed.
xiv CONTENTS
24 Composite Modeling of Masonry 489
24.1 Finite Element Model . . . . . . . . . . . . . . . . . . . . . . . . 489
24.1.1 Geometry Definition . . . . . . . . . . . . . . . . . . . . 490
24.1.2 Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . . 491
24.1.3 Material and Physical Properties . . . . . . . . . . . . . 492
24.1.4 Boundary Conditions . . . . . . . . . . . . . . . . . . . 493
24.2 Preliminary Linear Analysis . . . . . . . . . . . . . . . . . . . . 494
24.2.1 Deformation . . . . . . . . . . . . . . . . . . . . . . . . 495
24.3 Nonlinear Static Analysis . . . . . . . . . . . . . . . . . . . . . . 495
24.3.1 Displacements . . . . . . . . . . . . . . . . . . . . . . . 497
24.3.2 Stresses . . . . . . . . . . . . . . . . . . . . . . . . . . . 498
24.3.3 Plastic Strain as Crack Pattern . . . . . . . . . . . . . . 498
24.4 Including Creep Effects . . . . . . . . . . . . . . . . . . . . . . . 500
24.4.1 Material Properties . . . . . . . . . . . . . . . . . . . . 501
24.4.2 Transient Loading . . . . . . . . . . . . . . . . . . . . . 501
24.5 Nonlinear Transient Analysis . . . . . . . . . . . . . . . . . . . . 502
24.5.1 Displacements . . . . . . . . . . . . . . . . . . . . . . . 503
24.5.2 Stresses . . . . . . . . . . . . . . . . . . . . . . . . . . . 504
24.5.3 Strains . . . . . . . . . . . . . . . . . . . . . . . . . . . 505
Bibliography 507
Index 509
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis
Preface
This volume of the Diana User’s Manual describes how to apply the various
Diana modules for concrete and masonry analysis.
Cautionary note
Throughout this manual, it will be assumed that the reader has a
basic understanding of the Finite Element Method in general and of
concrete and masonry applications in particular.
Related volumes. Familiarity with notation conventions and general aspects
of Diana use as described in Volume Getting Started will be assumed. Some fa-
miliarity with Volumes Pre- and Postprocessing, Analysis Procedures, Element
Library, and Material Library will be assumed as well. Moreover, there are two
more volumes with examples of Diana analyses:
Volume Analysis Examples describes general examples, not specifically
related to concrete, masonry, or geotechnics.
Volume Geotechnical Analysis describes examples related to geotechnics.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis November 8, 2010 – First ed.
xvi Preface
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis
Glossary of Symbols
This glossary is additional to the general Glossary of Symbols for Diana. It
describes the symbols used particularly in concrete and masonry analysis.
1
Scalars
D11 Linear stiffness modulus [N/m2 ].
D22 Linear stiffness modulus [N/m2 ].
Gcr Shear modulus after cracking [N/m2 ].
Gf Fracture energy [N/m2 ].
K Conduction coefficient [W/(m2 ·K)].
c Volumetric thermal capacity [J/(m3 ·K)].
cA Arrhenius constant [K].
co Reinforcement coverage [m].
ft Tensile strength [N/m2 ].
m01 Reinforcement moment, X [N·m/m].
m02 Reinforcement moment, Y [N·m/m].
n01 Reinforcement force, normal, X [N / m].
n02 Reinforcement force, normal, Y [N / m].
n0c
1 Reinforcement force, combined, X [N / m].
n0c
2 Reinforcement force, combined, Y [N / m].
q 0 Reinforcement force, shear [N / m].
teq Reinforcement equivalent thickness [m].
zr Relative internal beam arm.
β Shear retention factor [−].
εc Creep strain [−].
εcr Crack strain [−].
εp Plastic strain [−].
1 SI-units in brackets.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis November 8, 2010 – First ed.
xviii Glossary of Symbols
εu Ultimate strain [−].
λ Thermal conductivity [W/(m·K)].
σy Yield stress of steel [N/m2 ].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis
Part I
General Introduction
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (I) November 8, 2010 – First ed.
Chapter 1
Basic Principles
Generally speaking a concrete and masonry analysis with Diana requires the
following actions.
Model definition. Typically you will define the model in the Preprocessing
environment of iDiana, as introduced in Volume Getting Started and formally
described in Volume Pre- and Postprocessing, or in FX+, as described in Volume
FX+ for DIANA.
Structural nonlinear analysis. In a concrete analysis, Module nonlin is
the core module, which handles the nonlinear constitutive models for concrete
and masonry-like materials in combination with load steps and/or time steps.
Heat flow analysis. A concrete analysis may also consist of a single heat
flow analysis to investigate the hardening process.
Phased analysis. A concrete analysis is often performed in phases to simulate
the various stages of construction. Diana offers Module phase to perform such
a ‘phased analysis’. This analysis handles the transfer from analysis results, like
displacements, strains and stresses, from one phase to a next phase.
Coupled flow–stress analysis. To analyze for instance the stress develop-
ment after pouring of concrete, or for a structural analysis of concrete members
subjected to a thermal load, Diana offers coupled flow–stress analysis.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (I) November 8, 2010 – First ed.
4 Basic Principles
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (I)
Part II
Structural Design
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
Chapter 2
Reinforcement Forces and
Moments for a Bridge
Name: ReBridge
Path: /Examples/ConcMas/ReBridge
Keywords: analys: linear static. constr: suppor. elemen: cq40s curved
shell. load: edge elemen face force weight. materi: elasti
isotro. option: direct groups units. post: binary femvie.
result: cauchy displa force moment reinfo stress total.
8000 10000 8000
(a) span
Lane 1 Lane 2
1000 3000 3000 500
8000
(b) cross-section
Figure 2.1: Bridge [mm]
This example aims at designing the reinforcements of a bridge. To prevent
failure of the bridge we have to know the amount and direction of reinforce-
ment needed. Diana allows for a relatively easy determination of the forces
and moments which are to be supported by the reinforcement, which will be
illustrated. In this example we construct a plate bridge consisting of massive
concrete [Fig. 2.1]. The bridge comprises three fields constructed as a continu-
ous plate. The first and last span is 8 meters long, the middle is 10 meters long.
The width of the deck is 8 meters.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
8 Reinforcement Forces and Moments for a Bridge
2.1 Finite Element Model
To build up the finite element model, we start iDiana and we enter the Design
environment with the model name BRIDGE.
iDiana
FEMGEN BRIDGE
Analysis and Units
Analysis Selection
Model Type: →Structural 3D
Units Definition
Length: →Millimeter
Mass: →Kilogram
Force: →Newton
In the Analysis and Units dialog we specify the model type for a three-dimen-
sional structural analysis and the adopted units [mm, kg, N].
2.1.1 Geometry Definition
To define the geometry we apply eight points P1 to P8 [Fig. 2.2].
Lane 2
3000
P4 P8
Lane 1
3000
Y
P3 P7
P2 P6
P1 P5
X
Z
2×500
8000
Figure 2.2: Top view (plan) of first span bridge [mm]
Points bridge.fgc
GEOMETRY POINT COORD 0 0
GEOMETRY POINT COORD 0 500
GEOMETRY POINT COORD 0 1000
GEOMETRY POINT COORD 0 4000
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
2.1 Finite Element Model 9
GEOMETRY POINT COORD 8000 0
GEOMETRY POINT COORD 8000 500
GEOMETRY POINT COORD 8000 1000
GEOMETRY POINT COORD 8000 4000
EYE FRAME
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY POINTS
With a series of GEOMETRY POINT commands, we define the coordinates of the
points. With the EYE FRAME command we display the specified points fitted in
the iDiana viewport. We display the points with their name labels [Fig. 2.3a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:15 points.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:16 surf.ps
Model: BRIDGE Model: BRIDGE
Analysis: DIANA Analysis: DIANA
Model Type: Structural 3D Model Type: Structural 3D
P4 P8
S3
P3 P7
S2
P2 P6
S1
P1 P5
Y Y
Z X Z X
(a) points (b) surfaces
Figure 2.3: Geometry with labels
Surfaces bridge.fgc
GEOMETRY SURFACE 4POINTS P1 P5 P6 P2
GEOMETRY SURFACE 4POINTS P2 P6 P7 P3
GEOMETRY SURFACE 4POINTS P3 P7 P8 P4
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY SURFACES ALL BLUE
We specify the lines and the surfaces for the model via some GEOMETRY SURFACE
commands with the four corner points. The VIEW and LABEL commands display
the surfaces with their names [Fig. 2.3b].
Divisions bridge.fgc
LABEL GEOMETRY LINES
LABEL GEOMETRY DIVISIONS
MESHING DIVISION FACTOR ALL .5
DRAWING DISPLAY
MESHING DIVISION L1 32
MESHING DIVISION L3 32
MESHING DIVISION L6 32
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
10 Reinforcement Forces and Moments for a Bridge
MESHING DIVISION L8 14
MESHING DIVISION L9 32
MESHING DIVISION L10 14
DRAWING DISPLAY
In order to get a mesh with the desired amount and size of the elements, we
change the divisions of the lines. We start with a VIEW command to show all
geometry without any labels. When labeling the divisions of the lines we see
that all the divisions equal to four. This is the default value of the division.
We wish to create quadratic elements which are mainly 500 mm square. To
do this we must change the divisions per line. We use the command MESHING
DIVISION FACTOR to multiply the division of all lines with the specified factor.
With the MESHING DIVISION command we change the division for the lines. The
final DRAWING DISPLAY command refreshes the drawing so we can see the final
divisions [Fig. 2.4a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:16 divi.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:16 sweep.ps
Model: BRIDGE Model: BRIDGE
Analysis: DIANA Analysis: DIANA
Model Type: Structural 3D Model Type: Structural 3D
L9
32
L9 L17
32 20
L10
14
L10
S3 14
S3 S6
L8 L8 L13
14 14 14
L6 L16
L7 S2 32 20 S5
2 L5 L12
L3 2 L15 2
L6 L4 32 20
32 S1 L2 S4 L11
L7 2
S2 L1 2 L14 2
2 L5 32 20
L3 2
L4 32
2 S1
L2
L1 2
32
Y Y
Z X Z X
(a) surface lines (b) after sweeping an edge
Figure 2.4: Geometry and divisions
Sweeping an edge bridge.fgc
CONSTRUCT SET OPEN EDGE2H
CONSTRUCT SET APPEND LINES L2 L5 L8
CONSTRUCT SET CLOSE
VIEW GEOMETRY +EDGE2H GREEN
MESHING DIVISION DEFAULT 20
GEOMETRY SWEEP EDGE2H SE1 TRANSLATE TR1 5000 0 0
EYE FRAME
LABEL GEOMETRY SURFACES ALL BLUE
First we make a group of lines EDGE2H using the command CONSTRUCT SET. To
check this group we color it green. We want all new lines to have a division
of 20. Therefore we change the default setting of the division. The GEOMETRY
SWEEP command sweeps the group EDGE2H using a translation of 5000 mm in
X-direction. The division of the lines will be set to the specified default value
[Fig. 2.4b].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
2.1 Finite Element Model 11
Geometry for wheel loads. The bridge must be loaded with concentrated
wheel loads. These loads should be located on the most unfavorable position.
The critical position of the wheel load, in transverse as well as in longitudinal
direction can be determined with an influence field analysis in Diana. In this
example we assume that the wheel loads act on the middle of the second span
(in longitudinal direction) and at the middle of the lanes in transverse direction.
Figure 2.5 shows the concentrated wheel loads (as defined according to the Eu-
ropean code ENV 1991-3 [3]) and the location on the bridge. The wheel prints
♥
♥
Lane 1
3000
2000
Wheel prints
400×400
600
8000 5000
Figure 2.5: Concentrated wheel load
are 400 × 400 millimeters.1 Comparing this figure with the current geometry
[Fig. 2.4b] we see that the wheel load is located on surface S6. We will delete
this surface and create a new surface, with two internal surfaces exactly at the
location of the wheel loads. In this way we are able to put the wheel loads
exactly at the right location.
bridge.fgc
UTILITY DELETE S6
yes
VIEW GEOMETRY ALL VIOLET
GEOMETRY POINT COORD 12200 1300 0
GEOMETRY POINT COORD 12600 1300 0
GEOMETRY POINT COORD 12600 1700 0
GEOMETRY POINT COORD 12200 1700 0
MESHING DIVISION DEFAULT 2
GEOMETRY SURFACE 4POINTS P13 P14 P15 P16
GEOMETRY COPY S7 S8 TRANSLATE 0 2000 0
LABEL GEOMETRY DIVISIONS
VIEW GEOMETRY +S7 GREEN
VIEW GEOMETRY +S8 GREEN
After deleting a surface, viewing all geometry and label the surfaces, we see
that only the surface is deleted. The lines and points of this surface remain. We
1 In practice we have to enlarge the wheel prints because of spreading of the load with an
approximate angle of 45°over the thickness of the asphalt and half the thickness of the bridge
when modeling it with shell elements. We will omit this in this example.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
12 Reinforcement Forces and Moments for a Bridge
do not delete these points and lines because we need them later on. With the
command GEOMETRY COPY we copy surface S7 using a translation of 2000 mm
in Y -direction. Now the two surfaces for the wheel prints have been made. We
display them in green [Fig. 2.6].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:16 wheelp.ps
Model: BRIDGE
Analysis: DIANA
Model Type: Structural 3D
32 20
2
2
2
2
14
14 14
2
2
2
2
32 20
2
2 2
32 20
2
2 2
32 20
Z X
Figure 2.6: Surfaces for wheel loads (green)
bridge.fgc
LABEL GEOMETRY LINES ALL
CONSTRUCT SET LANE APPEND L16 L13 L17 L8
CONSTRUCT SET WHEEL1 APPEND L18 L19 L20 L21
CONSTRUCT SET WHEEL2 APPEND L22 L23 L24 L25
VIEW GEOMETRY LANE GREEN
VIEW GEOMETRY +WHEEL1 BLUE
VIEW GEOMETRY +WHEEL2 BLUE
GEOMETRY SURFACE REGION S9 LANE WHEEL1 WHEEL2
VIEW GEOMETRY S9 RED
To ensure a proper mesh we will now remake a surface for the lane, with the
surfaces of the wheel loads as internal ‘holes’. We start with labeling the lines of
the current geometry. Then we make a set LANE with the lines along the outer
edge of the lane surface. These lines form a closed loop. Likewise we assemble
the lines along the edges of the wheel loads in two sets WHEEL1 and WHEEL2.
The geometry of the three sets is now displayed [Fig. 2.7a]. We create a region
surface with the lines in set LANE as boundary and the lines in the sets WHEE1
and WHEEL2 as internal ‘holes’. Finally, we display the new surface [Fig. 2.7b].
2.1.2 Meshing
Because a quarter of the bridge is defined, we may now create a finite element
mesh on the geometry.
bridge.fgc
VIEW GEOMETRY ALL
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
2.1 Finite Element Model 13
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:16 geowhe.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:16 georeg.ps
Model: BRIDGE Model: BRIDGE
Analysis: DIANA Analysis: DIANA
Model Type: Structural 3D Model Type: Structural 3D
Y Y
Z X Z X
(a) line sets (b) region surface
Figure 2.7: Making a region surface around the wheel loads
MESHING TYPES ALL QU8 CQ40S
MESHING GENERATE
VIEW OPTIONS SHRINK
VIEW HIDDEN SHADE
VIEW MESH S9 RED
VIEW MESH +S7 BLUE
VIEW MESH +S8 BLUE
VIEW OPTIONS COLOUR QUALITY
VIEW MESH ALL
We activate the complete geometry and select element type CQ40S (curved shell)
for all generic QU8 elements (8-node quadrilaterals). We generate the mesh and
then view it in ‘shrunken elements’ style. First only the mesh for the region
surface, with the elements below the wheel loads in blue [Fig. 2.8a]. Note that
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:16 mesh1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:16 mesh2.ps
Model: BRIDGE Model: BRIDGE
Analysis: DIANA Analysis: DIANA
Model Type: Structural 3D Model Type: Structural 3D
Y Y
Z X Z X
Quality
All Tests
PASS
(a) lane section with wheels (b) complete, colored for quality
Figure 2.8: Element mesh
the ‘holes’ for the wheel loads are not real holes: an element is generated for
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
14 Reinforcement Forces and Moments for a Bridge
each of the holes because the surfaces which represent them are still part of
the geometry. Finally, we display all the elements, colored according to their
‘quality’ [Fig. 2.8b]. We see that all elements are green which indicates that
none of the elements fails the quality test.
Expanding the mesh bridge.fgc
VIEW HIDDEN OFF
CONSTRUCT SET QUART APPEND ALL
GEOMETRY COPY QUART MIRROR Y 4000
CONSTRUCT SET HALF1 APPEND ALL
VIEW GEOMETRY HALF1 BLUE
EYE FRAME
Currently we only have a model for one quarter of the bridge. We can easily
expand this model to a complete model via two mirror transformations. First
we assemble the current geometry in a set QUART. We mirror this set via an
horizontal mirror plane at Y = 4000. This way the quarter geometry is mirrored
in Y -direction such that we obtain half the geometry of the complete bridge
model. We assemble the current geometry in a set HALF1 which we display in
blue [Fig. 2.9a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:17 geom1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:17 geomtot.ps
Model: BRIDGE Model: BRIDGE
Analysis: DIANA Analysis: DIANA
Model Type: Structural 3D Model Type: Structural 3D
Y Y
Z X Z X
(a) from quarter to half (b) from half to full: complete
Figure 2.9: Expanding the geometry
bridge.fgc
GEOMETRY COPY HALF1 HALF2 MIRROR X 13000
VIEW GEOMETRY +HALF2 VIOLET
EYE FRAME
MESHING GENERATE
VIEW HIDDEN SHADE
VIEW MESH
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
2.1 Finite Element Model 15
We repeat the mirror procedure, but now with a vertical mirror at X = 13000.
We assemble the mirrored geometry in a set HALF2 which we display in violet
[Fig. 2.9b]. Finally, we regenerate the mesh, now for the complete geometry,
and display it [Fig. 2.10].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:17 meshtot.ps
Model: BRIDGE
Analysis: DIANA
Model Type: Structural 3D
Z X
Quality
All Tests
PASS
Figure 2.10: Element mesh of bridge slab
2.1.3 Axes Consistency
We want to analyze local element output, for example distributed moments and
forces. For this, it is convenient to have consistent element axes.
bridge.fgc
VIEW HIDDEN OFF
VIEW GEOMETRY ALL
EYE ROTATE TO 45 30 30
LABEL GEOMETRY AXES ALL Z RED
GEOMETRY POINT COORD 0 0 1
CONSTRUCT COORDSYS RECTANGUL CS1 P1 P68 P38
PROPERTY ATTACH ALL COORDSYS CS1
GEOMETRY FLIP CONSISTENT ALL
LABEL GEOMETRY AXES ALL Z RED
DRAWING DISPLAY
We start with a three-dimensional view of the geometry. Then we display the
local z-axes with red arrows [Fig. 2.11a]. We see that there is no consistency in
the directions: some z-axes point upward, others downward. To solve this we
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
16 Reinforcement Forces and Moments for a Bridge
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:17 ax1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:17 ax2.ps
Model: BRIDGE Model: BRIDGE
Analysis: DIANA Analysis: DIANA
Model Type: Structural 3D Model Type: Structural 3D
Z Z
Y Y
X X
(a) before flipping - inconsistent (b) after flipping - consistent
Figure 2.11: Geometry local z-axes
define a rectangular coordinate system CS1 with its origin at point P1 (0,0,0),
the z-axis to point P68 (in global Z-direction) and the x-axis to point P38 (in
global X-direction). We attach this coordinate system to all geometry. Now
we use the FLIP CONSISTENT option to get consistent local z-axis directions. A
redisplay confirms the consistency [Fig. 2.11b].
2.1.4 Material and Physical Properties
We define the properties via the Property Manager dialog.
iDiana
View →Property Manager...
↑
Property Manager
↑Materials Material Name: CONCRETE
↑Linear Elasticity →Isotropic
↑Mass →Mass Density
↑Physical Properties Physical Property Name: THICK
↑Geometry →Curved Shell →Regular
We define a material CONCRETE with Young’s modulus E = 31000 N/mm2 ,
Poisson’s ratio ν = 0.2, and mass density ρ = 2.4×10−6 kg/mm3 . We also
define a physical property THICK with a thickness of 330 mm.
bridge.fgc
PROPERTY ATTACH ALL CONCRETE
PROPERTY ATTACH ALL THICK
We attach the defined properties to the complete geometry of the model.
2.1.5 Boundary Constraints
We define the supports (boundary constraints) with the following commands.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
2.1 Finite Element Model 17
bridge.fgc
EYE ANGLE 0
VIEW GEOMETRY ALL
LABEL GEOMETRY LINES
CONSTRUCT SET SUP1 APPEND L4 L7 L10 L34 L32 L29
CONSTRUCT SET OPEN SUPZ
CONSTRUCT SET APPEND SUP1
GEOMETRY COPY SUP1 SUP2 TRANSLATE 8000 0 0
GEOMETRY COPY SUP2 SUP3 TRANSLATE 10000 0 0
GEOMETRY COPY SUP3 SUP4 TRANSLATE 8000 0 0
CONSTRUCT SET CLOSE
VIEW GEOMETRY +SUPZ RED
We create a group SUP1 containing all the lines at the left edge of the bridge.
From this set we create a set SUPZ to contain all lines that must be supported
vertically. With three copy operations we copy the geometry of an existing set
into a new set using an appropriate translation in X-direction. Because target
lines do already exist, each copy operation will create a new set but no new
lines. For confirmation we display the new set SUPZ in red [Fig. 2.12a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:18 sups.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:18 constr.ps
Model: BRIDGE Model: BRIDGE
Analysis: DIANA Analysis: DIANA
Model Type: Structural 3D Model Type: Structural 3D
L26 L27 L38 L35 L80 L72 L71
L29 L28 L39 L81 L73 L74
L32 L30 L36 L75 L77
L31 L40 L82 L76
L41 L83
L42L84
L44
L43 L85L86
L33 L37 L78
L34 L79
L45 L87
L46L88
L48 L90
L47 L89
L9 L17 L62 L57
L24 L69
L25 L70
L23L68
L22 L67
L10 L58
L8 L13 L56
L20 L65
L21 L66
L19L64
L18 L63
L7 L6 L16 L61 L54 L55
L3 L5 L15 L12 L60 L53 L51
L4 L2 L11 L50 L52
L1 L14 L59 L49
Y
Z
Y
Z X
X
(a) sets for vertical supports (b) supports
Figure 2.12: Defining boundary constraints
bridge.fgc
PROPERTY BOUNDARY CONSTRAINT CO1 SUPZ Z
PROPERTY BOUNDARY CONSTRAINT CO2 P1 X Y
PROPERTY BOUNDARY CONSTRAINT CO3 P21 X
PROPERTY BOUNDARY CONSTRAINT CO4 P38 Y
MESHING GENERATE
EYE ROTATE TO 45 30 30
VIEW MESH
LABEL MESH CONSTRNT ALL
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
18 Reinforcement Forces and Moments for a Bridge
We define the constraints with appropriate specification of the supported de-
gree(s) of freedom: Z for the set SUPZ, X and Y for the origin, X for the top-left
vertex and Y for the bottom-right vertex. We regenerate the mesh and display
the supports as spikes in a three-dimensional view [Fig. 2.12b].
2.1.6 Loads
We will first analyze the construction phase. In this phase the bridge is loaded
with the dead weight and a distributed load of asphalt. The load of the asphalt
is 3.22 kN/m2 . We apply these loads with the following commands:
bridge.fgc
PROPERTY LOADS GRAVITY LO1 ALL -9.8 Z
LABEL MESH OFF
LABEL MESH LOADS LO1 ORANGE
CONSTRUCT SET DECK APPEND SURFACES ALL
PROPERTY LOADS PRESSURE LO2 DECK -3.22E-3 Z
LABEL MESH OFF
LABEL MESH LOADS LO2 VIOLET
With the GRAVITY load class we apply the dead weight of the bridge. For the dis-
tributed asphalt load we define a set DECK and apply the load via the PRESSURE
load class. We display both loads with different colors [Fig. 2.13].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:18 load1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:19 load2.ps
Model: BRIDGE Model: BRIDGE
Analysis: DIANA Analysis: DIANA
Model Type: Structural 3D Model Type: Structural 3D
Z Z
Y Y
X X
(a) dead weight (b) distributed asphalt
Figure 2.13: View of the loads
2.2 Linear Analysis
Before we can run an analysis we must write the model to a file in Diana batch
format and initiate the analysis.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
2.2 Linear Analysis 19
iDiana
SAVE AS BRIDG1
yes
Bridge model for first analysis
UTILITY WRITE DIANA bridg1.dat
yes
FILE CLOSE
yes
Bridge model
ANALYSE BRIDG1
Analysis Setup
Input Data File(s) Path: bridg1.dat ↑ OK
Reading Input ··· ↑ OK
Select Analysis Type
Type →Structural linear static ↑ OK
DIANA
⇑Structural linear static →Edit...
Structural Linear Static Settings ↑ Output
Model • User
° Selection ↑ Modify
Model Selection ↑ Elements ↑ Add
Elements Selection
¤
g Axes for Transformation of Strains or Stresses
Relative Internal Beam Arms 1: 0.8
Coverages 1: 30
↑ OK
Model Selection ↑ OK
Structural Linear Static Settings Output
Result • User
° Selection ↑ Modify
Results Selection
→DISPLA →TOTAL →TRANSL →GLOBAL ↑ Add
→STRESS →TOTAL →CAUCHY →GLOBAL ↑ Add
→STRESS →TOTAL →DISFOR →LOCAL ↑ Add
→STRESS →TOTAL →DISMOM →LOCAL ↑ Add
→STRESS →TOTAL →DISFOR →REINFO ↑ Add
→STRESS →TOTAL →DISMOM →REINFO ↑ Add
↑ OK
Structural Linear Static Settings ↑ OK
DIANA
↑File →Save Command File As...
Save Command File As
File Name: lin.dcf ↑ Save
DIANA
↑Analysis →Run
Calculating · · · ↑ OK
DIANA
↑ File → Exit
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
20 Reinforcement Forces and Moments for a Bridge
In the Analysis Setup dialog we specify the parameters and options for the
analysis of the model. In the Elements Selection dialog we specify a coverage
co = 30 mm and a relative internal beam arm zr = 80% of the effective height
(= ht − co). In the Results Selection dialog we select appropriate output items.
We save the commands on a file lin.dcf which looks as follows.
lin.dcf
*FILOS
INITIA
*INPUT
*LINSTA
BEGIN OUTPUT
BEGIN SELECT
BEGIN ELEMEN
BEGIN REAXES
CO 30
ZR 0.8
END REAXES
END ELEMEN
END SELECT
DISPLA TOTAL TRANSL GLOBAL
STRESS TOTAL CAUCHY GLOBAL
STRESS TOTAL DISFOR LOCAL
STRESS TOTAL DISMOM LOCAL
STRESS TOTAL DISMOM REINFO
STRESS TOTAL DISFOR REINFO
END OUTPUT
*END
To assess the results we enter the iDiana Results environment with the name
of the model.
bridg1.fvc
FEMVIEW BRIDG1
VIEW MESH
VIEW OPTIONS EDGES OUTLINE
RESULTS LOADCASE LC1
We start with a two-dimensional outline view of the finite element mesh. We
select load case LC1 which includes the dead weight and the asphalt loading.
2.2.1 Displacements
To display the vertical displacement we give the following commands:
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
2.2 Linear Analysis 21
bridg1.fvc
RESULTS NODAL DTX....G DTZ
PRESENT CONTOUR LEVELS
EYE ROTATE TO 45 30 30
VIEW OPTIONS SHRINK
VIEW OPTIONS DEFORM USING DTX....G RESDTX
We select the nodal result attribute DTZ which represents the vertical displace-
ments. For these results we make a contour plot [Fig. 2.14a]. In the results
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:34 disp1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:34 disp2.ps
Model: BRIDG1 Model: BRIDG1
LC1: Load case 1 Deformation = 454
Nodal DTX....G DTZ LC1: Load case 1
Max = 0 Nodal DTX....G DTZ
Min = -3.37 Max = 0
Min = -3.37
-.306 -.306
-.612 -.612
-.918 -.918
-1.22 -1.22
Y -1.53 -1.53
-1.84 Z -1.84
-2.14 Y -2.14
Z X -2.45 -2.45
-2.75 -2.75
-3.06 X -3.06
(a) 2D outline view (b) 3D view in deformed model
Figure 2.14: Contour plot of vertical displacements
monitor we see that the maximum deflection is 3.37 mm. It is even more in-
structive to display the contour plot in a three-dimensional view of the mesh in
‘shrunken elements’ style. Therefore we change the viewing direction and apply
the SHRINK and DEFORM viewing options [Fig. 2.14b].
2.2.2 Stresses
To display the stresses we give the following commands.
bridg1.fvc
RESULTS ELEMENT EL.SXX.G SXX
RESULTS RANGE SURFACE BOTTOM
PRESENT CONTOUR LEVELS
RESULTS RANGE SURFACE TOP
PRESENT CONTOUR LEVELS
We select the element result attribute SXX which represents the stresses in the
global X-direction σXX . With the RANGE and SURFACE options we indicate
that we want to see the stresses in the lower plane. We display a contour plot
of the stresses in the lower plane [Fig. 2.15a]. Notice that positive (tension)
stresses (orange and red) occur in areas around the middle of the spans. We
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
22 Reinforcement Forces and Moments for a Bridge
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:35 sxx1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:35 sxx2.ps
Model: BRIDG1 Model: BRIDG1
Deformation = 454 Deformation = 454
LC1: Load case 1 LC1: Load case 1
Element EL.SXX.G SXX Element EL.SXX.G SXX
Bottom (first) surface Top (last) surface
Max = 2.78 Max = 5.18
Min = -5.18 Min = -2.78
2.06 4.46
1.33 3.74
.608 3.01
-.116 2.29
-.84 1.56
Z -1.56 Z .84
Y -2.29 Y .116
-3.01 -.608
-3.74 -1.33
X -4.46 X -2.06
(a) lower plane (b) upper plane
Figure 2.15: Stresses in X-direction (σXX )
also display the stresses in the upper plane [Fig. 2.15b]. Here the tension stresses
occur around the two mid support lines.
2.2.3 Local Element Axes
In the next sections we will assess the bending moments and forces. Because
these results are defined in local element directions we may check the consistency
of the element x-axes, which we had in mind during the preparation of the model
[§ 2.1.3 p. 15].
bridg1.fvc
EYE ANGLE 0
VIEW OPTIONS SHRINK OFF
VIEW OPTIONS DEFORM OFF
VIEW MESH
LABEL MESH AXES ELEMENT X RED QUICK
EYE ZOOM FACTOR 10
We switch off the current viewing options to get a two-dimensional view of
the mesh. Then we display the local x-axes directions [Fig. 2.16a]. Due to the
QUICK option iDiana will display only one arrow per element, instead of one
for each Gauss point. This way we are able to check the consistency of the
x-axis direction. We zoom in on the center of the model to confirm the axes
consistency even more [Fig. 2.16b].
bridg1.fvc
LABEL MESH OFF
RESULTS RANGE OFF
EYE FRAME
VIEW OPTIONS EDGES OUTLINE
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
2.2 Linear Analysis 23
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:35 xax1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:35 xax2.ps
Model: BRIDG1 Model: BRIDG1
Y Y
Z X Z X
(a) full model (b) zoomed in
Figure 2.16: Directions of local element x-axes
We revert to an outline view of the full model. Because moments and forces are
single surface results we switch off the surface range selection.
2.2.4 Distributed Bending Moments
We will now assess the bending moments.
bridg1.fvc
RESULTS ELEMENT EL.MXX.L MXX
PRESENT CONTOUR LEVELS
PRESENT GRAPH LINE NODES THROUGH 236 1745
We select the element result attribute MXX which represents the element bending
moments mxx . We display these in a contour plot [Fig. 2.17a]. We also display a
diagram for mxx along the center line of the bridge slab [Fig. 2.17b]. We define
the line with two nodes at both ends of the bridge. Here we specify the nodes by
their number. In practice it is more convenient to select them via the graphics
cursor.
bridg1.fvc
VIEW MESH
VIEW OPTIONS EDGES OUTLINE
RESULTS ELEMENT EL.MXX.L MYY
PRESENT CONTOUR LEVELS
PRESENT GRAPH LINE NODES THROUGH 236 1745
Bending moments in transverse direction myy are represented by the MYY result
attribute. We display a contour plot and a diagram [Fig. 2.18].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
24 Reinforcement Forces and Moments for a Bridge
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:35 mxxc.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:35 mxxd.ps
Model: BRIDG1 Model: BRIDG1
LC1: Load case 1 LC1: Load case 1
Element EL.MXX.L MXX Element EL.MXX.L MXX
Max = .941E5 Max/Min on whole graph:
Min = -.505E5 Ymax = .885E5
Ymin = -.479E5
Xmax = .26E5
*1E4 Xmin = 0
Variation along a line
10
8
E
L
E 6
M
E
N
T 4
E
L 2
.
M
X
X 0
. 0 .25 .5 .75 1 1.25 1.5 1.75 2 2.25 2.5 2.75
L
*1E4
M -2
X
X
-4
.809E5
.678E5
.547E5 -6
.415E5 DISTANCE
Y .284E5
.152E5
.211E4
Z X -.11E5
-.242E5
-.373E5
(a) contour plot (b) diagram for center line
Figure 2.17: Bending moment mxx
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:36 myyc.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:36 myyd.ps
Model: BRIDG1 Model: BRIDG1
LC1: Load case 1 LC1: Load case 1
Element EL.MXX.L MYY Element EL.MXX.L MYY
Max = .195E5 Max/Min on whole graph:
Min = -.808E4 Ymax = .177E5
Ymin = -.808E4
Xmax = .26E5
*1E4 Xmin = 0
Variation along a line
2
1.75
E 1.5
L
E 1.25
M
E
N 1
T
.75
E
L .5
.
M
X .25
X
. 0
L 0 .25 .5 .75 1 1.25 1.5 1.75 2 2.25 2.5 2.75
M -.25 *1E4
Y
Y -.5
.17E5 -.75
.145E5
.12E5 -1
.949E4 DISTANCE
Y .698E4
.447E4
.196E4
Z X -551
-.306E4
-.557E4
(a) contour plot (b) diagram for center line
Figure 2.18: Bending moment myy
2.2.5 Distributed Forces
We may assess the normal forces with the following commands.
bridg1.fvc
VIEW MESH
VIEW OPTIONS EDGES OUTLINE
RESULTS ELEMENT EL.NXX.L NXX
PRESENT CONTOUR FROM -0.1 TO 0.1 LEVELS 4
RESULTS ELEMENT EL.NXX.L NYY
PRESENT CONTOUR FROM -0.1 TO 0.1 LEVELS 4
Result attributes NXX and NYY respectively represent the normal forces nxx and
nyy . The two contour plots confirm that in this load case only bending moments
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
2.2 Linear Analysis 25
are present [Fig. 2.19]. The extreme values of the forces are virtually zero, as
indicated in the results monitor.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:36 nxx.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:36 nyy.ps
Model: BRIDG1 Model: BRIDG1
LC1: Load case 1 LC1: Load case 1
Element EL.NXX.L NXX Element EL.NXX.L NYY
Max = .524E-11 Max = .556E-11
Min = -.955E-11 Min = -.374E-11
Y .1 Y .1
.6E-1 .6E-1
.2E-1 .2E-1
Z X -.2E-1 Z X -.2E-1
-.6E-1 -.6E-1
-.1 -.1
(a) nxx (b) nyy
Figure 2.19: Normal forces [sic]
2.2.6 Reinforcement Moments
In this model membrane forces can be neglected [§ 2.2.5], so reinforcement
only needs to support bending moments. Because there are no torsional shear
stresses, the reinforcement moments are equal to the distributed moments. Note
that the results of the reinforcement moments in the lower and upper planes are
similar. This corresponds to the definition of requirement of reinforcement:
Positive reinforcement moments in a positive surface (in this model
the upper plane) require reinforcement. In a negative plane (lower),
due to the definition of moments, negative moments require rein-
forcement.
With a simple trick we can easily display the areas of the model that require
reinforcement: in a contour plot with VALUES 0, iDiana will display positive
values in red, and negative values in blue.
bridg1.fvc
RESULTS ELEMENT EL.M1R.S M1R
RESULTS RANGE SURFACE BOTTOM
PRESENT CONTOUR VALUES 0
RESULTS RANGE SURFACE TOP
PRESENT CONTOUR VALUES 0
RESULTS ELEMENT EL.M1R.S M2R
RESULTS RANGE SURFACE BOTTOM
PRESENT CONTOUR VALUES 0
RESULTS RANGE SURFACE TOP
PRESENT CONTOUR VALUES 0
Result attributes M1R and M2R are the reinforcement moments in X- and Y -
direction respectively. We display contour plots for the lower and upper planes
[Fig. 2.20]. Looking at the results we can conclude that reinforcement in X-
direction is required in the lower plane at the spans (blue) [Fig. 2.20a] and in
the upper plane above the support lines (red) [Fig. 2.20b]. Reinforcement in Y -
direction is required in the lower plane at the spans (blue) [Fig. 2.20c] and in the
upper plane also at the spans and a bit along the long edges (red) [Fig. 2.20d].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
26 Reinforcement Forces and Moments for a Bridge
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:37 m1r1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:37 m1r2.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:37 m2r1.ps
Model: BRIDG1 Model: BRIDG1 Model: BRIDG1
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Element EL.M1R.S M1R Element EL.M1R.S M1R Element EL.M1R.S M2R
Bottom (first) surface Top (last) surface Bottom (first) surface
Max = .94E5 Max = .946E5 Max = .195E5
Min = -.506E5 Min = -.504E5 Min = -.909E4
Y Y Y
Z X Z X Z X
0 0 0
(a) lower, X-dir. (b) upper, X-dir. (c) lower, Y -dir.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:37 m2r2.ps
Model: BRIDG1
LC1: Load case 1
Element EL.M1R.S M2R
Top (last) surface
Max = .198E5
Min = -.808E4
Z X
0
(d) upper, Y -dir.
Figure 2.20: Reinforcement moments (red is +, blue is −)
2.2.7 Reinforcement Forces
Reinforcement forces only occur if membrane forces are present. As this is not
the case in this model [§ 2.2.5] we expect these to be zero.
bridg1.fvc
RESULTS ELEMENT EL.N1R.S N1R
PRESENT CONTOUR FROM -0.1 TO 0.1 LEVELS 4
RESULTS ELEMENT EL.N1R.S N1R
PRESENT CONTOUR FROM -0.1 TO 0.1 LEVELS 4
Result attributes N1R and N2R respective represent the reinforcement forces n01
and n02 . The contour plots, and the results monitor, show zero forces indeed
[Fig. 2.21].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:37 n1r.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:37 n2r.ps
Model: BRIDG1 Model: BRIDG1
LC1: Load case 1 LC1: Load case 1
Element EL.N1R.S N1R Element EL.N1R.S N1R
Top (last) surface Top (last) surface
Max = .432E-11 Max = .432E-11
Min = -.352E-11 Min = -.352E-11
Y .1 Y .1
.6E-1 .6E-1
.2E-1 .2E-1
Z X -.2E-1 Z X -.2E-1
-.6E-1 -.6E-1
-.1 -.1
(a) n01 (b) n02
Figure 2.21: Reinforcement forces [sic]
2.2.8 Combined Moments and Forces
If both membrane forces and bending moments are present, the reinforcement
loading is expressed by forces equivalent to the combined results of these mem-
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
2.2 Linear Analysis 27
brane forces and bending moments. These combined reinforcement forces can
also be determined only if bending moments are present.
bridg1.fvc
RESULTS ELEMENT EL.N1R.S N1RC
RESULTS RANGE SURFACE BOTTOM
PRESENT CONTOUR VALUES 0
RESULTS RANGE SURFACE TOP
PRESENT CONTOUR VALUES 0
RESULTS ELEMENT EL.N1R.S N2RC
RESULTS RANGE SURFACE BOTTOM
PRESENT CONTOUR VALUES 0
RESULTS RANGE SURFACE TOP
PRESENT CONTOUR VALUES 0
Result attributes N1RC and N2RC respectively represent the reinforcement com-
bined moment and forces in the X- and Y -direction, n0c 0c
1 and n2 . These results
are reinforcement forces per unit length. Reinforcement is required for positive
values in the upper plane (red) [Fig. 2.22bd], and for negative values in the lower
plane (blue) [Fig. 2.22ac].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:38 n1rc1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:38 n1rc2.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:38 n2rc1.ps
Model: BRIDG1 Model: BRIDG1 Model: BRIDG1
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Element EL.N1R.S N1RC Element EL.N1R.S N1RC Element EL.N1R.S N2RC
Bottom (first) surface Top (last) surface Bottom (first) surface
Max = 211 Min = -392 Max = 394 Min = -210 Max = 37.9
Min = -81.1
Y Y Y
Z X Z X Z X
0 0 0
(a) lower, X-dir. (b) upper, X-dir. (c) lower, Y -dir.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:38 n2rc2.ps
Model: BRIDG1
LC1: Load case 1
Element EL.N1R.S N2RC
Top (last) surface
Max = 82.5
Min = -33.7
Z X
0
(d) upper, Y -dir.
Figure 2.22: Combined reinforcement moments and forces (red is +, blue is −)
We will design the reinforcement in X-direction in the lower plane, based
on the maximum combined reinforcement moment and forces (n0c 1;max = 211
N/mm [Fig. 2.22a]). If we divide n0c
1;max by the yield stress of the steel (σy = 435
N/mm2 ) we get a thickness teq of the ‘equivalent reinforcement plate’ with a
unit length:
n0c
1;max 211
teq = = = 0.485 mm (2.1)
σy 435
For one meter length we need 0.485 × 1000 = 485 mm2 . So for example we can
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
28 Reinforcement Forces and Moments for a Bridge
apply ∅10–160, i.e., reinforcement bars of 10 mm diameter at a center to center
distance of 160 mm.
Questions:
1. How much reinforcement is required in X-direction in the upper surface,
designed on the maximum reinforcement combined moment and forces?
2. How much reinforcement is required in Y -direction?
2.2.9 Shear Reinforcement
We may assess the shear reinforcement with the following commands.
bridg1.fvc
RESULTS ELEMENT EL.N1R.S QT
RESULTS RANGE SURFACE BOTTOM
PRESENT CONTOUR LEVELS
RESULTS RANGE SURFACE TOP
PRESENT CONTOUR LEVELS
Result attribute QT represents the shear reinforcement forces q 0 . We display
contour plots for the lower and upper plane [Fig. 2.23]. Note that the results
are equal for both surfaces and that 0 < q 0 ≤ 114.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:38 qt1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:39 qt2.ps
Model: BRIDG1 Model: BRIDG1
LC1: Load case 1 LC1: Load case 1
Element EL.N1R.S QT Element EL.N1R.S QT
Bottom (first) surface Top (last) surface
Max = 114 Min = .347 Max = 114
Min = .347
104 104
93.6 93.6
83.2 83.2
72.9 72.9
Y 62.5 Y 62.5
52.2 52.2
41.8 41.8
Z X 31.4 Z X 31.4
21.1 21.1
10.7 10.7
(a) lower (b) upper
Figure 2.23: Shear reinforcement forces
2.3 Prestress
In this example only bending moments have been considered so far. In the next
analysis we will investigate the effect of adding a compressive force. This pre-
stressing reduces the required amount of reinforcement. To model the prestress
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
2.3 Prestress 29
we can apply a distributed normal force in global X-direction (nxx ) at both
edges of the bridge. We add this distributed normal force to the model. The
rest of the model will not be changed. We want to prestress the bridge to such
an extend that no reinforcement is needed in the lower plane in X-direction.
Question:
3. What is the value of the prestress (nxx ) that must be applied so that no
reinforcement is required in the lower plane in X-direction?
We assume that the internal arm (zd ) stays the same. In practice the internal
arm depends on the ratio of moment and normal force. In this case we use the
same command file.
Answer: No torsional shear forces and moments occur because a symmet-
ric load is applied. So in this case it is possible to make an addition of the
reinforcement needed for separate membrane and bending behavior
¯ ¯
nxx mxx ¯¯ nxy mxy ¯¯
n0c = − + ¯ 2 − (2.2)
1,lo
2 zd zd ¯
such that the last part of the equation for the combined reinforcement forces is
zero. Zero reinforcement in X-direction in the lower plane means that n0c
1,lo = 0.
Bending moment mxx will not change when adding a normal force. We also
assume that the internal arm zd remains the same. All these conditions result
in the following equation:
nxx mxx nxy mxy
n0c
1,lo = − =0⇔ = (2.3)
2 zd 2 zd
where mxx /zd is equal to the reinforcement forces n0c
1,lo due to bending moments
only, no membrane forces and no torsional shear forces and moments. This is
a result of our previous analysis [Fig. 2.22a]. We observed that the maximum
reinforcement force of combined moments and forces is n0c 1;max = 211 N/mm.
We must add a compression distributed normal force nxx of 422 N/mm.
2.3.1 Applying Prestress
To add the prestress (the normal force) we revert to the iDiana Design envi-
ronment and change the model.
bridge.fgc
FEMGEN BRIDGE
VIEW GEOMETRY ALL
VIEW GEOMETRY +SUP1 RED
VIEW GEOMETRY +SUP4 BLUE
PROPERTY LOADS PRESSURE LOP1 SUP1 422 X
PROPERTY LOADS PRESSURE LOP2 SUP4 -422 X
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
30 Reinforcement Forces and Moments for a Bridge
VIEW MESH
LABEL MESH LOADS LOP1 RED
LABEL MESH LOADS +LOP2 BLUE
As a check, we display the two edges appropriate for the prestress in different
colors [Fig. 2.24a]. Then we apply the prestress load to the two edges: load
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:20 geops.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:20 loadps.ps
Model: BRIDGE Model: BRIDGE
Analysis: DIANA Analysis: DIANA
Model Type: Structural 3D Model Type: Structural 3D
Z Z
Y Y
X X
(a) edges of geometry (b) prestress load on mesh
Figure 2.24: Applying the prestress load
class PRESSURE in X direction. We check the new load by displaying it on a
three-dimensional view of the mesh [Fig. 2.24b].
2.3.2 Linear Analysis
The model is now ready for a second analysis.
iDiana
SAVE AS BRIDG2
yes
Bridge model for second analysis
UTILITY WRITE DIANA bridg2.dat
yes
FILE CLOSE
yes
ANALYSE BRIDG2
Analysis Setup
Input Data File(s) Path: bridg2.dat ↑ OK
···
We write a new input data file bridg2.dat. Then we close the model and launch
the Analysis Setup dialog. We perform an analysis with the new input data file
and the same command file lin.dcf that we used previously. The model for the
iDiana Results environment is now called BRIDG2. We enter this environment
as soon as the analysis has terminated.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
2.3 Prestress 31
bridg2.fvc
FEMVIEW BRIDG2
VIEW MESH
VIEW OPTIONS EDGES OUTLINE
RESULTS LOADCASE LC1
We display the mesh and select load case LC1 which now includes not only the
dead weight and the asphalt load, but also the prestress load.
2.3.3 Normal Forces and Stresses
As a first impression of the analysis we assess the forces and stresses in longi-
tudinal direction.
bridg2.fvc
RESULTS ELEMENT EL.NXX.L NXX
PRESENT CONTOUR LEVELS
RESULTS ELEMENT EL.SXX.G SXX
RESULTS RANGE SURFACE BOTTOM
PRESENT CONTOUR LEVELS
Result attribute NXX represents the the distributed normal forces nxx . These
can be used to check the input of the prestress. The contour plot shows an
evenly distributed normal force [Fig. 2.25a]. The results monitor and the legend
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:47 nxxps.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:48 sxx1ps.ps
Model: BRIDG2 Model: BRIDG2
LC1: Load case 1 LC1: Load case 1
Element EL.NXX.L NXX Element EL.SXX.G SXX
Max = -422 Bottom (first) surface
Min = -422 Max = 1.5 Min = -6.46
-422 .777
-422 .531E-1
-422 -.671
-422 -1.39
Y -422 Y -2.12
-422 -2.84
-422 -3.57
Z X -422 Z X -4.29
-422 -5.01
-422 -5.74
(a) normal forces nxx (b) stress σxx in lower plane
Figure 2.25: Prestressed model – primary results
show that the all values are equal to −422 which is equal to the input value of
the prestress [§ 2.3.1]. Therefore we may conclude that the model is correct.
We also select the global stresses σXX and display a contour plot for those
in the lower plane [Fig. 2.25b]. The results monitor shows that the stresses vary
from +1.5 to −6.5. So there are still tensile stresses which appear in the spans
(orange and red).
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
32 Reinforcement Forces and Moments for a Bridge
2.3.4 Reinforcement Forces
For the lower plane we display the distribution of the reinforcement forces in
the longitudinal direction. Note that the forces in the upper and lower plane
are the same.
bridg2.fvc
RESULTS ELEMENT EL.N1R.S N1RC
RESULTS RANGE SURFACE BOTTOM
PRESENT CONTOUR VALUE 0
RESULTS ELEMENT EL.N1R.S N1R
RESULTS RANGE SURFACE BOTTOM
PRESENT CONTOUR LEVELS
The zero-contour plot for the combined reinforcement forces n0c1 shows that these
are all negative [Fig. 2.26a]. The contour plot for the reinforcement force n01
shows that all values are equal to −211 [Fig. 2.26b]. The reinforcement forces
n01 are based on the membrane forces only. Because of the absence of shear
stresses, these forces are equal to half the distributed normal forces.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:48 n1rc1ps.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:48 n1r1ps.ps
Model: BRIDG2 Model: BRIDG2
LC1: Load case 1 LC1: Load case 1
Element EL.N1R.S N1RC Element EL.N1R.S N1R
Bottom (first) surface Bottom (first) surface
Max = -.205 Max = -211 Min = -211
Min = -603
-211
-211
-211
-211
Y Y -211
-211
-211
Z X Z X -211
-211
0 -211
(a) combined (b) force only
Figure 2.26: Prestressed model – reinforcement forces, X-dir., lower plane
Question:
4. Do you think that our calculation of the prestress was correct so that re-
inforcement in the lower plane in X-direction is not required?
2.3.5 Reinforcement Moments
For the lower plane we display the distribution of the reinforcement moments
in the longitudinal direction.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
2.4 Asymmetric Loading 33
bridg2.fvc
RESULTS ELEMENT EL.M1R.S M1R
RESULTS RANGE SURFACE BOTTOM
PRESENT CONTOUR VALUE 0
The zero-contour plot shows negative moments in the spans and positive above
the support lines [Fig. 2.27]. The reinforcement moments are based on bending
moments only. So the results are similar to the results of the model without
prestress [Fig. 2.20a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:48 m1r1ps.ps
Model: BRIDG2
LC1: Load case 1
Element EL.M1R.S M1R
Bottom (first) surface
Max = .94E5
Min = -.506E5
Z X
0
Figure 2.27: Prestressed model – reinforcement moment, X-dir., lower plane
2.4 Asymmetric Loading
In the two previous analyses we have applied a symmetric load. Hence no
torsional forces and moments do occur. However, in reality these torsional
forces and moments do arise. That is why we will finally apply an asymmetric
load. First we delete the two prestress loads.
Delete prestress load bridge.fgc
UTILITY DELETE LOADS LOP1
yes
UTILITY DELETE LOADS LOP2
yes
Here we delete the prestress loads LOP1 and LOP2 that we added for the second
model [§ 2.3.1].
2.4.1 Applying Load According to Eurocode
For the new asymmetric load we will check the bridge in ultimate limit state. In
this example we apply loads according to the Eurocode ENV 1991-3 [3] which
comprise the following [Fig. 2.28]:
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
34 Reinforcement Forces and Moments for a Bridge
q1
F1 F1
q3 F2 F2 q3
q2
3×500 2000 3000
8000
Figure 2.28: Asymmetric bridge load
q1 = 9.0 kN/m2 – a distributed traffic load on lane 1.
q2 = 2.5 kN/m2 – a distributed traffic load on lane 2.
q3 = 0.5 kN/m – a distributed load on the railing.
F1 = 300 kN – a concentrated tandem load (axle load) in lane 1.
F2 = 200 kN – a concentrated tandem load (axle load) in lane 2.
We will apply these loads in three steps: the railing loads, the axle loads, and
the distributed traffic loads.
Railing load bridge.fgc
CONSTRUCT SET RAIL1 APPEND LINES LIMITS VMIN 499 VMAX 501
CONSTRUCT SET RAIL2 APPEND LINES LIMITS VMIN 7499 VMAX 7501
CONSTRUCT SET RAILS APPEND RAIL1 RAIL2
VIEW GEOMETRY ALL
VIEW GEOMETRY +RAILS RED
PROPERTY LOADS PRESSURE LORA RAILS -0.5 Z
VIEW MESH
LABEL MESH LOADS LORA RED
We assemble the geometric parts of the railing in two sets: RAIL1 all lines within
499 < Y < 501 (actually Y = 500), and RAIL2 all lines within 7499 < Y < 7501
(actually Y = 7500). We also make a set RAILS with the lines of the two previous
sets. As a check we display the set RAILS, overlaid in red on the complete
geometry [Fig. 2.29a]. Finally, we apply the load q3 = 0.5 on the set RAILS,
pointing downward (in −Z-direction). The display on the mesh confirms the
correct location and direction of this load [Fig. 2.29b].
Axle loads bridge.fgc
CONSTRUCT SET AXLE1 APPEND S7 S8 S23 S24
CONSTRUCT SET AXLE2 APPEND S15 S16 S31 S32
VIEW GEOMETRY ALL
VIEW GEOMETRY +AXLE1 RED
VIEW GEOMETRY +AXLE2 BLUE
PROPERTY LOADS PRESSURE LOAX1 AXLE1 -0.9375 Z
PROPERTY LOADS PRESSURE LOAX2 AXLE2 -0.625 Z
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
2.4 Asymmetric Loading 35
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:21 georail.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:21 loadra.ps
Model: BRIDGE Model: BRIDGE
Analysis: DIANA Analysis: DIANA
Model Type: Structural 3D Model Type: Structural 3D
Z Z
Y Y
X X
(a) geometry (b) loading
Figure 2.29: Applying the railing load
VIEW MESH
LABEL MESH LOADS LOAX1 RED
LABEL MESH LOADS LOAX2 BLUE
The axle loads will be applied near the middle of the second span [Fig. 2.5 p. 11].
Note that we have already made the surfaces for the wheels [Fig. 2.6 p. 12]. We
assemble these surfaces in two sets, AXLE1 and AXLE2, which we display in red
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:21 geoax.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:22 loadax.ps
Model: BRIDGE Model: BRIDGE
Analysis: DIANA Analysis: DIANA
Model Type: Structural 3D Model Type: Structural 3D
Z Z
Y Y
X X
(a) geometry (b) loading
Figure 2.30: Applying the axle loads (wheels)
and blue respectively [Fig. 2.30a]. Then we apply the two loads on these sets
and display these on the mesh [Fig. 2.30b]. Note that the start of each arrow
indicates the proper location of the load.
Traffic loads bridge.fgc
CONSTRUCT SET LANE1 APPEND SURFACES LIMITS VMIN 999 VMAX 4001
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
36 Reinforcement Forces and Moments for a Bridge
CONSTRUCT SET LANE2 APPEND SURFACES LIMITS VMIN 3999 VMAX 7001
VIEW GEOMETRY ALL
VIEW GEOMETRY +LANE1 RED
VIEW GEOMETRY +LANE2 BLUE
PROPERTY LOADS PRESSURE LOTR1 LANE1 -9.0E-3 Z
PROPERTY LOADS PRESSURE LOTR2 LANE2 -2.5E-3 Z
VIEW MESH
LABEL MESH LOADS LOTR1 RED
LABEL MESH LOADS +LOTR2 BLUE
The traffic loads q1 and q2 will be applied on each of the lanes, inside the railing
[Fig. 2.28 p. 34]. We assemble the surfaces of these lanes in two sets: LANE1 all
surfaces within 999 < Y < 4001 and LANE2 all surfaces within 3999 < Y < 7001.
We display the sets in red and blue respectively [Fig. 2.31a]. Finally, we apply
the two loads on the sets and display these on the mesh [Fig. 2.31b].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:22 geolan.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:22 loadlan.ps
Model: BRIDGE Model: BRIDGE
Analysis: DIANA Analysis: DIANA
Model Type: Structural 3D Model Type: Structural 3D
Z Z
Y Y
X X
(a) geometry (b) loading
Figure 2.31: Applying the traffic loads (lanes)
2.4.2 Linear Analysis
The model is now ready for a third analysis.
iDiana
SAVE AS BRIDG3
yes
Bridge model for second analysis
UTILITY WRITE DIANA bridg3.dat
yes
FILE CLOSE
yes
ANALYSE BRIDG3
Analysis Setup
Input Data File(s) Path: bridg3.dat ↑ OK
···
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
2.4 Asymmetric Loading 37
We write a new input data file bridg3.dat. Then we close the model and launch
the Analysis Setup dialog. We perform an analysis with the new input data file
and the same command file lin.dcf that we used previously. The model for
the iDiana Results environment is now called BRIDG3. To assess the results we
enter the iDiana Results environment with the name of the model.
bridg3.fvc
FEMVIEW BRIDG3
VIEW MESH
VIEW OPTIONS EDGES OUTLINE
RESULTS LOADCASE LC1
Load case LC1 now includes the dead weight, the asphalt and the railing loading,
and the asymmetric traffic load.
2.4.3 Displacements
To assess the displacements we use commands like for the first analysis [§ 2.2.1
p. 20].
bridg3.fvc
RESULTS NODAL DTX....G DTZ
PRESENT CONTOUR LEVELS
EYE ROTATE TO 45 30 30
VIEW OPTIONS SHRINK
VIEW OPTIONS DEFORM USING DTX....G RESDTX
The vertical displacements [Fig. 2.32a] confirm the asymmetric nature of the
loading. The maximum deflection is now 19.5 mm, it occurs in the mid-span
at the axle loads (blue). This is also clear from the deformed mesh display
[Fig. 2.32b].
2.4.4 Combined Moments and Forces
To assess the combined reinforcement moments and forces we use commands
like for the first analysis [§ 2.2.8 p. 26].
bridg3.fvc
EYE ANGLE 0
VIEW OPTIONS SHRINK OFF
RESULTS ELEMENT EL.N1R.S N1RC
RESULTS RANGE SURFACE BOTTOM
PRESENT CONTOUR VALUES 0
RESULTS RANGE SURFACE TOP
PRESENT CONTOUR VALUES 0
RESULTS ELEMENT EL.N1R.S N2RC
RESULTS RANGE SURFACE BOTTOM
PRESENT CONTOUR VALUES 0
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
38 Reinforcement Forces and Moments for a Bridge
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:56 disp1a.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:56 disp2a.ps
Model: BRIDG3 Model: BRIDG3
LC1: Load case 1 Deformation = 78.5
Nodal DTX....G DTZ LC1: Load case 1
Max = 2.46 Nodal DTX....G DTZ
Min = -19.5 Max = 2.46
Min = -19.5
.467 .467
-1.53 -1.53
-3.52 -3.52
-5.51 -5.51
Y -7.51 -7.51
-9.5 Z -9.5
-11.5 Y -11.5
Z X -13.5 -13.5
-15.5 -15.5
-17.5 X -17.5
(a) 2D outline view (b) 3D view in deformed model
Figure 2.32: Contour plot of vertical displacements (asymmetric)
RESULTS RANGE SURFACE TOP
PRESENT CONTOUR VALUES 0
The zero-contour plots show where reinforcement is required [Fig. 2.33]. We
may compare this with the results of the first analysis [Fig. 2.22 p. 27].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:57 n1rc1a.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:57 n1rc2a.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:57 n2rc1a.ps
Model: BRIDG3 Model: BRIDG3 Model: BRIDG3
Deformation = 78.5 Deformation = 78.5 Deformation = 78.5
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Element EL.N1R.S N1RC Element EL.N1R.S N1RC Element EL.N1R.S N2RC
Bottom (first) surface Top (last) surface Bottom (first) surface
Max = .112E4 Max = .107E4 Max = 362 Min = -191
Min = -.102E4 Min = -.111E4
Y Y Y
Z X Z X Z X
0 0 0
(a) lower, X-dir. (b) upper, X-dir. (c) lower, Y -dir.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:57 n2rc2a.ps
Model: BRIDG3
Deformation = 78.5
LC1: Load case 1
Element EL.N1R.S N2RC
Top (last) surface
Max = 253 Min = -361
Z X
0
(d) upper, Y -dir.
Figure 2.33: Combined reinforcement moments and forces (asymmetric)
Question:
5. How much reinforcement is required, and where?
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
2.4 Asymmetric Loading 39
2.4.5 Shear Reinforcement
To assess the shear reinforcement we use commands like for the first analysis
[§ 2.2.9 p. 28].
bridg3.fvc
RESULTS ELEMENT EL.N1R.S QT
RESULTS RANGE SURFACE BOTTOM
PRESENT CONTOUR LEVELS
RESULTS RANGE SURFACE TOP
PRESENT CONTOUR LEVELS
The shear reinforcement forces now look also asymmetric [Fig. 2.34]. Com-
parison with the results of the first analysis [Fig. 2.23 p. 28] learns that the
asymmetric load induces considerably larger shear reinforcement forces.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:57 qt1a.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:58 qt2a.ps
Model: BRIDG3 Model: BRIDG3
Deformation = 78.5 Deformation = 78.5
LC1: Load case 1 LC1: Load case 1
Element EL.N1R.S QT Element EL.N1R.S QT
Bottom (first) surface Top (last) surface
Max = 390 Min = .477 Max = 390
Min = .477
354 354
319 319
283 283
248 248
Y 213 Y 213
177 177
142 142
Z X 107 Z X 107
71.2 71.2
35.8 35.8
(a) lower (b) upper
Figure 2.34: Shear reinforcement forces (asymmetric)
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
40 Reinforcement Forces and Moments for a Bridge
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
2.4 Asymmetric Loading 41
Answers to questions: 4. Yes, all negative n0c
1 in lower plane
1. In X-direction in upper plane: [Fig. 2.26a].
maximum n0c 1 = 394 N/mm, re-
quired steel area A = 906 mm2 /m. 5. The only method to check if we have
2. In Y -direction in upper plane 190 applied enough reinforcement is to
mm2 /m, in lower plane 87 mm2 /m. model the reinforcement and per-
3. See § 2.3 on page 29. form a nonlinear analysis!
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
42 Reinforcement Forces and Moments for a Bridge
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
Chapter 3
Fire under Concrete Slab
Name: Fire
Path: /Examples/ConcMas/Fire
Keywords: analys: flow flowst heat nonlin physic stagge transi. constr:
initia suppor temper. elemen: bq4ht chx60 flow grid hx8ht
potent reinfo solid taper. load: edge elemen force temper
time. materi: capaci conduc elasti isotro. option: direct
groups newton regula units. post: binary femvie. pre: femgen.
result: cauchy displa stress temper total.
P = 14.5 N/mm P = 14.5 N/mm
Y
reinforcement
1900 Z
o o oo o
150 o
15 oo
X
o oo
fire
o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o o oo
200 1200 2100 1200 200
4900
Figure 3.1: Slab with fire under it [mm]
This example demonstrates how to perform a staggered flow–stress analysis. It
aims at:
Setting up such flow–stress analysis,
Using iDiana features for three-dimensional modeling and results manip-
ulation.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
44 Fire under Concrete Slab
It concerns a reinforced concrete slab which is subjected to a temperature load-
ing at the bottom faces (fire) [Fig. 3.1]. The slab is 4900 mm long, 1900 mm
wide and 150 mm high. The reinforcement cover is 15 mm. A distributed load
is applied at the top face along two lines over the width of the slab. At the
bottom, the slab is heating up resulting in the temperature loading [Fig. 3.2].
[°C] [°C]
1200 120
1000 100
Temperature
Temperature
800 80
600 Bottom face 60 Lateral faces
400 40
200 20
0 0
0 50 100 150 200 250 [min] 0 50 100 150 200 250 [min]
Time Time
Figure 3.2: Temperature evolution
The adopted material parameters for constructing the model are presented in
Table 3.1 and Table 3.2 on page 50. All material properties have been defined
as linear elastic with no temperature dependencies.
These are unrealistic assumptions, made to simplify the model. Re-
sults should not be interpreted as representing the correct slab behav-
ior at least from a quantitative point of view.
3.1 Finite Element Model
Due to symmetry only a quarter of the slab should be modeled. To build up the
finite element model we start iDiana and enter the Design environment with
the model name.
iDiana
FEMGEN FIRELOAD
Analysis and Units
Analysis Selection
Model Type: →Heatflow-Stress Staggered 3D
Units Definition
Length: →Millimeter
Mass: →Kilogram
Time: →Minute
Temperature: →Celsius
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
3.1 Finite Element Model 45
In the Analysis and Units dialog we specify the analysis type along with adopted
units for the analysis.
3.1.1 Geometry Definition
For the geometry of one quarter of the model we define some points and lines.
By sweeping the lines we create the bottom surface. A sweep of the latter
creates a body for the slab geometry.
Points and lines fireload.fgc
GEOMETRY POINT COORD 0.0
GEOMETRY POINT COORD 200.0
GEOMETRY POINT COORD 1400.0
GEOMETRY POINT COORD 2450.0
EYE FRAME
GEOMETRY LINE STRAIGHT P1 P2 2
GEOMETRY LINE STRAIGHT P2 P3 12
GEOMETRY LINE STRAIGHT P3 P4 10
CONSTRUCT SET SELIN1 APPEND LINES ALL
We define three lines in the X-direction that correspond to the bottom front
line of the model. Simultaneously with the definition of a line we specify its
division. We put all lines in a set SELIN1.
Sweep to bottom surface and slab body fireload.fgc
GEOMETRY SWEEP SELIN1 SELIN2 10 TRANSLATE 0.0 950.0 0.0
EYE FRAME
CONSTRUCT SET BOTTOM APPEND ALL
GEOMETRY SWEEP BOTTOM TOP 12 TRANSLATE 0.0 0.0 150.0
CONSTRUCT SET SLAB APPEND ALL
We sweep the set SELIN1 in Y -direction to create the bottom surface of the
model. Implicitly we define the division in Y -direction for the created lines.
We put the geometry entities of the bottom surface in a set BOTTOM. A second
sweep operation in the Z-direction creates a surface in set TOP and a body for
the slab geometry. We put all current geometry in a set SLAB.
Display fireload.fgc
EYE ROTATE TO 41 30 30
VIEW GEOMETRY ALL VIOLET
VIEW GEOMETRY +BOTTOM BLUE
EYE FRAME
LABEL GEOMETRY SURFACES ALL BLUE
LABEL GEOMETRY LINES ALL VIOLET
We choose an appropriate viewing direction and display the geometry with dif-
ferent colors for the bottom surface and the slab [Fig. 3.3a]. For future reference
we label the surfaces and the lines with their names.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
46 Fire under Concrete Slab
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:33 geom1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:33 mesh1.ps
Model: FIRELOAD Model: FIRELOAD
Analysis: DIANA Analysis: DIANA
Model Type: Heatflow-Stress Staggered 3D Model Type: Heatflow-Stress Staggered 3D
L14
L25
S10
L4 L26
L15
S13S4
L17
S1 S14 L5
L18 S11
L7
L11 L8
L21
S7 S5
L1 L22
S2 L27
L12
L16
L2
S8 L6
S15 S12
L19
L9
S6
L23 L28
S3
L13
L3 S9 S16
L20
L10
Z Z
Y L24 Y
X X
(a) geometry (b) finite element mesh
Figure 3.3: Modeling the slab
3.1.2 Meshing
fireload.fgc
MESHING TYPES SLAB HE20 CHX60
MESHING GENERATE
VIEW MESH
VIEW HIDDEN SHADE
We select the HE20 generic element type and the quadratic solid brick CHX60
structural element for the slab. We generate the mesh and display it in hidden
shade style [Fig. 3.3b].
3.1.3 Boundary Elements
A complication with respect to the modeling of boundary elements for stag-
gered flow–stress analysis is that these elements are linearly interpolated, i.e.,
they have no mid-side nodes. In principle, these elements are incompatible with
quadratic structural elements that we use for the structural model. Fortunately,
for the flow part of the staggered analysis, Diana will internally convert quad-
ratic structural elements to linear heat flow elements and thus will not consider
mid-side nodes for the flow analysis. However, in the Design environment of
iDiana, where we must build the complete model, the meshing procedure will
not allow the incompatibility of elements. We must find a work-around solution
for this problem. The trick is to copy the set of lines along the boundary by
translation over a zero distance.
Geometry fireload.fgc
CONSTRUCT SET LATERA APPEND SURFACES S13 S7 S8 S9
CONSTRUCT SPACE TOLERANCE OFF
GEOMETRY COPY TOP BNDTOP TRANSLATE 0.0 0.0 0.0
GEOMETRY COPY BOTTOM BNDBOT TRANSLATE 0.0 0.0 0.0
GEOMETRY COPY LATERA BNDLAT TRANSLATE 0.0 0.0 0.0
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
3.1 Finite Element Model 47
VIEW GEOMETRY BNDTOP ORANGE
VIEW GEOMETRY +BNDLAT RED
VIEW GEOMETRY +BNDBOT BLUE
CONSTRUCT SET BOUNDS APPEND BNDTOP BNDLAT BNDBOT
MESHING DIVISION FACTOR BOUNDS 0.5
MESHING TYPES BOUNDS BQ4HT
We put the lateral surfaces on which boundary elements have to be applied in
a set LATERA. We copy the sets TOP, BOTTOM and LATERA to new sets BNDTOP,
BNDBOT and BNDLAT to model the boundaries. With the TRANSLATE option we
indicate a zero distance. iDiana would not have created new lines and points
without corrective action because any new point would exactly coincide with
an existing point. To force the creation of new points and lines we switch off
the tolerance check. We view the geometry of the boundaries with different
colors [Fig. 3.4a] and put them in a set BOUNDS. The surfaces of the boundaries
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:33 geom2.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:34 mesh2.ps
Model: FIRELOAD Model: FIRELOAD
Analysis: DIANA Analysis: DIANA
Model Type: Heatflow-Stress Staggered 3D Model Type: Heatflow-Stress Staggered 3D
Z Z
Y Y
X X
(a) geometry (b) finite element mesh
Figure 3.4: Modeling the boundaries
get their division numbers from their originators during the copy action. So we
simply halve the number of divisions via the FACTOR option. Finally we assign
the linear BQ4HT boundary flow element to the surfaces of the boundaries.
Meshing fireload.fgc
MESHING GENERATE
VIEW OPTIONS SHRINK
VIEW MESH BNDTOP ORANGE
VIEW MESH +BNDLAT RED
VIEW MESH +BNDBOT BLUE
We generate the complete mesh. We display the mesh of the boundaries in
the ‘shrunken elements’ style with different colors [Fig. 3.4b]. Although the
mesh seems to be fine we still have to make one final correction. Since the
surfaces in the slab have no common points with the surfaces in the boundaries,
the generated boundary elements will not be automatically connected to the
structural elements.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
48 Fire under Concrete Slab
Merging nodes fireload.fgc
VIEW MESH +SLAB GREEN
LABEL MESH NODES
EYE ZOOM FACTOR 5. 650. -630. 0.
MESHING MERGE ALL 0.001
DRAWING DISPLAY
We add the mesh of the slab to the display and label the nodes. We zoom in
on the bottom part of the model [Fig. 3.5a]. Looking at the end nodes of the
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:34 shmeshza.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:34 shmeshzb.ps
1969 1799 1608 1803 1972 1807 1611 1811 1969 1799 1608 1803 1972 1807 1611 1811
Model: FIRELOAD Model: FIRELOAD
1913
Analysis: DIANA 2115
1214 1916 2120
1219 1913
Analysis: DIANA 1214 1916 1219
Model Type:1897
Heatflow-Stress
1727 Staggered 3D 1731 1900 1735 1739 Model Type:1897
Heatflow-Stress
1727 Staggered 3D 1731 1900 1735 1739
1841 1844 1841 1844
1825 16551351 16591356 1828 16631361 16671366 1825 16551351 16591356 1828 16631361 16671366
1769 1772 1769 1772
1753 12601948 12651952 1756 12701956 12751496 1753 12601948 12651952 1756 12701956 12751496
1697 1700 1697 1700
1876 1880 1684 1884 1497 1876 1880 1684 1884 1497
1681 2049
1311 1681 1311
1625 2044
1306 1628 1625 1306 1628
1804 1973 1808 1612 1812 1490 1498 1804 1973 1808 1612 1812 1490 1498
1609 1454 1609 1454
2116
1215 1917 2121
1220 1215 1917 1220
1732 1901 1736 1740 1491 1499 1732 1901 1736 1740 1491 1499
1845 1455 1845 1455
1352 16601357 1829 16641362 16681367 1492 1500 1352 16601357 1829 16641362 16681367 1492 1500
1773 1456 1773 1456
1427 12661953 1757 12711957 12761485 1493 1281 1427 12661953 1757 12711957 12761485 1493 1281
1701 1457 1701 1457
1428 1881 1685 1885 1486 1494 1428 1881 1685 1885 1486 1494
2045
2242
1307 1629 2050
1312 1458 1307 1629 1312 1458
1429 1432 1809 1613 1813 1479 1487 1495 1429 1432 1809 1613 1813 1479 1487 1495
2243
1384 2122
1221 1449 1226
2127 1384 1221 1449 1226
1430 1433 1737 1741 1480 1488 1430 1433 1737 1741 1480 1488
2244
1385 1450 1385 1450
1431 1434 16651363 16691368 1481 1489 1431 1434 16651363 16691368 1481 1489
2245
1386 1451 1386 1451
1267 1435 12721438 12771474 1482 1282 1267 1435 12721438 12771474 1482 1282
2246
1387 1452 1387 1452
1436 1439 1475 1483 1436 1439 1475 1483
2247
1388 2051
2249
1313 1453 1388 1313 1453
1437 1440 1443 1476 1484 1437 1440 1443 1476 1484
2248
1222
2123 2250
1389 1227
2128 1222 1389 1227
1441 1444 1477 1441 1444 1477
2251
1390 1390
1442 1445 1478 1442 1445 1478
2252
1391 1391
1278 1446 1283 1278 1446 1283
Z 2253
1392 Z 1392
Y 1447 Y 1447
2254
1393 1393
X 1448 X 1448
2255
1228
2129 1228
(a) before merging (b) after merging
Figure 3.5: Merging nodes – displayed labels
boundary elements, we see overlapping numbers: one node for the boundary
element and another one for the structural element. Therefore, there is no
connection. To solve this problem we apply a merging operation. The parameter
1
value 0.001 indicates a tolerance of 1000 millimeter for the check on coincident
nodes. A second display of node labels now shows one single node at the end of
each boundary element [Fig. 3.5b].
3.1.4 Reinforcements
To model the reinforcement grid we will first define its corner points. Then we
will model the grid between these points.
Points fireload.fgc
VIEW OPTIONS SHRINK OFF
LABEL MESH OFF
VIEW MESH ALL
EYE FRAME
CONSTRUCT SET OPEN RPTS
GEOMETRY POINT COORD 0 0 15
GEOMETRY POINT COORD 2450 0 15
GEOMETRY POINT COORD 2450 950 15
GEOMETRY POINT COORD 0 950 15
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
3.1 Finite Element Model 49
CONSTRUCT SET CLOSE
VIEW GEOMETRY +RPTS RED
We define points at the four vertices of the reinforcement grid, 15 mm above the
bottom face [Fig. 3.1]. We put the new points in a set RPTS which we display
on the mesh [Fig. 3.6a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:34 mesh3.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:35 mreif.ps
Model: FIRELOAD Model: FIRELOAD
Analysis: DIANA Analysis: DIANA
Model Type: Heatflow-Stress Staggered 3D Model Type: Heatflow-Stress Staggered 3D
Z Z
Y Y
X X
(a) points (b) reinforcement
Figure 3.6: Modeling the reinforcement grid
Grid fireload.fgc
REINFORCE GRID SECTION P43 P44 P45 P46
REINFORCE GRID STEEL RE1
REINFORCE SET SETGRID APPEND ALL
VIEW REINFORCE +STEEL
We specify the reinforcement section between the four points. We define the
actual reinforcement as STEEL and put it in a set SETGRID. We display the
reinforcement in the mesh [Fig. 3.6b].
3.1.5 Material and Physical Properties
To specify the material and physical properties for the different components of
our model we launch the Property Manager dialog.
iDiana
View →Property Manager...
↑
Property Manager
specify properties
We will specify the properties for the concrete, the boundary, and the reinforce-
ment.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
50 Fire under Concrete Slab
Table 3.1: Thermo-mechanical concrete properties
Thermal conductivity λ 0.132 J/(min·mm·°C)
Thermal capacity c 2.3×10−3 J/(mm3 ·°C)
Young’s modulus E 42000 MPa
Poisson’s ratio ν 0.18
Thermal expansion coefficient α 10×10−6 °C−1
Boundary conduction coefficient K 4.8×10−2 J/(mm2 ·°C·min)
Concrete iDiana
Property Manager
↑ Materials Material Name: MASLAB
↑Flow →Isotropic
↑Expansion →Isotropic →Constnt params.
↑Linear elasticity →Isotropic
We specify the properties of the concrete elements in a material MASLAB [Table
3.1]. For flow we specify the thermal conductivity and the thermal capacity. For
expansion we specify the thermal expansion coefficient. As elastic properties we
specify Young’s modulus and Poisson’s ratio.
Boundary iDiana
Property Manager
Materials Material Name: MABOUN
↑Flow →Boundary →Convection Only
We define a material MABOUN for the boundary elements. We specify the con-
duction coefficient K [Table 3.1] which simulates the conduction with the envi-
ronment.
Table 3.2: Properties of reinforcement
Young’s modulus E 215000 MPa
Equivalent thickness t 0.48 mm
Reinforcement grid iDiana
Property Manager
Materials Material Name: MAREIN
↑Elastic →Reinforcement →Bonded
↑Physical Properties Physical Property Name: PHREIN
↑Geometry →Embedded Reinforcements →Grid
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
3.1 Finite Element Model 51
For the reinforcement grid we define a material MAREIN with a Young’s modulus
for elasticity [Table 3.2]. We also define a physical property PHREIN with an
equivalent thickness in the X- and Y -direction of 0.48 mm both. In our case the
local x-axis of the grid is the same as the global X-axis. Thus the components
of the local vector are {1, 0, 0}.
Properties assignment fireload.fgc
PROPERTY ATTACH SLAB MASLAB
PROPERTY ATTACH STEEL MAREIN PHREIN
PROPERTY ATTACH BOUNDS MABOUN
VIEW HIDDEN FILL COLOUR
VIEW OPTIONS COLOUR MATERIAL
VIEW MESH SLAB
VIEW MESH BOUNDS
We assign the material and the physical properties to the appropriate sets of
the model geometry. We check the assignment of the material properties by
displaying the mesh of the slab and the boundaries with colors modulated ac-
cording to the assigned material [Fig. 3.7]. Both displays show only one color.
The legend confirms that this color represents the proper material: respectively
MASLAB and MABOUN.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:35 matslab.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:35 matbnd.ps
Model: FIRELOAD Model: FIRELOAD
Analysis: DIANA Analysis: DIANA
Model Type: Heatflow-Stress Staggered 3D Model Type: Heatflow-Stress Staggered 3D
Z Z
Y Y
X X
Materials Materials
MASLAB MABOUN
(a) concrete slab (b) boundaries
Figure 3.7: Checking the material assignment
3.1.6 Mechanical Loading
The quarter model is loaded by a vertical line load, distributed in the Y -direction
[Fig. 3.1 p. 43]. We define this load for the structural analysis.
Line load fireload.fgc
PROPERTY LOADS PRESSURE 1 L19 -14.5 Z
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
52 Fire under Concrete Slab
CONSTRUCT TCURVE TC1 LIST 0.0 1.0 250.0 1.0
PROPERTY ATTACH LOADCASE 1 TCURVE TC1
VIEW HIDDEN OFF
VIEW MESH ALL
LABEL MESH LOADS
We specify the distributed force via the PRESSURE load class as load case 1. The
distributed force P = 14.5 N/mm acts downward, i.e., in the Z-direction, over
line L19. As we are going to perform a transient analysis, we have to specify the
time dependency of this load. We define a time curve with a constant value of
1 from time t = 0 to t = 250. Assignment of the time curve to the load case
thus defines a constant pressure load for the specified time interval. A display
of the load on the mesh confirms the correct specification [Fig. 3.8a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:35 loads.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:35 bound.ps
Model: FIRELOAD Model: FIRELOAD
Analysis: DIANA Analysis: DIANA
Model Type: Heatflow-Stress Staggered 3D Model Type: Heatflow-Stress Staggered 3D
Z Z
Y Y
X X
(a) loading (b) constraints
Figure 3.8: Boundary conditions for structural analysis
3.1.7 Boundary Constraints
The boundary constraints for the structural analysis consist of a symmetry
condition along the back and right surfaces of the model and a vertical support
on the bottom line [Fig. 3.1 p. 43].
Symmetry and supports fireload.fgc
PROPERTY BOUNDARY CONSTRAINT S10 Y
PROPERTY BOUNDARY CONSTRAINT S11 Y
PROPERTY BOUNDARY CONSTRAINT S12 Y
PROPERTY BOUNDARY CONSTRAINT S16 X
PROPERTY BOUNDARY CONSTRAINT L8 Z
LABEL MESH OFF
LABEL MESH CONSTRNT
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
3.1 Finite Element Model 53
We suppress the horizontal normal displacement of the surfaces along the sym-
metry faces.1 For the supports we suppress the vertical displacement along the
line at X = 1200. We display the mesh with constraint labels to confirm the
correct specification [Fig. 3.8b].
3.1.8 Temperature
For the transient analysis we must specify the temperature development in time
along the boundaries, i.e., the fire load. For the heat flow analysis we must also
specify the initial temperature of the model.
Fire load fireload.fgc
PROPERTY LOADS EXTTEMP 2 BNDTOP 1
PROPERTY LOADS EXTTEMP 3 BNDBOT 1
PROPERTY LOADS EXTTEMP 4 BNDLAT 1
CONSTRUCT TCURVE TC2 LIST 0 20 250 20
CONSTRUCT TCURVE TC3 LIST 0 20 15 400 50 800 100 1000 250 1200
CONSTRUCT TCURVE TC4 LIST 0 20 15 40 50 80 100 100 250 120
UTILITY GRAPH TCURVE TC2
UTILITY GRAPH TCURVE TC3
UTILITY GRAPH TCURVE TC4
PROPERTY ATTACH LOADCASE 2 TCURVE TC2
PROPERTY ATTACH LOADCASE 3 TCURVE TC3
PROPERTY ATTACH LOADCASE 4 TCURVE TC4
Via the EXTTEMP load class we define an ambient temperature of 1 °C for the
surfaces of the boundaries. For each surface we use a time curve to define the
time dependency of the temperature. For the top surface we assume a constant
environmental temperature of 20 °C. For the bottom and lateral surfaces we
make time curves according to Figure 3.2 on page 44. We plot graphs of the
time curves to check their specification [Fig. 3.9]. By assigning the time curves
to the load cases we define the time dependency of the external temperature.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:36 timec2.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:36 timec3.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:36 timec4.ps
Model: FIRELOAD Model: FIRELOAD Model: FIRELOAD
Analysis: DIANA Analysis: DIANA Analysis: DIANA
Model Type: Heatflow-Stress Staggered 3D Model Type: Heatflow-Stress Staggered 3D Model Type: Heatflow-Stress Staggered 3D
TCURVE : TC2 TCURVE : TC3 TCURVE : TC4
*1E3
22.5 1.2 140
20
120
1
17.5
100
15 .8
V V V
A 12.5 A A 80
L L L
U U .6 U
E 10 E E
60
7.5 .4
40
5
.2
20
2.5
0 0 0
0 25 50 75 100 125 150 175 200 225 250 275 0 25 50 75 100 125 150 175 200 225 250 275 0 25 50 75 100 125 150 175 200 225 250 275
TIME TIME TIME
(a) constant (b) fire (c) for lateral surface
Figure 3.9: Time curves for temperature
1 See Figure 3.1a for surface and line names.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
54 Fire under Concrete Slab
Initial temperature fireload.fgc
PROPERTY INITIAL INITEMP ALL 20.0
Finally we specify an initial temperature field of 20 °C for all parts of the model.
3.2 Staggered Flow–Stress Analysis
For a staggered flow–stress analysis we must perform a flow analysis followed
by a structural analysis. Prior to the actual analysis we write the model to an
input data file in Diana batch format.
Write input data file iDiana
UTILTY WRITE DIANA
yes
FILE CLOSE
yes
Fire under concrete slab
iDiana writes the model to an input data file fireload.dat. We close the
model and start with the heat flow analysis.
3.2.1 Transient Heat Flow Analysis
We initiate the transient heat flow analysis via the ANALYSE command.
Initiate analysis iDiana
ANALYSE FIRELOAD
Analysis Setup
specify analysis options
In the Analysis Setup dialog we specify the various analysis options for the heat
flow analysis. This results in the following batch analysis commands.
Analysis commands thermal.dcf
*FILOS
INITIA
*INPUT
*HEATTR
INITIA TEMPER INPUT FIELD=1
EXECUT SIZES 1(10) 5(8) 50(4)
BEGIN OUTPUT FILE="thermal"
TEMPER
END OUTPUT
*END
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
3.2 Staggered Flow–Stress Analysis 55
We start the transient heat flow analysis with an initial temperature field as
defined in the input data file. We execute time steps over an interval of 250
minutes ranging from 1 minute at the beginning of the analysis to 50 minutes
at the end. We ask for output of temperatures to a database THERMAL for the
iDiana Results environment.
Once the analysis run has terminated we enter the iDiana Results environ-
ment with the name of the database to assess the results.
Initiate postprocessing thermal.fvc
FEMVIEW THERMAL
UTILITY TABULATE LOADCASES
The tabulation shows the available load cases (time steps) with their result data.
Tabulated load cases loads.tb
; Model: THERMAL
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; TR1 1 TIME = 1 "Boundary case 1"
; Nodal : PTE....S
;
; TR1 2 TIME = 2 "Boundary case 1"
; Nodal : PTE....S
... lines skipped
; TR1 22 TIME = 250 "Boundary case 1"
; Nodal : PTE....S
3.2.2 Temperature Distribution and Development
We will make contour plots for the temperature distribution after 250 minutes of
fire, i.e., for the last time step. We will also assess the temperature development
in time.
Temperature after 250 minutes of fire thermal.fvc
VIEW MESH SLAB
VIEW OPTIONS EDGES OUTLINE
EYE ROTATE TO 41 30 30
EYE FRAME
RESULTS LOADCASE TR1 22
RESULTS NODAL PTE....S PTE
PRESENT CONTOUR LEVELS
EYE ROTATE TO 90
EYE FRAME
DRAWING DISPLAY
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
56 Fire under Concrete Slab
We display a bird’s-eye view of the mesh of the slab in outline style. We select
nodal result attribute PTE representing the temperatures. We select the last
time step, i.e., the situation after 250 minutes of fire. We display a contour plot
of the temperatures [Fig. 3.10a]. As the top surface of the slab stays rather cool
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:41 temps.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 temps2.ps
Model: THERMAL Model: THERMAL
TR1: Boundary case 1 TR1: Boundary case 1
Step: 22 TIME: 250 Step: 22 TIME: 250
Nodal PTE....S PTE Nodal PTE....S PTE
Max/Min on model set: Max/Min on model set:
Max = .13E4 Max = .13E4
Min = 31.8 Min = 31.8
.118E4 .118E4
.107E4 .107E4
953 953
838 838
723 Z 723
Z 608 608
Y 492 492
377 Y X 377
262 262
X 147 147
(a) bird’s-eye view (b) side view
Figure 3.10: Temperature contours after 250 minutes of fire
we do not see much of the contours. These are only discernible in the side faces.
A view perpendicular to the longitudinal side face gives a better view of the
temperature distribution [Fig. 3.10b].
Distribution over thickness thermal.fvc
VIEW MESH SLAB
CONSTRUCT SHAPE PLANE PLANEY Y 380
VIEW XSECTION PLANEY
EYE ROTATE TO 90
EYE FRAME
LABEL MESH NODES
RESULTS LOADCASE TR1 10 TR1 18 TR1 22
PRESENT GRAPH LINE NODES THROUGH 302 404
PRESENT OPTIONS GRAPH AXES SWAP
To make a graph of the temperature distribution over the thickness of the slab
we need two nodes to define a vertical line through the slab. Therefore we
redisplay the mesh of the slab and construct a shape PLANEY corresponding
to the plane at Y = 380. With the XSECTION option we define a plane cross-
section through the model. We make a normal view of this cross-section with
node numbers [Fig. 3.11a]. We can now choose two nodes which form a vertical
line through the thickness, for instance 302 and 404 at X = 1400 (see pointers).
We select the time steps corresponding to times t = 10, 50, and 250 minutes.
We make a single display with three graphs for the temperature distribution
along the line between the two nodes [Fig. 3.11b]. To get the distance along
the thickness in vertical direction we swap the X- and Y -axes of the graphs.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
3.2 Staggered Flow–Stress Analysis 57
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 cross.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 thgraph.ps
Model: THERMAL Model: THERMAL
Nodal PTE....S PTE
Max/Min on whole graph:
Ymax = 150 Ymin = 0
Xmax = .116E4 Xmin = 20.2
Variation along a line
TR1 10
TR1 18
TR1 22
160
140
120
D 100
I
32 38 374 380 386 392 398 404 1287 1293 1299 1305 1311 S
67 169 1112 1116 1120 1124 1128 574 1904 1908 1912 1916 1454
68 170 1023 1027 1031 1035 1039 575 1832 1836 1840 1844 1455 T 80
69 171 934 938 942 946 950 576 1760 1764 1768 1772 1456 A
70 172 845 849 853 857 861 577 1688 1692 1696 1700 1457
71 173 756 760 764 768 772 578 1616 1620 1624 1628 1458 N
4 10 272 278 284 290 296 302 1202 1208 1214 1220 1226
C
E 60
40
20
0
0 .2 .4 .6 .8 1 1.2
Z NODAL PTE....S PTE *1E3
Y X
(a) node numbers for cross-section (b) after 10, 50, and 250 minutes
Figure 3.11: Temperature distribution over the thickness
We observe that after 10 minutes of fire the temperature of the bottom face is
about 230 °C, after 50 minutes about 760 °C, and after 250 minutes about 1160
°C. The top surface hardly warms up, which confirms the blue contour in the
bird’s-eye view [Fig. 3.10a].
Animation thermal.fvc
VIEW XSECTION PLANEY
VIEW OPTIONS EDGES OUTLINE
RESULTS LOADCASE TR1
PRESENT CONTOUR FROM 25 TO 800 LEVELS 10
UTILITY SETUP ANIMATE LINEAR
DRAWING ANIMATE LOADCASES PLOTFILE teman
To conclude the results assessment of the heat flow analysis we make an ani-
mation of the temperature development in the previously defined longitudinal
cross-section at Y = 380. Note that we apply consistent contour levels for all
animation frames, otherwise the contours could not be compared. The PLOT-
FILE option yields the animation frames on files so that we can show them in a
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 iDIANA
teman001
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 iDIANA
teman002
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 iDIANA
teman003
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 teman004
Model: THERMAL Model: THERMAL Model: THERMAL Model: THERMAL
TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1
Step: 1 TIME: 1 Step: 2 TIME: 2 Step: 3 TIME: 3 Step: 4 TIME: 4
Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = 37.6 Max = 59.6 Max = 83.2 Max = 107 Min = 17.5
document [Fig. 3.12].
Min = 18.4
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 Min = 17.6
iDIANA
teman005
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 Min = 17.4
iDIANA
teman006
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 iDIANA
teman007
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 teman008
Model: THERMAL Model: THERMAL Model: THERMAL Model: THERMAL
TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1
Step: 5 TIME: 5 Step: 6 TIME: 6 Step: 7 TIME: 7 Step: 8 TIME: 8
Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = 132 Min = 17.5 Max = 157 Min = 17 Max = 182 Min = 16.3 Max = 207 Min = 15.8
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 iDIANA
teman009
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 iDIANA
teman010
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 iDIANA
teman011
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 teman012
Model: THERMAL Model: THERMAL Model: THERMAL Model: THERMAL
TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1
Step: 9 TIME: 9 Step: 10 TIME: 10 Step: 11 TIME: 15 Step: 12 TIME: 20
Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = 232 Min = 15.2 Max = 258 Min = 14.6 Max = 387 Min = 11.8 Max = 455 Min = 10.4
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 iDIANA
teman013
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 iDIANA
teman014
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 iDIANA
teman015
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 teman016
Model: THERMAL Model: THERMAL Model: THERMAL Model: THERMAL
TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1
Step: 13 TIME: 25 Step: 14 TIME: 30 Step: 15 TIME: 35 Step: 16 TIME: 40
Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = 517 Min = 10.6 Max = 578 Min = 12.3 Max = 639 Min = 15.5 Max = 700 Min = 16.8
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 iDIANA
teman0179.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 iDIANA
teman0189.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 iDIANA
teman0199.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 teman020
800 800 800 800
Model: THERMAL Model: 730
THERMAL Model: 730
THERMAL Model: 730
THERMAL 730
TR1: Boundary case 1 659
TR1: Boundary case 1 659
TR1: Boundary case 1 659
TR1: Boundary case 1 659
Step: 17 TIME: 45 Step: 18589 TIME: 50 Step: 19589 TIME: 100 Step: 20589 TIME: 150 589
Nodal PTE....S PTE 518
Nodal PTE....S PTE 518
Nodal PTE....S PTE 518
Nodal PTE....S PTE 518
Max/Min on model set: Max/Min448on model set: Max/Min448on model set: Max/Min448on model set: 448
Max = Z761 Min = 17 Max = Z821
377 Min = 17.2 Max = Z.105E4
377 Max = Z.113E4
377 377
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 teman021
iDIANA 307
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:42 Min = 23
teman022
307 Min = 27.6
307 307
800
236 800
236 800
236 800
236
Model:Y THERMAL Model: 730
166
THERMAL 730
166 X 730
166 X 730
166
X Y 659 X Y 659 Y 659 659
TR1: Boundary case 1 95.5
TR1: Boundary case 1 95.5 95.5 95.5
Step: 21 TIME: 200 Step: 22589
25 TIME: 250 589
25 589
25 589
25
Nodal PTE....S PTE 518
Nodal PTE....S PTE 518 518 518
Max/Min on model set: Max/Min448on model set: 448 448 448
Max = Z.122E4 Max =Z.13E4
377 Z 377 Z 377 377
Min = 30.2 Min = 31.8
307 307 307 307
DRAWING ANIMATE LOADCASES PLOTFILE teman 800
236 DRAWING ANIMATE LOADCASES PLOTFILE teman 800
236 DRAWING ANIMATE LOADCASES PLOTFILE teman 800
236 DRAWING ANIMATE LOADCASES PLOTFILE teman 800
236
730
166 X 730
166 X 730
166 X 730
166
Y X Y 659 Y 659 Y 659 659
95.5 95.5 95.5 95.5
589
25 589
25 589
25 589
25
518 518 518 518
448 448 448 448
Z Z 377 Z 377 Z 377 377
307 307 307 307
DRAWING ANIMATE LOADCASES PLOTFILE teman 800
236 DRAWING ANIMATE LOADCASES PLOTFILE teman 800
236 DRAWING ANIMATE LOADCASES PLOTFILE teman 800
236 DRAWING ANIMATE LOADCASES PLOTFILE teman 800
236
730
166 X 730
166 X 730
166 X 730
166
Y X Y 659 Y 659 Y 659 659
95.5 95.5 95.5 95.5
589
25 589
25 589
25 589
25
518 518 518 518
448 448 448 448
Z Z 377 Z 377 Z 377 377
307 307 307 307
DRAWING ANIMATE LOADCASES PLOTFILE teman 800
236 DRAWING ANIMATE LOADCASES PLOTFILE teman 800
236 DRAWING ANIMATE LOADCASES PLOTFILE teman 800
236 DRAWING ANIMATE LOADCASES PLOTFILE teman 800
236
730
166 X 730
166 X 730
166 X 730
166
Y X Y 659 Y 659 Y 659 659
95.5 95.5 95.5 95.5
589
25 589
25 589
25 589
25
518 518 518 518
448 448 448 448
Z Z 377 Z 377 Z 377 377
307 307 307 307
DRAWING ANIMATE LOADCASES PLOTFILE teman 800
236 DRAWING ANIMATE LOADCASES PLOTFILE teman 800
236 DRAWING ANIMATE LOADCASES PLOTFILE teman 236 DRAWING ANIMATE LOADCASES PLOTFILE teman 236
730
166 X 730
Y X Y 659 Y 166
659 X Y 166 X 166
95.5 95.5 95.5 95.5
Figure 3.12: Animation of temperature development in cross-section
589
25 589
25 25 25
518 518
448 448
Z Z 377 377
307 307
DRAWING ANIMATE LOADCASES PLOTFILE teman 236 DRAWING ANIMATE LOADCASES PLOTFILE teman 236 DRAWING ANIMATE LOADCASES PLOTFILE teman DRAWING ANIMATE LOADCASES PLOTFILE teman
Y X Y 166 X 166
95.5 95.5
25 25
DRAWING ANIMATE LOADCASES PLOTFILE teman DRAWING ANIMATE LOADCASES PLOTFILE teman
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
58 Fire under Concrete Slab
3.2.3 Structural Analysis
Diana has stored the temperature distribution for the whole model, and for each
time step, on the analysis database (filos file). So this temperature information
is available for the structural analysis of the concrete slab. To initiate the
structural analysis we enter the iDiana Index environment.
Initiate analysis iDiana
INDEX
ANALYSE FIRELOAD
Analysis Setup
specification of options
Via the Analysis Setup dialog we specify a Structural Nonlinear analysis and
choose to perform the mechanical analysis using the already existing filos file
by selecting Open Existing in the Filos File section. Furthermore we specify
the various analysis options for the mechanical analysis. This results in the
following batch analysis commands.
Analysis commands structural.dcf
*NONLIN
EXECUT TIME STEPS EXPLIC SIZES 1(10) 5(8) 50(4)
BEGIN OUTPUT
FILE "Structural"
DISPLA
STRESS
END OUTPUT
*END
Once the analysis run has terminated, we enter the iDiana Results environment
to assess the results.
Initiate postprocessing structural.fvc
FEMVIEW STRUCTURAL
UTILITY TABULATE LOADCASES
VIEW MESH SLAB
EYE ROTATE TO 41 30 30
The load case tabulation shows the available load cases (time steps) with their
result data. We start with a bird’s-eye view of the model of the concrete slab.
Tabulated load cases loads.tb
; Model: STRUCTURAL
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; MODEL STATIC "Model Properties"
; Element : REINGRID*
;
; LC1 1 TIME = 1 "Load case 1"
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
3.2 Staggered Flow–Stress Analysis 59
; Nodal : TDTX...G
; Element : EL.SXX.G RE.SXX.G
;
... lines skipped
; Nodal : TDTX...G
; Element : EL.SXX.G RE.SXX.G
; * Indicates loads data
The nodal attribute TDTX represents the total displacement. The element at-
tribute EL.SXX represents the stress in the concrete slab. The element attribute
RE.SXX represents the reinforcement stress.
3.2.4 Stresses in the Concrete Slab
We will assess the distribution and development of the stresses in the concrete
slab.
Von Mises stress after 250 minutes of fire structural.fvc
RESULTS LOADCASE LC1 22
VIEW OPTIONS DEFORM USING TDTX...G RESTDT 1
EYE FRAME
RESULTS ELEMENT EL.SXX.G SXX
RESULTS CALCULATE VONMISES
PRESENT CONTOUR FROM 0 TO 200 LEVELS 10
EYE DIRECTION 0 -1000 0
VIEW OPTIONS EDGES OUTLINE
EYE FRAME
DRAWING DISPLAY
We select the last available load case (time step) for the situation after 250
minutes of fire. Via the DEFORM option we ask iDiana to display any results
in a model deformed according to the true total displacements (×1). We select
result attribute SXX for the Cauchy stresses. From these stresses we let iDiana
calculate the equivalent Von Mises stresses σeq . We display a contour plot
with explicitly specified level values [Fig. 3.13a]. To get a better view of the
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:13 sigeq1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:14 sigeq2.ps
Model: STRUCTURAL Model: STRUCTURAL
Deformation = 1 Deformation = 1
LC1: Load case 1 LC1: Load case 1
Step: 22 TIME: 250 Step: 22 TIME: 250
Element VONMISES EL.SXX.G Element VONMISES EL.SXX.G
Calculated from: EL.SXX.G Calculated from: EL.SXX.G
Max/Min on model set: Max/Min on model set:
Max = 745 Min = 5.56 Max = 745 Min = 5.56
200 200
182 182
164 164
145 145
127 127
109 109
90.9 Z 90.9
Z 72.7 72.7
Y 54.5 54.5
36.4 Y X 36.4
18.2 18.2
X 0 0
(a) bird’s-eye view (b) side view
Figure 3.13: Von Mises stress in deformed model after 250 minutes of fire
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
60 Fire under Concrete Slab
stress distribution over the thickness of the slab we also make a view on the
longitudinal side face, with the model in outline style [Fig. 3.13b]. The contour
plots show that the higher stresses occur above the support, at X = 200 mm.
Distribution over thickness structural.fvc
VIEW MESH SLAB
CONSTRUCT SHAPE PLANE PLANEY Y 380
VIEW XSECTION PLANEY
LABEL MESH NODES
EYE ZOOM FACTOR 4 -900 110
RESULTS LOADCASE LC1 10 LC1 18 LC1 22
PRESENT GRAPH LINE NODES THROUGH 10 38
PRESENT OPTIONS GRAPH AXES SWAP
To make graphs of the stress distribution over the thickness we need nodes
in the top and bottom face. Like for the thermal analysis, we make a cross-
section at Y = 380. We get the appropriate node numbers from a zoomed-in
display [Fig. 3.14a] (see pointers). The graphs show the distribution of the Von
Mises stress at location (200,380) for times after 10, 50, and 250 minutes of fire
[Fig. 3.14b].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:14 strnod.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:14 seqgr.ps
Model: STRUCTURAL Model: STRUCTURAL
Deformation = 1 Deformation = 1
Element VONMISES EL.SXX.G
Calculated from: EL.SXX.G
Max/Min on whole graph:
Ymax = 150 Ymin = 0
Xmax = 322 Xmin = 12.3
Variation along a line
LC1 10
160 LC1 18
LC1 22
140
32 120
109 49
67
110 38
267 D 100
68 205 410 I
111 169 S
263 374
69 206 1132 T 80
1181 421 A
112 170
259 1112 380 N
70 207 1043 1092 1141 1185 C
113 171 E 60
255 1023 1116
71 208 954 1003 1052 1096
114 172
251 934 1027
4 209 865 40
914 963 1007
173
21 845 938
210 776 825 874 918
10 20
756 849
308 736 785 829
272 760
0
319 740
0 50 100 150 200 250 300 350
278
Z VONMISES EL.SXX.G
Y X
(a) node numbers for cross-section (b) after 10, 50, and 250 minutes
Figure 3.14: Graphing the Von Mises stress distribution over the thickness
Animation structural.fvc
VIEW XSECTION PLANEY
EYE FRAME
VIEW OPTIONS EDGES OUTLINE
RESULTS LOADCASE LC1
PRESENT CONTOUR FROM 0 TO 200 LEVELS 10
UTILITY SETUP ANIMATE LINEAR
DRAWING ANIMATE LOADCASES PLOTFILE seqan
We make an animation of the Von Mises stress development in the previously
defined longitudinal cross-section at Y = 380 [Fig. 3.15].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:14 seqan001
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:14 seqan002
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:15 seqan003
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:15 seqan004
3.2 Staggered Flow–Stress Analysis 61
Model: STRUCTURAL Model: STRUCTURAL Model: STRUCTURAL Model: STRUCTURAL
Deformation = 1 Deformation = 1 Deformation = 1 Deformation = 1
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Step: 1 TIME: 1 Step: 2 TIME: 2 Step: 3 TIME: 3 Step: 4 TIME: 4
Element VONMISES EL.SXX.G Element VONMISES EL.SXX.G Element VONMISES EL.SXX.G Element VONMISES EL.SXX.G
Calculated from: EL.SXX.G Calculated from: EL.SXX.G Calculated from: EL.SXX.G Calculated from: EL.SXX.G
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = 7.55 Min = .258 Max = 16.8 Min = .632 Max = 26.3 Min = .748 Max = 35.7 Min = 1.12
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:15 seqan005
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:15 seqan006
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:15 seqan007
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:15 seqan008
Model: STRUCTURAL Model: STRUCTURAL Model: STRUCTURAL Model: STRUCTURAL
Deformation = 1 Deformation = 1 Deformation = 1 Deformation = 1
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Step: 5 TIME: 5 Step: 6 TIME: 6 Step: 7 TIME: 7 Step: 8 TIME: 8
Element VONMISES EL.SXX.G Element VONMISES EL.SXX.G Element VONMISES EL.SXX.G Element VONMISES EL.SXX.G
Calculated from: EL.SXX.G Calculated from: EL.SXX.G Calculated from: EL.SXX.G Calculated from: EL.SXX.G
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = 46 Min = 1.08 Max = 56.9 Min = .881 Max = 68.2 Min = .677 Max = 79.7 Min = .582
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:15 seqan009
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:15 seqan010
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:15 seqan011
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:15 seqan012
Model: STRUCTURAL Model: STRUCTURAL Model: STRUCTURAL Model: STRUCTURAL
Deformation = 1 Deformation = 1 Deformation = 1 Deformation = 1
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Step: 9 TIME: 9 Step: 10 TIME: 10 Step: 11 TIME: 15 Step: 12 TIME: 20
Element VONMISES EL.SXX.G Element VONMISES EL.SXX.G Element VONMISES EL.SXX.G Element VONMISES EL.SXX.G
Calculated from: EL.SXX.G Calculated from: EL.SXX.G Calculated from: EL.SXX.G Calculated from: EL.SXX.G
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = 91.6 Min = .745 Max = 104 Min = .754 Max = 170 Min = 2.34 Max = 213 Min = 1.86
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:15 seqan013
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:15 seqan014
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:15 seqan015
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:15 seqan016
Model: STRUCTURAL Model: STRUCTURAL Model: STRUCTURAL Model: STRUCTURAL
Deformation = 1 Deformation = 1 Deformation = 1 Deformation = 1
LC1: Load case 1 LC1: Load
200 case 1 LC1: Load
200 case 1 LC1: Load
200 case 1 200
Step: 13 TIME: 25 Step: 182
14 TIME: 30 Step: 182
15 TIME: 35 Step: 182
16 TIME: 40 182
Element VONMISES EL.SXX.G Element 164VONMISES EL.SXX.G Element164 VONMISES EL.SXX.G Element164VONMISES EL.SXX.G 164
Calculated from: EL.SXX.G Calculated
145 from: EL.SXX.G Calculated
145 from: EL.SXX.G Calculated
145 from: EL.SXX.G 145
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = 253 Min = 2.51 Max = 127
291 Min = 2.72 Max = 127
329 Min = 2.91 Max = 127
366 Min = 3.64 127
iDIANA 9.4.3-02 : TNO Diana BV iDIANA109
28 OCT 2010 01:37:16 seqan017 9.4.3-02 : TNO Diana BV iDIANA109
28 OCT 2010 01:37:16 seqan018 9.4.3-02 : TNO Diana BV iDIANA109
28 OCT 2010 01:37:16 seqan019 9.4.3-02 : TNO Diana BV 109
28 OCT 2010 01:37:16 seqan020
Z Z90.9 Z90.9 Z90.9 90.9
Model: STRUCTURAL Model:72.7STRUCTURAL Model:72.7
STRUCTURAL Model:72.7
STRUCTURAL 72.7
Deformation = 1 54.5 = 1
Deformation 54.5 = 1
Deformation 54.5 = 1
Deformation 54.5
LC1: Load
Y case
X 1 36.4 case
LC1: Load
Y200 X 1 36.4 case
LC1: Load
Y200 X 1 36.4 case
LC1: Load
Y200 X 1 36.4
200
Step: 17 TIME: 45 18.2
Step: 182
18 TIME: 50 18.2
Step: 182
19 TIME: 100 18.2
Step: 182
20 TIME: 150 18.2
182
Element VONMISES EL.SXX.G Element 0 VONMISES EL.SXX.G
164 Element0 VONMISES EL.SXX.G
164 Element0 VONMISES EL.SXX.G
164 0
164
Calculated from: EL.SXX.G Calculated
145 from: EL.SXX.G Calculated
145 from: EL.SXX.G Calculated
145 from: EL.SXX.G 145
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = 402 Min = 4.61 Max = 127
439 Min = 5.27 Max = 127
594 Min = 3.47 Max = 127
654 Min = 1.71 127
iDIANA 9.4.3-02 : TNO Diana BV iDIANA109
28 OCT 2010 01:37:16 seqan021 9.4.3-02 : TNO Diana BV 109
28 OCT 2010 01:37:16 seqan022 109 109
Z DRAWING ANIMATE LOADCASES PLOTFILE seqan Z90.9 DRAWING ANIMATE LOADCASES PLOTFILE seqan Z90.9 DRAWING ANIMATE LOADCASES PLOTFILE seqan Z90.9 DRAWING ANIMATE LOADCASES PLOTFILE seqan 90.9
Model: STRUCTURAL Model:72.7
STRUCTURAL 72.7 72.7 72.7
Deformation = 1 54.5 = 1
Deformation 54.5 54.5 54.5
LC1: Load
Y case
X 1 LC1: Y 36.4 case
Load
200 X 1 36.4 X
Y200 36.4 X
Y200 36.4
200
Step: 21 TIME: 200 18.2
Step: 182
22 TIME: 250 18.2
182 18.2
182 18.2
182
Element VONMISES EL.SXX.G Element164VONMISES EL.SXX.G
0 0
164 0
164 0
164
Calculated from: EL.SXX.G Calculated
145 from: EL.SXX.G 145 145 145
Max/Min on model set: Max/Min on model set:
Max = 702 Min = 6.22 Max = 127
745 Min = 5.56 127 127 127
109 109 109 109
Z DRAWING ANIMATE LOADCASES PLOTFILE seqan Z90.9 DRAWING ANIMATE LOADCASES PLOTFILE seqan Z90.9 DRAWING ANIMATE LOADCASES PLOTFILE seqan Z90.9 DRAWING ANIMATE LOADCASES PLOTFILE seqan 90.9
72.7 72.7 72.7 72.7
54.5 54.5 54.5 54.5
Y X 36.4 X
Y200 36.4 X
Y200 36.4 X
Y200 36.4
200
18.2
182 18.2
182 18.2
182 18.2
182
0
164 0
164 0
164 0
164
145 145 145 145
127 127 127 127
109 109 109 109
Z DRAWING ANIMATE LOADCASES PLOTFILE seqan Z90.9 DRAWING ANIMATE LOADCASES PLOTFILE seqan Z90.9 DRAWING ANIMATE LOADCASES PLOTFILE seqan Z90.9 DRAWING ANIMATE LOADCASES PLOTFILE seqan 90.9
72.7 72.7 72.7 72.7
54.5 54.5 54.5 54.5
Y X 36.4 X
Y200 36.4 X
Y200 36.4 X
Y200 36.4
200
18.2
182 18.2
182 18.2
182 18.2
182
0
164 0
164 0
164 0
164
145 145 145 145
127 127 127 127
109 109 109 109
Z DRAWING ANIMATE LOADCASES PLOTFILE seqan Z90.9 DRAWING ANIMATE LOADCASES PLOTFILE seqan Z90.9 DRAWING ANIMATE LOADCASES PLOTFILE seqan Z90.9 DRAWING ANIMATE LOADCASES PLOTFILE seqan 90.9
72.7 72.7 72.7 72.7
54.5 54.5 54.5 54.5
Y X 36.4 X
Y200 Y36.4
200 X Y36.4 X 36.4
18.2
182 18.2
182 18.2 18.2
0
164 0164 0 0
145 145
127 127
109 109
DRAWING ANIMATE LOADCASES PLOTFILE seqan Z90.9 DRAWING ANIMATE LOADCASES PLOTFILE seqan 90.9 DRAWING ANIMATE LOADCASES PLOTFILE seqan DRAWING ANIMATE LOADCASES PLOTFILE seqan
Figure 3.15: Animation of Von Mises stress development in cross-section
Z
72.7 72.7
54.5 54.5
Y X Y36.4 X 36.4
18.2 18.2
0 0
DRAWING ANIMATE LOADCASES PLOTFILE seqan DRAWING ANIMATE LOADCASES PLOTFILE seqan
3.2.5 Stresses in the Reinforcement Grid
We will assess the distribution and development of the stresses in the reinforce-
ment grid.
Stress after 250 minutes of fire structural.fvc
VIEW MESH SETGRID
VIEW OPTIONS EDGES OUTLINE
VIEW OPTIONS DEFORM OFF
EYE ROTATE TO 41 30 30
EYE FRAME
RESULTS LOADCASE LC1 22
RESULTS ELEMENT RE.SXX.G SXX
PRESENT CONTOUR FROM 800 TO 2300 LEVELS 10
RESULTS ELEMENT RE.SXX.G SYY
DRAWING DISPLAY
We display a bird’s-eye view of the undeformed mesh of the reinforcement grid
in outline style. We select the last load case (time step) for the situation after
250 minutes of fire. We display contour plots, with equivalent level values, for
the stresses in the X- and Y -direction [Fig. 3.16].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:17 sxxrei.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:17 syyrei.ps
Model: STRUCTURAL Model: STRUCTURAL
LC1: Load case 1 LC1: Load case 1
Step: 22 TIME: 250 Step: 22 TIME: 250
Element RE.SXX.G SXX Element RE.SXX.G SYY
Max/Min on model set: Max/Min on model set:
Max = .259E4 Max = .238E4
Min = 489 Min = 352
.23E4 .23E4
.216E4 .216E4
.203E4 .203E4
.189E4 .189E4
.175E4 .175E4
.162E4 .162E4
.148E4 .148E4
Z .135E4 Z .135E4
Y .121E4 Y .121E4
.107E4 .107E4
936 936
X 800 X 800
(a) σXX (b) σY Y
Figure 3.16: Reinforcement stresses after 250 minutes of fire
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II) November 8, 2010 – First ed.
62 Fire under Concrete Slab
History plot structural.fvc
LABEL MESH ELEMENTS VIEWMODE BLUE
EYE ZOOM FACTOR 3 800 -550
RESULTS LOADCASE LC1
PRESENT GRAPH ELEMENT 699
PRESENT OPTIONS GRAPH AXES SWAP
We label the element numbers on the current contour plot. We zoom in on the
area with the high stresses and determine the element nearest to the highest
stress [Fig. 3.17a]. We select all load cases (time steps) and make a time graph
of the development of the stress σY Y for this element [Fig. 3.17b]. We swap the
axes to get the time horizontally.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:17 relm.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:17 resgr.ps
Model: STRUCTURAL Model: STRUCTURAL
LC1: Load case 1 Element RE.SXX.G SYY
Step: 22 TIME: 250 Max/Min on whole graph:
Element RE.SXX.G SYY Ymax = .225E4
Max/Min on model set: Ymin = 4.77
Max = .238E4 677 678 685 686 693 694 Xmax = 250
Min = 352 Xmin = 1
*1E3 Variation over loadcases
Element 699 Mean
2.25
679 680 687 688 695 696 2
E
L 1.75
E
M
E
682 689 690 697 698 N 1.5
T
R 1.25
E
.
700 S 1
691 692 699 X
X
. .75
G
S .5
701 702 Y
.23E4 Y
.216E4 .25
.203E4
.189E4
.175E4 0
.162E4 0 25 50 75 100 125 150 175 200 225 250 275
.148E4 TIME
Z .135E4
Y .121E4
.107E4
936
X 800
(a) location of element (b) time graph
Figure 3.17: Development of σY Y in the reinforcement
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (II)
Part III
Cracking and Failure
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
Chapter 4
Smeared Cracking in a
Notched Beam
Name: NotchSm
Path: /Examples/ConcMas/NotchSm
Keywords: analys: linear nonlin physic static. constr: suppor. elemen:
pstres q8mem. load: deform. materi: consta crack cutoff
elasti isotro linear retent smear soften. option: direct groups
newton regula units. post: binary femvie. pre: femgen. re-
sult: cauchy crack displa extern force green reacti strain stress
total.
50
50
5
450
Figure 4.1: Notched beam [mm]
This example aims at setting up and evaluating a finite element model based
on smeared cracking. More precisely, it concerns a single-edged notched beam
[Fig. 4.1]. The thickness of the beam is 100 mm. The notch is 5 mm wide and
50 mm deep. We assume that the load is concentrated in one point.
4.1 Finite Element Model
To build up the finite element model, we start iDiana and enter the Design
environment with the model name NOTCH.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
66 Smeared Cracking in a Notched Beam
iDiana
FEMGEN NOTCH
Analysis and Units
Analysis Selection
Model Type: →Structural 2D
Units Definition
Length: →Millimeter
Mass: →Kilogram
Force: →Newton
Time: →Second
Temperature: →Celsius
In the Analysis and Units dialog we specify that the model is for a structural two-
dimensional analysis of a plane stress condition. We also indicate the adopted
units [mm, kg, N, s, °C].
4.1.1 Geometry Definition
To define the geometry we apply six points P1 to P6 [Fig. 4.2].
P6 P5
P3 P4
Y
P1 P2
X
Figure 4.2: Points for geometry definition
Points notch.fgc
GEOMETRY POINT COORD 0
GEOMETRY POINT COORD 222.5
GEOMETRY POINT COORD 222.5 50
GEOMETRY POINT COORD 225 50
GEOMETRY POINT COORD 225 100
GEOMETRY POINT COORD 0 100
EYE FRAME
LABEL GEOMETRY POINTS
We specify the coordinates of the points in the XY -coordinate system. Note that
non-specified coordinates are zero by default and that iDiana will automatically
name the points sequentially: P1, P2, ..., P6. We display the points labeled with
their names and fitted in the viewport.
Lines and surface notch.fgc
GEOMETRY LINE STRAIGHT L1 P1 P2
GEOMETRY LINE STRAIGHT L2 P2 P3
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
4.1 Finite Element Model 67
GEOMETRY LINE STRAIGHT L3 P3 P4
GEOMETRY LINE STRAIGHT L4 P4 P5
GEOMETRY LINE STRAIGHT L5 P5 P6
GEOMETRY LINE STRAIGHT L6 P6 P1
CONSTRUCT SET LEFT APPEND LINES ALL
GEOMETRY SURFACE REGION S1 LEFT
VIEW GEOMETRY CURRENT RED
LABEL GEOMETRY LINES ALL RED
We construct successively six lines. Then, we construct a set named LEFT that
contains all the lines of the left-hand side part of the model. We display the
geometry and line labels in red [Fig. 4.3a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:42 geom1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:42 mesh1.ps
Model: NOTCH Model: NOTCH
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
L5
L6 L4
L3
L2
L1
Y Y
Z X Z X
(a) geometry (b) mesh
Figure 4.3: Half the model (left part)
4.1.2 Meshing
We may now create a finite element mesh on the defined geometry.
notch.fgc
MESHING OPTIONS ALGORITHM PAVING S1
MESHING DIVISION ELSIZE ALL 5
MESHING TYPES ALL QU4 Q8MEM
MESHING DIVISION AUTOMATIC
MESHING GENERATE
VIEW MESH
We select the QU4 generic element type and the Q8MEM linear plane stress el-
ement for the set LEFT of the model. With the ELSIZE option we request for
an average element size of 5 mm. The PAVING meshing algorithm can create a
quadrilateral free mesh on any type of surface and thus is well suited to mesh
the left surface of our model. We generate the mesh and display it in the default
wire netting style [Fig. 4.3b]. Note that the specified element size leads to a fine
mesh.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
68 Smeared Cracking in a Notched Beam
4.1.3 Mirror to Full Model
We may now complete the model by mirroring the geometry.
notch.fgc
GEOMETRY COPY S1 MIRROR X 225
VIEW GEOMETRY ALL RED
LABEL GEOMETRY POINTS ALL BLUE
EYE FRAME
MESHING GENERATE
VIEW MESH
We mirror the surface with respect to a vertical line at X = 225 mm, i.e., the
central axis of the model. We introduce a small imperfection by modifying the
location of point P3 to assure that the cracking will be initiated at the left side
of the symmetric model. The geometry now covers the whole model [Fig. 4.4a].
