FACULTY OF ENGINEERING

DEPARTMENT OF CIVIL ENGINEERING

STRUCTURAL MECHANICS SECTION
KASTEELPARK ARENBERG 40
B-3001 LEUVEN

Stabil
MATLAB toolbox
for Structural Mechanics

USER’S GUIDE
STABIL VERSION 3.1
APRIL 2020
REPORT BWM-2020-05
Contact information
Web http://bwk.kuleuven.be/bwm/stabil
Email stabil@kuleuven.be
Phone +32 16 32 16 82
Address Structural Mechanics Section
Department of Civil Engineering, KU Leuven
Kasteelpark Arenberg 40, B-3001 Leuven, Belgium

Copyright

(C) 2007–2020 KU Leuven, Structural Mechanics

Stabil is free software: you can redistribute it and/or modify it under the terms of the GNU General Public
License as published by the Free Software Foundation, either version 3 of the License, or (at your option) any
later version.
Stabil is distributed in the hope that it will be useful, but WITHOUT ANY WARRANTY; without even the
implied warranty of MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the GNU
General Public License for more details.
You should have received a copy of the GNU General Public License along with Stabil. If not, see https:
//www.gnu.org/licenses/.

Acknowledgements

Stabil has been developed in the frame of OOI Project 2006/20 ”An interactive and adaptive application for the
static and dynamic analysis of structures”, funded by the KU Leuven Educational Policy Unit. The financial
support is gratefully acknowledged.
Contents

1 Getting started 1
1.1 About Stabil . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1
1.2 Obtaining and installing Stabil . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1
1.3 Terms of use . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1
1.4 Scope and structure of this document . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2
2 Static analysis of structures 3
2.1 Example 1.1: static analysis of a frame . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3
2.2 Example 1.2: static analysis of a 3D frame . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10
2.3 Example 1.3: static analysis of a plate with a circular hole . . . . . . . . . . . . . . . . . . . . . . 19
2.4 Example 1.4: static analysis of a barrel vault roof . . . . . . . . . . . . . . . . . . . . . . . . . . . 21
3 Dynamic analysis of structures 25
3.1 Example 2.1: dynamic analysis of a frame . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 25
3.2 Example 2.2: dynamic analysis of a plate . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35
4 Element guide 37
5 Functions — By category 55
5.1 General functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55
5.2 Postprocessing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55
5.3 Dynamics . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 56
5.4 General shell functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 56
6 Functions — Alphabetical list 57
Bibliography 303
ii CONTENTS
Chapter 1

Getting started

1.1 About Stabil

Stabil is a MATLAB toolbox for structural mechanics, based on the finite element method. Classical finite
element beam and truss elements, as well as shell elements and elements for 2D and 3D elasticity have been
implemented, and the toolbox can be used to solve a variety of static and dynamic structural problems. In
addition, Stabil contains a number of postprocessing functions tailored to structural analysis, including plots of
member forces and displacements of a structure. The user can interact with Stabil at a low level of abstraction
or a high level of abstraction, which is further detailed in this manual. Due to this multi-level approach,
the toolbox is suitable for educational purposes and for use in a research environment: the high level functions
allow for an easy and efficient implementation of many common problems, while the low level functions facilitate
customization and the implementation of novel finite element techniques in a research context.
Stabil is written in standard MATLAB language, so that the source code is available to the user. No additional
MATLAB toolboxes are required and the toolbox can be used in a Windows, Linux, or MacOS environment.

1.2 Obtaining and installing Stabil

Stabil can be downloaded from the internet at https://bwk.kuleuven.be/bwm/stabil. It is
distributed as a ZIP archive, which should be extracted to a directory on the hard disk, e.g.
C:\Users\/%username/%\Documents\matlab\stabil. After extraction of the ZIP archive, this directory
should contain a number of m-files.
The Stabil directory must be subsequently added to the MATLAB path to make the toolbox functions available
in MATLAB:
- In MATLAB, click on ‘Set Path...’ in the ‘Home’ tab.
- Click on ‘Add Folder’ and select the Stabil directory.
- Save the path and close the dialog window.

1.3 Terms of use

Stabil is free software: you can redistribute it and/or modify it under the terms of the GNU General Public
License as published by the Free Software Foundation, either version 3 of the License, or (at your option) any
later version. The toolbox can be used and modified for educational and research purposes. However, it cannot
be used for consulting, nor commercialized in any form. Regardless of any provision of the GNU General Public
License, Stabil may not be used for commercial purposes without explicit written permission from the authors.
Furthermore, if you use Stabil for research, please include a reference to Stabil in scientific publications of your
work (articles, reports, books, etc.).
Stabil is distributed in the hope that it will be useful, but without any warranty; without even the implied
warranty of merchantability or fitness for a particular purpose. See the GNU General Public License for more
2 GETTING STARTED

details. You should have received a copy of the GNU General Public License along with Stabil. If not, see
https://www.gnu.org/licenses/.

1.4 Scope and structure of this document

The present document is the user’s guide to Stabil version 4.0. It is a combination of a reference guide, providing
an overview of all functions of Stabil, and a tutorial, presenting a set of examples to illustrate the use of Stabil.
This document is not meant as a textbook: a theoretical background is only considered where this is necessary
to define the functionality of Stabil in a clear way. The reader is referred to various works on Matrix analysis of
Structures [5], Finite Elements [1, 3, 4, 6–9], or Dynamics of Structures [2] for a broad theoretical background.
This document is composed of the following chapters:
Chapter 1. Getting started (p. 1)
The aim of this chapter is to get the user started with Stabil and the accompanying user’s guide. The installation
procedure of Stabil is explained, the terms of use of Stabil are clarified, and the scope and structure of the user’s
guide are discussed.
Chapter 2. Static analysis of structures (p. 3)
In this chapter, the use of stabil for the static analysis of structures is explained through a number of examples.
Chapter 3. Dynamic analysis of structures (p. 25)
In this chapter, the use of stabil for the dynamic analysis of structures is explained through a number of
examples.
Chapter 4. Element guide (p. 37)
This chapter presents an overview of the element types available in Stabil. The conventions (local coordinate
system, nodal connectivity) for each element type are given and reference is made to the Stabil functions related
to the element implementation.
Chapter 5. Functions — By category (p. 55)
This chapter gives an overview of all functions in Stabil, organized by category.
Chapter 6. Functions — Alphabetical list (p. 57)
This chapter consists of an alphabetical list of the functions in Stabil. The syntax, the input and output
arguments, and the use of each function are described in detail. The information provided in this chapter is
also accessible at the MATLAB prompt through the help command.
Chapter 2

Static analysis of structures

2.1 Example 1.1: static analysis of a frame

The basic concepts of the Stabil toolbox are introduced through the example of a simple frame structure, shown
in figure 2.1. The frame has a height and width of 4 m and is clamped at node 1 and pinned at node 5. An
internal hinge is present at nodes 2 and 3, and a diagonal brace is present between nodes 1 and 4. At node 4
a point load F = 5 kN is applied and the vertical beam on the left is loaded by a distributed load p = 2 kN/m.
The beams and columns have a concrete rectangular cross-section with a width of 0.2 m and a height of 0.4 m.
The concrete has a Young’s modulus of 30 GPa and a Poisson’s ratio of 0.2. The diagonal brace has a circular
steel cross-section with a diameter of 8 mm with a Young’s modulus of 210 GPa and a Poisson coefficient of 0.3.
2 kN
m 5 kN
3 4

4m

1 x 5

4m

Figure 2.1: Simple frame structure.

The code to compute the deformation and bending moment in the frame structure is listed below:

% StaBIL manual
% Example 1.1: static analysis of a frame
% Units: m, kN

% Nodes=[NodID X Y Z]
Nodes= [1 0 0 0;
2 0 4 0;
3 0 4 0;
4 4 4 0;
5 4 0 0;
6 1 5 0]; % reference node

% Check the node coordinates as follows:

figure
plotnodes(Nodes);
4 STATIC ANALYSIS OF STRUCTURES

% Element types -> {EltTypID EltName}

Types= {1 'beam';
2 'truss'};

b=0.10;
h=0.25;
r=0.004;

% Sections=[SecID A ky kz Ixx Iyy Izz yt yb zt zb]

Sections= [1 b*h Inf Inf 0 0 b*h^3/12 h/2 h/2 b/2 b/2;
2 pi*r^2 NaN NaN NaN NaN NaN NaN NaN NaN NaN];

% Materials=[MatID E nu];
Materials= [1 30e6 0.2; % concrete
2 210e6 0.3]; % steel

% Elements=[EltID TypID SecID MatID n1 n2 n3]

Elements= [1 1 1 1 1 2 6;
2 1 1 1 3 4 6;
3 1 1 1 5 4 6;
4 2 2 2 1 4 NaN];

% Check node and element definitions as follows:

hold('on');
plotelem(Nodes,Elements,Types);
title('Nodes and elements');

% Degrees of freedom
% Assemble a column matrix containing all DOFs at which stiffness is
% present in the model:
DOF=getdof(Elements,Types);

% Remove all DOFs equal to zero from the vector:

% - 2D analysis: select only UX,UY,ROTZ
% - clamp node 1
% - hinge at node 5
seldof=[0.03; 0.04; 0.05; 1.00; 5.01; 5.02];
DOF=removedof(DOF,seldof);

% Assembly of stiffness matrix K

K=asmkm(Nodes,Elements,Types,Sections,Materials,DOF);

% Nodal loads: 5 kN horizontally on node 4.

seldof=[4.01];
PLoad= [5];

% Assembly of the load vectors:

P=nodalvalues(DOF,seldof,PLoad);

% Distributed loads are specified in the global coordinate system

% DLoads=[EltID n1globalX n1globalY n1globalZ ...]
DLoads= [1 2 0 0 2 0 0];

P=P+elemloads(DLoads,Nodes,Elements,Types,DOF);

% Constraint equations: Constant=Coef1*DOF1+Coef2*DOF2+ ...

% Constraints=[Constant Coef1 DOF1 Coef2 DOF2 ...]
Constr= [0 1 2.01 -1 3.01;
0 1 2.02 -1 3.02];

% Add constraint equations

[K,P]=addconstr(Constr,DOF,K,P);

% Solve K * U = P
U=K\P;
EXAMPLE 1.1: STATIC ANALYSIS OF A FRAME 5

% Plot displacements
figure
plotdisp(Nodes,Elements,Types,DOF,U,DLoads,Sections,Materials)

% The displacements can be displayed as follows:

printdisp(Nodes,DOF,U);

% Compute element forces

Forces=elemforces(Nodes,Elements,Types,Sections,Materials,DOF,U,DLoads);

% The element forces can be displayed in a orderly table:

printforc(Elements,Forces);

% Plot element forces

figure
plotforc('norm',Nodes,Elements,Types,Forces,DLoads)
title('Normal forces')

figure
plotforc('sheary',Nodes,Elements,Types,Forces,DLoads)
title('Shear forces')

figure
plotforc('momz',Nodes,Elements,Types,Forces,DLoads)
title('Bending moments')

% Plot stresses
figure
plotstress('snorm',Nodes,Elements,Types,Sections,Forces,DLoads)
title('Normal stresses due to normal forces')

figure
plotstress('smomzt',Nodes,Elements,Types,Sections,Forces,DLoads)
title('Normal stresses due to bending moments around z: top')

figure
plotstress('smomzb',Nodes,Elements,Types,Sections,Forces,DLoads)
title('Normal stresses due to bending moments around z: bottom')

figure
plotstress('smax',Nodes,Elements,Types,Sections,Forces,DLoads)
title('Maximal normal stresses')

figure
plotstress('smin',Nodes,Elements,Types,Sections,Forces,DLoads)
title('Minimal normal stresses')

After the definition of model parameters, the analysis starts by defining the nodes of the model, where the nodes
are defined in the (x,y)-plane. The nodes are represented by a matrix that contain node numbers as a first
column, followed by the x, y and z coordinates of each node. Next, the element types are defined by a cell array,
Types, containing type numbers followed by a string (either beam or truss). The Sections matrix defines
the section properties (cross section, moments of inertia,. . . ). In a similar way, the Materials matrix defines
material properties (the Young’s modulus and Poisson coefficient). The model definition is then completed by
providing an element connectivity table Elements, which refers to the previously defined element, material,
section and node numbers. In order to uniquely define a local coordinate system for the beam elements, use is
made of a reference node (node 6). The local x-axis is directed from the first node of the element to the last
node, the local y-axis is perpendicular to the local x-axis with its origin corresponding to the first node of the
element, and pointing in the direction of the reference node. The same convention applies in a three-dimensional
setting, as indicated in the beam element reference sheet on page 38.
Next, the degrees of freedom (DOF’s) are specified. The DOF’s are defined using a node.index approach,
where the digits to the left of the decimal point refer to the node number and the digits to the right of the
decimal point refer to degree of freedom. By convention, the degrees of freedom 01, 02, and 03 correspond to
translations ux , uy , and uz in the global coordinate directions whereas the degrees of freedom 04, 05, and 06
6 STATIC ANALYSIS OF STRUCTURES

Node Ux [m] Uy [m] Uz [m] ϕx [rad] ϕy [rad] ϕz [rad]

1 0.0000e+0 0.0000e+0 0.0000e+0 0.0000e+0 0.0000e+0 0.0000e+0
2 6.6633e-3 3.2297e-6 0.0000e+0 0.0000e+0 0.0000e+0 -1.8161e-3
3 6.6633e-3 3.2297e-6 0.0000e+0 0.0000e+0 0.0000e+0 4.0356e-4
4 6.6538e-3 -3.6160e-5 0.0000e+0 0.0000e+0 0.0000e+0 -8.3665e-4
5 0.0000e+0 0.0000e+0 0.0000e+0 0.0000e+0 0.0000e+0 - 2.0769e-3
6 0.0000e+0 0.0000e+0 0.0000e+0 0.0000e+0 0.0000e+0 0.0000e+0
Element Node N [kN] Vy [kN] Vz [kN] T [kNm] My [kNm] Mz [kNm]
1 i 6.0557e-1 6.2201e+0 -0.0000e+0 -0.0000e+0 -0.0000e+0 -8.8804e+00
1 j 6.0557e-1 -1.7799e+0 0.0000e+0 0.0000e+0 0.0000e+0 -4.4409e-16
2 i -1.7799e+0 6.0557e-1 -0.0000e+0 -0.0000e+0 -0.0000e+0 0.0000e+00
2 j -1.7799e+0 6.0557e-1 0.0000e+0 0.0000e+0 0.0000e+0 2.4223e+00
3 i -6.7799e+0 -6.0557e-1 -0.0000e+0 -0.0000e+0 -0.0000e+0 6.6613e-16
3 j -6.7799e+0 -6.0557e-1 0.0000e+0 0.0000e+0 0.0000e+0 -2.4223e+00
4 i 8.7318e+0 -0.0000e+0 -0.0000e+0 -0.0000e+0 -0.0000e+0 0.0000e+00
4 j 8.7318e+0 0.0000e+0 0.0000e+0 0.0000e+0 0.0000e+0 -0.0000e+00

Table 2.1: Nodal displacements, reaction forces, and member forces for example 1.1.

correspond to rotations ϕx , ϕy , ϕz around the global coordinate axes. For example, DOF 3.02 represents the
translation uy of node 3. This approach of defining the degrees of freedom for the problem at hand is very
instructive, since it enforces reasoning on the kinematics of the structure and how boundary conditions are
accounted for. This manual input of the vector of degrees of freedom is seen as a low-level functionality of the
toolbox. Alternatively, the high-level functions (getdof, selectdof, removedof) could be used to generate and
process this DOF vector, allowing for more complex structural models to be analyzed in an efficient way.
The finite element stiffness matrix is next assembled using the asmkm function. This function takes the Nodes,
Elements, Types, Sections, and Materials variables that define the finite element model and assembles the
sparse global stiffness matrix K corresponding to the dof vector. The asmkm function is a high-level function
that loops over the various elements of the mesh and calls low-level functions that generate element stiffness
matrices.
In Stabil, both nodal loads as well as distributed loads on elements can be considered, and dedicated functions are
available to either generate nodal loads on DOFs (the nodalvalues function) or distributed loads on elements
(the elemloads function). The load vector P is available in the Matlab environment, and has the same size as
the dof-vector.
In order to account for the internal hinge between nodes 2 and 3, constraint equations are added to the system
of equations to couple the horizontal and vertical displacements of both nodes. This is achieved through the
function addconstr that modifies the stiffness matrix K to account for linear constraint equations that relate
various degrees of freedom in the system.
The finite element system of equations (Ku = f ) is solved using the Matlab \ (left divide, mldivide) command.
Since the global stiffness matrix K is a sparse matrix, a sparse solver is used by Matlab by default. The resulting
displacement vector u has the same size as the dof vector and the load vector P and is equally available in the
Matlab environment.
In Stabil, a number of postprocessing functions is available to easily plot the deformed structure or the resulting
member forces. Figure 2.2 shows the resulting displacement of the structure as obtained with the plotdisp
command. The plotdisp command takes the model definition (Nodes, Elements, Types), the displacement
solution and corresponding dof vector, and (optionally) the distributed load with the section and material
definitions (Sections, and Materials). A key feature of the Stabil toolbox is that the deformed shape is
plotted in an exact way, accounting for the (cubic) shape functions of the beam element and the deformation of
the element due to distributed loads. This allows to demonstrate how distributed loads are reduced to equivalent
nodal loads.
Figure 2.3 shows the member forces in the structure as plotted with the plotforc command. Like the plotdisp
command, the plotforc command accounts for the effect of distributed loads, as is apparent in the quadratic
variation of the bending moment in the left column in figure 2.3.
EXAMPLE 1.1: STATIC ANALYSIS OF A FRAME 7

Figure 2.2: Deformed frame structure.

8 STATIC ANALYSIS OF STRUCTURES

8.732

0.606 −6.780
−1.780 −1.780

8.732

0.606 −6.780

(a)

2.422
0.000 −2.422

0.792

−8.880 0.000

(b)

0.606
−1.780 0.606
−0.606

6.220 −0.606

(c)

Figure 2.3: (a) Normal forces [kN], (b) bending moments [kNm], and (c) shear forces [kN] in the frame structure.
EXAMPLE 1.1: STATIC ANALYSIS OF A FRAME 9

173714

−71
24 −271
−71

173714

24 −271
(a) normal forces

2325
0 −2325 0 2325
−2325

760 −760

−8525 0 8525 0
(b) bending moments around z: top (c) bending moments around z: bottom
173714 173714

−71
24 2254
2054 −71
24 −2597
−2397

785 −736

173714 173714

8549 −271 −8501 −271

(c) maximal (d) minimal

Figure 2.4: Normal stresses.

10 STATIC ANALYSIS OF STRUCTURES

2.2 Example 1.2: static analysis of a 3D frame

In order to demonstrate the three-dimensional capabilities of Stabil, the following example considers a 3D frame
structure (figure 2.5). The frame consists of rectangular concrete beams (Young’s modulus E = 35 × 109 N/m2
and Poisson coefficient ν = 0.2) with a height of 0.5 m and a width of 0.2 m and concrete columns of 0.3 m by
0.2 m.

205

307 206
105 206
203
303 106 308
5 203 106
103 204
6305 304 205
103 6 201 104 204
3 210
301 105310
309 306
3 201 104
101 1104 202
5 302
101 4 202
1 10 102
z
y 102
1 x
2

Figure 2.5: Example 1.2: nodes, elements, loads and boundary conditions.

The following input file is structured in a similar way as example 1.1. It starts by defining nodes, element types,
sections, and materials. Subsequently, the elements are defined by the use of a reference node. The reprow
command is employed to replicate rows of the Nodes and Elements matrix. The getdof and seldof commands
are then used to generate and process the DOF vector. After assembling the stiffness matrix and assembling the
loads, the system is solved, the forces and reaction forces are computed and results are finally plotted, resulting
in figures 2.6 to 2.9 for the different load cases and load combinations.

% StaBIL manual
% Example 1.2: static analysis of a 3D frame
% Units: m, kN

% Types={EltTypID EltName}
Types= {1 'beam';
2 'truss'};

% Sections
bCol=0.2; % Column section width
hCol=0.3; % Column section height
bBeam=0.2; % Beam section width
hBeam=0.5; % Beam section height
Atruss=0.001;
EXAMPLE 1.2: STATIC ANALYSIS OF A 3D FRAME 11

% Sections=[SecID A ky kz Ixx Iyy Izz yt yb zt zb]

Sections= [1 hCol*bCol Inf Inf 0.196*bCol^3*hCol bCol^3*hCol/12 ...
hCol^3*bCol/12 hCol/2 hCol/2 bCol/2 bCol/2; % Columns
2 hBeam*bBeam Inf Inf 0.249*bBeam^3*hBeam bBeam^3*hBeam/12 ...
hBeam^3*bBeam/12 hBeam/2 hBeam/2 bBeam/2 bBeam/2; % Beams
3 Atruss NaN NaN NaN NaN NaN NaN NaN NaN NaN];

% Materials=[MatID E nu rho];
Materials= [1 35e9 0.2 2500; %concrete
2 210e9 0.3 7850]; %steel

L=5;
H=3.5;
B=4;

% Nodes=[NodID X Y Z]
Nodes= [1 0 0 0;
2 L 0 0]
Nodes=reprow(Nodes,1:2,2,[2 0 0 H])
Nodes=[Nodes;
10 2 0 2] % reference node
Nodes=reprow(Nodes,1:7,2,[100 0 B 0])

figure
plotnodes(Nodes);

% Elements=[EltID TypID SecID MatID n1 n2 n3]

Elements=[ 1 1 1 1 1 3 10;
2 1 1 1 2 4 10];
Elements=reprow(Elements,1:2,1,[2 0 0 0 2 2 0])
Elements=[ Elements;
5 1 2 1 3 4 10;
6 1 2 1 5 6 10];
Elements=reprow(Elements,1:6,2,[100 0 0 0 100 100 100])
Elements=[ Elements;
301 2 3 2 3 103 NaN;
302 2 3 2 4 104 NaN];
Elements=reprow(Elements,19:20,1,[2 0 0 0 2 2 0])
Elements=reprow(Elements,19:22,1,[4 0 0 0 100 100 0])
Elements=[ Elements;
309 2 3 2 4 106 NaN;
310 2 3 2 6 104 NaN];

hold('on');
plotelem(Nodes,Elements,Types);
title('Nodes and elements');

% Plot elements in different colors in order to check the section definitions

figure
plotelem(Nodes,Elements(find(Elements(:,3)==1),:),Types,'r');
hold('on');
plotelem(Nodes,Elements(find(Elements(:,3)==2),:),Types,'g');
plotelem(Nodes,Elements(find(Elements(:,3)==3),:),Types,'b');
title('Elements: sections')

% Degrees of freedom
DOF=getdof(Elements,Types);

% Boundary conditions: hinges

seldof=[ 1.01; 1.02; 1.03; 2.01; 2.02; 2.03;
101.01; 101.02; 101.03; 102.01; 102.02; 102.03;
201.01; 201.02; 201.03; 202.01; 202.02; 202.03;];

DOF=removedof(DOF,seldof);
12 STATIC ANALYSIS OF STRUCTURES

% Assembly of stiffness matrix K

K=asmkm(Nodes,Elements,Types,Sections,Materials,DOF);

% Loads

% Own weight
DLoadsOwn=accel([0 0 9.81],Elements,Types,Sections,Materials);

% Wind load

% DLoads=[EltID n1globalX n1globalY n1globalZ ...]

DLoadsWind =[1 0 0 0 0 1500 0;
2 0 0 0 0 1500 0;
3 0 1500 0 0 1500 0;
4 0 1500 0 0 1500 0];

DLoads=multdloads(DLoadsOwn,DLoadsWind);

P=elemloads(DLoads,Nodes,Elements,Types,DOF);

% Solve K * U = P
U=K\P;

figure
plotdisp(Nodes,Elements,Types,DOF,U(:,1),DLoads(:,:,1),Sections,Materials)
title('Displacements: own weight')

figure
plotdisp(Nodes,Elements,Types,DOF,U(:,2),DLoads(:,:,2),Sections,Materials)
title('Displacements: wind')

% Compute forces
[ForcesLCS,ForcesGCS]=elemforces(Nodes,Elements,Types,Sections,Materials,DOF,U,DLoads);

% Compute reaction forces for load case 1

Freac=reaction(Elements,ForcesGCS(:,:,1),[1.03; 2.03; 101.03; 102.03; 201.03; 202.03])

% Plot element forces for load case 1

figure
plotforc('norm',Nodes,Elements,Types,ForcesLCS(:,:,1),DLoads(:,:,1))
title('Normal forces: Own weight')
figure
plotforc('sheary',Nodes,Elements,Types,ForcesLCS(:,:,1),DLoads(:,:,1))
title('Shear forces along y: Own weight')
figure
plotforc('shearz',Nodes,Elements,Types,ForcesLCS(:,:,1),DLoads(:,:,1))
title('Shear forces along z: Own weight')
figure
plotforc('momx',Nodes,Elements,Types,ForcesLCS(:,:,1),DLoads(:,:,1))
title('Torsional moments: Own weight')
figure
plotforc('momy',Nodes,Elements,Types,ForcesLCS(:,:,1),DLoads(:,:,1))
title('Bending moments around y: Own weight')
figure
plotforc('momz',Nodes,Elements,Types,ForcesLCS(:,:,1),DLoads(:,:,1))
title('Bending moments around z: Own weight')

% Plot element forces for load case 2

figure
plotforc('norm',Nodes,Elements,Types,ForcesLCS(:,:,2),DLoads(:,:,2))
title('Normal forces: Wind')
figure
plotforc('sheary',Nodes,Elements,Types,ForcesLCS(:,:,2),DLoads(:,:,2))
title('Shear forces along y: Wind')
figure
plotforc('shearz',Nodes,Elements,Types,ForcesLCS(:,:,2),DLoads(:,:,2))
EXAMPLE 1.2: STATIC ANALYSIS OF A 3D FRAME 13

title('Shear forces along z: Wind')

figure
plotforc('momx',Nodes,Elements,Types,ForcesLCS(:,:,2),DLoads(:,:,2))
title('Torsional moments: Wind')
figure
plotforc('momy',Nodes,Elements,Types,ForcesLCS(:,:,2),DLoads(:,:,2))
title('Bending moments around y : Wind')
figure
plotforc('momz',Nodes,Elements,Types,ForcesLCS(:,:,2),DLoads(:,:,2))
title('Bending moments around z: Wind')

% Load combinations

% Safety factors
gamma_own=1.35;
gamma_wind=1.5;

% Combination factors
psi_wind=1;

% Load combination (Ultimate Limit State, ULS)

U_ULS=gamma_own*U(:,1)+gamma_wind*psi_wind*U(:,2);
Forces_ULS=gamma_own*ForcesLCS(:,:,1)+gamma_wind*psi_wind*ForcesLCS(:,:,2);
DLoads_ULS(:,1)=DLoads(:,1,1)
DLoads_ULS(:,2:7)=gamma_own*DLoads(:,2:7,1)+gamma_wind*psi_wind*DLoads(:,2:7,2);

figure
plotdisp(Nodes,Elements,Types,DOF,U_ULS,DLoads_ULS,Sections,Materials)

printdisp(Nodes,DOF,U_ULS);

printforc(Elements,Forces_ULS);

% Plot element forces

figure
plotforc('norm',Nodes,Elements,Types,Forces_ULS,DLoads_ULS)
title('Normal forces: ULS')
figure
plotforc('sheary',Nodes,Elements,Types,Forces_ULS,DLoads_ULS)
title('Shear forces along y: ULS')
figure
plotforc('shearz',Nodes,Elements,Types,Forces_ULS,DLoads_ULS)
title('Shear forces along z: ULS')
figure
plotforc('momx',Nodes,Elements,Types,Forces_ULS,DLoads_ULS)
title('Torsional moments: ULS')
figure
plotforc('momy',Nodes,Elements,Types,Forces_ULS,DLoads_ULS)
title('Bending moments around y: ULS')
figure
plotforc('momz',Nodes,Elements,Types,Forces_ULS,DLoads_ULS)
title('Bending moments around z: ULS')

% Plot stresses
figure
plotstress('snorm',Nodes,Elements,Types,Sections,Forces_ULS,DLoads_ULS)
title('Normal stresses due to normal forces')
figure
plotstress('smomyt',Nodes,Elements,Types,Sections,Forces_ULS,DLoads_ULS)
title('Normal stresses due to bending moments around y: top')
figure
plotstress('smomyb',Nodes,Elements,Types,Sections,Forces_ULS,DLoads_ULS)
title('Normal stresses due to bending moments around y: bottom')
figure
plotstress('smomzt',Nodes,Elements,Types,Sections,Forces_ULS,DLoads_ULS)
title('Normal stresses due to bending moments around z: top')
14 STATIC ANALYSIS OF STRUCTURES

figure
plotstress('smomzb',Nodes,Elements,Types,Sections,Forces_ULS,DLoads_ULS)
title('Normal stresses due to bending moments around z: bottom')
figure
plotstress('smax',Nodes,Elements,Types,Sections,Forces_ULS,DLoads_ULS)
title('Maximal normal stresses')
figure
plotstress('smin',Nodes,Elements,Types,Sections,Forces_ULS,DLoads_ULS)
title('Minimal normal stresses')
EXAMPLE 1.2: STATIC ANALYSIS OF A 3D FRAME 15

(a) Displacements

(b) Normal forces (c) Torsional moments

(d) Shear forces along z (e) Shear forces along y

(f) Bending moments around y (g) Bending moments around z

Figure 2.6: Results for load case 1 of example 1.2.

16 STATIC ANALYSIS OF STRUCTURES

(a) Displacements

(b) Normal forces (c) Torsional moments

(d) Shear forces along z (e) Shear forces along y

(f) Bending moments around y (g) Bending moments around z

Figure 2.7: Results for load case 2 of example 1.2.

EXAMPLE 1.2: STATIC ANALYSIS OF A 3D FRAME 17

(a) Displacements

(b) Normal forces (c) Torsional moments

(d) Shear forces along z (e) Shear forces along y

(f) Bending moments around y (g) Bending moments around z

Figure 2.8: Results for load combination ULS of example 1.2.

18 STATIC ANALYSIS OF STRUCTURES

(a) normal forces

(b) bending moments around y: top (c) bending moments around y: bottom

(d) bending moments around z: top (e) bending moments around z: bottom

(f) maximal (g) minimal

Figure 2.9: Normal stresses for load combination ULS of example 1.2.
EXAMPLE 1.3: STATIC ANALYSIS OF A PLATE WITH A CIRCULAR HOLE 19

2.3 Example 1.3: static analysis of a plate with a circular hole

This example demonstrates the use of Stabil for the solution of 2D plane strain continuum problems. A thin
disk with a circular hole is subjected to uniaxial tension. The stress concentration around the hole is examined:

% StaBIL manual
% Example 1.3: static analysis of a plate with a circular hole

% Stress concentration around a circular hole in a disk.

r = 1; % Radius of hole [m]
L = 20; % Width of plate [m]
p = 1; % Uniform pressure [N/m^2]
n = 40; % Mesh parameter (nElem = m*n)
m = 20; % Mesh parameter
Types = {1 'shell8'}; % {EltTypID EltName}
Sections = [1 1]; % [SecID t]
Materials = [1 200000 0]; % [MatID E nu]

% define lines
Line1 = [r 0 0;L/2 0 0];
Line2 = [L/2 0 0;L/2 L/2 0;0 L/2 0];
Line3 = [0 L/2 0;0 r 0];
Line4 = [r*sin((0:5).'*pi/10) r*cos((0:5).'*pi/10) zeros(6,1)];

[Nodes,Elements,Edge1,Edge2,Edge3,Edge4] = makemesh(Line1,Line2,Line3,Line4,...
m,n,Types(1,:),Sections(1,1),Materials(1,1),'L2method','linear');

% Check mesh:
figure;
plotnodes(Nodes,'numbering','off');
hold('on')
plotelem(Nodes,Elements,Types,'numbering','off');
title('Nodes and elements');

% Select all dof:

DOF = getdof(Elements,Types);
% Apply boundary conditions:
% - Line1 and Line3: symmetry condition
seldof = [0.03;0.04;0.05;0.06;Edge1+0.02;Edge3+0.01];
DOF = removedof(DOF,seldof);

% Assemble K:
K = asmkm(Nodes,Elements,Types,Sections,Materials,DOF);

% Apply load to upper edge (equivalent nodal forces):

C = selectdof(DOF,Edge2(1:(end-1)/2+1)+0.02);
P = C.'*[1/6; repmat([2/3; 1/3],((length(Edge2)-1)/2-2)/2,1);2/3; 1/6]*p*L/m;
U = K\P;

% Calculate stress in cylindrical global coordinate system

[SeGCS]=elemstress(Nodes,Elements,Types,Sections,Materials,DOF,U,'gcs','cyl');

% Get nodal stress from element solution

[SnGCS] = nodalstress(Nodes,Elements,Types,SeGCS);

% plot results
figure;
plotstresscontourf('sx',Nodes,Elements,Types,SnGCS)
title('\sigma_{r}')
figure;
plotstresscontourf('sy',Nodes,Elements,Types,SnGCS)
title('\sigma_{\theta}')
figure;
20 STATIC ANALYSIS OF STRUCTURES

plotstresscontourf('sxy',Nodes,Elements,Types,SnGCS)
title('\sigma_{r\theta}')

Figure 2.10

(a) σθ (b) σr

(c) σrθ

Figure 2.10: Results for the hole-in-disk problem.

EXAMPLE 1.4: STATIC ANALYSIS OF A BARREL VAULT ROOF 21

2.4 Example 1.4: static analysis of a barrel vault roof

A barrel vault roof subjected to its self weight is analysed. The curved edges are simply supported and the
straight edges are free. Due to symmetry only a quarter of the roof is modelled and symmetry boundary
conditions are applied.

Edge 2: simply supported

Edge 1:
symmetry
Edge 3: conditions
free
boundary

zy
x

Edge 4: symmetry conditions

Figure 2.11: 8 × 8 mesh of a quarter of a cylindrical roof.

% StaBIL manual
% Example 1.4: static analysis of a barrel vault roof

% A BARREL VAULT ROOF SUBJECTED TO ITS SELF WEIGHT

% Reference: COOK, CONCEPTS AND APPL OF F.E.A., 2ND ED., 1981, PP. 284-287.

%% Parameters
R=25; % Radius of cylindrical roof
L=50; % Length of cylindrical roof
t=0.25; % Thickness of roof
theta = 40*pi/180; % Angle of cylindrical roof
E = 4.32*10^8; % Youngs modulus
nu = 0; % Poisson coefficient
rho = 36.7347; % Density
N = 8; % Number of elements

%% Mesh

% Lines = [x1 y1 z1;x2 y2 z2;...]

