Practical Aspects of Composites Analysis and

Optimization

2 1st Edition; Released: April 2018

Table of Contents
About This Book ............................................................................................................ 7
Acknowledgement ...................................................................................................... 10
1 Introduction to Composite Materials ................................................................. 11
1.1 Composite Materials ........................................................................................ 11
Particulate Composites ....................................................................................... 11
Laminated Composites ....................................................................................... 12
Fiber-Matrix Laminated Composites .................................................................. 12
Core-Stiffened Laminated Composites ............................................................... 16
1.2 Material Terminology ....................................................................................... 16
Microscopic ......................................................................................................... 16
Macroscopic ........................................................................................................ 17
Micromechanics .................................................................................................. 17
Macromechanics ................................................................................................. 17
Homogeneous ..................................................................................................... 17
Heterogeneous ................................................................................................... 17
Isotropic .............................................................................................................. 17
Orthotropic ......................................................................................................... 17
Anisotropic .......................................................................................................... 18
1.3 Ply Conventions................................................................................................. 18
1.4 Laminate Conventions and Definitions ............................................................. 18
Defining Laminates ............................................................................................. 20
Symmetric Laminates.......................................................................................... 20
Anti-Symmetric Laminates .................................................................................. 20
Balanced Laminates ............................................................................................ 21
Cross-Ply Laminates ............................................................................................ 21
Angle-Ply Laminates ............................................................................................ 22
General Laminates .............................................................................................. 22
1.5 Common Advantages and Drawbacks of Composite Design ............................ 23
2 Basics of Composite Analysis .............................................................................. 25
2.1 Composite Designable Material Properties ..................................................... 25
2.2 Understanding Composite Material Properties ............................................... 26
2.3 The [A] [B] [D] Matrix ....................................................................................... 30
2.4 Failure Theories of Composite Lamina............................................................. 31

3
 2.4.1 Maximum Stress Theory ............................................................................... 31
2.4.2 Maximum Strain Theory ............................................................................... 33
2.4.3 Tsai-Hill Failure Theory.................................................................................. 34
3 Composite Modeling in OptiStruct ..................................................................... 35
3.1 Composite Pre-Processing ............................................................................... 35
Model Browser.................................................................................................... 36
Entity Editor ........................................................................................................ 36
3.2 Composite Material Types ............................................................................... 37
3.3 Material and Element Orientation ................................................................... 39
3.4 Types of Laminate in HyperMesh - OptiStruct ................................................. 41
Interface Laminate .............................................................................................. 42
3.5 Different Composite Modeling Methods ......................................................... 43
i. Composite Zone-Based Shell Modeling ...................................................... 43
ii. Composite Ply-Based Shell Modeling ......................................................... 48
iii. Composite Ply-by-Ply Solid Modeling ......................................................... 53
3.6 Zone based Vs Ply based .................................................................................. 55
3.7 Tutorial: Assigning Material Orientation......................................................... 64
3.8 Tutorial: Difference between PCOMP and PCOMPG using FEA approach ...... 74
3.9 Tutorial: Creating Ply-based Laminates ........................................................... 86
3.10 Basic Composite Modeling in HyperMesh Videos ......................................... 96
4 Advanced Composite modeling in OptiStruct..................................................... 97
4.1 Importing composite data with HyperWorks ................................................... 97
4.2 Using HyperLaminate Module to Create Composite Structure ...................... 100
4.3 Useful tools and options in HyperMesh Aerospace module .......................... 105
5 Post-Processing for Composites ....................................................................... 115
5.1 Overview of Composite Post-Processing ....................................................... 115
5.2 Ply-Based Composite Post-Processing ........................................................... 116
5.3 Tutorial: Simulating a Plate with a Hole, Test Coupon .................................. 117
5.4 Exercise1: How changing the angle changes the results?.......................... 123
5.5 Exercise2: Create a laminate of T Shaped Beam as shown using sub-laminates
and interfaces. Use the T-Beam model file........................................................... 123
6 Composite Optimization ................................................................................... 125
6.1 Composite Design Characteristics and Challenges ......................................... 125
6.2 Composite Design Costs and Complexity ....................................................... 126

4
 6.3 Optimization-Assisted Composite Design ...................................................... 127
6.4 What is OptiStruct Optimization? .................................................................. 128
6.5 Optimization Setup Module in HyperMesh ................................................... 128
6.6 Factors affecting composite optimization ..................................................... 134
6.7 Extrapolating Optimization from Composite Analysis ................................... 134
6.8 Composite Optimization: Three Steps from Concept to Final Design ........... 135
ii. Size Optimization ...................................................................................... 137
6.8.1 Phase 1: Free Size Optimization .............................................................. 138
6.8.2 Phase 2: Size Optimization ...................................................................... 159
6.8.3 Phase 3: Composite Shuffling Optimization............................................ 165
6.8.4 Final Design Verification ......................................................................... 169
6.9 Tutorial: Bike Frame Optimization using PCOMP and PCOMPG ................... 169
6.10 Optimization Example Videos ..................................................................... 181
6.11 Tutorial: Composite Optimization on A Solar Car Carbon Fiber Shock Mount
.............................................................................................................................. 181
Introduction ...................................................................................................... 181
1. Free Size Optimization .................................................................................. 191
2. Size Optimization .......................................................................................... 204
3. Shuffle Optimization ..................................................................................... 212
Setup ................................................................................................................. 213
Shuffle Design Variable Update ........................................................................ 213
Results ............................................................................................................... 214
Example: Three-wheeler Motorbike – Composite optimization of the Fairing .... 217
Appendix A ................................................................................................................ 219
OptiStruct I/O Options Reference......................................................................... 219
CSTRAIN ............................................................................................................ 219
CSTRESS ............................................................................................................. 221
DISPLACEMENT ................................................................................................. 222
OUTPUT ............................................................................................................. 223
THICKNESS......................................................................................................... 225
Appendix B OptiStruct Analysis Bulk Data Reference ............................................... 227
MAT1 ................................................................................................................. 227
MAT9 ................................................................................................................. 231
MAT9ORT .......................................................................................................... 232

5
 PCOMP .............................................................................................................. 233
PCOMPG............................................................................................................ 233
PCOMPP ............................................................................................................ 233
PLY ..................................................................................................................... 237
PSHELL ............................................................................................................... 239
STACK – Ply laminate definition ........................................................................ 242
STACK - Interface laminate definition ............................................................... 245
Appendix C OptiStruct Optimization Bulk Data Reference ....................................... 249
DCOMP .............................................................................................................. 249
DCONADD ......................................................................................................... 259
DCONSTR ........................................................................................................... 260
DDVAL ............................................................................................................... 261
DDVAL ............................................................................................................... 262
DDVAL ............................................................................................................... 263
DSHUFFLE .......................................................................................................... 268
DSIZE ................................................................................................................. 271
DVPREL1 ............................................................................................................ 284

6
About This Book
An engineering student should not only have theoretical knowledge; but, should also
know the practical aspects of any subject. A student who learns theory in the class
should be able to apply it practically. This book aims to provide both theoretical and
practical knowledge of composites to the student.

This book covers basic introduction to composite materials, terminologies used in

composites with different failure theories used to predict the failure of the
composites. In the practical part, this book covers how to model a composite structure
in HyperMesh, how to perform analysis and three-phase optimization of a composite
structure using OptiStruct and how to Post-Process the results in HyperView and
HyperGraph.

This book also consists of some tutorials and exercises for students to practice on their
own. There are few videos/video-links in this eBook to understand the concepts very
quickly and easily.

And now - enjoy the latest edition of this book and keep on learning and exploring.

Best regards

Dr. Matthias Gölke

On behalf of “ The Altair University Team

P.S.: We would appreciate your feedback about your learning experience

(eMail altairuniversity@altair.com)

7
Model Files
The models referenced in this book can be downloaded using the link provided in the
exercises, respectively. These model files are based on the Altair Student Edition 2017.

Software
Obviously, to practice the “Composite Analysis and Optimization” you need to have
access to Altair Student Edition 2017 (or higher). As a student, you are eligible to
download and install the free Student Edition:

https://altairuniversity.com/free-altair-student-edition/

Note: From the different software packages listed in the download area, you just need
to download and install the “Bundled installation package for Modeling,
Visualization, Analysis and Optimization”

Support
In case you encounter issues (during installation
or on how to utilize OptiStruct) post your
question in the moderated Support Forum
https://forum.altair.com
It’s an active forum with several thousands of
posts – moderated by Altair experts!

8
Free eBooks
In case you are interested in more details about the “things” happening in the
background we recommend our free eBooks

https://altairuniversity.com/free-ebooks-2

Many different eLearning courses are available for free in the Learning & Certification
Program

A kind of prerequisite course (knowledge) before you start with the analysis and
optimization of composites is:

Learn Structural Analysis with Altair OptiStruct

https://certification.altairuniversity.com/course/view.php?id=71

This course is to introduce basic composite linear static analysis.

Learn Composite Analysis and Optimization with Altair OptiStruct

https://certification.altairuniversity.com/course/view.php?id=93

9
Acknowledgement
A very special Thank You goes to all the many colleagues who contributed in different
ways:
Premanand Suryavanshi for reviewing, testing and editing the tutorials contained in
this book.
Rahul Ponginan, and Sanjay Nainani for reviewing the book. For sure, your feedback
and suggestions had a significant impact on the “shape” and content of this book.
Jeffrey A. Wollschlager, Author of “Introduction to the Design and Analysis of
Composite Structures” for generously sharing his book with all of us and the
inspirational collaboration.
Mike Heskitt, Sean Putman & Dev Anand for all the support.
The entire OptiStruct Documentation team for putting together 1000’s of pages of
documentation and recently released OptiStruct verification problem manual.
Lastly, the OptiStruct Development team deserves huge credit for their passion &
dedication! It is so exciting to see how OptiStruct has evolved throughout the last
couple of years.

Thank you very much.

Your Altair University Team

Disclaimer
Every effort has been made to keep the book free from technical as well as other mistakes.
However, publishers and authors will not be responsible for loss, damage in any form and
consequences arising directly or indirectly from the use of this book.
© 2019 Altair Engineering, Inc. All rights reserved. No part of this publication may be
reproduced, transmitted, transcribed, or translated to another language without the written
permission of Altair Engineering, Inc. To obtain this permission, write to the
attention Altair Engineering legal department at:
1820 E. Big Beaver, Troy, Michigan, USA, or call +1-248-614-2400.

10
 1 Introduction to Composite
Materials
This chapter is entirely from Jeffrey A. Wollschlager’s “Introduction to the Design and
Analysis of Composite Structures” book.

The objective of this chapter is to present an overview of composite material

terminology commonly used in practice. The chapter begins with a brief review of
different types of composites that are commonly used and are generally available for
designing composite parts. One of the most broadly used composite types are fiber-
matrix laminated composites. The chapter continues by defining common elasticity
and mechanics of materials terminology. Finally, the chapter concludes by defining
ply and laminate conventions.

1.1 Composite Materials

A composite material is a material that is formed by combining two or more materials
on a macroscopic scale. The macroscopic scale is an important part of the definition
of a composite material, as this book does not cover the analysis or design of
composite materials at the microscopic scale. There are several basic composite
material forms commonly used and currently available for producing composites
parts, each of which is defined below.

Particulate Composites
Particulate composite materials are materials that are manufactured by spreading
pieces of chopped fiber material onto a film of matrix material. This book does not
cover the analysis or design of particulate composites.

Figure 1.1, Particulate Composite Ply Material

11
Laminated Composites
Laminated composite materials are materials that are made up of any number of
layered materials, of the same or different orientation, bonded together with a matrix
material. The layers of a laminated composite, typically called plies, can be made from
several materials, including adhesive plies, metallic-foil plies, fiber-matrix plies of
various fiber and matrix material combinations, and core plies of various core
materials.

Fiber-Matrix Laminated Composites

Fiber-matrix laminated composite materials are materials that are made up of any
number of fiber-matrix plies, of the same or different fiber orientation, layered and
bonded together with some matrix material. There are several types of fiber-matrix
ply materials commonly used and currently available in the manufacturing of fiber-
matrix laminated composite parts. The most common fiber materials used in fiber-
matrix ply material systems include various types of boron, carbon, glass, and Kevlar®
fibers. The most common matrix materials used in fiber-matrix ply material systems
include various types of thermosetting and thermoplastic epoxies. Fiber-matrix ply
materials can be classified into the following general categories; unidirectional plies,
2D plain weave plies, 2D 5-harness-satin (5HS) plies, and 3D woven fiber-matrix
materials.

Unidirectional ply materials are made up of “straight” fibers embedded in a matrix

material. Figure 1.2 shows a schematic of a unidirectional ply material. Typical
unidirectional ply thicknesses range from 0.005–0.015 inches with typical fiber
volumes between 0.45–0.70. Typical unidirectional ply material properties for several
common fiber-matrix ply material systems are given in table 1.1. For comparative
purposes, table 1.2 gives typical material properties for several common engineering
metals. The properties presented in both tables should only be used within the
exercises of this book and for general comparison purposes. The material property
values presented in table 1.1 and table 1.2 should not be used for any actual design
purposes.

12
 Figure 1.2, Unidirectional Ply Material

Table 1.1, Typical Unidirectional Ply Material Properties (psi)

Property
Boron-Epoxy Carbon-Epoxy Glass-Epoxy Kevlar®-Epoxy
(psi)

E1 30.0e6 22.0e6 7.0e6 11.0e6

E2 2.90e6 1.30e6 2.0e6 0.80e6

ν12 0.26 0.30 0.25 0.34

ν23 n/a 0.26 n/a n/a

G12 0.90e6 0.75e6 1.0e6 0.30e6

α1 (ε/oF) 3.0e−6 −0.30e−6 3.0e−6 −2.0e−6

α2 (ε/oF) 16.0e−6 18.0e−6 12.0e−6 40.0e−6

ρ (lbs/in3) 0.072 0.056 0.065 0.052

Xt 190,000 170,000 150,000 200,000

Xc 380,000 170,000 150,000 38,000

Yt 10,000 6,500 4,500 3,000

Yc 35,000 28,000 18,000 15,000

S 14,000 10,000 8,000 6,000

*Note: Properties are typical properties only and should not be used for design purposes.

13
 Table 1.2, Typical Engineering Metal Material Properties (psi)
Property
Aluminum Steel Titanium
(psi)

E 10.0e6 29.0e6 16.0e6

ν 0.33 0.30 0.31

G 3.76e6 11.2e6 6.11e6

α (/oF) 12.0e−6 6.0e−6 5.0e−6

ρ (lbs/in3) 0.101 0.282 0.160

Ftu 60,000 125,000 130,000

Fty 45,000 100,000 120,000

*Note: Properties are typical properties only and should not be used for design purposes.

2D plain weave ply materials are made up of two unidirectional ply fibers woven into
each other with a “1-over-1-under” pattern embedded in a matrix material. Typical
2D plain weave ply thicknesses range from 0.01–0.015 inches with typical fiber
volumes between 0.40–0.65. 2D plain weave plies have reduced longitudinal stiffness
as compared to their equivalent unidirectional ply product forms. The reduced
stiffness is due to the undulation of the fibers that must be pulled taut, even though
they are embedded within a matrix material, before complete load-carrying capacity
can be achieved. Figure 1.3 shows a schematic of a 2D plain weave ply material.

14
 Figure 1.3, 2D Plain Weave Ply Material

2D 5-harness-satin (5HS) weave materials are made up of two unidirectional ply fibers
woven into each other with a “1-under-4-over” pattern embedded in a matrix
material. Typical 2D 5HS weave ply thicknesses range from 0.01−0.015 inches with
typical fiber volumes between 0.40−0.60. 2D 5HS weave plies are longitudinally stiffer
than their 2D plain weave ply counterparts. However, 2D 5HS weave plies still exhibit
a decrease in longitudinal stiffness as compared to their equivalent unidirectional ply
material. As can be seen from figure 1.4, which depicts a 2D 5HS weave ply material,
approximately 80% of the 2D 5HS weave ply is equivalent to two orthogonal
unidirectional plies. The remaining 20% of the 2D 5HS ply contains the undulations of
the fibers due to the weave pattern. Therefore, typical 2D 5HS weave plies exhibit
approximately 1% decrease in longitudinal stiffness as compared to their equivalent
unidirectional ply material. Furthermore, it is appropriate to model a 2D 5HS weave
ply material as two orthogonal unidirectional plies with the unidirectional longitudinal
stiffness, E1, reduced by 1% and the thickness of the unidirectional plies equal to ½
the total thickness of the 2D 5HS weave ply material.

15
 Figure 1.4, 2D 5HS Weave Ply Material

3D weaves are made up of unidirectional fibers woven in 3-dimensional patterns

embedded within a matrix material. 3D weaves come in many different thickness and
fiber volumes, and they are typically custom-made for specific purposes.

Core-Stiffened Laminated Composites

Core-stiffened composite laminates are made up of two laminated composite face
sheets separated by a core material. Typical core materials include aluminum
honeycomb, carbon honeycomb, and foam. The laminated composite face sheets can
be any of the laminated composite material types defined above. Figure 1.5 shows a
schematic of a honeycomb core-stiffened and a foam core-stiffened laminate
composite.

Figure 1.5, Honeycomb and Foam Core-Stiffened Composite Laminates

1.2 Material Terminology

Microscopic
Microscopic is a term used to describe physical objects smaller than can easily be seen
by the naked eye and which require a lens or microscope to see clearly.

16
Macroscopic
Macroscopic is a term used to describe physical objects that are measurable and
observable by the naked eye and do not require a lens or microscope to see clearly.

Micromechanics
Micromechanics is the study of composite material behavior wherein the interaction
of the constituent materials is examined in detail as part of the definition and behavior
of the heterogeneous composite material.

Macromechanics
Macromechanics is the study of composite material behavior wherein the material is
assumed homogeneous and the effects of the constituent materials are detected only
as averaged apparent properties, otherwise called effective properties, of the
composite material.

Homogeneous
A homogeneous body has uniform properties throughout; thus, the material
properties of the body are independent on the position within the body.

Heterogeneous
A heterogeneous body has non-uniform properties throughout; thus, the material
properties of the body are dependent on the position within the body.

Isotropic
An isotropic body has material properties that are the same in all directions at a given
point within a body; thus, the material properties are independent of orientation at a
specified point within the body.

Orthotropic
An orthotropic body has material properties that are the same in each of three
orthogonal planes at a given point within a body; thus, the material properties are
dependent on orientation at a specified point within the body.

17
Anisotropic
An anisotropic body has material properties that are different in all directions at a
given point within a body; thus, the material properties are dependent on orientation
at a specified point within the body.

1.3 Ply Conventions

In the case of fiber-matrix unidirectional composite plies, the material coordinate
system 1-axis defines the fiber direction, the material coordinate system 2-axis
defines the transverse matrix direction, and the material coordinate system 3-axis
defines the through-thickness direction of a ply. The fiber orientation of a ply, theta,
is defined relative to the global system x-axis using right-hand rule to define positive
theta as shown in figure 1.6.

Figure 1.6, Ply Conventions

1.4 Laminate Conventions and Definitions

To facilitate discussions on laminated composites, we must first define the laminate
stacking sequence and ply z-coordinate conventions that will be used throughout this
book. The laminate stacking sequence and ply z-coordinate conventions used in this
book are typical of the most popular FEA solvers. However, the conventions are not
necessarily consistent with those used in all FEA solvers. It is recommended that users
consult the specific FEA solver documentation for the laminate conventions used

18
within that solver. Chapter 10 gives the relevant laminate stacking sequence and ply
z-coordinate conventions for several popular solvers.

The global coordinate system of a homogeneous or laminated plate is defined in

figure 1.7. Note that the xy-plane defined by the global coordinate system goes
through the middle surface of the plate with the z-axis “down” as defined using right-
hand rule for the xy-plane as shown in figure 1.7. Assuming a laminated plate, the
laminate stacking sequence and ply z-coordinate conventions are also defined in
figure 1.7. Plies are numbered 1 through n with the 1st ply defined as the most
negative z ply and the nth ply as the most positive z ply. Plies stack in the positive z-
axis direction (plate normal) from ply 1 to ply n. In addition, the z-coordinate value
for the kth ply is always defined as the most positive z-coordinate interface for that
ply. The z-coordinate of a ply is measured relative to the middle surface of the plate.
Therefore, ply 1 through ply (n ∕ 2) − 1 will have negative z-coordinates. Likewise, ply
(n ∕ 2) to ply n will have positive z-coordinates. Since, by definition, there will always
be (n + 1) ply interfaces, the z0 coordinate is typically defined as –t ∕ 2 unless a laminate
offset is applied.

Fig 1.7: Laminated Plate Stacking Sequence and Z-coordinates

19
Defining Laminates
Laminates are typically specified in the engineering community using the following
notation:

[ply1 / ply2 / (ply3 / ply4)n / …/ ply n] n s

The subscript n defines the number of repeating units within its given brackets, and
the subscript s defines a laminate as a symmetric laminate. For symmetric laminates,
only the negative z-coordinate plies are specified, as the positive z-coordinate plies of
the laminate can be readily determined from the symmetric definition. In addition,
an underlined ply specifies the ply as being symmetric about ½ of the ply and is not
repeated on the other half of the laminate. An underlined ply allows for symmetric
laminate definitions containing an odd number of plies; otherwise, symmetric
laminates will always have an even number of plies.

Symmetric Laminates
A symmetric laminate is defined as a laminate that is composed of plies such that the
thickness, angle (theta), and material of the plies are symmetric about the middle
surface of the laminate. For symmetric laminates, the [B] matrix is zero and exhibits
no extensional–bending or shear–twisting coupling behaviors. Examples of
symmetric laminates using engineering notation, assuming all plies have the same
thickness and material, are given below.

[0/45/90/45/0], which can also be written as [0/45/90]s

[45/-45/90/0/0/90/−45/45], which can also be written as [45/−45/90/0]s

Anti-Symmetric Laminates
An anti-symmetric laminate is defined as a laminate for which every +θ ply and −θ ply
on the negative z-half of the laminate, there exist a −θ ply and +θ ply respectively on
the positive z-half of the laminate with the same thickness and material at the same
stacking sequence location. In addition, 0 plies and 90 plies must be symmetric about

20
the middle surface of the laminate. Examples of anti-symmetric laminates using
engineering notation, assuming all plies have the same thickness and material, are
given below.

[0/90/−45/45/90/0]

[0/45/90/−45/45/90/−45/0]

Balanced Laminates
A balanced laminate is defined as a laminate for which every +θ ply there exists a −θ
ply of the same thickness and material. The definition of a balanced laminate does
not define where in the laminate stacking sequence the plies exist, just that there are
the same number of +θ plies and −θ plies in total for the laminate. Balanced laminates
have zero A14 and A24 components and exhibit no extensional–shear coupling
behavior. In addition, if a balanced laminate is also anti-symmetric, then the laminate
will additionally have zero D14 and D24 components and will also not exhibit bending-
twisting coupling behavior. Examples of balanced laminates using engineering
notation, assuming all plies have the same thickness and material, are given below.

[45/−45/−30/30]

[22.5/−22.5/90/−22.5/22.5]

Cross-Ply Laminates
A cross-ply laminate is defined as a laminate composed of only 0 plies and 90 plies of
the same thickness and material. Cross-ply laminates have zero A14, A24, D14, and D24
components and exhibit no extensional-shear or bending-twisting coupling behaviors.
In addition, if a cross-ply laminate is symmetric, then the laminate will additionally
have a zero [B] matrix and exhibit no extensional-bending or shear-twisting coupling
behaviors. Examples of cross-ply laminates using engineering notation, assuming all
plies have the same thickness and material, are given below.

[0/90/0/90/0]

[0/0/90/90/0/0/90]s

21
Angle-Ply Laminates
An angle-ply laminate is defined as a laminate composed of only +θ plies and −θ plies
of the same thickness and material. In general, angle-ply laminates have fully
populated [A], [B], and [D] matrices. However, if an angle-ply laminate is balanced,
then the laminate will have zero A14 and A24 components and exhibit no extensional-
shear coupling behavior. In addition, if an angle-ply laminate is symmetric, then the
laminate will additionally have a zero [B] matrix and exhibit no extensional-bending
or shear-twisting coupling behaviors. Examples of angle-ply laminates using
engineering notation, assuming all plies have the same thickness and material, are
given below.

[45/−45/−30/30]

[−30/30/60/30/−30]

General Laminates
A general laminate is defined as a laminate that does not fall into any of the previous
laminate definitions. General laminates generally exhibit fully populated [A], [B], and
[D] matrices, and therefore all types of coupling typically exist; extension-shear
coupling (A14 and A24 terms), extension-bending coupling ([B] matrix terms), shear-
twisting coupling ([B] matrix terms), and bending-twisting coupling (D14 and D24
terms).

Examples of general laminates using engineering notation, assuming all plies have the
same thickness and material, are given below.

[0/45/90/22.5/0/45]

[90/−45/0/90/−45/0]

22
1.5 Common Advantages and Drawbacks of
Composite Design
Why use composites for creating structural components?

• The material property of the composites can be engineered as per the application
requirements.
• The ability to impart the required material property gives them great advantage
when compared with traditional homogeneous materials like steel or aluminum.
• Composites have increased strength to weight ratios in use cases against isotropic
metals

For these reasons, applications like aerospace components, where the weight is a
decisive factor, can benefit tremendously with the usage of composite materials

Drawbacks

Laminate composite structures, such as glass fiber and carbon fiber, come with:

• Higher cost
• Limited supply of raw materials
• Complex manufacturing needs

23
24
 2 Basics of Composite
Analysis

2.1 Composite Designable Material Properties

Take the following problem:
A simple square steel plate in tension needs to have displacement of 0.1 in x-direction.

• Designing for above requirement is a simple task

• What is the associated displacement on the part for the same loading in the y-
direction?

Fig 2.1: A Square Steel Plate in Tension.

What if the displacement in the y-direction needs to be no more than 0.025 units?

Using isotropic vs orthotropic materials provide different approaches to this design

problem

• Steel, being an isotropic material, cannot change its properties in different

directions. Hence different behavior in different directions needs to be achieved
by changing the geometry.
• In case of composites, achieving the above is as simple as determining the correct
number of plies in x and y directions.

25
• Ability to design the material property gives lot of freedom to the designers but
increases the complexity of the design task.
• Note that Orthotropic designs must take into account undesirable behaviors like
extensional–shear coupling, bending-twist coupling, etc.

2.2 Understanding Composite Material Properties

Unlike Isotropic structures, laminated parts are generally modelled as orthotropic
materials, thus the stress-strain relationship is different from the isotropic stress-
strain matrix. Generally, any two engineering material constants are sufficient for
isotropic materials and these are independent of direction. But for orthotropic
materials this is not the case.

The stress-strain relationship for orthotropic materials can be written as (Eon 2.1):

…. 2.1

The orthotropic strain-stress relationship for plane stress conditions can be further
reduced, as (Eqn 2.2):

…… 2.2

Therefore, at least five constants are required for orthotropic materials.

The constitutive stress/strain relationship is written in the principal material 1-, 2-, 3-
coordinate system as (Eqn 2.3):

…… 2.3

26
To determine the global behavior of a ply, this relationship is transformed to the
global x-, y-, z- coordinate system (Eqn 2.4), using the 2D plane stress transformations:

….. 2.4

Where (Eqn 2.5) is the stiffness matrix in the global coordinate

system.