Finally, we re-generate and display the mesh [Fig. 4.4b].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:42 geom2.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:43 mesh3.ps
Model: NOTCH Model: NOTCH
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
P6 P5 P10
P3P9
P4
P1 P8
P2 P7
Y Y
Z X Z X
(a) geometry (b) final mesh
Figure 4.4: Full model
4.1.4 Material and Physical Properties
We launch the Property Manager dialog to define the material and physical
properties of the model.
iDiana
View →Property Manager...
↑
Property Manager
···
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
4.1 Finite Element Model 69
Concrete (nonlinear) iDiana
Property Manager
↑ Materials Material Name: MACONCRE
↑Linear Elasticity →Isotropic
↑Static Nonlinearity →Concrete and Brittle Materials →Multi-directional Fixed Crack
→Constant Stress Cut-off →Linear Tension Softening
→Ultimate Strain Based →Constant Shear Retention →No Plasticity
We define the properties of concrete in a material instance MACONCRE. For linear
elasticity we specify a Young’s modulus E = 31000 MPa and a Poisson’s ratio
ν = 0.15. For the nonlinear material properties we fill in the parameters for the
tensile strength ft = 2.4 MPa, the ultimate strain of the diagram εu = 0.013,
and a constant shear retention factor β = 0.001.
Concrete (linear) iDiana
Property Manager
↑ Materials Material Name: MACONLIN
↑Linear Elasticity →Isotropic
Since we know where the cracks are going to appear we are going to limit
the nonlinear material usage to the relevant region. This is done to reduce the
calculation time. In order to do so we need a second material with linear material
properties only. We define the properties of concrete in a material instance
MACONLIN. For linear elasticity we specify a Young’s modulus E = 31000 MPa
and a Poisson’s ratio ν = 0.15.
Thickness iDiana
Property Manager
↑ Physical Properties Physical Property Name: PHCONCRE
↑Geometry →Plane Stress →Regular
For the thickness of the concrete we define a physical property instance PHCON-
CRE for which we specify a thickness value t = 100 mm.
Assignment notch.fgc
PROPERTY ATTACH ALL MACONLIN PHCONCRE
CONSTRUCT PMODIFIER CENTROID CUBOID 214 49 -1 236 101 1
PROPERTY ATTACH MO1 MACONCRE PHCONCRE
We first assign the linear material and property instances to the entire geometry
of the model. Then we modify the properties for the relevant nonlinear region of
the model. Please note that the attachment of the PMODIFIER also changes
the physical property assignmenti which you do not want to change. It isw
therefore specified again in the second PROPERTY ATTACH command.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
70 Smeared Cracking in a Notched Beam
4.1.5 Supports and Loading
To define the supports and loading with respect to the geometric parts, we read
the appropriate points from the geometry plot [Fig. 4.4a].
Supports notch.fgc
PROPERTY BOUNDARY CONSTRAINT CO1 P1 X Y
PROPERTY BOUNDARY CONSTRAINT CO2 P7 Y
LABEL MESH CONSTRNT
We support the lower-left corner in X- and Y -direction and the lower-right
corner in Y -direction. The supported degrees of freedom show up as red spikes
[Fig. 4.5a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:43 constr.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:43 load.ps
Model: NOTCH Model: NOTCH
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
Y Y
Z X Z X
(a) supports (b) load
Figure 4.5: Boundary conditions
Load notch.fgc
PROPERTY LOADS DISPLACE LO1 P5 -1.0 Y
LABEL MESH OFF
LABEL MESH LOADS
The defined load corresponds to a unit displacement applied on top of the beam
just above the notch. This load shows up as a vertical violet arrow [Fig. 4.5b].
4.2 Preliminary Linear Analysis
First of all, we will perform a linear analysis in order to check the model. There-
fore, we write the just created finite element model to a an input data file in
Diana batch format.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
4.2 Preliminary Linear Analysis 71
iDiana
UTILITY WRITE DIANA
yes
FILE CLOSE
yes
Smeared cracking of a notched beam
ANALYSE NOTCH
Analysis Setup
···
Via the Analysis Setup dialog we activate the following batch commands.
linsta.dcf
*FILOS
INITIA
*INPUT
*LINSTA
*END
By default, Diana will write the analysis results to a database for the iDiana
Results environment. As soon as the job has finished, we enter this environment
with the name of the model
linsta.fvc
FEMVIEW LINSTA
VIEW MESH
VIEW OPTIONS EDGES OUTLINE
EYE FRAME
The VIEW and EYE commands display outlines of the non-deformed mesh in
green.
4.2.1 Deformation
To get the deformed mesh displayed we give the following commands
linsta.fvc
RESULTS LOADCASE LC1
RESULTS NODAL DTX....G RESDTX
PRESENT SHAPE
We select load case LC1 (the only one) and result attribute RESDTX which rep-
resents the nodal displacements. We display the deformed shape of the mesh
[Fig. 4.6a]. Note that iDiana chooses a red color and an appropriate multipli-
cation factor, in this case 22×.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
72 Smeared Cracking in a Notched Beam
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:48 lidfm.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:48 listr.ps
Model: LINSTA Model: LINSTA
LC1: Load case 1 LC1: Load case 1
Nodal DTX....G RESDTX Element PRINC STRESS ALL
Max = 1.18 Min = 0 Calculated from: EL.SXX.G
Factor = 22.3 Max = 252 Min = -136
Factor = .105
214
175
136
Y Y 97
58.2
19.3
-19.6
Z X Z X -58.4
-97.3
(a) deformation (×22) (b) principal stresses
Figure 4.6: Linear analysis results
4.2.2 Principal Cauchy Stresses
The principal stresses in the beam may still give a better understanding of the
behavior of the model.
linsta.fvc
RESULTS ELEMENT EL.SXX.G SXX
RESULTS CALCULATE P-STRESS ALL
PRESENT OPTIONS VECTORS MODULATE 10
PRESENT VECTORS
We select result attribute SXX which represents the Cauchy stresses in the el-
ement nodes. As only the primary stresses were stored, we ask iDiana to
calculate the principal stresses via the P-STRESS option. Although iDiana will
always display stress vectors with a size proportional to the stress value, stress
peaks are more convincing when the vectors are modulated with colors accord-
ing to their values as well. Therefore, we give the VECTORS MODULATE option
and ask for modulation with ten colors. Finally, we display the stress vectors
[Fig. 4.6b]. Note that the red vectors indicate the highest tension stresses and
the dark blue vectors the highest compression stresses.
4.3 Nonlinear Analysis
To perform the nonlinear analysis we enter the iDiana Index environment.
iDiana
INDEX
ANALYSE NOTCH
Analysis Setup
···
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
4.3 Nonlinear Analysis 73
Via the Analysis Setup dialog we choose for a Structural Nonlinear analysis and
create the following batch commands:
nonlin.dcf
*NONLIN
BEGIN EXECUT
BEGIN ITERAT
CONVER SIMULT
MAXITE=30
END ITERAT
BEGIN LOAD
BEGIN STEPS
BEGIN AUTOMA
SIZE=1.0
MAXSIZ=0.1
MINSIZ=0.001
END AUTOMA
END STEPS
END LOAD
END EXECUT
BEGIN OUTPUT
DISPLA TOTAL TRANSL
STRESS TOTAL CAUCHY
FORCE REACTI TRANSL
STRAIN CRACK GREEN
END OUTPUT
*END
You could also directly run the analysis in batch mode, with the input data
and command files:
diana notch.dat nonlin
When the analysis is completed, we can enter the iDiana Results environment
with the model name NONLIN to assess the analysis results.
nonlin.fvc
FEMVIEW NONLIN
UTILITY TABULATE LOADCASES
The load case tabulation shows the available load cases with their load factor
and available result items. Here we only show the first and last steps of the
tabulation:
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
74 Smeared Cracking in a Notched Beam
nllc.tb
;
; Model: NONLIN
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; MODEL STATIC "Model Properties"
; Element : THICKNES* CRKBANDW*
;
; LC1 1 LOAD = .25E-1 "Load case 1"
; Nodal : TDTX...G FBX....G
; Element : EL.SXX.G
; Gauss : EL.EKNN1
;
... lines skipped
; Nodal : TDTX...G FBX....G
; Element : EL.SXX.G
; Gauss : EL.EKNN1 EL.EKNN2
;
; LC1 54 LOAD = 1 "Load case 1"
; Nodal : TDTX...G FBX....G
; Element : EL.SXX.G
; Gauss : EL.EKNN1 EL.EKNN2
; * Indicates loads data
;
In all the steps we see the element attributes EL.SXX.G which represent the total
stresses in the elements and the Gaussian attributes EL.EKNN1 and EL.EKNN2
which represent the crack strains in the integration points, i.e., there are cracks
in the model.
4.3.1 Load–Displacement Diagram
We will first present the load–displacement diagram for the top center of the
beam. This requires the number of the node at that location.
nonlin.fvc
VIEW MESH
EYE ZOOM /CURSOR
LABEL MESH NODES
We display the mesh and drag a zoom window around the top center of the
model [Fig. 4.7a]. Then we label the mesh with node numbers and see that the
appropriate node is number 68 [Fig. 4.7b]. We can now issue the commands to
draw the load–displacement diagram.
nonlin.fvc
RESULTS LOADCASE LC1
RESULTS NODAL FBX....G FBY
PRESENT GRAPH NODE 68
First we select all available load cases, i.e., the load steps. Then we select the
nodal result attribute FBY which represents the vertical reaction force. The final
PRESENT command displays the load–displacement diagram [Fig. 4.8]. Note that
the horizontal axis of the graph represents the ‘load factor’ which is equivalent
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
4.3 Nonlinear Analysis 75
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:48 meshp.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:48 meshz.ps
Model: NONLIN Model: NONLIN
72 71 70 69 68 1036 1037 1038 1039
190 191 192 193 67 1160 1159 1158 1157
311 312 313 194 66 1161 1280 1279 1278
Y Y
Z X Z X
424 425 314 195 65 1162 1281 1392 1391
(a) general view and zoom window (b) zoom-in
Figure 4.7: Mesh with node numbers
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:48 lodis.ps
Model: NONLIN
Nodal FBX....G FBY
Max/Min on whole graph:
Ymax = .162E4
Ymin = 143
Xmax = 1
Xmin = .25E-1
*1E3 Variation over loadcases
Node 68
1.8
1.6
N 1.4
O
D
A
L 1.2
F
B 1
X
.
. .8
.
.
G .6
F
B .4
Y
.2
0
0 .1 .2 .3 .4 .5 .6 .7 .8 .9 1 1.1
LOAD
Figure 4.8: Load–displacement diagram at mid-span
to the multiplication factor for the applied vertical unit displacement at the top
center. The diagram clearly shows that at the end the structure has almost
collapsed, i.e., the analysis has reached the Ultimate Limit State.
4.3.2 Principal Cauchy Stresses
To assess the results in the mesh we first make a display of the full mesh without
node numbers.
nonlin.fvc
VIEW MESH
VIEW EDGES
EYE FRAME
LABEL MESH NODES OFF
RESULTS LOADCASE LC1 1
RESULTS ELEMEN EL.SXX.G SXX
RESULTS CALCULATE P-STRESS P1 2DSORT
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
76 Smeared Cracking in a Notched Beam
PRESENT CONTOUR LEVELS
RESULTS LOADCASE LC1 48
DRAWING DISPLAY
We select load case LC1 1 which represents the analysis results of the first step.
Then we select the Cauchy stresses from which we let iDiana calculate the
principal stresses. Due to the sorting option 2DSORT, the first stress will always
represent the maximum of the two principal stresses. We display these maximum
stresses in a contour plot [Fig. 4.9a]. We also select step 48 which represents
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:48 sxx1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:48 sxx48.ps
Model: NONLIN Model: NONLIN
LC1: Load case 1 LC1: Load case 1
Step: 1 LOAD: .25E-1 Step: 48 LOAD: .504
Element PRINC STRESS PMAX Element PRINC STRESS PMAX
Calculated from: EL.SXX.G Calculated from: EL.SXX.G
Max = 2.73 Min = -1.87 Max = 7.06 Min = -1.82
2.31 6.26
1.89 5.45
1.48 4.64
1.06 3.83
Y .639 Y 3.02
.221 2.22
-.197 1.41
Z X -.616 Z X .602
-1.03 -.206
-1.45 -1.01
(a) first load step (b) near Ultimate Limit State
Figure 4.9: Maximum principal stress
the situation just before the Ultimate Limit State. Only the DRAWING DISPLAY
command will do to display the results for the selected step [Fig. 4.9b].
4.3.3 Crack Pattern
We will now draw the crack pattern for the currently selected load step, i.e.,
near the Ultimate Limit State.
nonlin.fvc
RESULTS GAUSSIAN EL.EKNN1 EKNN
PRESENT DISC 0.2
VIEW OPTIONS DEFORM USING TDTX...G RESTDT
We select the Gaussian result attribute EKNN which represents the crack strains
in the integration points. We display the edges of the model in its deformed
shape and present the strains via the DISC option. This option shows the strains
as disks in three-dimensional space. In a two-dimensional view, i.e., viewed
perpendicular to the model, these disks show up as lines which clearly indicate
the crack pattern [Fig. 4.10].
Animation. It is very instructive to see the crack strain contours develop
with increasing load. Therefore we can produce an animation sequence (movie)
with the following commands.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
4.3 Nonlinear Analysis 77
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:48 epcrk.ps
Model: NONLIN
Deformation = 39.7
LC1: Load case 1
Step: 48 LOAD: .504
Gauss EL.EKNN1 EKNN
Max = .72E-1
Min = 0
Z X .48E-1
.24E-1
Figure 4.10: Crack pattern near Ultimate Limit State
nonlin.fvc
RESULTS LOADCASE LC1
PRESENT CONTOUR FROM 0 TO 0.08 LEVELS 10
DRAWING ANIMATE LOADCASES PLOTFILE anecr
First we select load cases for which crack strains have developed, i.e., without
load case 1. Be aware that in an animation sequence of contour plots the frames
of the animation all use the same color to represent a certain value. Therefore
we explicitly specify the values for the first and last contours and the number
of contour levels. The DRAWING command starts the animation. Due to the
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:49 anecr001
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:49 anecr002
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:49 anecr003
PLOTFILE option we can show the animation frames in a document. Figure 4.11
shows a subset of the frames.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:49 anecr004
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:49 anecr005
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:49 anecr006
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:49 anecr007
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:49 anecr008
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:49 anecr009
DRAWING ANIMATE LOADCASES PLOTFILE anecr DRAWING ANIMATE LOADCASES PLOTFILE anecr DRAWING ANIMATE LOADCASES PLOTFILE anecr
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:49 anecr010
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:49 anecr011
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:49 anecr012
DRAWING ANIMATE LOADCASES PLOTFILE anecr DRAWING ANIMATE LOADCASES PLOTFILE anecr DRAWING ANIMATE LOADCASES PLOTFILE anecr
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:49 anecr013
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:49 anecr014
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:50 anecr015
DRAWING ANIMATE LOADCASES PLOTFILE anecr DRAWING ANIMATE LOADCASES PLOTFILE anecr DRAWING ANIMATE LOADCASES PLOTFILE anecr
DRAWING ANIMATE LOADCASES PLOTFILE anecr DRAWING ANIMATE LOADCASES PLOTFILE anecr DRAWING ANIMATE LOADCASES PLOTFILE anecr
Figure 4.11: Crack strain development (cracking) – animation frames
DRAWING ANIMATE LOADCASES PLOTFILE anecr DRAWING ANIMATE LOADCASES PLOTFILE anecr DRAWING ANIMATE LOADCASES PLOTFILE anecr
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
78 Smeared Cracking in a Notched Beam
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
Chapter 5
Discrete Cracking in a
Notched Beam
Name: Notch
Path: /Examples/ConcMas/Notch
Keywords: analys: nonlin physic. constr: suppor tying. elemen: interf
l8if pstres q8mem struct. load: deform. materi: consta crack
discre elasti isotro nonlin secant shear soften unload. option:
direct groups newton regula units. post: binary femvie. pre:
femgen. result: cauchy displa force reacti stress total tracti.
50
50
5
450
Figure 5.1: Notched beam [mm]
This example aims at setting up and evaluating a finite element model based
on discrete cracking. More precisely, it concerns a single-edged notched beam
[Fig. 5.1]. The thickness of the beam is 100 mm. The notch is 5 mm wide and
50 mm deep. Just above the notch, we will anticipate for a central crack by
using line interface elements in the middle of the model. We assume that the
load is concentrated in one point.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
80 Discrete Cracking in a Notched Beam
5.1 Finite Element Model
To build up the finite element model, we start iDiana and enter the Design
environment with the model name NOTCH.
iDiana
FEMGEN NOTCH
Analysis and Units
Analysis Selection
Model Type: →Structural 2D
Units Definition
Length: →Millimeter
Mass: →Kilogram
Force: →Newton
Time: →Second
Temperature: →Celsius
In the Analysis and Units dialog we specify that the model is for a structural two-
dimensional analysis of a plane stress condition. We also indicate the adopted
units [mm, kg, N, s, °C].
5.1.1 Geometry Definition
To define the geometry we apply six points P1 to P6 [Fig. 5.2].
P6 P5
P3 P4
Y
P1 P2
X
Figure 5.2: Points for geometry definition
Points notch.fgc
GEOMETRY POINT COORD 0
GEOMETRY POINT COORD 222.5
GEOMETRY POINT COORD 222.5 50
GEOMETRY POINT COORD 225 50
GEOMETRY POINT COORD 225 100
GEOMETRY POINT COORD 0 100
EYE FRAME
LABEL GEOMETRY POINTS
We specify the coordinates of the points in the XY -coordinate system. Note that
non-specified coordinates are zero by default and that iDiana will automatically
name the points sequentially: P1, P2, ..., P6. We display the points labeled with
their names and fitted in the viewport.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
5.1 Finite Element Model 81
Lines and surface notch.fgc
GEOMETRY LINE STRAIGHT L1 P1 P2
GEOMETRY LINE STRAIGHT L2 P2 P3
GEOMETRY LINE STRAIGHT L3 P3 P4
GEOMETRY LINE STRAIGHT L4 P4 P5
GEOMETRY LINE STRAIGHT L5 P5 P6
GEOMETRY LINE STRAIGHT L6 P6 P1
CONSTRUCT SET LEFT APPEND LINES ALL
GEOMETRY SURFACE REGION S1 LEFT
VIEW GEOMETRY CURRENT RED
LABEL GEOMETRY LINES CURRENT BLUE
We construct successively six lines. Then, we construct a set named LEFT that
contains all the lines of the left-hand side part of the model. We display the
geometry in red with line labels in blue [Fig. 5.3a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:15 geom1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:16 mesh1.ps
Model: NOTCH Model: NOTCH
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
L5
L6 L4
L3
L2
L1
Y Y
Z X Z X
(a) geometry (b) mesh
Figure 5.3: Half the model (left part)
5.1.2 Meshing
We may now create a finite element mesh on the defined geometry.
notch.fgc
MESHING OPTIONS ALGORITHM PAVING S1
MESHING DIVISION ELSIZE ALL 5
MESHING TYPES ALL QU4 Q8MEM
MESHING DIVISION AUTOMATIC
MESHING GENERATE
VIEW MESH
We select the QU4 generic element type and the Q8MEM linear plane stress struc-
tural element for the set LEFT of the model. With the ELSIZE option we request
for an average element size of 5 mm. The PAVING meshing algorithm can create
a quadrilateral free mesh on any type of surface and thus is well suited to mesh
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
82 Discrete Cracking in a Notched Beam
the left surface of our model. We generate the mesh and display it in the default
wire netting style [Fig. 5.3b]. Note that the specified element size leads to a fine
mesh.
5.1.3 Expansion to Full Model
We may now complete the model by mirroring the surface S1 and putting in
between interface elements. In our case, the thickness of the interface is zero
and we would not be able to distinguish the two edges of the interface which is
rather inconvenient for checking connections, assigned properties and so on. To
overcome that, we will first model the two concrete parts with a virtual distance
in between and fill the gap with interface elements. Then we will close this gap
by moving the parts against each other in order to get zero thickness interface
elements.
Mirror transformation notch.fgc
GEOMETRY COPY S1 MIRROR X 250
VIEW GEOMETRY ALL VIOLET
EYE FRAME
LABEL GEOMETRY POINTS
We mirror surface S1 with respect to vertical line at X = 250 mm. Then we
display the geometry with point labels.
Filling the gap notch.fgc
GEOMETRY SURFACE 4POINTS P10 P11 P5 P4
VIEW OPTIONS SHRINK GEOMETRY 0.9
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY LINES ALL BLUE
LABEL GEOMETRY SURFACES ALL VIOLET
LABEL GEOMETRY DIVISION ALL WHITE
We fill the gap with a 4POINTS surface. We display the geometry in shrunken
style and with labels for lines, surfaces, and divisions [Fig. 5.4a].
Adding the interface notch.fgc
MESHING TYPES S3 IL22 L8IF
MESHING DIVISION AUTOMATIC
CONSTRUCT SET CRACK APPEND SURFACES S3
MESHING GENERATE
VIEW MESH
We add the crack interface for the mid-surface S3. We specify a division of
1 in the normal direction of the interface elements. We specify the element
type and apply a L8IF linear interface element to geometry S3. We create a set
CRACK which contains the interface elements. Finally, we generate and display
the mesh [Fig. 5.4b]. Note that we still have to close the gap. We will do this
after having defined and verified the material and physical properties and the
boundary conditions [§ 5.1.6].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
5.1 Finite Element Model 83
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:16 geom2.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:16 mesh3.ps
Model: NOTCH Model: NOTCH
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
L5 L13 L11
45 4 45
S3
L6 L4 L10 L12
20 10 10 20
S1 L3 L14 L9 S2
1 4 1
L2 L8
10 10
L1 L7
46 46
Y Y
Z X Z X
(a) geometry (b) mesh
Figure 5.4: Full model with interface in gap
5.1.4 Material and Physical Properties
We launch the Property Manager dialog to define the material and physical
properties of the model.
iDiana
View →Property Manager...
↑
Property Manager
···
Concrete and crack interface iDiana
Property Manager
Materials Material Name: MACONCRE
↑
↑Linear Elasticity →Isotropic
Materials Material Name: MACRACK
↑Linear Elasticity →Interfaces
↑Static Nonlinearity →Interfaces →Cracking →Discrete Cracking
→Nonlinear Tension Softening →Secant Mode-I Unloading
→Constant Shear Stiffness After Crack
We define the properties of concrete for the beam in a material instance MA-
CONCRE. For linear elasticity we specify a Young’s modulus E = 31000 MPa
and a Poisson’s ratio ν = 0.15. For the crack interfaces we define a mate-
rial instance MACRACK with linear stiffness moduli D11 = 1.0×108 N/mm3 and
D22 = 1.0×108 N/mm3 . We also specify the nonlinear material parameters for
discrete cracking in the interface: the tensile strength ft = 2.4 MPa, the fracture
energy Gf = 0.08 N/mm2 and the shear modulus after cracking Gcr = 0.001
MPa.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
84 Discrete Cracking in a Notched Beam
Thickness iDiana
Property Manager
↑Physical Properties Physical Property Name: PHCONCRE
↑Geometry →Plane Stress →Regular
Physical Properties Physical Property Name: PHCRACK
↑Interface →Line →Plane Stress
For the concrete of the beam we define a physical property instance PHCONCRE
with a thickness value t = 100 mm. For the interface elements we define a
physical property PHCRACK with a thickness also equal to t = 100 mm.
Assignment notch.fgc
PROPERTY ATTACH S1 MACONCRE PHCONCRE
PROPERTY ATTACH S2 MACONCRE PHCONCRE
PROPERTY ATTACH S3 MACRACK PHCRACK
VIEW OPTIONS EDGES OUTLINE
VIEW HIDDEN FILL COLOUR
VIEW OPTIONS COLOUR MATERIALS
VIEW MESH
VIEW OPTIONS COLOUR PHYSICAL
We assign the defined property instances to the concrete of the beam (surfaces
S1 and S2) and to the crack interface (surface S3). To verify the assignment we
display two outline views of the model with the elements colored according to
their assigned property [Fig. 5.5].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:17 meshma.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:17 meshph.ps
Model: NOTCH Model: NOTCH
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
Y Y
Z X Z X
Materials Physical
MACONCRE PHCONCRE
MACRACK PHCRACK
(a) material (b) physical
Figure 5.5: Model colored for properties assignment
5.1.5 Boundary Conditions
The boundary conditions of the model comprise the supports, the loading, and
the tyings (liner constraints). For convenience, we tie the two top nodes of the
interface and prescribe the displacement load of the master node. Doing so will
facilitate the determination of the total reaction force later on.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
5.1 Finite Element Model 85
Supports and tying notch.fgc
PROPERTY BOUNDARY CONSTRAINT P1 X Y
PROPERTY BOUNDARY CONSTRAINT P7 Y
PROPERTY BOUNDARY MPC RBEAM P11 P5 Y
VIEW HIDDEN OFF
LABEL MESH CONSTRNT
We support the lower-left corner in X- and Y -direction and the lower-right
corner in Y -direction. The supported degrees of freedom show up as red spikes
and the tying as a red line [Fig. 5.6a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:17 meshco.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:17 meshlo.ps
Model: NOTCH Model: NOTCH
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
3M 3S
Y Y
Z X Z X
(a) constraints (b) load
Figure 5.6: Boundary conditions
Load notch.fgc
PROPERTY LOADS DISPLACE P5 -1.0 Y
LABEL MESH OFF
LABEL MESH LOADS
The load corresponds to a unit displacement applied on top of the beam just
above the notch. The load appears as a violet arrow [Fig. 5.6b].
5.1.6 Moving Parts Together
Finally we connect the two parts of the concrete beam.
notch.fgc
GEOMETRY MOVE S2 TRANSLATE P11 P5
yes
MESHING GENERATE
VIEW MESH
VIEW OPTIONS SHRINK MESH 0.8
EYE ZOOM FACTOR 30 -25 5
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
86 Discrete Cracking in a Notched Beam
We close the interface by moving surface S2 on the right-hand side such that
point P11 takes the position of point P5. The geometry has now changed so we
must re-mesh the model. The display shows the final mesh [Fig. 5.7a]. To discern
the interfaces as separate lines we display the mesh in ‘shrunken elements’ mode
and zoom in on the area above the notch [Fig. 5.7b].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:18 mesh.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:18 meshz.ps
Model: NOTCH Model: NOTCH
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
Y Y
Z X Z X
(a) full mesh (b) zoomed-in on notch
Figure 5.7: Final mesh with closed interface gap
5.2 Preliminary Linear Analysis
First of all, we will perform a linear analysis in order to check the model. There-
fore, we write the just created finite element model to a file in Diana batch
format.
iDiana
UTILITY WRITE DIANA
yes
FILE CLOSE
yes
Discrete cracking of a notched beam
ANALYSE NOTCH
Analysis Setup
···
Via the Analysis Setup dialog we activate the following batch commands.
linsta.dcf
*FILOS
INITIA
*INPUT
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
5.2 Preliminary Linear Analysis 87
*LINSTA
BEGIN OUTPUT
DISPLA TOTAL TRANSL
STRESS TOTAL CAUCHY
STRESS TOTAL TRACTI INTPNT
END OUTPUT
*END
We have selected output of displacements, Cauchy stresses and tractions within
the interfaces to a database for the iDiana Results environment. After com-
pleting the analysis we enter this environment with the name of the model.
linsta.fvc
FEMVIEW LINSTA
VIEW MESH
VIEW OPTIONS EDGES OUTLINE
EYE FRAME
The VIEW and EYE commands display the outlines of the non-deformed mesh in
green.
5.2.1 Deformation
To get the deformed mesh displayed we give the following commands
linsta.fvc
RESULTS LOADCASE LC1
RESULTS NODAL DTX....G RESDTX
PRESENT SHAPE
We select load case LC1 (the only one) and result attribute RESDTX which rep-
resents the nodal displacements. We display the deformed shape of the mesh
[Fig. 5.8a]. Note that iDiana chooses a red color and an appropriate multipli-
cation factor, in this case 22×.
5.2.2 Principal Cauchy Stresses
The principal stresses in the beam may give a better understanding of the
behavior of the model.
linsta.fvc
RESULTS ELEMENT EL.SXX.G SXX
RESULTS CALCULATE P-STRESS ALL
VIEW OPTIONS EDGES MATERIALS
PRESENT OPTIONS VECTORS MODULATE 10
PRESENT VECTORS
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
88 Discrete Cracking in a Notched Beam
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:22 lidfm.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:23 lipstr.ps
Model: LINSTA Model: LINSTA
LC1: Load case 1 LC1: Load case 1
Nodal DTX....G RESDTX Element PRINC STRESS ALL
Max = 1.18 Min = 0 Calculated from: EL.SXX.G
Factor = 22.3 Max = 249 Min = -136
Factor = .106
210
172
133
Y Y 94.8
56.3
17.8
-20.7
Z X Z X -59.2
-97.7
(a) deformation (×22) (b) principal stresses
Figure 5.8: Linear analysis results in concrete
We select result attribute SXX which represents the Cauchy stresses in the el-
ement nodes. As only the primary stresses were stored, we ask iDiana to
calculate the principal stresses via the P-STRESS option. With the EDGES MA-
TERIALS view option we get the model displayed with only the material edges,
which is often more convenient than the full mesh as a background for the stress
display. Although iDiana will always display stress vectors with a size propor-
tional to the stress value, stress peaks are more convincing when the vectors
are modulated with colors according to their values as well. Therefore, we give
the VECTORS MODULATE option and ask for modulation with ten colors. Finally,
we display the stress vectors [Fig. 5.8b]. Note that the red vectors indicate
the highest tension stresses and the dark blue vectors the highest compression
stresses.
5.2.3 Interface Normal Tractions
To get the normal tractions of the interface elements displayed we give the
following commands.
linsta.fvc
RESULTS GAUSSIAN EL.STX.L STX
PRESENT VECTORS
We select result attribute STX which represents the normal traction tn of inter-
face elements. The resulting vector plot show the distribution of this traction
along the crack interface Figure 5.9.
5.3 Nonlinear Analysis
To perform the nonlinear analysis, we enter the iDiana Index environment.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
5.3 Nonlinear Analysis 89
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:23 litrac.ps
Model: LINSTA
LC1: Load case 1
Gauss EL.STX.L STX
Max = 202
Min = -163
Factor = .131
166
129
92.6
Y 56
19.5
-17
-53.5
Z X -90
-127
Figure 5.9: Linear analysis: interface normal tractions
iDiana
INDEX
ANALYSE NOTCH
Analysis Setup
···
Via the Analysis Setup dialog we create the following batch commands for the
nonlinear analysis:
nonlin.dcf
*FILOS
INITIA
*INPUT
READ
*NONLIN
BEGIN EXECUT
BEGIN ITERAT
BEGIN CONVER
SIMULT
END CONVER
END ITERAT
BEGIN LOAD
BEGIN STEPS
BEGIN AUTOMA
SIZE=1.0
MAXSIZ=0.02
MINSIZ=0.001
END AUTOMA
END STEPS
END LOAD
END EXECUT
BEGIN OUTPUT
DISPLA TOTAL TRANSL
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
90 Discrete Cracking in a Notched Beam
STRESS TOTAL CAUCHY
STRESS TOTAL TRACTI
FORCE REACTI TRANSL
END OUTPUT
*END
When the analysis is completed, we can enter the iDiana Results environment
with the model name NONLIN to assess the analysis results.
nonlin.fvc
FEMVIEW NONLIN
UTILITY TABULATE LOADCASES
The load case tabulation shows the available load cases (load steps) with their
result data. Here we only show the first and last steps of the tabulation:
nllc.tb
;
; Model: NONLIN
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; MODEL STATIC "Model Properties"
; Element : THICKNES*
;
; LC1 1 LOAD = .2E-1 "Load case 1"
; Nodal : TDTX...G FBX....G
; Element : EL.SXX.G EL.STX.L
;
; LC1 2 LOAD = .4E-1 "Load case 1"
... lines skipped
;
; LC1 49 LOAD = .98 "Load case 1"
; Nodal : TDTX...G FBX....G
; Element : EL.SXX.G EL.STX.L
;
; LC1 50 LOAD = 1 "Load case 1"
; Nodal : TDTX...G FBX....G
; Element : EL.SXX.G EL.STX.L
; * Indicates loads data
;
5.3.1 Load–Displacement Diagram
We will present a load–displacement diagram for the top center of the beam,
i.e., where we have applied the displacement load [Fig. 5.6b]. Via node labeling
and zooming we can determine that this is node 68.
nonlin.fvc
RESULTS LOADCASE LC1
RESULTS NODAL FBX....G FBY
PRESENT GRAPH NODE 68
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
5.3 Nonlinear Analysis 91
We select all load cases, these represent the displacement. We also select result
attribute FBY representing the reaction force in the nodes. These reaction forces
can be interpreted as ‘the load’ on the beam to achieve the displacement. The
graph of these values for node 68 then represents the load–displacement diagram
at the mid-span [Fig. 5.10a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:28 lodis.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:28 nlstx.ps
Model: NONLIN Model: NONLIN
Nodal FBX....G FBY Element EL.STX.L STX
Max/Min on whole graph: Max/Min on whole graph:
Ymax = .142E4 Ymax = 50 Ymin = 0
Ymin = 36.9 Xmax = 4.01 Xmin = -5.32
Xmax = 1 Variation along a line
Xmin = .2E-1 LC1 1
*1E3 Variation over loadcases LC1 50
Node 68
1.6 60
1.4
50
N
O 1.2
D
A
L 40
1 D
F I
B S
X .8 T 30
. A
. N
. C
. .6 E
G 20
F
B .4
Y
10
.2
0 0
0 .1 .2 .3 .4 .5 .6 .7 .8 .9 1 1.1 -6 -5 -4 -3 -2 -1 0 1 2 3 4 5
LOAD ELEMENT EL.STX.L STX
(a) load–displacement diagram (b) normal tractions along interface
Figure 5.10: Result graphs
5.3.2 Interface Normal Tractions
We will assess the distribution of the normal tractions along the crack interface.
nonlin.fvc
RESULTS LOADCASE LC1 1 LC1 50
RESULTS ELEMENT EL.STX.L STX
PRESENT GRAPH LINE NODES LIST 58 TO 68
PRESENT OPTIONS GRAPH AXES SWAP
We select the first and the last load step (1 and 50) and attribute STX which
represents the normal tractions of the interface. Then we display a graph of the
variation of the normal traction along a line through the nodes of the interface
[Fig. 5.10b]. To get a realistic graph we swap the axes via the SWAP option. The
distance is now along the vertical axis, i.e., in the same direction as the crack
interface. Note that the solid line is for the first step and the dashed line for
the last step.
5.3.3 Von Mises Stresses
We will assess the stresses for the first and last load step. In this case we let
iDiana calculate the equivalent Von Mises stresses.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
92 Discrete Cracking in a Notched Beam
nonlin.fvc
RESULTS LOADCASE LC1 1
RESULTS ELEMENT EL.SXX.G SXX
RESULTS CALCULATE VONMISES
PRESENT CONTOUR LEVELS
RESULTS LOADCASE LC1 50
DRAWING DISPLAY
For attribute SXX, the primary stresses, we let iDiana calculate the Von Mises
stresses. We display contour plots for the first and last load step (1 and 50)
[Fig. 5.11]. Note that the contour levels for the two steps are different: for the
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:28 nlseq1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:28 nlseq2.ps
Model: NONLIN Model: NONLIN
LC1: Load case 1 LC1: Load case 1
Step: 1 LOAD: .2E-1 Step: 50 LOAD: 1
Element VONMISES EL.SXX.G Element VONMISES EL.SXX.G
Calculated from: EL.SXX.G Calculated from: EL.SXX.G
Max = 2.91 Min = .797E-3 Max = 3.44 Min = .394E-4
2.64 3.13
2.38 2.81
2.12 2.5
1.85 2.19
Y 1.59 Y 1.88
1.32 1.56
1.06 1.25
Z X .794 Z X .938
.529 .626
.265 .313
(a) first load step (b) last load step
Figure 5.11: Nonlinear analysis: Von Mises equivalent stress
first load step the colors blue to red represent a stress range of approximately
0.0 < σeq < 2.9, for the last step the same colors represent a range of 0.0 <
σeq < 3.4.
Animation nonlin.fvc
RESULTS LOADCASE LC1
PRESENT CONTOUR FROM 0 TO 1.4 LEVELS 6
VIEW OPTIONS DEFORM USING TDTX...G RESTDT 30
UTILITY SETUP ANIMATE LINEAR
DRAWING ANIMATE LOADCASES PLOTFILE ani
We can display the development of the stress for increasing deformation in an
animation sequence. First, we select all available load cases. A proper animation
sequence with contours requires consistent color levels for the frames. Therefore,
we explicitly specify the values for the first and the last contour via the FROM
... TO option. With the DEFORM USING option the contours will be displayed
in the deformed model, here with a 30× magnification. The DRAWING ANIMATE
command starts the animation. The PLOTFILE option yields a file for each frame
so that we can show them in a document [Fig. 5.12]. Note the increasing stress in
the first six frames. This confirms the increasing load in the load–displacement
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
5.3 Nonlinear Analysis
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:29 ani001 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:29 ani002 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:29 ani003 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:29 ani004 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:29 ani005
93
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:29 ani006 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:29 ani007 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:29 ani008 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:30 ani009 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:30 ani010
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:30 ani011 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:30 ani012 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:30 ani013 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:30 ani014 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:30 ani015
DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:30 ani016 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:31 ani017 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:31 ani018 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:31 ani019 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:31 ani020
DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:31 ani021 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:31 ani022 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:31 ani023 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:31 ani024 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:31 ani025
DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:32 ani026 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:32 ani027 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:32 ani028 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:32 ani029 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:32 ani030
DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:32 ani031 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:32 ani032 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:32 ani033 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:33 ani034 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:33 ani035
DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:33 ani036 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:33 ani037 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:33 ani038 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:33 ani039 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:33 ani040
DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:33 ani041 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:33 ani042 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:34 ani043 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:34 ani044 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:34 ani045
DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:34 ani046 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:34 ani047 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:34 ani048 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:34 ani049 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:44:34 ani050
DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani
DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani
Figure 5.12: Nonlinear analysis: animation frames for Von Mises stress
DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani DRAWING ANIMATE LOADCASES PLOTFILE ani
diagram [Fig. 5.10a]. Then the crack arises, the stress decreases gradually and
is localized at the crack tip.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
94 Discrete Cracking in a Notched Beam
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
Chapter 6
Shear Failure in Reinforced
Concrete Beam
Name: Shear
Path: /Examples/ConcMas/Shear
Keywords: analys: nonlin physic. constr: suppor. elemen: bar cq16m
pstres reinfo. load: deform. materi: consta crack cutoff
elasti harden isotro linear plasti retent smear soften strain von-
mis. option: direct groups newton regula units. post: binary
femvie. result: cauchy crack displa force green increm reacti
strain stress total. analys: nonlin physic. constr: suppor.
elemen: bar cq16m pstres reinfo. load: force node. materi:
consta crack cutoff elasti harden isotro linear plasti retent smear
soften strain vonmis. option: adapti arclen direct groups loadin
newton normal regula size units update. post: binary femvie.
result: crack displa extern force green strain total.
F ♥
500
450 Y
X 30 1∅20, 2∅14
290
2050
Figure 6.1: Model of the reinforced concrete beam [mm]
This example demonstrates application of the multi–directional fixed crack model.
The model is a moderately deep beam [Fig. 6.1]. The thickness of the beam is
200 mm. In the finite element model we will apply 8-node quadrilateral plane
stress elements.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
96 Shear Failure in Reinforced Concrete Beam
6.1 Finite Element Model
To build up the finite element model, we start iDiana and we enter the Design
environment with the model name SHEAR.
iDiana
FEMGEN SHEAR
Analysis and Units
Analysis Selection
Model Type: →Structural 2D
Units Definition
Length: →Millimeter
Mass: →Kilogram
Force: →Newton
Time: →Second
Temperature: →Celsius
In the Analysis and Units dialog we specify the model type for two-dimensional
structural analysis and the adopted units [mm, kg, N, s, °C].
6.1.1 Geometry Definition
We will first define the bottom lines of the beam and then sweep these upward
to create the surface.
shear.fgc
GEOMETRY POINT COORD P1 0.0
GEOMETRY POINT COORD P2 290.0
GEOMETRY POINT COORD P3 1550.0
GEOMETRY POINT COORD P4 2050.0
GEOMETRY LINE STRAIGHT P1 P2 4
GEOMETRY LINE STRAIGHT P2 P3 26
GEOMETRY LINE STRAIGHT P3 P4 10
CONSTRUCT SET BOTLIN APPEND LINES ALL
GEOMETRY SWEEP BOTLIN TMPLIN 4 TRANSLATE TR1 0 60
GEOMETRY SWEEP TMPLIN TOPLIN 10 TRANSLATE TR2 0 390
EYE FRAME
VIEW GEOMETRY ALL GREEN
VIEW GEOMETRY +BOTLIN RED
VIEW GEOMETRY +TOPLIN BLUE
LABEL GEOMETRY POINTS
We define the coordinates of the end points of the bottom lines. Then we create
straight lines between the points while we also specify the meshing division.
We collect the lines in a set BOTLIN. We sweep (translate through space) the
set BOTLIN vertically to create surfaces. A subsequent sweep reaches to the top
line, with the new geometry assembled in a set TOPLIN. In the sweep operations
we also define the meshing division for created vertical lines. Finally we display
the geometry in green with the bottom and top lines overlayed in red and blue
[Fig. 6.2a].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
6.1 Finite Element Model 97
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:03 geom iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:03 reinf
Model: SHEAR Model: SHEAR
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
P9 P10 P11 P12
P5 P6 P7 P8
P1 P2 P3 P4
Y Y
Z X Z X
(a) sets and point labels (b) reinforcements
Figure 6.2: Geometry definition
6.1.2 Reinforcement
We define the location of the reinforcement with the following commands.
shear.fgc
GEOMETRY COPY P1 P13 TRANSLATE 0 29.9
GEOMETRY COPY P4 P14 TRANSLATE 0 29.9
REINFORCE BAR SECTION RE1 P13 P14
REINFORCE BAR BAR1 RE1
LABEL GEOMETRY OFF
VIEW GEOMETRY ALL YELLOW
VIEW REINFORCE +BAR1 RED
We copy the two bottom corner points to create the end points of the reinforce-
ment bar. Then we define the reinforcement section RE1 and the reinforcement
bar BAR1. Finally, we display the geometry in yellow with the reinforcement in
red [Fig. 6.2b].
6.1.3 Meshing
We will mesh the model with 8-node quadratic quadrilateral plane stress ele-
ments CQ16M.
shear.fgc
MESHING TYPES ALL QU8 CQ16M
MESHING GENERATE
VIEW HIDDEN SHADE
VIEW OPTIONS SHRINK MESH
VIEW MESH
VIEW HIDDEN OFF
VIEW REINFORCE +ALL RED
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
98 Shear Failure in Reinforced Concrete Beam
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:03 mesh1 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:03 mesh2
Model: SHEAR Model: SHEAR
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
Y Y
Z X Z X
(a) as generated (b) with reinforcements
Figure 6.3: Finite element mesh
We specify the element type to be applied to all surfaces as CQ16M. Then we
generate the mesh and display it in ‘filled shrunken elements’ style [Fig. 6.3a].
We also display the reinforcement in the mesh [Fig. 6.3b]. Note that this requires
an un-filled view of the mesh.
6.1.4 Material and Physical Properties
We launch the Property Manager dialog to define the material and physical
properties of the model.
iDiana
View →Property Manager...
↑
Property Manager
···
Concrete iDiana
Property Manager
↑Materials Material Name: MACONCRE
↑Linear Elasticity →Isotropic
↑Static Nonlinearity →Concrete and Brittle Materials →Multi-directional Fixed Crack
→Constant Stress Cut-off →Linear Tension Softening
→Ultimate Strain Based →Constant Shear Retention →No Plasticity
↑Physical Properties Physical Property Name: PHCONCRE
↑Geometry →Plane Stress →Regular
For the concrete we define a material instance MACONCRE. We specify the elastic
properties: Young’s modulus E = 28000 MPa and Poisson’s ratio ν = 0.2. As
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
6.1 Finite Element Model 99
nonlinear material properties we specify a tensile strength ft = 2.5 MPa, an
ultimate strain εu = 3.11×10−4 , and a constant shear retention factor β = 0.2.
We also define a physical property instance PHCONCRE with a thickness t = 200
mm.
Reinforcement iDiana
Property Manager
↑Materials Material Name: MASTEEL
↑Linear Elasticity →Reinforcement →Reinforcement Bonded
↑Static Nonlinearity →Reinforcement →Von Mises Plasticity → Ideal Plasticity
↑Physical Properties Physical Property Name: PHSTEEL
↑Geometry →Embedded Reinforcements →Bar
For the reinforcement we define a material instance MASTEEL. We specify a
Young’s modulus E = 210000 MPa and Von Mises plasticity with a yield stress
σy = 440 MPa. We also define a physical property instance PHSTEEL with a
cross-section area A = 622 mm2 .
Assignment shear.fgc
PROPERTY ATTACH ALL MACONCRE PHCONCRE
PROPERTY ATTACH BAR1 MASTEEL PHSTEEL
First we assign the properties of the concrete to the entire model. Then we
overrule the assignment for the reinforcement BAR1 with the appropriate prop-
erties.
6.1.5 Boundary Conditions
The boundary conditions involve the constraints (supports) and the loading
[Fig. 6.1].
Constraints shear.fgc
PROPERTY BOUNDARY CONSTRAINT P2 Y
PROPERTY BOUNDARY CONSTRAINT L10 X
PROPERTY BOUNDARY CONSTRAINT L17 X
LABEL MESH CONSTRNT
We define the constraints with respect to the geometric parts. The point on the
lower edge at X = 290 is supported vertically (Y -direction). Due to symmetry
conditions, the two lines of the right edge are supported horizontally. The
display confirms the correct definition [Fig. 6.4a].
Loading shear.fgc
PROPERTY LOADS DISPLACE P11 -1.0 Y
LABEL MESH OFF
LABEL MESH LOADS
The load corresponds to a vertical unit displacement of the beam top at 500
mm from the right edge [Fig. 6.4b].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
100 Shear Failure in Reinforced Concrete Beam
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:03 meshbc iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:03 meshlo
Model: SHEAR Model: SHEAR
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
Y Y
Z X Z X
(a) constraints (b) loading: fixed displacement
Figure 6.4: Boundary conditions
6.2 Nonlinear Analysis
We write the model to a file in Diana batch format and leave the iDiana Design
environment.
iDiana
UTILITY WRITE DIANA sheard.dat
FILE CLOSE
yes
Shear failure in reinforced concrete beam (displacement control)
ANALYSE SHEAR
Analysis Setup
···
The FILE CLOSE command brings us in the Index environment where we launch
the Analysis Setup dialog. Here we create the following batch commands for
the displacement-controlled nonlinear analysis:
sheard.dcf
*FILOS
INITIA
*INPUT
*NONLIN
BEGIN EXECUT
BEGIN LOAD
LOADNR=1
STEPS EXPLIC SIZES 1(15)
END LOAD
END EXECUT
BEGIN OUTPUT
DISPLA TOTAL TRANSL
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
6.2 Nonlinear Analysis 101
DISPLA INCREM TRANSL
FORCE REACTI TRANSL
STRESS TOTAL CAUCHY GLOBAL INTPNT
STRAIN CRACK GREEN
END OUTPUT
*END
We start the analysis and when it is completed we enter the iDiana Results
environment to assess the analysis results.
iDiana
FEMVIEW SHEARD
6.2.1 Load–Displacement Diagram
We will present a diagram of the load versus the displacement for the node on
top of the beam where the load has been applied. Therefore we need to know
the number of this node.
Node number sheard.fvc
VIEW MESH
LABEL MESH CONSTRNTS
LABEL MESH NODES
EYE ZOOM /CURSOR
We label the constraints and the node numbers on the mesh [Fig. 6.5a]. When
we drag a zoom window around the appropriate node on the top edge, the node
appears to be number 266 [Fig. 6.5b].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:12 meshf iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:12 meshz
Model: SHEARD Model: SHEARD
166 186 171 196 176271206281211291216301221311226321231331236341241351246361251371256381261391266426401436406446411456416466421
181 191 201 276 286 296 306 316 326 336 346 356 366 376 386 396 431 441 451 461 471
167 187 172 197 177272207282212292217302222312227322232332237342242352247362252372257382262392267427402437407447412457417467422
182 192 202 277 287 297 307 317 327 337 347 357 367 377 387 397 432 442 452 462 472
168 188 173 198 178273208283213293218303223313228323233333238343243353248363253373258383263393268428403438408448413458418468423
183 193 203 278 288 298 308 318 328 338 348 358 368 378 388 398 433 443 453 463 473
169 189 174 199 179274209284214294219304224314229324234334239344244354249364254374259384264394269429404439409449414459419469424
184 194 204 279 289 299 309 319 329 339 349 359 369 379 389 399 434 444 454 464 474
170 190 175 200 180275210285215295220305225315230325235335240345245355250365255375260385265395270430405440410450415460420470425
185 195 205 280 290 300 310 320 330 340 350 360 370 380 390 400 435 445 455 465 475 381 261 391 266 426 401 436
1
10 12 15
4 7 61 64
17 20 28 76 79
25 71 74
22 66 69 34 86 89
31 81 84 40 96 99
37 91 94 49 111114
46 106109
43 101104 55 121124
52 116119 144146
58 141126 149151
129 154156
132 159161
135 138
164
476
2
11 13 477
5 18 478
8 62 479
23 67 480
26 72 481
29 77 482
32 82 483
35 87 484
38 92 485
41 97 486
44 102487
47 107488
50 112489
53 117490
56 122491
59 142492
127147493
130152494
133157495
136162496
139
3 14 16
6 24 68 70
9 63 65
19 21 33 83 85
30 78 80
27 73 75 39 93 95
36 88 90 45 103105
42 98 100 51 113115
48 108110 57 123125
54 118120 145148
60 143128 150153
131 155158
134 160163
137 165
140
386 396 431
Y Y
382 262 392 267 427 402 437
Z X Z X
(a) full display (b) zoom-in
Figure 6.5: Mesh with labeled node numbers
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
102 Shear Failure in Reinforced Concrete Beam
Diagram sheard.fvc
RESULTS LOADCASE LC1
RESULTS NODAL FBX....G FBY
PRESENT GRAPH NODE 266
We select all available load cases (steps) and choose result attribute FBY which
represents the reaction forces in the node. The PRESENT command displays the
load–displacement diagram for node 266 [Fig. 6.6]. Note that the horizontal axis
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:12 lodis
Model: SHEARD
Nodal FBX....G FBY
Max/Min on whole graph:
Ymax = .864E5
Ymin = .251E5
Xmax = 15
Xmin = 1
*1E4 Variation over loadcases
Node 266
9
8
N
O
D 7
A
L
F 6
B
X
.
. 5
.
.
G
F 4
B
Y
3
2
0 2 4 6 8 10 12 14 16
LOAD
Figure 6.6: Load–displacement diagram
of the graph represents the ‘load factor’ which is equivalent to the multiplica-
tion factor for the applied vertical unit displacement. The load–displacement
diagram shows a discontinuity at step 8. Presumably this indicates the point of
yielding of the reinforcement.
6.2.2 Reinforcement Stresses
We will check the stresses along the reinforcement. Therefore we need to know
the numbers of the elements that represent the reinforcement bar.
Element numbers sheard.fvc
VIEW MESH
EYE FRAME ALL
LABEL MESH OFF
LABEL MESH ELEMENT VIEWMODE RED
We display a general view of the mesh and remove the existing labels. Then we
label the mesh with element numbers [Fig. 6.7]. The reinforcement bar appears
to be represented by element numbers 141 to 160.
Stress distribution sheard.fvc
RESULTS LOADCASE LC1 8 9
RESULTS GAUSSIAN RE.SXX.G SXX
PRESENT GRAPH LINE ELEMENT LIST 141 TO 160
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
6.2 Nonlinear Analysis 103
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:12 meshel
Model: SHEARD
41 46 51 56 61 66 71 76 81 86 91 96 101 106 111 116 121 126 131 136
42 47 52 57 62 67 72 77 82 87 92 97 102 107 112 117 122 127 132 137
43 48 53 58 63 68 73 78 83 88 93 98 103 108 113 118 123 128 133 138
44 49 54 59 64 69 74 79 84 89 94 99 104 109 114 119 124 129 134 139
45 50 55 60 65 70 75 80 85 90 95 100 105 110 115 120 125 130 135 140
1
141 3
142 5
143 7
144 9
145 11
146 13
147 15
148 17
149 19
150 21
151 23
152 25
153 27
154 29
155 31
156 33
157 35
158 37
159 39
160
2 4 6 8 10 12 14 16 18 20 22 24 26 28 30 32 34 36 38 40
Z X
Figure 6.7: Element numbers
We plot the stress distribution in the reinforcement for the moment of yielding
and just beyond, i.e., for steps 8 and 9. We select the result attribute RE.SXX
which represents the axial stress in the reinforcement bar. Then we display the
distribution of the reinforcement stress along the line from element 141 to 160
[Fig. 6.8a]. Note that for step 8 (solid line) the maximum stress σmax ≈ 400
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:12 resig iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:12 repla
Model: SHEARD Model: SHEARD
Gauss RE.SXX.G SXX LC1: Load case 1
Max/Min on whole graph: Step: 9 LOAD: 9
Ymax = 440 Gauss RE.SXX.G SXX
Ymin = -.376 Max = 440
Xmax = .193E4 Min = -5.74
Xmin = 0 Results shown:
Variation along a line Mapped to nodes
Mean value used for each element
450 LC1 8
LC1 9
400
G
A 350
U
S
S 300
I
A
N 250
R
E 200
.
S
X 150
X
.
G 100
S 50
X
X
0
0 .2 .4 .6 .8 1 1.2 1.4 1.6 1.8 2
-50 *1E3
DISTANCE
Y
Z X
435
(a) stress distribution (b) plastic zone
Figure 6.8: Stress in reinforcement
MPa which is less than the yield stress σy , but for load case 9 (dotted line)
σmax = σy = 440 MPa. Of course we can also display the stress distribution
in a contour plot, this will confirm the distribution as presented by the graph.
However, here we will apply a contour plot to show the plastic zone in the
reinforcement.
Plastic zone sheard.fvc
LABEL MESH OFF
VIEW OPTIONS EDGES OUTLINE
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
104 Shear Failure in Reinforced Concrete Beam
RESULTS LOADCASE LC1 9
PRESENT CONTOUR VALUES 435
First we display an outline view of the model without element numbers. We
select step 9 and draw a contour plot with one value 435 which is just below the
yield stress σy . In this case iDiana will display the zone where σ ≥ σy in red
[Fig. 6.8b]. This clearly indicates the plastic zone. The elastic zone is displayed
in blue.
6.2.3 Crack Development
We will assess the crack pattern for a specific step and as an animation.
Crack pattern for step sheard.fvc
RESULTS LOADCASE LC1 9
RESULTS GAUSSIAN EL.EKNN1 EKNN
PRESENT DISC 0.3
VIEW OPTIONS DEFORM USING TDTX...G RESTDT 10
We select step 9 and result attribute EL.EKNN which represents the normal crack
strains εcr
nn . With the DISC option we display the crack pattern. With the
DEFORM option the cracks are presented on the deformed model, in this case for
the total displacement with a 10× magnification [Fig. 6.9].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:12 crack
Model: SHEARD
Deformation = 10
LC1: Load case 1
Step: 9 LOAD: 9
Gauss EL.EKNN1 EKNN
Max = .401E-2
Min = -.336E-4
Z X 0
435
Figure 6.9: Crack pattern for step 9
Animation sheard.fvc
RESULTS LOADCASE LC1
DRAWING ANIMATE LOADCASE PLOTFILE ancr
We can display the development of the cracks for increasing deformation in
an animation sequence. Therefore we select all steps. The DRAWING ANIMATE
command starts the animation. The PLOTFILE option yields a file for each frame
so that we can show them in a document [Fig. 6.10].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
6.3 Force-Controlled Analysis
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:12 ancr001
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:12 ancr002
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:12 ancr003
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:12 ancr004
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:12 ancr005
105
Model: SHEARD Model: SHEARD Model: SHEARD Model: SHEARD Model: SHEARD
Deformation = 10 Deformation = 10 Deformation = 10 Deformation = 10 Deformation = 10
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Step: 1 LOAD: 1 Step: 2 LOAD: 2 Step: 3 LOAD: 3 Step: 4 LOAD: 4 Step: 5 LOAD: 5
Gauss EL.EKNN1 EKNN Gauss EL.EKNN1 EKNN Gauss EL.EKNN1 EKNN Gauss EL.EKNN1 EKNN Gauss EL.EKNN1 EKNN
Max = .165E-3 Max = .105E-2 Max = .164E-2 Max = .216E-2 Max = .261E-2
Min = 0 Min = 0 Min = 0 Min = 0 Min = 0
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:13 ancr006
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:13 ancr007
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:13 ancr008
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:13 ancr009
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:13 ancr010
Model: SHEARD Model: SHEARD Model: SHEARD Model: SHEARD Model: SHEARD
Deformation = 10 Deformation = 10 Deformation = 10 Deformation = 10 Deformation = 10
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Step: 6 LOAD: 6 Step: 7 LOAD: 7 Step: 8 LOAD: 8 Step: 9 LOAD: 9 Step: 10 LOAD: 10
Gauss EL.EKNN1 EKNN Gauss EL.EKNN1 EKNN Gauss EL.EKNN1 EKNN Gauss EL.EKNN1 EKNN Gauss EL.EKNN1 EKNN
Max = .301E-2 Max = .339E-2 Max = .373E-2 Max = .401E-2 Max = .457E-2
Min = 0 Min = 0 Min = 0 Min = -.336E-4 Min = 0
Y Y Y Y Y
Z 9.4.3-02
iDIANA X : TNO Diana BV 0
28 OCT 2010 01:57:13 ancr011
iDIANA Z9.4.3-02
X : TNO Diana BV 28 OCT 2010 01:57:13 ancr012
iDIANA Z X : TNO Diana BV
0 9.4.3-02 28 OCT 2010 01:57:13 ancr013 Z
iDIANA0 9.4.3-02X : TNO Diana BV Z
iDIANA 09.4.3-02
28 OCT 2010 01:57:13 ancr014 X
: TNO Diana BV 28 OCT 2010 01:57:13 ancr015 0
435 435 435 435 435
Model: SHEARD Model: SHEARD Model: SHEARD Model: SHEARD Model: SHEARD
Deformation = 10 Deformation = 10 Deformation = 10 Deformation = 10 Deformation = 10
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Step: 11 LOAD: 11 Step: 12 LOAD: 12 Step: 13 LOAD: 13 Step: 14 LOAD: 14 Step: 15 LOAD: 15
Gauss EL.EKNN1 EKNN DRAWING ANIMATE LOADCASE PLOTFILE ancr Gauss EL.EKNN1 EKNN DRAWING ANIMATE LOADCASE PLOTFILE ancr Gauss EL.EKNN1 EKNN DRAWING ANIMATE LOADCASE PLOTFILE ancr Gauss EL.EKNN1 EKNN DRAWING ANIMATE LOADCASE PLOTFILE ancr Gauss EL.EKNN1 EKNN DRAWING ANIMATE LOADCASE PLOTFILE ancr
Max = .592E-2 Max = .793E-2 Max = .921E-2 Max = .101E-1 Max = .117E-1
Min = 0 Min = 0 Min = 0 Min = 0 Min = 0
Y Y Y Y Y
Z X 0 Z X 0 Z X 0 Z X 0 Z X 0
435 435 435 435 435
DRAWING ANIMATE LOADCASE PLOTFILE ancr DRAWING ANIMATE LOADCASE PLOTFILE ancr DRAWING ANIMATE LOADCASE PLOTFILE ancr DRAWING ANIMATE LOADCASE PLOTFILE ancr DRAWING ANIMATE LOADCASE PLOTFILE ancr
Y Y Y Y Y
Z X 0 Z X 0 Z X 0 Z X 0 Z X 0
435 435 435 435 435
Figure 6.10: Animation frames for crack development
DRAWING ANIMATE LOADCASE PLOTFILE ancr DRAWING ANIMATE LOADCASE PLOTFILE ancr DRAWING ANIMATE LOADCASE PLOTFILE ancr DRAWING ANIMATE LOADCASE PLOTFILE ancr DRAWING ANIMATE LOADCASE PLOTFILE ancr
6.3 Force-Controlled Analysis
We will now investigate the behavior of the same model in a force-controlled
analysis rather than a displacement-controlled analysis.
6.3.1 Creating a Force Load
We must replace the displacement load uY = −1 mm by a force load FY = −10
kN. Therefore we open the model in the Design environment.
shear.fgc
FEMGEN SHEAR
UTILITY DELETE LOADS ALL
yes
PROPERTY LOADS FORCE P11 -1.0E+4 Y
VIEW MESH
LABEL MESH LOADS
UTILITY WRITE DIANA shearf.dat
yes
First we delete all loads on the model. Then we apply a force load on the
appropriate point and display the load on the mesh [Fig. 6.11]. Finally we write
the model to a new data file in Diana batch format.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:03 meshlo2
Model: SHEAR
Analysis: DIANA
Model Type: Structural 2D
Z X
Figure 6.11: Loading for force-controlled analysis
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
106 Shear Failure in Reinforced Concrete Beam
iDiana
FILE CLOSE
yes
Shear failure in reinforced concrete beam (force control)
ANALYSE SHEAR
Analysis Setup
···
6.3.2 Nonlinear Analysis
To perform the analysis we apply an automatic adaptive load increment based on
the number of iterations in combination with the Arc-length iteration method.
The upper limit of the step size could be set to 0.25 with a factor γ = 0.25.1
With such parameter values, the number of steps could be set to 100. As
output results, we choose the total displacements, the external forces, and the
crack strains. These options could yield the following command file.
shearf.dcf
*FILOS
INITIA
*INPUT
READ
*NONLIN
BEGIN EXECUT
BEGIN LOAD
LOADNR=1
BEGIN STEPS
BEGIN ITERAT
ARCLEN
GAMMA=0.25
MAXSIZ=0.25
NSTEPS=100
END ITERAT
END STEPS
END LOAD
ITERAT MAXITE=50
END EXECUT
BEGIN OUTPUT
DISPLA TOTAL TRANSL
FORCE EXTERN TRANSL
STRAIN CRACK GREEN
END OUTPUT
*END
1 For more information, see Volume Analysis Procedures of the Diana User’s Manual:
‘Iteration Based Adaptive Loading’ in Chapter Nonlinear Analysis.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
6.3 Force-Controlled Analysis 107
After the job has been terminated, we check the convergence of the analysis
process via the output messages of which the last ones are:
shearf.out
STEP 46 TERMINATED, CONVERGENCE AFTER 1 ITERATION
STEP 47 TERMINATED, CONVERGENCE AFTER 1 ITERATION
STEP 48 TERMINATED, NO CONVERGENCE AFTER 50 ITERATIONS
Obviously, the last load step did not converge. Presumably this indicates that
the structure has collapsed, i.e., it has reached the Ultimate Limit State. We
enter the iDiana Results environment to assess the analysis results.
iDiana
FEMVIEW SHEARF
6.3.3 Load–Displacement Diagram
We check the overall behavior of the force-controlled analysis via the load–
displacement diagram.
shearf.fvc
RESULTS LOADCASE LC1
RESULTS NODAL TDTX...G TDTY
PRESENT GRAPH NODE 266
PRESENT OPTIONS GRAPH AXES SWAP
The load cases (steps) now represent the real load in vertical direction. Result
attribute TDTY represents the vertical displacements. We display the load–
displacement diagram for the loading point. We swap the axes to get the
displacements along the horizontal axis and the load along the vertical axis
[Fig. 6.12]. Note that the displacements are negative (−Y ) and thus the graph
is to be read from right to left. The dip at the end of the graph indicates that
the structure has indeed reached its Ultimate Limit State.
6.3.4 Ultimate Limit State
To assess the Ultimate Limit State we will display the crack pattern and the
crack strain distribution.
Crack pattern shearf.fvc
RESULTS LOADCASE LC1 47
RESULTS GAUSSIAN EL.EKNN1 EKNN
PRESENT DISC 0.3
We select the last step that has converged and the normal crack strain εcr
nn . We
display the crack pattern via the DISC option [Fig. 6.13a].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
108 Shear Failure in Reinforced Concrete Beam
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:52 lodis2
Model: SHEARF
Nodal TDTX...G TDTY
Max/Min on whole graph:
Ymax = 8.27
Ymin = .25
Xmax = -.821E-1
Xmin = -9.28
Variation over loadcases
Node 266
9
L 5
O
A
D 4
0
-10 -9 -8 -7 -6 -5 -4 -3 -2 -1 0
NODAL TDTX...G TDTY
Figure 6.12: Load–displacement diagram
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:52 crack2 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:52 creps2
Model: SHEARF Model: SHEARF
LC1: Load case 1 Deformation = 10
Step: 47 LOAD: 8.27 LC1: Load case 1
Gauss EL.EKNN1 EKNN Step: 47 LOAD: 8.27
Max = .497E-2 Gauss EL.EKNN1 EKNN
Min = 0 Max = .497E-2
Min = 0
Results shown:
Mapped to nodes
.452E-2
.407E-2
.361E-2
.316E-2
Y Y .271E-2
.226E-2
.181E-2
Z X Z X .136E-2
.331E-2 .904E-3
.166E-2 .452E-3
(a) crack pattern (b) crack strain
Figure 6.13: Ultimate Limit State
Crack strain shearf.fvc
PRESENT CONTOUR LEVELS
VIEW OPTIONS DEFORM USING TDTX...G RESTDT 10
To gain an insight into the true value of the crack strain we display a contour
plot in a deformed mesh (10×) [Fig. 6.13b]. The results monitor indicates that
the maximum crack strain εcr nn is approximately equal to 0.005. Note that un-
cracked areas do not have crack strain and therefore remain empty.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
Chapter 7
Shear Wall Panel
Name: Panel
Path: /Examples/ConcMas/Panel
Keywords: analys: linear static. constr: suppor. elemen: cq16m grid
pstres reinfo taper. load: deform edge elemen force. materi:
consta crack elasti harden isotro multil plasti rotati soften strain
totstr vonmis work. option: direct groups units. post: bi-
nary femvie. pre: append femgen. result: cauchy displa
extern force green reacti strain stress total. analys: nonlin
physic. constr: suppor. elemen: cq16m grid pstres reinfo
taper. load: deform edge elemen force. materi: consta crack
elasti harden isotro multil plasti rotati soften strain totstr von-
mis work. option: direct groups newton regula units. post:
binary femvie. pre: append femgen. result: cauchy crack
displa force green plasti princi reacti status strain stress total.
analys: nonlin physic. constr: suppor. elemen: cq16m grid
pstres reinfo taper. load: deform edge elemen force. materi:
consta crack elasti harden isotro multil plasti rotati soften strain
totstr vonmis work. option: direct groups newton regula units.
post: binary femvie. pre: append femgen. result: cauchy
crack displa force green plasti princi reacti status strain stress
total.
This example presents the building and analysis of a finite element model of a
shear wall panel [Fig. 7.1]. The panel has been tested experimentally by Maier
and Thürliman [9]. It will be modeled using plane stress elements and adopting
the Total Strain based rotating crack model as constitutive material behav-
ior. First we will build and check the model. Then we will subjected it to a
monotonic load and finally, as an option, to a cyclic load.
7.1 Finite Element Model
To build up the finite element model we start iDiana and enter the Design
environment with the model name PANEL.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
110 Shear Wall Panel
u 240
ρy
ρx ρf
1200
Y
B X B
380
A A–A
1700 700
260 100 980 100 260
150
100
400
150
B–B
Figure 7.1: Geometric model of the shear wall panel
iDiana
FEMGEN PANEL
Analysis and Units
Analysis Selection
Model Type: →Structural 2D
Units Definition
Length: →Millimeter
Mass: →Kilogram
Force: →Newton
Time: →Second
Temperature: →Celsius
In the Analysis and Units dialog we specify that this is a model for two-dimen-
sional structural analysis. We also indicate the adopted units [mm, kg, N, s,
°C].
7.1.1 Geometry Definition
We will first define the two-dimensional square, also know as ‘the workbox’,
where the model is going to be build. Then we will subsequently define the
panel and the beam along the top. Note that the beam along the bottom will
not be modeled, it is considered as a rigid support for the panel.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
7.1 Finite Element Model 111
Workbox panel.fgc
CONSTRUCT SPACE WORK-BOX 1440 1440 -260 0
EYE FRAME WORK-BOX
For this model we choose the XY -axes as shown in Figure 7.1. Then the X-
coordinates of the model vary from −260 to 1440 and the Y -coordinates from
0 to 1440. With the WORK-BOX option we specify these coordinate limits and
frame the display to it.
Panel bottom panel.fgc
GEOMETRY POINT COORD P1 0 0
GEOMETRY POINT COORD P2 100 0
GEOMETRY POINT COORD P3 590 0
GEOMETRY POINT COORD P4 1080 0
GEOMETRY POINT COORD P5 1180 0
GEOMETRY POINT COORD P6 0 1200
GEOMETRY LINE STRAIGHT L1 P1 P2 4
GEOMETRY LINE STRAIGHT L2 P2 P3 10
GEOMETRY LINE STRAIGHT L3 P3 P4 10
GEOMETRY LINE STRAIGHT L4 P4 P5 4
CONSTRUCT SET BOTTOM APPEND LINES ALL
VIEW GEOMETRY BOTTOM VIOLET
VIEW GEOMETRY +P6 BLUE
We define the coordinates of points P1 to P5 at the bottom of the panel. We also
define a point P6 at the top-left corner of the panel. Then we define straight
lines between the points along the bottom of the model. Note that we also
specify the meshing division for each line. We collect all lines in a set BOTTOM
which we display in violet [Fig. 7.2a]. We also display the top-point in blue.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:58 geom1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:58 geom2.ps
Model: PANEL Model: PANEL
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
4 10 10 4
20 20 20 20 20
Y Y
Z X Z X
4 10 10 4
(a) bottom lines (b) swept for surfaces
Figure 7.2: Definition of the panel geometry
Panel sweep panel.fgc
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
112 Shear Wall Panel
GEOMETRY SWEEP BOTTOM SE1 20 TRANSLATE TR1 P1 P6
CONSTRUCT SET WALL APPEND SURFACES ALL
VIEW GEOMETRY WALL BLUE
LABEL GEOMETRY DIVISIONS
We sweep the lines in set BOTTOM upward over the distance from point P1 to
point P6. Simultaneously we specify the meshing division as 20. We collect
all surfaces in a set WALL which we display in blue [Fig. 7.2b]. We label this
geometry display with the applied meshing divisions.
Upper beam panel.fgc
GEOMETRY POINT COORD P11 0 1320
GEOMETRY POINT COORD P12 0 1440
GEOMETRY POINT COORD P13 -260 1200
GEOMETRY POINT COORD P14 1440 1200
CONSTRUCT SET OPEN BEAMUP
CONSTRUCT SET APPEND L5 L6 L7 L8
GEOMETRY LINE STRAIGHT L14 P13 P6
GEOMETRY LINE STRAIGHT L15 P10 P14
GEOMETRY SWEEP BEAMUP SE2 2 TRANSLATE TR2 P6 P11
GEOMETRY SWEEP L20 L29 2 TRANSLATE TR3 P11 P12
GEOMETRY SWEEP L16 L32 2 TRANSLATE TR4 P11 P12
GEOMETRY SWEEP L17 L34 2 TRANSLATE TR5 P11 P12
GEOMETRY SWEEP L18 L36 2 TRANSLATE TR6 P11 P12
GEOMETRY SWEEP L19 L38 2 TRANSLATE TR7 P11 P12
GEOMETRY SWEEP L21 L40 2 TRANSLATE TR8 P11 P12
CONSTRUCT SET CLOSE
VIEW OPTIONS SHRINK GEOMETRY 0.8
VIEW GEOMETRY BEAMUP ORANGE
LABEL GEOMETRY LINES CURRENT WHITE
DRAWING CONTENTS MONITOR OFF
To model the upper beam we define additional points P11 to P14. We create a
new set BEAMUP to contain all geometric parts of the upper beam. We define
the bottom line of the beam: the four lines along the border between the panel
and the beam and two new lines L14 and L15 at the left and right ends. Then
we sweep these lines upward over half the height of the beam (to point P11). A
series of sweeps until the top of the beam (to point P12) completes the beam
geometry. We display the geometry of the upper beam with line labels [Fig. 7.3a].
Due to the shrunken style we can easily discern the points, lines, and surfaces.
Note that we remove the monitor because it overlaps the geometry. For the
forthcoming definition of constraints and loads it is useful to collect various
parts of the model in sets of which we already have BOTTOM and BEAMUP. We
will now create another set for the top line of the beam.
Sets panel.fgc
CONSTRUCT SET TOP APPEND L29 L32 L34 L36 L38 L40
VIEW GEOMETRY ALL VIOLET
VIEW GEOMETRY +BEAMUP ORANGE
VIEW GEOMETRY +BOTTOM GREEN
VIEW GEOMETRY +TOP BLUE
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
7.1 Finite Element Model 113
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:58 geom3.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:58 geom4.ps
L29 L32 L34 L36 L38 L40 P21 P12 P22 P23 P24 P25 P26
S11 S12 S13 S14 S15 S16
L30 L31 L33 L35 L37 L39 L41
L20 L16 L17 L18 L19 L21 P19 P11 P15 P16 P17 P18 P20
S9 S5 S6 S7 S8 S10
L27 L22 L23 L24 L25 L26 L28
L14 L5 L6 L7 L8 L15 P13 P6 P7 P8 P9 P10 P14
S1 S2 S3 S4
Y Y
Z X Z X P1 P2 P3 P4 P5
(a) upper beam with line labels (b) complete geometry with labels
Figure 7.3: Finishing the geometry
LABEL GEOMETRY POINTS
LABEL GEOMETRY SURFACES ALL WHITE
We collect the lines along the top of the beam in a set TOP. To check the
geometry and the sets we display the full geometry in violet overlapped with
the sets in various colors [Fig. 7.3b]. We add point and surface labels which are
useful in forthcoming definitions of reinforcements, materials etc.
7.1.2 Reinforcement
We will now specify the reinforcement grids in the shear wall.
panel.fgc
REINFORCE GRID SECTION REIWAL P1 P5 P10 P6
REINFORCE GRID REIFOR REIWAL
REINFORCE GRID SECTION REISE1 P1 P2 P7 P6
REINFORCE GRID SECTION REISE2 P4 P5 P10 P9
REINFORCE GRID REIFL1 REISE1
REINFORCE GRID REIFL2 REISE2
REINFORCE SET REIFLA APPEND REIFL1 REIFL2
LABEL GEOMETRY OFF
VIEW GEOMETRY ALL YELLOW
VIEW REINFORCE +REIWAL BLUE
VIEW REINFORCE +REIFLA RED
We specify the grid sections via their corner points. We define a grid REIFOR
for the panel. We define two grids for the flanges: REIFL1 and REIFL2 which we
collect in a grid set REIFLA. We display the grid for the panel in blue and the
grids for the flanges in red over a geometry displayed in yellow [Fig. 7.4].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
114 Shear Wall Panel
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:59 reinf.ps
Z X
Figure 7.4: Reinforcement in geometry
7.1.3 Meshing
We will mesh the model with 8-node quadratic quadrilateral plane stress ele-
ments CQ16M.
panel.fgc
MESHING TYPES ALL QU8 CQ16M
MESHING GENERATE
VIEW HIDDEN SHADE
VIEW OPTIONS SHRINK MESH 0.9
VIEW MESH
VIEW HIDDEN OFF
VIEW REINFORCE +REIWAL BLUE
VIEW REINFORCE +REIFLA RED
We specify the element type to be applied to all surfaces as CQ16M. Then we
generate the mesh and display it in ‘filled shrunken elements’ style [Fig. 7.5a].
We also display the reinforcement in the mesh [Fig. 7.5b]. Note that this requires
an un-filled view of the mesh.
7.1.4 Material and Physical Properties
We will specify the material properties [Table 7.1] and the physical properties
[Fig. 7.1] for the model. Therefore we launch the Property Manager dialog.
iDiana
View →Property Manager...
↑
Property Manager
···
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
7.1 Finite Element Model 115
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:59 mesh1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:59 mesh2.ps
Y Y
Z X Z X
(a) as generated (b) with reinforcement grids
Figure 7.5: Finite element mesh
Table 7.1: Material parameters
Young’s modulus E 30000 N/mm2
Poisson’s ratio ν 0.15
Concrete Tensile strength ft 2.2 N/mm2
Ultimate tensile strain εcrk
ult 0.0014
Compressive strength fc 27.5 N/mm2
Young’s modulus E 200000 N/mm2
Reinforcement Yield strength fsy 574 N/mm2
Hardening modulus Esy 8000 N/mm2
Concrete material iDiana
Property Manager
Materials Material Name: CONLIN
↑
↑Linear Elasticity →Isotropic
Materials Material Name: CON
↑Linear Elasticity →Isotropic
↑Static Nonlinearity →Concrete and Brittle Materials →Total Strain Rotating Crack
→Direct Input →Multi-lin. Diag. in Tension
→Ideal in Compression →No lateral confinement behav.
→No lateral cracking reduction →No Poisson reduction
We consider the upper beam to be linear elastic: we define a material instance
CONLIN with Young’s modulus E = 30000 and Poisson’s ratio ν = 0.15. For the
concrete in the panel we define a material instance CON with the same elastic
properties: E = 30000 and ν = 0.15. For nonlinearity in the panel we choose
the Total Strain Rotating Crack model with a compressive strength fc = 27.5.
We specify the stress–strain diagram on an external file multln.dat.
multln.dat
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
116 Shear Wall Panel
TENPAR 2.2 0.0 0.0 0.0014
Concrete thickness iDiana
Property Manager
↑Physical Properties Physical Property Name: BEAMTH
↑Geometry →Plane Stress →Regular
Physical Properties Physical Property Name: FLTH
↑Geometry →Plane Stress →Regular
Physical Properties Physical Property Name: WALLTH
↑Geometry →Plane Stress →Regular
We define the various thicknesses of the concrete: for the beam an instance
BEAMTH with a thickness of 700, for the flanges an instance FLTH with a thickness
of 400, and for the panel an instance WALLTH with a thickness of 100.
Reinforcement grids iDiana
Property Manager
↑Materials Material Name: STEEL
↑Linear Elasticity →Reinforcement →Reinforcement Bonded
↑Static Nonlinearity →Reinforcement →Von Mises Plasticity → Work Hardening Diag.
↑Physical Properties Physical Property Name: REFL
↑Geometry →Embedded Reinforcements →Grid
Physical Properties Physical Property Name: REWA
↑Geometry →Embedded Reinforcements →Grid
For the reinforcement steel we define a material STEEL with a Young’s modulus
E = 200000 and Von Mises plasticity with a work hardening diagram from an
external file hardia.dat.
hardia.dat
HARDIA 5.74000E+02 0.00000E+00 85.74000E+02 1.0
Next we specify the thickness for the reinforcement grids. For the flanges we
define a property instance REFL with an equivalent thickness of 4.64 in the y-
direction (vertical). For the panel we define a property instance REWA with
an equivalent thickness of 1.03 in the x-direction (horizontal) and 1.16 in the
y-direction (vertical). Note that we must ensure that the local x-direction co-
incides with the global X-direction by checking the X-axis components in the
dialog window.
Assignment panel.fgc
PROPERTY ATTACH BEAMUP CONLIN BEAMTH
PROPERTY ATTACH WALL CON
PROPERTY ATTACH S1 FLTH
PROPERTY ATTACH S4 FLTH
PROPERTY ATTACH S2 WALLTH
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
7.1 Finite Element Model 117
PROPERTY ATTACH S3 WALLTH
VIEW HIDDEN SHADE
VIEW MESH
VIEW OPTIONS COLOUR MATERIALS
VIEW OPTIONS COLOUR PHYSICAL
PROPERTY ATTACH REIFOR STEEL REWA
PROPERTY ATTACH REIFLA STEEL REFL
We assign the material and physical properties to the various geometrical parts
and reinforcement grids of the model. For the geometry we check the assignment
via a colored display of the mesh [Fig. 7.6].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:59 meshma.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:59 meshph.ps
Y Y
Z X Z X Physical
Materials FLTH
CON WALLTH
CONLIN BEAMTH
(a) material (b) thickness
Figure 7.6: Property assignment for mesh
7.1.5 Boundary Conditions
The boundary conditions involve the constraints (supports) and the loading
[Fig. 7.1].
Constraints panel.fgc
PROPERTY BOUNDARY CONSTRAINT CO1 BOTTOM PINNED
VIEW HIDDEN OFF
LABEL MESH CONSTRNT
We apply constraints at the bottom of the geometry: the PINNED option indicates
a support in X- and Y -direction. We display the supports on the mesh [Fig. 7.7-
a].
Loads panel.fgc
PROPERTY LOADS PRESSURE LO1 1 TOP -366.95 Y
PROPERTY LOADS DISPLACE LO2 2 P16 1 X
LABEL MESH OFF
LABEL MESH LOADS
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
118 Shear Wall Panel
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:49:59 meshco.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:50:00 meshlo.ps
Y Y
Z X Z X
(a) constraints (b) loads
Figure 7.7: Boundary constraints
We apply two loads: a vertical pressure on the top of the beam and a horizontal
displacement of the beam center. The total vertical load is 433 kN, we distribute
this over the width of the model which results in 366.95 N/mm. It is important
that both loads are defined in different load cases. Here we specify the pressure
in load case 1 and the displacement in load case 2. We display both load cases
on the mesh [Fig. 7.7b].
7.2 Preliminary Linear Analysis
In order to check the model, we will run a linear analysis. By default the two
load cases are applied separately and nonlinearities will not be considered at
first. We write the model to a file panel.dat in Diana batch format.
iDiana
UTILITY WRITE DIANA
FILE CLOSE
yes
Shear Wall Panel
ANALYSE PANEL
Analysis Setup
···
Prior to the actual analysis we will change the integration scheme of the CQ16M
elements: for this model we prefer a 3×3 integration instead of the default 2×2
scheme. We specify the customized integration scheme on a data file data.dat
in Diana batch format.
data.dat
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
7.2 Preliminary Linear Analysis 119
’ELEMEN’
DATA
/ WALL BEAMUP / 1
’DATA’
1 NINTEG 3 3
’END’
We launch the Analysis Setup dialog via the ANALYSE command and activate
the following command file for the linear analysis.
linear.dcf
*FILOS
INITIA
*INPUT
READ FILE="panel.dat"
READ APPEND FILE="data.dat"
*LINSTA
*END
When the analysis is completed, we enter the iDiana Results environment with
the model name to assess the analysis results.
FEMVIEW LINSTA
VIEW MESH
VIEW OPTIONS EDGES OUTLINE
EYE FRAME
The VIEW and EYE commands display the outlines of the non-deformed mesh.
7.2.1 Stresses
We will display the distribution of vertical stresses for the two load cases.
linsta.fvc
RESULTS LOADCASE LC1
RESULTS ELEMENT EL.SXX.G SYY
PRESENT CONTOUR FROM -2.5 TO -5 LEVELS 9
RESULTS LOADCASE LC2
PRESENT CONTOUR FROM -10 TO 10 LEVELS 9
We select results attribute SYY which represents the vertical stresses σY Y . We
display a contour plot for both load cases [Fig. 7.8]. Note that we explicitly
specify the contour levels to gain a better insight in the stresses in the panel.
7.2.2 Displacements
To assess the displacements we display the mesh including the element edges.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
120 Shear Wall Panel
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:50:03 linstr1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:50:03 linstr2.ps
Model: LINSTA Model: LINSTA
LC1: Load case 1 LC2: Load case 2
Element EL.SXX.G SYY Element EL.SXX.G SYY
Max = .517 Max = 23.3
Min = -7.46 Min = -23.3
-5 10
-4.75 8
-4.5 6
-4.25 4
-4 2
Y -3.75 Y 0
-3.5 -2
-3.25 -4
Z X -3 Z X -6
-2.75 -8
-2.5 -10
(a) for vertical pressure (b) for horizontal displacement
Figure 7.8: Vertical stresses
linsta.fvc
VIEW OPTIONS EDGES ALL
RESULTS LOADCASE LC1
RESULTS NODAL DTX....G RESDTX
PRESENT CONTOUR FROM 0 TO 0.2 LEVELS 9
VIEW OPTIONS DEFORM USING DTX....G RESDTX
RESULTS LOADCASE LC2
PRESENT CONTOUR FROM 0 TO 1.05 LEVELS 9
VIEW OPTIONS DEFORM USING DTX....G RESDTX
We select results attribute RESDTX which represents the displacement vectors of
the nodes. We display a contour plot for the two load cases [Fig. 7.9]. Note the
use of the DEFORM option to display the contour plot on the deformed mesh.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:50:03 lindis1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:50:03 lindis2.ps
Model: LINSTA Model: LINSTA
Deformation = 622 Deformation = 105
LC1: Load case 1 LC2: Load case 2
Nodal DTX....G RESDTX Nodal DTX....G RESDTX
Max = .193 Min = 0 Max = 1.15 Min = 0
.2 1.05
.18 .945
.16 .84
.14 .735
.12 .63
Y .1 Y .525
.8E-1 .42
.6E-1 .315
Z X .4E-1 Z X .21
.2E-1 .105
0 0
(a) for vertical pressure (b) for horizontal displacement
Figure 7.9: Total displacements
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
7.3 Nonlinear Analysis 121
7.3 Nonlinear Analysis
We now specify a nonlinear analysis via the Analysis Setup dialog.
iDiana
ANALYSE PANEL
Analysis Setup
···
We will consider and apply the following analysis options.
Use physical nonlinear effects and specify plasticity and total strain based
cracking with the secant option.
Specify two execute blocks, the first one for the vertical load and the
second one for the monotonic displacement.
Use for the first load the displacement convergence norm only.
Use for the second load the energy convergence norm of 0.001 only.
Apply in the second execute block the second load using thirty steps of
size 1.0.
Use one output block for the whole analysis and specify:
– Displacements,
– Crack status and strain,
– Principal and global stresses,
– Global strains,
– Plasticity status and plastic strains,
– Reaction and residual forces.
We save the analysis specification as a command file:
nonlin.dcf
*FILOS
INITIA
*INPUT
READ FILE="panel.dat"
READ APPEND FILE="data.dat"
*NONLIN
BEGIN TYPE
BEGIN PHYSIC
PLASTI
TOTCRK
END PHYSIC
END TYPE
EXECUT
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
122 Shear Wall Panel
BEGIN EXECUT
BEGIN ITERAT
BEGIN CONVER
DISPLA OFF
ENERGY TOLCON=0.001
FORCE OFF
END CONVER
MAXITE=50
END ITERAT
BEGIN LOAD
LOADNR=2
STEPS EXPLIC SIZES 1.(30)
END LOAD
END EXECUT
BEGIN OUTPUT
DISPLA
FORCE
STATUS
STATUS CRACK
STRAIN
STRAIN TOTAL GREEN PRINCI
STRAIN CRACK
STRAIN PLASTI
STRESS
STRESS CRACK
STRESS TOTAL CAUCHY PRINCI
END OUTPUT
*END
We run the analysis and enter the iDiana results environment to assess the
results.
7.4 Load–Displacement Diagram
We will present a diagram of the load versus the displacement for the node in
the beam center where the displacement has been applied. Therefore we need
to know the number of this node.
Node number nonlin.fvc
VIEW MESH
LABEL MESH CONSTRNTS
LABEL MESH NODES
EYE ZOOM /CURSOR
We label the constraints and the node numbers on the mesh [Fig. 7.10a]. When
we drag a zoom window around the appropriate node it appears to be number
482 [Fig. 7.10b].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
7.4 Load–Displacement Diagram 123
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:20 meshf iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:20 meshz
Model: NONLIN Model: NONLIN
534 538 535 540 536
544
542
546
543553548555549557550559551561552568563570564572565574566576567
580
578
582
579 586 584 588 585
537 539 541545547 554 556 558 560 562 569 571 573 575 577581583 587 589
514 519 516 522 470
474
471
476
472483478485479487480489481491482498493500494502495504496506497
510
508
512
509 528 524 531 526 550 559 551 561 552 568 563 570 564
518 521 473475477 484 486 488 490 492 499 501 503 505 507511513 530 533
515 520 517 523 1 12
44
590
597
59623
65
646141
647 678162
67986 71197 743108
710183 775119
742204 807130
774225806301838322
839246871257903268
870343 935279
902364 967290
934385 428
406
9991031
998
966 1030
417
449 529 525 532 527
34
59155
59576
645 152
677 173
709 194
741 215
773 236
805 312
837 333
869 354
901 375
933 396
9654391029
997460
2 13
45
592
593
59424
644142
66
643 67587 70798
676163 739109
708184 771120
740205 803131
772226804302
835247867258
836323 899269
868344 931280
900365 963291
932386 429
995
996
407
964 418
1027
1028
450
35
59856
60277
650 153
682 174
714 195
746 216
778 237
810 313
842 334
874 355
906 376
938 397
970440
1034
1002
461 558 560 562 569 571
3 14
46
599
600
60125
649143
67
648 68088 71299
681164 744110
713185 776121
745206 808132
777227809303
840248872259
841324 904270
873345 936281
905366 968292
937387 4301032
1000
969
4081033
419
1001
451
36
60357
60778
653 154
685 175
717 196
749 217
781 238
813 314
845 335
877 356
909 377
941 398
973441
1037
1005
462
4 15
47
604
605
60626
652144
68
651 68389 715100
684165 747111
716186 779122
748207 811133
780228812304
843249875260
844325 907271
876346 939282
908367 971293
940388 4311035
1003
972
4091036
1004
420
452
37
60858
61279
656 155
688 176
720 197
752 218
784 239
816 315
848 336
880 357
912 378
944 399
976442
1040
1008
463
5
60916
48
610 27
655145
69
611
654 68690 718101
687166 750112
719187 782123
751208 814134
783229815305
846250878261
847326 910272
879347 942283
911368 974294
943389 4321038
10061039
1007
975
410421
453 480 489 481 491 482 498 493 500 494
38
61359
61780
659 156
691 177
723 198
755 219
787 240
819 316
851 337
883 358
915 379
947 400 1043
979443
1011
464
6 17
49
614
615
61628
658146
70
657 68991 721102
690167 753113
722188 785124
754209 817135
786230818306
849251881262
850327 913273
882348 945284
914369 977295
946390 4331041
1009
978
4111042
1010
422
454
39
61860
62281
662 157
694 178
726 199
758 220
790 241
822 317
854 338
886 359
918 380
950 401 1046
1014
982444
465
7 18
50
619
620
62129
661147
71
660 69292 724103
693168 756114
725189 788125
757210 820136
789231821307
852252884263
853328 916274
885349 948285
917370 980296
949391 4341044
1012
981
4121045
1013
423
455
40
62361
62782
665 158
697 179
729 200
761 221
793 242
825 318
857 339
889 360
921 381
953 402 1049
1017
985445
466 488 490 492 499 501
8 19
51
624
625
62630
664148
72
663 69593 727104
696169 759115
728190 791126
760211 823137
792232824308
855253887264
856329 919275
888350 951286
920371 983297
952392 1047
1015
435
984
4131048
1016
424
456
41
62862
63283
668 159
700 180
732 201
764 222
796 243
828 319
860 340
892 361
924 382
956 403 1052
1020
988446
467
9 20
52
629
630
63131
667149
73
666 69894 730105
699170 762116
731191 794127
763212 826138
795233827309
858254890265
859330 922276
891351 954287
923372 986298
955393 1050
1018
987
436
4141051
1019
425
457
42
63363
63784
671 160
703 181
735 202
767 223
799 244
831 320
863 341
895 362
927 383
959 404 1055
1023
991447
468
Y Y
10
53
63421
63574
63632
670150
669 733106
702171
70195 765117
734192 797128
766213 829139
798234830310
861255893266
862331 925277
894352 957288
926373 989299
958394 1053
10211054
1022
990
437
415426
458 108
742 204
775 119
774 225
807 130
806 301
839 246
838 322
871 257
870
43
63864
64285
674 161
706 182
738 203
770 224
802 245
834 321
866 342
898 363
930 384
962 405 1058
1026
994448
469
Z X Z X
11
54
63922
64075
64133
673151
672 70496 736107
705172 768118
737193 800129
769214 832140
801235833311
864256896267
865332 928278
897353 960289
929374 992300
961395 1056
1024
993
438
4161057
1025
427
459
(a) full display (b) zoom-in
Figure 7.10: Mesh with labeled node numbers
Diagram nonlin.fvc
RESULTS LOADCASE LC1 LC2
RESULTS NODAL FBX....G FBX
PRESENT GRAPH NODE 482
We select all available load cases (steps) and choose results attribute FBX which
represents the horizontal reaction force in the node. The PRESENT command
displays the load–displacement diagram for node 482 [Fig. 7.11]. Note that the
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:20 lodis.ps
Model: NONLIN
Nodal FBX....G FBX
Max/Min on whole graph:
Ymax = -.7E-10
Ymin = -.884E6
Xmax = 30
Xmin = 1
*1E5 Variation over loadcases
Node 482
0
0 2.5 5 7.5 10 12.5 15 17.5 20 22.5 25 27.5 30 32.5
-1
N -2
O
D
A
L -3
F
B -4
X
.
. -5
.
.
G -6
F
B -7
X
-8
-9
LOAD
Figure 7.11: Load–displacement diagram
horizontal axis is labeled with ‘load’ which means that it represents the load on
the model. In this case this is the factor for the forced horizontal displacement
in the nonlinear analysis. In the sequel of this example we will present analysis
results for steps 6 and 31 which represent a horizontal displacement uX of 5 and
30 mm.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
124 Shear Wall Panel
7.4.1 Principal Stress
Principal stresses can best be displayed as vectors, then we can see both their
size and their direction. iDiana will display a tensile stress with a straight line,
a compressive stress gets a small transverse dash at its end.
nonlin.fvc
LABEL MESH OFF
VIEW OPTIONS EDGES OUTLINE
EYE FRAME
RESULTS LOADCASE LC2 6
RESULTS ELEMENT EL.S1 S2
PRESENT VECTORS ALL 1.0
RESULTS LOADCASE LC2 31
PRESENT VECTORS ALL 1.0
We revert to a clean outline view of the model and select results attribute S12
which represents the principal stresses. We display a vector plot for two selected
steps [Fig. 7.12]. Note that both plots share the same enlargement factor (1×)
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:20 nonstr1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:20 nonstr2.ps
Model: NONLIN Model: NONLIN
LC2: Load case 2 LC2: Load case 2
Step: 6 LOAD: 5 Step: 31 LOAD: 30
Element EL.S1 S2 Element EL.S1 S2
Max = 2.1 Max = 3.22
Min = -36.4 Min = -35.4
Factor = 1 Factor = 1
Y Y
Z X -10.7 Z X -9.64
-23.5 -22.5
(a) uX = 5 mm (b) uX = 30 mm
Figure 7.12: Vectors for principal stress
and color modulation so that we can readily compare the results. Obviously
the tensile stresses are so small that they appear as dots, most notably in the
beam.
7.4.2 Plastic Strains in Reinforcements
Via the plot of the plastic strain in the reinforcements we can determine the
yield areas of the grids.
nonlin.fvc
RESULTS ELEMENT RE.EPXXG EPXX
RESULTS CALCULATE VONMISES
RESULTS LOADCASE LC2 6
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
7.4 Load–Displacement Diagram 125
PRESENT CONTOUR VALUE 0.001
RESULTS LOADCASE LC2 31
PRESENT CONTOUR VALUE 0.001
We select results attribute RE.EPXX which represents the plastic strain in the
reinforcements. From these we let iDiana calculate the equivalent Von Mises
plastic strain εpeq . We display a contour plot for the two selected steps. Note
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:20 nonvmi1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:20 nonvmi2.ps
Model: NONLIN Model: NONLIN
LC2: Load case 2 LC2: Load case 2
Step: 6 LOAD: 5 Step: 31 LOAD: 30
Element VONMISES RE.EPXXG Element VONMISES RE.EPXXG
Calculated from: RE.EPXXG Calculated from: RE.EPXXG
Max = .137E-2 Min = 0 Max = .367E-1 Min = 0
Y Y
Z X Z X
.1E-2 .1E-2
(a) uX = 5 mm (b) uX = 30 mm
Figure 7.13: Plastic areas in reinforcements (red)
that we do a little trick to get the yielding areas clearly displayed: we ask for
one contour at a small but significant value. In this case areas with εpeq > 0.001
appear in red, the other areas, which are still elastic, in blue.
7.4.3 Cracking
We will asses the cracking behavior of the model via the crack strains and the
crack pattern.
Crack strain panel.fvc
RESULTS GAUSSIAN EL.EKNN1 EKNN
RESULTS LOADCASE LC2 6
PRESENT CONTOUR FROM 0 TO 0.02 LEVELS 7
RESULTS LOADCASE LC2 31
PRESENT CONTOUR FROM 0 TO 0.02 LEVELS 7
The selected results attribute EKNN represents the normal crack strain εcrnn . We
display two contour plots with the same levels so that we can compare the colors
of the contours [Fig. 7.14]: areas without crack strain are dark blue, areas with
εcr
nn > 0.02 are red.
Animation panel.fvc
VIEW OPTIONS DEFORM USING TDTX...G RESTDT 4.0
RESULTS LOADCASE LC1 1 TO LC2 31
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
126 Shear Wall Panel
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:20 noncrk1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:20 noncrk2.ps
Model: NONLIN Model: NONLIN
LC2: Load case 2 LC2: Load case 2
Step: 6 LOAD: 5 Step: 31 LOAD: 30
Gauss EL.EKNN1 EKNN Gauss EL.EKNN1 EKNN
Max = .39E-2 Max = .357E-1
Min = -.626E-4 Min = -.642E-4
Results shown: Results shown:
Mapped to nodes Mapped to nodes
.2E-1 .2E-1
.175E-1 .175E-1
.15E-1 .15E-1
Y .125E-1 Y .125E-1
.1E-1 .1E-1
.75E-2 .75E-2
Z X .5E-2 Z X .5E-2
.25E-2 .25E-2
0 0
(a) uX = 5 mm (b) uX = 30 mm
Figure 7.14: Crack strains
DRAWING ANIMATE LOADCASES PLOTFILE ancr
utility setup animate exit
We can display the development of the crack strain for increasing deformation in
an animation sequence. For the deformation we select results attribute RESTDT,
the total displacement, and we apply a 4× magnification. We select all steps
and start the animation. The PLOTFILE option yields a file for each frame so
that we can show them in a document [Fig. 7.15].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:20
iDIANA ancr001
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:20
iDIANA ancr002
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:20
iDIANA ancr003
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:20
iDIANA ancr004
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:21
iDIANA ancr005
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:21
iDIANA ancr006
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:21 ancr007
.2E-1 .2E-1 .2E-1 .2E-1 .2E-1 .2E-1 .2E-1
.175E-1 .175E-1 .175E-1 .175E-1 .175E-1 .175E-1 .175E-1
.15E-1 .15E-1 .15E-1 .15E-1 .15E-1 .15E-1 .15E-1
Y Y .125E-1 Y .125E-1 Y .125E-1 Y .125E-1 Y .125E-1 Y .125E-1 .125E-1
.1E-1 .1E-1 .1E-1 .1E-1 .1E-1 .1E-1 .1E-1
.75E-2 .75E-2 .75E-2 .75E-2 .75E-2 .75E-2 .75E-2
Z X Z .5E-2
X Z .5E-2
X Z .5E-2
X Z .5E-2
X Z .5E-2
X Z .5E-2
X .5E-2
.25E-2 .25E-2 .25E-2 .25E-2 .25E-2 .25E-2 .25E-2
0 0 0 0 0 0 0
DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:21
iDIANA ancr008
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:21
iDIANA ancr009
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:21
iDIANA ancr010
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:21
iDIANA ancr011
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:21
iDIANA ancr012
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:21
iDIANA ancr013
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:21 ancr014
.2E-1 .2E-1 .2E-1 .2E-1 .2E-1 .2E-1 .2E-1
.175E-1 .175E-1 .175E-1 .175E-1 .175E-1 .175E-1 .175E-1
.15E-1 .15E-1 .15E-1 .15E-1 .15E-1 .15E-1 .15E-1
Y Y .125E-1 Y .125E-1 Y .125E-1 Y .125E-1 Y .125E-1 Y .125E-1 .125E-1
.1E-1 .1E-1 .1E-1 .1E-1 .1E-1 .1E-1 .1E-1
.75E-2 .75E-2 .75E-2 .75E-2 .75E-2 .75E-2 .75E-2
Z X Z .5E-2
X Z .5E-2
X Z .5E-2
X Z .5E-2
X Z .5E-2
X Z .5E-2
X .5E-2
.25E-2 .25E-2 .25E-2 .25E-2 .25E-2 .25E-2 .25E-2
0 0 0 0 0 0 0
DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:21
iDIANA ancr015
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:21
iDIANA ancr016
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:21
iDIANA ancr017
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:21
iDIANA ancr018
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:21
iDIANA ancr019
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:21
iDIANA ancr020
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:21 ancr021
.2E-1 .2E-1 .2E-1 .2E-1 .2E-1 .2E-1 .2E-1
.175E-1 .175E-1 .175E-1 .175E-1 .175E-1 .175E-1 .175E-1
.15E-1 .15E-1 .15E-1 .15E-1 .15E-1 .15E-1 .15E-1
Y Y .125E-1 Y .125E-1 Y .125E-1 Y .125E-1 Y .125E-1 Y .125E-1 .125E-1
.1E-1 .1E-1 .1E-1 .1E-1 .1E-1 .1E-1 .1E-1
.75E-2 .75E-2 .75E-2 .75E-2 .75E-2 .75E-2 .75E-2
Z X Z .5E-2
X Z .5E-2
X Z .5E-2
X Z .5E-2
X Z .5E-2
X Z .5E-2
X .5E-2
.25E-2 .25E-2 .25E-2 .25E-2 .25E-2 .25E-2 .25E-2
0 0 0 0 0 0 0
DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:22
iDIANA ancr022
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:22
iDIANA ancr023
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:22
iDIANA ancr024
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:22
iDIANA ancr025
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:22
iDIANA ancr026
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:22
iDIANA ancr027
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:22 ancr028
.2E-1 .2E-1 .2E-1 .2E-1 .2E-1 .2E-1 .2E-1
.175E-1 .175E-1 .175E-1 .175E-1 .175E-1 .175E-1 .175E-1
.15E-1 .15E-1 .15E-1 .15E-1 .15E-1 .15E-1 .15E-1
Y Y .125E-1 Y .125E-1 Y .125E-1 Y .125E-1 Y .125E-1 Y .125E-1 .125E-1
.1E-1 .1E-1 .1E-1 .1E-1 .1E-1 .1E-1 .1E-1
.75E-2 .75E-2 .75E-2 .75E-2 .75E-2 .75E-2 .75E-2
Z X Z .5E-2
X Z .5E-2
X Z .5E-2
X Z .5E-2
X Z .5E-2
X Z .5E-2
X .5E-2
.25E-2 .25E-2 .25E-2 .25E-2 .25E-2 .25E-2 .25E-2
0 0 0 0 0 0 0
DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:22 ancr029 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:22 ancr030 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:22 ancr031
.2E-1 .2E-1 .2E-1
.175E-1 .175E-1 .175E-1
.15E-1 .15E-1 .15E-1
Y .125E-1 Y .125E-1 Y .125E-1
.1E-1 .1E-1 .1E-1
.75E-2 .75E-2 .75E-2
Z X .5E-2 Z X .5E-2 Z X .5E-2
.25E-2 .25E-2 .25E-2
0 0 0
DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr DRAWING ANIMATE LOADCASES PLOTFILE ancr
Figure 7.15: Animation frames for crack strain development
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
7.5 Cyclic Loading 127
Crack pattern panel.fvc
RESULTS LOADCASE LC2 6
PRESENT DISC 0.2
RESULTS LOADCASE LC2 31
PRESENT DISC 0.2
With the DISC option the crack strain is displayed as a disc perpendicular to
the strain direction. In a two-dimensional view this disc degrades to a narrow
line which clearly shows the crack pattern [Fig. 7.16]. Note that all cracks are
displayed with lines of equal length. The significance of the crack can only be
seen from its color: red for the larger strains, blue for the smaller.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:23 noncpa1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:51:23 noncpa2.ps
Model: NONLIN Model: NONLIN
Deformation = 4 Deformation = 4
LC2: Load case 2 LC2: Load case 2
Step: 6 LOAD: 5 Step: 31 LOAD: 30
Gauss EL.EKNN1 EKNN Gauss EL.EKNN1 EKNN
Max = .39E-2 Max = .357E-1
Min = -.626E-4 Min = -.642E-4
Y Y
Z X .258E-2 Z X .238E-1
.126E-2 .119E-1
(a) uX = 5 mm (b) uX = 30 mm
Figure 7.16: Crack pattern
7.5 Cyclic Loading
We can use the same model to study the effect of cyclic loading We only need
to change the command file so that the model is loaded cyclic [Fig. 7.17]. Please
u [mm] 0
−2
−4
0 5 10 15 20 25 30
Steps
Figure 7.17: Cyclic loading diagram
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
128 Shear Wall Panel
note that in the model there are no time-dependent properties, so we can apply
the load in the steps command of the command file by changing the line in the
second EXECUT block to:
cyclic.dcf
STEPS EXPLIC SIZES 1.(1) -1.(2) 1.(1) \
1.(2) -1.(4) 1.(2) \
1.(4) -1.(8) 1.(4)
We could now proceed in the same way as for the monotonic loading.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
Chapter 8
Column–Beam Joint in a
Portal Frame
Name: Portal
Path: /Examples/ConcMas/Portal
Keywords: analys: nonlin physic. constr: suppor. elemen: bar cq16m
pstres reinfo. load: force node. materi: consta crack cutoff
elasti harden isotro linear plasti retent smear soften strain von-
mis. option: adapti arclen direct groups loadin newton normal
regula size units update. post: binary femvie. pre: femgen.
result: cauchy crack displa extern force green plasti strain
stress total.
500 500 500
F F
810
1500
Figure 8.1: Frame and loading [mm]
In this example we will apply a concrete material model combining cracking
and crushing phenomena. It concerns the column–beam joint of a portal frame
[Fig. 8.1]. The thickness of the frame is 70 mm. We assume that the load is
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
130 Column–Beam Joint in a Portal Frame
concentrated in two points. Due to the symmetry of the problem (geometry and
loading), one half of the frame will be modeled [Fig. 8.2].
560 ♥
F 2∅6
10
120
90 10 2∅6
30
10 10
870
750
2∅6 2∅6
X
120
810
Figure 8.2: Dimensions of the portal frame and reinforcement details [mm]
8.1 Finite Element Model
To build up the finite element model, we start iDiana and enter the Design
environment with the model name PORTAL.
iDiana
FEMGEN PORTAL
Analysis and Units
Analysis Selection
Model Type: →Structural 2D
Units Definition
Length: →Millimeter
Mass: →Kilogram
Force: →Newton
Time: →Second
Temperature: →Celsius
In the Analysis and Units dialog we specify the model type for two-dimensional
structural analysis and the adopted units [mm, kg, N, s, °C].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
8.1 Finite Element Model 131
8.1.1 Geometry Definition
portal.fgc
GEOMETRY POINT COORD P1 0
GEOMETRY POINT COORD P2 60
GEOMETRY POINT COORD P3 120
GEOMETRY POINT COORD P4 120 750
GEOMETRY POINT COORD P5 560 750
GEOMETRY POINT COORD P6 810 750
GEOMETRY POINT COORD P7 810 870
GEOMETRY POINT COORD P8 560 870
GEOMETRY POINT COORD P9 120 870
GEOMETRY POINT COORD P10 0 870
GEOMETRY POINT COORD P11 0 750
EYE FRAME
GEOMETRY SURFACE 4POINTS P1 +P2 P3 P4 P11
GEOMETRY SURFACE 4POINTS P11 P4 P9 P10
GEOMETRY SURFACE 4POINTS P4 P5 P8 P9
GEOMETRY SURFACE 4POINTS P5 P6 P7 P8
CONSTRUCT SET PORTAL APPEND ALL
VIEW GEOMETRY PORTAL VIOLET
LABEL GEOMETRY LINES CURRENT RED
We define the coordinates of the vertices of the portal. Then, we construct the
corresponding surfaces and append all the geometrical entities constructed so
far in the set PORTAL. The geometry is finally displayed with labeled line names
[Fig. 8.3a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:52:38 geom1 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:52:38 mesh1
Model: PORTAL Model: PORTAL
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D L8 L12 L15 Model Type: Structural 2D
L9
L7 L11 L14
L5 L10 L13
L1
L4
Y Y
Z X L2L6 L3 Z X
(a) geometry (b) mesh
Figure 8.3: Definition of the model
8.1.2 Meshing
The meshing procedure involves the specification of the divisons, the generation
of the mesh and the check via a display.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
132 Column–Beam Joint in a Portal Frame
portal.fgc
MESHING DIVISION LINE ALL 8
MESHING DIVISION LINE L2 4
MESHING DIVISION LINE L3 4
MESHING DIVISION LINE L4 -520
MESHING DIVISION LINE L1 520
MESHING DIVISION LINE L10 220
MESHING DIVISION LINE L12 -220
MESHING TYPES ALL QU8 CQ16M
MESHING GENERATE
VIEW MESH
First we define the line divisions to be adopted. Note that we apply a slight
grading toward the connection of the column and the beam. Then we choose
for all geometrical entities the 8-node quadrilateral plane stress element CQ16M.
Finally we generate and display the finite element mesh [Fig. 8.3b].
8.1.3 Reinforcement
We define the reinforcement bars according to Figure 8.2 on page 130
portal.fgc
GEOMETRY POINT COORD P12 10
GEOMETRY POINT COORD P13 10 870
GEOMETRY POINT COORD P14 110
GEOMETRY POINT COORD P15 110 840
GEOMETRY POINT COORD P16 90 760
GEOMETRY POINT COORD P17 810 760
GEOMETRY POINT COORD P18 0 860
GEOMETRY POINT COORD P19 810 860
REINFORCE BAR SECTION RE1 P12 P13
REINFORCE BAR SECTION RE2 P14 P15
REINFORCE BAR SECTION RE3 P16 P17
REINFORCE BAR SECTION RE4 P18 P19
REINFORCE BAR REBAR1 RE1
REINFORCE BAR REBAR2 RE2
REINFORCE BAR REBAR3 RE3
REINFORCE BAR REBAR4 RE4
REINFORCE SET REBAR APPEND REBAR1 REBAR2 REBAR3 REBAR4
VIEW GEOMETRY ALL YELLOW
VIEW REINFORCE +REBAR RED
VIEW OPTIONS SHRINK MESH
VIEW MESH
VIEW REINFORCE +REBAR RED
First we define the end-points of each reinforcement bar. Then we specify the
four reinforcement sections via the SECTION option. All reinforcements, REBAR1
to REBAR4, are combined in the reinforcement set REBAR. The VIEW commands
display the reinforcements in the geometry and in the mesh [Fig. 8.4].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
8.1 Finite Element Model 133
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:52:38 geomre iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:52:38 meshre
Model: PORTAL Model: PORTAL
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
Y Y
Z X Z X
(a) in geometry (b) in mesh
Figure 8.4: Defined reinforcement bars
8.1.4 Material and Physical Properties
To specify the material and physical properties of the model we launch the
Property Manager dialog.
iDiana
View Property Manager...
↑ →
Property Manager
···
Concrete iDiana
Property Manager
↑Materials Material Name: MACONCRE
↑Linear Elasticity →Isotropic
↑Static Nonlinearity →Concrete and Brittle Materials →Multi-directional Fixed Crack
→Constant Stress Cut-off →Linear Tension Softening
→Ultimate Strain Based →Constant Shear Retention
→Von Mises Plasticity →Ideal Plasticity
↑Physical Properties Physical Property Name: PHCONCRE
↑Geometry →Plane Stress →Regular
For the concrete part, we define a material instance MACONCRE. As parameters
for elasticity we specify a Young’s modulus E = 28000 MPa and a Poisson’s
ratio ν = 0.2. As nonlinear material parameters we specify a tensile strength
ft = 2.2 MPa, an ultimate strain εu = 1×10−3 , a constant shear retention factor
β = 0.2, and a yield stress fc = 25 MPa. We also define a physical property
instance PHCONCRE with a thickness value t = 70 mm.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
134 Column–Beam Joint in a Portal Frame
Reinforcement iDiana
Property Manager
↑Materials Material Name: MAREINFO
↑Linear Elasticity →Reinforcement →Reinforcement Bonded
↑Static Nonlinearity →Reinforcement →Von Mises Plasticity → Ideal Plasticity
↑Physical Properties Physical Property Name: PHREINFO
↑Geometry →Embedded Reinforcements →Bar
For the reinforcement we define a material instance MAREINFO. The parameter
for elasticity is a Young’s Modulus E = 210000 MPa and for nonlinearity a yield
stress σy = 450 MPa. We also create a physical property instance PHREINFO with
a cross-section area A = 56.55 mm2 .
Assignment portal.fgc
PROPERTY ATTACH PORTAL MACONCRE PHCONCRE
PROPERTY ATTACH REBAR MAREINFO PHREINFO
We assign the property instances to the appropriate geometrical parts: the
concrete properties to set PORTAL and the reinforcement properties to the bars
REBAR.
8.1.5 Boundary Conditions
The boundary conditions involve the constraints (supports) and the loading
[Fig. 8.1].
Constraints portal.fgc
PROPERTY BOUNDARY CONSTRAINT P2 X Y
PROPERTY BOUNDARY CONSTRAINT L14 X
VIEW REINFORCE OFF
LABEL MESH CONSTRNT
We define the constraints with respect to the geometric parts. The mid-point of
the column base is supported horizontally and vertically (X- and Y -direction).
Due to symmetry conditions, the line of the right edge is supported horizontally.
The display confirms the correct definition [Fig. 8.5a].
Load portal.fgc
PROPERTY LOAD FORCE P8 -200 Y
LABEL MESH OFF
LABEL MESH LOADS
The load is a vertical force of −200 N, applied on top of the beam [Fig. 8.5b].
8.2 Nonlinear Analysis
We write the model to a file in Diana batch format and leave the iDiana Design
environment.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
8.2 Nonlinear Analysis 135
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:52:38 meshco iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:52:38 meshlo
Model: PORTAL Model: PORTAL
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
Y Y
Z X Z X
(a) constraints (b) loading
Figure 8.5: Boundary conditions
iDiana
UTILITY WRITE DIANA
FILE CLOSE
yes
Column-Beam Joint in a Portal Frame
ANALYSE PORTAL
Analysis Setup
···
Via the Analysis Setup dialog we create or activate the following batch command
file for the nonlinear analysis.
portal.dcf
*FILOS
INITIA
*INPUT
*NONLIN
BEGIN EXECUT
BEGIN LOAD
LOADNR=1
BEGIN STEPS
BEGIN ITERAT
ARCLEN
GAMMA=0.25
MAXSIZ=5
NSTEPS=40
END ITERAT
END STEPS
END LOAD
END EXECUT
BEGIN OUTPUT
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
136 Column–Beam Joint in a Portal Frame
DISPLA
FORCE EXTERN
STRAIN PLASTI
STRAIN CRACK
STRESS
END OUTPUT
*END
Note the use of the Arc-length iteration control method which is particularly
useful in case of force-controlled analysis of structures with softening material.
For this example, it would have been easier to use a displacement-controlled
analysis. However, we will apply force-control for demonstration purposes. After
the job has been terminated, we check the convergence of the analysis process
via the output messages of which the last ones are:
shearf.out
STEP 22 TERMINATED, CONVERGENCE AFTER 6 ITERATIONS
STEP 23 TERMINATED, CONVERGENCE AFTER 2 ITERATIONS
STEP 24 TERMINATED, CONVERGENCE AFTER 4 ITERATIONS
Obviously the last step that reached convergence is 24. Presumably the struc-
ture has collapsed beyond that step, i.e., it has reached its Ultimate Limit State.
We enter the iDiana Results environment to assess the analysis results.
iDiana
FEMVIEW PORTAL
8.2.1 Load–Displacement Diagram
We will present the load versus the displacement of the node on which the force
has been applied. Therefore we need to know the number of this node.
Node number portal.fvc
VIEW MESH
LABEL MESH NODES
EYE ZOOM /CURSOR
We display the mesh labeled with node numbers [Fig. 8.6a]. We know that the
force load was applied on the top edge between the fourth and fifth element
from the right [Fig. 8.5b]. For a closer look we drag a zoom window over the
right part of the portal. The node number turns out to be 255 [Fig. 8.6b].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
8.2 Nonlinear Analysis 137
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:52:59 nodes.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:52:59 nodesz.ps
Model: PORTAL Model: PORTAL
165
447166
202
416
448 167
203
449168
204
450169
205
451246247248249
336
452453454455 250
337338339 340
456 251
341
457 252
342
458 253
343 254
459344334 255
460345335 362
461398394 363
462399395 364
463400396 365
464401397
465
197198 199200201326327328329 330 331 332 333
160161
193
415 162
194 163
195 164
196
430 236237238239
316 240
317318319 320 241
321 242
322 243324244325245390358391359392360393361
323
188189190191192306307308309 310 311 312 313 314 315 386 387 388 389
155156
184
414 157
185 158
186 159
187
429 226227228229
296 230
297298299 300 231
301 232
302 233304234305235382354383355384356385357
303
179180181182183286287288289 290 291 292 293 294 295 378 379 380 381
150151
175
413 152
176 153
177 154
178
428 216217218219
276 220
277278279 280 221
281 222
282 223284224285225374350375351376352377353
283
170171172173
431174
432266267268269
433434435436 270
437 271
438 272
439 273
440264274
441265275
442366370
443367371
444368372
445369373
446
1412
66128723108
34129
427
45 206207208209
256 210
257258259 260 211
261 212
262 213
263 214 215 346 347 348 349
56 77 98 119140 254 345 255 398 362 399 363 400 364 401 365
2411 35130
67138824109426
46
57 78 99 120141 460 461 462 463 464 465
3410 36131
68148925110425
47 334 335 394 395 396 397
58 79 100121142
4409 37132
69159026111424
48
59 80 101122143 244 325 245 390 358 391 359 392 360 393 361
5408 38133
70169127112423
49
60 81 102123144 314 315 386 387 388 389
6407 39134
71179228113422
50
61 82 103124145 234 305 235 382 354 383 355 384 356 385 357
7406 40135
72189329114421
51
294 295 378 379 380 381
62 83 104125146
8405 41136
73199430115420
52 224 285 225 374 350 375 351 376 352 377 353
63 84 105126147 274 275 370 371 372 373
441 442 443 444 445 446
9404 42137
74209531116419
53 214 265 215 366 346 367 347 368 348 369 349
64 85 106127148
403 43138
75219632117
10 418
54
Y Y
65 86 107128149
Z X Z X
402 44139
76229733118
11 417
55
(a) full display (b) zoom-in
Figure 8.6: Mesh with labeled node numbers
Diagram portal.fvc
RESULTS LOADCASE LC1
RESULTS NODAL TDTX...G TDTY
PRESENT GRAPH NODE 255
We select all load cases and result attribute TDTY which represents the vertical
displacements uY . We then display for node 255 the evolution of uY over the
load step values [Fig. 8.7]. Note that uY is negative and therefore the displace-
ment in the graph increases downward.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:52:59 loadis.ps
Model: PORTAL
Nodal TDTX...G TDTY
Max/Min on whole graph:
Ymax = -.257E-1
Ymin = -6.08
Xmax = 63.7
Xmin = 1
Variation over loadcases
Node 255
0
0 10 20 30 40 50 60 70
-1
N
O
D
A -2
L
T
D -3
T
X
.
. -4
.