Line1 = [0 0 0;0 0 L/2];
Line2 = [R*sin(theta*(0:0.1:1).') R*cos(theta*(0:0.1:1).')-R L*ones(11,1)/2];
Line3 = [R*sin(theta) R*cos(theta)-R L/2; R*sin(theta) R*cos(theta)-R 0];
Line4 = [R*sin(theta*(1:-0.1:0).') R*cos(theta*(1:-0.1:0).')-R zeros(11,1)];

% Specify element type for mesh

Materials = [1 E nu rho];
Sections = [1 t];
22 STATIC ANALYSIS OF STRUCTURES

Types = {1 'shell8'};

% Mesh the area between lines 1,2,3,4 with N * N elements of type shell8,
% section number 1 and material number 1.
[Nodes,Elements,Edge1,Edge2,Edge3,Edge4] = ...
makemesh(Line1,Line2,Line3,Line4,N,N,Types(1,:),1,1);

% Check mesh:
figure;
plotnodes(Nodes,'numbering','off');
hold('on')
plotelem(Nodes,Elements,Types,'numbering','off');
title('Nodes and elements');

%% Assemble stiffness matrix

% Select all dof:

DOF = getdof(Elements,Types);

% Apply boundary conditions:

% - Line1 and Line4: symmetry condition
% - Line2: simply supported
sdof = [Edge1+0.01;Edge1+0.06;Edge1+0.05;Edge2+0.02;Edge2+0.01;
Edge2+0.06;Edge4+0.03;Edge4+0.04;Edge4+0.05];
DOF = removedof(DOF,sdof);

% Assemble K:
K = asmkm(Nodes,Elements,Types,Sections,Materials,DOF);

%% Solution

% Apply gravitational acceleration and determine equivalent nodal forces:

DLoads=accel([0 9.8 0],Elements,Types,Sections,Materials);
P=elemloads(DLoads,Nodes,Elements,Types,DOF);

% Solve K * U = P:
U = K\P;

% Plot displacements:
figure;
plotdisp(Nodes,Elements,Types,DOF,U)
title('Displacements')

% Check target displacement:

TP1 = selectdof(DOF,intersect(Edge3,Edge4)+0.02);
Utp1 = TP1*U
ratio_u = -Utp1/0.3016

%% Stress

% Determine element stress in global and local(element) coordinate system:

[SeGCS,SeLCS,vLCS]=elemstress(Nodes,Elements,Types,Sections,Materials,DOF,U);

% print stress:
printstress(Elements,SeGCS)

% plot stress contour:

figure;
plotstresscontour('sx',Nodes,Elements,Types,SeGCS,'location','bot')
title('sx in gcs (element solution)')

% plot filled contours:

figure;
plotstresscontourf('sx',Nodes,Elements,Types,SeGCS,'location','bot')
title('sx in gcs (element solution)')
EXAMPLE 1.4: STATIC ANALYSIS OF A BARREL VAULT ROOF 23

figure;
plotstresscontour('sx',Nodes,Elements,Types,SeLCS,'location','bot')
title('sx in lcs')

% plot lcs for shell elements

figure;
plotlcs(Nodes,Elements,Types,vLCS)
title('local coordinate system')

% Calculate nodal solution

% SnGCS: stress arranged per element
% SnGCS2: stress arranged per node
[SnGCS,SnGCS2]=nodalstress(Nodes,Elements,Types,SeGCS);
[SnLCS,SnLCS2]=nodalstress(Nodes,Elements,Types,SeLCS);
figure;
plotstresscontour('sx',Nodes,Elements,Types,SnGCS,'location','bot');
title('sx in gcs (nodal solution)')

% Stress ratios:

ratio_sz = SnGCS2(intersect(Edge3,Edge4),16)/358420
ratio_st = SnGCS2(intersect(Edge4,Edge1),14)/(-213400)

%% Shell forces

% Shell forces (element solution):

[FeLCS]=elemshellf(Elements,Sections,SeLCS);
figure;
plotshellfcontour('my',Nodes,Elements,Types,FeLCS)
title('my (element solution)')

% Nodal solution:
[FnLCS,FnLCS2]=nodalshellf(Nodes,Elements,Types,FeLCS);
figure;
plotshellfcontour('my',Nodes,Elements,Types,FnLCS)
title('my (nodal solution)')

%% Principal stress

% Principal stresses:
[Spr,Vpr]=principalstress(Elements,SnGCS);
figure;
plotstresscontour('s1',Nodes,Elements,Types,Spr,'location','bot');
title('s1')
% plot principal stresses:
figure;
plotprincstress(Nodes,Elements,Types,Spr,Vpr)
title('principal stresses')
24 STATIC ANALYSIS OF STRUCTURES

zy
x

(a) Local coordinate systems (b) Displacements

5 5
x 10 x 10
0.0599 3.5841

−0.1401 3.2082

−0.3401 2.8323

−0.5401 2.4564

−0.7401 2.0804

−0.9401 1.7045

−1.1401 1.3286

−1.3401 0.9527

−1.5401 zy 0.5768 zy
x x
MIN
−1.7401 0.2008 MIN

−1.9401 −0.1751
MAX
MAX
−2.1401 −0.551

(c) σxx at bottom of shell in GCS (element solution) (d) σxx at bottom of shell in LCS (element solution)

2079.965

1881.9048

1683.8446

1485.7844

1287.7242

1089.6639

891.6037

693.5435

495.4833 zy
zy
x
MAX x
297.4231

99.3629
MIN
−98.6973

(e) my in LCS (nodal solution) (f) Principal stresses at top of shell

Figure 2.12: Cylindrical roof: results.

Chapter 3

Dynamic analysis of structures

3.1 Example 2.1: dynamic analysis of a frame

The frame that was treated in section 2.1 is reconsidered, computing the eigenmodes and dynamic response of
the structure.
2 kN
m 5 kN
3 4

4m
y

1 x 5

4m

Figure 3.1: Simple frame structure.

3.1.1 Model

% StaBIL manual
% Example 2.1: dynamic analysis: model
% Units: m, N

L=4;
H=4;
nElemCable=8;

% Nodes=[NodID X Y Z]
Nodes= [1 0 0 0;
2 L 0 0];
Nodes=reprow(Nodes,1:2,4,[2 0 H/4 0]);
Nodes= [Nodes;
11 0 H 0];
Nodes=reprow(Nodes,11,3,[1 L/4 0 0]);
Nodes= [Nodes;
15 1 5 0]; % reference node
Nodes= [Nodes;
26 DYNAMIC ANALYSIS OF STRUCTURES

16 0 0 0];
Nodes=reprow(Nodes,16,nElemCable,[1 L/nElemCable H/nElemCable 0]);

% Check the node coordinates as follows:

figure
plotnodes(Nodes);

% Element types -> {EltTypID EltName}

Types= {1 'beam'};

b=0.10;
h=0.25;
r=0.004;

% Sections=[SecID A ky kz Ixx Iyy Izz]

Sections= [1 b*h Inf Inf 0 0 b*h^3/12;
2 pi*r^2 Inf Inf 0 0 pi*r^4/4];

% Materials=[MatID E nu];
Materials= [1 30e9 0.2 2500; % concrete
2 210e9 0.3 7850]; % steel

% Elements=[EltID TypID SecID MatID n1 n2 n3]

Elements= [1 1 1 1 1 3 15;
2 1 1 1 2 4 15];
Elements=reprow(Elements,1:2,3,[2 0 0 0 2 2 0]);
Elements=[ Elements;
9 1 1 1 11 12 15;
10 1 1 1 12 13 15;
11 1 1 1 13 14 15;
12 1 1 1 14 10 15;
13 1 2 2 16 17 15];
Elements=reprow(Elements,13,(nElemCable-1),[1 0 0 0 1 1 0]);

% Check node and element definitions as follows:

hold('on');
plotelem(Nodes,Elements,Types);
title('Nodes and elements');

% Degrees of freedom
DOF=getdof(Elements,Types);

% Boundary conditions
seldof=[0.03; 0.04; 0.05; 1.01; 1.02; 1.06; 2.01; 2.02; 16.01; 16.02];

DOF=removedof(DOF,seldof);

% Assembly of stiffness matrix K

[K,M]=asmkm(Nodes,Elements,Types,Sections,Materials,DOF);

% DLoads=[EltID n1globalX n1globalY n1globalZ ...]

DLoads=[1 2000 0 0 2000 0 0;
3 2000 0 0 2000 0 0;
5 2000 0 0 2000 0 0;
7 2000 0 0 2000 0 0];
b=elemloads(DLoads,Nodes,Elements,Types,DOF); % Spatial distribution, nodal (nDOF * 1)

% Constraint equations: Constant=Coef1*DOF1+Coef2*DOF2+ ...

% Constraints=[Constant Coef1 DOF1 Coef2 DOF2 ...]
Constr= [0 1 9.01 -1 11.01;
0 1 9.02 -1 11.02;
0 1 10.01 -1 (16.01+nElemCable);
0 1 10.02 -1 (16.02+nElemCable)];

[K,b,M]=addconstr(Constr,DOF,K,b,M);
EXAMPLE 2.1: DYNAMIC ANALYSIS OF A FRAME 27

3.1.2 Eigenmodes

% StaBIL manual
% Example 2.1: dynamic analysis: eigenvalue problem
% Units: m, N

% Assembly of M and K
tutorialdyna;

% Eigenvalue problem
nMode=12;
[phi,omega]=eigfem(K,M,nMode);

% Display eigenfrequenties
disp('Lowest eigenfrequencies [Hz]');
disp(omega/2/pi);

% Plot eigenmodes
figure;
plotdisp(Nodes,Elements,Types,DOF,phi(:,1),'DispMax','off')
figure;
plotdisp(Nodes,Elements,Types,DOF,phi(:,2),'DispMax','off')
figure;
plotdisp(Nodes,Elements,Types,DOF,phi(:,5),'DispMax','off')
figure;
plotdisp(Nodes,Elements,Types,DOF,phi(:,8),'DispMax','off')
figure;
plotdisp(Nodes,Elements,Types,DOF,phi(:,11),'DispMax','off')
figure;
plotdisp(Nodes,Elements,Types,DOF,phi(:,12),'DispMax','off')

% Animate eigenmodes
figure;
animdisp(Nodes,Elements,Types,DOF,phi(:,1))
title('Eigenmode 1')

figure;
animdisp(Nodes,Elements,Types,DOF,phi(:,2))
title('Eigenmode 2')

figure;
animdisp(Nodes,Elements,Types,DOF,phi(:,5))
title('Eigenmode 5')

figure;
animdisp(Nodes,Elements,Types,DOF,phi(:,8))
title('Eigenmode 8')

figure;
animdisp(Nodes,Elements,Types,DOF,phi(:,11))
title('Eigenmode 11')

figure;
animdisp(Nodes,Elements,Types,DOF,phi(:,12))
title('Eigenmode 12')

3.1.3 Modal superposition: time domain: piecewise exact integration

% StaBIL manual
% Example 2.1: dynamic analysis: modal superposition: piecewise exact integration
% Units: m, N

% Assembly of M and K
28 DYNAMIC ANALYSIS OF STRUCTURES

(a) Eigenmode 1 (b) Eigenmode 2

(b) Eigenmode 5 (c) Eigenmode 8

(d) Eigenmode 11 (e) Eigenmode 12

Figure 3.2: Results of example 2.1.

tutorialdyna;

% Sampling parameters
T=2.5; % Time window
dt=0.002; % Time step
N=T/dt; % Number of samples
EXAMPLE 2.1: DYNAMIC ANALYSIS OF A FRAME 29

t=[0:N-1]*dt; % Time axis

% Eigenvalue analysis
nMode=12; % Number of modes to take into account
[phi,omega]=eigfem(K,M,nMode); % Calculate eigenmodes and eigenfrequencies
xi=0.07; % Constant modal damping ratio

% Excitation
bm=phi.'*b; % Spatial distribution, modal (nMode * 1)
q=zeros(1,N); % Time history (1 * N)
q((t>=0.50) & (t<0.60))=1; % Time history (1 * N)
pm=bm*q; % Modal excitation (nMode * N)

% Modal analysis
x=msupt(omega,xi,t,pm,'zoh');

% Modal displacements -> nodal displacements

u=phi*x; % Nodal response (nDOF * N)

% Figures
figure;
plot(t,x);
title('Modal response (piecewise linear exact integration)');
xlabel('Time [s]');
xlim([0 4.1])
ylabel('Displacement [m kg^{0.5}]');
legend([repmat('Mode ',nMode,1) num2str([1:nMode].')]);

figure;
c=selectdof(DOF,[9.01; 13.02; 17.02]);
plot(t,c*u);
title('Nodal response (piecewise linear exact integration)');
xlabel('Time [s]');
xlim([0 4.1])
ylabel('Displacement [m]');
legend('9.01','13.02','17.02');

% Movie
figure;
animdisp(Nodes,Elements,Types,DOF,u);

% Display
disp('Maximum modal response');
disp(max(abs(x),[],2));

disp('Maximum nodal response 9.01 13.02 17.02');

disp(max(abs(c*u),[],2));

3.1.4 Modal superposition: transform to frequency domain

% StaBIL manual
% Example 2.1: dynamic analysis: direct method: frequency domain
% Units: m, N

% Assembly of M and K
tutorialdyna;

% Sampling parameters
N=2048; % Number of samples
dt=0.002; % Time step
T=N*dt; % Period
F=N/T; % Sampling frequency
df=1/T; % Frequency resolution
t=[0:N-1]*dt; % Time axis
30 DYNAMIC ANALYSIS OF STRUCTURES

f=[0:N/2-1]*df; % Positive frequencies corresponding to FFT [Hz]

Omega=2*pi*f; % Idem [rad/s]

% Eigenvalue analysis
nMode=12; % Number of modes to take into account
[phi,omega]=eigfem(K,M,nMode); % Calculate eigenmodes and eigenfrequencies
xi=0.07; % Constant modal damping ratio

% Excitation
bm=phi.'*b; % Spatial distribution, modal (nMode * 1)
q=zeros(1,N); % Time history (1 * N)
q((t>=0.50) & (t<0.60))=1; % Time history (1 * N)
Q=fft(q); % Frequency content (1 * N)
Q=Q(1:N/2); % Frequency content, positive freq (1 * N/2)
Pm=bm*Q; % Modal excitation, positive freq (nMode * N/2)

% Modal analysis
[X,H]=msupf(omega,xi,Omega,Pm); % Modal response, positive freq (nMode * N/2)

% F-dom -> t-dom

X=[X, zeros(nMode,1), conj(X(:,end:-1:2))];
x=ifft(X,[],2); % Modal response (nMode * N)

% Modal displacements -> nodal displacements

u=phi*x; % Nodal response (nDOF * N)

% Figures
figure;
subplot(3,2,1);
plot(t,q,'.-');
xlim([0 4.1])
ylim([0 1.2]);
title('Excitation time history');
xlabel('Time [s]');
ylabel('Force [N/m]');

subplot(3,2,2);
plot(f,abs(Q)/F,'.-');
title('Excitation frequency content');
xlabel('Frequency [Hz]');
ylabel('Force [N/m/Hz]');

subplot(3,2,4);
plot(f,abs(H),'.-');
title('Modal transfer function');
xlabel('Frequency [Hz]');
ylabel('Displacement [m/N]');
legend([repmat('Mode ',nMode,1) num2str([1:nMode].')]);

subplot(3,2,6);
plot(f,abs(X(:,1:N/2))/F,'.-');
title('Modal response');
xlabel('Frequency [Hz]');
ylabel('Displacement [m kg^{0.5}/Hz]');

subplot(3,2,5);
plot(t,x);
title('Modal response (calculation in f-dom)');
xlabel('Time [s]');
xlim([0 4.1])
ylabel('Displacement [m kg^{0.5}]');

figure;
plot(t,x);
title('Modal response (calculation in f-dom)');
xlabel('Time [s]');
EXAMPLE 2.1: DYNAMIC ANALYSIS OF A FRAME 31

xlim([0 4.1])
ylabel('Displacement [m kg^{0.5}]');
legend([repmat('Mode ',nMode,1) num2str([1:nMode].')]);

figure;
c=selectdof(DOF,[9.01; 13.02; 17.02]);
plot(t,c*u);
title('Nodal response (calculation in f-dom)');
xlabel('Time [s]');
xlim([0 4.1])
ylabel('Displacement [m]');
legend('9.01','13.02','17.02');

% Movie
figure;
animdisp(Nodes,Elements,Types,DOF,u);

% Display
disp('Maximum modal response');
disp(max(abs(x),[],2));

disp('Maximum nodal response 9.01 13.02 17.02');

disp(max(abs(c*u),[],2));

3.1.5 Direct time integration

% StaBIL manual
% Example 2.1: dynamic analysis: direct time integration: trapezium rule
% Units: m, N

% Assembly of M, K and C
tutorialdyna;
[phi,omega]=eigfem(K,M); % Calculate eigenmodes and eigenfrequencies
xi=0.07; % Damping ratio
nModes=length(K)-size(Constr,1);
C=M.'*phi(:,1:nModes)*diag(2*xi*omega(1:nModes))*phi(:,1:nModes).'*M;
% Modal -> full damping matrix C

% Sampling parameters
T=2.5; % Time window
dt=0.002; % Time step
N=T/dt; % Number of samples
t=[0:N-1]*dt; % Time axis

% Excitation
q=zeros(1,N); % Time history (1 * N)
q((t>=0.50) & (t<0.60))=1; % Time history (1 * N)
p=b*q; % Nodal excitation (nDOF * N)

% Direct time integration - trapezium rule

alpha=1/4;
delta=1/2;
theta=1;
u=newmark(M,C,K,dt,p,[alpha delta theta]);

% Figures
figure;
c=selectdof(DOF,[9.01; 13.02; 17.02]);
plot(t,c*u);
title(['Nodal response (direct time integration)']);
xlabel('Time [s]');
xlim([0 4.1])
ylabel('Nodal displacements [m]');
legend('9.01','13.02','17.02');
32 DYNAMIC ANALYSIS OF STRUCTURES

Excitation time history Excitation frequency content

0.1

1 0.08

Force [N/m/Hz]
0.8
Force [N/m]

0.06
0.6
0.04
0.4

0.2 0.02

0 0
0 1 2 3 4 0 10 20 30 40 50
Time [s] Frequency [Hz]

Modal transfer function

Mode 1
0.8
Mode 2
Mode 3

Displacement [m/N]
Mode 4 0.6
Mode 5
Mode 6 0.4
Mode 7
Mode 8
Mode 9 0.2
Mode 10
Mode 11 0
Mode 12 0 10 20 30 40 50
Frequency [Hz]

Modal response (calculation in f−dom) −3 Modal response

x 10
0.15 8
Displacement [m kg0.5/Hz]
Displacement [m kg0.5]

0.1 6

0.05 4

0 2

−0.05 0
0 1 2 3 4 0 10 20 30 40 50
Time [s] Frequency [Hz]

Figure 3.3: Modal superposition in frequency domain.

% Movie
figure;
animdisp(Nodes,Elements,Types,DOF,u);

% Display
disp('Maximum nodal response 9.01 13.02 17.02');
disp(max(abs(c*u),[],2));

3.1.6 Direct solution in the frequency domain

% StaBIL manual
% Example 2.1: dynamic analysis: modal superposition: transform to f-dom
EXAMPLE 2.1: DYNAMIC ANALYSIS OF A FRAME 33

0.1 0.1
Mode 1 Mode 1
Mode 2 Mode 2
0.08 0.08
Mode 3 Mode 3
Mode 4 Mode 4
Displacement [m kg0.5]

Displacement [m kg0.5]
0.06 Mode 5 0.06 Mode 5
Mode 6 Mode 6
Mode 7 Mode 7
0.04 0.04
Mode 8 Mode 8
Mode 9 Mode 9
0.02 Mode 10 0.02 Mode 10
Mode 11 Mode 11
Mode 12 Mode 12
0 0

−0.02 −0.02

−0.04 −0.04
0 0.5 1 1.5 2 2.5 3 3.5 4 0 0.5 1 1.5 2 2.5 3 3.5 4
Time [s] Time [s]
(a) Modal superposition in time domain (b) Modal superposition in frequency domain

Figure 3.4: Modal response: comparison.

% Units: m, N

% Assembly of M, K and C
tutorialdyna;
[phi,omega]=eigfem(K,M); % Calculate eigenmodes and eigenfrequencies
xi=0.07; % Damping ratio
nModes=length(K)-size(Constr,1);
C=M.'*phi(:,1:nModes)*diag(2*xi*omega(1:nModes))*phi(:,1:nModes).'*M;
% Modal -> full damping matrix C

% Sampling parameters
N=2048; % Number of samples
dt=0.002; % Time step
T=N*dt; % Period
F=N/T; % Sampling frequency
df=1/T; % Frequency resolution
t=[0:N-1]*dt; % Time axis
f=[0:N/2-1]*df; % Positive frequencies corresponding to FFT [Hz]
Omega=2*pi*f; % Idem [rad/s]

% Excitation
q=zeros(1,N); % Time history (1 * N)
q((t>=0.50) & (t<0.60))=1; % Time history (1 * N)
Q=fft(q); % Frequency content (1 * N)
Q=Q(1:N/2); % Frequency content, positive freq (1 * N/2)
Pd=b*Q; % Nodal excitation, positive freq (nDOF * N/2)

% Solution for each frequency

Ud=zeros(size(Pd));
for k=1:N/2
Kd=-Omega(k)^2*M+Omega(k)*i*C+K;
Ud(:,k)=Kd\Pd(:,k);
end

% F-dom -> t-dom

Ud=[Ud, zeros(length(K),1), conj(Ud(:,end:-1:2))];
u=ifft(Ud,[],2); % Nodal response (nDOF * N)

% Figures
figure;
c=selectdof(DOF,[9.01; 13.02; 17.02]);
plot(t,c*u);
title('Nodal response (direct method in f-dom)');
xlabel('Time [s]');
xlim([0 4.1])
34 DYNAMIC ANALYSIS OF STRUCTURES

ylabel('Displacement [m]');
legend('9.01','13.02','17.02');

% Movie
figure;
animdisp(Nodes,Elements,Types,DOF,u);

% Display
disp('Maximum nodal response 9.01 13.02 17.02');
disp(max(abs(c*u),[],2));

3.1.7 Comparison

−3 −3
x 10 x 10
5 5
9.01 9.01
13.02 13.02
4 4
17.02 17.02

3 3
Displacement [m]

Displacement [m]
2 2

1 1

0 0

−1 −1

−2 −2
0 0.5 1 1.5 2 2.5 3 3.5 4 0 0.5 1 1.5 2 2.5 3 3.5 4
Time [s] Time [s]
(a) Modal superposition in time domain (b) Modal superposition in frequency domain
−3 −3
x 10 x 10
5 5
9.01 9.01
13.02 13.02
4 4
17.02 17.02
Nodal displacements [m]

3 3
Displacement [m]

2 2

1 1

0 0

−1 −1

−2 −2
0 0.5 1 1.5 2 2.5 3 3.5 4 0 0.5 1 1.5 2 2.5 3 3.5 4
Time [s] Time [s]
(b) Direct time integration (c) Direct method in frequency domain

Figure 3.5: Nodal response: comparison.

Time domain Freq domain

Computational cost in seconds Modal superposition 0.167 0.147
Direct method 0.213 0.789
EXAMPLE 2.2: DYNAMIC ANALYSIS OF A PLATE 35

3.2 Example 2.2: dynamic analysis of a plate

In this example the eigenfrequencies of a simply supported rectangular plate are calculated using shell4 and
compared with the theoretical solution.

% StaBIL manual
% Example 2.2: dynamic analysis of a plate

% dynamic plate problem (dkt element)

% parameters

Lx = 10; % length x-direction

Ly = 10; % length y-direction
t = 1; % thickness plate
E = 200000; % E-modulus
nu = 0.3; % Poisson-coeff.
rho = 7000; % mass density
m = 20; % number of elements in x-direction
n = 20; % number of elements in y-direction
Types = {1 'shell4'}; % {EltTypID EltName}
Sections = [1 t]; % [SecID t]
Materials = [1 E nu rho]; % [MatID E nu]

% mesh

Line1 = [0 0 0;Lx 0 0];

Line2 = [Lx 0 0;Lx Ly 0];
Line3 = [Lx Ly 0;0 Ly 0];
Line4 = [0 Ly 0;0 0 0];

[Nodes,Elements,Edge1,Edge2,Edge3,Edge4] = makemesh(Line1,Line2,Line3,Line4,n,m,Types(1,:),1,1);
figure;
plotnodes(Nodes);
figure;
plotelem(Nodes,Elements,Types);

% DOFs (simply supported plate)

DOF = getdof(Elements,Types);
sdof = [0.01;0.02;0.06;[Edge1;Edge2;Edge3;Edge4]+0.03;[Edge1;Edge3]+0.05;[Edge2;Edge4]+0.04];
DOF = removedof(DOF,sdof);

% K & M

[K,M] = asmkm(Nodes,Elements,Types,Sections,Materials,DOF);

% eigenmodes

nMode = 10;
[phi,omega] = eigfem(K,M,nMode);
figure;
animdisp(Nodes,Elements,Types,DOF,phi(:,1));

% analytical solution

[mm,nn] = meshgrid((1:m),(1:n));
aomega = sqrt(E*t^2/(12*(1-nu^2)*rho))*((mm*pi/Lx).^2+(nn*pi/Ly).^2);
aomega = reshape(aomega,numel(aomega),1);
aomega = sort(aomega);
ratio = omega./aomega(1:nMode)
36 DYNAMIC ANALYSIS OF STRUCTURES

(a) 0.1268 Hz (b) 0.3170 Hz

(c) 0.3170 Hz (d) 0.5050 Hz

Figure 3.6: The first four eigenmodes of a thin plate.

fFEM [Hz] fanalytical [Hz] fFEM /fanalytical

0.1268 0.1270 0.9983
0.3170 0.3176 0.9982
0.3170 0.3176 0.9982
0.5050 0.5082 0.9939
0.6355 0.6352 1.0004
0.6355 0.6352 1.0004
0.8202 0.8258 0.9932
0.8202 0.8258 0.9932
1.0848 1.0799 1.0046
1.0848 1.0799 1.0046

Table 3.1: Eigenfrequencies of a thin plate.

Chapter 4

Element guide

This chapter presents an overview of the element types available in Stabil. The conventions (local coordinate
system, nodal connectivity) for each element type are given and reference is made to the Stabil functions related
to the element implementation.
38 ELEMENT GUIDE

beam
Tj
Vyj Nj
Myj
y j
x
Mzj
z
Vyi
Myi i
Ti

Ni
Mzi

Description
Euler-Bernoulli beam element with a cubic interpolation of the beam deflection.

Functions

dof_beam Element degrees of freedom for a beam element. p.117

ke_beam Beam element stiffness and mass matrix in global coordinate system. p.168
kelcs_beam Beam element stiffness and mass matrix in local coordinate system. p.164
trans_beam Transform coordinate system for a beam element. p.291
loads_beam Equivalent nodal forces for a beam element in the GCS. p.192
loadslcs_beam Equivalent nodal forces for a beam element in the LCS. p.189
accel_beam Compute the distributed loads for a beam due to an acceleration. p.59
forces_beam Compute the element forces for a beam element. p.153
forceslcs_beam Compute the element forces for a beam element in the LCS. p.151
nelcs_beam Shape functions for a beam element. p.206
nedloadlcs_beam Shape functions for a distributed load on a beam element. p.205
coord_beam Coordinates of the beam elements for plotting. p.78
disp_beam Return matrices to compute the displacements of the deformed beams. p.99
dispgcs2lcs_beam Transform the element displacements to the LCS for a beam. p.97
fdiagrgcs_beam Return matrices to plot the forces in a beam element. p.144
fdiagrlcs_beam Force diagram for a beam element in LCS. p.148
sdiagrgcs_beam Return matrices to plot the stresses in a beam element. p.253
sdiagrlcs_beam Stress diagram for a beam element in LCS. p.256
ELEMENT GUIDE 39

truss
Nj
y j
x

Ni

Description
Linear truss element.

Functions

dof_truss Element degrees of freedom for a truss element. p.134

ke_truss Truss element stiffness and mass matrix in global coordinate system. p.186
kelcs_truss Truss element stiffness and mass matrix in local coordinate system. p.167
trans_truss Transform coordinate system for a truss element. p.297
loads_truss Equivalent nodal forces for a truss element in the GCS. p.199
accel_truss Compute the distributed loads for a truss due to an acceleration. p.66
forces_truss Compute the element forces for a truss element. p.155
forceslcs_truss Compute the element forces for a truss element in the LCS. p.152
coord_truss Coordinates of the truss elements for plotting. p.96
disp_truss Return matrices to compute the displacements of the deformed trusses. p.115
dispgcs2lcs_truss Transform the element displacements to the LCS for a truss. p.98
fdiagrgcs_truss Return matrices to plot the forces in a truss element. p.146
sdiagrgcs_truss Return matrices to plot the stresses in a truss element. p.255
40 ELEMENT GUIDE

plane3
3

1
y

Description
The plane3 element is a 3-node linear isoparametric 2D triangular plane element, commonly referred to as the
“Constant Strain Triangle” (CST).

Functions

dof_plane3 Element degrees of freedom for a plane3 element. p.121

ke_plane3 Element stiffness and mass matrix in global coordinate system. p.173
coord_plane3 Coordinates of the plane3 element for plotting. p.83
disp_plane3 Return matrices to compute the displacements of the deformed element. p.103
se_plane3 Compute the element stresses for a plane3 element in the GCS. p.264
selcs_plane3 Compute the element stresses for a plane3 element in the LCS. p.257
patch_plane3 Patch information of the plane3 elements for plotting. p.213
ELEMENT GUIDE 41

plane4
4
3

1
y

Description
The plane4 element is a 4-node linear isoparametric 2D quadrilateral plane element.

Functions

dof_plane4 Element degrees of freedom for a plane4 element. p.122

ke_plane4 Element stiffness and mass matrix in global coordinate system. p.174
coord_plane4 Coordinates of the plane3 element for plotting. p.84
disp_plane4 Return matrices to compute the displacements of the deformed element. p.104
se_plane4 Compute the element stresses for a plane4 element in the GCS. p.265
selcs_plane4 Compute the element stresses for a plane4 element in the LCS. p.258
patch_plane4 Patch information of the plane4 elements for plotting. p.214
42 ELEMENT GUIDE

plane6
3
5
6
4 2

1
y

Description
The plane6 element is a 6-node quadratic isoparametric 2D triangular plane element.

Functions

dof_plane6 Element degrees of freedom for a plane6 element. p.123

ke_plane6 Element stiffness and mass matrix in global coordinate system. p.175
coord_plane6 Coordinates of the plane3 element for plotting. p.85
disp_plane6 Return matrices to compute the displacements of the deformed element. p.105
se_plane6 Compute the element stresses for a plane6 element in the GCS. p.266
selcs_plane6 Compute the element stresses for a plane6 element in the LCS. p.259
patch_plane6 Patch information of the plane6 elements for plotting. p.215
ELEMENT GUIDE 43

plane8
4 7
3

8 6
5 2

1
y

Description
The plane8 element is a 8-node quadratic isoparametric 2D rectangular plane element.

Functions

dof_plane8 Element degrees of freedom for a plane8 element. p.124

ke_plane8 Element stiffness and mass matrix in global coordinate system. p.176
coord_plane8 Coordinates of the plane3 element for plotting. p.86
disp_plane8 Return matrices to compute the displacements of the deformed element. p.106
se_plane8 Compute the element stresses for a plane8 element in the GCS. p.267
selcs_plane8 Compute the element stresses for a plane8 element in the LCS. p.260
patch_plane8 Patch information of the plane8 elements for plotting. p.216
44 ELEMENT GUIDE

plane10
3
7
8
10 6
9 2
5
1 4
y

Description
The plane10 element is a 10-node cubic isoparametric 2D triangular plane element.

Functions

dof_plane10 Element degrees of freedom for a plane10 element. p.119

ke_plane10 Element stiffness and mass matrix in global coordinate system. p.171
coord_plane10 Coordinates of the plane3 element for plotting. p.81
disp_plane10 Return matrices to compute the displacements of the deformed element. p.101
ELEMENT GUIDE 45

plane15
3
9
10 8
15
11 14 7
13
12 2
6
1 4 5
y

Description
The plane15 element is a 15-node quartic isoparametric 2D triangular plane element.

Functions

dof_plane15 Element degrees of freedom for a plane8 element. p.120

ke_plane15 Element stiffness and mass matrix in global coordinate system. p.172
coord_plane15 Coordinates of the plane3 element for plotting. p.82
disp_plane15 Return matrices to compute the displacements of the deformed element. p.102
46 ELEMENT GUIDE

solid4
4

z
1
2

x y

Description
The solid4 element is a 4-node linear isoparametric 3D solid tetrahedral element.

Functions

dof_solid4 Element degrees of freedom for a solid4 element. p.132

ke_solid4 Element stiffness and mass matrix in global coordinate system. p.184
coord_solid4 Coordinates of the plane3 element for plotting. p.94
patch_solid4 Patch information of the solid4 elements for plotting. p.222
ELEMENT GUIDE 47

solid8
8

5 7
6

4
z
1 3

x y 2

Description
The solid8 element is a 8-node linear isoparametric 3D solid element.

Functions

dof_solid8 Element degrees of freedom for a solid4 element. p.133

ke_solid8 Element stiffness and mass matrix in global coordinate system. p.185
coord_solid8 Coordinates of the plane3 element for plotting. p.95
patch_solid8 Patch information of the solid8 elements for plotting. p.223
48 ELEMENT GUIDE

solid10
4
10
8 3
7 9
z 6
1
5
2

x y

Description
The solid10 element is a 10-node quadratic isoparametric 3D solid tetrahedral element.

Functions

dof_solid10 Element degrees of freedom for a solid10 element. p.129

ke_solid10 Element stiffness and mass matrix in global coordinate system. p.181
coord_solid10 Coordinates of the plane3 element for plotting. p.91
disp_solid10 Return matrices to compute the displacements of the deformed element. p.111
patch_solid10 Patch information of the solid10 elements for plotting. p.220
ELEMENT GUIDE 49

solid15
12 6
4 11
10
5 15
13 14
9 3
z
1 8
7
2

x y

Description
The solid15 element is a 15-node quadratic isoparametric 3D solid tetrahedral element.

dof_solid15 Element degrees of freedom for a solid15 element. p.130

ke_solid15 Element stiffness and mass matrix in global coordinate system. p.182
coord_solid15 Coordinates of the plane3 element for plotting. p.92
disp_solid15 Return matrices to compute the displacements of the deformed element. p.112
50 ELEMENT GUIDE

solid20
8 15 7
16
5 14
13
6
20 19
17 18
4 11
12 3
z
1 10
9
2

x y

Description
The solid20 element is a 20-node quadratic isoparametric 3D solid tetrahedral element.