Here are the transformation equations “filled out”:

…… 2.5

The xy-plane defined by the global coordinate system goes through the middle surface
of the plate with z-axis defined using right hand rule. The 1st ply is always defined as
the most negative z-ply

27
 Fig 2.3: Ply distance from mid-plane
For a homogenous single ply plate of constant thickness, the mid-plane forces can be
written in terms of stress variation through the thickness of the plate as (Eqn 2.6):

…… 2.6

For a laminated plate made up of ‘n’ constant thickness plies the mid-plane forces can
be written in terms of the sum of the stress variation through the thickness of each
ply as (Eqn 2.7):

28
 ……. 2.7

For a homogenous single ply plate of constant thickness, the mid-plane moments can
be written in terms of stress variation through the thickness of the plate as (Eqn 2.8):

……. 2.8

For a laminated plate made up of ‘n’ constant thickness plies the mid-plane moments
can be written in terms of the sum of the stress variation through the thickness of
each ply as (Eqn 2.9):

……. 2.9

By adding the subscript “k” to designate the equation on the laminated coordinates
for each ply the general stress-strain relationship becomes (Eqn 2.10),

……. 2.10

Substituting the above into the equation 2.6 for mid-plane forces, it is shown:

29
 ……. 2.11

……. 2.12

Similarly, for mid-plane moments:

zk

{M x } = ∑ ∫ ([Q ]k ({ε x } + z {k } − {α } ∆T ))zdz

n
o
k k k x k ……. 2.13
k =1 z k −1

OR

{M x } = [B ]{ε x o }+ [D]{k }− {M }
x
T
x
……. 2.14

Where:

[A] = ∑ ([Q ]k (zk − zk −1 ))

n

……. 2.15
k =1

[B ] = 1 ∑ ([Q ] k (zk2 − zk2−1 ))

n

2 ……. 2.16
k =1

[D ] = 1 ∑ ([Q ]k (zk3 − zk3−1 ))

n
……. 2.17
3 k =1

2.3 The [A] [B] [D] Matrix

The definition of the relationship between the mid-plane generalized forces and strain
can be written as (Eqn 2.18):

……. 2.18

The [A], [B] and [D] matrices in the above relation have a lot of significance in
designing the laminates of a composite structure

30
By looking at these matrices the designer can determine:

• Various behaviors, such as whether the laminate is balanced

• The nature of any coupling(s) between extension, shear, bending, twisting etc.
• The [A] matrix relates mid-plane forces to mid-plane strains defining the
extensional behavior of the laminate
• The [B] matrix relates mid-plane forces to plate curvatures and mid-plane
moments to mid-plane strains.
• The [D] matrix relates mid-plane moments to plate curvatures defining the
bending behavior of the laminate

2.4 Failure Theories of Composite Lamina

A design of a structure is successful when the materials are used efficiently and the
structure is safe. Failure theories are developed to compare the stresses in the
material with the failure criteria. Failure criteria are usually the yield and ultimate
strength/point of the material. For a brittle material failure point is the ultimate point
in stress-strain curve; whereas, for ductile material failure point is the yield point in
the stress-strain curve.

None of the failure criteria used for isotropic materials can be used to predict the
failure of the composite lamina. Because, the weakest plane of the lamina may not be
aligned in the “principal stresses” direction. Therefore, the principal stresses concept
is used very less in the case of composite materials. Hence, several failure theories are
developed separately for composites. Related failure theories for composites are
discussed below.

2.4.1 Maximum Stress Theory

This theory is similar to maximum normal stress theory by Rankine and maximum
shear stress theory by Tresca, applied for isotropic materials. According to this theory
the stresses in the lamina are resolved to normal and shear stresses in the local axes
and predict the failure modes of a composite lamina by comparing the individual
stresses with respect to their ultimate stress, i.e. if any one of the normal or shear

31
stresses of a lamina is equal to or exceeds the corresponding ultimate stress, then the
lamina is said to fail.

Following are the few strength parameters used in this theory:

 For unidirectional lamina

• Ultimate Longitudinal tensile stress, (𝝈𝝈𝑻𝑻𝟏𝟏 )𝒖𝒖𝒖𝒖𝒖𝒖
• Ultimate Longitudinal compressive stress, (𝝈𝝈𝑪𝑪𝟏𝟏 )𝒖𝒖𝒖𝒖𝒖𝒖
• Ultimate Transverse tensile stress, (𝝈𝝈𝑻𝑻𝟐𝟐 )𝒖𝒖𝒖𝒖𝒖𝒖
• Ultimate Transverse compressive stress, (𝝈𝝈𝑪𝑪𝟐𝟐 )𝒖𝒖𝒖𝒖𝒖𝒖
• Ultimate In-plane shear stress, (𝝉𝝉𝟏𝟏𝟏𝟏 )𝒖𝒖𝒖𝒖𝒖𝒖

𝜎𝜎2
𝜏𝜏

𝜎𝜎1 𝜎𝜎1

𝜏𝜏
𝜎𝜎2

The lamina is considered to be failed if any of the following equations 2.19 are violated

−(𝝈𝝈𝒄𝒄𝟏𝟏 )𝒖𝒖𝒖𝒖𝒖𝒖 < 𝝈𝝈𝟏𝟏 < (𝝈𝝈𝑻𝑻𝟏𝟏 )𝒖𝒖𝒖𝒖𝒖𝒖, or

−(𝝈𝝈𝒄𝒄𝟐𝟐 )𝒖𝒖𝒖𝒖𝒖𝒖 < 𝝈𝝈𝟐𝟐 < (𝝈𝝈𝑻𝑻𝟐𝟐 )𝒖𝒖𝒖𝒖𝒖𝒖, or ……. 2.19

−(𝝉𝝉𝟏𝟏𝟏𝟏 )𝒖𝒖𝒖𝒖𝒖𝒖 < 𝝉𝝉𝟏𝟏𝟏𝟏 < (𝝉𝝉𝟏𝟏𝟏𝟏 )𝒖𝒖𝒖𝒖𝒖𝒖

Note*: All the strength parameters are treated as positive, normal stresses are positive
if tensile and negative if compressive.

32
2.4.2 Maximum Strain Theory
This theory is similar to St. Venant’s maximum normal strain and Tresca’s maximum
shear stress theory applied for isotropic materials. According to this theory the strains
in the lamina are resolved to the local axes and the failure modes of a composite
lamina are predicted by comparing the individual strains with respect to their ultimate
strains, i.e. if any one of the normal or shear strains of a lamina is equal to or exceeds
the corresponding ultimate strain, then the lamina is said to fail.

Following are the few strength parameters used in this theory:

 For unidirectional lamina

• Ultimate Longitudinal tensile strain, (𝜺𝜺𝑻𝑻𝟏𝟏 )𝒖𝒖𝒖𝒖𝒖𝒖
• Ultimate Longitudinal compressive strain, (𝜺𝜺𝑪𝑪𝟏𝟏 )𝒖𝒖𝒖𝒖𝒖𝒖
• Ultimate Transverse tensile strain, (𝜺𝜺𝑻𝑻𝟐𝟐 )𝒖𝒖𝒖𝒖𝒖𝒖
• Ultimate Transverse compressive strain, (𝜺𝜺𝑪𝑪𝟐𝟐 )𝒖𝒖𝒖𝒖𝒖𝒖
• Ultimate In-plane shear strain, (𝜸𝜸𝟏𝟏𝟏𝟏 )𝒖𝒖𝒖𝒖𝒖𝒖

The lamina is considered to be failed if any of the following equations 2.20 are violated

−(𝜺𝜺𝒄𝒄𝟏𝟏 )𝒖𝒖𝒖𝒖𝒖𝒖 < 𝜺𝜺𝟏𝟏 < (𝜺𝜺𝑻𝑻𝟏𝟏 )𝒖𝒖𝒖𝒖𝒖𝒖 , or

−(𝜺𝜺𝒄𝒄𝟐𝟐 )𝒖𝒖𝒖𝒖𝒖𝒖 < 𝜺𝜺𝟐𝟐 < (𝜺𝜺𝑻𝑻𝟐𝟐 )𝒖𝒖𝒖𝒖𝒖𝒖 , or ……. 2.20

−(𝜸𝜸𝟏𝟏𝟏𝟏 )𝒖𝒖𝒖𝒖𝒖𝒖 < 𝜸𝜸𝟏𝟏𝟏𝟏 < (𝜸𝜸𝟏𝟏𝟏𝟏 )𝒖𝒖𝒖𝒖𝒖𝒖

Note*: All the strength parameters are treated as positive, normal strains are positive
if tensile and negative if compressive.

33
2.4.3 Tsai-Hill Failure Theory
This theory is based on the Von-Mises distortional energy yield criterion for isotropic
material as anisotropic materials. Distortion energy is a total strain energy in the body.
Material is assumed to fail when the distortion energy exceeds the yield
point/strength of the material. Hill adopted the Von- Mises’ distortional energy yield
criterion to anisotropic materials. Then, Tsai adapted it to a unidirectional lamina. This
theory is popularly used in composite analysis. In this theory stresses are calculated
in the material direction on layer by layer basis.
Material is said to fail if it satisfies the following equation 2.21

(𝝈𝝈𝟏𝟏 ⁄𝑭𝑭𝟏𝟏 )𝟐𝟐 + (𝝈𝝈𝟐𝟐 ⁄𝑭𝑭𝟐𝟐 )𝟐𝟐 + (𝝉𝝉𝟏𝟏𝟏𝟏 ⁄𝑭𝑭𝟔𝟔 )𝟐𝟐 − (𝝈𝝈𝟏𝟏 𝝈𝝈𝟐𝟐 ⁄𝑭𝑭𝟏𝟏 )𝟐𝟐 > 𝟏𝟏 ……. 2.21

where,

𝑭𝑭𝟏𝟏 = (𝝈𝝈𝑻𝑻𝟏𝟏 )𝒖𝒖𝒖𝒖𝒖𝒖 if, 𝝈𝝈𝟏𝟏 > 𝟎𝟎.

𝑭𝑭𝟏𝟏 = (𝝈𝝈𝑪𝑪𝟏𝟏 )𝒖𝒖𝒖𝒖𝒖𝒖 if, 𝝈𝝈𝟏𝟏 < 𝟎𝟎.

𝑭𝑭𝟐𝟐 = (𝝈𝝈𝑻𝑻𝟐𝟐 )𝒖𝒖𝒖𝒖𝒖𝒖 if, 𝝈𝝈𝟐𝟐 > 𝟎𝟎.

𝑭𝑭𝟐𝟐 = (𝝈𝝈𝑪𝑪𝟐𝟐 )𝒖𝒖𝒖𝒖𝒖𝒖 if, 𝝈𝝈𝟐𝟐 < 𝟎𝟎.

𝑭𝑭𝟔𝟔 = (𝝉𝝉𝟏𝟏𝟏𝟏 )𝒖𝒖𝒖𝒖𝒖𝒖

There are other different failure mode theories which are used to predict the failure
of composite structures. These theories provide distinct criteria for failure matrix,
fiber and interface. Puck and Hashim-Rotem failure theories are examples of such
theories.

34
 3 Composite Modeling in
OptiStruct
This Chapter contains contents from Jeffrey A. Wollschlager’s “Introduction to the
Design and Analysis of Composite Structures” book. (Grey texts)

3.1 Composite Pre-Processing

Modeling laminate composites for FEA requires more information than isotropic
parts:
• Part Geometry
• Ply Geometry
• Material Data
• Mesh Data
• Material Alignment Information
• Lay-up sequence
• Z-Offset Information
• Drape Information

Which of these must be created while pre-processing depends on how much of this
information is available in the input data.

Composites can be modeled using both Shell and solid elements. At least one layer of
solid elements should be modeled when modelling with solids. This ends up to be a
huge number of elements. Majority of parts are modeled with shell elements instead
of solids. Analysis of composite shells is very like the solution of standard shell
elements. In OptiStruct, shell elements are assigned with PCOMP, PCOMPG or
PCOMPP and solid elements are assigned with PSOLID. Composite materials are
modeled with orthotropic material models. MAT8 is the commonly used orthotropic
material model for shells and MAT9 or MAT9ORT for solids.

Modeling composites in the HyperMesh Desktop interface is mostly done through the
Model Browser and the Entity Editor

35
Model Browser
• The Model View in the Model Browser is enabled by default
• A tree-structure of each type of entity in the model is shown
• New model entities may be created by right-clicking in the open area
• Right-clicking a model entity shows a context-sensitive menu for modifying that
entry

Entity Editor
• Provides detailed information about the selected entry in the Model Browser
• Offers easy editing and manipulation of fields in each card
• Links to tools, panels, and dialog boxes to enhance the creation and linking of
entities

Fig 3.1: snapshot of Model and entity browser

36
3.2 Composite Material Types

The following are most commonly used orthotropic material types in OptiStruct:

 MAT8

This is used to define the material properties for linear temperature-independent

orthotropic material for two-dimensional elements. The MAT8 card is most
commonly used to represent planar orthotropic material for composites

Where:

Fig 3.2: snapshot of MAT 8 card used in HyperMesh for OptiStruct

solver
The above bulk data card entries directly correspond to that of the following matrices
(Eqn 3.1 and 3.2):

37
 ……. 3.1

……. 3.2

 MAT2

This is used to define the material properties for linear temperature-independent and
anisotropic material for two-dimensional elements

Where:

Fig 3.3: snapshot of MAT2 card used in HyperMesh for OptiStruct solver

 MAT1

This is used to define the material properties for linear temperature independent
isotropic material for two dimensional elements

38
Where:

Fig 3.4: snapshot of MAT1 card used in HyperMesh for OptiStruct solver

3.3 Material and Element Orientation

Orthotropic materials are directionally dependent i.e., material properties are not the
same in all three directions. Consider a sample material property which is defined as:

E1 = 1.3e5 MPa E2 = E3 = 9650 MPa

u12 = u13 = 0.3 u23 = 0.6
G12 = G13 = 3450 MPa G23 = 3100 MPa
E1 is much stronger than E2.
By default, the orientation considered is element orientation which is dependent on
node numbering. All elements may not have same orientation and the element
coordinate system is always defined by the bi-section of vectors from G1-G3 and G2-
G4.

39
Material Orientation by default (based on Material Orientation by specifying

element node numbering) material orientation angle 90o

Fig 3.5: Image showing material orientations with and without material
orientation system
Using local coordinate system, one can specify E1 and E2 directions for orthotropic
materials. This system defines the material direction and hence it is called Material
system or one can define element material orientation for individual elements
independently within each element as an angle rotated by THETA degrees from the x-
axis of the element coordinate system.

Fig 3.6: Image showing element orientation using angle

The X-direction of material system is considered as E1 direction or 0o of the fiber.
Similarly, Y-direction of material system is considered as E2 direction or 90o of the

40
fiber. This material system will provide reference to ply angle definition. Note that
element coordinate system and material coordinate system are not the same.

Fig 3.7: Image showing alignment of element orientation using local

system
Here using a local coordinate system, X -direction is defined through MCID for
individual elements. One can assign or map the material coordinate system to
elements in HyperMesh using 2D Composite module.

3.4 Types of Laminate in HyperMesh - OptiStruct

A laminate is a stack of plies stacked in the direction of the element normal.

Fig 3.8: Image illustrating how laminate is stacked

In HyperMesh, Laminate entities are used to define laminates, which make up a
laminated structure by defining the stacking sequence of ply entities.

41
Ply Laminates

Ply laminates are used to define laminates which make up flat or slightly curved
laminated structures. Ply laminates stack ply entities.

Sub-laminate

Sub-laminates are very like ply laminates in that they also stack ply entities. However,
they define only a portion of a laminate to be used as components of an interface
laminate structure. However, the ply order defined within a sub-laminate must
remain in the defined order. The exact stacking sequence of the plies of the sub-
laminates may need to be created according to the interface definitions within an
interface laminate

Interface Laminate
Interface laminates are used to define laminates which make up complex laminated
structures that “wrap around” corners. Interface laminates stack sub-laminates. The
stack direction for the sub-laminates of an interface laminate is in the direction of the
element's normal. An interface definition defines which “surface” plies of two sub-
laminates touch, or interface, with each other. Each sub-laminate stacked within an
interface laminate must have at least one interface definition.

Fig 3.9: Image illustrating use of interface for creating laminate with sub-laminates

42
Creating a laminate from shell elements requires creating property cards to define the
ply and sequence information. There are 3 main types of property cards to choose,
for creating shell laminate properties:

• PCOMPP: Composite Laminate Property

• PCOMPG: Composite Laminate Property allowing for global ply identification
• PCOMP: Composite Laminate Property

PCOMP and PCOMP (G) are zone based properties used for modelling zone based
laminates whereas PCOMPP is a ply based modelling property.

3.5 Different Composite Modeling Methods

In general, there are three different composite modeling methods; zone-based shell
modeling, ply-based shell modeling, and ply-by-ply solid modeling.

i. Composite Zone-Based Shell Modeling

Composite shell zone-based modeling is the traditional approach to building
composite models. It requires a property definition for each laminate zone within a
composite structure. Therefore, at each ply drop or addition location, another
laminate zone property definition must be defined. Each laminate zone property
definition must completely define the laminate within that laminate zone. Plies that
extend through multiple laminate zones must be redefined in each laminate zone
property definition. The duplication of ply data within each laminate zone property
definition causes inefficient data handling and ultimately necessitated the need for
developing an alternative composite modeling approach. This lead to the composite
shell ply-based modeling approach discussed next.

The general process to develop a composite zone-based shell model for the design
and analysis of composite structures is described in this section. The modeling
procedures discussed are generally generic to all finite element solvers, however we
will be explicitly developing models using the finite element solver OptiStruct.

43
1. Create shell elements by generating a finite element mesh using a suitable finite
element pre-processor (Altair HyperMesh). Composite shell elements are defined
in OptiStruct through the GRID, CTRIA3, and CQUAD4 bulk data cards.

2. Assign element normal. An element normal defines the laminate stacking

sequence direction for a given element. The laminate stacking sequence is given
as the order in which the plies are defined within a laminate zone property
definition. Typically ply 1 is the first ply defined and ply n is the last ply defined
within a laminate zone property definition. Plies stack in the direction of the
element normal from ply 1 to ply n. Therefore, defining the element normal
correctly is of critical importance. It is recommended that users consult the
specific solver documentation for the element normal conventions used within
that solver.

Fig 3.10: Zone-Based Element Normal and Stacking Sequence Definitions

3. Assign element material coordinate system. The element material coordinate

system x-axis defines the direction of a 0o ply for an element. Furthermore, the
ply fiber direction θk, defined for each kth ply within a laminate zone property
definition, is always relative to the element material coordinate system x-axis as

44
 shown in figure 3.11. There are several methods for defining the element
material coordinate system for various finite element analysis solvers. However,
most solvers define the element material coordinate system x-axis as an angle θ
from the G1-G2 vector about the element normal as shown in figure 3.11. It is
recommended that users consult the specific solver documentation for the
element material coordinate system conventions used within that solver.

Fig 3.11: Zone-Based Element Material System and Ply Orientation

4. Create homogeneous ply materials for each unique ply material that is utilized
within the laminates that make up the composite structure. In general, most
solvers support the creation of plane stress isotropic, transversely isotropic, and
orthotropic homogeneous ply materials. Homogeneous ply materials are defined
in OptiStruct through the MAT1 (isotropic), MAT2 (anisotropic), or MAT8
(orthotropic) bulk data cards.

5. Create laminate zone property definition for each laminate zone of the
composite structure. A laminate zone is a constant thickness zone of the
laminate. Laminate zone boundaries are defined by ply shape boundaries. At
each ply shape boundary, a new laminate constant thickness zone must exist.
Laminate zones are defined as properties in most finite element analysis solvers.
The laminate stacking sequence within a laminate zone is given as the order in
which the plies are defined within the laminate zone property definition. Typically
ply 1 is the first ply defined and ply n is the last ply defined within a laminate zone

45
 property definition. Plies stack in the direction of the element normal from ply 1
to ply n. See figure 3.12 for a schematic of a laminate zone property stacking
sequence definition. For each ply defined in a laminate zone property definition,
the following ply data is typically required;

• Ply global identification number, GPLYID filed on the PCOMPG bulk data card
defines a unique id for each ply.
• Ply material identification number, MID field on the PCOMPG bulk data card
defines the plane stress stiffness matrix in the material coordinate system [Q]
for the ply.
• Ply thickness, tk field on the PCOMPG bulk data card.
• Ply fiber direction, θk field on the PCOMPG bulk data card. The ply fiber
direction is always relative to the element material coordinate system x-axis
as defined in figure 3.11.
• Ply results, SOUT field on the PCOMPG bulk data card determines whether to
calculate and output results for the ply or not.

Laminate zone properties are defined in OptiStruct through the PCOMP and
PCOMPG bulk data cards. It is generally recommended to use the PCOMPG bulk
data card over the PCOMP bulk data card.

6. Assign laminate zone properties to the elements that represent the laminate
zones defined by the laminate zone property definitions. This process assigns an
element stiffness matrix, in this case the ABD matrix of the laminate zone that the
element is within. Laminate zone properties are assigned to elements in
OptiStruct through the PID field on the CTRIA3 or CQUAD4 bulk data cards.

7. Create boundary conditions applied to the composite model that simulate the in-
situ environments under investigation.

• Constraints are defined in OptiStruct through the SPC bulk data card.

46
 • Forces and Moments are defined in OptiStruct through the FORCE and
MOMENT bulk data cards respectively.
• Pressures on shell elements are defined in OptiStruct through the PLOAD2
bulk data card.
• Initial and Model temperature distributions are defined in OptiStruct through
the TEMP or TEMPD bulk data cards.

8. Create load steps for each load case that the composite model is to be analyzed
for by combining appropriate boundary conditions that simulate the in-situ
environments of the composite structure under investigation. Load steps are
defined in OptiStruct through the SUBCASE, ANALYSIS, TITLE, SPC, LOAD, and
TEMPERATURE(LOAD) subcase control cards.

9. Create control cards to define initial temperatures, output results, output

formats, and solver controls.
• The initial temperature distribution is defined in OptiStruct through the
TEMPERATURE(INITIAL) subcase control card.
• Displacement output is defined in OptiStruct through the DISPLACEMENT i/o
options card.
• Composite ply-level strain output is defined in OptiStruct through the
CSTRAIN i/o options card. If thermal boundary conditions are applied, then it
is important to request ply-level mechanical strain output using the MECH
option on the CSTRAIN i/o options card.
• Composite ply-level stress output is defined in OptiStruct through the
CSTRESS i/o options card.
• Composite ply-level failure index output is defined in OptiStruct through the
SB and FT fields on the PCOMP or PCOMPG bulk data cards. CFAILURE i/o
Control card is used.
• Output file formats are defined in OptiStruct through the OUPTUT i/o options
card. Typically, H3D (binary file for post-processing in Altair HyperView) and
ASCII (text file) file formats are requested.

47
10. Export the solver input file representing the composite analysis model from the
pre-processor (HyperMesh) and solve the composite analysis by submitting the
solver input file to the solver executable (OptiStruct).

11. Post-process the composite analysis results. The most important results for
composite models are the ply-level mechanical strains and stresses in the material
coordinate system. Note that the mechanical strain tensors must be used
whenever there is a thermal boundary condition applied. If there is no thermal
boundary condition applied, then the mechanical strain tensor is equivalent to
the total strain tensor and the default output from most solvers can be used
directly.

ii. Composite Ply-Based Shell Modeling

Composite shell ply-based modeling is a relatively new technique for building
composite models that attempts to mimic the composite manufacturing process of
cutting and stacking plies “on top” of each other to construct a composite structure.
In the composite ply-based modeling approach, plies are defined as physical entities
of a given material with thickness and shape. Plies are then stacked “on top” of each
other in a specified order. In this way, a ply is defined only once. In addition, since
the ply shape for all plies are known, the laminate zones are automatically derived.
The principal advantage of ply-based modeling is the ability to easily make design
updates to composite models via addition and subtraction of plies and modification
of ply shapes, which automatically recalculates the laminate zones for the composite
model.

The general process to develop a composite ply-based shell model for the design and
analysis of composite structures is described in this section. The modeling procedures
discussed are generic to all finite element solvers, however we will be explicitly
developing models using the finite element solver OptiStruct.

48
1. Create shell elements by generating a finite element mesh using a suitable finite
element pre-processor (Altair HyperMesh). Composite shell elements are
defined in OptiStruct through the GRID, CTRIA3, and CQUAD4 bulk data cards.

2. Assign element normal. An element normal defines the laminate stacking

sequence direction for a given element. The laminate stacking sequence is given
as the order in which the plies are defined within a laminate zone property
definition. Typically ply 1 is the first ply defined and ply n is the last ply defined
within a laminate zone property definition. Plies stack in the direction of the
element normal from ply 1 to ply n. An element normal is defined in OptiStruct
by the order of the grids on the CTRIA3 and CQUAD4 bulk data cards.

Fig 3.12: Ply-Based Element Normal and Stacking Sequence Definitions

3. Assign element material coordinate system. The element material coordinate
system x-axis defines the direction of a 0o ply for an element. Furthermore, the
ply nominal fiber direction θk, defined for each kth ply, is always relative to the
element material coordinate system x-axis as shown in figure 3.13. Also, the ply
actual fiber direction θi, defined for each element of the ply shape, is always
relative to the nominal fiber direction and defines the actual fiber direction for
the ith element of the kth ply. There are several methods for defining the element
material coordinate system for various finite element analysis solvers. However,

49
 most solvers define the element material coordinate system x-axis as an angle θ
from the G1-G2 vector about the element normal as shown in figure 3.13. An
element material coordinate system is defined in OptiStruct through the θ field
on the CTRIA3 or CQUAD4 bulk data cards.

Fig 3.13: Ply-Based Element Material System and Ply Orientation

4. Create homogeneous ply materials for each unique ply material that is utilized
within the laminates that make up the composite structure. In general, most
solvers support the creation of plane stress isotropic, transversely isotropic, and
orthotropic homogeneous ply materials. Homogeneous ply materials are defined
in OptiStruct through the MAT1 (isotropic), MAT2 (anisotropic), or MAT8
(orthotropic) bulk data cards.

5. Create plies that make up the composite structure. The principal difference
between a ply and a ply definition within a laminate zone property definition of
zone-based shell modeling is that a ply additionally defines the ply shape along
with the ply data of material, thickness, and fiber direction. It is the ply shape
data that is the critical piece of data that allows for the automatic calculation of
the composite laminate zones. By defining a ply in this way, building composite
models is exactly analogous to the composite structures manufacturing process

50
 where a ply is cut to shape and then stacked to build up a laminated composite
structure. For each ply the following ply data is typically required;

• Ply material identification number, MID field on the PLY bulk data card defines
the plane stress stiffness matrix in the material coordinate system [Q] for the
ply.
• Ply thickness, tk field on the PLY bulk data card.
• Ply nominal fiber direction, θk field on the PLY bulk data card. The ply fiber
direction is always relative to the element material coordinate system x-axis
as defined in figure 3.13.
• Ply actual fiber direction, θi field defined on the DRAPE bulk data card for each
element of the ply shape. The DID field on the PLY bulk data card references
the drape table which defines the actual fiber directions for each element of
the ply. The ply actual fiber direction is always relative to the ply nominal
fiber direction as defined in figure 3.13. Typically, the ply actual fiber
direction θi is used to interface with draping solvers and obtain more accurate
fiber directions for the ply as it is actually manufactured on the final part.
• Ply results, SOUT field on the PLY bulk data card determines whether or not
to calculate and output results for the ply.
• Ply shape. The ply shape is typically defined by a set of elements that
represent the actual ply shape on the mesh of the composite structure and is
defined by the ESID field on the PLY bulk data card.

It is recommended that users consult the OptiStruct solver documentation for the
ply definitions used within. Plies are defined in OptiStruct through the PLY bulk
data card. The actual fiber orientation angle for a ply is defined in OptiStruct
through the DRAPE bulk data card.