G
T -5
D
T
Y
-6
-7
LOAD
Figure 8.7: Load–displacement diagram
8.2.2 Crack Development
We will assess the crack pattern for a specific step and as an animation.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
138 Column–Beam Joint in a Portal Frame
Crack pattern for step portal.fvc
VIEW MESH
EYE FRAME
VIEW OPTIONS EDGES OUTLINE
LABEL MESH NODES OFF
RESULTS LOADCASE LC1 24
RESULTS GAUSSIAN EL.EKNN1 EKNN
PRESENT DISC 0.3
PRESENT OPTIONS DISC MODULATE 10
VIEW OPTIONS DEFORM USING TDTX...G RESTDT 20
We revert to an outline view of the full mesh without node numbers. We select
the last step which represents the Ultimate Limit State. Result attribute EKNN
represents the normal crack strains εcr
nn . With the DISC option we display the
crack pattern [Fig. 8.8]. With the DEFORM option the results are presented on
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:52:59 crkuls.ps
Model: PORTAL
Deformation = 20
LC1: Load case 1
Step: 24 LOAD: 63.7
Gauss EL.EKNN1 EKNN
Max = .904E-2
Min = 0
.813E-2
.723E-2
.632E-2
Y .542E-2
.452E-2
.361E-2
.271E-2
Z X .181E-2
.904E-3
Figure 8.8: Crack pattern at Ultimate Limit State
the deformed mesh, in this case for the total displacements RESTDT and with
a 20× magnification. Due to the color modulation we can easily discern the
cracks with the largest normal strain, these are red in color.
Animation portal.fvc
RESULTS LOADCASE LC1 5 to LC1 24
PRESENT OPTIONS DISC MODULATE OFF
DRAWING ANIMATE LOADCASES PLOTFILE crack
We can display the development of the cracks for increasing deformation in an
animation sequence. Therefore we select the steps for which cracks have arisen:
5 to 24. We switch off color modulation to get all cracks displayed in the same
color. The DRAWING ANIMATE command starts the animation. The PLOTFILE
option yields a file for each frame so that we can show them in a document
[Fig. 8.9].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
8.2 Nonlinear Analysis 139
iDIANA 9.4.3-02 : TNO Diana BV iDIANA 28
9.4.3-02
OCT 2010
: TNO
01:52:59
Diana crack001
BV iDIANA 28
9.4.3-02
OCT 2010
: TNO
01:52:59
Diana crack002
BV iDIANA 28
9.4.3-02
OCT 2010
: TNO
01:52:59
Diana crack003
BV iDIANA 28
9.4.3-02
OCT 2010
: TNO
01:52:59
Diana crack004
BV iDIANA 28
9.4.3-02
OCT 2010
: TNO
01:52:59
Diana crack005
BV iDIANA 28
9.4.3-02
OCT 2010
: TNO
01:52:59
Diana crack006
BV 28 OCT 2010 01:52:59 crack007
Y Y Y Y Y Y Y
Z X Z X Z X Z X Z X Z X Z X
iDIANA 9.4.3-02 : TNO Diana BV iDIANA 28
9.4.3-02
OCT 2010
: TNO
01:52:59
Diana crack008
BV iDIANA 28
9.4.3-02
OCT 2010
: TNO
01:52:59
Diana crack009
BV iDIANA 28
9.4.3-02
OCT 2010
: TNO
01:52:59
Diana crack010
BV iDIANA 28
9.4.3-02
OCT 2010
: TNO
01:52:59
Diana crack011
BV iDIANA 28
9.4.3-02
OCT 2010
: TNO
01:53:00
Diana crack012
BV iDIANA 28
9.4.3-02
OCT 2010
: TNO
01:53:00
Diana crack013
BV 28 OCT 2010 01:53:00 crack014
DRAWING ANIMATE LOADCASES PLOTFILE crack DRAWING ANIMATE LOADCASES PLOTFILE crack DRAWING ANIMATE LOADCASES PLOTFILE crack DRAWING ANIMATE LOADCASES PLOTFILE crack DRAWING ANIMATE LOADCASES PLOTFILE crack DRAWING ANIMATE LOADCASES PLOTFILE crack DRAWING ANIMATE LOADCASES PLOTFILE crack
Y Y Y Y Y Y Y
Z X Z X Z X Z X Z X Z X Z X
iDIANA 9.4.3-02 : TNO Diana BV iDIANA 9.4.3-02
28 OCT 2010
: TNO
01:53:00
Diana BV
crack015 iDIANA 9.4.3-02
28 OCT 2010
: TNO
01:53:00
Diana BV
crack016 iDIANA 9.4.3-02
28 OCT 2010
: TNO
01:53:00
Diana BV
crack017 iDIANA 9.4.3-02
28 OCT 2010
: TNO
01:53:00
Diana BV
crack018 iDIANA 9.4.3-02
28 OCT 2010
: TNO
01:53:00
Diana BV
crack019 28 OCT 2010 01:53:00 crack020
DRAWING ANIMATE LOADCASES PLOTFILE crack DRAWING ANIMATE LOADCASES PLOTFILE crack DRAWING ANIMATE LOADCASES PLOTFILE crack DRAWING ANIMATE LOADCASES PLOTFILE crack DRAWING ANIMATE LOADCASES PLOTFILE crack DRAWING ANIMATE LOADCASES PLOTFILE crack DRAWING ANIMATE LOADCASES PLOTFILE crack
Y Y Y Y Y Y
Z X Z X Z X Z X Z X Z X
DRAWING ANIMATE LOADCASES PLOTFILE crack DRAWING ANIMATE LOADCASES PLOTFILE crack DRAWING ANIMATE LOADCASES PLOTFILE crack DRAWING ANIMATE LOADCASES PLOTFILE crack DRAWING ANIMATE LOADCASES PLOTFILE crack DRAWING ANIMATE LOADCASES PLOTFILE crack
Figure 8.9: Animation frames for crack development
8.2.3 Principal Stress
Due to the STRESS command in the OUTPUT block of the analysis commands
[§ 8.2] Diana has only stored the total Cauchy stresses. Thus, to display the
principal stresses we must first have them calculated by iDiana.
Calculation portal.fvc
VIEW OPTIONS DEFORM OFF
RESULTS LOADCASE LC1
RESULTS ELEMENT EL.SXX.G SXX
RESULTS CALCULATE P-STRESS ALL
We switch off the deformed model option and select all available load cases. The
SXX result attribute represents the total Cauchy stresses. Via the CALCULATE
option we let iDiana calculate the principal stresses.
Vector plot portal.fvc
RESULTS LOADCASE LC1 1
PRESENT VECTORS
RESULTS LOADCASE LC1 24
PRESENT VECTORS
For the first and last load cases we display vector plots of the principal stresses
via the VECTORS option [Fig. 8.10]. Note that the two plots have totally different
scaling factors and color levels for the vectors. So the two plots cannot be
compared mutually.
8.2.4 Concrete Crushing via Plastic Strain
To assess the crushing of the concrete we will display the Von Mises plastic
strains. These are not available as a results and must be calculated from the
Cauchy plastic strains.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
140 Column–Beam Joint in a Portal Frame
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:00 pstre1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:00 pstre2.ps
Model: PORTAL Model: PORTAL
LC1: Load case 1 LC1: Load case 1
Step: 1 LOAD: 1 Step: 24 LOAD: 63.7
Element PRINC STRESS ALL Element PRINC STRESS ALL
Calculated from: EL.SXX.G Calculated from: EL.SXX.G
Max = .244 Min = -.547 Max = 14.8 Min = -43.6
Factor = 132 Factor = 1.66
Y Y
Z X -.198E-1 Z X -4.63
-.283 -24.1
(a) for first load case (b) at Ultimate Limit State
Figure 8.10: Vector plots of the principal stresses
portal.fvc
RESULTS ELEMENT EL.EPXXG EPXX
RESULTS CALCULATE VONMISES
PRESENT CONTOUR LEVELS
We select the last load case, i.e., the Ultimate Limit State. The result attribute
EPXX represents the Cauchy plastic strains. From these we let iDiana calculate
the Von Mises plastic strains. We display these in a contour plot [Fig. 8.11a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:01 epvm.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:01 epvmz.ps
Model: PORTAL Model: PORTAL
LC1: Load case 1 LC1: Load case 1 50 51 52 139 77
Step: 24 LOAD: 63.7 Step: 24 LOAD: 63.7
Element VONMISES EL.EPXXG Element VONMISES EL.EPXXG
Calculated from: EL.EPXXG Calculated from: EL.EPXXG
Max = .24E-2 Min = 0 Max = .24E-2 Min = 0
46 47 48 138 67
42 43 44 137 57
140 141
.218E-2 .218E-2
.197E-2 .197E-2
.175E-2 .175E-2
.153E-2 .153E-2
Y .131E-2 Y .131E-2
.109E-2 .109E-2
.874E-3 .874E-3
Z X .655E-3 Z X 11 21 31 136 .655E-3
.437E-3 .437E-3
.218E-3 .218E-3
(a) full model (b) zoom-in
Figure 8.11: Von Mises plastic strain at Ultimate Limit State
portal.fvc
EYE ZOOM /CURSOR
VIEW OPTIONS EDGES ALL
LABEL MESH ELEMENTS VIEWMODE RED
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
8.2 Nonlinear Analysis 141
RESULTS LOADCASE LC1
PRESENT GRAPH ELEMENT 31
We zoom in on the crushed concrete area and ask for labeling element num-
bers. We can identify the element with larger plastic strains to be number 31
[Fig. 8.11b]. We then select all available load cases and display the evolution of
the Von Mises plastic strain as a function of the load step value [Fig. 8.12]. We
can detect the onset of crushing at a load value of about 50.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:01 evolvm.ps
Model: PORTAL
Element VONMISES EL.EPXXG
Calculated from: EL.EPXXG
Max/Min on whole graph:
Ymax = .762E-3 Ymin = 0
Xmax = 63.7 Xmin = 1
Variation over loadcases
*1E-4 Element 31 Mean
8
V
O 6
N
M
I 5
S
E
S
4
E
L
. 3
E
P
X
X 2
G
0
0 10 20 30 40 50 60 70
LOAD
Onset of crushing
Figure 8.12: Evolution with loading of the Von Mises plastic strain
8.2.5 Yielding in Reinforcement
We will assess the yielding of the reinforcement by displaying the plastic strain
and the stress in the model and as graphs.
Display in model portal.fvc
VIEW MESH
EYE FRAME
VIEW OPTIONS EDGES OUTLINE
LABEL MESH OFF
RESULTS LOADCASE LC1 24
RESULTS ELEMENT RE.EPXXG EPXX
PRESENT SYMBOL
PRESENT CONTOUR VALUES 0
We display an outline view of the full model without labels. Then we select
load case LC1 24, representing the last load step or the Ultimate Limit State
(ULS). Reinforcement results attribute EPXX represents the plastic strains εp .
Via the SYMBOL option we display these as symbols [Fig. 8.13a]. The size and
the color of the symbols (triangles) vary according to the represented value.
We also display a one-contour plot with a contour value 0 [Fig. 8.13b]. This
clearly indicates the plastic zones in red, i.e., where εp > 0. Both displays show
that yielding only occurs in the right end of the lower reinforcement bar in the
horizontal beam.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
142 Column–Beam Joint in a Portal Frame
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:01 plares.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:01 plarec.ps
Model: PORTAL Model: PORTAL
LC1: Load case 1 LC1: Load case 1
Step: 24 LOAD: 63.7 Step: 24 LOAD: 63.7
Element RE.EPXXG EPXX Element RE.EPXXG EPXX
Max = .597E-2 Max = .597E-2
Min = -.16E-2 Min = -.16E-2
Symbol factor = 1
All values
.53E-2
.455E-2
.379E-2
.303E-2
Y .227E-2 Y
.152E-2
.758E-3
0
Z X -.758E-3 Z X
-.152E-2 0
(a) symbol representation (b) plastic zones
Figure 8.13: Plastic strain in reinforcements (ULS)
Elements for reinforcements portal.fvc
VIEW EDGES
LABEL MESH ELEMENTS VIEWMODE RED
To get the elements that model the reinforcement bars we display the mesh with
element numbers [Fig. 8.14.] With a bit of zooming in we note that the elements
for the lower bar in the horizontal beam are 140 to 154 and for the upper bar
155 to 172.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:01 frael.ps
Model: PORTAL
15554
53
12615655
15756
15887
15988
160161162 163 92
89 90 91 164 93
165 94
166 95
167 96
168 169
109 170
110 171
111 172
112
49 50 51 52
125 13977 78 79 80 81 82 83 84 85 86 105 106 107 108
45 46 47 48
124 13867 68 69 70 71 72 73 74 75 76 101 102 103 104
41 42 43 44
123 137
14057
14158 59 60 61
142143144 145 62
146 63
147 64
148 65
149 66
150 97
151 98
152 99
153 100
154
1 11 21 31
122 136
2 12 22 32
121 135
3 13 23 33
120 134
4 14 24 34
119 133
5 15 25 35
118 132
6 16 26 36
117 131
7 17 27 37
116 130
8 18 28 38
115 129
9 19 29 39
114 128
Y
10 20 30 40
113 127
Z X
Figure 8.14: Element numbers
Graphs of plastic strain and total stress portal.fvc
PRESENT GRAPH LINE ELEMENTS LIST 140 TO 154
RESULTS ELEMENT RE.SXX.G SXX
PRESENT GRAPH LINE ELEMENTS LIST 155 TO 172
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
8.2 Nonlinear Analysis 143
We display a graph of the distribution of the currently selected results attribute,
i.e., the plastic strain, along the lower reinforcement bar [Fig. 8.15a]. Note that
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:01 plareg.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:01 frasxx.ps
Model: PORTAL Model: PORTAL
LC1: Load case 1 LC1: Load case 1
Step: 24 LOAD: 63.7 Step: 24 LOAD: 63.7
Element RE.EPXXG EPXX Element RE.SXX.G SXX
Max/Min on whole graph: Max/Min on whole graph:
Ymax = .219E-2 Ymax = 422
Ymin = 0 Ymin = -131
*1E-3 Xmax = 674 Xmax = 764
Xmin = 0 Xmin = 0
2.25 Variation along a line 500 Variation along a line
Mean value used for each element Mean value used for each element
2
E 400
E
L L
E 1.75 E
M M 300
E
N 1.5 E
T N
T
R 1.25 200
E R
E
. .
E 1
S 100
P X
X X
X .
G .75 G
0
E S 0 100 200 300 400 500 600 700 800
P .5
X
X X
X -100
.25
0 -200
0 100 200 300 400 500 600 700 DISTANCE
DISTANCE
(a) plastic strain in lower bar (b) total stress in upper bar
Figure 8.15: Plasticity in horizontal reinforcement bars (ULS)
the bar itself is specified as a polyline via the LIST option with element numbers.
The graph confirms the distribution of the plastic strains as displayed on the
model [Fig. 8.13].
Finally, we select results attribute SXX which represents the total stresses
in the reinforcements. We display their distribution along the upper bar as a
graph [Fig. 8.15b]. In the results monitor we see a maximum value of 422 which
is well below the yield stress σy = 450 MPa. This confirms the elastic state of
the entire upper bar as displayed in the contour plot [Fig. 8.13b].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
144 Column–Beam Joint in a Portal Frame
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
Chapter 9
Reinforced Concrete Slab
Name: Maekawa
Path: /Examples/ConcMas/Maekawa
Keywords: analys: nonlin physic. constr: suppor. elemen: cq40s
curved grid reinfo shell taper. load: deform. materi: elasti
harden isotro linear maekaw multil plasti soften strain vonmis
work. option: bfgs direct newton nonsym regula secant units.
post: binary femvie. pre: femgen. result: cauchy crack
displa force green plasti princi reacti strain stress total.
25 15
F
50 70
100
Z 25
15
1800 Y X
1800 Y X
(a) three-dimensional model and load (b) reinforcement location
Figure 9.1: Reinforced concrete slab [mm]
This example illustrates the use of the Modified Maekawa concrete model for
describing reinforced concrete behavior in both the tensile and the compressive
regime. We will apply the Diana-Maekawa model to describe the concrete slab
behavior under an out of plane loading [Fig. 9.1].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
146 Reinforced Concrete Slab
Model and loading. The structure consists of a square 1800×1800 mm con-
crete slab with a thickness of 100 mm and vertically supported along the edges
[Fig. 9.1a]. The slab is subjected to a point load at the center, perpendicular to
the slab surface.
Concrete and reinforcement properties. For the plain concrete we will
assume a Young’s modulus E = 28300 MPa, a Poisson’s ratio ν = 0.2, and
a compressive strength fc = 37 MPa. For the steel of the bar reinforcements
we assume Von Mises plasticity with work hardening, a Young’s modulus E =
2.1×105 MPa and a yield stress σy = 380 MPa.
The reinforcement bars are located in four layers [Fig. 9.1b]: the bars in X-
direction at a distance of 25 mm from the outer surfaces of the slab, and the
bars in Y -direction at distance of 15 mm. The steel percentages are 0.78% for
each of the four layers.
9.1 Finite Element Model
Due to the symmetry of this model we may limit ourselves to model only one
quarter of the slab: both X and Y from 0 to 900. Therefore we start iDiana
and enter the Design environment to make the finite element model for this
example, named SLAB.
iDiana
FEMGEN SLAB
Analysis and Units
Analysis Selection
Model Type: →Structural 3D
Units Definition
Length: →Millimeter
Mass: →Kilogram
Time: →Second
In the Analysis and Units dialog we indicate that this is a three-dimensional
model for structural analysis because we will apply shell elements. Furthermore
we indicate that we will apply the units mm, kg, s.
9.1.1 Slab Geometry
We simply specify the geometry of the quarter slab by a single surface between
the corner points.
slab.fgc
GEOMETRY POINT 0.0 0.0 50.0
GEOMETRY POINT 900.0 0.0 50.0
GEOMETRY POINT 900.0 900.0 50.0
GEOMETRY POINT 0.0 900.0 50.0
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
9.1 Finite Element Model 147
EYE FRAME
GEOMETRY SURFACE 4POINTS P1 P2 P3 P4
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY SURFACES ALL VIOLET
LABEL GEOMETRY POINTS ALL RED
LABEL GEOMETRY LINES ALL RED
We display the defined geometry and the surface name in violet, and the point
and line names in red [Fig. 9.2].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:38:04 geom.ps
Model: SLAB
Analysis: DIANA
Model Type: Structural P4
3D L3 P3
L4
S1
L2
Z X P1 L1 P2
Figure 9.2: Defined geometry of slab
9.1.2 Concrete Properties and Thickness
The properties and thickness of the concrete can be specified via the Property
Manager dialog.
iDiana
View →Property Manager...
↑
Property Manager
↑Materials Material Name: MA1
↑Linear Elasticity →Isotropic
↑Static Nonlinearity →Concrete and brittle materials →Mod. Maekawa concrete model
→Total Strain fixed crack →Constant shear retention
→Linear softening in tension →No crack-reclosing option
↑Physical Properties Physical Property Name: PH1
↑Geometry →Curved Shell →Regular
We define a material MA1. First we specify the linear elastic isotropic values:
Young’s modulus E = 28300 and Poisson’s ratio ν = 0.2. Then we specify the
properties for static nonlinearity: a correction factor for plasticity evaluation
of 1.0, a shear retention factor β = 0.10, a compressive strength fc = 37, a
tensile strength ft = 2.55, a Mode-I fracture energy GIf = 0.2307, and a crack
bandwidth h = 100. We define a physical property PH1: a thickness of 100.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
148 Reinforced Concrete Slab
Properties assignment slab.fgc
PROPERTY ATTACH S1 MA1 PH1
Finally we assign the specified properties to the geometric surface S1 which
models the concrete slab.
9.1.3 Meshing
Now we let iDiana generate the mesh for this model.
slab.fgc
MESHING TYPES ALL QU8 CQ40S
MESHING DIVISION SURFACE S1 8 8
MESHING GENERATE
VIEW MESH
First we indicate that the model must be meshed with CQ40S shell elements.
Because these elements have mid-side nodes we specify eight divisions along the
surface edges to get a 4×4 mesh. Finally we display a two-dimensional view of
the mesh in the default style [Fig. 9.3a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:38:04 mesh.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:38:04 reinfo.ps
Model: SLAB Model: SLAB
Analysis: DIANA Analysis: DIANA
Model Type: Structural 3D Model Type: Structural 3D
Y
Z
Y
Z X
X
(a) generated mesh of slab (b) reinforcement grids
Figure 9.3: Finite element model
9.1.4 Reinforcement Grids
We specify the location of the grids by their distance from the mid plane of the
slab: 35 mm for the outer grids and 25 mm for the inner grids.
slab.fgc
REINFORCE GRID SECTION S1 SURFACE -35.0
REINFORCE GRID SECTION S1 SURFACE -25.0
REINFORCE GRID SECTION S1 SURFACE 25.0
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
9.1 Finite Element Model 149
REINFORCE GRID SECTION S1 SURFACE 35.0
REINFORCE GRID GRID1 RE1
REINFORCE GRID GRID2 RE2
REINFORCE GRID GRID3 RE3
REINFORCE GRID GRID4 RE4
Note that each grid consists of a single section which covers the entire slab, i.e.,
surface S1. To verify the position of the grids we make a bird’s-eye view of the
model.
slab.fgc
EYE ROTATE TO 45 30 30
VIEW REINFORCE +GRID1 BLUE
VIEW REINFORCE +GRID2 RED
VIEW REINFORCE +GRID3 RED
VIEW REINFORCE +GRID4 BLUE
These commands display the finite element model which is the slabs’ mid plane
(green) and confirm the correct positions of the outer grids (blue) and the inner
grids (red) [Fig. 9.3b].
9.1.5 Steel Amount and Properties
We define the properties of the reinforcement steel and the amount of reinforce-
ment steel via the Property Manager dialog.
Material properties iDiana
View →Property Manager...
↑
Property Manager
↑ Materials Material Name: MA2
↑Linear Elasticity →Reinforcement →Reinforcement Bonded
↑Static Nonlinearity →Reinforcement →Von Mises Plasticity → Work Hardening Diagram
We define a material MA2 with Young’s modulus E = 210000. We submit the
hardening diagram for the reinforcement steel via an external file in Diana batch
format of which we specify the name: steel.dat in this case. The contents of
this file are as follows.
steel.dat
HARDIA 3.8E2 0.0 3.8E3 0.1
This input data indicates a linear work hardening diagram [Fig. 9.4].
Physical properties iDiana
Property Manager
↑Physical Properties Physical Property Name: PH2
↑Geometry →Embedded Reinforcements →Grid
Physical Properties Physical Property Name: PH3
↑Geometry →Embedded Reinforcements →Grid
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
150 Reinforced Concrete Slab
σy
3800
380
0 κ
0 0.1
Figure 9.4: Hardening diagram for reinforcement steel
We define a physical property PH2 for the grid with the bars in X-direction: we
specify an equivalent thickness in x-direction of 0.78, an equivalent thickness
in y-direction of 0., and the x-axis components (1.,0.,0.) for the global X-
direction. We also define property PH3 for the grid with the bars in Y -direction:
an equivalent thickness in x-direction of 0., an equivalent thickness in y-direction
of 0.78, and the x-axis components (1.,0.,0.) for the global X-direction.
Properties assignment slab.fgc
PROPERTY ATTACH GRID1 MA2 PH3
PROPERTY ATTACH GRID2 MA2 PH2
PROPERTY ATTACH GRID3 MA2 PH2
PROPERTY ATTACH GRID4 MA2 PH3
Finally we assign the steel material to all the grids and the two sets of physical
properties to the appropriate grids.
9.1.6 Boundary Constraints
The boundary constraints of the model are twofold: (1) a fixed displacement of
the center point of the complete plate which simulates the vertical force F and,
(2) the vertical supports and symmetry constraints along the edges of the slab.
Fixed displacement slab.fgc
PROPERTY LOADS DISPLACE P3 -1.0 Z
VIEW MESH
LABEL MESH LOADS ALL
These commands define a fixed unit displacement of point P3 in the negative
Z-direction. Note that point P3 actually is the center of the complete slab.
We redisplay the mesh to remove the displayed reinforcement grids, and then
display the displacement as a violet arrow [Fig. 9.5a].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
9.2 Nonlinear Analysis 151
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:38:05 load.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:38:05 bcons.ps
Model: SLAB Model: SLAB
Analysis: DIANA Analysis: DIANA
Model Type: Structural 3D Model Type: Structural 3D
Z Z
Y Y
X X
(a) fixed displacement (b) supports and symmetry constraints
Figure 9.5: Boundary constraints
Supports and symmetry constraints slab.fgc
PROPERTY BOUNDARY CONSTRAINT L1 Z
PROPERTY BOUNDARY CONSTRAINT L4 Z
PROPERTY BOUNDARY CONSTRAINT L2 X RY
PROPERTY BOUNDARY CONSTRAINT L3 Y RX
LABEL MESH OFF
LABEL MESH CONSTRNT
Along lines L1 and L4 we suppress the Z-displacement to model the vertical sup-
port. Along lines L2 and L3 we specify the symmetry conditions, one translation
and one rotation respectively uX = 0, φY = 0, and uY = 0, φX = 0. Note that
it is not necessary to specify φZ = 0 because the shell elements have no such
degree of freedom. Finally we verify the constraints by letting iDiana display
these as red spikes [Fig. 9.5b].
9.2 Nonlinear Analysis
Loading. In the nonlinear analysis we will apply the load, i.e., the displace-
ment of the center of the slab, as depicted in Figure 9.6. In total, 101 loading
load
2.0
1.5
1.0
0.5
0
1 21 31 51 61 81 101 steps
Figure 9.6: Loading program applied on the concrete slab
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
152 Reinforced Concrete Slab
steps will be applied in a three-cycle sawtooth pattern: 20 steps of 0.05 in
downward direction followed by 10 steps of −0.05 in upward direction. After
the third loading cycle the loading point is moved upward to a position of −1.0.
Analysis commands and options. To perform the nonlinear analysis of
model SLAB we write a input data file in Diana batch format.
iDiana
UTILITY WRITE DIANA
yes
FILE CLOSE
yes
Reinforced concrete slab
ANALYSE SLAB
Analysis Setup
···
We close the model and launch the Analysis Setup dialog where we activate the
batch commands for nonlinear analysis.
Preliminary slab.dcf
*FILOS
INITIA
*INPUT
*NONLIN
TYPE PHYSIC
BEGIN OUTPUT FEMVIEW
DISPLA
FORCE REACTI
STRESS PRINCI INTPNT
STRAIN PLASTI PRINCI INTPNT
STRAIN CRACK INTPNT
END OUTPUT
With the preliminary commands we perform some tasks which must precede
the actual execution of load steps.
Loading slab.dcf
BEGIN EXECUT
BEGIN LOAD
BEGIN STEPS
BEGIN EXPLIC
SIZE 0.0
END EXPLIC
END STEPS
LOADNR=1
END LOAD
END EXECUT
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
9.2 Nonlinear Analysis 153
BEGIN EXECUT
BEGIN LOAD
STEPS EXPLIC SIZES 0.05(20) -0.05(10) 0.05(20) -0.05(10) 0.05(20) \
-0.05(20)
LOADNR=1
END LOAD
BEGIN ITERAT
METHOD SECANT
MAXITE=50
BEGIN CONVER
ENERGY CONTIN TOLCON=0.0001
FORCE OFF
DISPLA OFF
END CONVER
END ITERAT
END EXECUT
*END
The load steps are specified according to Figure 9.6. For the reinforcement grids
no results are calculated. During the first loading stage (up to the 21st load
step) it is interesting to monitor the growth of the plastic and the cracking re-
gions. These regions are strongly related to the distribution of the compressive
and tensile stresses. To illustrate the capability of the Diana-Maekawa model
in describing both (large deformation) plasticity and cracking which occur si-
multaneously during out-of-plane loading of the slab we will show the growth
of plastic and cracking regions at various steps.
As soon as the analysis has been terminated we enter the iDiana Results
environment with the model name to assess the analysis results.
slab.fvc
FEMVIEW SLAB
CONSTRUCT SET CSLAB APPEND ELEMENTS 1 TO 16
VIEW MESH CSLAB
EYE ANGLE 0 0
First we put all the elements of the concrete slab in a set called CSLAB. We
display the undeformed mesh of the slab in the default green ‘wire netting’
style, without the reinforcements. We also specify a viewing direction from
Z = ∞ to the origin of the model XY Z-axes system. We will now display the
results of step 11, 21, 31, and 81.
Step 11 slab.fvc
RESULTS LOADCASE LC1 11
RESULTS RANGE SURFACE TOP
RESULTS GAUSSIAN EL.EKNN1 EKNN
PRESENT OPTION DISC MODULATE 10
PRESENT DISC
RESULTS RANGE SURFACE BOTTOM
PRESENT DISC
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
154 Reinforced Concrete Slab
RESULTS GAUSSIAN EL.S1 S1
RESULTS RANGE SURFACE TOP
PRESENT OPTION VECTOR MODULATE 10
PRESENT VECTOR
RESULTS RANGE SURFACE BOTTOM
PRESENT VECTOR
RESULTS GAUSSIAN EL.EP1 EP3
RESULTS RANGE SURFACE TOP
PRESENT CONTOUR FROM 0 to -0.2E-4 LEVELS 10
First we select load case LC1 11 which represents the results of step 11. Then we
select the crack-strain results in normal direction to the cracks: attribute EKNN
in the integration points (first crack in integration point). These crack-strains
represent how much the cracks are opened. A suitable display option for cracks
is DISC which shows them as disks. These disks have the same orientation as
the cracks and their color indicates the opening of the crack.
Secondly we select the result S1 in the integration points, which is the first
principal stress σ1 , i.e., the most positive (tensile) principal stress. These results
are visualized as vectors, oriented in the direction of the principal stress and with
size and color modulated according to the magnitude of the stress.
The third result that we select is EP3 which represents the third principal
plastic strain εp.3 , i.e., the most negative (compressive) plastic strain. These
results are displayed as contour plots, scaled by the plastic strain at step 81.
Steps 21, 31, and 81. By selecting load case LC1 21, LC1 31, and LC1 81,
followed by the same commands as shown above we get the same results dis-
played for steps 21 (extreme loading in first cycle), 31 (end of first cycle), and
81 (extreme loading in third cycle).
9.2.1 Results for Step 11
The slab is supported in Z-direction at the outer edges, and free to curve in
Z-direction at the symmetry edges. Therefore it will globally deform as a bowl.
This results in compression at the top surface and tension in radial direction at
the bottom surface. However, because the corners of the slab are restricted to
move upward, we may expect bending effects in the opposite direction there.
We find a nice symmetric crack distribution at the bottom surface of the
slab [Fig. 9.7a-bottom]. The largest crack opening occurs close to the midpoint
of the slab, where the curvature is largest. The direction of the first principal
stress in the bottom surface appears to be perpendicular to the crack directions
[Fig. 9.7b-bottom]. The principal stresses are all less than, or equal to 2.55
which is the value specified for the tensile strength ft of concrete [§ 9.1.2 p. 147].
In the top surface of the slab no cracks can be noticed yet [Fig. 9.7a-top]. The
highest tensile stress can be found near the corners of the slab in radial direction
[Fig. 9.7b-top].
The plastic strain in both surfaces is very small [Fig. 9.7c], while over the
major part in the bottom surface it is even equal to zero. Note that the Maekawa
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
9.2 Nonlinear Analysis 155
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:23 cr_11t.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:23 s1_11t.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:23 ep3_11t.ps
Model: SLAB Model: SLAB Model: SLAB
LC1: Load case 1 LC1: Load case 1
Step: 11 LOAD: .5 Step: 11 LOAD: .5
Gauss EL.S1 S1 Gauss EL.EP1 EP3
Top (last) surface Top (last) surface
Max = 1.5 Max = -.403E-10
Min = .828E-2 Min = -.22E-6
Factor = 51.4 Results shown:
Mapped to nodes
-.2E-4
-.182E-4
-.164E-4
1.35 -.145E-4
1.2 -.127E-4
1.05 -.109E-4
Y Y .902 Y -.909E-5
.753 -.727E-5
.604 -.545E-5
.455 -.364E-5
Z X Z X .306 Z X
-.182E-5
.157 0
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:23 cr_11b.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:23 s1_11b.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 ep3_11b.ps
Model: SLAB Model: SLAB Model: SLAB
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Step: 11 LOAD: .5 Step: 11 LOAD: .5 Step: 11 LOAD: .5
Gauss EL.EKNN1 EKNN Gauss EL.S1 S1 Gauss EL.EP1 EP3
Bottom (first) surface Bottom (first) surface Bottom (first) surface
Max = .958E-4 Max = 2.53 Min = .348 Max = -.497E-11
Min = .246E-4 Factor = 30.4 Min = -.246E-6
Results shown:
Mapped to nodes
-.2E-4
-.182E-4
-.164E-4
.887E-4 2.31 -.145E-4
.815E-4 2.09 -.127E-4
.744E-4 1.88 -.109E-4
Y .673E-4 Y 1.66 Y -.909E-5
.602E-4 1.44 -.727E-5
.531E-4 1.22 -.545E-5
.459E-4 1 -.364E-5
Z X .388E-4 Z X .784 Z X
-.182E-5
.317E-4 .566 0
(a) cracks (b) max. tensile stress (c) max. compressive strain
Figure 9.7: Results for step 11 at top and bottom surface
model only generates plastic strain under compressive loadings.
9.2.2 Results for Step 21
At step 21 the crack pattern as found in step 11 has extended considerably in the
bottom surface whereas the top surface is still uncracked [Fig. 9.8a]. However,
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 cr_101t.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 s1_101t.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 ep3_101t.ps
Model: SLAB Model: SLAB Model: SLAB
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Step: 21 LOAD: 1 Step: 21 LOAD: 1 Step: 21 LOAD: 1
Gauss EL.EKNN1 EKNN Gauss EL.S1 S1 Gauss EL.EP1 EP3
Top (last) surface Top (last) surface Top (last) surface
Max = .501E-4 Max = 2.5 Max = -.175E-9
Min = 0 Min = .153E-1 Min = -.845E-5
Factor = 30.8 Results shown:
Mapped to nodes
-.2E-4
-.182E-4
-.164E-4
.451E-4 2.25 -.145E-4
.401E-4 2 -.127E-4
.351E-4 1.76 -.109E-4
Y .301E-4 Y 1.51 Y -.909E-5
.251E-4 1.26 -.727E-5
.2E-4 1.01 -.545E-5
.15E-4 .761 -.364E-5
Z X .1E-4 Z X .512 Z X
-.182E-5
.501E-5 .264 0
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 cr_101b.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 s1_101b.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 ep3_101b.ps
Model: SLAB Model: SLAB Model: SLAB
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Step: 21 LOAD: 1 Step: 21 LOAD: 1 Step: 21 LOAD: 1
Gauss EL.EKNN1 EKNN Gauss EL.S1 S1 Gauss EL.EP1 EP3
Bottom (first) surface Bottom (first) surface Bottom (first) surface
Max = .382E-3 Max = 2.55 Min = .648 Max = -.147E-10
Min = .144E-5 Factor = 30.2 Min = -.984E-6
Results shown:
Mapped to nodes
-.2E-4
-.182E-4
-.164E-4
.344E-3 2.36 -.145E-4
.306E-3 2.17 -.127E-4
.268E-3 1.98 -.109E-4
Y .23E-3 Y 1.79 Y -.909E-5
.192E-3 1.6 -.727E-5
.154E-3 1.41 -.545E-5
.116E-3 1.22 -.364E-5
Z X .776E-4 Z X 1.03 Z X
-.182E-5
.395E-4 .838 0
(a) cracks (b) max. tensile stress (c) max. compressive strain
Figure 9.8: Results for step 21 at top and bottom surface
the stress pattern has changed [Fig. 9.8b]. Around the midpoint of the slab
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
156 Reinforced Concrete Slab
the crack strains at the bottom have increased considerably. Because of the
softening behavior, the maximum stress in the normal direction has strongly
reduced. Hence, the maximum stress now works in another direction. In the
top surface near the corner point the maximum tensile stress is nicely limited
to the tensile strength of the concrete [Fig. 9.8b-top]. Moreover, we observe
strong plastic deformations at the top surface around the midpoint of the slab
[Fig. 9.8c-top].
9.2.3 Results for Step 31
At step 31 the load has again been reduced to half the value of the prescribed
displacement at step 21. The crack patterns for step 31 [Fig. 9.9a] are almost
identical to those of step 21. However, the legend indicates that the crack strains
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 cr_151t.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 s1_151t.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 ep3_151t.ps
Model: SLAB Model: SLAB Model: SLAB
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Step: 31 LOAD: .5 Step: 31 LOAD: .5 Step: 31 LOAD: .5
Gauss EL.EKNN1 EKNN Gauss EL.S1 S1 Gauss EL.EP1 EP3
Top (last) surface Top (last) surface Top (last) surface
Max = .703E-4 Max = .212 Max = -.173E-9
Min = 0 Min = -.616E-1 Min = -.845E-5
Factor = 362 Results shown:
Mapped to nodes
-.2E-4
-.182E-4
-.164E-4
.633E-4 .185 -.145E-4
.563E-4 .158 -.127E-4
.492E-4 .13 -.109E-4
Y .422E-4 Y .103 Y -.909E-5
.352E-4 .754E-1 -.727E-5
.281E-4 .48E-1 -.545E-5
.211E-4 .206E-1 -.364E-5
Z X .141E-4 Z X -.682E-2 Z X
-.182E-5
.703E-5 -.342E-1 0
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 cr_151b.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 s1_151b.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 ep3_151b.ps
Model: SLAB Model: SLAB Model: SLAB
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Step: 31 LOAD: .5 Step: 31 LOAD: .5 Step: 31 LOAD: .5
Gauss EL.EKNN1 EKNN Gauss EL.S1 S1 Gauss EL.EP1 EP3
Bottom (first) surface Bottom (first) surface Bottom (first) surface
Max = .238E-3 Max = .355 Max = -.147E-10
Min = .495E-4 Min = -.261E-1 Min = -.984E-6
Factor = 217 Results shown:
Mapped to nodes
-.2E-4
-.182E-4
-.164E-4
.219E-3 .317 -.145E-4
.2E-3 .279 -.127E-4
.182E-3 .241 -.109E-4
Y .163E-3 Y .203 Y -.909E-5
.144E-3 .164 -.727E-5
.125E-3 .126 -.545E-5
.106E-3 .883E-1 -.364E-5
Z X .873E-4 Z X .502E-1 Z X
-.182E-5
.684E-4 .121E-1 0
(a) cracks (b) max. tensile stress (c) max. compressive strain
Figure 9.9: Results for step 31 at top and bottom surface
are zero which means that the cracks are fully closed. The stress pattern of step
31 at the bottom surface is different from step 11, which has the same load
factor, because the model has been cracked in step 31 [Fig. 9.9b]. The plastic
strains [Fig. 9.9c] are almost identical to those of step 21. This could be expected
because plastic deformation can only occur with increasing loading.
9.2.4 Results for Step 81
The results for step 81 show patterns similar to those for step 21 [Fig. 9.10],
except that there more cracks in the bottom surface and now also the top
surface has been cracked.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
9.2 Nonlinear Analysis 157
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 cr_401t.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 s1_401t.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 ep3_401t.ps
Model: SLAB Model: SLAB Model: SLAB
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Step: 81 LOAD: 2 Step: 81 LOAD: 2 Step: 81 LOAD: 2
Gauss EL.EKNN1 EKNN Gauss EL.S1 S1 Gauss EL.EP1 EP3
Top (last) surface Top (last) surface Top (last) surface
Max = .195E-3 Max = 2.52 Max = -.744E-9
Min = .397E-5 Min = .578E-2 Min = -.233E-4
Factor = 30.6 Results shown:
Mapped to nodes
-.2E-4
-.182E-4
-.164E-4
.176E-3 2.27 -.145E-4
.157E-3 2.01 -.127E-4
.138E-3 1.76 -.109E-4
Y .119E-3 Y 1.51 Y -.909E-5
.995E-4 1.26 -.727E-5
.804E-4 1.01 -.545E-5
.613E-4 .759 -.364E-5
Z X .422E-4 Z X .508 Z X
-.182E-5
.231E-4 .257 0
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 cr_401b.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 s1_401b.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 ep3_401b.ps
Model: SLAB Model: SLAB Model: SLAB
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Step: 81 LOAD: 2 Step: 81 LOAD: 2 Step: 81 LOAD: 2
Gauss EL.EKNN1 EKNN Gauss EL.S1 S1 Gauss EL.EP1 EP3
Bottom (first) surface Bottom (first) surface Bottom (first) surface
Max = .851E-3 Max = 2.53 Min = 1.01 Max = -.288E-10
Min = .274E-5 Factor = 30.3 Min = -.385E-5
Results shown:
Mapped to nodes
-.2E-4
-.182E-4
-.164E-4
.766E-3 2.38 -.145E-4
.681E-3 2.23 -.127E-4
.596E-3 2.08 -.109E-4
Y .512E-3 Y 1.92 Y -.909E-5
.427E-3 1.77 -.727E-5
.342E-3 1.62 -.545E-5
.257E-3 1.46 -.364E-5
Z X .172E-3 Z X 1.31 Z X
-.182E-5
.875E-4 1.16 0
(a) cracks (b) max. tensile stress (c) max. compressive strain
Figure 9.10: Results for step 81 at top and bottom surface
9.2.5 Deformation
The following commands display the deformed shape for step 81 (which was
already selected for the last plot).
slab.fvc
VIEW MESH CSLAB
EYE ANGLE -77 20
RESULTS NODAL TDTX...G RESTDT
PRESENT SHAPE
First we display the undeformed mesh under an appropriate viewing angle, by
default in green. Then we select the TDT results attribute which represents
the total displacements of the nodes. Finally the SHAPE option displays the
deformed shape of the mesh, by default in red, with an appropriate scaling
factor for the displacements [Fig. 9.11a].
9.2.6 Load–Displacement Diagram
Finally we display the load–displacement diagram between the point load and
the vertical displacement of the mid-point of the slab.
slab.fvc
PRESENT GRAPH RESULTS
NODAL TDTX...G TDTZ
1
NODAL FBX....G FBZ
LOADCASES
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
158 Reinforced Concrete Slab
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 shape401.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:24 lod-def.ps
Model: SLAB Model: SLAB
LC1: Load case 1 Max/Min on whole graph:
Step: 81 LOAD: 2 Ymax = .187E5 Ymin = 0
Nodal TDTX...G RESTDT Xmax = 0 Xmin = -2
Max/Min on model set: Variation over loadcases
Max = 2 Node 25
Min = .153E-1
Factor = 38.5 *1E4
2
1.8
N 1.6
O
D
A 1.4
L
F 1.2
B
X 1
.
.
. .8
.
G
.6
F
B
Z .4
.2
0
-2.25 -2 -1.75 -1.5 -1.25 -1 -.75 -.5 -.25 0
Z NODAL TDTX...G TDTZ
Y
X
(a) for step 81 (b) load–displacement diagram
Figure 9.11: Deformation
LC1
25
We activate graph presentation of results. For the horizontal axis we select the
total displacements. The we indicate that we have a single vertical axis which
represents the total load in Z-direction FBZ. Finally we indicate that the graph
must be plotted over all load cases and for node 25. Now iDiana plots the graph
[Fig. 9.11b]. The concrete slab is subjected to the concentrated load, increased
and reduced alternatively, until the vertical displacement of the mid-point is
approximately 2 mm, i.e., 2% of the slab thickness. Then it is unloaded until
the external load is approximately zero.
The diagram shows that hysteresis has occurred during loading–unloading
of the slab. We also can observe a typical characteristic of the Maekawa com-
pression model: the unloading directions change with increasing maximum de-
formations ever experienced.
9.3 Concluding Remarks
Based on this example we have demonstrated the capability of the Diana-
Maekawa model to describe the reinforced concrete behavior in both compres-
sive regime and tensile regime. Besides, we have also shown that the Diana-
Maekawa model is capable of describing (nonlinear) deformation behavior of
reinforced concrete, in which plasticity, cracking and hysteresis occur simulta-
neously.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
Chapter 10
Fire near Concrete Safety
Tank
Name: FiTank
Path: /Examples/ConcMas/FiTank
Keywords: analys: linear static. constr: suppor. elemen: axisym cl12i
cq16a grid interf reinfo struct taper. load: edge elemen force
prestr reinfo weight. materi: elasti isotro. option: direct
groups units. post: binary femvie. pre: femgen. result:
cauchy displa stress total. analys: flow flowst heat nonlin
stagge transi. constr: initia suppor temper. elemen: axisym
b2aht cl12i cq16a flow interf potent q4aht struct taper. load:
edge elemen flux force prestr reinfo temper time weight. ma-
teri: capaci compli conduc consta crack creep cutoff drucke
elasti isotro linear plasti retent smear soften temper transi von-
mis. option: direct groups units. post: binary femvie. pre:
femgen. result: flux temper total. analys: flow flowst heat
nonlin physic stagge transi. constr: initia suppor temper. el-
emen: axisym b2aht cl12i cq16a flow grid interf potent q4aht
reinfo struct taper. load: edge elemen flux force prestr re-
info temper time weight. materi: capaci compli conduc consta
crack creep cutoff drucke elasti harden isotro linear plasti re-
tent smear soften strain temper transi vonmis. option: direct
groups newton regula units. post: binary femvie tabula. pre:
femgen. result: cauchy crack creep displa elasti flux green
plasti strain stress temper total.
In this example we will analyze a concrete safety tank for the storage of liquefied
natural gas (lng) [Fig. 10.1]. The tank consists of an inner steel tank and an
outer concrete safety tank. Under normal service conditions the lng will be
contained in the inner steel tank. The steel tank is not taken into account in
this example. We concentrate on the outer concrete safety tank, which will
be loaded in case of leakage of the steel tank. The initial load consists of the
gravity and the prestress by the prestressing cables. The concrete structure will
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
160 Fire near Concrete Safety Tank
♥
dome
300
beam
1452
225
39200
30000
wall
450
Y 960
800
floor
430 X
24775
Figure 10.1: Safety tank – idealized model [mm]
be loaded on the floor by a hydrostatic pressure. In case of leakage of the inner
tank the wall of the safety tank will also be loaded by the hydrostatic pressure.
We will also subject this model to a nonlinear staggered flow–stress analysis of
a fire load.
10.1 Model for Linear Structural Analysis
We will model the concrete tank with CQ16A axisymmetric elements with a
reinforcing grid and CL12I interface elements for the foundation. We now enter
the iDiana Design environment to build the model.
iDiana
FEMGEN TANK
Analysis and Units
Analysis Selection
Model Type: →Structural Axisymmetric
Units Definition
Length: →Millimeter
Mass: →Kilogram
Time: →Second
Temperature: →Celsius
In the Analysis and Units dialog we indicate that the model is for axisymmetric
structural analysis and that we will apply the mm-kg-s-°C unit system.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.1 Model for Linear Structural Analysis 161
tankli.fgc
DRAWING CONTENTS MONITOR OFF
CONSTRUCT SPACE WORK-BOX SIZE 26200 40400 0
EYE FRAME WORK-BOX
CONSTRUCT PARAMETER TFLOOR 800
CONSTRUCT PARAMETER TFLOORN -800
CONSTRUCT PARAMETER TWALL 450
CONSTRUCT PARAMETER HWALL 30000
CONSTRUCT PARAMETER HBEAM 1452
CONSTRUCT PARAMETER TDOME 300
To get a clean viewport during preprocessing we switch off the results monitor.
To achieve that the model to be build immediately fits in the viewport of the
iDiana window we specify a ‘workbox’ which surrounds the outer limits of the
model. We arrange a proper fit of the workbox in the viewport. Finally we
assign some values to parameters that we will use in the subsequent modeling
commands: TFLOOR for the floor thickness, TFLOORN for the thickness in the
−Y -direction, TWALL for the wall thickness, HWALL for the height of the wall,
HBEAM for the height of the beam, and TDOME for the dome thickness.
We will describe the commands that actually build the model in separate
sections: the floor [§ 10.1.1], the wall [§ 10.1.2], the beam [§ 10.1.3], the dome
[§ 10.1.4], the foundation interface [§ 10.1.5], and the reinforcements [§ 10.1.6].
10.1.1 Floor
The floor is a simple rectangle with dimension 26185×800 mm. However, despite
its simple geometry, we must pay attention to the position of the wall. To get
a consistent mesh there must be geometric points directly below the wall.
Top surface tankli.fgc
GEOMETRY POINT P1 0 TFLOOR
GEOMETRY SWEEP P1 P2 -930 TRANSLATE 24775 0 0 DEPENDENT
GEOMETRY SWEEP P2 P3 TRANSLATE TWALL 0 0 DEPENDENT
GEOMETRY SWEEP P3 P4 204 TRANSLATE 960 0 0 DEPENDENT
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY POINTS
LABEL GEOMETRY LINES ALL VIOLET
First we define a point P1 on the floor top surface at the upper left corner
directly with its coordinates in the two-dimensional XY -space (Z = 0). Then
we sweep this point along the top surface: to point P2 at the inner side of the
wall. We declare the translation to be dependent on the original point: should
we ever move that, then iDiana will keep the distance between the two points.
The sweep operation also creates a line L1 where the value of -930 specifies
the fineness of the mesh along the new line: thirty divisions and, due to the -9,
a strongly decreasing division, i.e., a gradual mesh refinement toward the end
of the line. Because CQ16A elements have midside nodes, each element requires
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
162 Fire near Concrete Safety Tank
two divisions. Therefore we must specify twice as much divisions as we want to
have elements along a line.
A second sweep to the right of P2 along the wall thickness creates point P3
and line L2. Here we let iDiana apply the default division in four equal parts.
The last sweep along the ‘overhang’ of the floor to the right of P3 (960 mm)
creates point P4 and line L3. The value of 204 yields four divisions with moderate
refinement toward the start of the line. Finally we display the currently defined
geometry with labels for points and lines [Fig. 10.2a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:29 geoflp.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:29 geofl.ps
Y Y
Z X P1 L1 P2
L2
P3P4
L3 Z X L7 L1
LCMB1 L2
L3
S1 L8
L4
LCMB2 L5
L6
(a) lines and points on top (b) lines and surface
Figure 10.2: Floor geometry
Thickness tankli.fgc
GEOMETRY LCMB LCMB1 L1 L2 L3
GEOMETRY SWEEP LCMB1 LCMB2 6 TRANSLATE 0 TFLOORN 0 DEPENDENT
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY LINES ALL VIOLET
LABEL GEOMETRY SURFACES
We assemble the lines in a ‘combined line’ via the LCMB option. To complete
the geometry of the floor we sweep the combined line downward over the floor
thickness and simultaneously specify a division of six equal parts. The sweeping
operation on a line not only creates a new line but also a surface S1. We display
the floor geometry in violet with labels for lines and surfaces [Fig. 10.2b].
Meshing tankli.fgc
MESHING TYPES 4SIDES QU8 CQ16A
MESHING GENERATE
VIEW MESH
On the created surface we generate a finite element mesh. We specify that
surfaces with four sides should be meshed with QU8 elements, i.e., eight-node
quadrilaterals for which we choose the specific CQ16A Diana element. Finally
we generate and display the mesh [Fig. 10.3a]. Note the refinement of the mesh
in horizontal direction toward the junction of wall and floor.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.1 Model for Linear Structural Analysis 163
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:29 meshfl.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:29 meshwa.ps
Y Y
Z X Z X
(a) floor (b) floor–wall
Figure 10.3: Floor and wall mesh
10.1.2 Wall
We may now continue with the modeling of the wall. Therefore we will first
define its geometry and then perform the meshing.
Geometry tankli.fgc
VIEW GEOMETRY ALL VIOLET
GEOMETRY SWEEP P2 TRANSLATE 0 HWALL 0 DEPENDENT
GEOMETRY SPLIT L9 P10 0.5
MESHING DIVISION L9 60
MESHING DIVISION L10 60
GEOMETRY LCMB LCMB3 L9 L10
GEOMETRY SWEEP LCMB3 TRANSLATE TWALL 0 0 DEPENDENT
First we switch from mesh display to geometry display. Then we sweep point
P2, the inner wall–floor junction, over the height of the wall which will create
the connecting line, automatically called L9.
Because we want to create more than 99 divisions along the wall, we split
the new line in two parts, which modifies line L9 and creates a new line L10. We
define the division of the lines with value 60 which in total will create 120 divi-
sions along the wall. Since further on in this chapter, we will apply quadratic
structural elements and linear boundary elements, gradual mesh refinement to-
wards the top and bottom ends of the wall is not applied. In iDiana gradual
mesh refinement using both linear and quadratic elements yields incompatible
results.
Prior to sweeping the new lines over the thickness of the wall we assemble
them in a new combined line called LCMB3. After the sweep, which creates a
surface S2, we may perform the meshing of the wall.
Meshing tankli.fgc
MESHING TYPES 4SIDES QU8 CQ16A
MESHING GENERATE
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
164 Fire near Concrete Safety Tank
VIEW MESH
We generate the mesh for the currently defined geometry. The mesh, as gener-
ated for floor and wall together, is then displayed [Fig. 10.3b]. Note the refine-
ment toward the floor–wall junction.
10.1.3 Beam
The modeling of the beam is a bit more complicated than that of the floor and
the wall. Figure 10.4 shows the points, lines and surfaces involved. First we will
demonstrate the definition of the geometry of the square surface S3 at the right
hand side of the beam. Then the tapered surface S4 will be defined. Finally we
will perform the meshing operation of the beam.
L26
P26 P14 P15 P16
L18 L32 L33 L16 L17 LCMB5 = L16 + L17
P27
S4
L23
L30 L31
S3 L24
L25 = L22 + L23
rin = 39570 P21
L22
L14 L15 LCMB4 = L14 + L15
P9 P13
P12
L10
Figure 10.4: Modeling the beam
Surface S3 tankli.fgc
VIEW GEOMETRY ALL VIOLET
GEOMETRY SWEEP P12 TRANSLATE 225 0 0
GEOMETRY LCMB LCMB4 L14 L15
GEOMETRY COPY LCMB4 LCMB5 TRANSLATE 0 HBEAM 0 DEPENDENT
GEOMETRY POINT PC 0 430 0
GEOMETRY LINE CIRCLE PC 39570
GEOMETRY POINT INTERSECT L10 L18
GEOMETRY SURFACE 4POINTS +P21 P14 +P15 P16 P13 +P12 P9
We start with sweeping point P12 along 225 mm in the X-direction. This creates
point P13 and line L15. The lines L14 and L15 are then combined to line LCMB4.
The combined line is then copied to a new combined line LCMB5 over the height
of the beam, which automatically creates points P14, P15 and P16, and lines L16
and L17.
The difficulty now is to find the intersection point of the inner dome and
wall surfaces (P21). The position of this point cannot be determined directly
from the dimensions of the idealized model [Fig. 10.1 p. 160]. The solution to
the problem is to let iDiana calculate the intersection of two lines. One of
these, L10, was already created during the modeling of the wall. The other
one, L18, is the inner circle line of the dome. We define the center of the
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.1 Model for Linear Structural Analysis 165
dome PC at XY -coordinate (0,430); the radius of the inner surface of the dome
rin = 39200 + 800 − 430 = 39570. With these two parameters we define a circle.
iDiana will create four lines for the circle of which the first one, L18, is the
northeasterly sector. Now we let iDiana determine the intersection point (P21).
Now that all required points have been determined, we specify a new surface
(S3). Note that we must terminate with a corner point.
Surface S4 tankli.fgc
GEOMETRY LINE CIRCLE PC 39870
GEOMETRY POINT INTERSECT P26 L16 L26
GEOMETRY LINE PC P26
GEOMETRY POINT INTERSECT P27 L30 L18
GEOMETRY LINE ARC P21 P27 PC 6
GEOMETRY SURFACE 4POINTS P21 P27 P26 P14
To define the tapered surface S4, which actually connects the beam to the dome,
we start with a circle with radius 39870 = rin + tdome (the northeasterly sector
becoming line L26). Then we let iDiana calculate the intersection point between
the circle and the top line of the beam (P26). The determination of point P27
requires a construction line from P26 to the center of the dome circles (L30).
The intersection of this line and the inner dome circle delivers point P27, the
last point needed to define the surface S4 via the 4POINTS option.
The 4POINTS option defines the surface with straight edges. Therefore
we must predefine the line L31 as a circular arc via the ARC option.
Meshing tankli.fgc
MESHING TYPES 4SIDES QU8 CQ16A
MESHING DIVISION L33 6
MESHING DIVISION L22 2
MESHING DIVISION L17 2
MESHING DIVISION L24 6
MESHING DIVISION L15 2
MESHING GENERATE
VIEW MESH
EYE ZOOM FACTOR 10 12000. 10000. 0.
First we specify how the surfaces must be meshed with respect to element types
and division. For lines not mentioned, iDiana will apply a default division of
four equal parts. We generate and display the mesh [Fig. 10.5a]. Because the
modeling of the beam was rather complicated we check the mesh by zooming-
in. Here we specify an enlargement of 10× and a shift of the eye to a position
just below the beam [Fig. 10.5b]. In a truly interactive session it would be
more handy to indicate a zoom window with the graphics cursor [Vol. Getting
Started].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
166 Fire near Concrete Safety Tank
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:30 meshbe.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:30 meshbez.ps
Y Y
Z X Z X
(a) overall display (b) zoomed-in on beam
Figure 10.5: Floor–wall–beam mesh
10.1.4 Dome
The inner and outer points at the zenith of the dome (P18 and P23) have been
created implicitly with the inner and outer circles of the dome when we defined
the beam geometry [§ 10.1.3]. Therefore we can now define the geometry of the
dome, without defining any new points or lines.
Surface S5 tankli.fgc
EYE FRAME
VIEW GEOMETRY ALL VIOLET
GEOMETRY LINE ARC P23 P26 PC 98
GEOMETRY LINE ARC P27 P18 PC 98
GEOMETRY SURFACE 4POINTS P23 P26 P27 P18
We revert to an overall display of the model. Once more we predefine the lines
of a new surface (S5) to be pure circular arcs. Like for the wall, we do not define
a meshing division for the dome either.
Meshing tankli.fgc
CONSTRUCT SET TANK APPEND SURFACES ALL
MESHING TYPES TANK QU8 CQ16A
MESHING GENERATE
VIEW MESH
For the sake of convenience we collect all the currently defined surfaces in a set
called TANK. Then we generate and display the mesh [Fig. 10.6].
10.1.5 Foundation Interface
The pile foundation is modeled in a smeared sense by means of a linear elastic
bedding. The reason for this is that the element size at the floor is too large to
model the piles individually by springs at nodal points. If the force on particular
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.1 Model for Linear Structural Analysis 167
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:30 meshdo.ps
Z X
Figure 10.6: Complete mesh for concrete tank
piles itself has to be analyzed by, for instance, spring elements at nodal points
then the element size at the floor should have been smaller than the distance
between the piles.
Note that the modeling of a bedding by springs at the nodal points will
generally not obtain the correct distributed support, due to the quadratic in-
terpolation function of the connected continuum elements. Using interface el-
ements for this purpose will automatically take account of the interpolation
scheme, while in addition the axisymmetric surface geometry of the bedding is
evaluated automatically.
tankli.fgc
VIEW GEOMETRY ALL VIOLET
GEOMETRY SWEEP LCMB2 LCMB6 1 TRANSLATE 0 -100 0 DEPENDENT
MESHING TYPES S6 IL33 CL12I BASE LCMB6
MESHING GENERATE
VIEW MESH
EYE ZOOM FACTOR 10. 11000. -19000. 0.
To model the foundation interface we simply sweep the combined line LCMB2,
which forms the bottom line of the floor [Fig. 10.2 p. 162], downward over an
arbitrary distance.1 The sweep operation creates appropriate lines and points,
and a surface S6 to form the geometry of the foundation interface [Fig. 10.7].
We apply IL33 interface elements which match the QU8 elements for the floor.
With the BASE option we specify the orientation of the interface elements, i.e.,
the line that is attached to the material or to the ‘world’. Otherwise we could
possibly get interface elements with three nodes in vertical direction. Finally
we generate the mesh and display it zoomed-in on the the floor–wall connection
[Fig. 10.8a].
tankli.fgc
1 To get a discernible foundation ‘thickness’ we apply a distance of 100.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
168 Fire near Concrete Safety Tank
QU8
BASE LCMB2
IL33 S6
LCMB6
Figure 10.7: Modeling the foundation interface
VIEW OPTIONS COLOUR TYPES
VIEW HIDDEN SHADE
VIEW OPTIONS SHRINK 0.9
We display the mesh in ‘shrunken’ style, filled with a separate color for the
element type: structural elements in red, interfaces in orange [Fig. 10.8b].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:30 meshif.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:30 meshfil.ps
Y Y
Z X Z X
Element Types
QU8
IL33
(a) zoom-in on floor–wall (b) shrunken and color filled for types
Figure 10.8: Mesh with foundation
10.1.6 Reinforcement
For the reinforcement grids, which show up as lines in an axisymmetric model,
we must define some new points and then put in the reinforcement grids. For
this example we will not explain the definition of each reinforcement in detail but
limit ourselves to some general remarks about definition of grid reinforcements
in an axisymmetric model. In this model there are reinforcements which show
up as straight lines and as curved lines.
Straight lines. The straight line reinforcements are located in the floor, the
wall and the beam. These are defined with single sections by two end points via
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.1 Model for Linear Structural Analysis 169
the following commands.
tankli.fgc
GEOMETRY COPY P5 P32 TRANSLATE 0 65 0
GEOMETRY COPY P8 P33 TRANSLATE 0 65 0
REINFORCE GRID SECTION AXI-SYM P32 P33
REINFORCE GRID GR1 RE1
REINFORCE ATTACH GR1 S1
GEOMETRY COPY P1 P34 TRANSLATE 0 -65 0
GEOMETRY COPY P4 P35 TRANSLATE 0 -65 0
REINFORCE GRID SECTION AXI-SYM P34 P35
REINFORCE GRID GR2 RE2
REINFORCE ATTACH GR2 S1
GEOMETRY COPY P6 P36 TRANSLATE 50 0 0
GEOMETRY COPY P36 P37 TRANSLATE 0 3000 0
REINFORCE GRID SECTION AXI-SYM P36 P37
REINFORCE GRID GR3 RE3
REINFORCE ATTACH GR3 TANK
GEOMETRY COPY P14 P40 TRANSLATE 50 0 0
REINFORCE GRID SECTION AXI-SYM P36 P40
REINFORCE GRID GR4 RE4
REINFORCE ATTACH GR4 TANK
GEOMETRY COPY P7 P38 TRANSLATE -50 0 0
GEOMETRY COPY P38 P39 TRANSLATE 0 3000 0
REINFORCE GRID SECTION AXI-SYM P38 P39
REINFORCE GRID GR5 RE5
REINFORCE ATTACH GR5 TANK
GEOMETRY COPY P15 P41 TRANSLATE -50 0 0
REINFORCE GRID SECTION AXI-SYM P38 P41
REINFORCE GRID GR6 RE6
REINFORCE ATTACH GR6 TANK
GEOMETRY COPY P7 P42 TRANSLATE 0 200 0
GEOMETRY COPY P8 P43 TRANSLATE 0 200 0
REINFORCE GRID SECTION AXI-SYM P42 P43
REINFORCE GRID GR7 RE7
REINFORCE ATTACH GR7 S1
GEOMETRY COPY P3 P44 TRANSLATE 0 -200 0
GEOMETRY COPY P4 P45 TRANSLATE 0 -200 0
REINFORCE GRID SECTION AXI-SYM P44 P45
REINFORCE GRID GR8 RE8
REINFORCE ATTACH GR8 S1
GEOMETRY POINT ONLINE P46 P6 P7 0.5
GEOMETRY POINT ONLINE P47 P37 P39 0.5
REINFORCE GRID SECTION AXI-SYM P46 P47
REINFORCE GRID GR9 RE9
REINFORCE ATTACH GR9 TANK
GEOMETRY COPY P46 P48 TRANSLATE 0 15500 0
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
170 Fire near Concrete Safety Tank
REINFORCE GRID SECTION AXI-SYM P47 P48
REINFORCE GRID GR10 RE10
REINFORCE ATTACH GR10 TANK
GEOMETRY COPY P46 P49 TRANSLATE 0 24000 0
REINFORCE GRID SECTION AXI-SYM P48 P49
REINFORCE GRID GR11 RE11
REINFORCE ATTACH GR11 TANK
GEOMETRY POINT ONLINE P50 P14 P15 0.5
REINFORCE GRID SECTION AXI-SYM P49 P50
REINFORCE GRID GR12 RE12
REINFORCE ATTACH GR12 TANK
GEOMETRY COPY P13 P51 TRANSLATE -150 0 0
GEOMETRY COPY P16 P52 TRANSLATE -150 0 0
REINFORCE GRID SECTION AXI-SYM P51 P52
REINFORCE GRID GR13 RE13
REINFORCE ATTACH GR13 S3
The general principle is that we define the end points of a reinforcement and
translate these over the distance of the concrete cover. Then we define a grid
section between the two end points. We define each reinforcement to consist of
a single section which we attach to an appropriate part of the geometry.
Curved lines. In this model, there are two curved line reinforcements, located
in the roof and continuing in the beam. In the roof, the reinforcements have
a concrete cover of 50 mm at the inner and outer sides of the roof. To get an
accurate course of these reinforcements we use two sections per reinforcement
with four points each. In this case, iDiana will approximate the course of the
reinforcements with a third-order curve. The commands to define the curved
reinforcements in the roof and the beam are as follows.
tankli.fgc
GEOMETRY COPY P18 P53 TRANSLATE 0.0 50.0 0.0
GEOMETRY COPY P53 P54 TRANSLATE 4828.5 -295.3 0.0
GEOMETRY COPY P53 P55 TRANSLATE 9584.9 -1176.9 0.0
GEOMETRY COPY P53 P56 TRANSLATE 14198.5 -2631.5 0.0
GEOMETRY COPY P53 P57 TRANSLATE 18600.5 -4637.6 0.0
GEOMETRY COPY P53 P58 TRANSLATE 22725.1 -7165.2 0.0
GEOMETRY COPY P53 P59 TRANSLATE 26511.0 -10176.6 0.0
REINFORCE GRID SECTION AXI-SYM P53 P54 P55 P56
REINFORCE GRID SECTION AXI-SYM P56 P57 P58 P59
REINFORCE GRID GR14 RE14 RE15
REINFORCE ATTACH GR14 TANK
CONSTRUCT PARAMETER RIRO 1.005048
GEOMETRY POINT ONLINE P60 PC P53 RIRO
GEOMETRY POINT ONLINE P61 PC P54 RIRO
GEOMETRY POINT ONLINE P62 PC P55 RIRO
GEOMETRY POINT ONLINE P63 PC P56 RIRO
GEOMETRY POINT ONLINE P64 PC P57 RIRO
GEOMETRY POINT ONLINE P65 PC P58 RIRO
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.1 Model for Linear Structural Analysis 171
GEOMETRY POINT ONLINE P66 PC P59 RIRO
REINFORCE GRID SECTION AXI-SYM P60 P61 P62 P63
REINFORCE GRID SECTION AXI-SYM P63 P64 P65 P66
REINFORCE GRID GR15 RE16 RE17
REINFORCE ATTACH GR15 TANK
The first point of the reinforcement along the inner side of the roof, P53, is
defined via a vertical translation of 50 mm of the inner top point of the roof, P18.
Then we apply six angular increments, of ∆α = 7° each, to define six more points
at a radial distance of 50 mm from the inner side of the roof. The translations
were calculated via X = rinr sin α and Y = rinr (1−cos α) where rinr is the radius
of the reinforcement along the inner side of the roof: rinr = rin + 50 = 39620.
We define the two sections RE14 and RE15 with four consecutive points each and
then the complete reinforcement RE14 with these two sections. Note that the last
point, P59, lies outside the beam, which causes the reinforcement in the iDiana
model to stick out of the element mesh. Fortunately, Diana will correct this
when evaluating the reinforcements for the individual elements of the mesh.
The radius of the reinforcement along the outer surface of the roof is rour =
rin + 300 − 50 = 39820. We define a parameter RIRO which represents the ratio
of the radii of the outer and inner reinforcements: rour /rinr = 39820/39620 ≈
1.005048. We apply this parameter to define points along the outer reinforce-
ment with respect to corresponding points along the inner reinforcement and
the center of the roof, PC. Finally we define two sections, RE16 and RE17, in grid
reinforcement GR15.
Reinforcement display tankli.fgc
VIEW HIDDEN OFF
VIEW OPTIONS SHRINK OFF
VIEW REINFORCE +ALL
EYE FRAME
EYE ZOOM FACTOR 10. 12000. 10000. 0.
EYE FRAME
EYE ZOOM FACTOR 10. 11000. -19000. 0.
To display the reinforcements we first revert to a mesh display in wire netting
style by switching off the ‘hidden’ and ‘shrunken’ view styles. Then we display all
the reinforcements, by default in orange [Fig. 10.9]. Due to the plus sign in +ALL,
iDiana will not erase the current display: the reinforcements are superposed to
the element mesh display. We display two details of the reinforcements: near the
beam and the floor–wall connection [Fig. 10.10]. Note the curved reinforcements
sticking out of the beam.
10.1.7 Supports
In this axisymmetric model, only the bottom line of the foundation interface is
supported in vertical direction.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
172 Fire near Concrete Safety Tank
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:33 reinf.ps
Z X
Figure 10.9: Reinforcements
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:33 reinfb.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:33 reinfw.ps
Y Y
Z X Z X
(a) beam (b) floor–wall
Figure 10.10: Reinforcements details
tankli.fgc
PROPERTY BOUNDARY CONSTRAINT LCMB6 Y
EYE FRAME
VIEW MESH
VIEW HIDDEN OFF
LABEL MESH CONSTRNT
EYE ZOOM FACTOR 10. 11000. -19000. 0.
We apply a constraint in Y -direction (uY = 0) along the combined line LCMB6,
which is the bottom line of the foundation interface. Because iDiana cannot
display supports in a hidden viewed mesh, we switch that off. We display the
supports on the complete mesh [Fig. 10.11a]. To get a better view, we zoom in
on the floor–wall junction [Fig. 10.11b].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.1 Model for Linear Structural Analysis 173
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:33 meshsup.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:33 meshzup.ps
Y Y
Z X Z X
(a) full model (b) floor–wall
Figure 10.11: Supports on mesh
10.1.8 Loading
Different load cases are defined to be able to analyze the subsequent loading by
dead weight and prestress, by normal service load and by a calamity load. To
start with a clean view of the mesh we zoom out on the total mesh and switch
off the support labels.
Dead weight tankli.fgc
EYE FRAME
LABEL MESH OFF
PROPERTY LOADS GRAVITY WEIGHT 1 ALL -9.8 Y
LABEL MESH LOADS WEIGHT
First we define the dead weight of the model via the GRAVITY load class. We
name the load WEIGHT and specify it as load case 1. The gravity acceleration
g = 9.8 acts downward, i.e., in the −Y -direction. To check the load we display it
on the mesh [Fig. 10.12a]. Note that iDiana draws an arrow pointing downward
on each element of the mesh.
Reinforcement prestress tankli.fgc
LABEL MESH OFF
PROPERTY LOADS PRESTRES LOP1 2 GR7 0. 1200.
PROPERTY LOADS PRESTRES LOP2 2 GR8 0. 1200.
PROPERTY LOADS PRESTRES LOP3 2 GR9 1200. 1200.
PROPERTY LOADS PRESTRES LOP4 2 GR10 1200. 1200.
PROPERTY LOADS PRESTRES LOP5 2 GR11 1200. 1200.
PROPERTY LOADS PRESTRES LOP6 2 GR12 1200. 1200.
PROPERTY LOADS PRESTRES LOP7 2 GR13 0. 1000.
VIEW REINFORCE
LABEL MESH LOADS 2
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
174 Fire near Concrete Safety Tank
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:33 loadwei.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:34 loadpre.ps
.12E4
.12E4
.12E4
Y Y
.12E4
Z X Z X 0
0
(a) weight (b) prestress
Figure 10.12: Permanent loads
We define the prestress load in the reinforcement grids via the PRESTRES load
class. We name the loads LOP1 to LOP7 and specify it as load case 2. For each
0 0
prestressed grid we specify the stress in the two directions σxx and σzz [Vol.
Element Library]. To check the load we display the reinforcements with load
0
labels, i.e., the values for σxx for the prestressed reinforcements [Fig. 10.12b].
Note that the reinforcement grids in the floor and roof are not prestressed.
Service load tankli.fgc
LABEL MESH OFF
PROPERTY LOADS PRESSURE SERVICE 3 L1 0.147 NORMAL
VIEW MESH
LABEL MESH LOADS SERVICE
Next we define the service load, a pressure on the floor of the tank. We specify
this as load case 3 with the PRESSURE load class. This pressure acts perpendic-
ularly on line L1, i.e., in the normal direction. The loads labeling on the mesh
proves the correct downward direction [Fig. 10.13a].
Calamity load tankli.fgc
LABEL MESH OFF
PROPERTY LOADS PRESSURE CALAMI 4 LCMB3 1.0 NORMAL
CONSTRUCT SCURVE HYD GLOBAL Y LIST 800 0.147 30800 0.0
PROPERTY ATTACH CALAMI SCURVE HYD
LABEL MESH LOADS CALAMI
Finally we define a calamity load which occurs when the inner steel tank col-
lapses. In that case the liquid causes an additional hydrostatic pressure on the
inner side of the concrete wall. We specify this as load case 4 with the PRESSURE
load class. The hydrostatic load acts perpendicularly (normal) on the combined
line LCMB3.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.1 Model for Linear Structural Analysis 175
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:34 loadser.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:34 loadcal.ps
Y Y
Z X Z X
(a) service (b) calamity
Figure 10.13: External loads
At first we define a constant pressure of 1. Then we define a space curve
named HYD to specify the hydrostatic tapering of the pressure in the global
Y -direction: 0.147 at the bottom of the wall (Y = 800), to zero at the top of
the wall (Y = 30800). Finally we attach the space curve to the calamity load
which may be considered as a multiplication.
The labeling shows the correct tapering and direction of the load [Fig. 10.13-
b]. Note that iDiana displays only one arrow for each element where the length
represents the mean value of the pressure load along the edge of the element. In
reality the load is passed to Diana as a varying edge load with correct values
at the nodes.
10.1.9 Properties
To complete the finite element model we must now specify material and physical
properties for its various parts: the concrete tank, the reinforcements, and the
foundation interface.
Concrete tank iDiana
View →Property Manager...
↑
Property Manager
↑ Materials Material Name: CONCRETE
↑Linear Elasticity →Isotropic
↑Mass →Mass density
For the concrete tank we define an isotropic material CONCRETE with Young’s
modulus E = 17500 MPa, Poisson’s ratio ν = 0.2, and mass density ρ =
2400×10−9 kg/mm3 .
tankli.fgc
PROPERTY ATTACH TANK MATERIAL CONCRETE
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
176 Fire near Concrete Safety Tank
We assign the material CONCRETE to the set TANK which comprises all surfaces
that model the tank.
Reinforcement iDiana
View →Property Manager...
↑
Property Manager
↑Materials Material Name: STEEL
↑Linear Elasticity →Isotropic
↑Physical Properties Physical Property Name: GRT1
↑Geometry →Embedded Reinforcements →Grid
Physical Properties Physical Property Name: GRT2
...
For the embedded reinforcement grids we specify a material STEEL with E =
210000 MPa. Furthermore we have specified nine sets of physical properties,
GRT1, GRT2 etc., with values for the equivalent thicknesses of the grids in their
two directions, tangential Z and in-plane XY .
tankli.fgc
PROPERTY ATTACH GR1 STEEL GRT1
PROPERTY ATTACH GR2 STEEL GRT1
PROPERTY ATTACH GR3 STEEL GRT2
PROPERTY ATTACH GR4 STEEL GRT3
PROPERTY ATTACH GR5 STEEL GRT2
PROPERTY ATTACH GR6 STEEL GRT3
PROPERTY ATTACH GR7 STEEL GRT4
PROPERTY ATTACH GR8 STEEL GRT4
PROPERTY ATTACH GR9 STEEL GRT5
PROPERTY ATTACH GR10 STEEL GRT6
PROPERTY ATTACH GR11 STEEL GRT5
PROPERTY ATTACH GR12 STEEL GRT7
PROPERTY ATTACH GR13 STEEL GRT10
PROPERTY ATTACH GR14 STEEL GRT11
PROPERTY ATTACH GR15 STEEL GRT11
We assign the material STEEL and the appropriate thickness to each reinforce-
ment.
Foundation interface iDiana
View →Property Manager...
↑
Property Manager
↑Materials Material Name: SOILSP
↑Linear Elasticity →Interfaces
↑Physical Properties Physical Property Name: FOUNDA
↑Geometry →Interface →Line
The foundation interface is a soil spring for which we specify the ‘material’
properties a material named SOILSP with the linear stiffness moduli D11 =
6.922×10−2 and D22 = 1.0×10−5 , respectively for the normal and shear trac-
tion. The interface elements require the configuration of the model, in this case
‘axisymmetric’. Therefore we define a physical property FOUNDA.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.2 Linear Structural Analysis 177
tankli.fgc
PROPERTY ATTACH S6 SOILSP FOUNDA
We assign the properties of the interface to its surface.
Check properties tankli.fgc
VIEW HIDDEN FILL COLOUR
VIEW OPTIONS COLOUR MATERIAL
VIEW MESH
EYE ZOOM FACTOR 10. 11000. -19000. 0.
EYE FRAME
VIEW OPTIONS COLOUR PHYSICAL
VIEW MESH
EYE ZOOM FACTOR 10. 11000. -19000. 0.
In finite element modeling it is good practice to thoroughly check the generated
model prior to the actual analysis. In this case we may check the properties
assignment by color modulation. The MATERIALS option displays the mesh with
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:35 materi.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:35 materiz.ps
Y Y
Z X Z X
Materials Materials
CONCRETE CONCRETE
SOILSP SOILSP
(a) full model (b) floor–wall
Figure 10.14: Elements color filled for material properties
the elements colored according to their assigned material property [Fig. 10.14].
The PHYSICAL option colors the elements according to their assigned physical
property [Fig. 10.15]. Note that no physical properties were assigned to the
concrete tank.
10.2 Linear Structural Analysis
To perform the analysis of the model we write an input data file in Diana batch
format.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
178 Fire near Concrete Safety Tank
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:35 physic.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:35 physicz.ps
Y Y
Z X Z X
Physical Physical
No Physical No Physical
FOUNDA FOUNDA
(a) full model (b) floor–wall
Figure 10.15: Elements color filled for physical properties
iDiana
UTILTY WRITE DIANA
yes
FILE CLOSE
yes
Concrete safety tank
ANALYSE TANK
Analysis Setup
specify analysis options
We close the model and launch the Analysis Setup dialog where we indicate a
Linear Static analysis type and output of displacements and stresses which gives
the following batch command file.
linsta.dcf
*FILOS
INITIA
*INPUT
*LINSTA
BEGIN OUTPUT FEMVIE
DISPLA TOTAL TRANSL GLOBAL
STRESS TOTAL CAUCHY LOCAL INTPNT
END OUTPUT
*END
The analysis results are written to a data base for the iDiana Results environ-
ment. We now enter this environment to assess the analysis results.
linsta.fvc
FEMVIEW TANK
VIEW MESH
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.2 Linear Structural Analysis 179
EYE FRAME
We display the undeformed model in green, nicely fitted in the iDiana viewport.
10.2.1 Deformation for Load Cases
As a first check of the analysis results we make plots of the deformed structure
for all load cases.
linsta.fvc
RESULTS LOADCASE LC1
RESULTS NODAL DTX....G RESDTX
PRESENT SHAPE FACTOR 500
RESULTS LOADCASE LC2
RESULTS NODAL DTX....G RESDTX
PRESENT SHAPE FACTOR 500
RESULTS LOADCASE LC3
RESULTS NODAL DTX....G RESDTX
PRESENT SHAPE FACTOR 500
RESULTS LOADCASE LC4
RESULTS NODAL DTX....G RESDTX
PRESENT SHAPE FACTOR 500
Here we display the deformations of the load cases 500× enlarged [Fig. 10.16].
These deformations inspire confidence in the model.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:39 dfmwei.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:39 dfmpre.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:39 dfmser.ps
Model: LINSTA Model: LINSTA Model: LINSTA
LC1: Load case 1 LC2: Load case 2 LC3: Load case 3
Nodal DTX....G RESDTX Nodal DTX....G RESDTX Nodal DTX....G RESDTX
Max = 6.39 Max = 8.48 Max = 2.21
Min = .931E-5 Min = .191E-4 Min = .101E-4
Factor = 500 Factor = 500 Factor = 500
Y Y Y
Z X Z X Z X
(a) weight (b) prestress (c) service
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:39 dfmcal.ps
Model: LINSTA
LC4: Load case 4
Nodal DTX....G RESDTX
Max = 8.05
Min = .32E-4
Factor = 500
Z X
(d) calamity
Figure 10.16: Deformation ×500 for basic load cases
10.2.2 Combining Load Cases
In reality there are three different loadings which we will now combine from
the basic load cases. iDiana will prompt us for the load cases of each load
combination, including a multiplication factor and a descriptive text.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
180 Fire near Concrete Safety Tank
linsta.fvc
RESULTS CALCULATE COMBINE EMPTY
LC1
1
LC2
1
GO
empty tank
ALL
RESULTS CALCULATE COMBINE FULL
LC1
1
LC2
1
LC3
1
GO
fully filled tank
ALL
RESULTS CALCULATE COMBINE CALAMI
LC1
1
LC2
1
LC3
1
LC4
1
GO
calamity
ALL
UTILITY TABULATE LOADCASES
This command sequence creates three load combinations: EMPTY a load combi-
nation with only weight and prestress loading [§ 10.2.3]; FULL the fully filled tank
with weight, prestress and service loading [§ 10.2.4]; CALAMI the calamity situa-
tion when the liquid directly fills the concrete tank [§ 10.2.5]. The ALL answer
after the descriptive text for each combination indicates that all results should
be calculated for the defined load combination. We tabulate all load cases that
are now known to iDiana.
Tabulated load cases linstalc.tb
;
; Model: LINSTA
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; MODEL STATIC "Model Properties"
; Element : REINGRID*
;
; LC1 STATIC "Load case 1"
; Nodal : DTX....G
; Gauss : EL.SXX.L RE.SXX.L
;
; LC2 STATIC "Load case 2"
; Nodal : DTX....G
; Gauss : EL.SXX.L RE.SXX.L
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.2 Linear Structural Analysis 181
;
; LC3 STATIC "Load case 3"
; Nodal : DTX....G
; Gauss : EL.SXX.L RE.SXX.L
;
; LC4 STATIC "Load case 4"
; Nodal : DTX....G
; Gauss : EL.SXX.L RE.SXX.L
;
; EMPTY STATIC "empty tank"
; Combination: LC1 *1 LC2 *1
; Nodal : DTX....G
; Gauss : EL.SXX.L RE.SXX.L
;
; FULL STATIC "fully filled tank"
; Combination: LC1 *1 LC2 *1 LC3 *1
; Nodal : DTX....G
; Gauss : EL.SXX.L RE.SXX.L
;
; CALAMI STATIC "calamity"
; Combination: LC1 *1 LC2 *1 LC3 *1 LC4 *1
; Nodal : DTX....G
; Gauss : EL.SXX.L RE.SXX.L
; * Indicates loads data
;
Prepare results display linsta.fvc
VIEW MESH TANK
VIEW EDGES
DRAWING CONTENTS AXES OFF
We display the mesh of set TANK, i.e., the tank only, without the interface
elements. As we only display the edges of the mesh we get a clear view in
combination with analysis results. To get an undisturbed picture we remove
the displayed axes.
10.2.3 Empty Tank
For the empty tank we will now first display the principal Cauchy stresses and
then the equivalent Von Mises stresses.
Principal Cauchy stress linsta.fvc
RESULTS LOADCASE EMPTY
RESULTS GAUSSIAN EL.SXX.L SXX
RESULTS CALCULATE P-STRESS ALL
PRESENT OPTIONS VECTORS MODULATE 10
PRESENT VECTORS
EYE ZOOM FACTOR 10. 11000 -19000 0
PRESENT VECTORS
We display the principal stresses for the EMPTY load combination [Fig. 10.17a]:
dead weight and prestressing in the reinforcements. The large blue vectors show
that the wall to floor connection is highly stressed. This is made perfectly clear
when we zoom in on that part of the model [Fig. 10.17b]. Note that we must
re-display the stress vectors to get them properly scaled.
Stress concentrations can made still more clear with a contour plot of the
equivalent Von Mises stress.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
182 Fire near Concrete Safety Tank
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:39 empsp.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:40 empsp_fw.ps
Model: LINSTA
EMPTY: empty tank
Gauss PRINC STRESS ALL
Calculated from: EL.SXX.L
Max/Min on model set:
Max = .92 Min = -7.42
Factor = 454
.86E-1 .86E-1
-.748 -.748
-1.58 -1.58
-2.41 -2.41
-3.25 -3.25
-4.08 -4.08
-4.92 -4.92
-5.75 -5.75
-6.58 -6.58
(a) full model (b) floor-wall connection
Figure 10.17: Principal stresses for empty tank
Equivalent Von Mises stress linsta.fvc
EYE FRAME
VIEW OPTIONS DEFORM USING DTX....G RESDTX 200
RESULTS CALCULATE VONMISES
PRESENT CONTOUR LEVELS 10
EYE ZOOM FACTOR 10. 11000 -19000 0
We display analysis results in a deformed mesh with the deformation to be taken
as 200× the calculated displacements. We let iDiana calculate the Von Mises
stresses and display these in a contour plot [Fig. 10.18].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:40 empsv.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:40 empsv_fw.ps
6.06 6.06
5.48 5.48
4.89 4.89
4.3 4.3
3.72 3.72
3.13 3.13
2.55 2.55
1.96 1.96
1.38 1.38
.79 .79
Figure 10.18: Von Mises stress contours for empty tank
10.2.4 Fully Filled Tank
Now we will display the analysis results of the fully filled tank: deformation,
principal stresses and Von Mises stresses.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.2 Linear Structural Analysis 183
Deformation linsta.fvc
VIEW OPTIONS DEFORM OFF
EYE FRAME
RESULTS LOADCASE FULL
RESULTS NODAL DTX....G RESDTX
PRESENT SHAPE FACTOR 200
We switch off the ‘deformed’ view option and create an outline view of the
undeformed mesh in green [Fig. 10.19a]. We switch to the full load case where
we select the nodal displacements as analysis result. Finally we display a 200×
enlarged picture of the deformed model outlines in red [Fig. 10.19a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:40 fuldf.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:40 fulsp.ps
.108
-.704
-1.52
-2.33
-3.14
-3.95
-4.76
-5.58
-6.39
(a) deformation ×200 (b) principal stress
Figure 10.19: Analysis results for fully filled tank
Principal stresses linsta.fvc
VIEW OPTIONS DEFORM USING DTX....G RESDTX 200
RESULTS GAUSSIAN EL.SXX.L SXX
RESULTS CALCULATE P-STRESS ALL
PRESENT VECTORS
EYE ZOOM FACTOR 10. 11000 -19000 0
PRESENT VECTORS
EYE FRAME
EYE ZOOM FACTOR 10. 12000 11000 0
We let iDiana calculate the principal stresses and then display them in vector
style in a deformed outline of the complete model [Fig. 10.19b]. The stresses
in the empty tank seem to relax when the service load is added (hydrostatic
pressure on the floor). We observe that the maximum stresses appear near the
wall–floor and the wall–dome junctions, as expected. To examine these areas in
more detail we zoom-in [Fig. 10.20].
Von Mises stresses linsta.fvc
EYE FRAME
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
184 Fire near Concrete Safety Tank
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:40 fulsp_fw.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:40 fulsp_wd.ps
.108 .108
-.704 -.704
-1.52 -1.52
-2.33 -2.33
-3.14 -3.14
-3.95 -3.95
-4.76 -4.76
-5.58 -5.58
-6.39 -6.39
Figure 10.20: Maximum principal stresses for fully filled tank
RESULTS CALCULATE VONMISES
PRESENT CONTOUR LEVELS 10
EYE ZOOM FACTOR 10 11000 -19000 0
EYE FRAME
EYE ZOOM FACTOR 10 12000 11000 0
We display the complete model with the Von Mises stress contours for the fully
filled tank [Fig. 10.21]. For better examination of the significant areas we zoom
in on the floor–wall and the beam [Fig. 10.22].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:40 fulsv.ps
6.11
5.52
4.93
4.34
3.75
3.16
2.57
1.98
1.39
.795
Figure 10.21: Von Mises stress contours for fully filled tank
10.2.5 Calamity Situation
To finish this example we will display the analysis results of the calamity load
where the inner tank has collapsed and the liquid directly acts as an hydrostatic
pressure on the wall of the concrete safety tank. The commands are like those
for the fully filled tank in the previous section, except that we will not make
zoomed-in plots now.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.3 Model for Flow–Stress Analysis 185
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:40 fulsv_fw.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:40 fulsv_wd.ps
6.11 6.11
5.52 5.52
4.93 4.93
4.34 4.34
3.75 3.75
3.16 3.16
2.57 2.57
1.98 1.98
1.39 1.39
.795 .795
Figure 10.22: Von Mises stress contours for fully filled tank (details)
linsta.fvc
VIEW OPTIONS DEFORM OFF
EYE FRAME
RESULTS LOADCASE CALAMI
RESULTS NODAL DTX....G RESDTX
PRESENT SHAPE FACTOR 200
VIEW OPTIONS DEFORM USING DTX....G RESDTX 200
RESULTS GAUSSIAN EL.SXX.L SXX
RESULTS CALCULATE P-STRESS ALL
PRESENT VECTORS
RESULTS CALCULATE VONMISES
PRESENT CONTOUR LEVELS 10
We subsequently display the deformation of the tank in the calamity situa-
tion 200× enlarged and the principal stress vectors in the deformed shape of
the model [Fig. 10.23]. The last picture shows the Von Mises stress contours
[Fig. 10.24]. We may conclude that the prestressing of the wall is almost com-
pensated by the internal hydrostatic pressure.
10.3 Model for Flow–Stress Analysis
We continue the analysis of the reinforced concrete safety tank with a nonlinear
flow–stress analysis. The considered nonlinear phenomena are: transient creep,
plasticity, cracking and temperature dependent material properties. The tank
will be subjected to an external fire load. It is assumed that a neighboring tank
at a distance of 50 m, is burning with a surface temperature of 2000 °C at an
environmental temperature of 25 °C.
A nonlinear heat flow analysis will be carried out with Diana’s Module
heattr. The results of the flow analysis will then be incorporated in a struc-
tural nonlinear analysis as prescribed temperatures on the nodal points. The
sequence of a flow analysis followed by a structural analysis is a so-called stag-
gered coupled flow–stress analysis [Vol. Analysis Procedures]. For such a stag-
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
186 Fire near Concrete Safety Tank
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:40 caldf.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:40 calsp.ps
.298
-.552
-1.4
-2.25
-3.1
-3.95
-4.8
-5.66
-6.51
(a) deformation ×200 (b) principal stress
Figure 10.23: Analysis results for calamity situation
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:41 calsv.ps
5.73
5.18
4.62
4.07
3.52
2.97
2.41
1.86
1.31
.757
Figure 10.24: Von Mises stress contours for calamity situation
gered analysis we must prepare a single model with appropriate elements and
properties for both types of analysis. Therefore we launch iDiana and enter
the Design environment with the name of the model.
tankfs.fgc
FEMGEN TANK
PROPERTY FE-PROG DIANA HTSTAG AX
yes
With the HTSTAG AX option we indicate that the model will be applied for stag-
gered flow–stress analysis in an axisymmetric configuration. We will specify
additional data for the heat flow analysis [§ 10.3.1], and for the nonlinear struc-
tural analysis [§ 10.3.2].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.3 Model for Flow–Stress Analysis 187
10.3.1 Model for Heat Flow Analysis
For the heat flow analysis Diana will automatically transform the structural el-
ements with appropriate flow properties, like conductivity and capacity, to flow
elements [Vol. Analysis Procedures]. In this example we must modify the model
as used in the linear elastic analysis. The additional data for the flow analy-
sis comprises the radiation, material properties of the concrete, the boundary
conditions, and an initial temperature field.
10.3.1.1 Radiation
For the heat flow analysis we must describe the heat radiation along the outside
of the concrete tank. Therefore we will apply boundary elements B2AHT. The
outside of the concrete tank comprises a number of lines that we first must
determine. We start with displaying all lines of the geometry.
tankfs.fgc
EYE FRAME
VIEW HIDDEN OFF
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY LINES ALL VIOLET
CONSTRUCT SET OUTER APPEND LINES L8 L3 L12 L13 L15 L24 L17 L16 L33 L34
VIEW GEOMETRY OUTER VIOLET
LABEL GEOMETRY LINES CURRENT VIOLET
We display all lines of the geometry with their labels [Fig. 10.25a]. From this
display we determine the lines that together form the outer boundary. We
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:52 geolin.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:52 geoout.ps
L36
L34 L34
L35
L27
L19
L33
L16
LCMB5
L32L17
L24 L33
L16
L17
L24
L23
L31
L25
L22
L14
LCMB4
L15 L15
L13
L10 L13
L26
L18
L30 L11
LCMB3
L12
L9 L12
Y Y
Z X L7 L1
LCMB1 L2
L3L8 Z X L3
L8
L40 L4
LCMB2
L37
LCMB6 L5
L
L386
L41
L39
(a) all lines (b) outer lines
Figure 10.25: Geometry lines
assemble these lines in a set called OUTER. To check the correct contents of this
set we display its lines only, with their labels [Fig. 10.25b]. The display shows a
complete set of lines along the outer boundary of the model.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
188 Fire near Concrete Safety Tank
Modeling incompatible elements. An awkward complication with respect
to the modeling of the boundary elements for staggered flow–stress analysis is
that these are linearly interpolated, i.e., they have no mid-side node. In prin-
ciple these elements are incompatible with the edges of the quadratic CQ16A
elements that we must apply for the structural model of the tank. Fortunately,
for the flow analysis part of the staggered flow–stress analysis, Diana inter-
nally converts quadratic structural elements to linear flow elements, in this case
Q4AHT elements which certainly are compatible with the linear boundary ele-
ments. However, in the Design environment of iDiana, where we must build the
complete model, the meshing procedure would not allow the incompatibility of
elements. We must find a work-around solution for this problem: the trick is to
copy the set of lines along the boundary by translation over a virtual distance.
tankfs.fgc
CONSTRUCT SPACE TOLERANCE OFF
GEOMETRY COPY OUTER BOUND TRANSLATE 0 0 0
VIEW GEOMETRY BOUND VIOLET
LABEL GEOMETRY LINES CURRENT VIOLET
We copy the set OUTER to a new set BOUND over a zero distance. Without
corrective action iDiana would not create new lines and points because any
new point would exactly coincide with an existing point. In other words: each
new point would be located within the default tolerance distance of an existing
point and would therefore not be created! To force creation of new points and
lines we switch off the tolerance check before starting the copy operation. To
check whether this operation has been performed correctly we display the new
set [Fig. 10.26a]. We notice that new lines L42, L43, . . . , L51 have been created.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:52 geobnd.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:53 geodiv.ps
L51
49
L50
L49
L48
L47
3 213
L46
1
L45
30
L44
30
Y Y
Z X L43
L42 Z X
202
3
(a) lines (b) divisions
Figure 10.26: Geometry for boundary
Meshing. We are now ready to perform the meshing operation. We must not
forget to adapt the number of divisions for the linear boundary elements: these
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.3 Model for Flow–Stress Analysis 189
require one division per element whereas the quadratic CQ16A elements required
two divisions per element [§ 10.1.1 p. 162].
tankfs.fgc
MESHING TYPES BOUND BE2 B2AHT
MESHING DIVISION FACTOR BOUND 0.5
LABEL GEOMETRY OFF
LABEL GEOMETRY DIVISIONS CURRENT RED
We assign the B2AHT element type to the lines in set BOUND. The lines in this
set got their number of divisions from their originators during the copy action.
So here we may simply halve the number of divisions via the FACTOR option.
Note that iDiana only adapts the real number of divisions; the grading factor
will not be changed.
As a check we let the currently displayed geometry, i.e., the lines in set
BOUND, be labeled with their divisions [Fig. 10.26b]. For instance along the
outer surface of the dome we see a division of 49. This is indeed half the number
of divisions as we specified for the dome itself [§ 10.1.4 p. 166].
tankfs.fgc
MESHING GENERATE
VIEW MESH ALL
VIEW MESH +BOUND RED
VIEW OPTIONS SHRINK 0.7
EYE ZOOM FACTOR 15. 12000. 11000. 0.
Here we finally let the mesh be generated and display it completely in green wire
netting style. To clearly discern the boundary elements from the structural
elements we apply two viewing options First we display the elements in set
BOUND in red where the plus sign prevents the already displayed mesh to be
erased. Then we apply shrinkage to display the elements shrunken to 70 %
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:53 mesh.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:53 meshbm.ps
Y Y
Z X Z X
(a) entirely (b) beam
Figure 10.27: Generated mesh
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
190 Fire near Concrete Safety Tank
of their original size [Fig. 10.27a]. We now clearly see the boundary elements
displayed along the outer surface of the model. For a still better check we zoom
in on the beam at the dome–wall connection [Fig. 10.27b]. Here we clearly see
one boundary element along the edge of each structural element.
Although the mesh seems to be OK we still have to make one final correction.
Since the lines in set BOUND have no points in common with the lines in set
OUTER, the generated boundary elements will not be automatically connected
to the structural part. We will first prove this and than repair the defect.
tankfs.fgc
EYE ZOOM FACTOR 5. 0. 800. 0.
LABEL MESH NODES
MESHING MERGE ALL 1.
LABEL MESH NODES
We zoom in a bit further on the beam at the dome–wall connection and label
the nodes with their numbers [Fig. 10.28a]. Looking at the end nodes of the
red boundary elements we see overlapping numbers: one node for the boundary
element and another one for the structural element. No connection! To solve
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:53 meshno.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:53 meshnom.ps
699
1258 715 702
1259 721 705
1257 728 709
1254 699 715 702 721 705 728 709
712 718 724 731 712 718 724 731
Y Y
698 714 701 720 704 727 708
1255 698 714 701 720 704 727 708
Z X Z X
(a) before merging (b) after merging
Figure 10.28: Node labels
this problem we apply a merging operation on the mesh. The parameter value
of 1 indicates an absolute tolerance of one millimeter for the check on coinciding
nodes. A second display of node labels now shows one single node at the end of
each boundary element [Fig. 10.28b].
10.3.1.2 Material Properties
The data as specified for the linear elastic analysis [§ 10.1.9 p. 175] is to be
supplemented with the material data for the heat flow analysis part of the stag-
gered flow–stress analysis. Therefore we launch the Property Manager dialog to
specify the additional data.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.3 Model for Flow–Stress Analysis 191
iDiana
View Property Manager...
↑ →
Property Manager
···
The concrete and the boundary elements require special material properties for
the heat flow analysis. The reinforcements do not play a part in the heat flow
analysis, these do not require additional data.
Concrete iDiana
Property Manager
↑ Materials Material Name: CONCRETE
↑Flow →Isotropic
↑External →External Data from File
We select the material CONCRETE and specify the initial conductivity k =
1.78×10−3 and capacitance c = 2.369×10−3 . For the concrete we must also
specify the temperature dependence of the conductivity and the capacitance.
These dependencies must be supplied on a data file in Diana batch format
[Vol. Material Library].
conc.dat
TEMPER 0. 20. 24.5 100. 105. 115.
200. 500. 795. 1200. 2000.
CONDIS 1.780E-3 1.780E-3 1.780E-3 1.363E-3 1.335E-3 1.280E-3
1.233E-3 1.068E-3 0.850E-3 0.850E-3 0.850E-3
CAPATT 2.369E-3 2.369E-3 2.360E-3 2.443E-3 9.310E-3 6.170E-3
2.138E-3 2.374E-3 2.680E-3 2.938E-3 2.938E-3
The CONDIS values are the conductivities and the CAPATT values the capaci-
tances for the corresponding temperatures in TEMPER. During definition of the
additional properties for nonlinear structural analysis we will add the tempera-
ture dependence of some more material properties to this file.
Boundary elements iDiana
Property Manager
Materials Material Name: BCONDUC
↑Flow →Boundary
↑External →External Data from File
For the boundary elements we define a new material BCONDUC. with a conduc-
tion coefficient K = 2.75×10−6 . Furthermore we must specify the temperature
dependence of the conduction coefficient on an external data file in Diana batch
format [Vol. Material Library].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
192 Fire near Concrete Safety Tank
bounfl.dat
TEMPER 25. 75. 125. 175. 225. 275.
325. 375. 425. 475. 525. 575.
625. 675. 725.
CONVTT 2.754E-6 3.520E-6 4.460E-6 5.590E-6 6.940E-6 8.510E-6
10.300E-6 12.400E-6 14.800E-6 17.500E-6 20.500E-6 23.800E-6
31.600E-6 36.100E-6 27.5
The CONVTT values are the conduction coefficients for the corresponding tem-
peratures in TEMPER.
tankfs.fgc
PROPERTY ATTACH BOUND MATERIAL BCONDUC
We assign the material BCONDUC to the set BOUND, i.e., to all boundary elements.
10.3.1.3 Boundary Conditions
The boundary conditions for the flow analysis comprise the heat flux into the
concrete via the outer surface, and the fixed environmental temperature of the
boundary elements. These boundary conditions will be defined in one single
boundary case. In the Design environment the constituents of a boundary case
must be defined as a load case. For the transient heat flow analysis we must
also specify the variation in time of the defined boundary case.
Heat flux. We assume that a flux of q = 0.015 runs through all vertical faces
and a flux of q = 0.005 through the dome.
tankfs.fgc
CONSTRUCT SET OUTVERT APPEND LINES L8 L12 L13 L24
PROPERTY LOADS FLUX FL1 1 OUTVERT 0.015
PROPERTY LOADS FLUX FL2 1 L34 0.005
Looking at the display of the outer lines [Fig. 10.25b] we assemble the vertical
lines in a set OUTVERT. Then we specify a FLUX load FL1 for boundary case
1 along the lines in this set. A second flux load FL2 is defined along line L34
representing the outer surface of the dome.
tankfs.fgc
EYE FRAME
VIEW OPTIONS SHRINK OFF
LABEL MESH OFF
LABEL MESH LOADS FL1
LABEL MESH LOADS FL2 BLUE
We first revert to a regular display of the complete mesh and then display the
two loads in different colors [Fig. 10.29a].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.3 Model for Flow–Stress Analysis 193
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:53 meshflx.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:53 meshtem.ps
.5E-2
.5E-2
.5E-2
.5E-2
.5E-2
.5E-2
.5E-2
.5E-2
.5E-2
.5E-2
.5E-2
.5E-2 25
22
5252
5252
5252
5252
5252
52
.5E-2
.5E-2
.5E-2
.5E-2
.5E-2 52
5252
5252
.5E-2
.5E-2
.5E-2
.5E-2 5252
5252
.5E-2
.5E-2
.5E-2
.5E-2 5252
5252
.5E-2
.5E-2
.5E-2 5252
525
.5E-2
.5E-2
.5E-2 525
.5E-2
.5E-2
.5E-2 25
25
25
.5E-2
.5E-2
.5E-2 25
25
25
.5E-2
.5E-2 25
25
.5E-2
.5E-2 25
25
.5E-2
.5E-2 25
25
.5E-2
.5E-2 25
25
.5E-2
.5E-2 25
25
.5E-2
.5E-2 25
25
25
25
25
25
25
25
.15E-1 25
.15E-1 25
.15E-1 25
25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
Y .15E-1 Y 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
.15E-1 25
Z X .15E-1
.15E-1 Z X 25
25
225
5
25
.15E-1
.15E-1 25
(a) heat flux (b) external temperature
Figure 10.29: Boundary conditions for flow analysis
Environmental temperature. Via the boundary elements we can model the
fixed environmental temperature of 25 °C.
tankfs.fgc
PROPERTY LOADS EXTTEMP ETM 1 BOUND 25.
LABEL MESH OFF
LABEL MESH LOADS ETM
We define the fixed temperature via the EXTTEMP load class. Here the load
is named ETM and added to boundary case 1. We display the defined load
[Fig. 10.29b].
Variation in time. For a transient heat flow analysis Diana always requires
the variation in time of the boundary conditions. In the Design environment
we may specify this variation with a so-called time curve. In this example we
assume that the defined boundary case 1 does not change in time.
tankfs.fgc
CONSTRUCT TCURVE LIST 0.0 1.0 10000000.0 1.0
PROPERTY ATTACH LOADCASE 1 TCURVE TC1
We define a time curve for a time interval from t = 0 to infinity with a constant
multiplication factor of 1. By default iDiana names the time curve TC1. We
assign the time curve to boundary case 1.
10.3.1.4 Initial Temperature Field
By default Diana will assume a zero temperature field at the start of a transient
heat flow analysis. In this example the environmental temperature is 25 °C
and we may assume that this also is the initial temperature of the structure.
Therefore we must define an initial temperature field of 25 °C for all nodes of
the concrete tank.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
194 Fire near Concrete Safety Tank
tankfs.fgc
PROPERTY INITIAL INITEMP IC1 TANK 25
VIEW MESH TANK
LABEL MESH INITIAL CURRENT WHITE
EYE ZOOM FACTOR 15. 12000. 11000. 0.
We specify an initial condition named IC1 for all nodes in set TANK, i.e., in the
concrete structure. The INITEMP class indicates an initial temperature field. We
display the mesh for set TANK. Then we label all nodes of the the currently
displayed part of the mesh with their initial temperature [Fig. 10.30a]. As the
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:54 meshit1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:54 meshit2.ps
25 25
25
25 25
2522
22 52
2
52
2 52
2
52 52
2 52 25
25
25
2 552
5552
2
552
52
52
52
552
2
52
5552
2
52
25552
52
22
52
552
52
2
52
552
522
5252
522 52 25
55 5522
52
25552
52
22
52
552
52
2
5 52
52
2
52 52
52
22 52
52 25
5552
52
52
552
52
2
5552
52
2
5 52
52
252
52 25
2 5
255
22
552
5
252
2
552
2
55252 25
525
252
5
2
552
2
555
52
55 25
2222
52 525
22
5 55
5
25525
25
2525 25
2525
2525
25
25
2525
2525 25
2525
25
25
2525
2525 25 25 25 25 25 25 25 25 25 25 25 25 25
25
25
2525
2525
25
25
2525
2525
25
25
2525
2525 25
25
2525
2525
25
25 25
2525
25
2525
25
25 25 25
25
2525
25
25
2525
25 25 25 25
2525
25
2525
2525
25
25
2525
2525
25
25
25
25 25
25
25
25
25
25
25 25 25 25 25 25 25 25
25
2525
25
25
2525
25
25
25
25 25
25
25
25
25
25
25
2525
25
2525
25
2525
25
25
25
25
2525 25
25
25
25
25
25
25
25
2525
25
25 25 25 25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25 25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25 25 25 25 25 25 25 25 25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25 25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25 25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25 25 25 25 25 25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25 25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25 25 25 25 25 25 25 25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25 25 25 25 25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25 25 25 25 25 25 25 25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25 25 25 25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25 25 25 25 25 25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
Y 25
25
25
25
25
25
25
25 Y
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25 25 25 25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
25
Z X 25 25 25 25 25 25 25 25 25 2525 25 25 2525 252525 2525 2525
2525 2525
2525 2525
2525 25
25 252525
25 25
25 25
2525
25
2525
25
2525
25
25
25
25
2525
25
2525 Z X
25
25 25 25 25 25 25 25 25 25 25
25252525
25
2525 25
25 25
25
25 25
25
25 25
25
25 25
25
25
25
25 25
25
25 25
25
25
2525
25
25 25 25 25 25 25 25 25 2525 2525 25252525
2525 25
25252525
25 25
2525
25 25
25
2525
2525
25
2525
25
25 25 25 25 25
(a) entirely (b) beam
Figure 10.30: Initial temperature field
default label color for initial fields (orange) is hardly visible on paper we explic-
itly ask to display the labels in WHITE, this will give labels in black on the plot
file (and in this manual). Because of the overlapping labels we zoom in on the
beam at the dome–roof connection and then the values of 25 clearly stand out
at each node [Fig. 10.30b].
10.3.2 Model for Nonlinear Structural Analysis
For the nonlinear structural analysis we must adapt and supply some data for
the model that we used in the linear elastic analysis. This data involves the
loading and some additional material properties.
10.3.2.1 Loading
For the nonlinear analysis of the fire load we have two basic load cases: the
weight plus service load which we now combine in load case 1, and the prestress
of the reinforcements which remains load case 2. The calamity load is not needed
in the nonlinear analysis. To adapt the loading for the nonlinear analysis we
give the following commands in the iDiana Design environment.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.3 Model for Flow–Stress Analysis 195
tankfs.fgc
UTILITY DELETE LOADS SERVICE
yes
PROPERTY LOADS PRESSURE SERVICE 1 L1 0.147 NORMAL
UTILITY DELETE LOADS CALAMI
yes
First we delete the service load. Then we redefine the same service load and
add it to load case 1, i.e., the weight load. Finally we delete the calamity load.
tankfs.fgc
EYE FRAME
VIEW HIDDEN OFF
LABEL MESH OFF
LABEL MESH LOADS 1
LABEL MESH OFF
VIEW REINFORCE
LABEL MESH LOADS 2
To check the modified load cases we let iDiana display them. First we revert to
a display of the full mesh in green wire-netting style. Then we display load case
1 [Fig. 10.31a] for the mesh, and load case 2, the prestress, for the reinforcements
[Fig. 10.31b]. Note for load case 1 the arrows for all elements which represent
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:54 load1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:54 load2.ps
.5E-2
25
.5E-2
2.5E-2
5.5E-2
225.5E-2
5.5E-2
25.5E-2
225.5E-2
5.5E-2
25.5E-2
225.5E-2
5.5E-2
225.5E-2
5.5E-2
225.5E-2
5.5E-2
225.5E-2
5.5E-2
25.5E-2
25.5E-2
225.5E-2
5.5E-2
2 5.5E-2
2 5.5E-2
25.5E-2
225.5E-2
5.5E-2
225.5E-2
5.5E-2
2 5.5E-2
2 5.5E-2
25
25
.5E-2
25
.5E-2
25
.5E-2
25
.5E-2
25
.5E-2
25
.5E-2
25
.5E-2
25
.5E-2
25
.5E-2
25
.5E-2
25
.5E-2
25
.5E-2
25
.5E-2
25
.5E-2
25
.5E-2
25
.5E-2
25
.5E-2
25
.5E-2
25
25
25
25
25
25
25
.15E-1
25
.15E-1
25 0
.15E-1
25
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25 .12E4
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25 .12E4
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25 .12E4
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
Y .15E-1
25 Y
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25
.15E-1
25 .12E4
Z X .15E-1
25
25
225
5
.15E-1
25 Z X 0
.15E-1
.15E-1
25 0
(a) case 1: weight and service (b) case 2: prestress
Figure 10.31: Loads for nonlinear analysis
the weight load, and the additional arrows on top of the floor which represent
the pressure of the liquid in the inner tank. The display of load case 2, the
prestress in the reinforcement, is exactly the same as in the model for linear
analysis [Fig. 10.12b].
Variation in time. For a transient nonlinear analysis Diana always requires
the variation in time of the loading conditions. In this example we assume that
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
196 Fire near Concrete Safety Tank
the defined load case 1, weight and service load, does not change in time. We
may apply the same time curve as for the variation of the boundary conditions
in the heat flow model [§ 10.3.1.3 p. 193].
tankfs.fgc
PROPERTY ATTACH LOADCASE 1 TCURVE TC1
We assign the time curve to load case 1.
10.3.2.2 Material Properties
The data as specified for the linear elastic analysis is to be supplemented with the
material data for nonlinear thermal analysis. Therefore we launch the Property
Manager dialog to specify the additional data.
iDiana
View Property Manager...
↑ →
Property Manager
···
For this example we must specify additional material properties for the concrete
and for the reinforcement steel. We assume that the foundation interface be-
haves linearly. Therefore there is no need to add any nonlinear material data
to material SOILSP.
Concrete iDiana
Property Manager
↑ Materials Material Name: CONCRETE
↑Expansion →Isotropic - Constant Params.
↑Static Nonlinearity →Concrete and Brittle Materials →Multi-directional Fixed Crack
→Constant Stress Cut-off →Linear Tension Softening
→Ultimate Strain Based →Constant Shear Retention
→Drucker-Prager Plasticity →Ideal Plasticity
↑External →External Data from File
We select the material CONCRETE and and specify the thermal expansion co-
efficient α = 1.2×10−5 . For static nonlinearity we specify th tensile strength
ft = 1.8, the ultimate strain of the tension softening diagram εcr
u = 0.0019, the
constant shear retention factor β = 0.2, the cohesion c = 8.66, friction angle
sin φ = 0.5, and dilatancy angle sin ψ = 0.5.
For the concrete we must also specify the temperature dependence of the
Young’s modulus, the thermal expansion coefficient, and the tensile strength.
These dependencies must be added to the data file in Diana batch format
that we prepared for the temperature dependent properties for the flow analysis
[§ 10.3.1.2 p. 191].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.3 Model for Flow–Stress Analysis 197
conc.dat
TEMYOU 0. 17500. 70. 17500. 850. 0.
TEMALP 0. 1.2E-5 400. 1.2E-5 425. 2.4E-5 800. 2.4E-5
TEMYLD 0. 8.66 200. 8.66 850. 0.
The TEMYOU data item specifies the temperature influence on the Young’s mod-
ulus: E = 17500 until 70 °C and then decreases linearly to zero at 850 °C. The
TEMALP data item specifies the temperature influence on the thermal expansion
coefficient: α = 1.2×10−5 until 400 °C, then increases linearly to 2.4×10−5 at
425 °C and remains constant until 800 °C. The TEMYLD data item specifies the
temperature influence on the tensile strength: ft = 8.66 until 200 °C, then de-
creases linearly to zero at 850 °C. The external data file for concrete material
properties is now complete and we supply its name to iDiana via the Property
Manager dialog.
Reinforcement steel iDiana
Property Manager
Materials Material Name: STEEL
↑Expansion →Isotropic - Constant Params.
↑Static Nonlinearity →Reinforcement →Von Mises Plasticity → Ideal Plasticity
↑External →External Data from File
For the reinforcement steel we must also specify the material properties for non-
linear thermal analysis. Therefore we select the material STEEL and specify the
thermal expansion coefficient α = 1.2×10−5 . For static nonlinearity we specify
the yield stress σy = 400. Like for the concrete, the temperature dependence of
the reinforcement is specified via an external file.
steel.dat
TEMYOU 0. 210000. 150. 210000. 750. 0.
TEMALP 0. 1.2E-5 900. 1.2E-5
TEMYLD 0. 400. 300. 400. 750. 0.
High strength steel iDiana
Property Manager
Materials Material Name: →STEEL →STEELH
↑Static Nonlinearity →Reinforcement →Von Mises Plasticity → Ideal Plasticity
↑External →External Data from File
For the linear elastic analysis there was no difference between normal steel and
high strength steel. Both steel qualities have the same E, ν, and α. However, for
the nonlinear analysis we must specify another yield stress for the high strength
steel that usually is applied for the prestressed reinforcement. Therefore we
choose the STEEL material and then change the name in STEELH. In doing so
we create a copy of material STEEL. Now we edit the new material STEELH by
changing the yield stress to σy = 1800. We must also modify the temperature
dependent properties via another external file.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
198 Fire near Concrete Safety Tank
steelh.dat
TEMYOU 0. 210000. 150. 210000. 750. 0.
TEMALP 0. 1.2E-5 900. 1.2E-5
TEMYLD 0. 1800. 300. 1800. 750. 0.
Property assignment tankfs.fgc
PROPERTY ATTACH GR7 STEELH
PROPERTY ATTACH GR8 STEELH
PROPERTY ATTACH GR9 STEELH
PROPERTY ATTACH GR10 STEELH
PROPERTY ATTACH GR11 STEELH
PROPERTY ATTACH GR12 STEELH
PROPERTY ATTACH GR13 STEELH
We assign material STEELH to the prestressed reinforcements, GR7 to GR13 [§ 10.1.8
p. 174]. To check the proper assignment we give the following commands.
tankfs.fgc
LABEL MESH OFF
LABEL REINFORCE MATERIALS ALL RED
Here we see the reinforcements in the roof and floor labeled with STEEL and
those in the wall and beams with STEELH [Fig. 10.32]. The latter are indeed the
prestressed reinforcements.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:55 reimat.ps
STEEL
STEELH
STEELH
STEELH
STEEL
STEEL
STEELH
Y
STEEL
STEELH
STEEL
STEEL STEELH
STEEL STEELH
Z X
Figure 10.32: Materials for reinforcements
10.4 Staggered Flow–Stress Analysis
For a staggered flow–stress analysis we must perform a flow analysis followed
by a structural analysis.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.4 Staggered Flow–Stress Analysis 199
10.4.1 Transient Nonlinear Heat Flow Analysis
In this case we perform a transient heat flow analysis to determine the tem-
perature changes in time. The analysis is also nonlinear because the material
properties for the flow model depend on the temperature [§ 10.3.1.2 p. 190]. We
write an input data file in Diana batch format and initiate the analysis.
iDiana
UTILITY WRITE DIANA
yes
FILE CLOSE
yes
Fire load on concrete safety tank
ANALYSE TANK
Analysis Setup
specification of options
Via the Analysis Setup dialog we specify the various analysis options for heat
flow analysis. Here we perform eight time steps of 15, 45, 120, 180, 240, 300,
360, and 360 seconds respectively. The time steps represent 14 , 1, 3, 6, 10, 15,
21, and 27 minutes of fire time. The resulting batch analysis commands are as
follows.
flow.dcf
*FILOS
INITIA
*INPUT
*HEATTR
MODEL MATRIX CAPACI LUMPED
BEGIN INITIA
TEMPER
NONLIN
END INITIA
BEGIN EXECUTE
NONLIN
SIZES 15. 45. 120. 180. 240. 300. 360. 360.
END EXECUTE
*END
During the analysis Diana writes log lines which indicate the convergence.
flow.out
STEP 1 TERMINATED, CONVERGENCE AFTER 2 ITERATIONS
STEP 2 TERMINATED, CONVERGENCE AFTER 2 ITERATIONS
STEP 3 TERMINATED, CONVERGENCE AFTER 2 ITERATIONS
STEP 4 TERMINATED, CONVERGENCE AFTER 3 ITERATIONS
STEP 5 TERMINATED, CONVERGENCE AFTER 3 ITERATIONS
STEP 6 TERMINATED, CONVERGENCE AFTER 3 ITERATIONS
STEP 7 TERMINATED, CONVERGENCE AFTER 3 ITERATIONS
STEP 8 TERMINATED, CONVERGENCE AFTER 3 ITERATIONS
This shows that each of the steps has reached convergence. We may now enter
the iDiana Results environment to assess the analysis results.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
200 Fire near Concrete Safety Tank
flow.fvc
FEMVIEW FLOW
UTILITY TABULATE LOADCASES
VIEW MESH TANK
VIEW OPTIONS EDGES OUTLINE
The tabulation shows the the available load cases and analysis results.
flowlc.tb
;
; Model: FLOW
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; TR1 1 TIME = 15 "Boundary case 1"
; Nodal : PTE....S
; Element : EL.FLX.L
;
; TR1 2 TIME = 60 "Boundary case 1"
; Nodal : PTE....S
; Element : EL.FLX.L
;
; TR1 3 TIME = 180 "Boundary case 1"
; Nodal : PTE....S
; Element : EL.FLX.L
;
; TR1 4 TIME = 360 "Boundary case 1"
; Nodal : PTE....S
; Element : EL.FLX.L
;
; TR1 5 TIME = 600 "Boundary case 1"
; Nodal : PTE....S
; Element : EL.FLX.L
;
; TR1 6 TIME = 900 "Boundary case 1"
; Nodal : PTE....S
; Element : EL.FLX.L
;
; TR1 7 TIME = .126E4 "Boundary case 1"
; Nodal : PTE....S
; Element : EL.FLX.L
;
; TR1 8 TIME = .162E4 "Boundary case 1"
; Nodal : PTE....S
; Element : EL.FLX.L
;
Note that Module heattr has automatically created eight load cases, one for
each step. We display the outlines of the model for set TANK, i.e., the concrete.
Now we are ready to fill this with contour plots of the temperatures.