Functions

dof_solid20 Element degrees of freedom for a solid20 element. p.131

ke_solid20 Element stiffness and mass matrix in global coordinate system. p.183
coord_solid20 Coordinates of the plane3 element for plotting. p.93
disp_solid20 Return matrices to compute the displacements of the deformed element. p.113
patch_solid20 Patch information of the solid10 elements for plotting. p.221
ELEMENT GUIDE 51

shell4
4

3
1
z

x y

Description
Shell element consisting of a bilinear membrane element and four overlaid DKT triangles for the bending
stiffness.

Functions

dof_shell4 Element degrees of freedom for a shell4 element. p.126

ke_shell4 Shell4 element stiffness and mass matrix in global coordinate system. p.178
kelcs_shell4 Shell4 element stiffness and mass matrix in local coordinate system. p.166
trans_shell4 Transform coordinate system for a shell4 element. p.293
ke_dkt DKT plate element stiffness and mass matrix. p.169
q_dkt Q matrix for a DKT element. p.247
sh_qs4 Shape functions for a quadrilateral serendipity element with 4 nodes. p.274
sh_t Shape functions for a triangular plate element. p.276
se_shell4 Compute the element stresses for a shell4 element. p.268
selcs_shell4 Compute the element stresses for a shell4 element. p.261
accel_shell4 Compute the distributed loads for a shell due to an acceleration. p.61
loads_shell4 Equivalent nodal forces for a shell4 element in the GCS. p.194
loadslcs_shell4 Equivalent nodal forces for a shell4 element in the LCS. p.191
pressure_shell4 Equivalent nodal forces for a shell4 element in the GCS due to a pressure. p.239
coord_shell4 Coordinates of the shell4 elements for plotting. p.88
disp_shell4 Matrices to compute the displacements of the deformed shell. p.108
scontour_shell4 Matrix to plot contours in a shell4 element. p.251
patch_shell4 Patch information of the shell4 elements for plotting. p.217
grid_shell4 Grid in natural coordinates for mapped meshing. p.162
52 ELEMENT GUIDE

shell6
3
6 5
1 4
z 2

x y

Description
This element is based on chapter 15 of Zienkiewicz [9].

dof_shell6 Element degrees of freedom for a shell4 element. p.127

ke_shell6 Shell6 element stiffness and mass matrix in global coordinate system. p.179
ke_dkt DKT plate element stiffness and mass matrix. p.169
q_dkt Q matrix for a DKT element. p.247
se_shell6 Compute the element stresses for a shell4 element. p.269
accel_shell6 Compute the distributed loads for a shell due to an acceleration. p.62
loads_shell6 Equivalent nodal forces for a shell6 element in the GCS. p.195
pressure_shell6 Equivalent nodal forces for a shell6 element in the GCS due to a pressure. p.240
coord_shell6 Coordinates of the shell6 elements for plotting. p.89
disp_shell6 Matrices to compute the displacements of the deformed shell. p.109
patch_shell6 Patch information of the shell6 elements for plotting. p.218
ELEMENT GUIDE 53

shell8
4
8 7
3
1
z 5 6
2

x y

Description
This element is based on chapter 15 of Zienkiewicz [9].

Functions

dof_shell8 Element degrees of freedom for a shell8 element. p.128

ke_shell8 shell8 element stiffness and mass matrix in global coordinate system. p.180
sh_qs8 Shape functions for a quadrilateral serendipity element with 8 nodes. p.275
b_shell8 B matrix for a shell8 element in global coordinate system. p.73
se_shell8 Compute the element stresses for a shell8 element. p.270
accel_shell8 Compute the distributed loads for a shell due to an acceleration. p.63
loads_shell8 Equivalent nodal forces for a shell8 element in the GCS. p.196
pressure_shell8 Equivalent nodal forces for a shell8 element in the GCS due to a pressure. p.241
coord_shell8 Coordinates of the shell8 elements for plotting. p.90
disp_shell8 Matrices to compute the displacements of the deformed shell. p.110
scontour_shell8 Matrix to plot contours in a shell8 element. p.252
patch_shell8 Patch information of the shell8 elements for plotting. p.219
grid_shell8 Grid in natural coordinates for mapped meshing. p.163
54 ELEMENT GUIDE

mass
ϕz

uz
1
ux uy
z
ϕx ϕy

x y

Description
Single point concentrated mass element with 6 degrees of freedom.

Functions

dof_mass Element degrees of freedom for a mass element. p.118

ke_mass Element stiffness and mass matrix in global coordinate system. p.170
coord_mass Coordinates of the mass element for plotting. p.80
disp_mass Return matrices to compute the displacements of the deformed element. p.100
patch_mass Patch information of the mass elements for plotting. p.212
Chapter 5

Functions — By category

5.1 General functions

getdof Get the vector with the degrees of freedom of the model. p.159
asmkm Assemble stiffness and mass matrix. p.70
removedof Remove DOF with Dirichlet boundary conditions equal to zero. p.249
addconstr Add constraint equations to the stiffness matrix and load vector. p.67
tconstr Return matrices to apply constraint equations. p.288
nodalvalues Construct a vector with the values at the selected DOF. p.210
elemloads Equivalent nodal forces. p.138
accel Compute the distributed loads due to an acceleration. p.58
elemforces Compute the element forces. p.137
elemdisp Select the element displacements from the global displacement vector. p.136
selectdof Select degrees of freedom. p.262
unselectdof Unselect degrees of freedom. p.299
selectnode Select nodes by location. p.263
reprow Replicate rows from a matrix. p.250
multdloads Combine distributed loads. p.204

5.2 Postprocessing

plotnodes Plot the nodes. p.232

plotelem Plot the elements. p.227
plotdisp Plot the displacements. p.225
plotforc Plot the forces. p.229
plotlcs Plot the local element coordinate systems. p.231
plotstress Plot the stresses. p.236
plotstresscontour Plot stress contours. p.237
plotstresscontourf Plot filled contours of stresses. p.238
animdisp Animate the displacements. p.68
getmovie Get the movie from a figure where an animation has been played. p.160
printdisp Display the displacements in the command window. p.243
printforc Display the forces in the command window. p.244
56 FUNCTIONS — BY CATEGORY

5.3 Dynamics

eigfem Compute eigenmodes and eigenfrequencies. p.135

msupt Modal superposition in the time domain. p.203
msupf Modal superposition in the frequency domain. p.202
cdiff Direct time integration for dynamic systems - central diff. method. p.74
newmark Direct time integration for dynamic systems - Newmark method p.207
wilson Direct time integration for dynamic systems - Wilson-theta method p.302

5.4 General shell functions

elempressure Equivalent nodal forces for pressure ⊥ shell surface. p.139

gaussq Gauss points for 2D numerical integration. p.156
nodalshellf Compute the nodal shell forces/moments from element solution. p.208
nodalstress Compute the nodal stresses from element solution. p.209
plotprincstress Plot the principal stresses. p.233
plotshellfcontour Plot contour lines of forces/moments per unit length. p.234
plotstresscontour Plot stress contour lines. p.237
plotshellfcontourf Plot filled contours of shell forces. p.235
principalstress Compute the principal stresses and directions. p.242
printshellf Display forces/moments in command window (shell elements). p.245
printstress Display stresses in command window (shell elements). p.246
Chapter 6

Functions — Alphabetical list

58 FUNCTIONS — ALPHABETICAL LIST

accel
ACCEL Compute the distributed loads due to an acceleration.

DLoads=accel(Accelxyz,Nodes,Elements,Types,Sections,Materials)
computes the distributed loads due to an acceleration.
In order to simulate gravity, accelerate the structure in the direction
opposite to gravity.

Accelxyz Acceleration [Ax Ay Az] (1 * 3)

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
Sections Section definitions [SecID SecProp1 SecProp2 ...]
Materials Material definitions [MatID MatProp1 MatProp2 ... ]
DLoads Distributed loads [EltID n1globalX n1globalY n1globalZ ...]

See also ELEMLOADS, ACCEL_BEAM, ACCEL_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 59

accel beam
ACCEL_BEAM Compute the distributed loads for a beam due to an acceleration.

DLoads=accel_beam(Accelxyz,[],Elements,Sections,Materials,Options)
computes the distributed loads for a beam due to an acceleration.
In order to simulate gravity, accelerate the structure in the direction
opposite to gravity.

Accelxyz Acceleration [Ax Ay Az] (1 * 3)

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Sections Section definitions [SecID SecProp1 SecProp2 ...]
Materials Material definitions [MatID MatProp1 MatProp2 ... ]
Options Element options {Option1 Option2 ...}
DLoads Distributed loads [EltID n1globalX n1globalY n1globalZ ...]

See also ACCEL, ACCEL_TRUSS.

60 FUNCTIONS — ALPHABETICAL LIST

accel shell2
ACCEL_SHELL2 Compute the distributed loads for a SHELL2 element due to an acceleration.

DLoads=accel_shell2(Accelxyz,Nodes,Elements,Sections,Materials,Options)
computes the distributed loads for a SHELL2 element due to an acceleration.
In order to simulate gravity, accelerate the structure in the direction
opposite to gravity.

Accelxyz Acceleration [Ax Ay Az] (1 * 3)

Nodes Node definitions [NodeID x y z]
Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Sections Section definitions [SecID SecProp1 SecProp2 ...]
Materials Material definitions [MatID MatProp1 MatProp2 ... ]
Options Element options {Option1 Option2 ...}
DLoads Distributed loads [EltID n1globalX n1globalY n1globalZ ...]
FUNCTIONS — ALPHABETICAL LIST 61

accel shell4
ACCEL_SHELL4 Compute the distributed loads for shell4 elements due to an
acceleration.

DLoads = accel_shell4(Accelxyz,[],Elements,Sections,Materials,Options)
computes the distributed loads for shell4 elements due to an acceleration.
In order to simulate gravity, accelerate the structure in the direction
opposite to gravity.

Accelxyz Acceleration [Ax Ay Az] (1 * 3)

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Sections Section definitions [SecID SecProp1 SecProp2 ...]
Materials Material definitions [MatID MatProp1 MatProp2 ... ]
Options Element options {Option1 Option2 ...}
DLoads Distributed loads [EltID n1globalX n1globalY n1globalZ ...]

See also ACCEL, ACCEL_TRUSS.

62 FUNCTIONS — ALPHABETICAL LIST

accel shell6
ACCEL_SHELL6 Compute the distributed loads for shell6 elements due to an acceleration.

DLoads = accel_shell6(Accelxyz,[],Elements,Sections,Materials,Options)
computes the distributed loads for shell8 elements due to an acceleration.
In order to simulate gravity, accelerate the structure in the direction
opposite to gravity.

Accelxyz Acceleration [Ax Ay Az] (1 * 3)

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Sections Section definitions [SecID SecProp1 SecProp2 ...]
Materials Material definitions [MatID MatProp1 MatProp2 ... ]
Options Element options struct. Fields:
-MatType: ’isotropic’ (default) or ’orthotropic’
DLoads Distributed loads [EltID n1globalX n1globalY n1globalZ ...]

See also ACCEL, ACCEL_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 63

accel shell8
ACCEL_SHELL8 Compute the distributed loads for shell8 elements due to an acceleration.

DLoads = accel_shell8(Accelxyz,[],Elements,Sections,Materials,Options)
computes the distributed loads for shell8 elements due to an acceleration.
In order to simulate gravity, accelerate the structure in the direction
opposite to gravity.

Accelxyz Acceleration [Ax Ay Az] (1 * 3)

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Sections Section definitions [SecID SecProp1 SecProp2 ...]
Materials Material definitions [MatID MatProp1 MatProp2 ... ]
Options Element options struct. Fields:
-MatType: ’isotropic’ (default) or ’orthotropic’
DLoads Distributed loads [EltID n1globalX n1globalY n1globalZ ...]

See also ACCEL, ACCEL_TRUSS.

64 FUNCTIONS — ALPHABETICAL LIST

accel solid20
ACCEL_SOLID20 Compute the distributed loads for solid20 elements due to an
acceleration.

DLoads = accel_solid20(Accelxyz,[],Elements,Sections,Materials,Options)
computes the distributed loads for solid20 elements due to an acceleration.
In order to simulate gravity, accelerate the structure in the direction
opposite to gravity.

Accelxyz Acceleration [Ax Ay Az] (1 * 3)

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Sections Section definitions [SecID SecProp1 SecProp2 ...]
Materials Material definitions [MatID MatProp1 MatProp2 ... ]
Options Element options {Option1 Option2 ...}
DLoads Distributed loads [EltID n1globalX n1globalY n1globalZ ...]

See also ACCEL, ACCEL_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 65

accel solid8
ACCEL_SOLID8 Compute the distributed loads for solid8 elements due to an
acceleration.

DLoads = accel_solid8(Accelxyz,[],Elements,Sections,Materials,Options)
computes the distributed loads for solid8 elements due to an acceleration.
In order to simulate gravity, accelerate the structure in the direction
opposite to gravity.

Accelxyz Acceleration [Ax Ay Az] (1 * 3)

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Sections Section definitions [SecID SecProp1 SecProp2 ...]
Materials Material definitions [MatID MatProp1 MatProp2 ... ]
Options Element options {Option1 Option2 ...}
DLoads Distributed loads [EltID n1globalX n1globalY n1globalZ ...]

See also ACCEL, ACCEL_TRUSS.

66 FUNCTIONS — ALPHABETICAL LIST

accel truss
ACCEL_TRUSS Compute the distributed loads for a truss due to an acceleration.

DLoads=accel_truss(Accelxyz,[],Elements,Sections,Materials,Options)
computes the distributed loads for a truss due to an acceleration.
In order to simulate gravity, accelerate the structure in the direction
opposite to gravity.

Accelxyz Acceleration [Ax Ay Az] (1 * 3)

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Sections Section definitions [SecID SecProp1 SecProp2 ...]
Materials Material definitions [MatID MatProp1 MatProp2 ... ]
Options Element options {Option1 Option2 ...}
DLoads Distributed loads [EltID n1globalX n1globalY n1globalZ ...]

See also ACCEL, ACCEL_BEAM.

FUNCTIONS — ALPHABETICAL LIST 67

addconstr
ADDCONSTR Add constraint equations to the stiffness matrix and load vector.

[K,F]=addconstr(Constr,DOF,K,F)
[K,F,M]=addconstr(Constr,DOF,K,[],M)
[K,F,M]=addconstr(Constr,DOF,K,F,M)
modifies the stiffness matrix, the mass matrix and the load vector according
to the applied constraint equations. The dimensions of the stiffness matrix,
the mass matrix and the load vector are kept the same. The resulting
stiffness and mass matrix are not symmetric anymore. This function can be
used as well to apply imposed displacements.

Constr Constraint equation:

Constant=CoefS*SlaveDOF+CoefM1*MasterDOF1+CoefM2*MasterDOF2+...
[Constant CoefS SlaveDOF CoefM1 MasterDOF1 CoefM2 MasterDOF2 ...]
DOF Degrees of freedom (nDOF * 1)
K Stiffness matrix (nDOF * nDOF)
F Load vector (nDOF * nSteps)
M Mass matrix (nDOF * nDOF)
68 FUNCTIONS — ALPHABETICAL LIST

animdisp
ANIMDISP Animate the displacements.

DispScal=animdisp(Nodes,Elements,Types,DOF,U)
animates the displacements.

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
DOF Degrees of freedom (nDOF * 1)
U Displacements (nDOF * nSteps)
DispScal Displacement scaling

ANIMDISP(...,ParamName,ParamValue) sets the value of the specified

parameters. The following parameters can be specified:
’DispScal’ Displacement scaling. Default: ’auto’.
’Handle’ Plots in the axis with this handle. Default: current axis.
’Fps’ Frames per second. Default: 12.
’CreateMovie’ Saves the movie in the userdata of the axis of the figure.
Use getmovie to get the movie from the axis. Default: ’off’.
’Counter’ Displays the number of the frame for transient displacements.
Default: ’on’.
Additional parameters are redirected to the PLOTDISP function which plots
the individual frames of the movie.

See also GETMOVIE, PLOTDISP.

FUNCTIONS — ALPHABETICAL LIST 69

argdimchk
ARGDIMCHK Validate input argument dimensions.

msg = ARGDIMCHK(arg1,size1,arg2,size2,...) returns an appropriate error

message if the dimensions of arg1,arg2,... do not comply with size1,size2,...
respectively. If they do comply, an empty matrix is returned.
size1,size2,... are cell arrays consisting of at least 2 cells. Each cell
corresponds to a dimension of arg1,arg2,... and contains a number (to
constrain the dimension explicitly) or a string (to constrain the dimension
implicitly). E.g. the expression:

ERROR(ARGDIMCHK( ...
omega,{’nMode’, 1 }, ...
Phi, {’nDof’, ’nMode’ }, ...
xi, {’nMode’, 1 }, ...
b, {’nDof’, 1 }, ...
q, { 1, ’nOmega’}, ...
Omega,{ 1, ’nOmega’}, ...
c, {’nSelDof’,’nDof’ }));

checks if omega,Phi,xi,b,q,Omega,c are all 2-dimensional variables and if

SIZE(omega,2)==1 SIZE(Phi,2)==SIZE(omega,1)
SIZE(xi,1)==SIZE(omega,1) SIZE(xi,2)==1
SIZE(b,1)==SIZE(Phi,1) SIZE(b,2)==1
SIZE(q,1)==1 SIZE(Omega,1)==1
SIZE(Omega,2)==SIZE(q,2) SIZE(c,2)==SIZE(Phi,1)
If not, an appropriate error message is shown.
70 FUNCTIONS — ALPHABETICAL LIST

asmkm
ASMKM Assemble stiffness and mass matrix.

[K,M] = ASMKM(Nodes,Elements,Types,Sections,Materials,DOF)
K = ASMKM(Nodes,Elements,Types,Sections,Materials,DOF)
K = ASMKM(Nodes,Elements,Types,Sections,Materials)
assembles the stiffness and the mass matrix using the finite element method.

[K,~,dKdx] = ASMKM(Nodes,Elements,Types,Sections,Materials,DOF,dNodesdx,dSectionsdx)
assembles the stiffness matrix using the finite element method and
additionally computes the derivatives of the stiffness matrix with
respect to the design variables x. The derivatives of the mass matrix
have not yet been implemented.

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ...}
Sections Section definitions [SecID SecProp1 SecProp2 ...]
Materials Material definitions [MatID MatProp1 MatProp2 ...]
DOF Degrees of freedom (nDOF * 1)
dNodesdx Node definitions derivatives (SIZE(Nodes) * nVar)
dSectionsdx Section definitions derivatives (SIZE(Sections) * nVar)
K Stiffness matrix (nDOF * nDOF)
M Mass matrix (nDOF * nDOF)
dKdx Stiffness matrix derivatives (CELL(nVar,1))

See also KE_TRUSS, KE_BEAM.

FUNCTIONS — ALPHABETICAL LIST 71

be plane3
e_plane3 is a function.
[BeGCS] = be_plane3(Node, Section, Material, UeGCS, Options, gcs)
72 FUNCTIONS — ALPHABETICAL LIST

b shell6
B_SHELL6 b matrix for a shell6 element in global coordinate system.

[Bg,J] = b_shell6(Ni,dN_dxi,dN_deta,zetar,Node,h,v1i,v2i,v3i) returns

the element b matrix in the global coordinate system and the Jacobian
of the parametric transformation. Both are evaluated in the natural
coordinates (xi,eta and zetar) which were used to calculate
Ni,dN_dxi,dN_deta and zetar.

Node Node definitions [x y z] (6 * 3)

Nodes should have the following order:
3
| \
6 5
| \
1--4--2
Ni Shape functions for quadratic serendipity element (6 * 1)
dN_dxi first derivatives of shape functions Ni (6 * 1)
dN_deta first derivatives of shape functions Ni (6 * 1)
h scalar or vector containing thickness scalar or (6 * 1)
v(1,2,3)i components of the local coordinate system in node i (6 * 3)
d Nodal offset from shell mid plane scalar (default = 0)
Bg b matrix of shell8 element (6 * 36)
J Jacobian of the parametric transformation (3 * 3)

See also SE_SHELL8, KE_SHELL8.

FUNCTIONS — ALPHABETICAL LIST 73

b shell8
B_SHELL8 b matrix for a shell8 element in global coordinate system.

[Bg,J] = b_shell8(Ni,dN_dxi,dN_deta,zetar,Node,h,v1i,v2i,v3i) returns

the element b matrix in the global coordinate system and the Jacobian
of the parametric transformation. Both are evaluated in the natural
coordinates (xi,eta and zetar) which were used to calculate
Ni,dN_dxi,dN_deta and zetar.

Node Node definitions [x y z] (8 * 3)

Nodes should have the following order:
4----7----3
| |
8 6
| |
1----5----2
Ni Shape functions for quadratic serendipity element (8 * 1)
dN_dxi first derivatives of shape functions Ni (8 * 1)
dN_deta first derivatives of shape functions Ni (8 * 1)
h scalar or vector containing thickness scalar or (8 * 1)
v(1,2,3)i components of the local coordinate system in node i (8 * 3)
d Nodal offset from shell mid plane scalar (default = 0)
Bg b matrix of shell8 element (6 * 48)
J Jacobian of the parametric transformation (3 * 3)

See also SE_SHELL8, KE_SHELL8.

74 FUNCTIONS — ALPHABETICAL LIST

cdiff
CDIFF Direct time integration for dynamic systems - central diff. method.
[u,t] = CDIFF(M,C,K,dt,p,u0,u1) applies the central difference method for
the calculation of the nodal displacements u of the dynamic system with
the system matrices M, C and K due to the excitation p.

M Mass matrix (nDof * nDof)

C Damping matrix (nDof * nDof)
K Stiffness matrix (nDof * nDof)
dt Time step of the integration scheme (1 * 1). Should be small enough
to ensure the stability and the precision of the integration scheme.
p Excitation (nDof * N). p(:,k) corresponds to time point t(k).
u0 Displacements at time point t(1)-dt (nDof * 1). Defaults to zero.
u1 Displacements at time point t(1) (nDof * 1). Defaults to zero.
u Displacements (nDof * N). u(:,k) corresponds to time point t(k).
t Time axis (1 * N), defined as t = [0:N-1] * dt.
FUNCTIONS — ALPHABETICAL LIST 75

checkunique
CHECKUNIQUE Check if vector contains unique elements.

checkunique(p,name)
find non-unique elements in a vector and print error

p Vector with elements to be checked

name Name of elements in p
76 FUNCTIONS — ALPHABETICAL LIST

cmat isotropic
CMAT_ISOTROPIC Constitutive matrix for isotropic materials.

[C,C_lambda,C_mu]==cmat_isotropic(problem,Section,Material)
computes the constitutive matrix for isotropic materials.

problem
Section Section definition
Material Material definition
C Constitutive matrix (nStress * nStrain)
C_lambda Contribution of lambda to C (nStress * nStrain)
C_mu Contribution of mu to C (nStress * nStrain)
FUNCTIONS — ALPHABETICAL LIST 77

cmat shell8
CMAT_SHELL8 Constitutive matrix for shell8 element

C = cmat_shell8(MatType,Material,k)
C = cmat_shell8(MatType,Material)
returns the constitutive matrix for shell8 elements.

MatType Material type: ’isotropic’ or ’orthotropic’

Material Material definition
isotropic: [E nu rho]
orthotropic: [Exx Eyy nuxy muxy muyz muzx theta rho]
k Geometric coefficient for non-uniform shear stress (default = 1.2)
C Constitutive matrix (5 * 5)

See also KE_SHELL8

78 FUNCTIONS — ALPHABETICAL LIST

coord beam
COORD_BEAM Coordinates of the beam elements for plotting.

[X,Y,Z]=coord_beam(Nodes,NodeNum)
returns the coordinates of the beam elements for plotting.

Nodes Node definitions [NodID x y z] (nNodes * 4)

NodeNum Node numbers [NodID1 NodID2 NodID3] (nElem * 3)
X X coordinates (2 * nElem)
Y Y coordinates (2 * nElem)
Z Z coordinates (2 * nElem)

See also COORD_TRUSS, PLOTELEM.

FUNCTIONS — ALPHABETICAL LIST 79

coord kbeam
COORD_BEAM Coordinates of the beam elements for plotting.

coord_beam(Nodes,NodeNum)
returns the coordinates of the beam elements for plotting.

Nodes Node definitions [NodID x y z] (nNodes * 4)

NodeNum Node numbers [NodID1 NodID2 NodID3] (nElem * 3)
X X coordinates (2 * nElem)
Y Y coordinates (2 * nElem)
Z Z coordinates (2 * nElem)

See also COORD_TRUSS, PLOTELEM.

80 FUNCTIONS — ALPHABETICAL LIST

coord mass
COORD_MASS Coordinates of the mass element for plotting.

[X,Y,Z]=coord_mass(Nodes,NodeNum)
returns the coordinates of the mass element for plotting.

Nodes Node definitions [NodID x y z] (nNode * 4)

NodeNum Node numbers [NodID1] (nElem * 1)
X X coordinates (1 * nElem)
Y Y coordinates (1 * nElem)
Z Z coordinates (1 * nElem)

See also COORD_BEAM, PLOTELEM.

FUNCTIONS — ALPHABETICAL LIST 81

coord plane10
COORD_PLANE10 Coordinates of the plane elements for plotting.

[X,Y,Z] = coord_plane10(Nodes,NodeNum)
returns the coordinates of the plane10 elements for plotting.

Nodes Node definitions [NodID x y z] (nNodes * 4)

NodeNum Node numbers [NodID1 NodID2 ...] (nElem * 10)
X X coordinates (15 * nElem)
Y Y coordinates (15 * nElem)
Z Z coordinates (15 * nElem)

See also COORD_TRUSS, PLOTELEM.

82 FUNCTIONS — ALPHABETICAL LIST

coord plane15
COORD_PLANE15 Coordinates of the plane elements for plotting.

[X,Y,Z] = coord_plane15(Nodes,NodeNum)
returns the coordinates of the plane15 elements for plotting.

Nodes Node definitions [NodID x y z] (nNodes * 4)

NodeNum Node numbers [NodID1 NodID2 ...] (nElem * 15)
X X coordinates (15 * nElem)
Y Y coordinates (15 * nElem)
Z Z coordinates (15 * nElem)

See also COORD_TRUSS, PLOTELEM.

FUNCTIONS — ALPHABETICAL LIST 83

coord plane3
COORD_PLANE3 Coordinates of PLANE3 element sides for plotting.

[X,Y,Z]=coord_plane3(Nodes,Nodenumbers)
returns the coordinates of PLANE3 element sides for plotting.

Nodes Node definitions [NodID x y z] (nNodes * 3)

Nodenumbers Node numbers [NodID1 NodID2 NodID3] (nElem * 3)
X X coordinates (3 * nElem)
Y Y coordinates (3 * nElem)
Z Z coordinates (3 * nElem)
84 FUNCTIONS — ALPHABETICAL LIST

coord plane4
COORD_PLANE4 Coordinates of the plane elements for plotting.

[X,Y,Z] = coord_plane4(Nodes,NodeNum)
returns the coordinates of the plane4 elements for plotting.

Nodes Node definitions [NodID x y z] (nNodes * 4)

NodeNum Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 4)
X X coordinates (4 * nElem)
Y Y coordinates (4 * nElem)
Z Z coordinates (4 * nElem)

See also COORD_TRUSS, PLOTELEM.

FUNCTIONS — ALPHABETICAL LIST 85

coord plane6
COORD_PLANE6 Coordinates of the plane elements for plotting.

[X,Y,Z] = coord_plane6(Nodes,NodeNum)
returns the coordinates of the plane6 elements for plotting.

Nodes Node definitions [NodID x y z] (nNodes * 4)

NodeNum Node numbers [NodID1 NodID2 ...] (nElem * 6)
X X coordinates (6 * nElem)
Y Y coordinates (6 * nElem)
Z Z coordinates (6 * nElem)

See also COORD_TRUSS, PLOTELEM.

86 FUNCTIONS — ALPHABETICAL LIST

coord plane8
COORD_PLANE8 Coordinates of the shell8 elements for plotting.

coord_plane8(Nodes,NodeNum)
returns the coordinates of the plane8 elements for plotting.

Nodes Node definitions [NodID x y z] (nNodes * 4)

NodeNum Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 8)
X X coordinates (20 * nElem)
Y Y coordinates (20 * nElem)
Z Z coordinates (20 * nElem)

See also COORD_TRUSS, PLOTELEM.

FUNCTIONS — ALPHABETICAL LIST 87

coord shell2
COORD_SHELL2 Coordinates of SHELL2 elements for plotting.

[X,Y,Z]=coord_shell2(Nodes,NodeNum)
returns the coordinates of the SHELL2 elements for plotting.

Nodes Node definitions [NodID x y z] (nNodes * 4)

NodeNum Node numbers [NodID1 NodID2] (nElem * 2)
X X coordinates (2 * nElem)
Y Y coordinates (2 * nElem)
Z Z coordinates (2 * nElem)
88 FUNCTIONS — ALPHABETICAL LIST

coord shell4
COORD_SHELL4 Coordinates of the shell elements for plotting.

[X,Y,Z] = coord_shell4(Nodes,NodeNum)
returns the coordinates of the shell4 elements for plotting.

Nodes Node definitions [NodID x y z] (nNodes * 4)

NodeNum Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 4)
X X coordinates (4 * nElem)
Y Y coordinates (4 * nElem)
Z Z coordinates (4 * nElem)

See also COORD_TRUSS, PLOTELEM.

FUNCTIONS — ALPHABETICAL LIST 89

coord shell6
COORD_SHELL6 Coordinates of the shell6 elements for plotting.

[X,Y,Z] = coord_shell6(Nodes,NodeNum)
returns the coordinates of the shell6 elements for plotting.

Nodes Node definitions [NodID x y z] (nNodes * 4)

NodeNum Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 6)
X X coordinates (15 * nElem)
Y Y coordinates (15 * nElem)
Z Z coordinates (15 * nElem)

See also COORD_TRUSS, PLOTELEM.

90 FUNCTIONS — ALPHABETICAL LIST

coord shell8
COORD_SHELL8 Coordinates of the shell8 elements for plotting.

[X,Y,Z] = coord_shell8(Nodes,NodeNum)
returns the coordinates of the shell8 elements for plotting.

Nodes Node definitions [NodID x y z] (nNodes * 4)

NodeNum Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 8)
X X coordinates (20 * nElem)
Y Y coordinates (20 * nElem)
Z Z coordinates (20 * nElem)

See also COORD_TRUSS, PLOTELEM.

FUNCTIONS — ALPHABETICAL LIST 91

coord solid10
COORD_SOLID10 Coordinates of SOLID10 element sides for plotting.

[X,Y,Z]=coord_solid10(Nodes,Nodenumbers)
returns the coordinates of SOLID10 element sides for plotting.

Nodes Node definitions [NodID x y z] (nNodes * 4)

Nodenumbers Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 4)
X X coordinates (4 * nElem)
Y Y coordinates (4 * nElem)
Z Z coordinates (4 * nElem)
92 FUNCTIONS — ALPHABETICAL LIST

coord solid15
COORD_SOLID8 Coordinates of SOLID15 element sides for plotting.

[X,Y,Z]=coord_solid15(Nodes,Nodenumbers)
returns the coordinates of SOLID15 element sides for plotting.

Nodes Node definitions [NodID x y z] (nNodes * 4)

Nodenumbers Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 4)
X X coordinates (4 * nElem)
Y Y coordinates (4 * nElem)
Z Z coordinates (4 * nElem)
FUNCTIONS — ALPHABETICAL LIST 93

coord solid20
COORD_SOLID20 Coordinates of SOLID20 element sides for plotting.

[X,Y,Z]=coord_solid20(Nodes,Nodenumbers)
returns the coordinates of SOLID20 element sides for plotting.

Nodes Node definitions [NodID x y z] (nNodes * 4)

Nodenumbers Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 4)
X X coordinates (4 * nElem)
Y Y coordinates (4 * nElem)
Z Z coordinates (4 * nElem)
94 FUNCTIONS — ALPHABETICAL LIST

coord solid4
COORD_SOLID4 Coordinates of SOLID4 element sides for plotting.

[X,Y,Z]=coord_rshell(Nodes,Nodenumbers)
returns the coordinates of RSHELL element sides for plotting.

Nodes Node definitions [NodID x y z] (nNodes * 4)

Nodenumbers Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 4)
X X coordinates (4 * nElem)
Y Y coordinates (4 * nElem)
Z Z coordinates (4 * nElem)
FUNCTIONS — ALPHABETICAL LIST 95

coord solid8
COORD_SOLID8 Coordinates of SOLID8 element sides for plotting.

[X,Y,Z]=coord_solid8(Nodes,Nodenumbers)
returns the coordinates of the SOLID8 element sides for plotting.

Nodes Node definitions [NodID x y z] (nNodes * 4)

Nodenumbers Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 4)
X X coordinates (4 * nElem)
Y Y coordinates (4 * nElem)
Z Z coordinates (4 * nElem)
96 FUNCTIONS — ALPHABETICAL LIST

coord truss
COORD_TRUSS Coordinates of the truss elements for plotting.

[X,Y,Z]=coord_truss(Nodes,NodeNum)
returns the coordinates of the truss elements for plotting.

Nodes Node definitions [NodID x y z] (nNodes * 4)

NodeNum Node numbers [NodID1 NodID2] (nElem * 2)
X X coordinates (2 * nElem)
Y Y coordinates (2 * nElem)
Z Z coordinates (2 * nElem)

See also COORD_BEAM, PLOTELEM.

FUNCTIONS — ALPHABETICAL LIST 97

dispgcs2lcs beam
DISPGCS2LCS_BEAM Transform the element displacements to the LCS for a beam.

UeLCS=dispgcs2lcs_beam(UeGCS,Node)
transforms the element displacements from the GCS to the LCS for a beam
element.

Node Node definitions [x y z] (3 * 3)

UeGCS Displacements in the GCS (12 * 1)
UeLCS Displacements in the LCS (12 * 1)

See also DISPGCS2LCS_TRUSS.

98 FUNCTIONS — ALPHABETICAL LIST

dispgcs2lcs truss
DISPGCS2LCS_TRUSS Transform the element displacements to the LCS for a truss.

UeLCS=dispgcs2lcs_truss(UeGCS,Node)
transforms the element displacements from the GCS to the LCS for a truss
element.

Node Node definitions [x y z] (2 * 3)

UeGCS Displacements in the GCS (6 * 1)
UeLCS Displacements in the LCS (6 * 1)

See also DISPGCS2LCS_BEAM.

FUNCTIONS — ALPHABETICAL LIST 99

disp beam
DISP_BEAM Return matrices to compute the displacements of the deformed beams.