6. Create laminates by stacking plies in a given stacking sequence order. Typically

ply 1 is the first ply defined and ply n is the last ply defined within a stack
definition. Plies stack in the direction of the element normal from ply 1 to ply n

51
 as shown in figure 3.12. Laminates are defined in OptiStruct through the STACK
bulk data card.
7. Create ply-based properties. In zone-based composite modeling, a laminated
zone property definition defines a laminate zone. On assignment of a laminated
zone property definition to an element, the element stiffness matrix is completely
defined. However, in the case of ply-based modeling, a ply-based property is
simply a template property defining element level laminate property definitions,
such as element offset defined by Z0 on the PCOMPP bulk data card. Assignment
of a ply-based property to an element “tags” the element as having a ply-based
laminate definition. Elements actual property is then automatically resolved from
the ply and stack definitions that are defined by the PLY and STACK bulk data cards
above. Ply-based properties are defined in OptiStruct through the PCOMPP bulk
data card.

Repeat step 8 to 13.

8. Assign ply-based properties to the elements

9. Create boundary

10. Create load steps

11. Create control cards

12. Export the solver input file Post-process the composite analysis results.

13. Post-process the composite analysis results

At first glance, it may appear that the composite ply-based modeling method is
more cumbersome than the composite zone-based modeling method based solely on
the number of steps required to build the composite models between the two
methods. However, upon modification of any composites model, due to a design

52
update, the efficiency of the composite ply-based modeling techniques become
readily apparent. In addition, composite ply-based modeling techniques have
significant advantages for composite design optimization.

iii. Composite Ply-by-Ply Solid Modeling

Composite ply-by-ply solid modeling is the most accurate modeling technique and is
the only method which can accurately capture through-thickness effects. However,
ply-by-ply solid modeling requires a solid layer of elements for each ply. ply-by-ply
solid models are still commonly developed for the design and analysis of composite
structural joints.

1. Create solid elements by generating a finite element mesh for each ply using a
suitable finite element pre-processor (Altair HyperMesh). A layer of solid
elements is required for each ply. Composite solid elements are defined in
OptiStruct through the GRID, CPENTA, and CHEXA bulk data cards.

2. Create a material coordinate system for each unique ply fiber direction. The ply
fiber 1-direction is always the material coordinate system x-axis for a rectangular
coordinate system. The ply matrix 2-direction is always the material coordinate
system y-axis for a rectangular coordinate system. Finally, the ply through-
thickness 3-direction is always the material coordinate system z-axis for a
rectangular coordinate system. Material coordinate systems are defined in
OptiStruct with the COORD1R or CORD2R bulk data cards.

Fig 3.14: Solid Element Material Coordinate System Definition

53
3. Create a homogeneous solid ply material for each unique ply material that is
utilized within the laminates that make up the composite structure. In general,
most solvers support the creation of isotropic, transversely isotropic, and
orthotropic homogeneous ply materials. Homogeneous ply materials are defined
in OptiStruct through the MAT1 (isotropic), MAT9ORT (orthotropic), or MAT9
(anisotropic) bulk data cards.

4. Create a solid ply property definition for each ply of the composite structure. Ply
properties are defined in OptiStruct through the PSOLID bulk data card. For each
ply the following solid ply property data is typically required;
• Ply material identification number, MID field on the PSOLID bulk data card
defines the stiffness matrix in the material coordinate system for the ply.
• Ply fiber direction, CORDM field on the PSOLID bulk data card which
references a material coordinate system definition.

5. Assign solid ply properties to the elements that represent the ply. This process
assigns an element its stiffness matrix through the PID field on the CPENTA or
CHEXA bulk data cards.

6. Create boundary conditions applied to the composite model that simulate the in-
situ environments under investigation.

• Constraints are defined in OptiStruct through the SPC bulk data card.
• Forces and Moments are defined in OptiStruct through the FORCE and
MOMENT bulk data cards respectively.
• Pressures on solid element faces are defined in OptiStruct through the
PLOAD4 bulk data card.
• Initial and Model temperature distributions are defined in OptiStruct through
the TEMP or TEMPD bulk data cards.

7. Create load steps

8. Create control cards

54
9. Export the solver input file

10. Post-process the composite analysis results.

3.6 Zone based Vs Ply based

For a zone based model, the part/model is divided into several zones and each
laminate zone requires a property. Any changes in laminate stacking or plies need
rework of zones.

Zone-based modeling limitations include:

1. Data duplication
2. Difficult to interpret ply shape
3. No relationship to the manufacturing process
4. Model updates require multiple steps

55
 Fig 3.15: Illustration of zone-based modelling
For OptiStruct solver, PCOMP and PCOMP (G) are two properties which are used for
modelling zone-based laminate modelling.

PCOMP

Below is the PCOMP card used for modeling zone-based models in HyperMesh:

Fig 3.16: PCOMP card image

PCOMP defines the structure and properties of a composite lay-up which is then
assigned to an element. If a ply runs through different zones, no associativity between
PCOMPs is maintained.

56
 Fig 3.17: Image illustrating disadvantage of PCOMP

The following example illustrates limitations of using PCOMP (zone based)

This is an aircraft structure with several zones and junctions. Each zone has a PCOMP
and each PCOMP is a laminate with several plies. The laminate layout is shown with
the figure for a better understanding.

Fig 3.18: Aircraft structure modelled with PCOMP

57
The results of the structure after analysis are shown below:

Fig 3.19: Results of aircraft structure using PCOMP, stress in ply 3

Upon observing, the stress value does not vary gradually in the top face region, but
suddenly decreases to a lower value across zones. This example shows that, for the
results to be meaningful during post-processing of the PCOMP results, we must
correlate the ply results to their corresponding ply property.

This highlights that, during the post-processing of PCOMP components, plotting

results based on just the ply number is not sufficient. One must keep track of ply
properties (material, thickness, orientation, failure index, etc.) on your own during
post-processing with this method. In cases that use large and complex models, it
becomes tedious to track the individual ply properties during post-processing.

This drawback with PCOMP can be avoided with the use of the PCOMPG card for
property definition. Using the PCOMPG card, one can assign a global ply number for
each ply and post-process the results based on global ply number.

PCOMPG
PCOMPG defines the structure and properties of a composite lay-up allowing for
global ply identification which is then assigned to an element. Plies of different
PCOMPG definitions can have a relationship using global ply IDs.

58
 Fig 3.20: Image illustrating PCOMPG
The same example of aircraft structure if modelled with PCOMPG, the results are
completely different

59
 Fig 3.21: Results of aircraft structure using PCOMPG, stress in ply 3
Post-processing the results based on global ply number eliminates the need to track
the ply number and corresponding ply properties on the components. The results are
displayed based on the global ply number, irrespective of the ply order, so you can
choose any one global ply number and view results across the whole component. If a
ply is not present in any given region, no result is displayed.

60
PCOMPP
PCOMPP is a ply-based modeling approach for modern composite analysis

Fig 3.22: Ply based modelling approach

Some of the advantages of ply-based modelling are:

• No data duplication
• Plies are defined as “physical objects” with respect to shape
• Direct relationship to the manufacturing process
• Model updates require single step

PCOMPP property facilitates modelling flexibility for ply based modelling of laminates
in HyperMesh. Ply definition, stacking and the property are defined separately
through independent cards (PLY, STACK, and PCOMPP).

• PLY card defines fiber orientation and layout

• STACK card sets the sequence of PLYs into a laminate

61
Element properties are set implicitly through STACK and PLY, replacing PCOMP and
PCOMPG explicit laminate definitions. This provides additional flexibility in
manipulating laminates in both analysis and optimization.

Where:

Fig 3.23: PCOMPP card image from HyperMesh

PLY defines the properties of ply used in ply-based composite definition

Where:

Fig 3.24: Ply card image from HyperMesh

The STACK defines the stacking information and sequence for ply-based composite
definition

62
Where:

Fig 3.25: Stack card image from HyperMesh

Using ply-based modelling it is easy to create laminates with several sub-laminates

and interfaces

Where:

Fig 3.26: Stack card with sub-laminate and interfaces image from
HyperMesh

63
3.7 Tutorial: Assigning Material Orientation
In this tutorial, you will learn how to assign element material orientation using the
following:

• System ID
• Vector
• Angle

Step 1: Load the OptiStruct user profile.

1. Start HyperMesh Desktop.
2. In the User Profile dialog, select OptiStruct.
3. Click OK.

Step 2: Retrieve and view the file, composites.hm.

1. Open a model file by clicking File > Open > Model from the menu bar, or

clicking on the Standard toolbar.

2. In the Open Model dialog, open the composites.hm file. A model appears in
the graphics area.

Fig 4.6: Model view in Graphic Area

64
Step 3: Update all of the elements to the correct element types for
OptiStruct.
1. Open the Element Type panel by clicking Mesh > Assign > Element Type
from the menu bar.
2. Click elems >> all. HyperMesh selects all the element types (1D, 2D, and
3D).
3. Click update.
4. Return to the main menu by clicking return.

Step 4: Assign element material coordinate direction using system ID.

1. Open the Composites panel by clicking composites from the 2D page.
2. Go to the material orientation subpanel.
3. Set the entity selector to elems.
4. Click elems >> all.
5. Set the Material orientation method to by system ID.
6. Activate the system selector.
7. Select the rectangular system on top of ball as indicated in the following
image.

Note: The system ID = 1.

65
 Fig 4.7: Selecting the System
8. Click color and select a display color for the review vectors or lines.
9. In the size = field, enter 2.0.

Note: This value specifies, in model units, how large the review vectors are when
displayed.

10. Click assign

66
 Fig 4.8: visualization of Material Orientation

11. Open the Card Edit panel by clicking on the Collectors toolbar.
12. Set the entity selector to elems.
13. Select any element in the model.
14. Click edit.
15. In the Card Previewer dialog, review the card.

Note: This function assigns the ID of the coordinate system to the selected
elements. This can be verified by reviewing the MCID field of the
CQUAD4 card populated with System ID 1 for the currently loaded
OptiStruct user profile. How each analysis code interprets this
information varies. For OptiStruct, refer to the CQUAD4 and PCOMP
(G) bulk data cards in the Bulk Data Section of the OptiStruct Reference
Manual. For visualization purposes HyperMesh also projects the x­axis
of the selected coordinate system onto the face of the shell elements
to define the x­axis of the material coordinate system. If you later
modify the system, the element material coordinate directions change
implicitly.

16. Exit the Card Previewer by clicking return.

67
 17. Exit the Card Edit panel and return to the Composites panel by clicking
return.

Step 5: Assign element material coordinate direction using a system axis.

In this step, you should be in the Composites panel, material orientation subpanel.

1. Set the entity selector to elems.

2. Click elems >> all.
3. Set the Material orientation method to by system axis.
4. Activate the system selector.
5. Select the rectangular system on top of ball as indicated in the following
image.

Note: The system ID = 1.

6. Under the system selector, set the switch to local 2­axis.

7. In the size= field, enter 2.0.

Note: This value specifies, in model units, how large the review vectors are when
displayed.

8. Click color and select a display color for the review vectors or lines.
9. Click project.
10. Open the Card Edit panel.
11. Set the entity selector to elems.
12. Select any element in the model.
13. Click edit.
14. In the Card Previewer dialog, review the card.

Note: This function assigns a material angle to the selected elements, which for
OptiStruct is defined as the angle between the vector direction connecting node1 and
node2 of the shell element (that is, the element coordinate system x­axis) and the
projection of the selected local axis onto the surface of the shell element. This can be
verified by reviewing the THETA field of the CQUAD4 card populated with an angle (in

68
degrees) for the currently loaded OptiStruct user profile. Each element in this case
will have a unique THETA value as defined by the projection. How each analysis code
interprets this information varies. For OptiStruct, refer to the CQUAD4 and PCOMP
(G) bulk data cards in the Bulk Data Section of the OptiStruct Reference Manual. For
visualization purposes HyperMesh also projects the local axis of the selected
coordinate system onto the face of the shell elements to define the x­axis of the
material coordinate system.

15. Exit the Card Previewer.

16. Exit the Card Edit panel and return to the Composites panel.

Step 6: Assign element material coordinate direction using a vector.

In this step you should be in the Composites panel, material orientation subpanel.

1. Set the entity selector to elems.

2. Click elems >> all.

3. Set the Material orientation method to by vector.

4. Set the orientation selector to vector.

5. Activate the vector selector.

6. Select the radial r vector from the spherical coordinate system on the bottom
of the ball.

Note: The r­axis will flash once when you click on it.

7. Click B.

8. Select the origin of the local spherical system as the base.

9. In the size = field, enter 2.0.

Note: This value specifies, in model units, how large the review vectors are when
displayed.

10. Click color and select a display color for the review vectors or lines.

69
 11. Click project.

12. Open the Card Edit panel.

13. Set the entity selector to elems.

14. Select any element in the model.

15. Click edit.

16. In the Card Previewer dialog, review the card.

Note: This function assigns a material angle to the selected elements, which for
OptiStruct is defined as the angle between the vector direction connecting node1 and
node2 of the shell element (that is, the element coordinate system x­axis) and the
projection of the selected vector onto the surface of the shell element. This can be
verified by reviewing the THETA field of the CQUAD4 card populated with an angle (in
degrees) for the currently loaded OptiStruct user profile. Each element in this case
will have a unique THETA value as defined by the projection. How each analysis code
interprets this information varies. For OptiStruct, refer to the CQUAD4 and PCOMP
(G) bulk data cards in the Bulk Data Section of the OptiStruct Reference Manual. For
visualization purposes HyperMesh also projects the selected vector onto the face of
the shell elements to define the x­axis of the material coordinate system.

17. Exit the Card Previewer.

18. Exit the Card Edit panel and return to the Composites panel.

Step 7: Assign element material coordinate direction using an angle.

In this step you should be in the Composites panel, material orientation subpanel.

1. Set the entity selector to elems.

2. Click elems >> all.

3. Set the Material orientation method to by angle.

4. In the angle = field, enter 45.00.

5. In the size = field, enter 2.0.

70
Note: This value specifies, in model units, how large the review vectors are when
displayed.

6. Click color and select a display color for the review vectors or lines.

7. Click set.

8. Open the Card Edit panel.

9. Set the entity selector to elems.

10. Select any element in the model.

11. Click edit.

12. In the Card Previewer dialog, review the card.

Note: This function assigns a material angle of 45 degrees to the selected elements,
which for OptiStruct is defined as the angle 45 degrees from the vector direction
connecting node1 and node2 of the shell element (that is, the element coordinate
system x­axis) using right hand rule. In order to use right hand rule, the normal
direction of the element must be known and can be determined from the Tools page,
Normals panel. This can be verified by reviewing the THETA field of the CQUAD4 card
populated with a 45­degree angle for the currently loaded OptiStruct user profile.
Each element in this case will have a THETA of 45 degrees. How each analysis code
interprets this information varies. For OptiStruct, refer to the CQUAD4 and PCOMP
(G) bulk data cards in the Bulk Data Section of the OptiStruct Reference Manual. For
visualization purposes HyperMesh defines a vector using OptiStruct convention on
the face of the shell elements to define the x­axis of the material coordinate system.
This option should be used only in situations where great care has been taken to
assure that the node1­node2 direction of the shell elements are initially aligned
properly.
13. Exit the Card Previewer.

14. Exit the Card Edit panel and return to the Composites panel.

71
Step 8: Review ply directions.
In this step you should be in the Composites panel.

1. Go to ply directions subpanel.

2. Use the switch to select zone based model.
3. Set the entity selector to elems.
4. Click elems >> by collector.
5. Select the collector, yellow_sample.

Note: The yellow_sample collector has a PCOMP card image assigned to it with
the following laminate definitions (45/60/90). The PCOMP definition assigned
to the yellow_sample collector can be reviewed in the card editor.

6. Click select.
7. In the ply = field, enter 1.

Note:This defines the ply number to review.

8. Open the Card Edit panel.

9. Set the entity selector to props.
10. Click props.
11. Select yellow_sample.
12. Click select.
13. Click edit.
14. In the Card Previewer dialog, review the card.

Note: The first ply defined on the PCOMP card is the most negative z­axis ply as
determined from the element normal. All ply angles on the PCOMP card are relative
to the material coordinate direction set in the above exercises using right hand rule.
In order to use right hand rule, the normal direction of the element must also be
known and can be determined from the Tools page, Normals panel. For OptiStruct,
refer to the PCOMP(G) bulk data cards in the Bulk Data Section of the OptiStruct
Reference Manual.

15. Exit the Card Previewer.

72
 16. Exit the Card Edit panel and return to the Composites panel.
17. In the size = field, enter 2.0.

Note:This value specifies, in model units, how large the review vectors are when
displayed.

18. Click color and select a display color for the review vectors or lines.
19. Click review.
20. Review additional ply angles, reselect elements, and enter a ply ID by clicking
review.

Note: Elements that do not have ply angles assigned will not be displayed. Ply
directions are set through card images in the solver template; an example is PCOMP
card for OptiStruct.

Here is a short video on how to check element normal and assign material orientation.

Checking element normals and assigning material orientation using

HyperMesh - Altair University

73
3.8 Tutorial: Difference between PCOMP and
PCOMPG using FEA approach
Step 1: Launch HyperMesh, set the OptiStruct User Profile and retrieve the
file
1. Launch HyperMesh.
2. Select OptiStruct from the User Profiles dialog and click OK.
3. Click File > open. An Open Model browser window opens.

Note: If HyperMesh Desktop was launched, use: File > open > Model.

4. Select the frame.hm file you saved to your working directory from the
OptiStruct.zip
5. Click Open. The frame.hm database is loaded into the current HyperMesh
session, replacing any existing data.

Step 2: Review the model setup in HyperMesh

The structural model has been already set up and can be solved without any further
modifications. Review the model setup before submitting the job.

The model is set up for linear static analysis. As mentioned earlier, only half of the
structure is modeled; and to impose the half symmetry boundary conditions, all the
nodes on the symmetry plane are constrained in dof1, dof5, and dof6.

All the components are modeled with the PCOMP property which lists the plies
(stacking sequence) from the bottom surface upwards, with respect to the element’s
normal direction, as shown in the image below (Fig 4.9).

Fig 4.9: Ply stacking sequence with respect to element normal

74
Components in this model that have names starting with the word "Flange" represent
junctions in which different components are connected together. While reviewing,
closely watch the flange area formed by the Skin and Rib components (highlighted in
the following figure). Review the ply lay­up of the Skin_inner, Rib, Flange1_Rib_Skin,
and Flange2_Rib_Skin components (laminate layout is shown in the bottom portion
of the following figure). Note that few plies are common for the Skin_inner,
Flange1_Rib_Skin, Flange2_Rib_Skin, and Skin_outer components, but appear in
different stacking sequence in each component. For example, the 4th ply in
Skin_inner is the 3rd ply in Flange2_Rib_Skin and the 2nd ply in Skin_outer
components.

Fig 4.10: Ply stacking for the Skin_inner, Rib, Skin_outer, Flangel_Rib_Skin
components
1. From the 2D page, click HyperLaminate to enter the Graphic User
Interface (GUI).
This opens the HyperLaminate (GUI) in which the ply lay­up information
can be defined, reviewed and edited. Material properties and design
variables can also be created and edited here.
2. Expand the Laminates portion of the tree structure on the left­hand side
of the screen.
3. Select the Skin_inner PCOMP.
Details of the laminate appear in the GUI.

75
 4. Verify that the lay­up definition for Skin_inner matches the first 5 entries
of the table below, which is the lay­up information of Flange1_Rib_Skin
component.
5. Select the Rib PCOMP and verify that the 3rd and 4th lay­up definition for
Rib matches the 6th and 7th entries in the following table.
6. Select the Flange1_Rib_Skin PCOMP to view the ply lay­up definitions.
Verify that the lay­up definition for Flange1_Rib_Skin matches the
following table.
Observe that the first 5 P1 (Major) Stress are the same as Skin_inner
lay­ups and that the last two lay­ups are the same as the 3rd and 4th
lay­up of Rib, as shown in the last figure. You can verify how other flanges
are modeled.
7. You can also review the other components. Once the review is completed,
select Exit from the File menu. Exit the HyperLaminate GUI and return to
HyperMesh

Laminate properties of Flange1_Rib_Skin:

Ply
Material Thickness T Orientation SOUT
Number

1 carbon_fiber 1.2 45 YES

2 matrix 0.2 90 YES

3 carbon_fiber 1.2 ­45 YES

4 matrix 0.2 ­90 YES

5 carbon_fiber 1.2 90 YES

6 matrix 0.2 ­45 YES

7 carbon_fiber 1.2 45 YES

Table 4.1: Laminate properties of Flange1_Rib_Skin

Step 3: Submit the Job

1. From the Analysis page, enter the OptiStruct panel.

76
 2. Following the input file: field, click Save as. A Save As browser window
opens.
3. Select the directory where you would like to write the OptiStruct model
file and enter the name for the model, frame_PCOMP.fem, in the input
file: field.
4. Click Save.

The name and location of the frame_PCOMP.fem file displays in the input file: field.

5. Set the export options: toggle to all.

6. Set the run options: toggle to analysis.
7. Set the memory options: toggle to memory default.
8. Click OptiStruct. This launches the OptiStruct job.

If the analysis is successful, no error messages are reported to the shell. The analysis
is complete when the message Process completed successfully appears in the shell.

The default files written to the directory are:

frame_PCOMP.html HTML report of the analysis, giving a summary of the

problem formulation and the analysis results.

frame_PCOMP.out OptiStruct output file containing specific information

on the file setup, the set up of your optimization
problem, estimates for RAM and disk space required
for the run, information for each of the optimization
iterations, and compute time information. Review this
file for warnings and errors.

frame_PCOMP.h3d HyperView binary results file.

77
 frame_PCOMP.stat Summary of analysis process, providing CPU
information for each step during analysis process.

The frame_PCOMP.out file is a good place to look for error messages that will help to
debug the input deck if any errors are present.

Step 4: View the results/Post­processing

1. Click HyperView from the OptiStruct panel. HyperView launches and the
model results are automatically loaded into HyperView.
2. Click Close to close the message window.
3. Click the Contour toolbar .
4. Select the first switch below Result type: and select Composite stresses(s).
5. Select the second switch and select the P1 (Major) Stress.
6. Select 3 for the Layers option.
7. In the field below, Averaging method: select None.

Fig 4.11: Contour Results Panel in HyperView

8. Click Apply. This contours the maximum principle stress for the 3rd ply of all
the components in the model.

9. Click the Isometric view icon in the Standard Views toolbar to see the
model, as shown in the following figure 4.12.

78
 Fig 4.12: Stress distribution on the top face of the frame
The stress value does not vary gradually in the top face region, but suddenly decreases
to a lower value across the Flange2_Rib_Skin component. Looking at the table of
laminate properties of
Flange1_Rib_Skin again, observe that the 3rd ply property of the Flange2_Rib_Skin
component is of a matrix material and the third plies in the components adjacent to
it (Flange1_Rib_Skin and Skin_outer) are of a carbon fiber material. The sudden
changes in the stress values occur because we are looking at stress on two different
materials. This example shows that, for the results to be meaningful during
post­processing of the PCOMP results, you have to correlate the ply results to their
corresponding ply property.

This highlights that, during the post­processing of PCOMP components, plotting

results based on just the ply number is not sufficient. You have to keep track of ply
properties (material, thickness, orientation, failure index, etc.) on your own during
post­processing with this method. In cases that use large and complex models, it
becomes tedious to track the individual ply properties during postprocessing.

79
This drawback to using PCOMP can be avoided with the use of the PCOMPG card for
property definition. Using the PCOMPG card, you can assign a global ply number for
each ply and post­process the results based on global ply number. The following steps
explain the procedure to redefine the model with PCOMPG property.

Step 5: Redefine the model setup in HyperMesh

1. Close the HyperView window and return to HyperMesh.

2. Note: Click to return to the previous page where HyperMesh is open, if

you are using HyperMesh Desktop.
3. From the 2D page, select the HyperLaminate panel. This opens the
HyperLaminate GUI in which the ply lay­up information can be defined,
reviewed and edited.
4. Click Tools > Laminate Options. This opens a new window in which the default
ply lay­up options can be set.
5. Click the Convention: switch and select Total.
6. Click OK to close the window. This sets up Total as the default option
whenever a new component is created.

Fig 4.13: Laminate information with global ply number

Now you create new PCOMPG components with global ply numbers defined as shown
in the above figure 4.13. As discussed earlier, the 4th ply in Skin_inner is the 3rd ply
in Flange2_Rib_Skin and the 2nd ply in Skin_outer components. Therefore, all of
these plies will be defined with the same global ply ID 4. Similarly, all other plies are
to be defined, as shown in the above figure.

80
 7. Expand the laminates portion of the tree structure on the left­hand side of
the screen.
8. Right­click PCOMPG and a menu appears. Click New. This creates new
component, which is named NewLaminate1 by default, and the tree structure
is expanded.

9. Rename the component to Skin_inner_GPLY by right­clicking and select

Rename in the text field and overwrite the default component name.

10. In the Add/Update plies: section under the field GPLYID, enter 1.

11. Select the pull­down menu below Material and select carbon_fiber.

12. Below the Thickness T1 field, enter 1.2.

13. Below the Orientation field, enter 45.

14. Select the pull­down menu below SOUT and select YES.

15. Click Add New Ply to add the ply information.

16. Repeat this procedure to add 4 more plies with the properties shown in the
table:

GPLYID Material Thickness T Orientation SOUT

2 matrix 0.2 90 YES

3 carbon_fiber 1.2 ­45 YES

4 matrix 0.2 ­90 YES

5 carbon_fiber 1.2 90 YES

17. Click Update Laminate at the bottom of the window to update the lay­up
information. The graphical display of lay­up information now appears in the
field below the Review tab, on the right side of the GUI.

18. Create a new PCOMPG component with name Rib_GPLY and the ply lay­up,
as shown in the following table:

81
 GPLYID Material Thickness T Orientation SOUT

11 carbon_fiber 1.2 0 YES

12 matrix 0.2 45 YES

13 matrix 0.2 ­45 YES

14 carbon_fiber 1.2 45 YES

Referring to the figure showing laminate information with global ply number
above (fig 4.13), you will create the Flange1_Rib_Skin_GPLY component.

19. Right­click Skin_inner_GPLY and select Duplicate from the menu to create an
identical component.

20. Rename the component as Flange1_Rib_Skin_GPLY by right­clicking and

select rename in the text field and overwrite the component name.

21. Add 2 more plies with the properties shown in the following table using the
Add New Ply feature.

GPLYID Material Thickness T Orientation SOUT

13 matrix 0.2 ­45 YES

14 carbon_fiber 1.2 45 YES

The new component Flange1_Rib_Skin_GPLY was created. Its first 5 plies are the
same as Skin_inner_GPLY and its last 2 plies are the 3rd and 4th plies of the Rib
component.

To reduce the number of steps in this tutorial, the ply lay­up information of other
components is already defined with PCOMPG property and appropriate laminate
information in the
updated_PCOMPG_properties.fem file you saved to your working directory from
the OptiStruct.zip file. This file is imported into HyperMesh to update (overwrite)
the properties instead of manually updating them.

82
The updated_PCOMPG_properties.fem file is saved in OptiStruct input file format.
Open this in any text editor to review how the components are defined with
PCOMPG properties. A section of the file is shown below (Fig 4.14).

Fig 4.14: Components defined with PCOMPG

22. Click File > Exit. This will exit the HyperLaminate GUI and return to
HyperMesh.
23. Click File > Import > Solver Deck.
24. Toggle and expand the Import options and check the box next to FE
overwrite.
25. This option overwrites the old PCOMP properties with PCOMPG properties
defined in the updated_PCOMPG_properties.fem file.