10.4.1.1 Temperatures
To display the temperature field we first select load cases TR1 8 which represents
the last time step, i.e., after twenty-seven minutes of fire.
flow.fvc
RESULTS LOADCASE TR1 8
RESULTS NODAL PTE....S PTE
PRESENT CONTOUR LEVELS
EYE ZOOM FACTOR 15. 11000. 11000. 0.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.4 Staggered Flow–Stress Analysis 201
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:39:00 flowte8a.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:39:00 flowte8b.ps
Model: FLOW Model: FLOW
TR1: Boundary case 1 TR1: Boundary case 1
Step: 8 TIME: .162E4 Step: 8 TIME: .162E4
Nodal PTE....S PTE Nodal PTE....S PTE
Max/Min on model set: Max/Min on model set:
Max = 112 Min = 25 Max = 112 Min = 25
104 104
96.3 96.3
88.4 88.4
80.4 80.4
Y 72.5 Y 72.5
64.6 64.6
56.7 56.7
Z X 48.8 Z X 48.8
40.8 40.8
32.9 32.9
(a) entirely (b) beam
Figure 10.33: Temperature contours after 27 minutes of fire
We select the PTE result attribute which represents the temperatures in the
nodes. We displays a contour plot of the temperature [Fig. 10.33a]. In the
results monitor iDiana writes the extreme temperature to be 112 °C. We also
zoom in on the beam and the upper part of the wall [Fig. 10.33b]. This shows
that the heat of the fire has penetrated into the concrete over about 150 mm
which is about one-third of the wall thickness.
Variation in time. We will apply two options to see the development of the
temperature in time: an animation sequence and a history plot.
Animation flow.fvc
PRESENT CONTOUR FROM 26 TO 100 LEVELS 10
RESULTS LOADCASE TR1
UTILITY SETUP ANIMATE LINEAR
UTILITY SETUP ANIMATE SPEED 20
DRAWING ANIMATE LOADCASES PLOTFILE temper
In an animation sequence of contour plots we must be aware that the frames
of the animation all use the same colors to represent a certain value. Therefore
we explicitly specify the values for the first and last contour. We select all time
steps (load cases) to get an animation with eight frames. For an animation of
an increasing temperature two more options are applicable: the sequence and
speed of the frames display. We may set these beforehand. Here we display
the frames linearly, i.e., sequentially from the first to the last and then starting
again at the first. The heating process is rather slow and we make the animation
a bit more realistic by slowing it down to 20% of the maximum speed. Now we
have set all appropriate parameters and options and may start the animation.
By default the animation appears on the screen. Here we apply the PLOTFILE
option to get the frames on files which we can show in a document [Fig. 10.34].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
202 Fire near Concrete Safety Tank
iDIANA 9.4.3-02 : TNO Diana BV iDIANA 9.4.3-02
28 OCT: 2010
TNO Diana
02:39:00
BV temper001 iDIANA 9.4.3-02
28 OCT: 2010
TNO Diana
02:39:00
BV temper002 iDIANA 9.4.3-02
28 OCT: 2010
TNO Diana
02:39:00
BV temper003 28 OCT 2010 02:39:00 temper004
Model: FLOW Model: FLOW Model: FLOW Model: FLOW
TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1
Step: 1 TIME: 15 Step: 2 TIME: 60 Step: 3 TIME: 180 Step: 4 TIME: 360
Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = 25.8 Min = 25 Max = 28.4 Min = 25 Max = 35.1 Min = 25 Max = 45.1 Min = 25
100 100 100 100
93.3 93.3 93.3 93.3
86.5 86.5 86.5 86.5
79.8 79.8 79.8 79.8
73.1 73.1 73.1 73.1
66.4 66.4 66.4 66.4
15 s 1 min 3 min 6 min
Y Y 59.6 Y 59.6 Y 59.6 59.6
52.9 52.9 52.9 52.9
46.2 46.2 46.2 46.2
iDIANA
Z 9.4.3-02
X : TNO Diana BV Z 28 39.5 9.4.3-02 : TNO Diana BV
X OCT 2010 02:39:00 temper005
iDIANA Z X 39.5 28 OCT 2010 02:39:00 temper006
iDIANA
Z 9.4.3-02
X : TNO Diana BV 39.5 39.5
28 OCT 2010 02:39:01 temper007
32.7 32.7 32.7 32.7
26 26 26 26
Model: FLOW Model: FLOW Model: FLOW
TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1
Step: 5 TIME: 600 Step: 6 TIME: 900 Step: 7 TIME: .126E4
Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE
Max/Min on model set: DRAWING ANIMATE LOADCASES PLOTFILE temper Max/Min
DRAWING on model LOADCASES
ANIMATE set: PLOTFILE temper Max/Min on model set:
DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper
Max = 58.3 Min = 25 Max = 74.4 Min = 25 Max = 93.5 Min = 25
100 100 100
93.3 93.3 93.3
86.5 86.5 86.5
79.8 79.8 79.8
73.1 73.1 73.1
66.4 66.4 66.4
10 min 15 min 21 min
Y 9.4.3-02 : TNO Diana BV 59.6
Y 59.6
Y 59.6
iDIANA 28 OCT 2010 02:39:01 temper008
52.9 52.9 52.9
46.2 46.2 46.2
Model: FLOW 39.5 39.5 39.5
Z X case 1
TR1: Boundary Z X Z X
32.7 32.7 32.7
Step: 8 TIME: .162E4 26 26 26
Nodal PTE....S PTE
Max/Min on model set:
Max = 112 Min = 25
DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper
100
93.3
86.5
79.8
73.1
66.4
27 min
Y 59.6
52.9
46.2
Z X 39.5
32.7
26
Figure 10.34: Animation sequence of temperature contours
DRAWING ANIMATE LOADCASES PLOTFILE temper
History plot. To plot the temperature history we must choose a significant
node, in this case on the outer edge of the beam. We may indicate the node
with a cursor hit or with its number. For both methods of indication we need
a display of the mesh.
flow.fvc
VIEW MESH
LABEL MESH NODES
DRAWING CONTENTS POINTER POSITION
DRAWING CONTENTS POINTER DELETE
PRESENT GRAPH NODE 388
We choose for indication via the node number and therefore label all displayed
nodes [Fig. 10.35a]. We decide to take node 388 as location for a history plot
and then mark the node with an arrow for which we specify the position of
the tail and head with the graphics cursor. Finally we draw a graph for the
temperature history of node 388 [Fig. 10.35b].
10.4.2 Transient Nonlinear Structural Analysis
In the structural analysis we can apply the development of the nodal temper-
atures in time, as obtained in a transient heat flow analysis [§ 10.4.1 p. 199]
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.4 Staggered Flow–Stress Analysis 203
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:39:01 flowbn.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:39:01 flowtg.ps
Model: FLOW 804 Model: FLOW
Nodal PTE....S PTE
853 Max/Min on whole graph:
Ymax = 112
902 Ymin = 25.8
740 739 738 699 702 705 709 Xmax = .162E4
Xmin = 15
737 Variation over loadcases
Node 388
734 736 120
735
110
733 698 701 704 708
N 100
O
732 D
A 90
L
697 700 703 707 P 80
T
E 70
.
.
. 60
.
396 395 394 706 S
50
P
T
E 40
30
393 392 391
20
0 .2 .4 .6 .8 1 1.2 1.4 1.6 1.8
Y TIME *1E3
Z X 390 389 388
(a) node location (b) graph
Figure 10.35: Temperature history
[Fig. 10.34 p. 202]. These temperatures are still available on the filos file. To
initiate the transient nonlinear structural analysis we may enter the iDiana
Index environment.
iDiana
INDEX
ANALYSE TANK
Analysis Setup
specification of options
Via the Analysis Setup dialog we specify the various options resulting in the
following command file which performs a transient analysis up to 23 minutes.
Note that we do not initialize a new filos file!.
struct.dcf
*NONLIN
BEGIN OUTPUT TABULA
BEGIN SELECT
ELEMEN 176 289 290
BEGIN REINFO 1-15
ELEMEN 176 289 290
END REINFO
STEPS 1 4 5 7
END SELECT
STRAIN ELASTI LOCAL INTPNT
STRAIN CREEP LOCAL INTPNT
STRAIN PLASTI LOCAL INTPNT
STRAIN CRACK INTPNT
STRESS TOTAL LOCAL INTPNT
END OUTPUT
BEGIN OUTPUT FEMVIEW BINARY
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
204 Fire near Concrete Safety Tank
DISPLA TOTAL
STRAIN CRACK
END OUTPUT
BEGIN TYPE
BEGIN PHYSIC
CREEP FIRST
CRACKI CONSIS
END PHYSIC
END TYPE
BEGIN EXECUT
BEGIN START
INITIA STRESS INPUT LOAD=2 FACTOR=1.0
STEPS OFF
END START
END EXECUT
BEGIN EXECUT
TIME STEPS EXPLIC SIZES 1.E-10 400 100 400 400 40(2)
BEGIN ITERAT
BEGIN CONVER
ENERGY CONTIN TOLCON=0.0001
FORCE OFF
DISPLA OFF
END CONVER
END ITERAT
END EXECUT
*END
The presented time steps were chosen by trial and error to achieve convergence
within a reasonable number of iterations. To achieve convergence it is important
that only a limited number of cracks arise per time step.
The structural analysis yields two types of output. In tabular form we get
the strains and stresses for some selected steps. The displacements and crack
strains are written to a database STRUCT for the iDiana Results environment.
The analysis did not converge anymore for further time steps, as the roof almost
completely collapsed due to cracking [Fig. 10.38].
10.4.2.1 Deformation
We enter the Results environment of iDiana to make plots of the deformed
model. iDiana immediately shows the undeformed model in green.
struct.fvc
FEMVIEW TANK
RESULTS LOADCASE LC1 1
RESULTS NODAL TDTX...G RESTDT
PRESENT SHAPE
RESULTS LOADCASE LC1 7
PRESENT SHAPE
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.4 Staggered Flow–Stress Analysis 205
We select the nodal results attribute TDT which represents the total displace-
ments. Then we respectively select load case LC1 1 for the first step which is the
situation after application of the initial load, and LC1 7 which is the situation
after the last executed time step, i.e., after 23 minutes of fire. We display the
deformed model in red [Fig. 10.36]. In the results monitor we see that iDiana
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:39:12 dfm1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:39:12 dfm7.ps
Model: STRUCT Model: STRUCT
LC1: Load case 1 LC1: Load case 1
Step: 1 TIME: .1E-9 Step: 7 TIME: .138E4
Nodal TDTX...G RESTDT Nodal TDTX...G RESTDT
Max = 9.28 Max = 6.22
Min = .199E-4 Min = .106E-4
Factor = 362 Factor = 541
Y Y
Z X Z X
(a) at initial load (306×) (b) after 23 minutes of fire (456×)
Figure 10.36: Deformed model
has automatically chosen multiplication factors for the deformation of 306 and
456 respectively. Therefore the two displays may not be compared as such.
For proper comparison we could redraw the deformed shapes with an explicitly
specified multiplication factor, equal for both displays. However, it is more in-
structive to show the development of the deformation in an animation sequence.
Animation struct.fvc
RESULTS LOADCASE LC1
UTILITY SETUP ANIMATE LINEAR
DRAWING ANIMATE LOADCASES PLOTFILE deform
For a complete animation sequence we select all load cases (time steps). We
apply the same options for the animation as we did for the temperature de-
velopment. The development of the deformation shows up clearly [Fig. 10.37].
Note that iDiana now applies a multiplication factor of 456× for all frames.
10.4.2.2 Strains
Below we show a fragment of the tabular output with the elastic and creep
strains after 23 minutes of fire (step 7).
struct.tb
Analysis type NONLIN
Step nr. 7
Time 1.380E+03
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
206 Fire near Concrete Safety Tank
iDIANA 9.4.3-02 : TNO Diana BV iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:39:12 deform001
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:39:12 deform002
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:39:13 deform003
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:39:13 deform004
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:39:13 deform005
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:39:13 deform006 28 OCT 2010 02:39:13 deform007
Model: STRUCT Model: STRUCT Model: STRUCT Model: STRUCT Model: STRUCT Model: STRUCT Model: STRUCT
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1 LC1: Load case 1 LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Step: 1 TIME: .1E-9 Step: 2 TIME: 400 Step: 3 TIME: 500 Step: 4 TIME: 900 Step: 5 TIME: .13E4 Step: 6 TIME: .134E4 Step: 7 TIME: .138E4
Nodal TDTX...G RESTDT Nodal TDTX...G RESTDT Nodal TDTX...G RESTDT Nodal TDTX...G RESTDT Nodal TDTX...G RESTDT Nodal TDTX...G RESTDT Nodal TDTX...G RESTDT
Max = 9.28 Max = 8.25 Max = 8.01 Max = 7.13 Max = 6.36 Max = 6.29 Max = 6.22
Min = .199E-4 Min = .964E-5 Min = .729E-5 Min = .148E-5 Min = .917E-5 Min = .988E-5 Min = .106E-4
Factor = 541 Factor = 541 Factor = 541 Factor = 541 Factor = 541 Factor = 541 Factor = 541
Y Y Y Y Y Y Y
Z X Z X Z X Z X Z X Z X Z X
DRAWING ANIMATE LOADCASES PLOTFILE deform DRAWING ANIMATE LOADCASES PLOTFILE deform DRAWING ANIMATE LOADCASES PLOTFILE deform DRAWING ANIMATE LOADCASES PLOTFILE deform DRAWING ANIMATE LOADCASES PLOTFILE deform DRAWING ANIMATE LOADCASES PLOTFILE deform DRAWING ANIMATE LOADCASES PLOTFILE deform
Figure 10.37: Animated deformation for seven time steps
Result STRAIN ELASTI GREEN
Axes LOCAL
Location of results INTPNT
Elmnr Intpt Eexx Eeyy Eezz Gexy
176 1 1.660E-04 -2.850E-04 -3.551E-04 -3.039E-05
2 8.145E-05 -3.028E-04 -2.286E-04 1.400E-04
3 5.457E-05 -9.835E-05 -9.372E-05 -4.039E-05
4 5.320E-06 -8.626E-05 -4.869E-05 -8.169E-05
289 1 4.767E-05 3.713E-05 -6.159E-05 1.083E-04
2 6.993E-05 2.393E-05 -6.227E-05 1.193E-04
3 6.054E-05 4.195E-05 -7.388E-05 1.161E-04
4 7.389E-05 2.680E-05 -7.436E-05 1.017E-04
290 1 5.920E-05 4.361E-05 -8.162E-05 1.105E-04
2 5.286E-05 4.046E-05 -8.137E-05 9.768E-05
3 4.221E-05 1.798E-05 -7.700E-05 5.326E-05
4 1.083E-05 1.817E-05 -7.271E-05 1.269E-05
Analysis type NONLIN
Step nr. 7
Time 1.380E+03
Result STRAIN CREEP GREEN
Axes LOCAL
Location of results INTPNT
Elmnr Intpt Ecxx Ecyy Eczz Gcxy
176 1 1.016E-04 -1.929E-04 -1.987E-04 -1.549E-05
2 3.052E-05 -1.169E-04 -7.646E-05 4.868E-05
3 1.280E-05 -2.661E-05 -2.084E-05 -3.986E-06
4 3.097E-06 -1.370E-05 -8.689E-06 -6.234E-06
289 1 4.083E-07 3.785E-07 -7.961E-07 7.829E-07
2 2.265E-07 1.158E-07 -2.483E-07 3.876E-07
3 5.339E-07 4.330E-07 -8.573E-07 1.023E-06
4 1.988E-07 1.205E-07 -2.644E-07 4.320E-07
290 1 5.614E-07 3.478E-07 -8.229E-07 1.007E-06
struct Page 8
Elmnr Intpt Ecxx Ecyy Eczz Gcxy
2 2.199E-07 1.028E-07 -2.514E-07 3.231E-07
3 4.317E-07 2.120E-07 -6.066E-07 6.887E-07
4 9.437E-08 7.182E-08 -1.786E-07 1.573E-07
10.4.2.3 Cracks
To display the crack pattern at the wall–roof connection we first zoom in on
that area.
struct.fvc
EYE ZOOM FACTOR 15. 11000. 11000. 0.
RESULTS LOADCASE LC1 4
RESULTS GAUSSIAN EL.EKNN1 EKNN
PRESENT DISC
RESULTS LOADCASE LC1 5
PRESENT DISC
RESULTS LOADCASE LC1 7
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
10.4 Staggered Flow–Stress Analysis 207
PRESENT DISC
We select steps 4, 5, and 7 which represent the situation after 15, 21.7, and
23 minutes. Furthermore we select the results attribute EKNN which represents
the normal crack strains. We display the crack strains as disks in the crack
plane. Because we look in the direction of this plane, the cracks appear as lines
[Fig. 10.38].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:39:13 crck4.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:39:13 crck5.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:39:13 crck7.ps
Model: STRUCT Model: STRUCT Model: STRUCT
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Step: 4 TIME: 900 Step: 5 TIME: .13E4 Step: 7 TIME: .138E4
Gauss EL.EKNN1 EKNN Gauss EL.EKNN1 EKNN Gauss EL.EKNN1 EKNN
Max = .773E-3 Max = .158E-2 Max = .182E-2
Min = 0 Min = 0 Min = 0
Y Y Y
Z X .515E-3 Z X .105E-2 Z X .121E-2
.258E-3 .526E-3 .607E-3
(a) after 15 minutes (b) after 21.7 minutes (c) after 23 minutes
Figure 10.38: Crack pattern
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
208 Fire near Concrete Safety Tank
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
Chapter 11
Gas Explosion in Tunnel
Name: Tunnel
Path: /Examples/ConcMas/Tunnel
Keywords: analys: dynami eigen linear nonlin physic static transi. con-
str: suppor tying. elemen: cl6tm cq16e grid mass pstrai
reinfo taper. load: edge elemen force time weight. materi:
consta crack cutoff elasti harden isotro linear massli plasti re-
tent smear soften strain vonmis. option: direct groups modifi
newmar newton units. post: binary femvie. pre: femgen.
result: cauchy crack displa green plasti status strain stress
total. analys: dynami eigen linear nonlin physic static transi.
constr: suppor tying. elemen: cl6tm cq16e grid mass pstrai
reinfo taper. load: edge elemen force time weight. materi:
consta crack cutoff elasti harden isotro linear massli plasti retent
smear soften strain vonmis. option: direct groups modifi new-
mar newton regula units. post: binary femvie. pre: femgen.
result: cauchy crack displa green plasti status strain stress
total veloci.
11.1 Description
This example involves an underwater tunnel of which a typical cross-section is
shown in Figure 11.1 on the next page. For comprehensive description of this
analysis example see Meyer [10], Van Mier [13] and Nauta [11].
11.1.1 Loading
The tunnel segment is subjected to a static loading by dead weight and sand and
water pressure and to a dynamic loading by an internal explosion. It has been
proved that both static and dynamic loading yield the same type of deformation
and moment distribution. Therefore, it is possible to model only one quarter of
the entire roof slab by finite elements and to apply boundary constraints which
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
210 Gas Explosion in Tunnel
♥ 10∅40
modeled part 6∅30
10∅30
9∅40
3∅40 + 4∅30
7.86 m
2 × 20∅30
14.90 m
Figure 11.1: Tunnel cross-section with reinforcement for a 1.5 m wide section
13800 kg/m2
Sand 2 m
ρ = 1900 kg/m3
Water 10 m
ρ = 1000 kg/m3
Explosion p MPa
Figure 11.2: Quarter roof slab – loading and supports
are applicable to both loadings [Fig. 11.2]. The weight of sand is modeled with
a layer of 2 m thickness and a mass density ρ = 1900 kg/m3 . For the weight of
water, a height of 10 m has been modeled. The pressure due to sand and water
is (2 × 1900 + 10 × 1000) = 13800 kg/m2 for a tunnel section of 1 m length.
11.1.2 Explosion
The explosion pressure [Fig. 11.3] starts with an instantaneous shock front, fol-
lowed by a parabolic decrement of the overpressure during 25 ms. Then the
overpressure remains constant during 100 ms, the ‘overpressure plateau’. In the
next 25 ms the depressurizing takes place.
11.1.3 Material Properties
The nonlinear behavior of concrete under tension has been described with a
cracking model as in Figure 11.4a. Table 11.1 gives the values of the material
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
11.1 Description 211
p
MPa
2.0
0.5
0.0 t
0 25 125 150 ms
Figure 11.3: Explosion – pressure in time
σ
σ σy
ft
Es
ε
Ec σy
ε
εcr
u
(a) Concrete (b) Reinforcement steel
Figure 11.4: Material models
parameters. The behavior under pressure is assumed to be elastic: no plasticity
Table 11.1: Material parameters for tunnel
Young’s modulus Ec 22000 MPa
Poisson’s ratio ν 0.2
Mass density ρ 2400 kg/m3
Concrete
Tensile strength ft 3.360 MPa
Ultimate crack strain εcr
u 0.001
Shear retention factor β 0.2
Reinforcement Young’s modulus Es 210000 MPa
steel Yield stress σy 528 MPa
check. The ultimate crack strain εcr
u has been determined with tension stiffening
according to:
fu
εcr
u = (11.1)
Eu
It is common practice not to count for the maximum steel stress, but to take a
kind of average:
528×106
εcr
u = × 0.4 ≈ 0.001 (11.2)
210000×106
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
212 Gas Explosion in Tunnel
Due to cracking, the shear stiffness will decrease. This effect, the so-called
‘aggregate interlock’, has been modeled via constant shear retention with a
reduction factor β = 0.2. For the reinforcement steel, the nonlinear behavior
has been described with plasticity according to the Von Mises yield criterion
[Fig. 11.4b]. Due to the effect of sudden dynamic loading, the material strength
is assumed to be 20% higher as it would be in static loading.
11.1.4 Finite Element Idealization
The quarter of the entire roof slab is modeled with 3×16 CQ16E plane strain el-
ements, with a 2×2 integration scheme, and reinforcement bars [Fig. 11.5]. The
Y
♥ P
F E
0.9
1.3
C D
X
A B
Z 0.5 0.5 2.5 4.5
Figure 11.5: Finite element model
boundary constraints have been determined from the results of a linear static
analysis applied on a two-dimensional frame model of the complete tunnel as
described by Meyer [10]. Right edge DE is supported horizontally (no rota-
tion). For left edge AF rotations are suppressed, but the edge is free to move
horizontally. This is modeled with linear constraints (tyings).
The sand and water, resting on the roof, affect the dynamic behavior of the
tunnel. To model this effect, we will attach mass elements along edge EF.
11.2 Finite Element Model
To make the finite element model we start iDiana and enter the Design envi-
ronment with the model name.
iDiana
FEMGEN ROOF
Analysis and Units
Analysis Selection
Model Type: → Structural Plane Strain
In the Analysis and Units dialog we specify that this model is for structural
plane strain analysis.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
11.2 Finite Element Model 213
11.2.1 Geometry Definition
We will define the geometry via points and a surface.
Points roof.fgc
GEOMETRY POINT PA 0.0 0.0
GEOMETRY POINT PB 1.0 0.0
GEOMETRY POINT PC 3.5 0.4
GEOMETRY POINT PD 8.0 0.4
GEOMETRY POINT PE 8.0 1.3
GEOMETRY POINT PF 0.0 1.3
EYE FRAME
VIEW GEOMETRY ALL RED
LABEL GEOMETRY POINTS
We specify the coordinates of points A to F [Fig. 11.5] and name them explic-
itly PA to PF. A plane strain model is situated in the XY -plane, i.e., the Z-
coordinates are zero. We may omit these in the definition of the geometrical
points. We display the specified points, labeled with their names, fitted in the
iDiana viewport [Fig. 11.6a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:30 points.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:30 geom.ps
Model: ROOF Model: ROOF
Analysis: DIANA Analysis: DIANA
Model Type: Structural plane strain Model Type: Structural plane strain
PF PE L6
L1
S1 L5
PC PD L4
L7
L3
PA PB L2 L8
Y Y
Z X Z X
(a) points (b) lines and surfaces
Figure 11.6: Geometry
Surfaces roof.fgc
GEOMETRY SURFACE 4POINTS PA +PB +PC PD PE PF
GEOMETRY SPLIT L2 0.5
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY LINES ALL VIOLET
LABEL GEOMETRY SURFACES ALL BLUE
We specify the geometrical surface between the points. We use the + symbol
to indicate points that are included in the surface side definition. We finish
the geometry by splitting line L2 in two halves, because we need a point in the
middle to properly define the supports. Here the SPLIT option splits line L2 in
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
214 Gas Explosion in Tunnel
two new lines, connected via a new point P7. Finally we display the defined
geometry, including labels for lines and surfaces [Fig. 11.6b]. Note that lines L2,
L8,L3 and L4 together form line L7.
11.2.2 Meshing
We are now ready to generate the finite element mesh of the roof.
Element types and divisions roof.fgc
MESHING TYPES ALL QU8 CQ16E
MESHING TYPES L6 BE3 CL6TM
MESHING DIVISION ELSIZE ALL 0.25
MESHING DIVISION PROPAGATE L1 6
We select the QU8 generic element type, and the CQ16E quadratic plane strain
Diana element for the surface of the model and the BE3 generic element type,
and the CL6TM distributed mass element for the top line. We specify the number
of divisions model wide using half the required element size. This is done because
quadratic elements use two divisions along an edge. To get a structured mesh
we need to make the division on the right side edge equal to the division on
the left side edge. Due to the PROPAGATE option iDiana will apply the same
division for lines opposite to the specified line. In this case, the same division
as line L1 for all vertical lines.
Generation and display roof.fgc
MESHING GENERATE
MESHING RENUMBER GLOBAL XYZ
VIEW MESH
VIEW OPTIONS SHRINK
We generate the mesh, renumber the nodes and display it in ‘shrunken element’
style [Fig. 11.7].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:30 mesh.ps
Model: ROOF
Analysis: DIANA
Model Type: Structural plane strain
Z X
Figure 11.7: Generated mesh
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
11.2 Finite Element Model 215
11.2.3 Reinforcements
For the reinforcement grids, which show up as lines in a plane strain model, we
must define some new points and then put in the reinforcement grids. In this
example all reinforcements are straight lines which we define by their two end
points combined with the AXI-SYM option to indicate that the grid only consists
of a single line, which is the case in axisymmetric and plane strain models. We
simply create the appropriate end points via the a translation of the geometry.
In some cases we copy an existing reinforcement. From a geometric point of
view there are five grids [Fig. 11.1]: a grid at 5 cm below the top surface, a grid
at 10 cm below the top surface, a grid at 5 cm above the bottom surface, and
two vertical grids which stick from the wall into the roof slab. Basically each
grid consists of one or more sections, where multiple sections are necessary if
the reinforcement is bent.
Top roof.fgc
GEOMETRY COPY PF TRANSLATE 0.0 -0.05 0.0
GEOMETRY COPY P2 TRANSLATE 5.5 0.0 0.0
REINFORCE GRID SECTION RE1 AXI-SYM P2 P3
REINFORCE GRID GR1 RE1
GEOMETRY COPY P3 TRANSLATE 1.0 0.0 0.0
REINFORCE GRID SECTION RE2 AXI-SYM P3 P4
REINFORCE GRID GR2 RE2
GEOMETRY COPY P4 TRANSLATE 1.5 0.0 0.0
REINFORCE GRID SECTION RE3 AXI-SYM P4 P5
REINFORCE GRID GR3 RE3
Because the top grid has three different cross-sections, we must define three
separate reinforcements: GR1 from X = 0 to 5.5, GR2 to 6.5, and GR3 to the
right end of the model at X = 8.
Sub-top roof.fgc
GEOMETRY COPY P2 TRANSLATE 0.0 -0.05 0.0
GEOMETRY COPY P6 TRANSLATE 3.5 0.0 0.0
REINFORCE GRID SECTION RE4 AXI-SYM P6 P7
REINFORCE GRID GR4 RE4
GEOMETRY COPY P7 TRANSLATE 1.0 0.0 0.0
REINFORCE GRID SECTION RE5 AXI-SYM P7 P8
REINFORCE GRID GR5 RE5
REINFORCE COPY GR5 GR6 TRANSLATE 1.0 0.0 0.0
The sub-top grid is located 10 cm below the top surface, or 5 cm below the top
grid. Here we create the start point of the sub-top grid by a 5 cm downward
translation of the start point of the top grid. Like the top grid, the sub-top
grid has three different cross-sections so we must define three separate rein-
forcements: GR4 up to X = 3.5, GR5 up to X = 4.5, and GR6 up to X = 5.5.
Since GR5 and GR6 have an identical shape we simply use REINFORCE COPY to
generate GR6.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
216 Gas Explosion in Tunnel
Bottom roof.fgc
GEOMETRY COPY PA TRANSLATE 0.0 0.05 0.0
GEOMETRY COPY PB TRANSLATE 0.0 0.05 0.0
REINFORCE GRID SECTION RE7 AXI-SYM P10 P11
GEOMETRY COPY PC TRANSLATE 0.0 0.05 0.0
REINFORCE GRID SECTION RE8 AXI-SYM P11 P12
REINFORCE GRID GR7 RE7 RE8
GEOMETRY COPY PD TRANSLATE 0.0 0.05 0.0
REINFORCE GRID SECTION RE9 AXI-SYM P12 P13
REINFORCE GRID GR8 RE9
The bottom grid has two different cross-sections so we must define two rein-
forcements. The first one, GR7, has a bent near point B [Fig. 11.5] which is 5
cm above the geometrical point P2. Because of the bent, GR7 comprises two
sections: RE7 and RE8. The second reinforcement of the bottom grid, GR8, ends
at the right end of the model, 5 cm above point P4.
Wall–roof roof.fgc
GEOMETRY COPY P1 TRANSLATE 0.04 0.0 0.0
GEOMETRY COPY P14 TRANSLATE 0.0 0.87 0.0
REINFORCE GRID SECTION RE10 AXI-SYM P14 P15
REINFORCE GRID GR9 RE10
REINFORCE COPY GR9 GR10 TRANSLATE .42 0 0
The last two reinforcement grids, GR9 and GR10, stick vertically into roof slab,
respectively at X = 0.54 and X = 0.96 and over two-third of the height of the
slab: 32 × 1.3 ≈ 0.866667. Since GR9 and GR10 have an identical shape we simply
use REINFORCE COPY to generate GR10.
Reinforcement display roof.fgc
VIEW OPTIONS SHRINK OFF
VIEW REINFORCE +GR1 RED
VIEW REINFORCE +GR2 BLUE
VIEW REINFORCE +GR3 RED
VIEW REINFORCE +GR4 BLUE
VIEW REINFORCE +GR5 VIOLET
VIEW REINFORCE +GR6 BLUE
VIEW REINFORCE +GR7 RED
VIEW REINFORCE +GR8 BLUE
VIEW REINFORCE +GR9 VIOLET
VIEW REINFORCE +GR10 BLUE
LABEL REINFORCE GRID
We display the various reinforcements with different colors to be able to dis-
tinguish the location of the connection points [Fig. 11.8]. For instance the top
reinforcement grid is displayed in red–blue–red, and the sub-top in blue–violet–
blue. We display each reinforcement grid labeled with its name.
11.2.4 Boundary Constraints
The boundary constraints comprise the rigid supports and the linear constraints
to keep the left edge of the model vertically.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
11.2 Finite Element Model 217
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:31 reinf.ps
Model: ROOF
Analysis: DIANA
Model Type: Structural plane strain
GR4 GR1 GR5 GR6 GR2 GR3
GR9 GR10 GR8
GR7
Z X
Figure 11.8: Reinforcements
roof.fgc
PROPERTY BOUNDARY CONSTRAINT L8 Y
PROPERTY BOUNDARY CONSTRAINT L5 X
PROPERTY BOUNDARY MPC RBEAM L1 PA X
LABEL REINFORCE OFF
VIEW REINFORCE OFF
DRAWING DISPLAY
LABEL MESH CONSTRNT
First we suppress the vertical (Y) displacement of line L8, which is the right half
of the roof–wall connection line. Then the horizontal (X) displacement of line L5
are suppressed, i.e., the right edge of the model. To keep the left edge vertically
we apply a special linear multi-point constraint, a so-called Rigid Beam MPC,
The MPC is applied along line L1 with the horizontal (X) displacement of point
PA as master degree of freedom. We display the defined boundary constraints
[Fig. 11.9a]. The supports show up at the nodes as red spikes. Letters S and M
respectively mark the slave and master degrees of freedom for the MPC.
11.2.5 Loading
Loading consists of three cases: dead weight (1), sand and water pressure (2)
and an initial value for the explosion pressure (3) of 1×106 N/m2 = 10 bar.
Dead weight roof.fgc
PROPERTY LOADS GRAVITY WEIGHT 1 ALL -9.81 Y
First we define the dead weight of the model via the GRAVITY load class. We
name the load WEIGHT and specify it as load case 1. The gravity acceleration
g = 9.81 acts downward, i.e., in the −Y -direction.
Sand and water pressure roof.fgc
PROPERTY LOADS PRESSURE PSAND 2 L6 S1 135378.0 NORMAL
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
218 Gas Explosion in Tunnel
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:31 bound.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:32 loads.ps
Model: ROOF Model: ROOF
Analysis: DIANA Analysis: DIANA
Model Type: Structural plane strain Model Type: Structural plane strain
3S
3S
3S
3S
3S
3S
3M
Y Y
Z X Z X
(a) constraints (b) load cases
Figure 11.9: Boundary conditions
PROPERTY LOADS PRESSURE PWATER 2 L1 580627.0 NORMAL
We define a pressure load, named PSAND, via the PRESSURE load class and in
load case 2. This load acts along the line L6 in the NORMAL direction. We define
the water pressure at the left, along line L1, and call it PWATER. This load also
belongs to load case 2.
Explosion roof.fgc
CONSTRUCT SET BOTTOM APPEND LINES L3 L4
PROPERTY LOADS PRESSURE PEXPIN 3 BOTTOM 1000000.0 NORMAL
PROPERTY LOADS PRESSURE PEXPRO 3 L1 -1887000.0 NORMAL
CONSTRUCT TCURVE LIST FILE ”timelo.dat”
PROPERTY ATTACH LOADCASE 3 TCURVE TC1
The initial explosion pressure along the bottom, lines L3 and L4, is defined as load
case 3. Due to the NORMAL option the load PEXPIN will always act perpendicular
to the element edge, even along the inclined line L3. According to Van Mier [13]
an additional horizontal distributed tension force must be added in the roof slab
at the left edge of the model. For that, we apply a PRESSURE load PEXPRO along
line L1.
Finally we must specify the time–load diagram of the explosion pressure
[Fig. 11.3]. This is done via a time curve of which the xy-coordinates are supplied
via an external file timelo.dat, as shown below. By attaching the time curve
to load case 3, the explosion pressure in time is fully specified.
Time–load diagram timelo.dat
0.000 0.0000
1.E-6 2.0000
0.001 1.8824
0.002 1.7696
0.003 1.6616
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
11.2 Finite Element Model 219
0.004 1.5584
0.005 1.4600
0.006 1.3664
0.007 1.2776
0.008 1.1936
0.009 1.1144
0.010 1.0400
0.011 0.9704
0.012 0.9056
0.013 0.8456
0.014 0.7904
0.015 0.7400
0.016 0.6944
0.017 0.6536
0.018 0.6176
0.019 0.5864
0.020 0.5600
0.021 0.5384
0.022 0.5216
0.023 0.5096
0.024 0.5024
0.025 0.5000
0.125 0.5000
0.150 0.0000
1.000 0.0000
Load cases display roof.fgc
LABEL MESH OFF
LABEL MESH LOADS 1 VIOLET
LABEL MESH LOADS 2 BLUE
LABEL MESH LOADS 3 ORANGE
To check the applied load cases, and particularly their direction, we display
them with various colors [Fig. 11.9b]. The little violet arrows for all elements
indicate the dead weight. The blue ones, in two sizes, respectively display the
sand and water pressure. In orange we see the explosion pressure along the
bottom and the larger horizontal tension force along the left edge.
11.2.6 Material and Physical Properties
We will now specify material and physical properties for the concrete, water and
sand, and the reinforcements via the Property Manager dialog.
iDiana
View →Property Manager...
↑
Property Manager
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
220 Gas Explosion in Tunnel
↑Materials Material Name: CONCRETE
↑Linear Elasticity →Isotropic
↑Mass →Mass Density
↑Static Nonlinearity →Concrete and Brittle Materials →Multi-directional Fixed Crack
→Constant Stress Cut-off →Linear Tension Softening
→Constant Shear Retention →No Plasticity
Materials Material Name: STEEL
↑Linear Elasticity →Isotropic
↑Static Nonlinearity →Reinforcement →Von Mises Plasticity →Ideal Plasticity
→Reinforcement Bonded
Materials Material Name: SOIL
↑Mass →Distributed mass→Isotropic
↑Physical Properties Physical Property Name: GRT1
↑Geometry →Embedded Reinforcements →Grid
···
Physical Properties Physical Property Name: GRT9
↑Geometry →Embedded Reinforcements →Grid
Concrete. We define the material properties for concrete in a material named
CONCRETE [Table 11.1]. We specify the linear isotropic values for Ec , ν, and ρ.
For the cracking parameters we specify ft , εcr
u , and β.
Reinforcement. We define the material properties for the reinforcements in
a material named STEEL [Table 11.1]. We specify the linear isotropic value for
Es . For the plasticity parameters we specify σy . For the reinforcements we must
also specify the equivalent thicknesses. Therefore we define nine sets of physical
properties, GRT1 to GRT9. For each set we give the values for the equivalent
thicknesses of the grids in their two directions, tangential Z and in-plane XY .
Water and sand. We define the mass represention water and sand in a ma-
terial named SOIL. We specify the isotropic value.
Property assignment roof.fgc
PROPERTY ATTACH ALL MATERIAL CONCRETE
PROPERTY ATTACH L6 SOIL
PROPERTY ATTACH GR1 STEEL GRT1
PROPERTY ATTACH GR2 STEEL GRT2
PROPERTY ATTACH GR3 STEEL GRT3
PROPERTY ATTACH GR4 STEEL GRT4
PROPERTY ATTACH GR5 STEEL GRT5
PROPERTY ATTACH GR6 STEEL GRT6
PROPERTY ATTACH GR7 STEEL GRT7
PROPERTY ATTACH GR8 STEEL GRT8
PROPERTY ATTACH GR9 STEEL GRT9
PROPERTY ATTACH GR10 STEEL GRT9
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
11.3 Linear Static Analysis 221
First we assign the material CONCRETE to the complete geometry of the model.
Then we assign the material SOIL to the mass elements on line L6. Finally we
assign the material STEEL and the appropriate thickness to each reinforcement.
11.3 Linear Static Analysis
To check the correctness and the behavior of the model it is useful to do a linear
static analysis. Therefore we write an input data file in Diana batch analysis
format and initiate the analysis.
iDiana
UTILITY WRITE DIANA
yes
FILE CLOSE
yes
Roof slab
ANALYSE ROOF
Analysis Setup
specification of options
In the Analysis Setup dialog we choose for Linear Static analysis and output of
displacements and stresses leading to the following batch commands.
linsta.dcf
*FILOS
INITIA
*INPUT
*LINSTA
BEGIN OUTPUT FEMVIE
DISPLA TOTAL TRANSL GLOBAL
STRESS TOTAL CAUCHY LOCAL INTPNT
END OUTPUT
*END
The analysis results are written to a data base for the iDiana Results environ-
ment. As soon as the analysis job is terminated we may enter this environment
to assess the results.
linsta.fvc
FEMVIEW LINSTA
VIEW MESH
EYE FRAME
We display the undeformed model in green, nicely fitted in the iDiana viewport.
We will now assess the analysis results of the three load cases. As a first check
we make plots of the deformed structure for each load case.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
222 Gas Explosion in Tunnel
11.3.1 Dead Weight
We select the results of the dead weight which was defined as load case LC1.
linsta.fvc
RESULTS LOADCASE LC1
RESULTS NODAL DTX....G RESDTX
PRESENT SHAPE
The result attribute DT indicates the displacements in the nodes. We display
the deformed mesh in red [Fig. 11.10a]. Note that iDiana has automatically
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:36 dfm1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:36 dfm2.ps
Model: LINSTA Model: LINSTA
LC1: Load case 1 LC2: Load case 2
Nodal DTX....G RESDTX Nodal DTX....G RESDTX
Max = .108E-2 Max = .669E-2
Min = .48E-5 Min = .14E-4
Factor = 435 Factor = 70.3
Y Y
Z X Z X
(a) dead weight (435×) (b) sand and water pressure (70.3×)
Figure 11.10: Deformations
scaled the displacements such that the deformation becomes evident. In this
case the enlarging factor is 435×. The results monitor indicates the maximum
displacement to be about 1 mm. Note that the mass of the CL6TM elements is
not taken into account in linear static analysis.
11.3.2 Sand and Water Pressure
For the results of the sand and water pressure we select load case LC2.
linsta.fvc
RESULTS LOADCASE LC2
RESULTS NODAL DTX....G RESDTX
PRESENT SHAPE
This displays the scaled deformation [Fig. 11.10b]. The maximum displacement
is about 6.7 mm and the automatic scale factor is 70.3×. This causes the two
deformations to look quite similar.
11.3.3 Initial Explosion
For the results of the initial explosion pressure we select load case LC3.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
11.3 Linear Static Analysis 223
linsta.fvc
RESULTS LOADCASE LC3
RESULTS NODAL DTX....G RESDTX
PRESENT SHAPE
RESULTS GAUSSIAN El.SXX.L SXX
RESULTS CALCULATE P-STRESS ALL
PRESENT VECTORS
Again we display the deformation [Fig. 11.11a]. Here we observe a much larger
maximum displacement of about 50 mm. Because this is the most significant
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:36 dfm3.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:36 pst3.ps
Model: LINSTA Model: LINSTA
LC3: Load case 3 LC3: Load case 3
Nodal DTX....G RESDTX Gauss PRINC STRESS ALL
Max = .497E-1 Calculated from: EL.SXX.L
Min = .3E-3 Max = .573E8
Factor = 9.47 Min = -.342E8
Factor = .822E-8
Y Y
Z X Z X .268E8
-.37E7
(a) deformation (9.5×) (b) principal stress
Figure 11.11: Results of initial explosion
load case, we also assess the stresses, as determined in the integration points.
After having selected the primary stresses in the integration points we apply
the P-STRESS option to let iDiana calculate the principal stresses. We display
the principal stresses in vector style with default color modulation [Fig. 11.11b].
The results monitor indicates the maximum stress to be 57.3 MPa which is far
beyond the tensile strength of the concrete [Fig. 11.4a]. In other words: this
example requires a nonlinear analysis!
Von Mises stress. The vector plot clearly indicates the direction and the
size of the stresses. However, a more clear insight into the distribution of the
stresses is given by a contour plot of the equivalent Von Mises stress.
linsta.fvc
RESULTS CALCULATE VONMISES
PRESENT CONTOUR LEVELS
PRESENT PEAKS
First we let iDiana calculate the Von Mises stresses via the VONMISES option
and then present these stresses in contour style [Fig. 11.12a]. Here the red areas
indicate the highest stress and the blue ones the lowest. To highlight the precise
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
224 Gas Explosion in Tunnel
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:36 vms3.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:36 vmsp3.ps
Model: LINSTA Model: LINSTA
LC3: Load case 3 LC3: Load case 3
Gauss VONMISES EL.SXX.L Gauss VONMISES EL.SXX.L
Calculated from: EL.SXX.L Calculated from: EL.SXX.L
Max = .444E8 Max = .444E8
Min = .212E7 Min = .212E7
Results shown:
Mapped to nodes
MIN
MAX
.406E8
.367E8
.329E8
.29E8
Y .252E8 Y
.214E8
.175E8
Z X .137E8 Z X
.981E7
.596E7
(a) stress contours (b) peak stress locations
Figure 11.12: Von Mises stress due to initial explosion
location of the peak stresses we give the PRESENT PEAKS command. The red
marker with the ‘MAX’ label indicates that the highest stresses due to explosion
appear near the roof–wall connection point [Fig. 11.12b].
11.4 Eigenvalue Analysis
To verify the dynamic behavior of the finite element model we will perform an
eigenvalue analysis and plot the eigenmodes in the iDiana Results environment.
The batch commands for the eigenvalue analysis are as follows.
eigen.dcf
*EIGEN
MODEL OFF
EXECUT NMODES=6
*END
The default values for parameters of an eigenvalue analysis with Module eigen
are appropriate in most cases. Here we only ask for some more eigenpairs than
the default of one: via the NMODES parameter we ask for six eigenpairs. Note that
we neither initialize the analysis database (filos file) nor read any input data.
The complete model is still available from the previous linear static analysis of
the modified model. Note also that it is not necessary to perform the evaluation
and assembling process: we switch it off via the MODEL command. We run the
analysis with the above command file.
diana eigen
As soon as the analysis job is terminated we enter the iDiana Results environ-
ment to assess the analysis results.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
11.4 Eigenvalue Analysis 225
eigen.fvc
FEMVIEW EIGEN
UTILITY TABULATE LOADCASES
VIEW MESH
The available load cases and analysis results are tabulated as follows.
eiglc.tb
;
; Model: EIGEN
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; MODEL STATIC "Model Properties"
; Element : REINGRID*
;
; MO1 0 FREQUENCY = 6.4 "Mode 1"
; Nodal : DTX....G
;
; MO2 0 FREQUENCY = 28.8 "Mode 2"
; Nodal : DTX....G
;
; MO3 0 FREQUENCY = 37.4 "Mode 3"
; Nodal : DTX....G
;
; MO4 0 FREQUENCY = 62.1 "Mode 4"
; Nodal : DTX....G
;
; MO5 0 FREQUENCY = 98.8 "Mode 5"
; Nodal : DTX....G
;
; MO6 0 FREQUENCY = 109 "Mode 6"
; Nodal : DTX....G
; * Indicates loads data
;
Note that Module eigen has automatically created six load cases with names
starting with MO followed by a mode number. We also see the values of the
corresponding eigenfrequencies. We start with a display of the undeformed
mesh, by default in green wire netting style.
11.4.1 Eigenfrequencies
Diana also writes the eigenfrequencies on the standard output file, together
with the generalized masses and the relative error in each frequency.
eigen.out
EIGEN-FREQUENCIES:
0.64012E+01( 1) 0.28799E+02( 2) 0.37407E+02( 3) 0.62134E+02( 4)
0.98849E+02( 5) 0.10880E+03( 6)
RELATIVE ERROR ||R|| / ||Kx||:
0.00000E+00( 1) 0.00000E+00( 2) 0.00000E+00( 3) 0.00000E+00( 4)
0.00000E+00( 5) 0.00000E+00( 6)
MODE FREQUENCY GEN. MASS PARTICIPATION
1 0.64012E+01 0.10000E+01 0.25162E+03
11.4.2 Eigenmodes
To display the eigenmodes we give the following commands.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
226 Gas Explosion in Tunnel
eigen.fvc
RESULTS LOADCASE MO1 0
RESULTS NODAL DTX....G RESDTX
PRESENT SHAPE
RESULTS LOADCASE MO2 0
PRESENT SHAPE
RESULTS LOADCASE MO3 0
PRESENT SHAPE
RESULTS LOADCASE MO4 0
PRESENT SHAPE
RESULTS LOADCASE MO5 0
PRESENT SHAPE
RESULTS LOADCASE MO6 0
PRESENT SHAPE
We select the various modes MO1 to MO6. As results item we select DT for the
displacements. We display the deformed meshes of the six eigenmodes in red
[Fig. 11.13].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:38 eigm1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:38 eigm2.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:38 eigm3.ps
Model: EIGEN Model: EIGEN Model: EIGEN
MO1: Mode 1 MO2: Mode 2 MO3: Mode 3
Step: 0 FREQUENCY: 6.4 Step: 0 FREQUENCY: 28.8 Step: 0 FREQUENCY: 37.4
Nodal DTX....G RESDTX Nodal DTX....G RESDTX Nodal DTX....G RESDTX
Max = 1 Min = .433E-2 Max = 1 Min = .34E-1 Max = 1 Min = .132
Factor = .471 Factor = .47 Factor = .471
Y Y Y
Z X Z X Z X
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:38 eigm4.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:38 eigm5.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:38 eigm6.ps
Model: EIGEN Model: EIGEN Model: EIGEN
MO4: Mode 4 MO5: Mode 5 MO6: Mode 6
Step: 0 FREQUENCY: 62.1 Step: 0 FREQUENCY: 98.8 Step: 0 FREQUENCY: 109
Nodal DTX....G RESDTX Nodal DTX....G RESDTX Nodal DTX....G RESDTX
Max = 1 Min = .172E-1 Max = 1 Min = .147E-1 Max = 1 Min = .103
Factor = .47 Factor = .47 Factor = .47
Y Y Y
Z X Z X Z X
Figure 11.13: Eigenmodes
11.5 Initial Static Nonlinear Analysis
It is necessary that the transient nonlinear analysis starts (at time t = 0) from
a static equilibrium situation. Therefore an initial static nonlinear analysis is
required to apply the dead weight and sand and water pressure. We perform
two ‘automatic’ load steps of size 1.
static.dcf
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
11.5 Initial Static Nonlinear Analysis 227
*NONLIN
MODEL OFF
BEGIN TYPE
BEGIN TRANSI
METHOD NEWMAR
DYNAMI MASS CONSIS
END TRANSI
PHYSIC
END TYPE
BEGIN OUTPUT FEMVIE
SELECT STEPS LAST
STRESS TOTAL LOCAL INTPNT
STRAIN CRACK INTPNT
STRAIN PLASTI LOCAL INTPNT
DISPLA TOTAL
STATUS PLASTI
STATUS CRACK
END OUTPUT
BEGIN EXECUT
BEGIN LOAD
STEPS AUTOMA SIZE=1.0 MINSIZ=1.0E-6
LOADNR=1
END LOAD
BEGIN ITERAT
METHOD NEWTON MODIFI
MAXITE=20
BEGIN CONVER
ENERGY TOLCON=0.0001
FORCE OFF
DISPLA OFF
END CONVER
END ITERAT
END EXECUT
BEGIN EXECUT
BEGIN LOAD
STEPS AUTOMA SIZE=1.0 MINSIZ=1.0E-6
LOADNR=2
END LOAD
BEGIN ITERAT
METHOD NEWTON MODIFI
MAXITE=20
BEGIN CONVER
ENERGY TOLCON=0.0001
FORCE OFF
DISPLA OFF
END CONVER
END ITERAT
END EXECUT
*END
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
228 Gas Explosion in Tunnel
Note the MODEL OFF command which suppresses the model evaluation. We may
skip this because it was performed in the preliminary linear static analysis. We
run the job with this file
diana static tunnel.dat
After a nonlinear analysis it is good practice to check if the iteration processes of
the steps have converged. In the Analysis Progress window and in the standard
output file Diana has written log lines which indicate the convergence:
static.out
STEP 1 TERMINATED, CONVERGENCE AFTER 1 ITERATION
STEP 2 TERMINATED, CONVERGENCE AFTER 12 ITERATIONS
This shows that each of the steps has reached convergence. We may now enter
the iDiana Results environment to assess the analysis results.
static.fvc
FEMVIEW STATIC
UTILITY TABULATE LOADCASES
VIEW MESH
RESULTS LOADCASE LC2 2
The available load cases appear tabulated as follows.1
statlc.tb
;
; Model: STATIC
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; MODEL STATIC "Model Properties"
; Element : REINGRID* CRKBANDW*
;
; LC1 1 LOAD = 1 "Load case 1"
; Nodal : TDTX...G
; Gauss : EL.SXX.L RE.SXX.L RE.EPXXL RE.STPL1 RE.STPL2
;
; LC2 2 LOAD = 1 "Load case 2"
; Nodal : TDTX...G
; Gauss : EL.SXX.L EL.EKNN1 EL.STCR1 RE.SXX.L RE.EPXXL RE.STPL1 RE.STPL2
; * Indicates loads data
;
Note that Module nonlin has automatically created two load cases, one for
each step. The name of the load cases consists of two parts: the name of the
model load case that was used in the step, and the step number. Here we will
assess the analysis results of the last step: LC2 2.
11.5.1 Deformation
We plot the deformation after the last step with the following commands.
1 Dueto small differences in accuracy during the iteration procedure, the actual load case
numbers may differ per computer.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
11.5 Initial Static Nonlinear Analysis 229
static.fvc
RESULTS NODAL TDTX...G RESTDT
PRESENT SHAPE
This gives a display of the deformed mesh [Fig. 11.14]. Here we see a maximum
displacement of 8.5 mm and an automatically determined scale factor of 55×.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:40 statdfm.ps
Model: STATIC
LC2: Load case 2
Step: 2 LOAD: 1
Nodal TDTX...G RESTDT
Max = .854E-2
Min = .641E-4
Factor = 55.1
Z X
Figure 11.14: Deformed mesh after initial static nonlinear analysis (55×)
11.5.2 Crack Formation
We assess the crack formation via the normal crack strain εcr
nn and the crack
status. Both were directly determined in the Diana analysis run.
static.fvc
RESULTS GAUSSIAN EL.EKNN1 EKNN
PRESENT CONTOUR LEVELS
VIEW OPTIONS EDGES OUTLINE
PRESENT OPTIONS DISC MODULATE 5
PRESENT DISC FACTOR 0.4
We select result attribute EKNN which represents the normal crack strain εcr nn
in the integration points. We make a contour plot for those elements that have
crack strain at all [Fig. 11.15a]. Obviously cracks appear at the roof’s outer side
near the roof–wall connection and at the roof’s inner side in the middle between
the walls. This is in accordance with the deformation [Fig. 11.14].
To actually plot the cracks we start with an outline view of the model and
the reinforcements. In such display of the model, a crack pattern will show up
more clearly. We ask for color modulation of the cracks with five colors for
the crack strain. Finally we display each crack as a disc in the crack plane.
Because we look in the direction of the crack plane we see a single line for
each crack, together these lines show the crack pattern [Fig. 11.15b]. Note the
FACTOR option which reduces the cracks to a length that fits nicely in the model
display.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
230 Gas Explosion in Tunnel
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:40 statcre.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:40 statcrp.ps
Model: STATIC Model: STATIC
LC2: Load case 2 LC2: Load case 2
Step: 2 LOAD: 1 Step: 2 LOAD: 1
Gauss EL.EKNN1 EKNN Gauss EL.EKNN1 EKNN
Max = .172E-3 Max = .172E-3
Min = 0 Min = 0
Results shown:
Mapped to nodes
.156E-3
.14E-3
.125E-3
.109E-3
Y .936E-4 Y
.78E-4
.624E-4 .137E-3
.468E-4 .103E-3
Z X Z X .686E-4
.312E-4
.156E-4 .343E-4
(a) contour plot (b) crack pattern
Figure 11.15: Normal crack strain
static.fvc
EYE ZOOM FACTOR 3 -2.7 0.3 0
EYE ROTATE RIGHT 10
EYE ROTATE LEFT 10
RESULTS GAUSSIAN EL.STCR1 STCRCK
PRESENT SYMBOL
We demonstrate some more possibilities of displaying cracks and their status.
First we zoom in on the upper left corner of the model. Then we rotate the
viewing point ten degrees to the right. Now we get a side-glance on the disks
of the cracks which causes them to be displayed as slender ellipses [Fig. 11.16-
a]. After having neutralized the eye rotation we select result attribute STCRCK
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:40 statcrpz.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:40 statcrs.ps
Model: STATIC Model: STATIC
LC2: Load case 2 LC2: Load case 2
Step: 2 LOAD: 1 Step: 2 LOAD: 1
Gauss EL.EKNN1 EKNN Gauss EL.STCR1 STCRCK
Max = .172E-3 Symbol factor = 1
Min = 0 Fully_l Fully Open Loading
Partia_l Partially Open Loadi
No Crack Yet
Partia_u Partially Open Unloa
Fully_u Fully Open Unloading
Closed Closed Crack
Partia_l Partia_l Partia_l Partia_l Partia_l Partia_l Partia_l Partia_l Partia_l Partia_l
Y Y
.137E-3
.103E-3
Z X .686E-4 Z X
.343E-4
(a) crack pattern (b) status labels
Figure 11.16: Crack status at upper-left surface
which represents the crack status. We display the status for each crack with a
symbol, i.e., as a text string near the crack location [Fig. 11.16b]. In this case
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
11.5 Initial Static Nonlinear Analysis 231
we see a string ‘Partia l’ for all cracks, which stands for ‘partially open loading
active’. See ‘crack status’ in Volume Analysis Procedures for a description of
possible crack statuses.
11.5.3 Stresses
For the initial static nonlinear analysis we will now display the stresses in the
reinforcements and in the concrete. Before doing that we give the EYE FRAME
command to revert to a display of the entire model.
Reinforcement static.fvc
EYE FRAME
RESULTS GAUSSIAN RE.SXX.L SXX
PRESENT OPTIONS SYMBOL TRIANGLE RANGE ALL
PRESENT SYMBOL
PRESENT CONTOUR LEVELS
We select the result attribute RE.SXX which represents the σxx stresses in the
reinforcements. Then we make a symbol plot with triangles for the complete
range of values, scaled and color modulated according to the represented value
[Fig. 11.17a]. In the monitor we see that the extreme values for σxx range from
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:40 statrss.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:40 statrsc.ps
Model: STATIC Model: STATIC
LC2: Load case 2 LC2: Load case 2
Step: 2 LOAD: 1 Step: 2 LOAD: 1
Gauss RE.SXX.L SXX Gauss RE.SXX.L SXX
Max = .67E8 Max = .67E8
Min = -.813E8 Min = -.813E8
Symbol factor = 1 Results shown:
All values Mapped to nodes
Fully_l = 2
Partia_l = 1
= 0
Partia_u = -1
Fully_u = -2
Closed = -3
.593E8 .535E8
.445E8 .401E8
.297E8 .266E8
.148E8 .131E8
Y .373E-8 Y -.376E6
-.148E8 -.139E8
-.297E8 -.273E8
-.445E8 -.408E8
Z X -.593E8 Z X
-.543E8
-.741E8 -.678E8
(a) symbol display (b) contour plot
Figure 11.17: Stress in reinforcements
+67 MPa to −81 MPa. Although the symbol display clearly shows the stress
distribution, a contour plot of the stresses looks more natural [Fig. 11.17b]. Here
we simply see the reinforcement colored according to the local stress. Note that
in both displays the color modulation is from red for the extreme positive value
(tension), via yellowish green for zero stress, to blue for the extreme negative
value (compression). Compared to the crack displays [Fig. 11.15], we see tension
stress in the reinforcements at places where cracks arise.
Concrete static.fvc
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
232 Gas Explosion in Tunnel
RESULTS GAUSSIAN EL.SXX.L SXX
RESULTS CALCULATE P-STRESS ALL
PRESENT VECTORS
RESULTS CALCULATE VONMISES
PRESENT CONTOUR LEVELS
We select the result attribute EL.SXX which represents the total Cauchy stresses
in the elements of the model. We let iDiana calculate the principal stresses.
Then we display the principal stresses in vector style with default color modu-
lation [Fig. 11.18a]. The results monitor indicates a stress variation from +3.36
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:40 statcsp.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:40 statcsv.ps
Model: STATIC Model: STATIC
LC2: Load case 2 LC2: Load case 2
Step: 2 LOAD: 1 Step: 2 LOAD: 1
Gauss PRINC STRESS ALL Gauss VONMISES EL.SXX.L
Calculated from: EL.SXX.L Calculated from: EL.SXX.L
Max = .336E7 Max = .754E7
Min = -.982E7 Min = .509E6
Factor = .479E-7 Results shown:
Mapped to nodes
.69E7
.626E7
.562E7
.498E7
Y Y .434E7
.371E7
.307E7
Z X Z X .243E7
-.104E7 .179E7
-.543E7 .115E7
(a) principal stress vectors (b) Von Mises stress contours
Figure 11.18: Stress in concrete
MPa (tension, red) to −9.82 MPa (compression, blue). The Von Mises stress
contours also clearly display the stress distribution [Fig. 11.18b]. These vary
from 7.5 MPa to 0.51 MPa. Note that the blue areas here indicate the lowest
stress values.
11.5.4 Plasticity in Reinforcements
From the displayed reinforcement stress [Fig. 11.17], we know that the yield
stress σy = 528 MPa has nowhere been reached. We will confirm this by dis-
playing the plastic strain.
static.fvc
RESULTS GAUSSIAN RE.EPXXL EPXX
PRESENT CONTOUR LEVELS
The result attribute RE.EPXX represents the plastic strain εpxx in the reinforce-
ment. The contour plot shows all reinforcements entirely in blue [Fig. 11.19].
The results monitor indicates both extreme values to be zero and the legend also
shows zeros only. All this means that at the end of the initial static nonlinear
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
11.6 Transient Nonlinear Dynamic Analysis 233
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:41 statrpl.ps
Model: STATIC
LC2: Load case 2
Step: 2 LOAD: 1
Gauss RE.EPXXL EPXX
Max = 0 Min = 0
Results shown:
Mapped to nodes
0
0
0
0
Y 0
0
0
Z X 0
0
0
Figure 11.19: Plastic strain in reinforcement (none!)
analysis the reinforcements are still fully elastic. Starting from the static equi-
librium state of the model we may now continue with the transient nonlinear
dynamic analysis.
11.6 Transient Nonlinear Dynamic Analysis
Before starting the transient nonlinear dynamic analysis we will discuss some
considerations concerning the various options for such analysis. In particular
we will clarify the choices that we will make for this example.
11.6.1 Consideration of Options
In a transient nonlinear dynamic analysis the main options to consider are the
time integration scheme, the size of the time steps, and the equilibrium iteration
process.
11.6.1.1 Time Integration
By default Diana will apply a Newmark-β time integration scheme with pa-
rameters β = 14 and γ = 21 . This scheme is unconditionally stable, the time
step size ∆t only affects the accuracy. We will apply this default scheme for
this example. For more information on time integration schemes see Volume
Analysis Procedures.
11.6.1.2 Time Step Size
An explosion pressure as shown in Figure 11.3 on page 211 may be considered
as a wave propagation problem. Generally speaking, such a problem interacts
with a large number of natural frequencies. To determine the time step size ∆t,
it is important to handle a sufficiently high stop (cut-off) frequency fco to get
the necessary accuracy of the solution.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
234 Gas Explosion in Tunnel
Under the assumption that ten steps will do to describe one period of the
1
shock wave (at a ratio ∆t = 10 T the error is less than 3%) the time step is
Tco 1 1
∆t = = = = 0.2×10−3 s (11.3)
n n × fco 10 × 500
if we set fco at 500 Hz. Also the nature of the time–load diagram influences the
choice of the time step size: ∆t must be sufficiently small to fit sudden changes
in the loading.
11.6.1.3 Automatic Time Increments
In this example we bypass troubles with setting an appropriate time step size
by choosing for the automatic time increments option. The SDIRK2 method
ensures sufficiently accurate results [Vol. Analysis Procedures].
11.6.1.4 Equilibrium Iteration
Due to nonlinear effects, an iteration to equilibrium is necessary within each time
step. In this example we use the default Regular Newton–Raphson iteration
scheme. As convergence criterion for the iteration process we use the default
value for the internal energy.
11.6.2 Performing Time Steps
The transient analysis of the model involves time steps up to time t = 250 ms
We prepare the following command file for these time steps.
dynami.dcf
*NONLIN
MODEL OFF
TYPE OFF
BEGIN OUTPUT FEMVIEW
DISPLA TOTAL
VELOCI
STRESS TOTAL LOCAL INTPNT
STRAIN CRACK INTPNT
STRAIN PLASTI LOCAL INTPNT
STATUS PLASTI
STATUS CRACK
END OUTPUT
BEGIN EXECUT
BEGIN TIME
BEGIN STEPS
BEGIN AUTOMA
SIZE=0.250
MINSIZ=1.0E-6
SDIRK2
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
11.6 Transient Nonlinear Dynamic Analysis 235
END AUTOMA
END STEPS
END TIME
BEGIN ITERAT
BEGIN CONVER
ENERGY TOLCON=1.0E-6
FORCE OFF
DISPLA OFF
END CONVER
END ITERAT
END EXECUT
*END
We run the analysis job with the shown command file.
diana dynami
Diana writes all the analysis results to a model DYNAMI for the iDiana Results
environment.
dynami.fvc
FEMVIEW DYNAMI
UTILITY TABULATE LOADCASES
VIEW MESH
We enter the Results environment with the name of the model. The tabulation
of the load cases shows the end time for each load case.2
dynlc.tb
;
; Model: DYNAMI
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; MODEL STATIC "Model Properties"
; Element : REINGRID* CRKBANDW*
;
; LC3 3 TIME = .1E-5 "Load case 3"
; Nodal : TDTX...G TVTX...G
; Gauss : EL.SXX.L EL.EKNN1 EL.STCR1 RE.SXX.L RE.EPXXL RE.STPL1 RE.STPL2
;
; LC3 4 TIME = .634E-4 "Load case 3"
; Nodal : TDTX...G TVTX...G
; Gauss : EL.SXX.L EL.EKNN1 EL.STCR1 RE.SXX.L RE.EPXXL RE.STPL1 RE.STPL2
;
... lines omitted
; Gauss : EL.SXX.L EL.EKNN1 EL.EKNN2 EL.STCR1 EL.STCR2 RE.SXX.L RE.EPXXL RE.STPL1 RE.STPL2
;
; LC3 1243 TIME = .25 "Load case 3"
; Nodal : TDTX...G TVTX...G
; Gauss : EL.SXX.L EL.EKNN1 EL.EKNN2 EL.STCR1 EL.STCR2 RE.SXX.L RE.EPXXL RE.STPL1 RE.STPL2
;
; LC3 1244 TIME = .25 "Load case 3"
; Nodal : TDTX...G TVTX...G
; Gauss : EL.SXX.L EL.EKNN1 EL.EKNN2 EL.STCR1 EL.STCR2 RE.SXX.L RE.EPXXL RE.STPL1 RE.STPL2
; * Indicates loads data
;
2 Due
to small differences in accuracy during the iteration procedure, the actual load case
(step) numbers may differ per computer.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
236 Gas Explosion in Tunnel
11.6.3 Results after Start of Explosion
At time t = 25 ms the explosion is at the beginning of the overpressure plateau
[Fig. 11.3]. We assess the results for this time by selecting the appropriate step.
Displacements and velocities dynami.fvc
RESULTS LOADCASE LC3 241
RESULTS NODAL TDTX...G RESTDT
PRESENT SHAPE
RESULTS NODAL TVTX...G RESTVT
PRESENT VECTORS
The result attribute TDT represents the total displacements which we present as
a deformed shape [Fig. 11.20a]. The results monitor shows a maximum displace-
ment of 17 mm. The result attribute TVT represents the velocity field which we
present as a vector plot [Fig. 11.20b]. The maximum velocity is about 2 m/s.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:28:47 dynd1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:28:47 dynv1.ps
Model: DYNAMI Model: DYNAMI
LC3: Load case 3 LC3: Load case 3
Step: 241 TIME: .25E-1 Step: 241 TIME: .25E-1
Nodal TDTX...G RESTDT Nodal TVTX...G RESTVT
Max = .168E-1 Max = 1.95
Min = .296E-2 Min = .174E-3
Factor = 28 Factor = .241
Y Y
Z X Z X 1.3
.65
(a) total deformation ×28 (b) velocity field ×0.24
Figure 11.20: Nonlinear dynamic analysis results at t = 25 ms (1)
Cracks and reinforcement stress dynami.fvc
RESULTS GAUSSIAN EL.EKNN1 EKNN
PRESENT DISC FACTOR 0.4
RESULTS GAUSSIAN RE.SXX.L SXX
PRESENT SYMBOL
The result attribute EKNN represents the normal crack strain. Combined with
the DISC option we get the crack pattern displayed [Fig. 11.21a]. Note that there
is only a small area without cracks. Furthermore we select the reinforcement
stresses via the RE.SXX result attribute and display these as symbols, by default
modulated in size and color [Fig. 11.21b]. The maximum stress is 528 MPa,
which is equal to the yield stress.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
11.6 Transient Nonlinear Dynamic Analysis 237
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:28:47 dync1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:28:47 dyns1.ps
Model: DYNAMI Model: DYNAMI
LC3: Load case 3 LC3: Load case 3
Step: 241 TIME: .25E-1 Step: 241 TIME: .25E-1
Gauss EL.EKNN1 EKNN Gauss RE.SXX.L SXX
Max = .413E-2 Min = 0 Max = .528E9
Min = -.818E8
Symbol factor = 1
All values
.488E9
.427E9
.366E9
.305E9
Y Y .244E9
.183E9
.122E9
.61E8
Z X .275E-2 Z X 0
.138E-2 -.61E8
(a) crack pattern (b) reinforcement stresses
Figure 11.21: Nonlinear dynamic analysis results at t = 25 ms (2)
11.6.4 Results at End of Explosion
At time t = 150 ms the explosion has come to an end [Fig. 11.3]. We assess the
results for this time by selecting the appropriate step and then display the same
results as for t = 25 ms.
dynami.fvc
RESULTS LOADCASE LC3 540
RESULTS NODAL TDTX...G RESTDT
PRESENT SHAPE
RESULTS NODAL TVTX...G RESTVT
PRESENT VECTORS
RESULTS GAUSSIAN EL.EKNN1 EKNN
PRESENT DISC FACTOR 0.4
RESULTS GAUSSIAN RE.SXX.L SXX
PRESENT SYMBOL
These commands display the results in the same style as explained previously
[Fig. 11.22]. The maximum displacement has increased to 36 cm, the maximum
velocity to 4 m/s. The model now shows cracks in virtually every element. The
maximum reinforcement stress is still 528 MPa, but we see this reached at many
more places.
11.6.5 Results at End of Analysis
We select the last step to assess the results at the end of the transient analysis,
i.e., for t = 250 ms.
dynami.fvc
RESULTS LOADCASE LC3 1244
RESULTS NODAL TDTX...G RESTDT
PRESENT SHAPE
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
238 Gas Explosion in Tunnel
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:28:47 dynd2.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:28:47 dynv2.ps
Model: DYNAMI Model: DYNAMI
LC3: Load case 3 LC3: Load case 3
Step: 540 TIME: .15 Step: 540 TIME: .15
Nodal TDTX...G RESTDT Nodal TVTX...G RESTVT
Max = .357 Max = 3.51
Min = .145E-2 Min = .153E-1
Factor = 1.32 Factor = .134
Y Y
Z X Z X 2.35
1.18
(a) total deformation ×1.3 (b) velocity field
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:28:47 dync2.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:28:47 dyns2.ps
Model: DYNAMI Model: DYNAMI
LC3: Load case 3 LC3: Load case 3
Step: 540 TIME: .15 Step: 540 TIME: .15
Gauss EL.EKNN1 EKNN Gauss RE.SXX.L SXX
Max = .907E-1 Max = .528E9
Min = 0 Min = -.521E9
Symbol factor = 1
All values
.525E9
.42E9
.315E9
.21E9
Y Y .105E9
0
-.105E9
-.21E9
Z X .605E-1 Z X -.315E9
.302E-1 -.42E9
(c) crack pattern (d) reinforcement stresses
Figure 11.22: Nonlinear dynamic analysis results at t = 150 ms
RESULTS NODAL TVTX...G RESTVT
PRESENT VECTORS
RESULTS GAUSSIAN EL.EKNN1 EKNN
PRESENT DISC FACTOR 0.4
RESULTS GAUSSIAN RE.SXX.L SXX
PRESENT SYMBOL
Once more we display the results in the familiar style [Fig. 11.23]. The maximum
displacement has increased to about 60 cm. The maximum velocity is 7.6 m/s
and its direction is a bit indeterminate. The model is on the way back: the
crack pattern has hardly changed. The maximum reinforcement stress is still
528 MPa.
11.6.6 History Diagrams
The presentation of results in the previous sections, i.e., for specific times and
in a model display, gives a reasonable impression of their development in time.
However, a more precise insight requires the presentation of the results in the
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
11.6 Transient Nonlinear Dynamic Analysis 239
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:28:47 dynd3.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:28:47 dynv3.ps
Model: DYNAMI Model: DYNAMI
LC3: Load case 3 LC3: Load case 3
Step: 1244 TIME: .25 Step: 1244 TIME: .25
Nodal TDTX...G RESTDT Nodal TVTX...G RESTVT
Max = .596 Max = 1.17
Min = .162E-1 Min = .249E-1
Factor = .789 Factor = .404
Y Y
Z X Z X .786
.405
(a) total deformation ×0.69 (b) velocity field
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:28:47 dync3.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:28:47 dyns3.ps
Model: DYNAMI Model: DYNAMI
LC3: Load case 3 LC3: Load case 3
Step: 1244 TIME: .25 Step: 1244 TIME: .25
Gauss EL.EKNN1 EKNN Gauss RE.SXX.L SXX
Max = .176 Min = 0 Max = .528E9
Min = -.512E9
Symbol factor = 1
All values
.52E9
.416E9
.312E9
.208E9
Y Y .104E9
0
-.104E9
-.208E9
Z X .118 Z X -.312E9
.588E-1 -.416E9
(c) crack pattern (d) reinforcement stresses
Figure 11.23: Nonlinear dynamic analysis results at t = 250 ms
form of a history diagram, i.e., a graph with the time along the horizontal axis.
Therefore we select all load cases, i.e., all the saved time steps.
dynami.fvc
RESULTS LOADCASE LC3
PRESENT OPTIONS GRAPH LINES THICK
PRESENT OPTIONS GRAPH POINTS SYMBOLS OFF
RESULTS NODAL TDTX...G TDTY
PRESENT GRAPH NODE 38
RESULTS NODAL TVTX...G TVTY
PRESENT GRAPH NODE 38
We set some style options for graph plotting: thick lines without marker sym-
bols. Then we select the TDTY nodal result attribute which represents the total
vertical displacement uY . We make a history plot for uY at node 38 [Fig. 11.24-
a]. This node3 is the bottom point at the midspan of the roof slab (point D in
3 To get the node number you may give the LABEL MESH NODES command.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III) November 8, 2010 – First ed.
240 Gas Explosion in Tunnel
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:28:47 dynhd.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:28:47 dynhv.ps
Model: DYNAMI Model: DYNAMI
Nodal TDTX...G TDTY Nodal TVTX...G TVTY
Max/Min on whole graph: Max/Min on whole graph:
Ymax = .536 Ymax = 4.22
Ymin = -.853E-2 Ymin = -1.03
Xmax = .25 Xmax = .25
Xmin = .1E-5 Xmin = .1E-5
Variation over loadcases Variation over loadcases
Node 38 Node 38
.6 5
.5 4
N N
O O
D D
A .4 A 3
L L
T T
D .3 V 2
T T
X X
. .
. .2 . 1
. .
G G
T .1 T 0
D V 0 .25E-1 .5E-1 .75E-1 .1 .125 .15 .175 .2 .225 .25 .275
T T
Y Y
0 -1
0 .25E-1 .5E-1 .75E-1 .1 .125 .15 .175 .2 .225 .25 .275
-.1 -2
TIME TIME
(a) vertical displacement (b) vertical velocity
Figure 11.24: History plot for midspan bottom of slab
Figure 11.5 on page 212). Similarly we make a history plot for result attribute
TVTY which represents the total vertical velocity u̇Y [Fig. 11.24b]. Note that the
two history plots confirm the development of the displacement and velocity as
obtained in the previous sections.
iDiana offers another instructive way of presenting the development of anal-
ysis results in time: an animation sequence. This would be good practice for
ambitious users. See for instance the animation of the crack development in a
reinforced concrete beam [§ 6.2.3 p. 104].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (III)
Part IV
Creep and Shrinkage
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
Chapter 12
Post-tensioned Concrete
Beam
Name: PostTe
Path: /Examples/ConcMas/PostTe
Keywords: analys: nonlin physic. constr: suppor. elemen: bar beam
class2 ishape l7ben reinfo. load: elemen force line reinfo
weight. materi: concre consta crack creep cutoff elasti harden
isotro kelvin nonlin plasti retent shrink smear soften strain tem-
per time viscoe vonmis. option: adapti arclen direct groups
linese loadin newton normal regula size units update. post:
binary femvie. pre: append femgen. result: cauchy crack
displa green moment plasti strain stress total.
A B
Y P1 P2
X
A B
30 m 30 m
500
cBB = 90
300
850 200
250 cAA = 130
800
Figure 12.1: Post-tensioned beam [mm]
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
244 Post-tensioned Concrete Beam
This example deals with a post-tensioned concrete beam on three supports
[Fig. 12.1]. It illustrates the use of post-tensioned tendons, and the perfor-
mance of Limit State analyses with cracking. The beam is loaded by dead
weight, by post-tensioning and by distributed permanent and live loads P1 and
P2 from the girders. We will perform three analyses on the model: Preliminary,
Serviceability Limit State (SLS), and Ultimate Limit State (ULS).
Preliminary analysis.
We will start with a preliminary linear elastic analysis [§ 12.2]. In this
analysis the concrete is loaded by the post-tensioned tendon, by dead
weight at the age of seven days, and by the permanent load at the age of
fourteen days (P1 = P2 = 10 kN/m).
Serviceability Limit State analysis.
After completion of the preliminary linear analysis we will perform the
nonlinear SLS analysis [§ 12.3]. This analysis includes aging, creep, and
shrinkage over five years according to the CEB-FIP model code.
Ultimate Limit State analysis.
Finally we will perform the ULS analysis with the same model and an
increasing live load until collapse [§ 12.4].
12.1 Finite Element Model
To build up the finite element model we start iDiana and enter the Design
environment with the model name.
iDiana
FFEMGEN POSTTE
Analysis and Units
Analysis Selection
Model Type: →Structural 2D
Units Definition
Length: →Meter
Force: →Newton
Time: →Day
Temperature: →Celsius
In the Analysis and Units dialog we specify that the model will be applied for a
two-dimensional structural analysis. We also specify the adopted units for the
analysis [m, N, day, °C]. Note that time unit has been defined as day. Attention
should be given to the mass unit which is given by:
2
[ f orce ] × [ time ]
[ mass ] = (12.1)
[ length ]
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
12.1 Finite Element Model 245
In our particular case we have
N·day2 N·s2
[ mass ] = = (3600 × 24)2 ≈ 7.46×109 kg (12.2)
m m
12.1.1 Beam
We will model the beam with a single line along its length.
Geometry postte.fgc
GEOMETRY POINT COORD P1 0
GEOMETRY POINT COORD P2 30
GEOMETRY POINT COORD P3 60
EYE FRAME
GEOMETRY LINE STRAIGHT L1 P1 P2
GEOMETRY LINE STRAIGHT L2 P2 P3
CONSTRUCT SET BEAM APPEND ALL
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY POINTS
LABEL GEOMETRY LINES ALL VIOLET
We define the coordinates of the end and middle points of the beam. Then,
we construct the corresponding lines. We append all the geometrical entities
constructed so far in the set BEAM. We display the geometry of the beam with
labels [Fig. 12.2a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:05 geom1 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:05 mesh1
Model: POSTTE Model: POSTTE
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
P1 L1 P2 L2 P3
Y Y
Z X Z X
(a) geometry (b) mesh
Figure 12.2: Modeling the beam
Meshing postte.fgc
MESHING DIVISION LINE ALL 15
MESHING TYPES STRAIGHT BE2 L7BEN
MESHING GENERATE
VIEW OPTIONS SHRINK MESH
VIEW MESH
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
246 Post-tensioned Concrete Beam
We specify that the two lines should be divided in fifteen elements each. We
indicate that the lines should be meshed with the 2-node class-II beam ele-
ment L7BEN. We display the mesh in ‘shrunken elements’ style so that we can
distinguish the thirty elements [Fig. 12.2b].
12.1.2 Reinforcement
We specify the reinforcement bar (tendon) with sections between points.
Points postte.fgc
GEOMETRY POINT COORD P4 11.65 -.5
GEOMETRY POINT COORD P5 29.1 .6217
GEOMETRY POINT COORD P6 30 .68
GEOMETRY POINT COORD P7 30.9 .6217
GEOMETRY POINT COORD P8 47.45 -.5
VIEW GEOMETRY ALL BLUE
LABEL GEOMETRY POINTS
We define the end-points of each reinforcement bar according to Figure 12.1.
We display the geometry with point labels [Fig. 12.3a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:05 geometry iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:05 meshrei
Model: POSTTE Model: POSTTE
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
P5P6P7
P1 P4 P2 P8 P3
Y Y
Z X Z X
(a) geometry (a) generated mesh
Figure 12.3: Modeling the reinforcement in the beam
Sections in bar postte.fgc
REINFORCE BAR SECTION RE1 P1 P4 P5
REINFORCE BAR SECTION RE2 P5 P6 P7
REINFORCE BAR SECTION RE3 P7 P8 P3
REINFORCE BAR TENDON RE1 RE2 RE3
VIEW MESH
VIEW REINFORCE +TENDON
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
12.1 Finite Element Model 247
We specify the three reinforcement sections between appropriate points. Finally
we define the reinforcement bar called TENDON as an assembly of the three
sections. We display the mesh along with the reinforcement [Fig. 12.3b].
12.1.3 Material and Physical Properties
We launch the Property Manager to specify the properties of the reinforcement
tendon and the concrete beam.
iDiana
View →Property Manager...
↑
Property Manager
···
12.1.3.1 Material Properties
We will specify the properties of the reinforcement steel and the concrete of the
beam.
Reinforcement steel iDiana
Property Manager
↑ Materials Material Name: MATENDON
↑Linear Elasticity →Reinforcement →Reinforcement not bonded
↑Static Nonlinearity →Reinforcement →Von Mises plasticity →Ideal plasticity
For the reinforcement steel we define a material MATENDON. As elastic property
we specify a Young’s modulus E = 2.1×1011 Pa. We also indicate that the steel
is not bonded to the surrounding concrete. For plasticity we specify the Von
Mises model with a yield stress σy = 1.86×109 Pa.
Concrete beam iDiana
Property Manager
Materials Material Name: MABEAM
↑Linear Elasticity →Isotropic
↑Mass →Mass density
↑Static nonlinearity →Concrete and Brittle Materials →Multi-directional Fixed Crack
→Constant stress cut-off →Hordijk Tension Softening
→Constant Shear Retention →No plasticity
↑External →External Data from File
For the concrete beam we define a material MABEAM. We specify a Young’s
modulus E = 3.975×1010 Pa and a Poisson’s ratio ν = 0.3. For the present
study, the concrete has a mass density ρ = 2500 kg/m3 . Using Equation (12.2),
we can also express that ρ = 3.35×10−7 × 7.46×109 kg/m3 . Therefore we
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
248 Post-tensioned Concrete Beam
specify a concrete density of 3.35×10−7 N·m/day2 . Furthermore we use the
multi–directional fixed crack model with tensile strength ft = 4.75×106 Pa,
fracture energy Gf = 100 N/m, numerical crack bandwidth h = 2 m, constant
shear retention factor β = 0.2 and the Hordijk softening curve for which we
accept the default parameters c1 = 3 and c2 = 6.93.
The material parameters for the nonlinear creep and shrinkage behavior we
specify according to the CEB-FIP Model Code 1990 [Vol. Material Library]:
Young’s modulus at 28 days E28 = 3.975×104 MPa, mean compressive strength
at 28 days fc28 = 63 MPa, notational size hc = 580 mm, and an age at the
element birth tel = 7 days. These parameters we add via an external file.
mabeam.dat
12.1.3.2 Physical Properties
We will specify the dimensions of the beam and the tendon.
Concrete beam iDiana
Property Manager
↑ Physical Properties Physical Property Name: PHBEAM
↑Geometry →Beam →Class II (Bernoulli numeric) →Predefined shapes → I-shape
For the concrete beam we define a physical property PHBEAM with an I-shaped
cross-section: height h = 1.4 m, width of the upper flange b1 = 0.5 m, width of
the lower flange b2 = 0.8 m, thickness of the upper flange t1 = 0.3 m, thickness
of the lower flange t2 = 0.25 m, the thickness of the web t3 = 0.2 m.
Reinforcement tendon iDiana
Property Manager
Physical Properties Physical Property Name: PHTENDON
↑Embedded reinforcements →Bar
For the reinforcement tendon we define a physical property PHTENDON with a
cross-section area A = 2.886×10−3 m2 .
12.1.3.3 Assignment
We have now defined all properties for the model and we must assign them to
the appropriate geometrical parts.
postte.fgc
PROPERTY ATTACH BEAM MABEAM PHBEAM
PROPERTY ATTACH TENDON MATENDON PHTENDON
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
12.1 Finite Element Model 249
12.1.4 Checking the Mesh and the Reinforcement
postte.fgc
VIEW MESH
VIEW OPTIONS SHRINK OFF
EYE ROTATE TO -49 -30 -30
EYE FRAME
VIEW HIDDEN SHADE
VIEW OPTIONS HIDDEN PHYSICAL
VIEW OPTIONS HIDDEN TRANSPARENT
VIEW REINFORCE +TENDON BLUE
VIEW HIDDEN OFF
We display the mesh in the default wire netting style by unselecting the ‘shrunken
element’ style view mode and we choose an appropriate eye point. Then we dis-
play a shaded view of the mesh. Additionally, we apply the PHYSICAL and
TRANSPARENT options, to get a more realistic representation of the beam cross-
section profile and tendon location [Fig. 12.4a]. Because iDiana only applies
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:05 hid3d iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:05 tendon
Model: POSTTE Model: POSTTE
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
Y Y
X X
Z Z
(a) beam with profile (b) tendon
Figure 12.4: Mesh of beam and tendon location
transparency on-screen we cannot see the tendon in the figure in this document,
obtained via an iDiana plotfile. The tendon is visible via the plotfile if we
switch off the shaded view [Fig. 12.4b].
12.1.5 Boundary Conditions and Loading
We will define the supports and the loading.
Supports postte.fgc
PROPERTY BOUNDARY CONSTRAINT CO1 P1 X Y
PROPERTY BOUNDARY CONSTRAINT CO2 P2 Y
PROPERTY BOUNDARY CONSTRAINT CO3 P3 Y
LABEL MESH CONSTRNT
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
250 Post-tensioned Concrete Beam
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:05 supp iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:05 loads
Model: POSTTE Model: POSTTE
Model: POSTTE Analysis: DIANA Analysis: DIANA
Analysis: DIANA Model Type: Structural 2D Model Type: Structural 2D
Model Type: Structural 2D .44E7
.44E7
.44E7
.44E7
.44E7
.44E7
Y Y
.44E7
X X
Z Z
1 2
Model: POSTTE Model: POSTTE
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
Y
X
Y Y
X X
Z
Z Z
3 4
(a) supports (b) loading
Figure 12.5: Supports and loading
Loading postte.fgc
PROPERTY LOADS GRAVITY LO1 1 BEAM -73231258.E3 Y
PROPERTY LOADS POSTTENS LO2 1 TENDON 4.4E6 4.4E6 0.01 0.01 0.22 0.01
PROPERTY LOADS PRESSURE LO3 2 BEAM -10.E3 Y
PROPERTY LOADS PRESSURE LO4 3 L1 -15.E3 Y
PROPERTY LOADS PRESSURE LO5 4 L2 -15.E3 Y
DRAWING VIEWPORT SETUP FOUR
LABEL MESH OFF
LABEL MESH LOADS LO2 WHITE
DRAWING VIEWPORT USE TRIGHT
LABEL MESH OFF
LABEL MESH LOADS LO3 VIOLET
DRAWING VIEWPORT USE BLEFT
LABEL MESH OFF
LABEL MESH LOADS LO4 ORANGE
DRAWING VIEWPORT USE BRIGHT
LABEL MESH OFF
LABEL MESH LOADS LO5 RED
Load case 1 contains the dead weight LO1 and the post-tensioning load LO2.
Note the particular value of the gravity acceleration g = 9.81 m/s2 = 7.32×1010
m/day2 . Load cases 2, 3, and 4 contain the live loads LO3, LO4, and LO5. With
the VIEWPORT option we initiate a multiple-viewport display and label the mesh
with all loads, except the gravity load, in various colors [Fig. 12.5b].
12.1.6 Specifying the Reinforcement Shape
As far as iDiana, the model is now complete. However, we can improve its data
by specifying the shape of the reinforcement. Therefore we must first write the
model to a file in Diana batch input format.
Write input file iDiana
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
12.2 Preliminary Linear Analysis 251
UTILITY WRITE DIANA
yes
Post-tensioned concrete beam
FILE CLOSE
We can open the generated data file postte.dat and inspect it. We may edit
this file to specify that the three sections of the reinforcement have a parabolic
shape. The appropriate part of the input data file should look as follows:
Include reinforcement shape postte.dat
... lines omitted
’REINFORCEMENTS’
LOCATI
4 BAR
LINE 0.000000E+00 0.000000E+00 0.000000E+00
0.116500E+02 -0.500000E+00 0.000000E+00
0.291000E+02 0.621700E+00 0.000000E+00
PARABO 0. 1. 0.
LINE 0.291000E+02 0.621700E+00 0.000000E+00
0.300000E+02 0.680000E+00 0.000000E+00
0.309000E+02 0.621700E+00 0.000000E+00
PARABO 0. 1. 0.
LINE 0.309000E+02 0.621700E+00 0.000000E+00
0.474500E+02 -0.500000E+00 0.000000E+00
0.600000E+02 0.119209E-06 0.000000E+00
PARABO 0. 1. 0.
MATERIALS
/ 4 / 1
GEOMETRY
/ 4 / 2
... lines omitted
In table ’REINFORCEMENTS’ we have added the PARABO input item to the three
sections. The input data indicates that the axis of the parabola is in the Y -
direction, i.e., vertical.
12.2 Preliminary Linear Analysis
Now we prepare the following command file for the preliminary linear static
analysis.
linsta.dcf
*FILOS
INITIA
*INPUT
*LINSTA
*END
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
252 Post-tensioned Concrete Beam
We perform the analysis with the appropriate input data and command files:
diana postte.dat linsta
Once the analysis is completed, we start iDiana and enter the Results environ-
ment. In preparation to the assessment of the analysis results we will tabulate
the available analysis results and display the mesh with element numbers for
the beam and tendon.
Tabulate available results linsta.fvc
FEMVIEW LINSTA
UTILITY TABULATE LOADCASES
The tabulation of the available load cases with their analysis result attributes
is shown below.
loads.tb
;
; Model: LINSTA
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; MODEL STATIC "Model Properties"
; Element : REINBAR* CROSSE*
;
; LC1 STATIC "Load case 1"
; Nodal : DTX....G FEX....G* FBX....G
; Element : EL.EXX.G EL.SXX.G EL.NX..L EL.MX..L RE.EXX.G RE.SXX.G RE.NX..L
;
; LC2 STATIC "Load case 2"
; Nodal : DTX....G FEX....G* FBX....G
; Element : EL.EXX.G EL.SXX.G EL.NX..L EL.MX..L RE.EXX.G RE.SXX.G RE.NX..L
;
; LC3 STATIC "Load case 3"
; Nodal : DTX....G FEX....G* FBX....G
; Element : EL.EXX.G EL.SXX.G EL.NX..L EL.MX..L RE.EXX.G RE.SXX.G RE.NX..L
;
; LC4 STATIC "Load case 4"
; Nodal : DTX....G FEX....G* FBX....G
; Element : EL.EXX.G EL.SXX.G EL.NX..L EL.MX..L RE.EXX.G RE.SXX.G RE.NX..L
; * Indicates loads data
;
The nodal attributes DT, FE, and FB represent the displacement, the external
force and the reaction force. The element attributes EL.E, EL.S, EL.N, and EL.M,
represent the total strain, the total stress, the element force and the element
moment. The reinforcement attributes RE.E and RE.S represent the total strain
and the total stress within the reinforcement.
Display element numbers linsta.fvc
VIEW MESH BEAM
LABEL MESH ELEMENTS VIEWMODE RED
VIEW MESH ALL
VIEW MESH -BEAM
LABEL MESH ELEMENTS VIEWMODE RED
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
12.2 Preliminary Linear Analysis 253
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:09 beamel.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:09 tendel.ps
Model: LINSTA Model: LINSTA
45464748 49 50
1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 23 24 25 26 27 28 29 30 31 32 33 34 35 36 37 38 39 40 41 42 43 44 51 52 53 54 55 56 57 58 59 60 61 62
Y Y
Z X Z X
(a) beam (b) tendon
Figure 12.6: Mesh with element numbers
In the mesh displays [Fig. 12.6] we can easily determine the numbers of the
elements at the beginning and end point of the model. We will need these
numbers to display the analysis results: the stress in the reinforcement tendon
[§ 12.2.1], the bending moments in the beam [§ 12.2.2], and the shear and normal
forces in the beam [§ 12.2.3].
12.2.1 Reinforcement Stress
We will assess the stress in the reinforcement for load case 1, dead weight plus
post-tensioning.
Distribution linsta.fvc
RESULTS LOADCASE LC1
RESULTS ELEMENT RE.SXX.G SXX
PRESENT GRAPH LINE ELEMENTS LIST 31 TO 62
We select the load case 1 and choose the result attribute for the reinforcement
stress. We display the distribution of the reinforcement stress as a graph along
the line of elements that represent the tendon [Fig. 12.7a].
Check for plastic yield linsta.fvc
LABEL MESH OFF
PRESENT CONTOUR VALUE 1.86E9
The graph shows that the stress nowhere exceeds the yield stress σy = 1.89×109 .
We can confirm this easily via a contour plot with one contour for the value of
the yield stress [Fig. 12.7b]. The tendon is all blue, indicating that it is elastic
all over.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
254 Post-tensioned Concrete Beam
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:09 tensxx.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:09 tensxxc.ps
Model: LINSTA Model: LINSTA
LC1: Load case 1 LC1: Load case 1
Element RE.SXX.G SXX Element RE.SXX.G SXX
Max/Min on whole graph: Max/Min on model set:
Ymax = .141E10 Max = .141E10
Ymin = .131E10 Min = .13E10
Xmax = 58.1
*1E9 Xmin = 0
Variation along a line
1.42 Mean value used for each element
E 1.4
L
E
M
E
N 1.38
T
R
E 1.36
.
S
X
X
. 1.34
G
S
X
X 1.32
1.3
0 10 20 30 40 50 60
DISTANCE Y
Z X
.186E10
(a) distribution (b) check for plastic yield
Figure 12.7: Stress in tendon for dead weight plus post-tensioning
12.2.2 Bending Moments in the Beam
We will assess the bending moment in the beam for two load cases: the dead
weight plus post-tensioning and the live load on the left half of the model.
Dead weight plus post-tensioning linsta.fvc
RESULTS ELEMENT EL.MX..L MZ
PRESENT GRAPH LINE ELEMENTS LIST 1 TO 30
We select the bending moment MZ in the beam as analysis result. We display
the distribution as a graph along the line of elements that represent the concrete
beam [Fig. 12.8a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:09 beamz1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:09 beamz3.ps
Model: LINSTA Model: LINSTA
LC1: Load case 1 LC3: Load case 3
Element EL.MX..L MZ Element EL.MX..L MZ
Max/Min on whole graph: Max/Min on whole graph:
Ymax = .108E7 Ymax = .816E6
Ymin = -.152E7 Ymin = -.128E7
Xmax = 58 Xmax = 58
*1E6 Xmin = 0 *1E6 Xmin = 0
Variation along a line Variation along a line
1.25 Mean value used for each element 1 Mean value used for each element
1 .75
.75
E E .5
L L
E .5 E
M M .25
E .25 E
N N
T T 0
0
0 10 20 30 40 50 60 0 10 20 30 40 50 60
E E
L -.25 L -.25
. .
M -.5 M
X X -.5
. .
. -.75 .
L L -.75
-1
M M -1
Z -1.25 Z
-1.5 -1.25
-1.75 -1.5
DISTANCE DISTANCE
(a) dead weight plus post-tensioning (b) live load on left half
Figure 12.8: Bending moment in beam
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
12.2 Preliminary Linear Analysis 255
Live load on left half linsta.fvc
RESULTS LOADCASE LC3
DRAWING DISPLAY
We select load case 3 which represents the live load P1 on the left part of the
model. We only have to redisplay the model to get the distribution graph
[Fig. 12.8b].
12.2.3 Forces in the Beam
We will asses the shear force and the normal force in the beam for the dead
weight plus post-tensioning load.
Shear force linsta.fvc
RESULTS LOADCASE LC1
RESULTS ELEMENT EL.NX..L QY
PRESENT GRAPH LINE ELEMENTS LIST 1 TO 30
We select the the load case for the dead weight plus post-tensioning. We also
select the shear force QY of the beam elements. We display the distribution as
a graph along a line of elements that represent the beam [Fig. 12.9.]
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:09 beaqy1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:09 beanx1.ps
Model: LINSTA Model: LINSTA
LC1: Load case 1 LC1: Load case 1
Element EL.NX..L QY Element EL.NX..L NX
Max/Min on whole graph: Max/Min on whole graph:
Ymax = .258E6 Ymax = -.379E7
Ymin = -.252E6 Ymin = -.408E7
Xmax = 58 Xmax = 58
*1E5 Xmin = 0 *1E6 Xmin = 0
Variation along a line Variation along a line
3 Mean value used for each element -3.78 Mean value used for each element
-3.8
2 -3.83
E E
L L -3.85
E E
M M -3.88
E 1 E
N N
T T -3.9
E E -3.93
L 0 L
. 0 10 20 30 40 50 60 . -3.95
N N
X X -3.98
. .
. -1 . -4
L L
Q N -4.03
Y -2 X
-4.05
-4.08
-3 -4.1
DISTANCE 0 10 20 30 40 50 60
DISTANCE
(a) shear force (b) normal force
Figure 12.9: Force in beam for dead weight plus post-tensioning
Normal force linsta.fvc
RESULTS ELEMENT EL.NX..L NX
DRAWING DISPLAY
We select the normal force NX of the beam elements. We only have to redisplay
the model to get the distribution graph [Fig. 12.9b].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
256 Post-tensioned Concrete Beam
12.3 Serviceability Limit State Analysis
We will perform a nonlinear analysis for the Serviceability Limit State (SLS).
This analysis applies the creep and shrinkage modeling features of Diana. How-
ever, prior to the analysis we will adapt the model with respect of the integration
schemes of the elements.
12.3.1 Adapting the Element Integration Scheme
The default integration scheme of the beam cross-section is not appropriate
for this nonlinear analysis. Indeed, under integration along the beam is not
recommended for physical nonlinear analysis. Moreover, a three-point scheme
within the cross-section is also too low. With the the following additional data
file we can overrule the default integration scheme.
data.dat
’ELEMEN’
DATA
/ BEAM / 1
’DATA’
1 NINTEG 3 11
NUMINT GAUSS SIMPSO
’END’
With the NINTEG input data item we adopt three integration points along the
beam and eleven integration points in each rectangle of the I-shaped cross-
section. This gives a reasonable dense distribution of points along the height
of the I-profile [Fig. 12.10].1 Note that integration points 11 and 12 are on the
outer fibers of the cross-section and that there are two pairs of overlapping
integration points: (1, 33) and (22, 23).
12.3.2 Running the Analysis
For the Serviceability Limit State analysis we apply the command file as shown
below.
SLS analysis commands creep.dcf
*INPUT
READ APPEND FILE="data.dat" TABLE ELEMEN DATA
*NONLIN
: Output item definition
BEGIN OUTPUT
DISPLA TOTAL TRANSL
STRESS TOTAL FORCE
STRESS TOTAL MOMENT
1 See Volume Element Library for integration schemes of beam elements.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
12.3 Serviceability Limit State Analysis 257
11
1
33
28
23
22
17
12
Figure 12.10: Integration points in I-shape cross-section
STRESS TOTAL CAUCHY
STRAIN TOTAL GREEN
STRAIN SHRINK GREEN
END OUTPUT
: Only transient nonlinearity
: Crack model deactivated
BEGIN TYPE
BEGIN PHYSIC
CRACKI OFF
END PHYSIC
END TYPE
: Post-tensioning and dead weight
BEGIN EXECUTE
BEGIN LOAD
LOADNR=1
BEGIN STEPS
EXPLICIT SIZES 1.
END STEPS
END LOAD
END EXECUTE
: 7 days of creep and shrinkage
BEGIN EXECUTE
PHYSIC BOND
BEGIN TIME
BEGIN STEPS
EXPLICIT SIZES 0.3E-1 0.7E-1 0.2 0.7 2.(3)
END STEPS
END TIME
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
258 Post-tensioned Concrete Beam
ITERAT MAXITE=20
END EXECUTE
: Permanent load
BEGIN EXECUTE
PHYSIC BOND
BEGIN LOAD
LOADNR=2
STEPS EXPLICIT SIZES 1.
END LOAD
ITERAT MAXITE=20
END EXECUTE
: 5 years of creep and shrinkage
BEGIN EXECUTE
PHYSIC BOND
BEGIN TIME
BEGIN STEPS
EXPLICIT SIZES 0.3E-1 0.7E-1 0.2 0.7 2. 7. 20. 70. 265. 365.(4)
END STEPS
END TIME
ITERAT MAXITE=20
END EXECUTE
*END
In the TYPE command block we switch off the use of cracking. The PHYSIC BOND
command, it the last three EXECUT blocks indicates that the tendon fully sticks
to the concrete beam after applying dead weight and post-tensioning loading.
We run the analysis with the appropriate data and command files.
diana postte.dat creep
Once the analysis has terminated we enter the iDiana Results environment
with the model name.
iDiana
FEMVIEW CREEP
12.3.3 Prestress Relaxation in the Tendon
We will assess the relaxation of the prestress in the tendon. First we will show
the stress distribution at specific points in time. Then we make a time-graph
for a specific point of the tendon.
Distribution creep.fvc
RESULTS LOADCASE LC1 1 LC1 8 LC2 9 LC1 22
RESULTS ELEMENT RE.SXX.G SXX
PRESENT GRAPH LINE ELEMENTS LIST 31 TO 62
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
12.3 Serviceability Limit State Analysis 259
We select some load cases that represent the situation of the model at four
specific points in time:
LC1 1 Application of post-tensioning and dead weight,
LC1 8 seven days of creep and shrinkage,
LC2 9 application of permanent load,
LC1 22 five years of creep and shrinkage.
Then we select the stress σXX in the tendon. We display the stress distribution
as multiple graphs along a line of elements that represent the reinforcement
tendon [Fig. 12.11a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:23 relten.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:23 reltim.ps
Model: CREEP Model: CREEP
Element RE.SXX.G SXX Element RE.SXX.G SXX
Max/Min on whole graph: Max/Min on whole graph:
Ymax = .141E10 Ymax = .134E10
Ymin = .124E10 Ymin = .128E10
Xmax = 58.1 Xmax = .183E4
Xmin = 0 Xmin = .3E-1
*1E9 Variation along a line *1E9 Variation over loadcases
Mean value used for each element Element 46 Mean
1.42 LC1 1 1.35
LC1 8
LC2 9
1.4 LC1 22 1.34
E E
L 1.38 L
E E 1.33
M M
E E
N 1.36 N
T T 1.32
R 1.34 R
E E 1.31
. .
S 1.32 S
X X
X X 1.3
. 1.3 .
G G
S 1.28 S 1.29
X X
X X
1.26 1.28
1.24 1.27
0 10 20 30 40 50 60 0 .2 .4 .6 .8 1 1.2 1.4 1.6 1.8 2
DISTANCE TIME *1E3
(a) distribution at four points in time (b) evolution in time for mid-point
Figure 12.11: Prestress relaxation in the tendon
Evolution in time creep.fvc
RESULTS LOADCASE LC1 2 TO LC1 22
PRESENT GRAPH ELEMENT 46
We select all load cases that represent time steps. We make a time-graph for
the element at the mid-point of the tendon [Fig. 12.11b].
12.3.4 Stress Relaxation in the Beam
Another interesting phenomenon to present with respect to long-term behavior
of prestressed concrete structure is relaxation of concrete.
Evolution in time creep.fvc
RESULTS LOADCASE LC1 10 TO LC1 22
RESULTS ELEMENT EL.SXX.G SXX
RESULTS RANGE SURFACE 11 12
PRESENT GRAPH ELEMENT 15
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
260 Post-tensioned Concrete Beam
We first select the last thirteen load cases corresponding to a five-year period
of time after the application of the permanent load and during which creep
and shrinkage effects are analyzed. Then we choose the normal stress σXX in
the beam. As locations for the results to be shown we select the upper and
lower fiber of the concrete beam via the SURFACE option. Note that the surface
numbers correspond to the integration point numbers in the vertical direction
[Fig. 12.10 p. 257]: surfaces 11 and 12 represent the outer fibers of the beam.
Finally we present the time evolution of the stress for the middle element of the
beam [Fig. 12.12].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:53:23 relcon.ps
Model: CREEP
Element EL.SXX.G SXX
2 surfaces
Max/Min on whole graph:
Ymax = -.449E7
Ymin = -.112E8
Xmax = .183E4
*1E7 Xmin = 7.03
Variation over loadcases
-.4 Element 15 Mean
-.5
E
L
E -.6
M
E
N
T -.7
E
L -.8
.
S
X
X -.9
.
G
S -1
X
X
-1.1
-1.2
0 .2 .4 .6 .8 1 1.2 1.4 1.6 1.8 2
TIME *1E3
Figure 12.12: Time evolution of the normal stress in the beam
12.4 Ultimate Limit State Analysis
We will now perform the Ultimate Limit State analysis including cracking mod-
eling. During this analysis the following sequence is analyzed after the prelimi-
nary analysis:
Application of a live load on one field: P1 = 25 kN/m, P2 = 10 kN/m,
Application of a live load on two fields: P1 = 25 kN/m, P2 = 25 kN/m,
Increase the live load until failure.
In the ULS analysis we will apply the two live loads P1 and P2 with two separate
load increments. We will then increase the live loads until failure of the beam.
As output results we will ask for the total displacements, the total stresses , the
plastic strains, and the crack strains. To perform the ULS analysis we apply
the following command file.
ULS analysis commands uls.dcf
*FILOS
INITIA
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
12.4 Ultimate Limit State Analysis 261
*INPUT
READ FILE="postte.dat"
READ APPEND FILE="data.dat" TABLE ELEMEN DATA
*NONLIN
: Output item definition
BEGIN OUTPUT
DISPLA TOTAL TRANSL
STRESS TOTAL MOMENT Z
STRESS TOTAL CAUCHY XX INTPNT
STRESS TOTAL CAUCHY XX
STRAIN PLASTI GREEN XX
STRAIN CRACK
END OUTPUT
: Post-tensioning and dead weight
BEGIN EXECUTE
BEGIN LOAD
LOADNR=1
BEGIN STEPS
EXPLICIT SIZES 1.
END STEPS
END LOAD
END EXECUTE
: 7 days of creep and shrinkage
BEGIN EXECUTE
PHYSIC BOND
BEGIN TIME
BEGIN STEPS
EXPLICIT SIZES 0.3E-1 0.7E-1 0.2 0.7 2.(3)
END STEPS
END TIME
ITERAT MAXITE=20
END EXECUTE
: Permanent load
BEGIN EXECUTE
PHYSIC BOND
BEGIN LOAD
LOADNR=2
STEPS EXPLICIT SIZES 1.
END LOAD
ITERAT MAXITE=20
END EXECUTE
: Live load field 1
BEGIN EXECUTE
PHYSIC BOND
BEGIN LOAD
LOADNR=3
STEPS EXPLICIT SIZES 1.
END LOAD
ITERAT MAXITE=20
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
262 Post-tensioned Concrete Beam
END EXECUTE
: Live load field 2
BEGIN EXECUTE
PHYSIC BOND
BEGIN LOAD
LOADNR=4
STEPS EXPLICIT SIZES 1.
END LOAD
ITERAT MAXITE=20
END EXECUTE
: Increase permanent load until
: reinforcement yielding at support
BEGIN EXECUTE
PHYSIC BOND
BEGIN LOAD
LOADNR=2
BEGIN STEPS
BEGIN ITERAT
ARCLEN
INISIZ=0.25
NSTEPS=100
END ITERAT
END STEPS
END LOAD
BEGIN ITERAT
MAXITE=20
LINESE
BEGIN CONVER
DISPLA OFF
FORCE OFF
ENERGY CONTINU
END CONVER
END ITERAT
END EXECUTE
*END
With these commands we apply automatic adaptive load increments based on
the number of iterations in combination with Arc-length control. The initial
size of the load step is set to 0.25. With such parameter values, the number
of steps could be set to 100. The Line Search algorithm is applied within the
equilibrium iteration and the convergence criterion will be only energy-based.
We run the analysis with the appropriate data and command files.
diana postte.dat uls
Once the analysis has terminated we enter the iDiana Results environment
with the model name.
iDiana
FEMVIEW ULS
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
12.4 Ultimate Limit State Analysis 263
12.4.1 Plastic Yield in the Tendon
We will assess the plastic yield of the tendon at time of failure and its develop-
ment in time.
Plastic strain at failure uls.fvc
VIEW MESH ALL
VIEW MESH -BEAM
RESULTS LOADCASE LC2 37
RESULTS ELEMENT RE.EPXXG EPXX
PRESENT SYMBOL
PRESENT CONTOUR VALUE 0
We display the model of the tendon only. Then we select the last converged
step representing the situation at failure. We choose the plastic strain εpxx in
the reinforcement as analysis result. We then present symbols with sizes and
colors modulated according to the value of εpxx [Fig. 12.13a]. A clear display
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:29 plastr.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:29 plastrc.ps
Model: ULS Model: ULS
LC2: Load case 2 LC2: Load case 2
Step: 37 LOAD: 6.2 Step: 37 LOAD: 6.2
Element RE.EPXXG EPXX Element RE.EPXXG EPXX
Max/Min on model set: Max/Min on model set:
Max = .116 Max = .116
Min = -.779E-2 Min = -.779E-2
Symbol factor = 1
All values
.111
.99E-1
.866E-1
.743E-1
Y .619E-1 Y
.495E-1
.371E-1
.248E-1
Z X .124E-1 Z X
0 0
(a) plastic strain (b) plastic areas
Figure 12.13: Plastic yield in the tendon at failure
of the plastic areas in the tendon is obtained with a single contour for a zero
value [Fig. 12.13b]. Blue indicates εpxx ≤ 0 for no plastic yield, red is εpxx > 0
for plastic yield.
Plastic yield in time uls.fvc
RESULTS LOADCASE LC2
UTILITY SETUP ANIMATE LINEAR
DRAWING ANIMATE LOADCASES PLOTFILE plan
PRESENT GRAPH ELEMENT 37 46
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
264 Post-tensioned Concrete Beam
We select all LC2 load cases which represent the load steps. While maintaining
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:29 plan006
Model:
iDIANA ULS
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:29 plan007
LC2: Load case 2
Step: 16 LOAD: 4.04
Model:
iDIANA ULS
the contour value of zero we can now easily make an animation sequence of the
Element 9.4.3-02
RE.EPXXG :EPXX
TNO Diana BV 28 OCT 2010 01:54:29 plan008
LC2: Load
Max/Min oncase
model2 set:
Step:
Max = 17
0ULS LOAD:
Min = 04.24
Model:
Element 9.4.3-02
iDIANA RE.EPXXG :EPXX
TNO Diana BV 28 OCT 2010 01:54:29 plan009
LC2: Load
Max/Min oncase
model2 set:
Step:
Max = 18 LOAD: 4.38
.294E-3
Model: ULS
development of the plastic area. Here we show the frames for a load factor 4
iDIANA
Element 9.4.3-02
RE.EPXXG :EPXX
TNO Diana BV 28 OCT 2010 01:54:30 plan010
Min
LC2:=Load
-.108E-3
case 2
Max/Min on model set:
Step:
Max = 19 LOAD: 4.5
.101E-2
Model:
iDIANA
Element ULS
9.4.3-02 : TNO
RE.EPXXG EPXX Diana BV 28 OCT 2010 01:54:30 plan012
Min
LC2:=Load
-.121E-3
Max/Min oncase
model2 set:
Step:
Max = 20 LOAD: 4.58
.174E-2
Model: ULS
and beyond, i.e., from the start of the plastic yield [Fig. 12.14a].
iDIANA
Element 9.4.3-02 :EPXXTNO Diana BV 28 OCT 2010 01:54:30 plan012
Min
LC2: 0 RE.EPXXG
=Load case 2
Max/Min on model set:
Step:
Max = 22 LOAD: 4.74
.254E-2
Model:
iDIANA
Element ULS
9.4.3-02 : TNO
RE.EPXXG EPXX Diana BV 28 OCT 2010 01:54:30 plan013
Min
LC2:=Load
-.871E-4
Max/Min oncase
model2 set:
Step:
Max = 22 LOAD: 4.74
.382E-2
Model:
iDIANA
Element ULS
9.4.3-02
RE.EPXXG :EPXX
TNO Diana BV 28 OCT 2010 01:54:30 plan014
Min
LC2:=Load
-.257E-3
case 2
Max/Min on model set:
Step:
Max = 23 LOAD: 4.89
.382E-2
Model:
iDIANA
Element ULS
9.4.3-02 : TNO
RE.EPXXG EPXX Diana BV 28 OCT 2010 01:54:30 plan015
Min
LC2:=Load
-.257E-3
Max/Min oncase
model2 set:
Step:
Max = 24 LOAD: 5.05
.515E-2
Model:
iDIANA
Element ULS
9.4.3-02
RE.EPXXG :EPXX
TNO Diana BV 28 OCT 2010 01:54:30 plan016
Min
LC2:=Load
-.435E-3
case 2 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:30 plstev.ps
Max/Min on model set:
Step:
Max = 25 LOAD: 5.24
.687E-2
Model:
iDIANA
Element ULS
9.4.3-02 : TNO
RE.EPXXG EPXX Diana BV 28 OCT 2010 01:54:30 plan017
Min
LC2:=Load
-.663E-3 Model: ULS
Max/Min oncase
model2 set:
Element RE.EPXXG EPXX
Step:
Max = 26 LOAD: 5.52
.89E-2
Model:
iDIANA
Element ULS
9.4.3-02
RE.EPXXG :EPXX
TNO Diana BV 28 OCT 2010 01:54:30 plan018 Max/Min on whole graph:
Min
LC2:=Load
-.863E-3
case 2 Ymax = .834E-1
Max/Min on model set:
Step:
Max = 27 LOAD: 5.71
.125E-1 Ymin = 0
Model:
iDIANA
Element ULS
9.4.3-02 : TNO
RE.EPXXG EPXX Diana BV 28 OCT 2010 01:54:30 plan019
Min
LC2:=Load
-.111E-2 Xmax = 6.2
Max/Min oncase
model2 set:
Xmin = 1
Step:
Max = 28 LOAD: 5.77
.171E-1
Model:
iDIANA
Element ULS
9.4.3-02
RE.EPXXG :EPXX
TNO Diana BV 28 OCT 2010 01:54:30 plan020 *1E-2 Variation over loadcases
Min
LC2:=Load
-.141E-2
case 2 Element 37 Mean
Max/Min on model set: 9
Step:
Max = 29 LOAD: 5.85
.204E-1 Element 46 Mean
Model:
iDIANA
Element ULS
9.4.3-02 : TNO
RE.EPXXG EPXX Diana BV 28 OCT 2010 01:54:30 plan021
Min
LC2:=Load
-.163E-2
Max/Min oncase
model2 set:
Step:
Max = 30 LOAD: 5.92
.25E-1
Model:
iDIANA
Element ULS
9.4.3-02
RE.EPXXG :EPXX
TNO Diana BV 28 OCT 2010 01:54:30 plan022 8
Min
LC2:=Load
-.193E-2
case 2 E
Max/Min
Y onLOAD:
model set:
Step:
Max = 31
.316E-1 5.99 L
Model:
iDIANA
Element ULS
9.4.3-02 : TNO
RE.EPXXG EPXX Diana BV 28 OCT 2010 01:54:30 plan023
Min
LC2:=Load
-.236E-2
case 2 set: E 7
Max/Min
Y onLOAD:
model M
Step:
Max = Z32
.409E-1 6.03
Model:
iDIANA
Element ULS X
9.4.3-02
RE.EPXXG :EPXX
TNO Diana BV 28 OCT 2010 01:54:30 plan024 E
Min
LC2:=Load
-.296E-2
case 2 N 6
Max/Min
Y onLOAD:
model set: 0
Step:
Max = Z33
.484E-1 6.06 T
Model:
iDIANA
Element ULS X
9.4.3-02 : TNO
RE.EPXXG EPXX Diana BV 28 OCT 2010 01:54:30 plan025
Min
LC2:=Load
-.344E-2
case 2 set:
Max/Min
Y onLOAD:
model 0 R 5
Step:
Max = Z34
.54E-1 6.09
Model:
iDIANA
Element ULS X
9.4.3-02
RE.EPXXG :EPXX
TNO Diana BV 28 OCT 2010 01:54:30 plan026 E
Min
LC2:=Load
-.38E-2
case 2 .
Max/Min
Y onLOAD:
model set: DRAWING ANIMATE LOADCASES PLOTFILE plan 0
Step:
Max = Z35
.623E-1 6.12 E 4
Model:
iDIANA
Element ULS X
9.4.3-02 : TNO
RE.EPXXG EPXX Diana BV 28 OCT 2010 01:54:30 plan027
Min
LC2:=Load
-.434E-2
case 2 set: P
Max/Min
Y onLOAD:
model DRAWING ANIMATE LOADCASES PLOTFILE plan 0 X
Step:
Max = Z36
.736E-1 6.16
Model:
Element ULS X
RE.EPXXG EPXX X
Min
LC2:=Load
-.507E-2
case 2 G 3
Max/Min
Y onLOAD:
model set: DRAWING ANIMATE LOADCASES PLOTFILE plan 0
Step:
Max = Z37
.891E-1 6.2
Element X
RE.EPXXG EPXX
Min = -.607E-2 E
Max/Min
Y on model set: DRAWING ANIMATE LOADCASES PLOTFILE plan 0 P 2
Max = Z.116 X X
Min = -.779E-2
Y DRAWING ANIMATE LOADCASES PLOTFILE plan 0 X
Z X 1
Y DRAWING ANIMATE LOADCASES PLOTFILE plan 0
Z X
0
Y DRAWING ANIMATE LOADCASES PLOTFILE plan 0 1 2 3 4 5 6 7
Z X
LOAD
Y DRAWING ANIMATE LOADCASES PLOTFILE plan 0
Z X
Y DRAWING ANIMATE LOADCASES PLOTFILE plan 0
Z X
Y DRAWING ANIMATE LOADCASES PLOTFILE plan 0
Z X
Y DRAWING ANIMATE LOADCASES PLOTFILE plan 0
Z X
Y DRAWING ANIMATE LOADCASES PLOTFILE plan 0
Z X
Y DRAWING ANIMATE LOADCASES PLOTFILE plan 0
(a) animation of plastic area
Z X
Y
Z
Y
X
DRAWING ANIMATE LOADCASES PLOTFILE plan
DRAWING ANIMATE LOADCASES PLOTFILE plan
0
0
(b) time-graph for plastic strain
Z X
Y DRAWING ANIMATE LOADCASES PLOTFILE plan 0
Z X
Y
Z
Y
Z
X
X
Figure 12.14: Time evolution of plastic yield in the tendon
DRAWING ANIMATE LOADCASES PLOTFILE plan
DRAWING ANIMATE LOADCASES PLOTFILE plan
0
DRAWING ANIMATE LOADCASES PLOTFILE plan 0
Z X
DRAWING ANIMATE LOADCASES PLOTFILE plan 0
From the element number display of the tendon we can determine the ele-
DRAWING ANIMATE LOADCASES PLOTFILE plan
DRAWING ANIMATE LOADCASES PLOTFILE plan
ments in the plastic areas [Fig. 12.6b]: 37 in the left mid-span, 46 at the mid-
support. We make a time-graph for the evolution of the plastic strain in the
tendon for these elements [Fig. 12.14b]. The CEB-FIP model code regulations
specify a maximum elongation for the tendon of εu = 3.5%. From the time-
graph we can conclude that the ULS stage will be reached at load factor of 6,
which is load case LC2 32.
12.4.2 Stress in the Tendon
We will assess the distribution of the stress in the tendon at various stages of
the analysis.
Stress distribution uls.fvc
RESULTS ELEMENT RE.SXX.G SXX
RESULTS LOADCASE LC3 10
PRESENT GRAPH LINE ELEMENTS LIST 31 TO 62
RESULTS LOADCASE LC4 11
DRAWING DISPLAY
RESULTS LOADCASE LC2 32
DRAWING DISPLAY
We select the stress σxx in the reinforcement tendon as analysis result. Then
we select load case LC3 10 which represents the situation after application of live
load P1 . For this result we display the distribution as a graph along the line of
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
12.4 Ultimate Limit State Analysis 265
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:30 sxxlv1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:30 sxxlv2.ps
Model: ULS Model: ULS
LC3: Load case 3 LC4: Load case 4
Step: 10 LOAD: 1 Step: 11 LOAD: 1
Element RE.SXX.G SXX Element RE.SXX.G SXX
Max/Min on whole graph: Max/Min on whole graph:
Ymax = .141E10 Ymax = .141E10
Ymin = .129E10 Ymin = .129E10
*1E9 Xmax = 58.1 *1E9 Xmax = 58.1
Xmin = 0 Xmin = 0
1.42 Variation along a line 1.42 Variation along a line
Mean value used for each element Mean value used for each element
1.4 1.4
E E
L L
E E
M 1.38 M 1.38
E E
N N
T T
1.36 1.36
R R
E E
. .