[Ax,Ay,Az,B,Cx,Cy,Cz] = DISP_BEAM(Nodes,Elements,DOF,DLoads,Sections,Materials,Points)
[Ax,Ay,Az,B,Cx,Cy,Cz] = DISP_BEAM(Nodes,Elements,DOF,DLoads,Sections,Materials)
[Ax,Ay,Az,B] = DISP_BEAM(Nodes,Elements,DOF,[],Sections,Materials)
[Ax,Ay,Az,B] = DISP_BEAM(Nodes,Elements,DOF)
returns the matrices to compute the displacements of the deformed
beams. The coordinates of the specified points along the deformed
beam elements are computed using X=Ax*U+Cx*DLoad+B(:,1);
Y=Ay*U+Cy*DLoad+B(:,2) and Z=Az*U+Cz*DLoad+B(:,3). The matrices
Cx,Cy and Cz superimpose the displacements that occur due to the
distributed loads if all nodes are fixed.

[Ax,Ay,Az,B,Cx,Cy,Cz,dAxdx,dAydx,dAzdx,dCxdx,dCydx,dCzdx]
= DISP_BEAM(Nodes,Elements,DOF,DLoads,Sections,Materials,Points,dNodesdx,
dDLoadsdx(,dSectionsdx))
additionally computes the derivatives of the displacements with
respect to the design variables x.

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
DOF Degrees of freedom (nDOF * 1)
DLoads Distributed loads [EltID n1globalX n1globalY n1globalZ ...]
(use an empty array [] when shear deformation is
considered but no DLoads are present)
Sections Section definitions [SecID SecProp1 SecProp2 ...]
Materials Material definitions [MatID MatProp1 MatProp2 ... ]
Points Points in the local coordinate system (1 * nPoints)
dNodesdx Node definitions derivatives (SIZE(Node) * nVar)
dDLoadsdx Distributed loads derivatives (SIZE(DLoad) * nVar)
Ax Matrix to compute the x-coordinates of the deformations
Ay Matrix to compute the y-coordinates of the deformations
Az Matrix to compute the z-coordinates of the deformations
B Matrix which contains the x-, y- and z-coordinates of the
undeformed structure
Cx Matrix to compute the x-coordinates of the deformations
Cy Matrix to compute the y-coordinates of the deformations
Cz Matrix to compute the z-coordinates of the deformations
dAxdx, dAydx, dAzdx, dCxdx, dCydx, dCzdx
Derivatives of the matrices to compute the coordinates of the
interpolation points after deformation

See also DISP_TRUSS, PLOTDISP, NELCS_BEAM, NEDLOADLCS_BEAM.

100 FUNCTIONS — ALPHABETICAL LIST

disp mass
DISP_MASS Matrices to compute the displacements of the deformed mass element

[Ax,Ay,Az,B,Cx,Cy,Cz]
=disp_beam(Nodes,Elements,DOF,EltIDDLoad,Sections,Materials,Points)
[Ax,Ay,Az,B,Cx,Cy,Cz]
=disp_beam(Nodes,Elements,DOF,EltIDDLoad,Sections,Materials)
[Ax,Ay,Az,B]
=disp_beam(Nodes,Elements,DOF,[],Sections,Materials)
[Ax,Ay,Az,B]
=disp_beam(Nodes,Elements,DOF)

returns the matrices to compute the displacements of the deformed mass.

The coordinates of the node of the mass element are
computed using X=Ax*U+B(:,1); Y=Ay*U+B(:,2) and
Z=Az*U+B(:,3). The matrices Cx,Cy and Cz superimpose the
displacements that occur due to the distributed loads if all nodes are fixed.

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
DOF Degrees of freedom (nDOF * 1)
Ax Matrix to compute the x-coordinates of the deformations
Ay Matrix to compute the y-coordinates of the deformations
Az Matrix to compute the z-coordinates of the deformations
B Matrix which contains the x-, y- and z-coordinates of the
undeformed structure
Cx Matrix to compute the x-coordinates of the deformations
Cy Matrix to compute the y-coordinates of the deformations
Cz Matrix to compute the z-coordinates of the deformations

See also DISP_TRUSS, PLOTDISP, DISP_SHELL8.

FUNCTIONS — ALPHABETICAL LIST 101

disp plane10
DISP_PLANE10 Matrices to compute the displacements of the deformed plane.

[Ax,Ay,Az,B] = disp_plane10(Nodes,Elements,DOF,U)
returns the matrices to compute the displacements of the deformed plane.
The coordinates of the nodes of the plane10 element are
computed using X=Ax*U+B(:,1); Y=Ay*U+B(:,2) and
Z=Az*U+B(:,3).

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
DOF Degrees of freedom (nDOF * 1)
Ax Matrix to compute the x-coordinates of the deformations
Ay Matrix to compute the y-coordinates of the deformations
Az Matrix to compute the z-coordinates of the deformations
B Matrix which contains the x-, y- and z-coordinates of the
undeformed structure

See also DISP_TRUSS, PLOTDISP, DISP_SHELL4.

102 FUNCTIONS — ALPHABETICAL LIST

disp plane15
DISP_PLANE15 Matrices to compute the displacements of the deformed plane.

[Ax,Ay,Az,B] = disp_plane15(Nodes,Elements,DOF,U)
returns the matrices to compute the displacements of the deformed plane.
The coordinates of the nodes of the plane15 element are
computed using X=Ax*U+B(:,1); Y=Ay*U+B(:,2) and
Z=Az*U+B(:,3).

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
DOF Degrees of freedom (nDOF * 1)
Ax Matrix to compute the x-coordinates of the deformations
Ay Matrix to compute the y-coordinates of the deformations
Az Matrix to compute the z-coordinates of the deformations
B Matrix which contains the x-, y- and z-coordinates of the
undeformed structure

See also DISP_TRUSS, PLOTDISP, DISP_SHELL4.

FUNCTIONS — ALPHABETICAL LIST 103

disp plane3
DISP_PLANE3 Matrices to compute the displacements of the deformed plane3.

[Ax,Ay,Az,B] = disp_plane3(Nodes,Elements,DOF,U)
returns the matrices to compute the displacements of the deformed plane3 element.
The coordinates of the nodes of the plane3 element are
computed using X=Ax*U+B(:,1); Y=Ay*U+B(:,2) and
Z=Az*U+B(:,3).

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
DOF Degrees of freedom (nDOF * 1)
Ax Matrix to compute the x-coordinates of the deformations
Ay Matrix to compute the y-coordinates of the deformations
Az Matrix to compute the z-coordinates of the deformations
B Matrix which contains the x-, y- and z-coordinates of the
undeformed structure

See also DISP_TRUSS, PLOTDISP, DISP_SHELL8.

104 FUNCTIONS — ALPHABETICAL LIST

disp plane4
DISP_PLANE4 Matrices to compute the displacements of the deformed plane4.

[Ax,Ay,Az,B] = disp_plane4(Nodes,Elements,DOF,U)
returns the matrices to compute the displacements of the deformed plane4.
The coordinates of the nodes of the plane4 element are
computed using X=Ax*U+B(:,1); Y=Ay*U+B(:,2) and
Z=Az*U+B(:,3).

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
DOF Degrees of freedom (nDOF * 1)
Ax Matrix to compute the x-coordinates of the deformations
Ay Matrix to compute the y-coordinates of the deformations
Az Matrix to compute the z-coordinates of the deformations
B Matrix which contains the x-, y- and z-coordinates of the
undeformed structure

See also DISP_TRUSS, PLOTDISP, DISP_SHELL8.

FUNCTIONS — ALPHABETICAL LIST 105

disp plane6
DISP_PLANE6 Matrices to compute the displacements of the deformed plane.

[Ax,Ay,Az,B] = disp_plane6(Nodes,Elements,DOF,U)
returns the matrices to compute the displacements of the deformed plane.
The coordinates of the nodes of the plane6 element are
computed using X=Ax*U+B(:,1); Y=Ay*U+B(:,2) and
Z=Az*U+B(:,3).

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
DOF Degrees of freedom (nDOF * 1)
Ax Matrix to compute the x-coordinates of the deformations
Ay Matrix to compute the y-coordinates of the deformations
Az Matrix to compute the z-coordinates of the deformations
B Matrix which contains the x-, y- and z-coordinates of the
undeformed structure

See also DISP_TRUSS, PLOTDISP, DISP_SHELL4.

106 FUNCTIONS — ALPHABETICAL LIST

disp plane8
DISP_PLANE8 Return matrices to compute the displacements of the deformed elements.

[Ax,Ay,Az,B]=disp_plane8(Nodes,Elements,DOF)
returns the matrices to compute the displacements of the deformed elements.
The coordinates of the specified points along the deformed beams element are
computed using
X=Ax*U+B(:,1)
Y=Ay*U+B(:,2)
Z=Az*U+B(:,3)

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
DOF Degrees of freedom (nDOF * 1)
Points Points in local coordinate system (1 * nPoints)
Ax Matrix to compute the x-coordinates of the deformations
Ay Matrix to compute the y-coordinates of the deformations
Az Matrix to compute the z-coordinates of the deformations
B Matrix which contains the x-, y- and z-coordinates of the
undeformed structure
FUNCTIONS — ALPHABETICAL LIST 107

disp shell2
DISP_SHELL2 Return matrices to compute the displacements of deformed SHELL2 elements.

[Ax,Ay,Az,B,Cx,Cy,Cz]
=disp_shell2(Nodes,Elements,DOF,EltIDDLoad,Sections,Materials,Points)
[Ax,Ay,Az,B,Cx,Cy,Cz]
=disp_shell2(Nodes,Elements,DOF,EltIDDLoad,Sections,Materials)
[Ax,Ay,Az,B]
=disp_shell2(Nodes,Elements,DOF,[],Sections,Materials)
[Ax,Ay,Az,B]
=disp_shell2(Nodes,Elements,DOF)

returns the matrices to compute the displacements of deformed SHELL2 elements.

The coordinates of the specified points along the deformed SHELL2 element are
computed using X=Ax*U+Cx*DLoad+B(:,1); Y=Ay*U+Cy*DLoad+B(:,2) and
Z=Az*U+Cz*DLoad+B(:,3). The matrices Cx,Cy and Cz superimpose the
displacements that occur due to the distributed loads if all nodes are fixed.
In the current implementation, Cx=Cy=Cz=0, i.e. the local effect of the
distributed loads is ignored.

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
DOF Degrees of freedom (nDOF * 1)
EltIDDLoad Elements with distributed loads [EltID]
(use empty array [] when shear deformation is considered
but no DLoads are present)
Sections Section definitions [SecID SecProp1 SecProp2 ...]
Materials Material definitions [MatID MatProp1 MatProp2 ... ]
Points Points in the local coordinate system (1 * nPoints)
Ax Matrix to compute the x-coordinates of the deformations
Ay Matrix to compute the y-coordinates of the deformations
Az Matrix to compute the z-coordinates of the deformations
B Matrix which contains the x-, y- and z-coordinates of the
undeformed structure
Cx Matrix to compute the x-coordinates of the deformations
Cy Matrix to compute the y-coordinates of the deformations
Cz Matrix to compute the z-coordinates of the deformations
108 FUNCTIONS — ALPHABETICAL LIST

disp shell4
DISP_SHELL4 Matrices to compute the displacements of the deformed shell4.

[Ax,Ay,Az,B] = disp_shell4(Nodes,Elements,DOF,U)
returns the matrices to compute the displacements of the deformed shell4.
The coordinates of the nodes of the shell4 element are
computed using X=Ax*U+B(:,1); Y=Ay*U+B(:,2) and
Z=Az*U+B(:,3).

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
DOF Degrees of freedom (nDOF * 1)
Ax Matrix to compute the x-coordinates of the deformations
Ay Matrix to compute the y-coordinates of the deformations
Az Matrix to compute the z-coordinates of the deformations
B Matrix which contains the x-, y- and z-coordinates of the
undeformed structure

See also DISP_TRUSS, PLOTDISP, DISP_SHELL8.

FUNCTIONS — ALPHABETICAL LIST 109

disp shell6
DISP_SHELL6 Matrices to compute the displacements of the deformed shell.

[Ax,Ay,Az,B] = disp_shell6(Nodes,Elements,DOF,U)
returns the matrices to compute the displacements of the deformed shell.
The coordinates of the nodes of the shell6 element are
computed using X=Ax*U+B(:,1); Y=Ay*U+B(:,2) and
Z=Az*U+B(:,3).

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
DOF Degrees of freedom (nDOF * 1)
Ax Matrix to compute the x-coordinates of the deformations
Ay Matrix to compute the y-coordinates of the deformations
Az Matrix to compute the z-coordinates of the deformations
B Matrix which contains the x-, y- and z-coordinates of the
undeformed structure

See also DISP_TRUSS, PLOTDISP, DISP_SHELL4.

110 FUNCTIONS — ALPHABETICAL LIST

disp shell8
DISP_SHELL8 Matrices to compute the displacements of the deformed shell.

[Ax,Ay,Az,B] = disp_shell8(Nodes,Elements,DOF,U)
returns the matrices to compute the displacements of the deformed shell.
The coordinates of the nodes of the shell8 element are
computed using X=Ax*U+B(:,1); Y=Ay*U+B(:,2) and
Z=Az*U+B(:,3).

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
DOF Degrees of freedom (nDOF * 1)
Ax Matrix to compute the x-coordinates of the deformations
Ay Matrix to compute the y-coordinates of the deformations
Az Matrix to compute the z-coordinates of the deformations
B Matrix which contains the x-, y- and z-coordinates of the
undeformed structure

See also DISP_TRUSS, PLOTDISP, DISP_SHELL4.

FUNCTIONS — ALPHABETICAL LIST 111

disp solid10
DISP_SOLID10 Return matrices to compute the displacements of the deformed elements.

[Ax,Ay,Az,B]=disp_solid10(Nodes,Elements,DOF,Points)
[Ax,Ay,Az,B]=disp_solid10(Nodes,Elements,DOF)
returns the matrices to compute the displacements of the deformed elements.
The coordinates of the specified points along the deformed beams element are
computed using X=Ax*U+B(:,1); Y=Ay*U+B(:,2) and Z=Az*U+B(:,3).

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
DOF Degrees of freedom (nDOF * 1)
Points Points in local coordinate system (1 * nPoints)
Ax Matrix to compute the x-coordinates of the deformations
Ay Matrix to compute the y-coordinates of the deformations
Az Matrix to compute the z-coordinates of the deformations
B Matrix which contains the x-, y- and z-coordinates of the
undeformed structure

See also DISP_TRUSS, PLOTDISP.

112 FUNCTIONS — ALPHABETICAL LIST

disp solid15
DISP_SOLID15 Return matrices to compute the displacements of the deformed elements.

[Ax,Ay,Az,B]=disp_solid15(Nodes,Elements,DOF,Points)
[Ax,Ay,Az,B]=disp_solid15(Nodes,Elements,DOF)
returns the matrices to compute the displacements of the deformed elements.
The coordinates of the specified points along the deformed beams element are
computed using X=Ax*U+B(:,1); Y=Ay*U+B(:,2) and Z=Az*U+B(:,3).

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
DOF Degrees of freedom (nDOF * 1)
Points Points in local coordinate system (1 * nPoints)
Ax Matrix to compute the x-coordinates of the deformations
Ay Matrix to compute the y-coordinates of the deformations
Az Matrix to compute the z-coordinates of the deformations
B Matrix which contains the x-, y- and z-coordinates of the
undeformed structure

See also DISP_TRUSS, PLOTDISP.

FUNCTIONS — ALPHABETICAL LIST 113

disp solid20
DISP_SOLID20 Return matrices to compute the displacements of the deformed elements.

[Ax,Ay,Az,B]=disp_solid20(Nodes,Elements,DOF,Points)
[Ax,Ay,Az,B]=disp_solid20(Nodes,Elements,DOF)
returns the matrices to compute the displacements of the deformed elements.
The coordinates of the specified points along the deformed beams element are
computed using X=Ax*U+B(:,1); Y=Ay*U+B(:,2) and Z=Az*U+B(:,3).

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
DOF Degrees of freedom (nDOF * 1)
Points Points in local coordinate system (1 * nPoints)
Ax Matrix to compute the x-coordinates of the deformations
Ay Matrix to compute the y-coordinates of the deformations
Az Matrix to compute the z-coordinates of the deformations
B Matrix which contains the x-, y- and z-coordinates of the
undeformed structure

See also DISP_TRUSS, PLOTDISP.

114 FUNCTIONS — ALPHABETICAL LIST

disp solid8
DISP_SOLID8 Return matrices to compute the displacements of the deformed elements.

[Ax,Ay,Az,B]=disp_solid8(Nodes,Elements,DOF,Points)
[Ax,Ay,Az,B]=disp_solid8(Nodes,Elements,DOF)
returns the matrices to compute the displacements of the deformed elements.
The coordinates of the specified points along the deformed beams element are
computed using X=Ax*U+B(:,1); Y=Ay*U+B(:,2) and Z=Az*U+B(:,3).

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
DOF Degrees of freedom (nDOF * 1)
Points Points in local coordinate system (1 * nPoints)
Ax Matrix to compute the x-coordinates of the deformations
Ay Matrix to compute the y-coordinates of the deformations
Az Matrix to compute the z-coordinates of the deformations
B Matrix which contains the x-, y- and z-coordinates of the
undeformed structure

See also DISP_TRUSS, PLOTDISP.

FUNCTIONS — ALPHABETICAL LIST 115

disp truss
DISP_TRUSS Return matrices to compute the displacements of the deformed trusses.

[Ax,Ay,Az,B]=disp_truss(Nodes,Elements,DOF,[],[],[],Points)
[Ax,Ay,Az,B]=disp_truss(Nodes,Elements,DOF)
returns the matrices to compute the displacements of the deformed
trusses. The coordinates of the specified points along the deformed
truss elements are computed using X=Ax*U+B(:,1); Y=Ay*U+B(:,2)
and Z=Az*U+B(:,3).

[Ax,Ay,Az,B,Cx,Cy,Cz,dAxdx,dAydx,dAzdx,dCxdx,dCydx,dCzdx]
= DISP_TRUSS(Nodes,Elements,DOF,EltIDDLoad,Sections,Materials,Points,dNodesdx,
dDLoadsdx(,dSectionsdx))
additionally computes the derivatives of the displacements with
respect to the design variables x.

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
DOF Degrees of freedom (nDOF * 1)
Points Points in the local coordinate system (1 * nPoints)
dNodesdx Node definitions derivatives (SIZE(Node) * nVar)
dDLoads Distributed loads derivatives (SIZE(DLoad) * nVar)
Ax Matrix to compute the x-coordinates of the deformations
Ay Matrix to compute the y-coordinates of the deformations
Az Matrix to compute the z-coordinates of the deformations
B Matrix which contains the x-, y- and z-coordinates of the
undeformed structure
dAxdx, dAydx, dAzdx, dCxdx, dCydx, dCzdx
Derivatives of the matrices to compute the coordinates of the
interpolation points after deformation

See also DISP_BEAM, PLOTDISP.

116 FUNCTIONS — ALPHABETICAL LIST

dloadgcs2lcs
DLOADGCS2LCS Distributed load transformation from GCS to LCS.

DLoadLCS = DLOADGCS2LCS(T,DLoad)
transforms the distributed load definitions in the global
coordinate system (algebraic convention) to the local coordinate
system (beam convention).

[DLoadLCS,dDLoadLCSdx] = DLOADGCS2LCS(T,DLoad,dTdx,dDLoaddx)
transforms the distributed load definitions in the global
coordinate system (algebraic convention) to the local coordinate
system (beam convention), and additionally computes the derivatives
of the distributed load information with respect to the design
variables x.

T Element transformation matrix (6 * 6)

DLoad Distributed loads in GCS [n1globalX; n1globalY; n1globalZ; ...]
(6/8 * nLC * nDLoads)
dTdx Transformation matrix derivatives (6 * 6 * nVar)
dDLoaddx Distributed loads derivatives (GCS) (SIZE(DLoad) * nVar)
DLoadLCS Distributed loads in LCS [n1localX; n1localY; n1localZ; ...]
(6/8 * nLC * nDLoads)
dDLoadLCSdx Distributed loads derivatives (LCS) (SIZE(DLoadLCS) * nVar)
FUNCTIONS — ALPHABETICAL LIST 117

dof beam
DOF_BEAM Element degrees of freedom for a beam element.

DOF = dof_beam(NodeNum) builds the vector with the

builds the vector with the degrees of freedom for the beam element.

NodeNum Node definitions [NodID1 NodID2] (1 * 2)

DOF Degrees of freedom (12 * 1)

See also GETDOF.

118 FUNCTIONS — ALPHABETICAL LIST

dof mass
DOF_MASS Element degrees of freedom for a mass element.

dof = dof_truss(NodeNum) builds the vector with the

labels of the degrees of freedom for which stiffness is present in the
mass element.

NodeNum Node numbers [NodID1] (1)

dof Degrees of freedom (6 * 1)

See also GETDOF.

FUNCTIONS — ALPHABETICAL LIST 119

dof plane10
DOF_PLANE10 Element degrees of freedom for a plane10 element.

dof = dof_plane10(NodeNum) builds the vector with the

labels of the degrees of freedom for which stiffness is present in the
plane10 element.

NodeNum Node definitions [NodID1 NodID2 ... NodIDn] (1 * 10)

dof Degrees of freedom (20 * 1)

See also GETDOF.

120 FUNCTIONS — ALPHABETICAL LIST

dof plane15
DOF_PLANE15 Element degrees of freedom for a plane15 element.

dof = dof_plane15(NodeNum) builds the vector with the

labels of the degrees of freedom for which stiffness is present in the
plane15 element.

NodeNum Node definitions [NodID1 NodID2 ... NodIDn] (1 * 15)

dof Degrees of freedom (30 * 1)

See also GETDOF.

FUNCTIONS — ALPHABETICAL LIST 121

dof plane3
DOF_PLANE3 Element degrees of freedom for a plane3 element.

dof = dof_plane3(NodeNum) builds the vector with the

labels of the degrees of freedom for which stiffness is present in the
plane3 element.

NodeNum Node definitions [NodID1 NodID2 NodID3] (1 * 3)

dof Degrees of freedom (6 * 1)

See also GETDOF.

122 FUNCTIONS — ALPHABETICAL LIST

dof plane4
DOF_PLANE4 Element degrees of freedom for a plane4 element.

dof = dof_plane4(NodeNum) builds the vector with the

labels of the degrees of freedom for which stiffness is present in the
plane4 element.

NodeNum Node definitions [NodID1 NodID2 ... NodIDn] (1 * 4)

dof Degrees of freedom (8 * 1)

See also GETDOF.

FUNCTIONS — ALPHABETICAL LIST 123

dof plane6
DOF_PLANE6 Element degrees of freedom for a plane6 element.

dof = dof_plane6(NodeNum) builds the vector with the

labels of the degrees of freedom for which stiffness is present in the
plane6 element.

NodeNum Node definitions [NodID1 NodID2 ... NodIDn] (1 * 6)

dof Degrees of freedom (12 * 1)

See also GETDOF.

124 FUNCTIONS — ALPHABETICAL LIST

dof plane8
of_plane8 is a function.
dof = dof_plane8(Nodenumbers)
FUNCTIONS — ALPHABETICAL LIST 125

dof shell2
DOF_SHELL2 Element degrees of freedom for a SHELL2 element.

DOF = dof_shell2(NodeNum) returns a vector with the degrees of freedom for

a SHELL2 element.

NodeNum Node definitions [NodID1 NodID2] (1 * 2)

DOF Degrees of freedom (12 * 1)
126 FUNCTIONS — ALPHABETICAL LIST

dof shell4
DOF_SHELL4 Element degrees of freedom for a shell4 element.

dof = dof_shell4(NodeNum) builds the vector with the

labels of the degrees of freedom for which stiffness is present in the
shell4 element.

NodeNum Node definitions [NodID1 NodID2 ... NodIDn] (1 * 4)

dof Degrees of freedom (24 * 1)

See also GETDOF.

FUNCTIONS — ALPHABETICAL LIST 127

dof shell6
DOF_SHELL6 Element degrees of freedom for a shell6 element.

dof = dof_shell6(NodeNum) builds the vector with the

labels of the degrees of freedom for which stiffness is present in the
shell6 element.

NodeNum Node definitions [NodID1 NodID2 ... NodIDn] (1 * 6)

dof Degrees of freedom (36 * 1)

See also GETDOF.

128 FUNCTIONS — ALPHABETICAL LIST

dof shell8
DOF_SHELL8 Element degrees of freedom for a shell8 element.

dof = dof_shell8(NodeNum) builds the vector with the

labels of the degrees of freedom for which stiffness is present in the
shell8 element.

NodeNum Node definitions [NodID1 NodID2 ... NodIDn] (1 * 8)

dof Degrees of freedom (48 * 1)

See also GETDOF.

FUNCTIONS — ALPHABETICAL LIST 129

dof solid10
DOF_SOLID10 Element degrees of freedom for a solid10 element.

dof = dof_solid10(NodeNum) builds the vector with the

labels of the degrees of freedom for which stiffness is present in the
solid10 element.

NodeNum Node definitions [NodID1 NodID2 ... NodIDn] (1 * 4)

dof Degrees of freedom (30 * 1)

See also GETDOF.

130 FUNCTIONS — ALPHABETICAL LIST

dof solid15
DOF_SOLID15 Element degrees of freedom for a solid10 element.

dof = dof_solid15(NodeNum) builds the vector with the

labels of the degrees of freedom for which stiffness is present in the
solid15 element.

NodeNum Node definitions [NodID1 NodID2 ... NodIDn] (1 * 4)

dof Degrees of freedom (45 * 1)

See also GETDOF.

FUNCTIONS — ALPHABETICAL LIST 131

dof solid20
DOF_SOLID20 Element degrees of freedom for a solid20 element.

dof = dof_solid20(NodeNum) builds the vector with the

labels of the degrees of freedom for which stiffness is present in the
solid20 element.

NodeNum Node definitions [NodID1 NodID2 ... NodIDn] (1 * 4)

dof Degrees of freedom (60 * 1)

See also GETDOF.

132 FUNCTIONS — ALPHABETICAL LIST

dof solid4
DOF_SOLID4 Element degrees of freedom for a solid4 element.

dof = dof_solid4(NodeNum) builds the vector with the

labels of the degrees of freedom for which stiffness is present in the
solid4 element.

NodeNum Node definitions [NodID1 NodID2 NodID3 NodID4] (1 * 4).

dof Degrees of freedom (12 * 1).

See also GETDOF.

FUNCTIONS — ALPHABETICAL LIST 133

dof solid8
DOF_SOLID8 Element degrees of freedom for a solid8 element.

dof = dof_solid8(NodeNum) builds the vector with the

labels of the degrees of freedom for which stiffness is present in the
solid8 element.

NodeNum Node definitions [NodID1 NodID2 ... NodIDn] (1 * 4)

dof Degrees of freedom (24 * 1)

See also GETDOF.

134 FUNCTIONS — ALPHABETICAL LIST

dof truss
DOF_TRUSS Element degrees of freedom for a truss element.

dof = dof_truss(NodeNum) builds the vector with the degrees of freedom

for the truss element.

NodeNum Node numbers [NodID1 NodID2] (1 * 2)

dof Degrees of freedom (6 * 1)

See also GETDOF.

FUNCTIONS — ALPHABETICAL LIST 135

eigfem
EIGFEM Compute the eigenmodes and eigenfrequencies of the finite element model.

[phi,omega]=eigfem(K,M,nMode)
[phi,omega]=eigfem(K,M)
computes the eigenmodes and eigenfrequencies of the finite element model.

K Stiffness matrix (nDOF * nDOF)

M Mass matrix (nDOF * nDOF)
nMode Number of eigenmodes and eigenfrequencies (default: all)
phi Eigenmodes (in columns) (nDOF * nMode)
omega Eigenfrequencies [rad/s] (nMode * 1)
136 FUNCTIONS — ALPHABETICAL LIST

elemdisp
ELEMDISP Select the element displacements from the global displacement vector.

UeGCS = elemdisp(Type,NodeNum,DOF,U) selects the element

displacements from the global displacement vector.

Type Element type e.g. ’beam’,’truss’, ...

NodeNum Node numbers (1 * nNodes)
DOF Degrees of freedom (nDOF * 1)
U Displacements (nDOF * nLC)
UeGCS Element displacements

See also ELEMFORCES, DOF_BEAM, DOF_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 137

elemforces
ELEMFORCES Compute the element forces.

[ForcesLCS,ForcesGCS] = ELEMFORCES(Nodes,Elements,Types,Sections,Materials,DOF,U,DLoads,TLoads)
[ForcesLCS,ForcesGCS] = ELEMFORCES(Nodes,Elements,Types,Sections,Materials,DOF,U)
computes the element forces in the local (beam convention) and the
global (algebraic convention) coordinate system.

[ForcesLCS,ForcesGCS,dForcesLCSdx,dForcesGCSdx]
= ELEMFORCES(Nodes,Elements,Types,Sections,Materials,DOF,U,DLoads,TLoads,
dNodesdx,dSectionsdx,dUdx,dDLoadsdx)
additionally computes the derivatives of the element forces with
respect to the design variables x.

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ...}
Sections Section definitions [SecID SecProp1 SecProp2 ...]
Materials Material definitions [MatID MatProp1 MatProp2 ...]
DOF Degrees of freedom (nDOF * 1)
U Displacements (nDOF * nLC)
DLoads Distributed loads [EltID n1globalX n1globalY n1globalZ ...]
TLoads Temperature loads [EltID Tyt Tyb Tzt Tzb]
dNodesdx Node definitions derivatives (SIZE(Nodes) * nVar)
dSectionsdx Section definitions derivatives (SIZE(Sections) * nVar)
dUdx Displacements derivatives (nDOF * nLC * nVar)
dDLoadsdx Distributed loads derivative (SIZE(DLoads) * nVar)
ForcesLCS Element forces in LCS (beam convention) [N Vy Vz T My Mz] (nElem * 12 * nLC)
ForcesGCS Element forces in GCS (algebraic convention) (nElem * 12 * nLC)
dForcesLCSdx Element forces derivatives in LCS (nElem * 12 * nLC * nVar)
dForcesGCSdx Element forces derivatives in GCS (nElem * 12 * nLC * nVar)

See also FORCES_TRUSS, FORCES_BEAM.

138 FUNCTIONS — ALPHABETICAL LIST

elemloads
ELEMLOADS Equivalent nodal forces.

F = ELEMLOADS(DLoads,Nodes,Elements,Types,DOF)
computes the equivalent nodal forces of a distributed load
(in the global coordinate system).

[F,dFdx] = ELEMLOADS(DLoads,Nodes,Elements,Types,DOF,dDLoadsdx,dNodesdx)
additionally computes the derivatives of the equivalent nodal forces
with respect to the design variables x.

DLoads Distributed loads [EltID n1globalX n1globalY n1globalZ ...]

Nodes Node definitions [NodID x y z]
Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
DOF Degrees of freedom (nDOF * 1)
dDLoadsdx Distributed loads derivatives (SIZE(DLoads) * nVar)
dNodesdx Node definitions derivatives (SIZE(Nodes) * nVar)
F Load vector (nDOF * nLC)
dFdx Load vector derivatives (nDOF * nLC * nVar)

See also LOADS_TRUSS, LOADS_BEAM, NODALVALUES.

FUNCTIONS — ALPHABETICAL LIST 139

elempressure
ELEMPRESSURE Equivalent nodal forces for a pressure load on a shell element.

F = elempressure(Pressures,Nodes,Elements,Types,DOF)
computes the equivalent nodal forces of a distributed pressure
(in the local coordinate system xyz, with z perpendicular to the surface).

Pressures Pressure on surface or edge [EltID n1localZ n2localZ n3localZ ...]

Nodes Node definitions [NodID x y z]
Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
DOF Degrees of freedom (nDOF * 1)
F Load vector (nDOF * 1)

See also PRESSURE_SHELL8, PRESSURE_SHELL4, NODALVALUES.

140 FUNCTIONS — ALPHABETICAL LIST

elemsize
ELEMSIZE Compute element length/area/volume.

S = ELEMSIZE(Nodes,Elements,Types)
computes the size of all elements, depending on element type. For a 1D
line element it computes length, for a 2D plate element it computes
area, and for a 3D solid element it computes volume.

[S,dSdx] = ELEMSIZE(Nodes,Elements,Types,dNodesdx)
additionaly computes the derivatives of the size with respect to the
design variables x.

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
dNodesdx Node definitions derivatives (SIZE(Nodes) * nVar)
S Element sizes
dSdx Element sizes derivatives

See also SIZE_BEAM, SIZE_TRUSS, ELEMVOLUMES.

FUNCTIONS — ALPHABETICAL LIST 141

elemstress
ELEMSTRESS Compute the element stresses.

[SeGCS,SeLCS,vLCS] = elemstress(Nodes,Elements,Types,Sections,Materials,DOF,U)
[SeGCS,SeLCS] = elemstress(Nodes,Elements,Types,Sections,Materials,DOF,U)
SeGCS = elemstress(Nodes,Elements,Types,Sections,Materials,DOF,U)
computes the element stresses in the global and the local coordinate system.

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
Sections Section definitions [SecID SecProp1 SecProp2 ...]
Materials Material definitions [MatID MatProp1 MatProp2 ... ]
DOF Degrees of freedom (nDOF * 1)
U Displacements (nDOF * 1)
elemstress(...,ParamName,ParamValue) sets the value of the specified
parameters. The following parameters can be specified:
’GCS’ Sets the gcs in which SeGCS is computed.
Default: ’cart’. Type of values:
’cart’: cartesian coordinate system
’cyl’ : cylindrical coordinate system
’sph’ : spherical coordinate system

SeGCS Element stresses in GCS in corner nodes IJKL and

at top/mid/bot of shell (nElem * 72)
72 = 6 stresscomp. * 4 nodes * 3 locations
[sxx syy szz sxy syz sxz]
SeLCS Element stresses in LCS in corner nodes IJKL and
at top/mid/bot of shell (nElem * 72)
[sxx syy szz sxy syz sxz]
vLCS Unit vectors of LCS (nElem * 9)

See also SE_SHELL8, SE_SHELL4.

142 FUNCTIONS — ALPHABETICAL LIST

elemtloads
ELEMTLOADS Equivalent nodal forces for temperature loading.

F=elemtloads(TLoads,Nodes,Elements,Types,Sections,Materials,DOF)
computes the equivalent nodal forces of a temperature gradient
(in the global coordinate system).

TLoads Temperature gradient [EltID Tyt Tyb Tzt Tzb]

Tkt and Tkb correspond to the temperatures at the top and
the bottom of the profile when the k-axis (LCS) points up (k=y,z)
Nodes Node definitions [NodID x y z]
Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Type definitions {TypID EltName Option1 ... }
Sections Section definitions [SecID A ky kz Ixx Iyy Izz yt yb zt zb]
Materials Material definitions [MatID E nu rho alpha]
DOF Degrees of freedom (nDOF * 1)
F Load vector (nDOF * 1)

See also TLOADS_TRUSS, TLOADS_BEAM.

FUNCTIONS — ALPHABETICAL LIST 143

elemvolumes
ELEMVOLUMES Compute element volumes.