26. Click on the folder icon next to File: and select the
updated_PCOMPG_properties.fem file and click Import.
27. Click Close.

Step 6: Review the imported properties in HyperLaminate

1. From the 2D page, go to the HyperLaminate panel.
2. Expand the laminates portion of the tree structure on the left­hand side of
the screen.
3. All of the components now appear under PCOMPG. The components created
earlier (Skin_inner_GPLY, Rib_GPLY, and Flange1_Rib_Skin_GPLY) are still
present. There is no element associated with these components. Review the
PCOMPG components to view the laminate definitions.

83
 4. Click File > Exit.

Step 7: Submit the Job

1. From the Analysis page, enter the OptiStruct panel.

2. Following the input file: field, click Save as.

3. In the Save file browser window, select the directory where you would like to
write the OptiStruct model file and enter frame_PCOMPG.fem as the name
for the model.

4. Click Save.

5. The name and location of the frame_PCOMPG.fem file displays in the input
file: field.

6. Set the export options: toggle to all.

7. Set the run options: toggle to analysis.

8. Set the memory options: toggle to memory default.

9. Click OptiStruct. This launches the OptiStruct job.

If the job is successful, new results files can be seen in the directory where the model
file was written. The frame_PCOMPG.out file is a good place to look for error
messages that will help to debug the input deck, if any errors are present.

The default files written to the directory are:

frame_PCOMPG.html HTML report of the analysis, giving a summary of

the problem formulation and the analysis results.

frame_PCOMPG.out OptiStruct output file containing specific

information on the file setup, the set up of your
optimization problem, estimates for the amount
of RAM and disk space required for the run,

84
 information for each of the optimization
iterations, and compute time information. Review
this file for warnings and errors.

HyperMesh binary results file.

frame_PCOMPG.res

HyperView binary results file.

frame_PCOMPG.h3d

frame_PCOMPG.stat Summary of analysis process, providing CPU

information for each step during analysis
process.

Step 8: View the results/Post­processing

1. When the message Process completed successfully is received in the
command window, click HyperView in the OptiStruct panel. The results are
automatically loaded into HyperView.

A message window may appear with information about the successful loading
of the model and result files into HyperView.

2. Click Close to close the message window.

3. Click the Contour toolbar .

4. Select the first switch below Result type: and select Composite stresses (s).

5. Select the second switch and select P1 (Major) Stress.

6. For the Layers field, select PLY 3.

7. For Averaging method: select None.

8. Click Apply. This plots the maximum principle stress for global ply 3. The
results are not plotted

85
 in the regions where, global ply 3 is not present.

Click the Isometric view icon in the Standard Views toolbar.

Fig 4.15: Isometric view of the model

Post­processing the results based on global ply number eliminates the need to track
the ply number and corresponding ply properties on the components. The results are
displayed based on the global ply number, irrespective of the ply order, so you can
choose any one global ply number and view results across the whole component. If a
ply is not present in any given region, no result is displayed.

3.9 Tutorial: Creating Ply-based Laminates

This tutorial introduces the user to creating a simple but complete and running model
from geometric data and material properties.

Step 1: Open HyperMesh Desktop with the OptiStruct user profile

Step 2: Create nodes to bound the composite plate mesh geometry

1. On the Geom page, enter the nodes panel.

2. With the XYZ option selected, enter the node coordinates {-50,20,0}. Click
create

86
 to create the node.

3. Create seven more nodes at coordinates: {-20,20,0}, {10,20,0}, {50,20,0}, {-

20,-20,0}, {10,-20,0}, {50,-20,0}, and {-50,-20,0}.

Step 3: Create lines to serve as ply boundaries

1. From the Geom page, select the lines panel.

2. With the Linear Nodes option selected and the node list entity selector
active, select the top left and bottom left nodes in that order and click create
to create a line between those two nodes.
3. Repeat step 2 to create 3 more vertical lines parallel to the first at each of the
created node locations.

4. Similarly, create lines between each pair of adjacent nodes on the ‘top’ and
‘bottom’ of the rectangle to enclose each rectangle.

87
Step 4: Create a new MAT8 material with the following parameters

Fig 4.16: Material Entity Editor

88
Step 5: Create a new PCOMPP property with default parameters and assign
to the component

Fig 4.17: Property Entity Editor

Step 6: Create the plies using the geometric lines as boundaries

1. In the Model Browser, right-click to select Create > Ply.
2. For the first ply, set the Name: to Ply1 with a Thickness of 1, an Orientation
angle of 0 degrees, and a Material of Biaxial. Change the Shape: drop-down
entity selector to Line and select the outermost lines, signifying the ply is to
represent the complete plate

89
 Fig 4.18: Create Ply Window

3. For the second ply, set the Name: to Ply2 with a Thickness of 1, an
Orientation angle of 0 degrees, a Material of Biaxial and a shape using lines
of the outline of the two rightmost sections.

Tip: Do not select the dividing line between the sections.

4. For the third ply, set the Name: to Ply3 with a Thickness of 1, an Orientation
angle of 0 degrees, a Material of Biaxial and shape of only the outline of the
rightmost rectangle.

5. For the final ply, set the Name: to Ply4 with a Thickness of 1, an Orientation
angle of 0 degrees, a Material of Biaxial and shape comprising the total plate.

90
 Fig 4.19: Model Browser

Step 7: Create the laminate

1. Right-click in the Model Browser and select Create > Laminate. Name the
new laminate.

2. Click in the first cell of the first row to select Ply1 in the drop-down selector.
Information about the ply is populated on the rest of the row.

3. For rows 2, 3, and 4 of the laminate, select Ply2, Ply3, and Ply4 respectively.
Plies may not be used multiple times within a single laminate.

4. Click Create to create the laminate. Close the Create Laminate dialog box.

Step 8: Set composite visualization options for element color by prop, 2d

detailed element representation, and composite layers

Fig 4.20: Composite Visualization

91
Step 9: Create the 2d mesh
1. On the 2D page, select the skin panel. Set the mesh type to mesh, w/o surf.

2. With the line list entity selector active, select the four ‘vertical’ lines in the
model from left to right.

3. Click create to accept the selection and go to the mesh parameters panel. Set
the element size to 5, click recalc all, and click mesh. HyperMesh creates 160
elements from the line selections.

92
 Fig 4.21: Skin mesh review

4. Click return twice to exit the skin meshing panel.

Step 10: Realize the plies to convert the geometric boundaries to element
sets
1. In the Model Browser, right-click on the Ply container of the model tree and
select Realize.
2. Select the auto1 component as the Realization region: and set the Projection
options:

to Project Normal to target mesh for CPD/Geom data.

93
 Fig 4.22: Ply Realization Panel
3. Click Realize to have HyperMesh Desktop project the line data onto the mesh
to determine the mesh ply shapes.

Fig 4.23: Ply Visualization

94
Step 11: Edit the PCOMPP card and set Z0 to 0 to set the bottom surface of
the plate geometry coincident with the bottom surface of the base ply

Fig 4.24: Re-positioning of plies using Z offset

95
3.10 Basic Composite Modeling in HyperMesh
Videos
i. Pre-Processing for composite Analysis:
Here is a short video on basic ply based modelling of composites in
HyperMesh:

Preprocessing for composite analysis using HyperMesh - Altair University

ii. Creating Sub-laminates and Interface laminates:

Here is a short video on creating sub-laminates and Interface laminates in
HyperMesh.

Creating sub laminates and interface laminates using HyperMesh - Altair

University

96
 4 Advanced Composite
modeling in OptiStruct

4.1 Importing composite data with HyperWorks

If composite data is available or designed with a CAD tool like CATIA, one can import
and carry further modelling without re-creating everything from the beginning.
HyperMesh reads composite data from CAD files while importing geometry.
HyperMesh can read composite data from either CatPart from CATIA composites and
FiberSim.

Using CATIA Composite Link:

Use the CATIA Composites Link option to import drape data. This method is separate
from the CATIA Reader Support, where drape data is not imported. You need to use
the CATIA composite (Simulyt) module and export a HDF5 file and then use that to
import in HyperMesh using the CATIA composite connection.

1. First import a CAD model (without composite data) using the CATIA geometry
import method.
2. Use the CATIA composite connection to import the HDF5 files created from
the Simulyt interface in CATIA.
3. When realizing the plies, use the CATIA Composite Link drape map by
proximity method in the Ply Realization dialog.
4. When exporting the composite data to CAD including draping, use the
geometry export option CATIA Composites.

97
 Fig 4.1: CATIA Import options from HyperMesh

Here is a short video on how to import composite model from CATIA and Visualize.

https://altairuniversity.com/learning-library/import-catia-composite-data/

98
Using FiberSim:
The following entities are supported by the FiberSim HDF5 reader in HyperMesh:

1. Plies: Name, thickness and fiber orientation information is directly read and
mapped as a Ply entity in HyperMesh. Plies that point to woven and stack
materials are split/separated into multiple plies with half the thickness and
correct orientation angles. These split ply names always have _1 and _2 suffix
in them for each identification.

2. Data Map/Table: Data map with element set (ply shapes), material
orientation angles (orient1, orient2, draping corrections) thickness
corrections, reference direction and normal information for each ply is
preserved/mapped in the table entity in HyperMesh, therefore each ply has
a table associated with it. HyperMesh does not create nodes and elements in
the database from FiberSim triangulation data to define ply shapes. Instead,
it preserves this information in a table so that when these plies are mapped
(realized) on actual good mesh, HyperMesh uses this triangular information
to define the ply boundary and extract the actual elements.

3. Laminates: One laminate per HDF5 component with all the ply sequence
preserved as per layer_id value.

4. Materials: Material names and their mechanical properties are read and
mapped to solver cards automatically depending on the user profile loaded
while importing the model. Currently mechanical properties such as E1, E2,
E3, G12, G13, G23, Alpha1, Alpha2 and Alpha_ref temperatures are mapped
to solver material attributes

5. Rosette/Systems: All the system definitions available in the HDF5 file will be
imported into one system collector in HyperMesh. Currently HyperMesh does
not preserve the ply and system relationship.

99
4.2 Using HyperLaminate Module to Create
Composite Structure
HyperLaminate is a HyperMesh module that facilitates the creation, review and
edition of composite laminates. In support of this process certain materials and design
variables are also supported by the HyperLaminate module.

The HyperLaminate Solver (HLS), which is accessed through the HyperLaminate

module, uses classical laminated plate theory for simple in-plane analysis of
composite laminates.

The current HyperMesh database is only updated with information from the current
HyperLaminate session on exit from HyperLaminate (except with Abaqus materials,
which are updated simultaneously in HyperMesh and HyperLaminate), so while it is
possible to work in HyperMesh while HyperLaminate is running, this is not advisable.
Any changes made to those entities which HyperLaminate touches (materials,
component collectors and design variables) may result in synchronization problems
and loss of data.

Laminate Browser
The Laminate Browser, located on the left side of the HyperLaminate window,
provides a vertical tree view of the materials, laminates, and HLS loadcases in your
model. For the OptiStruct and Nastran user profiles the browser also includes size
design variables.

On launching HyperLaminate, the Laminate Browser is populated with all the relevant
materials, laminate definitions, HLS loadcases, and size design variables existing in the
HyperMesh database, for the active user profile.

100
 Fig 4.2: Laminate Browser from HyperLaminate

Define/Edit Pane
The Define/Edit Pane, the central pane of the HyperLaminate window, allows you to
edit the definition of the selected entity. On selecting an entity in the Laminate
Browser, the Define/Edit pane is populated with the current definition.

Fig 4.3: Define/Edit pane for Materials

101
This pane allows to define and edit materials, add material and define laminates. For
laminates, the Define/Edit pane allows the laminate name, HyperMesh entity color,
stacking sequence convention, and the ply lay-up order to be edited. In addition, HLS
loadcases may be selected (through the Assign LoadCases button) and solved
(through the Calculate button) for the current laminate.

There are a number of options (conventions) for the stacking sequence:

a) Total: The Ply lay-up order table describes the laminate in its entirety.

b) Symmetric: The Ply lay-up order table describes the bottom half of the laminate.
The top half of the laminate is the mirror image of the bottom half. The ply angles
used for the top half are the same as the ply angles used in the bottom half.

c) Antisymmetric: The Ply lay-up order table describes the bottom half of the
laminate. The top half of the laminate is the mirror image of the bottom half. The ply
angles used for the top half have the opposite sign to the ply angles used in the
bottom half (but 0, 90, 180, 270, and 360 remain as 0, 90, 180, 270, and 360,
respectively).

d) Symmetric-Midlayer: The Ply lay-up order table describes the bottom half of the
laminate and a midlayer (or core). The midlayer is the last ply defined in the table. The
top half of the laminate is the mirror image of the bottom half. The midlayer is not
reflected. The ply angles used for the top half are the same as the ply angles used in
the bottom half. Due to the midlayer, the total number of plies is always odd.

e) Antisymmetric-Midlayer: The Ply lay-up order table describes the bottom half of
the laminate and a midlayer (or core). The midlayer is the last ply defined in the table.
The top half of the laminate is the mirror image of the bottom half. The midlayer is
not reflected. The ply angles used for the top half have the opposite sign to the ply
angles used in the bottom half (but 0, 90, 180, 270, and 360 remain as 0, 90, 180, 270,
and 360, respectively). Due to the midlayer, the total number of plies is always odd.

102
f) Repeat: The Ply lay-up order table describes a single sub-laminate which is repeated
a number of times. The number of repetitions is determined by the number entered
in the Repetitions: field (which is activated when this Convention is chosen).

Fig 4.4: Laminate Definition pane

The Define/Edit pane for Laminates also provides access to the HyperLaminate Solver.
Several inplane loading scenarios (HLS loadcases) may be solved for a given laminate.
The HLS loadcases are selected on the LoadCase Definition dialog, which is launched
by clicking on the Assign LoadCases button.

HyperLaminate Solver
The HyperLaminate Solver (HLS) uses classical laminated plate theory to analyze
composite laminates subject to various in-plane and thermal loading conditions.

The solver is integrated into the HyperLaminate module of HyperMesh. The following
functionalities are provided:

1. to define and edit HLS loadcases

103
 2. to select a subset of HLS loadcases for analysis for each laminate
3. to perform the analysis
4. to review the results of the analysis for each laminate
5. to export the results to an external file

When a laminate is selected from the Laminate Browser, an Assign LoadCases button
is present in the lower left corner of the Define/Edit pane. This button launches the
LoadCase Definition GUI, allowing you to select which HLS loadcases the current
laminate will be analyzed for.

Fig 4.5: HyperLaminate Loadcase Definition box

Once the desired loadcases are selected, the analysis can be performed for the
current laminate by clicking the Calculate button. Once the analysis is complete
several results tabs will appear in the Review/Results pane, namely:

• Stiffness/Material Matrix
• Mid-Plane Results
• Global System Results
• Material System Results
• Principal Results
• Invariant Results

These results will remain so long as the laminate is not updated. Once a laminate is
updated, the results will no longer be valid and therefore the results tabs are

104
removed. Clicking the Calculate button will re-launch the HyperLaminate Solver and
populate the results tabs for the updated laminate definition.

4.3 Useful tools and options in HyperMesh

Aerospace module
Import and model PCOMP using .csv file
Here is an exercise which helps to model a laminate using PCOMP, in turn using a .csv
file. You should copy the file: blade.hm, sample.csv

Step 1: Open HyperMesh Desktop with the Aerospace User Profile

1. Open HyperMesh Desktop.
2. In the User Profiles dialog box, set Application: to Engineering Solutions and
select the radio button option for Aerospace with solver selection set to
OptiStruct.

Fig 4.25: Aerospace user profile

This setting enables the Aerospace toolbar menu options in HyperMesh Desktop.

Step 2: Open the model blade.hm in HyperMesh Desktop

105
 Fig 4.26: Blade Model in HM

Step 3: Review the existing properties in the model

1. Using the Model Browser, expand the Property section of the model tree.
2. Click on each of the four properties in the model to populate that property
into the Entity Editor beneath the Model Browser.

106
 Fig 4.27: Property Entity Editor

3. Note that the card image for the existing properties is either PSHELL or
PSOLID, indicating that these properties are for the MAT1 shells or solid
elements in the model.

Step 4: Review the sample.csv file in a text editor

1. Open the sample.csv file in a text editor and review the file.

Fig 4.28: CSV file in a text editor

The headers indicate the information required in each column: the id of the new
PCOMP entry, the ID of the material used in that PCOMP, the thickness of the PCOMP,
and the orientation(s) of each layer within the PCOMP entry. Note that each of the

107
orientation listings does not have to be the same length: some of the rows in this file
indicate 4 orientations and some list only 3.

2. Close the text editor and return to HyperMesh Desktop.

Step 5: Use the sample.csv file to create new PCOMP entries

1. In the Aerospace menu, select Aerospace > Composites > PCOMP from CSV.
2. Use the Select file button to select sample.csv

Fig 4.29: Importing CSV file

3. Click Create to generate new PCOMP entries from the existing information in
sample.csv.

Step 6: Review the new property entries

1. Expand the Property section in the Model Browser to review the new entries.

Fig 4.30: Model Browser

108
 2. Use the Entity Editor to review each property and compare with the
information in sample.csv.

Using Orientation tools

This exercise introduces the user to using the element orientation tools within the
Aerospace Toolbar to set the zero-angle direction for each element. The model
provided is a plate with hole test coupon.

Fig 4.31: Plate with hole test coupon

Step 1: Open coupon.hm using the Aerospace User Profile in HyperMesh

Desktop

Step 2: Use the Model Browser to review the existing geometry and mesh
1. Using the Model Browser, expand the Component section of the model tree.

2. Click the mesh display icon to toggle off the mesh display for the
plate_with_hole component.

This reveals 3 lines within the model: one horizontal line along the top edge of the
coupon, a vertical line spanning half the left edge of the coupon, and a circular arc
inscribed within the hole in the center of the plate.

109
Note also that the plate is angularly offset with respect to all 3 global axes.

3. Toggle the mesh display for the plate_with_hole component back on.

Step 3: Review the existing element-based orientation

1. On the 2D page, enter the composites panel.

2. In the material orientation subpanel, click on the comps entity selector to choose
the plate_with_hole component.

3. Click review to show the current material orientation as a vector at the centroid of
each element.

Fig 4.32: Material orientation

4. Note that the current material orientation is set to the default, which is set as
the direction of each element first two nodes.
5. Exit the composites panel.

Step 4: Set the material orientation using the curves available in the model
1. In the Aerospace menu, click Aerospace > Composites > Material Orientation
to bring
up the Material Orientation dialog box.

110
2. Use the elems entity selector to select all the elements in the model.
3. With the Orientation Method: set to By curve, enable the Lines entity selector
and click the line at the top of the test coupon.
4. Click Apply to use the endpoints of this line to define the new zero-degree
direction for this component.

Fig 4.33: Material Orientation Window

5. Reselect all elements in the model and use the line along the left edge of the
plate to redefine the zero-degree material orientation.

111
 6. Finally, use the circular line around the hole in the center of the plate to define
the zero degree material orientation

Fig 4.34: Material Orientation assigned to the model using different methods

Sewing tool
Use this tool to connect two dissimilar 2D shell meshes using RBE3 connection. If the
nodes are close to each other within a tolerance they will snap without creating the
RBE3 connection.

112
1. Select the global finite element model (GFEM). The free edges that need to
be connected will be displayed.
2. Select the detailed finite element model (DFEM). The free edges that need to
be connected will be displayed. The Height and Node Snap tolerances will
automatically be calculated. You can change these.
3. Click Sew. This will connect 2D shell meshes with RBE3 elements.

Fig 4.35: Two dissimilar materials connected using RBE3 elements

113
114
 5 Post-Processing for
Composites

5.1 Overview of Composite Post-Processing

Composites post-processing is enhanced in HyperView with the reorganization of ply
results as layers. Output results depends on the control cards defined in the Pre-
process. For composite analysis basically CSTRESS, CSTRAIN and CFAILURE will be
defined in the control cards. CSTRESS is used to contour plot the composite stress
results of the model, CSTRAIN is used to contour plot the composite strain results of
the model, whereas, CFAILURE is defined to contour plot the elements/region which
fails during the analysis according to the failure theory defined in the property.

• Ply results are grouped together

• The ply filter is applied through layers in the Contour, Iso, and Tensor plot panels
• Quickly cycle through the plies for a given result type

Standard aggregation modes include min/max/extreme/sum/average/range

• These process the results across multiple plies and contour plot the corresponding
values
• The Layer Filter allows you to aggregate the results only on selected plies
• An Envelope loadstep provides a snapshot of results taken from multiple
loadsteps

115
 Fig 5.1: Composite results in HyperView

5.2 Ply-Based Composite Post-Processing

Individual ply results are available when using ply-based modeling

• Strain tensor components (e)

• Stress tensor components (s)
• Principal/Invariant strain (e1, evm)
• Principal/Invariant stress (s1, svm)
• Traditional failure theories (Max Strain, Tsai-Wu, Hill, etc…)

Automatically search through ALL plies for Min/Max

• Min/Max result
• Min/Max layer

116
 Fig 5.2: Contour plot of composite strain for individual ply

5.3 Tutorial: Simulating a Plate with a Hole, Test

Coupon

This tutorial requires the user to set up, load, and analyze a standard plate coupon
with a hole in the center. The analysis will require users to create everything
necessary for the analysis in the HyperMesh Desktop environment except for the
mesh and material properties.

Step 1: Open the model in HyperMesh Desktop with the OptiStruct user profile

Step 2: Update the plate_with_hole element orientations to align with the global X-
axis

117
 Fig 5.3: Plate with hole model
Step 3: Create a new PCOMPP property card with the following properties and assign the
property to the plate_with_hole component

118
Step 4: Create four plies which use all elements in the model to define the
ply shape and which have the following parameters
Tip: Ensure that Output results is checked.

Name Material Thickness Orientation Color

Zero mat8 0.05 0 Blue

Forty-five mat8 0.05 45 Yellow

Ninety mat8 0.05 90 Red

Negative Forty-five mat8 0.05 -45 Green

Fig 5.4: Create Laminate Window

Step 5: Create a new laminate, stacking the plies in the following order

Step 6: Create a new load collector named SPC

Fig 5.5: Load collector entity editor

Step 7: Create SPC constraints in DOFs 1-6 along the X- edge of the plate
1. In the Analysis page, enter the constraints panel.
2. With the nodes entity selector active, select the row of nodes along the X-
edge of the mesh.
3. Ensure that all of the DOF check boxes are marked and click create. Click
return to close the constraints panel.

119
 Fig 5.6: Model constrained at one end

Step 8: Create a new load collector named Force

Step 9: Create a force of 10 units in the Y-axis direction on node 2111

1. In the Analysis page, enter the forces panel.
2. With the nodes entity selector active, select node 2111 using the by id option.
3. Set the system toggle to global system, the magnitude to 10, and the
direction dropdown to y-axis.
4. Click create to create the force. Click return to close the forces panel.

120
Fig 5.7: Model with Constrains and Load
Step 10: Create a linear static loadstep named Lateral with the SPC set to the SPC
load collector and LOAD set to Force load collector

Fig 5.8: Loadstep Entity Editor

Step 11: Enable output of composite strain and composite stress results
1. On the Analysis page, enter the control cards panel.
2. Click next and click on the GLOBAL_OUTPUT_REQUEST button.
3. Check the box for CSTRAIN and set FORMAT(1) to H3D, TYPE(1) to ALL, and
OPTION(1) to ALL.
4. Check the box for CSTRESS and set FORMAT(1) to H3D, TYPE(1) to ALL, and
OPTION(1) to ALL.
5. Click return to exit the GLOBAL_OUTPUT_REQUEST section.

121
Step 12: Save the model and run in OptiStruct

Step 13: Post-process the stress and strain contours from the plate analysis
in HyperView
1. Load <filename>.h3d in HyperView for post-processing

Fig 5.9: Normal X Strains of plate_with_hole_analysis.h3d

Fig 5.10: Displacement profile of plate_with_hole_analysis.h3d

122
Here is a short video on Plate-with-Hole analysis

Analysis of a composite plate - Altair University

5.4 Exercise1: How changing the angle changes the

results?

Create a similar plate with same single ply and material direction - 0o in X-axis. Fix one
end of the plate and apply a force of 100N in X-direction and record Normal stress.
Change material direction by 10o each time till 90o without changing the direction of
force. Observe the changes in results.

5.5 Exercise2: Create a laminate of T Shaped Beam

as shown using sub-laminates and interfaces.
Use the T-Beam model file.

123
Tip: Use PCOMPP property for modelling
(Reference: https://youtu.be/LCrF1QlCdM)

124
 6 Composite Optimization
This Chapter contains contents from Jeffrey A. Wollschlager’s “Introduction to the
Design and Analysis of Composite Structures” book. (Grey texts)

6.1 Composite Design Characteristics and

Challenges
Composite material structures offer unprecedented freedom and flexibility: material
properties can be locally tailored

• How can FE simulation assist in determining the best use of these characteristics?

Characteristics Challenges

Design Complexity: how to

Enhanced material properties optimally define geometry,
Materials, patches, plies,
angles, stacking sequence?

Development phase
Complex manufacturing compression:
processes How to reduce design time?

How to mitigate re-design risk?

How to evaluate manufacturing

Manufacturing costs costs vs. design performances?

Fig 6.1: Composite Design Characteristics and Challenges

125
6.2 Composite Design Costs and Complexity
The trade-offs between design and manufacturing are intrinsically related to the
mechanical efficiency of part design and the cost to manufacture

Integrated ribs
Manufacturing Ply drop-offs
Costs Complex stacking
Manufacturing
Complexity Plate design
Ply drop-offs
Complex stacking

Plate design
One laminate
Complex stacking

Plate design One

laminate Quasi isotropic
n
[0°, 90°, +-45]S

Mechanical Design
efficiency complexity

Fig 6.2: Composite Design Costs and Complexity

126
 6.3 Optimization-Assisted Composite Design
Optimization-assisted composite design infuses the traditional design process with
FE-based manufacturing considerations and streamlined composite design
automation tools

Geometry
Design Design
definition
(CAD) (CAD)

Structural
Design Integrated
optimization
(CAE)
(CAD) design
Verification Verification
and analysis
(CAE) (CAE)
Virtual
verification Verification
(CAE)
Optimization
(CAE)

Physical
verification Physical Test Physical Test Physical Test

(a) (b) (c)

Fig 6.3: a) Traditional design. b) Optimization improvement of existing design.

c) Optimization driven design process

OptiStruct optimization transforms FE models into insightful optimized design

solutions

• Solution for concept and pre-design of complex composite structures

• Streamlined process based on structural optimization and process automation

127
6.4 What is OptiStruct Optimization?
OptiStruct optimization solves for the optimum value of an objective function based
upon the response of the model to its load cases by changing model geometry and
properties

• OptiStruct is a gradient-approach optimization platform

• OptiStruct can utilize any of the analysis types available in the HyperWorks suite
• OptiStruct iterates your solution based on responses from your existing model
and load cases

Fig 6.4: Optimization concept

6.5 Optimization Setup Module in HyperMesh

Optimization entities can be created in HyperMesh in one of three areas

Fig 6.5: a) Optimization option

128
 Fig 6.5: b) Model Browser

Fig 6.5: c) Optimization Menu

i. Definition of Design Variables

Fig 6.6: a) Optimization Panel

129
 Fig 6.6: b) Optimization Menu

Fig 6.6: c) Model Browser - Optimization View

130
 ii. Definition of Responses

Fig 6.7: a) Optimization Menu

Fig 6.7: b) Model Browser - Optimization View

Fig 6.7: c) Optimization > Responses option

Fig 6.7: d) Optimization > Responses Panel

131
 iii. Definition of Design Constraints

Fig 6.8: a) Optimization Menu

Fig 6.8: b) Model Browser - Optimization View

Fig 6.8: c) Optimization > dconstraints option

Fig 6.8: d) Optimization > dconstraints Panel

132
 iv. Definition of Objective

Fig 6.9: a) Optimization > Objective Panel

Fig 6.9: b) Optimization Menu

Fig 6.9: c) Model Browser -
Optimization View

Fig 6.9: d) Optimization > Objective option

133
6.6 Factors affecting composite optimization
Factors which affect the composite optimization are:

• Part Geometry
• Ply Geometry
• Material Data
• Mesh Data
• Material Alignment Information
• Lay-up sequence
• Z-Offset Information
• Drape Information

In an analysis, each of these factors contributes to the overall performance of the part
Composite optimization seeks to maximize performance and minimize the
opportunity for part failure.