S 1.34 S 1.34
X X
X X
. .
G G
1.32 1.32
S S
X X
X X
1.3 1.3
1.28 1.28
0 10 20 30 40 50 60 0 10 20 30 40 50 60
DISTANCE DISTANCE
(a) for live load P1 (b) for live load P2
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:30 sxxuls.ps
Model: ULS
LC2: Load case 2
Step: 32 LOAD: 6.03
Element RE.SXX.G SXX
Max/Min on whole graph:
Ymax = .186E10
Ymin = .13E10
*1E9 Xmax = 58.1
Xmin = 0
1.9 Variation along a line
Mean value used for each element
1.8
E
L
E
M 1.7
E
N
T
1.6
R
E
.
S 1.5
X
X
.
G
1.4
S
X
X
1.3
1.2
0 10 20 30 40 50 60
DISTANCE
(c) at ULS
Figure 12.15: Distribution of the tendon stresses along the beam
elements that represent the tendon [Fig. 12.15a]. In the same way we present
the stress distribution for load case LC4 11 which represents the situation after
application of live load P2 [Fig. 12.15b]. The situation at ULS is represented by
load case LC2 32 for which we also display the distribution [Fig. 12.15c].
12.4.3 Crack Development in the Beam
We will assess the crack development in the beam. First the crack pattern in
the ULS state and then the evaluation of the cracks in time.
ULS state uls.fvc
DRAWING VIEWPORT SETUP TWO-HORIZ
VIEW MESH BEAM
EYE FRAME
RESULTS GAUSSIAN EL.EKNN1 EKNN
RESULTS RANGE SURFACE 11
PRESENT DISC .3
DRAWING VIEWPORT USE 2
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
266 Post-tensioned Concrete Beam
RESULTS RANGE SURFACE 12
PRESENT DISC .3 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:30 crak001
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:30 crak002
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:30 crak003
We setup a Graphics Window with two viewports and display the mesh of the iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:30 crak004
beam in the top viewport. We select the crack strain εcr as analysis result. Note
iDIANA 9.4.3-02 : TNO Diana BV
iDIANA 9.4.3-02 : TNO Diana BV
28 OCT 2010 01:54:30 crak005
28 OCT 2010 01:54:31 crak006
that the currently selected load case is still that for the ULS State: LC2 32. We
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:31 crak007
select surface 11 and 12, for the upper and lower fiber of the beam, and display
iDIANA 9.4.3-02 : TNO Diana BV
Model: ULS
28 OCT 2010 01:54:31 crak008 1
εcr as discs to get a clear impression of the crack pattern [Fig. 12.16a].
Deformation = 1
LC2: Load case
iDIANA 2
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:31 crak009 1
Step: 14 LOAD: 2.93
Gauss EL.EKNN1 EKNN
Model: ULS
All surfaces
Deformation = 1 set:
Max/Min on model
LC2:
Max =Load
iDIANA case 2
9.4.3-02
.686E-3 : TNO Diana BV 28 OCT 2010 01:54:31 crak010 1
Step:
Min = 15
0 LOAD: 3.78
Gauss EL.EKNN1 EKNN
Model: ULS
All surfaces
Deformation = 1 set:
Max/Min on model
LC2:
Max =Load
iDIANA case 2
9.4.3-02
.132E-2 : TNO Diana BV 28 OCT 2010 01:54:31 crak011 1
Step:
Min = 16
0 LOAD: 4.04
Gauss EL.EKNN1 EKNN
Model:
All ULS
surfaces
Deformation = 1 set:
Max/Min on model
LC2:
Max =Load
iDIANA case 2
9.4.3-02
.163E-2 : TNO Diana BV 28 OCT 2010 01:54:31 crak012 1
Step:
Min = 17
0 LOAD: 4.24
Gauss EL.EKNN1 EKNN
Model: ULS
All surfaces
Deformation = 1 set:
Max/Min on model
LC2:
Max =Load
iDIANA case 2
9.4.3-02
.188E-2 : TNO Diana BV 28 OCT 2010 01:54:31 crak013 1
Step:
Min = 18
0 LOAD: 4.38
Gauss EL.EKNN1 EKNN
Model: ULS
All surfaces
Y
Deformation = 1 set:
Max/Min on model
LC2:
Max =Load
iDIANA case 2
9.4.3-02
.231E-2 : TNO Diana BV 28 OCT 2010 01:54:31 crak014 1
Step:
Min = 19
0 LOAD: 4.5 0
GaussZ EL.EKNN1
X EKNN 0
Model:
Y ULS
All surfaces
Deformation = 1 set:
Max/Min on model
LC2:=Load
iDIANA
Max case 2
9.4.3-02
.283E-2 : TNO Diana BV 28 OCT 2010 01:54:31 crak015 2
1
Step:
Min = 20
0 LOAD: 4.58 0
GaussZ EL.EKNN1
X EKNN 0
Model:
Y ULS
All surfaces
Deformation = 1 set:
Max/Min on model DRAWING ANIMATE LOADCASES PLOTFILE crak
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:30 crkuls.ps LC2:
Max Load
iDIANA
= .34E-2 case 2 = 0
9.4.3-02
Min : TNO Diana BV 2
28 OCT 2010 01:54:31 crak016 1
Step: 21 LOAD: 4.65 0
GaussZ EL.EKNN1
X EKNN 0
Model: ULS Model:
Y ULS
All surfaces
LC2: Load case 2 Deformation = 1 set:
Max/Min on model DRAWING ANIMATE LOADCASES PLOTFILE crak
Step: 32 LOAD: 6.03 LC2:
Max =Load
iDIANA case 2
9.4.3-02
.377E-2 : TNO Diana BV 2
28 OCT 2010 01:54:31 crak017 1
Step:
Min = 22
0 LOAD: 4.74 0
Gauss EL.EKNN1 EKNN GaussZ EL.EKNN1
X EKNN
Surface 11 Model: 0
Max/Min on model set: Y ULS
All surfaces
DRAWING ANIMATE LOADCASES PLOTFILE crak
Deformation = 1 set:
Max/Min on model
Max = .476E-1 LC2:=Load
iDIANA
Max case 2
9.4.3-02
.431E-2 : TNO Diana BV 2
28 OCT 2010 01:54:31 crak018 1
Min = 0 Step:
Min = 23
0 LOAD: 4.89 0
GaussZ EL.EKNN1
X EKNN 0
Model:
Y ULS
All surfaces
Deformation = 1 set:
Max/Min on model DRAWING ANIMATE LOADCASES PLOTFILE crak
LC2:=Load
iDIANA
Max case 2
9.4.3-02
.525E-2 : TNO Diana BV 2
28 OCT 2010 01:54:31 crak019 1
Step:
Min = 24
0 LOAD: 5.05 0
GaussZ EL.EKNN1
X EKNN 0
Model:
Y ULS
All surfaces
Deformation = 1
Max/Min on model set: DRAWING ANIMATE LOADCASES PLOTFILE crak
LC2:=Load
iDIANA
Max case 2
9.4.3-02
.647E-2 : TNO Diana BV 2
28 OCT 2010 01:54:31 crak020 1
Step:
Min = 25
0 LOAD: 5.24 0
GaussZ EL.EKNN1
X EKNN 0
Model:
Y ULS
All surfaces
Deformation = 1
Max/Min on model set: DRAWING ANIMATE LOADCASES PLOTFILE crak
LC2:=Load
iDIANA
Max case 2
9.4.3-02
.793E-2 : TNO Diana BV 2
28 OCT 2010 01:54:31 crak021 1
Step:
Min = 26
0 LOAD: 5.52 0
GaussZ EL.EKNN1
X EKNN 0
Model:
Y ULS
All surfaces
Deformation = 1 set:
Max/Min on model DRAWING ANIMATE LOADCASES PLOTFILE crak
Y
LC2:=Load
iDIANA
Max case 2
9.4.3-02
.105E-1 : TNO Diana BV 2
28 OCT 2010 01:54:31 crak022 1
Step:
Min = 027 LOAD: 5.71 0
GaussZ EL.EKNN1
X EKNN 0
0 Model:
Z X 0 All Y ULS
surfaces
DRAWING ANIMATE LOADCASES PLOTFILE crak
Deformation = 1 set:
Max/Min on model
LC2:=Load
iDIANA
Max case 2
9.4.3-02
.139E-1 : TNO Diana BV 2
28 OCT 2010 01:54:31 crak023 1
1 Step:
Min = 28
0 LOAD: 5.77 0
GaussZ EL.EKNN1
X EKNN 0
Model: ULS
All surfaces
Y
Model: ULS Deformation = 1 set:
Max/Min on model DRAWING ANIMATE LOADCASES PLOTFILE crak
LC2: Load case 2 LC2:=Load
iDIANA
Max case 2
9.4.3-02
.162E-1 : TNO Diana BV 2
28 OCT 2010 01:54:31 crak024 1
Step: 32 LOAD: 6.03 Step:
Min = 29
0 LOAD: 5.85 0
Gauss EL.EKNN1 EKNN GaussZ EL.EKNN1
X EKNN 0
Surface 12 Model:
Y ULS
All surfaces
Max/Min on model set: Deformation = 1 set:
Max/Min on model DRAWING ANIMATE LOADCASES PLOTFILE crak
Max = .231E-1 LC2:
Max =Load case 2
.196E-1 2
1
Min = 0 Step:
Min = 30
0 LOAD: 5.92 0
GaussZ EL.EKNN1
X EKNN 0
Model:
Y ULS
All surfaces
Deformation = 1 set:
Max/Min on model DRAWING ANIMATE LOADCASES PLOTFILE crak
LC2:
Max = .243E-1 2
Load case 2
1
Step:
Min = 31
0 LOAD: 5.99 0
GaussZ EL.EKNN1
X EKNN 0
Model:
Y ULS
All surfaces
Deformation = 1 set:
Max/Min on model DRAWING ANIMATE LOADCASES PLOTFILE crak
LC2:
Max = .311E-1 2
Load case 2
1
Step:
Min = 32
0 LOAD: 6.03 0
GaussZ EL.EKNN1
X EKNN 0
Model:
Y ULS
All surfaces
Deformation = 1 set:
Max/Min on model DRAWING ANIMATE LOADCASES PLOTFILE crak
LC2:
Max =Load case 2
.366E-1 2
1
Step:
Min = 33
0 LOAD: 6.06 0
GaussZ EL.EKNN1
X EKNN 0
Model:
Y ULS
All surfaces
Deformation = 1 set:
Max/Min on model DRAWING ANIMATE LOADCASES PLOTFILE crak
Y LC2:
Max =Load case 2
.407E-1 2
1
Step:
Min = 34
0 LOAD: 6.09 0
GaussZ EL.EKNN1
X EKNN 0
0 Model:
Y ULS
All surfaces
Z X 0 Deformation = 1 set:
Max/Min on model DRAWING ANIMATE LOADCASES PLOTFILE crak
LC2:
Max =Load case 2
.467E-1 2
1
Step:
Min = 35
0 LOAD: 6.12 0
2 GaussZ EL.EKNN1
X EKNN 0
Model:
Y ULS
All surfaces
Deformation = 1 set:
Max/Min on model DRAWING ANIMATE LOADCASES PLOTFILE crak
LC2:
Max =Load
.55E-1caseMin
2 = 0 2
1
Step: 36 LOAD: 6.16 0
GaussZ EL.EKNN1
X EKNN 0
Model:
Y ULS
All surfaces
Deformation = 1 set:
Max/Min on model DRAWING ANIMATE LOADCASES PLOTFILE crak
LC2:
Max =Load case 2
.663E-1 2
Step:
Min = 37
0 LOAD: 6.2 0
(a) at ULS, upper en lower fiber
GaussZ EL.EKNN1
X EKNN 0
All surfaces
Y
Max/Min on model set: DRAWING ANIMATE LOADCASES PLOTFILE crak
Max = .859E-1 2
Min = 0 0
Z X 0
Y DRAWING ANIMATE LOADCASES PLOTFILE crak
2
0
Z X 0
Y DRAWING ANIMATE LOADCASES PLOTFILE crak
2
0
Z X 0
Y DRAWING ANIMATE LOADCASES PLOTFILE crak
2
0
Z X
(b) animation in deformed model
0
Y DRAWING ANIMATE LOADCASES PLOTFILE crak
2
0
Z X 0
DRAWING ANIMATE LOADCASES PLOTFILE crak
2
DRAWING ANIMATE LOADCASES PLOTFILE crak
Figure 12.16: Crack pattern in beam
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
12.4 Ultimate Limit State Analysis 267
Crack development animation uls.fvc
RESULTS LOADCASE LC2 14 TO LC2 37
RESULTS RANGE OFF
VIEW OPTIONS DEFORM USING TDTX...G RESTDT 1
DRAWING ANIMATE LOADCASES PLOTFILE crak
We select all load cases for which crack strain has arisen, i.e., load case LC2 14
(load factor 2.9) and beyond. We switch off the range (surface) selection to get
the cracks in one display. We also indicate that the model must be drawn in
its true deformed state (factor 1). The animation clearly shows the behavior of
the concrete beam [Fig. 12.16b].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
268 Post-tensioned Concrete Beam
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
Chapter 13
Long Term Behavior of RC
Beam
Name: RCbeam
Path: /Examples/ConcMas/RCbeam
Keywords: analys: nonlin physic. constr: suppor. elemen: bar beam
cl9be class3 rectan reinfo. load: force node weight. materi:
concre consta crack creep cutoff elasti isotro maxwel nonlin re-
tent shrink smear soften temper viscoe. option: adapti ar-
clen direct loadin newton regula size spheri units. post: binary
femvie. result: cauchy crack displa green status strain stress
total.
F F
A
1000 1100 1000
A–A
2∅6
160
5∅12
750
Figure 13.1: Jaccoud & Favre – Geometry C-series [mm]
From 1979 to 1982 a series of long term experiments on reinforced simply sup-
ported concrete slabs were carried out at the l’Ecole Polytechnique Fédérale de
Lausanne in Switzerland. Figure 13.1 shows the dimensions of the slab and its
boundary conditions. The results of the experiments were published by Jac-
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
270 Long Term Behavior of RC Beam
coud & Favre [7]. In 1993 the RILEM committee TC 114 adopted the so-called
C-series as benchmark tests for computer software for creep and shrinkage, see
Espion [6] and Vonk et al. [15].
This example illustrates the calculation and validation of the long term be-
havior of the C-series reinforced concrete slab. At an age of 28 days, five slabs,
denoted C11 to C15, were loaded up to different load levels, representing ap-
proximately 20 to 60 % of the theoretical failure load. The numerical analysis
is executed for experiment C11 and C15. For these experiments the time de-
pendent deflection of the mid span was measured for a time span of one year.
In experiment C11 no cracking occurred. The reinforcement remained elastic
during both tests.
13.1 Finite Element Model
Since the slab and loading scheme are symmetrical, it is sufficient to model only
one half of the slab. The half is modeled by seven three-node CL9BE beam
elements [Fig. 13.2]. The CL9BE element is a numerically integrated two-dimen-
Y
♥
X
Figure 13.2: Idealized finite element model
sional element in which shear deformation is included according to the Mindlin–
Reissner theory [Vol. Element Library]. The input data file is as follows:
Input data beam.dat
Jaccoud & Favre, reinforced concrete slab, C-series
’UNITS’
TIME DAY
LENGTH MM
MASS 7.46496e+12 0.
: FORCE 7.46496e+12*KG*MM/DAY**2 = 1. N
’COORDINATES’
1 .00000E+00 .00000E+00 .00000E+00
2 .10000E+03 .00000E+00 .00000E+00
3 .20000E+03 .00000E+00 .00000E+00
4 .30000E+03 .00000E+00 .00000E+00
5 .40000E+03 .00000E+00 .00000E+00
6 .50000E+03 .00000E+00 .00000E+00
7 .60000E+03 .00000E+00 .00000E+00
8 .70000E+03 .00000E+00 .00000E+00
9 .80000E+03 .00000E+00 .00000E+00
10 .90000E+03 .00000E+00 .00000E+00
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
13.1 Finite Element Model 271
11 .10000E+04 .00000E+00 .00000E+00
12 .11375E+04 .00000E+00 .00000E+00
13 .12750E+04 .00000E+00 .00000E+00
14 .14125E+04 .00000E+00 .00000E+00
15 .15500E+04 .00000E+00 .00000E+00
16 .00000E+00 -51. .00000E+00
17 .15500E+04 -51. .00000E+00
18 .00000E+00 54. .00000E+00
19 .15500E+04 54. .00000E+00
’ELEMEN’
CONNEC
1 CL9BE 1 2 3
2 CL9BE 3 4 5
3 CL9BE 5 6 7
4 CL9BE 7 8 9
5 CL9BE 9 10 11
6 CL9BE 11 12 13
7 CL9BE 13 14 15
MATERI
/ 1-7 / 1
DATA
/ 1-7 / 1
GEOMET
/ 1-7 / 1
’REINFO’
LOCATI
1 BAR
LINE 16 17
2 BAR
LINE 18 19
GEOMET
1 2
2 3
MATERI
/ 1 2 / 2
’MATERI’
:Concrete
1 YOUNG 29300.
POISON 0.2
: density 2.500000e-06 kg/mm^3
DENSIT 3.348979e-19
:Reinforcement
2 YOUNG 2.1E+5
’DATA’
1 NUMINT GAUSS SIMPSO
NINTEG 2 9
’GEOMET’
1 RECTAN 160.0 750.0
2 CROSSE 565.0
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
272 Long Term Behavior of RC Beam
3 CROSSE 57.0
’SUPPORTS’
1 TR 2
15 TR 1 RO 3
’LOADS’
CASE 1
NODAL
11 FORCE 2 -1.E+3
CASE 2
WEIGHT
: gravity = 9.81 m/sec^2
2 -73231258.E6
COMBIN
1 1 1.
2 2 1.
:C11
3 1 2.885 2 1.
’END’
In axial direction, the default 2-point reduced Gauss integration is used to pre-
vent shear locking. In thickness direction the 9-point Simpson integration is
used. This scheme has proved to be sufficiently accurate in similar calculations.
Because of the two-dimensional idealization, all reinforcements at one side are
modeled by one embedded bar with default integration scheme per part (two-
point Gauss).
Load set 1 is a unit nodal load F = 1 kN, load set 2 is dead weight loading
and load set 3 is the combined load for experiment C11 (F = 2.885 kN).
13.2 Preliminary Linear Analysis
The model, loads and boundary conditions are checked by running a linear
elastic analysis with the following command file.
lin.dcf
*FILOS
INITIA
*INPUT
*LINSTA
BEGIN OUTPUT FEMVIE
SELECT LOADS 3 /
DISPLA
STRESS FORCE
STRESS MOMENT
END OUTPUT
*END
The FEMVIE output option will deliver a database with analysis results for as-
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
13.2 Preliminary Linear Analysis 273
sessment in the iDiana Results environment. We run Diana with the input
data file and the command file.
diana beam.dat lin
When the analysis has terminated we enter the iDiana Results environment to
assess the analysis results.
lin.fvc
FEMVIEW LIN
VIEW OPTIONS SHRINK
VIEW OPTIONS HIDDEN BEAMS QUICK 100
VIEW MESH ALL
VIEW HIDDEN SHADE
LABEL MESH CONSTRNT
With these commands we get a shrunken elements view of the mesh where
the beam elements and reinforcements are displayed with artificially enlarged
cross-sections [Fig. 13.3a]. The top and bottom row of elements denote the
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:27 mesh.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:27 ledfm.ps
Model: LIN Model: LIN
LC3: Load case 3
Nodal DTX....G RESDTX
Max = .838
Min = .126E-2
Factor = 109
Y Y
Z X Z X
(a) undeformed mesh (b) elastic deformation for C11
Figure 13.3: Finite element model
reinforcements, the mid row is for the beam elements. Finally we display the
boundary constraints on the mesh.
13.2.1 Displacements
To display the displacements we first switch off the viewing options to get the
mesh simply displayed with green lines.
lin.fvc
LABEL MESH OFF
VIEW HIDDEN OFF
VIEW OPTIONS SHRINK OFF
RESULTS LOADCASE LC3
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
274 Long Term Behavior of RC Beam
RESULTS NODAL DTX....G RESDTX
PRESENT SHAPE
We select the results of LC3, i.e., load set 3 of the input data. Then we select the
nodal displacements, represented by result attribute RESDTX. The SHAPE option
then displays the deformed mesh in red [Fig. 13.3b]. In the results monitor we
observe that the calculated maximum deflection of the mid span uY = 0.838.
This is in reasonable accordance with the analytical value:
5 q l4 Fa ¡ 2 ¢
uY = + 3 l − 4 a2
384 EI 24 EI (13.1)
= 0.469 + 0.395 = 0.864 mm
with a = 1000 mm the distance from load to support, l = 3100 mm the span,
F = 2885 N the point load, q = 2.943 N/mm the distributed dead weight load,
and EI = 7.547×1012 N·mm2 the sum of bending stiffness contributions. The
first experimental value, measured 5 minutes after loading, is uY = 1.1 mm.
13.2.2 Shear Force and Bending Moment
To display the distribution of the shear force and the bending moment we switch
to a graphics window with two viewports. Thus we can simultaneously display
the results in two different ways: a diagram and a contour plot.
Shear force lin.fvc
DRAWING VIEWPORT SETUP TWO-HORIZ
DRAWING VIEWPORT USE TLEFT
EYE ANGLE 0
EYE FRAME
RESULTS ELEMENT EL.NX..L QY
PRESENT DIAGRAM
DRAWING VIEWPORT COPY TLEFT TO BLEFT
PRESENT CONTOUR LEVELS 5
For the shear force we display a two-dimensional view of the model in the XY -
plane: via the ANGLE option we specify a zero view angle with respect to the
Z-axis. Then we select attribute QY for the shear force QY . The diagram is
displayed in the top viewport and the contour plot in the bottom [Fig. 13.4a].
In the diagram we clearly see the discontinuity at the location of the load.
Bending moment lin.fvc
DRAWING VIEWPORT USE TLEFT
EYE ROTATE TO 90 0 0
RESULTS ELEMENT EL.MX..L MZ
PRESENT DIAGRAM
DRAWING VIEWPORT COPY TLEFT TO BLEFT
PRESENT CONTOUR LEVELS 5
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
13.3 Material Parameters 275
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:27 leqy.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:27 lemz.ps
Model: LIN Model: LIN
LC3: Load case 3 LC3: Load case 3
Element EL.NX..L QY Element EL.MX..L MZ
Max = -.476E-9 Max = -.981E4
Min = -.745E4 Min = -.644E7
Factor = .122E-1 Factor = .142E-4
Y Z
Z X Y X
1 1
Model: LIN Model: LIN
LC3: Load case 3 LC3: Load case 3
Element EL.NX..L QY Element EL.MX..L MZ
Max = -.476E-9 Max = -.981E4
Min = -.745E4 Min = -.644E7
Y -.124E4 Z -.108E7
-.248E4 -.215E7
-.372E4 -.322E7
Z X -.496E4 Y X -.43E7
-.621E4 -.537E7
2 2
(a) shear force (b) bending moment
Figure 13.4: Linear elastic stress for C11
For the bending moment we display the model in the XZ-plane. Then we select
attribute MZ for the bending moment MZ . Again we display the diagram in the
top viewport and the contour plot in the bottom [Fig. 13.4b].
13.3 Material Parameters
Apart from the usual elastic properties, input is needed to model creep, shrink-
age and cracking. The material models in this example are based on the CEB-
FIP Model Code 1990 [2].
Creep. Creep is modeled by rheologic Maxwell chains, consisting of several
parallel spring and dashpot chains. The properties of these chains can be de-
rived from experimental curves or standard creep models like CEB-FIP by curve
fitting. In the past, tools and handbooks were developed for this purpose. In
Diana, parameter determination from experimental or standard creep or relax-
ation curves is directly part of the code.
Input data for the CEB-FIP creep model are: the initial age of loading t0 ,
the modulus of elasticity Et0 , the mean compressive strength fcm , the notational
size h0 , the cement type, the relative humidity RH and the ambient temperature
Tenv .
Shrinkage. Shrinkage is modeled as age-dependent initial strain. The CEB-
FIP shrinkage model requires no additional input data, compared to the creep
model. The input data specified below leads to a basic shrinkage strain εsh
0 =
5.55650×10−4 .
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
276 Long Term Behavior of RC Beam
Cracking. A multi–directional fixed crack model is used, with constant stress
cut-off, nonlinear tension softening and constant shear retention. The additional
input data are: tensile strength ft , fracture energy Gf , crack bandwidth hcr and
the shear retention factor β.
Input material data. By assuming constant distribution of average proper-
ties and using standard models, the numerical calculations will result in true
predictions without any curve fitting to the experiments. The input data [Ta-
ble 13.1], are determined directly from the reported results of experiments on
Table 13.1: Input data from experiments
Initial Young’s modulus Et0 29.3 kN/mm2
Tensile strength ft 2.8 N/mm2
Mean compressive strength fcm 30.55 N/mm2
Concrete age at loading t0 28 days
Relative ambient humidity RH 60
Ambient temperature Tenv 20 °C
Notational member size h0 132 mm
prisms or cubes, the reported environment conditions, and the slab geometry.
The remaining data are estimated [Table 13.2], where hcr is estimated from stir-
Table 13.2: Estimated input data
Normal hardening cement
Estimated crack bandwidth hcr 200 mm
Poisson’s ratio ν 0.2
Fracture energy Gf 0.06 N·mm/mm2
Constant shear retention factor β 0.2
rup spacing and Gf is for CEB-FIP grade C20 with a maximum aggregate size
of 16 mm.
It must be noted that a rather large experimental scatter is observed for
results of identical experiments on different cubes and slabs. The elastic prop-
erties in the ’MATERI’ table are extended with the required material data for
the nonlinear analysis. The material input data is as follows.
materi.dat
’UNITS’
TIME DAY
LENGTH MM
MASS 7.46496e+12 0.
: FORCE 7.46496e+12*KG*MM/DAY**2 = 1. N
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
13.4 Nonlinear Analysis 277
TEMPER CELSIUS
’MATERI’
:Concrete
1
:Elastic properties
YOUN28 29300.
POISON 0.2
: density 2.500000e-06 kg/mm^3
DENSIT 3.348979e-19
:Creep and shrinkage according to CEB-FIP model code 1990
CREEPN MC1990
SHRINN MC1990
FCM28 30.55
H 132.
LODAGE 28.
CEMTYP NR
RH 60.
TEMPER 20.
:Cracking
CRACK 1
CRKVAL 2.8
TAUCRI 1
BETA 0.2
TENSIO 3
GF 0.06
CRACKB 200.
:Reinforcement
2 YOUNG 2.1E+5
’END’
Diana will translate the creep input to Maxwell chains, which are the actual
input for a nonlinear analysis.
13.4 Nonlinear Analysis
It is assumed that both shrinkage and creep start from the moment of loading,
with an initial concrete age of 28 days and a calculation time of 0 days. The dead
weight in load set 1 and the point load in load set 2 are applied using load steps.
Automatic load step control is used in case of cracking. The subsequent creep
and shrinkage are analyzed using time steps in days. The time stepping scheme
is composed by incrementing the step size logarithmically, starting from 25 %
of the lowest relaxation time and maximized by 5 % of the highest relaxation
time.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
278 Long Term Behavior of RC Beam
13.4.1 Experiment C11
In this experiment the structure must remain uncracked. Therefore, the point
load can be applied in one step without size control. Afterward the effect of
creep and shrinkage is analyzed for a period of 365 days. The analysis commands
are:
creep1.dcf
*FILOS
INITIA
*INPUT
READ FILE="beam.dat"
READ FILE="materi.dat"
*NONLIN
TYPE PHYSIC
BEGIN OUTPUT FEMVIE
SELECT STEPS ALL
DISPLA GLOBAL
END OUTPUT
BEGIN OUTPUT FEMVIE APPEND
MODEL OFF
SELECT STEPS 2 LAST
STRESS TOTAL CAUCHY
END OUTPUT
: Apply dead weight load
BEGIN EXECUT
BEGIN LOAD
STEPS EXPLIC SIZES 1.0
LOADNR=2
END LOAD
BEGIN ITERAT
BEGIN CONVER
ENERGY TOLCON=1.0E-6
FORCE OFF
DISPLA OFF
END CONVER
END ITERAT
OUTPUT OFF
END EXECUT
: Apply point weight
BEGIN EXECUT
BEGIN LOAD
STEPS EXPLIC SIZES 2.885
LOADNR=1
END LOAD
BEGIN ITERAT
MAXITE=50
BEGIN CONVER
ENERGY TOLCON=1.0E-6
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
13.4 Nonlinear Analysis 279
FORCE OFF
DISPLA OFF
END CONVER
END ITERAT
END EXECUT
: Shrinkage and creep
BEGIN EXECUT
TIME STEPS EXPLIC SIZES 0.1E-5 0.2E-5 0.7E-5 0.2E-4 0.7E-4 0.2E-3 \
0.7E-3 0.2E-2 0.7E-2 0.2E-1 0.7E-1 0.2 0.7 \
2.0 7.0 20.0 35.0(2) 50.0(4) 65.0
BEGIN ITERAT
MAXITE=50
BEGIN CONVER
ENERGY TOLCON=1.0E-6
FORCE OFF
DISPLA OFF
END CONVER
END ITERAT
END EXECUT
*END
Now we run Diana as follows.
diana creep1
When the analysis has terminated we enter the iDiana Results environment to
assess the analysis results.
iDiana
FEMVIEW CREEP1
We will assess the development of the deflection of the beam and of the axial
stresses.
13.4.1.1 Deflection in Time
To make a history plot of the deflection of the beam we select all load cases
(time steps) and attribute TDTY for the vertical displacement uY .
creep1.fvc
RESULTS LOADCASE LC1 3 TO LC1 25
RESULTS NODAL TDTX...G TDTY
PRESENT GRAPH NODE 15
We make a graph for the selected result in node 15, i.e., the mid-span loca-
tion [Fig. 13.5]. The predicted creep deflection of the mid-span after a year is
∆uY = 3.12 − 0.84 = 2.28 mm [Eq. (13.1) p. 274], while the analysis result is
∆uY = 3.12 − 0.46 = 2.66 mm (see results monitor). The measured value from
experiments is ∆uY = 4.6 − 1.1 = 3.5 mm.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
280 Long Term Behavior of RC Beam
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:33 c1defl.ps
Model: CREEP1
Nodal TDTX...G TDTY
Max/Min on whole graph:
Ymax = -.84
Ymin = -3.12
Xmax = 365
Xmin = .1E-5
Variation over loadcases
Node 15
-.75
-1
N -1.25
O
D
A -1.5
L
T -1.75
D
T
X -2
.
.
. -2.25
G
T -2.5
D
T -2.75
Y
-3
-3.25
0 50 100 150 200 250 300 350 400
TIME
Figure 13.5: C11: Deflection in time
13.4.1.2 Axial Stress
We will now display the axial stresses in the beam and the reinforcement at two
points in time: just after loading and after 365 days.
Just after loading creep1.fvc
DRAWING VIEWPORT SETUP TWO-HORIZ
VIEW MESH
EYE ANGLE 0
EYE FRAME
RESULTS LOADCASE LC1 2
RESULTS ELEMENT EL.SXX.G SXX
PRESENT SYMBOL
DRAWING VIEWPORT USE BLEFT
RESULTS LOADCASE LC1 2
RESULTS ELEMENT RE.SXX.G SXX
PRESENT SYMBOL
We make two viewports: the top one for the beam elements and the bottom for
the reinforcements. We select LC1 2 for time step 2, which is just after loading.
Result attribute SXX represents the axial stress σxx which we display with sym-
bols (triangles). iDiana modulates the symbols with size and color according
to the values they represent. In the top viewport we display the stresses for the
beam elements and in the bottom for the reinforcements [Fig. 13.6a].
After 365 days creep1.fvc
DRAWING VIEWPORT USE TLEFT
RESULTS LOADCASE LC1 25
RESULTS ELEMENT EL.SXX.G SXX
PRESENT SYMBOL
DRAWING VIEWPORT USE BLEFT
RESULTS LOADCASE LC1 25
RESULTS ELEMENT RE.SXX.G SXX
PRESENT SYMBOL
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
13.4 Nonlinear Analysis 281
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:33 c1sxxb.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:34 c1sxxe.ps
Model: CREEP1 Model: CREEP1
LC1: Load case 1 LC1: Load case 1
Step: 2 LOAD: 2.88 Step: 25 TIME: 365
Element EL.SXX.G SXX Element EL.SXX.G SXX
Max = -.299E-2 Max = -.152
Min = -1.96 Min = -2.02
Symbol factor = 1 Symbol factor = 1
All values All values
-.196 -.187
-.392 -.374
-.588 -.56
-.783 -.747
-.979 -.934
Y -1.18 Y -1.12
-1.37 -1.31
-1.57 -1.49
-1.76 -1.68
Z X -1.96 Z X -1.87
1 1
Model: CREEP1 Model: CREEP1
LC1: Load case 1 LC1: Load case 1
Step: 2 LOAD: 2.88 Step: 25 TIME: 365
Element RE.SXX.G SXX Element RE.SXX.G SXX
Max = 8.55 Max = -35.3
Min = -9.58 Min = -100
Symbol factor = 1 Symbol factor = 1
All values All values
7.25 -39.1
5.44 -45.6
3.63 -52.1
1.81 -58.6
-.222E-15 -65.1
Y -1.81 Y -71.6
-3.63 -78.1
-5.44 -84.6
-7.25 -91.1
Z X -9.07 Z X -97.6
2 2
(a) just after loading (b) after 365 days
Figure 13.6: C11: axial stress in beam (top) and reinforcements (bottom)
Here we select time step 25 which represents the time point after 365 days.
Analogous to the time point just after loading we display the axial stresses with
symbols in the two viewports [Fig. 13.6b]. Note that the colors and sizes of the
triangles in the four viewports do not represent the same values.
13.4.2 Experiment C15
In this experiment the structure will show cracking already during loading.
Therefore the point load is applied with automatic step size control via the
Spherical Path Arc-length method. Afterward again the effect of creep and
shrinkage is analyzed for a period of 365 days. The complete command file for
this analysis is as follows:
creep2.dcf
*FILOS
INITIA
*INPUT
READ FILE="beam.dat"
READ FILE="materi.dat"
*NONLIN
TYPE PHYSIC
: Apply dead weight load
BEGIN EXECUT
BEGIN LOAD
STEPS EXPLIC SIZES 1.0
LOADNR=2
END LOAD
BEGIN ITERAT
BEGIN CONVER
ENERGY TOLCON=1.0E-6
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
282 Long Term Behavior of RC Beam
FORCE OFF
DISPLA OFF
END CONVER
END ITERAT
BEGIN OUTPUT FEMVIE
DISPLA GLOBAL
END OUTPUT
END EXECUT
: Apply point load
BEGIN EXECUT
BEGIN LOAD
BEGIN STEPS
BEGIN ITERAT
INISIZ=4.0
MINSIZ=1.0
NSTEPS=50
GAMMA=0.5
NITERA=6
ARCLEN SPHERI
END ITERAT
END STEPS
LOADNR=1
END LOAD
BEGIN ITERAT
MAXITE=50
BEGIN CONVER
ENERGY TOLCON=1.0E-6
FORCE OFF
DISPLA OFF
END CONVER
END ITERAT
BEGIN OUTPUT FEMVIE APPEND
DISPLA GLOBAL
STATUS CRACK
STRAIN CRACK
STRESS TOTAL CAUCHY
END OUTPUT
STOP LOAD TOTAL=15.725
END EXECUT
: Shrinkage and creep
BEGIN EXECUT
TIME STEPS EXPLIC SIZES 0.1E-5 0.2E-5 0.7E-5 0.2E-4 0.7E-4 0.2E-3 \
0.7E-3 0.2E-2 0.7E-2 0.2E-1 0.7E-1 0.2 0.7 \
2.0 7.0 20.0 35.0(2) 50.0(4) 65.0
BEGIN ITERAT
MAXITE=50
BEGIN CONVER
ENERGY TOLCON=1.0E-6
FORCE OFF
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
13.4 Nonlinear Analysis 283
DISPLA OFF
END CONVER
END ITERAT
BEGIN OUTPUT FEMVIE APPEND
DISPLA GLOBAL
STATUS CRACK
STRAIN CRACK
STRESS TOTAL CAUCHY
END OUTPUT
END EXECUT
*END
We run Diana with this command file:
diana creep2
We enter the iDiana Results environment to asses the analysis results.
iDiana
FEMVIEW CREEP2
For experiment C15 we will asses the deflection in time, the crack pattern, and
the axial stress.
13.4.2.1 Deflection in Time
We will make two history plots of the deflection of the beam: one which only
covers the time until just after the application of the load, and another one
which covers the full time span of one year.
creep2.fvc
RESULTS LOADCASE LC2 1 TO LC1 22
RESULTS NODAL TDTX...G TDTY
PRESENT GRAPH NODE 15
RESULTS LOADCASE LC1 23 TO LC1 45
PRESENT GRAPH NODE 15
First we select the time steps up to step 22, which represent the time span
until just after application of the load. The graph [Fig. 13.7a] shows the load–
deflection curve of the mid-span. Note the temporary decrease of the load at
the moment of initial cracking, calculated by the automatic step size control.
Output shows that the point load has been applied in eight steps. The calculated
deflection of the mid-span after complete loading is uY = 13.1 mm, while the
instantaneously measured value is uY = 10 mm.
The second graph [Fig. 13.7b] shows the development of the deflection over
one year, i.e., all time steps. The predicted creep deflection after a year is
∆uY = 21.14 − 13.13 = 8.01 mm. The result of the Diana analysis is ∆uY =
21.1 − 13.1 = 8.0 mm. The measured value from experiments is ∆uY = 19.5 −
10.0 = 9.5 mm.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
284 Long Term Behavior of RC Beam
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:08 c5defl0.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:08 c5defl.ps
Model: CREEP2 Model: CREEP2
Nodal TDTX...G TDTY Nodal TDTX...G TDTY
Max/Min on whole graph: Max/Min on whole graph:
Ymax = -.455 Ymax = -13.1
Ymin = -13.1 Ymin = -21.1
Xmax = 15.7 Xmax = 365
Xmin = 1 Xmin = .1E-5
Variation over loadcases Variation over loadcases
Node 15 Node 15
0 -13
0 2 4 6 8 10 12 14 16
-14
-2
N N
O O -15
D D
A -4 A
L L -16
T T
D -6 D -17
T T
X X
. . -18
. -8 .
. .
G G
-19
T -10 T
D D
T T -20
Y Y
-12
-21
-14 -22
LOAD 0 50 100 150 200 250 300 350 400
TIME
(a) until just after loading (b) over a full year
Figure 13.7: C15: deflection in time
13.4.2.2 Crack Pattern
To plot a crack pattern we select attribute EKNN which represents the normal
crack strain εcr
nn .
creep2.fvc
VIEW MESH
EYE ANGLE 0
EYE FRAME
RESULTS RANGE SURFACE ALL
RESULTS LOADCASE LC1 22
RESULTS GAUSSIAN EL.EKNN1 EKNN
PRESENT OPTIONS DISC MODULATE 5
PRESENT DISC FACTOR 0.5
RESULTS LOADCASE LC1 45
PRESENT DISC FACTOR 0.5
Crack strains are available in the integration points of the beam elements. In
iDiana these are called ‘Gaussian’ results. For beam elements Gaussian results
are presented for ‘surfaces’ of integration points. By default only the top surface
is selected. Here we select all surfaces via the RANGE and SURFACE options. With
the DISC option we display the crack pattern just after the application of the
load (step 22) and after one year (step 45) [Fig. 13.8].
13.4.2.3 Axial Stress
Also the axial stresses are displayed at two points in time: just after loading
and after 365 days.
creep2.fvc
DRAWING VIEWPORT SETUP TWO-HORIZ
RESULTS LOADCASE LC1 22
RESULTS ELEMENT EL.SXX.G SXX
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
13.4 Nonlinear Analysis 285
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:08 c5eknnb.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:08 c5eknne.ps
Model: CREEP2 Model: CREEP2
LC1: Load case 1 LC1: Load case 1
Step: 22 LOAD: 15.7 Step: 45 TIME: 365
Gauss EL.EKNN1 EKNN Gauss EL.EKNN1 EKNN
All surfaces All surfaces
Max = .17E-2 Max = .235E-2
Min = 0 Min = 0
Y Y
.136E-2 .188E-2
.102E-2 .141E-2
Z X .681E-3 Z X .939E-3
.341E-3 .47E-3
(a) just after loading (b) after 365 days
Figure 13.8: C15: crack pattern in beam
PRESENT SYMBOL
DRAWING VIEWPORT USE BLEFT
RESULTS LOADCASE LC1 22
RESULTS ELEMENT RE.SXX.G SXX
PRESENT SYMBOL
DRAWING VIEWPORT USE TLEFT
RESULTS LOADCASE LC1 45
RESULTS ELEMENT EL.SXX.G SXX
PRESENT SYMBOL
DRAWING VIEWPORT USE BLEFT
RESULTS LOADCASE LC1 45
RESULTS ELEMENT RE.SXX.G SXX
PRESENT SYMBOL
We make two viewports: the top one for the beam elements and the bottom
for the reinforcements. Result attribute SXX represents the axial stress σxx . We
respectively select steps 22 and 45 to display the stresses just after loading and
after one year [Fig. 13.9].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
286 Long Term Behavior of RC Beam
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:08 c5sxxb.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:56:08 c5sxxe.ps
Model: CREEP2 Model: CREEP2
LC1: Load case 1 LC1: Load case 1
Step: 22 LOAD: 15.7 Step: 45 TIME: 365
Element EL.SXX.G SXX Element EL.SXX.G SXX
Max = 3.07 Max = 3.66
Min = -13.6 Min = -9.01
Symbol factor = 1 Symbol factor = 1
All values All values
1.67 2.53
0 1.27
-1.67 -.666E-15
-3.34 -1.27
-5.01 -2.53
Y -6.68 Y -3.8
-8.35 -5.07
-10 -6.33
-11.7 -7.6
Z X -13.4 Z X -8.87
1 1
Model: CREEP2 Model: CREEP2
LC1: Load case 1 LC1: Load case 1
Step: 22 LOAD: 15.7 Step: 45 TIME: 365
Element RE.SXX.G SXX Element RE.SXX.G SXX
Max = 276 Max = 296
Min = -23.6 Min = -161
Symbol factor = 1 Symbol factor = 1
All values All values
269 274
239 229
209 183
180 137
150 91.4
Y 120 Y 45.7
89.8 -.142E-13
59.8 -45.7
29.9 -91.4
Z X 0 Z X -137
2 2
(a) just after loading (b) after 365 days
Figure 13.9: C15: axial stress in beam (top) and reinforcements (bottom)
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
Chapter 14
Concrete Viaduct
Name: Viaduct
Path: /Examples/ConcMas/Viaduct
Keywords: analys: nonlin phase physic. constr: suppor. elemen: bar
cq16m pstres reinfo taper. load: prestr reinfo time weight.
materi: concre creep elasti isotro kelvin shrink time viscoe. op-
tion: direct groups newton regula units. post: binary femvie.
result: cauchy displa stress total.
0.58 m
FE model
cast slab Y
X
I-beams
cross-beam Z
column 14 m
Figure 14.1: Composite viaduct
This example illustrates the nonlinear structural analysis of a viaduct composed
of prefabricated and cast concrete. Time dependent deformations and stresses
are predicted using phased analysis and models for shrinkage and creep. In the
construction of (partly) cast concrete structures like viaducts, often concrete of
different ages is used. In these cases, creep and shrinkage will cause redistri-
bution of strains and stresses in the composite. This example focuses on the
analysis of a viaduct with a span of 14 m and a thickness of 0.58 m [Fig. 14.1].
The self-bearing driving floor is constructed with prefab prestressed I-shaped
beams and a cast slab above and in between. The transverse floor ends are con-
nected to cross-beams which are in turn supported by columns. The dimensions
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
288 Concrete Viaduct
of the I-beam’s cross-section and reinforcement [Fig. 14.2] were supplied by the
Dutch Ministry of Public Works, see Beem [1].
Y 7000 ♥
X (a) reinforcement
250
400
6-9 6 80
5 90
4 5
4 120
580
500
170
3 3 30
2 2 90
1 1
8 250 160 250
400 (b) support (c) cast slab 660
8-9 (d) I-beam
400
Figure 14.2: I-beam and cast slab [mm]
The instantaneous response and creep effects due to prestress, dead weight
and shrinkage will be analyzed during two different phases in the structures
lifetime.
1. Transport and construction – The prestressed I-beams (with prestrained
cables) are analyzed for a period of three months after production. The
beams are transported from production to construction site during this
period, but the positions of the supports stay approximately the same
[Fig. 14.3a].
2. In use – The composite floor with cast slab, cross-beam and prestressed
I-beams is analyzed for a period of seventy years, starting immediately
after casting of the slab [Fig. 14.3b].
14.1 Finite Element Model
Since the structure and loading scheme are symmetrical, it is sufficient to model
only the left half of the structure, see the indicated area in Figure 14.1 on
the previous page. Though the interaction between slab and I-beam is three
dimensional, a restriction to two dimensional plane stress idealization with lon-
gitudinal cross-section is made for the sake of simplicity. For this example we
use 880 eight-node quadrilateral CQ16M plane stress elements with a default 2×2
Gauss integration scheme. Each phase is characterized by its own model and
constraints.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
14.1 Finite Element Model 289
7000 ♥
500
150 (a) Phase 1: ‘Transport & construction’
7250 ♥
580
400
(b) Phase 2: ‘In use’
400
Figure 14.3: Phases of analysis
Phase one. The element model consists of one I-beam of 35×12 = 420 ele-
ments in ABCD [Fig. 14.4a]. Five reinforcement cables are modeled with embed-
C
D
Y
A
B
X (a) elements & supports
X (b) reinforcement cables
Figure 14.4: Finite element model phase one (I-beam)
ded BAR reinforcements [Fig. 14.4b]. Constraints are dead weight, prestress of
the cables, one discrete vertical support at the inner side of the cross-beam and
suppressed horizontal displacement at the right side (symmetry).
Phase two. Elements are added to the model of phase one [Fig. 14.5a]: 3×4 =
12 elements for the cross-beam, 2×14 = 28 elements for the support stir-up and
35×12 = 420 elements for the cast slab. Points J and K are indicated for refer-
ence during input preparation and interpretation of analysis results. Reinforce-
ment bars are modeled with four embedded BAR reinforcements [Fig. 14.5b].
The cross-section area of each bar is equal to the total area of the actual bars in
Z-direction of a single beam, i.e., smeared reinforcement [Fig. 14.2c]. To model
the column, the vertical support is moved to the bottom of the cross-beam. Fur-
ther constraints are dead weight, initial stress in the I-beam and reinforcement
stress from the previous phase.
The element distribution in Y -direction was determined aiming at equal
dimensions, taking into account the various geometrical areas. In X-direction
the element distribution was determined mainly by the used maximum element
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
290 Concrete Viaduct
Y
K
J
X (a) elements & supports
X (b) reinforcement bars
Figure 14.5: Addition to finite element model for phase two (slab and cross-
beam)
height/width ratio of 1/5. The used transverse thickness (in Z-direction) is
equal to the width of the lower flange of one I-beam. Slab and I-beam contribute
to the total transverse thickness by separate elements with varying thicknesses
[Fig. 14.6]. The reinforcement location of straight parts is indicated with two-
(a) I-beam (b) cast slab
Figure 14.6: Thickness modeling
node sections, the location of curved parts with three-node sections. The default
2-point Gauss integration scheme is used for the generated reinforcement parts
in the elements.
14.1.1 Element Mesh and Reinforcement
The finite element meshes for beam, slab and cross-beam and their transverse
thicknesses are given on a previously made input data file in Diana batch
format. We will now discuss the various parts of the complete input data file
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
14.1 Finite Element Model 291
for phase 1: element mesh, reinforcements, geometric and material properties,
supports, and loading.
Element mesh nlph.dat
CONCRETE VIADUCT
’UNITS’
TIME DAY
LENGTH MM
MASS 7.46496E+12 0.00000E+00
’COORDINATES’
1 0.000000E+00 -1.000000E+02 0.000000E+00
2 6.250000E+01 -1.000000E+02 0.000000E+00
... lines skipped
4037 3.250000E+02 8.000000E+02 0.000000E+00
4038 2.500000E+02 8.200000E+02 0.000000E+00
’ELEMENTS’
CONNECT
1 CQ16M 1 2 3 10 17 16 15 8
2 CQ16M 3 4 5 12 19 18 17 10
... lines skipped
879 CQ16M 2467 2468 2469 2544 2619 2618 2617 2542
880 CQ16M 2469 2470 2471 2546 2621 2620 2619 2544
MATERI
/ 1-12 / 1
/ 13-432 / 2
/ 433-880 / 3
GEOMET
/ 1-82 783-880 / 8
/ 83-117 / 9
/ 118-257 / 10
/ 258-292 / 11
/ 293-327 / 12
/ 328-362 / 13
/ 363-432 / 14
/ 433-467 / 15
/ 468-607 / 16
/ 608-642 / 17
/ 643-677 / 18
/ 678-712 / 19
/ 713-782 / 10
’GROUPS’
ELEMEN
1 CROSSBEAM / 1-12 /
2 IBEAM / 13-432 /
3 SLAB / 433-880 /
NODES
4 SUPPORT1 / 63 /
5 MIDSPAN1 / 134 /
6 MIDSPAN2 / 134-418(71) 560 631 773-1270(71) 1412-1767(71)
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
292 Concrete Viaduct
1909-2122(71) 2396 2471 2546 2621 /
7 SUPPORT2 / 4 /
Table ’UNITS’ was added because it is intended to use days instead of the
default seconds in transient analysis. The above data models the finite element
mesh with CQ16M elements [Fig. 14.4a]. We show some detail plots of the I-
beam [Fig. 14.7] and cast slab [Fig. 14.8] with element and node numbers which
we will use for further reference in data preparation and analysis runs. The plots
for I-beam and slab show the overlapping elements: different element numbers
attached to the same node numbers. Note that we assemble some elements and
nodes in groups, this is for ease of reference in analysis commands.
iDIANA 0.0-04 : TNO Diana BV 02 AUG 2005 15:09:06 mesh2.ps iDIANA 0.0-04 : TNO Diana BV 02 AUG 2005 15:09:06 mesh3.ps
2052 2053 2054 2055 2056 2057 2058 2059 2060 2061 2110 2111 2112 2113 2114 2115 2116 2117 2118 2119 2120 2121 2122
1981 398 1983 399 1985 400 1987 401 1989 402 2039 427 2041 428 2043 429 2045 430 2047 431 2049 432 2051
1910 1911 1912 1913 1914 1915 1916 1917 1918 1919 1968 1969 1970 1971 1972 1973 1974 1975 1976 1977 1978 1979 1980
1839 363 1841 364 1843 365 1845 366 1847 367 1897 392 1899 393 1901 394 1903 395 1905 396 1907 397 1909
1697 1698 1699 1700 1701 1702 1703 1704 1705 1706 1755 1756 1757 1758 1759 1760 1761 1762 1763 1764 1765 1766 1767
1626 328 1628 329 1630 330 1632 331 1634 332 1684 357 1686 358 1688 359 1690 360 1692 361 1694 362 1696
1555 1556 1557 1558 1559 1560 1561 1562 1563 1564 1613 1614 1615 1616 1617 1618 1619 1620 1621 1622 1623 1624 1625
1484 293 1486 294 1488 295 1490 296 1492 297 1542 322 1544 323 1546 324 1548 325 1550 326 1552 327 1554
1413 1414 1415 1416 1417 1418 1419 1420 1421 1422 1471 1472 1473 1474 1475 1476 1477 1478 1479 1480 1481 1482 1483
1342 258 1344 259 1346 260 1348 261 1350 262 1400 287 1402 288 1404 289 1406 290 1408 291 1410 292 1412
1200 1201 1202 1203 1204 1205 1206 1207 1208 1209 1258 1259 1260 1261 1262 1263 1264 1265 1266 1267 1268 1269 1270
1129 223 1131 224 1133 225 1135 226 1137 227 1187 252 1189 253 1191 254 1193 255 1195 256 1197 257 1199
1058 1059 1060 1061 1062 1063 1064 1065 1066 1067 1116 1117 1118 1119 1120 1121 1122 1123 1124 1125 1126 1127 1128
987 188 989 189 991 190 993 191 995 192 1045 217 1047 218 1049 219 1051 220 1053 221 1055 222 1057
916 917 918 919 920 921 922 923 924 925 974 975 976 977 978 979 980 981 982 983 984 985 986
845 153 847 154 849 155 851 156 853 157 903 182 905 183 907 184 909 185 911 186 913 187 915
774 775 776 777 778 779 780 781 782 783 832 833 834 835 836 837 838 839 840 841 842 843 844
703 118 705 119 707 120 709 121 711 122 761 147 763 148 765 149 767 150 769 151 771 152 773
561 562 563 564 565 566 567 568 569 570 619 620 621 622 623 624 625 626 627 628 629 630 631
490 83 492 84 494 85 496 86 498 87 548 112 550 113 552 114 554 115 556 116 558 117 560
348 349 350 351 352 353 354 355 356 357 406 407 408 409 410 411 412 413 414 415 416 417 418
277 48 279 49 281 50 283 51 285 52 335 77 337 78 339 79 341 80 343 81 345 82 347
206 207 208 209 210 211 212 213 214 215 264 265 266 267 268 269 270 271 272 273 274 275 276
135 13 137 14 139 15 141 16 143 17 193 42 195 43 197 44 199 45 201 46 203 47 205
57 58 59 60 61 62 63 67 68 69 70 71 72 73 122 123 124 125 126 127 128 129 130 131 132 133 134
50 10 52 11 54 12 56
43 44 45 46 47 48 49
36 7 38 8 40 9 42
29 30 31 32 33 34 35
22 4 24 5 26 6 28
15 16 17 18 19 20 21
8 1 10 2 12 3 14
1 2 3 4 5 6 7
I-beam and cross-beam near support I-beam near mid-span
Figure 14.7: Plots of beam details
iDIANA 0.0-04 : TNO Diana BV 02 AUG 2005 15:09:06 mesh4.ps iDIANA 0.0-04 : TNO Diana BV 02 AUG 2005 15:09:06 mesh5.ps
2547 2548 2549 2550 2551 2552 2553 2554 2555 2556 2557 2558 2559 2560 2609 2610 2611 2612 2613 2614 2615 2616 2617 2618 2619 2620 2621
2472 844 2474 845 2476 846 2478 847 2480 848 2482 849 2484 850 2534 875 2536 876 2538 877 2540 878 2542 879 2544 880 2546
2397 2398 2399 2400 2401 2402 2403 2404 2405 2406 2407 2408 2409 2410 2459 2460 2461 2462 2463 2464 2465 2466 2467 2468 2469 2470 2471
2322 807 2324 808 2326 809 2328 810 2330 811 2332 812 2334 813 2384 838 2386 839 2388 840 2390 841 2392 842 2394 843 2396
2243 2244 2245 2246 2052 2053 2054 2055 2056 2057 2058 2059 2060 2061 2110 2111 2112 2113 2114 2115 2116 2117 2118 2119 2120 2121 2122
2238 805 2240 806 1981 748 1983 749 1985 750 1987 751 1989 752 2039 777 2041 778 2043 779 2045 780 2047 781 2049 782 2051
2233 2234 2235 2236 1910 1911 1912 1913 1914 1915 1916 1917 1918 1919 1968 1969 1970 1971 1972 1973 1974 1975 1976 1977 1978 1979 1980
2228 803 2230 804 1839 713 1841 714 1843 715 1845 716 1847 717 1897 742 1899 743 1901 744 1903 745 1905 746 1907 747 1909
2223 2224 2225 2226 1697 1698 1699 1700 1701 1702 1703 1704 1705 1706 1755 1756 1757 1758 1759 1760 1761 1762 1763 1764 1765 1766 1767
2218 801 2220 802 1626 678 1628 679 1630 680 1632 681 1634 682 1684 707 1686 708 1688 709 1690 710 1692 711 1694 712 1696
2213 2214 2215 2216 1555 1556 1557 1558 1559 1560 1561 1562 1563 1564 1613 1614 1615 1616 1617 1618 1619 1620 1621 1622 1623 1624 1625
2208 799 2210 800 1484 643 1486 644 1488 645 1490 646 1492 647 1542 672 1544 673 1546 674 1548 675 1550 676 1552 677 1554
2203 2204 2205 2206 1413 1414 1415 1416 1417 1418 1419 1420 1421 1422 1471 1472 1473 1474 1475 1476 1477 1478 1479 1480 1481 1482 1483
2198 797 2200 798 1342 608 1344 609 1346 610 1348 611 1350 612 1400 637 1402 638 1404 639 1406 640 1408 641 1410 642 1412
2193 2194 2195 2196 1200 1201 1202 1203 1204 1205 1206 1207 1208 1209 1258 1259 1260 1261 1262 1263 1264 1265 1266 1267 1268 1269 1270
2188 795 2190 796 1129 573 1131 574 1133 575 1135 576 1137 577 1187 602 1189 603 1191 604 1193 605 1195 606 1197 607 1199
2183 2184 2185 2186 1058 1059 1060 1061 1062 1063 1064 1065 1066 1067 1116 1117 1118 1119 1120 1121 1122 1123 1124 1125 1126 1127 1128
2178 793 2180 794 987 538 989 539 991 540 993 541 995 542 1045 567 1047 568 1049 569 1051 570 1053 571 1055 572 1057
2173 2174 2175 2176 916 917 918 919 920 921 922 923 924 925 974 975 976 977 978 979 980 981 982 983 984 985 986
2168 791 2170 792 845 503 847 504 849 505 851 506 853 507 903 532 905 533 907 534 909 535 911 536 913 537 915
2163 2164 2165 2166 774 775 776 777 778 779 780 781 782 783 832 833 834 835 836 837 838 839 840 841 842 843 844
2158 789 2160 790 703 468 705 469 707 470 709 471 711 472 761 497 763 498 765 499 767 500 769 501 771 502 773
2153 2154 2155 2156 561 562 563 564 565 566 567 568 569 570 619 620 621 622 623 624 625 626 627 628 629 630 631
2148 787 2150 788 490 433 492 434 494 435 496 436 498 437 548 462 550 463 552 464 554 465 556 466 558 467 560
2143 2144 2145 2146 348 349 350 351 352 353 354 355 356 357 406 407 408 409 410 411 412 413 414 415 416 417 418
2138 785 2140 786 277
2133 2134 2135 2136 206
2128 783 2130 784 135
57 58 59 60 61
near support near mid-span
Figure 14.8: Plots of cast slab details
Reinforcements nlph.dat
’REINFORCEMENTS’
LOCATI
1 BAR
LINE 4001 4002
ELEMEN 13-432 /
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
14.1 Finite Element Model 293
2 BAR
LINE 4003 4004
ELEMEN 13-432 /
3 BAR
LINE 4005 4006
ELEMEN 13-432 /
4 BAR
LINE 4007 4008
ELEMEN 13-432 /
LINE 4008 4016 4016
PARABO 0. 1. 0.
ELEMEN 13-432 /
LINE 4016 4018
ELEMEN 13-432 /
5 BAR
LINE 4011 4012
ELEMEN 13-432 /
LINE 4012 4020 4020
PARABO 0. 1. 0.
ELEMEN 13-432 /
LINE 4020 4022
ELEMEN 13-432 /
6 BAR
LINE 4025 4026
ELEMEN 433-880 /
8 BAR
LINE 4029 4030
ELEMEN 1-12 /
LINE 4030 4031 4032
ELEMEN 1-12 /
LINE 4032 4033
ELEMEN 1-12 /
LINE 4033 4034 4035
ELEMEN 1-12 /
LINE 4035 4036
ELEMEN 1-12 /
9 BAR
LINE 4029 4030
ELEMEN 1-12 /
LINE 4030 4031 4032
ELEMEN 1-12 /
LINE 4032 4037
ELEMEN 1-432 /
LINE 4037 4038 4025
ELEMEN 433-880 /
MATERI
/ 1-5 8-9 / 4
/ 6 / 5
GEOMET
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
294 Concrete Viaduct
/ 1 / 1
/ 2 4-5 / 2
/ 3 / 3
/ 6 / 4
/ 8 / 6
/ 9 / 7
Bends in reinforcements 4 and 5 are specified with parabolic sections with co-
inciding end- and midpoints, for instance point 4016 in bar 4. This is to assure
that the subsequent LINE section is tangential to the parabolic section. The
above data will add the reinforcements to the finite element mesh [Fig. 14.4b].
Geometric properties nlph.dat
’GEOMET’
1 CROSSE 384.845
2 CROSSE 153.938
3 CROSSE 76.97
4 CROSSE 2945.
6 CROSSE 804.
7 CROSSE 603.
8 THICK 660.
9 THICK 660. 660. 660. 410. 160. 160. 160. 410.
10 THICK 160.
11 THICK 160. 160. 160. 200. 240. 240. 240. 200.
12 THICK 240. 240. 240. 280. 320. 320. 320. 280.
13 THICK 320. 320. 320. 360. 400. 400. 400. 360.
14 THICK 400.
15 THICK 1.E-6 1.E-6 1.E-6 250. 500. 500. 500. 250.
16 THICK 500.
17 THICK 500. 500. 500. 460. 420. 420. 420. 460.
18 THICK 420. 420. 420. 380. 340. 340. 340. 380.
19 THICK 340. 340. 340. 300. 260. 260. 260. 300.
20 THICK 260.
The CROSSE items specify the various cross-sectional areas of the reinforcement
bars. The THICK items specify the thickness of the quadrilateral plane stress
elements [Fig. 14.6 p. 290]. Note that some elements have uniform thickness and
others are tapered.
14.1.2 Material Definition
The material characterizations for creep and shrinkage are based on the CEB-
FIP Model Code 1990 [2]. Diana transforms the user input for CEB-FIP models
to the parameters for the models used for the numerical analysis.
14.1.2.1 Shrinkage
Diana models shrinkage straightforwardly as age-dependent initial strain. The
CEB-FIP shrinkage model requires no additional input data, compared to the
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
14.1 Finite Element Model 295
creep model [Vol. Material Library].
14.1.2.2 Creep, Relaxation and Elasticity
The viscoelastic Kelvin Chain model [Vol. Material Library] is used to predict
age dependent creep, relaxation and elastic deformation for arbitrary loading.
Diana derives the parameters for the aging Kelvin Chain model by fitting
and a creep curve from the CEB-FIP creep model. Input data for parameter
determination are: the initial age of the concrete at the start of analysis t0 ,
Young’s modulus of elasticity at the age of twenty-eight days Et=28 , the mean
compressive strength fcm , the notational size h0 , the cement class, the relative
humidity of the ambient environment RH and the ambient temperature Tenv .
Table 14.1 shows the material data as used for the analysis, either as input
or as default values. A NOBOND specification has been added to the material
Table 14.1: Material parameters
t
en
)
55
am
m
)
(C
20
e
be
rc
(C
am
fo
s-
t
pu
n
s
ab
be
ro
ei
In
Sl
R
C
I-
Young’s modulus Et28 YOUNG 39750 30000 37600 210000 N/mm2
Poisson’s ratio ν POISON 0.3 0.3 0.3 -
Mass density ρ DENSIT 2.5×10−6 2.5×10−6 2.5×10−6 - kg/mm3
Notational size h0 H 580 580 - - mm
Mean comp. stren. fcm FCM 63 28 - - N/mm2
Relative humidity RH RH 80% 80% - -
Ambient temp. Tenv TEMPER 20 20 - - °C
Cement type CEMTYP nr nr - -
Initial age t0 AGING 1.0 0.01 - - day
properties of the slab reinforcement to enforce zero initial reinforcement stress
immediately after casting. The notational size h0 is calculated from the cross-
section of the member Ac and the perimeter u which is in contact with the
atmosphere.
2Ac
h0 =
u
For both slab and I-beam it is assumed that the notational size equals the com-
posed thickness of beam and slab. The initial age of the beam’s concrete after
AGING equals the moment of loading by prestress. The initial age of the slab’s
concrete after AGING is chosen such that just little initial stiffness is available.
In this example, the elastic and viscous material properties are strongly age
dependent.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
296 Concrete Viaduct
The I-beam is loaded by prestress, continuous shrinkage and dead weight
after one day of curing and by the additional slab dead weight after 89
days. The stiffness of the I-beam at the age of 89 days is about 80 %
larger than at the initial age of one day.
The slab is loaded by dead weight and continuous shrinkage, almost im-
mediately after casting. Therefore the initial stiffness is close to zero.
Loading at different ages will result in different creep curves, because of the age-
dependent stiffness and viscous properties. If no unique loading age is available,
age dependent Kelvin Chains can fit these different creep curves. To show this
we have performed two small tests at different loading ages, see the appendix
of this chapter [§ 14.3 p. 308].
Material properties nlph.dat
’MATERI’
: concrete cross-beam
1 YOUNG 3.76E+4
POISON 0.3
: density 2.5E-6 kg/mm^3
DENSIT 3.34898E-19
: concrete I-beam (grade C55)
2 YOUN28 3.975E+4
POISON 0.3
DENSIT 3.34898E-19
CREEPN MC1990
SHRINN MC1990
H 580.
FCM28 63.
AGING 1.
: concrete cast slab (grade C20)
3 YOUN28 3.0E+4
POISON 0.3
DENSIT 3.34898E-19
CREEPN MC1990
SHRINN MC1990
H 580.
FCM28 28.
AGING 0.01
: reinforcement steel FeP1860 and FeB500 in I-beams with initial bond
4 YOUNG 2.1E+5
POISON 0.3
: reinforcement steel FeB500 in slab without initial bond
5
YOUNG 2.1E+5
POISON 0.3
NOBOND
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
14.2 Phased Analysis 297
14.1.3 Boundary Conditions
The boundary conditions for this model involve the supports, symmetry condi-
tions and the loading.
Supports and symmetry conditions nlph.dat
’DIRECTIONS’
1 1. 0. 0.
2 0. 1. 0.
3 0. 0. 1.
’SUPPOR’
/ SUPPORT1 / TR 2
/ MIDSPAN2 / TR 1
We support the bottom-left node vertically, uY = 0. Due to symmetry the
vertical line through the mid-span can not have a horizontal displacement, uX =
0.
Loading nlph.dat
’LOADS’
CASE 1
WEIGHT
2 -7.32313E+13
CASE 2
REINFO
/ 1-5 /
PRESTR 1006.
’TIMELO’
LOAD 1
TIMES 0. 1.E+5 /
FACTOR 1.0 1.0 /
’END’
The model is completed with input of dead weight (load case 1) and reinforce-
ment prestress (load case 2). In table ’TIMELO’ we specify a time–load diagram
for a constant dead weight load.
14.2 Phased Analysis
We will perform a nonlinear analysis with two phases in one single analysis job.
However, the commands and input data will be presented separately.
14.2.1 Phase One
The model for phase one contains only the I-beam elements. This leads to the
following commands, which also apply the initial load.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
298 Concrete Viaduct
Initial loading nlph.dcf
*PHASE
BEGIN ACTIVE
ELEMEN IBEAM
REINFO 1-5
END ACTIVE
*NONLIN
TYPE PHYSIC
BEGIN OUTPUT FEMVIEW BINARY FILE="PHASE1"
BEGIN SELECT
ELEMEN IBEAM
REINFO NONE
END SELECT
DISPLA
DISPLA PHASE
STRESS GLOBAL NODES
END OUTPUT
BEGIN EXECUT
BEGIN START
BEGIN INITIA
BEGIN STRESS
BEGIN INPUT
LOAD=2
FACTOR=1
END INPUT
END STRESS
END INITIA
STEPS OFF
END START
END EXECUT
The *PHASE commands select the I-beam as the active part of the model. This
selection is necessary to skip the elements of the slab and cross-beam, which
become active in phase two. Note that selection of elements includes selection of
the reinforcements in those elements. As the first part in the nonlinear analysis,
the I-beam is loaded with the initial reinforcement stress from load set 2 and
initial dead weight from load set 1.
Transient analysis nlph.dcf
BEGIN EXECUT
TIME STEPS EXPLIC SIZES 1.0E-10
ITERAT CONVER FORCE
END EXECUT
BEGIN EXECUT
BEGIN TIME
BEGIN STEPS
BEGIN EXPLIC
SIZES 0.0001 0.0003 0.0006 0.001 0.003 0.005\
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
14.2 Phased Analysis 299
0.01(4) 0.025(4) 0.05(5) 0.1(6) 0.25(4)\
0.5(4) 1.(6) 2.5(4) 5.(4) 9. 10.(4)
END EXPLIC
END STEPS
END TIME
ITERAT CONVER FORCE
END EXECUT
The second part of the nonlinear analysis of phase one is the calculation of creep
and shrinkage for a period of 89 days. The time stepping scheme is composed
by incrementing the step size approximately logarithmic. Step sizes are related
to the range of retardation times of the various Kelvin units. Note that we
perform a real-life analysis to get accurate results.
14.2.2 Phase Two
The model for phase two contains the I-beam elements, the cross-beam elements
and the slab elements [Fig. 14.5 p. 290]. To complete the model, we must replace
the I-beam support from phase one by a cross-beam support. Therefore we apply
the following input data file.
ph2.dat
CONCRETE VIADUCT
’SUPPOR’
/ SUPPORT2 / TR 2
/ MIDSPAN2 / TR 1
’TIMELO’
LOAD 1
TIMES 89.0 100000.0 /
FACTOR 1.0 1.0 /
’END’
The model for phase two is defined by addition of the slab and cross-beam
elements to the selection of active elements in Module phase. This leads to the
following commands.
Load and stress nlph.dcf
*INPUT
READ FILE="ph2.dat" TABLE SUPPOR TIMELO
*PHASE
BEGIN ACTIVE
ELEMEN IBEAM CROSSBEAM SLAB
REINFO 1-5 6 8 9
END ACTIVE
*NONLIN
TYPE PHYSIC
BEGIN OUTPUT FEMVIEW BINARY FILE="PHASE2"
BEGIN SELECT
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
300 Concrete Viaduct
ELEMEN IBEAM
REINFO NONE
END SELECT
DISPLA
DISPLA PHASE
STRESS GLOBAL NODES
END OUTPUT
BEGIN EXECUT
BEGIN START
TIME=89
INITIA STRESS PHASE
STEPS OFF
END START
END EXECUT
In the first part the dead weight load is applied, including the additional slab
weight. For the elements and reinforcements of the I-beam the initial stresses
and deformations are automatically equal to the stresses at the end of the pre-
vious phase.
The additional dead weight load will cause deformation and stress incre-
ments, Diana superposes these to the existing deformation and stress at the
end of phase one. The calculated instantaneous displacement increment asked
by DISPLA PHASE is found from the tabulated output.
As stated before, the stresses in the specified slab reinforcements are enforced
zero by using the NOBOND input option. This is to prevent their contribution to
the stiffness of deforming slab elements in this stage. Another way to achieve this
would have been to use a separate phase without slab reinforcement for the static
analysis and a separate phase with input of the additional slab reinforcement
for transient analysis.
Transient analysis nlph.dcf
BEGIN EXECUT
TIME STEPS EXPLIC SIZES 1.0E-10
ITERAT CONVER FORCE
END EXECUT
BEGIN EXECUT
BEGIN TIME
BEGIN STEPS
BEGIN EXPLIC
SIZES 0.0001 0.0003 0.0006 0.001 0.003 0.005\
0.01(4) 0.025(4) 0.05(5) 0.1(6) 0.25(4) 0.5(4) 1.(6)\
2.5(4) 5.(4) 10.(2) 20.(2) 50.(2) 100. 200.(2) 300.\
500.(2) 1000.(5) 3000.
END EXPLIC
END STEPS
END TIME
ITERAT CONVER FORCE
PHYSIC BOND REINFO 6
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
14.2 Phased Analysis 301
END EXECUT
*END
The second part of the nonlinear analysis is the calculation of creep and shrink-
age for a period of 10000 days (≈ 27.5 years). As in phase one, the time stepping
scheme is composed by incrementing the step size approximately logarithmic and
related to the range of retardation times of the Kelvin units. The bond between
slab and reinforcement is switched on with the PHYSIC BOND command.
The stresses and strains in the slab are a result of complex interactions. The
shrinkage of the slab is partly suppressed by the reinforcement and the I-beam,
causing additional tension in the slab and pressure in the I-beam. Therefore the
distributions of the normal stress along the mid-span for slab and I-beam are
no longer linear. On the other hand, the creep of the I-beam due to the dead
weight of the slab will cause a redistribution of stress from the I-beam to the
slab.
14.2.3 Analysis and Results
Now we may perform the nonlinear analysis with two phases in one single run.
diana nlph
After the analysis has been terminated we may asses the results. We will produce
and discuss the analysis results for the two phases separately.
14.2.3.1 Phase One
Output of the first phase for results assessment with iDiana is on a database
PHASE1. We now enter the Results environment for the first phase.
phase1.fvc
FEMVIEW PHASE1
UTILITY TABULATE LOADCASES
The tabulation of the load cases shows that there are load cases named LC1 for
load case one with indices for each step of the first phase.
nlph1lc.tb
;
; Model: PHASE1
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; MODEL STATIC "Model Properties"
; Element : THICKNES* REINBAR*
;
; LC1 1 TIME = .1E-9 "Load case 1"
; Nodal : TDTX...G PDTX...G
; Element : EL.SXX.G
;
; LC1 2 TIME = .1E-3 "Load case 1"
; Nodal : TDTX...G PDTX...G
; Element : EL.SXX.G
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
302 Concrete Viaduct
;
; LC1 3 TIME = .4E-3 "Load case 1"
; Nodal : TDTX...G PDTX...G
; Element : EL.SXX.G
;
; LC1 4 TIME = .1E-2 "Load case 1"
In the iDiana Results environment we will produce some graphs to represent
the stresses in the beam.
Just after loading phase1.fvc
RESULTS LOADCASE LC1 1
PRESENT OPTIONS GRAPH LINES OFF
RESULTS ELEMENT EL.SXX.G SXX
PRESENT GRAPH LINE NODES LIST 2052 TO 2122
PRESENT GRAPH LINE NODES THROUGH 134 2122
To plot the resulting initial stress distributions in some cross-sections we select
the first step: LC1 1. Here we want to produce graphs for the variation of the
stress along a line in the model. The sequence of the points (nodes) on such a
line may be arbitrary. Therefore the drawing of graphs with lines is not quite
appropriate: we switch that off. Then we select the horizontal stress σXX in the
beam via the SXX attribute. Nodes 2052–2122 represent the upper side DC of
the beam [Fig. 14.7 p. 292]. We draw a graph, with symbols only, with the line
through these nodes as horizontal axis, and the selected stress σXX as vertical
axis [Fig. 14.9a]. The second graph takes the line through nodes 134 and 2122 as
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:29 p1startbsup.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:29 p1startbsmi.ps
Model: PHASE1 Model: PHASE1
LC1: Load case 1 LC1: Load case 1
Step: 1 TIME: .1E-9 Step: 1 TIME: .1E-9
Element EL.SXX.G SXX Element EL.SXX.G SXX
Max/Min on whole graph: Max/Min on whole graph:
Ymax = .193 Ymax = -2.73
Ymin = -9.18 Ymin = -7.2
Xmax = .7E4 Xmax = 500
Xmin = 0 Xmin = 0
1 Variation along a line -2.5 Variation along a line
0 -3
0 1 2 3 4 5 6 7 8
E -1 *1E3 E
L L -3.5
E E
M -2 M
E E -4
N N
T -3 T
-4.5
E -4 E
L L -5
. .
S -5 S
X X -5.5
X -6 X
. .
G G -6
-7
S S
X -8 X -6.5
X X
-9 -7
-10 -7.5
DISTANCE 0 100 200 300 400 500 600
DISTANCE
(a) upper side DC (b) mid-span BC
Figure 14.9: Phase one, stress in I-beam just after loading
the horizontal axis, which represents the mid-span cross-section BC [Fig. 14.9b].
The local stress wiggles at the left side of the plots along the beam axes are
caused by the sudden drop of reinforcement stress at the ends of the prestrained
cables.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
14.2 Phased Analysis 303
After 89 days phase1.fvc
RESULTS LOADCASE LC1 53
RESULTS ELEMENT EL.SXX.G SXX
PRESENT GRAPH LINE NODES LIST 2052 TO 2122
PRESENT GRAPH LINE NODES THROUGH 134 2122
To get graphs of the results after a period of 89 days of creep and shrinkage we
select the last step of phase one: LC1 53. We draw graphs for σXX along the
same lines through the model [Fig. 14.10].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:29 p1endbsup.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:29 p1endbsmi.ps
Model: PHASE1 Model: PHASE1
LC1: Load case 1 LC1: Load case 1
Step: 53 TIME: 89 Step: 53 TIME: 89
Element EL.SXX.G SXX Element EL.SXX.G SXX
Max/Min on whole graph: Max/Min on whole graph:
Ymax = .158 Ymax = -2.83
Ymin = -8.83 Ymin = -6.77
Xmax = .7E4 Xmax = 500
Xmin = 0 Xmin = 0
1 Variation along a line -2.5 Variation along a line
0 -3
0 1 2 3 4 5 6 7 8
E E
L -1 *1E3 L -3.5
E E
M M
E -2 E
N N -4
T T
-3
E E -4.5
L -4 L
. .
S S -5
X -5 X
X X
. . -5.5
G -6 G
S S -6
X -7 X
X X
-8 -6.5
-9 -7
DISTANCE 0 100 200 300 400 500 600
DISTANCE
(a) upper side DC (b) mid-span BC
Figure 14.10: Phase one, stress in I-beam after 89 days
The results of the first phase may also be used to make history plots of
displacement and stress at distinct points.
Graph options phase1.fvc
RESULTS LOADCASE LC1
PRESENT OPTIONS GRAPH AXES XLOG
PRESENT OPTIONS GRAPH LINES NORMAL
PRESENT OPTIONS GRAPH POINTS SYMBOLS OFF
First we select all load cases for history plots of the first phase of the analysis.
With the XLOG option we ask for a logarithmic scale of the horizontal (time)
axis, which is appropriate in this case because of the large variation in time step
size. We ask iDiana to draw graphs with lines of normal thickness and switch
off the display of symbols for points on the graph.
Stress in I-beam phase1.fvc
RESULTS ELEMENT EL.SXX.G SXX
PRESENT GRAPH ELEMENT 47
PRESENT GRAPH ELEMENT 432
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
304 Concrete Viaduct
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:29 p1strB.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:29 p1strC.ps
Model: PHASE1 Model: PHASE1
Element EL.SXX.G SXX Element EL.SXX.G SXX
Max/Min on whole graph: Max/Min on whole graph:
Ymax = -6.6 Ymin = -7 Ymax = -2.93
Xmax = 89 Xmin = .1E-9 Ymin = -3.01
Variation over loadcases Xmax = 89
Element 47 Mean Xmin = .1E-9
Variation over loadcases
Element 432 Mean
-6.55 -2.92
-6.6 -2.93
E E
L -6.65 L -2.94
E E
M M
E -6.7 E
N N -2.95
T T
-6.75
E E -2.96
L -6.8 L
. .
S S -2.97
X -6.85 X
X X
. . -2.98
G -6.9 G
S S -2.99
X -6.95 X
X X
-7 -3
-7.05 -3.01
.1E-9 .464E-8 .215E-6 .1E-4 .464E-3 .215E-1 1 46.4 .215E4 .1E-9 .464E-8 .215E-6 .1E-4 .464E-3 .215E-1 1 46.4 .215E4
TIME Log Scale TIME Log Scale
(a) at point B (b) at point C
Figure 14.11: History plot of stress in I-beam
For the stress, we select locations near the bottom and top of the mid-span
[Fig. 14.4a]: element 47 for point B and element 432 for point C [Fig. 14.11]. For
elements, there are stress values in each node. However, a history plot requires
only one value per time point, therefore iDiana will automatically calculate the
average value for the selected elements.
Vertical displacement phase1.fvc
RESULTS NODAL TDTX...G TDTY
PRESENT GRAPH NODE 134
The history plot of the displacement shows the upheaval by prestressing in phase
one in the first 89 days [Fig. 14.12].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:29 p1disB.ps
Model: PHASE1
Nodal TDTX...G TDTY
Max/Min on whole graph:
Ymax = 14.6 Ymin = 10
Xmax = 89 Xmin = .1E-9
Variation over loadcases
Node 134
15
14.5
N 14
O
D
A 13.5
L
T 13
D
T
X 12.5
.
.
. 12
G
T 11.5
D
T 11
Y
10.5
10
.1E-9 .464E-8 .215E-6 .1E-4 .464E-3 .215E-1 1 46.4 .215E4
TIME Log Scale
Figure 14.12: History plot of displacement of point B
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
14.2 Phased Analysis 305
14.2.3.2 Phase Two
Output of the second phase for results assessment with iDiana is on a database
PHASE2. We now enter the Results environment for the first phase.
phase2.fvc
FEMVIEW PHASE2
UTILITY TABULATE LOADCASES
The tabulation of the load cases shows that there are load cases named LC1 for
load case one with indices for each step of the second phase.
nlph2lc.tb
;
; Model: PHASE2
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; MODEL STATIC "Model Properties"
; Element : THICKNES* REINBAR*
;
; LC1 1 TIME = 89 "Load case 1"
; Nodal : TDTX...G PDTX...G
; Element : EL.SXX.G
;
; LC1 2 TIME = 89 "Load case 1"
; Nodal : TDTX...G PDTX...G
; Element : EL.SXX.G
;
; LC1 3 TIME = 89 "Load case 1"
; Nodal : TDTX...G PDTX...G
; Element : EL.SXX.G
;
; LC1 4 TIME = 89 "Load case 1"
We will make graphs of the horizontal stress in the I-beam at two stages:
just after the slab has been casted, and after 10000 days which is the end time
of the analysis.
Just after loading phase2.fvc
RESULTS LOADCASE LC1 1
RESULTS ELEMENT EL.SXX.G SXX
PRESENT GRAPH LINE NODES LIST 2052 TO 2122
PRESENT GRAPH LINE NODES THROUGH 134 2122
We select step 1 of phase two: LC1 1, i.e., just after the additional loading with
the slab’s dead weight. The stresses in the I-beam [Fig. 14.13] show an opposite
linear pressure distribution at the mid-span, with pressures increasing in the
upper beam fibers and decreasing in the lower fibers.
After 10000 days phase2.fvc
RESULTS LOADCASE LC1 66
RESULTS ELEMENT EL.SXX.G SXX
PRESENT GRAPH LINE NODES LIST 2052 TO 2122
PRESENT GRAPH LINE NODES THROUGH 134 2122
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
306 Concrete Viaduct
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:31 p2startbsup.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:31 p2startbsmi.ps
Model: PHASE2 Model: PHASE2
LC1: Load case 1 LC1: Load case 1
Step: 1 TIME: 89 Step: 1 TIME: 89
Element EL.SXX.G SXX Element EL.SXX.G SXX
Max/Min on whole graph: Max/Min on whole graph:
Ymax = .222 Ymax = -.852
Ymin = -10.3 Ymin = -10.3
Xmax = .7E4 Xmax = 500
Xmin = 0 Xmin = 0
2 Variation along a line 0 Variation along a line
0 100 200 300 400 500 600
-1
0
E 0 1 2 3 4 5 6 7 8 E -2
L L
E *1E3 E
M -2 M -3
E E
N N
T T -4
-4
E E -5
L L
. .
S -6 S -6
X X
X X -7
. .
G G
-8 -8
S S
X X -9
X X
-10
-10
-12 -11
DISTANCE DISTANCE
(a) upper side DC (b) mid-span BC
Figure 14.13: Phase two, stress in I-beam just after loading
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:32 p2endbsup.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:32 p2endbsmi.ps
Model: PHASE2 Model: PHASE2
LC1: Load case 1 LC1: Load case 1
Step: 66 TIME: .101E5 Step: 66 TIME: .101E5
Element EL.SXX.G SXX Element EL.SXX.G SXX
Max/Min on whole graph: Max/Min on whole graph:
Ymax = -.793 Ymax = -1.31
Ymin = -7.08 Ymin = -7.08
Xmax = .7E4 Xmax = 500
Xmin = 0 Xmin = 0
0 Variation along a line -1 Variation along a line
0 1 2 3 4 5 6 7 8
*1E3
-1
-2
E E
L L
E -2 E
M M -3
E E
N N
T -3 T
-4
E E
L -4 L
. .
S S -5
X X
X -5 X
. .
G G
-6
S -6 S
X X
X X
-7
-7
-8 -8
DISTANCE 0 100 200 300 400 500 600
DISTANCE
(a) upper side DC (b) mid-span BC
Figure 14.14: Phase two, stress in I-beam after 10000 days
For the results after 10000 days we select the last step of phase two: LC1 66. The
other commands display the graphs for the stresses in the I-beam [Fig. 14.14].
The results of the second phase may also be used to make history plots of
displacement and stress at distinct points.
Graph options phase2.fvc
RESULTS LOADCASE LC1
PRESENT OPTIONS GRAPH AXES XLOG
PRESENT OPTIONS GRAPH LINES NORMAL
PRESENT OPTIONS GRAPH POINTS SYMBOLS OFF
First we select all load cases for history plots of the second phase of the analysis.
With the XLOG option we ask for a logarithmic scale of the horizontal (time)
axis, which is appropriate in this case because of the large variation in time step
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
14.2 Phased Analysis 307
size. We ask iDiana to draw graphs with lines of normal thickness and switch
off the display of symbols for points on the graph.
Stress in I-beam phase2.fvc
RESULTS ELEMENT EL.SXX.G SXX
PRESENT GRAPH ELEMENT 47
PRESENT GRAPH ELEMENT 432
For the stress, we select locations near the bottom and top of the mid-span
[Fig. 14.4a]: element 47 for point B and element 432 for point C [Fig. 14.15]. For
elements, there are stress values in each node. However, a history plot requires
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:32 p2strB.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:32 p2strC.ps
Model: PHASE2 Model: PHASE2
Element EL.SXX.G SXX Element EL.SXX.G SXX
Max/Min on whole graph: Max/Min on whole graph:
Ymax = -1.28 Ymax = -6.78
Ymin = -1.65 Ymin = -9.87
Xmax = .101E5 Xmax = .101E5
Xmin = 89 Xmin = 89
Variation over loadcases Variation over loadcases
Element 47 Mean Element 432 Mean
-1.25 -6.5
-1.3
-7
E E
L L
E -1.35 E
M M -7.5
E E
N N
T -1.4 T
-8
E E
L -1.45 L
. .
S S -8.5
X X
X -1.5 X
. .
G G
-9
S -1.55 S
X X
X X
-9.5
-1.6
-1.65 -10
46.4 100 215 464 .1E4 .215E4 .464E4 .1E5 .215E5 46.4 100 215 464 .1E4 .215E4 .464E4 .1E5 .215E5
TIME Log Scale TIME Log Scale
(a) at point B (b) at point C
Figure 14.15: History plot of stress in I-beam
only one value per time point, therefore iDiana will automatically calculate the
average value for the selected elements.
Vertical displacement phase2.fvc
RESULTS NODAL TDTX...G TDTY
PRESENT GRAPH NODE 134
After the upheaval by prestressing in phase one in the first 89 days, the elastic
deflection due to the slab’s weight indicates the start of phase two. The his-
tory plot of the displacement shows that the elastic deflection, caused by the
additional weight of the slab in phase two, is initially followed by further creep
deflection [Fig. 14.16]. After about two hundred days however the deflection
changes into an upheaval. This upheaval is caused by shrinkage which is hin-
dered mainly at the top by the relatively large amount of reinforcement number
6. You may check yourself that an analysis without reinforcement 6 results
in continuously increasing deflection by creep. Generally speaking, the graphs
show an increasing upheaval in time, an increase of pressure in the lower fiber
of the beam (at B) and a decrease in the upper fiber (at C).
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
308 Concrete Viaduct
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:32 p2disB.ps
Model: PHASE2
Nodal TDTX...G TDTY
Max/Min on whole graph:
Ymax = 1.51
Ymin = -1.22
Xmax = .101E5
Xmin = 89
Variation over loadcases
Node 134
1.75
1.5
1.25
N
O
D 1
A
L .75
T
D .5
T
X .25
.
. 0
. 46.4 100 215 464 .1E4 .215E4 .464E4 .1E5 .215E5
G
-.25 Log Scale
T
D -.5
T
Y -.75
-1
-1.25
TIME
Figure 14.16: History plot of displacement of point B
14.3 Appendix: Aging Study
In these tests we compare aging Kelvin Chains to non-aging Maxwell Chains.
These tests represent two main ages at loading of the I-beam’s concrete: dead
material 1 material 1
F nonaging F
material 2 material 2
F aging F
(a) initial loading at age 1 day (b) initial loading at age 89 days
Figure 14.17: Models to investigate aging of concrete
weight and prestress load at the age of one day [Fig. 14.17a] and the additional
slab weight at the age of 89 days [Fig. 14.17b].
1. Non-aging Maxwell Chains, loading age t0 = 1 or 89 days.
2. Aging Kelvin Chain, initial age t0 = 1 days.
14.3.1 Loading Age One Day
The input data for the first test, with a loading age of one day, is as follows.
test1.dat
TEST AGING CREEP, I-BEAM
’UNITS’
TIME DAY
LENGTH MM
FORCE N
’COORDI’ DI=2
1 0. 0.
2 1. 0.
3 1. 0.
’ELEMEN’
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
14.3 Appendix: Aging Study 309
CONNEC
1 L2TRU 1 2
2 L2TRU 1 3
MATERI
1 1
2 2
GEOMET
/ 1-2 / 1
’MATERI’
1 YOUN28 3.975E+04
POISON 0.3
CREEPN MC1990
H 580.
FCM28 63.
LODAGE 1.
2 YOUN28 3.975E+04
POISON 0.3
CREEPN MC1990
H 580.
FCM28 63.
AGING 1.
’GEOMET’
1 CROSSE 1.
’SUPPOR’
1 TR 1
’LOADS’
CASE 1
NODAL
/ 2-3 / FORCE 1 1.
’TIMELO’
LOAD 1
TIMES 0.0 100000.0 /
FACTOR 1.0 1.0 /
’END’
Note the use of table ’UNITS’. This table is added because it is intended to use
days instead of the default seconds in transient analysis. The commands for the
first test are as follows.
test1.dcf
*FILOS
INITIA
*INPUT
*NONLIN
TYPE PHYSIC
BEGIN OUTPUT TABULA
SELECT ELEMEN ALL / INTPNT 1
STRAIN TOTAL GREEN LOCAL NOAXES
END OUTPUT
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
310 Concrete Viaduct
BEGIN EXECUT
BEGIN TIME
BEGIN STEPS
BEGIN EXPLIC
SIZES 1.E-10 0.0001 0.0003 0.0006\
0.001 0.003 0.005\
0.01(4) 0.025(4) 0.05(5) 0.1(6)\
0.25(4) 0.5(4) 1.(6)\
2.5(4) 5.(4) 10.(6)\
100.0 300.0 500.0\
1000.0 3000.0 5000.0
END EXPLIC
END STEPS
END TIME
BEGIN ITERAT
METHOD NEWTON REGULA
MAXITE=5
END ITERAT
END EXECUT
*END
We run the job with these files.
diana test1
An output fragment is shown below:
test1.tb
Analysis type NONLIN
Step nr. 53
Time 9.000E+01
Result STRAIN TOTAL GREEN
Axes LOCAL
Location of results NODES
Elmnr Nodnr Exx Eyy Ezz
1 1 6.886E-05 -2.066E-05 -2.066E-05
2 6.886E-05 -2.066E-05 -2.066E-05
2 1 6.757E-05 -2.027E-05 -2.027E-05
3 6.757E-05 -2.027E-05 -2.027E-05
14.3.2 Loading Age 89 Days
The input data for the second test, with a loading age of 89 days, is as follows.
test2.dat
’MATERI’
1 YOUN28 3.975E+04
POISON 0.3
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
14.3 Appendix: Aging Study 311
CREEPN MC1990
H 580.
FCM28 63.
LODAGE 90.
2 YOUN28 3.975E+04
POISON 0.3
CREEPN MC1990
H 580.
FCM28 63.
AGING 1.
’TIMELO’
LOAD 1
TIMES 0.0 89.0 89.0 100000.0 /
FACTOR 0.0 0.0 1.0 1.0 /
’END’
In the commands for the second test, as shown below, we do not initialize the
filos file. Only input tables ’MATERI’ and ’TIMELO’ are read to overwrite the
data of the first test.
test2.dcf
*INPUT
*NONLIN
TYPE PHYSIC
BEGIN OUTPUT TABULA
SELECT ELEMEN ALL / INTPNT 1
STRAIN TOTAL GREEN LOCAL NOAXES
END OUTPUT
BEGIN EXECUT
TIME STEPS EXPLIC SIZES 89.0
BEGIN ITERAT
BEGIN CONVER
FORCE CONTIN
DISPLA OFF
END CONVER
END ITERAT
END EXECUT
BEGIN EXECUT
BEGIN TIME
BEGIN STEPS
BEGIN EXPLIC
SIZES 1.E-10 0.0001 0.0003 0.0006\
0.001 0.003 0.005\
0.01(4) 0.025(4) 0.05(5) 0.1(6)\
0.25(4) 0.5(4) 1.(6)\
2.5(4) 5.(4) 10.(6)\
100.0 300.0 500.0\
1000.0 3000.0 5000.0
END EXPLIC
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
312 Concrete Viaduct
END STEPS
END TIME
END EXECUT
*END
Now run the second job.
diana test2
An output fragment is shown below:
test2.tb
Analysis type NONLIN
Step nr. 61
Time 1.009E+04
Result STRAIN TOTAL GREEN
Axes LOCAL
Location of results NODES
Elmnr Nodnr Exx Eyy Ezz
1 1 4.854E-05 -1.456E-05 -1.456E-05
2 4.854E-05 -1.456E-05 -1.456E-05
2 1 4.910E-05 -1.473E-05 -1.473E-05
3 4.910E-05 -1.473E-05 -1.473E-05
The displayed output fragments, taken from test1.tb and test2.tb, show that
the values for aging Kelvin Chains (element 1) are close to the values for the
non-aging Maxwell Chains (element 2).
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
Chapter 15
Stress Ribbon Bridge
Name: Srbrid
Path: /Examples/ConcMas/Srbrid
Keywords: analys: geomet nonlin phase physic. constr: suppor tying.
elemen: bar beam cable cl6tr cl9be class3 reinfo truss zones.
load: anchor elemen force line postte reinfo temper. materi:
concre consta crack creep cutoff elasti isotro linear maxwel re-
tent smear soften temper viscoe. option: adapti arclen direct
lagran loadin modifi newton regula size spheri total. post: bi-
nary femvie. pre: append. result: cauchy displa moment
stress total.
At the Technical University of Catalonia, a draft design of a Stress Ribbon bridge
has been made. The design, such as described by Cobo Del Arco and Aparicio
Bengoechea [4], is the basis for the current example on a phased geometric
and physical nonlinear analysis. Figure 15.1 on the following page shows the
geometry of the bridge where Asb is the cross-sectional area of all four suspension
cables, Asp the cross-sectional area of the six prestressing cables and Ac the total
cross-sectional area of the bridge segments. For this example, the symmetry
about the longitudinal axis of the bridge allows a two-dimensional approach.
A Stress Ribbon bridge comprises the load carrying mechanisms of a cable,
a beam and an arch. The erection, which is carried out in sequences, begins
with suspending cables between abutments on both sides of a crossing. The
cables provide the support for bridge segments, which are interconnected after
being positioned on the suspension cables. Prestress cables, running through
the bridge segments as well as the abutments, are then inserted. Flexural stiff-
ness is finely provided by post-tensioning the prestress cables from behind the
abutments.
Analysis in phases. The analysis is performed in two phases. Phase 1 deals
with the behavior of the suspension cables, when subjected to the dead weight
loading of the bridge segments. In phase 2, the deformed geometry of the cables
is used as the initial geometry of the bridge segments. The bridge segments,
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
314 Stress Ribbon Bridge
abutment precast concrete segments
40 m
anchors for suspension cables
handrail
precast concrete 2 suspension
segment cables 24 ∅0.6
pavement 3 posttension fascia beam
cables 19 ∅0.6
10
NA 30
17.5 20
15 10 10 10 10 10 15 40 10 20
100 115
250
Asb = 0.01344 m2 Asp = 0.01596 m2 Ac = 1.0 m2
Figure 15.1: Geometry of stress ribbon bridge [cm]
including the prestress cables are connected to the suspension cables, and the
combined system is posttensioned. The prestress cables are bonded to the bridge
segments, and additional external loading is applied. Finally, the structure is
subjected to thermal contraction and creep.
15.1 Phase 1
In phase 1, the bearing cables are suspended between the abutments. The cables
are subjected to a horizontal force, which gives the desired vertical displacement
due to dead weight of the cables and the bridge segments. The horizontal force
is estimated by the following analytical expression [4]:
q0 l 2
H0 = = 1.03×107 N (15.1)
8f0
with H0 the horizontal force, q0 = 2.575×104 N/m the distributed dead weight
of bridge segments and cables, f0 = 2 m the desired deflection at midspan and
l = 80 m the span length.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
15.1 Phase 1 315
15.1.1 Finite Element Model
The suspension cables are represented by 40 (2 m long) three-node truss ele-
ments CL6TR as shown in Figure 15.2. See also Volume Element Library. As
q0 (dead weight bridge segments & cables)
H0
Figure 15.2: Finite element model for phase 1, truss elements CL6TR
post-tensioning of the bridge (in phase 2) is assumed to take place from one end,
the symmetry conditions are not utilized. The finite element model, including
properties, supports, and loading, is given on a previously made input data file
in Diana batch format. We will now discuss the various parts of the complete
input data file for phase 1.
Element mesh phas1.dat
STRESS RIBBON BRIDGE
’COORDI’
1 0.000000E+00 0.000000E+00 0.000000E+00
2 1.000000E+00 0.000000E+00 0.000000E+00
... lines skipped
80 7.900000E+01 0.000000E+00 0.000000E+00
81 8.000000E+01 0.000000E+00 0.000000E+00
’ELEMEN’
CONNEC
1 CL6TR 1 2 3
2 CL6TR 3 4 5
... lines skipped
39 CL6TR 77 78 79
40 CL6TR 79 80 81
MATERI
/ 1-40 / 1
GEOMET
/ 1-40 / 1
Material and geometrical properties phas1.dat
’MATERI’
1 YOUNG 2.00000E+11
THERMX 1.00000E-05
’GEOMET’
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
316 Stress Ribbon Bridge
1 ZAXIS 0.0 0.0 1.0
:total cross sectional area of the 4 suspension cables /1/
CROSSE 0.01344
Young’s modulus and the total cross-sectional area of the four suspension cables
are taken from the article by Cobo Del Arco and Aparicio Bengoechea [4].
Supports and loading phas1.dat
’SUPPOR’
/ 1 81 / TR 2
81 TR 1
’LOADS’
CASE 1
:horizontal force on suspension cables
NODAL
1 FORCE 1 -1.03E7
CASE 2
:distributed load (deadweight bridge segments and suspension cables)
:2.575E4 from paper by del Arco et al, see Bibliography
ELEMEN
/ 1-40 / LINE
FORCE -2.575E4
DIRECT 2
CASE 3
:negligible initial stress in suspension cables
ELEMEN
/ 1-40 / PRESTR 1.0E3
’TEMPER’
0. 1. 1.E10
/ 1-40 /
20. 10. 10.
’END’
Three load cases are defined:
Case 1: the horizontal force H0 in the suspension cable.
Case 2: the dead weight q0 of the bridge segments and cables.
Case 3: a negligible prestress force in the suspension cables. The prestress is
applied as an initial load in phase 1, to provide a negligible lateral stiffness
of the truss elements. The stiffness is a result of the geometric nonlinear
formulation.
The input file also contains a ’TEMPER’ table to be used for the analysis of
thermal contraction of the assembled model in phase 2.
15.1.2 Initialization and Nonlinear Analysis
Before the nonlinear analysis of phase 1 is carried out, we must perform the
following tasks:
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
15.1 Phase 1 317
Initialize the database.
Read and evaluate the input file.
Initialize phase 1.
Assemble the finite element model.
Generate and store the element matrices.
Generate and store the load vectors.
First we will discuss the commands that initialize the analysis and then the
commands that actually perform the load steps of the nonlinear analysis: the
horizontal force on the suspension cables and the distributed load.
Initialization phas1.dcf
*FILOS
INITIALIZE
*INPUT
*PHASE
*NONLIN
BEGIN TYPE
BEGIN PHYSIC
CRACKI SECANT
VISCOE
END PHYSIC
GEOMET
END TYPE
OUTPUT OFF
:initial stress in suspension cables
BEGIN EXECUT
BEGIN START
BEGIN INITIA
BEGIN STRESS
BEGIN INPUT
LOAD=3
FACTOR=1
END INPUT
END STRESS
END INITIA
STEPS OFF
END START
END EXECUT
Preceding the actual phased nonlinear analysis, usually a complete linear anal-
ysis is performed. However, this is not necessary and omitted in this example
because the linear elastic stiffness matrix would give zero terms on the diagonal,
which inhibits solution of the system of equations. The zero terms represent the
lack of stiffness in the lateral direction of the truss elements. In the nonlinear
analysis we solve this problem by subjecting the truss elements to a negligible
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
318 Stress Ribbon Bridge
initial stress via the EXECUT START INITIA STRESS INPUT command for Module
nonlin.
For the initialization, under TYPE PHYSIC, we also specify the phenomena
which will be used in the complete analysis: viscoelastic material behavior due
to shrinkage in the bridge segments (VISCOE) and cracking of concrete via the
secant crack normal stiffness (CRACKI SECANT).
Load steps phas1.dcf
:horizontal force on suspension cables
BEGIN EXECUT
BEGIN LOAD
BEGIN STEPS
BEGIN ENERGY
INISIZ=0.25
NSTEPS=10
MAXSIZ=1.E+06
MINSIZ=0.001
ARCLEN SPHERI
END ENERGY
END STEPS
LOADNR=1
END LOAD
BEGIN ITERAT
METHOD NEWTON REGULA
MAXITE=20
CONVER FORCE CONTIN TOLCON=1.E-06
CONVER DISPLA CONTIN TOLCON=1.E-06
END ITERAT
STOP LOAD TOTAL=1
END EXECUT
:distributed load (dead weight bridge segments and suspension cables)
BEGIN EXECUT
BEGIN LOAD
BEGIN STEPS
BEGIN ENERGY
INISIZ=0.25
NSTEPS=10
MAXSIZ=1.E+06
MINSIZ=0.001
ARCLEN SPHERI
END ENERGY
END STEPS
LOADNR=2
END LOAD
BEGIN ITERAT
METHOD NEWTON REGULA
MAXITE=20
CONVER FORCE CONTIN TOLCON=1.E-06
CONVER DISPLA CONTIN TOLCON=1.E-06
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
15.2 Phase 2 319
END ITERAT
STOP LOAD TOTAL=1
BEGIN OUTPUT FEMVIEW BINARY
SELECT STEPS LAST
DISPLA TOTAL
STRESS CAUCHY LOCAL INTPNT
END OUTPUT
END EXECUT
*END
The first EXECUT block concerns the prescribed horizontal force, the second
belongs to the dead weight of the bridge segments. Both executions are per-
formed with Spherical Path Arc-length control, by specifying the ARCLEN SPHERI
command. The STOP LOAD TOTAL 1.0 command ensures that the execution is
terminated when the total load factor for the current load reaches the value 1.0.
As the deformed geometry of phase 1 is to be used as the initial geometry for
the bridge segments, the displacements of all the nodes are selected for output.
We may now perform the execution of phase 1 by starting Diana with the input
data and command files as discussed above:
diana phas1
When the analysis job has terminated we enter the iDiana Results environment
to display the deformed truss model.
Deformed model phas1.fvc
FEMVIEW PHAS1
RESULTS LOADCASE LC2 8
RESULTS NODAL TDTX...G RESTDT
PRESENT SHAPE
The TDT results attribute represents the total displacements. For these we select
‘load case’ PH1 8 which is the last executed load step. We display the result as
a deformed shape [Fig. 15.3].
15.2 Phase 2
For phase 2 we must specify additional data: material properties, the finite
element model, and some data to analyze the thermal contraction.
15.2.1 Material Models
The bridge segments are prefabricated concrete elements, 1 m long (in the lon-
gitudinal direction of the bridge), and 5 m wide [Fig. 15.1 p. 314]. The concrete
is modeled according to a multi–directional fixed crack model for tensile states
of stress, combined with a creep model for long duration compressive states
of stress. The input in batch format of the material properties of the bridge
segments (material 2), and the prestressing cables (material 3) is shown below.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
320 Stress Ribbon Bridge
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:57:57 p1dfm.ps
Model: PHAS1
LC2: Load case 2
Step: 8 LOAD: 1
Nodal TDTX...G RESTDT
Max = 2 Min = 0
Factor = 2.35
Z X
Figure 15.3: Nonlinear deformations after phase 1
phas2.dat
’MATERI’
2 YOUN28 0.35E5
POISON 0.2
THERMX 1.0E-5
:creep according to model code 1990
CREEPN MC1990
FCM28 35.0
:2Ac/u=98.0 mm
H 98.
LODAGE 28
CEMTYP NR
RH 60
TEMPER 10
:Cracking
CRACK 1
CRKVAL 3.0E6
TAUCRI 1
BETA 0.2
TENSIO 1
TENVAL 4.0E-3
3 YOUNG 2.0E11
NOBOND
See Volume Material Library for description of these input data items.
15.2.1.1 Cracking
A multi–directional fixed crack model with a constant stress cut-off criterion is
used, The cut-off value equals the tensile strength of concrete, which is taken as
ft = 3 MPa. The softening branch of the stress–strain diagram, subsequent to
cracking, is linear and in accordance with a tension stiffening model. The latter
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
15.2 Phase 2 321
implies that the ultimate stress inducing tensile strain is governed by the yield
stress of the reinforcement:
1 fy
εcr
u = = 4×10−3 (15.2)
2 Es
where fy = 1600 MPa is the yield stress of the prestress steel. The shear
modulus, with reference to the crack plane, is reduced by a constant shear
retention factor β = 0.2, at the onset of cracking.
15.2.1.2 Creep
Creep is modeled by rheological Maxwell chains , consisting of several parallel
spring and dashpot chains. The properties of the chains can be derived from
experimental curves or standard creep models like CEB-FIP by curve fitting. In
the past, tools and handbooks have been developed for this purpose. In Diana,
parameter determination from experimental or standard creep or relaxation
curves is directly part of the code.
Input data for the CEB-FIP creep model are: the initial age of loading t0 ,
the modulus of elasticity Et0 the mean compressive strength fcm , the cement
type, the relative humidity RH, and the ambient temperature Tenv , and the
notational size h0 . The notational size is defined as:
2Ac
h0 = (15.3)
u
with Ac the cross-sectional area of the member and u the perimeter of the
cross-section in contact with the atmosphere.
It should be noticed that the units belonging to the creep model (day, MPa,
mm, °C) refer to the CEB-FIP code, and are independent of other input data,
which in the present example are in SI units. The input parameters belonging
to the CEB-FIP creep model must be transformed to a viscoelastic model in
Diana syntax, before applicable in a nonlinear analysis.
15.2.2 Finite Element Model
In phase 2 of the analysis, the model is extended by CL9BE beam elements ,
representing the bridge segments [Fig. 15.4]. The initial geometry of the beam
q0 (dead weight bridge segments & cables)
CL9BE beam elements
CL6TR truss elements
Figure 15.4: Finite element model for phase 2
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
322 Stress Ribbon Bridge
elements follow the deformed shape of the phase 1 truss model. This requires
a new set of nodes to be defined. The coordinates of the nodes are found by
adding the final displacements of the nodes in phase 1, as given on the tabular
output file phas1.tb, to the coordinates of the nodes defined in phase 1. The
prestressing cable is located in the bridge segments’ center of gravity, and is
consequently connected directly to the beam nodes.
After the bridge segments have been positioned, the cavity for the suspension
cable is filled with concrete. Hence, the suspension cable is bonded to the bridge
segments. This is achieved by tying the truss nodes to the beam nodes, see input
table ’TYINGS’.
The end node of the truss model, which in phase 1 was subjected to a
horizontal force (load case 1), remains its displaced position (0.17 m) in phase
2, by fixing it in the horizontal direction. This is why load case 1 is left out
in file phas2.dat. We specify two additional loads, case 2 and case3. Load
case 2 is the dead weight q0 of the bridge segments and cables. This load is
defined as time dependent, however with a constant value in the time domain
of interest. This is necessary in order to perform time stepping in connection
with thermal contraction and creep. Load case 3, which was initiated in phase
1 as a negligible prestress load in the suspension cables, is redefined as the post-
tension load in the input file for phase 2. In magnitude this load is equal to
the horizontal force H0 in the suspension cables, which was applied in phase 1.
As explained earlier, the horizontal load is limited by buckling. In reality, the
end support would be fixed during all phases of the construction, thus allowing
horizontal translation of the suspension cables. However, this distinction is not
significant. Below we show some significant fragments of the additional input
data for the finite element model for phase 2.
phas2.dat
’COORDI’
101 -1.721000E-01 .000000E+00 .000000E+00
102 8.269000E-01 -9.865000E-02 .000000E+00
... lines skipped
180 7.900103E+01 -9.865000E-02 .000000E+00
181 8.000000E+01 .000000E+00 .000000E+00
’ELEMEN’
CONNEC
101 CL9BE 101 102 103
102 CL9BE 103 104 105
... lines skipped
139 CL9BE 177 178 179
140 CL9BE 179 180 181
MATERI
/ 101-140 / 2
GEOMET
/ 101-140 / 2
DATA
/ 101-140 / 1
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
15.2 Phase 2 323
’REINFORCEMENTS’
LOCATI
1 BAR
101 101 102 103
102 103 104 105
... lines skipped
139 177 178 179
140 179 180 181
MATERI
1 3
GEOMET
1 3
’GEOMET’
2 NZONES 2
ZONE2D -0.175 1.150 0.025 1.50 0.025 2.50 0.125 2.50
:Cross-sectional area of prestressing cables from paper
:by del Arco et al, see Bibliography
3 CROSSE 0.01596
’DATA’
1 NUMINT GAUSS SIMPSO
NINTEG 2 3
’LOADS’
:Deadweight of bridge segments and cables
CASE 2
ELEMEN
/ 1-40 / LINE
FORCE -2.575E4
DIRECT 2
:Posttension load in prestress cables equal to H0, applied in phase 1
CASE 3
REINFO
1 ANCHOR 101
FORCE 1.03258E7
SHEAR 0.10
:After the bridge-segments have been positioned, it is anticipated
:that the suspension cables are grouted in the conduits. Hence, that
:the suspension cables are bonded to the bridge segments. This is
:modelled by tying the truss nodes to the beam nodes.
’TYINGS’
EQUAL TR 1 2
2 102
3 103
... lines skipped
79 179
80 180
:The support table is appended to the support table from
:phase 1, see phas2l1.com and phas1.dat
’SUPPOR’
1 TR 1
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
324 Stress Ribbon Bridge
101 TR 1
101 TR 2
181 TR 1
181 TR 2
15.2.3 Thermal Contraction
The additional input data for phase 2 also contains a ’TEMPER’ table to be used
for the analysis of thermal contraction of the assembled model.
phas2.dat
’TEMPER’
0. 1. 1.E10
/ 1-40 /
20. 10. 10.
/ 101-140 /
20. 10. 10.
0. 0. 0.
’END’
15.2.4 Nonlinear Analysis
The nonlinear analysis of phase 2 comprises the following steps:
Initialization and application of dead weight.
Prestressing of the cables.
Bonding of the prestress cables and simultaneous application of additional
loadings.
Time stepping for creep analysis.
15.2.4.1 Initialization and Dead Weight
Before initializing phase 2 of the nonlinear analysis, the tables of the input file
for phase 2 are read and appended by Module input.
phas2l1.dcf
*INPUT
READ TABLE DATA
READ APPEND TABLE GEOMET MATERI COORDI ELEMEN SUPPOR
READ TABLE LOADS REINFO TYINGS TEMPER
*PHASE
*NONLIN
BEGIN TYPE
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
15.2 Phase 2 325
PHYSIC
GEOMET
END TYPE
OUTPUT OFF
BEGIN EXECUT
BEGIN START
INITIA STRESS PHASE
STEPS EXPLIC SIZE 1.
LOAD LOADNR=2
END START
BEGIN ITERAT
METHOD NEWTON REGULA
MAXITE=1
CONVER FORCE CONTIN TOLCON=1.E-06
CONVER DISPLA CONTIN TOLCON=1.E-06
END ITERAT
END EXECUT
In phased modeling, external loads which are active in one phase, must be
applied again in each subsequent phase, if still active. However, the internal
force vector remains unchanged when entering a new phase. The command
EXECUTE START STEPS implies that the external force vector (the out-of-balance
force) is applied incrementally. As equilibrium was satisfied at the end of phase
1, the external load vector is applied in one increment. In the present example,
this is consequently merely a reapplication of the external load vector, which
is in equilibrium with the internal forces left over from phase 1. It should be
noticed that the horizontal force applied at the end of the truss model need not
be entered again, because the support has been fixed in the horizontal direction
in phase 2. The output file shows that equilibrium is obtained immediately.
15.2.4.2 Cable Prestressing
In the first part of phase 2, the prestress cable is posttensioned from one end by a
force equal to 70% of the horizontal force in the truss elements. Due to the fixed
supports at both ends of the bridge, additional prestress cause snap-through.
For the analysis we prepare the following batch commands.
phas2l1.dcf
BEGIN EXECUT
BEGIN LOAD
BEGIN STEPS
BEGIN ENERGY
INISIZ=0.1
NSTEPS=20
MAXSIZ=1.E+06
MINSIZ=0.001
ARCLEN SPHERI
END ENERGY
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
326 Stress Ribbon Bridge
END STEPS
LOADNR=3
END LOAD
BEGIN ITERAT
METHOD NEWTON MODIFI
MAXITE=20
CONVER FORCE CONTIN TOLCON=1.E-06
CONVER DISPLA CONTIN TOLCON=1.E-06
END ITERAT
STOP LOAD TOTAL=0.7
BEGIN OUTPUT FEMVIE BINARY
SELECT STEPS LAST
DISPLA TOTAL
STRESS CAUCHY LOCAL INTPNT
STRESS MOMENT
END OUTPUT
END EXECUT
*END
Now we may start Diana to execute the first part of phase 2.
diana phas2l1 phas2.dat
After termination of the analysis job we enter the iDiana Results environment
to display the analysis results.
phas2l1.fvc
FEMVIEW PHAS2L1
RESULTS LOADCASE LC3 8
RESULTS NODAL TDTX...G RESTDT
PRESENT SHAPE FACTOR 1
RESULTS GAUSSIAN RE.SXX.L SXX
PRESENT CONTOUR LEVELS
Again we select the total displacements of the last step. We display a true-
scale plot of the deformation [Fig. 15.5a]. The SXX result attribute represents
the normal stress which we display as a contour plot [Fig. 15.5b]. In the results
monitor we see that σxx varies from 446×106 to 454×106 .
15.2.4.3 Bonding Prestress Cables and Additional Load
After post-tensioning, the prestress cable is bonded and additional vertical load-
ing, due to railing, bridge pavement and service load is applied. Therefore we
prepare the following command file.
phas2l2.dcf
*NONLIN
MODEL OFF
TYPE OFF
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
15.2 Phase 2 327
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:07 p2l1dfm.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:07 p2l1sxx.ps
Model: PHAS2L1 Model: PHAS2L1
LC3: Load case 3 LC3: Load case 3
Step: 8 LOAD: .7 Step: 8 LOAD: .7
Nodal TDTX...G RESTDT Gauss RE.SXX.L SXX
Max = 1.9 Min = 0 Max = .454E9
Factor = 1 Min = .446E9
Results shown:
Mapped to nodes
.453E9
.452E9
.452E9
.451E9
Y Y .45E9
.449E9
.449E9
Z X Z X .448E9
.447E9
.446E9
(a) deformation, true-scale (b) contour of normal stress
Figure 15.5: Phase 2 results
BEGIN EXECUT
BEGIN LOAD
BEGIN STEPS
BEGIN ENERGY
INISIZ=0.25
NSTEPS=40
MAXSIZ=1E+06
MINSIZ=0.001
ARCLEN SPHERI
END ENERGY
END STEPS
LOADNR=2
END LOAD
BEGIN ITERAT
METHOD NEWTON REGULA
MAXITE=20
CONVER FORCE CONTIN TOLCON=1.E-06
CONVER DISPLA CONTIN TOLCON=1.E-06
END ITERAT
PHYSIC BOND REINFO 1
STOP LOAD TOTAL=2.01
BEGIN OUTPUT FEMVIE BINARY
BEGIN SELECT
STEPS LAST
ELEMEN 1-40 102-140
END SELECT
DISPLA TOTAL
STRESS CAUCHY LOCAL INTPNT
STRESS MOMENT
END OUTPUT
END EXECUT
*END
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
328 Stress Ribbon Bridge
We start Diana to perform this step in the analysis of phase 2.
diana phas2l2 phas2.dat
After termination of the analysis we enter the iDiana Results environment.
phas2l2.fvc
FEMVIEW PHAS2L2
RESULTS LOADCASE LC2 12
RESULTS GAUSSIAN RE.SXX.L SXX
PRESENT CONTOUR LEVELS
We select step 12 (the last step) and again make a contour plot of the normal
stresses [Fig. 15.6]. In the results monitor we see that σxx varies from 492×106
to 501×106 .
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:10 p2l2sxx.ps
Model: PHAS2L2
LC2: Load case 2
Step: 12 LOAD: 2.01
Gauss RE.SXX.L SXX
Max = .501E9
Min = .492E9
Results shown:
Mapped to nodes
.5E9
.499E9
.498E9
.498E9
Y .497E9
.496E9
.495E9
Z X .495E9
.494E9
.493E9
Figure 15.6: Phase 2 normal stress after bonding and additional load
15.2.4.4 Time Stepping for Creep
The bridge is then subjected to a decreased ambient temperature of 10 °C.
Finally creep is simulated for a period of 12000 days (≈ 33 years). The time
stepping scheme is composed by logarithmically incrementing the step size.1
The command sequence for the time stepping is as follows.
phas2t.dcf
*NONLIN
MODEL OFF
TYPE OFF
BEGIN EXECUT
1 Accumulation of the increments in the SIZE command of file phas2t.dcf gives 1.0368×109
s which is 12000 days.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
15.2 Phase 2 329
TIME STEPS EXPLIC SIZE 1.0
BEGIN ITERAT
METHOD NEWTON REGULA
MAXITE=20
BEGIN CONVER
ENERGY TOLCON=1.E-06
FORCE OFF
DISPLA OFF
END CONVER
END ITERAT
PHYSIC BOND REINFO 1
BEGIN OUTPUT FEMVIE BINARY
DISPLA TOTAL
END OUTPUT
END EXECUT
BEGIN EXECUT
BEGIN TIME
BEGIN STEPS
BEGIN EXPLIC
SIZE 1.E0 2.E0 7.E0 2.E1 7.E1 2.E2 7.E2 \
2.E3 7.E3 2.E4 7.E4 2.E5 7.E5 2.E6 \
7.E6 2.E7 7.E7 2.E8 7.E8 3.68E7
END EXPLIC
END STEPS
END TIME
BEGIN ITERAT
METHOD NEWTON REGULA
MAXITE=20
CONVER FORCE CONTIN TOLCON=1.E-10
CONVER DISPLA CONTIN TOLCON=1.E-10
END ITERAT
PHYSIC BOND REINFO 1
BEGIN OUTPUT FEMVIE BINARY APPEND
MODEL OFF
DISPLA TOTAL
END OUTPUT
END EXECUT
*END
We start Diana to perform the creep analysis in phase 2.
diana phas2t phas2.dat
After termination we enter the iDiana Results environment.
phas2t.fvc
FEMVIEW PHAS2T
RESULTS LOADCASE LC1 33
RESULTS NODAL TDTX...G RESTDT
PRESENT SHAPE FACTOR 1
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV) November 8, 2010 – First ed.