V = ELEMVOLUMES(Nodes,Elements,Types,Sections)
computes the volume for all elements.

[V,dVdx] = ELEMVOLUMES(Nodes,Elements,Types,Sections,dNodesdx,dSectionsdx)
computes the volume for all elements, as well as the derivatives of the
volume with respect to the design variables x.

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
Sections Section definitions [SecID SecProp1 SecProp2 ...]
dNodesdx Node definitions derivatives (SIZE(Nodes) * nVar)
dSectionsdx Section dervinitions derivatives (SIZE(Sections) * nVar)
V Element volumes (nElem * 1)
dVdx Element volumes derivatives (nElem * nVar)

See also VOLUME_BEAM, VOLUME_TRUSS, ELEMSIZES.

144 FUNCTIONS — ALPHABETICAL LIST

fdiagrgcs beam
FDIAGRGCS_BEAM Return matrices to plot the forces in a beam element.

[ElemGCS,FdiagrGCS,ElemExtGCS,ExtremaGCS,Extrema]
= fdiagrgcs_beam(ftype,Forces,Node,[],[],DLoad,Points)
[ElemGCS,FdiagrGCS,ElemExtGCS,ExtremaGCS,Extrema]
= fdiagrgcs_beam(ftype,Forces,Node,[],[],DLoad)
returns the coordinates of the points along the beam in the global
coordinate system and the coordinates of the forces with respect to the beam
in the global coordinate system. These can be added in order to plot the
forces: ElemGCS+FdiagrGCS. The coordinates of the points with extreme values
and the coordinates of the extreme values with respect to the beam are given
as well and can be similarly added: ElemExtGCS+ExtremaGCS. Extrema is the
list with the correspondig extreme values.

ftype ’norm’ Normal force (in the local x-direction)

’sheary’ Shear force in the local y-direction
’shearz’ Shear force in the local z-direction
’momx’ Torsional moment (around the local x-direction)
’momy’ Bending moment around the local y-direction
’momz’ Bending moment around the local z-direction
Forces Element forces in LCS (beam convention) [N; Vy; Vz; T; My; Mz]
(12 * 1)
Node Node definitions [x y z] (3 * 3)
DLoad Distributed loads [n1globalX; n1globalY; n1globalZ; ...]
(6 * 1)
Points Points in the local coordinate system (1 * nPoints)
ElemGCS Coordinates of the points along the beam in GCS (nPoints * 3)
FdiagrGCS Coordinates of the force with respect to the beam in GCS
(nValues * 3)
ElemExtGCS Coordinates of the points with extreme values in GCS (nValues * 3)
ExtremaGCS Coordinates of the extreme values with respect to the beam in GCS
(nValues * 3)
Extrema Extreme values (nValues * 1)

See also PLOTFORC, FDIAGRLCS_BEAM, FDIAGRGCS_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 145

fdiagrgcs shell2
FDIAGRGCS_SHELL2 Return matrices to plot the forces in a SHELL2 element.

[ElemGCS,FdiagrGCS,ElemExtGCS,ExtremaGCS,Extrema]
= fdiagrgcs_shell2(ftype,Forces,Node,Section,Material,DLoad,Points)
[ElemGCS,FdiagrGCS,ElemExtGCS,ExtremaGCS,Extrema]
= fdiagrgcs_shell2(ftype,Forces,Node,Section,Material,DLoad)
returns the coordinates of the points along the SHELL2 in the global
coordinate system and the coordinates of the forces with respect to the element
in the global coordinate system. These can be added in order to plot the
forces: ElemGCS+FdiagrGCS. The coordinates of the points with extreme values
and the coordinates of the extreme values with respect to the element are given
as well and can be similarly added: ElemExtGCS+ExtremaGCS. Extrema is the
list with the correspondig extreme values.

ftype ’Nphi’ Normal force (per unit length) in meridional direction

’Qphi’ Transverse force (per unit length) in meridional direction
’Mphi’ Bending moment (per unit length) in meridional direction
’Ntheta’ Normal force (per unit length) in circumferential direction
’Mtheta’ Bending moment (per unit length) in circumferential direction
Forces Element forces in LCS (beam convention) [N; Vy; 0; 0; 0; Mz] (12 * 1)
Node Node definitions [x y z] (3 * 3)
DLoad Distributed loads [n1globalX; n1globalY; n1globalZ; ...] (6 * 1)
Points Points in the local coordinate system (1 * nPoints)
ElemGCS Coordinates of the points along the element in GCS (nPoints * 3)
FdiagrGCS Coordinates of the force with respect to the element in GCS (nValues * 3)
ElemExtGCS Coordinates of the points with extreme values in GCS (nValues * 3)
ExtremaGCS Coordinates of the extreme values with respect to the element in GCS
(nValues * 3)
Extrema Extreme values (nValues * 1)
146 FUNCTIONS — ALPHABETICAL LIST

fdiagrgcs truss
FDIAGRGCS_TRUSS Return matrices to plot the forces in a truss element.

[ElemGCS,FdiagrGCS,ElemExtGCS,ExtremaGCS,Extrema]
= fdiagrgcs_truss(ftype,Forces,Node,[],[],[],Points)
[ElemGCS,FdiagrGCS,ElemExtGCS,ExtremaGCS,Extrema]
= fdiagrgcs_truss(ftype,Forces,Node)
returns the coordinates of the points along the truss in the global
coordinate system and the coordinates of the forces with respect to the truss
in the global coordinate system. These can be added in order to plot the
forces: ElemGCS+FdiagrGCS. The coordinates of the points with extreme values
and the coordinates of the extreme values with respect to the truss are given
as well and can be similarly added: ElemExtGCS+ExtremaGCS. Extrema is the
list with the correspondig extreme values.

ftype ’norm’ Normal force (in the local x-direction)

Forces Element forces in LCS [N; 0; 0; 0; 0; 0](12 * 1)
Node Node definitions [x y z] (3 * 3)
Points Points in the local coordinate system (1 * nPoints)
ElemGCS Coordinates of the points along the truss in GCS (nPoints * 3)
FdiagrGCS Coordinates of the force with respect to the truss in GCS
(nValues * 3)
ElemExtGCS Coordinates of the points with extreme values in GCS (nValues * 3)
ExtremaGCS Coordinates of the extreme values with respect to the truss in GCS
(nValues * 3)
Extrema Extreme values (nValues * 1)

See also PLOTFORC, FDIAGRGCS_BEAM.

FUNCTIONS — ALPHABETICAL LIST 147

fdiagrlcs
FDIAGRLCS Return force diagrams in LCS.

FdiagrLCS = FDIAGRLCS(ftype,Nodes,Elements,Types,Forces,DLoads,Points)
FdiagrLCS = FDIAGRLCS(ftype,Nodes,Elements,Types,Forces,DLoads)
FdiagrLCS = FDIAGRLCS(ftype,Nodes,Elements,Types,Forces)
computes element force values in all interpolation points (in beam
convention) for beam and truss elements.

[FdiagrLCS,dFdiagrLCSdx]
= FDIAGRLCS(ftype,Nodes,Elements,Types,Forces,DLoads,...
Points,dNodesdx,dForcesdx,dDLoadsdx)
additionally computes the derivatives of the force values with
respect to the design variables x.

ftype ’norm’ Normal force (in the local x-direction)

’sheary’ Shear force in the local y-direction
’shearz’ Shear force in the local z-direction
’momx’ Torsional moment (around the local x-direction)
’momy’ Bending moment around the local y-direction
’momz’ Bending moment around the local z-direction
Nodes Node definitions [NodID x y z]
Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
Forces Element forces in LCS (beam convention) [N Vy Vz T My Mz]
(nElem * 12)
DLoads Distributed loads [EltID n1globalX n1globalY n1globalZ ...]
Points Points in the local coordinate system (1 * nPoints)
dNodesdx Node definitions derivatives (SIZE(Nodes) * nVar)
dForcesdx Element forces in LCS derivatives (SIZE(Forces) * nVar)
dDLoadsdx Distributed loads derivatives (SIZE(DLoads) * nVar)
FdiagrLCS Element force values at the points (nElem * nPoints * nLC)
dFdiagrLCSdx Element force values derivatives (nElem * nPoints * nLC * nVar)

See also PLOTFORC, FDIAGRGCS_BEAM, FDIAGRGCS_TRUSS.

148 FUNCTIONS — ALPHABETICAL LIST

fdiagrlcs beam
FDIAGRLCS_BEAM Force diagram for a beam element in LCS.

[FdiagrLCS,loc,Extrema] = FDIAGRLCS_BEAM(ftype,Forces,DLoadLCS,L,Points)
computes the elements forces at the specified points. The extreme
values for an element with a single DLoad are analytically determined.
The extreme values for an element with multiple DLoads are calculated
in the interpolation points only.

[FdiagrLCS,loc,Extrema,dFdiagrLCSdx]
= FDIAGRLCS_BEAM(ftype,Forces,DLoadLCS,L,Points,dForcesdx,dDLoadLCSdx,dLdx)
additionally computes the derivatives of the element force values with
respect to the design variables x.

ftype ’norm’ Normal force (in the local x-direction)

’sheary’ Shear force in the local y-direction
’shearz’ Shear force in the local z-direction
’momx’ Torsional moment (around the local x-direction)
’momy’ Bending moment around the local y-direction
’momz’ Bending moment around the local z-direction
Forces Element forces in LCS (beam convention) [N; Vy; Vz; T; My; Mz](12 * nLC)
DLoadLCS Distributed loads in LCS [n1localX; n1localY; n1localZ; ...] (6 * nLC)
L Beam length
Points Points in the local coordinate system (1 * nPoints)
dForcesdx Element forces in LCS derivatives (SIZE(Forces) * nVar)
dDLoadLCSdx Distributed loads derivatives (SIZE(DLoadLCS) * nVar)
dLdx Beam length derivatives (1 * nVar)
FdiagrLCS Element forces at the points (1 * nPoints * nLC)
loc Locations of the extreme values (nValues * nLC)
Extrema Extreme values (nValues * nLC)
loc and Extrema are only calculated when nLC = 1 (for plotting).
If this is not the case their calculation is omitted for effiency.
dFdiagrLCSdx Element force value derivatives (1 * nPoints * nLC * nVar)

See also FDIAGRGCS_BEAM.

FUNCTIONS — ALPHABETICAL LIST 149

fdiagrlcs shell2
FDIAGRLCS_SHELL2 Force diagram for a SHELL2 element in LCS.

[FdiagrLCS,loc,Extrema] = fdiagrlcs_shell2(ftype,Forces,DLoadLCS,L,Points)
computes the elements forces at the specified points. The extreme values are
obtained by enumeration.

ftype ’Nphi’ Normal force (per unit length) in meridional direction

’Qphi’ Transverse force (per unit length) in meridional direction
’Mphi’ Bending moment (per unit length) in meridional direction
’Ntheta’ Normal force (per unit length) in circumferential direction
’Mtheta’ Bending moment (per unit length) in circumferential direction
Forces Element forces in LCS (beam convention) [N; Vy; 0; 0; 0; Mz] (12 * 1)
DLoadLCS Distributed loads in LCS [n1localX; n1localY; n1localZ; ...]
(6 * 1) or (12 * 1)
Points Points in the local coordinate system (1 * nPoints)
FdiagrLCS Element forces at the points (1 * nPoints)
loc Locations of the extreme values (nValues * 1)
Extrema Extreme values (nValues * 1)
150 FUNCTIONS — ALPHABETICAL LIST

fdiagrlcs truss
FDIAGRLCS_TRUSS Force diagram for a truss element in LCS.

[FdiagrLCS,loc,Extrema] = FDIAGRLCS_TRUSS(ftype,Forces,DLoadLCS,L,Points)
computes the element forces at the specified points.

[FdiagrLCS,loc,Extrema,dFdiagrLCSdx]
= FDIAGRLCS_TRUSS(ftype,Forces,DLoadLCS,L,Points,dForcesdx,dDLoadLCSdx,dLdx)
additionally computes the derivatives of the element force values with
respect to the design variables x.

ftype ’norm’ Normal force (in the local x-direction)

Forces Element forces in LCS [N; 0; 0; 0; 0; 0] (12 * 1)
Node Node definitions [x y z] (3 * 3)
Points Points in the local coordinate system (1 * nPoints)
dForcesdx Element forces in LCS derivatives (SIZE(Forces) * nVar)
FdiagrLCS Element forces at the points (1 * nPoints * nLC)
loc Locations of the extreme values (nValues * nLC)
Extrema Extreme values (nValues * nLC)
dFdiagrLCSdx Element force value derivatives (1 * nPoints * nLC * nVar)

See also FDIAGRGCS_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 151

forceslcs beam
FORCESLCS_BEAM Compute the element forces for a beam element in the LCS.

Forces = FORCESLCS_BEAM(KeLCS,UeLCS,DLoadLCS,L,TLoadLCS,A,E,alpha,Iyy,Izz,hy,hz)
Forces = FORCESLCS_BEAM(KeLCS,UeLCS,DLoadLCS,L)
Forces = FORCESLCS_BEAM(KeLCS,UeLCS)
computes the element forces for the beam element in the local
coordinate system (algebraic convention).

[Forces,dForcesdx] = FORCESLCS_BEAM(KeLCS,UeLCS,DLoadLCS,L,[],[],[],...
[],[],[],[],[],dKeLCSdx,dUeLCSdx,dDLoadLCSdx,dLdx)
[Forces,dForcesdx] = FORCESLCS_BEAM(KeLCS,UeLCS,[],[],[],[],[],[],[],...
[],[],[],dKeLCSdx,dUeLCSdx,dDLoadLCSdx,dLdx)
additionally computes the derivatives of the element forces with
respect to the design variables x.

KeLCS Element stiffness matrix (12 * 12)

UeLCS Displacements (12 * nLC)
DLoadLCS Distributed loads [n1localX; n1localY; n1localZ; ...]
L Beam length
DLoadLCS Distributed loads [n1localX; n1localY; n1localZ; ...]
(6 * 1)
TLoadLCS Temperature load [dTm; dTy; dTz] (3 * 1)
A Cross-sectional area
E Young’s modulus
alpha Linear thermal expansion coefficient
Iyy Area moment of inertia for bending around local y-axis
Izz Area moment of inertia for bending around local z-axis
hy Profile height (in local y-direction)
hz Profile height (in local z-direction)
dKeLCSdx Element stiffness matrix derivatives (CELL(nVar,1))
dUeLCSdx Displacements derivatives (SIZE(UeLCS) * nVar)
dDLoadLCSdx Distributed loads derivatives (SIZE(DLoadLCS) * nVar)
dLdx Beam length derivatives (1 * nVar)
Forces Element forces [N; Vy; Vz; T; My; Mz] (12 * nLC)
dForcesdx Element forces derivatives (12 * nLC * nVar)

See also FORCES_BEAM, FORCESLCS_TRUSS, ELEMFORCES

152 FUNCTIONS — ALPHABETICAL LIST

forceslcs truss
FORCESLCS_TRUSS Compute the element forces for a truss element in the LCS.

Forces = FORCESLCS_TRUSS(KeLCS,UeLCS,dTm,A,E,alpha)
Forces = FORCESLCS_TRUSS(KeLCS,UeLCS)
computes the element forces for the truss element in the local coordinate
system (algebraic convention).

[Forces,dForcesdx] = FORCESLCS_TRUSS(KeLCS,UeLCS,[],[],[],[],dKeLCSdx,dUeLCSdx)
additionally computes the derivatives of the element forces with
respect to the design variables x.

KeLCS Element stiffness matrix (6 * 6)

UeLCS Displacements (6 * nLC)
dKeLCSdx Element stiffness matrix derivatives (CELL(nVar,1))
dUeLCSdx Displacements derivatives (SIZE(UeLCS) * nVar)
Forces Element forces [N; 0; 0](6 * nLC)
dForcesdx Element forces derivatives (6 * nLC * nVar)

See also FORCES_TRUSS, FORCESLCS_BEAM, ELEMFORCES

FUNCTIONS — ALPHABETICAL LIST 153

forces beam
FORCES_BEAM Compute the element forces for a beam element.

[ForcesLCS,ForcesGCS] = FORCES_BEAM(Node,Section,Material,UeGCS,DLoad,TLoad,Options)
[ForcesLCS,ForcesGCS] = FORCES_BEAM(Node,Section,Material,UeGCS,DLoad)
[ForcesLCS,ForcesGCS] = FORCES_BEAM(Node,Section,Material,UeGCS)
computes the element forces for the beam element in the local and
the global coordinate system (algebraic convention).

[ForcesLCS,ForcesGCS,dForcesLCSdx,dForcesGCSdx]
= FORCES_BEAM(Node,Section,Material,UeGCS,DLoad,TLoad,Options,dNodedx,...
dSectiondx,dUeGCSdx,dDLoaddx)
= FORCES_BEAM(Node,Section,Material,UeGCS,[],[],Options,dNodedx,...
dSectiondx,dUeGCSdx)
additionally computes the derivatives of the element forces with
respect to the design variables x.

Node Node definitions [x y z] (3 * 3)

Section Section definition [A ky kz Ixx Iyy Izz]
Material Material definition [E nu]
UeGCS Displacements (12 * nLC)
DLoad Distributed loads [n1globalX; n1globalY; n1globalZ; ...]
(6 * 1)
TLoad TLoad [dTm; dTy; dTz] (3 * 1)
Options Element options {Option1 Option2 ...}
dNodedx Node definitions derivatives (SIZE(Node) * nVar)
dSectiondx Section definitions derivatives (SIZE(Section) * nVar)
dUeGCSdx Displacements derivatives (SIZE(UeGCS) * nVar)
dDLoaddx Distributed loads derivatives (SIZE(DLoad) * nVar)
ForcesLCS Element forces in the LCS (12 * nLC)
ForcesGCS Element forces in the GCS (12 * nLC)
dForcesLCSdx Element forces derivatives in LCS (12 * nLC * nVar)
dForcesGCSdx Element forces derivatives in GCS (12 * nLC * nVar)

See also FORCESLCS_BEAM, ELEMFORCES.

154 FUNCTIONS — ALPHABETICAL LIST

forces shell2
FORCES_BEAM Compute the element forces for a SHELL2 element.

[ForcesLCS,ForcesGCS]=forces_shell2(Node,Section,Material,UeGCS,DLoad,TLoad,Options)
[ForcesLCS,ForcesGCS]=forces_shell2(Node,Section,Material,UeGCS,DLoad)
[ForcesLCS,ForcesGCS]=forces_shell2(Node,Section,Material,UeGCS)
computes the element forces for the SHELL2 element in the local and the
global coordinate system (algebraic convention).

Node Node definitions [x y z] (3 * 3)

Section Section definition [h]
Material Material definition [E nu]
UeGCS Displacements (12 * 1)
DLoad Distributed loads [n1globalX; n1globalY; n1globalZ; ...]
(6 * 1)
TLoad TLoad [dTm; dTy; dTz] (3 * 1)
Options Element options {Option1 Option2 ...}
ForcesLCS Element forces in the LCS (12 * 1)
ForcesGCS Element forces in the GCS (12 * 1)
FUNCTIONS — ALPHABETICAL LIST 155

forces truss
FORCES_TRUSS Compute the element forces for a truss element.

[ForcesLCS,ForcesGCS] = FORCES_TRUSS(Node,Section,Material,UeGCS,[],TLoad)
[ForcesLCS,ForcesGCS] = FORCES_TRUSS(Node,Section,Material,UeGCS)
computes the element forces for the truss element in the local and the
global coordinate system (algebraic convention).

[ForcesLCS,ForcesGCS,dForcesLCSdx,dForcesGCSdx]
= FORCES_TRUSS(Node,Section,Material,UeGCS,[],TLoad,[],dNodedx,...
dSectiondx,dUeGCSdx)
additionally computes the derivatives of the element forces with
respect to the design variables x.

Node Node definitions [x y z] (2 * 3)

Section Section definition [A]
Material Material definition [E]
UeGCS Displacements (6 * nLC)
TLoad Temperature load [dTm]
Options Element options {Option1 Option2 ...}
dNodedx Node definitions derivatives (SIZE(Node) * nVar)
dSectiondx Section definitions derivatives (SIZE(Section) * nVar)
dUeGCSdx Displacements derivatives (SIZE(UeGCS) * nVar)
dDLoaddx Distributed loads derivatives (SIZE(DLoad) * nVar)
ForcesLCS Element forces in the LCS (12 * nLC)
ForcesGCS Element forces in the GCS (12 * nLC)
dForcesLCSdx Element forces derivatives in LCS (12 * nLC * nVar)
dForcesGCSdx Element forces derivatives in GCS (12 * nLC * nVar)

See also FORCESLCS_TRUSS, ELEMFORCES.

156 FUNCTIONS — ALPHABETICAL LIST

gaussq
GAUSSQ Gauss points for 2D numerical integration.

[x,H] = gaussq(n) returns the coordinates and weights for a 2D

gauss-legendre quadrature.

n number of points in one direction = 2 or 3

x coordinates of gauss-points (n^2 * 2)
H weights used in summation (1 * n^2)

See also KE_SHELL8, KELCS_SHELL4

FUNCTIONS — ALPHABETICAL LIST 157

gaussqtet
GAUSSQTET Gauss points for 3D numerical integration on a tetrahedron.

[x,H] = gaussqtet(n) returns the coordinates and weights for a 3D

gauss-legendre quadrature on a tetrahedron. The coordinates are
returned in natural coordinates (i.e. no volume coordinates)

n number of integration points

x coordinates of the integration points (n * 3)
H weights used in summation (1 * n)

See also GAUSSQ, GAUSSQTRI

158 FUNCTIONS — ALPHABETICAL LIST

gaussqtri
GAUSSQTRI Gauss points for 2D numerical integration on a triangle.

[x,H] = gaussqtri(n) returns the coordinates and weights for a 2D

triangular gauss-legendre quadrature.

n number of integration points

x coordinates of the integration points (n * 2)
H weights used in summation (1 * n)

See also GAUSSQ

FUNCTIONS — ALPHABETICAL LIST 159

getdof
GETDOF Get the vector with the degrees of freedom of the model.

DOF=getdof(Elements,Types) builds the vector with the

labels of the degrees of freedom for which stiffness is present in the
finite element model.

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]

Types Element type definitions {TypID EltName Option1 ... }
DOF Degrees of freedom (nDOF * 1)

See also DOF_TRUSS, DOF_BEAM, GETDOF.

160 FUNCTIONS — ALPHABETICAL LIST

getmovie
GETMOVIE Get the movie from a figure where an animation has been played.

mov=getmovie(h)
gets the movie from the userdata of the axis of a figure where an animation
has been played. In order to save the movie in the userdata the animation
should have been played using animdisp(...,’CreateMovie’,’on’). This
function blocks the command prompt until the movie has become available.

h Axis handle.
mov Structured array with movie frames.

The movie can be played with movie(gcf,mov).

See also ANIMDISP, MOVIE.

FUNCTIONS — ALPHABETICAL LIST 161

grid plane4
GRID_PLANE4 Grid in natural coordinates for mapped meshing.

[s,t,NodeNum,Elements] = grid_plane4(m,n,Type,Section,Material)
returns matrices of a grid in the natural coordinate system, which can
be used for mapped meshing.

s s-coordinate of nodes (1 * nNodes)

t t-coordinate of nodes (1 * nNodes)
NodeNum Node numbers order on grid ((m+1) * (n+1))
Elements Node numbers are saved per element here (nElem * 8)
Type Type ID of meshed elements
Section Section ID of meshed elements
Material Material ID of meshed elements

See also MAKEMESH, GRID_SHELL8.

162 FUNCTIONS — ALPHABETICAL LIST

grid shell4
GRID_SHELL4 Grid in natural coordinates for mapped meshing.

[s,t,NodeNum,Elements] = grid_shell4(m,n,Type,Section,Material)
returns matrices of a grid in the natural coordinate system, which can
be used for mapped meshing.

s s-coordinate of nodes (1 * nNodes)

t t-coordinate of nodes (1 * nNodes)
NodeNum Node numbers order on grid ((m+1) * (n+1))
Elements Node numbers are saved per element here (nElem * 8)
Type Type ID of meshed elements
Section Section ID of meshed elements
Material Material ID of meshed elements

See also MAKEMESH, GRID_SHELL8.

FUNCTIONS — ALPHABETICAL LIST 163

grid shell8
GRID_SHELL8 Grid in natural coordinates for mapped meshing.

[s,t,NodeNum,Elements] = grid_shell8(m,n,Type,Section,Material)
returns matrices of a grid in the natural coordinate system, which can
be used for mapped meshing.

s s-coordinate of nodes (1 * nNodes)

t t-coordinate of nodes (1 * nNodes)
NodeNum Node numbers order on grid ((m+1) * (n+1))
Elements Node numbers are saved per element here (nElem * 12)
Type Type ID of meshed elements
Section Section ID of meshed elements
Material Material ID of meshed elements

See also MAKEMESH, GRID_SHELL4.

164 FUNCTIONS — ALPHABETICAL LIST

kelcs beam
KELCS_BEAM Beam element stiffness and mass matrix in local coordinate system.

[KeLCS,MeLCS] = KELCS_BEAM(L,A,ky,kz,Ixx,Iyy,Izz,E,nu,rho,Options)
[KeLCS,MeLCS] = KELCS_BEAM(L,A,ky,kz,Ixx,Iyy,Izz,E,nu,rho)
KeLCS = KELCS_BEAM(L,A,ky,kz,Ixx,Iyy,Izz,E,nu)
returns the element stiffness and mass matrix in the local coordinate system
for a two node beam element (isotropic material).

[KeLCS,~,dKeLCSdx] = KELCS_BEAM(L,A,ky,kz,Ixx,Iyy,Izz,E,nu,rho,Options,dLdx,dAdx,...
dkydx,dkzdx,dIxxdx,dIyydx,dIzzdx)
returns the element stiffness matrix in the local coordinate system
for a two node beam element (isotropic material), and additionally
computes the derivatives of the stiffness matrix with respect to the
design variables x. The derivatives of the mass matrix have not yet
been implemented.

L Beam length
A Beam cross section area
ky Shear deflection factor A_sy = ky * A
kz Shear deflection factor A_sz = kz * A
Ixx Moment of inertia
Iyy Moment of inertia
Izz Moment of inertia
E Young’s modulus
nu Poisson coefficient
rho Mass density
Options Options for the mass matrix: {’lumped’}, {’norotaroryinertia’}
dLdx Beam length derivatives (1 * nVar)
dAdx Beam cross section area derivatives (1 * nVar)
dkydx Shear deflection factor derivatives (1 * nVar)
dkzdx Shear deflection factor derivatives (1 * nVar)
dIxxdx Moment of inertia derivatives (1 * nVar)
dIyydx Moment of inertia derivatives (1 * nVar)
dIzzdx Moment of inertia derivatives (1 * nVar)
KeLCS Element stiffness matrix (12 * 12)
MeLCS Element mass matrix (12 * 12)
dKeLCSdx Element stiffness matrix derivatives (CELL(nVar,1))

See also KE_BEAM, KELCS_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 165

kelcs shell2
KELCS_SHELL2 SHELL2 element stiffness matrix in local coordinate system.

KeLCS = kelcs_shell2(r1,phi,L,h,E,nu) returns the element stiffness matrix

in the local coordinate system for a two-node axisymmetric shell element.
The global y-axis is assumed to be the axis of symmetry.

r1 Radial coordinate of node 1

phi Slope with respect to the xz-plane
h Shell thickness
E Young’s modulus
nu Poisson coefficient
KeLCS Element stiffness matrix (6 * 6)
166 FUNCTIONS — ALPHABETICAL LIST

kelcs shell4
KELCS_SHELL4 shell element stiffness and mass matrix in element
coordinate system.

[Ke,Me] = kelcs_shell4(Node_lc,h,E,nu,rho)
Ke = kelcs_shell4(Node_lc,h,E,nu)
returns the element stiffness and mass matrix in the element
coordinate system for a four node shell element (isotropic material).

Node Node definitions [x y z] (4 * 3)

Nodes should have the following order:
4---------3
| |
| |
| |
1---------2

h Shell thickness
E Young’s modulus
nu Poisson coefficient
rho Mass density
Options Element options [NOT available yet] {Option1 Option2 ...}
KeLCS Element stiffness matrix (24 * 24)
MeLCS Element mass matrix (24 * 24)

This element is a flat shell element that consists of a bilinear

membrane element and four overlaid DKT triangles for the bending
stiffness.

See also KE_SHELL8, ASMKM, KE_DKT.

FUNCTIONS — ALPHABETICAL LIST 167

kelcs truss
KELCS_TRUSS Truss element stiffness and mass matrix in local coordinate system.

[KeLCS,MeLCS] = KELCS_TRUSS(L,A,E,rho,Options)
[KeLCS,MeLCS] = KELCS_TRUSS(L,A,E,rho)
KeLCS = KELCS_TRUSS(L,A,E)
returns the element stiffness and mass matrix in the local coordinate system
for a two node truss element (isotropic material).

[KeLCS,~,dKeLCSdx] = KELCS_TRUSS(L,A,E,rho,Options,dLdx,dAdx)
returns the element stiffness matrix in the local coordinate system
for a two node truss element (isotropic material), and additionally
computes the derivatives of the stiffness matrix with respect to the
design variables x. The derivatives of the mass matrix have not yet
been implemented.

L Truss length
A Truss cross section area
E Young’s modulus
rho Mass density
Options Options for the mass matrix: {’lumped’}
dLdx Truss length derivatives (1 * nVar)
dAdx Truss cross section area derivatives (1 * nVar)
KeLCS Element stiffness matrix (6 * 6)
MeLCS Element mass matrix (6 * 6)
dKeLCSdx Element stiffness matrix derivatives (CELL(nVar,1))

See also KE_TRUSS, KELCS_BEAM.

168 FUNCTIONS — ALPHABETICAL LIST

ke beam
KE_BEAM Beam element stiffness and mass matrix in global coordinate system.

[Ke,Me] = KE_BEAM(Node,Section,Material,Options) returns the element

stiffness and mass matrix in the global coordinate system
for a two node beam element (isotropic material).

[Ke,~,dKedx] = KE_BEAM(Node,Section,Material,Options,dNodedx,dSectiondx)
returns the element stiffness matrix in the global coordinate system
for a two node beam element (isotropic material), and additionally
computes the derivatives of the stiffness matrix with respect to the
design variables x. The derivatives of the mass matrix have not yet
been implemented.

Node Node definitions [x y z] (3 * 3)

Section Section definition [A ky kz Ixx Iyy Izz]
Material Material definition [E nu rho]
Options Struct containing element options. Fields:
.lumped Construct lumped mass matrix:
{true | false (default)}
.rotationalInertia Include rotational inertia:
{true (default)| false}
dNodedx Node definitions derivatives (SIZE(Node) * nVar)
dSectiondx Section definitions derivatives (SIZE(Section) * nVar)
Ke Element stiffness matrix (12 * 12)
Me Element mass matrix (12 * 12)
dKedx Element stiffness matrix derivatives (CELL(nVar,1))

See also KELCS_BEAM, TRANS_BEAM, ASMKM, KE_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 169

ke dkt
KE_DKT DKT plate element stiffness and mass matrix.

[Ke,Me] = ke_dkt(Node,h,E,nu,rho)
Ke = ke_dkt(Node,h,E,nu)
returns the element stiffness and mass matrix in the global coordinate system
for a three node plate element (isotropic material) in the xy-plane.

Node Node definitions [x y] (3 * 2)

h Plate thickness (uniform or defined in nodes) [h]/[h1 h2 h3]
E Young’s modulus
nu Poisson coefficient
rho Mass density
Ke Element stiffness matrix (24 * 24)
Me Element mass matrix (24 * 24)

This element is a Discrete Kirchoff Triangle plate element. This code

is a MATLAB code based on the E-2 element FORTRAN coding, described in:
Construction of new efficient three-node triangular thin plate bending
elements, C. Jeyachandrabose and J. Kirkhope, Computers & Structures
Vol. 23, No. 5, pp. 587-603, 1986.

See also Q_DKT, SH_T, KE_DKT4.

170 FUNCTIONS — ALPHABETICAL LIST

ke mass
KE_MASS mass element system matrices in the global coordinate system.

[Ke,Me] = ke_mass(Node,Section,Material,Options) returns the element

stiffness and mass matrix in the global coordinate system for a
concentrated mass element

Node Node definitions [x1 y1 z1] (1 * 3)

Section Section definition [m]
Material Material definition []
Options Element options {Option1 Option2 ...}
Ke Element stiffness matrix (6 * 6)
Me Element mass matrix (6 * 6)
FUNCTIONS — ALPHABETICAL LIST 171

ke plane10
KE_PLANE10 plane element stiffness and mass matrix in global coordinate system.

[Ke,Me] = ke_plane10(Node,Section,Material,Options) returns the element

stiffness and mass matrix in the global coordinate system for a 10-node
plane triangular element. Plane10 only operates in the 2D xy-plane so that
z-coordinates should be equal to zero.

Node Node definitions [x y z] (10 * 3)

Nodes should have the following order:

3
| \
8 7
| \
9 10 6
| \
1--4--5--2

Section Section definition [h] (only used in plane stress)

Material Material definition [E nu rho]
Options Struct containing optional parameters. Fields:
.problem Plane stress or plane strain
{’2dstress’ (default) | ’2dstrain’}
.nXi Number of Gauss integration points
{1 | 3 | 4 | 6 | 7 (default) | 12 | 13 | 16 | 19 | 28 | 33 | 37}
Ke Element stiffness matrix (20 * 20)
Me Element mass matrix (20 * 20)

See also KE_BEAM, ASMKM, KE_TRUSS.

172 FUNCTIONS — ALPHABETICAL LIST

ke plane15
KE_PLANE15 plane element stiffness and mass matrix in global coordinate system.

[Ke,Me] = ke_plane15(Node,Section,Material,Options) returns the element

stiffness and mass matrix in the global coordinate system for a 15-node
plane triangular element. Plane15 only operates in the 2D xy-plane so that
z-coordinates should be equal to zero.

Node Node definitions [x y z] (15 * 3)

Nodes should have the following order:

3
| \
10 9
| \
11 15 8
| \
12 13 14 7
| \
1---4---5---6---2

Section Section definition [h] (only used in plane stress)

Material Material definition [E nu rho]
Options Struct containing optional parameters. Fields:
.problem Plane stress or plane strain
{’2dstress’ (default) | ’2dstrain’}
.nXi Number of Gauss integration points
{1 | 3 | 4 | 6 | 7 | 12 | 13 (default) | 16 | 19 | 28 | 33 | 37}
Ke Element stiffness matrix (30 * 30)
Me Element mass matrix (30 * 30)

See also KE_BEAM, ASMKM, KE_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 173

ke plane3
KE_PLANE3 plane element stiffness and mass matrix in global coordinate system.