6.7 Extrapolating Optimization from Composite

Analysis
Isotropic Material Failure Determination
• Von Mises Stress determines failure
• Geometry changes (shape or thickness) will prevent failure

Composite Material Failure Determination

• In what ply is the failure?

• Is the failure in the fiber or matrix?

• Will changing the stacking sequence prevent failure?

By these criteria we can deduce that for every composite part there is a combination
of number of plies at various ply angles, stacked in a given ply sequence for a given
geometry that constitutes an “optimum” – that is, the structure is as robustly
designed as possible for a given load set

134
6.8 Composite Optimization: Three Steps from
Concept to Final Design
Optimization can take a composite part all the way from initial concept to updated
product. Composite optimization-driven-design is a three-step process

 Phase I - Concept: Free-Size or Topology Optimization

• Free-Size and Topology design formulation
• Manufacturing constraints
 Phase II – Dimension: Ply-Bundle Size Optimization with ply-based FEA modeling
• All behavior constraints
• Manufacturing constraints
 Phase III – Sequence: Ply Stacking Sequence Optimization
• All behavior constraints
• Stacking manufacturing constraints

Fig 6.10: Optimization Process

Each step in the composite optimization process is able to integrate manufacturing

constraints appropriate to the optimization type.

135
i. Free Size Optimization

Free-Size Optimization is a concept-level optimization that optimizes the thickness of

each ply on an element-by-element basis.

SMEAR technology is used in composite design optimization, where the stacking

sequence of the laminate being optimized is initially indeterminate.

Laminate will have following effects on ABD matrices when smear technology is used
as the laminate type:

• [A]smear = Stacking Sequence independent

• [B]smear = 0 (Symmetric)
• [D]smear = [A]smear (T2/12) - Stacking Sequence Independent

The results of this optimization illustrates the optimized geometric ply boundaries

• Elements are grouped into sets according to these geometries

• This process is known as ‘ply tailoring’

Fig 6.11: i) Free Size Optimization graphical representation

136
ii. Size Optimization

Size Optimization is a fine-tuning-level optimization that optimizes the thickness of

tailored plies

• Ply-based modeling tracks the continuity of plies across patches automatically,

rather than requiring designers to track hundreds or thousands of ‘zones’
• Following a ply bundle sizing optimization, the number of plies required per
orientation can be established simply by dividing each ply thickness by the
thickness of the basic manufacturable ply

Sizing
optimization

Fig 6.11: ii) Size Optimization graphical representation

137
iii. Shuffling Optimization
Shuffling Optimization is a composite-specific optimization that shuffles the plies from
the results of the sizing optimization to determine the optimal stacking sequence

• The shuffling process establishes the final ply-book for the optimized composite
structure
• Composite shuffling optimization works within any additional manufacturing-
specific constraints imposed on the expected ply continuity within stacking
sequence

Sizing Shuffling
optimization optimization

Fig 6.11: iii) Shuffle Optimization graphical representation

6.8.1 Phase 1: Free Size Optimization

In Free Size Optimization, OptiStruct answers the question “What ply shapes, for each
ply layer, would build up the most efficient composite part?” based on the responses
and constraints associated with the specified objective.

• For example, consider the following cantilevered plate with a

point load at the unconstrained end (fig 6.12)
• The initial model contains plies at 0, 90, 45, and -45 degrees
• There is an initial thickness of each ply within each element
• This optimization considers performance independent of stacking sequence by
using SMEAR parameters (SMEAR technology is enabled by setting the LAM field
on the STACK card to SMEAR or SYMSMEAR)

138
• OptiStruct should produce a minimum mass structure (objective)
• The displacement at the load application point must not exceed 0.6 (constraint)
• The thickness of each ply is allowed to vary between zero and its initial thickness
for each element
• Ply angles cannot be altered in free size optimization, so the optimization will only
utilize the angles in the initial model – 0, 45, -45, and 90 degrees
• There is no limitation on the number of distinct ply angles which may be included
within a model

0°

+45°

-45°

90°
Superply Level

SMEAR-PARAMETER SET
constraints
DOF 123

90°
directio 3

0° direction

Fig 6.12: Cantilever plate subjected to point load

T0°

0°

90° T-45°
45°
-45°

PCOMP, PCOMPG, or PCOMPP

Variable: ‘Ti’ of each Super-Ply-Element

139
The general process for defining a composite free-size optimization is described in this
section.
1. Define composite free-size design variables
The composite free-size design variables are the thickness of every ply for every
element. Say for example, we are considering four plies 0/90/−45/45 with 2,240
elements. Therefore, 8,960 thickness design variables will exist in this composite free-
size optimization. Unlike topology optimization, in which the optimization algorithm
is “pushing” the design variables to either their lower or upper bound, the free-size
optimization algorithm allows the thickness design variables to “freely” be any value
between their lower and upper bounds. In this light, the composite free-size
optimization algorithm captures the coupling between total element thickness and
the relative percentage of each ply’s thickness to the total element thickness (i.e. the
laminate family). As an example, if the composite free-size optimization algorithm
decides it needs to increase an element thickness, it has a choice of ply by which to
achieve the increase in element thickness. If it chooses to increase the 0o ply
thickness, as opposed to the 90o ply thickness, the stiffness increase effect due to the
increase in element thickness will be significantly amplified in the 0o direction by the
selection of the 0o ply. Therefore, the free-size optimization algorithm is not only
optimizing on the total element thicknesses, but also on the relative percentage of
each ply’s thickness to the total element thickness (i.e. the laminate family). It is
important to state again that SMEAR technology should be utilized at the composite
free-sizing stage; thus, making the optimization problem stacking-sequence
independent. With SMEAR technology, regardless of the stacking sequence or how
ply thicknesses grow or shrink (i.e. add or remove plies within that ply layer), the
composite free-size results will be the same. Composite free-size design variables are
defined in OptiStruct through the DSIZE bulk data card.

140
 Fig 6.13: Composite Free-Size Design Variables

Free Size Optimization utilizes property identification numbers (PIDs) as a marker of

which elements make up the design space.

• For this reason, elements that are part of the optimization design-space must
have a separate property card from the non-design elements
• Multiple property cards may be referenced in one DSIZE entry
• All property referenced on a free size optimization DSIZE card share the same
parameters for manufacturing control, symmetry, etc.

The free size optimization panel, create subpanel allows design variable creation for
DSIZE

• For composite optimization, the optimization type must be set to the appropriate
property type: PCOMP or PCOMP(G)
• Minimum and maximum element thickness (via create subpanel) are not valid for
composite optimization

141
 Fig 6.13: Free size optimization panel

2. Define composite manufacturing constraints

The manufacturability of a new part is a critical design-level consideration. OptiStruct

is able to generate designs which meet various manufacturing criteria

• Manufacturing constraints include such design specifications as planar, radial, and

cyclical symmetries, pattern repetition across multiple parts
• Manufacturing constraints specific to composites, such as minimum laminate
thickness, may also be added to free-size optimization
• For the plate example, manufacturing constraints can be used to produce a
balanced laminate
• Ply Balance constraints request that OptiStruct produce identical structural
shapes and thickness contours for the 45 and -45 degree ply angles

Using Manufacturing Constraints for Practical Design Concepts

Minimum member size control (mindim) specifies the smallest dimension to be
retained in concept-level optimization designs

• Controls checker board effect and discreteness

• Min Member Size > 3 x mesh size
• The smallest mindim available in a run is dependent on average mesh size

142
 d = 60 d = 90

Fig 6.14: Different design pattern for different mindim

Without min member size

• Difficult to manufacture due to micro structures
• Results are mesh dependent

Pattern grouping
Pattern grouping provides model symmetry control during optimization
• The amount of control is indicated by how many planes of symmetry are needed
• Each plane of symmetry is specified by a normal vector
• 1-plane symmetry has one anchor node which serves as the base of the plane and
a first node which orients the vector
• 2- and 3-plane symmetries add second and third nodes, respectively, for
orthogonal planes

143
 Original Model

No grouping 1-pln symmetry (YZ) 1-pln symmetry (XZ) 2-pln symmetry (XZ & YZ)

Fig 6.15: Different pattern grouping results

Cyclic Repetition is pattern grouping for structures utilizing axial rotation symmetry
• Symmetry definitions are similar to planar pattern grouping
• Allows cyclic repetition of design features within a single domain
• User enters number of wedges and specifies an axis
• Use case: cyclic structures & non-symmetric loadcases

144
 Fig 6.16: Cyclic Repetition - Pattern grouping

Pattern repetition reproduces topological results in different structural components

Package spaces can be of:
• different sizes
• different meshes
• different components
• Scale patterns to different design regions
• Applied results may also be spatially reoriented according to user control

Fig 6.17: a) Topology without pattern

145
 Package Space
Package Space

Package Space
Package Space
F

3
2

4
1

Fig 6.17: b) Beam with 4 design areas:

All package spaces shall have similar topology
Package
Space 1

Fig 6.17: c) Topology with pattern repetition: 3 repetitions

A practical application example of pattern repetition is airplane wing ribs

• Same topology on every rib

• Scaling factor to account for different sizes of design space

Fig 6.18: a) Without pattern repetition

146
 Fig 6.18: b) With pattern repetition

The free size optimization panel update subpanel allows the modification of basic
design variable information for DSIZE design variable cards

Fig 6.19: a) Free size optimization update sub-panel

The free size optimization panel parameters subpanel allows users to adjust the
minimum dimension of members formed by the optimization

• Used to eliminate small members

• Also eliminates checkerboard results

Fig 6.19: b) Free size optimization parameters sub-panel

The free size optimization panel pattern grouping subpanel allows the creation of
planar and radial symmetry options

147
 Fig 6.19: c) Free size optimization pattern grouping sub-panel
The free size optimization panel pattern repetition subpanel allows users to create
scaled and replicated pattern repetition zones within the optimization model design
space

Fig 6.19: d) Free size optimization pattern repetition sub-panel

Composite-Specific Manufacturing Constraints for Optimization

In the free size optimization panel, composites subpanel allows the creation of
composite-specific manufacturing constraints for optimization. Composite
manufacturing constraints provide a mechanism for the free-size optimization
algorithm to produce manufacturable designs and avoid the trivial “all 0 degree”
optimized design result. The composite manufacturing constraints include; total
laminate thickness constraints, ply group percentage constraints, ply balancing
constraints, ply group constant thickness constraints, and ply group drop off
constraints. Each composite manufacturing constraint is defined in figure 6.20(a)
through figure 6.20(f) below. Composite manufacturing constraints for free-size
optimization are defined in OptiStruct through the DSIZE bulk data card, COMP
continuation lines.

148
 n
LT = ∑ tk , i
k =1

LTMIN < LT < LTMAX

Fig 6.20: a) Total Laminate Thickness Manufacturing Constraint

n
LT = ∑ tk , i
k =1

PGT = ∑ tk ,i

PGT
PGP =
LT
PGPMIN < PGP < PGPMAX
Fig 6.20: b) Ply Group Percentage Manufacturing Constraint

149
 PGT 1 = ∑ tk ,i

PGT 2 = ∑ tk ,i

PGT 1 = PGT 2
Fig 6.20: c) Ply Group Balancing Manufacturing Constraint

PGT = ∑ tk ,i

PGT = CTHICK
Fig 6.20: d) Ply Group Constant Thickness Constraint

∆t tk ,i − tk ,1+ i
PDMAX = tan(θ ) = =
∆d ∆d
Fig 6.20: e) Ply Group Drop Off Constraint

150
 Fig 6.20: f) Free size optimization composites sub-panel

3. Define Response, Constraint & Objective

After creating the design variable, the responses, constraint, and objective can be set
up
Response: Measurement of system performance
• For this example, the responses would be total mass & displacement at node
where load is applied

Constraint Functions: Bounds on response functions of the system that need to be

satisfied for the design to be acceptable

• For the plate example, the maximum displacement at the load application point
must be less than 0.6

Objective Function: Any response function of the system to be optimized. The

response is a function of the design variables

• The design objective is to have a lightweight structure; the objective function will
be to minimize the mass

Optimization Responses Available Within OptiStruct

These responses are commonly used in optimization with OptiStruct:
• Mass (MASS) and Volume (VOLUME) – Total and Regional
• Compliance, strain energy (COMP) – Total and Regional

C = 1�2 𝑈𝑈 𝑇𝑇 𝑓𝑓 ; with ku = f or C = 1�2 𝑈𝑈 𝑇𝑇 𝐾𝐾𝐾𝐾 = 1�2 ∫ 𝜀𝜀 𝑇𝑇 𝜎𝜎𝜎𝜎𝜎𝜎 …… 6.2

151
• Weighted Compliance (WCOMP) - 𝐶𝐶𝑤𝑤 = ∑ 𝑊𝑊𝑖𝑖 𝐶𝐶𝑖𝑖 = 1�2 ∑ 𝑊𝑊𝑖𝑖 𝑈𝑈𝑖𝑖 𝑓𝑓𝑖𝑖 …… 6.3

�𝜆𝜆𝑖𝑖 …… 6.4
• Natural Frequency (FREQ) - 𝑓𝑓𝑖𝑖 =
2𝜋𝜋
• Inverse of Weighted Eigenvalues (WFREQ)
𝑤𝑤𝑖𝑖
𝑓𝑓𝑤𝑤 = ∑ ; with [𝐾𝐾𝑖𝑖 − 𝜆𝜆𝑖𝑖 𝑚𝑚]𝑈𝑈𝑖𝑖 = 0 …… 6.5
𝜆𝜆𝑖𝑖

• Combination of Weighted Compliance and Weighted Inverse Eigenvalues (COMB)

∑𝑊𝑊𝑖𝑖�
𝜆𝜆𝑖𝑖 …… 6.6
𝑆𝑆 = ∑ 𝑊𝑊𝑖𝑖 𝐶𝐶𝑖𝑖 + 𝑁𝑁𝑁𝑁𝑁𝑁𝑁𝑁 ∑ 𝑊𝑊𝑖𝑖
NF = 𝐶𝐶𝑚𝑚𝑚𝑚𝑚𝑚 𝜆𝜆𝑚𝑚𝑚𝑚𝑚𝑚

Other Optimization Responses Available in OptiStruct

Other common optimization responses include:
• Nodal Displacements (DISP)
• Stress (STRESS)
• Buckling Mode (LAMA)
• Center of Gravity (COG)
• Force (FORCE)
• Mass Moments of Inertia (INERTIA)
• Strain (STRAIN)
• Composite stress, strain, failure (CSTRESS, CSTRAIN, CFAILURE)
• Frequency response displacements, velocity, acceleration (FRDISP, FRVELO,
FRACCL)
• Frequency response stress (FRSTRE), strain (FRSTRA), force (FRFORC)

152
Defining Response, Constraint & Objective in OptiStruct

The response optimization panel allows the creation of responses of various types

Fig 6.21: a) Response optimization panel

The dconstraint optimization panel links the created responses with upper- or lower-
bound constraints

• Note that some responses are only valid within the context of an applied loadstep
• In this case, HyperMesh Desktop will ask the user to specify which loadstep should
be used for evaluating the constraint

Fig 6.21: b) dconstraint optimization panel

The objective optimization panel determines which response is to be used as the
objective
An objective may be set to:

• Minimize or maximize a response

• Min(mass) – minimize the mass of the total model
• Minmax or maxmin an objective reference
• Minmax(stress) – minimize the maximum stress for the selected elements

The response used within the objective may not be used for any other constraint

153
 Fig 6.21: c) objective optimization panel

4. Create control cards

Create control cards to define additional optimization output results and output
formats. Thickness optimization results and automatic free-size to size model output
generation should be requested. Thickness optimization results are requested in
OptiStruct through the THICKNESS i/o options card. Optimization output formats are
defined in OptiStruct through the OUTPUT i/o options card. Use OUTPUT, FSTOSZ to
automatically output a size model containing the “sliced” ply results from the free-
size model.

5. Post-process the composite free-size optimization results.

When post-processing Free Size Optimization, results should be considered on several

levels:

• Global: was the optimization able to achieve objectives and meet constraints?
• Tailored Patch: What are the size, shape, and ply depth of the optimized regions?
• Response: Is the analysis of the optimized structure reasonable?

When contour plotting thickness results, the total thickness of the composite layup
may be broken down by ply angle

154
 Fig 6.22: a) Free size optimization results

For each ply angle, the tailored patch shapes represent superply bundles which are
generally split into four levels of resolution

• Users can define a different number of ply bundles per orientation to tune the
complexity of the design
• The super ply bundles can be visualized using the Contour panel or the isosurface
display
• The elements within each tailored patch ply bundle can be automatically exported
by OptiStruct

155
 0° Plies

90° Plies

+45° Plies
Linked by Ply
Balance
Manufacturing
Constraint

-45° Plies

Fig 6.22: b) Tailored patch shapes

Free-Size to Size Optimization Output Automation

Using the control card output parameter FSTOSZ instructs OptiStruct to generate
element sets and new property cards from ply bundles at the end of Phase 1
optimization

• Useful for transitioning automatically from FreeSize to Size Optimization

• Creates a new *.sizing.fem deck
• Number of ply bundles can be specified in the output

156
 0

90

45

-45

Level setting Ply-Bundles: 0° plies Level setting Ply-Bundles: ±45° plies

Level setting Ply-Bundles: 90° plies

Fig 6.23: Level setting Ply-Bundles for different orientations

There are two important output files; *_des.h3d and *_sizing.#.fem. The *_des.h3d
file contains the composite free-size optimization thickness results which can be
contour plotted to facilitate interpretations of the resulting optimized ply shapes.
However, the most important output file is the *_sizing.#.fem file. This file contains
a “run ready” composite size optimization input file. While this file is “run ready”, it
is highly suggested to import and modify this model within a pre-processor

157
(HyperMesh) as necessary. The significant advantage to the *_sizing.#.fem file is that
optimized ply shapes from the composite free-size optimization are contained in this
file; and design variables and design variable property relationships for the thickness
of each ply shape are automatically generated. Ply shapes are generated for each ply
by “slicing” the composite free-size optimization thicknesses of a single ply for every
element as shown in figure 6.20 (e). This process is repeated for every ply and the
resulting composite free-size ply shapes are shown in figure 6.24.

Fig 6.24: Composite Free-Size Ply Shape Generation

The ply numbering convention within OptiStruct is [LPPSNN].

Where;
• L is the laminate number (1, 2, 3, …) ≤ 9
• P is the ply number (01, 02, 03, …) ≤ 99
• S is the ply shape number for the given ply (1, 2, 3, …) ≤ 9
• NN counts the ply iterates for a given ply shape (01, 02, 03, …) ≤ 99

158
 Ply11100 (0°-Bundle1) Ply11200 (0°-Bundle2)

Ply11300 (0°-Bundle3) Ply11400 (0°-Bundle4)

Fig 6.25: design variables & Plies converted to sizing optimizations

Utilizing composite optimization FSTOSZ automation can also be used to extrapolate

cost/weight studies of proposed design changes to composite parts

6.8.2 Phase 2: Size Optimization

This step of the composite design optimization methodology answers the question;
“Exactly how many plies of each ply shape are required to satisfy strength and
manufacturing engineering requirements?” At this stage, both the part shape and the
ply shapes define the constant thickness zones are known. However, exactly how
many plies of each ply shape that are required to meet strength and manufacturing
engineering targets is unknown and needs to be determined through composite size
optimization technology. Composite size optimization is detailed design optimization
as opposed to composite free-size optimization which is concept design optimization.

159
• Size optimization models can be easily created from free-size optimizations
through FSTOSZ output parameter
• The optimization results determine the required number of plies per patch
• All behavior constraints and manufacturing constraints carry over from free-size
model using FSTOSZ
• Each ply bundle has a design variable (DESVAR) and design variable property
relationship (DVPREL)

Bundle1 Bundle2

Bundle3 Bundle4

Level setting Ply-Bundles: 0° plies

Bundle1 Bundle2
Bundle1 Bundle2

Bundle3 Bundle4 Bundle3 Bundle4

Level setting Ply-Bundles: ±45° Level setting Ply-Bundles: 90°

Fig 6.26: Level setting Ply-Bundles for different orientations

The general process for defining a composite size optimization is described in this
section.
1. Import the composite free-size *_sizing.#.fem file.
Make sure that all the ply bundles have the same initial thickness (i.e. sum of each ply
thickness in a bundle is same as the thickness of each ply given before free-size

160
optimization). Also make sure that a manufacturing thickness is defined for each ply
using the TMANUF field on the PLY bulk data card. This causes discrete ply thicknesses
to be selected during the composite size optimization. Finally, laminates should be
defined with symmetric smear technology by setting the LAM field on the STACK bulk
data card to SYSSMEAR. Symmetric smear makes the problem stacking-sequence
independent and ensures that a symmetric laminate will result by automatically
doubling the number of plies.

2. Define composite size design variables and design variable property

relationships
The *_sizing.#.fem file automatically defines design variables and design variable
property relationships for the thickness of each ply shape resulting from the
composite free-size optimization. However, it is suggested that the design variable
upper and lower bound limits be adjusted appropriately. By default, OUTPUT FSTOSZ
produces 4 ply shapes for each ply. Since we are considering 0/90/45/-45 plies in our
example, there will be 16 design variables. Design variables are defined in OptiStruct
through the DESVAR bulk data card. Design variable property relationships are
defined in OptiStruct through the DVPREL1 bulk data card.

3. Define composite manufacturing constraints

for the composite size optimization. The *_sizing.#.fem file automatically defines
composite manufacturing constraints as copies of those which were defined in the
composite free-size optimization. Composite manufacturing constraints provide a
mechanism for the size optimization algorithm to produce manufacturable designs
and avoid the trivial “all 0 degree” optimized design result. The composite
manufacturing constraints include; total laminate thickness constraints, ply group
percentage constraints, ply balancing constraints, ply group constant thickness
constraints, and ply group drop off constraints

161
4. Define responses
For the composite size optimization, if needed you can change response type like,
strains, stresses etc...

5. Define constraints
For the composite size optimization, you can define new constraint. For example, you
can give strain as a constraint.

6. Define the objective

For the composite size optimization, the objective can be minimize stress.

7. Create control cards

To define additional optimization output results and output formats. Thickness
optimization results and automatic size to shuffling model output generation should
be requested. Thickness optimization results are requested in OptiStruct through the
THICKNESS i/o options card. Optimization output formats are defined in OptiStruct
through the OUTPUT i/o options card. Use OUTPUT, SZTOSH to automatically output
a shuffling model containing the ply thickness results (i.e. # of plies) from the size
model.

8. Size Optimization Setup – Design Variable Notes

Using FSTOSZ to export a Size Optimization setup will link DESVAR and DCOMP entries
with DVPRELS

• Manufacturing entries from DSIZE are automatically carried over to DCOMP

• All DVPRELs and DESVARs are linked and sizing parameters are automatically
created

Activating the output parameter SZTOSH takes the results of the completed size
optimization and prepares a *.shuffling.fem deck for composite shuffling optimization

162
 Fig 6.27: a) SZTOSH control card panel

9. Size Optimization Results

The results of size optimization give the optimum thickness for each ply bundle

• When ply thickness is known, this thickness can be converted into number of plies
• Results are output under the final iteration listed in the *.prop file following
optimization

90 DEG
0 DEG

45 DEG - 45 DEG

Fig 6.27: b) Size Optimization Results

The results of size optimization give the optimum thickness for each ply bundle

163
 Fig 6.27: c) Optimum thickness for each ply bundle

10. Post-process the composite size optimization results

The most important output file is the *_shuffling.#.fem file. This file contains the
number of plies of each ply shape which are required to meet the strength and
manufacturing engineering targets. Importing the *_shuffling.#.fem into a
preprocessor (HyperMesh) shows the final number of plies for each ply shape. In

164
addition, the .out file contains the same information for each iteration of the
composite size optimization. Reviewing this file after each optimization is a suggested
practice. Still, even after a composite size optimization, the final design is not
completely defined. The exact stacking sequence for the plies is still unknown and
will be determined in the next step, composite shuffling optimization.

6.8.3 Phase 3: Composite Shuffling Optimization

This step of the composite design optimization methodology answers the question;
“What are possible stacking sequences that satisfy final part manufacturing
requirements?” At this stage many things are known; including the part shape, the
ply shapes which define the constant thickness zones, and even the exact number of
plies of each ply shape are known. However, exactly how to stack those plies to meet
manufacturing engineering requirements is unknown and needs to be determined
through composite shuffling optimization.

• Shuffling optimization models can be created from size optimizations through

SZTOSH output parameter
• The optimization results determine the final stacking sequence for the model
• Ply book rules can be entered on the composite shuffle panel parameter
subpanel

Ply Shuffling

Fig 6.28: a) Ply shuffling – Optimum stacking order

The general process for defining a composite shuffling optimization is described in this
section

165
1. Import the composite size *_shuffling.#.fem file
2. Add shuffling design variable manufacturing constraints
Typically, the maximum successive number of plies for all ply orientations are limited
to four with zero violation. The maximum successive number of plies for a given layer
is defined via the MAXSUCC continuation line on the DSHUFFLE bulk data card. A
cover stacking sequence is typically defined as [-45/0/45/90] with as many repeats as
necessary. The cover stacking sequence defines the plies at the top and bottom
surface of the laminate. The cover stacking sequence is defined via the COVER
continuation line on the DSHUFFLE bulk data card. Finally, a core stacking sequence
can be defined with as many repeats as necessary. The core stacking sequence
defines the plies at the middle surface of the laminate. The core stacking sequence is
defined via the CORE continuation line on the DSHUFFLE bulk data card.

Fig 6.28: b) composite shuffle panel parameter subpanel

3. Post-process the composite shuffling optimization results

The most important output file is the *.prop file. This file contains the final stacking
sequence which meets the strength and manufacturing engineering targets.
Importing the *.prop with FE-overwrite into a preprocessor (HyperMesh) will produce
the final verification model. In addition, the *.shuffle.html file contains information
on the stacking sequence as the shuffling optimization iterations progressed to the
final stacking sequence. This file can provide useful information and it is suggested
practice to review the file contents. However, the final design is not complete. The
final design must be verified to meet the desired strength and manufacturing
engineering targets. This last step will be discussed in the next section.