330 Stress Ribbon Bridge
RESULTS LOADCASE LC1
RESULTS NODAL TDTX...G TDTY
PRESENT GRAPH NODE 41
Again we display a true-scale plot of the deformation for the last step (33)
[Fig. 15.7a]. Then we select all steps (‘load cases’) and result attribute TDTY
which represents the vertical displacement. Now we can display a graph of the
deflection of the mid span (node 41) as a function of time [Fig. 15.7b].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:22 p2tdfm.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:58:22 p2tgdy.ps
Model: PHAS2T Model: PHAS2T
LC1: Load case 1 Nodal TDTX...G TDTY
Step: 33 TIME: .104E10 Max/Min on whole graph:
Nodal TDTX...G RESTDT Ymax = -1.99
Max = 2.04 Min = 0 Ymin = -2.04
Factor = 1 Xmax = .104E10
Xmin = 1
Variation over loadcases
Node 41
-1.98
-1.99
N
O
D
A
L -2
T
D
T
X -2.01
.
.
.
G
-2.02
T
D
T
Y -2.03
-2.04
0 .2 .4 .6 .8 1 1.2
Y TIME *1E9
Z X
(a) final deformation, true-scale (b) mid-span deflection in time
Figure 15.7: Phase 2 results for creep
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (IV)
Part V
Young Hardening Concrete
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
Chapter 16
Hydration of Concrete
Column
Name: Colhtnl
Path: /Examples/ConcMas/Colhtnl
Keywords: analys: flow flowst heat nonlin physic stagge transi. constr:
initia suppor temper tying. elemen: axisym b2aht cq16a flow
potent q4aht. load: elemen temper time. materi: capaci
conduc consta crack cutoff elasti hydrat isotro linear power re-
tent smear soften viscoe. option: direct newton regula units.
post: binary femvie. pre: femgen. result: cauchy reacti
stress temper total.
Y
0.1 m
X
r =1m
Figure 16.1: Concrete column
This example shows the transient temperature, maturity, and stress develop-
ment in a part of a hydrating concrete column, radius 1 m [Fig. 16.1], during
the first four days after pouring. A slice with thickness 0.1 m of the column is
analyzed, using axisymmetric elements.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
334 Hydration of Concrete Column
16.1 Finite Element Model
We will create a structural model with ten axisymmetric CQ16A elements in
X-direction. For the heat flow analysis Diana will automatically transfer these
elements to Q4AHT elements. The heat flow analysis also requires a bound-
ary element along the outer edge of the column slice (X = 1) to simulate the
convection to the external environment and the environmental temperature.
Therefore we apply a B2AHT element which Diana will automatically skip dur-
ing the structural analysis. To create the finite element model we start iDiana
and enter the Design environment with the model name.
iDiana
FEMGEN COLHTNL
Analysis and Units
Analysis Selection
Model Type: →HeatFlow-Stress Staggered Axisymmetric
Units Definition
Temperature: → Celsius
In the Analysis and Units dialog we specify that the model will be used for
an axisymmetric staggered heat flow–structural analysis. We also specify the
applied units because one of them is not SI: the temperature is in °C instead of
the default K.
Workbox colhtnl.fgc
CONSTRUCT SPACE WORK-BOX 1. 0.1 0.
EYE FRAME WORK-BOX
We define a workbox around the model and let it just fit into the iDiana
viewport.
16.1.1 Geometry Definition
To define the geometry of the model we first define the position of the four
corner points.
Points colhtnl.fgc
GEOMETRY POINT 0.0
GEOMETRY POINT 1.0
GEOMETRY POINT 1.0 0.1
GEOMETRY POINT 0.0 0.1
GEOMETRY SURFACE 4POINTS P1 P2 P3 P4
GEOMETRY LINE STRAIGHT P2 P3
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY POINTS
LABEL GEOMETRY LINES ALL VIOLET
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
16.1 Finite Element Model 335
The SURFACE 4POINTS option defines the surface for this model via the corner
points. Via the the LINE STRAIGHT option we define a separate line for the
boundary element. This is necessary because of the different meshing division
for the structural element CQ16A and the flow boundary element B2AHT. The
first has a midside node which yields two divisions per element, the latter has
no midside node and yields one division. We display the defined geometry with
labels for points and lines [Fig. 16.2a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:04 geom.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:05 mesh.ps
Model: COLHTNL Model: COLHTNL
Analysis: DIANA Analysis: DIANA
Model Type: Heatflow-Stress Staggered axi-symmetric Model Type: Heatflow-Stress Staggered axi-symmetric
P4 L3 P3 13 44 14 45 15 46 16 47 17 48 18 49 19 50 20 51 21 52 22 53 2
L4
33 34 35 36 37 38 39 40 41 42 43
L2
L5 2 3 4 5 6 7 8 9 10 11 1
P1 L1 P2 3 23 4 24 5 25 6 26 7 27 8 28 9 29 10 30 11 31 12 32 1
Y Y
Z X Z X
(a) geometry (b) generated mesh
Figure 16.2: Defining the finite element mesh
16.1.2 Meshing
The actual meshing of the model is performed via the following commands.
colhtnl.fgc
MESHING DIVISION ELSIZE ALL 0.05
MESHING TYPES ALL QU8 CQ16A
MESHING DIVISION L5 1
MESHING TYPES L5 BE2 B2AHT
MESHING GENERATE
VIEW OPTIONS SHRINK
VIEW MESH
LABEL MESH NODES
LABEL MESH ELEMENTS
With the ELSIZE option we first specify a division of size 0.05 which will yield a
mesh with a single line of square elements: two divisions just fill up the vertical
dimension of 0.1, i.e., one CQ16A element. The TYPES option assigns the CQ16A
element to all surfaces of the model. For the boundary element we explicitly
define a single division and assign the B2AHT element to the additional line that
we have defined earlier.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
336 Hydration of Concrete Column
The GENERATE option now generates the mesh. Generally a MESHING MERGE
command is required to mutually connect the nodes along the boundary line
and the surface. In this particular case we may skip this operation because the
boundary element is directly connected to the corner nodes of the surface. Fi-
nally we display the generated mesh with node and element numbers [Fig. 16.2b].
Note the SHRINK option which activates the ‘shrunken elements’ style, otherwise
we could not distinguish the boundary element.
16.1.3 Material Properties
The heat analysis uses a variable called degree of reaction to calculate the heat
production caused by the hydration. Resulting from heat analysis are time
dependent temperature and degree of reaction. These are input for a Power
Law model, which is used for the description of the viscoelastic behavior in the
stress calculation. Instead of a Power Law model we may also apply a Kelvin
or Maxwell Chain model. The properties of these models can also be a function
of temperature and degree of reaction.
In general, usage of Kelvin or Maxwell Chain models is recommended be-
cause these are superior in the description of long term behavior. For creep in
early-age concrete only relatively short time spans have to be analyzed. The
stress fluctuations during this period may be more pronounced than in long-term
processes. Therefore it may be advantageous to develop the creep function in
a Taylor series, as Diana does for the Power Law, rather than using a Kelvin
or Maxwell chain model. See also De Borst & Van Den Boogaard [5] for back-
ground theory.
Cracking will occur if the tensile thermal stresses exceed the cracking stress
value.
iDiana
View →Property Manager...
↑
Property Manager
···
We launch the Property Manager dialog to specify the material properties for
the structural elements and the boundary elements.
Structural elements iDiana
Property Manager
↑ Materials Material Name: MA1
↑Flow →Isotropic
↑Linear Elasticity →Isotropic
↑Static Nonlinearity →Concrete and Brittle Materials →Multi-directional Fixed Crack
→Constant Stress Cut-off →Linear Tension Softening
→Constant Shear Retention →No Plasticity
↑Transient Nonlinearity →Power Law Viscoelasticity
↑External →External Data from File
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
16.1 Finite Element Model 337
For the CQ16A elements we define a material MA1 with properties for heat flow
analysis and for structural analysis. For the flow we specify a conductivity
k = 0.0026 and a capacitance c = 2650. For linear elasticity we specify a Young’s
modulus E = 1.75×1010 and a Poisson’s ratio ν = 0.2. For static nonlinearity we
specify a tensile strength ft = 8.0×105 , an ultimate crack strain εcr
u = 0.033, and
a constant shear retention factor β = 0.2. For transient nonlinearity we specify
the power of the creep function p = 0.3, the development point td = 144000.0,
the creep coefficient α = 3.0, and the power of the time dependent part of the
creep function d = 0.35.
The properties which depend on time and/or the degree of reaction must
be input via an external data file in Diana batch format. For this example we
apply a file materi.dat which looks as follows.
materi.dat
CONREA 0. 4.0E-3 1. 2.6E-3
CAPART 2950. 2917. 2903. 2886. 2870. 2850. 2827. 2797.
2767. 2737. 2707. 2678. 2650.
PRDKAR .320 .686 .850 .960 1.000 .890 .620 .400
.230 .130 .060 .020 .000
REACTI .100 .200 .240 .290 .340 .400 .470 .560
.650 .739 .828 .917 1.00
MAXPRD 73528.
ALPHA .72E9
ARRHEN 5995.
The CONREA input data record specifies the conductivity k as a linear function
of the degree of reaction r. Then CAPART specifies the values of the capacitance
c and PRDKAR the values of the heat production q, both for the degrees of reac-
tion in REACTI. Finally, MAXPRD specifies the totally produced heat, ALPHA the
maximum heat production α, and ARRHEN the Arrhenius constant cA . See also
Volume Material Library for more information on these input data records.
Boundary iDiana
Property Manager
Materials Material Name: MA2
↑Flow →Boundary →Convection only
For the B2AHT boundary element we define a material MA2 with a conduction
coefficient K = 0.025 which simulates the conduction to the environment.
Property assignment colhtnl.fgc
PROPERTY ATTACH S1 MA1
PROPERTY ATTACH L5 MA2
We assign material MA1 to surface S1 which comprises the CQ16A elements and
material MA2 to line L5 which comprises the B2AHT boundary element.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
338 Hydration of Concrete Column
16.1.4 Boundary and Initial Conditions
For the flow analysis the boundary condition involves the external temperature.
Moreover we must specify the initial temperature of the model. For the struc-
tural model the boundary condition involves the rigid supports and a linear
constraint, respectively to keep the lower and upper edges horizontally.
Flow colhtnl.fgc
PROPERTY LOADS EXTTEMP L5 25.0
CONSTRUCT TCURVE LIST 0.0 1.0 10000000.0 1.0
PROPERTY ATTACH LOADCASE 1 TC1
PROPERTY INITIAL INITEMP ALL 25.0
LABEL MESH OFF
LABEL MESH INITIAL ALL BLUE
The EXTTEMP load class defines an ambient temperature of 25 °C, i.e., along line
L5 which has been meshed with a boundary element. By default iDiana will
assume load case 1 for this ‘load’. Because this is a transient analysis, we must
also specify the development of the ambient temperature in time; in this case
we assume a constant temperature. We specify a time curve with a constant
factor 1.0 from t = 0 to t ≈ ∞. By default the name of the time curve will
be TC1. Assigning the time curve to the external temperature, load case 1, we
define the time dependency of the external temperature.
A transient heat flow analysis also requires a specified initial temperature.
Here we specify a uniform temperature of 25 °C for all nodes via the INITEMP
initial condition class. As a check we display the initial temperature on the
mesh [Fig. 16.3a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:05 initem.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:05 bcons.ps
Model: COLHTNL Model: COLHTNL
Analysis: DIANA Analysis: DIANA
Model Type: Heatflow-Stress Staggered axi-symmetric Model Type: Heatflow-Stress Staggered axi-symmetric
25 25 25 25 25 25 25 25 25 25 25 25 25 25 25 25 25 25 25 25 25 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3M
25 25 25 25 25 25 25 25 25 25 25
25 25 25 25 25 25 25 25 25 25 25 25 25 25 25 25 25 25 25 25 25
Y Y
Z X Z X
(a) initial temperature (b) structural constraints
Figure 16.3: Boundary and initial conditions
Structural colhtnl.fgc
PROPERTY BOUNDARY CONSTRAINT L4 X
PROPERTY BOUNDARY CONSTRAINT L1 Y
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
16.2 Nonlinear Transient Heat Flow Analysis 339
PROPERTY BOUNDARY MPC RBEAM L3 P3 Y
LABEL MESH OFF
LABEL MESH CONSTRNT
For the structural model we specify the rigid supports: the horizontal displace-
ment uX = 0 along the central axis of the model, which is line L5, and the
vertical displacement uY = 0 along the bottom edge, which is line L1.
To simulate that the model is a slice out of and infinitely long column we
apply a ‘Rigid Beam’ multi-point constraint along the top edge. The MPC RBEAM
option forces the vertical displacements uY along line L3 to be equal to the uY
of the starting point P3 of that line. In other words: the top edge is forced
to remain horizontally. As a check we display the boundary constraints on the
mesh [Fig. 16.3b].
16.2 Nonlinear Transient Heat Flow Analysis
The first stage in a staggered flow–stress analysis is the flow analysis. In this
case we perform a transient heat flow analysis to determine the temperature
changes in time. The analysis is also nonlinear because the material properties
for the flow model depend on the degree of reaction. We write an input data
file in batch analysis format and initiate the analysis.
iDiana
UTILITY WRITE DIANA
yes
FILE CLOSE
yes
Hydration of concrete column
ANALYSE COLHTNL
Analysis Setup
specification of options
The ANALYSE command initiates the analysis of the model. In the Analysis
Setup dialog we may specify the various options for heat flow analysis, resulting
in the following batch analysis commands.
colhtnl.dcf
*FILOS
INITIA
*INPUT
*HEATTR
MODEL MATRIX CAPACI LUMPED
BEGIN INITIA
NONLIN HYDRAT
TEMPER INPUT
END INITIA
BEGIN EXECUT
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
340 Hydration of Concrete Column
ALPHA=0.67
SIZES 7200.0(40)
BEGIN NONLIN
ITERAT MAXITE=100
HYDRAT ITERAT
END NONLIN
END EXECUT
BEGIN OUTPUT FEMVIE BINARY
SELECT STEPS 1-40(3)
TEMPER
REACTI INTPNT
END OUTPUT
The *HEATTR command invokes Module heattr for transient heat flow analy-
sis. This module automatically adapts the finite element model for heat flow
analysis: the CQ16A elements will be changed to Q4HT elements.
With the SIZES command in the EXECUT block we take forty steps of two
hours each resulting in a concrete age of eighty hours. For output we select the
temperatures in the nodes and the degree of reaction in the integration points of
the elements for steps 1, 4, 7, · · · , 37, 40. See also Volume Analysis Procedures
for description of the various commands and options.
As soon as the analysis run has terminated we enter the iDiana Results
environment to assess the results.
colhtnl.fvc
FEMVIEW COLHTNL
UTILITY TABULATE LOADCASES
RESULTS LOADCASE ALL
The load case tabulation shows the available load cases (steps) with their results
data. Below we show only the first four load cases.
flcs.tb
;
; Model: COLHTNL
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; TR1 1 TIME = .72E4 "Boundary case 1"
; Nodal : PTE....S
; Gauss : EL.DGR.S
;
; TR1 4 TIME = .288E5 "Boundary case 1"
; Nodal : PTE....S
; Gauss : EL.DGR.S
;
; TR1 7 TIME = .504E5 "Boundary case 1"
; Nodal : PTE....S
; Gauss : EL.DGR.S
;
; TR1 10 TIME = .72E5 "Boundary case 1"
; Nodal : PTE....S
; Gauss : EL.DGR.S
;
The nodal attribute PTE represents the temperature and the Gaussian attribute
EL.DGR the degree of reaction. We select ALL load cases for results presentation.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
16.2 Nonlinear Transient Heat Flow Analysis 341
16.2.1 Temperatures
To assess the temperatures we select these via the NODAL option and the PTE
attribute name.
Contour animation colhtnl.fvc
RESULTS NODAL PTE....S PTE
UTILITY SETUP ANIMATE LINEAR
PRESENT
28 OCT 2010 CONTOUR
01:34:12 FROM 25 TO 45 LEVELS 9
temper001
DRAWING ANIMATE LOADCASES PLOTFILE temper
A very instructive manner to display the temperature development in time is
the animation sequence of temperature contours. Here we setup a sequence to
be displayed LINEAR, i.e., from the beginning to the end and then starting all
over again. In order to get corresponding contours, the same color for the same
temperature in each frame, we explicitly specify the contour levels: 9 levels
between 25° and 45° which yields contour limits at whole odd values: 25°, 27°,
· · · , 45° [Fig. 16.4-left].
We put the animation on the screen with the DRAWING ANIMATE LOADCASES
command. After twenty seconds the animation stops and iDiana will prompt us
what to do: restart?, exit?, etc. In this case we type ‘exit’ to stop the animation.
Due to the PLOTFILE option iDiana has saved each frame of the animation in a
separate file: temper001, temper002, . . . , temper014. This allows us to show
the animation frames in a document [Fig. 16.4]. Note that the temperature
reaches a maximum of about 45° at the center of the column after about 26
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:12 temper001
Model: COLHTNL
TR1: Boundary case 1
Step: 1 TIME: .72E4
Nodal PTE....S PTE
Max = 26.9
Min = 26.1
hours.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:12 temper002
Model: COLHTNL
TR1: Boundary case 1
Step: 4 TIME: .288E5
Nodal PTE....S PTE
Max = 38.4
Min = 30.5
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:12 temper003
Model: COLHTNL
TR1: Boundary case 1
Step: 7 TIME: .504E5
Nodal PTE....S PTE
2h
Max = 42.7
Min = 30.3
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:12 temper004
Model: COLHTNL
TR1: Boundary case 1
Step: 10 TIME: .72E5
Nodal PTE....S PTE
8h
Max = 44.4
Min = 29.7
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:12 temper005
Model: COLHTNL 45
TR1: Boundary case 1 43
Step: 13 TIME: .936E5 41
Nodal PTE....S PTE 39
14 h
Max = 44.9 Min = 29.1
37
iDIANA
Y 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:12 temper006 35
33
31
Model: COLHTNL 45
Z X case 1
TR1: Boundary 29
43
27
Step: 16 TIME: .115E6 41
Nodal PTE....S PTE 25
39
20 h
Max = 44.6 Min = 28.6
37
iDIANA
Y 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:12 temper007 35
33
45 Model: COLHTNL
Z X case 1
TR1: Boundary
Step: 19 TIME: .137E6
Nodal PTE....S PTE
DRAWING ANIMATE LOADCASES PLOTFILE temper 31
45
29
43
27
41
25
39
26 h
Max = 43.9 Min = 28.2
43 iDIANA
Y 9.4.3-02 : TNO Diana BV
Model: COLHTNL
DRAWING ANIMATE LOADCASES PLOTFILE temper
37
28 OCT 2010 01:34:12 temper008 35
33
31
45
29
Z X case 1
TR1: Boundary
41 Step: 22 TIME: .158E6
Nodal PTE....S PTE
43
27
41
25
39
32 h
Max = 43 Min = 27.9
37
iDIANA
Y 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:12 temper009 35
39 Model: COLHTNL
Z X case 1
TR1: Boundary
Step: 25 TIME: .18E6
Nodal PTE....S PTE
DRAWING ANIMATE LOADCASES PLOTFILE temper
33
31
45
29
43
27
41
25
39
37 38 h
Max = 41.9
Min = 27.6 37
iDIANA
Y 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:12 temper010 35
33
DRAWING ANIMATE LOADCASES PLOTFILE temper 31
Model: COLHTNL 45
29
35
Z X case 1
TR1: Boundary 43
Step: 28 TIME: .202E6 27
41
25
Nodal PTE....S PTE 39
44 h
Max = 40.7 Min = 27.3
37
iDIANA
Y 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:12 temper011 35
33 Model: COLHTNL
Z X case 1
TR1: Boundary
Step: 31 TIME: .223E6
Nodal PTE....S PTE
DRAWING ANIMATE LOADCASES PLOTFILE temper
33
31
45
29
43
27
41
25
39
31 50 h
Max = 39.5 Min = 27.1
37
iDIANA
Y 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:12 temper012 35
33
DRAWING ANIMATE LOADCASES PLOTFILE temper 31
Model: COLHTNL 45
29
29 Z X case 1
TR1: Boundary
Step: 34 TIME: .245E6
Nodal PTE....S PTE
43
27
41
25
39
56 h
Max = 38.4 Min = 26.9
37
iDIANA
Y 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:12 temper013 35
27 Model: COLHTNL
Z X case 1
TR1: Boundary
Step: 37 TIME: .266E6
DRAWING ANIMATE LOADCASES PLOTFILE temper
33
31
45
29
43
27
41
25
Nodal PTE....S PTE
25 Max = 37.3 Min = 26.8
iDIANA
Y 9.4.3-02 : TNO Diana BV
Model: COLHTNL
DRAWING ANIMATE LOADCASES PLOTFILE temper 62
39
37
28 OCT 2010 01:34:12 temper014 35
33
31 h
45
29
Z X case 1
TR1: Boundary 43
Step: 40 TIME: .288E6 27
41
25
Nodal PTE....S PTE 39
68 h
Max = 36.3 Min = 26.6
37
Y 35
33
DRAWING ANIMATE LOADCASES PLOTFILE temper 31
45
29
Z X 43
27
41
25
39
74 h
37
Y 35
33
DRAWING ANIMATE LOADCASES PLOTFILE temper 31
45
29
Z X 43
27
TFILE temper 41
25
39
80 h
37
Y 35
33
DRAWING ANIMATE LOADCASES PLOTFILE temper 31
45
29
Z X 43
27
41
25
39
37
Y 35
33
DRAWING ANIMATE LOADCASES PLOTFILE temper 31
Figure 16.4: Animation sequence of temperature contours
45
29
Z X 43
27
41
25
39
37
Y 35
33
DRAWING ANIMATE LOADCASES PLOTFILE temper 31
Z X 29
27
25
DRAWING ANIMATE LOADCASES PLOTFILE temper
History plot. Another format to show the variation of the temperature in
time is the history plot for a specific location.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
342 Hydration of Concrete Column
History plot colhtnl.fvc
PRESENT GRAPH NODE 3
We display the history plot for the selected node 3, which is located at the
column center [Fig. 16.5a]. The graph confirms the conclusion of the animation
sequence: a maximum of 45.3° after about 26 hours.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:12 temph.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:12 dgrh.ps
Model: COLHTNL Model: COLHTNL
Nodal PTE....S PTE Gauss EL.DGR.S DGR
Max/Min on whole graph: Max/Min on whole graph:
Ymax = 44.9 Ymax = .991
Ymin = 26.9 Ymin = .166
Xmax = .288E6 Xmax = .288E6
Xmin = .72E4 Xmin = .72E4
Variation over loadcases Variation over loadcases
Node 3 Element 2 Mean
46 1 Element 11 Mean
44 .9
G
A
N 42
U .8
O
S
D
S
A 40 I .7
L A
N
P 38
T .6
E
E 36
L
.
. .5
.
D
. 34
G
.
R
S
. .4
32 S
P
T
D .3
E 30
G
R
28 .2
26 .1
0 .25 .5 .75 1 1.25 1.5 1.75 2 2.25 2.5 2.75 3 0 .25 .5 .75 1 1.25 1.5 1.75 2 2.25 2.5 2.75 3
TIME *1E5 TIME *1E5
(a) temperature at column center (b) degree of reaction
Figure 16.5: History plots
16.2.2 Degree of Reaction
It is interesting to see the development in time of the degree of reaction at the
column center and at the outer surface. The degree of reaction is available for
the element integration points: the GAUSSIAN result attribute DGR. As location
we choose element 2 at the column center and element 11 at the outer surface
[Fig. 16.2b].
History plot colhtnl.fvc
RESULTS GAUSSIAN EL.DGR.S DGR
PRESENT GRAPH ELEMENT 2 11
For the selected elements we display two graphs in one axes system [Fig. 16.5-
b]. These show that heat activates the hydration of concrete. At the warmer
column center the degree of reaction develops more quickly and to a higher
value than at the cooler outer surface. Respectively see the solid line with ‘+’
markers, and the dashed line with ‘*’ markers.
16.3 Nonlinear Structural Analysis
To perform the nonlinear structural analysis we may now directly invoke Module
nonlin. This module automatically transforms the finite element model to
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
16.3 Nonlinear Structural Analysis 343
structural: the Q4HT elements will be reverted to CQ16A, the B2AHT boundary
element will be deactivated and the temperatures resulting from the previous
flow analysis will be transformed to an internal time–temperature table for
structural analysis. In the analysis form we only have to specify options for the
actual structural analysis, resulting in the following batch commands.
colhtnl.dcf
*NONLIN
TYPE PHYSIC
BEGIN OUTPUT FEMVIEW BINARY
SELECT STEPS 1-22(3) 26 31 44 LAST
STRESS TOTAL LOCAL
END OUTPUT
BEGIN EXECUT
TIME STEPS EXPLIC SIZE 3600.(2) 7200.(33) 600.(6) 1200.(33)
BEGIN ITERAT
BEGIN CONVER
ENERGY
FORCE OFF
DISPLA OFF
END CONVER
END ITERAT
END EXECUT
*END
For output we select the total stresses for some steps, including the last one.
With the EXECUT commands we perform 74 time steps until time t = 80 h. See
also Volume Analysis Procedures for description of the various commands and
options.
Crack logging colhtnl.out
STEP 74 TERMINATED, CONVERGENCE AFTER 1 ITERATION
END TIME: 2.880E+05
CRACKING LOGGING SUMMARY
GROUP NAME CRACK, OPEN, CLOSED, ACTIVE, INACTI, ARISES, RE-OPENS, CLOSES
TOTAL MODEL 0 0 0 0 0 0 0 0
When the analysis run has terminated we check whether cracking has occurred.
At the tail of the standard output file we see the crack logging information
for the last step. The zeros indicate that no cracking has occurred during the
analysis.
Available results colhtnl.fvc
FEMVIEW COLHTNL
UTILITY TABULATE LOADCASES
RESULTS LOADCASE LC1
We enter the iDiana Results environment to assess the stresses. The load case
tabulation shows the available load cases (steps) with their results data. Below
we show only the first five load cases.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
344 Hydration of Concrete Column
nlcs.tb
;
; Model: S_COLHTNL
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; MODEL STATIC "Model Properties"
; Element : CRKBANDW*
;
; LC1 1 TIME = .36E4 "Load case 1"
; Element : EL.SXX.L
;
; LC1 4 TIME = .216E5 "Load case 1"
; Element : EL.SXX.L
;
; LC1 7 TIME = .432E5 "Load case 1"
; Element : EL.SXX.L
;
; LC1 10 TIME = .648E5 "Load case 1"
; Element : EL.SXX.L
;
The result attribute SXX represents the stresses in the element nodes. We select
ALL load cases for results presentation.
16.3.1 Stresses
We will now assess the stress distribution over the model and its development
in time. First we will make some contour and history plots of the Von Mises
equivalent stress, then a few vector plots of the principal stresses.
Von Mises stress – animation colhtnl.fvc
RESULTS ELEMENT EL.SXX.L SXX
RESULTS CALCULATE VONMISES
UTILITY SETUP ANIMATE LINEAR
PRESENT CONTOUR FROM 1500 TO 800000 LEVELS 6
DRAWING ANIMATE LOADCASES PLOTFILE pstres
With the SXX results attribute we select the primary stresses. Being scalar
values, the Von Mises stresses are more suitably for contour plots. We ask
iDiana to calculate these via the VONMISES option. Like for the temperatures
we set up an animation sequence for stresses of all available load cases (steps)
[Fig. 16.6a]. Note that the stress gradually increases in the first 30 hours and
that the highest stresses occur at the outer surface. To confirm this we make a
history plot for the element near the center and at the outer surface, respectively
element 2 and 11.
History plot colhtnl.fvc
PRESENT GRAPH ELEMENT 2 11
We make two history plots [Fig. 16.6b]. The solid line, for the outer surface,
shows a maximum stress of 4×105 after about 30 hours. The dashed line, for
the center, shows a maximum stress of 7.3×105 after about 18 hours.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:13 pstres001
16.3 Nonlinear Structural Analysis 345
Model: S_COLHTNL
LC1: Load case 1
Step: 1 TIME: .36E4
Element VONMISES EL.SXX.L
Calculated from: EL.SXX.L
Max = .14E5 Min = .133E4
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:13 pstres002
Model: S_COLHTNL
LC1: Load case 1
Step: 4 TIME: .216E5
Element VONMISES EL.SXX.L
Calculated from: EL.SXX.L
Max = .406E6
Min = .531E5
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:13 pstres003
Model: S_COLHTNL
LC1: Load case 1
Step: 7 TIME: .432E5
Element VONMISES EL.SXX.L
1h
Calculated from: EL.SXX.L
Max = .774E6
Min = .156E6
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:13 pstres004
Model: S_COLHTNL
LC1: Load case 1 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:14 pstrh.ps
Step: 10 TIME: .648E5
Element VONMISES EL.SXX.L
6h
Calculated from: EL.SXX.L
Max = .808E6 Model: S_COLHTNL
Min = .224E6
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:13 pstres005 Element VONMISES EL.SXX.L
Model: S_COLHTNL Calculated from: EL.SXX.L
LC1: Load case 1
Step: 13 TIME: .864E5 Max/Min on whole graph:
Element VONMISES EL.SXX.L .8E6 Ymax = .713E6
12 h
Calculated from: EL.SXX.L
Max = .723E6 .686E6
.572E6
Ymin = .341E4
Min = Y.257E6
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:13 pstres006
.458E6 Xmax = .288E6
.344E6 Xmin = .36E4
Model: S_COLHTNL
Z
LC1: Load X
case 1 .23E6 *1E5
Step: 16 TIME: .108E6 .116E6 Variation over loadcases
Element VONMISES EL.SXX.L .15E4
.8E6
8 Element 2 Mean
18 h
Calculated from: EL.SXX.L
Max = .6E6 Min = .258E6 .686E6
.572E6
Element 11 Mean
iDIANA
Y 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:14 pstres007
.458E6
DRAWING ANIMATE LOADCASES PLOTFILE pstres .344E6
Model: S_COLHTNL
Z
LC1: Load X
case 1 .23E6 7
.8E6 Step: 19 TIME: .13E6
Element VONMISES EL.SXX.L
.116E6
.15E4
.8E6
27 h
Calculated from: EL.SXX.L
.686E6
Max = .471E6
.572E6
V
.686E6 Min = Y.243E6
iDIANA 9.4.3-02 : TNO Diana BV
Model: S_COLHTNL
Z
LC1: Load X
case 1
DRAWING ANIMATE LOADCASES PLOTFILE pstres
28 OCT 2010 01:34:14 pstres008
.458E6
.344E6
.23E6
O 6
N
Step: 22 TIME: .151E6 .116E6 M
.572E6 Element VONMISES EL.SXX.L .15E4
.8E6 I 5
30 h
Calculated from: EL.SXX.L
.686E6
Max = .384E6
Min = Y.218E6
iDIANA 9.4.3-02 : TNO Diana BV .572E6
28 OCT 2010 01:34:14 pstres009
S
.458E6 E
.458E6 Model: S_COLHTNL
Z
LC1: Load X
case 1
Step: 26 TIME: .18E6
DRAWING ANIMATE LOADCASES PLOTFILE pstres .344E6
.23E6
.116E6
S
4
Element VONMISES EL.SXX.L .15E4
E
.344E6 .8E6
36 h
Calculated from: EL.SXX.L
.686E6
Max = .279E6
Min = Y.175E6
iDIANA 9.4.3-02 : TNO Diana BV .572E6
28 OCT 2010 01:34:14 pstres010
L
DRAWING ANIMATE LOADCASES PLOTFILE pstres
.458E6 . 3
.344E6
.23E6 Model: S_COLHTNL
Z
LC1: Load X
case 1
Step: 31 TIME: .216E6
Element VONMISES EL.SXX.L
.23E6
.116E6
.15E4
.8E6
S
X
X
42 h
Calculated from: EL.SXX.L
.116E6 Max = .179E6 Min = .14E5
iDIANA
Y 9.4.3-02 : TNO Diana BV
Model: S_COLHTNL
DRAWING ANIMATE LOADCASES PLOTFILE pstres
.686E6
.572E6
28 OCT 2010 01:34:14 pstres011
.458E6
.344E6
. 2
L
.15E4 Z
LC1: Load X
case 1
Step: 44 TIME: .252E6
Element VONMISES EL.SXX.L
.23E6
.116E6
.15E4
.8E6 1
50 h
Calculated from: EL.SXX.L
Max = .135E6 .686E6
Min = Y.137E5
iDIANA 9.4.3-02 : TNO Diana BV .572E6
28 OCT 2010 01:34:14 pstres012
.458E6
DRAWING ANIMATE LOADCASES PLOTFILE pstres .344E6
Model: S_COLHTNL
Z
LC1: Load X
case 1 .23E6 0
Step: 74 TIME: .288E6 .116E6
Element VONMISES EL.SXX.L .15E4
.8E6
0 .25 .5 .75 1 1.25 1.5 1.75 2 2.25 2.5 2.75 3
60 h
Calculated from: EL.SXX.L
.686E6
Max = .268E6 Min = .14E5
.572E6
TIME *1E5
Y
.458E6
DRAWING ANIMATE LOADCASES PLOTFILE pstres .344E6
Z X .23E6
.116E6
.15E4
.8E6
s 70 h
.686E6
Y .572E6
.458E6
DRAWING ANIMATE LOADCASES PLOTFILE pstres .344E6
Z X .23E6
.116E6
.15E4
.8E6
80 h
.686E6
Y .572E6
.458E6
DRAWING ANIMATE LOADCASES PLOTFILE pstres .344E6
Z X .23E6
.116E6
.15E4
.8E6
(b) history plot
.686E6
Y .572E6
.458E6
(a) animation of contours
DRAWING ANIMATE LOADCASES PLOTFILE pstres .344E6
Z X .23E6
.116E6
.15E4
.8E6
.686E6
Y .572E6
.458E6
DRAWING ANIMATE LOADCASES PLOTFILE pstres .344E6
Z X .23E6
.116E6
.15E4
Figure 16.6: Von Mises stress
DRAWING ANIMATE LOADCASES PLOTFILE pstres
Principal stress – vector plots colhtnl.fvc
RESULTS ELEMENT EL.SXX.L SXX
RESULTS CALCULATE P-STRESS ALL
RESULTS LOADCASE LC1 10
PRESENT VECTORS
RESULTS LOADCASE LC1 16
PRESENT VECTORS
RESULTS LOADCASE LC1 44
PRESENT VECTORS
RESULTS LOADCASE LC1 74
PRESENT VECTORS
To get a better idea of the stress distribution, in particular the areas of tension
and compression, we make vector plots of the principal stresses at the most
critical times, 18 and 30 hours, and after 70 and 80 hours. Due to the P-STRESS
option iDiana will calculate the principal stresses. The step numbers 10, 16, 44,
and 74 respectively correspond with times of 18, 30, 70, and 80 hours. We make
vector plots for these times [Fig. 16.7]. We see that the altering temperature
gradients in combination with the viscoelastic behavior cause altering compres-
sion (blue) and tension zones (red). Until 70 hours there is compression near the
center and tension near the outer surface. Finally a compression stress begins to
develop near the outer surface. In the results monitors we may see the extreme
values for the stresses, as indicated in Table 16.1.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
346 Hydration of Concrete Column
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:14 str18.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:14 str30.ps
Model: S_COLHTNL Model: S_COLHTNL
LC1: Load case 1 LC1: Load case 1
Step: 10 TIME: .648E5 Step: 16 TIME: .108E6
Element PRINC STRESS ALL Element PRINC STRESS ALL
Calculated from: EL.SXX.L Calculated from: EL.SXX.L
Max = .808E6 Max = .6E6 Min = -.761E6
Min = -.632E6 Factor = .773E-7
Factor = .728E-7
Y Y
Z X .328E6 Z X .146E6
-.152E6 -.307E6
(a) after 18 hours (b) after 30 hours
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:14 str70.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:14 str80.ps
Model: S_COLHTNL Model: S_COLHTNL
LC1: Load case 1 LC1: Load case 1
Step: 44 TIME: .252E6 Step: 74 TIME: .288E6
Element PRINC STRESS ALL Element PRINC STRESS ALL
Calculated from: EL.SXX.L Calculated from: EL.SXX.L
Max = .102E6 Max = .903E5
Min = -.196E6 Min = -.267E6
Factor = .301E-6 Factor = .22E-6
Y Y
Z X .279E4 Z X -.288E5
-.964E5 -.148E6
(c) after 70 hours (d) after 80 hours
Figure 16.7: Principal stresses
Table 16.1: Extreme stresses
Time
t 18 30 70 80 h
Tension σt 0.808 0.600 0.102 0.090 MPa
Compression σc −0.632 −0.761 −0.196 −0.267 MPa
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
Chapter 17
Thermal and Flow–Stress
Analysis of a Box Girder
Name: Girder
Path: /Examples/ConcMas/Girder
Keywords: analys: flow heat nonlin transi. constr: initia temper. el-
emen: bc3ht cq8ht ct6ht flow potent. load: elemen temper
time. materi: adiaba capaci conduc hydrat isotro. option:
direct groups units. post: binary femvie. result: reacti tem-
per total. analys: flow flowst heat nonlin physic stagge transi.
constr: initia suppor temper. elemen: b2ht cq16e ct12e flow
potent pstrai q4ht t3ht. load: elemen temper time weight.
materi: adiaba capaci conduc elasti hydrat isotro shrink. op-
tion: direct groups newton regula units. post: binary femvie.
result: cauchy displa green princi reacti strain stress temper
total.
0.625 12.75 0.625
0.65
0.25
0.40
1.60
0.25
0.25
4.00 6.00 4.00
Figure 17.1: Cross-section of the box girder [m]
The objective of this example is to analyze the thermal behavior of a multi-cell
box girder [Fig. 17.1]. This kind of structure is employed for the construction
of bridges or viaducts. In our case, the box girder is made of high performance
concrete. We will perform two analyses: first a thermal flow analysis and then a
staggered flow–stress analysis. These analyses require different models: we will
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
348 Thermal and Flow–Stress Analysis of a Box Girder
first build the model for thermal analysis [§ 17.1], then we will adapt the model
for the flow–stress analysis [§ 17.3].
17.1 Model for Thermal Analysis
To build up the finite element model, we start iDiana and enter the Design
environment with the model name GIRDER.
iDiana
FEMGEN GIRDER
Analysis and Units
Analysis Selection
Model Type: →Heat Flow 2D
Units Definition
Length: →Meter
Mass: →Kilogram
Time: →Day
Temperature: →Celsius
In the Analysis and Units dialog we specify the model type for two-dimensional
heat flow analysis and the adopted units [m, kg, day, °C].
17.1.1 Geometry Definition
Due to symmetry conditions, we will just model a half part of the structure.
♥
P Q R S T
O
J K L M
H
I
2.25
G
2.00
1.60
0.25
1.35
D E F
A B C
2.60
3.00
6.375
7.00
Figure 17.2: Detailed geometry of the model [m]
Points girder.fgc
GEOMETRY POINT COORD 0
GEOMETRY POINT COORD 2.6
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
17.1 Model for Thermal Analysis 349
GEOMETRY POINT COORD 3
GEOMETRY POINT COORD 0 0.25
GEOMETRY POINT COORD 2.6 0.25
GEOMETRY POINT COORD 3 0.25
GEOMETRY POINT COORD 6.375 1.35
GEOMETRY POINT COORD 6.375 1.6
GEOMETRY POINT COORD 7 1.6
GEOMETRY POINT COORD 02
GEOMETRY POINT COORD 2.6 2
GEOMETRY POINT COORD 32
GEOMETRY POINT COORD 6.375 2
GEOMETRY POINT COORD 72
GEOMETRY POINT COORD 0 2.25
GEOMETRY POINT COORD 2.6 2.25
GEOMETRY POINT COORD 3 2.25
GEOMETRY POINT COORD 6.375 2.25
GEOMETRY POINT COORD 7 2.25
EYE FRAME
LABEL GEOMETRY POINTS
With a series of GEOMETRY POINT commands, we define the coordinates of points
A to T [Fig. 17.2]. The EYE and LABEL commands display the geometry entities
defined so far with point name labels [Fig. 17.3a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:22 geom1 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:22 geom2
Model: GIRDER Model: GIRDER
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 2D Model Type: Heat flow 2D
P15 P16 P17 P18 P19 L20 L23 L26 L28
L21 S6 L19S7 L22 S8 L25 S9 L27
P10 P11 P12 P13 P14 L18 L12 L24 L16
L17
S5
L15
P8 P9 L14
S10
L13 L9 L29
P7
S4 L10
L11 S3
L8
P4 P5 P6 L3 L7
L4 S1 L2 S2 L6
P1 P2 P3 L1 L5
Y Y
Z X Z X
(a) points (b) lines and surfaces
Figure 17.3: Geometry with labels
Surfaces girder.fgc
GEOMETRY SURFACE 4POINTS P1 P2 P5 P4
GEOMETRY SURFACE 4POINTS P2 P3 P6 P5
GEOMETRY SURFACE 4POINTS P3 P7 P8 P6
GEOMETRY SURFACE 4POINTS P5 P6 P12 P11
GEOMETRY SURFACE 4POINTS P8 P9 P14 P13
GEOMETRY SURFACE 4POINTS P10 P11 P16 P15
GEOMETRY SURFACE 4POINTS P11 P12 P17 P16
GEOMETRY SURFACE 4POINTS P12 P13 P18 P17
GEOMETRY SURFACE 4POINTS P13 P14 P19 P18
GEOMETRY SURFACE 3POINTS P8 P7 P9
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
350 Thermal and Flow–Stress Analysis of a Box Girder
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY POINTS OFF
LABEL GEOMETRY LINES ALL VIOLET
LABEL GEOMETRY SURFACES ALL BLUE
We define each surface via four corner points. We display the entire geometry
in violet, remove the point name labels, and add the line and surface labels
[Fig. 17.3b].
Sets girder.fgc
CONSTRUCT SET GIRDER APPEND ALL
CONSTRUCT SET BOUNDA APPEND LINES L1 L3 L5 L8 L10 L17 L15 L11 L13
CONSTRUCT SET BOUNDA APPEND LINES L18 L20 L23 L24 L26 L28 L27 L29
VIEW GEOMETRY GIRDER BLUE
VIEW GEOMETRY BOUNDA RED
We define two useful sets: GIRDER which contains the complete geometry, and
BOUNDA which contains all lines along the boundary of the model. For confir-
mation we display these sets in blue and red respectively [Fig. 17.4].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:22 geogir iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:22 geobou
Model: GIRDER Model: GIRDER
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 2D Model Type: Heat flow 2D
Y Y
Z X Z X
(a) girder (b) boundary
Figure 17.4: Geometry sets
17.1.2 Meshing
For the meshing we must define the coarseness and the element types.
Generation girder.fgc
MESHING DIVISION LINE ALL 6
MESHING TYPES ALL QU8 CQ8HT
MESHING TYPES S10 TR6 CT6HT
MESHING TYPES BOUNDA BE3 BC3HT
MESHING GENERATE
VIEW MESH ALL
VIEW MESH +BOUNDA RED
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
17.1 Model for Thermal Analysis 351
We define a division of 6 for all lines. Then, we choose the element types. For
the overall model, we select the 8-node quadrilateral heat flow element CQ8HT.
However, for the triangular surface S10 it is more convenient to use a triangular
element and thus we adopt the CT6HT heat flow element. The lines in set BOUNDA
are modeled with 3-node boundary elements BC3HT. We generate the mesh and
display it with the boundary elements in red [Fig. 17.5a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:22 mesh1 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:22 mesh2
Model: GIRDER Model: GIRDER
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 2D Model Type: Heat flow 2D
Y Y
Z X Z X Quality
All Tests
ASPECT
PASS
(a) colored for sets (b) colored for quality
Figure 17.5: Initial mesh
Quality check girder.fgc
VIEW HIDDEN SHADE
VIEW OPTIONS COLOUR QUALITY
VIEW MESH
We display the mesh with each element filled with color according to its quality
[Fig. 17.5b]. Elements which pass all quality criteria are filled with green. Here
we see some elements filled with yellow, indicating that these have an ‘aspect
defect’, i.e., the length to height ratio is too large. This can be solved by a mesh
refinement of the affected geometry parts.
Refinement girder.fgc
CONSTRUCT SET SELIN APPEND LINES L1 L3 L18 L20 L24 L26
MESHING DIVISION LINE SELIN 10
MESHING DIVISION LINE L8 12
MESHING DIVISION LINE L10 12
MESHING GENERATE
VIEW MESH
LABEL MESH QUALITY
We redefine some line divisions which yields a suitable mesh that passes the
quality test, i.e., all elements are green in color [Fig. 17.6a].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
352 Thermal and Flow–Stress Analysis of a Box Girder
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:22 mesh iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:23 meshma
Model: GIRDER Model: GIRDER
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 2D Model Type: Heat flow 2D
Y Y
Z X Z X
Quality Materials
All Tests MACONC
PASS MABOUN
(a) for quality (b) for materials
Figure 17.6: Final mesh, with color fill
17.1.3 Material Properties
We launch the Property Manager dialog to specify the material properties of
the model according to Table 17.1. Note that we must covert the values for λ
and K to the time unit in day.
Table 17.1: Material properties
Volumetric thermal capacity c 2675 kJ/(m3 ·K)
Thermal conductivity λ 2 W/(m·K)
Conduction coefficient K 8 W/(m2 ·K)
iDiana
View →Property Manager...
↑
Property Manager
···
We will define materials for the concrete and the boundary.
Concrete iDiana
Property Manager
↑ Materials Material Name: MACONC
↑Flow →Isotropic
↑External →External Data from File
For the heat flow elements (modeling the concrete) we specify the thermal prop-
erties in a material MACONC: conductivity λ = 172800 J/(day·m·K) and capac-
itance c = 2.675×106 J/(m3 ·K). The properties that depend on time must be
input via an external data file in Diana batch format:
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
17.1 Model for Thermal Analysis 353
concrete.dat
ADIAB 0.0 20.00
0.1 24.98
0.2 29.47
0.3 33.51
0.4 37.15
0.5 40.42
0.6 43.37
0.7 46.02
0.8 48.41
0.9 50.57
1.0 52.50
1.5 59.65
2.0 63.88
2.5 66.38
3.0 67.86
4.0 69.25
5.0 69.73
10. 70.00
60. 70.00
ARRHEN 6000.
The ADIAB data item specifies the temperature values in °C at different ages
during the development of the hydration reaction in adiabatic conditions. To
generate this series of values the following formula has been used (see JSCE [8]):
¡ ¢
Tadiab = 20 + 50 1 − exp (−1.05 t) (17.1)
The ARRHEN data item specifies the Arrhenius constant cA = 6000 K.
Boundary iDiana
Property Manager
Materials Material Name: MABOUN
↑Flow →Boundary →Convection only
For the boundary elements, we define a material MABOUN. and specify a con-
duction coefficient K = 700×103 J/(m2 ·K·day) which simulates the conduction
with the environment.
Assignment girder.fgc
PROPERTY ATTACH GIRDER MACONC
PROPERTY ATTACH BOUNDA MABOUN
VIEW OPTIONS COLOUR MATERIALS
We assign the materials to the corresponding sets of the model. As a check we
display the mesh with the elements colored according to their assigned material:
red for the concrete, orange for the boundary [Fig. 17.6b].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
354 Thermal and Flow–Stress Analysis of a Box Girder
17.1.4 Boundary and Initial Conditions
The boundary condition involves the external temperature. Moreover, we must
specify the initial temperature fields of the model.
External temperature girder.fgc
PROPERTY LOADS EXTTEMP BOUNDA 20.
VIEW HIDDEN OFF
VIEW MESH
LABEL MESH LOADS ALL RED
CONSTRUCT TCURVE TC1 LIST 0 1 30 1
PROPERTY ATTACH LOADCASE 1 TC1
The EXTTEMP load class defines an ambient temperature of 20 °C for the lines
that have been meshed with boundary elements (set BOUNDA). By default,
iDiana will consider this load as load case 1. We label the mesh with the
external temperatures of the boundary in red [Fig. 17.7a]. As we are about
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:23 meshlo iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:23 meshin
Model: GIRDER Model: GIRDER
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 2D Model Type: Heat flow 2D
20 20 20 20 20 202020 20 20 20 20 20 20 20 2020 20 20 20
20 20 20 20
20 20 20
20 20 20 20
20 20 20
20 20
20
20 20
20
2020
20 20 20
20 20 20
20 20 20
20 20
20
2020202020
20
20 2020
20
20 20 20 20
20 20 20 20
20 20 20
20 20 20 20
20 20 20
20 20
20
20 20
20
2020
20 20 20
20 20 20
20 20 20
20 202020
20
20 202020
20
20 202020
2020
20 20 20 20
20 20 20 20
20 20 20
20 20 20
20 20 20
20
2020
20
2020
2020
20
20 20 20
20 20 20
20 20 20
20 20
202020
2020202020
20
2020
20 202020
20
202020
20
20 20 20 20 20 20 20 20 20 20 20 20 20 20 20 20 20 20 20 20 20 20 20
2020
20 20
20
20 20 20 20 20 20 20 20
20
20 20
20 202020
20 20 202020
20 202020
20 202020
20
20 20 20 20 20202020 2020
20 20
202020
20
202020
20
20
20 2020
20202020
20202020
202020
20 20 20
20 20
202020
20202020
20
20 20
20 20
20 20
2020 20 20
20 202020
20 20 20
20
20 20 20 20
20 20
20 20 20202020 20 20 20
20 20 20
20 20 20 20
20 20
20 20 20
20
20 20 20
20 20 20
20 20
20 20
2020 20 20
20 20
20 20 20
20
20 20 20
20 20 20 20 20202020 20 20
20 20
20 20 20
20
20 20 20
20
20 20 20 20
20 20
20 20 20 20 20 20 20 20
20 20 20
20 20 20
20 20 20 20
20 20 20
20 20
20 20
2020 20 20
20
20 20 20
20 20 20
20 20 20
20 20 20 20
20
20 20 20
20 20
20
20 20 20 20
20
2020
20 20
20 202020 20
20 20 20 20 20 202020 20 20
20
20
20 20
20 20
20
20 20
20 20
20
20 20
20 20 20 20
20
20 20 20
20 20 20
20
20
20
20
20
20
20
20
20
20
20
20
20
20
20
Y Y
Z X Z X
(a) external for boundary elements (b) initial in nodes
Figure 17.7: Temperatures
to perform a transient analysis, we must also specify the development of the
ambient temperature in time. Here we assume a constant environmental tem-
perature. Via the TCURVE LIST options, we specify a time curve with a constant
factor 1.0 from t = 0 to 30 days. By assigning the time curve to load case 1 we
define the time dependency of the external temperature.
Initial temperature girder.fgc
PROPERTY INITIAL INITEMP ALL 20.
LABEL MESH OFF
LABEL MESH INITIAL ALL BLUE
A transient heat flow analysis requires a specified initial temperature. Via the
INITEMP class we define an initial uniform temperature of 20 °C for all nodes.
We label the mesh with the initial temperatures in blue [Fig. 17.7b].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
17.2 Transient Nonlinear Heat Flow Analysis 355
17.2 Transient Nonlinear Heat Flow Analysis
To perform the transient heat flow analysis, we must first write an input data
file in Diana batch format.
iDiana
UTILITY WRITE DIANA
yes
FILE CLOSE
yes
Thermal analysis of a box girder
ANALYSE GIRDER
Analysis Setup
···
With the ANALYSE command we launch the Analysis Setup dialog. We indicate
to perform a Transient Heat Transfer analysis with an initial degree of hydration
equal to 0.01 and an initial temperature field as defined in our data file. We
specify an analysis in 25 steps, ranging from 0.2 days at the beginning to 5 days
at the end. For each step we define a maximum of 25 iterations with an update
of the degree of reaction after each iteration. For output results, we select the
temperature and the degree of reaction. We save the commands in Diana batch
format on a file girder.dcf which looks as follows.
girder.dcf
*FILOS
INITIA
*INPUT
READ
*HEATTR
BEGIN INITIA
NONLIN HYDRAT DGRINI=0.01
TEMPER INPUT FIELD=1
END INITIA
BEGIN EXECUT
BEGIN NONLIN
HYDRAT ITERAT
ITERAT MAXITE=25
END NONLIN
SIZES 0.2(10) 0.5(6) 1(5) 5(4)
END EXECUT
BEGIN OUTPUT FEMVIEW BINARY
REACTI TOTAL INTPNT
TEMPER
END OUTPUT
*END
After termination of the analysis we enter the iDiana Results environment with
the name of the model to assess the analysis results.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
356 Thermal and Flow–Stress Analysis of a Box Girder
girder.fvc
FEMVIEW GIRDER
UTILITY TABULATE LOADCASES
The load case tabulation shows the available load cases with their available
result data. Below we show the head and tail of this tabulation.
Tabulated load cases loads.tb
;
; Model: GIRDER
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; TR1 1 TIME = .2 "Boundary case 1"
; Nodal : PTE....S
; Gauss : EL.DGR.S
;
; TR1 2 TIME = .4 "Boundary case 1"
; Nodal : PTE....S
; Gauss : EL.DGR.S
... lines skipped
; TR1 25 TIME = 30 "Boundary case 1"
; Nodal : PTE....S
; Gauss : EL.DGR.S
;
Each load case TR1 represents one time step of the transient analysis for the
indicated TIME. Attribute PTE represents the temperatures in the nodes and
DGR the degree of reaction in the Gauss points.
17.2.1 Temperature Within the Concrete
To assess the temperature we start with an outline view of the model.
girder.fvc
VIEW MESH
VIEW OPTIONS EDGES OUTLINE
RESULTS NODAL PTE....S PTE
RESULTS LOADCASE TR1 1
PRESENT CONTOUR LEVEL
We select the temperatures for the first load case (t = 0.2 days) and display
these in a contour plot [Fig. 17.8a].
Temperature evolution. We will now focus on the evolution of the temper-
ature for the warmest part of the model.
girder.fvc
VIEW OPTIONS EDGES ALL
LABEL MESH NODES /PICK
First we put back the inner grid of the mesh. With the graphics cursor (cross-
hair) we pick the node labels corresponding to the maximum temperatures, i.e.,
the red areas [Fig. 17.9].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
17.2 Transient Nonlinear Heat Flow Analysis 357
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:35 tempco
Model: GIRDER
TR1: Boundary case 1
Step: 1 TIME: .2
Nodal PTE....S PTE
Max = 27.6
Min = 23.7
27.3
26.9
26.5
26.2
Y 25.8
25.5
25.1
Z X 24.7
24.4
24
Figure 17.8: Temperature contours at time t = 0.2 days
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:35 nodes iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:35 nodes
Model: GIRDER Model: GIRDER
TR1: Boundary case 1 TR1: Boundary case 1
Step: 1 TIME: .2 Step: 1 TIME: .2
Nodal PTE....S PTE Nodal PTE....S PTE
Max = 27.6 Max = 27.6
Min = 23.7 Min = 23.7
289 289
205 205
27.3 27.3
26.9 26.9
26.5 26.5
26.2 26.2
Y 25.8 Y 25.8
25.5 25.5
25.1 25.1
Z X 24.7 Z X 24.7
24.4 24.4
24 24
(a) node 205 (b) node 289
Figure 17.9: Picking the warmest nodes
girder.fvc
RESULTS LOADCASE ALL
PRESENT OPTIONS GRAPH POINTS SYMBOLS OFF
PRESENT GRAPH NODE 205 289
We select all available load cases (time steps) and draw a graph of the evolution
of the temperature in time for the two selected nodes [Fig. 17.10]. The graphs
show that a maximum of 37 °C is reached for node 289 after about 1 day.
Animation girder.fvc
VIEW MESH
LABEL MESH OFF
VIEW OPTIONS EDGES OUTLINE
UTILITY SETUP ANIMATE LINEAR
PRESENT CONTOUR FROM 20.5 TO 34 LEVELS 8
DRAWING ANIMATE LOADCASES PLOTFILE temper
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
358 Thermal and Flow–Stress Analysis of a Box Girder
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:35 tempev
Model: GIRDER
Nodal PTE....S PTE
Max/Min on whole graph:
Ymax = 36.9
Ymin = 20.2
Xmax = 30
Xmin = .2
Variation over loadcases
Node 205
38 Node 289
36
N 34
O
D
A
L 32
P
T 30
E
.
. 28
.
.
S 26
P
T 24
E
22
20
0 2.5 5 7.5 10 12.5 15 17.5 20 22.5 25 27.5 30 32.5
TIME
Figure 17.10: Evolution of the temperature in the warmest nodes
A very instructive manner to display the temperature evolution is an anima-
tion sequence of temperature contours. We revert to a clean outline view of
the mesh. In an animation sequence of contour plots, we must be aware that
the frames of the animation all use the same levels for color representation.
Therefore, we explicitly specify the values for the first and the last contour via
the FROM....TO option. We start the animation on the screen with the DRAWING
ANIMATE LOADCASES command. Due to the PLOTFILE option we can show the
iDIANA 9.4.3-02 : TNO Diana BV
Model: GIRDER
TR1: Boundary case 1
Step: 1 TIME: .2
Nodal PTE....S PTE
28 OCT 2010 01:37:35 temper001
iDIANA 9.4.3-02 : TNO Diana BV
Model: GIRDER
TR1: Boundary case 1
Step: 2 TIME: .4
Nodal PTE....S PTE
28 OCT 2010 01:37:35 temper002
iDIANA 9.4.3-02 : TNO Diana BV
Model: GIRDER
TR1: Boundary case 1
Step: 3 TIME: .6
Nodal PTE....S PTE
28 OCT 2010 01:37:35 temper003
iDIANA 9.4.3-02 : TNO Diana BV
Model: GIRDER
TR1: Boundary case 1
Step: 4 TIME: .8
Nodal PTE....S PTE
28 OCT 2010 01:37:36 temper004
iDIANA 9.4.3-02 : TNO Diana BV
Model: GIRDER
TR1: Boundary case 1
Step: 5 TIME: 1
Nodal PTE....S PTE
28 OCT 2010 01:37:36 temper005
Max = 27.6 Max = 32.6 Max = 35.4 Min = 26 Max = 36.7 Max = 36.9
Min = 23.7 Min = 25.3 Min = 26.2 Min = 26.1
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:36 temper006
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:36 temper007
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:36 temper008
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:36 temper009
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:36 temper010
Model: GIRDER Model: GIRDER Model: GIRDER Model: GIRDER Model: GIRDER
TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1
4.8 h 9.6 h 14.4 h 19.2 h 1.0 d
Step: 6 TIME: 1.2 Step:
34 7 TIME: 1.4 Step:
34 8 TIME: 1.6 Step:
34 9 TIME: 1.8 Step:
34 10 TIME: 2 34
Nodal PTE....S PTE Nodal PTE....S PTE
32.5 Nodal PTE....S PTE
32.5 Nodal PTE....S PTE
32.5 Nodal PTE....S PTE
32.5 32.5
Max = 36.5 Max 31
= 35.6 Min = 25 Max 31
= 34.5 Max 31
= 33.3 Max 31
= 32.1 31
Min = 25.6 Min = 24.3 Min = 23.8 Min = 23.3
29.5 29.5 29.5 29.5 29.5
Y 28Y 28Y 28Y 28Y 28
26.5 26.5 26.5 26.5 26.5
25 25 25 25 25
Z X 23.5
Z X 23.5
Z X 23.5
Z X 23.5
Z X 23.5
22 22 22 22 22
20.5 20.5 20.5 20.5 20.5
DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:36 temper011
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:36 temper012
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:36 temper013
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:36 temper014
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:36 temper015
Model: GIRDER Model: GIRDER Model: GIRDER Model: GIRDER Model: GIRDER
TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1
1.2 d 1.4 d 1.6 d 1.8 d 2.0 d
Step: 11 TIME: 2.5 Step:
34 12 TIME: 3 Step:
34 13 TIME: 3.5 Step:
34 14 TIME: 4 Step:
34 15 TIME: 4.5 34
Nodal PTE....S PTE Nodal PTE....S PTE
32.5 Nodal PTE....S PTE
32.5 Nodal PTE....S PTE
32.5 Nodal PTE....S PTE
32.5 32.5
Max = 29.5 Max 31
= 27.4 Max 31
= 25.9 Max 31
= 24.7 Max 31
= 23.8 31
Min = 22.4 Min = 21.8 Min = 21.4 Min = 21.1 Min = 20.9
29.5 29.5 29.5 29.5 29.5
Y 28Y 28Y 28Y 28Y 28
26.5 26.5 26.5 26.5 26.5
25 25 25 25 25
Z X 23.5
Z X 23.5
Z X 23.5
Z X 23.5
Z X 23.5
22 22 22 22 22
20.5 20.5 20.5 20.5 20.5
DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:36 temper016
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:36 temper017
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:36 temper018
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:36 temper019
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:36 temper020
Model: GIRDER Model: GIRDER Model: GIRDER Model: GIRDER Model: GIRDER
TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1
3.5 d 3.0 d 3.5 d 4.0 d 4.5 d
Step: 16 TIME: 5 Step:
34 17 TIME: 6 Step:
34 18 TIME: 7 Step:
34 19 TIME: 8 Step:
34 20 TIME: 9 34
Nodal PTE....S PTE Nodal PTE....S PTE
32.5 Nodal PTE....S PTE
32.5 Nodal PTE....S PTE
32.5 Nodal PTE....S PTE
32.5 32.5
Max = 23.2 Max 31
= 22.3 Max 31
= 21.8 Max 31
= 21.5 Max 31
= 21.2 31
Min = 20.8 Min = 20.7 Min = 20.6 Min = 20.5 Min = 20.4
29.5 29.5 29.5 29.5 29.5
Y 28Y 28Y 28Y 28Y 28
26.5 26.5 26.5 26.5 26.5
25 25 25 25 25
Z X 23.5
Z X 23.5
Z X 23.5
Z X 23.5
Z X 23.5
22 22 22 22 22
20.5 20.5 20.5 20.5 20.5
DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:36 temper021
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:36 temper022
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:36 temper023
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:37 temper024
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:37 temper025
Model: GIRDER Model: GIRDER Model: GIRDER Model: GIRDER Model: GIRDER
TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1
5d 6d 7d 8d 9d
Step: 21 TIME: 10 Step: 34
22 TIME: 15 Step: 23 34TIME: 20 Step: 24 TIME:
34 25 Step: 25 TIME:
34 30 34
Nodal PTE....S PTE Nodal 32.5
PTE....S PTE Nodal PTE....S
32.5 PTE Nodal PTE....S
32.5 PTE Nodal PTE....S PTE
32.5 32.5
Max = 21 Min = 20.4 Max = 31
20.6 Max = 20.4
31 Max = 20.3 31 Max = 20.2 31 31
Min = 20.2 Min = 20.2 Min = 20.1 Min = 20.1
29.5 29.5 29.5 29.5 29.5
Y 28Y 28Y 28Y 28Y 28
26.5 26.5 26.5 26.5 26.5
25 25 25 25 25
Z X 23.5
Z X 23.5
Z X 23.5
Z X 23.5
Z X 23.5
22 22 22 22 22
20.5 20.5 20.5 20.5 20.5
DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper
10 d 15 d 20 d 25 d 30 d
34 34 34 34 34
32.5 32.5 32.5 32.5 32.5
31 31 31 31 31
29.5 29.5 29.5 29.5 29.5
Y Y28 Y28 Y28 Y28 28
26.5 26.5 26.5 26.5 26.5
25 25 25 25 25
Z X Z23.5 X Z23.5 X Z23.5 X Z23.5 X 23.5
22 22 22 22 22
20.5 20.5 20.5 20.5 20.5
Figure 17.11: Concrete temperature in time
DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper
frames in this document [Fig. 17.11]. Note that the darkest blue represents all
areas with a temperature below 20.5 °C. We may conclude that the model has
cooled down completely after about 20 days, which confirms the graph of the
temperature evolution [Fig. 17.10].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
17.2 Transient Nonlinear Heat Flow Analysis 359
17.2.2 Degree of Reaction
In the animation sequence we can see that the temperature reaches a maximum
value in the core of the right hand side of the box girder. On the other hand,
within the thinner parts, the increase of the temperature remains quite low.
Therefore, it is interesting to compare the development in time of the degree of
reaction for these two specific areas of the model.
girder.fvc
RESULTS LOADCASE TR1 5
PRESENT CONTOUR LEVELS
LABEL MESH ELEMENTS /PICK
We select the fifth load case, corresponding to time t = 1 day for which the
maximum value of the temperature is reached within the concrete. We display
a contour plot of the temperatures at this time, with default levels. Then we
pick the two elements for which we want to assess the degree of reaction: first
for the warmest part [Fig. 17.12a] and then for the coldest part [Fig. 17.12b].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:37 temp1d iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:37 temp1d
Model: GIRDER Model: GIRDER
TR1: Boundary case 1 TR1: Boundary case 1
Step: 5 TIME: 1 Step: 5 TIME: 1
Nodal PTE....S PTE Nodal PTE....S PTE
Max = 36.9 Max = 36.9
Min = 26.1 Min = 26.1
128 128
103 103
35.9 35.9
34.9 34.9
34 34
33 33
Y 32 Y 32
31 31
30 30
Z X 29 Z X 29
28.1 28.1
27.1 27.1
(a) warmest, element 128 (b) coldest, element 103
Figure 17.12: Picking the warmest and coldest elements at t = 1 day
girder.fvc
RESULTS GAUSSIAN EL.DGR.S DGR
RESULTS LOADCASE ALL
PRESENT GRAPH ELEMENT 128 103
We select result attribute DGR which represents the degree of reaction. For
the two selected elements we draw graphs of the development of the degree of
reaction in time for the two selected elements [Fig. 17.13]. The graphs show that
heat activates the hydration of concrete.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
360 Thermal and Flow–Stress Analysis of a Box Girder
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:37 degrea
Model: GIRDER
Gauss EL.DGR.S DGR
Max/Min on whole graph:
Ymax = .956
Ymin = .163
Xmax = 30
Xmin = .2
Variation over loadcases
Element 128 Mean
1 Element 103 Mean
.9
G
A
U .8
S
S
I .7
A
N
.6
E
L
. .5
D
G
R
. .4
S
D .3
G
R
.2
.1
0 2.5 5 7.5 10 12.5 15 17.5 20 22.5 25 27.5 30 32.5
TIME
Figure 17.13: Degree of reaction in the warmest and coldest part of the model
17.3 Model for Flow–Stress Analysis
As this model has been defined for a heat flow analysis, we must now make it
suitable for a flow–stress analysis. To adapt the model we open it in the iDiana
Design environment.
girder.fgc
FEMGEN GIRDER
PROPERTY FE-PROG DIANA HTSTAG PE
yes
With the HTSTAG PE option we indicate that the model will be applied for stag-
gered flow–stress analysis in a plane strain configuration. Due to the change of
the model type, iDiana warns us that all element type assignments along with
all analysis specific data will be removed. We confirm this deleting operation.
When you change the analysis type iDiana will remove the mesh,
the materials and the loads.
17.3.1 Meshing
As iDiana has removed the mesh, we must remesh the model for flow–stress
analysis. This requires the application of plane strain elements for the stress
analysis and boundary elements for the potential flow analysis.
Plane strain elements girder.fgc
MESHING TYPES GIRDER QU8 CQ16E
MESHING TYPES S10 TR6 CT12E
We change the element types adopted in the previous heat flow analysis to the
quadratic plane strain elements CQ16E and CT12E.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
17.3 Model for Flow–Stress Analysis 361
Boundary elements. A complication with respect to the modeling of bound-
ary elements for staggered flow–stress analysis is that these elements are linearly
interpolated, i.e., they have no mid-side nodes. Indeed, for the flow part of the
staggered analysis, Diana will internally convert quadratic structural elements
to linear heat flow elements and thus will not consider mid-side nodes for the
potential flow analysis. However, in the Design environment of iDiana, where
we must build the complete model, the meshing procedure would not allow the
incompatibility of elements. We must find a work-around solution for this prob-
lem. The trick is to copy the set of lines along the boundary by translation over
a virtual distance.
girder.fgc
CONSTRUCT SPACE TOLERANCE OFF
GEOMETRY COPY BOUNDA OUTER TRANSLATE 0 0 0
MESHING TYPES OUTER BE2 B2HT
MESHING DIVISION FACTOR OUTER .5
MESHING GENERATE
VIEW MESH ALL
VIEW MESH +OUTER RED
VIEW OPTIONS SHRINK
We copy the set BOUNDA to a new set OUTER where the TRANSLATE option
indicates a zero distance. Without corrective action, iDiana would not have
created new lines and points because any new point would exactly coincide with
an existing point. To force the creation of new points and lines we switch off
the tolerance check. We assign the B2HT element type to the lines of set OUTER.
Note that the lines in this set have got their divisions from their originators
during the copy action. So here we may simply halve the number of divisions
via the FACTOR option. Finally we generate the mesh and display it in ‘shrunken
element’ style [Fig. 17.14].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:27 meshc.ps
Model: GIRDER
Analysis: DIANA
Model Type: Heatflow-Stress Staggered plane strain
Z X
Figure 17.14: Generated mesh
Merging the mesh. Although the mesh seems to be correct we still have to
make one final correction. Since the lines in the set OUTER have no common
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
362 Thermal and Flow–Stress Analysis of a Box Girder
points with the lines in the set BOUNDA, the generated boundary elements will
not be automatically connected to the structural part.
girder.fgc
EYE ZOOM FACTOR 12 -2.7 1.5
LABEL MESH NODES
MESHING MERGE ALL 0.001
DRAWING DISPLAY
We zoom on the top left hand side part of the model and label the nodes with
their numbers [Fig. 17.15a]. Looking at the end nodes of the boundary elements,
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:27 meshza.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:27 meshzb.ps
Model: GIRDER Model: GIRDER
Analysis: DIANA Analysis: DIANA
Model Type: Heatflow-Stress Staggered plane strain Model Type: Heatflow-Stress Staggered plane strain
322
52 361 323
51 52 309 51
355 356 303 304
316 350 317 270 298 271
344 345 292 293
310 339 311 264 287 265
333 334 281 282
42
305 328 43
306 42 276 43
Y Y
Z X Z X
(a) before merging (b) after merging
Figure 17.15: Merging the mesh for nodes
we see overlapping numbers: one node for the boundary element and another
one for the structural element, indicating that there is no connection. To solve
this problem we apply a merging operation on the mesh. The parameter value
0.001 indicates a tolerance of one millimeter for the check on coinciding nodes.
A second display of node labels now shows one single node at the end of each
boundary element [Fig. 17.15b].
17.3.2 Material Properties
We may now launch the Property Manager dialog to specify the material prop-
erties for the various components of the model.
iDiana
View →Property Manager...
↑
Property Manager
···
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
17.3 Model for Flow–Stress Analysis 363
Concrete iDiana
Property Manager
↑ Materials Material Name: MACONC
↑Flow →Isotropic
↑Expansion →Isotropic-constnt params.
↑Linear elasticity →Predefined concrete classes
↑External →External Data from File
For the box girder, we define the same thermal material properties as for the first
case study in a material named MACONC [§ 17.1.3 p. 352]: a thermal conductivity
λ = 173×103 J/(day·m·K) and a thermal capacity c = 2675×103 J/(m3 ·K).
For this example, we must specify additional material properties for the linear
elastic behavior of the concrete [Table 17.2]. We specify the value of the thermal
Table 17.2: Material properties for concrete
Thermal expansion coefficient α 1.2×10−5
Concrete class CEB-FIP C30
Young’s modulus E ≈17000 MPa
expansion coefficient. Furthermore we specify the basic elastic properties from
the Model Code Regulations for concrete. where we choose the CEB-FIP model
Code and a C30-class concrete. However, as we are about to study the behavior
of young hardening concrete, the proposed value for Young’s modulus E =
34000 MPa is too large. As a first approximation, we divide it by 2 and input
E = 17000 MPa. For the concrete, we must also specify the development of the
autogenous shrinkage with time. This dependency must be added to the data
file in Diana batch format.
concrete2.dat
ADIAB 0.0 20.00
0.1 24.98
0.2 29.47
0.3 33.51
0.4 37.15
0.5 40.42
0.6 43.37
0.7 46.02
0.8 48.41
0.9 50.57
1.0 52.50
1.5 59.65
2.0 63.88
2.5 66.38
3.0 67.86
4.0 69.25
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
364 Thermal and Flow–Stress Analysis of a Box Girder
5.0 69.73
10. 70.00
80. 70.00
ARRHEN 6000.
SHRINF 6.62E-06 1.07E-05 1.40E-05 1.70E-05 1.98E-05 3.11E-05
4.03E-05 4.82E-05 5.51E-05 6.14E-05 6.71E-05 7.24E-05
7.73E-05 8.19E-05 1.01E-04 1.16E-04 1.28E-04 1.37E-04
SHTIME 0.2 0.4 0.6 0.8 1.0 2.0
3.0 4.0 5.0 6.0 7.0 8.0
9.0 10. 15. 20. 25. 30.
The SHRINF data item specifies the shrinkage strains εsh at the respective con-
crete age t given in SHTIME (ranging from 0 to 30 days). To generate this series
of shrinkage values, the following formula has been used (see JSCE [8]):
³ 0.7
´
εsh = 207.7 1 − exp−0.1 t ×10−6 (17.2)
The external data file concrete2.dat for concrete material properties is now
complete and we may supply its name to iDiana via the Property Manager
dialog.
Boundary iDiana
Property Manager
Materials Material Name: MABOUN
↑Flow →Boundary →Convection only
For the boundary elements, we define a material MABOUN with the same a
conduction coefficient as for the flow analysis: K = 700×103 J/(m2 ·K·day).
Assignment girder.fgc
PROPERTY ATTACH GIRDER MACONC
PROPERTY ATTACH OUTER MABOUN
We assign the materials to the corresponding sets of the model.
17.3.3 Flow Boundary and Initial Conditions
Like for the flow analysis we specify the external temperature and the initial
temperature field of the model.
External and initial temperature girder.fgc
PROPERTY LOADS EXTTEMP OUTER 20
PROPERTY ATTACH LOADCASE 1 TC1
PROPERTY INITIAL INITEMP ALL 20
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
17.3 Model for Flow–Stress Analysis 365
17.3.4 Mechanical Loading and Boundary Constraints
For the flow–stress analysis we must also specify the mechanical loading, which
consists of the dead weight, and the boundary constraints.
Dead weight girder.fgc
PROPERTY LOADS GRAVITY 2 ALL -9.81E-6 Y
CONSTRUCT TCURVE TC2 LIST 0 0 7 0 7.1 1 60 1
UTILITY GRAPH TCURVE TC2
PROPERTY ATTACH LOADCASE 2 TC2
For the nonlinear structural analysis, we define the dead weight of the model via
the GRAVITY load class. We specify it as load case 2. The gravity acceleration
g = 9.81×10−6 MN/kg acts downward, i.e., in the Y -direction. However, we
suppose that the box girder will stand its dead weight at a later age of 7 days.
Via the TCURVE LIST option, we specify a time curve as a unit step function with
a factor 0 from t = 0 to 7 days and a factor 1 from t = 7 to 30 days [Fig. 17.16a].
We assign the created time curve TC2 to load case 2 and thus define the time
dependency for the dead weight.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:28 tcwei.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:28 mesup.ps
Model: GIRDER Model: GIRDER
Analysis: DIANA Analysis: DIANA
Model Type: Heatflow-Stress Staggered plane strain Model Type: Heatflow-Stress Staggered plane strain
TCURVE : TC2
1.2
.8
V
A
L
U .6
E
.4
.2
0
0 10 20 30 40 50 60 70
TIME Y
Z X
(a) time curve for dead weight (b) mechanical supports
Figure 17.16: Load and supports for structural analysis
Boundary constraints girder.fgc
VIEW GEOMETRY GIRDER
EYE FRAME ALL
LABEL GEOMETRY LINES
LABEL GEOMETRY POINTS
PROPERTY BOUNDARY CONSTRAINT L4 X
PROPERTY BOUNDARY CONSTRAINT L21 X
PROPERTY BOUNDARY CONSTRAINT P3 Y
VIEW MESH ALL
LABEL MESH CONSTRNT
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
366 Thermal and Flow–Stress Analysis of a Box Girder
The boundary constraints of the model consist of a symmetry condition along
the left edge and a vertical support on point C [Fig. 17.2 p. 348]. To specify these
constraints correctly we display the point and line labels in the geometry of the
model. For the symmetry condition we suppress the horizontal displacement on
the lines along the left edge. The vertical support is applied to the appropriate
point of the geometry. The display of the mesh with labeled constraints confirms
the correct specification [Fig. 17.16b].
17.4 Staggered Flow–Stress Analysis
To perform the staggered flow–stress analysis we write an input data file in
Diana batch format. Then, we may start the analysis.
iDiana
UTILITY WRITE DIANA girder2
FILE CLOSE
yes
Flow-stress analysis of a box girder
ANALYSE GIRDER2
Analysis Setup
···
The ANALYSE command initiates the analysis of the model named GIRDER2. Via
the Analysis Setup dialog, we run a Transient Heat Transfer analysis with ap-
propriate options. When this analysis is terminated, we choose to perform a
subsequent analysis. Using the same Filos file we change the analysis type to
Structural Nonlinear. In the Analysis Setup dialog we may specify the vari-
ous analysis options for the mechanical analysis. These operations should be
equivalent to the following batch analysis commands.
girder2.dcf
*FILOS
INITIA
*INPUT
*HEATTR
BEGIN INITIA
NONLIN HYDRAT DGRINI=0.01
TEMPER INPUT FIELD=1
END INITIA
BEGIN EXECUT
BEGIN NONLIN
HYDRAT ITERAT
ITERAT MAXITE=30
END NONLIN
SIZES 0.2(10) 0.5(6) 1(5) 5(4)
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
17.4 Staggered Flow–Stress Analysis 367
END EXECUT
BEGIN OUTPUT FEMVIE BINARY
FILE GIRDER
REACTI TOTAL INTPNT
TEMPER
END OUTPUT
*NONLIN
BEGIN EXECUT
TIME STEPS EXPLIC SIZES 0.2(10) 0.5(6) 1(5) 5(4)
ITERAT CONVER SIMULT
END EXECUT
BEGIN OUTPUT FEMVIE BINARY
FILE GIRDER2
DISPLA
STRAIN TEMPER
STRESS
STRESS TOTAL CAUCHY PRINCI
TEMPER
END OUTPUT
*END
The *HEATTR command invokes module heattr for a transient heat flow anal-
ysis. This module automatically adapts the finite element model for heat flow
analysis: the CQ16E and CT12E elements will be changed respectively to Q4HT
and T3HT elements. The commands are the same as for heat flow analysis
and they have already been commented [§ 17.2 p. 355]. To perform the nonlin-
ear structural analysis, we invoke module nonlin. This module automatically
transforms the heat flow model to a structural model: the Q4HT and T3HT re-
spectively revert to CQ16E and CT12E elements. The B2HT boundary elements
will be deactivated and the temperature values resulting from the previous flow
analysis will be transformed to an internal time–temperature table for struc-
tural analysis. In the Analysis Setup dialog we only have to specify options
for the actual structural analysis. For output we select for all time steps, the
displacement, the stresses and their transformation in the principal stress space,
the strains and the temperatures. As soon as the analysis run is terminated, we
enter the iDiana Results environment to assess the results.
girder2.fvc
FEMVIEW GIRDER2
UTILITY TABULATE LOADCASES
RESULTS LOADCASE ALL
The load case tabulation shows the available load cases (time steps) with their
result data.
Tabulated load cases loadfs.tb
;
; Model: GIRDER2
;
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
368 Thermal and Flow–Stress Analysis of a Box Girder
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; LC2 1 TIME = .2 "Load case 2"
; Nodal : TDTX...G
; Element : EL.ETMPG EL.SXX.G EL.S1 EL.TE..S
;
; LC2 2 TIME = .4 "Load case 2"
; Nodal : TDTX...G
; Element : EL.ETMPG EL.SXX.G EL.S1 EL.TE..S
... lines skipped
; LC2 25 TIME = 30 "Load case 2"
; Nodal : TDTX...G
; Element : EL.ETMPG EL.SXX.G EL.S1 EL.TE..S
;
We recognize the various result attributes: TDTX the total displacement, EL.ETMPS
the thermal strain, EL.SXX the stress, EL.S1 the principal stress, and EL.TE tem-
perature extrapolated to the element nodes. We select all available load cases
to start the result presentation.
17.4.1 Thermal Strain
We will now assess the thermal strain distribution over the model and its de-
velopment in time.
girder2.fvc
RESULTS ELEMENT EL.ETMPG ETMPXX
UTILITY SETUP ANIMATE LINEAR
PRESENT CONTOUR FROM 0 TO 1.8E-4 LEVELS 8
VIEW OPTIONS DEFORM USING TDTX...G RESTDT 500
DRAWING ANIMATE LOADCASES PLOTFILE epsth
We set up an animation sequence for the thermal strains of all time steps
[Fig. 17.17]. Via the DEFORM option we get all results displayed in the de-
formed model. It is interesting to notice that the largest thermal strains occur
in the thicker parts of the model. Also note that when the dead weight starts
to act, after seven days, the thermal strain development has almost come to an
end.
17.4.2 Principal Stress
We will now assess at the effect of the dead weight on the major principal stress.
After 7 days girder2.fvc
VIEW OPTIONS DEFORM OFF
RESULTS ELEMENT EL.S1 S1
RESULTS LOADCASE LC2 18
PRESENT CONTOUR FROM 0 TO 1.4 LEVELS 6
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
17.4 Staggered Flow–Stress Analysis 369
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth001 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth002 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth003 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth004 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth005
Model: GIRDER2 Model: GIRDER2 Model: GIRDER2 Model: GIRDER2 Model: GIRDER2
Deformation = 500 Deformation = 500 Deformation = 500 Deformation = 500 Deformation = 500
LC2: Load case 2 LC2: Load case 2 LC2: Load case 2 LC2: Load case 2 LC2: Load case 2
Step: 1 TIME: .2 Step: 2 TIME: .4 Step: 3 TIME: .6 Step: 4 TIME: .8 Step: 5 TIME: 1
Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX
Max = .924E-4 Max = .152E-3 Max = .184E-3 Max = .198E-3 Max = .199E-3
Min = .458E-4 Min = .654E-4 Min = .736E-4 Min = .757E-4 Min = .714E-4
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth006 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth007 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth008 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth009 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth010
4.8 h 9.6 h 14.4 h 19.2 h 1.0 d
Model: GIRDER2 Model: GIRDER2 Model: GIRDER2 Model: GIRDER2 Model: GIRDER2
Deformation
Y = 500 Deformation
Y = 500 Deformation
Y = 500 Deformation
Y = 500 Deformation
Y = 500
LC2: Load case 2 LC2: Load case 2 LC2: Load case 2 LC2: Load case 2 LC2: Load case 2
Step: 6 TIME: 1.2 Step: 7 TIME: 1.4 Step: 8 TIME: 1.6 Step: 9 TIME: 1.8 Step: 10 TIME: 2
Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX
Max = Z.192E-3
X Max = Z.181E-3
X Max = Z.168E-3
X Max = Z.153E-3
X Max = Z.138E-3
X
Min = .631E-4 Min = .549E-4 Min = .475E-4 Min = .411E-4 Min = .356E-4
DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth011 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth012 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth013 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth014 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth015
1.2 d 1.4 d 1.6 d 1.8 d 2.0 d
Model: GIRDER2 Model: GIRDER2 Model: GIRDER2 Model: GIRDER2 Model: GIRDER2
Deformation
Y = 500 Deformation
Y = 500 Deformation
Y = 500 Deformation
Y = 500 Deformation
Y = 500
LC2: Load case 2 LC2: Load case 2 LC2: Load case 2 LC2: Load case 2 LC2: Load case 2
Step: 11 TIME: 2.5 Step: 12 TIME: 3 Step: 13 TIME: 3.5 Step: 14 TIME: 4 Step: 15 TIME: 4.5
Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX
Max = Z.107E-3
X Max = Z.833E-4
X Max = Z.654E-4
X Max = Z.522E-4
X Max = Z.425E-4
X
Min = .264E-4 Min = .193E-4 Min = .147E-4 Min = .12E-4 Min = .103E-4
DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth016 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth017 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth018 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:48 epsth019 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:49 epsth020
3.5 d 3.0 d 3.5 d 4.0 d 4.5 d
Model: GIRDER2 Model: GIRDER2 Model: GIRDER2 Model: GIRDER2 Model: GIRDER2
Deformation
Y = 500 Deformation
Y = 500 Deformation
Y = 500 Deformation
Y = 500 Deformation
Y = 500
LC2: Load case 2 LC2: Load case 2 LC2: Load case 2 LC2: Load case 2 LC2: Load case 2
Step: 16 TIME: 5 Step: 17 TIME: 6 Step: 18 TIME: 7 Step: 19 TIME: 8 Step: 20 TIME: 9
Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX
Max = Z.353E-4
X Max = Z.264E-4
X Max = Z.207E-4
X Max = Z.169E-4
X Max = Z.142E-4
X
Min = .92E-5 Min = .773E-5 Min = .663E-5 Min = .575E-5 Min = .502E-5
DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:49 epsth021
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:49 epsth022
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:49 epsth023
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:49 epsth024
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:49 epsth025
5d 6d 7d 8d 9d
Model: GIRDER2 Model: GIRDER2 Model: GIRDER2 Model: GIRDER2 Model: GIRDER2
Deformation
Y = 500 Deformation
Y = 500 DeformationY = 500 Deformation =Y 500 Deformation = 500
Y
LC2: Load case 2 LC2: Load case 2 LC2: Load case 2 LC2: Load case 2 LC2: Load case 2
Step: 21 TIME: 10 Step: 22 TIME: 15 Step: 23 TIME: 20 Step: 24 TIME: 25 Step: 25 TIME: 30
Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX Element EL.ETMPG ETMPXX
Max = Z.121E-4
X Z
Max = .721E-5 X Z
Max = .472E-5 X Max = .318E-5Z X Max = .216E-5 Z X
Min = .442E-5 Min = .267E-5 Min = .177E-5 Min = .121E-5 Min = .826E-6
DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth
Z X 10 d Y
Z X 15 d Y
Z X 20 d Y
Z X 25 d Y
Z X 30 d
DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth DRAWING ANIMATE LOADCASES PLOTFILE epsth
Figure 17.17: Thermal strains and deformation in time
Via the S1 result attribute we select the first principal stress. We choose load
case 18 which corresponds to time t = 7 days, just before the application of the
dead weight. The PRESENT command gives the contour plot We draw a contour
plot with explicitly specified level values [Fig. 17.18a]. In the results monitor we
see that the largest values obtained are around 0.13 MPa. These occur near the
exchanging surfaces of the thicker part of the model.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:49 sigp1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:49 sigp2.ps
Model: GIRDER2 Model: GIRDER2
LC2: Load case 2 LC2: Load case 2
Step: 18 TIME: 7 Step: 19 TIME: 8
Element EL.S1 S1 Element EL.S1 S1
Max = .126 Max = 1.95
Min = -.332E-1 Min = -.607
1.4 1.4
1.2 1.2
Y 1 Y 1
.8 .8
.6 .6
Z X .4 Z X .4
.2 .2
0 0
(a) at t = 7 days (b) at t = 8 days
Figure 17.18: First principal stress
After 8 days girder2.fvc
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
370 Thermal and Flow–Stress Analysis of a Box Girder
RESULTS LOADCASE LC2 19
DRAWING DISPLAY
We select load case 19 which corresponds to time t = 8 days, just after the
application of the dead weight. The DRAWING DISPLAY command updates the
current view [Fig. 17.18b]. Note that the dead weight considerably increases the
major principal stress up to 1.95 MPa.
17.4.3 Longitudinal Stress
From the animation sequence of the temperature in the thermal analysis [Fig. 17.11
p. 358] we saw that the temperature reached a maximum value in the core of the
right hand side of the box girder. On the other hand, within the thinner parts,
the increase of temperature remained quite low. Therefore, it is interesting to
compare the development in time of the longitudinal stress for these two specific
areas of the model.
girder2.fvc
VIEW MESH
VIEW OPTIONS EDGES OUTLINE
LABEL MESH ELEMENTS VIEWMODE RED
RESULTS LOADCASE ALL
RESULTS ELEMENT EL.SXX.G SZZ
PRESENT GRAPH ELEMENT 80 125
On a new model display we label the elements with their number in red [Fig. 17.19-
a]. We determine the elements in the areas with extreme temperatures. We se-
lect for all load cases, the SZZ stress result attribute. For this result we display
two graphs: one for each element [Fig. 17.19b].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:49 elmsfs.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:49 gszz.ps
Model: GIRDER2 Model: GIRDER2
Element EL.SXX.G SZZ
Max/Min on whole graph:
Ymax = 2.18
Ymin = -3.22
Xmax = 30
Xmin = .2
Variation over loadcases
Element 80 Mean
3 Element 125 Mean
2
140 141 142 143 144 151
152
153 164 165 166 167 168 175176177 E
135 136 137 138 139 148
149
150 159 160 161 162 163 172173174 L
130 131 132 133 134 145
146
147 154 155 156 157 158 169170171 E
127128129 M 1
124125126 E
118
119
120 121122123 N
178183
179 186
184 T
111 180185
181
105 182 0
99 E
110 L 0 2.5 5 7.5 10 12.5 15 17.5 20 22.5 25 27.5 30 32.5
115
116
117 104
98 .
109 S -1
103
97 X
108 X
102
107 96 .
112
113
114
101 G
95 -2
106
80 81 82 83 84 919293 100 S
75 76 77 78 79 888990 94 Z
70 71 72 73 74 858687 Z
-3
-4
TIME
Y
Z X
Figure 17.19: Evolution of the longitudinal stress σZZ
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
Chapter 18
Wall with Cooling Pipes
Name: Walcoo
Path: /Examples/ConcMas/Walcoo
Keywords: analys: flow heat nonlin transi. constr: initia temper. el-
emen: bq4ht coolpi flow hx8ht l2ht potent. load: elemen
temper time. materi: adiaba capaci conduc hydrat isotro. op-
tion: direct groups units. post: binary femvie. pre: append
femgen. result: equage inttmp reacti temper total.
1.00
2.50
out
Z
Y
X
5.00
in
Figure 18.1: Geometry of wall with cooling pipes [m]
This example provides an introduction to the application of Diana’s cooling
pipe elements. The studied structure is a concrete wall with a cooling circuit
[Fig. 18.1]. This structure is 5 m long and has a thickness of 1 m and a height
of 4.8 m. Figure 18.2 shows a detailed description of the cooling pipe positions,
along with adopted boundary conditions.
18.1 Finite Element Model
To build the finite element model for this example, we start iDiana and enter
the Design environment with the name of the model: WALL.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
372 Wall with Cooling Pipes
convective exchange
0.90
2.50
4×0.40
Z Z
X q=0 Y q=0
0.20 4.60 0.20
5.00 q is boundary flux
Figure 18.2: Wall cross-sections [m]
iDiana
FEMGEN WALL
Analysis and Units
Analysis Selection
Model Type: →Heat Flow 3D
Units Definition
Length: →Meter
Time: →Day
Temperature: →Celsius
In the dialog Analysis and Units we indicate that the model is for a three-di-
mensional heat flow analysis. We also specify the adopted units for the analysis
[m, day, °C].
18.1.1 Geometry Definition
We will define the geometry in two parts: first the wall and then the cooling
pipes.
18.1.1.1 Wall
We start by defining the geometry of the bottom surface of the concrete wall.
For a better understanding of the model description, we present a top view of
the concrete wall [Fig. 18.3].
Bottom points wall.fgc
GEOMETRY POINT COORD 0
GEOMETRY POINT COORD .2
GEOMETRY POINT COORD 4.8
GEOMETRY POINT COORD 5
GEOMETRY POINT COORD 0 .5
GEOMETRY POINT COORD .2 .5
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
18.1 Finite Element Model 373
I J K
L
0.50
E F G
H
Y
0.50
A B C
D
X
0.20 4.60 0.20
Figure 18.3: Top view of the concrete wall [m]
GEOMETRY POINT COORD 4.8 .5
GEOMETRY POINT COORD 5 .5
GEOMETRY POINT COORD 0 1
GEOMETRY POINT COORD .2 1
GEOMETRY POINT COORD 4.8 1
GEOMETRY POINT COORD 5 1
EYE FRAME ALL
VIEW GEOMETRY ALL BLUE
LABEL GEOMETRY POINTS
We define the coordinates of points A to L. All points of the bottom surface of
the concrete wall are located in the XY -plane, i.e., Z-coordinates are equal to
zero. We may omit them in the definition of the geometrical points. We label
the specified points with their names and fitted in the viewport [Fig. 18.4a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:38 geom1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:38 geom2.ps
Model: WALL Model: WALL
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 3D Model Type: Heat flow 3D
P9 P10 P11 P12 L12 L15 L17
L13
S4 S5 S6
L11 L14 L16
P5 P6 P7 P8 L3 L7 L10
L4
S1 S2 S3
L2 L6 L9
P1 P2 P3 P4 L1 L5 L8
Y Y
Z X Z X
(a) points (b) lines and surfaces
Figure 18.4: Geometry of wall bottom
Bottom surfaces wall.fgc
GEOMETRY SURFACE 4POINTS P1 P2 P6 P5
GEOMETRY SURFACE 4POINTS P2 P3 P7 P6
GEOMETRY SURFACE 4POINTS P3 P4 P8 P7
GEOMETRY SURFACE 4POINTS P5 P6 P10 P9
GEOMETRY SURFACE 4POINTS P6 P7 P11 P10
GEOMETRY SURFACE 4POINTS P7 P8 P12 P11
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
374 Wall with Cooling Pipes
CONSTRUCT SET BOTWAL APPEND ALL
VIEW GEOMETRY ALL BLUE
LABEL GEOMETRY LINES ALL RED
LABEL GEOMETRY SURFACES ALL BLUE
We create six surfaces in the bottom of the wall. Their geometry components
are assembled in a set BOTWAL. Finally, we display the line labels for the current
geometry [Fig. 18.4b].
Bottom sets and divisions wall.fgc
CONSTRUCT SET SELIN1 APPEND LINES L1 L3 L12 L17 L10 L8
CONSTRUCT SET SELIN2 APPEND LINES L5 L7 L15
MESHING DIVISION LINE ALL 2
MESHING DIVISION LINE SELIN1 1
MESHING DIVISION LINE SELIN2 8
We define some sets containing lines for which we want to have the same division.
Sets SELIN1 and SELIN2 contain all the lines in the X-direction. Then we specify
the line division to be applied in each set.
Sweeping the bottom wall.fgc
LABEL GEOMETRY OFF
EYE ROTATE TO 41 30 30
GEOMETRY SWEEP BOTWAL MID1 2 TRANSLATE 0 0 .4
GEOMETRY SWEEP MID1 MID2 2 TRANSLATE 0 0 .4
GEOMETRY SWEEP MID2 MID3 2 TRANSLATE 0 0 .4
GEOMETRY SWEEP MID3 MID4 2 TRANSLATE 0 0 .4
GEOMETRY SWEEP MID4 TOPWAL 3 TRANSLATE 0 0 .9
EYE FRAME ALL
CONSTRUCT SET WALL APPEND ALL
VIEW GEOMETRY WALL BLUE
To prepare ourselves for the transformation to a three-dimensional model, we
choose an appropriate eye point [Fig. 18.5a]. Then we sweep, translate through
space, the original profile BOTWAL to create a body. This operation is repeated
several times in order to create geometrical entities for each plane containing
cooling pipes (sets MID1 to MID4). We also create the top plane which is defined
as set TOPWAL. For each sweeping operation we define the division for created
lines in the Z-direction. All the geometry entities created so far are put together
in the set WALL [Fig. 18.5b].
18.1.1.2 Cooling Pipes
From the previously created geometry entities we will now pick up the lines
corresponding to the cooling pipe discretization. As the cooling pipes are located
in the vertical mid-plane of the wall we will apply one half of the wall.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
18.1 Finite Element Model 375
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:38 geomw0.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:38 geomw1.ps
Model: WALL Model: WALL
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 3D Model Type: Heat flow 3D
Z Z
Y Y
X X
(a) bottom surfaces (b) swept to bodies
Figure 18.5: Making the three-dimensional geometry of the wall
Right hand side of wall wall.fgc
LABEL GEOMETRY BODIES
CONSTRUCT SET RIGWAL APPEND BODIES B4 B5 B6 B10 B11 B12 B16 B17 B18
CONSTRUCT SET RIGWAL APPEND BODIES B22 B23 B24 B28 B29 B30
VIEW GEOMETRY RIGWAL
LABEL GEOMETRY LINES CURRENT RED
We display the body labels and create a set RIGWAL containing the geometrical
entities of the right hand side part of the wall. Then we display the line labels
in red [Fig. 18.6a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:38 geom3.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:38 geom4.ps
Model: WALL Model: WALL
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 3D L146L145 Model Type: Heat flow 3D
L144
L136
L159
L160
L155
L117L116
L156
L130
L115
L107 L131
L88 L87
L126
L101
L127
L78L86 L102
L59 L58 L148
L97
L98L72
L49L57 L73
L30 L29 L140
L68
L69L43
L20L28 L44
L13 L12
L39
L40 L119 L150
L3 L11 L147
L111 L149
L143
L90
L161
L82 L162
L61
L157
L158 L121
L53 L118L132
L32 L120L133
L114
L92
L24 L128
L89 L103
L15 L129
L85L91 L104
L63
L7 L99
L60 L74
L100
L56L62 L75
L34
L70
L31 L45
L71
L27L33 L46
L17
L41
L14
L42
Z L10L16 Z
Y Y
X X
(a) right hand side (b) full, with cooling pipes
Figure 18.6: Geometry display of wall
Lines of cooling pipes wall.fgc
CONSTRUCT SET OPEN COOLPI
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
376 Wall with Cooling Pipes
CONSTRUCT SET APPEND LINES L27 L24 L69 L53 L99 L82 L127 L111 L114
CONSTRUCT SET CLOSE
VIEW GEOMETRY WALL
VIEW GEOMETRY +COOLPI RED
We construct set COOLPI by picking up the appropriate lines. Finally, we display
the geometry of the cooling pipes in red in the complete geometry of the wall
[Fig. 18.6b].
18.1.2 Meshing
We may now create a finite element mesh on the defined geometry. The mesh
consists not only of the wall with cooling pipes but also comprises the boundary
of the wall.
18.1.2.1 Wall and Cooling Pipes
wall.fgc
MESHING TYPES WALL HE8 HX8HT
MESHING TYPES COOLPI BE2 L2HT
MESHING GENERATE
VIEW MESH
VIEW HIDDEN SHADE
We select the HE8 generic element type and the linear HX8HT heat flow element
for the set WALL of the model. For the cooling pipes, we select the BE2 generic
element type and the linear L2HT cooling pipe element. We generate the mesh
and display it in the hidden shade style [Fig. 18.7a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:38 mesh1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:39 mesh2.ps
Model: WALL Model: WALL
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 3D Model Type: Heat flow 3D
Z Z
Y Y
X X
(a) wall (b) boundary
Figure 18.7: Finite element mesh
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
18.1 Finite Element Model 377
18.1.2.2 Boundary Elements
We must describe the heat convection along the outside surfaces of the concrete
structure. We start by defining all the concerned surfaces of the geometry.
Selection wall.fgc
VIEW GEOMETRY ALL WHITE
VIEW HIDDEN OFF
EYE ROTATE TO 0
CONSTRUCT SET BOUNDA APPEND CURSOR POLYGON
CONSTRUCT SET BOUNDA APPEND TOPWAL
First we display the geometry in the default style. Then, we rotate the model
to get its top view in the XY -plane. We create a set BOUNDA using the CURSOR
POLYGON option. By drawing a polygon as shown in Figure 18.8, we append in
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:38 polygon.ps
Model: WALL
Analysis: DIANA
Model Type: Heat flow 3D
Z X
Figure 18.8: Cursor selection with a polygon
this set all the surfaces that lie within this polygon. Finally, we append to the
set BOUNDA the top surface TOPWAL of the model with another CONSTRUCT SET
command.
Meshing wall.fgc
MESHING TYPES BOUNDA QU4 BQ4HT
MESHING GENERATE
VIEW MESH BOUNDA
EYE ROTATE TO 41 30 30
VIEW OPTIONS SHRINK
We select the QU4 generic element type and the linear BQ4HT heat flow boundary
element for the set BOUNDA of our model. We regenerate the mesh and display
the mesh of the boundaries in the ‘shrunken element’ style [Fig. 18.7b].
18.1.3 Materials and Physical Properties
We must now specify the material and physical properties for the different com-
ponents of our model. We launch the Property Manager dialog.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
378 Wall with Cooling Pipes
iDiana
View Property Manager...
↑ →
Property Manager
···
We must define the properties of the concrete, the boundary elements and the
cooling pipes.
18.1.3.1 Concrete
For this example we adopt the parameter values for the thermal behavior of the
concrete according to Table 18.1.
Table 18.1: Thermal properties of concrete
Thermal conductivity λ 173×103 J/(m·K·day)
Thermal capacity c 2675×103 J/(m3 ·K)
Arrhenius constant cA 5000 K
Boundary conduction coefficient K 700×103 J/(m2 ·K·day)
iDiana
Property Manager
↑ Materials Material Name: MAWALL
↑Flow →Isotropic
↑External →External Data from File
We define the material properties of the wall in a material named MAWALL. We
specify the values for thermal conductivity and capacity. The properties that
depend on time must be input via an external data file concrete.dat in Diana
batch format.
concrete.dat
ADIAB 0.0 20.00
0.1 24.98
0.2 29.47
0.3 33.51
0.4 37.15
0.5 40.42
0.6 43.37
0.7 46.02
0.8 48.41
0.9 50.57
1.0 52.50
1.5 59.65
2.0 63.88
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
18.1 Finite Element Model 379
2.5 66.38
3.0 67.86
4.0 69.25
5.0 69.73
10. 70.00
60. 70.00
ARRHEN 6000.
EQUAGE ARRTYP
The ADIAB data item specifies the temperature values in °C at different ages
(ranging from 0 to 60 days) during the development of the hydration reaction
in adiabatic conditions. The ARRHEN item specifies the Arrhenius constant cA .
Finally, Diana needs some additional input data to calculate the equivalent age.
Here, we specify an Arrhenius-type equivalent age. The reference temperature
TEMREF is not specified. Diana will assume a default value of 20 °C.
18.1.3.2 Boundary Elements
iDiana
Property Manager
Materials Material Name: MABOUN
↑Flow →Boundary
For the boundary elements we define a material MABOUN. We specify the value
for the conduction coefficient K [Table 18.1] which simulates the conduction
with the environment.
18.1.3.3 Cooling Pipes
We adopt the properties of the cooling pipes according to Table 18.2.
Table 18.2: Properties of the cooling pipes
Conduction coefficient K 2160×106 J/(m2 ·K·day)
Fluid discharge × capacitance Qf × c 100×106 J/(K·day)
Perimeter l 8.48×10−2 m
iDiana
Property Manager
Materials Material Name: MACOOL
↑Flow →Cooling Pipe
For the cooling pipe elements we define a material MACOOL. We specify the
value for the conduction coefficient K which simulates the convection exchange
between the cooling pipe and the surrounding concrete material. We also specify
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
380 Wall with Cooling Pipes
a value for the product of the fluid discharge and the fluid capacity. The last
two parameters, corresponding to times at which cooling starts and stops, are
left empty. This means that the cooling pipe elements will be active during the
entire heat flow analysis.
iDiana
Property Manager
↑ Physical Properties Physical Property Name: PHCOOL
↑Geometry →Cooling Pipe
For the cooling pipes we must also define a physical property: the perimeter.
Therefore we open the Physical Properties tab and define a property instance
PHCOOL. We specify the pipe perimeter l.
18.1.3.4 Properties Attachment
wall.fgc
PROPERTY ATTACH WALL MAWALL
PROPERTY ATTACH COOLPI MACOOL PHCOOL
PROPERTY ATTACH BOUNDA MABOUN
We attach the materials and the physical properties to the corresponding sets.
18.1.4 Boundary and Initial Conditions
The boundary condition involves the external temperature. Moreover, we must
specify the initial temperature fields of the model.
Ambient temperature wall.fgc
PROPERTY LOADS EXTTEMP BOUNDA 20
CONSTRUCT TCURVE TC1 LIST 0 1 60 1
PROPERTY ATTACH LOADCASE 1 TC1
The EXTTEMP load class defines an ambient temperature of 20 °C for the sur-
faces that have been meshed with boundary elements (set BOUNDA). By default,
iDiana will consider this load as load case 1. As we are about to perform a tran-
sient analysis, we must also specify the development of the ambient temperature
with time. In this example we assume a constant environmental temperature.
We specify a time curve with a constant factor 1.0 from t = 0 to 60 days. We
assign the time curve to load case 1 and thus defines the time dependency of
the external temperature.
Initial temperature wall.fgc
PROPERTY INITIAL INITEMP ALL 20
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
18.1 Finite Element Model 381
A transient heat flow analysis also requires a specified initial temperature. Here,
we define an initial uniform temperature of 20 °C for all nodes via the INITEMP
class.
The initial temperature of the cooling pipe elements must be input via an
external file in Diana batch format. It aims at defining the ’COOLPI’ table
that will be read as additional input data records during the heat flow analysis.
For each cooling circuit, we must define the number of the node where the fluid
enters the pipe along with initial fluid temperatures in the subsequent nodes of
the cooling pipe in the fluid flow direction. We are going to pick up the starting
nodes of the cooling circuit.
wall.fgc
VIEW OPTIONS SHRINK OFF
VIEW MESH COOLPI
LABEL MESH NODES
We display the mesh of the cooling circuit in normal style with node labels
[Fig. 18.9]. The starting node is labeled as number 10. Thus, we create the file
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:30:39 mesh3.ps
Model: WALL
Analysis: DIANA
Model Type: Heat flow 3D
39
41
29 38
28 37
19
20 27 36
9 18
26 35
8 17
25 34
7 16
24 33
6 15
23 32
5 14
22 31
13 40
4
12 21
3 30
2 11
1
10
Z
Y
Figure 18.9: Node numbers for cooling pipe mesh
coolpi.dat which contains the starting node and the initial temperature of the
fluid of each cooling circuit.
coolpi.dat
’COOLPI’
1 STRTNO 10
TEMPER 10.
For this example we choose a uniform temperature of 10 °C.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
382 Wall with Cooling Pipes
18.2 Transient Nonlinear Heat Flow Analysis
To perform the transient heat flow analysis, we must first write an input data
file in Diana batch format. Then we start the analysis.
iDiana
UTILITY WRITE DIANA
yes
FILE CLOSE
yes
Wall with cooling pipes
ANALYSE WALL
Analysis Setup
specification of options
The ANALYSE command initiates the analysis of the model named WALL. In
the Analysis Setup dialog we may specify the various analysis options for the
transient heat flow analysis. The specification should result in the following
batch analysis commands.
wall.dcf
*FILOS
INITIA
*INPUT
*INPUT
READ APPEND FILE "coolpi.dat" TABLE COOLPI
*HEATTR
BEGIN INITIA
BEGIN NONLIN
EQUAGE
HYDRAT DGRINI=0.01
END NONLIN
TEMPER INPUT FIELD=1
END INITIA
BEGIN EXECUT
BEGIN NONLIN
HYDRAT ITERAT
BEGIN ITERAT
CONVER TEMPER TOLCON=0.0001
MAXITE=30
END ITERAT
END NONLIN
SIZES 0.2(10) 0.5(6) 1(25)
END EXECUT
BEGIN OUTPUT
FILE "wall"
EQUAGE TOTAL INTPNT
INTTMP
REACTI TOTAL INTPNT
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
18.2 Transient Nonlinear Heat Flow Analysis 383
TEMPER
END OUTPUT
*END
The second *INPUT command specifies that table ’COOLPI’ should be read from
file coolpi.dat. The *HEATTR command invokes module heattr for a transient
heat flow analysis. The INITIA commands initiate this analysis. We specify an
initial degree of hydration equal to 0.01 and an initial temperature field as
defined in our data file. We also ask for the calculation of the equivalent age
with the EQUAGE command. With the SIZES command of the EXECUT block, we
define 41 steps ranging from 0.2 days at the beginning of the analysis to 1 day
at the end of the analysis. For output results, we select the temperatures, the
degree of reaction, the equivalent age and the internal temperature of cooling
pipes.
Once the analysis run has terminated, we enter the iDiana Results environ-
ment to assess the results.
wall.fvc
FEMVIEW WALL
UTILITY TABULATE LOADCASES
The load case tabulation shows the available load cases (time steps) with their
result data. Below we show the head and tail of this tabulation.
Tabulated load cases loads.tb
;
; Model: WALL
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; TR1 1 TIME = .2 "Boundary case 1"
; Nodal : PTE....S
; Element : EL.PTE.S
; Gauss : EL.DGR.S EL.EQA.S
;
... lines skipped
;
; TR1 41 TIME = 30 "Boundary case 1"
; Nodal : PTE....S
; Element : EL.PTE.S
; Gauss : EL.DGR.S EL.EQA.S
;
We see the various result attributes: PTE represents the temperature, EL.PTE
represents the internal temperature of cooling pipes, EL.DGR represents the de-
gree of reaction, and EL.EQA represents the equivalent age.
18.2.1 Temperature within the Concrete
We will display the temperature in the concrete in two ways: a transverse cross-
section of the wall and a longitudinal cross-section along the cooling pipes. For
the latter display we will also make an animation sequence to see the develop-
ment of the temperature in time.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
384 Wall with Cooling Pipes
Transverse cross-section wall.fvc
VIEW MESH WALL
EYE ROTATE TO 41 30 30
CONSTRUCT SHAPE PLANE MIDX X 2.51
VIEW XSECTION MIDX
EYE ROTATE TO 90 90
EYE FRAME
VIEW OPTIONS EDGES OUTLINE
RESULTS LOADCASE TR1 1
RESULTS NODAL PTE....S PTE
PRESENT CONTOUR LEVELS
We display a bird’s-eye view of the concrete wall. Then, we construct a shape
MIDX corresponding to the medium plane perpendicular to the X-axis. Via the
XSECTION option we define a transverse cross-section through the three-dimen-
sional solid model. We display this cross-section in a two-dimensional outline
view. We select the temperatures for the first time step and display these as
contours [Fig. 18.10a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:06 temp2.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:06 temp2a.ps
Model: WALL Model: WALL
TR1: Boundary case 1 TR1: Boundary case 1
Step: 1 TIME: .2 Step: 1 TIME: .2
Nodal PTE....S PTE Nodal PTE....S PTE
Max/Min on model set: Max/Min on model set:
Max = 29.9 Max = 29.9
Min = 10.1 Min = 10.1
28.1 28.1
26.3 26.3
24.5 24.5
22.7 22.7
Z 20.9 20.9
19.1 Z 19.1
17.3 Y 17.3
X Y 15.5 15.5
13.7 13.7
11.9 X 11.9
(a) transverse cross-section (b) longitudinal cross-section
Figure 18.10: Temperature contours at t = 0.2 day
Longitudinal cross-section wall.fvc
VIEW MESH RIGWAL
EYE ROTATE TO 41 30 30
EYE FRAME
VIEW HIDDEN SHADE
PRESENT CONTOUR LEVELS
In order to present the three-dimensional nature of the problem we display
the set RIGWAL and move the viewing position. We also set the view mode to
the ‘hidden shade’ style. Again we display a contour plot of the temperatures
[Fig. 18.10b].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
18.2 Transient Nonlinear Heat Flow Analysis 385
Animation wall.fvc
RESULTS LOADCASE ALL
UTILITY SETUP ANIMATE LINEAR
PRESENT CONTOUR FROM 10 TO 37 LEVELS 7
DRAWING ANIMATE LOADCASES PLOTFILE temper
A very instructive manner to display the temperature development in time is the
animation sequence of temperature contours. Therefore we select all available
time steps (load cases). With the LINEAR option we get the frames displayed
sequentially from the first to the last and then starting again at the first. In
an animation sequence of contour plots, we must be aware that the frames of
the animation all use the same color to represent a certain value. Therefore, we
explicitly specify the values for the first and the last contour via the FROM ...
TO option. Due to the PLOTFILE option we can put the frames of the animation
in a document. Here we show the frames for the first nine days [Fig. 18.11].
iDIANA 9.4.3-02 : TNO Diana BV iDIANA 9.4.3-02
28 OCT :2010
TNO 02:31:06
Diana BV temper001 iDIANA 9.4.3-02
28 OCT :2010
TNO 02:31:06
Diana BV temper002 iDIANA 9.4.3-02
28 OCT :2010
TNO 02:31:06
Diana BV temper003 iDIANA 9.4.3-02
28 OCT :2010
TNO 02:31:06
Diana BV temper004 28 OCT 2010 02:31:06 temper005
Model: WALL Model: WALL Model: WALL Model: WALL Model: WALL
TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1
Step: 1 TIME: .2 Step: 2 TIME: .4 Step: 3 TIME: .6 Step: 4 TIME: .8 Step: 5 TIME: 1
Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = 29.9 Max = 34.6 Max = 38.5 Max = 40.7 Max = 41.6
Min = 10.1 Min = 10.1 Min = 10.1 Min = 10.1 Min = 10.1
37 37 37 37 37
33.6 33.6 33.6 33.6 33.6
30.2 30.2 30.2 30.2 30.2
26.9 26.9 26.9 26.9 26.9
Z Z 23.5 Z 23.5 Z 23.5 Z 23.5 23.5
4.8 h 9.6 h 14.4 h 19.2 h 1.0 d
Y Y 20.1 Y 20.1 Y 20.1 Y 20.1 20.1
16.8 16.8 16.8 16.8 16.8
13.4 13.4 13.4 13.4 13.4
X
iDIANA 9.4.3-02 : TNO Diana BV X
iDIANA 9.4.3-02
28 OCT :2010
TNO 02:31:07
Diana BV temper006
10 X
iDIANA 9.4.3-02
28 OCT :2010
TNO 02:31:07
Diana BV temper007
10 X
iDIANA 9.4.3-02
28 OCT :2010
TNO 02:31:07
Diana BV temper008
10 X
iDIANA 9.4.3-02
28 OCT :2010
TNO 02:31:07
Diana BV temper009
10 28 OCT 2010 02:31:07 temper010
10
Model: WALL Model: WALL Model: WALL Model: WALL Model: WALL
TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1
Step: 6 TIME: 1.2 Step: 7 TIME: 1.4 Step: 8 TIME: 1.6 Step: 9 TIME: 1.8 Step: 10 TIME: 2
Nodal PTE....S PTE DRAWING ANIMATE LOADCASES PLOTFILE temper
Nodal PTE....S PTE DRAWING ANIMATE LOADCASES PLOTFILE temper
Nodal PTE....S PTE DRAWING ANIMATE LOADCASES PLOTFILE temper
Nodal PTE....S PTE DRAWING ANIMATE LOADCASES PLOTFILE temper
Nodal PTE....S PTE DRAWING ANIMATE LOADCASES PLOTFILE temper
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = 41.6 Max = 40.9 Max = 39.9 Max = 38.7 Max = 37.5 Min = 10
Min = 10.1 Min = 10.1 Min = 10.1 Min = 10.1
37 37 37 37 37
33.6 33.6 33.6 33.6 33.6
30.2 30.2 30.2 30.2 30.2
26.9 26.9 26.9 26.9 26.9
Z Z 23.5 Z 23.5 Z 23.5 Z 23.5 23.5
1.2 d 1.4 d 1.6 d 1.8 d 2.0 d
Y Y 20.1 Y 20.1 Y 20.1 Y 20.1 20.1
16.8 16.8 16.8 16.8 16.8
13.4 13.4 13.4 13.4 13.4
X
iDIANA 9.4.3-02 : TNO Diana BV X28 OCT :2010
iDIANA 9.4.3-02 TNO 02:31:07
Diana BV temper011
10 X28 OCT :2010
iDIANA 9.4.3-02 TNO 02:31:07
Diana BV temper012
10 X28 OCT :2010
iDIANA 9.4.3-02 TNO 02:31:07
Diana BV temper013
10 X28 OCT :2010
iDIANA 9.4.3-02 TNO 02:31:07
Diana BV temper014
10 28 OCT 2010 02:31:07 temper015
10
Model: WALL Model: WALL Model: WALL Model: WALL Model: WALL
TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1
Step: 11 TIME: 2.5 Step: 12 TIME: 3 Step: 13 TIME: 3.5 Step: 14 TIME: 4 Step: 15 TIME: 4.5
Nodal PTE....S PTE DRAWING ANIMATE LOADCASES PLOTFILE temper
Nodal PTE....S PTE DRAWING ANIMATE LOADCASES PLOTFILE temper
Nodal PTE....S PTE DRAWING ANIMATE LOADCASES PLOTFILE temper
Nodal PTE....S PTE DRAWING ANIMATE LOADCASES PLOTFILE temper
Nodal PTE....S PTE DRAWING ANIMATE LOADCASES PLOTFILE temper
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = 34.4 Min = 10 Max = 31.7 Min = 10 Max = 29.3 Min = 10 Max = 27.4 Min = 10 Max = 25.8 Min = 10
37 37 37 37 37
33.6 33.6 33.6 33.6 33.6
30.2 30.2 30.2 30.2 30.2
26.9 26.9 26.9 26.9 26.9
Z Z 23.5 Z 23.5 Z 23.5 Z 23.5 23.5
2.5 d 3.0 d 3.5 d 4.0 d 4.5 d
Y Y 20.1 Y 20.1 Y 20.1 Y 20.1 20.1
16.8 16.8 16.8 16.8 16.8
13.4 13.4 13.4 13.4 13.4
X
iDIANA 9.4.3-02 : TNO Diana BV X28 OCT
iDIANA 9.4.3-02 : TNO
2010Diana
02:31:07
BV temper016
10 28X OCT
iDIANA 9.4.3-02 : TNO
2010Diana
02:31:07
BV temper01710 28 XOCT
iDIANA 9.4.3-02 : TNO
2010Diana
02:31:07
BV temper018 10 iDIANA 9.4.3-02 X: TNO
28 OCT 2010Diana
02:31:07
BV temper019 10 28 OCT 2010 02:31:07 temper020 10
Model: WALL Model: WALL Model: WALL Model: WALL Model: WALL
TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1
Step: 16 TIME: 5 Step: 17 TIME: 6 Step: 18 TIME: 7 Step: 19 TIME: 8 Step: 20 TIME: 9
Nodal PTE....S PTE DRAWING ANIMATE LOADCASES PLOTFILE Nodal
temperPTE....S PTE DRAWING ANIMATE LOADCASES PLOTFILE temper
Nodal PTE....S PTE DRAWING ANIMATE LOADCASES PLOTFILE temper
Nodal PTE....S PTE DRAWING ANIMATE LOADCASES PLOTFILE
Nodal temper
PTE....S PTE DRAWING ANIMATE LOADCASES PLOTFILE temper
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = 24.5 Min = 10 Max = 22.8 Min = 10 Max = 21.7 Min = 10 Max = 20.9 Min = 10 Max = 20.5 Min = 10
37 37 37 37 37
33.6 33.6 33.6 33.6 33.6
30.2 30.2 30.2 30.2 30.2
26.9 26.9 26.9 26.9 26.9
Z Z 23.5 Z 23.5 Z 23.5 Z 23.5 23.5
5.0 d 6.0 d 7.0 d 8.0 d 9.0 d
Y Y 20.1 Y 20.1 Y 20.1 Y 20.1 20.1
16.8 16.8 16.8 16.8 16.8
13.4 13.4 13.4 13.4 13.4
X X 10 X 10 X 10 X 10 10
DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper DRAWING ANIMATE LOADCASES PLOTFILE temper
Figure 18.11: Concrete temperature animation sequence
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
386 Wall with Cooling Pipes
18.2.2 Degree of Reaction and Equivalent Age
Looking at the animation sequence, we can see that the temperature reaches
a maximum value in the core of the top part of the wall. On the other hand,
near the cooling circuit the temperature increase remains quite low. Therefore,
it is interesting to compare the development in time of the degree of reaction
for these two specific areas of the model.