[Ke,Me] = ke_plane3(Node,Section,Material,Options) returns the element

stiffness and mass matrix in the global coordinate system for a 3-node
CST element. Plane3 only operates in the 2D xy-plane so that
z-coordinates should be equal to zero.

Node Node definitions [x y z] (3 * 3)

Section Section definitions [h] (only used in plane stress)
Material Material definition [E nu rho]
Options Struct containing optional parameters. Fields:
.problem Plane stress or plane strain
{’2dstress’ (default) | ’2dstrain’}
Ke Element stiffness matrix (6 * 6)
Me Element mass matrix (6 * 6)
174 FUNCTIONS — ALPHABETICAL LIST

ke plane4
KE_PLANE4 plane element stiffness and mass matrix in global coordinate system.

[Ke,Me] = ke_plane4(Node,Section,Material,Options) returns the element

stiffness and mass matrix in the global coordinate system for a 4-node
plane element. Plane4 only operates in the 2D xy-plane so that
z-coordinates should be equal to zero.

Node Node definitions [x y z] (4 * 3)

Nodes should have the following order:

4---3
| |
1---2

Section Section definition [h] (only used in plane stress)

Material Material definition [E nu rho]
Options Struct containing optional parameters. Fields:
.problem Plane stress, plane strain or axisymmetrical
{’2dstress’ (default) | ’2dstrain’ | ’axisym’}
.bendingmodes Include (non-conforming) bending modes
{true (default) | false}
.integration Full (2x2) or reduced (1x1) integration
{’full’ (default) | ’reduced’}
Ke Element stiffness matrix (8 * 8)
Me Element mass matrix (8 * 8)

See also KE_BEAM, ASMKM, KE_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 175

ke plane6
KE_PLANE6 plane element stiffness and mass matrix in global coordinate system.

[Ke,Me] = ke_plane6(Node,Section,Material,Options) returns the element

stiffness and mass matrix in the global coordinate system for a 6-node
plane triangular element. Plane6 only operates in the 2D xy-plane so that
z-coordinates should be equal to zero.

Node Node definitions [x y z] (6 * 3)

Nodes should have the following order:

3
| \
6 5
| \
1--4--2

Section Section definition [h] (only used in plane stress)

Material Material definition [E nu rho]
Options Struct containing optional parameters. Fields:
.problem Plane stress or plane strain
{’2dstress’ (default) | ’2dstrain’}
.nXi Number of Gauss integration points
{1 | 3 | 4 | 6 | 7 (default) | 12 | 13 | 16 | 19 | 28 | 33 | 37}
Ke Element stiffness matrix (12 * 12)
Me Element mass matrix (12 * 12)

See also KE_BEAM, ASMKM, KE_TRUSS.

176 FUNCTIONS — ALPHABETICAL LIST

ke plane8
KE_PLANE8 plane element stiffness and mass matrix in global coordinate system.

[Ke,Me] = ke_plane8(Node,Section,Material,Options) returns the element

stiffness and mass matrix in the global coordinate system for a 8-node
plane element. Plane8 only operates in the 2D xy-plane so that
z-coordinates should be equal to zero.

Node Node definitions [x y z] (8 * 3)

Section Section definition [h] (only used in plane stress)
Material Material definition [E nu rho]
Options Struct containing optional parameters. Fields:
.problem Plane stress or plane strain
{’2dstress’ (default) | ’2dstrain’ | ’axisym’}
Ke Element stiffness matrix (16 * 16)
Me Element mass matrix (16 * 16)
FUNCTIONS — ALPHABETICAL LIST 177

ke shell2
KE_SHELL2 SHELL2 element stiffness matrix in global coordinate system.

Ke = ke_shell2(Node,Section,Material) returns the element stiffness

matrix in the global coordinate system for a two-node axisymmetric shell
element. The global y-axis is assumed to be the axis of symmetry.

Node Node definitions [x y z] (3 * 3)

Section Section definition [h]
Material Material definition [E nu]
Ke Element stiffness matrix (6 * 6)
178 FUNCTIONS — ALPHABETICAL LIST

ke shell4
KE_SHELL4 shell element stiffness and mass matrix in global coordinate system.

[Ke,Me] = ke_shell4(Node,Section,Material,Options)
Ke = ke_shell4(Node,Section,Material,Options)
returns the element stiffness and mass matrix in the global coordinate system
for a four node shell element (isotropic material).

Node Node definitions [x y z] (4 * 3)

Nodes should have the following order:
4---------3
| |
| |
| |
1---------2

Section Section definition [h]

Material Material definition [E nu rho]
Options Element options {Option1 Option2 ...}
Ke Element stiffness matrix (24 * 24)
Me Element mass matrix (24 * 24)

This shell element consists of a bilinear membrane element and

four overlaid DKT triangles for the bending stiffness.

See also KE_BEAM, ASMKM, KE_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 179

ke shell6
KE_SHELL6 shell element stiffness and mass matrix in global coordinate system.

[Ke,Me] = ke_shell6(Node,Section,Material,Options)
Ke = ke_shell6(Node,Section,Material,Options)
returns the element stiffness and mass matrix in the global coordinate system
for an eight node shell element.

Node Node definitions [x y z] (6 * 3)

Nodes should have the following order:
3
| \
6 5
| \
1--4--2

Section Section definition [h] or [h1 h2 h3]

(uniform thickness or defined in corner nodes(1,2,3))
Material Material definition [E nu rho] or
[Exx Eyy nuxy muxy muyz muzx theta rho]
Options Element options struct. Fields:
-LCSType: determine the reference local element
coordinate system. Values:
’element’ (default) or ’global’
-MatType: ’isotropic’ (default) or ’orthotropic’
-Offset: nodal offset from shell midplane. Values:
’top’, ’mid’ (default), ’bot’ or numerical value
Ke Element stiffness matrix (36 * 36)
Me Element mass matrix (36 * 36)

This element is based on chapter 15 of

The Finite Element Method: for Solid and Structural Mechanics,
Zienkiewicz (2005).

See also KE_BEAM, ASMKM, KE_TRUSS.

180 FUNCTIONS — ALPHABETICAL LIST

ke shell8
KE_SHELL8 Shell element stiffness and mass matrix in global coordinate system.

[Ke,Me] = ke_shell8(Node,Section,Material,Options)
Ke = ke_shell8(Node,Section,Material,Options)
returns the element stiffness and mass matrix in the global coordinate system
for an eight node shell element.

Node Node definitions [x y z] (8 * 3)

Nodes should have the following order:
4----7----3
| |
8 6
| |
1----5----2

Section Section definition [h] or [h1 h2 h3 h4]

(uniform thickness or defined in corner nodes(1,2,3,4))
Material Material definition [E nu rho] or
[Exx Eyy nuxy muxy muyz muzx theta rho]
Options Element options struct. Fields:
-LCSType: determine the reference local element
coordinate system. Values:
’element’ (default) or ’global’
-MatType: ’isotropic’ (default) or ’orthotropic’
-Offset: nodal offset from shell midplane. Values:
’top’, ’mid’ (default), ’bot’ or numerical value
-RotaryInertia: 0 (default) or 1
Ke Element stiffness matrix (48 * 48)
Me Element mass matrix (48 * 48)

This element is based on chapter 15 of

The Finite Element Method: for Solid and Structural Mechanics,
Zienkiewicz (2005).

See also KE_BEAM, ASMKM, KE_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 181

ke solid10
KE_SOLID10 Compute the element stiffness and mass matrix for a solid10 element.

[Ke,Me] = ke_solid10(Node,Section,Material,Options) computes element

stiffness and mass matrix in the global coordinate system for a solid10
element.

Node Node definitions [x y z] (10 * 3)

Nodes should have the following order:

4
/ | \
8 | 10
/ 9 \
1--- |-7--3
\ | /
5 | 6
\ | /
2

Section Section definition []

Material Material definition [E nu rho]
Options Struct containing optional parameters. Fields:
.nXi Number of Gauss integration points
{1 | 4 (default) | 5}
Ke Element stiffness matrix (30 * 30)
Me Element mass matrix (30 * 30)

See also KE_BEAM, ASMKM, KE_TRUSS.

182 FUNCTIONS — ALPHABETICAL LIST

ke solid15
KE_SOLID15 Compute the element stiffness and mass matrix for a solid15 element.

[Ke,Me] = ke_solid15(Node,Section,Material,Options) computes element

stiffness and mass matrix in the global coordinate system for a solid15
prismatic element.

Node Node definitions [x y z] (15 * 3)

Nodes should have the following order:
6
/ | \
12 | 11
/ 15 \
/ | \
4 ---10 ----5
| 3 |
| / \ |
13 9 8 14
| / \ |
|/ \|
1 --- 7 --- 2

Section Section definition []

Material Material definition [E nu rho]
Options Element options struct. Fields: []
Ke Element stiffness matrix (45 * 45)
Me Element mass matrix (45 * 45)
FUNCTIONS — ALPHABETICAL LIST 183

ke solid20
KE_SOLID20 Compute the element stiffness and mass matrix for a solid20 element.

[Ke,Me] = ke_solid20(Node,Section,Material,Options) computes element

stiffness and mass matrix in the global coordinate system for a solid20
element.

Node Node definitions [x y z] (20 * 3)

Nodes should have the following order:
8---15----7
/| /|
16 | 14 |
/ 20 / 19
/ | / |
5---13----6 |
| 4--11|----3
| / | /
17 12 18 10
| / | /
|/ |/
1----9----2

Section Section definition []

Material Material definition [E nu rho]
Options Element options struct. Fields: []
Ke Element stiffness matrix (60 * 60)
Me Element mass matrix (60 * 60)

See also KE_BEAM, ASMKM, KE_TRUSS.

184 FUNCTIONS — ALPHABETICAL LIST

ke solid4
KE_SOLID4 Compute the element stiffness and mass matrix for a solid4 element.

[Ke,Me] = ke_solid4(Node,Section,Material,Options) computes element

stiffness and mass matrix in the global coordinate system for a solid4
element.

Node Node definitions [x y z] (4 * 3)

Nodes should have the following order:

4
/ | \
/ | \
/ | \
1--- |----3
\ | /
\ | /
\ | /
2

Section Section definition []

Material Material definition [E nu rho]
Options Element options struct. Fields: []
Ke Element stiffness matrix (12 * 12)
Me Element mass matrix (12 * 12)

See also KE_BEAM, ASMKM, KE_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 185

ke solid8
KE_SOLID8 Compute the element stiffness and mass matrix for a solid8 element.

[Ke,Me] = ke_solid8(Node,Section,Material,Options)
[Ke,Me] = ke_solid8(Node,Section,Material,Options)
computes element stiffness and mass matrix in the global coordinate system
for a solid8 element.

Node Node definitions [x y z] (8 * 3)

Nodes should have the following order:
8---------7
/| /|
/ | / |
/ | / |
5---------6 |
| 4-----|---3
| / | /
| / | /
|/ |/
1---------2

Section Section definition []

Material Material definition [E nu rho]
Options Element options struct. Fields: []
Ke Element stiffness matrix (24 * 24)
Me Element mass matrix (24 * 24)

See also KE_BEAM, ASMKM, KE_TRUSS.

186 FUNCTIONS — ALPHABETICAL LIST

ke truss
KE_TRUSS Truss element stiffness and mass matrix in global coordinate system.

[Ke,Me] = KE_TRUSS(Node,Section,Material,Options) returns the element

stiffness and mass matrix in the global coordinate system
for a two node truss element (isotropic material).

[Ke,~,dKedx] = KE_TRUSS(Node,Section,Material,Options,dNodedx,dSectiondx)
returns the element stiffness matrix in the global coordinate system
for a two node truss element (isotropic material), and additionally
computes the derivatives of the stiffness matrix with respect to the
design variables x. The derivatives of the mass matrix have not yet
been implemented.

Node Node definitions [x1 y1 z1; x2 y2 z2] (2 * 3)

Section Section definition [A]
Material Material definition [E nu rho]
Options Struct containing element options. Fields:
.lumped Construct lumped mass matrix:
{true | false (default)}
dNodedx Node definitions derivatives (SIZE(Node) * nVar)
dSectiondx Section definitions derivatives (SIZE(Section) * nVar)
Ke Element stiffness matrix (6 * 6)
Me Element mass matrix (6 * 6)
dKedx Element stiffness matrix (CELL(nVar,1))

See also KELCS_TRUSS, TRANS_TRUSS, ASMKM, KE_BEAM.

FUNCTIONS — ALPHABETICAL LIST 187

lconstr
LCONSTR Add linear constraint equations to the stiffness matrix and load vector
using Lagrange multipliers.

[L,K,F]=lconstr(Constr,DOF,K,F)
[L,K,F,M]=lconstr(Constr,DOF,K,[],M)
[L,K,F,M]=lconstr(Constr,DOF,K,F,M)
modifies the stiffness matrix, the mass matrix and the load vector according
to the applied constraint equations. The dimensions of the stiffness matrix,
the mass matrix and the load vector increase with the number of constraints.
The resulting stiffness and mass matrix are symmetric.

Constr Constraint equation:

Constant=CoefS*SlaveDOF+CoefM1*MasterDOF1+CoefM2*MasterDOF2+...
[Constant CoefS SlaveDOF CoefM1 MasterDOF1 CoefM2 MasterDOF2 ...]
DOF Degrees of freedom (nDOF * 1)
L Selection matrix for displacements: U = L*(K\F); (nDOF * (nDOF+nConstr))
K Stiffness matrix (nDOF * nDOF)
F Load vector (nDOF * nSteps)
M Mass matrix (nDOF * nDOF)
188 FUNCTIONS — ALPHABETICAL LIST

linkandcheck
LINKANDCHECK Link two matrices and check for presence.

p3=linkandcheck(p1,p2,name)
Link two matrices and check for presence

p1 Vector with elements to be link and checked

p2 Vector with elements to be link and checked
name Name of elements in p2
p3 Lowest absolute index in p2 for each element in p1
FUNCTIONS — ALPHABETICAL LIST 189

loadslcs beam
LOADSLCS_BEAM Equivalent nodal forces for a beam element in the LCS.

FLCS = LOADSLCS_BEAM(DLoadLCS,L)
computes the equivalent nodal forces of a distributed load
(in the local coordinate system).

[FLCS,dFLCSdx] = LOADSLCS_BEAM(DLoadLCS,L,dDLoadLCSdx,dLdx)
additionally computes the derivatives of the equivalent nodal forces
with respect to the design variables x.

DLoadLCS Distributed loads [n1localX; n1localY; n1localZ; ...] (6/8 * nLC)

L Beam length
dDLoadLCSdx Distributed loads derivatives (6/8 * nLC * nVar)
dLdx Beam length derivatives (1 * nVar)
FLCS Load vector (12 * nLC)
dFLCSdx Load vector derivatives (12 * nLC * nVar)

See also LOADS_BEAM.

190 FUNCTIONS — ALPHABETICAL LIST

loadslcs shell2
LOADSLCS_SHELL2 Equivalent nodal forces for a SHELL2 element in the LCS.

FLCS = loadslcs_shell2(DLoadLCS,L)
computes the equivalent nodal forces of a distributed load
(in the local coordinate system).

DLoadLCS Distributed loads [n1localX; n1localY; n1localZ; ...]

(6 * 1)
L Element length
FLCS Load vector (12 * 1)
FUNCTIONS — ALPHABETICAL LIST 191

loadslcs shell4
LOADSLCS_SHELL4 Equivalent nodal forces for a shell4 element in the LCS.

F = loadslcs_shell4(DLoadLCS,Node)
computes the equivalent nodal forces of a distributed load
(in the local coordinate system).

DLoadLCS Distributed loads [n1localX; n1localY; n1localZ; ...]

in corner Nodes (12 * 1)
Node Node definitions [x y z] (4 * 3)
FLCS Load vector (24 * 1)

See also LOADSLCS_BEAM, ELEMLOADS, LOADS_TRUSS.

192 FUNCTIONS — ALPHABETICAL LIST

loads beam
LOADS_BEAM Equivalent nodal forces for a beam element in the GCS.

F = LOADS_BEAM(DLoad,Node)
computes the equivalent nodal forces of a distributed load
(in the global coordinate system).

[F,dFdx] = LOADS_BEAM(DLoad,Node,dDLoaddx,dNodedx)
additionally computes the derivatives of the equivalent nodal forces
with respect to the design variables x.

DLoad Distributed loads [n1globalX; n1globalY; n1globalZ; ...]

(6/8 * nLC * nDLoads)
Node Node definitions [x y z] (3 * 3)
dDLoaddx Distributed loads derivatives (6/8 * nLC * nVar * nDLoads)
dNodedx Node definitions derivatives (SIZE(Node) * nVar)
F Load vector (12 * nLC)
dFdx Load vector derivatives (12 * nLC * nVar)

See also LOADSLCS_BEAM, ELEMLOADS, LOADS_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 193

loads shell2
LOADS_SHELL2 Equivalent nodal forces for a SHELL2 element in the GCS.

F = loads_shell2(DLoad,Node)
computes the equivalent nodal forces of a distributed load
(in the global coordinate system).

DLoad Distributed loads [n1globalX; n1globalY; n1globalZ; ...]

(6 * 1)
Node Node definitions [x y z] (3 * 3)
F Load vector (6 * 1)
194 FUNCTIONS — ALPHABETICAL LIST

loads shell4
LOADS_SHELL4 Equivalent nodal forces for a shell4 element in the GCS.

F = loads_shell4(DLoad,Node)
computes the equivalent nodal forces of a distributed load
(in the global coordinate system).

DLoad Distributed loads [n1globalX; n1globalY; n1globalZ; ...]

in corner Nodes (12 * 1)
Node Node definitions [x y z] (4 * 3)
F Load vector (24 * 1)

See also LOADSLCS_BEAM, ELEMLOADS, LOADS_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 195

loads shell6
LOADS_SHELL6 Equivalent nodal forces for a shell6 element in the GCS.

F = loads_shell6(DLoad,Node)
computes the equivalent nodal forces of a distributed load
(in the global coordinate system).

DLoad Distributed loads [n1globalX; n1globalY; n1globalZ; ...]

in corner Nodes (9 * 1)
Node Node definitions [x y z] (6 * 3)
F Load vector (36 * 1)

See also LOADSLCS_BEAM, ELEMLOADS, LOADS_TRUSS.

196 FUNCTIONS — ALPHABETICAL LIST

loads shell8
LOADS_SHELL8 Equivalent nodal forces for a shell8 element in the GCS.

F = loads_shell8(DLoad,Node)
computes the equivalent nodal forces of a distributed load
(in the global coordinate system).

DLoad Distributed loads [n1globalX; n1globalY; n1globalZ; ...]

in corner Nodes (12 * 1)
Node Node definitions [x y z] (8 * 3)
F Load vector (48 * 1)

See also LOADSLCS_BEAM, ELEMLOADS, LOADS_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 197

loads solid20
LOADS_SOLID20 Equivalent nodal forces for a solid20 element.

F = loads_solid20(DLoad,Node)
computes the equivalent nodal forces of a distributed load
(in the global coordinate system).

DLoad Distributed loads [n1globalX; n1globalY; n1globalZ; ...]

in corner Nodes (24 * 1)
Node Node definitions [x y z] (8 * 3)
F Load vector (24 * 1)

See also LOADSLCS_BEAM, ELEMLOADS, LOADS_TRUSS.

198 FUNCTIONS — ALPHABETICAL LIST

loads solid8
LOADS_SOLID8 Equivalent nodal forces for a solid8 element.

F = loads_solid8(DLoad,Node)
computes the equivalent nodal forces of a distributed load
(in the global coordinate system).

DLoad Distributed loads [n1globalX; n1globalY; n1globalZ; ...]

in Nodes (24 * 1)
Node Node definitions [x y z] (8 * 3)
F Load vector (24 * 1)

See also LOADSLCS_BEAM, ELEMLOADS, LOADS_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 199

loads truss
LOADS_TRUSS Equivalent nodal forces for a truss element in the GCS.

F = LOADS_TRUSS(DLoad,Node)
computes the equivalent nodal forces of a distributed load
(in the global coordinate system).

[F,dFdx] = LOADS_TRUSS(DLoad,Node,dDLoaddx,dNodedx)
additionally computes the derivatives of the equivalent nodal forces
with respect to the design variables x.

DLoad Distributed load [n1globalX n1globalY n1globalZ ...]

(6/8 * nLC)
Node Node definitions [x y z] (2 * 3)
dDLoaddx Distributed load derivatives (6/8 * nLC * nVar)
dNodedx Node definitions derivatives (SIZE(Node) * nVar)
F Load vector (6 * nLC)
dFdx Load vector derivatives (6 * nLC * nVar)

See also ELEMLOADS, LOADS_BEAM.

200 FUNCTIONS — ALPHABETICAL LIST

lsolver
LSOLVER Solves linear system of equations.

[U,fK] = lsolver(K,P,save_factor,check_crpoint,fK)
solves the linear system K*U=P.

K Coefficient matrix [n * n]
P Right-hand side [n * 1]
save_factor Save factorization {true | false}
check_crpoint Check critical points {true | false}
fK Struct containing factorization of K
FUNCTIONS — ALPHABETICAL LIST 201

meshcat
eshcat is a function.
[Nodes, Elements] = meshcat(varargin)
202 FUNCTIONS — ALPHABETICAL LIST

msupf
MSUPF Modal superposition in the frequency domain.

[X,H] = MSUPF(omega,xi,Omega,Pm) calculates the modal transfer functions H

and the modal displacements x(t) = X * EXP(i * Omega * t) of a dynamic
system with the eigenfrequencies omega and the modal damping ratios xi due
to the modal excitation pm(t) = Pm * EXP(i * Omega * t).

omega Eigenfrequencies [rad/s] (nMode * 1)

xi Modal damping ratios [ - ] (nMode * 1) or (1 * 1), constant modal
damping is assumed in the (1 * 1) case.
Omega Excitation frequencies [rad/s] (1 * N).
Pm Complex amplitude of the modal excitation (nMode * N).
X Complex amplitude of the modal displacements (nMode * N).
H Modal transfer functions (nMode * N).
FUNCTIONS — ALPHABETICAL LIST 203

msupt
MSUPT Modal superposition in the time domain.

x = MSUPT(omega,xi,t,pm,x1,y1,interp) calculates the modal displacements

x(t) of a dynamic system with the eigenfrequencies omega and the modal
damping ratios xi due to the modal excitation pm(t), given the initial
conditions x1 and y1.
The solution of the modal differential equations is performed by means of
the piecewise exact method. Interp can be ’foh’ (first order hold) or ’zoh’
(zero order hold). In the first case the excitation is assumed to vary
linearly within each time step while in the second case it is assumed to be
constant: if t(k) <= t < t(k+1) then p(t) = p(k).

omega Eigenfrequencies [rad/s] (nMode * 1)

xi Modal damping ratios [ - ] (nMode * 1) or (1 * 1), constant modal
damping is assumed in the (1 * 1) case.
t Time points (1 * N) of the sampling of p, x and t.
pm Modal excitation (nMode * N).
x1 Modal displacements at time point t(1) (nMode * 1), defaults to zero.
y1 Modal velocities at time point t(1) (nMode * 1), defaults to zero.
interp Interpolation scheme: ’foh’ or ’zoh’, defaults to ’foh’.
x Modal displacements (nMode * N).
204 FUNCTIONS — ALPHABETICAL LIST

multdloads
MULTDLOADS Combine distributed loads.

DLoads = MULTDLOADS(DLoads_1,DLoads_2,...,DLoads_k)
combines the distributed loads of multiple load cases into one 3D array.
Each 3D-plane corresponds to a single load case. In the presence of
partial distributed loads, every row will have identical starting
and ending points in the 3rd dimension to allow for accurate combination
of load cases. A distributed load with a starting and/or ending point
value of ’NaN’ will be considered as a load on the entire element
Calculations will be more efficient compared to a partial distributed
load with starting point equal to zero and ending point equal to the
length of the element.

DLoads_k Distributed loads [EltID n1globalX n1globalY n1globalZ ...]

without partial DLoads: (nElem_k * 7)
with partial DLoads: (nElem_k * 9)
DLoads Distributed loads [EltID n1globalX n1globalY n1globalZ ...]
(maxnElem * 7 * k)
(maxnElem * 9 * k)

See also ELEMLOADS.

FUNCTIONS — ALPHABETICAL LIST 205

nedloadlcs beam
NEDLOADLCS_BEAM Interpolation functions for a distributed load on a beam element.

NeLCS = NEDLOADLCS_BEAM(Points)
NeLCS = NEDLOADLCS_BEAM(Points,phi_y,phi_z)
determines the values of the interpolation functions for a distributed
load in the specified points (LCS). These are used to compute the
displacements that occur due to the distributed loads if all nodes are
fixed.

NeLCS = NEDLOADLCS_BEAM(Points,[],[],a,b,L)
NeLCS = NEDLOADLCS_BEAM(Points,phi_y,phi_z,a,b,L)
determines the values of the interpolation functions for a partial
distributed load in the specified points (LCS). The load starts at a
distance ’a’ and ends at distance ’b’ from the first node of the element:
1) from 0 to a: no DLoad,
2) from a to b: DLoad,
3) from b to L: no DLoad.

[NeLCS,dNeLCSdx] = NEDLOADLCS_BEAM(Points,[],[],a,b,L,dadx,dbdx,dLdx)
[NeLCS,dNeLCSdx] = NEDLOADLCS_BEAM(Points,phi_y,phi_z,a,b,L,dadx,dbdx,dLdx)
additionally computes the derivatives of the interpolation functions of
a partial distributed load with respect to the design variables x.
Note: the derivatives of the interpolation functions for a distributed
load on the complete element are zero.

Points Points in the local coordinate system (1 * nPoints)

phi_y Shear deformation constant in y dir (scalar)
phi_z Shear deformation constant in z dir (scalar)
a Local starting point for the DLoad (scalar)
b Local ending point for the DLoad (scalar)
L Element length (scalar)
dadx Local starting point derivatives (1 * nVar)
dbdx Local ending point derivatives (1 * nVar)
dLdx Element length derivatives (1 * nVar)
NeDLoad Interpolated values (nPoints * 6)
dNeDLoaddx Interpolated values derivatives (nPoints * 6 *nVar)

See also DISP_BEAM, NELCS_BEAM.

206 FUNCTIONS — ALPHABETICAL LIST

nelcs beam
NELCS_BEAM Shape functions for a beam element.

NeLCS = nelcs_beam(Points)
NeLCS = nelcs_beam(Points,phi_y,phi_z)
determines the values of the shape functions in the specified points.

Points Points in the local coordinate system (1 * nPoints).

phi_y Shear deformation constant in the y-direction (1 * 1).
phi_z Shear deformation constant in the z-direction (1 * 1).
NeLCS Values (nPoints * 12).

See also DISP_BEAM.

FUNCTIONS — ALPHABETICAL LIST 207

newmark
NEWMARK Direct time integration for dynamic systems - Newmark method
[u,v,a,t] = NEWMARK(M,C,K,dt,p,u0,v0,a0,[alpha delta]) applies the Newmark
method for the calculation of the nodal displacements u, velocities v and
accelerations a of the dynamic system with the system matrices M, C and K
due to the excitation p.

M Mass matrix (nDof * nDof)

C Damping matrix (nDof * nDof)
K Stiffness matrix (nDof * nDof)
dt Time step of the integration scheme (1 * 1). Should be small enough
to ensure the stability and the precision of the integration scheme.
p Excitation (nDof * N). p(:,k) corresponds to time point t(k).
u0 Displacements at time point t(1)-dt (nDof * 1). Defaults to zero.
v0 Velocities at time point t(1)-dt (nDof * 1). Defaults to zero.
a0 Accelerations at time point t(1)-dt (nDof * 1). Defaults to zero.
u Displacements (nDof * N). u(:,k) corresponds to time point t(k).
t Time axis (1 * N), defined as t = [0:N-1] * dt.
208 FUNCTIONS — ALPHABETICAL LIST

nodalshellf
NODALSHELLF Compute the nodal shell forces/moments per unit length
from the element solution.

[FnLCS,FnLCS2] = nodalshellf(Nodes,Elements,Types,FeLCS) computes the

nodal forces from the element solution.

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
Sections Section definitions [SecID SecProp1 SecProp2 ...]
FeLCS Element forces/moments per unit length in corner nodes IJKL
(nElem * 32) [Nx Ny Nxy Mx My Mxy Vx Vy]
FnLCS Nodal forces/moments per unit length in corner nodes IJKL
(nElem * 32) [Nx Ny Nxy Mx My Mxy Vx Vy]
FnLCS2 Nodal forces per node (nNodes * 9)
(9 = NodID + 8 fcomp.)
[NodID Nx Ny Nxy Mx My Mxy Vx Vy]
See also ELEMSHELLF.
FUNCTIONS — ALPHABETICAL LIST 209

nodalstress
NODALSTRESS Compute the nodal stresses from the element solution.

[Sn,Sn2] = nodalstress(Nodes,Elements,Types,Se)
computes the nodal stresses from the element solution.

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
Sections Section definitions [SecID SecProp1 SecProp2 ...]
Se Element stresses in corner nodes IJKL and
at top/mid/bot of shell (nElem * 72)
72 = 6 stresscomp. * 4 nodes * 3 locations
[sxx syy szz sxy syz sxz ...]
Sn Nodal stress in corner nodes IJKL and
at top/mid/bot of shell (nElem * 72)
72 = 6 stresscomp. * 4 nodes * 3 locations
[sxx syy szz sxy syz sxz ...]
Sn2 Nodal stresses per node
at top/mid/bot of shell (nNodes * 19)
(19 = NodID + 3 locations * 6 scomp.)
[NodID sxx syy szz sxy syz sxz ...]
See also ELEMSTRESS.
210 FUNCTIONS — ALPHABETICAL LIST

nodalvalues
NODALVALUES Construct a vector with the values at the selected DOF.

F=nodalvalues(DOF,seldof,values)
constructs a vector with the values at the selected DOF. This function can
be used to obtain a load vector, initial displacements, velocities or
accelerations.

DOF Degrees of freedom (nDOF * 1)

seldof Selected degrees of freedom [NodID.dof] (nValues * 1)
values Corresponding values [Value] (nValues * nSteps)
F Load vector (nDOF * nSteps)

See also ELEMLOADS.

FUNCTIONS — ALPHABETICAL LIST 211

patch beam
PATCH_BEAM Patch information of the beam elements for plotting.

[pxyz,pind,pvalue] = patch_beam(Nodes,NodeNum,Values) returns matrices

to plot patches of beam elements.

Nodes Node definitions [NodID x y z].

NodeNum Node numbers [NodID1 NodID2 NodID3] (nElem * 3).
Values Values assigned to nodes used for coloring (nElem * 3).
pxyz Coordinates of Nodes (3*nElem * 3).
pind Indices of Nodes (nElem * 3).
pvalue Values arranged per Node (3*nElem * 1).
212 FUNCTIONS — ALPHABETICAL LIST

patch mass
PATCH_MASS Patch information of the mass elements for plotting.

[pxyz,pind,pvalue] = patch_mass(Nodes,NodeNum,Values) returns matrices

to plot patches of mass elements.

Nodes Node definitions [NodID x y z].

NodeNum Node numbers [NodID1 NodID2 NodID3] (nElem).
Values Values assigned to nodes used for coloring (nElem).
pxyz Coordinates of Nodes (nElem * 3).
pind Indices of Nodes (nElem).
pvalue Values arranged per Node (nElem).
FUNCTIONS — ALPHABETICAL LIST 213

patch plane3
PATCH_PLANE4 Patch information of the plane4 elements for plotting.

[pxyz,pind,pvalue] = patch_plane4(Nodes,NodeNum,Values) returns matrices

to plot patches of plane4 elements.

Nodes Node definitions [NodID x y z]

NodeNum Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 4)
Values Values assigned to nodes used for coloring (nElem * 4)
pxyz Coordinates of Nodes (4*nElem * 3)
pind indices of Nodes (nElem * 4)
pvalue Values arranged per Node (4*nElem * 1)

See also PLOTSTRESSCONTOURF, PLOTSHELLFCONTOURF.

214 FUNCTIONS — ALPHABETICAL LIST

patch plane4
PATCH_PLANE4 Patch information of the plane4 elements for plotting.

[pxyz,pind,pvalue] = patch_plane4(Nodes,NodeNum,Values) returns matrices

to plot patches of plane4 elements.

Nodes Node definitions [NodID x y z]

NodeNum Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 4)
Values Values assigned to nodes used for coloring (nElem * 4)
pxyz Coordinates of Nodes (4*nElem * 3)
pind Indices of Nodes (nElem * 4)
pvalue Values arranged per Node (4*nElem * 1)

See also PLOTSTRESSCONTOURF, PLOTSHELLFCONTOURF.

FUNCTIONS — ALPHABETICAL LIST 215

patch plane6
PATCH_PLANE4 Patch information of the plane4 elements for plotting.

[pxyz,pind,pvalue] = patch_plane4(Nodes,NodeNum,Values) returns matrices

to plot patches of plane4 elements.

Nodes Node definitions [NodID x y z]

NodeNum Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 4)
Values Values assigned to nodes used for coloring (nElem * 4)
pxyz Coordinates of Nodes (4*nElem * 3)
pind indices of Nodes (nElem * 4)
pvalue Values arranged per Node (4*nElem * 1)

See also PLOTSTRESSCONTOURF, PLOTSHELLFCONTOURF.

216 FUNCTIONS — ALPHABETICAL LIST

patch plane8
PATCH_PLANE4 Patch information of the plane4 elements for plotting.

[pxyz,pind,pvalue] = patch_plane4(Nodes,NodeNum,Values) returns matrices

to plot patches of plane4 elements.

Nodes Node definitions [NodID x y z]

NodeNum Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 4)
Values Values assigned to nodes used for coloring (nElem * 4)
pxyz Coordinates of Nodes (4*nElem * 3)
pind indices of Nodes (nElem * 4)
pvalue Values arranged per Node (4*nElem * 1)

See also PLOTSTRESSCONTOURF, PLOTSHELLFCONTOURF.

FUNCTIONS — ALPHABETICAL LIST 217

patch shell4
PATCH_SHELL4 Patch information of the shell4 elements for plotting.

[pxyz,pind,pvalue] = patch_shell4(Nodes,NodeNum,Values) returns matrices

to plot patches of shell4 elements.

Nodes Node definitions [NodID x y z]

NodeNum Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 4)
Values Values assigned to nodes used for coloring (nElem * 4)
pxyz Coordinates of Nodes (4*nElem * 3)
pind indices of Nodes (nElem * 4)
pvalue Values arranged per Node (4*nElem * 1)

See also PLOTSTRESSCONTOURF, PLOTSHELLFCONTOURF.

218 FUNCTIONS — ALPHABETICAL LIST

patch shell6
PATCH_SHELL6 Patch information of the shell6 elements for plotting.

[pxyz,pind,pvalue] = patch_shell6(Nodes,NodeNum,Values) returns matrices

to plot patches of shell6 elements.