166
Shuffling Optimization Results
The results of shuffling optimization give the final stacking sequence for the part

• Results are highly dependent on manufacturing conditions specified for

optimization

Reversed
Pairing Core Cover
Successive Successive Pairing
Initial No rules constraint [0/45/- [0/45/-
ply limit = 3 ply limit = 2 constraint
45/-45 45/90] 45/90]
45/-45

90 0 0 0 0 0 0 0

90 0 0 0 0 0 0 45

90 0 0 -45 0 0 0 -45

90 0 -45 0 0 0 45 90

45 45 0 0 45 45 -45 0

45 -45 45 45 -45 -45 45 0

45 45 45 45 45 -45 -45 0

45 -45 45 90 -45 45 45 45

-45 -45 90 45 45 45 -45 -45

-45 45 45 45 -45 -45 90 -45

-45 45 -45 -45 45 -45 90 45

-45 -45 -45 -45 -45 45 90 -45

0 90 90 90 90 90 90 45

0 90 90 90 90 90 -45 90

0 90 90 -45 90 90 45 90

167
 0 90 -45 90 90 90 0 90

The results of shuffling optimization give the final stacking sequence for the part
• Results are available visually in an *.html file & STACK written in *.prop file

Fig 6.29: a) Stacking sequence - *.html file

Stacking Sequence before Optimization

Stacking Sequence after Optimization

Fig 6.29: b) Stacking sequence before and after optimization

168
6.8.4 Final Design Verification
This step of the composite design optimization methodology verifies the final design
meets the strength and manufacturing engineering requirements by performing an
analysis on the final design as given from the results of the shuffling optimization.

6.9 Tutorial: Bike Frame Optimization using

PCOMP and PCOMPG

In this tutorial, you learn the steps required to perform a ply orientation optimization
for a composite structure. The figure 6.30. below illustrates the model that will be
used for this exercise.

Fig 6.30: Bike frame model

Model file: https://altairuniversity.com/learning-library/composite-optimization-

tutorial-bike-frame/

169
The optimization problem for this tutorial is stated as:

Objective : Minimize volume.

Constraints : A given maximum Nodal Displacement.

Design Variables : Layer thickness.

In this tutorial, You will :

• Set-up a size optimization of a Composite Bike Frame.

• Post-process the composite size optimization results in HyperView.

1. Import the model:

Goto file > open > bicycle_frame.hm > open.
You can see bicycle_frame model in the graphic area

You can see that Properties, Materials and Control cards are already assigned
to the model as shown below figure 6.31.

170
 Fig 6.31: Model Browser view

2. Create Load Collectors:

Let us imagine the type of loads acting on the bicycle frame. The first load would be
point load on the pedal (downward direction) and second will be the moment caused
due to pedalling.

• Hence, to define the above loads, right click on the model browser > Create >
load Collector > name it as Crank.
• Then from Analysis panel goto Forces > Create > nodes, select a node at the
centre of the spider as shown in the image below.
• Enter value for the magnitude as -100 (downward load) and direction to Z-axis.
And leave rest all the parameters as shown in the image.
• Click Create. And you can see a force of magnitude 100N created.

171
 Fig 6.32: Force applied to the model

Now keeping same (Crank) load collector current, let us assign moment load.

• Goto Analysis panel > Moments > Create > nodes, select the same centre node
of the spider as before. Let the magnitude be 100 and direction X-axis (Pedalling
Direction), leave rest all parameters same as shown in below image. Click create.
You can see a moment force in the X-direction created.

172
 Fig 6.33: Moment applied to the model

3. Defining Boundary Constraints:

• Constraints (All DOF) will be applied to the rear wheel location of the frame and
to the Head-tube location (Handle) of the frame.
• Right click on the model browser > create > Load collector, name it as SPC.
• Now, goto Analysis panel > Constraints > create > nodes, select the two node as
shown in the image below. And set all other parameters as shown. Click create.

173
 Fig 6.34: SPC applied to the rear wheel location of the frame

Similarly assign constraints for the Head-Tube.

Fig 6.35: SPC applied to the Head-tube (Handle location) of the frame

4. Creating Load Steps:

• Goto Analysis panel > Load steps, click name and enter Crank. Toggle type to
Linear-Static.

174
• Check the box preceding SPC, click on the entry field and select the SPC load-
collector from the list.
• Next, check the box preceding load. Click on the entry field and select the Crank
Load-collector from the list.
• Leave rest all parameters as shown in the below image and click create. Return.

5. Set-up the Design variables:

Here, we set-up a limit to which extent the thickness of each ply is allowed to deform
from its original value, by defining upper and lower bound value.

To set-up this, goto 2d panel > Hyperlaminate, this launches a Hyperlaminate GUI.
Perform the following steps:
i. Expand Design Variable in the laminate browser, the DESVAR branch will
appear.
ii. Right click on DESVAR, click New.
iii. Rename it as “thk1” and set all other parameter as shown below.

175
 Where, “Initial value” is the thickness of the original ply and “Upper-bound” value
is the allowable deformation value.
iv. In a similar manner, and with identical values, create a total of 5 Design
Variables.

v. Now, the above Desvar’s is assigned to “Seat-Tube”.

In the same GUI, click on laminates in the laminate browser and expand the
PCOMP tree and select Seat-tube laminate.
Check the optimization box. New fields appear in the Ply lay-up order table, which
allows you to assign the Design Variables to each ply.
Click on the field under Designvar and assign thk1 to the first ply and thk2 to the
second and so on as shown in below image.

Fig 6.36: Assigning thickness under Designvar field

176
vi. Now in the same manner assign the Design variables to “top-tube” and
“bottom-tube” laminates.
vii. Exit the Hyperlaminate GUI by closing.

6. Create a Displacement and Volume Response:

Create a response to measure the total displacement of the node where the loads
have been applied and set the objective to minimize this response.

Goto Analysis panel > Optimization > Responses, name the Response = Disp. Click the
response type and switch to Static displacement. Click on nodes and select the node
at the bottom bracket on which loads were applied, click total disp. Click create.

In same panel rename Response = Volume, switch the response type to Volume >
Total. Click create.

Return to optimization panel.

7. Create constraints on the Displacement Response:

In the optimization panel, goto > dconstraints, constraint name = Disp. Set the upper-
bound value as 1.8. Click response and select Disp from the response list. Click on
loadsteps and select Crank. Click create.

*A constraint is defined on the Response Disp. It states that any solution (min vol)
needs to have a displacement lesser than 1.8mm is to be feasible.

177
8. Define Objective:
The objective is to minimize volume. To define this, goto Analysis > optimization
panel > Objective, toggle to “min” and Response = Volume. Click create. Return
twice.

9. Run the optimization:

In the Analysis panel, Click optistruct. Set all other parameters as shown in the image
below and click save as.

Click optistruct to run the Analysis. After the analysis is complete, a dialogue box
opens as shown below.

178
10. Post-Processing the composite size optimization results in the
Hyperview: ( Reviewing the results in HyperGraph)

In the same window shown in the above image click on view and select
bicycle_frameopt_hist.mvw file. It takes you to HyperGraph window. This file contains
Objective, Constraints and Design Variable’s against iteration history. You can see 9

pages of graph by clicking this icon.

179
The first page shows the Objective function.

Second page shows Maximum Constraints Violations.

The next pages shows the Design Variables for each iterations.

180
6.10 Optimization Example Videos
This below video demonstrates Optimization of composite structures using
HyperMesh- OptiStruct

Altair University _OptiStruct for Composite Analysis _Optimization -

Altair

6.11 Tutorial: Composite Optimization on A Solar

Car Carbon Fiber Shock Mount
(written by Arnold Kadiu, University of Michigan)

Introduction
The purpose of this tutorial is to give engineers a firsthand experience with composite
analysis and optimization. It is based off a simplified shock mount used on a Solar Car
Vehicle. The model is used to demonstrate the process of optimizing a carbon fiber
laminate. The mount is optimized using a realistic set of constraints, loads, materials,
and program parameters.

The tutorial was prepared with HyperWorks version 17.2. The pre-processing was
executed with HyperMesh, the post-processing with HyperView, for the analysis and

181
optimization OptiStruct was used. A basic knowledge of HyperMesh is assumed when
completing this tutorial.

The mount is a layered carbon fiber piece that is adhered to the main structure of the
Solar Car. There were many different types of loads that are applied to this mount,
but due to it being a shock load, the largest predicted force was used. The model has
already been meshed, RBE-2 elements have been used, forces have been applied and
loadsteps have been made. For every section the appropriate hm/fem files are
available. This allows each section to be completed independently of another.

Model Setup

With composites, it is essential that after meshing the components the element
normals and orientations must all point in the same direction. This allows the engineer
to accurately analyze for materials heading in specific directions and optimize
effectively.
This is absolutely necessary for composites due to the different fiber directions. It is
recommended that the element normals and orientations are adjusted each time. A
few single elements that are misoriented can cause a completely inaccurate
optimization; wasting resources and time. Open model called:
shock_mount_element_adjustment.hm

Checking Element Normals

The elements are checked to see whether the element normals are facing the same
direction. To do this go to:

2D > Composites > element normals > elems > display normals

Notice that the menu below is set to color display normals, this can also be set to
vector display normals. They will both convey

Menu to View/Edit Element Normals

182
It is apparent in the image below that the element normals are not all facing the same
direction. This can be problematic in the setup and optimization.

Element Normals Are Different

Adjusting Element Normals

The elements must be adjusted to make sure that the model can be correctly finished.
Go to:

2D > Composites > element normals > elems > adjust normal

Figure: Adjusting Element Normals After

After adjusting the normals, they should all face the same direction, i.e. they are the
same color or the vectors are facing the same direction.

183
 Element Normals Pointing in The Same Direction

Checking Element Orientation

To check the orientation of the elements, go to:

2D > Composites > element orientation > elems > review

Orientations Are Not Facing the Same Direction

184
Adjusting Element Orientation

This step will change the elements so that they all align in the same coordinate system,
thus making sure that the 0 deg is the same for all the elements.

2D > Composites > element orientation > elems > system (by system id) > assign

Adjusting Element Orientation

Elements All Facing Same Direction

Material Creation

With isotropic materials such as steel or aluminum the strength is the same in all
direction, with composites this is not the case. This ties directly with the previous part
where we insured that all the elements are pointing the same direction. We will be
creating an orthotropic material, carbon fiber. Particularly with orthotropic materials,
it is essential to get as many of the properties of the material as possible. File is:
SM_Material_Setup.hm

185
To create a material, go to the top menu and go to: Materials > Create

Alternatively, right click in the model assembly > create> material

Once the material is created then the properties need to be input into the MAT8 Card.
The values given are just representative numbers for the purpose of this tutorial.

MAT8 Card Image

Creating A Laminate

In order to describe the various layers, thicknesses and orientation of each of the
composite layers many plies must be created. These plies then become a part of a
laminate/STACK. Creating the different layers using this method allows the use of the
PCOMPP property in conjunction with the laminate. We will only focus on the 00, 900,
and ±450. It is very possible to make the layers in orientations with 150 steps. Open
model SM_Laminate_Setup.hm

Creating Plies

Now that the material has been created, the individual plies must be made. A ply is a
representation of a layer of material which in this case is carbon fiber. To prepare for
optimization we will be creating thick layers of each direction, a superply, so that
OptiStruct can properly optimize the mount. For this step the ply is not a
manufacturable thickness, meaning a layer of carbon fiber will not be 2mm. That will
be added later steps in the optimization.

Right click in model browser > create > Ply > (Fill in Fields) > Elements > by collector
(shock mount) > Create

Try to keep a consistent naming structure to keep track of the plies.

186
For the optimization later we need to create the following plies:

Creating the Laminate

The created plies are now stacked into a Laminate. The laminate option is set to
smear, Other options are available and can be explored.

To create a laminate, go to: Model browser > Create > Laminate > add plies > create

187
Creating the Property

Now create a property using the PCOMPP card image. Right click in the model browser
and go to create Property. Once created, enter in a maximum interlaminar shear
stress, this example is based on the Hoffman theory.

Maximum Allowable
shear stress

Now that the property has been created, it needs to be applied to the elements. Right
click on the property in the model browser and go to assign. From there go to
elements > by collector > Shock Mount

Visualizing the Model

Now that the plies have been created, the laminate generated, the property created
and applied; the layers of the composite can now be seen. Adjust the settings on the
visualization panel. Afterwards change the colors on the individual plies by
highlighting all of the plies, right clicking on the color and choosing autocolor. Now
the plies can be seen independently. If desired, each ply can be selected or deselected
to view separately.

Visualizing the Plies

188
Baseline Analysis

In order to see how well the optimized model compares to the original we need to
analysis the model as is first to see how well performs in this configuration.

The mass of our initial model is 0.87 kg. This can be found by going to tools and then
selecting mass calc. For our analysis we would also like to look at CFAILURE, CSTRAIN
and CSTRESS (composite strain and stress) To activate this go to: Analysis > control
cards > GLOBAL_OUTPUT_REQUEST

Run the analysis: Analysis > OptiStruct

It is advised to keep the analysis files in a separate directory than your model files to
avoid confusion.

Once the analysis has run open the results in HyperView. Look at displacement. This
can be done by going to the visualization bar and then selecting the shock mount as
your component and apply.

It is recommended that the rigids are hidden to minimize confusion.

189
 Initial Displacement
Do the same to view Composite Stresses

Composite Stresses
In these results it shows the max stress at 63.9 𝑁𝑁�𝑚𝑚𝑚𝑚2 which is 63.9 MPa. However,
this number is not an entirely accurate number because it describes stress

190
concentrations are the single element. We can adjust the visualization to only show
values above a certain stress. After going to the following menu, we can see which
elements act as extreme outliers. We will set the value at 50.

Elements Over 50 MPa

Mass 0.87 KG
Displacement 0.0118 mm
Composite Stress (Max element) 63.9 MPa

1. Free Size Optimization

The primary focus will be on free size, size and shuffle optimizations. The metrics that
will measure the effectiveness of the optimization are maximizing the stiffness and

191
keeping mass under 400 grams. The optimization will be done using the load provided,
which is the maximum force the mount will receive.

The free size optimization will take the large plies, superplies, and change the
thickness of the composite plies according to the parameters it is given. Remember
that free size optimization can only take away material not add it. By varying the
thickness of each ply with a particular fiber orientation for every element, the total
laminate thickness can change throughout the structure. That is why the superplies
were created above to ensure that OptiStruct can create the most efficient structure.

Setup

Setup for a free size optimization involves creating a number of parameters and
responses for OptiStruct to follow when performing the optimization. Additional
control cards will also be added to output the results in the desired format. The ones
used in this tutorial are only some of the options available when choosing response
and parameters for the optimization.

Defining the Free Size Design Variable

Create a new free size design variable. Its type will be set to STACK, make sure the
variable is created before continuing. Go to: Analysis > optimization > free size >
create

Creating Design Variable

Manufacturing Constraints

Manufacturing constraints will be added to make the optimization more feasible to

manufacture. First, we will set a minimum dimension through the parameters menu.
This makes it so OptiStruct will not optimize element groups smaller than a specified

192
size. The next thing is the balance constrain which makes certain ply directions
symmetric. And last we will specify is the thickness constraint, which limits how thick
or thin OptiStruct can make the laminate.

Setting the Minimum Dimension

Set the size of the mindim to 25 mm. This means that OptiStruct will make no ply
smaller than 25 mm on any side. This number will vary significantly based on the
application. The next step is making sure the 45° and -45° plies are placed
symmetrically and that the thickness of the laminate does not exceed 8mm or get
thinner than 2.

Creating Thickness Constraints

Creating Symmetry Constraint

193
Defining Responses for The Optimization

In this tutorial the responses “mass” and “compliance” are going to be used.
Many other responses and constraints can be used. Mass will be given an upper bound
of 400 grams and the objective of the optimization will be to minimize compliance.
This means that OptiStruct will create optimizations that stay under 400 grams while
minimizing compliance. Note that this is not trying to minimize stress. To create a
response: Analysis > optimization > responses

Creating Mass Response

Creating Compliance Response

Analysis > optimization >dconstraints

Setting Upper Limit of Mass to 400 Grams

Analysis > optimization > objective

Creating Objective to Minimize Compliance

194
Adjusting the Control Cards

In order for the optimization to run more optimal to our model, some changes are
made to the output settings and the control cards.

Analysis > optimization > opti control

Changing Max Iterations

In the above image the number of max design iterations is changed from 30 to 60.
This allows the program to continue trying iterations past 30 if it has not converged
on a solution by that point. In addition to this the OUTPUT Control Card must be
changed to export a detailed free size optimization result.

Analysis > control cards > OUTPUT

Control Card OUTPUT – FSTOSZ

Running the Optimization

Now the optimization can begin. Make sure that the run options is set to optimization
and the memory options is set reasonably. Leaving it at default is advised if hardware
specifications are unknown. However, if the specifications are known, increasing the
amount of maximum memory could allow the optimization to run much quicker.
However, for this tutorial, leaving it to the default value is enough.

Analysis > OptiStruct > optimization

195
 Running the Optimization
Free Size Results

Once the optimization has run press both the view out button and HyperView button.
Each shows different information in a different manner.

From view out we can see that all the constraints were met and that the optimization
has converged onto a feasible result.

196
Results in HyperView

The results in HyperView are more visual so they can assist more on the conceptual
level. Looking at the thickness of the elements is a good starting point.

Free Size Optimization Thickness Results

From the thickness results we can see that there are clear indications that less
material is needed and spots where more material could be beneficial. There is a large
section where the mount is at the upper limit of thickness and a large section where
it is at the lower limit. In these situations, it is up to the engineer to decide whether
changing the constraints is allowed with the design constraints and time constraints.
This is why it is always advised to include more material than thought into the
optimization.

197
Material Thickness More Than 6.6 mm Thick

198
 Material Less Than 3mm Thick
Viewing the Model in HyperMesh

Now that the element thicknesses have been viewed, it’s time to view the mounts
stress and displacement compared to the original. To do this the solver deck must be
imported into HyperMesh. Open SM_Free size.hm

199
Once the model is loaded, take the opportunity to look at the optimization at a ply by
ply level by selecting and deselecting plies on the left hand side.

Free Size Plies Visualized

Comparing Analysis Results

Run a basic analysis of the model to get a comparison stress, displacement, and mass.

200
 Post-Processing Of Free Size Optimization

Changes in Results After Optimization

These results show the effectiveness of OptiStruct. Mass and displacement went
down significantly. The stresses are also more distributed as opposed to the pre-
optimized model. Stress is up, but it should decrease in the later optimizations.

Changing the Original Model

As mentioned previously the engineer has the option to revise this model in order to
give OptiStruct more freedom when optimizing the structure. In this hypothetical
example the engineer has gone back and decided that the mount can be at its thickest
4 more mm and at its thinnest 0.5 fewer mm. Also, to give the program more choice,
each superply shall have a thickness of 5mm. However, further freedoms were limited

201
at this point because the engineer has decided that the cost to manufacture a
composite thicker than 12 mm is too costly.

The things that need to change:

• Each superply is 5 mm thick

• Max thickness of laminate is 12 mm
• Min thickness of laminate is 1.5 mm

Changing SuperPly Thickness

Changing Laminate Thickness

Run the Optimization and Compare the Models

Run the optimization and then import the result back into HyperMesh similar to the
previous steps. Then compare the results.

202
New Free Size Plies Visualized

203
 New Composite Stresses
Original Free_Size Free_Size_5mm
Mass 0.87 KG 0.50 Kg 0.55Kg
Displacement 0.0118 mm 0.13 mm 0.0045 mm
Composite Stress (Max
63.9 MPa 87.1 MPa 33.7 MPa
element)

As visible in the image above with these new constraints and freedoms, the laminate
is far more optimized with the new set of constraints. The mass will be reduced to 400
grams in the next optimization.

2. Size Optimization
The model as it is now can’t be manufactured. Each layer does not have a real
thickness or multiple of it. It also does not have other constraints that must be taken
into account to create a realistic composite. The discrete size optimization will change
it so each ply falls within a window of thicknesses.

204
Setup

To set up the size optimization, each ply will have a min and max thickness and an
individual ply thickness will be given. More responses and constraints can be added
at this point in the optimization if desired. To begin, open the file that was just
analysed or the file named SM_Free size_sizing.14.fem

Understanding the Naming System for Plies

If you look to the model browser, the name of each of the plies has changed from
what it was originally. This was done during the optimization process and has a basic
nomenclature to understand its meaning.

205
Adjusting TMANUF

In this step the ply property TMANUF, manufacturing thickness value, will be
specified. This setting forces the ply to be a multiple of the number inputted. In this
case 0.25 mm will be used. Each ply bundle must be a multiple of this number. This
number varies on the material chosen.

Adjusting TMANUF
Adjusting Ply Design Variables

Each ply had its own design variable created in the free size process. Now those are
going to be edited to make them more in line with the goals in mind. Each upper
boundary will be changed according to the table below. Make sure to update each
layer. These values vary based on what the engineer would like for the size of the ply
bundles.

206
Analysis > Optimization > size

Listed Upper Ply Bounds

Additional Setting Changes

In addition to the changes that have been made, the main design variable should be
changed to a composite size design variable and the output file must also be changed
into a size optimization output. Make sure to update the variable when finished.

To the main design variable go to:

Analysis > Composite size > Parameters

From there select the old Design for dcomp and change the parameters to suit the
same parameters as before.

• Min Thickness: 1.5

• Max thickness: 12
• Ply Balance: ±45°

207
 Updating Design Variable

The output file must also be changed to size optimization output. Change it to SZTOSH.
Go to:

Analysis > control cards > OUTPUT

Run the Optimization

Run the optimization like the previous models.

Run the optimization by going to:

Analysis > OptiStruct > optimization

Size Results

As before view the output file and view the results in HyperView. In this case it seems
that OptiStruct could not converge on a solution that meets all of the criteria. It
appears that the mass constraint has been violated by 16 grams on the final iteration.
It ends up being a 4% over the design criteria, in this case we will deem this acceptable.

If this violation can’t be tolerated, then changes must be made to minimum

thickness, maximum thickness, max ply thickness, or a number of other variables,
however, these are not a guarantee that the optimization will converge to a solution.

208
 Mass Constraint Violated
Results in HyperView

Open the results in HyperView. In this case we can see that the material thickness
easily conforms to the thickness constraints created.

Size Optimization Element Thickness

Results in HyperMesh

Import the solver deck into a new model. The file to import is called
SM_sizing.14_shuffling.9.fem

Once open visualize the plies as done previously. There will be many more plies than
before, this is because each ply is now representative of an actual layer of carbon

209
fiber, whereas before, each ply was an arbitrary thickness of carbon fiber. Now there
are a total of 47 plies.

Plies Visualized

Comparing Analysis Results

Now that the plies have been visualized, the size results must be compared to free
size results. We should expect the displacement and stress numbers to rise slightly,
due to the layer thicknesses being non optimal and the actual mass decreasing. We
do however expect the estimated mass of 416 grams to be accurate.

In the results we can see that this is true. Displacement has increased to 0.0106 mm
and max composite stresses have increase to 52 MPa.

210
After Size Optimization: Displacement Results

Size Optimization: Stress Results

211
 Original Free_Size Free_Size_5mm Size

Mass 0.87 KG 0.50 Kg 0.55Kg 0.416 Kg

Displacement 0.0118 mm 0.13 mm 0.0045 mm 0.017 mm

Composite Stress (Max

63.9 MPa 87.1 MPa 33.7 MPa 55.4 MPa
element)

Clearly, an increase in displacement is unwanted, however the mount is now a

realistic representation of the part and meets our original design constraints. Also,
our values should further improve with the shuffle optimization and the part is still
better than the original model while being less than half the original mass.

3. Shuffle Optimization
In this set the optimal ply sequence will be determined. Currently, the ply schedule is
still vaguely the same as the original. This means it still follows the order by which we
created the original plies: 90, -45, +45, and 0 (looking at it from the outside of the
mount to the inside). This can be verified by visualizing the plies and then unselecting
the plies starting from the bottom. With the shuffle optimization, the plies will be
moved around in the schedule based on the constraints, load cases and responses
that we specify.

212
Setup
In this example little is needed besides a new set of constraints for the shuffle
optimization. However, in this step more responses and constraints can be added in
addition to the ones already created. The ones already created can be replaced as
well. For example, the mass constraint no longer applies because during the shuffle
optimization no mass is added or taken away. The mass response/constraint could be
replaced with a stress response/constraint.

Shuffle Design Variable Update

In this step the shuffle design variable will be updated and the parameters for the
shuffle will be specified. Go to:

Analysis > composite shuffle > parameters

Select the dshuffle as the original design name selected. Afterwards select edit so that
a constraint for successive plies can be created. This constraint is created based on
the application. Generally unidirectional plies cannot be stacked in sequence more
than 4-5 plies. However, since this is a thin mount we will stick to a max of 2 plies in
succession. This could hurt our theoretical results, but the theoretical results will be a
closer representation of the real world results. The max succession of plies is
determined on a case by case basis.

Editing DSHUFFLE

• DSHUFFLE_NUMBER_OF_MAXSUCC: number of ply constraints

• MANGLE: angle of ply specified

213
• MSUCC: How many plies can be placed in sequence
• VSUCC: Number of times the constraint is allowed to be violated

Lastly select the pairing constraint to have a 45 degree constraint.

Make sure to update at the end.

Results
Run the file like the previous files by going to:

Analysis > OptiStruct > OptiStruct

If the mass constraint hasn’t been removed, it will tell you a constraint has been
violated because the mount will still weigh .416 kg. Once the files have run, view the
results.

Shuffle Optimization: Displacement

214
 Shuffle Optimization: Stress Results

Original Free_Size Free_Size_5mm Size Shuffule

Mass 0.87 KG 0.50 Kg 0.55Kg 0.416 Kg 0.416 Kg

Displacement 0.0118 mm 0.13 mm 0.0045 mm 0.017 mm 0.016 mm

Composite Stress
63.9 MPa 87.1 MPa 33.7 MPa 55.4 MPa 56.7 MPa
(Max element)

To view the Stacking Sequence, open the below html file in your folder.

215
216
Example: Three-wheeler Motorbike – Composite
optimization of the Fairing

Conceptual Design of a 3-Wheeler Motorbike – Composite optimization of the

fairing - Altair University

Conceptual Design of a 3-Wheeler Motorbike – Composite optimization of the

fairing - Altair University

217
Conceptual Design of a 3-Wheeler Motorbike – Composite optimization of the
fairing - Altair University

Conceptual Design of a 3-Wheeler Motorbike – Composite optimization of the fairing

- Altair University

218
Appendix A
All the Appendix in this book are taken from Jeffrey A. Wollschlager’s “Introduction to
the Design and Analysis of Composite Structures” book.

OptiStruct I/O Options Reference

CSTRAIN
Defines composite ply strain output. Composite ply strains are output at the middle
of each ply.

CSTRAIN (FORMAT, TYPE, EXTRA) = OPTION

Argument Description
FORMAT Defines the output format. (Default = blank)

ASCII - Results are output to the ASCII file formats.

H3D - Results are output to the *.h3d file format.
OP2 - Results are output to the *.op2 file format.
Blank - Results are output in all active formats defined on the OUTPUT
card.

TYPE Defines the strain components to output. (Default = ALL)

ALL – All strain components and principals are output.

PRINC – Only principal strains are output.

EXTRA Defines extra parameters for composite strain output.

MECH - Total and mechanical strains are output.

219
 THERM - Total and thermal strains are output.

OPTION Defines the output options. (Default = ALL)

ALL – Results are output for all elements.

NONE – Results are not output.
SID – Results are output for all elements defined by the element set
identification number.

PID – Results are output for all elements that reference the properties
defined by the property set identification number.

220
CSTRESS
Defines composite ply stress output. Composite ply stresses are output at the middle
of each ply.

CSTRESS (FORMAT, TYPE) = OPTION

Argument Description
FORMAT Defines the output format. (Default = blank)

ASCII - Results are output to the ASCII file formats.

H3D - Results are output to the *.h3d file format.
OP2 - Results are output to the *.op2 file format.
Blank - Output in all formats defined on the OUTPUT card.

TYPE Defines the stress components to output. (Default = ALL)

ALL – All stress components, principals, and failure indices are output.
PRINC – Only principal stresses are output.
FI – Only failure indices are output.