Finding the extreme temperatures wall.fvc
RESULTS LOADCASE TR1 6
EYE ROTATE TO 90 90
VIEW XSECTION MIDX
EYE FRAME
PRESENT CONTOUR LEVELS
LABEL MESH ELEMENTS VIEWMODE BLUE
First, we select the sixth load case corresponding to time t = 1.2 days for which
the maximum value of the temperature is reached within the concrete. We
display the contour plot of the temperatures for the transverse cross-section,
including the element numbers in blue [Fig. 18.12a]. Therefore, we may locate
two elements in the left hand side column: element number 795 is located on the
warmest part of the concrete and element number 597 is located on the coldest
part in between the cooling pipes.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:09 temp-all.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:09 evol-reac.ps
Model: WALL Model: WALL
TR1: Boundary case 1 Gauss EL.DGR.S DGR
Step: 6 TIME: 1.2 291 299 Max/Min on whole graph:
Nodal PTE....S PTE Ymax = .958
Max/Min on model set: Ymin = .145
Max = 41.6 811 819 365 Xmax = 30
Min = 10.1 Xmin = .2
Variation over loadcases
Element 597 Mean
1 Element 795 Mean
795 803 366
.9
G
A
779 787 367 U .8
S
S
I .7
693 701 249 A
N
.6
677 685 250 E
L
. .5
D
613 621 193 G
R
. .4
597 605 194 S
D .3
533 541 137 G
R
.2
38.7
517 525 138
35.9
33 .1
30.1 0 2.5 5 7.5 10 12.5 15 17.5 20 22.5 25 27.5 30 32.5
453 461 81 27.3
Z TIME
24.4
21.5
437 445 82 18.7
X Y
15.8
12.9
(a) temperatures at t = 1.2 days (b) degree of reaction in time
Figure 18.12: Assessment of the degree of reaction
Degree of reaction in time wall.fvc
RESULTS LOADCASE ALL
RESULTS GAUSSIAN EL.DGR.S DGR
PRESENT GRAPH ELEMENT 597 795
We select the degree of reaction results for all time steps. For the two elements
with the extreme temperatures we display time graphs of the degree of reaction
[Fig. 18.12b]. These show that heat activates the hydration of concrete. In the
same way, we can display the evolution of the equivalent age.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
18.2 Transient Nonlinear Heat Flow Analysis 387
Equivalent age wall.fvc
RESULTS GAUSSIAN EL.EQA.S EQA
DRAWING DISPLAY
We select the degree-of-reaction results attribute and update the current view
of the graph [Fig. 18.13]. We notice that on the warmest part teq > t, whereas
on the coldest part teq = t.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:09 evol-age.ps
Model: WALL
Gauss EL.EQA.S EQA
Max/Min on whole graph:
Ymax = 34 Ymin = .247
Xmax = 30 Xmin = .2
Variation over loadcases
Element 597 Mean
Element 795 Mean
35
G 30
A
U
S
S 25
I
A
N
20
E
L
.
E 15
Q
A
.
S 10
E
Q
A 5
0
0 2.5 5 7.5 10 12.5 15 17.5 20 22.5 25 27.5 30 32.5
TIME
Figure 18.13: Evolution of the equivalent age with time
18.2.3 Temperature of Coolant
Finally we will assess the evolution of the outlet temperature of the coolant.
Cooling pipe elements wall.fvc
VIEW MESH COOLPI
EYE ROTATE TO 41 30 30
EYE FRAME
LABEL MESH ELEMENTS ALL RED
We rotate the model in order to get a suitable three-dimensional view. Then
we display the cooling circuit mesh with element numbers [Fig. 18.14a]. From
this view, we can easily read that element 38 corresponds to the end part of the
cooling circuit.
Temperature wall.fvc
RESULTS ELEMENT EL.PTE.S PTE
PRESENT GRAPH ELEMENT 38
We select the temperature results for the cooling pipes and display the graph
corresponding to element number 38 [Fig. 18.14b].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
388 Wall with Cooling Pipes
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:09 evol-cpe.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:09 evol-temp.ps
Model: WALL Model: WALL
Element EL.PTE.S PTE
Max/Min on whole graph:
40 Ymax = 12.4
37 Ymin = 10.4
39 Xmax = 30
Xmin = .2
36 Variation over loadcases
27 Element 38 Mean
12.5
35
19 26 12.2
17
18 E
34 L 12
25 E
16
8 M
33 E
24 N 11.8
15 T
7
32 E 11.5
23 L
14
6 .
31 P 11.2
22 T
13 E
5 . 11
30 S
21
12
4 38 P 10.8
T
20 E
11
3 10.5
29
10 10.2
2 28
0 2.5 5 7.5 10 12.5 15 17.5 20 22.5 25 27.5 30 32.5
TIME
Z 1
Y
9
X
(a) getting the element number (b) evolution in time
Figure 18.14: Assessment of the outlet temperature of the coolant
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
Chapter 19
Cooling Pipes in a Tunnel
Name: Coolpi
Path: /Examples/ConcMas/Coolpi
Keywords: analys: flow heat nonlin transi. constr: initia temper. el-
emen: bq4ht coolpi flow hx8ht l2ht potent. load: elemen
temper time. materi: adiaba capaci conduc hydrat isotro. op-
tion: direct groups units. post: binary femvie. pre: append
femgen. result: inttmp reacti temper total.
6.90
Z
Y
X
1.20
1.90
20 1.30
2.80
Figure 19.1: Tunnel segment with cooling pipes [m]
This example presents the use of cooling pipe elements within Diana. The
studied structure is a U-shaped concrete tunnel with three cooling circuits in
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
390 Cooling Pipes in a Tunnel
its walls. The cooling is active during the hardening process of the concrete.
Due to symmetry we will model only one half-part of the U-shaped structure
[Fig. 19.1]. This part consists of an already existing base slab, with a thickness
of 1.2 m and a width of 6 m, on which has been cast a wall with a thickness
of 1.3 m and a height of 6.9 m. This structure is 20 m long and is laying on
a soil foundation. Figure 19.2 shows a detailed description of the cooling pipe
positions, along with adopted boundary conditions.
0.45 0.40 0.45
fluid entry
fluid discharge
2.15
convective exchange
q boundary flux
0.75
♥
circuit 1 0.75
6.90
circuit 2
0.75
0.50
Tenv = 20°C 0.50
0.50
circuit 3
0.50
Z
0.50
1.20 q=0
q=0
2.80 1.30 1.90
Figure 19.2: Tunnel cross-section in Y Z-plane [m]
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
19.1 Finite Element Model 391
19.1 Finite Element Model
To make the finite element model, we start iDiana and then enter the Design
environment with the model name.
iDiana
FFEMGEN TUNNEL
Analysis and Units
Analysis Selection
Model Type: →Heat Flow 3D
Units Definition
Length: →Meter
Time: →Day
Temperature: →Celsius
In the Analysis and Units dialog we indicate that it is a model for three-dimen-
sional heat flow analysis. We also specify the applied units [m, day, °C].
19.1.1 Geometry Definition
We will define the geometry of the wall in three parts: the wall, the cooling
pipes, and the slab.
19.1.1.1 Wall
To construct our model, we start by defining the geometry of the bottom surface
of the concrete wall. For a better understanding of the model description, we
present a top view of the concrete wall [Fig. 19.3]. We define the coordinates of
points A to P.
D N P C
0.45
L F H J
0.40 Y cooling pipes
K E G I
0.45
A M O B
X
0.45 19.10 0.45
Figure 19.3: Top view of the concrete wall [m]
Points tunnel.fgc
GEOMETRY POINT 0
GEOMETRY POINT 20
GEOMETRY POINT 20 1.3
GEOMETRY POINT 0 1.3
GEOMETRY POINT 0.45 0.45
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
392 Cooling Pipes in a Tunnel
GEOMETRY POINT 0.45 0.85
GEOMETRY POINT 19.55 0.45
GEOMETRY POINT 19.55 0.85
GEOMETRY POINT 20 0.45
GEOMETRY POINT 20 0.85
GEOMETRY POINT 0 0.45
GEOMETRY POINT 0 0.85
GEOMETRY POINT 0.45
GEOMETRY POINT 0.45 1.3
GEOMETRY POINT 19.55
GEOMETRY POINT 19.55 1.3
Note that if we only specify the X- and Y -coordinates the iDiana will assume
Z = 0 by default which is OK for the points in the bottom surface. If we only
specify X, like for the first two points, then both Y and Z will be zero. Also by
default, iDiana will name the specified points sequentially P1, P2, . . . , P16.
Display geometry tunnel.fgc
EYE FRAME ALL
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY POINTS
We display the specified points, labeled with their names and fitted in the
iDiana viewport [Fig. 19.4a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:18 wapnts.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:18 wasurf.ps
Model: TUNNEL Model: TUNNEL
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 3D Model Type: Heat flow 3D
P4 P14 P16P3 L9
L10 L17 L24
S3L8 S6 S9
L16L23
P12P6 P8 P10 L7L6 L15 L22
S2L5 S5 S8
L14L21
P11P5 P7 P9 L4L3 L13 L20
S1 S4 S7
P1 P13 P15P2 L1L2 L11 L12L19
L18
Y Y
Z X Z X
(a) points (b) lines and surfaces
Figure 19.4: Wall geometry in the XY -plane
Surfaces tunnel.fgc
GEOMETRY SURFACE 4POINTS P1 P13 P5 P11
GEOMETRY SURFACE 4POINTS P11 P5 P6 P12
GEOMETRY SURFACE 4POINTS P12 P6 P14 P4
GEOMETRY SURFACE 4POINTS P13 P15 P7 P5
GEOMETRY SURFACE 4POINTS P5 P7 P8 P6
GEOMETRY SURFACE 4POINTS P6 P8 P16 P14
GEOMETRY SURFACE 4POINTS P15 P2 P9 P7
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
19.1 Finite Element Model 393
GEOMETRY SURFACE 4POINTS P7 P9 P10 P8
GEOMETRY SURFACE 4POINTS P8 P10 P3 P16
CONSTRUCT SET BOTWAL APPEND SURFACES ALL
Nine surfaces are created which together represent the model of the bottom
surface of the wall. We assemble their geometry components in the set BOTWAL.
Display geometry tunnel.fgc
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY LINES ALL VIOLET
LABEL GEOMETRY SURFACES ALL BLUE
We display the defined geometry in violet including labels for lines and surfaces
[Fig. 19.3b].
Meshing division tunnel.fgc
CONSTRUCT SET SELIN1 APPEND LINES L2 L4 L5 L7 L8 L10
CONSTRUCT SET SELIN1 APPEND LINES L12 L19 L14 L21 L16 L23
CONSTRUCT SET SELIN2 APPEND LINES L1 L3 L6 L9 L18 L20 L22 L24
CONSTRUCT SET SELIN3 APPEND LINES L11 L13 L15 L17
MESHING DIVISION LINE SELIN1 3
MESHING DIVISION LINE SELIN2 1
MESHING DIVISION LINE SELIN3 20
We define some sets containing lines for which we want to have the same division.
The set SELIN1 contains all the lines in the Y -direction whereas sets SELIN2 and
SELIN3 contain all the lines in the X-direction. Then we specify the line division
to be applied in each set.
Display geometry tunnel.fgc
VIEW GEOMETRY SELIN1 RED
VIEW GEOMETRY +SELIN2 BLUE
VIEW GEOMETRY +SELIN3 VIOLET
LABEL GEOMETRY DIVISION SELIN1 RED
LABEL GEOMETRY DIVISION SELIN2 BLUE
LABEL GEOMETRY DIVISION SELIN3 GREEN
We display the defined geometry, including division labels for lines, in different
colors for each set [Fig. 19.5a]. Note the ‘+’ sign which causes the various sets
to be superposed to the current display.
Sweep to three-dimensional model tunnel.fgc
EYE ROTATE TO 41 30 30
GEOMETRY SWEEP BOTWAL MID1 2 TRANSLATE TR1 0 0 .5
GEOMETRY SWEEP MID1 MID2 2 TRANSLATE TR2 0 0 .5
GEOMETRY SWEEP MID2 MID3 2 TRANSLATE TR3 0 0 .5
GEOMETRY SWEEP MID3 MID4 2 TRANSLATE TR4 0 0 .5
GEOMETRY SWEEP MID4 MID5 2 TRANSLATE TR5 0 0 .5
GEOMETRY SWEEP MID5 MID6 2 TRANSLATE TR6 0 0 .75
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
394 Cooling Pipes in a Tunnel
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:18 wamedi.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:18 wasw.ps
Model: TUNNEL Model: TUNNEL
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 3D Model Type: Heat flow 3D
3 13 20 1
3 13
3 13 20
3 13
3 13 20
31 3
1 20
Y
Z
Y
Z X
X
(a) meshing divisions (b) swept surfaces
Figure 19.5: Final geometry of the wall
GEOMETRY SWEEP MID6 MID7 2 TRANSLATE TR7 0 0 .75
GEOMETRY SWEEP MID7 MID8 2 TRANSLATE TR8 0 0 .75
GEOMETRY SWEEP MID8 TOPWAL 6 TRANSLATE TR9 0 0 2.15
To prepare ourselves for the transformation to a three-dimensional model we
choose an appropriate eye point. Then we sweep, i.e., translate through space,
the original profile BOTWAL to create a body. This operation is repeated several
times in order to create geometrical entities for each plane containing cooling
pipes (sets MIDi with i = 1, . . . , 8) and also to create the top plane which is
defined as set TOPWAL. Via these sweeping operations we also define the division
for created lines in the Z-direction to be 2 and 6.
Make set and display geometry tunnel.fgc
CONSTRUCT SET WALCON APPEND ALL
EYE FRAME
VIEW GEOMETRY ALL VIOLET
We assemble all the geometry entities created so far in the set WALCON. Finally
we display the wall geometry in violet, fitting in the viewport, [Fig. 19.5b].
19.1.1.2 Cooling Pipes
From the geometry entities which have been previously created, we will pick up
the lines corresponding to the cooling pipe discretization. The same methodol-
ogy will be repeated for each of the three cooling circuits.
First circuit tunnel.fgc
EYE ROTATE TO 0
CONSTRUCT SET COOTMP APPEND CURSOR POLYGON /CURSOR
EYE ROTATE TO 90
VIEW GEOMETRY COOTMP VIOLET
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
19.1 Finite Element Model 395
EYE FRAME
LABEL GEOMETRY LINES COOTMP RED
CONSTRUCT SET COOLP1 APPEND LINES L324 L317 L331 L277 L298 L237 L251 L197
CONSTRUCT SET COOLP1 APPEND LINES L218 L157 L171 L117 L124
UTILITY DELETE SET COOTMP
yes
We change the eye point to display a top view of the wall [Fig. 19.6a]. We create
a ‘dummy’ set named COOTMP. Here we use the graphics cursor to control the
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:18 cp1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:18 cp1vw.ps
Model: TUNNEL Model: TUNNEL
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 3D Model Type: Heat flow 3D
L347 L357 L364
L372
L371 L378
L382
L307 L317 L324
L332
L331 L338
L342
L267 L277 L284
L292
L291 L298
L302
L227 L237 L244
L252
L251 L258
L262
L187 L197 L204
L212
L211
L147 L157 L218
L222
L164
L172
L171
L107 L117 L178
L182
L124
L132
L131
L67 L77 L138
L142
L84
L92
L91
L27 L37 L98
L102
L44
L52
L51
L3 L13 L62
L58
L20
Y Z
Z X Y X
(a) cursor selection with polygon (b) selected geometry
Figure 19.6: Defining the first circuit of cooling pipes
append operation based on the position of a part of the screen. With the
POLYGON option we create a quadrilateral around the second horizontal line.
By double clicking for the last vertex of the quadrilateral, the set COOTMP is
created. Then we display the created set in violet and rotate the eye point 90°
around the X-axis to get an in-plane view [Fig. 19.6b]. We label the lines of
COOTMP in red. We create the set COOLP1 by picking up the appropriate lines.
This set corresponds to the first cooling circuit. Then we delete the set COOTMP
with the UTILITY DELETE command.
Second circuit tunnel.fgc
EYE ROTATE TO 0
VIEW GEOMETRY ALL VIOLET
CONSTRUCT SET COOTMP APPEND CURSOR POLYGON /CURSOR
EYE ROTATE TO 90
VIEW GEOMETRY COOTMP VIOLET
EYE FRAME
LABEL GEOMETRY LINES COOTMP RED
CONSTRUCT SET COOLP2 APPEND LINES L326 L319 L333 L279 L299 L239 L253 L199
CONSTRUCT SET COOLP2 APPEND LINES L219 L159 L173 L119 L126
UTILITY DELETE SET COOTMP
yes
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
396 Cooling Pipes in a Tunnel
First we switch back to the original top view of the wall [Fig. 19.7a]. Then we
create the set COOTMP by defining a quadrilateral around the third horizontal
line. Then we display the created set in violet and rotate it over 90° around the
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:18 cp2.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:18 cp2vw.ps
Model: TUNNEL Model: TUNNEL
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 3D Model Type: Heat flow 3D
L350 L359 L366
L374
L373 L379
L383
L310 L319 L326
L334
L333 L339
L343
L270 L279 L286
L294
L293 L299
L303
L230 L239 L246
L254
L253 L259
L263
L190 L199 L206
L214
L213
L150 L159 L219
L223
L166
L174
L173
L110 L119 L179
L183
L126
L134
L133
L70 L79 L139
L143
L86
L94
L93
L30 L39 L99
L103
L46
L54
L53
L6 L15 L63
L59
L22
Y Z
Z X Y X
(a) cursor selection with polygon (b) selected geometry
Figure 19.7: Defining the second circuit of cooling pipes
X-axis to get an in-plane view [Fig. 19.7b]. We label the lines of COOTMP in red.
For the second circuit we define the set COOLP2 by specifying the appropriate
lines. Once more we delete the set COOTMP.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:18 cp3a.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:18 cp3b.ps
Model: TUNNEL Model: TUNNEL
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 3D Model Type: Heat flow 3D
Y Z
Z X Y X
(a) first cursor selection (b) second cursor selection
Figure 19.8: Defining the third circuit of cooling pipes
Third circuit tunnel.fgc
EYE ROTATE TO 0
VIEW GEOMETRY ALL VIOLET
CONSTRUCT SET COOTMP APPEND CURSOR POLYGON /CURSOR
VIEW GEOMETRY COOTMP VIOLET
EYE ROTATE TO 90
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
19.1 Finite Element Model 397
CONSTRUCT SET COOTMP2 APPEND CURSOR POLYGON /CURSOR
VIEW GEOMETRY COOTMP2 VIOLET
EYE ROTATE TO 41 30 30
LABEL GEOMETRY LINES COOTMP2 RED
CONSTRUCT SET COOLP3 APPEND LINES L44 L37 L77 L84 L99 L39 L79 L69 L29
UTILITY DELETE SET COOTMP2
yes
UTILITY DELETE SET COOTMP
yes
Like before, we start by displaying the top view of the concrete wall. Then
we define a set COOTMP via a quadrilateral polygon around the two medium
horizontal lines [Fig. 19.8a]. We rotate the eye point 90° around the X-axis to
get an in-plane view. Now we define a second set COOTMP2 via a quadrilateral
polygon [Fig. 19.8b]. We display the obtained set COOTMP2 and move the view-
ing position to get a nice three-dimensional representation of our geometry. We
label the lines in red [Fig. 19.9a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:18 cp3vw.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:19 cpall.ps
Model: TUNNEL Model: TUNNEL
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 3D Model Type: Heat flow 3D
L69
L93
L91
L29
L79
L77
L39
L37
Z L78L86
L99 Z
L84
L85
L98 L103
Y L38L46
L102 Y
L45
L44
X X
(a) third circuit (b) all circuits
Figure 19.9: Three-dimensional view of cooling pipe circuits
We may pick up lines corresponding to the third cooling circuit and there-
fore construct the set COOLP3. Unfortunately the labels for lines do overlap
[Fig. 19.9a]. Eventually, line labels can be more easily read with some EYE
ZOOM commands. Then we delete temporary sets COOTMP2 and COOTMP.
All three circuits tunnel.fgc
VIEW GEOMETRY COOLP1 VIOLET
VIEW GEOMETRY +COOLP2 RED
VIEW GEOMETRY +COOLP3 BLUE
CONSTRUCT SET COOLPI APPEND COOLP1 COOLP2 COOLP3
To check the geometry of the cooling pipe circuits we display these with different
colors [Fig. 19.9b]. The creation of a set COOLPI, which contains the complete
cooling circuit geometry, terminates the definition of the cooling pipe circuits.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
398 Cooling Pipes in a Tunnel
19.1.1.3 Slab
For a better understanding of the modeling process we present a top view of the
concrete slab [Fig. 19.10].
S W X T
1.90
D N P C
L F H J
Y
1.30 K E G I
A M O B
X
2.80
Q U V R
Figure 19.10: Top view of the concrete slab
Make set tunnel.fgc
CONSTRUCT SET OPEN TOPBAS
CONSTRUCT SET APPEND BOTWAL
VIEW GEOMETRY BOTWAL
EYE ROTATE TO 0
We open a set TOPBAS in which we will include all the geometrical entities that
form the top surface of the slab. We first append the set BOTWAL. As this set
is part of the top surface of the concrete slab, we display a top view of this set
on the screen.
Points tunnel.fgc
GEOMETRY POINT COORD 0 -2.8
GEOMETRY POINT COORD 20 -2.8
GEOMETRY POINT COORD 0 1.9
GEOMETRY POINT COORD 20 1.9
GEOMETRY POINT COORD .45 -2.8
GEOMETRY POINT COORD 19.55 -2.8
GEOMETRY POINT COORD 19.55 1.9
GEOMETRY POINT COORD .45 1.9
VIEW GEOMETRY TOPBAS VIOLET
LABEL GEOMETRY POINTS
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
19.1 Finite Element Model 399
We define the coordinates of points Q to X [Fig. 19.10]. All the points of the top
surface of the concrete slab are situated in the XY -plane. So we may omit the
Z-coordinates, iDiana will assume zero values by default. After the definition
we display the defined points labeled with their names [Fig. 19.11a]. We may
now apply the specified points to define surfaces.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:19 slpnts.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:19 slsurf.ps
Model: TUNNEL Model: TUNNEL
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 3D Model Type: Heat flow 3D
Open Sets: TOPBAS
P163
P168 P167
P164 L397 L395 L393
L398
L396 L394
L392
P4 P14 P16P3 L9
L10 L17 L24
P12P6 P8 P10 L8 L16L23
L7L6
L5
L15 L22
L14L21
P11P5 P7 P9 L4L3 L13 L20
P1 P13 P15P2 L1L2 L11 L12L19
L18
L387
L386 L389
L391
P161
P165 P166
P162 L385 L388 L390
Y Y
Z X Z X
(a) points (b) surfaces
Figure 19.11: Geometry of the slab
Surfaces tunnel.fgc
GEOMETRY SURFACE 4POINTS P161 P165 P13 P1
GEOMETRY SURFACE 4POINTS P165 P166 P15 P13
GEOMETRY SURFACE 4POINTS P166 P162 P2 P15
GEOMETRY SURFACE 4POINTS P16 P3 P164 P167
GEOMETRY SURFACE 4POINTS P14 P16 P167 P168
GEOMETRY SURFACE 4POINTS P4 P14 P168 P163
CONSTRUCT SET CLOSE
VIEW GEOMETRY TOPBAS VIOLET
LABEL GEOMETRY LINES CURRENT BLUE
We define six quadrilateral surfaces. As all the geometrical entities have been
defined for the top surface of the concrete slab we may now close the active set
TOPBAS. We display this set in violet with line labels in blue [Fig. 19.11b].
Meshing division tunnel.fgc
CONSTRUCT SET SELIN4 APPEND LINES L388 L395
CONSTRUCT SET SELIN5 APPEND LINES L385 L390 L393 L397
CONSTRUCT SET SELIN6 APPEND LINES L387 L386 L389 L391
CONSTRUCT SET SELIN7 APPEND LINES L392 L394 L396 L398
MESHING DIVISION LINE SELIN4 20
MESHING DIVISION LINE SELIN5 1
MESHING DIVISION LINE SELIN6 8
MESHING DIVISION LINE SELIN7 2
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
400 Cooling Pipes in a Tunnel
Like for the construction of the concrete wall, we define some sets containing
lines for which we want to have the same division. The sets SELIN4 and SELIN5
contains the new created lines in the X-direction whereas sets SELIN6 and SELIN7
contain the new created lines in the Y -direction. Then we specify the line
division to be applied in each set. The number of division chosen for SELIN4 and
SELIN5 are the same as for SELIN3 and SELIN2. Thus, we ensure a regular square
mesh of the top surface of the concrete slab.
Make set tunnel.fgc
CONSTRUCT SET OPEN BASCON
GEOMETRY SWEEP TOPBAS BOTBAS 4 TRANSLATE TR10 0 0 -1.2
CONSTRUCT SET CLOSE
With a sweeping operation we create a body with four line divisions in the Z-
direction. The surface set which results from the translation of TOPBAS in the
−Z direction is called BOTBAS. It represents the bottom surface of the concrete
slab. All the involved geometrical entities for the creation of this body are
placed in the set BASCON.
19.1.1.4 Complete Model
Prior to the actual meshing procedure we propose a three-dimensional display
of the complete model geometry.
Display tunnel.fgc
EYE ROTATE TO 41 30 30
VIEW GEOMETRY BASCON VIOLET
VIEW GEOMETRY +WALCON BLUE
VIEW GEOMETRY +COOLPI RED
EYE FRAME
We display the slab in violet, the wall in blue, and the cooling pipe circuits in
red [Fig. 19.12a].
19.1.2 Meshing
We may now create a finite element mesh on the defined geometry.
tunnel.fgc
MESHING TYPES WALCON HE8 HX8HT
MESHING TYPES BASCON HE8 HX8HT
MESHING TYPES COOLPI BE2 L2HT
MESHING GENERATE
VIEW MESH
VIEW HIDDEN SHADE
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
19.1 Finite Element Model 401
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:19 geomod.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:20 mesh.ps
Model: TUNNEL Model: TUNNEL
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 3D Model Type: Heat flow 3D
Z Z
Y Y
X X
(a) geometry (b) mesh
Figure 19.12: Complete model
We select the HE8 generic element type and the linear HX8HT heat flow element
for the sets WALCON and BASCON of the model. For the cooling pipes we select
the BE2 generic element type and the linear L2HT cooling pipe element. We
generate the mesh and display it in the hidden shade style [Fig. 19.12b].
19.1.3 Boundary Elements
We must describe the heat convection along the outside surfaces of the concrete
structure composed by the base slab and the wall. We start by defining all the
concerned surfaces of the geometry.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:20 bnd1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:20 bnd2.ps
Model: TUNNEL Model: TUNNEL
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 3D Model Type: Heat flow 3D
Z Y
X Y Z X
(a) first polygon (b) second polygon
Figure 19.13: Boundary selection
Geometry selection tunnel.fgc
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
402 Cooling Pipes in a Tunnel
VIEW GEOMETRY ALL VIOLET
VIEW HIDDEN OFF
EYE ROTATE TO 90 90
EYE FRAME
CONSTRUCT SET BOUNDA APPEND CURSOR POLYGON /CURSOR
EYE ROTATE TO 0
EYE FRAME
CONSTRUCT SET BOUNDA APPEND CURSOR POLYGON /CURSOR
VIEW GEOMETRY BOUNDA VIOLET
EYE ROTATE TO 41 30 30
EYE FRAME
We display the geometry in the default style and rotate the model to get its
view in the Y Z-plane. Then we create a set BOUNDA via a polygon that we
draw with the cursor [Fig. 19.13a]. We append in this set all the surfaces inside
this polygon. Now we rotate the geometry in order to get a top view of the
model. We append the end faces of the model to the set BOUNDA via another
polygon [Fig. 19.13b], and thus finish the construction of exchange surface geom-
etry. Finally we display the geometry corresponding to the boundary surfaces
[Fig. 19.14a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:20 bndgeo.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:21 bndmes.ps
Model: TUNNEL Model: TUNNEL
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 3D Model Type: Heat flow 3D
Z Z
Y Y
X X
(a) geometry (b) element mesh
Figure 19.14: Boundary model
Meshing tunnel.fgc
MESHING TYPES BOUNDA QU4 BQ4HT
MESHING GENERATE
VIEW MESH BOUNDA
VIEW OPTION SHRINK
For the meshing process we select the QU4 generic element type and the linear
BQ4HT heat flow boundary element for the set BOUNDA of our model. We recre-
ate the mesh, including boundary elements. Finally we display the mesh for set
BOUNDA in shrunken element style [Fig. 19.14b].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
19.1 Finite Element Model 403
19.1.4 Material and Physical Properties
We must now specify the material and physical properties for the various com-
ponents of our model via the Property Manager dialog.
iDiana
View →Property Manager...
↑
Property Manager
···
We specify the various materials for the concrete, the boundary elements, and
the cooling pipes. Note that the material properties of the slab just consist
of a single definition of the thermal conductivity and capacitance whereas the
concrete wall needs further properties to take account of the heat production
induced by the hydration reaction.
Base slab concrete iDiana
Property Manager
↑ Materials Material Name: MABASE
↑Flow →Isotropic
For the base slab we define a material MABASE: a thermal conductivity λ =
231×103 J/(m·K·day) and a thermal capacity C = 2700×103 J/(m3 ·K).
Wall concrete iDiana
Property Manager
Materials Material Name: MAWALL
↑Flow →Isotropic
↑External →External Data from File
For the wall we define a material MAWALL: a thermal conductivity λ = 231×103
J/(m·K·day) and a thermal capacity C = 2700×103 J/(m3 ·K). The properties
which depend on time must be input via an external data file in Diana batch
format. For this example we apply the following file.
Hydration in time wall.dat
ADIAB 0.0 20.00
0.1 24.81
0.2 29.11
0.3 32.97
0.4 36.42
0.5 39.51
0.6 42.28
0.7 44.76
0.8 46.98
0.9 48.97
1.0 50.75
1.5 57.22
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
404 Cooling Pipes in a Tunnel
2.0 60.94
2.5 63.09
3.0 64.32
4.0 65.44
5.0 65.82
10. 66.00
60. 66.00
ARRHEN 5000.
The ADIAB data item specifies the temperature values in °C at different ages
(ranging from 0 days to 60 days) during the development of the hydration reac-
tion in adiabatic conditions. The ARRHEN item specifies the Arrhenius constant
CA . See also Volume Material Library for more information on these input data
items.
Boundary elements iDiana
Property Manager
Materials Material Name: MABOUND
↑Flow →Boundary →Convection only
For the boundary elements we define a material MABOUND with a conduction
coefficient to simulate the conduction with the environment: K = 1210×103
J/(m2 ·K·day).
Cooling pipes iDiana
Property Manager
Materials Material Name: MACOOL
↑Flow →Cooling Pipe
↑Physical Properties Physical Property Name: PHCOOL
↑Geometry →Cooling Pipe
For the cooling pipes we define a material MACOOL with a conduction coeffi-
cient which simulates the convection exchange between the cooling pipe and the
surrounding concrete material: K = 2160×106 J/(m2 ·K·day). We also specify
a value for the fluid discharge times the heat capacitance Qf × c = 100×106
J/(day·K). The last two items in the dialog, corresponding to times at which
cooling starts and stops, are left free. This means that the cooling pipe elements
will be active during the entire heat flow analysis. We also define a physical
property PHCOOL to simulate the thermal behavior of the cooling pipe elements.
Here we specify a pipe perimeter l = 8.48×10−2 m.
Property assignment tunnel.fgc
PROPERTY ATTACH WALCON MAWALL
PROPERTY ATTACH BASCON MABASE
PROPERTY ATTACH COOLPI MACOOL PHCOOL
PROPERTY ATTACH BOUNDA MABOUND
We assign the properties to the corresponding sets.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
19.1 Finite Element Model 405
19.1.5 Boundary and Initial Conditions
The boundary condition of the model involves the external temperature. More-
over, we must specify the initial temperature fields of the model.
External temperature tunnel.fgc
PROPERTY LOADS EXTTEMP BOUNDA 15
CONSTRUCT TCURVE TC1 LIST 0 1 60 1
PROPERTY ATTACH LOADCASE 1 TC1
The EXTTEMP load class defines an ambient temperature of 15 °C for the surfaces
that have been meshed with boundary elements, i.e., the set BOUNDA. By default,
iDiana will consider this load as load case 1.
Because we are about to perform a transient analysis, we must also specify
the development of the ambient temperature with time. In the present case we
assume a constant environmental temperature. We specify a time curve with a
constant factor 1 from t = 0 to t = 60 days. We assign the time curve to load
case 1. This defines the time dependency of the external temperature.
Initial temperature of concrete tunnel.fgc
PROPERTY INITIAL INITEMP ALL 15
A transient heat flow analysis also requires a specified initial temperature. Here,
we define an initial uniform temperature of 15 °C for all nodes via the INITEMP
initial condition class.
Initial temperature of cooling pipes. The initial temperature of the cool-
ing pipe elements must be input via an external file in Diana batch format.
It aims at defining the ’COOLPI’ table which will be read as additional input
data during the heat flow analysis. For each cooling circuit we must define the
number of the node where the fluid enters the pipe along with initial fluid tem-
peratures in the subsequent nodes of the cooling pipe in the fluid flow direction.
For further information see also Volume Element Library. We will now first pick
up the starting nodes of each cooling circuit.
tunnel.fgc
VIEW OPTION SHRINK OFF
VIEW MESH COOLP1
VIEW MESH +COOLP2 RED
VIEW MESH +COOLP3 BLUE
EYE ZOOM /CURSOR
LABEL MESH NODES COOLP1 VIOLET
LABEL MESH NODES COOLP2 RED
LABEL MESH NODES COOLP3 BLUE
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
406 Cooling Pipes in a Tunnel
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:21 meshcp.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:34:21 meshcpz.ps
247 269
Model: TUNNEL Model: TUNNEL 354
Analysis: DIANA Analysis: DIANA
Model Type: Heat flow 3D Model Type: Heat flow 3D 289
246 268
203 311
225
310
245
159 202 224
181
115 158 201
137 180 223
72 114 222 157
93 136
27 71 113
51 92 135
26 70134
6 50 91
2590
45
Z Z
Y Y
X X
(a) complete (b) zoomed-in with node numbers
Figure 19.15: Mesh of cooling pipes
We first switch off the shrunken element style option. Then we display the
mesh of each cooling circuit in three different colors [Fig. 19.15a]. For a better
view we make a zoom of the right hand side part of the cooling pipe system.
Finally we label the element nodes in the same color as for the displayed meshes
[Fig. 19.15b]. In the display we determine the three starting nodes: 134, 135
and 45. We apply these node numbers in the external data file.
coolpi.dat
’COOLPI’
1 STRTNO 134
TEMPER 10.
2 STRTNO 135
TEMPER 10.
3 STRTNO 45
TEMPER 10.
’END’
Via input table ’COOLPI’ we describe the temperature in the cooling pipes. For
each cooling circuit, data item STRTNO specifies the starting node and TEMPER
the temperature of the fluid. For this example we have chosen a uniform tem-
perature of 10 °C.
19.2 Transient Nonlinear Heat Flow Analysis
To perform the transient heat flow analysis, we must first write an input data
file in Diana batch format. Then we may close the model and start the analysis.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
19.2 Transient Nonlinear Heat Flow Analysis 407
iDiana
UTILITY WRITE DIANA
yes FILE CLOSE
yes
U-shaped tunnel with cooling pipes
ANALYSE TUNNEL
Analysis Setup
specification of options
Via the Analysis Setup dialog we specify a transient heat flow analysis and
activate the appropriate options. This results in the following batch analysis
commands.
tunnel.dcf
*FILOS
INITIA
*INPUT
*INPUT
READ APPEND FILE="coolpi.dat"
*HEATTR
BEGIN INITIA
BEGIN NONLIN
EQUAGE OFF
HYDRAT DGRINI=0.01
END NONLIN
TEMPER INPUT
END INITIA
BEGIN EXECUT
SIZES 0.2(10) 0.5(10) 1.0(3) 10.0(2)
END EXECUT
BEGIN OUTPUT FEMVIEW BINARY
TEMPER
REACTI
INTTMP
END OUTPUT
*END
The second *INPUT command specifies that data in batch format must be read
from an external file. This is the file with the temperature initialization of
the cooling pipes. The *HEATTR command invokes module heattr for a tran-
sient heat flow analysis. The INITIA command initiates the transient heat flow
analysis. We specify an initial degree of hydration equal to 0.01 and an initial
temperature field as defined in our data file. With the SIZES command in the
EXECUTE block, we define 25 steps ranging from 0.2 days at the beginning of
the analysis to 10 days at the end of the analysis. For output results we select
the temperatures, the degree of reaction, and the internal temperature of the
cooling pipes. All the results will be output at the nodes. As soon as the anal-
ysis run is terminated we enter the iDiana Results environment to assess the
results.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
408 Cooling Pipes in a Tunnel
tunnel.fvc
FEMVIEW TUNNEL
UTILITY TABULATE LOADCASES
RESULTS LOADCASE TR1 1
The load case tabulation shows the available load cases (time steps) with their
result data. Here we show only the first four load cases.
lc.tb
;
; Model: TUNNEL
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; TR1 1 TIME = .2 "Boundary case 1"
; Nodal : PTE....S
; Element : EL.PTE.S EL.DGR.S
;
; TR1 2 TIME = .4 "Boundary case 1"
; Nodal : PTE....S
; Element : EL.PTE.S EL.DGR.S
;
; TR1 3 TIME = .6 "Boundary case 1"
; Nodal : PTE....S
; Element : EL.PTE.S EL.DGR.S
;
; TR1 4 TIME = .8 "Boundary case 1"
; Nodal : PTE....S
; Element : EL.PTE.S EL.DGR.S
;
The nodal attribute PTE represents the temperature, the element attribute
EL.PTE represents the internal temperature of the cooling pipes and the ele-
ment attribute EL.DGR represents the degree of reaction. To start the results
presentation we select the first load case.
19.2.1 Temperature within Concrete
To display the temperatures in the concrete we first define a cross-section and
then display a contour plot.
Cross-section tunnel.fvc
VIEW MESH WALCON
EYE ROTATE TO 41 30 30
VIEW HIDDEN SHADE
CONSTRUCT SHAPE PLANE XSEC X 10.5
VIEW XSECTION XSEC
EYE LOCATE
EYE FRAME
First we activate the concrete wall by displaying the set WALCON. We create a
three-dimensional view in ‘hidden shade’ style. Then we define a plane cross-
section through our three-dimensional solid model at X = 10.5. In this case we
apply a PLANE shape. Via the XSECTION viewing option we display the cross-
section. Finally we draw the outlines of the model with dashed lines. This
clearly shows the location of the cross-section [Fig. 19.16a].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
19.2 Transient Nonlinear Heat Flow Analysis 409
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:19 xsec.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:20 tempc.ps
Model: TUNNEL Model: TUNNEL
TR1: Boundary case 1
Step: 1 TIME: .2
Nodal PTE....S PTE
Max/Min on model set:
Max = 18.7 Min = 10
17.9
17.1
16.3
15.5
Z 14.7
Z 14
Y 13.2
X Y 12.4
11.6
X 10.8
(a) cross-section definition via shape (b) contours
Figure 19.16: Concrete temperature
Contour plot tunnel.fvc
EYE LOCATE OFF
EYE NORMAL
VIEW OPTIONS EDGES OUTLINE
RESULTS NODAL PTE....S PTE
PRESENT CONTOUR LEVELS
We now switch off the location lines and display a ‘normal’ view of the cross-
section. With the EDGES OUTLINE viewing option we remove the inner grid of
the mesh within the cross-section. Then, we select the temperature results via
the NODAL option and the PTE attribute name. The CONTOUR LEVELS presenta-
tion option displays the temperature contours obtained for the first time step
[Fig. 19.16b].
Animation tunnel.fvc
RESULTS LOADCASE ALL
UTILITY SETUP ANIMATE LINEAR
PRESENT CONTOUR FROM 10 TO 40 LEVELS 9
DRAWING ANIMATE LOADCASES PLOTFILE temper
A very instructive manner to display the temperature development in time is
the animation sequence of temperature contours. First, we select all available
load cases. Then we set up the animation. The LINEAR option display the frames
sequentially from the first to the last and then starting again at the first. In
an animation sequence of contour plots it is important that the frames of the
animation all use the same color to represent a certain value. Therefore we
explicitly specify the values for the first and the last contour: 10° and 40°.
Now we have set all the parameters and options and finally we start the ani-
mation on the screen where the PLOTFILE option causes each of the frames to be
saved also on a separate file: temper001.ps, temper002.ps, . . . , temper025.ps.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:20 temper001
Model: TUNNEL
TR1: Boundary case 1
Step: 1 TIME: .2
Nodal PTE....S PTE
Max/Min on model set:
Max = 18.7 Min = 10
410 Cooling Pipes in a Tunnel
iDIANA 9.4.3-02 : TNO
iDIANA
Diana
9.4.3-02
BV : TNO
iDIANA
Diana
9.4.3-02
BV : TNO
iDIANA
Diana
9.4.3-02
BV : TNO
iDIANA
Diana
9.4.3-02
28BVOCT 2010
: TNO
iDIANA
01:36:20
Diana
9.4.3-02
28BV
temper001
OCT 2010
: TNO
iDIANA
01:36:20
Diana
9.4.3-02
28BV
temper002
OCT 2010
: TNO
iDIANA
01:36:20
Diana
9.4.3-02
28BV
temper003
OCT 2010
: TNO
iDIANA
01:36:20
Diana
9.4.3-02
28BV
temper004
OCT 2010
: TNO
iDIANA
01:36:20
Diana
9.4.3-02
28BV
temper005
OCT 2010
: TNO
iDIANA
01:36:20
Diana
9.4.3-02
28BV
temper006
OCT 2010
: TNO
iDIANA
01:36:20
Diana
9.4.3-02
28BV
temper007
OCT 2010
: TNO
iDIANA
01:36:20
Diana
9.4.3-02
28BV
temper008
OCT 2010
: TNO
01:36:20
Diana28BV
temper009
OCT 2010 01:36:20
28 temper010
OCT 2010 01:36:20
28 temper011
OCT 2010 01:36:20
28 temper012
OCT 2010 01:36:20 temper013
Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL
TR1: Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case 1
Step: 1 TIME: .2 Step: 2 TIME: .4 Step: 3 TIME: .6 Step: 4 TIME: .8 Step: 5 TIME: 1 Step: 6 TIME: 1.2 Step: 7 TIME: 1.4 Step: 8 TIME: 1.6 Step: 9 TIME: 1.8 Step: 10 TIME: 2 Step: 11 TIME: 2.5Step: 12 TIME: 3 Step: 13 TIME: 3.5
Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max = 18.7 Min = 10Max = 17.4 Min = 10Max = 21.2 Min = 10Max = 26.3 Min = 10Max = 31.2 Min = 10Max = 34.5 Min = 10Max = 37.7 Min = 10Max = 40 Min = 10 Max = 41.4 Min = 10 Max = 41.8 Min = 10Max = 41.7 Min = 10Max = 40.1 Min = 10Max = 37.7 Min = 10
40 40 40 40 40 40 40 40 40 40 40 40 40
37 37 37 37 37 37 37 37 37 37 37 37 37
34 34 34 34 34 34 34 34 34 34 34 34 34
31 31 31 31 31 31 31 31 31 31 31 31 31
28 28 28 28 28 28 28 28 28 28 28 28 28
Z Z Z Z Z Z 25 Z 25 Z 25 Z 25 Z 25 Z 25 Z 25 Z 25 25 25 25 25 25
22 22 22 22 22 22 22 22 22 22 22 22 22
19 19 19 19 19 19 19 19 19 19 19 19 19
X Y X Y X Y X Y X Y X Y 16 X Y 16 X Y 16 X Y 16 X Y 16 X Y 16 X Y 16 X Y 16 16 16 16 16 16
13 13 13 13 13 13 13 13 13 13 13 13 13
10 10 10 10 10 10 10 10 10 10 10 10 10
4.8 h 9.6 h 14 h 19 h
DRAWING ANIMATE LOADCASES
DRAWING PLOTFILE
ANIMATE LOADCASES
temper
DRAWING PLOTFILE
ANIMATE LOADCASES
temper
DRAWING PLOTFILE
ANIMATE LOADCASES
temper
DRAWING PLOTFILE 1d
ANIMATE LOADCASES
temper
DRAWING PLOTFILE temper 1.2 d 1.4 d 1.6 d 1.8 d
ANIMATE LOADCASES
DRAWING PLOTFILE
ANIMATE LOADCASES
temper
DRAWING PLOTFILE
ANIMATE LOADCASES
temper
DRAWING PLOTFILE
ANIMATE LOADCASES
temper
DRAWING PLOTFILE
ANIMATE LOADCASES
temper 2d
DRAWING PLOTFILE
ANIMATE LOADCASES
temper 2.5 d
DRAWING PLOTFILE 3d
ANIMATE LOADCASES
temper 3.5 d
DRAWING PLOTFILE
ANIMATE LOADCASES
temper PLOTFILE temper
iDIANA 9.4.3-02 : TNO
iDIANA
Diana
9.4.3-02
BV : TNO
iDIANA
Diana
9.4.3-02
BV : TNO
iDIANA
Diana
9.4.3-02
BV : TNO
iDIANA
Diana
9.4.3-02
28BVOCT 2010
: TNO
iDIANA
01:36:20
Diana
9.4.3-02
28BV
temper014
OCT 2010
: TNO
iDIANA
01:36:20
Diana
9.4.3-02
28BV
temper015
OCT 2010
: TNO
iDIANA
01:36:20
Diana
9.4.3-02
28BV
temper016
OCT 2010
: TNO
iDIANA
01:36:20
Diana
9.4.3-02
28BV
temper017
OCT 2010
: TNO
iDIANA
01:36:20
Diana
9.4.3-02
28BV
temper018
OCT 2010
: TNO
iDIANA
01:36:21
Diana
9.4.3-02
28BV
temper019
OCT 2010
: TNO
iDIANA
01:36:21
Diana
9.4.3-02
28BV
temper020
OCT 2010
: TNO
01:36:21
Diana28BV
temper021
OCT 2010 01:36:21
28 temper022
OCT 2010 01:36:21
28 temper023
OCT 2010 01:36:21
28 temper024
OCT 2010 01:36:21 temper025
Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL Model: TUNNEL
TR1: Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case TR1:
1 Boundary case 1
Step: 14 TIME: 4 Step: 15 TIME: 4.5Step: 16 TIME: 5 Step: 17 TIME: 5.5Step: 18 TIME: 6 Step: 19 TIME: 6.5Step: 20 TIME: 7 Step: 21 TIME: 8 Step: 22 TIME: 9 Step: 23 TIME: 10 Step: 24 TIME: 20 Step: 25 TIME: 30
Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max/Min on model set:
Max = 35 Min = 10 Max = 32.5 Min = 10 Max = 30.2 Min = 10Max = 28.1 Min = 10Max = 26.2 Min = 10Max = 24.6 Min = 10Max = 23.1 Min = 10Max = 21 Min = 10 Max = 19.5 Min = 10 Max = 18.3 Min = 10Max = 16.1 Min = 10Max = 15.1 Min = 10
40
37
34
31
28
Z 25
22
19
X Y
40
37
40
37
40
37
40
37
40
37
40
37
40
37
40
37
40
37 16 40
37
40
37
40
37
34 34 34 34 34 34 34 34 34 34 34 34
31
28
25
31
28
25
31
28
25
31
28
25
31
28
25
31
28
25
31
28
25
31
28
25
31
28
25
13 31
28
25
31
28
25
31
28
25
Z Z Z Z Z Z Z Z Z Z Z Z
22
19
16
22
19
16
22
19
16
22
19
16
22
19
16
22
19
16
22
19
16
22
19
16
22
19
16
10 22
19
16
22
19
16
22
19
16
X Y X Y X Y X Y X Y X Y X Y X Y X Y X Y X Y X Y
13 13 13 13 13 13 13 13 13 13 13 13
10 10 10 10 10 10 10 10 10 10 10 10
4d
DRAWING ANIMATE LOADCASES
DRAWING PLOTFILE 4.5 d
ANIMATE LOADCASES
temper
DRAWING PLOTFILE 5d
ANIMATE LOADCASES
temper
DRAWING PLOTFILE 5.5 d
ANIMATE LOADCASES
temper
DRAWING PLOTFILE temper 6d
ANIMATE LOADCASES
DRAWING PLOTFILE 6.5 d
ANIMATE LOADCASES
temper
DRAWING PLOTFILE
ANIMATE LOADCASES
temper 7d
DRAWING PLOTFILE
ANIMATE LOADCASES
temper 8d
DRAWING PLOTFILE
ANIMATE LOADCASES
temper 9d
DRAWING PLOTFILE
ANIMATE LOADCASES
temper
DRAWING PLOTFILE10 d 20 d 30 d
ANIMATE LOADCASES
temper
DRAWING PLOTFILE
ANIMATE LOADCASES
temper PLOTFILE temper
Figure 19.17: Concrete temperature animation sequence
DRAWING ANIMATE LOADCASES PLOTFILE temper
When the animation stops, iDiana prompts us what to do: restart?, exit?, etc.
We choose exit to leave the animation menu. The saved files allow us to show
the frames stationary in a document [Fig. 19.17].
Three-dimensional view tunnel.fvc
VIEW MESH WALCON
EYE ROTATE TO 41 30 30
EYE FRAME
VIEW HIDDEN SHADE
CONSTRUCT SHAPE PLANE YSEC Y 0.45
VIEW CUTAWAY YSEC BOTTOM
VIEW OPTIONS EDGES OUTLINE
EYE LOCATE
In order to represent the three-dimensional nature of the problem we will plot
the temperature contours in a longitudinal plane. We revert to a three-dimen-
sional ‘hidden shade’ view of the wall. Then we define the plane, called YSEC,
at Y = 0.45. The CUTAWAY viewing option shows the model in a ‘cutaway’ view
along the plane, with the BOTTOM part removed. Finally we produce an outline
view which shows the location of the cross-section plane [Fig. 19.18a].
Contour plot tunnel.fvc
RESULTS LOADCASE TR1 10
PRESENT CONTOUR FROM 10 TO 40 LEVELS 9
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
19.2 Transient Nonlinear Heat Flow Analysis 411
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:21 ycut3d.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:22 temp3d.ps
Model: TUNNEL Model: TUNNEL
TR1: Boundary case 1
Step: 10 TIME: 2
Nodal PTE....S PTE
Max/Min on model set:
Max = 41.8 Min = 10
40
37
34
31
28
25
Z Z 22
Y Y 19
16
13
X X 10
(a) cutaway view (b) temperature in cutaway plane
Figure 19.18: Temperature in longitudinal direction
In the animation sequence [Fig. 19.17], we see that the temperature reaches a
maximum after two days, i.e., at step number 10. We select this step via the
LOADCASE option and then display the temperature contours [Fig. 19.18b]. Note
that we apply the same levels as in the animation sequence.
19.2.2 Degree of Reaction
Looking at the animation sequence [Fig. 19.17], we can see that the temperature
reaches a maximum value in the core of the top part of the wall. On the
other hand, near the cooling circuit the temperature increase remains quite low.
Therefore, it is interesting to compare the development in time of the degree of
reaction for these two specific areas of the model.
Selection tunnel.fvc
EYE LOCATE OFF
VIEW XSECTION XSEC
EYE NORMAL
VIEW OPTIONS EDGES ALL
LABEL MESH ELEMENTS ’elem-old’
We revert to a cross-section view. The EDGES ALL option puts the inner grid of
the mesh back on the cross-section. We now get a contour plot of the tempera-
tures in the cross-section. Now we must get numbers of two elements for which
we want to assess the degree of reaction. Therefore we activate the graphics
cursor, by double-clicking the ’elem old’ option, which we then use to select
two elements in the middle column [Fig. 19.19a]: the first one is located on the
warmest part of the concrete, the second one on the coldest part in between the
cooling pipes. iDiana respectively shows element numbers 6169 and 3733.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
412 Cooling Pipes in a Tunnel
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:22 mesh2e.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:22 degrea.ps
Model: TUNNEL Model: TUNNEL
TR1: Boundary case 1 Element EL.DGR.S DGR
Step: 10 TIME: 2 Max/Min on whole graph:
Nodal PTE....S PTE Ymax = .998
Max/Min on model set: Ymin = .207E-1
Max = 41.8 Min = 10 Xmax = 30
Xmin = .2
Variation over loadcases
6169 Element 6169 Mean
1 Element 3733 Mean
.9
E
L .8
E
M
E .7
N
T
.6
E
L .5
.
D
G .4
R
.
S .3
D
G .2
R
3733 40 .1
37
34
31 0
28 0 2.5 5 7.5 10 12.5 15 17.5 20 22.5 25 27.5 30 32.5
Z 25 TIME
22
19
X Y 16
13
10
(a) element picking with cursor (b) graphs for two elements
Figure 19.19: Degree of reaction development in time
Drawing graphs tunnel.fvc
RESULTS LOADCASE ALL
RESULTS ELEMENT EL.DGR.S DGR
PRESENT GRAPH ELEMENT 6169 3733
We select the degree of reaction results for all load cases. For the two element
numbers that we picked up previously we display two graphs in one axes system
[Fig. 19.19b]. The graphs show that heat activates the hydration of concrete.
19.2.3 Internal Temperature of Cooling Pipe
Finally, we are going to assess the evolution of the temperature within the
cooling pipes.
Element numbers display tunnel.fvc
VIEW MESH COOLP1
EYE ROTATE TO 41 30 30
EYE FRAME
LABEL MESH ELEMENTS VIEWMODE VIOLET
VIEW MESH COOLP2
LABEL MESH ELEMENTS VIEWMODE VIOLET
VIEW MESH COOLP3
LABEL MESH ELEMENTS VIEWMODE VIOLET
We first rotate the model in order to get a suitable three-dimensional view.
Then we display each cooling circuit individually with labeled element numbers
[Fig. 19.20a-c]. From these views we can easily read the element numbers which
correspond to the end part of the cooling circuits.
Drawing graphs tunnel.fvc
RESULTS ELEMENT EL.PTE.S PTE
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
19.2 Transient Nonlinear Heat Flow Analysis 413
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:22 cp1elnr.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:22 cp2elnr.ps
Model: TUNNEL Model: TUNNEL
354348
352328 353
351 347
327 304
284 346
283
326 264260 303
262240 263 345
325 302
261 282 259 344
239 216 301
196 324 176 258
281 343
174 238 323 175172 215 300
173152 195 280 130 171 214 257 342
110 151 194 237 322 299
279 129 170 213 256 341
109 150 193 236 321 298
278 128 169 255 340
108 149 235 212 297
192 320
277 127 168 211 254 339
107 148 191 234 319 296
276 126 167 210 253 338
106 147 190 233 318 295
275 125 166 252 337
105 146 189 232 209 294
317
274 124 165 208 251 336
104 145 188 231 316 293
273 123 164 207 250 335
103 144 187 230 315 292
272 122 163 249 334
102 143 186 229 206 291
314
271 121 162 205 248 333
101 142 185 228 313 290
270 120 161 204 247 332
100 141 184 227 312 289
269 119 160 246 331
203
99 140 183 226 311 288
225
268 118 159 202 245 330
98 139 182 310 287
267 117 158 201 244 329
97 138 224 309 286
181 266 243 350
349 116 157 200
96 137 180 223 285
265 115 156 199 242
95 136 179 222 306
308
241307
114 155 198
94 135 178 221305
113 154 197
93 134 177
112 220
153219
Z 92 218
133217 Z
Y Y 111
91 132
131
X X
(a) circuit 1 (b) circuit 2
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:22 cp3elnr.ps
Model: TUNNEL
47
46
45 87
367
12 43 86
23 66
42 85
22 65
41 84
21 64
40 83
20 63
39 82
19 62
38 81
18 61
37 80
17 60
36 79
16 59
35 78
15 58
34 77
14 57
33 76
13 56
32 75
12 55
31 74
11 54
30 73
10 53
29 72
9 52
28 71
8 51
27 70
Z 7 50
Y 26 69
6 49
25 68
5 48 90
X 24 89
4 88
44
(c) circuit 3
Figure 19.20: Element numbers for cooling pipes
PRESENT GRAPH ELEMENT 349 350 88
We select the temperature results for the cooling pipes via the EL.PTE attribute
name. We display three graphs in one axes system corresponding respectively
to element numbers 349, 350 and 88 [Fig. 19.21]. The development in time of
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:36:22 cptmpg.ps
Model: TUNNEL
Element EL.PTE.S PTE
Max/Min on whole graph:
Ymax = 20.1
Ymin = 10.7
Xmax = 30
Xmin = .2
Variation over loadcases
Element 349 Mean
21 Element 350 Mean
Element 88 Mean
20
E 19
L
E
M 18
E
N
T 17
E 16
L
.
P 15
T
E 14
.
S
13
P
T 12
E
11
10
0 2.5 5 7.5 10 12.5 15 17.5 20 22.5 25 27.5 30 32.5
TIME
Figure 19.21: Temperature development in cooling pipes
the internal temperature is exactly the same for element number 349 and for
element number 350. This is due to the symmetry along the middle XZ-plane
of the concrete wall. Moreover, we may notice that the internal temperatures
for the third cooling circuit reaches lower values than for those of the two other
cooling circuits. Indeed, the concentration of cooling pipe elements is larger on
the bottom part of the concrete wall than on the top part. This results in lower
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
414 Cooling Pipes in a Tunnel
values of internal temperature due to a larger density of cooling elements.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
Chapter 20
Early Age Behavior of a
Purification Wall
Name: PurWal
Path: /Examples/ConcMas/PurWal
Keywords: analys: flow flowst heat nonlin phase physic stagge transi.
constr: initia suppor temper. elemen: b2ht cq16e ct12e
flow potent pstrai q4ht t3ht. load: elemen node temper time
weight. materi: adiaba capaci conduc elasti hydrat isotro ma-
turi power viscoe. option: direct groups newton regula units.
post: binary femvie. pre: femgen. result: cauchy displa
reacti stress temper total.
plane strain
0.70
2.30 wall
28.60
0.80 base
5.30
soil foundation
Figure 20.1: Specimen of the wall [m]
This example combines a coupled flow–stress analysis with a phased analysis,
applied on a purification wall [Fig. 20.1]. The base of the structure consists of
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
416 Early Age Behavior of a Purification Wall
a slab of 0.8 m thick and 5.3 m wide. After thirty-six days a water-purification
wall has been cast on the base. The wall is 0.7 m thick and 2.3 m high. The
structure is 28.6 m long and directly founded on the underlaying soil. The
casts of the base slab and the wall have been removed when the concrete was
seven days old. To completely analyze the structure we will perform a staggered
analysis for each of the two construction phases: the casting of the slab and the
casting of the wall.
20.1 Finite Element Model
Due to the large length of the structure we may apply plain strain elements with
the same discretization in space for the thermal and the stress analysis. These
isoparametric elements are quadratically interpolated with eight nodes for the
concrete parts and six nodes for the soil foundation. To make the finite element
model we start iDiana and enter the Design environment with the model name.
iDiana
FEMGEN PURWAL
Analysis and Units
Analysis Selection
Model Type: →Heatflow-Stress Staggered Plane Strain
Units Definition
Length: →Meter
Mass: →Kilogram
Time: →Day
Temperature: →Celsius
In the Analysis and Units dialog we specify that the model will be applied for
a staggered heat flow–stress analysis in a plane strain configuration. We also
specify the applied units [m, kg, day, °C].
20.1.1 Geometry Definition
We will define the geometry of the two-dimensional model in the XY -plane
[Fig. 20.2]. First the points and then the surfaces between the points.
Points purwal.fgc
GEOMETRY POINT COORD 0.00 0.00
GEOMETRY POINT COORD 5.00 0.00
GEOMETRY POINT COORD 5.00 3.00
GEOMETRY POINT COORD 2.65 3.00
GEOMETRY POINT COORD 0.35 3.00
GEOMETRY POINT COORD 0.00 3.00
GEOMETRY POINT COORD 2.65 3.80
GEOMETRY POINT COORD 0.35 3.80
GEOMETRY POINT COORD 0.00 3.80
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
20.1 Finite Element Model 417
♥
q is boundary flux
K J
q=0
uX = 0 convective exchange
I H G
T = 20°
6.10
F
C
E D
3.80
T = 20°
3.00
uX = 0
Y
A
B
X T = 20°
0.35 uY = 0
2.65
5.00
Figure 20.2: Two-dimensional geometry and boundary conditions [m, °C]
GEOMETRY POINT COORD 0.35 6.10
GEOMETRY POINT COORD 0.00 6.10
EYE FRAME ALL
DRAWING CONTENTS MONITOR POSITION 1.00 0.95
VIEW GEOMETRY ALL BLUE
LABEL GEOMETRY POINTS
We specify the XY -coordinates of points A to K. Note that we may omit the
Z-coordinates. By default iDiana will assume these to be zero. We display the
specified points, labeled with their names and fitted in the iDiana viewport
[Fig. 20.3a]. To ensure visibility for the entire model we move the monitor to
the right.
Surfaces purwal.fgc
GEOMETRY SURFACE 4POINTS P9 P8 P10 P11
CONSTRUCT SET WALCON APPEND S1
GEOMETRY SURFACE 4POINTS P6 +P5 P4 P7 +P8 P9
CONSTRUCT SET BASCON APPEND S2
GEOMETRY SURFACE 4POINTS P1 P2 P3 +P4 +P5 P6
CONSTRUCT SET FOUNDA APPEND S3
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY LINES ALL VIOLET
LABEL GEOMETRY SURFACES ALL RED
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
418 Early Age Behavior of a Purification Wall
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:40 geom1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:41 geom2.ps
Model: PURWAL Model: PURWAL
Analysis: DIANA Analysis: DIANA
P11 P10 Model Type: Heatflow-Stress Staggered plane strain L3 Model Type: Heatflow-Stress Staggered plane strain
L4
S1
L2
P9 P8 P7 L1 L11
L9
L5
S2
L8
P6 P5 P4 P3 L6 L10L7 L16 L15
L12
S3
L14
Y Y
Z X P1 P2 Z X L13
(a) points (b) lines and surfaces
Figure 20.3: Geometry
We create three surfaces, representing the foundation, the base slab and the pu-
rification wall. We assemble the geometry components in sets FOUNDA, BASCON
and WALCON respectively. Finally, we display the defined geometry including
labels for lines and surfaces [Fig. 20.3b]. Note that line L10 corresponds to the
association of lines L6 and L7, that line L11 corresponds to the association of
lines L1 and L9, and that line L16 corresponds to the association of lines L6, L7
and L15.
20.1.2 Meshing
We may now create a finite element mesh on the defined geometry. First we will
mesh the soil foundation and then the concrete structure comprising the wall
and the base slab.
Soil foundation purwal.fgc
MESHING DIVISION LINE L6 10
MESHING DIVISION LINE L7 30
MESHING DIVISION LINE L12 916
MESHING DIVISION LINE L13 8
MESHING DIVISION LINE L14 8
MESHING DIVISION LINE L15 -408
MESHING TYPES S3 TR6 CT12E
MESHING OPTIONS ALGORITHM DELAUNAY S3 2
MESHING GENERATE
VIEW MESH FOUNDA
VIEW HIDDEN SHADE
VIEW OPTIONS SHRINK MESH
VIEW OPTIONS COLOUR OFF
LABEL MESH QUALITY
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
20.1 Finite Element Model 419
By meshing the surface representing the foundation, we have to ensure the
continuity of the element size between the base slab and the soil part. Moreover,
away from the concrete structure, a coarser mesh is satisfactory. Therefore we
explicitly specify the divisions of the lines. The Delaunay meshing algorithm
can create a triangular free mesh on any type of surface and thus is well suited
to mesh the bottom surface of the model. We select therefore the triangular
CT12E plane strain element. We generate the mesh and display it in color-filled
style. Then we apply the QUALITY option to have the elements colored according
to their ‘shape quality’ [Fig. 20.4a]. The green color indicates the elements that
have passed the quality tests, in this case all of them.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:41 mesh1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:41 mesh2.ps
Model: PURWAL Model: PURWAL
Analysis: DIANA Analysis: DIANA
Model Type: Heatflow-Stress Staggered plane strain Model Type: Heatflow-Stress Staggered plane strain
Y Y
Z X Z X
(a) soil foundation (quality) (b) concrete structure added
Figure 20.4: Mesh display
Wall and base slab purwal.fgc
MESHING TYPES S1 QU8 CQ16E
MESHING TYPES S2 QU8 CQ16E
MESHING DIVISION LINE L1 10
MESHING DIVISION LINE L2 26
MESHING DIVISION LINE L3 10
MESHING DIVISION LINE L4 26
MESHING DIVISION LINE L5 10
MESHING DIVISION LINE L8 10
MESHING DIVISION LINE L9 30
MESHING GENERATE
LABEL MESH OFF
VIEW MESH +BASCON RED
VIEW MESH +WALCON BLUE
We select the quadrilateral quadratic CQ16E plane strain element for the surfaces
of the slab and the wall. We specify the divisions of the lines in order to get a
mesh as much regular as possible. Then we generate the mesh and superpose it
on the display with different colors for the slab and the wall [Fig. 20.4b].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
420 Early Age Behavior of a Purification Wall
20.1.3 Modeling the Boundary
For the heat flow analysis, we must describe the heat convection along the
outside of the concrete structure composed by the base slab and the wall. We
should keep in mind that for the heat flow analysis, Diana will automatically
transform the quadratic structural elements to linear flow elements. Therefore,
we will apply linear boundary elements.
Lines along boundaries purwal.fgc
VIEW GEOMETRY ALL
LABEL GEOMETRY POINTS
CONSTRUCT SET OPEN BOUNDA
CONSTRUCT SET OPEN BOUND2
GEOMETRY LINE STRAIGHT P11 P10 5
GEOMETRY LINE STRAIGHT P10 P8 13
CONSTRUCT SET CLOSE
CONSTRUCT SET OPEN BOUTMP
GEOMETRY LINE STRAIGHT P9 P8 5
CONSTRUCT SET CLOSE
CONSTRUCT SET OPEN BOUND1
GEOMETRY LINE STRAIGHT P8 P7 15
GEOMETRY LINE STRAIGHT P7 P4 5
CONSTRUCT SET CLOSE
CONSTRUCT SET CLOSE
We start by redefining the appropriate lines of the geometry. All these lines
correspond to the outside of the concrete structure and were previously created
automatically due to the definition of the surfaces S1 and S2 but with twice as
much elements as in the present case. We put the lines of the boundary in some
useful sets for the phased analysis:
BOUND2 with boundary elements of the purification wall that will be activated
during the second phase of the analysis,
BOUND1 with the boundary elements of the base slab that will be activated
during the first phase of the analysis,
BOUTMP with the boundary elements of the base slab that will be activated
during the first phase of the analysis but deactivated during the second
phase.
Note that we also put all boundary elements in a set called BOUNDA.
Geometry display purwal.fgc
VIEW GEOMETRY BOUND2 BLUE
VIEW GEOMETRY +BOUND1 VIOLET
VIEW GEOMETRY +BOUTMP RED
LABEL GEOMETRY LINES BOUND2 BLUE
LABEL GEOMETRY LINES BOUND1 VIOLET
LABEL GEOMETRY LINES BOUTMP RED
We display the defined geometry with different colors for the sets and including
labels for lines [Fig. 20.5a].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
20.1 Finite Element Model 421
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:42 geobnd.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:42 meshall.ps
Model: PURWAL Model: PURWAL
Analysis: DIANA Analysis: DIANA
L17 Model Type: Heatflow-Stress Staggered plane strain Model Type: Heatflow-Stress Staggered plane strain
L18
L19 L20
L21
Y Y
Z X Z X
(a) lines of geometry (b) element mesh
Figure 20.5: Modeling the boundary
Meshing and display purwal.fgc
MESHING TYPES BOUNDA BE2 B2HT
MESHING GENERATE
MESHING MERGE ALL 0.001
VIEW MESH ALL GREEN
VIEW MESH +BOUNDA WHITE
For the boundaries we select the linear heat flow boundary element B2HT and
generate the mesh. Since the lines in the set BOUNDA have no common points
with the outer lines of sets WALCON and BASCON, the generated boundary el-
ements will not be connected to the structural part. To solve this problem,
we apply a merging operation on the mesh for the concerned outer lines of the
model. The parameter value 0.001 indicates a tolerance of one millimeter for
the check on coinciding nodes. Finally we display the mesh with different colors
for the structural elements and for the boundaries [Fig. 20.5b].1
20.1.4 Material Properties
We must now specify material properties for the soil, the concrete and the
boundary. Therefore we launch the Property Manager dialog.
iDiana
View →Property Manager...
↑
Property Manager
···
1 In a document, the color option WHITE yields black.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
422 Early Age Behavior of a Purification Wall
Soil iDiana
Property Manager
↑ Materials Material Name: SOIL
↑Flow →Isotropic
↑Linear Elastic →Isotropic
↑Mass →Mass Density
↑Expansion →Isotropic - constant params.
We define the material properties for thermo-mechanical soil behavior in a ma-
terial named SOIL, according to Table 20.1. For the isotropic flow properties
Table 20.1: Thermo-mechanical soil properties
Thermal conductivity λ 191 kJ/(m·K·day)
Thermal capacity c 3200 kJ/(m3 ·K)
Young’s modulus E 630 MPa
Poisson’s ratio ν 0.3
Mass density ρ 1720 kg/m3
Thermal expansion coefficient α 7×10−6 K−1
we specify the thermal conductivity and capacity. For linear elasticity we spec-
ify Young’s modulus and Poisson’s ratio. Then we specify the mass density.
Finally, for isotropic expansion, we specify the thermal expansion coefficient.
Concrete iDiana
Property Manager
Materials Material Name: CONCRETE
↑External →External Data from File
For a material CONCRETE we specify the thermal and mechanical properties of
concrete according to Table 20.2. These values apply for slowly hardening con-
crete according to the formulas provided by the Japan Society of Civil Engineers
(JSCE) [8]. They define the compressive strength, the tensile strength and the
Young’s modulus. A large number of these material properties are either tem-
perature or time dependent. In this context, we create a data file in Diana
batch format.
concrete.dat
CONDUC 3.110000E+02
CAPACI 2.675000E+03
ADIAB 0.0 20.00
0.1 23.94
0.2 27.50
0.3 30.72
0.4 33.63
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
20.1 Finite Element Model 423
Table 20.2: Properties of slowly hardening concrete
Cement quality SL
` ´
Adiabatic temp. rise Tadiab 36 1 − exp−1.25t °C
Arrhenius constant cA 5000 K
Thermal conductivity λ 311 kJ/(K·m·day)
Thermal capacity c 2765 kJ/(K·m3 )
Convection coefficient, cast h 700 kJ/(K·m2 ·day)
Convection coefficient, no cast h 1500 kJ/(K·m2 ·day)
Mass density ρ 2300 kg/m3
Young’s modulus E 27000 MPa
Poisson’s ratio ν 0.2
Thermal expansion coefficient α 10−5 °C−1
t
Compressive fc (t) ×fc (91) MPa
6.2 + 0.93 t
strength
fc (91) 29 MPa
p
Tensile strength ft (t) 0.35 fc (t) MPa
p
Young’s modulus EC (t) 4700 φ(t) fc (t) MPa
for 0 ≤ t < 3 days φ(t) 0.73
for 3 ≤ t < 5 days φ(t) 0.135 t + 0.325
for t ≥ 5 days φ(t) 1.00
0.5 36.26
0.6 38.63
0.7 40.78
0.8 42.72
0.9 44.48
1.0 46.07
1.5 51.99
2.0 55.56
2.5 57.72
3.0 59.02
4.0 60.28
5.0 60.74
10. 61.00
70. 61.00
ARRHEN 5000.
YOUNG 27000.
THERMX 10.E-6
POISON 0.2
DENSIT 2300.
POWER 0.3 33. 1. 0.3
YOUHAR JSCE
YOUN91 27000.
CEMTYP SL
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
424 Early Age Behavior of a Purification Wall
FTTIME 0. 0.25 0.5 0.75 1. 2. 3. 4. 5. 6. 7. 8. 9.
10. 15. 20. 30. 70.
FTVALU 0. 0.37 0.52 0.62 0.71 0.94 1.09 1.2 1.28 1.34 1.4
1.44 1.48 1.51 1.63 1.69 1.77 1.87
The ADIAB data item specifies the temperature values in °C during adiabatic hy-
dration reaction development at different ages ranging from 0 to 70 days. These
values are calculated according to the formula for Tadiab [Table 20.2]. To model
viscoelasticity Diana offers the young hardening concrete model according to
JSCE. For that, we must use the Double Power Law model and specify YOUHAR
as JSCE [Vol. Material Library]. The Power Law is used with the parameters
a = 1.0 and p = d = 0.3 and a development time td = 33 days. Two more
parameters are required: YOUN91 for fc (91) and CEMTYP for the cement quality
[Table 20.2]. Finally, the two series of values FTTIME and FTVALU correspond to
the evolution of the tensile strength according to the formula for ft (t) [Table
20.2]. These two series are necessary to calculate the crack index. All the other
data items, respectively CONDUC, CAPACI, ARRHEN, YOUNG, THERMX, POISON and
DENSIT, have been defined according to Table 20.2. These last seven items could
also have been defined via the Property Manager dialog.
Convection along boundary iDiana
Property Manager
Materials Material Name: CONVEC1
↑
↑External →External Data from File
External File Name: convec1.dat
Materials Material Name: CONVEC2
↑External →External Data from File
External File Name: convec2.dat
We specify the convection coefficient for the boundary elements, along with their
time dependencies, via two files in Diana batch input format.
convec1.dat
CONVEC 7.000000E+02
TIME 0. 7. 7.0001 70.
CONVTT 7.000000E+02 7.000000E+02 1.500000E+03 1.500000E+03
convec2.dat
CONVEC 7.000000E+02
TIME 0. 43. 43.0001 70.
CONVTT 7.000000E+02 7.000000E+02 1.500000E+03 1.500000E+03
In both data files, the CONVEC data item is defined according to Table 20.2. The
sudden changes of CONVTT data item correspond to the removal of the concrete
form work. For the first phase, it happens at the age of seven days as defined in
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
20.1 Finite Element Model 425
convec1.dat. As the phased analysis will be performed by using a continuous
time, i.e., time will not be set to zero at the start of the second phase but
reinitialized to 36 days which corresponds to the end-time of the first phase.
File convec2.dat has to provide a change of the convection coefficient at the
age of 36 + 7 = 43 days.
Assignment purwal.fgc
PROPERTY ATTACH FOUNDA MATERIAL SOIL
PROPERTY ATTACH BASCON MATERIAL CONCRETE
PROPERTY ATTACH WALCON MATERIAL CONCRETE
PROPERTY ATTACH BOUTMP MATERIAL CONVEC1
PROPERTY ATTACH BOUND1 MATERIAL CONVEC1
PROPERTY ATTACH BOUND2 MATERIAL CONVEC2
Finally, we assign the materials to the corresponding sets of the model.
20.1.5 Boundary Conditions and Loading
For a model in a staggered analysis we must specify the boundary conditions
for the flow analysis, and the mechanical load for the structural stress analysis.
For both we must also specify their dependency of time.
Boundary conditions for flow analysis. The boundary conditions for the
flow analysis comprise the fixed temperature on the outer surfaces of the soil
foundation and the convective flux on the outer surfaces of the concrete structure
[Fig. 20.3 p. 418]. We will define these boundary conditions in two separate
boundary cases. In the Design environment, a boundary case is considered
as a load case and its constituents must be defined via the PROPERTY LOADS
command.
purwal.fgc
VIEW GEOMETRY ALL
LABEL GEOMETRY LINES
PROPERTY LOADS FIXTEMP 1 L13 20.
PROPERTY LOADS FIXTEMP 1 L14 20.
PROPERTY LOADS FIXTEMP 1 L15 20.
PROPERTY LOADS EXTTEMP 2 BOUNDA 20.
VIEW MESH
VIEW OPTIONS SHRINK OFF
LABEL MESH LOADS 1
LABEL MESH LOADS 2 BLUE
With the FIXTEMP load class we specify a prescribed temperature on the lines
along the boundary. These first three boundary conditions constitute the first
load case. For the boundary elements, we must also specify the external tem-
perature so that Diana can calculate the convective flux at the outer surface of
the concrete. With the EXTTEMP load class we define the second load case that
contains the external temperature for the boundary elements. We display the
mesh with the two defined load cases as labels [Fig. 20.6a].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
426 Early Age Behavior of a Purification Wall
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:43 load1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:43 load2.ps
Model: PURWAL Model: PURWAL
Analysis: DIANA Analysis: DIANA
20
20
20
20
20 Model Type: Heatflow-Stress Staggered plane strain Model Type: Heatflow-Stress Staggered plane strain
20
20
20
20
20
20
20
20
20
20
20
20
20
20
20
20
20
20202020202020202020202020202020
20
20
20
20
20
202020 20 20 20 20 20 20
20
20
20
20
20
20
Y Y
20
Z X Z X
20 20 20 20 20 20 20 20 20
(a) flow boundary conditions (b) dead weight
Figure 20.6: Loading
Dead weight purwal.fgc
PROPERTY LOADS GRAVITY 3 ALL -9.81E-6 2
LABEL MESH LOADS OFF
LABEL MESH LOADS 3
For the nonlinear structural analysis we define the dead weight of the model via
the GRAVITY load class as load case 3. The gravity acceleration g = 9.81×10−6
MN/kg acts downward, i.e., in the −Y direction. To check the load we display
its labels (arrows) on the mesh [Fig. 20.6b].
Time dependency purwal.fgc
CONSTRUCT TCURVE TCDUM LIST 0 1. 70 1.
PROPERTY ATTACH LOADCASE 1 TCDUM
PROPERTY ATTACH LOADCASE 2 TCDUM
PROPERTY ATTACH LOADCASE 3 TCDUM
For transient coupled flow–stress analysis Diana requires the variation in time
of the heat flow boundary conditions and the mechanical loading. We specify
this variation with a so-called time curve. We assume that the defined load
cases 1, 2 and 3 do not change in time. Via the LIST option we specify a time
interval from t = 0 to t = 70 days with a constant multiplication factor of 1.
We assign the time curve to load cases 1, 2 and 3.
20.1.6 Boundary Constraints
The boundary constraints of the model consist of a symmetry condition along
the left edge, a vertical support of the bottom edge, and a horizontal support
of the right edge of the foundation.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
20.1 Finite Element Model 427
Symmetry and supports purwal.fgc
PROPERTY BOUNDARY CONSTRAINT L4 X
PROPERTY BOUNDARY CONSTRAINT L5 X
PROPERTY BOUNDARY CONSTRAINT L12 X
PROPERTY BOUNDARY CONSTRAINT L13 Y
PROPERTY BOUNDARY CONSTRAINT L14 X
LABEL MESH OFF
LABEL MESH CONSTRNT
We prevent the horizontal and vertical displacements of the appropriate lines
along the edges of the model. We display these boundary constraints on the
mesh [Fig. 20.7a].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:43 supp.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:43 initem.ps
Model: PURWAL Model: PURWAL
Analysis: DIANA Analysis: DIANA
Model Type: Heatflow-Stress Staggered plane strain 20
2020
2020
2020
2020
20
20 Model Type: Heatflow-Stress Staggered plane strain
20
20
20
2020
20
20
2020
2020
2020
2020
20
20
20
20
20
2020
20
20
2020
2020
2020
2020
20
20
20
20
20
2020
20
20
2020
2020
2020
2020
20
20
20
20
20
2020
20
20
2020
2020
2020
2020
20
20
20
20
20
2020
20
20
2020
2020
2020
2020
20
20
20
20
20
2020
20
20
2020
2020
2020
2020
20
20
20
20
20
2020
20
20
2020
2020
2020
2020
20
20
20
20
20
2020
20
20
2020
2020
2020
2020
20
20
20
20
20
2020
20
20
2020
2020
2020
2020
20
20
20
20
20
2020
20
20
2020
2020
2020
2020
20
20
20
20
20
2020
20
20
2020
2020
2020
2020
20
20
20
20
20
2020
20
20
2020
2020
2020
2020
20
20
20
20
20
2020
20
20
20 20
20
20
202020
20
2020
20 20
20 20
20 20
20 20
20 20
202020 20
20202020
20 20
202020
2020 20
202020
20
20 20
20
20 20202020202020202020202020202020
20
20
20 20
20
20
20
20 20
20
2020
20 20
20 20
20 20
20 20
20 20
202020 20
20202020
20 20
202020
2020 20
202020
20
20 20
20
20 20202020202020202020202020202020
20
20
20 20
20
20
20
20 20
20
2020
20 20
20 20
20 20
20 20
20 20
202020 20
20202020
20 20
202020
2020 20
202020
20
20 20
20
20 20202020202020202020202020202020
20
20
20 20
20
20
20
20 20
20
2020
20 20
20 20
20 20
20 20
20 20
202020 20
20202020
20 20
202020
2020 20
202020
20
20 20
20
20 20202020202020202020202020202020
20
20
20 20
20
20
20
20 20
20
2020
20 20
20 20
20 20
20 20
20 20
202020 20
20202020
20 20
202020
2020 20
202020
20
20 20
20
20 20202020202020202020202020202020
20
20
20
20
20
2020
20
2020
20
20
2020
20
20
2020
2020
2020
2020
2020
2020
20
20
20
202020
20
2020
20
2020
020
220 20
20
20 2020
202020
20
2020
20
20
2 2020 20 20 20 20
020 20 20
202020 20
2 20
02 0 20
220
020
2 0 202 02020
2 0 20
2020 20 20 20 202020202020 20 20
202020 20 20 20 20 20 20
2020 20 20 20
20 2020 20 20 20 20 2020 20 20 20
2020 20 20 20 20 20 20
20 20 20
20 20 20 20 20 20
2020 20 20 20 20
202020 20 20
20 20 20 20
20 20 20 20
2020 20
20
20 20 20 20 20 20
20
20 20
20 20 20 20
20 20 20
20 20 20 20
Y Y
20 20 20 20 20 20
Z X Z X
20 20 20 20 20 20 20 20 20
(a) symmetry conditions and supports (b) initial temperatures
Figure 20.7: Boundary constraints and initial conditions
20.1.7 Initial Temperature Field
By default Diana will assume a zero temperature field at the start of a transient
heat flow analysis. However, in this example the environmental temperature
is 20 °C and we may assume that this is also the initial temperature of the
structure.
purwal.fgc
PROPERTY INITIAL INITEMP ALL 20.
LABEL MESH OFF
LABEL MESH INITIAL ALL RED
We specify an initial condition of 20 °C for all nodes of the model. We display
the values of the initial temperature on the mesh [Fig. 20.7b].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
428 Early Age Behavior of a Purification Wall
20.2 First Stage – Casting the Base Slab
The first stage of our analysis is a staggered flow–stress analysis. This analysis
is nonlinear because the material properties for the model depend on the tem-
perature and on the time. First, we write an input data file in Diana batch
format.
iDiana
UTILITY WRITE DIANA
yes
FILE CLOSE
yes
Early age behavior of a purification wall
ANALYSE PURWAL
Analysis Setup
specification of options
The ANALYSE command initiates the analysis of the model named PURWAL. Via
the Analysis Setup dialog we specify that this is a phased analysis. We define set
FOUNDA, BASCON, BOUND1 and BOUTMP as active and run the analysis. Then we
click Next in the Analysis Setup dialog. Therefore, we may specify a transient
heat transfer analysis. In the Analysis Setup dialog we may specify the various
analysis options for the heat flow analysis. Then we click Next. Using the same
filos file, we change the analysis type to Structural Nonlinear. Once more
we may specify the various analysis options for the mechanical analysis. These
operations result in the following batch analysis commands.
phase1.dcf
*FILOS
INITIA
*INPUT
*PHASE
ACTIVE ELEMEN FOUNDA BASCON BOUND1 BOUTMP
*HEATTR
BEGIN INITIA
BEGIN NONLIN
EQUAGE OFF
HYDRAT DGRINI=0.01
END NONLIN
TEMPER INPUT
END INITIA
EXECUT SIZES 0.1(20) 0.5(10) 1.0(3) 5.0(4) 6.0
BEGIN OUTPUT FEMVIE FILE="FLOW1"
TEMPER
REACTI
END OUTPUT
*NONLIN
BEGIN TYPE
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
20.2 First Stage – Casting the Base Slab 429
BEGIN PHYSIC
TEMPER
VISCOE
END PHYSIC
END TYPE
BEGIN EXECUTE
TIME STEPS EXPLIC SIZES 0.1(20) 0.5(10) 1.0(3) 5.0(4) 6.0
BEGIN ITERAT
BEGIN CONVER
SIMULT
FORCE TOLCON=1.0E-10
DISPLA TOLCON=1.0E-10
END CONVER
END ITERAT
END EXECUT
BEGIN OUTPUT FEMVIE FILE="STRUC1"
DISPLA
STRESS
STRESS TOTAL CAUCHY CRKIND
END OUTPUT
*END
When the analysis has terminated we enter the iDiana Results environment.
20.2.1 Heat Flow Analysis Results
We enter the Results environment with model FLOW1 to assess the heat flow
analysis results of the first construction stage.
Node numbers flow1.fvc
FEMVIEW FLOW1
VIEW MESH BASCON
EYE FRAME
LABEL MESH NODES
We display the mesh of the base slab and label the node numbers [Fig. 20.8a].
We will need these numbers to display the analysis results.
Temperature in time flow1.fvc
RESULTS LOADCASE TR1
RESULTS NODAL PTE....S PTE
PRESENT GRAPH NODE 1 234 237
In order to study the evolution of the temperature in time, we select for all load
cases (time steps) the PTE nodal result. We make a graph of the temperature
evolution at three different nodes along the axis of symmetry of the model
corresponding to the top, the middle and the bottom of the base slab [Fig. 20.8-
b]. It appears that the temperature in the core of the slab reaches a maximum
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
430 Early Age Behavior of a Purification Wall
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:59 basno.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:59 teslab.ps
Model: FLOW1 Model: FLOW1
Nodal PTE....S PTE
Max/Min on whole graph:
Ymax = 38.9
Ymin = 20.1
Xmax = 36
Xmin = .1
Variation over loadcases
Node 1
40 Node 234
Node 237
38
1 2 3 4 5 6 263 269 275 281 287 293 299 305 311 317 323 329 335 341 347 N 36
O
D
233238243248253258 264 270 276 282 288 294 300 306 312 318 324 330 336 342 348 A 34
L
P 32
234239244249254259 265 271 277 283 289 295 301 307 313 319 325 331 337 343 349 T
E 30
.
235240245250255260 266 272 278 284 290 296 302 308 314 320 326 332 338 344 350 .
. 28
.
S
236241246251256261 267 273 279 285 291 297 303 309 315 321 327 333 339 345 351 26
P
T
237242247252257262 268 274 280 286 292 298 304 310 316 322 328 334 340 346 352 E 24
22
20
0 5 10 15 20 25 30 35 40
Y TIME
Z X
(a) nodes (b) time graph
Figure 20.8: Temperature evolution in the base slab
around the 16th time step, i.e., approximately around 1.6 days. We will now look
at the temperature distribution in the concrete slab at the time corresponding
to the maximum temperature rise.
Temperature after 1.6 days flow1.fvc
RESULTS LOADCASE TR1 16
PRESENT GRAPH LINE NODES THROUGH 234 349
VIEW MESH BASCON
VIEW OPTIONS EDGES OUTLINE
PRESENT CONTOUR LEVELS
We select the load case TR1 16 which corresponds to the maximum temperature
rise. With the NODES THROUGH option, by clicking once on the first node and
twice on the second node, we display the horizontal temperature distribution in
the core of the concrete slab [Fig. 20.9b]. We also make a contour plot of the
temperature distribution in an outline view of the base slab [Fig. 20.9b].
20.2.2 Structural Analysis Results
We enter the Results environment with model STRUC1 to assess the structural
analysis results of the first construction stage.
Element numbers struc1.fvc
FEMVIEW STRUC1
VIEW MESH BASCON
EYE FRAME
LABEL MESH ELEMENTS VIEWMODE VIOLET
We display the mesh of the base slab, including the element numbers [Fig. 20.10-
a]. We will need these numbers to display the analysis results.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
20.2 First Stage – Casting the Base Slab 431
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:59 tdslab.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:54:59 tcslab.ps
Model: FLOW1 Model: FLOW1
TR1: Boundary case 1 TR1: Boundary case 1
Step: 16 TIME: 1.6 Step: 16 TIME: 1.6
Nodal PTE....S PTE Nodal PTE....S PTE
Max/Min on whole graph: Max/Min on model set:
Ymax = 38.8 Max = 38.8 Min = 20
Ymin = 29.8
Xmax = 2.65
Xmin = 0
39 Variation along a line
38
N 37
O
D
A 36
L
P 35
T
E 34
.
.
. 33
.
S
32
P
T
E 31
30
37.1
35.4
29 33.7
0 .25 .5 .75 1 1.25 1.5 1.75 2 2.25 2.5 2.75 32
DISTANCE Y 30.3
28.6
26.9
Z X 25.1
23.4
21.7
(a) horizontal distribution in the core (b) contour plot
Figure 20.9: Temperature in the base slab after 1.6 days
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:00 basel.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:00 slabszz.ps
Model: STRUC1 Model: STRUC1
Element EL.SXX.G SZZ
Max/Min on whole graph:
Ymax = 1.81
Ymin = -.451
Xmax = 36
Xmin = .1
Variation over loadcases
Element 66 Mean
2 Element 68 Mean
Element 70 Mean
1.75
E
L 1.5
66 71 76 81 86 91 96 101 106 111 116 121 126 131 136 141 146 151 156 161 E
M
E 1.25
N
67 72 77 82 87 92 97 102 107 112 117 122 127 132 137 142 147 152 157 162 T
1
E
L .75
68 73 78 83 88 93 98 103 108 113 118 123 128 133 138 143 148 153 158 163 .
S
X .5
69 74 79 84 89 94 99 104 109 114 119 124 129 134 139 144 149 154 159 164 X
.
G .25
70 75 80 85 90 95 100 105 110 115 120 125 130 135 140 145 150 155 160 165 S
Z 0
Z 0 5 10 15 20 25 30 35 40
-.25
-.5
TIME
Y
Z X
(a) elements (b) time graph for σZZ
Figure 20.10: Stress evolution in the base slab
Transverse stress in time struc1.fvc
RESULTS LOADCASE LC3
RESULTS ELEMENT EL.SXX.G SZZ
PRESENT GRAPH ELEMENT 66 68 70
In order to study the evolution of the transverse stress σZZ in time, we select for
all load cases the SZZ element result. Then we make graphs of the evolution of
the transverse stress for three elements at the symmetry axis [Fig. 20.10b]. We
note that the increase of the temperature in the heating phase at low Young’s
modulus values generates small compressive stress. In the cooling phase, at
higher Young’s modulus values, the decrease of temperature leads to more sig-
nificant stresses in tension. As expected, we also note that in the core of the slab
the tensile stresses reach larger values than near the bottom and top surfaces.
Crack index struc1.fvc
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
432 Early Age Behavior of a Purification Wall
VIEW MESH
VIEW OPTIONS EDGES OUTLINE
LABEL MESH ELEMENTS OFF
RESULTS LOADCASE LC3 38
RESULTS ELEMENT EL.ICR.S ICR
PRESENT CONTOUR LEVELS
PRESENT CONTOUR FROM 2 TO 1 LEVELS 5
In this context it is interesting to investigate the crack index output result. We
start with an outline view of the base slab. The time graphs [Fig. 20.10b] show
that the stress reaches its largest value at the end time of the analysis, i.e.,
after thirty-six days. Therefore we select the last load case. Then we select the
element result ICR which represents the crack index. We display a contour plot
of the crack index with default levels [Fig. 20.11a]. We can clearly see that the
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:01 icr1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:01 icr2.ps
Model: STRUC1 Model: STRUC1
LC3: Load case 3 LC3: Load case 3
Step: 38 TIME: 36 Step: 38 TIME: 36
Element EL.ICR.S ICR Element EL.ICR.S ICR
Max/Min on model set: Max/Min on model set:
Max = 7.91 Max = 7.91
Min = .956 Min = .956
7.28
6.65
6.02
5.38 1
Y 4.75 Y 1.17
4.12 1.33
3.49 1.5
Z X 2.85 Z X 1.67
2.22 1.83
1.59 2
(a) default levels (b) customized levels: cracked area in red
Figure 20.11: Crack index contours after 36 days
major part of the base slab exhibits a crack index less than 1.0. In order to have
a better overview of the crack index values, we display the crack index contour
with a more refined level scale [Fig. 20.11b]. Here the area with a crack index
less than 1.0 is displayed in red. We can conclude that cracks will arise in the
core of the base slab.
Animation struc1.fvc
RESULTS LOADCASE LC3
UTILITY SETUP ANIMATE LINEAR
DRAWING ANIMATE LOADCASES PLOTFILE szz1
We make an animation sequence of the development of the crack index by dis-
playing a contour plot for each time step. Due to the PLOTFILE option we can
put the frames of the animation in a document. Because there is no crack in-
dex less than 2.0 until 6.5 days we show the frames for that time and beyond
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
20.3 Second Stage – Casting the Wall
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:02 szz1029
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:02 szz1030
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:02 szz1031
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:02 szz1032
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:02 szz1033
433
Model: STRUC1 Model: STRUC1 Model: STRUC1 Model: STRUC1 Model: STRUC1
LC3: Load case 3 LC3: Load case 3 LC3: Load case 3 LC3: Load case 3 LC3: Load case 3
Step: 29 TIME: 6.5 Step: 30 TIME: 7 Step: 31 TIME: 8 Step: 32 TIME: 9 Step: 33 TIME: 10
Element EL.ICR.S ICR Element EL.ICR.S ICR Element EL.ICR.S ICR Element EL.ICR.S ICR Element EL.ICR.S ICR
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = 11.2 Max = 10.4 Max = 7.73 Max = 7.41 Max = 7.31
Min = 2.05 Min = 1.86 Min = 1.54 Min = 1.37 Min = 1.26
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:02 iDIANA
szz10349.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:02 iDIANA
szz10359.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:02 iDIANA
szz10369.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:02 iDIANA
szz10379.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:02 szz1038
Model: STRUC1 Model: STRUC1 Model: STRUC1 Model: STRUC1 Model: STRUC1
LC3: Load case 3 LC3: Load case 3 LC3: Load case 3 LC3: Load case 3 LC3: Load case 3
6.5 d 7d 8d 9d 10 d
Step: 34 TIME: 15 Step: 35 TIME: 20 Step: 36 TIME: 25 Step: 37 TIME: 30 Step: 38 TIME: 36
Element EL.ICR.S ICR Element EL.ICR.S ICR Element EL.ICR.S ICR Element EL.ICR.S ICR Element EL.ICR.S ICR
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = 7.63 Min = 1.1 Max = 17.72 Max = 7.79
1 Max = 7.92 1 Min = .97 Max = 7.91 1 1
Min = 1.17
1.01 Min = .978
1.17 1.17 Min = .956 1.17 1.17
Y Y Y Y Y
1.33 1.33 1.33 1.33 1.33
1.5 1.5 1.5 1.5 1.5
Z X 1.67
Z X 1.67
Z X 1.67
Z X 1.67
Z X 1.67
1.83 1.83 1.83 1.83 1.83
2 2 2 2 2
DRAWING ANIMATE LOADCASES PLOTFILE szz1 DRAWING ANIMATE LOADCASES PLOTFILE szz1 DRAWING ANIMATE LOADCASES PLOTFILE szz1 DRAWING ANIMATE LOADCASES PLOTFILE szz1 DRAWING ANIMATE LOADCASES PLOTFILE szz1
Z X
15 d 1
Y1.17
1.33
1.5
Z1.67 X
1.83
20 d 1
Y1.17
1.33
1.5
Z1.67 X
1.83
25 d 1
Y1.17
1.33
1.5
Z1.67 X
1.83
30 d 1
Y1.17
1.33
1.5
Z1.67 X
1.83
36 d 1
1.17
1.33
1.5
1.67
1.83
2 2 2 2 2
Figure 20.12: Crack index animation sequence
DRAWING ANIMATE LOADCASES PLOTFILE szz1 DRAWING ANIMATE LOADCASES PLOTFILE szz1 DRAWING ANIMATE LOADCASES PLOTFILE szz1 DRAWING ANIMATE LOADCASES PLOTFILE szz1 DRAWING ANIMATE LOADCASES PLOTFILE szz1
[Fig. 20.12]. From the animation sequence we can expect the first cracks to arise
sometime between twenty to twenty-five days.
20.3 Second Stage – Casting the Wall
We will now perform the second staggered flow–stress analysis that corresponds
to the second construction stage. We enter the Index environment of iDiana
to start these analyses.
iDiana
INDEX
ANALYSE PURWAL
The ANALYSE command initiates the analysis of the model named PURWAL. Via
the Analysis Setup dialog we specify that this is a Phased analysis. However,
we must specify that we open an existing filos file. We define set FOUNDA,
BASCON, WALCON, BOUND1 and BOUND2 as active and run the analysis. Then,
we click Next. Therefore, we may specify a Transient Heat Transfer analysis.
The Analysis Setup dialog appears where we may specify the various analysis
options for the heat flow analysis. Then we click Next. Using the same filos
file, we change the analysis type to Structural Nonlinear analysis. Once more
the Analysis Setup dialog appears where we may specify the various analysis
options for the mechanical analysis. These operations result in the following
batch analysis commands.
phase2.dcf
*PHASE
BEGIN ACTIVE
ELEMEN FOUNDA BASCON WALCON BOUND1 BOUND2 /
END ACTIVE
*HEATTR
BEGIN INITIA
BEGIN NONLIN
EQUAGE OFF
HYDRAT DGRINI=0.01
END NONLIN
TIME=36.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
434 Early Age Behavior of a Purification Wall
TEMPER INPUT
END INITIA
EXECUT SIZES 0.1(20) 0.5(10) 1.0(3) 5.0(4)
BEGIN OUTPUT FEMVIE FILE="FLOW2"
TEMPER
REACTI
END OUTPUT
*NONLIN
BEGIN TYPE
BEGIN PHYSIC
TEMPER
VISCOE
END PHYSIC
END TYPE
BEGIN EXECUT
BEGIN START
TIME=36.0
INITIA STRESS PHASE
LOAD LOADNR=3
STEPS
END START
BEGIN ITERAT
BEGIN CONVER
SIMULT
FORCE TOLCON=1.0E-10
DISPLA TOLCON=1.0E-10
END CONVER
END ITERAT
END EXECUT
BEGIN EXECUTE
TIME STEPS EXPLIC SIZES 0.1(20) 0.5(10) 1.0(3) 5.0(4)
BEGIN ITERAT
BEGIN CONVER
SIMULT
FORCE TOLCON=1.0E-10
DISPLA TOLCON=1.0E-10
END CONVER
END ITERAT
END EXECUTE
BEGIN OUTPUT FEMVIE FILE="STRUC2"
DISPLA
STRESS
STRESS TOTAL CAUCHY CRKIND
END OUTPUT
*END
The structure of this command file is completely similar to the phase1.dcf file.
For each module *HEATTR and *NONLIN, the initial time is set to 36 days to
ensure the time continuation between the two construction stages. There is also
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
20.3 Second Stage – Casting the Wall 435
an INITIA STRESS PHASE command to initiate a new phase in the nonlinear
analysis and apply load number 3 explicitly. After the analysis has terminated
we enter the iDiana Results environment.
20.3.1 Heat Flow Analysis Results
We enter the Results environment with model FLOW2 to assess the heat flow
analysis results of the second construction stage. The entire mesh is automati-
cally displayed in the outline style.
Degree of reaction flow2.fvc
FEMVIEW FLOW2
RESULTS LOADCASE TR1 1
RESULTS ELEMENT EL.DGR.S DGR
PRESENT CONTOUR LEVELS
We select the first load case TR1 1 and present a contour plot of the degree of
reaction [Fig. 20.13]. It can be clearly seen that the hydration reaction has just
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:20 dgrini.ps
Model: FLOW2
TR1: Boundary case 1
Step: 1 TIME: 36.1
Element EL.DGR.S DGR
Max = 1
Min = .176E-1
.912
.822
.733
.643
Y .554
.465
.375
Z X .286
.196
.107
Figure 20.13: Degree of reaction contours
started in the purification wall (r = 0.176×10−1 ) whereas it has already come
to an end in the base slab (r = 1).
Temperature flow2.fvc
VIEW MESH WALCON
EYE FRAME
LABEL MESH NODES
RESULTS NODAL PTE....S PTE
RESULTS LOADCASE TR1
PRESENT GRAPH NODE 37
We display the mesh of the wall with node numbers and determine a node in the
core of the purification wall, i.e., on the symmetry edge [Fig. 20.14a]. We make
a time graph for the evolution of the temperature at this node [Fig. 20.14b].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
436 Early Age Behavior of a Purification Wall
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:20 walno.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:20 tewall.ps
Model: FLOW2 Model: FLOW2
Nodal PTE....S PTE
798081828384 Max/Min on whole graph:
Ymax = 38.2 Ymin = 20
Xmax = 66 Xmin = 36.1
737475767778 Variation over loadcases
Node 37
676869707172 40
616263646566 38
555657585960 N 36
O
D
A 34
495051525354 L
P 32
434445464748 T
E 30
.
373839404142 .
. 28
.
313233343536 S
26
P
T
252627282930 E 24
192021222324 22
131415161718 20
35 37.5 40 42.5 45 47.5 50 52.5 55 57.5 60 62.5 65 67.5
Y TIME
7 8 9 101112
Z X
1 2 3 4 5 6
(a) nodes (b) time graph
Figure 20.14: Temperature in the core of the wall
Animation flow2.fvc
VIEW MESH
LABEL MESH NODES OFF
VIEW MESH +BASCON
EYE FRAME
VIEW OPTIONS EDGES OUTLINE
UTILITY SETUP ANIMATE LINEAR
PRESENT CONTOUR FROM 20 TO 36 LEVELS 7
DRAWING ANIMATE LOADCASES PLOTFILE tem2
We make an animation sequence of the development of the temperature in the
concrete structure by displaying a contour plot for each time step. We ensure
consistent levels for all frames. Due to the PLOTFILE option we can put the
frames of the animation in a document. Here we show a selection of the frames
for times from 36 to 51 days [Fig. 20.15].
20.3.2 Structural Analysis Results
We enter the Results environment with model STRUC2 to assess the structural
analysis results of the second construction stage.
struc2.fvc
FEMVIEW STRUC2
UTILITY TABULATE LOADCASES
The load case tabulation shows the available load cases with their result data.
Tabulated load cases loads.tb
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
20.3 Second Stage – Casting the Wall 437
iDIANA 9.4.3-02 : TNO Diana BV iDIANA 9.4.3-02 : TNO
28 OCT
Diana
2010
BV 01:55:21 tem2004 iDIANA 9.4.3-02 : TNO
28 OCT
Diana
2010
BV 01:55:21 tem2007 iDIANA 9.4.3-02 : TNO
28 OCT
Diana
2010
BV 01:55:21 tem2010 iDIANA 9.4.3-02 : TNO
28 OCT
Diana
2010
BV 01:55:21 tem2015 28 OCT 2010 01:55:21 tem2020
Model: FLOW2 Model: FLOW2 Model: FLOW2 Model: FLOW2 Model: FLOW2
TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1
Step: 4 TIME: 36.4 Step: 7 TIME: 36.7 Step: 10 TIME: 37 Step: 15 TIME: 37.5 Step: 20 TIME: 38
Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = 23.7 Min = 20 Max = 32.3 Min = 20 Max = 36.6 Min = 20 Max = 38.1 Min = 20 Max = 36.3 Min = 20
36 36 36 36 36
34 34 34 34 34
32 32 32 32 32
Y Y 30 Y 30 Y 30 Y 30 30
28 28 28 28 28
26 26 26 26 26
Z X Z X 24 Z X 24 Z X 24 Z X 24 24
22 22 22 22 22
20 20 20 20 20
iDIANA 9.4.3-02 : TNO Diana BV 36.4 d iDIANA 9.4.3-02 : TNO28Diana
DRAWING ANIMATE LOADCASES PLOTFILE tem2
OCT 2010 36.7 d
BV 01:55:21 tem2022 iDIANA 9.4.3-02 : TNO28Diana
DRAWING ANIMATE LOADCASES PLOTFILE tem2
OCT 2010
BV 01:55:21 tem2024 37 d iDIANA 9.4.3-02 : TNO28Diana
DRAWING ANIMATE LOADCASES PLOTFILE tem2
OCT 2010
BV 01:55:21 tem2028 37.5 d iDIANA 9.4.3-02 : TNO28Diana
DRAWING ANIMATE LOADCASES PLOTFILE tem2
OCT 2010
BV 01:55:22 tem2032 38 d
DRAWING ANIMATE LOADCASES PLOTFILE tem2
28 OCT 2010 01:55:22 tem2034
Model: FLOW2 Model: FLOW2 Model: FLOW2 Model: FLOW2 Model: FLOW2
TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1 TR1: Boundary case 1
Step: 22 TIME: 39 Step: 24 TIME: 40 Step: 28 TIME: 42 Step: 32 TIME: 45 Step: 34 TIME: 51
Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE Nodal PTE....S PTE
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = 32.3 Min = 20 Max = 28.4 Min = 20 Max = 23.7 Min = 20 Max = 20.9 Min = 20 Max = 20.5 Min = 20
36 36 36 36 36
34 34 34 34 34
32 32 32 32 32
Y Y 30 Y 30 Y 30 Y 30 30
28 28 28 28 28
26 26 26 26 26
Z X Z X 24 Z X 24 Z X 24 Z X 24 24
22 22 22 22 22
20 20 20 20 20
39 d
DRAWING ANIMATE LOADCASES PLOTFILE tem2
40 d
DRAWING ANIMATE LOADCASES PLOTFILE tem2
42 d
DRAWING ANIMATE LOADCASES PLOTFILE tem2
45 d
DRAWING ANIMATE LOADCASES PLOTFILE tem2
51 d
DRAWING ANIMATE LOADCASES PLOTFILE tem2
Figure 20.15: Temperature animation sequence
;
; Model: STRUC2
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; LC3 1 LOAD = 1 "Load case 3"
; Nodal : TDTX...G
; Element : EL.SXX.G EL.ICR.S
;
; LC3 2 TIME = 36.1 "Load case 3"
; Nodal : TDTX...G
; Element : EL.SXX.G EL.ICR.S
;
... lines skipped
;
; LC3 38 TIME = 66 "Load case 3"
; Nodal : TDTX...G
; Element : EL.SXX.G EL.ICR.S
;
We see the various result attributes: TDT represents the total displacements,
EL.S represents the total stresses, and EL.ICR represents the crack index. The
first load case corresponds to the results obtained after the INITIA command
block of the *NONLIN structural analysis in the command file phase2.dcf. All
the other load cases correspond to time step results of the EXECUTE command
block.
Transverse stress struc2.fvc
VIEW MESH BASCON
VIEW MESH +WALCON
EYE FRAME
VIEW OPTIONS EDGES OUTLINE
RESULTS LOADCASE LC3 1
RESULTS ELEMENT EL.SXX.G SZZ
PRESENT CONTOUR LEVELS
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
438 Early Age Behavior of a Purification Wall
We display the concrete part of the model in outline style. To get a statement
of the stress configuration at the start of the second phase, we select the first
load case and the SZZ result attribute which represents the transverse stress. We
display this in a contour plot [Fig. 20.16]. Here we can check the continuity of
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:23 wallszz.ps
Model: STRUC2
LC3: Load case 3
Step: 1 LOAD: 1
Element EL.SXX.G SZZ
Max/Min on model set:
Max = 1.82
Min = -.168E-1
1.66
1.49
1.32
1.15
Y .987
.82
.653
Z X .485
.318
.151
Figure 20.16: Transverse stress at start of second phase
stress with the previous phased analysis. In the transversal direction, the wall
is nearly free of stress whereas the base slab is subjected to quite significant
tensile stresses.
Elements in wall struc2.fvc
VIEW MESH WALCON
EYE FRAME
LABEL MESH ELEMENTS VIEWMODE VIOLET
We will present some element results for the wall. Therefore we display its
mesh with element numbers [Fig. 20.17]. We can easily pick up the numbers
of the elements at the bottom part, the core part, and the upper part of the
purification wall.
Crack index struc2.fvc
RESULTS LOADCASE LC3 2 TO LC3 38
RESULTS ELEMENT EL.ICR.S ICR
PRESENT GRAPH ELEMENT 1 31 61
RESULTS LOADCASE LC3 25 TO LC3 38
DRAWING DISPLAY
We show the evolution of the crack index during the second phase. We select
all load cases that correspond to time steps. We select the ICR results attribute
which represents the crack index. We display the evolution of the crack index for
the selected elements [Fig. 20.18a]. It appears that the most critical crack index
values arise at the end of the construction stage, i.e., beyond 40 days. For a more
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
20.3 Second Stage – Casting the Wall 439
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:23 wallel.ps
Model: STRUC2
6162636465
5657585960
5152535455
4647484950
4142434445
3637383940
3132333435
2627282930
2122232425
1617181920
1112131415
6 7 8 9 10
Y
1 2 3 4 5
Z X
Figure 20.17: Mesh with element numbers of the purification wall
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:24 icr3.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:55:24 icr4.ps
Model: STRUC2 Model: STRUC2
Element EL.ICR.S ICR Element EL.ICR.S ICR
Max/Min on whole graph: Max/Min on whole graph:
Ymax = 100 Ymax = 12 Ymin = 1.36
Ymin = 1.36 Xmax = 66 Xmin = 40
Xmax = 66 Variation over loadcases
Xmin = 36.1 Element 1 Mean
Variation over loadcases Element 31 Mean
Element 1 Mean Element 61 Mean
110 Element 31 Mean 12
Element 61 Mean
100
E 90 E 10
L L
E E
M 80 M
E E
N N 8
T 70 T
E 60 E
L L 6
. .
I 50 I
C C
R 40 R
. . 4
S S
30
I I
C 20 C
R R 2
10
0 0
35 37.5 40 42.5 45 47.5 50 52.5 55 57.5 60 62.5 65 67.5 40 42.5 45 47.5 50 52.5 55 57.5 60 62.5 65 67.5
TIME TIME
(a) all time steps (b) from 40 to 66 days
Figure 20.18: Crack index evolution in the wall
refined evolution of the crack index we select the steps that correspond to times
from 40 to 66 days and update the current view to get the new graph [Fig. 20.18-
b]. It appears that crack index values range from 100 to 1.5. Therefore, the risk
of cracking is lower for the wall than for the base slab.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
440 Early Age Behavior of a Purification Wall
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
Chapter 21
Adiabatic Hydration of
Concrete
Name: Hydrat
Path: /Examples/ConcMas/Hydrat
Keywords: analys: flow heat nonlin transi. constr: initia temper. el-
emen: flow potent q4ht. load: flux node time. materi:
adiaba capaci conduc hydrat isotro. option: direct. post:
binary femvie tabula. result: reacti temper total.
insulation
k
conductiviy
0.004
0 r
0 0.5 1.0
1 concrete c
capacitance
3000
2500 r
X 0 0.5 1.0
degree of reaction
1
(a) model (b) material properties
Figure 21.1: Adiabatic hydration of concrete
Diana can calculate the heat production due to hydration of cement or vul-
canization of rubber. This example concerns chemical heat production due to
hydration of cement. See also the publication by Reinhardt et al. [12]. The
model is an insulated piece of young concrete as shown in Figure 21.1a. The
initial temperature (at time t = 0) is 25 °C. The heat production q starts at
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
442 Adiabatic Hydration of Concrete
time t = 0. The lower graph in Figure 21.1b shows the dependency of the ca-
pacitance c on the degree of reaction r. The conductivity k depends linearly on
the degree of reaction r as shown in the upper graph. Due to the insulation,
the hydration process occurs without loss of heat, i.e., it is adiabatic.
First Diana derives the degree of reaction dependent part of the heat pro-
duction qr from input of the experimentally measured adiabatic temperature
development. The purpose of this example is now to check if a subsequent
transient analysis with Module heattr will yield the same temperature devel-
opment as was input previously. Because of the degree of reaction dependent
material properties, the solution of this problem must be obtained in a nonlinear
analysis.
21.1 Finite Element Model
To model the concrete we use one single Q4HT element in the two-dimensional
XY -coordinate space. The complete input data file for this model is as follows.
adiab.dat
ADIABATIC HYDRATION OF CONCRETE
’COORDINATES’ DI=2
1 0.0 0.0
2 1.0 0.0
3 1.0 1.0
4 0.0 1.0
’ELEMENTS’
CONNECTIVITY
1 Q4HT 1 2 3 4
MATERI
1 1
GEOMET
1 1
DATA
1 1
’GEOMET’
1 THICK 1.
’DATA’
1 NINTEG 1 1
’MATERIA’
1 CONDUC 2.6E-3
CAPACI 2650.
REACTI .0 .100 .200 .240 .290 .340 .400 .470 .560
.650 .739 .828 .917 1.00
CONREA 0. 4.0E-3 1. 2.6E-3
CAPART 2984. 2950. 2917. 2903. 2886. 2870. 2850. 2827. 2797.
2767. 2737. 2707. 2678. 2650.
ARRHEN 5995.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
21.2 Nonlinear Transient Analysis 443
ADIAB 0. 25.0
1.800E+03 25.01
97 lines skipped
1.764E+05 4.897E+01
1.782E+05 4.898E+01
1.800E+05 4.898E+01
’BOUNDA’
CASE 1
NODAL
1 Q 0.
’TIMEBO’
BOUNDA 1
TIME 0.0 10000000.0 /
FACTOR 1.0 1.0 /
’INIVAR’
TEMPER 1
/ 1-4 / / 25.0(4) /
’END’
The material properties are specified in table ’MATERI’. For the preliminary
analysis we specify the conductivity and capacitance with CONDUC and CAPACI
respectively. The material properties are specified for the thirteen degrees of
reaction in REACTI, the values for capacitance at these degrees of reaction are
specified with CAPART. The linear relation between the conductivity and the
degree of reaction is specified with CONREA for two points. ADIAB specifies the
measured transient temperature development during adiabatic hydration.
Tables ’BOUNDA’ and ’TIMEBO’ specify a boundary case which Diana always
needs when solving the system of equations. For this example this boundary
case is a dummy, it does not affect the analysis results. Finally, table ’INIVAR’
specifies the initial temperature of the concrete for the four nodes with the
POTENT input. The heat production formulation in Diana with the Arrhenius
constant (input ARRHEN) requires that this temperature is in °C [Vol. Material
Library].
21.2 Nonlinear Transient Analysis
In this example we initialize a filos file, read the input data file, and perform
the nonlinear transient analysis in one job. We apply the following command
file in batch format where the commands under *HEATTR specify how to perform
a transient heat flow analysis.
adiab.dcf
*FILOS
INITIA
*INPUT
*HEATTR
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
444 Adiabatic Hydration of Concrete
MODEL MATRIX CAPACI LUMPED
BEGIN INITIA
NONLIN HYDRAT DGRINI=0.01
TEMPER INPUT
END INITIA
BEGIN EXECUT
ALPHA=0.67
SIZES 1800.0(100)
BEGIN NONLIN
BEGIN ITERAT
MAXITE=10
TOLCON=0.01
END ITERAT
HYDRAT ITERAT
END NONLIN
END EXECUT
BEGIN OUTPUT TABULA
SELECT NODES 1
TEMPER
REACTI INTPNT
END OUTPUT
BEGIN OUTPUT FEMVIE
SELECT NODES 1
TEMPER
REACTI INTPNT
END OUTPUT
*END
The INITIA commands specify the initial condition. The NONLIN HYDRAT com-
mand initiates a nonlinear transient analysis with heat generation due to cement
hydration. Parameter DGRINI specifies the value for initial degree of reaction.
The TEMPER INPUT command states that the analysis starts with the initial
temperature as specified in table ’INIVAR’.
The EXECUT commands cause the analysis to be performed. The ALPHA pa-
rameter specifies a time integration parameter α = 32 which yields the Galerkin
integration method. The SIZES command specifies the sizes (in seconds) for
the hundred time steps of half an hour each. The NONLIN ITERAT commands
specify a nonlinear iteration process with a maximum of ten iterations. The
HYDRAT ITERAT command causes an implicit update of the degree of reaction
during each iteration.
The OUTPUT commands specify the analysis results to be output. There are
two output devices: TABULA for tabular output and FEMVIE for assessment with
iDiana. In both cases we select output for node 1 of the temperature and the
degree of reaction of each step.
We now perform the analysis with these commands and the input data file:
diana adiab
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
21.2 Nonlinear Transient Analysis 445
Convergence. To check the convergence of the nonlinear analysis we may
filter out the lines with the word SOLUTION from the standard output file. Below
we show the last ones that pass through this ‘filter’:
adiab.out
We see that the steps converged within one iteration to the specified tolerance
of 0.01 .
21.2.1 Temperature and Degree of Reaction
For the selected node 1, the temperature (labeled PTE) and the degree of reaction
(labeled DGR) are written to the tabular output file after each time step. Below,
we show the fragments of this output for the first and the last time step.
adiab.tb
Analysis type FLOW
Time 1.800E+03
Step nr. 1
Result TEMPER TOTAL
Nodnr PTE
1 2.505E+01
Analysis type FLOW
Time 1.800E+03
Step nr. 1
Result REACTI TOTAL
Location of results INTPNT
Elmnr Intpt DGR
1 1 1.205E-02
lines skipped
Analysis type FLOW
Time 1.800E+05
Step nr. 100
Result TEMPER TOTAL
Nodnr PTE
1 4.871E+01
Analysis type FLOW
Time 1.800E+05
Step nr. 100
Result REACTI TOTAL
Location of results INTPNT
Elmnr Intpt DGR
1 1 9.980E-01
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V) November 8, 2010 – First ed.
446 Adiabatic Hydration of Concrete
21.2.2 Time Response
To assess the time response we start up iDiana and enter the Results environ-
ment with the name of the model ‘ADIAB’.
adiab.fvc
FEMVIEW ADIAB
RESULTS LOADCASE ALL
RESULTS NODAL PTE....S PTE
PRESENT GRAPH NODE 1
RESULTS GAUSSIAN EL.DGR.S DGR
PRESENT GRAPH ELEMENT 1
For history plots we select all load cases (time steps), via the RESULTS LOADCASE
command. Then we select the NODAL result attribute PTE which represents the
temperatures. With the PRESENT GRAPH command and the NODE option we get
a history plot of the temperature in node 1 [Fig. 21.2a]. Comparison of the
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:56 gtemp.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:37:56 gdgre.ps
Model: ADIAB Model: ADIAB
Nodal PTE....S PTE Gauss EL.DGR.S DGR
Max/Min on whole graph: Max/Min on whole graph:
Ymax = 48.7 Ymin = 25 Ymax = .998
Xmax = .18E6 Xmin = .18E4 Ymin = .12E-1
Variation over loadcases Xmax = .18E6
Node 1 Xmin = .18E4
Variation over loadcases
Element 1 Mean
50 1
47.5 .9
G
A .8
N 45
U
O
S
D
S .7
A 42.5 I
L A
N .6
P 40
T E
E 37.5
L .5
.
.
.
D
. 35
G .4
.
R
S
.
32.5 S .3
P
T
D .2
E 30
G
R
27.5 .1
25 0
0 .2 .4 .6 .8 1 1.2 1.4 1.6 1.8 2 0 .2 .4 .6 .8 1 1.2 1.4 1.6 1.8 2
TIME *1E5 TIME *1E5
(a) temperature (b) degree of reaction
Figure 21.2: History plots (transient response)
transient temperatures with the input of the adiabatic temperature development
shows a very good resemblance for the chosen value of the initial degree of
reaction. However, you could verify yourself that taking a smaller initial degree
of reaction will result in a time shift of the temperature curve, and that taking a
larger value will result in a reversed time shift and a corresponding temperature
shift.
Finally we select the degree of reaction in the integration points via the
GAUSSIAN option and the DGR result attribute. Here we get a history plot of the
mean value for element 1 [Fig. 21.2b].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (V)
Part VI
Masonry Modeling
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
Chapter 22
Interfaces in Masonry Wall
Name: Wall
Path: /Examples/ConcMas/Wall
Keywords: analys: nonlin physic. constr: suppor. elemen: cl12i
cq16m interf pstres struct. load: temper weight. materi:
brittl crack discre elasti isotro linear secant shear soften unload
zero. option: direct groups newton regula units. post: binary
femvie. pre: femgen. result: cauchy displa stress total.
♥ potential crack
symmetry
2.40 wall t = 0.10
rim
0.20 beam t = 0.20
6.00
Figure 22.1: Model
This example illustrates the application of interface elements in a masonry wall
[Fig. 22.1]. The complete wall is 2.40 m high, 6.00 m long and 0.10 m thick.