Nodes Node definitions [NodID x y z]

NodeNum Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 6)
Values Values assigned to nodes used for coloring (nElem * 6)
pxyz Coordinates of Nodes (6*nElem * 3)
pind indices of Nodes (nElem * 8)
pvalue Values arranged per Node (6*nElem * 1)

See also PLOTSTRESSCONTOURF, PLOTSHELLFCONTOURF.

FUNCTIONS — ALPHABETICAL LIST 219

patch shell8
PATCH_SHELL8 Patch information of the shell8 elements for plotting.

[pxyz,pind,pvalue] = patch_shell8(Nodes,NodeNum,Values)
returns matrices to plot patches of shell8 elements.

Nodes Node definitions [NodID x y z]

NodeNum Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 8)
Values Values assigned to nodes used for coloring (nElem * 8)
pxyz Coordinates of Nodes (8*nElem * 3)
pind indices of Nodes (nElem * 8)
pvalue Values arranged per Node (8*nElem * 1)

See also PLOTSTRESSCONTOURF, PLOTSHELLFCONTOURF.

220 FUNCTIONS — ALPHABETICAL LIST

patch solid10
PATCH_SOLID20 Patch information of the solid10 elements for plotting.

[pxyz,pind,pvalue] = patch_solid20(Nodes,NodeNum,Values)
returns matrices to plot patches of solid10 elements.

Nodes Node definitions [NodID x y z]

NodeNum Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 10)
Values Values assigned to nodes used for coloring (nElem * 4)
pxyz Coordinates of Nodes (4*nElem * 3)
pind indices of Nodes (nElem * 4)
pvalue Values arranged per Node (4*nElem * 1)

See also PATCH_SHELL20.

FUNCTIONS — ALPHABETICAL LIST 221

patch solid20
PATCH_SOLID20 Patch information of the solid20 elements for plotting.

[pxyz,pind,pvalue] = patch_solid20(Nodes,NodeNum,Values)
returns matrices to plot patches of solid20 elements.

Nodes Node definitions [NodID x y z]

NodeNum Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 20)
Values Values assigned to nodes used for coloring (nElem * 8)
pxyz Coordinates of Nodes (8*nElem * 3)
pind indices of Nodes (nElem * 8)
pvalue Values arranged per Node (8*nElem * 1)

See also PATCH_SHELL8.

222 FUNCTIONS — ALPHABETICAL LIST

patch solid4
PATCH_SOLID4 Patch information of the solid4 elements for plotting.

[pxyz,pind,pvalue] = patch_solid20(Nodes,NodeNum,Values)
returns matrices to plot patches of solid4 elements.

Nodes Node definitions [NodID x y z]

NodeNum Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 10)
Values Values assigned to nodes used for coloring (nElem * 4)
pxyz Coordinates of Nodes (4*nElem * 3)
pind indices of Nodes (nElem * 4)
pvalue Values arranged per Node (4*nElem * 1)

See also PATCH_SHELL20.

FUNCTIONS — ALPHABETICAL LIST 223

patch solid8
PATCH_SOLID8 Patch information of the solid8 elements for plotting.

[pxyz,pind,pvalue] = patch_solid8(Nodes,NodeNum,Values)
returns matrices to plot patches of solid8 elements.

Nodes Node definitions [NodID x y z]

NodeNum Node numbers [NodID1 NodID2 NodID3 NodID4] (nElem * 8)
Values Values assigned to nodes used for coloring (nElem * 8)
pxyz Coordinates of Nodes (8*nElem * 3)
pind indices of Nodes (nElem * 8)
pvalue Values arranged per Node (8*nElem * 1)

See also PATCH_SHELL8.

224 FUNCTIONS — ALPHABETICAL LIST

patch truss
PATCH_TRUSS Patch information of the truss elements for plotting.

[pxyz,pind,pvalue] = patch_truss(Nodes,NodeNum,Values) returns matrices

to plot patches of truss elements.

Nodes Node definitions [NodID x y z].

NodeNum Node numbers [NodID1 NodID2 NodID3] (nElem * 2).
Values Values assigned to nodes used for coloring (nElem * 2).
pxyz Coordinates of Nodes (2*nElem * 3).
pind Indices of Nodes (nElem * 2).
pvalue Values arranged per Node (2*nElem * 1).
FUNCTIONS — ALPHABETICAL LIST 225

plotdisp
PLOTDISP Plot the displacements.

plotdisp(Nodes,Elements,Types,DOF,U,DLoads,Sections,Materials)
plotdisp(Nodes,Elements,Types,DOF,U,[],Sections,Materials)
plotdisp(Nodes,Elements,Types,DOF,U)
DispScal=plotdisp(Nodes,Elements,Types,DOF,U,DLoads,Sections,Materials)
plots the displacements. If DLoads, Sections and Materials are supplied, the
displacements that occur due to the distributed loads if all nodes are fixed,
are superimposed.

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
DOF Degrees of freedom (nDOF * 1)
U Displacements (nDOF * 1)
DLoads Distributed loads [EltID n1globalX n1globalY n1globalZ ...]
(use empty array [] when shear deformation (in beam element)
is considered but no DLoads are present)
Sections Section definitions [SecID SecProp1 SecProp2 ...]
Materials Material definitions [MatID MatProp1 MatProp2 ... ]
DispScal Displacement scaling

plotdisp(...,ParamName,ParamValue) sets the value of the specified

parameters. The following parameters can be specified:
’DispScal’ Displacement scaling. Default: ’auto’.
’DispMax’ Mention maximal displacement. Default: ’on’.
’Undeformed’ Plots the undeformed mesh. Default: ’k:’.
’Handle’ Plots in the axis with this handle. Default: current axis.
Additional parameters are redirected to the PLOT3 function which plots
the deformations.

[DispScal,h] = plotdisp(...) returns a struct h with handles to all the

objects in the plot.

See also DISP_TRUSS, DISP_BEAM, PLOTELEM.

226 FUNCTIONS — ALPHABETICAL LIST

plotdispx
PLOTDISPX Plot element quantity on deformed elements.

plotdispx(Nodes,Elements,Types,DOF,U,x);
[h,DispScal] = plotdispx(Nodes,Elements,Types,DOF,U,x,varargin)
plots element quantity on deformed elements.

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
DOF Degrees of freedom (nDOF * 1)
U Displacements (nDOF * 1)
x Elements quantity to plot (nElem * 1)
plotdispx(...,ParamName,ParamValue) sets the value of the
specified parameters. The following parameters can be specified:
’GCS’ Plot the GCS. Default: ’on’.
’minmax’ Add location of min and max stress. Default: ’off’.
’colorbar’ Add colorbar. Default: ’off’.
’Undeformed’ Plots the undeformed mesh. {’on’ | ’off’ (default)}
’ncolor’ Number of colors in colormap. Default: 10.
’Handle’ Plots in the axis with this handle. Default: current axis.
Additional parameters are redirected to the PATCH function which plots
the elements.
FUNCTIONS — ALPHABETICAL LIST 227

plotelem
PLOTELEM Plot the elements.

plotelem(Nodes,Elements,Types)
plots the elements.

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }

plotelem(...,ParamName,ParamValue) sets the value of the specified

parameters. The following parameters can be specified:
’Numbering’ Plots the element numbers. Default: ’on’.
’GCS’ Plots the global coordinate system. Default: ’on’.
’Handle’ Plots in the axis with this handle. Default: current axis.
Additional parameters are redirected to the PLOT3 function which plots
the elements.

h = PLOTELEM(...) returns a struct h with handles to all the objects

in the plot.

See also COORD_TRUSS, COORD_BEAM, PLOTDISP.

228 FUNCTIONS — ALPHABETICAL LIST

plotelemx
PLOTELEMX Plot element quantity on elements.

plotelemx(Nodes,Elements,Types,x) plots element quantity on elements.

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
x Elements quantity to plot (nElem * 1)
plotelemx(...,ParamName,ParamValue) sets the value of the
specified parameters. The following parameters can be specified:
’GCS’ Plot the GCS. Default: ’on’.
’minmax’ Add location of min and max stress. Default: ’off’.
’colorbar’ Add colorbar. Default: ’off’.
’Undeformed’ Plots the undeformed mesh. Default: ’k-’.
’ncolor’ Number of colors in colormap. Default: 10.
’Handle’ Plots in the axis with this handle. Default: current axis.
Additional parameters are redirected to the PATCH function which plots
the elements.

See also ELEMSTRESS.

FUNCTIONS — ALPHABETICAL LIST 229

plotforc
PLOTFORC Plot element member forces.

plotforc(ftype,Nodes,Elements,Types,Sections,Materials,Forces,DLoads)
plotforc(ftype,Nodes,Elements,Types,Sections,Materials,Forces)
plots the element member forces (in accordance to the beam convention).

ftype ’norm’ Normal force (in the local x-direction)

(for truss ’sheary’ Shear force in the local y-direction
and beam ’shearz’ Shear force in the local z-direction
elements) ’momx’ Torsional moment (around the local x-direction)
’momy’ Bending moment around the local y-direction
’momz’ Bending moment around the local z-direction
ftype ’Nphi’ Normal force (per unit length) in meridional direction
(for ’Qphi’ Transverse force (per unit length) in meridional direction
shell2 ’Mphi’ Bending moment (per unit length) in meridional direction
elements) ’Ntheta’ Normal force (per unit length) in circumferential direction
’Mtheta’ Bending moment (per unit length) in circumferential direction
Nodes Node definitions [NodID x y z]
Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
Sections Section definitions [SecID SecProp1 SecProp2 ...]
Materials Material definitions [MatID MatProp1 MatProp2 ... ]
Forces Element forces in LCS (beam convention) [N Vy Vz T My Mz]
(nElem * 12)
DLoads Distributed loads [EltID n1globalX n1globalY n1globalZ ...]

plotforc(...,ParamName,ParamValue) sets the value of the specified

parameters. The following parameters can be specified:
’ForcScal’ Force scaling. Default: ’auto’.
’MinMax’ Display minimum and maximum value. Default: ’off’.
’Values’ Force values. Default: ’on’.
’Undeformed’ Plots the undeformed mesh. Default: ’k-’.
’Handle’ Plots in the axis with this handle. Default: current axis.
Additional parameters are redirected to the PLOT3 function which plots
the forces.

[ForcScal,h] = plotforc(...) returns a struct h with handles to all the

objects in the plot.

See also FDIAGRGCS_BEAM, FDIAGRGCS_TRUSS.

230 FUNCTIONS — ALPHABETICAL LIST

plotgcs
lotgcs is a function.
h = plotgcs(lref, h)
FUNCTIONS — ALPHABETICAL LIST 231

plotlcs
PLOTLCS Plot the local element coordinate systems.

[h,vLCS] = plotlcs(Nodes,Elements,Types)
[h,vLCS] = plotlcs(Nodes,Elements,Types,[],varargin)
plotlcs(Nodes,Elements,Types,vLCS,varargin)

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
vLCS Element coordinate systems (nElem * 9)
plotlcs(...,ParamName,ParamValue) sets the value of the specified
parameters. The following parameters can be specified:
’GCS’ Plot the GCS. Default: ’on’.
’Undeformed’ Plots the undeformed mesh. Default: ’k-’.
’Handle’ Plots in the axis with this handle. Default: current
axis.

See also ELEMSTRESS

232 FUNCTIONS — ALPHABETICAL LIST

plotnodes
PLOTNODES Plot the nodes.

plotnodes(Nodes)
plots the nodes.

Nodes Node definitions [NodID x y z]

plotnodes(...,ParamName,ParamValue) sets the value of the specified

parameters. The following parameters can be specified:
’Numbering’ Plots the node numbers. Default: ’on’.
’GCS’ Plots the global coordinate system. Default: ’on’.
’Handle’ Plots in the axis with this handle. Default: current axis.
Additional parameters are redirected to the PLOT3 function which plots
the nodes.

h = PLOTNODES(...) returns a struct h with handles to all the objects

in the plot.

See also PLOTELEM, PLOTDISP.

FUNCTIONS — ALPHABETICAL LIST 233

plotprincstress
PLOTPRINCSTRESS Plot the principal stresses in shell elements.

plotprincstress(Nodes,Elements,Types,Spr,Vpr)
plots the principal stresses in shell elements with a vector plot.

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
Spr Principal stresses (nElem * 72) [s3 s2 s1 0 0 0 ...]
Vpr Principal dir. matrix (output from principalstress)
{nElem * 12}
plotprincdir(...,ParamName,ParamValue) sets the value of the specified
parameters. The following parameters can be specified:
’location’ Location (top,mid,bot). Default: ’top’.
’GCS’ Plot the GCS. Default: ’on’.
’VectScal’ Vector scaling. Default: ’auto’.
’Undeformed’ Plots the undeformed mesh. Default: ’k-’.
’Handle’ Plots in the axis with this handle. Default: current
axis.

See also PRINCIPALSTRESS.

234 FUNCTIONS — ALPHABETICAL LIST

plotshellfcontour
PLOTSHELLFCONTOUR Plot forces/moments per unit length in shell elements.

plotshellfcontour(ftype,Nodes,Elements,Types,F)
plots force contours (output from ELEMSHELLF/NODALSHELLF).

ftype ’Nx’ Membrane forces

’Ny’
’Nxy’
’Mx’ Bending moments
’My’
’Mxy’
’Vx’ Shear forces
’Vy’
Nodes Node definitions [NodID x y z]
Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
F Forces/moments per unit length
(nElem * 32) [Nx Ny Nxy Mx My Mxy Vx Vy]
plotshellfcontour(...,ParamName,ParamValue) sets the value of the specified
parameters. The following parameters can be specified:
’Ncontour’ Number of contours. Default: ’10’.
’GCS’ Plot the GCS. Default: ’on’.
’Undeformed’ Plots the undeformed mesh. Default: ’k-’.
’Handle’ Plots in the axis with this handle. Default: current axis.

See also ELEMSHELLF, SCONTOUR_SHELL8, SCONTOUR_SHELL4.

FUNCTIONS — ALPHABETICAL LIST 235

plotshellfcontourf
PLOTSHELLFCONTOURF Plot filled contours of shell forces in shell elements.

plotshellfcontourf(stype,Nodes,Elements,Types,F)
plotshellfcontourf(stype,Nodes,Elements,Types,F,DOF,U)
plots force contours (output from ELEMSTRESS).

ftype ’Nx’ Membrane forces

’Ny’
’Nxy’
’Mx’ Bending moments
’My’
’Mxy’
’Vx’ Shear forces
’Vy’
Nodes Node definitions [NodID x y z]
Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
F Forces/moments per unit length
(nElem * 32) [Nx Ny Nxy Mx My Mxy Vx Vy]
DOF Degrees of freedom (nDOF * 1)
U Displacements (nDOF * 1)
plotshellfcontourf(...,ParamName,ParamValue) sets the value of the
specified parameters. The following parameters can be specified:
’GCS’ Plot the GCS. Default: ’on’.
’ncolor’ Number of colors in colormap. Default: 10.
’Handle’ Plots in the axis with this handle. Default: current axis.

See also ELEMSHELLF, PATCH_SHELL8, PATCH_SHELL4.

236 FUNCTIONS — ALPHABETICAL LIST

plotstress
PLOTSTRESS Plot the stresses.

plotstress(stype,Nodes,Elements,Types,Sections,Materials,Forces,DLoads)
plotstress(stype,Nodes,Elements,Types,Sections,Materials,Forces)
plots the stresses.

stype ’snorm’ Normal stress due to normal force

(for truss ’smomyt’ Normal stress due to bending moment
and beam around the local y-direction at the top
elements) ’smomyb’ Normal stress due to bending moment
around the local y-direction at the bottom
’smomzt’ Normal stress due to bending moment
around the local z-direction at the top
’smomzb’ Normal stress due to bending moment
around the local z-direction at the bottom
’smax’ Maximal normal stress (normal force and bending moment)
’smin’ Minimal normal stress (normal force and bending moment)
stype ’sNphi’ Stress due to normal force in meridional direction
(for ’sMphiT’ Stress at the top due to bending moment in
meridional direction
shell2 ’sMphiB’ Stress at the bottom due to bending moment in
meridional direction
elements) ’sNtheta’ Stress due to normal force in circumferential direction
’sMthetaT’ Stress at the top due to bending moment in
circumferential direction
’sMthetaB’ Stress at the bottom due to bending moment in
circumferential direction
Nodes Node definitions [NodID x y z]
Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
Sections Section definitions [A ky kz Ixx Iyy Izz yt yb zt zb]
Materials Material definitions [MatID MatProp1 MatProp2 ... ]
Forces Element forces in LCS (beam convention) [N Vy Vz T My Mz]
(nElem * 12)
DLoads Distributed loads [EltID n1globalX n1globalY n1globalZ ...]

plotstress(...,ParamName,ParamValue) sets the value of the specified

parameters. The following parameters can be specified:
’StressScal’ Stress scaling. Default: ’auto’.
’MinMax’ Display minimum and maximum value. Default: ’off’.
’Values’ Stress values. Default: ’on’.
’Undeformed’ Plots the undeformed mesh. Default: ’k-’.
’Handle’ Plots in the axis with this handle. Default: current axis.
Additional parameters are redirected to the PLOT3 function which plots
the stresses.

[StressScal,h] = plotstress(...) returns a struct h with handles to all the

objects in the plot.

See also SDIAGRGCS_BEAM, SDIAGRGCS_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 237

plotstresscontour
PLOTSTRESSCONTOUR Plot stress contour lines in shell elements.

plotstresscontour(stype,Nodes,Elements,Types,S)
plots stress contours (output from ELEMSTRESS/NODALSTRESS).

stype ’sx’ Normal stress (in the global/local x-direction)

’sy’
’sz’
’sxy’ Shear stress
’syz’
’sxz’
Nodes Node definitions [NodID x y z]
Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
S Element stresses in GCS/LCS [sxx syy szz sxy syz sxz]
(nElem * 72)
plotstresscontour(...,ParamName,ParamValue) sets the value of the specified
parameters. The following parameters can be specified:
’location’ Location (top,mid,bot). Default: ’top’.
’Ncontour’ Number of contours. Default: ’10’.
’GCS’ Plot the GCS. Default: ’on’.
’Undeformed’ Plots the undeformed mesh. Default: ’k-’.
’Handle’ Plots in the axis with this handle. Default: current axis.

See also ELEMSTRESS, SCONTOUR_SHELL8, SCONTOUR_SHELL4.

238 FUNCTIONS — ALPHABETICAL LIST

plotstresscontourf
PLOTSTRESSCONTOURF Plot filled contours of stresses.

plotstresscontourf(stype,Nodes,Elements,Types,S)
plotstresscontourf(stype,Nodes,Elements,Types,S,DOF,U)
plots stress contours (output from ELEMSTRESS).

stype ’sx’ Normal stress (in the global/local x-direction)

’sy’
’sz’
’sxy’ Shear stress
’syz’
’sxz’
Nodes Node definitions [NodID x y z]
Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
S Element stresses in GCS/LCS [sxx syy szz sxy syz sxz]
(nElem * 72)
plotstresscontourf(...,ParamName,ParamValue) sets the value of the
specified parameters. The following parameters can be specified:
’location’ Location (top,mid,bot). Default: ’top’.
’GCS’ Plot the GCS. Default: ’on’.
’minmax’ Add location of min and max stress. Default: ’on’.
’colorbar’ Add colorbar. Default: ’on’.
’ncolor’ Number of colors in colormap. Default: 10.
’Handle’ Plots in the axis with this handle. Default: current axis.

See also ELEMSTRESS.

FUNCTIONS — ALPHABETICAL LIST 239

pressure shell4
PRESSURE_SHELL4 Equivalent nodal forces for a shell4 element in the GCS
due to a pressure normal to the element surface.

F = pressure_shell4(Pressure,Node)
computes the equivalent nodal forces of a pressure load normal to the
elements surface.

Pressure Distributed pressure in corner Nodes [p1lobalZ; ...]

(4 * 1)
Node Node definitions [x y z] (4 * 3)
F Load vector (24 * 1)

See also ELEMPRESSURE, PRESSURE_SHELL8.

240 FUNCTIONS — ALPHABETICAL LIST

pressure shell6
PRESSURE_SHELL8 Equivalent nodal forces for a shell6 element in the GCS
due to a pressure normal to the element surface.

F = pressure_shell(Pressure,Node)
computes the equivalent nodal forces of a pressure load normal to
the elements surface.

Pressure Distributed loads in corner Nodes [p1localZ; ...]

(3 * 1)
Node Node definitions [x y z] (6 * 3)
F Load vector (36 * 1)

See also ELEMPRESSURE, PRESSURE_SHELL4.

FUNCTIONS — ALPHABETICAL LIST 241

pressure shell8
PRESSURE_SHELL8 Equivalent nodal forces for a shell8 element in the GCS
due to a pressure normal to the element surface.

F = pressure_shell(Pressure,Node)
computes the equivalent nodal forces of a pressure load normal to
the elements surface.

Pressure Distributed loads in corner Nodes [p1localZ; ...]

(4 * 1)
Node Node definitions [x y z] (8 * 3)
F Load vector (48 * 1)

See also ELEMPRESSURE, PRESSURE_SHELL4.

242 FUNCTIONS — ALPHABETICAL LIST

principalstress
PRINCIPALSTRESS Compute the principal stresses and directions in shell elements.

[Spr,Vpr] = principalstress(Elements,SeGCS)
computes the principal stresses and directions.

Elements Element definitions [EltID TypID SecID MatID n1 n2...]

SeGCS Element stresses in GCS in corner nodes IJKL and
at top/mid/bot of shell (nElem * 72)
72 = 6 stresscomp. * 4 nodes * 3 locations
[sxx syy szz sxy syz sxz ...]
Spr Principal stress (nElem * 72)
[s1 s2 s3 0 0 0 ...]
Vpr Principal stress directions {nElem * 12}

See also ELEMSTRESS, PLOTPRINCDIR.

FUNCTIONS — ALPHABETICAL LIST 243

printdisp
PRINTDISP Display the displacements in the command window.

printdisp(Nodes,DOF,U)
displays the displacements in the command window.

Nodes Node definitions [NodID x y z]

DOF Degrees of freedom (nDOF * 1)
U Displacements (nDOF * 1)

See also PRINTFORC, PLOTDISP.

244 FUNCTIONS — ALPHABETICAL LIST

printforc
PRINTFORC Display the forces in the command window.

printforc(Elements,Forces)
displays the forces in the command window.

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]

Forces Element forces [N Vy Vz T My Mz] (nElem * 12)

See also PRINTDISP.

FUNCTIONS — ALPHABETICAL LIST 245

printshellf
PRINTSHELLF Display forces/moments in command window (shell elements).

printshellf(Elements,F)
displays shell forces in command window.

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]

F Shellf matrix [Nx Ny Nxy Mx My Mxy Vx Vy] (nElem * 32)

See also PRINTSTRESS.

246 FUNCTIONS — ALPHABETICAL LIST

printstress
PRINTSTRESS Display stress in command window (shell elements).

printstress(Elements,S,location) displays stress in command window.

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]

S Stress matrix [sx sy sz sxy syz szx] (nElem * 72)

See also PRINTSHELLF.

FUNCTIONS — ALPHABETICAL LIST 247

q dkt
Q_DKT Q matrix for a DKT element.

Q = Q_DKT(b,c,det) returns the Q matrix of the DKT element,

which is used to compute the curvatures of the plate element

b Geometrical property of the triangle (see ke_dkt) (3 * 1)

c Geometrical property of the triangle (3 * 1)
det Determinant of the parametric transformation (=2*area of
triangle)

See also KE_DKT, KELCS_SHELL4, SE_SHELL4.

248 FUNCTIONS — ALPHABETICAL LIST

reaction
REACTION Compute the reaction forces for a degree of freedom.

Freac=reaction(Elements,ForcesGCS,seldof)
computes the reaction forces for a degree of freedom.

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]

ForcesGCS Element forces in GCS (nElem * 12)
seldof Selected DOF labels (kDOF * 1)
Freac Reaction force

See also ELEMFORCES.

FUNCTIONS — ALPHABETICAL LIST 249

removedof
REMOVEDOF Remove DOF with Dirichlet boundary conditions equal to zero.

DOF=removedof(DOF,seldof) removes the specified Dirichlet boundary

conditions from the degrees of freedom vector.

DOF Degrees of freedom (nDOF * 1)

seldof Dirichlet boundary conditions equal to zero [NodID.dof]

See also GETDOF.

250 FUNCTIONS — ALPHABETICAL LIST

reprow
REPROW Replicate rows from a matrix.

Matrix=reprow(Matrix,RowSel,nTime,RowInc)
replicates the selected rows from a matrix a number of times and adds them
below the existing rows. The k-th time the increment RowInc is added k times
to the copied rows.

Matrix Matrix (nRow * nCol)

RowSel Rows to be copied (1 * kRow)
nTime Number of times
RowInc Increments that are added to the different columns of the copied
rows (1 * nCol)
FUNCTIONS — ALPHABETICAL LIST 251

scontour shell4
SCONTOUR_SHELL4 Matrix to plot contours in a shell4 element.

Scontour = scontour_shell4(Node,Stress,Svalues) returns a matrix used

for plotting contours in a shell4 element.

Node Node definitions [x y z] (4 * 3)

Stress Stress in nodes (4 * 1)
Svalues Values of contours (nContour * 1)
Scontour Coordinates of contours in GCS

See also PLOTSTRESSCONTOUR, PLOTSHELLFCONTOUR.

252 FUNCTIONS — ALPHABETICAL LIST

scontour shell8
SCONTOUR_SHELL8 Matrix to plot contours in a shell8 element.

Scontour = scontour_shell8(Node,Stress,Svalues) returns a matrix used

for plotting contours in a shell4 element.

Node Node definitions [x y z] (4 * 3)

Stress Stress in nodes (4 * 1) or (8 * 1)
Svalues Values of contours (nContour * 1)
Scontour Coordinates of contours in GCS

See also PLOTSTRESSCONTOUR, PLOTSHELLFCONTOUR.

FUNCTIONS — ALPHABETICAL LIST 253

sdiagrgcs beam
SDIAGRGCS_BEAM Return matrices to plot the stresses in a beam element.

[ElemGCS,SdiagrGCS,ElemExtGCS,ExtremaGCS,Extrema]
= sdiagrgcs_beam(stype,Forces,Node,Section,[],DLoad,Points)
[ElemGCS,SdiagrGCS,ElemExtGCS,ExtremaGCS,Extrema]
= sdiagrgcs_beam(Forces,Node,Section,[],DLoad)
returns the coordinates of the points along the beam in the global
coordinate system and the coordinates of the stresses with respect to the beam
in the global coordinate system. These can be added in order to plot the
stresses: ElemGCS+SdiagrGCS. The coordinates of the points with extreme values
and the coordinates of the extreme values with respect to the beam are given
as well and can be similarly added: ElemExtGCS+ExtremaGCS. Extrema is the
list with the corresponding extreme values.

stype ’snorm’ Normal stress due to normal force

’smomyt’ Normal stress due to bending moment
around the local y-direction at the top
’smomyb’ Normal stress due to bending moment
around the local y-direction at the bottom
’smomzt’ Normal stress due to bending moment
around the local z-direction at the top
’smomzb’ Normal stress due to bending moment
around the local z-direction at the bottom
’smax’ Maximal normal stress (normal force and bending moment)
’smin’ Minimal normal stress (normal force and bending moment)
Forces Element forces in LCS (beam convention) [N; Vy; Vz; T; My; Mz]
(12 * 1)
Node Node definitions [x y z] (3 * 3)
Section Section definition [A ky kz Ixx Iyy Izz yt yb zt zb]
DLoad Distributed loads [n1globalX; n1globalY; n1globalZ; ...]
(6 * 1)
Points Points in the local coordinate system (1 * nPoints)
ElemGCS Coordinates of the points along the beam in GCS (nPoints * 3)
SdiagrGCS Coordinates of the stress with respect to the beam in GCS
(nValues * 3)
ElemExtGCS Coordinates of the points with extreme values in GCS (nValues * 3)
ExtremaGCS Coordinates of the extreme values with respect to the beam in GCS
(nValues * 3)
Extrema Extreme values (nValues * 1)

See also PLOTSTRESS, SDIAGRLCS_BEAM, SDIAGRGCS_TRUSS.

254 FUNCTIONS — ALPHABETICAL LIST

sdiagrgcs shell2
SDIAGRGCS_SHELL2 Return matrices to plot the stresses in a SHELL2 element.

[ElemGCS,SdiagrGCS,ElemExtGCS,ExtremaGCS,Extrema]
= sdiagrgcs_shell2(ftype,Forces,Node,Section,Material,DLoad,Points)
[ElemGCS,SdiagrGCS,ElemExtGCS,ExtremaGCS,Extrema]
= sdiagrgcs_shell2(ftype,Forces,Node,Section,Material,DLoad)
returns the coordinates of the points along the SHELL2 in the global
coordinate system and the coordinates of the stresses with respect to the element
in the global coordinate system. These can be added in order to plot the
stresses: ElemGCS+SdiagrGCS. The coordinates of the points with extreme values
and the coordinates of the extreme values with respect to the element are given
as well and can be similarly added: ElemExtGCS+ExtremaGCS. Extrema is the
list with the correspondig extreme values.

ftype ’sNphi’ Stress due to normal force in meridional direction

’sMphiT’ Stress at the top due to bending moment in
meridional direction
’sMphiB’ Stress at the bottom due to bending moment in
meridional direction
’sNtheta’ Stress due to normal force in circumferential direction
’sMthetaT’ Stress at the top due to bending moment in
circumferential direction
’sMthetaB’ Stress at the bottom due to bending moment in
circumferential direction
Forces Element forces in LCS (beam convention) [N; Vy; 0; 0; 0; Mz] (12 * 1)
Node Node definitions [x y z] (3 * 3)
DLoad Distributed loads [n1globalX; n1globalY; n1globalZ; ...] (6 * 1)
Points Points in the local coordinate system (1 * nPoints)
ElemGCS Coordinates of the points along the element in GCS (nPoints * 3)
FdiagrGCS Coordinates of the force with respect to the element in GCS (nValues * 3)
ElemExtGCS Coordinates of the points with extreme values in GCS (nValues * 3)
ExtremaGCS Coordinates of the extreme values with respect to the element in GCS
(nValues * 3)
Extrema Extreme values (nValues * 1)
FUNCTIONS — ALPHABETICAL LIST 255

sdiagrgcs truss
SDIAGRGCS_TRUSS Return matrices to plot the stresses in a truss element.

[ElemGCS,SdiagrGCS,ElemExtGCS,ExtremaGCS,Extrema]
= sdiagrgcs_truss(stype,Forces,Node,Section,[],[],Points)
[ElemGCS,SdiagrGCS,ElemExtGCS,ExtremaGCS,Extrema]
= sdiagrgcs_truss(stype,Forces,Node,Section)
returns the coordinates of the points along the truss in the global
coordinate system and the coordinates of the stresses with respect to the truss
in the global coordinate system. These can be added in order to plot the
stresses: ElemGCS+SdiagrGCS. The coordinates of the points with extreme values
and the coordinates of the extreme values with respect to the truss are given
as well and can be similarly added: ElemExtGCS+ExtremaGCS. Extrema is the
list with the corresponding extreme values.

stype ’snorm’ Normal stress due to normal force

Forces Element forces in LCS [N; 0; 0; 0; 0; 0](12 * 1)
Node Node definitions [x y z] (3 * 3)
Section Section definition [A ky kz Ixx Iyy Izz yt yb zt zb]
Points Points in the local coordinate system (1 * nPoints)
ElemGCS Coordinates of the points along the truss in GCS (nPoints * 3)
SdiagrGCS Coordinates of the force with respect to the truss in GCS
(nValues * 3)
ElemExtGCS Coordinates of the points with extreme values in GCS (nValues * 3)
ExtremaGCS Coordinates of the extreme values with respect to the truss in GCS
(nValues * 3)
Extrema Extreme values (nValues * 1)

See also PLOTSTRESS, SDIAGRGCS_BEAM.

256 FUNCTIONS — ALPHABETICAL LIST

sdiagrlcs beam
SDIAGRLCS_BEAM Stress diagram for a beam element in LCS.

[SdiagrLCS,loc,Extrema] = sdiagrlcs_beam(ftype,Forces,DLoadLCS,L,Points)
computes the stresses at the specified points. The extreme values are
analytically determined.

stype ’snorm’ Normal stress due to normal force

’smomyt’ Normal stress due to bending moment
around the local y-direction at the top
’smomyb’ Normal stress due to bending moment
around the local y-direction at the bottom
’smomzt’ Normal stress due to bending moment
around the local z-direction at the top
’smomzb’ Normal stress due to bending moment
around the local z-direction at the bottom
’smax’ Maximal normal stress (normal force and bending moment)
’smin’ Minimal normal stress (normal force and bending moment)
Forces Element forces in LCS (beam convention) [N; Vy; Vz; T; My; Mz](12 * 1)
DLoadLCS Distributed loads in LCS [n1localX; n1localY; n1localZ; ...](6 * 1)
Points Points in the local coordinate system (1 * nPoints)
Section Section definition [A ky kz Ixx Iyy Izz yt yb zt zb]
SdiagrLCS Stresses at the points (1 * nPoints)
loc Locations of the extreme values (nValues * 1)
Extrema Extreme values (nValues * 1)

See also SDIAGRGCS_BEAM.

FUNCTIONS — ALPHABETICAL LIST 257

selcs plane3
SELCS_PLANE3 Compute the element stresses for a plane3 element.

[SeLCS] = selcs_plane3(Node,Section,Material,UeGCS,Options)
computes the element stresses in the
local coordinate system for the plane3 element.

Node Node definitions [x y z] (4 * 3)

Section Section definition [h] (only used in plane stress)
Material Material definition [E nu rho]
UeLCS Displacements (6 * nSteps)
Options Element options {Option1 Option2 ...}
SeLCS Element stresses in LCS in corner nodes IJKL
(9 * nTimeSteps) [sxx syy sxy]

See also ELEMSTRESS, SE_PLANE3.

258 FUNCTIONS — ALPHABETICAL LIST

selcs plane4
SELCS_PLANE4 Compute the element stresses for a plane4 element.

[SeLCS] = selcs_plane4(Node,Section,Material,UeGCS,Options)
computes the element stresses in the
local coordinate system for the plane4 element.

Node Node definitions [x y z] (4 * 3)

Section Section definition [h] (only used in plane stress)
Material Material definition [E nu rho]
UeLCS Displacements (8 * nSteps)
Options Element options {Option1 Option2 ...}
SeLCS Element stresses in LCS in corner nodes IJKL
(12 * nTimeSteps) [sxx syy sxy] for plane stress / plane strain problems
(16 * nTimeSteps) [sxx stheta syy sxy] for axisymmetric problems

See also ELEMSTRESS, SE_PLANE4.