OPTION Defines the output options. (Default = ALL)

ALL – Results are output for all elements.

NONE – Results are not output.
SID – Results are output for all elements defined by the element set
identification number.

PID – Results are output for all elements that reference the properties
defined by the property set identification number.

221
DISPLACEMENT
Defines grid point displacement output.

DISPLACEMENT (FORMAT) = OPTION

Argument Description
FORMAT Defines the output format. (Default = blank)

ASCII - Results are output to the ASCII file formats.

H3D - Results are output to the *.h3d file format.
OP2 - Results are output to the *.op2 file format.
Blank - Results are output in all active formats defined on the OUTPUT
card.

OPTION Defines the output options. (Default = ALL)

ALL – Results are output for all grids.

NONE – Results are not output.
SID – Results are output for all grids defined by the node set
identification number.

222
OUTPUT
Defines active output formats for an analysis or optimization run.

OUTPUT, FORMAT, FREQUENCY

Argument Description
FORMAT Defines the output format.

Analysis Results Output Formats

H3D - Results are output to the binary *.h3d file format.
OP2 - Results are output to the binary *.op2 file format.
ASCII - Results are output to the OptiStruct ASCII file formats (*.cstr
composite stress/strain, *.disp displacement, *.force, *.gpf grid point
forces, *.load applied load, *.mpcf multi-point constraint forces,
*.spcf single point constraint forces, *.strs stress/strain)

PUNCH - Results are output to the Nastran *.pch file format.

Optimization Results Output Formats

FSTOSZ - Automatic generation of a size optimization model at the
last iteration of the free-size optimization. (*_sizing.#.fem)

SZTOSH - Automatic generation of a shuffling optimization model at

the last iteration of the size optimization model. (*_shuffling.#.fem)

DESVAR - Outputs the updated design variables for the given iteration
to the *.desvar and/or *.out files.

PROPERTY - Outputs the updated property cards for the given

iteration to the *.prop and/or *.out files.

223
FREQUENCY Defines the frequency at which results are output.
(Default = FL)

FIRST - Results are output for the first iteration only.

LAST - Results are output for the last iteration only.
FL - Results are output for the first and last iterations.
ALL - Results are output for all iterations.
N= - Results are output for the Nth iteration.
NONE - Results are not output.

224
THICKNESS
Defines element and ply thickness output for topology, free-size, and size design
optimizations.

THICKNESS (FORMAT, COMP) = OPTION

Argument Description
FORMAT Defines the output format. (Default = blank)

ASCII - Results are output to the ASCII file formats.

H3D - Results are output to the *.h3d file format.
OP2 - Results are output to the *.op2 file format.
Blank - Output in all formats defined on the OUTPUT card.

COMP Defines composite ply thickness output options.

(Default = DESIGN)

ALL - Outputs the thickness of all plies

DESIGN - Only outputs the thickness of designable plies.
NOPLY - No ply thickness is output.

OPTION Defines the output options. (Default = ALL)

ALL – Results are output for all elements.

NONE – Results are not output.

225
226
Appendix B
OptiStruct Analysis Bulk Data Reference
MAT1
Defines a linear elastic, temperature independent, isotropic material definition for
rod, beam, shell, and solid elements.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

MAT1 MID E G ν ρ α TREF GE

ST SC SS

Field Comments
MID Material identification number.

E Young’s modulus of the material.

G Shear modulus of the material.

ν Poisson’s ratio of the material.

ρ Mass density of the material.

α Coefficient of thermal expansion of the material.

TREF Reference stress free temperature of the material. Can be overridden by

the TREF field on the PCOMP/G or PCOMPP cards. Typically not used.

GE Damping coefficient of the material.

ST Tension stress allowable of the material.

SC Compression stress allowable of the material.

SS Shear stress allowable of the material.

Note: Stress allowables are used in laminated plate failure theory

calculations if the FT field is specified on the PCOMP/G or PCOMPP card.

227
MAT2

Defines a linear elastic, temperature independent, anisotropic material definition for

shell elements.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

MAT2 MID Q11 Q12 Q13 Q22 Q23 Q33 ρ

α1 α2 α3 TREF GE ST SC SS

Field Comments
MID Material identification number.

Qij Components of the plane stress stiffness matrix in the material

coordinate system. See Chapter 3 for details on calculation of the plane
stress stiffness matrix for a given linear elastic material law.

ρ Mass density of the material.

αi Coefficient of thermal expansion of the material in the 1-, 2-, and 3-

directions.

TREF Reference stress free temperature of the material. Can be overridden by

the TREF field on the PCOMP/G or PCOMPP cards. Typically not used.

GE Damping coefficient of the material.

ST Tension stress allowable of the material.
SC Compression stress allowable of the material.
SS Shear stress allowable of the material.

Note: Stress allowables are used in laminated plate failure theory

calculations if the FT field is specified on the PCOMP/G or PCOMPP card.

228
MAT8

Defines a linear elastic, temperature independent, orthotropic material definition for

shell elements.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

MAT8 MID E1 E2 ν12 G12 G13 G23 ρ

α1 α2 TREF Xt Xc Yt Yc S

GE F12 STRN …

Field Comments
MID Material identification number.

E1 Modulus of elasticity of the material in the 1-direction (fiber).

E2 Modulus of elasticity of the material in the 2-direction (matrix).

ν12 Poisson’s ratio of the material on the 1-plane in the 2-direction.

G12 Shear modulus of the material on the 1-plane in the 2-direction.

G13 Shear modulus of the material on the 1-plane in the 3-direction.

G23 Shear modulus of the material on the 2-plane in the 3-direction.

ρ Mass density of the material.

αi Coefficient of thermal expansion of the material in the 1-direction (fiber)

and 2-direction (matrix).

TREF Reference stress free temperature of the material. Can be overridden by

the TREF field on the PCOMP/G or PCOMPP cards. Typically not used.

Xt Tension stress or strain allowable of the material in the 1-direction (fiber).

Xc Compression stress or strain allowable of the material in the 1-direction

(fiber).

229
Yt Tension stress or strain allowable of the material in the 2-direction
(matrix).

S In-Plane shear stress or shear strain allowable of the material.

GE Damping coefficient of the material.

F12 Tsai-Wu interaction term. Used only if FT field is set to TSAI.

STRN Indicates if Xt, Xc, Yt, Yc, and S fields are entered as stress allowables (0
or blank) or strain allowables (1). (Default = blank).

230
MAT9
Defines a linear elastic, temperature independent, anisotropic material definition for
solid elements.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

MAT9 MID C11 C12 C13 C14 C15 C16 C22

C23 C24 C25 C26 C33 C34 C35 C36

C44 C45 C46 C55 C56 C66 ρ α1

α2 α3 α4 α5 α6 TREF GE

Field Comments
MID Material identification number.

Cij Stiffness matrix coefficients of the material as defined in

chapter 3.

ρ Mass density of the material.

αi Coefficient of thermal expansion vector of the material as defined in

chapter 3.

TREF Reference stress free initial temperature of the material. Overridden by

the TEMPERATURE(INITIAL) card in the subcase control section. Typically
not used.

GE Damping coefficient of the material.

231
MAT9ORT
Defines a linear elastic, temperature independent, orthotropic material definition for
solid elements.
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

MAT9ORT MID E1 E2 E3 ν12 ν23 ν31 ρ

G12 G23 G31 α1 α2 α1 TREF GE

Field Comments
MID Material identification number.

E1 Modulus of elasticity of the material in the 1-direction (fiber).

E2 Modulus of elasticity of the material in the 2-direction (matrix).

E3 Modulus of elasticity of the material in the 3-direction.

ν12 Poisson’s ratio of the material on the 1-plane in the 2-direction.

ν23 Poisson’s ratio of the material on the 2-plane in the 3-direction.

ν31 Poisson’s ratio of the material on the 3-plane in the 1-direction.

G12 Shear modulus of the material on the 1-plane in the 2-direction.

G23 Shear modulus of the material on the 2-plane in the 3-direction.

G31 Shear modulus of the material on the 1-plane in the 3-direction.

Equivalent to G13.

ρ Mass density of the material.

α1 Coefficient of thermal expansion of the material in the 1-direction.

α2 Coefficient of thermal expansion of the material in the 2-direction.

α3 Coefficient of thermal expansion of the material in the 3-direction.

TREF Reference stress free initial temperature of the material. Overridden by

the TEMPERATURE(INITIAL) card in the subcase control section. Typically
not used.
GE Damping coefficient of the material.

232
PCOMP
Defines the property definition of a laminated plate for composite zone-based shell
modeling.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

PCOMP PID Z0 NSM SB FT TREF GE LAM

MID1 t1 θ1 SOUT1 MID2 t2 θ2 SOUT2

MID3 t3 θ3 SOUT3 MID4 t4 θ4 SOUT4

PCOMPG
Defines the property definition of a laminated plate with global ply identification for
composite zone-based shell modeling.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

PCOMPG PID Z0 NSM SB FT TREF GE LAM

GPLYID1 MID1 t1 θ1 SOUT1

GPLYID2 MID2 t2 θ2 SOUT2

GPLYID3 MID3 t3 θ3 SOUT3

PCOMPP
Defines the property definition of a laminated plate for composite ply based
modeling.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

PCOMPP PID Z0 NSM SB FT TREF GE

Field Comments
PID Property identification number.

Z0 Distance from the element reference plane to the bottom ply of the
laminated plate. See figures below for Z0 conventions. (Default: −T ∕ 2)

233
NSM Nonstructural mass per unit area applied to the laminated plate.

SB Interlaminate shear stress allowable of the laminated plate.

FT Laminate failure output option. If blank, no failure output calculations

are performed on the laminate. In addition, material allowable fields on
the ply MAT cards and the SB field must be entered to perform failure
output calculations. (Default: blank)

HILL - Tsai-Hill failure theory.

HOFF - Hoffman failure theory.

TSAI - Tsai-Wu failure theory.

STRN - Max Strain failure theory.

TREF Reference stress free temperature of the laminated plate. Overrides the
TREF field on the MAT card referenced by each ply. If TREF is not
specified, then each TREF field on the MAT card referenced by each ply
must have the same TREF value.

GE Damping coefficient of the laminated plate.

LAM Laminate stacking sequence option. If blank all plies must be specified.
(Default = blank)

SYM - Only plies on the bottom half of the laminate need to be specified.
This option is not valid for PCOMPG card.

MEM - All plies must be specified, however only [A] matrix terms are
calculated. Therefore, the laminated plate exhibits extension behavior
only. Any Z0 entry is ignored and set to the default value (−T ∕ 2).

234
BEND - All plies must be specified, however only [D] matrix terms are
calculated. Therefore, the laminated plate exhibits bending behavior
only. Any Z0 entry is ignored and set to the default value (−T ∕ 2).

SMEAR - All plies must be specified and SMEAR technology is utilized to

calculate the ABD matrix of the laminate. Any Z0 entry is ignored and set
to the default value (−T ∕ 2).

SMEARZ0 - All plies must be specified and SMEAR technology is utilized

to calculate the ABD matrix of the laminate. The Z0 entry is considered
in the calculation of the ABD matrix. Unlike SMEAR technology,
SMEARZ0 will develop a B matrix due to the Z0 term. If Z0 is set to the
default value (−T ∕ 2), then SMEAR and SMEARZ0 will produce the same
ABD matrix.

SMCORE - All plies must be specified. The last ply specified must be the
core layer. All other plies define the “top” and “bottom” face sheet
laminates. Half of the total thickness of the laminate is placed on the
“top” of the core. The other half of the laminate thickness is placed on
the “bottom” of the core. SMEAR Core technology is utilized to calculate
the ABD matrix of the laminate. Any Z0 entry is ignored and set to the
default value (−T ∕ 2).

SYMEM - Only plies on the bottom half of laminate need to be specified,

however only [A] matrix terms are calculated. Therefore, the laminated
plate exhibits extension behavior only. Any Z0 entry is ignored and set to
the default value (−T ∕ 2). This option is not valid for PCOMPG card.

SYBEND - Only plies on the bottom half of the laminate need to be

specified, however only [D] matrix terms are calculated. Therefore, the
laminated plate exhibits bending behavior only. Any Z0 entry is ignored
and set to the default value (−T ∕ 2). This option is not valid for PCOMPG
card.

235
 SYSMEAR - Only plies on the bottom half of the laminate need to be
specified and SMEAR technology is utilized to calculate the ABD matrix of
the laminate.

GPLYIDk Global ply identification number of the kth ply. Must be unique with
respect to all other plies defined on the current PCOMP/G card.

MIDk Material identification number of the kth ply. Must refer to a MAT1,
MAT2, or MAT8 card. If MIDk is not specified for a ply, then the default is
the last defined ply’s MIDk.

tk Nominal thickness of the kth ply. If tk is not specified for a ply, then the
default is the last defined ply’s tk.

θk Nominal fiber orientation angle, in degrees, of the kth ply relative to the
x-axis of the element material coordinate system. See figures below for
θk conventions.

SOUTk Stress, strain, and failure output option of the kth ply. Ply stress, strain,
and failure output is given at the middle of each ply. In addition, OUTPUT
CSTRESS and/or OUTPUT CSTRAIN cards must be defined in the I/O
section to get output for the ply. (Default = NO)

NO – do not output stress, strain, or failure for the kth ply.

YES – output stress, strain, and failure for the kth ply.

236
PLY
Defines a ply for composite ply-based shell modeling

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

PLY ID MIDk tk θκ SOUTk TMANUFk DIDk

ESID1 ESID2 ESID3 ESID4 ESID5 ESID6 ESID7 ESID8

ESID9 …

Field Comments
ID Ply identification number.

MIDk Material identification number of the kth ply. Must refer to a MAT1,
MAT2, or MAT8 card.

tk Nominal thickness of the kth ply.

θκ Nominal fiber orientation angle, in degrees, of the kth ply relative to the
x-axis of the element material coordinate system. See figure below for θ
conventions. (Default = 0.0)

SOUTk Stress, strain, and failure output option of the kth ply. Ply stress, strain,
and failure output is given at the middle of each ply. In addition, OUTPUT
CSTRESS and/or OUTPUT CSTRAIN cards must be defined in the I/O
section to get output for the ply. (Default = NO)

NO – do not output stress, strain, or failure for the kth ply.

YES – output stress, strain, and failure for the kth ply

TMANUFk Actual manufactured ply thickness of the kth ply. This parameter is utilized
in composite size optimization to automatically create discrete design

237
 variables such that the thickness of the ply bundle is equal to an integer
multiple of TMANUF.

DIDk DRAPE data table identification number of the kth ply. A drape data table
is used to define draping data for a ply. A drape data table defines a ply’s
actual fiber orientation angle and thickness by specifying variations from
a ply’s nominal fiber orientation angle and thickness at the centroid of
each element that makes up the shape of a ply.

ESIDi Element set identification numbers that define the elements that define
shape of the ply. The superset of all elements defined by all referenced
element set IDs define the shape of the ply.

238
PSHELL
Defines the property definition of a homogeneous shell element.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

PSHELL PID MID1 T MID2 12I/T3 MID3 Ts/T NSM

Z1 Z2 MID4 T0 ZOFFS

Field Comments
PID Property identification number.

MID1 Material identification number for extension behavior of the plate. Must
reference a MAT1, MAT2, or MAT8 card. This field must not be blank. If
homogenizing by reference to a MAT2 card, see section 7.4 for calculation
of the equivalent homogenized material matrix [Q1 ] .

T Total thickness of the plate. Can by overridden by the Ti fields on the

CQUAD4 and/or CTRIA3 cards.

MID2 Material identification number for bending behavior of the plate. If blank,
then the plate has membrane behavior only. In addition, MID3 and MID4
fields must also be blank. If homogenizing by reference to a MAT2 card,
see section 7.4 for calculation of the equivalent homogenized material
matrix [Q2 ] .

12I/T3 Bending stiffness ratio of the plate. (Default = 1.0)

MID3 Material identification number for transverse shear behavior of the plate.
If blank, then MID2 field is used to calculate the transverse shear behavior
of the plate. If MID3 field is referenced by a MAT2 card, then Q33 field on
the MAT2 card must be blank. If MID3 field is referenced by a MAT8 card,
then G23 and G13 fields must not be blank. If homogenizing by reference

239
 to a MAT2 card, see section 7.4 for calculation of the equivalent
homogenized material matrix [Q3 ] .

Ts/T Transverse shear ratio of the plate. The transverse shear thickness
divided by the total thickness of the homogenized plate. (Default =
0.8333)

NSM Non-structural mass per unit area applied to the plate.

Z1 The first z-coordinate distance at which to calculate the stress and strain
output for the plate, typically the bottom of the plate. (Default: −T ∕ 2)

Z2 The second z-coordinate distance at which to calculate the stress and

strain output for the plate, typically the top of the plate. (Default: T ∕ 2)

MID4 Material identification number for extension-bending coupling behavior

of the plate. Cannot reference the same material as the MID1 or MID2
fields. If homogenizing by reference to a MAT2 card, see section 7.4 for
calculation of the equivalent homogenized material matrix [Q4 ] .

T0 Minimum homogeneous shell thickness. Valid for topology and free-size

optimization with MAT1 card only. Can be overridden by the T0 field on
the DSIZE card, THICK option. (Default = blank)

ZOFFS Offset from the element grid point plane to the reference plane of the
plate element. Can be overridden by the ZOFFS field on the CQUAD4
and/or CTRIA3 cards. See figures below for ZOFFS conventions.

240
241
STACK – Ply laminate definition
Defines the stacking sequence of a composite laminate for composite ply based
modeling using the ply laminate definition of the STACK card.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

STACK ID LAM PLY PLY PLY PLY PLY PLY

ID1 ID2 ID3 ID4 ID5 ID6

PLY … PLY
ID7 IDn

Field Comments
ID Stack identification number.

LAM Laminate stacking sequence option. If blank all plies must be specified.
(Default = blank)

SYM - Only plies on the bottom half of the laminate need to be specified.
This option is not valid for PCOMPG card.
MEM - All plies must be specified, however only [A] matrix terms are
calculated. Therefore, the laminated plate exhibits extension behavior
only. Any Z0 entry is ignored and set to the default value (−T ∕ 2).
BEND - All plies must be specified, however only [D] matrix terms are
calculated. Therefore, the laminated plate exhibits bending behavior
only. Any Z0 entry is ignored and set to the default value (−T ∕ 2).
SMEAR - All plies must be specified and SMEAR technology is utilized to
calculate the ABD matrix of the laminate. Any Z0 entry is ignored and set
to the default value (−T ∕ 2).
SMEARZ0 - All plies must be specified and SMEAR technology is utilized
to calculate the ABD matrix of the laminate. The Z0 entry is considered in
the calculation of the ABD matrix. Unlike SMEAR technology, SMEARZ0
will develop a B matrix due to the Z0 term. If Z0 is set to the default value
(−T ∕ 2), then SMEAR and SMEARZ0 will produce the same ABD matrix.

242
 SMCORE - All plies must be specified. The last ply specified must be the
core layer. All other plies define the “top” and “bottom” face sheet
laminates. Half of the total thickness of the laminate is placed on the
“top” of the core. The other half of the laminate thickness is placed on
the “bottom” of the core. SMEAR Core technology is utilized to calculate
the ABD matrix of the laminate. Any Z0 entry is ignored and set to the
default value (−T ∕ 2).

SYMEM - Only plies on the bottom half of laminate need to be specified,

however only [A] matrix terms are calculated. Therefore, the laminated
plate exhibits extension behavior only. Any Z0 entry is ignored and set to
the default value (−T ∕ 2). This option is not valid for PCOMPG card.

SYBEND - Only plies on the bottom half of the laminate need to be

specified, however only [D] matrix terms are calculated. Therefore, the
laminated plate exhibits bending behavior only. Any Z0 entry is ignored
and set to the default value (−T ∕ 2).This option is not valid for PCOMPG
card.

SYSMEAR - Only plies on the bottom half of the laminate need to be

specified and SMEAR technology is utilized to calculate the ABD matrix of
the laminate.

PLYIDk Ply identification number for the kth ply, defined in the order of the ply
laminate stacking sequence as given in the figure below.

243
244
STACK - Interface laminate definition
Defines the stacking sequence of a composite laminate for composite ply based
modeling using the interface laminate definition of the STACK card.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

STACK ID

SUB …

INT …

Continuation lines to define sub-laminates.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

SUB SIDi SNAMEi SPLY SPLY SPLY SPLY SPLY

IDi1 IDi2 IDi3 IDi4 IDi5

SPLY … SPLY
IDi6 ID1n

Continuation lines to define interface definitions.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

INT IPLYIDi1 IPLYIDi2

Field Comments
ID Stack identification number.

SUB Keyword used to define the start of a sub-laminate definition data block.
Multiple sub-laminate definitions can be defined on a single STACK card,
each of which begins with the SUB keyword.

SIDi Sub-laminate identification number for the ith sub-laminate definition.

SNAMEi Sub-laminate name for the ith sub-laminate definition.

245
SPLYIDik Sub-laminate ply identification number for the ith sub-laminate definition
for the kth ply, defined in the order of the sub-laminate stacking sequence
as defined in the figure below.

INT Keyword used to define the start of an interface definition data block.
Multiple interface definitions can be defined on a single STACK card, each
of which begins with the INT keyword. Each interface definition defines
exactly one interface laminate of a complete integrated structure.
IPLYIDi1

IPLYIDi2 Interface ply identification numbers defining the ith interface laminate
definition. Interface plies can be either the 1st or nth ply of a sub-laminate
definition and must come from different sub-laminates. IPLYIDi1 and
IPLYIDi2 stack in the direction of the element normal at the interface
between the two sub-laminates, which defines the directions the sub-
laminates stack. The interface laminate stacking sequence follows
directly as defined on the two sub-laminate stacking sequence definitions
from their interface plies to the ply on the opposite side of the sub-
laminate definition in their respective directions from the two interface
plies as defined in the figure below.

246
247
248
Appendix C
OptiStruct Optimization Bulk Data
Reference
DCOMP
Defines composite size optimization design manufacturing constraints.
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

DCOMP ID ETYPE EID1 EID2 EID3 EID4 EID5 EID6

EID7 …

Continuation to define total laminate thickness manufacturing constraints.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

LAMTHK LTMIN LTMAX LTSET LTEXC

Continuation lines to define ply group thickness percentage manufacturing

constraints.
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

PLYPCT PPGRP PPMIN PPMAX PPOPT PPSET PPEXC

Continuation lines to define ply group balancing manufacturing constraints.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

BALANCE BGRP1 BGRP2 BOPT

Continuation lines to define ply group constant thickness manufacturing constraints.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

CONST CGRP CTHICK COPT

Continuation lines to define ply group drop off manufacturing constraints.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

PLYDRP PDGRP PDTYP PDMAX PDOPT PDSET PDEXC

249
Field Comments
ID Composite size optimization manufacturing constraint identification
number.

ETYPE Entity type.

PCOMP – Specifies that the composite manufacturing constraints apply

to a PCOMP zone-based laminate definition
STACK – Specifies that the composite manufacturing constraints apply to
a STACK ply-based laminate definition.

EIDi Entity identification number. Must be PCOMP identification numbers for

ETYPE = PCOMP. Must be STACK identification numbers for ETYPE =
STACK.

LAMTHK Keyword used to define total laminate thickness manufacturing

constraints. Multiple LAMTHK definitions can be defined on a single
DCOMP card, each of which begins with the LAMTHK keyword.

n
LT = ∑ tk , i
k =1

LTMIN < LT < LTMAX

250
LTMIN Minimum laminate total thickness for the laminate total thickness
manufacturing constraint. (LTMIN > 0.0)

LTMAX Maximum laminate total thickness for the laminate total thickness
manufacturing constraint. (LTMAX > LTMIN)

LTSET Element set identification number defining the elements to which the
laminate thickness manufacturing constraint applies. (Default = All
Elements)
LTEXC Ply exclusion option indicating plies that are to be excluded from the
laminate thickness calculation for the laminate thickness manufacturing
constraint. (Default = CORE)

NONE - No plies are excluded from the calculation.

CORE - The core layer within a SMCORE laminate definition (i.e. the last
layer defined in the laminate definition) is excluded from the calculation.
If the referenced PCOMP or STACK card is not defined as a SMCORE
laminate, then there is no core layer defined.
CONST - Any ply defined with a CONST ply thickness manufacturing
constraint is excluded from the calculation.
BOTH – Both the core layer within a SMCORE laminate definition and any
ply defined with a CONST ply thickness manufacturing constraint are
excluded from the calculation.

PLYPCT Keyword used to define ply group percent thickness manufacturing

constraints. Multiple PLYPCT definitions can be defined on a single
DCOMP card, each of which begins with the PLYPCT keyword.

251
 n
LT = ∑ tk , i
k =1

PGT = ∑ tk ,i

PGT
PGP =
LT
PPMIN < PGP < PPMAX

PPGRP Ply group identification to which the ply group percent thickness
manufacturing constraint applies. Ply groups can be identified by nominal
fiber orientation angle, ply sets, or individual ply identification numbers
depending on the PPOPT setting.

PPMIN Minimum ply group percent thickness for the ply group percent thickness
manufacturing constraint. (PPMIN > 0.0)
PPMAX Maximum ply group percent thickness for the ply group percent thickness
manufacturing constraint. (PPMAX > PTMIN)

PPOPT Ply group identification option for the ply group percent thickness
manufacturing constraint. (Default = BYANG)

BYANG - Specifies that PPGRP is defined as a real number representing a

nominal fiber orientation angle. The ply group is defined as all the plies
which have the given nominal fiber orientation angle.

252
 BYSET - Specifies that PPGRP is defined as a ply set identification number.
The ply group is the set of plies which are defined in the referenced ply
set.

BYPLY – Specifies that PPGRP is defined as a single ply identification

number. The ply group is the individual ply referenced by the ply
identification number.

PPSET Element set identification number defining the elements to which the ply
group percent thickness manufacturing constraint applies. (Default = All
Elements)

PPEXC Ply exclusion option indicating plies that are to be excluded from the ply
group percent thickness calculation for the ply group percent thickness
manufacturing constraint. (Default = CORE)

NONE - No plies are excluded from the calculation.

CORE - The core layer within a SMCORE laminate definition (i.e. the last
layer defined in the laminate definition) is excluded from the calculation.
If the referenced PCOMP or STACK card is not defined as a SMCORE
laminate, then there is no core layer defined.

CONST - Any ply defined with a CONST ply thickness manufacturing

constraint is excluded from the calculation.

BOTH – Both the core layer within a SMCORE laminate definition and any
ply defined with a CONST ply thickness manufacturing constraint are
excluded from the calculation.

BALANCE Keyword used to define ply group balance manufacturing constraints.

Multiple BALANCE definitions can be defined on a single DCOMP card,
each of which begins with the BALANCE keyword.

253
 PGT 1 = ∑ tk ,i

PGT 2 = ∑ tk ,i

PGT 1 = PGT 2

BGRP1 Ply group #1 identification to which the ply group balance manufacturing
constraint applies. Ply groups can be identified by nominal fiber
orientation angle, ply sets, or individual ply identification numbers
depending on the BOPT setting.

BGRP2 Ply group #2 identification to which the ply group balance manufacturing
constraint applies. Ply groups can be identified by nominal fiber
orientation angle, ply sets, or individual ply identification numbers
depending on the BOPT setting.

BOPT Ply group identification option for the ply group balance manufacturing
constraint. (Default = BYANG)

BYANG - Specifies that BGRP1 and BGRP2 are defined as real numbers
representing the nominal fiber orientation angles. The ply group is
defined as all the plies which have the given nominal fiber orientation
angle.
BYSET - Specifies that BGRP1 and BRRP2 are defined as ply set
identification numbers. The ply group is the set of plies which are defined
in the referenced ply set.