The wall is placed on a beam with a square cross-section of 0.20×0.20 m. Wall
and beam are connected via a rim. We assume that a crack may arise in the
wall along the vertical symmetry line. In this example we will concentrate
on the methods for creating the model, rather than examining the results of
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
450 Interfaces in Masonry Wall
the analysis. To show the possibilities of connecting parts of the model with
interface elements we will model the complete structure instead of only one half.
22.1 Finite Element Model
We will model the masonry wall and the beam with CQ16M plane stress elements
and the rim and potential crack with CL12I structural interface elements. The
elements of the rim behave linearly, those of the crack nonlinearly. We launch
iDiana and enter the Design environment with the name of the model.
iDiana
FEMGEN WALL
Analysis and Units
Analysis Selection
Model Type: → Structural 2D
Via the Analysis and Units dialog we indicate that this is a model for two-di-
mensional structural analysis.
22.1.1 Geometry Definition
First we will place all geometry points in such a way that the two parts of the
wall and the beam can be modeled separately. Later on we will move some parts
to their final location.
Points wall.fgc
GEOMETRY POINT COORD 0.0
GEOMETRY POINT COORD 3.0
GEOMETRY POINT COORD 6.0
GEOMETRY POINT COORD 6.0 0.2
GEOMETRY POINT COORD 3.0 0.2
GEOMETRY POINT COORD 0.0 0.2
EYE FRAME
GEOMETRY POINT COORD 3.2 0.4
GEOMETRY POINT COORD 6.2 0.4
GEOMETRY POINT COORD 6.2 2.8
GEOMETRY POINT COORD 3.2 2.8
EYE FRAME
GEOMETRY POINT COORD -0.2 0.4
GEOMETRY POINT COORD 2.8 0.4
GEOMETRY POINT COORD 2.8 2.8
GEOMETRY POINT COORD -0.2 2.8
EYE FRAME
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY POINTS ALL VIOLET
We define the coordinates of the points, omitting the zero’s for the default
Y = 0 and Z = 0 coordinates. We scale the display such that all currently
defined points fit in the viewport. Finally we display the points with labels
[Fig. 22.2].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
22.1 Finite Element Model 451
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:13 points.ps
Model: WALL
Analysis: DIANA
Model Type: Structural 2D
P14 P13 P10 P9
P11 P12 P7 P8
P6 P5 P4
P1 P2 P3
Z X
Figure 22.2: Created points
Surfaces for beam wall.fgc
CONSTRUCT SET OPEN JOIST
GEOMETRY SURFACE 4POINTS P1 P2 P5 P6
GEOMETRY SURFACE 4POINTS P2 P3 P4 P5
CONSTRUCT SET CLOSE
We create the surfaces for the beam and include these in a set called JOIST.1
This is done for easier modeling and postprocessing. This set will be available
in the Results environment.
Surfaces for wall wall.fgc
CONSTRUCT SET OPEN WALL
GEOMETRY SURFACE 4POINTS P11 P12 P13 P14
GEOMETRY SURFACE 4POINTS P7 P8 P9 P10
CONSTRUCT SET CLOSE
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY SURFACES
We create the surfaces for the wall and assemble these in a set named WALL.
We display the current geometry, including surface labels [Fig. 22.3a]. Note that
there is a gap in between the three surfaces. This is for easier modeling of the
interface between the surfaces.
Surfaces for interfaces wall.fgc
CONSTRUCT SET OPEN INT
CONSTRUCT SET OPEN RIM
GEOMETRY SURFACE 4POINTS P6 P5 P12 P11
GEOMETRY SURFACE 4POINTS P5 P4 P8 P7
CONSTRUCT SET CLOSE RIM
CONSTRUCT SET OPEN CRACK
1 Because BEAM is a reserved word for iDiana commands, we have chosen the set name
JOIST.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
452 Interfaces in Masonry Wall
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:13 surface.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:13 interface.ps
Model: WALL Model: WALL
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
L10 L20 L14
L11 L15
S3 S4 S3 S7 S4
L9 L13
L8 L21 L12
L17 S5 L19 S6
L16 L18
L3 L7
S1 S2 L4 S1 S2
L2 L6
L1 L5
Y Y
Z X Z X
(a) for wall and beam (b) all, interfaces included
Figure 22.3: Surfaces
GEOMETRY SURFACE 4POINTS P7 P10 P13 P12
CONSTRUCT SET CLOSE
CONSTRUCT SET CLOSE
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY LINES ALL VIOLET
LABEL GEOMETRY SURFACES
Finally we generate and assemble the surfaces for the interfaces in three different
sets: INT with all interfaces, RIM with the interfaces in between wall and beam,
CRACK with the interface in between the two wall parts. We display the complete
geometry of the model, including labels for lines and surfaces [Fig. 22.3b].
22.1.2 Meshing
We have now completely defined the geometry of the model and may perform
the meshing process.
Generate mesh wall.fgc
MESHING DIVISION SURFACE INT 24 1
MESHING DIVISION SURFACE JOIST 24 6
MESHING DIVISION SURFACE WALL 24 24
MESHING TYPES INT IL33 CL12I
MESHING TYPES S5 IL33 CL12I BASE L3
MESHING TYPES S6 IL33 CL12I BASE L7
MESHING TYPES S7 IL33 CL12I BASE L9
MESHING TYPES JOIST QU8 CQ16M
MESHING TYPES WALL QU8 CQ16M
MESHING GENERATE
First we specify the divisions for a regular mesh. Note that for the interface
surfaces in set INT the division in the ‘thickness’ direction is one. Then we
specify the Diana element type for the various parts: the generic QU8 eight-
node quadrilateral for the wall and the beam, and the matching generic IL33
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
22.1 Finite Element Model 453
interface element, respectively mapped to the specific CQ16M and CL12I Diana
elements. Note that for each interface surface we must specify the line that is
connected to the material via the BASE option. Finally we generate the mesh.
Display mesh wall.fgc
VIEW MESH
VIEW HIDDEN SHADE
VIEW OPTIONS COLOUR TYPES
VIEW OPTIONS COLOUR OFF
VIEW MESH JOIST RED
VIEW MESH +WALL GREEN
VIEW MESH +RIM BLUE
VIEW MESH +CRACK VIOLET
EYE FRAME
We make a ‘shaded hidden view’ which for this two-dimensional model simply
means that the elements will be filled with color. Then we display the elements
in a color according to their type: the QU8 quadrilateral elements in red and the
IL33 interface elements in orange [Fig. 22.4a]. To check if the sets of elements
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:14 meshtyp.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:14 meshset.ps
Model: WALL Model: WALL
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
Y Y
Z X Z X
Element Types
QU8
IL33
(a) color for element types (b) color for sets
Figure 22.4: Generated mesh
have been filled correctly we display the various sets where the + sign causes
superposition of the specified part on the current display [Fig. 22.4b]. Note the
small triangular gap at the junction of sets CRACK and RIM. This is due to the
provisional gaps between the surfaces. We will remove this gap presently by
gluing the surfaces together [§ 22.1.6].
22.1.3 Supports
To define the supports with respect to the geometric parts and display them on
the mesh we give the following commands.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
454 Interfaces in Masonry Wall
wall.fgc
PROPERTY BOUNDARY CONSTRAINT L1 Y
PROPERTY BOUNDARY CONSTRAINT L5 Y
PROPERTY BOUNDARY CONSTRAINT P2 X
VIEW HIDDEN OFF
VIEW OPTION SHRINK
VIEW MESH
LABEL MESH CONSTRNT
We define three sets of supports: CO1 which suppresses the translation in Y -
direction of line L1, CO2 which suppresses the translation in Y -direction of line
L5, and CO3 which suppresses the translation in X-direction of point P2. Then
we display the mesh in ‘shrunken elements’ style with labels for the supports:
spikes in the direction of the suppressed translation [Fig. 22.5].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:14 sup.ps
Model: WALL
Analysis: DIANA
Model Type: Structural 2D
Z X
Figure 22.5: Supports
22.1.4 Material and Physical Properties
We may now continue with the specification of material and physical properties
in the Property Manager dialog.
iDiana
View →Property Manager...
↑
Property Manager
···
Material properties iDiana
Property Manager
↑ Materials Material Name: CONCRETE
↑Linear Elasticity →Isotropic
↑Mass →Mass Density
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
22.1 Finite Element Model 455
Materials Material Name: MASONRY
↑Linear Elasticity →Isotropic
↑Mass →Mass Density
↑Expansion →Isotropic - Constant Params.
Materials Material Name: MATRIM
↑Linear Elasticity →Interfaces
Materials Material Name: MATCRK
↑Linear Elasticity →Interfaces
↑Static Nonlinearity →Interfaces →Cracking →Discrete Cracking →Linear Tension Softening
→Secant Mode-I Unloading →Zero Shear Stiffn. aft Crack
We create two elastic isotropic materials: a material named CONCRETE with
E = 30×109 , ν = 0.2, and ρ = 2400; and a material named MASONRY with
E = 5×109 , ν = 0.2, ρ = 1800, and α = 10−5 . Then we define a material
named MATRIM with properties for the interface elements of the rim: the linear
stiffness moduli D11 = 333×1010 and D22 = 139×1010 , respectively for the
normal and shear traction. For a material MATCRK we specify the properties for
discrete cracking in the interface elements: the stiffness moduli D11 = D22 =
1.0×1010 , the tensile strength ft = 1×1010 , and the fracture energy Gf = 100
[Vol. Material Library].
Physical properties iDiana
Property Manager
↑Physical Properties Physical Property Name: THKB
↑Geometry →Plane Stress →Regular
Physical Properties Physical Property Name: THKW
↑Geometry →Plane Stress →Regular
Physical Properties Physical Property Name: INTER
↑Geometry →Interface →Line →Plane Stress
As physical properties we define two thicknesses THKB with t = 0.2 and THKW
with t = 0.1. For the interface elements we specify a set of physical properties
named INTER the thickness t = 0.1.
Properties assignment wall.fgc
PROPERTY ATTACH JOIST CONCRETE THKB
PROPERTY ATTACH WALL MASONRY THKW
PROPERTY ATTACH RIM MATRIM INTER
PROPERTY ATTACH CRACK MATCRK INTER
We have now defined all properties for the model and must assign them to
the appropriate geometrical parts (sets). The beam gets the material proper-
ties CONCRETE and the thickness THKB. The wall gets the material properties
MASONRY and the thickness THKW. The horizontal interface gets the material
properties MATRIM and the physical properties INTER. Finally the vertical inter-
face gets the material properties MATCRK and the physical properties INTER.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
456 Interfaces in Masonry Wall
Check assignment wall.fgc
LABEL MESH OFF
VIEW OPTIONS COLOUR MATERIALS
VIEW HIDDEN SHADE
VIEW OPTIONS COLOUR PHYSICAL
VIEW HIDDEN SHADE
To check the properties assignment we display a mesh with color modulation for
the material properties [Fig. 22.6a], and for the physical properties [Fig. 22.6b].
The displays and the legend confirm the correctness of the properties assign-
ment. Note that the interface elements for crack and rim have different material
properties (green and yellow) but that the physical properties are the same (yel-
low).
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:14 meshmat.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:14 meshphy.ps
Model: WALL Model: WALL
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
Y Y
Z X Materials Z X
CONCRETE Physical
MASONRY THKB
MATRIM THKW
MATCRK INTER
(a) material properties (b) physical properties
Figure 22.6: Color modulated mesh properties
22.1.5 Loading
For this model the loading comprises dead weight only.
Dead weight wall.fgc
PROPERTY LOADS GRAVITY ALL -10. Y
We apply gravity load for the entire model with g = 10 m/s2 .
22.1.6 Gluing the Surfaces Together
Now that the modeling is completed, the parts can be moved to their final
position.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
22.1 Finite Element Model 457
Move parts wall.fgc
CONSTRUCT TRANSFRM TRANSLATE TR1 P12 P5
CONSTRUCT TRANSFRM TRANSLATE TR2 P7 P5
GEOMETRY MOVE S3 TR1
yes
GEOMETRY MOVE S4 TR2
yes
MESHING GENERATE
We define two transformations: TR1 is defined by the translation vector from
point P12 to P5 which will move the beam to the wall, TR2 is defined by the
translation vector from point P7 to P5 which will close the vertical crack inter-
face. We apply the two transformations to the appropriate surfaces, which will
move the two parts of the wall to their final position. This modification to the
geometry cancels the mesh, therefore we must re-generate it.
Check moved parts wall.fgc
VIEW OPTIONS COLOUR OFF
VIEW OPTIONS SHRINK
VIEW HIDDEN SHADE
VIEW MESH
VIEW HIDDEN OFF
VIEW GEOMETRY JOIST RED
VIEW GEOMETRY +WALL GREEN
VIEW GEOMETRY +INT BLUE
To check whether the transformations have been applied correctly we display the
final model [Fig. 22.7a]. Note that the interface elements are no longer visible
because these have a zero thickness. However, a display of the geometry with
various colors for the sets proves their existence [Fig. 22.7b].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:14 mesh.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:14 geomet.ps
Model: WALL Model: WALL
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
Y Y
Z X Z X
(a) element mesh (b) geometry
Figure 22.7: Final model
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
458 Interfaces in Masonry Wall
22.1.7 Temperature in Time
The time-dependency of the temperature of the wall must be supplied via an
input data file in Diana batch format.
temper.dat
’TEMPER’
0.0 100.0
/ WALL /
0.0 -100.0
’END’
This input in table ’TEMPER’ defines a temperature decrement of 100° in 100 s
for all elements in the wall.
22.2 Transient Nonlinear Analysis
Now that we have checked the final model, we may write it to a file in Diana
batch input format and initiate the analysis.
iDiana
UTILITY WRITE DIANA
yes
FILE CLOSE
yes
wall
ANALYSE WALL
Analysis Setup
···
Via the Analysis Setup dialog we activate the following batch commands for the
nonlinear analysis of this example [Vol. Analysis Procedures].
wall.dcf
*FILOS
INITIA
*INPUT
*INPUT
READ FILE="temper.dat"
*NONLIN
TYPE PHYSIC
BEGIN OUTPUT FEMVIEW BINARY
DISPLA TOTAL
STRESS TOTAL GLOBAL
END OUTPUT
BEGIN EXECUT
BEGIN LOAD
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
22.2 Transient Nonlinear Analysis 459
STEPS EXPLIC SIZE 1.
LOADNR=1
END LOAD
BEGIN ITERAT
METHOD NEWTON REGULA
MAXITE=20
BEGIN CONVER
ENERGY TOLCON=1E-08
FORCE OFF
DISPLA OFF
END CONVER
END ITERAT
END EXECUT
BEGIN EXECUT
TIME STEPS EXPLIC SIZE 1.(15)
BEGIN ITERAT
METHOD NEWTON REGULA
MAXITE=20
BEGIN CONVER
ENERGY CONTIN TOLCON=1E-08
FORCE OFF
DISPLA OFF
END CONVER
END ITERAT
END EXECUT
*END
The first *INPUT command reads input file wall.dat with the generated mesh.
The READ command after the second *INPUT command reads file temper.dat
with the time-dependent temperature of the wall [§ 22.1.7]. As we execute fifteen
time steps of one second each, the wall is cooled down 15° in this analysis.
wall.fvc
FEMVIEW WALL
UTILITY TABULATE LOADCASES
When the analysis has been terminated we enter the iDiana Results environ-
ment to assess the results. The tabulation shows the available results.
reslc.tb
;
; Model: WALL
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; MODEL STATIC "Model Properties"
; Element : THICKNES*
;
; LC1 1 LOAD = 1 "Load case 1"
; Nodal : TDTX...G
; Element : EL.SXX.G
;
; LC1 2 TIME = 1 "Load case 1"
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
460 Interfaces in Masonry Wall
; Nodal : TDTX...G
; Element : EL.SXX.G
;
; LC1 3 TIME = 2 "Load case 1"
... remainder skipped
Note that Diana has passed sixteen load cases to the Results environment of
iDiana: all named LC1 but with increasing step numbers for each executed step
in the nonlinear analysis.
22.2.1 Deformation and Horizontal Stress
We will display the deformation and the horizontal stress for the first and the
last time step and as an animation.
First and last step wall.fvc
VIEW MESH WALL
RESULT LOADCASE LC1 1
VIEW OPTION DEFORM USING TDTX...G RESTDT 1500
RESULT ELEMENT EL.SXX.G SXX
PRESENT CONTOUR LEVELS 25
RESULT LOADCASE LC1 16
VIEW OPTION DEFORM USING TDTX...G RESTDT 1500
RESULT ELEMENT EL.SXX.G SXX
PRESENT CONTOUR LEVELS 25
We ask iDiana to display any results in a mesh which shows the deformation
1500× enlarged. We select the first load case (time step) and the horizontal
stresses σXX as analysis result. We display the values of these stresses in a
color filled contour style with twenty-five levels [Fig. 22.8a]. We make a similar
display for the last step [Fig. 22.8b]. Note that in the last step the crack interface
is clearly open and that, due to the lack of contact between the two walls, the
stress distributions are separated.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:26 ressxx1.ps iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:26 ressxx16.ps
Model: WALL Model: WALL
Deformation = .15E4 Deformation = .15E4
LC1: Load case 1 LC1: Load case 1
Step: 1 LOAD: 1 Step: 16 TIME: 15
Element EL.SXX.G SXX Element EL.SXX.G SXX
Max/Min on model set: Max/Min on model set:
Max = .224E4 Max = .715E6
Min = -.683E4 Min = -.177E6
.189E4 .68E6
.154E4 .646E6
.119E4 .612E6
841 .578E6
492 .543E6
144 .509E6
-205 .475E6
-554 .44E6
-902 .406E6
-.125E4 .372E6
-.16E4 .337E6
-.195E4 .303E6
-.23E4 .269E6
-.265E4 .235E6
-.299E4 .2E6
-.334E4 .166E6
-.369E4 .132E6
-.404E4 .973E5
-.439E4 .63E5
Y -.474E4 Y .287E5
-.509E4 -.557E4
-.544E4 -.399E5
Z X -.578E4 Z X -.742E5
-.613E4 -.108E6
-.648E4 -.143E6
(a) first step (b) last step
Figure 22.8: Deformation and horizontal stress
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
22.2 Transient Nonlinear Analysis 461
Animation wall.fvc
PRESENT CONTOUR FROM -0.143E6 TO 0.681E6 LEVELS 25
RESULT LOADCASE LC1
DRAWING ANIMATE LOADCASE PLOTFILE anima
Since we used time increments in the nonlinear analysis we can ask iDiana to
create an animation of the behavior of the wall in time. In order to get the
same color modulation for stress values over the respective time steps, we take
over the extreme contour bounding values of the last step contours [Fig. 22.8b].
Then we select all load cases and make an animated display. Here we ask for a
plot file of each frame so that we can present the animation as a still [Fig. 22.9].
The frames must be read from left to right and from top to bottom. Note that
the crack begins to show up at step 6.
iDIANA 9.4.3-02 : TNO Diana BV
Model: WALL
Deformation = .15E4
LC1: Load case 1
Step: 1 LOAD: 1
28 OCT 2010 02:31:27 anima001
iDIANA 9.4.3-02 : TNO Diana BV
Model: WALL
Deformation = .15E4
LC1: Load case 1
Step: 2 TIME: 1
28 OCT 2010 02:31:27 anima002
iDIANA 9.4.3-02 : TNO Diana BV
Model: WALL
Deformation = .15E4
LC1: Load case 1
Step: 3 TIME: 2
28 OCT 2010 02:31:27 anima003
iDIANA 9.4.3-02 : TNO Diana BV
Model: WALL
Deformation = .15E4
LC1: Load case 1
Step: 4 TIME: 3
28 OCT 2010 02:31:27 anima004
Element EL.SXX.G SXX Element EL.SXX.G SXX Element EL.SXX.G SXX Element EL.SXX.G SXX
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = .224E4 Max = .395E5 Max = .857E5 Max = .132E6
Min = -.683E4 Min = -.105E5 Min = -.227E5 Min = -.349E5
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:28 anima005
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:28 anima006
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:28 anima007
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:28 anima008
Model: WALL Model: WALL Model: WALL Model: WALL
Deformation = .15E4 Deformation = .15E4 Deformation = .15E4 Deformation = .15E4
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Step: 5 TIME: 4 Step: 6 TIME: 5 Step: 7 TIME: 6 Step: 8 TIME: 7
Element EL.SXX.G SXX Element EL.SXX.G SXX Element EL.SXX.G SXX Element EL.SXX.G SXX
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = .178E6 Max = .224E6 Max = .271E6 Max = .317E6
Min = -.471E5 Min = -.594E5 Min = -.716E5 Min = -.838E5
Y Y Y Y
Z X Z X Z X Z X
DRAWING ANIMATE LOADCASE PLOTFILE anima DRAWING ANIMATE LOADCASE PLOTFILE anima DRAWING ANIMATE LOADCASE PLOTFILE anima DRAWING ANIMATE LOADCASE PLOTFILE anima
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:28 anima009
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:28 anima010
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:28 anima011
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:28 anima012
Model: WALL Model: WALL Model: WALL Model: WALL
Deformation = .15E4 Deformation = .15E4 Deformation = .15E4 Deformation = .15E4
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Step: 9 TIME: 8 Step: 10 TIME: 9 Step: 11 TIME: 10 Step: 12 TIME: 11
Element EL.SXX.G SXX Element EL.SXX.G SXX Element EL.SXX.G SXX Element EL.SXX.G SXX
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = .363E6 Max = .409E6 Max = .454E6 Max = .498E6
Min = -.959E5 Min = -.108E6 Min = -.12E6 Min = -.131E6
Y Y Y Y
Z X Z X Z X Z X
DRAWING ANIMATE LOADCASE PLOTFILE anima DRAWING ANIMATE LOADCASE PLOTFILE anima DRAWING ANIMATE LOADCASE PLOTFILE anima DRAWING ANIMATE LOADCASE PLOTFILE anima
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:28 anima013
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:28 anima014
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:29 anima015
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:29 anima016
Model: WALL Model: WALL Model: WALL Model: WALL
Deformation = .15E4 Deformation = .15E4 Deformation = .15E4 Deformation = .15E4
LC1: Load case 1 LC1: Load case 1 LC1: Load case 1 LC1: Load case 1
Step: 13 TIME: 12 Step: 14 TIME: 13 Step: 15 TIME: 14 Step: 16 TIME: 15
Element EL.SXX.G SXX Element EL.SXX.G SXX Element EL.SXX.G SXX Element EL.SXX.G SXX
Max/Min on model set: Max/Min on model set: Max/Min on model set: Max/Min on model set:
Max = .542E6 Max = .59E6 Max = .652E6 Max = .715E6
Min = -.143E6 Min = -.154E6 Min = -.166E6 Min = -.177E6
Y Y Y Y
Z X Z X Z X Z X
DRAWING ANIMATE LOADCASE PLOTFILE anima DRAWING ANIMATE LOADCASE PLOTFILE anima DRAWING ANIMATE LOADCASE PLOTFILE anima DRAWING ANIMATE LOADCASE PLOTFILE anima
Y Y Y Y
Z X Z X Z X Z X
Figure 22.9: Animation of deformation and horizontal stress
DRAWING ANIMATE LOADCASE PLOTFILE anima DRAWING ANIMATE LOADCASE PLOTFILE anima DRAWING ANIMATE LOADCASE PLOTFILE anima DRAWING ANIMATE LOADCASE PLOTFILE anima
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
462 Interfaces in Masonry Wall
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
Chapter 23
Discrete Modeling of
Masonry
Name: MasonDi
Path: /Examples/ConcMas/MasonDi
Keywords: analys: linear static. constr: suppor tying. elemen: interf
l8if pstres q8mem struct. load: deform. materi: elasti isotro.
option: direct groups units. post: binary femvie. result:
cauchy displa extern force green reacti strain stress total tracti.
analys: nonlin physic. constr: suppor tying. elemen: interf
l8if pstres q8mem struct. load: deform. materi: elasti isotro.
option: direct groups newton nonsym regula units. post:
binary femvie. result: cauchy displa force green princi reacti
strain stress total tracti. analys: nonlin physic. constr:
suppor tying. elemen: interf l8if pstres q8mem struct. load:
deform. materi: elasti isotro. option: direct groups newton
nonsym regula units. post: binary femvie. result: cauchy
displa force green princi reacti strain stress total tracti.
In this example we will assess a masonry structure in shear, similar to that of
a test specimen as shown in Figure 23.1a. The assessment of this specimen has
been published by van Zijl et al. [14]. We will create a finite element model
[Fig. 23.1b], using the ‘Simplified Modeling Method with Brick Crack Interface’.
To model the bricks we will apply Q8MEM elements (plane stress, linear, 4-node)
with Q8IF linear interface elements for the brick joint- and brick crack-interfaces.
The interface elements will have a nominal width of 0.5 mm. For each masonry
brick there will be eight plane stress elements and two interface elements.
Modeling strategy. We will build the complete model in three steps. First
we will create half a brick with interface elements to represent the brick crack
and the brick joint. This part will then be meshed, the axes of the interface
elements checked, and some properties attached. Then we will copy the half
brick into a basic block of two bricks. Finally we will copy the two brick model
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
464 Discrete Modeling of Masonry
iDIANA 0.0-04 : TNO Diana BV 24 MAY 2005 11:47:37 modelfe
Z X Materials
GROUT
(b) finite element model
MASONRY
CRACK
(a) test specimen
Figure 23.1: Masonry structure
several times into a complete wall after which the hole will be cut away.
Material models. In this example we will keep the material in the bricks and
brick crack interfaces linear. This means that only the brick joints can crack
during the analysis. Therefore we could have used the ‘Simplified Modeling
Method’ in this case. However, for educational purposes, we have chosen the
‘Simplified Modeling Method with Brick Crack Interface’.
23.1 Finite Element Model
To build the finite element model we start iDiana and enter the Design envi-
ronment with the name of a new model for which we choose BRICK.
iDiana
FEMGEN BRICK
Analysis and Units
Analysis Selection
Model Type: →Structural 2D
Units Definition
Length: →Millimeter
Force: →Newton
Time: →Second
In the dialog Analysis and Units we indicate that the model is for a two-dimen-
sional structural analysis and specify the adopted units [mm, N, s].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
23.1 Finite Element Model 465
Meshing parameters brick.fgc
CONSTRUCT SPACE TOLERANCE ABSOLUTE 0.1
MESHING DIVISION DEFAULT 2
First we create a proper environment for the model, i.e., setting tolerances and
devisions for meshing . Since we are going to model interfaces with a thickness
of 0.5 millimeter we set an absolute modeling tolerance of 0.1 millimeter. Then
we change the default of four element divisions along a new line to 2. This
complies with the eight structural elements and two interface elements that will
be created in every brick.
23.1.1 Modeling Half a Brick
We will define and mesh the geometry of one half of a brick.
Geometry brick.fgc
GEOMETRY POINT 0.0 0.0 0.0
GEOMETRY SWEEP P1 TRANSLATE 104.75 0.0 0.0
EYE FRAME
GEOMETRY SWEEP L1 TRANSLATE 0.0 0.5 0.0
GEOMETRY SWEEP L2 TRANSLATE 0.0 50.0 0.0
EYE FRAME
GEOMETRY SWEEP L7 TRANSLATE 0.5 0.0 0.0
VIEW OPTIONS SHRINK GEOMETRY 0.9
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY SURFACES ALL VIOLET
We define the geometry of half a brick using one point and several sweep com-
mands. This includes the interface elements on two sides [Fig. 23.2a]. The
surface at the bottom (S1) represents the brick joint. The surface at the right
(S3) represents the brick crack interface.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:28 geom1 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:28 mesh1
Model: BRICK Model: BRICK
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
S2 S3
S1
Y Y
Z X Z X
Element Types
IL22
QU4
(a) geometry (b) mesh
Figure 23.2: Modeling half a brick
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
466 Discrete Modeling of Masonry
Mesh brick.fgc
MESHING TYPES S1 IL22 L8IF BASE L1
MESHING TYPES S2 QU4 Q8MEM
MESHING TYPES S3 IL22 L8IF BASE L7
MESHING DIVISION AUTOMATIC
MESHING GENERATE
VIEW OPTIONS COLOUR TYPES
VIEW MESH
VIEW OPTIONS SHRINK MESH 0.9
VIEW HIDDEN FILL COLOUR
To mesh the current geometry we first complete the meshing type definition,
then generate and view the mesh of the half brick [Fig. 23.2b]. Note the 2×2
quadrilateral elements (QU4, orange) and the interface elements (IL22, red).
Axes. When using interface elements in two-dimensional analysis it is very
important that their axes are correctly aligned. The general rule of thumb is
that the interface element local z-axis should be aligned in the same direction
as the global Z-axis.
brick.fgc
VIEW HIDDEN OFF
EYE DIRECTION 1 1 1
EYE FRAME
LABEL MESH AXES ALL Z RED
GEOMETRY FLIP S3
MESHING GENERATE
LABEL MESH AXES ALL Z BLUE
The first bird’s-eye view of the mesh shows that the axes of the brick joint
interface are not aligned correctly [Fig. 23.3a]. Therefore we flip the axes via
the FLIP option. The second view shows that the local z-axes are correctly
aligned [Fig. 23.3b].
23.1.2 Material and Physical Properties
To define the material and physical properties we launch the Property Manager
dialog.
iDiana
View →Property Manager...
↑
Property Manager
···
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
23.1 Finite Element Model 467
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:29 inax1 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:29 inax2
Model: BRICK Model: BRICK
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
Y Y
Z X Z X
(a) as generated (b) after flip
Figure 23.3: Local z-axes of elements (note the interfaces!)
Material properties iDiana
Property Manager
Materials Material Name: MASONRY
↑
↑Linear Elasticity →Isotropic
Materials Material Name: CRACK
↑Linear Elasticity →Interfaces
Materials Material Name: GROUT
↑Linear Elasticity →Interfaces
↑Static Nonlinearity →Interfaces →Combined Crack-Shear-Crush
→Constant Mode II Fract. Energy
We define the parameters for three material instances [Table 23.1]: MASONRY
for the brick elements with linear elastic properties, CRACK for the brick crack
interfaces with linear stiffnesses, and GROUT for the brick joint interfaces with
linear stiffnesses and nonlinear properties for the combined cracking-shearing-
crushing model.
Physical properties iDiana
Property Manager
↑Physical Properties Physical Property Name: INTERFAC
↑Geometry →Interface →Line →Plane Stress
Physical Properties Physical Property Name: PLANE
↑Geometry →Plane stress →Regular
Here we specify the thickness of the model, for which we choose 100 mm. We
create two property instances, both with a thickness of 100 mm: INTERFAC for
the interface elements, and PLANE for the brick elements.
Attachment brick.fgc
VIEW GEOMETRY ALL
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
468 Discrete Modeling of Masonry
Table 23.1: Material parameters
Young’s modulus E 1.74×104 N/mm2
Bricks
Poisson’s ratio ν 0.15
Linear normal stiffness D11 1.0×104 N/mm2
Cracks
Linear tangential stiffness D22 1.0×103 N/mm2
Linear normal stiffness D11 83.0 N/mm3
Linear tangential stiffness D22 36.0 N/mm3
Tensile strength ft 0.25 N/mm2
Fracture energy Gf 0.018 N/mm
Cohesion c 0.35 N/mm2
Friction angle tan φ 0.75
Dilatancy angle tan ψ 0.60
Joints Residual friction coefficient Φ 0.75
Confining normal stress for ψ0 σu −1.3 N/mm2
Exponential degradation coefficient δ 5.0
Cap critical compressive strength fc 8.5 N/mm2
Shear traction control factor Cs 9.0
Compressive fracture energy Gfc 5.0 N/mm
Equivalent plastic relative displacement κp 0.093
Fracture energy factor b 0.05
PROPERTY ATTACH S1 GROUT INTERFAC
PROPERTY ATTACH S2 MASONRY PLANE
PROPERTY ATTACH S3 CRACK INTERFAC
We attach the material and physical properties to the appropriate parts of the
model.
23.1.3 Creating the Two-brick Model
To expand the half brick model to two bricks we will copy it two times. We
must take special attention to the correct assignment of material properties.
Copying geometry brick.fgc
CONSTRUCT SET COMPLETE APPEND SURFACES ALL
GEOMETRY COPY COMPLETE TRANSLATE 0.0 50.5 0.0
EYE ROTATE TO 0
VIEW GEOMETRY ALL VIOLET
EYE FRAME
CONSTRUCT SET COMPLETE APPEND SURFACES ALL
GEOMETRY COPY COMPLETE TRANSLATE -105.25 0.0 0.0
VIEW GEOMETRY ALL VIOLET
EYE FRAME
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
23.1 Finite Element Model 469
For convenience we assemble all surfaces in set COMPLETE before the transla-
tion. First we copy the geometry over 50.5 mm (the brick’s height) in vertical
direction [Fig. 23.4a]. Again we put all surfaces, including the ones just created,
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:29 geom2 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:29 geom3
Model: BRICK Model: BRICK
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
Y Y
Z X Z X
(a) first copy (b) second copy
Figure 23.4: Making the geometry of the two-brick model
into the set COMPLETE. A subsequent translation, now over 105.25 mm (half
the brick’s width) in horizontal direction creates the geometry of the two-brick
model [Fig. 23.4b]. Actually, the model now comprises two half bricks with one
full brick on top. Although the geometry is OK, we must correct the attachment
of the materials to the interfaces.
Geometry and materials brick.fgc
LABEL GEOMETRY MATERIALS ALL RED
LABEL GEOMETRY SURFACES ALL BLUE
PROPERTY ATTACH S3 MATERIAL GROUT
PROPERTY ATTACH S12 MATERIAL GROUT
LABEL GEOMETRY MATERIALS ALL RED
LABEL GEOMETRY SURFACES ALL BLUE
The geometry labels [Fig. 23.5a] show that surfaces S3 and S12 have the material
for the crack attached (CRACK), while this should be the material for the joints
(GROUT). We correct this via the two PROPERTY ATTACH commands. The new
geometry labels confirm the correction [Fig. 23.5b].
23.1.4 Expansion to the Complete Model
We will now expand the two-brick model to the complete geometry of the ma-
sonry wall specimen. The expansion involves two copy operations: first hori-
zontally then vertically. After the copy operations we must not forget to apply
a line of interface elements along the upper edge of the model.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
470 Discrete Modeling of Masonry
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:29 geomma1 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:29 geomma2
Model: BRICK Model: BRICK
Analysis: DIANA Analysis: DIANA
Model Type: Structural 2D Model Type: Structural 2D
MASONRY CRACK MASONRY CRACK MASONRY GROUT MASONRY CRACK
S11 S12 S5 S6 S11 S12 S5 S6
GROUT GROUT GROUT GROUT
S10 S4 S10 S4
MASONRY CRACK MASONRY CRACK MASONRY CRACK MASONRY GROUT
S8 S9 S2 S3 S8 S9 S2 S3
GROUT GROUT GROUT GROUT
S7 S1 S7 S1
Y Y
Z X Z X
(a) after copy (b) corrected
Figure 23.5: Material assignment to geometry of the two-brick model
Horizontal copy brick.fgc
LABEL GEOMETRY OFF
CONSTRUCT SET COMPLETE APPEND SURFACES ALL
GEOMETRY COPY COMPLETE 4 TRANSLATE 210.5 0.0 0.0
EYE FRAME
LABEL GEOMETRY LINES L146 RED
LABEL GEOMETRY LINES L155 RED
UTILITY DELETE LINES L146 L155
yes
All current surfaces are assembled in a set COMPLETE. This set is then copied
four times in horizontal direction over a distance equal to the width of a brick
(210.5 mm). The resulting geometry now comprises two full layers of bricks
[Fig. 23.6a]. Note that we must delete the two lines which represent superfluous
interfaces near the right edge.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:29 geom4 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:29 geom5
Model: BRICK
Analysis: DIANA
Model Type: Structural 2D
L155
L146
Y Y
Z X Z X
(a) 4× copied horizontally (b) 7× copied vertically
Figure 23.6: Expansion of the two-brick geometry
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
23.1 Finite Element Model 471
Vertical copy brick.fgc
CONSTRUCT SET COMPLETE APPEND SURFACES ALL
GEOMETRY COPY COMPLETE 7 TRANSLATE 0.0 101.0 0.0
EYE FRAME
DRAWING CONTENTS MONITOR OFF
Again, we collect all current surfaces in a set COMPLETE. Now this set is copied
seven times in vertical direction over a distance equal to the thickness of two
brick layers (101 mm). The geometry now completely covers the specimen of
the masonry wall [Fig. 23.6b].
Interfaces along upper edge. The model still lacks a line of appropriate
interfaces along its upper edge. You can apply these easily by copying an hori-
zontal line of interfaces, for instance with the following commands.
brick.fgc
CONSTRUCT SET TMP APPEND SURFACES LIMITS VMIN 757.4 VMAX 758.1
VIEW GEOMETRY ALL YELLOW
VIEW GEOMETRY +TMP BLUE
GEOMETRY COPY TMP UPINT TRANSLATE 0 50.5 0
VIEW GEOMETRY +UPINT RED
We select all surfaces along the lower edge of the upper brick layer with Y -
coordinates in the range 757.5 ≤ Y ≤ 758.0.1 With the LIMITS option we collect
the surfaces (interfaces) which are located completely within the specified range
of Y -coordinates in a set TMP. To check if the set is correctly filled we highlight
it in blue [Fig. 23.7a]. We copy this set vertically over a distance of the thickness
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:30 geom6a iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:30 geom6b
Y Y
Z X Z X
(a) selected row (blue) (b) copied to upper edge (red)
Figure 23.7: Copying interfaces onto the upper edge
of a brick layer (50.5 mm) to apply the appropriate interfaces along the upper
layer. For a final check we display the new interfaces in red [Fig. 23.7b].
1 To check this, zoom in on this edge, display point labels, and tabulate some points.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
472 Discrete Modeling of Masonry
23.1.5 Cutting the Hole
To finish the geometry definition of the brick wall specimen we must cut away
the hole near the center of the wall.
brick.fgc
CONSTRUCT SET HOLE APPEND SURFACES LIMITS 315.50 526.00 252.75 555.75
VIEW GEOMETRY ALL YELLOW
VIEW GEOMETRY +HOLE GREEN
UTILITY DELETE POINTS HOLE
yes
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY TYPES ALL BLUE
Here we assemble all surfaces in the hole (including the interfaces!) in a set
HOLE. The specified limits of the area exactly coincide with the center line of
the joints. To check the hole, we display the set in green [Fig. 23.8a]. If we
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:30 hole iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:30 geomfin
L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF
Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM
L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF
Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM
L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF
Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM
L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF
Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM
L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF
Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM
L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF
Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM
L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF
Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM
L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF
Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM
L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF
Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM
L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF
Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM
L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF
Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM
L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF
Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM
L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF
Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM
L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF
Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM
L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF
Y Y
Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM
L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF
Z X Z X Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEML8IF Q8MEM
L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF L8IF
(a) hole highlighted (b) hole cut away
Figure 23.8: Geometry with hole
delete the points in this set iDiana will also delete all the lines and surfaces
attached to these points. This way, the interfaces along the edges of the hole
are also deleted. This is confirmed with a display of the remaining geometry,
including labels for the assigned element types [Fig. 23.8b].
23.1.6 Boundary Constraints and Loading
The boundary constraints and loading must be applied along the top and bottom
edges of the model. Therefore we will define some sets. To clean up things, we
will first delete the sets that have been defined so far.
Sets brick.fgc
UTILITY DELETE SETS ALL
yes
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
23.1 Finite Element Model 473
CONSTRUCT SET BOTTOM APPEND LIMITS VMAX .25
CONSTRUCT SET TOP APPEND LIMITS VMIN 808.25
VIEW GEOMETRY BOTTOM VIOLET
VIEW GEOMETRY +TOP BLUE
LABEL GEOMETRY POINTS TOP
We define two sets: BOTTOM for the lower edge and TOP for the upper edge. The
sets are simply specified via the LIMITS option: BOTTOM is filled with everything
below a vertical coordinate of 0.25 and TOP with everything above 808.25. We
display the sets to confirm their accurate definition [Fig. 23.9a]. Note that due
to the very narrow vertical limit values the sets only contain lines and points.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:30 geombnd iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:31 geomcolo
P668 P667
P666 P665
P672 P671
P670 P669
P676 P675
P674 P673
P680 P679
P678 P677
P684 P683
P682 P681
CO2 CO2 CO2 CO2 CO2 CO2 CO2 CO2 CO2 LO1 CO2
Y Y
Z X Z X
CO1 CO1 CO1 CO1 CO1 CO1 CO1 CO1 CO1 CO1
(a) sets for boundaries (b) labels in geometry
Figure 23.9: Constraints and loading
Boundary conditions and loading brick.fgc
PROPERTY BOUNDARY CONSTRAINT BOTTOM X Y
PROPERTY BOUNDARY CONSTRAINT TOP Y
PROPERTY BOUNDARY MPC RBEAM TOP P682 X
PROPERTY LOADS DISPLACE P682 -1 X
VIEW GEOMETRY ALL VIOLET
LABEL GEOMETRY CONSTRNT ALL BLUE
LABEL GEOMETRY LOADS ALL RED
The lower edge is supported in X- and Y -direction and the upper edge in Y -
direction only. Furthermore, we apply a multi-point constraint to prevent hor-
izontal deformation of the upper edge. Finally, for loading we apply a unit
displacement in horizontal −X-direction of a point on the upper edge. Due
to the multi-point constraint this load involves a uniform displacement of the
entire upper edge.
23.1.7 Generating the Final Mesh
We are now ready to generate and check the mesh of the complete model of the
masonry wall specimen.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
474 Discrete Modeling of Masonry
Mesh and materials brick.fgc
MESHING GENERATE
VIEW OPTIONS SHRINK MESH 0.8
VIEW HIDDEN FILL
VIEW OPTIONS COLOUR MATERIAL
VIEW MESH ALL
EYE ZOOM FACTOR 4 160 160
We generate the mesh and display it in ‘shrunken elements’ style, with colors
modulated according to assigned materials [Fig. 23.10a]. The individual bricks,
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:31 meshfin iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:31 meshfinz
Y Y
Z X Materials
Z X Materials
GROUT MASONRY
MASONRY GROUT
CRACK CRACK
(a) full view (b) zoomed-in
Figure 23.10: Final mesh, colors modulated for materials
each with a 4×2 element mesh, are clearly outlined by the interface elements
representing the joints. The vertical cracks show up as interface elements along
the vertical center line of each brick. This is even more obvious when we zoom
in on the model [Fig. 23.10b].
Boundary conditions brick.fgc
EYE FRAME
VIEW HIDDEN OFF
VIEW OPTIONS COLOUR OFF
VIEW MESH ALL
LABEL MESH CONSTRNT
LABEL MESH OFF
LABEL MESH LOADS
To check the boundary conditions we display these on the full mesh. The sup-
ports show up as red spikes and the linear constraints as a continuous red line
[Fig. 23.11a]. The load, i.e., the horizontal displacement, shows up as a violet
arrow [Fig. 23.11b].
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
23.2 Linear Analysis 475
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:31 meshcns iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:32 meshlod
3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S 3S
3M 3S 3S
Y Y
Z X Z X
(a) constraints (b) load
Figure 23.11: Boundary conditions of the mesh
23.2 Linear Analysis
The model is now finished and ready for analysis. We write it to an input data
file bricka.dat in Diana batch format and then close it.
iDiana
UTILITY WRITE DIANA bricka
yes
FILE CLOSE
yes
Discrete Modeling of Masonry
ANALYSE BRICK
Analysis Setup
···
The ANALYSE command launches the Analysis Setup dialog where we can accept
all the default settings for a Structural Linear Static analysis. This results in
the following batch command file.
linear.dcf
*FILOS
INITIA
*INPUT
*LINSTA
*END
We run the analysis with the input data file and this command file. When
the analysis has terminated there is an iDiana database with analysis results
(model name LINEAR). To assess these results we enter the Results environment
with the model name.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
476 Discrete Modeling of Masonry
linear.fvc
FEMVIEW LINEAR
VIEW MESH
VIEW OPTIONS EDGES OUTLINE
RESULTS LOADCASE LC1
We display the outlines of the model and select load case 1 (the only one avail-
able).
23.2.1 Displacements
Displaying the deformed model is a good way to check if there are any errors in
the model. We start with displaying the undeformed mesh.
linear.fvc
RESULTS NODAL DTX....G RESDTX
PRESENT SHAPE
First we select the load case and then the nodal result attribute RESDTX which
represents the displacement vector. The shape of the deformed mesh is displayed
in red [Fig. 23.12a]. It shows that there are no errors in the model. Note
that iDiana applies a default multiplication factor to make the deformation
discernible (see the legend).
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:38 lindfm iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:38 lineeq
Model: LINEAR Model: LINEAR
LC1: Load case 1 Deformation = 67.3
Nodal DTX....G RESDTX LC1: Load case 1
Max = 1 Min = 0 Element VONMISES EL.EXX.G
Factor = 67.3 Calculated from: EL.EXX.G
Max = .309E-3
Min = .192E-4
.282E-3
.256E-3
.23E-3
.203E-3
Y Y .177E-3
.151E-3
.124E-3
Z X Z X .981E-4
.718E-4
.455E-4
(a) deformation (b) Von Mises strain
Figure 23.12: Results of linear analysis
23.2.2 Strains
We also assess the strains due to the linear analysis.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
23.3 Nonlinear Analysis 477
linear.fvc
VIEW OPTIONS DEFORM USING DTX....G RESDTX
RESULT ELEMENT EL.EXX.G EXX
RESULTS CALCULATE VONMISES
PRESENT CONTOUR LEVELS
With the DEFORM option we display the outlines of the deformed model. Then
we select the strains via result attribute EXX and let iDiana calculate the equiv-
alent Von Mises strains. We display these in a contour plot [Fig. 23.12b]. Note
that the highest strains occur near the upper corners of the hole.
23.3 Nonlinear Analysis
To perform the analysis of the cracks in the model we enter the iDiana Index
environment and initiate a subsequent analysis.
iDiana
INDEX
ANALYSE BRICK
Analysis Setup
···
In the Analysis Setup dialog we indicate a Structural Nonlinear analysis. We
choose options for load steps, iteration procedure, output2 , etc. The options
should result in the following batch commands.
nonlin.dcf
*FILOS
INITIA
*INPUT
*NONLIN
BEGIN EXECUT
BEGIN ITERAT
METHOD NEWTON REGULA
BEGIN CONVER
DISPLA OFF
ENERGY TOLCON=0.0001
FORCE TOLCON=0.001
SIMULT
END CONVER
MAXITE=50
END ITERAT
BEGIN LOAD
2 Hint: To get output in the integration points of the elements click Properties in the Results
Selection dialog and then, in the Result Item Properties dialog, set the Location to Integration
points.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
478 Discrete Modeling of Masonry
LOADNR=1
BEGIN STEPS
BEGIN AUTOMA
SIZE=8.15
MAXSIZ=0.2
END AUTOMA
END STEPS
END LOAD
END EXECUT
BEGIN OUTPUT FEMVIE BINARY
DISPLA
FORCE
STRAIN TOTAL TRACTI INTPNT
STRAIN TOTAL GREEN LOCAL INTPNT
STRAIN TOTAL GREEN PRINCI INTPNT
STRESS TOTAL CAUCHY LOCAL INTPNT
STRESS TOTAL CAUCHY PRINCI INTPNT
END OUTPUT
*END
Now we run Diana with these commands and the brick.dat input data file.
Once the analysis has terminated we enter the iDiana Results environment to
assess the results.
nonlin.fvc
FEMVIEW NONLIN
UTILITY TABULATE LOADCASES
The tabulation of the load cases shows all the performed load steps together
with their load factors. The latter being equal to the horizontal displacement
uX of the upper edge. We show only the head and tail of the tabulation:
.tb
;
; Model: NONLIN
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; MODEL STATIC "Model Properties"
; Element : THICKNES*
;
... lines skipped
; Nodal : TDTX...G FBX....G
; Gauss : EL.PTX.L EL.EXX.L EL.E1 EL.SXX.L EL.S1
; * Indicates loads data
;
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
23.3 Nonlinear Analysis 479
23.3.1 Displacements
To inspect the behavior of the model in the nonlinear analysis we will plot the
load–displacement diagram for all load steps. We will also display the deformed
mesh.
Load–displacement diagram nonlin.fvc
RESULTS LOADCASE LC1
RESULTS NODAL FBX....G FBX
PRESENT GRAPH NODE 1387
For the horizontal axis we select all load cases, i.e., the load factors for each step.
For the vertical axis we select the calculated horizontal force FX represented
by result attribute FBX. The specified node is the one at the horizontal load on
the upper edge of the model [Fig. 23.11b] and thus we get a load–displacement
diagram for the upper edge [Fig. 23.13a]. The diagram shows a rather steep
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:08 lodis iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:08 nlidfm
Model: NONLIN Model: NONLIN
Nodal FBX....G FBX LC1: Load case 1
Max/Min on whole graph: Step: 22 LOAD: 2.45
Ymax = .53E5 Nodal TDTX...G RESTDT
Ymin = .796E4 Max = 2.46 Min = 0
Xmax = 8.15 Factor = 27.4
Xmin = .102
*1E4 Variation over loadcases
Node 1387
5.5
N 4.5
O
D
A 4
L
F 3.5
B
X 3
.
.
. 2.5
.
G
2
F
B
X 1.5
.5
0 1 2 3 4 5 6 7 8 9
LOAD Y
Z X
(a) load–displacement for top (b) deformation (27×) at uX ≈ 2.5 mm
Figure 23.13: Displacement
increment to FX ≈ 54000 at a horizontal displacement uX ≈ 2.5 mm. Then
follows a gradual decline until FX ≈ 35000 at uX ≈ 8 mm.
Deformation nonlin.fvc
RESULTS LOADCASE LC1 22
RESULTS NODAL TDTX...G RESTDT
VIEW MESH
PRESENT SHAPE
VIEW OPTIONS EDGES OUTLINE
To assess the deformation we choose a load step for which the force is about at
its maximum, i.e., at uX ≈ 2.5 mm. We select the total displacements, attribute
RESTDT, and plot a deformed mesh [Fig. 23.13b]. Note that iDiana applies an
automatic multiplication factor of approximately 27×. The most significant
cracks show up along the diagonal from the lower-left to the upper-right corner.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
480 Discrete Modeling of Masonry
23.3.2 Stresses in the Bricks
The following commands display a contour plot of the principal stresses.
nonlin.fvc
VIEW OPTIONS EDGES ALL
VIEW OPTIONS DEFORM USING TDTX...G RESTDT
RESULTS GAUSSIAN EL.S1 S1
PRESENT CONTOUR LEVELS
RESULTS GAUSSIAN EL.S1 S2
PRESENT CONTOUR LEVELS
Here we make two plots: result attribute S1 represents the first principal stress
[Fig. 23.14a], and S2 the second which shows mainly compression [Fig. 23.14b].
As principal stresses only occur in the bricks, the other elements (the interfaces)
have no color and therefore clearly show the cracks.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:08 nlis1 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:08 nlis2
Model: NONLIN Model: NONLIN
Deformation = 27.4 Deformation = 27.4
LC1: Load case 1 LC1: Load case 1
Step: 22 LOAD: 2.45 Step: 22 LOAD: 2.45
Gauss EL.S1 S1 Gauss EL.S1 S2
Max = 8.29 Max = .32
Min = -4.68 Min = -9.48
Results shown: Results shown:
Mapped to nodes Mapped to nodes
7.11 -.571
5.93 -1.46
4.75 -2.35
3.57 -3.24
Y 2.4 Y -4.14
1.22 -5.03
.369E-1 -5.92
Z X -1.14 Z X -6.81
-2.32 -7.7
-3.5 -8.59
(a) σ1 (b) σ2
Figure 23.14: Principal stress in the bricks at uX ≈ 2.5 mm
23.3.3 Crack Strain
Instead of the deformation, the crack strains in the interfaces provide for an
even more distinct way of displaying the cracks in the model.
nonlinb.fvc
RESULTS GAUSSIAN EL.PTX.L PTX
PRESENT CONTOUR LEVELS
The result attribute PTX represents the crack strain perpendicular to the inter-
face. A contour plot of this result fills the open cracks with colors [Fig. 23.15].
These crack strains may also be interpreted as a measure for the width of the
crack: from very narrow (blue) to wide open (red).
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
23.3 Nonlinear Analysis 481
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:09 nlcrk.ps
Model: NONLIN
Deformation = 27.4
LC1: Load case 1
Step: 22 LOAD: 2.45
Gauss EL.PTX.L PTX
Max = .943
Min = -.303
Results shown:
Mapped to nodes
.83
.716
.603
.49
Y .377
.264
.15
Z X .371E-1
-.761E-1
-.189
Figure 23.15: Crack strains at uX ≈ 2.5 mm
Animation. It is rather spectacular to see the cracks develop with increasing
deformation in an animation, i.e., a movie. We must ensure that all frames of
the movie have the same scaling for the deformation and contour levels.
nonlin.fvc
RESULTS LOADCASE LC1
VIEW OPTIONS DEFORM USING TDTX...G RESTDT 15
PRESENT CONTOUR FROM -1 TO 3.4 LEVELS 10
DRAWING ANIMATE LOADCASES PLOTFILE ancrk
We select all load cases to get as much frames as possible. Then we ensure a
fixed deformation scaling factor of 15×, and consistent contour levels. We start
the animation via the DRAWING ANIMATE command. Due to the PLOTFILE option
we can show the frames in this document. Here we only show a subset of twenty
frames [Fig. 23.16].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
482 Discrete Modeling of Masonry
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:09 ancrk001
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:09 ancrk004
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:09 ancrk006
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:10 ancrk010
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:10 ancrk013
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:10 ancrk019
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:11 ancrk023
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:11 ancrk024
DRAWING ANIMATE LOADCASES PLOTFILE ancrk DRAWING ANIMATE LOADCASES PLOTFILE ancrk DRAWING ANIMATE LOADCASES PLOTFILE ancrk DRAWING ANIMATE LOADCASES PLOTFILE ancrk
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:11 ancrk025
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:11 ancrk026
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:11 ancrk027
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:11 ancrk028
DRAWING ANIMATE LOADCASES PLOTFILE ancrk DRAWING ANIMATE LOADCASES PLOTFILE ancrk DRAWING ANIMATE LOADCASES PLOTFILE ancrk DRAWING ANIMATE LOADCASES PLOTFILE ancrk
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:11 ancrk029
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:12 ancrk030
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:12 ancrk031
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:12 ancrk032
DRAWING ANIMATE LOADCASES PLOTFILE ancrk DRAWING ANIMATE LOADCASES PLOTFILE ancrk DRAWING ANIMATE LOADCASES PLOTFILE ancrk DRAWING ANIMATE LOADCASES PLOTFILE ancrk
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:12 ancrk033 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:12 ancrk034 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:12 ancrk035
DRAWING ANIMATE LOADCASES PLOTFILE ancrk DRAWING ANIMATE LOADCASES PLOTFILE ancrk DRAWING ANIMATE LOADCASES PLOTFILE ancrk DRAWING ANIMATE LOADCASES PLOTFILE ancrk
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:42:12 ancrk036
DRAWING ANIMATE LOADCASES PLOTFILE ancrk DRAWING ANIMATE LOADCASES PLOTFILE ancrk DRAWING ANIMATE LOADCASES PLOTFILE ancrk
DRAWING ANIMATE LOADCASES PLOTFILE ancrk
Figure 23.16: Crack development – animation frames
23.4 Additional Exercise
It is also of interest to analyze the structure where the top edge is still rigidly
connected in X-direction but also allowed to move vertically. Assuming that
the model itself is identical to that already used we can prepare the modified
model.
brick.fgc
FEMGEN BRICK
UTILITY TABULATE CONSTRNT ALL
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
23.4 Additional Exercise 483
UTILITY DELETE CONSTRNT CO2
yes
PROPERTY BOUNDARY MPC RBEAM TOP P682 Y
VIEW MESH
VIEW OPTIONS SHRINK
LABEL MESH CONSTRNT
The tabulation shows that constraint CO2 represents the vertical support of the
top edge. We replace this support by a multi-point constraint in Y -direction to
keep the edge straight. The labeling of the constraints confirms their correctness
[Fig. 23.17].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:40:33 meshcnsb
3S
4S 3S
4S 3S
4S 3S
4S 3S
4S 3S
4S 3S
4S 3S
4S 3S
4S 3S
4S 3S
4S 3S
4S 3S
4S 3S
4S 3S
4S 3S
4S 3S
4S 3S
4S 3S
4S
4M
3M 3S
4S 3S
4S
Z X
Figure 23.17: Modified constraints
23.4.1 Nonlinear Analysis
For this analysis we write a new data file in Diana batch format.
iDiana
UTILITY WRITE DIANA brickb
yes
We run the analysis with the new input data file brickb.dat and the same
command file as for the previous analysis [§ 23.3 p. 477].
diana brickb.dat nonlin.dcf nonlinb
This analysis yields a model NONLINB for the iDiana Results environment. We
enter this environment when the analysis has terminated.
nonlinb.fvc
FEMVIEW NONLINB
UTILITY TABULATE LOADCASES
The head and tail of the load cases tabulation are now:
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
484 Discrete Modeling of Masonry
.tb
;
; Model: NONLINB
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; MODEL STATIC "Model Properties"
; Element : THICKNES*
;
... lines skipped
; Nodal : TDTX...G FBX....G
; Gauss : EL.PTX.L EL.EXX.L EL.E1 EL.SXX.L EL.S1
; * Indicates loads data
;
We will assess the results in a similar way as for the previous model.
23.4.2 Displacements
Load-displacement diagram nonlinb.fvc
RESULTS LOADCASE LC1
RESULTS NODAL FBX....G FBX
PRESENT GRAPH NODE 1387
The diagram shows a peak force at uX ≈ 0.3 mm followed by a steep decline
[Fig. 23.18a]. The force reaches a zero value at uX ≈ 2 mm and remains like
that al the way until the end of the analysis.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:03 lodisb iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:03 nlidfmb
Model: NONLINB Model: NONLINB
Nodal FBX....G FBX LC1: Load case 1
Max/Min on whole graph: Step: 4 LOAD: .283
Ymax = .119E5 Nodal TDTX...G RESTDT
Ymin = 1.48 Max = .292 Min = 0
Xmax = 8.15 Factor = 231
Xmin = .102
*1E4 Variation over loadcases
Node 1387
1.2
1
N
O
D
A
L .8
F
B
X .6
.
.
.
.
G .4
F
B
X
.2
0
0 1 2 3 4 5 6 7 8 9
LOAD Y
Z X
(a) load–displacement for top (b) deformation (230×) at uX ≈ 0.3 mm
Figure 23.18: Displacements
Deformation nonlinb.fvc
RESULTS LOADCASE LC1 4
RESULTS NODAL TDTX...G RESTDT
VIEW MESH
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
23.4 Additional Exercise 485
PRESENT SHAPE
VIEW OPTIONS EDGES OUTLINE
To assess the deformation we choose a load step for which the force is about at its
maximum, i.e., at uX ≈ 0.3 mm. The deformation now shows up [Fig. 23.18b].
The automatic multiplication factor is now approximately 230×. Open cracks
are visible near the lower-left and upper-right corners of the hole and also near
the upper-left and lower-right corners of the wall.
23.4.3 Stresses in the Bricks
nonlinb.fvc
VIEW OPTIONS EDGES ALL
VIEW OPTIONS DEFORM USING TDTX...G RESTDT
RESULTS GAUSSIAN EL.S1 S1
PRESENT CONTOUR LEVELS
RESULTS GAUSSIAN EL.S1 S2
PRESENT CONTOUR LEVELS
The pictures show the stress distribution in the bricks [Fig. 23.19].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:03 nlis1b iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:03 nlis2b
Model: NONLINB Model: NONLINB
Deformation = 231 Deformation = 231
LC1: Load case 1 LC1: Load case 1
Step: 4 LOAD: .283 Step: 4 LOAD: .283
Gauss EL.S1 S1 Gauss EL.S1 S2
Max = .67 Max = .236
Min = -.567 Min = -1.82
Results shown: Results shown:
Mapped to nodes Mapped to nodes
.557 .485E-1
.445 -.139
.332 -.326
.22 -.513
Y .107 Y -.701
-.498E-2 -.888
-.117 -1.08
Z X -.23 Z X -1.26
-.342 -1.45
-.455 -1.64
(a) σ1 (b) σ2
Figure 23.19: Principal stress in bricks at uX ≈ 0.3 mm
23.4.4 Crack Strain
nonlinb.fvc
RESULTS GAUSSIAN EL.PTX.L PTX
PRESENT CONTOUR LEVELS
The normal crack strain is now displayed in the deformed model [Fig. 23.20].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
486 Discrete Modeling of Masonry
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:03 nlcrkb.ps
Model: NONLINB
Deformation = 231
LC1: Load case 1
Step: 4 LOAD: .283
Gauss EL.PTX.L PTX
Max = .116
Min = -.159E-1
Results shown:
Mapped to nodes
.104
.919E-1
.799E-1
.679E-1
Y .56E-1
.44E-1
.32E-1
Z X .2E-1
.803E-2
-.395E-2
Figure 23.20: Crack strains at uX ≈ 0.3 mm
Animation nonlinb.fvc
RESULTS LOADCASE LC1
VIEW OPTIONS DEFORM USING TDTX...G RESTDT 7
PRESENT CONTOUR FROM 0 TO 6.0 LEVELS 8
DRAWING ANIMATE LOADCASES PLOTFILE ancrkb
We ensure a fixed deformation scaling factor of 7× and consistent contour levels.
We show the first twelve frames (until uX ≈ 6 mm).
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
23.4 Additional Exercise 487
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:03
iDIANA
ancrkb001
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:03
iDIANA
ancrkb002
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:03
iDIANA
ancrkb003
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:03 ancrkb004
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:04
iDIANA
ancrkb005
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:04
iDIANA
ancrkb006
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:04
iDIANA
ancrkb007
9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:04 ancrkb008
DRAWING ANIMATE LOADCASES PLOTFILE ancrkb DRAWING ANIMATE LOADCASES PLOTFILE ancrkb DRAWING ANIMATE LOADCASES PLOTFILE ancrkb DRAWING ANIMATE LOADCASES PLOTFILE ancrkb
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:04 ancrkb009 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:04 ancrkb010 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:04 ancrkb011
DRAWING ANIMATE LOADCASES PLOTFILE ancrkb DRAWING ANIMATE LOADCASES PLOTFILE ancrkb DRAWING ANIMATE LOADCASES PLOTFILE ancrkb DRAWING ANIMATE LOADCASES PLOTFILE ancrkb
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 01:43:04 ancrkb012
DRAWING ANIMATE LOADCASES PLOTFILE ancrkb DRAWING ANIMATE LOADCASES PLOTFILE ancrkb DRAWING ANIMATE LOADCASES PLOTFILE ancrkb
DRAWING ANIMATE LOADCASES PLOTFILE ancrkb
Figure 23.21: Crack development – animation frames
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
488 Discrete Modeling of Masonry
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
Chapter 24
Composite Modeling of
Masonry
Name: WalShr
Path: /Examples/ConcMas/WalShr
Keywords: analys: linear static. constr: suppor tying. elemen: cq16m
pstres. load: deform. materi: elasti harden hill isotro plasti
rankin strain. option: direct groups units. post: binary
femvie. result: displa total. analys: nonlin physic. con-
str: suppor tying. elemen: cq16m pstres. load: deform.
materi: elasti harden hill isotro plasti rankin strain. option:
direct groups newton regula units. post: binary femvie. re-
sult: cauchy displa force green plasti princi reacti strain stress
total. analys: nonlin physic. constr: suppor tying. elemen:
cq16m pstres. load: deform time. materi: elasti harden hill
isotro maxwel plasti rankin strain viscoe. option: direct groups
newton regula units. post: binary femvie. result: cauchy dis-
pla force green plasti princi reacti strain stress total.
In this example we will assess the same structure as in the example ‘Discrete
Modeling of Masonry’ [Ch. 23 p. 463]. However, here we will model the bricks
and joints together as a single homogeneous material. The constraints will be
as in the additional exercise [§ 23.4 p. 482]: the top of the structure can move
vertically but remains straight and horizontal. The finite element model is a
mesh of 25×19 elements with a 5×7 elements hole [Fig. 24.1].
24.1 Finite Element Model
In the iDiana Design environment we will make a model WALL.
iDiana
FEMGEN WALL
Analysis and Units
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
490 Composite Modeling of Masonry
420 210 420
250
800 300
250
1050
Figure 24.1: Masonry structure and finite element model [mm]
Analysis Selection
Model Type: →Structural 2D
Units Definition
Length: →Millimeter
Force: →Newton
Time: →Second
In the Analysis and Units dialog we specify that this is a model for two-dimen-
sional structural analysis. We also specify the adopted units [mm, N, s].
24.1.1 Geometry Definition
We create the basic geometry with a series of GEOMETRY POINT and GEOMETRY
SWEEP commands.
wall.fgc
GEOMETRY POINT COORD P1 0
GEOMETRY SWEEP P1 P2 TRANSLATE TR1 420
GEOMETRY SWEEP P2 P3 TRANSLATE TR2 210
GEOMETRY SWEEP P3 P4 TR1
VIEW GEOMETRY ALL VIOLET
EYE FRAME
Note that we preserve the horizontal distance of 420 in a translation TR1 to re-
use it in the third sweep operation. The initial geometry now comprises three
lines which we consider to be the bottom edge of the model [Fig. 24.2a]. We will
now assemble these lines in a set BOTTOM and sweep this vertically to create
the two-dimensional geometry.
wall.fgc
CONSTRUCT SET BOTTOM APPEND LINES ALL
GEOMETRY SWEEP BOTTOM MID1 TRANSLATE TR3 0 250
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
24.1 Finite Element Model 491
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:33 geom1 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:33 geom2
Model: WALL
Analysis: DIANA
Model Type: Structural 2D P13 L18 P14 L19 P15 L20 P16
S7 S8 S9
L21 L22 L23 L24
P9 L11 P10 L12 P11 L13 P12
S4 S5 S6
L14 L15 L16 L17
P5 L4 P6 L5 P7 L6 P8
S1 S2 S3
L7 L8 L9 L10
Y Y
Z X Z XP1 L1 P2 L2 P3 L3 P4
(a) initial lines (b) two-dimensional
Figure 24.2: Geometry definition
GEOMETRY SWEEP MID1 MID2 TRANSLATE TR4 0 300
GEOMETRY SWEEP MID2 TOP TR3
VIEW GEOMETRY ALL VIOLET
EYE FRAME
LABEL GEOMETRY POINTS ALL RED
LABEL GEOMETRY LINES ALL BLUE
LABEL GEOMETRY SURFACES ALL VIOLET
DRAWING CONTENTS MONITOR OFF
UTILITY DELETE SURFACES S5
yes
The VIEW command displays the full geometry. For future comfort we label all
the geometric parts [Fig. 24.2b]. Since the center surface, S5, is not required we
delete it.
24.1.2 Meshing
We will now create a finite element mesh on the defined geometry. We assign
element type CQ16M (quadratic, 8-node, plane stress) to all surfaces.
wall.fgc
MESHING TYPES ALL QU8 CQ16M
MESHING DIVISION ELSIZE ALL 21
MESHING GENERATE
VIEW OPTIONS SHRINK
VIEW MESH
LABEL MESH AXES ALL X RED
LABEL MESH AXES ALL Y BLUE
For a 25×19 element mesh the elements have a width of 1050/25 = 42 and
a height of 800/19 = 42.1. Because of the quadratic elements we must half
this size to get the 25×19 mesh. The VIEW commands display the mesh in
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
492 Composite Modeling of Masonry
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:33 mesh1 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:33 mesh2
Y Y
Z X Z X
(a) as generated (b) element axes
Figure 24.3: Mesh
green ‘shrunken-elements’ style [Fig. 24.3a]. Because of the orthotropic nature
of brickwork we also check the orientation of the element axes [Fig. 24.3b]. The
red arrows show that all element x-axes point in vertical direction. The blue
arrows show the horizontal direction of the element y-axes.
24.1.3 Material and Physical Properties
To define the material and physical properties we launch the Property Manager
dialog.
iDiana
View →Property Manager...
↑
Property Manager
···
Material properties iDiana
Property Manager
↑ Materials Material Name: BRICKS
↑Linear Elasticity →Isotropic
↑Static Nonlinearity →Masonry →Rankine-Hill anisotropic plast → Crack rate independent
For the masonry we define a material instance BRICKS. First we specify the
Young’s modulus and Poisson’s ratio for linear elasticity. Then we choose the
Rankine–Hill anisotropic plasticity model with independent crack rate. For this
model we fill in the parameters according to Table 24.1. Note that due to the
orientation of the element axes x indicates a property in vertical direction and
y in horizontal direction.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
24.1 Finite Element Model 493
Table 24.1: Material parameters for masonry (Rankine–Hill)
Young’s modulus E 8000 N/mm2
Poisson’s ratio ν 0.15
Tensile strength in x-direction ft.x 0.25 N/mm2
Tensile strength in y-direction ft.y 0.35 N/mm2
Alpha shear stress contribution ατ 1.0
Alpha h αh 1.0
Compressive strength in x-direction fc.x 8.5 N/mm2
Compressive strength in y-direction fc.y 8.5 N/mm2
Beta coupling normal stresses β −1.0
Gamma contribution shear stress γ 3.0
Rankine fracture energy in x-direction Gft.x 0.018 N/mm
Rankine fracture energy in y-direction Gft.y 0.054 N/mm
Hill fracture energy in x-direction Gfc.x 15.0 N/mm
Hill fracture energy in y-direction Gfc.y 20.0 N/mm
Equivalent plastic strain κp 0.0012
Physical properties iDiana
Property Manager
↑ Physical Properties Physical Property Name: THICK
↑Geometry →Plane Stress →Regular
Here we specify the thickness of the model, for which we choose 100 mm.
Attachment wall.fgc
PROPERTY ATTACH ALL BRICKS THICK
Finally we assign the defined properties to the geometry of the model.
24.1.4 Boundary Conditions
We apply the boundary conditions and loading using the following commands
so that the top of the structure is free to move in the vertical direction and has
a unit displacement in horizontal direction.
wall.fgc
CONSTRUCT SET TOP APPEND L18 L19 L20
PROPERTY BOUNDARY CONSTRAINT CO1 BOTTOM X Y
PROPERTY LOADS DISPLA LO1 P13 -1 X
PROPERTY BOUNDARY MPC RBEAM CO2 TOP P13 X
PROPERTY BOUNDARY MPC RBEAM CO3 TOP P13 Y
LABEL MESH OFF
LABEL MESH CONSTRNT
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
494 Composite Modeling of Masonry
LABEL MESH OFF
LABEL MESH LOADS
The labeling of constraints and loading shows the supports of the bottom edge,
the constraints of the top edge [Fig. 24.4a], and the load [Fig. 24.4b].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:34 mesh3 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:34 mesh4
2M
3M3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S3S
2S
Y Y
Z X Z X
(a) constraints (b) loading
Figure 24.4: Boundary conditions
24.2 Preliminary Linear Analysis
First of all, we will perform a linear analysis in order to check the model. There-
fore, we write a model to a file wall.dat in Diana batch format.
iDiana
UTILITY WRITE DIANA
yes
FILE CLOSE
yes
Smeared Cracking of Masonry
ANALYSE WALL
Analysis Setup
···
The ANALYSE command launches the Analysis Setup dialog where we initiate a
Structural Linear Static analysis. We ask for a results database LINSME with
displacements. This results in the following batch command file.
linsme.dcf
*FILOS
INITIA
*INPUT
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
24.3 Nonlinear Static Analysis 495
*LINSTA
OUTPUT DISPLA
*END
When the analysis has terminated we enter the iDiana Results environment
with the name of the model.
linsme.fvc
FEMVIEW LINSME
VIEW MESH
VIEW OPTIONS EDGES OUTLINE
We display an outline view of the mesh.
24.2.1 Deformation
To get the deformed mesh displayed we give the familiar commands.
linsme.fvc
RESULTS LOADCASE LC1
RESULTS NODAL DTX....G RESDTX
PRESENT SHAPE
The plot shows a deformed shape as expected [Fig. 24.5].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:31:37 lindis.ps
Model: LINSME
LC1: Load case 1
Nodal DTX....G RESDTX
Max = 1 Min = 0
Factor = 66.6
Z X
Figure 24.5: Linear deformation
24.3 Nonlinear Static Analysis
To perform the analysis of the cracks in the model we enter the iDiana Index
environment and initiate a subsequent analysis.
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
496 Composite Modeling of Masonry
iDiana
INDEX
ANALYSE WALL
Analysis Setup
···
In the Analysis Setup dialog we indicate a Structural Nonlinear analysis. We
choose options for load steps, iteration procedure, output1 , etc. The options
should result in the following batch commands.
nonsme.dcf
*FILOS
INITIA
*INPUT
*NONLIN
BEGIN EXECUT
BEGIN ITERAT
BEGIN CONVER
DISPLA OFF
FORCE TOLCON=1.0E-6
END CONVER
END ITERAT
BEGIN LOAD
LOADNR=1
BEGIN STEPS
BEGIN AUTOMA
SIZE=0.15
MAXSIZ=0.02
END AUTOMA
END STEPS
END LOAD
END EXECUT
BEGIN OUTPUT FEMVIE BINARY
DISPLA
FORCE
STRAIN PLASTI GREEN LOCAL INTPNT
STRAIN PLASTI GREEN PRINCI INTPNT
STRAIN TOTAL GREEN LOCAL INTPNT
STRESS TOTAL CAUCHY PRINCI INTPNT
END OUTPUT
*END
Now we can perform the analysis with the input data and command files.
1 Hint: To get output in the integration points of the elements click Properties in the Results
Selection dialog and then, in the Result Item Properties dialog, set the Location to Integration
points.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
24.3 Nonlinear Static Analysis 497
diana wall.dat nonsme
Once the analysis has terminated we enter the iDiana Results environment to
assess the results.
FEMVIEW NONSME
UTILITY TABULATE LOADCASES
The tabulation of the load cases shows all the performed load steps together
with their load values. We show only the head and tail of the tabulation:
nllc.tb
;
; Model: NONSME
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; MODEL STATIC "Model Properties"
; Element : THICKNES* CRKBANDW*
;
... lines skipped
; Nodal : TDTX...G FBX....G
; Gauss : EL.EPXXL EL.EP1 EL.EXX.L EL.S1
; * Indicates loads data
;
24.3.1 Displacements
To inspect the behavior of the model in the nonlinear analysis we will assess the
displacements
Load–displacement diagram nonsme.fvc
RESULTS LOADCASE LC1
RESULTS NODAL FBX....G FBX
PRESENT GRAPH NODE 962
We plot the load–displacement diagram for all load steps. For the horizontal
axis we select all load cases, i.e., the horizontal displacement for each step. For
the vertical axis we select the calculated horizontal force FX represented by
result attribute FBX. The specified node is at the upper left corner of the model
and thus we get a load–displacement diagram for the upper edge [Fig. 24.6a].
Deformation nonsme.fvc
RESULTS LOADCASE LC1 52
RESULTS NODAL TDTX...G RESTDT
VIEW MESH
PRESENT SHAPE
VIEW OPTIONS EDGES OUTLINE
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
498 Composite Modeling of Masonry
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:33:27 lodis iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:33:27 nlidfm
Model: NONSME Model: NONSME
Nodal FBX....G FBX LC1: Load case 1
Max/Min on whole graph: Step: 52 LOAD: .111
Ymax = .112E5 Nodal TDTX...G RESTDT
Ymin = 637 Max = .114 Min = 0
Xmax = .15 Factor = 587
Xmin = .3E-2
*1E4 Variation over loadcases
Node 962
1.2
1
N
O
D
A
L .8
F
B
X .6
.
.
.
.
G .4
F
B
X
.2
0
0 .2E-1 .4E-1 .6E-1 .8E-1 .1 .12 .14 .16
LOAD Y
Z X
(a) load–displacement diagram (b) deformation at uX ≈ 0.1 mm
Figure 24.6: Displacements
To assess the deformation we choose a load step for which the force is just beyond
its maximum, i.e., at a horizontal displacement uX ≈ 0.1 mm. We select the
total displacements, attribute RESTDT, and plot a deformed mesh [Fig. 24.6b].
Note that iDiana applies an automatic multiplication factor.
24.3.2 Stresses
The following commands display a contour plot of the principal stresses.
nonsme.fvc
VIEW OPTIONS EDGES ALL
VIEW OPTIONS DEFORM USING TDTX...G RESTDT
RESULTS GAUSSIAN EL.S1 S1
PRESENT CONTOUR LEVELS
RESULTS GAUSSIAN EL.S1 S2
PRESENT CONTOUR LEVELS
Here we make two plots for the principal stresses in the integration points: result
attribute S1 represents the first principal stress [Fig. 24.7a], and S2 the second
[Fig. 24.7b].
24.3.3 Plastic Strain as Crack Pattern
Displaying the plastic strain gives a good indication of the ‘cracked’ areas in the
model. Therefore we select result attribute EP1 which represents the principal
plastic strain.
nonsme.fvc
RESULTS GAUSSIAN EL.EP1 EP1
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
24.3 Nonlinear Static Analysis 499
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:33:27 nlis1 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:33:27 nlis2
Model: NONSME Model: NONSME
Deformation = 587 Deformation = 587
LC1: Load case 1 LC1: Load case 1
Step: 52 LOAD: .111 Step: 52 LOAD: .111
Gauss EL.S1 S1 Gauss EL.S1 S2
Max = .284 Max = .957E-1
Min = -.48 Min = -1.33
Results shown: Results shown:
Mapped to nodes Mapped to nodes
.215 -.335E-1
.146 -.163
.761E-1 -.292
.666E-2 -.421
Y -.628E-1 Y -.55
-.132 -.68
-.202 -.809
Z X -.271 Z X -.938
-.341 -1.07
-.41 -1.2
(a) σ1 (b) σ2
Figure 24.7: Principal stress at uX ≈ 0.1 mm
PRESENT CONTOUR LEVELS
This gives a contour plot of the principal plastic strain [Fig. 24.8]. Note that
areas without a plastic strain, which may be considered as ‘uncracked’, show
up in dark blue. Although reached at lesser deformation, the ‘crack pattern’ is
similar to that of the Brick Crack Interface model [Fig. 23.20 p. 486].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:33:28 nlep1
Model: NONSME
Deformation = 587
LC1: Load case 1
Step: 52 LOAD: .111
Gauss EL.EP1 EP1
Max = .194E-2
Min = 0
Results shown:
Mapped to nodes
.177E-2
.159E-2
.141E-2
.124E-2
Y .106E-2
.883E-3
.706E-3
Z X .53E-3
.353E-3
.177E-3
Figure 24.8: Principal plastic strain at uX ≈ 0.1 mm
Animation. The following commands initiate an animation of the develop-
ment of the principal plastic strain.
nonsme.fvc
RESULTS LOADCASE LC1 1 TO 59 STEPS 2
VIEW OPTIONS DEFORM USING TDTX...G RESTDT 500
PRESENT CONTOUR FROM 0 TO 0.0015 LEVELS 10
DRAWING ANIMATE LOADCASES
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
500 Composite Modeling of Masonry
We choose for a movie frame for each odd numbered load step until the maximum
displacement uX ≈ 0.124 mm. Furthermore we ensure a fixed deformation
scaling factor of 500× and consistent contour levels. The animation implies the
frames of Figure 24.9.
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:33:28iDIANA
anepp001
9.4.3-02 : TNO Diana BV 28 OCT 2010 02:33:28iDIANA
anepp002
9.4.3-02 : TNO Diana BV 28 OCT 2010 02:33:28iDIANA
anepp003
9.4.3-02 : TNO Diana BV 28 OCT 2010 02:33:28 anepp004
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:33:28iDIANA
anepp005
9.4.3-02 : TNO Diana BV 28 OCT 2010 02:33:28iDIANA
anepp006
9.4.3-02 : TNO Diana BV 28 OCT 2010 02:33:28iDIANA
anepp007
9.4.3-02 : TNO Diana BV 28 OCT 2010 02:33:28 anepp008
drawing animate loadcases plotfile anepp drawing animate loadcases plotfile anepp drawing animate loadcases plotfile anepp drawing animate loadcases plotfile anepp
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:33:29 anepp009 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:33:29 anepp010 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:33:29 anepp011
drawing animate loadcases plotfile anepp drawing animate loadcases plotfile anepp drawing animate loadcases plotfile anepp drawing animate loadcases plotfile anepp
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:33:29 anepp012
drawing animate loadcases plotfile anepp drawing animate loadcases plotfile anepp drawing animate loadcases plotfile anepp
drawing animate loadcases plotfile anepp
Figure 24.9: Plastic strain development (cracking) – animation frames
24.4 Including Creep Effects
We will now add properties for creep of the masonry to the model WALL, as
made in §24.1. The modified model requires a transient analysis, i.e., with time
steps instead of load steps. To modify the model we re-enter the iDiana Design
environment with the model name.
iDiana
FEMGEN WALL
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
24.4 Including Creep Effects 501
24.4.1 Material Properties
Analysis of creep effects requires the additional specification of a viscoelasticity
material model. To modify the material we launch the Property Manager.
iDiana
View →Property Manager...
↑
Property Manager
↑ Materials Material Name: BRICKS
↑External →External Data from File
Maxwell Chain viscoelasticity. We model the actual creep of the material
with a Maxwell Chain viscoelasticity model. This must be supplied via an
external input data file in Diana batch format.
maxwell.dat
MAXWEL 7
,1 YOUNG 2800.
,2 YOUNG 200.
RELTIM 1.0
,3 YOUNG 1000.
RELTIM 10.
,4 YOUNG 1000.
RELTIM 100.
,5 YOUNG 1000.
RELTIM 1000.
,6 YOUNG 1000.
RELTIM 10000.
,7 YOUNG 1000.
RELTIM 100000.
This specifies a Maxwell Chain with seven units each comprising a Young’s
modulus and a relaxation time.
24.4.2 Transient Loading
As creep analysis is transient it is performed via time steps. Consequently, the
load must be defined with respect to time. In iDiana this can be achieved via
a time curve.
wall.fgc
CONSTRUCT TCURVE TC1 LIST 0 0 36000 100
PROPERTY ATTACH LO1 TC1
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
502 Composite Modeling of Masonry
These commands define a time curve which increases linearly from 0 at time
t = 0 to 100 at time t = 36000 s (ten hours). We attach this time curve to the
already specified load LO1 which represents a unit horizontal displacement of the
upper edge of the model [§ 24.1.4 p. 493]. During the transient analysis Diana
will now apply the value of the time curve at a certain time as a multiplication
factor for the displacement.
24.5 Nonlinear Transient Analysis
Prior to the actual analysis we write a complete input data file in Diana batch
format for the modified model.
iDiana
UTILITY WRITE DIANA wallcrp
Here we write a data file wallcrp.dat. To perform the analysis we choose
options similar to those used for the previous model.
noncrp.dcf
*FILOS
INITIA
*INPUT
*NONLIN
BEGIN EXECUT
BEGIN ITERAT
BEGIN CONVER
DISPLA OFF
FORCE TOLCON=1.0E-6
END CONVER
END ITERAT
BEGIN TIME
BEGIN STEPS
BEGIN AUTOMA
SIZE=50
MAXSIZ=0.02
END AUTOMA
END STEPS
END TIME
END EXECUT
BEGIN OUTPUT FEMVIE BINARY
DISPLA
FORCE
STRAIN PLASTI GREEN LOCAL INTPNT
STRAIN PLASTI GREEN PRINCI INTPNT
STRAIN TOTAL GREEN LOCAL INTPNT
STRESS TOTAL CAUCHY PRINCI INTPNT
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
24.5 Nonlinear Transient Analysis 503
END OUTPUT
*END
Note that instead of load steps we now perform time steps, see the TIME com-
mand block. Now we can perform the analysis with the input data and command
file.
diana wallcrp.dat noncrp
Once the analysis has terminated we enter the iDiana Results environment to
assess the results.
FEMVIEW NONCRP
UTILITY TABULATE LOADCASES
The tabulation of the load cases shows all the performed time steps together
with their time values. We show only the head and tail of the tabulation:
nlcrlc.tb
;
; Model: NONCRP
;
; LOADCASE DATA
;
; Name Details and results stored
; ---- --------------------------
;
; MODEL STATIC "Model Properties"
; Element : THICKNES* CRKBANDW*
;
... lines skipped
; Nodal : TDTX...G FBX....G
; Gauss : EL.EXX.L EL.S1
; * Indicates loads data
;
24.5.1 Displacements
To inspect the behavior of the model in the nonlinear transient analysis we will
assess the displacements.
Time–load diagram noncrp.fvc
RESULTS LOADCASE LC1
RESULTS NODAL FBX....G FBX
PRESENT GRAPH NODE 962
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
504 Composite Modeling of Masonry
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:20 timlod iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:20 nlicrdfm
Model: NONCRP Model: NONCRP
Nodal FBX....G FBX LC1: Load case 1
Max/Min on whole graph: Step: 54 TIME: 45.2
Ymax = .109E5 Nodal TDTX...G RESTDT
Ymin = 580 Max = .128 Min = 0
Xmax = 50 Factor = 520
Xmin = 1
*1E4 Variation over loadcases
Node 962
1.2
1
N
O
D
A
L .8
F
B
X .6
.
.
.
.
G .4
F
B
X
.2
0
0 5 10 15 20 25 30 35 40 45 50 55
TIME Y
Z X
(a) time–load diagram (b) deformation at uX ≈ 0.13 mm
Figure 24.10: Behavior from transient creep analysis
We plot the time–load diagram for all time steps. For the horizontal axis we
select all load cases, i.e., the time for each step. For the vertical axis we select
the calculated horizontal force FX represented by result attribute FBX. The
specified node is at the upper left corner of the model and thus we get a time–
load diagram for the upper edge [Fig. 24.10a]. Note that at time t = 50 s the
horizontal displacement uX = 0.14 mm, so the horizontal scale of the time–
load diagram is equal to that of the load–displacement diagram of the non-
viscous analysis [Fig. 24.6 p. 498]. The two diagrams are quite similar. The only
noticeable difference is that the time–load diagram shows a maximum force
which is a little bit lower than that of the load–displacement diagram.
Deformation noncrp.fvc
RESULTS LOADCASE LC1 54
RESULTS NODAL TDTX...G RESTDT
VIEW MESH
PRESENT SHAPE
VIEW OPTIONS EDGES OUTLINE
To assess the deformation we choose a time step for which the force is just
beyond its maximum, i.e., at time t = 45 s where the displacement uX ≈ 0.13
mm. We select the total displacements, attribute RESTDT, and plot a deformed
mesh [Fig. 24.10b]. Note that iDiana applies an automatic multiplication factor.
24.5.2 Stresses
The following commands display a contour plot of the principal stresses.
noncrp.fvc
VIEW OPTIONS EDGES ALL
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
24.5 Nonlinear Transient Analysis 505
VIEW OPTIONS DEFORM USING TDTX...G RESTDT
RESULTS GAUSSIAN EL.S1 S1
PRESENT CONTOUR LEVELS
RESULTS GAUSSIAN EL.S1 S2
PRESENT CONTOUR LEVELS
Here we make two plots for the principal stresses in the integration points: result
attribute S1 represents the first principal stress [Fig. 24.11a], and S2 the second
[Fig. 24.11b].
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:21 nlicrs1 iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:21 nlicrs2
Model: NONCRP Model: NONCRP
Deformation = 520 Deformation = 520
LC1: Load case 1 LC1: Load case 1
Step: 54 TIME: 45.2 Step: 54 TIME: 45.2
Gauss EL.S1 S1 Gauss EL.S1 S2
Max = .286 Max = .101
Min = -.464 Min = -1.29
Results shown: Results shown:
Mapped to nodes Mapped to nodes
.218 -.258E-1
.15 -.152
.815E-1 -.279
.133E-1 -.405
Y -.55E-1 Y -.531
-.123 -.658
-.191 -.784
Z X -.26 Z X -.91
-.328 -1.04
-.396 -1.16
(a) σ1 (b) σ2
Figure 24.11: Principal stress due to transient creep at uX ≈ 0.13 mm
24.5.3 Strains
The Maxwell viscoelastic model does not deliver uniquely defined plastic strains.
So, instead of the plastic strain we will now make a contour plot of the total
strain.
noncrp.fvc
RESULTS GAUSSIAN EL.EXX.L EXX
PRESENT CONTOUR LEVELS
Result attribute EXX represents the total vertical strain εxx . The contour plot
[Fig. 24.12], is similar to that of the plastic strain [Fig. 24.8 p. 499].
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
506 Composite Modeling of Masonry
iDIANA 9.4.3-02 : TNO Diana BV 28 OCT 2010 02:38:21 nlicrexx
Model: NONCRP
Deformation = 520
LC1: Load case 1
Step: 54 TIME: 45.2
Gauss EL.EXX.L EXX
Max = .189E-2
Min = -.13E-3
Results shown:
Mapped to nodes
.17E-2
.152E-2
.134E-2
.115E-2
Y .97E-3
.787E-3
.603E-3
Z X .42E-3
.237E-3
.537E-4
Figure 24.12: Total vertical strain due to transient creep at uX ≈ 0.13 mm
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
Bibliography
[1] Beem, R. C. A. Analysis of composed concrete beam. Tech. Rep. BSW
93-06A, Bouwdienst Rijkswaterstaat, Utrecht, 1993. (In Dutch).
[2] CEB-FIP. CEB-FIP Model Code 1990. Comité Euro-International du
Béton, 1993.
[3] CEN. Eurocode 1: Basis of design and actions on structures – Part 3:
Traffic loads on bridges. Tech. Rep. ENV 1991-3, European Committee for
Standardization (CEN), 1995.
[4] Cobo del Arco, D., and Aparicio Bengoechea, A. C. Analytical
and numerical static analysis of stress ribbon bridges. In Bridge Assessment
Management and Design, B. I. G. Barr, H. R. Evans, and J. E. Harding,
Eds. Elsevier Science B.V., 1994, pp. 341–346.
[5] de Borst, R., and van den Boogaard, A. H. Finite-element modeling
of deformation and cracking in early-age concrete. J. Eng. Mech. Div.,
ASCE 120, 12 (1994), 2519–2534.
[6] Espion, B. Benchmark examples for creep and shrinkage analysis com-
puter programs. In Proc. 5th Int. RILEM Symposium on Creep and Shrink-
age of Concrete (Barcelona, 1993), pp. 877–888.
[7] Jaccoud, J. P., and Favre, R. Flèche des structures en béton armé.
Annales de l’institut technique de bâtiment et des Travaux Publics, 406
(1982).
[8] JSCE. Japan Concrete Specification. Tech. rep., Japan Society of Civil
Engineers, 1999. in Japanese.
[9] Maier, J., and Thürliman, B. Bruchversuche an Stahlbetonscheiben.
Tech. Rep. 8003-1, Zürich, 1985.
[10] Meyer, C. Analysis of underwater tunnel for internal gas explosion. In
Proc. IABSE Coll. Computational Mechanics of Concrete Structures – Ad-
vances and Applications (Delft, 1987).
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
508 BIBLIOGRAPHY
[11] Nauta, P. Dynamische belastingen (II), computerprogramma’s voor
dynamica-berekeningen – DIANA. Cement 44, 6 (1991), 64–66.
[12] Reinhardt, H. W., Blaauwendraad, J., and Jongedijk, J. Temper-
ature development in concrete structures taking account of state dependent
properties. In Proc. Int. Conf. Concrete at Early Ages (Paris, 1982).
[13] van Mier, J. G. M. Examples of non-linear analysis of reinforced concrete
structures with DIANA. Heron 32, 3 (1987).
[14] van Zijl, G. P. A. G., Rots, J. G., and Vermeltvoort, A. T. Mod-
elling shear-compression in masonry. In Proc. 9th Canadian Masonry Sym-
posium (Fredericton, NB, Canada, 2001), P. H. Bischoff, J. L. Dawe, A. B.
Schriver, and A. J. Valsangkar, Eds., no. ISBN 1-55131-040-6, University
of New Brunswick. (CDROM).
[15] Vonk, R. A., Rots, J. G., Kanstad, T., Ulm, F. J., and Navratil,
J. Examples of evaluation of computer codes for creep and shrinkage
analysis of concrete structures computer programs. In Proc. 5th Int.
RILEM Symposium on Creep and Shrinkage of Concrete (Barcelona, 1993),
pp. 889–924.
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
Index
Page numbers. Bold face numbers in- crack development, 76, 104, 138, 267,
dicate pages with formal information about 481
the entry, e.g., a syntax description (36). crack strain development, 126
Italic numbers point to an instructive ex- deformation, 205
ample of how the concept in question might setup, 201, 205
be used (132 ). Underlined numbers refer stress development, 60, 92, 344, 461
to theoretical backgrounds on the subject temperature development, 57, 201,
(95). 341, 358, 409
thermal strain development, 368
Keywords. Sans serif type style refers ARC option
to the interactive interface (EYE). Type- line, 165
writer style refers to the batch interface Arc-length control, 106, 136, 262, 281,
(YOUNG). 319
ARCLEN command, 319
ARRHEN input, 337, 353, 379, 404, 443
Arrhenius constant, 337, 353, 379, 404,
Symbols 443
Autogenous shrinkage, 363
2DSORT option, 76
Automatic load increments, 262
4POINTS option, 165
Automatic time increments, 234
Axes
A consistency check, 15, 466, 492
AXI-SYM option, 215
Accuracy
Axisymmetric elements, 160
nonlinear iteration, 233
staggered analysis, 333
Adaptive loading, 262
ADIAB input, 353, 379, 404, 424, 443
Adiabatic hydration, 353, 379, 424, 442 B
Aggregate interlock
B2AHT element, 187
constant shear retention, 212
staggered analysis, 334
Aging, 244
B2HT element
phased structural analysis, 295
staggered analysis, 361, 421
ALPHA input, 337
Bar reinforcement
ALPHA parameter
nonlinear analysis, 272
transient heat flow, 444
nonlinear phased analysis, 289
ANGLE option
BASE option
view angle, 274
quadrilateral surface, 167, 453
ANIMATE option
BC3HT element, 351
drawing, 341
Beam elements, 246
Animation
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
510 INDEX
nonlinear phased analysis, 321 CL9BE element
Bedding, 166 nonlinear analysis, 270
Bending moments nonlinear phased analysis, 321
beam elements, 254 Class-II beams, 246
diagram, 23 Colhtnl example, 333
Bernoulli beams, 248 Color modulation
BOND command, 258, 301 geometric parts, 400, 420
’BOUNDA’ table labeling, 393
concrete hydration, 443 mesh properties, 84, 177, 456, 466,
Boundary case, 192 474
Boundary conditions sets in mesh, 406, 421
potential flow, 338 Combination of load cases, 179
transient potential flow, 192, 405 Combined line, 162
Boundary constraints Commands
display, 339 eigenvalue analysis, 224
Boundary elements static nonlinear analysis, 153
conduction coefficient, 404 transient heat flow, 443
heat flow, 46, 187, 351, 377, 401 transient nonlinear analysis, 235
staggered analysis, 188, 420 Compressive strength
Box girder concrete, 275
thermal analysis, 355 Concrete
BQ4HT element, 47, 377, 402 bridge, 7
Brick elements, 46 cracking, 83, 153, 210
Bridge creep, 248, 269, 295
nonlinear phased analysis, 313 fire load, 43, 185
reinforcement forces and moments, 7 heat flow, 54, 352, 378
Bridge loading, 11 hydration, see Hydration
Maekawa model, 145
C nonlinear material properties, 196, 247
nonlinear phased analysis, 319
CALCULATE option, 139 post-tensioned, 243
CAPACI input shear failure, 95
concrete hydration, 443 shrinkage, 248, 294, 363
Capacitance slab, 145
concrete hydration, 443 slowly hardening, 422
heat flow, 191 thermoelastic properties, 49
CAPART input, 337, 443 young hardening, 333, 424, 441
CAPATT input, 191 CONDIS input, 191
CEB-FIP code, 264, 275, 363 CONDUC input
concrete creep, 248, 295, 321 concrete hydration, 443
concrete shrinkage, 248, 294 Conduction coefficient
CEMTYP input boundary elements, 379, 404
young hardening concrete, 424 cooling pipe elements, 379, 404
CHX60 element, 46 Conductivity
CL12I element, 160, 450 concrete hydration, 443
CL6TM element flow elements, 191
transient nonlinear analysis, 214 CONREA input, 337, 443
CL6TR element CONSISTENT option, 16
nonlinear phased analysis, 315 Constraints
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
INDEX 511
labeling, 18, 151 Crack pattern, 76, 104, 127, 207, 229
Contour plots Maekawa model, 155
crack index, 432 masonry, 480
crack strain, 108, 125 plastic strain, 498
degree of reaction, 435 Ultimate Limit State, 107, 138, 265
displacement, 21, 119 Crack status, 230
display style, 460 Crack strain, 76, 229
plastic strain, 125, 140, 232, 499 contour plot, 108
reinforcement stress, 61, 231 masonry, 480
stress, 21, 119, 182, 344, 460 Cracking, 65, 79, 129, 229, 248
temperature, 55, 201, 341, 356, 384, fracture energy, 276
409 interface elements, 455
thermal strain, 368 nonlinear phased analysis, 320
total strain, 505 staggered analysis, 336
CONVEC input transient nonlinear analysis, 210
boundary elements, 424 Creep, 248
Convection masonry, 500
boundary elements, 424 phased analysis, 295, 322
Convergence, 204 Creep curves, 275, 295, 321
nonlinear analysis, 107, 228 Creep strain, 205
transient heat flow, 445 Cross-section
Convergence criteria, 121, 234, 262 bar reinforcement, 294
CONVTT input Cross-section view, 56, 408
boundary elements, 192, 424 CROSSE input
Cooling pipe elements, 371, 376 reinforcements, 294
internal temperature, 412 Crushing, 129, 139
material input, 379, 404 masonry, 467
meshing, 394 CT12E element, 367
Coolpi example, 389 staggered analysis, 360, 419
’COOLPI’ table, 406 CT6HT element, 351
Coordinate systems, 16 Cursor picking, 377, 395, 411
CQ16A element, 160 CUTAWAY option, 410
staggered, 188 Cutaway view, 410
staggered analysis, 334
CQ16E element, 367
D
staggered analysis, 360, 419
transient nonlinear analysis, 212, 214 DEFORM option, 21, 59, 120, 477
CQ16M element, 97, 114, 132, 450 Deformed mesh, 71, 87, 479, 498
masonry, 491 animation, 205
nonlinear phased analysis, 288 results plot, 92, 120, 138, 182, 460
CQ40S element, 13 Degree of reaction, 336, 337
concrete cracking, 148 output, 342, 359, 386, 411, 435, 445
CQ8HT element, 351 Delaunay meshing, 419
Crack bandwidth Dependent transformation, 161
estimated, 276 DGR output, 445
Crack development, 137, 481 DGRINI parameter, 444
Crack index Diagram
staggered analysis, 432, 439 bending moment, 23
tensile strength input, 424 DISC option, 76, 104, 127, 138, 154
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
512 INDEX
Disc plot, 207 380, 405, 425
display style, 229
Discrete cracking, 79, 455
F
DISPLA command
phased analysis, 300 FACTOR option
Displacement-controlled analysis, 100 disc plot scaling, 229
DISPLAY option, 10 meshing divisions, 10, 47, 189, 361
Distributed load, 18 FEMVIE output device, 272
DIVISION option, 10 transient heat flow, 444
Divisions for meshing, 10, 214 Fire example, 43
Dynamic analysis Fire load, 53, 185
transient nonlinear, 209 FiTank example, 159
FIXTEMP load class, 425
E FLIP option, 16, 466
Flow elements, 351, 376
E output Flow–stress analysis, 43, 54, 185, 415
linear static analysis, 310 FLUX load class, 192
Edge representation, 409 Force-controlled analysis, 105, 136
EDGES option Foundation
edge representation view, 409 interface elements, 166
mesh display, 88, 411 FTTIME input, 424
Eigenfrequency FTVALU input, 424
explosion, 225
Eigenmode
G
explosion, 225
Eigenvalue analysis Galerkin integration
explosion, 224 transient heat flow, 444
Elastic strain, 205 Gauss integration, 272
Element numbers GAUSSIAN option, 342
labeling, 102 results selection, 446
ELSIZE option, 67, 335 Gaussian results
Energy norm, 262 crack strain, 74, 76, 284
ENV 1991-3 code, 11, 33 degree of reaction, 342, 356, 446
EQUAGE command, 407 Geometric nonlinearity
Equivalent age phased analysis, 313
output, 387 Girder example, 347
European code, see ENV Grading of line divisions, 132
EXECUT command GRAPH option
nonlinear phased analysis, 318 time response, 446
staggered analysis, 340, 343 Graph plotting, 412
transient heat flow, 444 display style, 239
Explosion, 209 history, 62, 202, 239
Extreme result result along line, 23, 56, 143, 253,
in monitor, 21, 143 302
EXTTEMP load class, 53, 193, 338, 354, Gravity, 173
flow–stress analysis, 365
Gravity acceleration
staggered analysis, 426
GRAVITY load class, 18
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
INDEX 513
flow–stress analysis, 365, 426 *INPUT command, 407
structural analysis, 173, 217 Input data
Grid reinforcement, 49, 113, 148, 160, 215 heat flow analysis, 442
Groups, 292 reinforcements, 294
INPUT option
initial stresses, 318
H
transient heat flow, 444
Hardening Insulation, 442
reinforcement steel, 116, 149 Integration schemes
Von Mises plasticity, 146 beam elements, 256
HE elements, 401 nonlinear analysis, 256
Heat flow analysis, 54, 348, 406 Interface elements, 160
transient nonlinear, 382 cracking, 79, 82, 455, 463
Heat production modeling, 82, 166, 451, 453
maturing concrete, 441 structural, 450
*HEATTR command, 367, 407, 443 Intersection point, 165
staggered analysis, 340 ITERAT command
Hidden view, 376 nonlinear heat flow, 444
History plot ITERAT option
nonlinear phased analysis, 303, 306 transient heat flow, 444
transient heat flow, 342, 446 Iterative solution procedure
transient nonlinear analysis, 62, 238, transient nonlinear analysis, 234
279
HSTAG option, 186, 360 J
HX8HT element, 376, 401
HYDRAT command, 444 JSCE code
Hydrat example, 441 young hardening concrete, 424
Hydration, 379 JSCE input
adiabatic, 441 young hardening concrete, 424
staggered analysis, 333, 424
transient heat flow, 359, 403, 441,
K
444
Hysteresis Kelvin Chain model, 336
reinforced concrete, 158 aging, 295
I L
IL elements L2HT element, 376, 401
structural, 167, 453 L7BEN element, 246
INITEMP initial condition class, 194, 338, L8IF element, 82
354, 381, 405 Labeling the model
INITIA command supports, 18
nonlinear phased analysis, 318 surfaces, 9
transient heat flow, 444 LCMB option, 162
Initial conditions LIMITS option
flow analysis, 338, 354, 381, 405 append to set, 471
Initial potential field, 193, 338, 427 LINE input
’INIVAR’ table reinforcements, 294
potential flow analysis, 443 Line names
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
514 INDEX
labeling, 374 MODEL command
Line Search, 262 eigenvalue analysis, 224
Linear static analysis, 118, 251 nonlinear analysis, 228
LIST option MODULATE option
polyline, 143 vector colors, 72, 88
time curve, 354, 426 Monitor
LOAD command display position, 417
nonlinear stop criterion, 319 MPC option, 339
Load–displacement diagram, 74, 91, 102, Multi–directional fixed crack model, 95,
123, 137, 497 248, 320
masonry, 479 Multi-point constraints, 339
Ultimate Limit State, 107 Multiple viewports, 250
LOADCASES option
animation, 341
N
Loading
labeling, 250 Newmark integration, 233
Logarithmic scale for graph, 303, 306 NINTEG input
beam elements, 256
M NMODES parameter
eigenvalue analysis, 224
Maekawa example, 145 NOBOND input, 295, 300
Maekawa model, 145 Node numbers
MasonDi example, 463 labeling, 48, 101, 122, 136
Masonry, 449, 492 NONLIN command
composite modeling, 489 transient heat flow, 444
discrete modeling, 463 Nonlinear analysis, 88, 121, 458
transient creep, 500 cracking, 72, 134
Material properties dynamic, 233
aging concrete, 295 heat flow, 406
heat flow, 352, 403 phased, 297, 313
MATERIALS option Serviceability Limit State, 256
colored elements, 177 staggered, 342
edge display, 88 Ultimate Limit State, 260
Maturity, 333 Normal force
MAXPRD input, 337 beam elements, 255
Maxwell Chain model, 336 Notch example, 79
concrete creep, 275, 308, 321 Notched beam, 65, 79
masonry creep, 501 NotchSm example, 65
Merge
mesh, 48, 190, 362, 421
O
tolerance, 190, 421
Mesh quality, 351, 419 OUTLINE option
labeling, 14 postprocessing, 409
Meshing
algorithm, 67, 81
P
axisymmetric model, 160
Mirror transformation, 14 P-STRESS option, 72, 88, 223, 345
Mirroring Panel example, 109
geometry copy, 68, 82 PARABO input
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
INDEX 515
reinforcement bars, 251 Post-tensioning, 243
Parameter, 161, 171 PostTe example, 243
Paving meshing, 67, 81 POTENT input
PAVING option, 67, 81 transient heat flow, 443
Peak values, 224 Power Law, 336
PEAKS option viscoelasticity, 424
highlighting, 224 PRDKAR input, 337
*PHASE command Predefined shapes for beam elements, 248
nonlinear analysis, 298 Prefab concrete, 319
PHASE option phased analysis, 287
nonlinear analysis, 300 PRESSURE load class, 18, 52, 174, 218
Phased analysis, 287 PRESTRES load class, 174
nonlinear, 297, 313 Prestress, see Reinforcement
staggered, 415 Principal stress, 223, 232
PHYSIC command contour plot, 76, 369
nonlinear analysis options, 301 vector plot, 72, 87, 124, 139, 181
PHYSICAL option PROPAGATE option, 214
beam display, 249 PTE output
colored elements, 177 heat flow, 445
Physical properties Purification wall, 415
heat flow, 403 PurWal example, 415
PINNED option, 117
PLANE option
Q
shape, 408
Plane shape, 408 Q4AHT element
Plane strain elements staggered analysis, 334
flow–stress analysis, 360 Q4HT element, 367
staggered analysis, 419 concrete hydration, 442
transient nonlinear analysis, 212 Q8IF element, 463
Plane stress elements, 81, 97, 109, 114, Q8MEM element, 67, 81, 463
132, 450, 463 QU elements
cracking, 67 structural, 162
masonry, 491 Quadrilateral meshing, 67, 81
nonlinear phased analysis, 288 QUALITY option
Plastic strain, 232 colored elements, 419
concrete crushing, 140 QUICK option
contour plot, 498 local axes display, 22
reinforcement, 124, 141, 263
Plastic yield
R
reinforcement, 263
PLOTFILE option Radiation, 187
animation, 341, 409 RANGE option
Point names results selection, 21, 284
labeling, 349, 373 Rankine–Hill plasticity, 492
Pointer display position, 202 RBEAM option, 339
POLYGON option RCbeam example, 269
cursor selection, 395 REACTI input, 337, 443
Portal example, 129 READ command, 459
Portal frame, 129 ReBridge example, 7
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
516 INDEX
RECTANGUL option Shape, 56
coordinate system, 16 Shear example, 95
REGION option Shear failure
surface definition, 13 concrete, 95
Regular Newton–Raphson iteration Shear force
nonlinear analysis, 234 beam elements, 255
’REINFO’ table, 251 Shear locking, 272
Reinforcement Shear retention
concrete creep, 321 constant, 212, 321
display, 49, 97, 98, 114, 132, 148, Shear wall panel, 109
171, 216, 247 Shell elements
labeling, 216 concrete cracking, 148
material, 176 curved, 13
modeling, 48, 97, 113, 132, 168, 215, SHRINF input, 364
246 SHRINK option, 336
nonlinear analysis, 146, 272 Shrinkage, 248, 363
phased analysis, 288 phased analysis, 294, 318
plasticity, 104, 124, 141, 263 Shrinkage strain, 275, 364
post-tensioned, 243 Shrunken elements view, 47
stress in bar, 103, 253, 264 SHTIME input, 364
stress in grid, 61 Simpson integration, 272
thickness, 176, 220 SIZES command
transient nonlinear analysis, 209 transient heat flow, 340, 444
Reinforcement forces and moments, 7 SLS, 256
Reinforcement moments Smeared cracking, 65
contour plot, 25 Softening, 136
Reinforcement prestress, 28, 174, 313 Soil
cables, 297 thermo-mechanical properties, 422
Reinforcement steel, 51, 99, 134 Solid elements, 46
plasticity, 247 Space curve, 175
Relaxation SPHERI command, 319
concrete, 259 Spherical Path, 281, 319
prestress, 258 SPLIT option, 213
Relaxation function, 295 Spring elements, 167
Rigid Beam MPC, 217, 339 Srbrid example, 313
Rotating crack model, 109 Staggered analysis, 43, 54, 185, 366
concrete hydration, 339, 416
elements, 46
S
START command
Safety tank, 159 nonlinear phased analysis, 318
SDIRK2 method, 234 STOP command, 319
SECANT option STRAIGHT option
cracking, 318 line definition, 335
SECTION option Strain
reinforcement bar, 132 transient nonlinear analysis, 205
Serviceability Limit State, see SLS Stress
Set in time, 62, 370
colored display, 17 nonlinear analysis, 231
SET option, 10 STRESS command
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
INDEX 517
initial stresses, 318 Temperature evolution, 56, 57, 356, 429
Stress evolution Temperature influence
young hardening concrete, 431 concrete, 196
STRTNO input, 406 reinforcement, 197
Supports Temperature load, 44
graphic display, 18, 117 flow–stress analysis, 53
SURFACE option nonlinear phased analysis, 324
results, 21, 260, 284 TEMYLD input
SWAP option, 56, 91 Drucker–Prager plasticity, 197
SWEEP option, 10 TEMYOU input
Sweeping parts, 10, 45, 96, 112, 161, 162, linear elasticity, 197
374, 394 Tensile strength
Switch analysis type, 342 concrete, 196, 220, 276, 424
SYMBOL option discrete cracking, 455
results presentation, 141 Tension softening, 147
Symbols for results presentation Tension stiffening
cracks, 230 concrete, 211, 320
plastic strain, 141, 263 Thermal analysis, 355
Symbols, glossary of, xvii Thermal expansion
Symmetry, 52, 297, 426 temperature dependent, 197
Thermal strain
concrete, 368
T
THICK input
T3HT element, 367 plane stress elements, 294
TABULA output device Time curve, 193, 196, 405
transient heat flow, 444 boundary conditions, 426
Tabular output, 205 load, 52, 365, 501
transient heat flow, 444 temperature, 53, 338, 354, 380
TABULATE option Time dependency
load cases, 356, 383 staggered analysis, 426
Tapered thickness Time integration
plane stress elements, 294 transient nonlinear analysis, 233
TCURVE option, 354 Time steps
TEMALP input nonlinear analysis, 234
linear elasticity, 197 Time–load diagram
TEMPER command nonlinear analysis, 218, 297
transient heat flow, 444 ’TIMELO’ table
TEMPER input, 191 nonlinear analysis, 297
cooling pipe elements, 406 TOTAL option
’TEMPER’ table, 458 nonlinear stop criterion, 319
nonlinear phased analysis, 324 Total Strain cracking, 115
Temperature Traction
concrete, 200, 356, 383, 408 linear static analysis, 88
contour plot, 55, 201, 384 Traffic load
cooling pipe, 387 ENV 1991-3 code, 33
heat flow, 341, 446 Transient analysis
vs. time, 458 heat flow, 339, 355, 406
Temperature analysis nonlinear, 202, 233, 299, 502
staggered, 333 staggered, 54, 198, 333
Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI) November 8, 2010 – First ed.
518 INDEX
Transient creep, 500 VISCOE command, 318
Transient flow analysis Viscoelasticity
nonlinear, 339, 355, 382, 406, 443 concrete creep, 295, 424
TRANSLATE option masonry, 501
geometry copy, 47 shrinkage, 318
Transparency, 249 staggered analysis, 336
TRANSPARENT option, 249 VONMISES option, 223, 344
TRIANGLE option Von Mises plasticity, 146
result symbol, 231 reinforcement, 99, 116
Triangular meshing, 419 Von Mises stress
Truck load contour plot, 59, 91, 182, 223, 232,
ENV 1991-3 code, 11, 33 344
Truss elements peak values, 223
nonlinear phased analysis, 315
Tunnel
W
concrete cooling, 390
dynamic analysis, 209 Walcoo example, 371
Tunnel example, 209 Wall example, 449
Tyings WalShr example, 489
no rotation, 212 Wheel load, 11
truss–beam, 322 WHITE option, 194
’TYINGS’ table WORK-BOX option
truss–beam, 322 framing, 111
TYPE command Workbox, 161
nonlinear analysis, 258 framing, 111, 334
U X
ULS, 75, 107, 136, 260 XLOG option, 303, 306
Ultimate Limit State, see ULS XSECTION option
’UNITS’ table model view, 56, 384, 408
concrete creep, 292, 309
Y
V
YOUHAR input
VALUES option Japanese Code, 424
contour plot, 25 YOUN91 input, 424
Vector plots Young’s modulus
interface traction, 88 temperature dependent, 197
principal stress, 72, 87, 124, 139, 181,
223, 345
Z
velocity, 236
VECTORS option, 139 Zooming, 165
color and style, 72, 88
Velocity
transient analysis, 236
Viaduct example, 287
Viewport control, 250
VIEWPORT option, 250
November 8, 2010 – First ed. Diana-9.4.3 User’s Manual – Concrete and Masonry Analysis (VI)
You might also like
- Notes On Cracked and Uncracked Concrete Sections...100% (4)Notes On Cracked and Uncracked Concrete Sections...22 pages
- 2019-20-Ce Seismic Analysis and Design of g+4 Residential Building in Moderate and High Earthquake Zones - 05No ratings yet2019-20-Ce Seismic Analysis and Design of g+4 Residential Building in Moderate and High Earthquake Zones - 0554 pages
- 2022 Bookmatter ReinforcedConcreteWithWorkedExNo ratings yet2022 Bookmatter ReinforcedConcreteWithWorkedEx18 pages
- Analysis of A Reinforced Concrete BuildingNo ratings yetAnalysis of A Reinforced Concrete Building119 pages
- Reinforced Concrete With Worked Examples (Franco Angotti, Matteo Guiglia, Piero Marro Etc.) (Z-Library)100% (2)Reinforced Concrete With Worked Examples (Franco Angotti, Matteo Guiglia, Piero Marro Etc.) (Z-Library)860 pages
- Manual For The Design of Reinforced Concrete Building Structures To EC2No ratings yetManual For The Design of Reinforced Concrete Building Structures To EC215 pages
- Analysis of Reinforced Concrete Maluos BNo ratings yetAnalysis of Reinforced Concrete Maluos B67 pages
- Computational Methods in Reinforced Concrete100% (1)Computational Methods in Reinforced Concrete211 pages
- Durham E-Theses: Tension Stiffening in Reinforced Concrete Members With Large Diameter ReinforcementNo ratings yetDurham E-Theses: Tension Stiffening in Reinforced Concrete Members With Large Diameter Reinforcement119 pages
- Reinforced Concrete With Worked Examples: Franco Angotti Matteo Guiglia Piero Marro Maurizio OrlandoNo ratings yetReinforced Concrete With Worked Examples: Franco Angotti Matteo Guiglia Piero Marro Maurizio Orlando860 pages
- TR-2-82 Connections For Precast BuildingsNo ratings yetTR-2-82 Connections For Precast Buildings310 pages
- 2022-23-CE DESIGN OF RESIDENTIAL BUILDING (G+2) BY USING REVIT - (5) - Batch-28No ratings yet2022-23-CE DESIGN OF RESIDENTIAL BUILDING (G+2) BY USING REVIT - (5) - Batch-2837 pages
- MSC Thesis JRMoraal Wind Turbine Foundation Model100% (1)MSC Thesis JRMoraal Wind Turbine Foundation Model97 pages
- Model Report of 230KV Transformer Foundation at FaridpurNo ratings yetModel Report of 230KV Transformer Foundation at Faridpur97 pages
- General Static Analysis of FE Structures: Sofistik 2025No ratings yetGeneral Static Analysis of FE Structures: Sofistik 2025220 pages
- 2022-23-Ce-Analysis and Design of (G+3) Commercial Building Using Etabs-5No ratings yet2022-23-Ce-Analysis and Design of (G+3) Commercial Building Using Etabs-554 pages
- Ansys Modeling of Flexural Behavior of RC Beam Strengthening by FRP100% (3)Ansys Modeling of Flexural Behavior of RC Beam Strengthening by FRP57 pages
- Pre and Post-Process Tools in Finite Element Analysis: Universitat de Girona100% (1)Pre and Post-Process Tools in Finite Element Analysis: Universitat de Girona213 pages
- TibertLicThesis-Numerical Analyses of Cable Roof Structures100% (1)TibertLicThesis-Numerical Analyses of Cable Roof Structures196 pages
- Numerical Analyses of Cable Roof Structures - Gunnar TibertNo ratings yetNumerical Analyses of Cable Roof Structures - Gunnar Tibert196 pages
- Preface Xvii Author Xix: 1 Setting Up The Project 1No ratings yetPreface Xvii Author Xix: 1 Setting Up The Project 110 pages
- Seismic Analysis and Design 4 Storey Using Staad 200422No ratings yetSeismic Analysis and Design 4 Storey Using Staad 200422175 pages
- ALMAR - Fatigue Handbook - Offshore Steel Structures (1985) COMPLETE VERSIONNo ratings yetALMAR - Fatigue Handbook - Offshore Steel Structures (1985) COMPLETE VERSION532 pages
- WILCKEN - Alpha Factors For The Calculation of Forecasted Operational LimitsNo ratings yetWILCKEN - Alpha Factors For The Calculation of Forecasted Operational Limits67 pages
- Buckling of S-Ffened Plates According To DNV RP C201No ratings yetBuckling of S-Ffened Plates According To DNV RP C20116 pages
- Edit This Text For Your Title: MEK 4450 Marine Operations. 1-1No ratings yetEdit This Text For Your Title: MEK 4450 Marine Operations. 1-154 pages
- Nonsurgical Lip and Eye Rejuvenation Techniques: Gabriella Fabbrocini Maria Pia de Padova Antonella Tosti90% (10)Nonsurgical Lip and Eye Rejuvenation Techniques: Gabriella Fabbrocini Maria Pia de Padova Antonella Tosti125 pages
- Assignment, 2020) - I Am Working As Asst. Manager (Environment, Health &No ratings yetAssignment, 2020) - I Am Working As Asst. Manager (Environment, Health &3 pages
- p0467v1-1 Estimation and Tendering - Some Contextual Factors100% (1)p0467v1-1 Estimation and Tendering - Some Contextual Factors12 pages
- CE5106-2021 - Ch4 - Dynamic Compaction Method+DesignNo ratings yetCE5106-2021 - Ch4 - Dynamic Compaction Method+Design37 pages
- Method Statement For Antibacterial PaintNo ratings yetMethod Statement For Antibacterial Paint7 pages
- Peikko Solutionsforparkingconstruction BrochureNo ratings yetPeikko Solutionsforparkingconstruction Brochure12 pages
- Reflected Ceiling Plan Floor Tile Layout: Legend0% (1)Reflected Ceiling Plan Floor Tile Layout: Legend1 page
- General Conditions of Contract Clause 31 and Special Conditions of Contract Clause 10 SimplifiedNo ratings yetGeneral Conditions of Contract Clause 31 and Special Conditions of Contract Clause 10 Simplified2 pages
- List of House Types: 1 Detached Single-Unit HousingNo ratings yetList of House Types: 1 Detached Single-Unit Housing10 pages
- Faculty of Architeecture and Planning, Aktu LucknowNo ratings yetFaculty of Architeecture and Planning, Aktu Lucknow29 pages
- Road Pavement Design For Frost Prone AreNo ratings yetRoad Pavement Design For Frost Prone Are4 pages
- BOQ For Repair Work of 40'X20' Building at A/Selesthimaduwa VidyalayaNo ratings yetBOQ For Repair Work of 40'X20' Building at A/Selesthimaduwa Vidyalaya9 pages
- Construction of Proposed Subsidiary Training Centre of BSF at Chakur, Latur (Maharashtra) Bill of Quantities For Civil Works - Swimming Pool Nit NoNo ratings yetConstruction of Proposed Subsidiary Training Centre of BSF at Chakur, Latur (Maharashtra) Bill of Quantities For Civil Works - Swimming Pool Nit No16 pages