254
 BYPLY – Specifies that BGRP1 and BGRP2 are defined as single ply
identification numbers. The ply group is the individual ply referenced by
the ply identification number.
CONST Keyword used to define ply group constant thickness manufacturing
constraints. Multiple CONST definitions can be defined on a single
DCOMP card, each of which begins with the CONST keyword.

PGT = ∑ tk ,i

PGT = CTHICK

CGRP Ply group identification to which the ply group constant thickness
manufacturing constraint applies. Ply groups can be identified by nominal
fiber orientation angle, ply sets, or individual ply identification numbers
depending on the COPT setting.

CTHICK Constant ply group thickness for the ply group constant thickness
manufacturing constraint. (CTHICK > 0.0)

COPT Ply group identification option for the ply group constant thickness
manufacturing constraint. (Default = BYANG)

BYANG - Specifies that CGRP is defined as a real number representing the

nominal fiber orientation angle. The ply group is defined as all the plies
which have the given nominal fiber orientation angle.

255
BYSET - Specifies that CGRP is defined as a ply set identification number.
The ply group is the set of plies which are defined in the referenced ply
set.
BYPLY – Specifies that CGRP is defined as a single ply identification
number. The ply group is the individual ply referenced by the ply
identification number.

256
PLYDRP Keyword used to define ply group drop off manufacturing constraints.
Multiple PLYDRP definitions can be defined on a single DCOMP card, each
of which begins with the PLYDRP keyword.

PDGRP Ply group identification to which the ply group drop off manufacturing
constraint applies. Ply groups can be identified by nominal fiber
orientation angle, ply sets, or individual ply identification numbers
depending on the PDOPT setting.

PDTYPE Specifies type of ply group drop of manufacturing constraint to apply.

(Default = TOTDRP)

TOTDRP uses the total laminate drop method to calculate the ply drop
manufacturing constraint.

n n
PDMAX = ∆t = ∑ tk ,i − ∑ tk ,i +1
k =1 k =1

PDMAX Maximum ply group drop off based on the PDTYPE setting. (PPMAX > 0)

PDOPT Ply group identification option for the ply group drop off manufacturing
constraint. (Default = BYANG)

BYANG - Specifies that PPGRP is defined as a real number representing a

nominal fiber orientation angle. The ply group is defined as all the plies
which have the given nominal fiber orientation angle.
BYSET - Specifies that PPGRP is defined as a ply set identification number.
The ply group is the set of plies which are defined in the referenced ply
set.

257
 BYPLY – Specifies that PPGRP is defined as a single ply identification
number. The ply group is the individual ply referenced by the ply
identification number.

PDSET Element set identification number defining the elements to which the ply
group drop off manufacturing constraint applies. (Default = All Elements)

PDEXC Ply exclusion option indicating plies that are to be excluded from the ply
group drop off calculation for the ply group drop off manufacturing
constraint. (Default = CORE)

NONE - No plies are excluded from the calculation.

CORE - The core layer within a SMCORE laminate definition (i.e. the last
layer defined in the laminate definition) is excluded from the calculation.
If the referenced PCOMP or STACK card is not defined as a SMCORE
laminate, then there is no core layer defined.
CONST - Any ply defined with a CONST ply thickness manufacturing
constraint is excluded from the calculation.
BOTH – Both the core layer within a SMCORE laminate definition and any
ply defined with a CONST ply thickness manufacturing constraint are
excluded from the calculation.

258
DCONADD
Defines an optimization design constraint as a combination of DCONSTR design
constraint definitions.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

DCONADD DCID DC1 DC2 DC3 DC4 DC5 DC6 DC7

DC8 …

Field Comments

DCID Design constraint identification number.

DCi DCONSTR identification numbers used to create a new design constraint

as the combination of referenced DCONSTR identification numbers.

259
DCONSTR
Defines an optimization design constraint.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

DCONSTR DCID RID LBOUND UBOUND LFREQ UFREQ

Field Comments
DCID Design constraint identification number.

RID Design response identification number for which to apply the design
constraint.

LBOUND Design constraint lower bound value for the referenced design response.

UBOUND Design constraint upper bound value for the referenced design response.

LFREQ Design constraint lower bound frequency value. This value only applies
to frequency design responses related to frequency response subcases.
The design constraints bounds, LBOUND and UBOUND, are applied only
if the loading frequency falls between LFREQ and UFREQ.

UFREQ Design constraint upper bound frequency value. This value only applies
to frequency design responses related to frequency response subcases.
The design constraints bounds, LBOUND and UBOUND, are applied only
if the loading frequency falls between LFREQ and UFREQ.

260
DDVAL
Defines a discrete design value list for an optimization design variable.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

DDVAL ID DVAL1 DVAL2 DVAL3 DVAL4 DVAL5 DVAL6 DVAL7

DVAL8 …

Alternate form of the DDVAL card:

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

DDVAL ID DVAL1 THRU DVAL2 BY INC

DVAL1 THRU DVAL2 BY INC

Field Comments
ID Discrete design value list identification number.

DVALi Discrete design values. Can be listed in any order.

THRU Keyword used in alternate discrete design value list definition.

BY Keyword used in alternate discrete design value list definition.

INC Discrete design value increment. The list of discrete design values
generated by the alternate format is DVAL1 + (n)(INC), where n = 0, 1, 2,
…n. The last discrete design value is always DVAL2 even if the range is not
evenly divisible by INC.

261
DDVAL
Defines a discrete design value list for an optimization design variable.
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

DDVAL ID DVAL1 DVAL2 DVAL3 DVAL4 DVAL5 DVAL6 DVAL7

DVAL8 …

Alternate form of the DDVAL card:

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

DDVAL ID DVAL1 THRU DVAL2 BY INC

DVAL1 THRU DVAL2 BY INC

Field Comments
ID Discrete design value list identification number.

DVALi Discrete design values. Can be listed in any order.

THRU Keyword used in alternate discrete design value list definition.

BY Keyword used in alternate discrete design value list definition.

INC Discrete design value increment. The list of discrete design values
generated by the alternate format is DVAL1 + (n)(INC), where n = 0, 1, 2,
…n. The last discrete design value is always DVAL2 even if the range is not
evenly divisible by INC.

262
DDVAL
Defines a discrete design value list for an optimization design variable.
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

DDVAL ID DVAL1 DVAL2 DVAL3 DVAL4 DVAL5 DVAL6 DVAL7

DVAL8 …

Alternate form of the DDVAL card:

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

DDVAL ID DVAL1 THRU DVAL2 BY INC

DVAL1 THRU DVAL2 BY INC

Field Comments
ID Discrete design value list identification number.

DVALi Discrete design values. Can be listed in any order.

THRU Keyword used in alternate discrete design value list definition.

BY Keyword used in alternate discrete design value list definition.

INC Discrete design value increment. The list of discrete design values
generated by the alternate format is DVAL1 + (n)(INC), where n = 0, 1, 2,
…n. The last discrete design value is always DVAL2 even if the range is not
evenly divisible by INC.

263
Design Responses Table
Response RTYPE PTYPE ATTA ATTB ATTi

Mass MASS Property - COMB PID

Card or SUM MID
MAT Blank = All

Mass Fraction MASSFRAC Property - COMB PID

Card or SUM MID
MAT Blank = All

Volume VOLUME Property - COMB PID

Card or SUM MID
MAT Blank = All

Volume VOLFRAC Property - COMB PID

Fraction Card or SUM MID
MAT Blank = All

Center of COG Property Center of Gravity COMB PID

Gravity Card or Item Code MID
MAT Blank = All

Moment of INERTIA Property Moment of COMB PID

Inertia Card or Inertia Item Code MID
MAT Blank = All

Compliance COMP Property - COMB PID

Card or SUM MID
MAT Blank = All

Weighted WCOMP Property - - PID

Compliance Card or MID
MAT Blank = All

Displacement DISP - Displacement - GID

Component Item
Code

Normal Mode FREQ - Normal Mode - -

Frequency Number

Buckling LAMA - Buckling Mode - -

Mode Number
Eigenvalue

Homogeneous STRESS Property Homogeneous - PID

Stress Card or Stress Item Code EID
(Z1, Z2) ELEM Blank = All

Homogeneous STRAIN Property Homogeneous - PID

Strain Card or Strain Item Code EID
(Z1, Z2) ELEM Blank = All

Composite Ply CSTRESS PCOMPG Composite Ply ALL PID

Stress PLY Stress Item Code G# EID
(mid of ply) ELEM (global PLYID
ply #) Blank = All

Composite Ply CSTRAIN PCOMPG Composite Ply ALL PID

Strain PLY Strain Item Code G# EID
(mid of ply) ELEM (global PLYID
ply #) Blank = All

264
 Composite Ply CFAILURE PCOMPG Composite Ply ALL PID
Failure PLY Failure Item G# EID
(mid of ply) ELEM Code (global PLYID
ply #) Blank = All

Static Force FORCE Property Static Force Item - PID

Card or Code EID
MAT Blank = All

SPC Forces SPCFORCE Component DOF GID

(1-6)

GPF Balance GPFORCE GID Component DOF EID

(1-6)

Homogeneous Stress or Strain Item Codes

Element Component ASCII Code

All Solid Elements σvm / εvm SVM

σ1 / ε1 SMAP

σ2 / ε2 SMDP

σ3 / ε3 SMIP

σx / εx SXX

σy / εy SYY

σz / εz SZZ

τxy / γxy SXY

τyz / γyz SYZ

τxz / γxz SXZ

All Shell Elements σvm / εvm SVMB

(Both Sides) σ1 / ε1 SMPB

σ3 / ε3 SMIPB

σx / εx SXB

σy / εy SYB

τxy / γxy SXYB

(Z1) σvm / εvm SVM1

σ1 / ε1 SMP1

σ3 / ε3 SMIP1

σx / εx SX1

σy / εy SY1

τxy / γxy SXY1

265
 (Z2) σvm / εvm SVM2

σ1 / ε1 SMP2

σ3 / ε3 SMIP2

σx / εx SX2

σy / εy SY2

τxy / γxy SXY2

Composite Ply Stress or Strain Item Codes

Type Component Code

(Total Stress/Strain) σ1 / ε1 S1

σ2 / ε2 S2

τ12 / γ12 S12

τ23 / γ23 S2Z

τ13 / γ13 S1Z

σ1 / ε1 (principal) SMAP

σ3 / ε3 (principal) SMIP

(Mechanical Strain) εm,1 MS1

εm,2 MS2

γm,12 MS12

εm,1 (principal) MSMAP

εm,3 (principal) MSMIP

(Thermal Strain) εt,1 TS1

εt,2 TS2

γt,12 TS12

εt,1 (principal) TSMAP

εt,3 (principal) TSMIP

Composite Ply Failure Item Codes

Theory Code

Maximum Strain STRN

Tsai-Hill HILL

266
Tsai-Wu TSAI

267
DSHUFFLE
Defines shuffling optimization design variables and design manufacturing constraints.
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

DSHUFFLE ID PTYPE PID1 PID2 PID3 PID4 PID5 PID6

PID7 …

Continuation lines to define a maximum successive layers constraint.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

MAXSUCC MANGLE MSUCC VSUCC

Continuation line to define a pairing constraint.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

PAIR PANGLE1 PANGLE2 POPT

Continuation line to define a core layer stacking sequence constraint.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

CORE CREP CANG1 CANG2 CANG3 CANG4 CANG5 CANG6

CANG7 …

Continuation line to define a cover layer stacking sequence constraint.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

COVER VREP VANG1 VANG2 VANG3 VANG4 VANG5 VANG6

VANG7 …

Field Comments
ID Free-size optimization design variable and design manufacturing
constraint identification number

PTYPE Property type on which to apply the free-size design variables and design
manufacturing constraints.

PCOMP - Defines PCOMP identification numbers follow.

268
 PCOMPG - Defines PCOMPG identification numbers follow.
STACK – Defines STACK identification numbers follow.

PIDi List of property identification numbers of PTYPE on which to apply the

shuffle optimization design variables and design manufacturing
constraints.

MAXSUCC Keyword used to define shuffling optimization maximum number of

successive plies for a given angle constraint.

MANGLE Ply orientation, in degrees, to which the MAXSUCC constraint is applies.

MSUCC Maximum number of successive plies for the angle defined by MANGLE.
(Integer > 0)

VSUCC Allowable percentage violation for the MAXSUCC constraint. 0.0 indicates
that this constraint cannot be violated (Default = 0.0)

PAIR Keyword used to define shuffling optimization pairing constraint.

PANGLE1 First ply orientation, in degrees, to which the PAIR constraint is applied.
(only 45.0 allowed at this time)

PANGLE2 Second ply orientation, in degrees, to which the PAIR constraint is applies.
(only -45.0 allowed at this time)

POPT Pairing constraint option. SAME indicates that the stacking sequence
should remain the same for consecutive pairs. REVERSE indicates that the
stacking sequence should be reversed for alternate pairs.

269
CORE Keyword used to define shuffling optimization core layer stacking
sequence constraint. The core layer is defined by the plies around the
middle surface of the laminate.

CREP Number of times the core layer stacking sequence should be repeated
(Integer > 0, Default = 1)

CANG# Ply orientations, in degrees, defining the core layer stacking sequence.

COVER Keyword used to define shuffling optimization cover layer stacking

sequence constraint. The cover layer is defined by the plies at the
top/bottom surface of the laminate.

VREP Number of times the cover layer stacking sequence should be repeated
(Integer > 0, Default = 1)

VANG# Ply orientations, in degrees, defining the cover layer stacking sequence

270
DSIZE
Defines free-size optimization design variables and design manufacturing constraints.
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

DSIZE ID PTYPE PID1 PID2 PID3 PID4 PID5 PID6

PID7 …

Continuation lines to define zone-based free-size optimization groups.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

GROUP EG1 EG2 EG3 EG4 EG5 EG6

EG7 …

Continuation line to define a homogeneous shell thickness constraint.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

THICK T0 T1

Continuation line to define a homogeneous shell von Mises stress constraint.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

STRESS UBOUND

Continuation line to define a member size manufacturing constraint.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

MEMBSIZ MINDIM

Continuation lines to define total laminate thickness manufacturing constraints.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

COMP LAMTHK LTMIN LTMAX LTSET LTEXC

Continuation lines to define ply group thickness percentage manufacturing

constraints.
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

COMP PLYPCT PPGRP PPMIN PPMAX PPOPT PPSET PPEXC

271
Continuation lines to define ply group balancing manufacturing constraints.
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

COMP BALANCE BGRP1 BGRP2 BOPT

Continuation lines to define ply group constant thickness manufacturing constraints.

(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

COMP CONST CGRP CTHICK COPT

Continuation lines to define ply group drop off manufacturing constraints.

(1) (2) (3) (4) (5) (6) (7) (8) (9) 10

COMP PLYDRP PDGRP PDTYPE PDMAX PDOPT PDSET PDEXC

PDDEF PDX PDY PDZ

Field Comments
ID Free-size optimization design variable and design manufacturing
constraint identification number

PTYPE Property type on which to apply the free-size design variables and design
manufacturing constraints.

PCOMP - Defines PCOMP identification numbers follow.

PCOMPG - Defines PCOMPG identification numbers follow.
PSHELL - Defines PSHELL identification numbers follow.
STACK – Defines STACK identification numbers follow.

PIDi List of property identification numbers of PTYPE on which to apply the

free-size optimization design variables and design manufacturing
constraints. For PTYPE = PCOMP, PCOMPG, or STACK; design variables
are automatically created for the thickness of each ply for each element
referenced by the property identification numbers. For PTYPE = PSHELL;
design variables are automatically created for the thickness of the

272
 homogeneous shell for each element referenced by the property
identification numbers.

GROUP Keyword used to define free-sizing optimization zone groups. Free-size

optimization zone groups are defined by element sets. For zone groups,
design variables are automatically created for the thickness of each ply
for each zone group. Therefore, the thickness of the plies within a zone
group will be uniform and no ply drops or additions will exist within the
zone group. Effectively, a zone group removes the element-by-element
nature of the free-size optimization design variables and considers all the
elements within the zone group as the same.

EGi Element set identification numbers defining the element within the zone
group.

THICK Keyword used to define a homogeneous thickness constraint. This

keyword is valid for PTYPE = PSHELL only. The THICK keyword can be
defined only once on a DSIZE card.

T0 Minimum homogeneous shell thickness for the homogeneous thickness

constraint. Overrides the T0 field on the PSHELL card. If no value is
entered, then the T0 field on the PSHELL card is used. If no value is
entered on the PSHELL card, then T0 = 0.0 is assumed. (Default = blank,
T0 > 0.0)

T1 Maximum homogeneous shell thickness for the homogeneous thickness

constraint. If no value is entered, then T field on the PSHELL card is used.
(Default = blank, T1 > T0)

273
STRESS Keyword used to define a homogeneous von Mises stress constraint. This
keyword is valid for PTYPE = PSHELL only. The STRESS keyword can be
defined only once on a DSIZE card.

UBOUND Upper bound value for the homogeneous von Mises stress constraint.
The von Mises stress cannot exceed this value. (UBOUND > 0.0)

MEMBSIZ Keyword used to define a member size manufacturing constraint. The

MEMBSIZ keyword can be defined only once on a DSIZE card.

MINDIM Minimum dimension of formed members for the member size

manufacturing constraint. Used to prevent the formation of small
members. (Default = blank – no minimum size control, MINDIM > 0.0).

COMP Keyword used to indicate the start of a composite manufacturing

constraint definition. The COMP keyword is followed by the specific
composite manufacturing constraint keyword being defined; LAMTHK,
PLYTHK, PLYPCT, BALANCE, CONST, or PLYDRP.

LAMTHK Keyword used to define total laminate thickness manufacturing

constraints. Multiple LAMTHK definitions can be defined on a single
DCOMP card, each of which begins with the LAMTHK keyword.

n
LGT = ∑ tk , i
k =1

LTMIN < LGT < LTMAX

274
LTMIN Minimum laminate total thickness for the laminate total thickness
manufacturing constraint. (LTMIN > 0.0)

LTMAX Maximum laminate total thickness for the laminate total thickness
manufacturing constraint. (LTMAX > LTMIN)

LTSET Element set identification number defining the elements to which the
laminate thickness manufacturing constraint applies. (Default = All
Elements)

LTEXC Ply exclusion option indicating plies that are to be excluded from the
laminate thickness calculation for the laminate thickness manufacturing
constraint. (Default = CORE)

NONE - No plies are excluded from the calculation.

CORE - The core layer within a SMCORE laminate definition (i.e. the last
layer defined in the laminate definition) is excluded from the calculation.
If the referenced PCOMP or STACK card is not defined as a SMCORE
laminate, then there is no core layer defined.
CONST - Any ply defined with a CONST ply thickness manufacturing
constraint is excluded from the calculation.
BOTH – Both the core layer within a SMCORE laminate definition and any
ply defined with a CONST ply thickness manufacturing constraint are
excluded from the calculation.

PLYPCT Keyword used to define ply group percent thickness manufacturing

constraints. Multiple PLYPCT definitions can be defined on a single
DCOMP card, each of which begins with the PLYPCT keyword.

275
 n
LT = ∑ tk , i
k =1

PGT = ∑ tk ,i

PGT
PGP =
LT
PPMIN < PGP < PPMAX

PPGRP Ply group identification to which the ply group percent thickness
manufacturing constraint applies. Ply groups can be identified by nominal
fiber orientation angle, ply sets, or individual ply identification numbers
depending on the PPOPT setting.

PPMIN Minimum ply group percent thickness for the ply group percent thickness
manufacturing constraint. (PPMIN > 0.0)

PPMAX Maximum ply group percent thickness for the ply group percent thickness
manufacturing constraint. (PPMAX > PTMIN)

PPOPT Ply group identification option for the ply group percent thickness
manufacturing constraint. (Default = BYANG)

BYANG - Specifies that PPGRP is defined as a real number representing a

nominal fiber orientation angle. The ply group is defined as all the plies
which have the given nominal fiber orientation angle.

276
 BYSET - Specifies that PPGRP is defined as a ply set identification number.
The ply group is the set of plies which are defined in the referenced ply
set.

BYPLY – Specifies that PPGRP is defined as a single ply identification

number. The ply group is the individual ply referenced by the ply
identification number.

PPSET Element set identification number defining the elements to which the ply
group percent thickness manufacturing constraint applies. (Default = All
Elements)

PPEXC Ply exclusion option indicating plies that are to be excluded from the ply
group percent thickness calculation for the ply group percent thickness
manufacturing constraint. (Default = CORE)

NONE - No plies are excluded from the calculation.

CORE - The core layer within a SMCORE laminate definition (i.e. the last
layer defined in the laminate definition) is excluded from the calculation.
If the referenced PCOMP or STACK card is not defined as a SMCORE
laminate, then there is no core layer defined.
CONST - Any ply defined with a CONST ply thickness manufacturing
constraint is excluded from the calculation.
BOTH – Both the core layer within a SMCORE laminate definition and any
ply defined with a CONST ply thickness manufacturing constraint are
excluded from the calculation.

BALANCE Keyword used to define ply group balance manufacturing constraints.

Multiple BALANCE definitions can be defined on a single DCOMP card,
each of which begins with the BALANCE keyword.

277
 PGT 1 = ∑ tk ,i

PGT 2 = ∑ tk ,i

PGT 1 = PGT 2

BGRP1 Ply group #1 identification to which the ply group balance manufacturing
constraint applies. Ply groups can be identified by nominal fiber
orientation angle, ply sets, or individual ply identification numbers
depending on the BOPT setting.

BGRP2 Ply group #2 identification to which the ply group balance manufacturing
constraint applies. Ply groups can be identified by nominal fiber
orientation angle, ply sets, or individual ply identification numbers
depending on the BOPT setting.

BOPT Ply group identification option for the ply group balance manufacturing
constraint. (Default = BYANG)

BYANG - Specifies that BGRP1 and BGRP2 are defined as real numbers
representing the nominal fiber orientation angles. The ply group is
defined as all the plies which have the given nominal fiber orientation
angle.
BYSET - Specifies that BGRP1 and BRRP2 are defined as ply set
identification numbers. The ply group is the set of plies which are defined
in the referenced ply set.

278
 BYPLY – Specifies that BGRP1 and BGRP2 are defined as single ply
identification numbers. The ply group is the individual ply referenced by
the ply identification number.

CONST Keyword used to define ply group constant thickness manufacturing

constraints. Multiple CONST definitions can be defined on a single
DCOMP card, each of which begins with the CONST keyword.

PGT = ∑ tk ,i

PGT = CTHICK

CGRP Ply group identification to which the ply group constant thickness
manufacturing constraint applies. Ply groups can be identified by nominal
fiber orientation angle, ply sets, or individual ply identification numbers
depending on the COPT setting.

CTHICK Constant ply group thickness for the ply group constant thickness
manufacturing constraint. (CTHICK > 0.0)

COPT Ply group identification option for the ply group constant thickness
manufacturing constraint. (Default = BYANG)

BYANG - Specifies that CGRP is defined as a real number representing the

nominal fiber orientation angle. The ply group is defined as all the plies
which have the given nominal fiber orientation angle.

279
 BYSET - Specifies that CGRP is defined as a ply set identification number.
The ply group is the set of plies which are defined in the referenced ply
set.
BYPLY – Specifies that CGRP is defined as a single ply identification
number. The ply group is the individual ply referenced by the ply
identification number.

PLYDRP Keyword used to define ply group drop off manufacturing constraints.
Multiple PLYDRP definitions can be defined on a single DCOMP card, each
of which begins with the PLYDRP keyword.

PDGRP Ply group identification to which the ply group drop off manufacturing
constraint applies. Ply groups can be identified by nominal fiber
orientation angle, ply sets, or individual ply identification numbers
depending on the PDOPT setting.

PDTYPE Specifies type of ply group drop of manufacturing constraint to apply.

(Default = PLYSLP)

PLYSLP uses the ply slope method to calculating ply drop manufacturing
constraint.

∆t tk ,i − tk ,i +1
PDMAX = tan(θ ) = =
∆d ∆d

PLYDRP uses the ply drop method to calculating ply drop manufacturing constraint

280
 PDMAX = ∆t = tk ,i − tk ,i +1

TOTSLP uses the total laminate slope method to calculating ply drop
manufacturing constraint. Same as PLYSLP but considering ALL the plies
as a total thickness, not just the kth ply, in PDGRP.

n n

∆t
∑ t k , i − ∑ t k , i +1
PDMAX = tan(θ ) = = k =1 k =1
∆d ∆d

TOTDRP uses the total laminate drop method to calculating ply drop
manufacturing constraint. Same as PLYDRP but considering ALL the plies
as a total thickness, not just the kth ply, in PDGRP.

n n
PDMAX = ∆t = ∑ tk ,i − ∑ tk ,i +1
k =1 k =1

PDMAX Maximum ply group drop off based on the PDTYPE setting. (PPMAX > 0)

281
PDOPT Ply group identification option for the ply group drop off manufacturing
constraint. (Default = BYANG)

BYANG - Specifies that PPGRP is defined as a real number representing a

nominal fiber orientation angle. The ply group is defined as all the plies
which have the given nominal fiber orientation angle.
BYSET - Specifies that PPGRP is defined as a ply set identification number.
The ply group is the set of plies which are defined in the referenced ply
set.
BYPLY – Specifies that PPGRP is defined as a single ply identification
number. The ply group is the individual ply referenced by the ply
identification number.

PDSET Element set identification number defining the elements to which the ply
group drop off manufacturing constraint applies. (Default = All Elements)

PDEXC Ply exclusion option indicating plies that are to be excluded from the ply
group drop off calculation for the ply group drop off manufacturing
constraint. (Default = CORE)

NONE - No plies are excluded from the calculation.

CORE - The core layer within a SMCORE laminate definition (i.e. the last
layer defined in the laminate definition) is excluded from the calculation.
If the referenced PCOMP or STACK card is not defined as a SMCORE
laminate, then there is no core layer defined.
CONST - Any ply defined with a CONST ply thickness manufacturing
constraint is excluded from the calculation.
BOTH – Both the core layer within a SMCORE laminate definition and any
ply defined with a CONST ply thickness manufacturing constraint are
excluded from the calculation.

282
PDDEF Optional definition to fine-tune the ply group drop off manufacturing
constraint by requesting directional drop off. DIRECT is currently the only
option available.

PDX/Y/Z Used to specify the drop off direction when DIRECT is used in the PDDEF
field. Defines the components of a direction vector, in the global
coordinate system, in which the drop off constraint is to be applied. For
example, if drop off control is required in the x-axis direction, then 1,0,0
should be entered for PDX, PDY, PDZ respectively.

283
DVPREL1
Defines property values, at each ith iteration of a size optimization, as a linear
combination of design variables.
Pi = C0 + ∑ (COEFi )( DVIDi )
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)

DVPREL1 ID TYPE PID PNAME C0

or FID

DVID1 COEF1 DVID2 COEF2 DVID3 COEF3 DVID4 COEF4

DVID5 COEF5 …

Field Comments
ID Design variable property relationship identification number.

TYPE Property type.

PID Property identification number of TYPE.

PNAME Property field variable name. (i.e. T for the thickness of a ply on the PLY
card)

FID Property field identification number. The first row has field identification
numbers 1 – 10, the second row has field identification numbers 11 – 20,
and so on. (i.e. 4 for the thickness of a ply on the PLY card)

C0 Constant in the linear combination equation. (Default = 0.0)

DVIDi Design variable identification numbers defining the design variable to link
in the linear combination equation.

COEFi Design variable coefficients in the linear combination equation. (Default

= 1.0)

284
285