FUNCTIONS — ALPHABETICAL LIST 259

selcs plane6
SELCS_PLANE6 Compute the element stresses for a plane6 element.

[SeLCS] = selcs_plane6(Node,Section,Material,UeGCS,Options)
computes the element stresses in the
local coordinate system for the plane6 element.

Node Node definitions [x y z] (6 * 3)

Nodes should have the following order:
3
| \
6 5
| \
1--4--2
Section Section definition [h] (only used in plane stress)
Material Material definition [E nu rho]
UeLCS Displacements (6 * nSteps)
Options Element options {Option1 Option2 ...}
SeLCS Element stresses in LCS in corner nodes IJKL
(9 * nTimeSteps) [sxx syy sxy]

See also ELEMSTRESS, SE_PLANE6.

260 FUNCTIONS — ALPHABETICAL LIST

selcs plane8
SELCS_PLANE8 Compute the element stresses for a plane4 element.

[SeLCS] = selcs_plane8(Node,Section,Material,UeGCS,Options)
computes the element stresses in the
local coordinate system for the plane8 element.

Node Node definitions [x y z] (4 * 3)

Section Section definition [h] (only used in plane stress)
Material Material definition [E nu rho]
UeLCS Displacements (8 * nSteps)
Options Element options {Option1 Option2 ...}
SeLCS Element stresses in LCS in corner nodes IJKL
(12 * nTimeSteps) [sxx syy sxy]

See also ELEMSTRESS, SE_PLANE8.

FUNCTIONS — ALPHABETICAL LIST 261

selcs shell4
SELCS_SHELL4 Compute the element stresses for a shell4 element.

[SeLCS] = selcs_shell4(Node,Section,Material,UeGCS,Options)
computes the element stresses in the global and the
local coordinate system for the shell4 element.

Node Node definitions [x y z] (4 * 3)

h Shell thickness
E Young’s modulus
nu Poisson coefficient
rho Mass density
UeLCS Displacements (24 * nTimeSteps)
Options Element options {Option1 Option2 ...}
SeLCS Element stresses in LCS in corner nodes IJKL and
at top/mid/bot of shell (72 * nTimeSteps)
[sxx syy szz sxy syz sxz]

See also ELEMSTRESS, SE_SHELL4.

262 FUNCTIONS — ALPHABETICAL LIST

selectdof
SELECTDOF Select degrees of freedom.

L=selectdof(DOF,seldof)
[L,I]=selectdof(DOF,seldof)
L=selectdof(DOF,seldof,’Ordering’,ordering)
creates the matrix to extract degrees of freedom from the global degrees of
freedom by matrix multiplication.

DOF Degrees of freedom (nDOF * 1)

seldof Selected DOF labels (kDOF * 1)
L Selection matrix (kDOF * nDOF)
I Index vector (kDOF * 1)
ordering ’seldof’,’DOF’ or ’sorted’ Default: ’seldof’
Ordering of L and I similar as seldof, DOF or sorted
FUNCTIONS — ALPHABETICAL LIST 263

selectnode
SELECTNODE Select nodes by location.

Nodesel=selectnode(Nodes,x,y,z)
Nodesel=selectnode(Nodes,xmin,ymin,zmin,xmax,ymax,zmax)
selects nodes by location.

Nodes Node definitions [NodID x y z]

Nodesel Node definitions of the selected nodes
264 FUNCTIONS — ALPHABETICAL LIST

se plane3
SE_PLANE3 Compute the element stresses for a plane3 element.

[SeGCS,SeLCS,vLCS] = se_plane3(Node,Section,Material,UeGCS,Options,GCS)
[SeGCS,SeLCS] = se_plane3(Node,Section,Material,UeGCS,Options,GCS)
SeGCS = se_plane3(Node,Section,Material,UeGCS,Options,GCS)
computes the element stresses in the global and the
local coordinate system for the shell3 element.

Node Node definitions [x y z] (3 * 3)

Nodes should have the following order:
3
| \
1--2
Section Section definition [h] (only used in plane stress)
Material Material definition [E nu rho]
UeGCS Displacements (8 * nTimeSteps)
Options Element options {Option1 Option2 ...}
GCS Global coordinate system in which stresses are returned
’cart’|’cyl’
SeGCS Element stresses in GCS in corner nodes IJKL
18 = 6 stress comp. * 3 nodes (18 * nTimeSteps)
[sxx syy szz sxy syz sxz]
SeLCS Element stresses in LCS in corner nodes IJKL
18 = 6 stress comp. * 3 nodes (18 * nTimeSteps)
[sxx syy szz sxy syz sxz]
vLCS Unit vectors of LCS (1 * 9)

See also ELEMSTRESS, SE_SHELL8.

FUNCTIONS — ALPHABETICAL LIST 265

se plane4
SE_PLANE4 Compute the element stresses for a plane4 element.

[SeGCS,SeLCS,vLCS] = se_plane4(Node,Section,Material,UeGCS,Options,GCS)
[SeGCS,SeLCS] = se_plane4(Node,Section,Material,UeGCS,Options,GCS)
SeGCS = se_plane4(Node,Section,Material,UeGCS,Options,GCS)
computes the element stresses in the global and the
local coordinate system for the shell4 element.

Node Node definitions [x y z] (4 * 3)

Nodes should have the following order:
4---3
| |
1---2
Section Section definition [h] (only used in plane stress)
Material Material definition [E nu rho]
UeGCS Displacements (8 * nTimeSteps)
Options Element options {Option1 Option2 ...}
GCS Global coordinate system in which stresses are returned
’cart’|’cyl’
SeGCS Element stresses in GCS in corner nodes IJKL
24 = 6 stress comp. * 4 nodes (24 * nTimeSteps)
[sxx syy szz sxy syz sxz]
SeLCS Element stresses in LCS in corner nodes IJKL
24 = 6 stress comp. * 4 nodes (24 * nTimeSteps)
[sxx syy szz sxy syz sxz]
vLCS Unit vectors of LCS (1 * 9)

See also ELEMSTRESS, SE_SHELL8.

266 FUNCTIONS — ALPHABETICAL LIST

se plane6
SE_PLANE6 Compute the element stresses for a plane6 element.

[SeGCS,SeLCS,vLCS] = se_plane6(Node,Section,Material,UeGCS,Options,GCS)
[SeGCS,SeLCS] = se_plane6(Node,Section,Material,UeGCS,Options,GCS)
SeGCS = se_plane6(Node,Section,Material,UeGCS,Options,GCS)
computes the element stresses in the global and the
local coordinate system for the plane6 element.

Node Node definitions [x y z] (8 * 3)

Nodes should have the following order:
3
| \
6 5
| \
1--4--2

Section Section definition [h] (only used in plane stress)

Material Material definition [E nu rho]
UeGCS Displacements (8 * nTimeSteps)
Options Element options {Option1 Option2 ...}
GCS Global coordinate system in which stresses are returned
’cart’|’cyl’
SeGCS Element stresses in GCS in corner nodes IJKL
48 = 6 stress comp. * 8 nodes (24 * nTimeSteps)
[sxx syy szz sxy syz sxz]
SeLCS Element stresses in LCS in corner nodes IJKL
48 = 6 stress comp. * 8 nodes (24 * nTimeSteps)
[sxx syy szz sxy syz sxz]
vLCS Unit vectors of LCS (1 * 9)

See also ELEMSTRESS, SE_PLANE8.

FUNCTIONS — ALPHABETICAL LIST 267

se plane8
SE_PLANE8 Compute the element stresses for a plane8 element.

[SeGCS,SeLCS,vLCS] = se_plane8(Node,Section,Material,UeGCS,Options,GCS)
[SeGCS,SeLCS] = se_plane8(Node,Section,Material,UeGCS,Options,GCS)
SeGCS = se_plane8(Node,Section,Material,UeGCS,Options,GCS)
computes the element stresses in the global and the
local coordinate system for the shell8 element.

Node Node definitions [x y z] (8 * 3)

Nodes should have the following order:
4----7----3
| |
8 6
| |
1----5----2
Section Section definition [h] (only used in plane stress)
Material Material definition [E nu rho]
UeGCS Displacements (8 * nTimeSteps)
Options Element options {Option1 Option2 ...}
GCS Global coordinate system in which stresses are returned
’cart’|’cyl’
SeGCS Element stresses in GCS in corner nodes IJKL
48 = 6 stress comp. * 8 nodes (24 * nTimeSteps)
[sxx syy szz sxy syz sxz]
SeLCS Element stresses in LCS in corner nodes IJKL
48 = 6 stress comp. * 8 nodes (24 * nTimeSteps)
[sxx syy szz sxy syz sxz]
vLCS Unit vectors of LCS (1 * 9)

See also ELEMSTRESS, SE_SHELL8.

268 FUNCTIONS — ALPHABETICAL LIST

se shell4
SE_SHELL4 Compute the element stresses for a shell4 element.

[SeGCS,SeLCS,vLCS] = se_shell4(Node,Section,Material,UeGCS,Options,GCS)
[SeGCS,SeLCS] = se_shell4(Node,Section,Material,UeGCS,Options,GCS)
SeGCS = se_shell4(Node,Section,Material,UeGCS,Options,GCS)
computes the element stresses in the global and the
local coordinate system for the shell4 element.

Node Node definitions [x y z] (4 * 3)

Nodes should have the following order:
Section Section definition [h]
Material Material definition [E nu rho]
UeGCS Displacements (24 * nTimeSteps)
Options Element options {Option1 Option2 ...}
GCS Global coordinate system in which stresses are returned
’cart’|’cyl’|’sph’
SeGCS Element stresses in GCS in corner nodes IJKL and
at top/mid/bot of shell (72 * nTimeSteps)
72 = 6 stress comp. * 4 nodes * 3 locations
[sxx syy szz sxy syz sxz]
SeLCS Element stresses in LCS in corner nodes IJKL and
at top/mid/bot of shell (72 * nTimeSteps)
[sxx syy szz sxy syz sxz]
vLCS Unit vectors of LCS (1 * 9)

See also ELEMSTRESS, SE_SHELL8.

FUNCTIONS — ALPHABETICAL LIST 269

se shell6
SE_SHELL6 Compute the element stresses for a shell6 element.

[SeGCS,SeLCS,vLCS] = se_shell6(Node,Section,Material,UeGCS,Options,gcs)
[SeGCS,SeLCS] = se_shell6(Node,Section,Material,UeGCS,Options,gcs)
SeGCS = se_shell6(Node,Section,Material,UeGCS,Options,gcs)
computes the element stresses in the global and the
local coordinate system for the shell6 element.

Node Node definitions [x y z] (6 * 3)

Nodes should have the following order:
3
| \
6 5
| \
1--4--2

Section Section definition [h] or [h1 h2 h3]

(uniform thickness or defined in corner nodes(1,2,3))
Material Material definition [E nu rho] or [Exx Eyy nuxy muxy muyz muzx theta rho]
UeGCS Displacements (36 * nTimeSteps)
Options Element options struct. Fields:
-LCSType: determine the reference local element
coordinate system. Values:
’element’ (default) or ’global’
-MatType: ’isotropic’ (default) or ’orthotropic’
-Offset: nodal offset from shell midplane. Values:
’top’, ’mid’ (default), ’bot’ or numerical value
GCS Global coordinate system in which stresses are returned
’cart’|’cyl’|’sph’
SeGCS Element stresses in GCS in corner nodes IJKL and
at top/mid/bot of shell (72 * nTimeSteps)
72 = 6 stress comp. * 4 nodes * 3 locations
(in a triangular element the fourth node is zero)
[sxx syy szz sxy syz sxz]
SeLCS Element stresses in LCS in corner nodes IJKL and
at top/mid/bot of shell (54 * nTimeSteps)
[sxx syy szz sxy syz sxz]
vLCS Unit vectors of LCS (3 * 3)

See also ELEMSTRESS, SE_SHELL4.

270 FUNCTIONS — ALPHABETICAL LIST

se shell8
SE_SHELL8 Compute the element stresses for a shell8 element.

[SeGCS,SeLCS,vLCS] = se_shell8(Node,Section,Material,UeGCS,Options,gcs)
[SeGCS,SeLCS] = se_shell8(Node,Section,Material,UeGCS,Options,gcs)
SeGCS = se_shell8(Node,Section,Material,UeGCS,Options,gcs)
computes the element stresses in the global and the
local coordinate system for the shell8 element.

Node Node definitions [x y z] (8 * 3)

Nodes should have the following order:
4----7----3
| |
8 6
| |
1----5----2

Section Section definition [h] or [h1 h2 h3 h4]

(uniform thickness or defined in corner nodes(1,2,3,4))
Material Material definition [E nu rho] or [Exx Eyy nuxy muxy muyz muzx theta rho]
UeGCS Displacements (48 * nTimeSteps)
Options Element options struct. Fields:
-LCSType: determine the reference local element
coordinate system. Values:
’element’ (default) or ’global’
-MatType: ’isotropic’ (default) or ’orthotropic’
-Offset: nodal offset from shell midplane. Values:
’top’, ’mid’ (default), ’bot’ or numerical value
GCS Global coordinate system in which stresses are returned
’cart’|’cyl’|’sph’
SeGCS Element stresses in GCS in corner nodes IJKL and
at top/mid/bot of shell (72 * nTimeSteps)
72 = 6 stress comp. * 4 nodes * 3 locations
[sxx syy szz sxy syz sxz]
SeLCS Element stresses in LCS in corner nodes IJKL and
at top/mid/bot of shell (72 * nTimeSteps)
[sxx syy szz sxy syz sxz]
vLCS Unit vectors of LCS (3 * 3)

See also ELEMSTRESS, SE_SHELL4.

FUNCTIONS — ALPHABETICAL LIST 271

se solid20
SE_SOLID20 Compute the element stresses for a solid20 element.

[SeGCS,SeLCS,vLCS] = se_solid20(Node,Section,Material,UeGCS,Options,gcs)
[SeGCS,SeLCS] = se_solid20(Node,Section,Material,UeGCS,Options,gcs)
SeGCS = se_solid20(Node,Section,Material,UeGCS,Options,gcs)
computes the element stresses in the global and the
local coordinate system for the solid20 element.

Node Node definitions [x y z] (20 * 3)

Nodes should have the following order:
8---15----7
/| /|
16 | 14 |
/ 20 / 19
/ | / |
5---13----6 |
| 4--11|----3
| / | /
17 12 18 10
| / | /
|/ |/
1----9----2
272 FUNCTIONS — ALPHABETICAL LIST

se solid8
SE_SOLID8 Compute the element stresses for a solid8 element.

[SeGCS,SeLCS,vLCS] = se_solid8(Node,Section,Material,UeGCS,Options,gcs)
[SeGCS,SeLCS] = se_solid8(Node,Section,Material,UeGCS,Options,gcs)
SeGCS = se_solid8(Node,Section,Material,UeGCS,Options,gcs)
computes the element stresses in the global and the
local coordinate system for the solid8 element.

Node Node definitions [x y z] (8 * 3)

Nodes should have the following order:
8---------7
/| /|
/ | / |
/ | / |
5---------6 |
| 4-----|---3
| / | /
| / | /
|/ |/
1---------2

Section Section definition []

Material Material definition [E nu rho]
UeGCS Displacements (48 * nTimeSteps)
Options Element options struct. Fields: []
GCS Global coordinate system in which stresses are returned
’cart’|’cyl’|’sph’
SeGCS Element stresses in GCS in nodes (48 * nTimeSteps)
48 = 6 stress comp. * 8 nodes
[sxx syy szz sxy syz sxz]
SeGCS Element stresses in GCS in nodes (48 * nTimeSteps)
48 = 6 stress comp. * 8 nodes
[sxx syy szz sxy syz sxz]
vLCS Unit vectors of LCS (3 * 3)

See also ELEMSTRESS, SE_SHELL4.

FUNCTIONS — ALPHABETICAL LIST 273

se truss
e_truss is a function.
[SeGCS, SeLCS, vLCS] = se_truss(Node, Section, Material, UeGCS, Options, gcs)
274 FUNCTIONS — ALPHABETICAL LIST

sh qs4
SH_QS4 Shape functions for a quadrilateral serendipity element with 4
nodes.

[Ni,dN_dxi,dN_deta] = sh_qs4(xi,eta) returns the shape functions and

its derivatives to the natural coordinates in the point (xi,eta).

xi Natural coordinate (scalar)

eta Natural coordinate (scalar)
Ni Shape functions in point (xi,eta) (4 * 1)
dN_dxi Derivative of Ni to xi (4 * 1)
dN_deta Derivative of Ni to eta (4 * 1)

See also KELCS_SHELL4.

FUNCTIONS — ALPHABETICAL LIST 275

sh qs8
SH_QS8 Shape functions for an 8 node quadrilateral serendipity element.

[Ni,dN_dxi,dN_deta] = sh_qs8(xi,eta) returns the shape functions and

its derivatives with respect to the natural coordinates in the point (xi,eta).

xi natural coordinate (scalar)

eta natural coordinate (scalar)
Ni shape functions in point (xi,eta) (8 * 1)
dN_dxi derivative of Ni to xi (8 * 1)
dN_deta derivative of Ni to eta (8 * 1)

see also KE_SHELL8.

276 FUNCTIONS — ALPHABETICAL LIST

sh t
SH_T Shape functions for a triangular plate element.

[Ni] = sh_t(L,b,c) returns the shape functions and

its derivatives in point L.

L Area coordinates [L1,L2,L3] (3 * 1)

b Geometrical property of the triangle (see ke_dkt) (3 * 1)
c Geometrical property of the triangle (3 * 1)
Ni Shape functions and derivatives (9 * 1)
in point L

These shape functions are used to determine the mass matrix of a

triangular plate element.

See also KE_DKT.

FUNCTIONS — ALPHABETICAL LIST 277

sh t10
SH_T10 Shape functions for a 10 node triangular element.

[Ni,dN_dxi,dN_deta] = sh_t10(xi,eta) returns the shape functions and

its derivatives with respect to the natural coordinates in the point (xi,eta)

xi natural coordinate (scalar)

eta natural coordinate (scalar)
Ni shape functions in point (xi,eta) (10 * 1)
dN_dxi derivative of Ni to xi (10 * 1)
dN_deta derivative of Ni to eta (10 * 1)

The nodes have the following order:

see also SH_T3, SH_T6, SH_T15.

278 FUNCTIONS — ALPHABETICAL LIST

sh t15
SH_T15 Shape functions for a 15 node triangular element.

[Ni,dN_dxi,dN_deta] = sh_t15(xi,eta) returns the shape functions and

its derivatives with respect to the natural coordinates in the point (xi,eta)*

xi natural coordinate (scalar)

eta natural coordinate (scalar)
Ni shape functions in point (xi,eta) (15 * 1)
dN_dxi derivative of Ni to xi (15 * 1)
dN_deta derivative of Ni to eta (15 * 1)

The nodes have the following order:

see also SH_T3, SH_T6, SH_T15.

FUNCTIONS — ALPHABETICAL LIST 279

sh t3
SH_T3 Shape functions for a 3 node triangular element.

[Ni,dN_dxi,dN_deta] = sh_t3(xi,eta) returns the shape functions and

its derivatives with respect to the natural coordinates in the point (xi,eta).

xi natural coordinate (scalar)

eta natural coordinate (scalar)
Ni shape functions in point (xi,eta) (3 * 1)
dN_dxi derivative of Ni to xi (3 * 1)
dN_deta derivative of Ni to eta (3 * 1)
280 FUNCTIONS — ALPHABETICAL LIST

sh t6
SH_T6 Shape functions for an 6 node triangular element.

[Ni,dN_dxi,dN_deta] = sh_t6(xi,eta) returns the shape functions and

its derivatives with respect to the natural coordinates in the point (xi,eta).

xi natural coordinate (scalar)

eta natural coordinate (scalar)
Ni shape functions in point (xi,eta) (6 * 1)
dN_dxi derivative of Ni to xi (6 * 1)
dN_deta derivative of Ni to eta (6 * 1)

see also KE_SHELL6.

FUNCTIONS — ALPHABETICAL LIST 281

sh vs20
SH_VS20 Shape functions for a volume serendipity element with 20 nodes.

[Ni,dNi_dxi,dNi_deta,dNi_dzeta] = sh_vs20(xi,eta,zeta)
returns the shape functions and its derivatives to the natural coordinates
in the point (xi,eta,zeta).

xi Natural coordinate (scalar)

eta Natural coordinate (scalar)
zeta Natural coordinate (scalar)
Ni Shape functions in point (xi,eta) (20 * 1)
dN_dxi Derivative of Ni to xi (20 * 1)
dN_deta Derivative of Ni to eta (20 * 1)
dN_dzeta Derivative of Ni to zeta (20 * 1)

See also KE_SOLID20.

282 FUNCTIONS — ALPHABETICAL LIST

sh vs8
SH_VS8 Shape functions for a volume serendipity element with 8 nodes.

[Ni,dNi_dxi,dNi_deta,dNi_dzeta] = sh_vs8(xi,eta,zeta)
returns the shape functions and its derivatives to the natural coordinates
in the point (xi,eta,zeta).

xi Natural coordinate (scalar)

eta Natural coordinate (scalar)
zeta Natural coordinate (scalar)
Ni Shape functions in point (xi,eta) (8 * 1)
dN_dxi Derivative of Ni to xi (8 * 1)
dN_deta Derivative of Ni to eta (8 * 1)
dN_dzeta Derivative of Ni to zeta (8 * 1)

See also KE_SOLID8.

FUNCTIONS — ALPHABETICAL LIST 283

size beam
SIZE_BEAM Compute beam element size (length).

S = SIZE_BEAM(Node) computes the element size (length) of a two node

beam element.

[S,dSdx] = SIZE_BEAM(Node,dNodedx) additionally computes the

derivatives of the element size with respect to the design variables x.

Node Node definitions [x y z] (3 * 3)

dNodedx Node definitions derivatives (SIZE(Node) * nVar)
S Element size
dSdx Element size derivatives

See also ELEMSIZES, ELEMVOLUMES, SIZE_TRUSS.

284 FUNCTIONS — ALPHABETICAL LIST

size plane6
size_plane6 Compute plane6 element size (area).

s = size_plane6(NodeNum) computes the size (area) of a plane6 element.

Node Node definitions [x y z] (6 * 3)

S Element size
FUNCTIONS — ALPHABETICAL LIST 285

size solid10
size_solid10 Compute solid10 element size (volume).

S = size_solid10(NodeNum) computes the size of a solid10 element.

Node Node definitions [x y z] (10 * 3)

S Element size
286 FUNCTIONS — ALPHABETICAL LIST

size solid4
size_solid4 Compute solid4 element size (volume).

s = size_solid4(NodeNum) computes the size (volume) of a solid4 element.

Node Node definitions [x y z] (4 * 3)

S Element size
FUNCTIONS — ALPHABETICAL LIST 287

size truss
SIZE_TRUSS Compute truss element size (length).

S = SIZE_TRUSS(Node) computes the element size (length) of a two node

truss element.

[S,dSdx] = SIZE_TRUSS(Node,dNodedx) additionally computes the

derivatives of the element size with respect to the design variables x.

Node Node definitions [x y z] (3 * 3)

dNodedx Node definitions derivatives (SIZE(Node) * nVar)
S Element size
dSdx Element size derivatives

See also ELEMSIZES, ELEMVOLUMES, SIZE_BEAM.

288 FUNCTIONS — ALPHABETICAL LIST

tconstr
TCONSTR Return matrices to apply constraint equations.

[T,Q0,MasterDOF]=tconstr(Constr,DOF)
returns matrices to apply constraint equations to the stiffness and mass
matrix and the load vector: Kr=T.’*K*T, Mr=T.’*M*T and Fr=T.’*(F-K*Q0).
The original displacement vector is computed using U=T*Ur+Q0.

Constr Constraint equation:

Constant=CoefS*SlaveDOF+CoefM1*MasterDOF1+CoefM2*MasterDOF2+...
[Constant CoefS SlaveDOF CoefM1 MasterDOF1 CoefM2 MasterDOF2 ...]
DOF Degrees of freedom (nDOF * 1)
FUNCTIONS — ALPHABETICAL LIST 289

tloads beam
TLOADS_BEAM Equivalent nodal forces for a beam element in the GCS.

F = tloads_beam(TLoad,Node,Section,Material)
computes the equivalent nodal forces of a temperature load
(in the global coordinate system).

TLoad Temperature loads [dTm; dTy; dTz] (3 * 1)

Node Node definitions [x y z] (2 * 3)
Section Section definitions [A ky kz Ixx Iyy Izz yt yb zt zb]
Material Material definitions [E nu rho alpha]
F Load vector (12 * 1)

See also ELEMTLOADS, TLOADS_TRUSS.

290 FUNCTIONS — ALPHABETICAL LIST

tloads truss
TLOADS_TRUSS Equivalent nodal forces for a truss element in the GCS.

F = tloads_truss(TLoad,Node,Section,Material)
computes the equivalent nodal forces of a temperature load
(in the global coordinate system).

TLoad Temperature loads [n1globalX; n1globalY; n1globalZ; ...]

(6 * 1)
Node Node definition [x y z] (2 * 3)
Section Section definition [A ...]
Material Material definition [E nu rho alpha]
F Load vector (6 * 1)

See also ELEMTLOADS, TLOADS_BEAM.

FUNCTIONS — ALPHABETICAL LIST 291

trans beam
TRANS_BEAM Transform coordinate system for a beam element.

t = TRANS_BEAM(Node)
computes the transformation matrix between the local and the global
coordinate system for the beam element.
[t,dtdx] = TRANS_BEAM(Node,dNodedx)
additionally computes the derivatives of the transformation matrix
with respect to the design variables x.

Node Node definitions [x y z] (3 * 3)

dNodedx Node definitions derivatives (SIZE(Node) * nVar)
t Transformation matrix (3 * 3)
dtdx Transformation matrix derivatives (3 * 3 * nVar)

See also KE_BEAM, TRANS_TRUSS.

292 FUNCTIONS — ALPHABETICAL LIST

trans shell2
TRANS_BEAM Transform coordinate system for a beam element.

t = trans_beam(Node)
computes the transformation matrix between the local and the global
coordinate system for the SHELL2 element.

Node Node definitions [x y z] (3 * 3)

t Transformation matrix (3 * 3)

See also KE_BEAM, TRANS_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 293

trans shell4
TRANS_SHELL4 Transform coordinate system for a shell4 element.

[t,Node_lc,W] = trans_shell4(Node)
[t,Node_lc] = trans_shell4(Node)
t = trans_shell4(Node)
computes the transformation matrix between the local and the global
coordinate system and the correction matrix for non-coplanar nodes
for the shell4 element.

Node Node definitions [x y z] (4 * 3)

t Transformation matrix (3 * 3)
Node_lc Nodes in LCS [x y z] (4 * 3)
W Correction matrix for warped elements
(24 * 24)

See also KE_BEAM, TRANS_TRUSS.

294 FUNCTIONS — ALPHABETICAL LIST

trans shell8
TRANS_SHELL8 Transform coordinate system of a shell8 element.

t = trans_shell8(Node)
t = trans_shell8(Node,Options)
computes the transformation matrix between the local and the global
coordinate system for stress computations.

Node Node definitions [x y z] (8 * 3)

t Transformation matrix (3 * 3)
Options Element options struct. Fields:
-LCSType: determine the reference local element
coordinate system. Values:
’element’ (default) or ’global’

See also SE_SHELL8, TRANS_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 295

trans solid20
TRANS_SOLID20 Transform coordinate system of a solid8 element.

t = trans_solid20(Node)
t = trans_solid20(Node,Options)
computes the transformation matrix between the local and the global
coordinate system for stress computations.

Node Node definitions [x y z] (20 * 3)

t Transformation matrix (3 * 3)

See also SE_SOLID20, TRANS_TRUSS.

296 FUNCTIONS — ALPHABETICAL LIST

trans solid8
TRANS_SOLID8 Transform coordinate system of a solid8 element.

t = trans_solid8(Node)
t = trans_solid8(Node,Options)
computes the transformation matrix between the local and the global
coordinate system for stress computations.

Node Node definitions [x y z] (8 * 3)

t Transformation matrix (3 * 3)

See also SE_SOLID8, TRANS_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 297

trans truss
TRANS_TRUSS Transform coordinate system for a truss element.

t = TRANS_TRUSS(Node)
computes the transformation matrix between the local and the global
coordinate system for the truss element.
[t,dtdx] = TRANS_TRUSS(Node,dNodedx)
additionally computes the derivatives of the transformation matrix
with respect to the design variables x.

Node Node definitions [x y z] (2 * 3)

dNodedx Node definitions derivatives (SIZE(Node) * nVar)
t Transformation matrix (3 * 3)
dtdx Transformation matrix derivatives (3 * 3 * nVar)

See also KE_TRUSS, TRANS_BEAM.

298 FUNCTIONS — ALPHABETICAL LIST

udiagrgcs
UDIAGRGCS Return displacement diagrams in GCS

[UxdiagrGCS,UydiagrGCS,UzdiagrGCS] = UDIAGRGCS(Nodes,Elements,Types,DOF,U,DLoads,
Sections,Materials,Points)
[UxdiagrGCS,UydiagrGCS,UzdiagrGCS] = UDIAGRGCS(Nodes,Elements,Types,DOF,U,DLoads,
Sections,Materials)
[UxdiagrGCS,UydiagrGCS,UzdiagrGCS] = UDIAGRGCS(Nodes,Elements,Types,DOF,U,[],
Sections,Materials)
[UxdiagrGCS,UydiagrGCS,UzdiagrGCS] = UDIAGRGCS(Nodes,Elements,Types,DOF,U)
computes the displacements of the interpolation points after
deformation in the global (algebraic) coordinate system. If DLoads,
Sections and Materials are supplied, the displacements that occur
due to distributed loads if all nodes are fixed, are superimposed.

[UxdiagrGCS,UydiagrGCS,UzdiagrGCS,dUxdiagrGCSdx,dUydiagrGCSdx,dUzdiagrGCSdx]
= UDIAGRGCS(Nodes,Elements,Types,DOF,U,DLoads,Sections,Materials,Points,
dNodesdx,dUdx,dDLoadsdx,dSectionsdx)
additionally computes the derivatives of the displacement values
with respect to the design variables x.

Nodes Node definitions [NodID x y z]

Elements Element definitions [EltID TypID SecID MatID n1 n2 ...]
Types Element type definitions {TypID EltName Option1 ... }
DOF Degrees of freedom (nDOF * 1)
U Displacements (nDOF * 1)
DLoads Distributed loads [EltID n1globalX n1globalY n1globalZ ...]
(use empty array [] when shear deformation (in beam element)
is considered but no DLoads are present)
Sections Section definitions [SecID SecProp1 SecProp2 ...]
Materials Material definitions [MatID MatProp1 MatProp2 ... ]
Points Points in the local coordinate system (1 * nPoints)
dNodesdx Node definitions derivatives (SIZE(Nodes) * nVar)
dUdx Displacements derivatives (SIZE(U) * nVar)
dDLoadsdx Distributed loads derivatives (SIZE(DLoads) * nVar)
UxdiagrGCS x-direction displacement values at the points (nElem * nPoints * nLC)
UydiagrGCS y-direction displacement values at the points (nElem * nPoints * nLC)
UzdiagrGCS z-direction displacement values at the points (nElem * nPoints * nLC)
dUxdiagrGCSdx x-direction displacement values derivatives (nElem * nPoints * nLC * nVar)
dUydiagrGCSdx y-direction displacement values derivatives (nElem * nPoints * nLC * nVar)
dUzdiagrGCSdx z-direction displacement values derivatives (nElem * nPoints * nLC * nVar)

See also PLOTDISP, DISP_TRUSS, DISP_BEAM.

FUNCTIONS — ALPHABETICAL LIST 299

unselectdof
UNSELECTDOF Unselect degrees of freedom.

L=unselectdof(DOF,seldof)
[L,I]=unselectdof(DOF,seldof)
creates the matrix to unselect degrees of freedom from the global degrees of
freedom.

DOF Degrees of freedom (nDOF * 1)

seldof Unselected dof labels (ndof * 1)
L Selection matrix ((nDOF-ndof) * nDOF)
I Index vector ((nDOF-ndof) * 1)

See also SELECTDOF.

clearpage

volume beam
VOLUME_BEAM Compute the volume of a beam element.

V = VOLUME_BEAM(Node,Section) computes the volume of a two-node beam

element.

[V,dVdx] = VOLUME_BEAM(Node,Section,dNodedx,dSectiondx) computes the

volume of a two node beam element, as well as the derivatives of the
volume with respect to the design variables x.

Node Node definitions [x y z] (3 * 3)

Sections Section definitions [SecID SecProp1 SecProp2 ...]
dNodedx Node definitions derivatives (SIZE(Node) * nVar)
dSectionsdx Section definitions derivatives (SIZE(Section) * nVar)
V Element volume (1 * 1)
dVdx Element volume derivatives (nVar * 1)

See also ELEMVOLUMES, VOLUME_TRUSS, ELEMSIZES, SIZE_BEAM.

clearpage

volume truss
VOLUME_TRUSS Compute the volume of a truss element.

V = VOLUME_TRUSS(Node,Section) computes the volume of a two-node truss

element.

[V,dVdx] = VOLUME_TRUSS(Node,Section,dNodedx,dSectiondx) computes the

volume of a two node truss element, as well as the derivatives of the
volume with respect to the design variables x.

Node Node definitions [x y z] (3 * 3)

300 FUNCTIONS — ALPHABETICAL LIST

Sections Section definitions [SecID SecProp1 SecProp2 ...]

dNodedx Node definitions derivatives (SIZE(Node) * nVar)
dSectionsdx Section definitions derivatives (SIZE(Section) * nVar)
V Element volume (1 * 1)
dVdx Element volume derivatives (nVar * 1)

See also ELEMVOLUMES, VOLUME_BEAM, ELEMSIZES, SIZE_TRUSS.

FUNCTIONS — ALPHABETICAL LIST 301

vtrans solid
VTRANS_SOLID Transformation matrix for stress and strain components in matrix (Voigt) notation.

[theta] = vtrans_solid(t)
[theta] = vtrans_solid(t,vtype)
computes the transformation matrix between the local and the global
coordinate system for t stress or strain vector in matrix notation.

t Transformation matrix (3 * 3)
vtype Vector type ’stress’ (default) | ’strain’
theta Stress transformation matrix (6 * 6)

See also TRANS_SOLID8, TRANS_SOLID20.

302 FUNCTIONS — ALPHABETICAL LIST

wilson
WILSON Direct time integration for dynamic systems - Wilson-theta method
[u,v,a,t] = WILSON(M,C,K,dt,p,u1,v1,[alpha delta theta]) applies the
Wilson-theta method for the calculation of the nodal displacements u,
velocities v and accelerations a of the dynamic system with the system
matrices M, C and K due to the excitation p.

M Mass matrix (nDof * nDof)

C Damping matrix (nDof * nDof)
K Stiffness matrix (nDof * nDof)
dt Time step of the integration scheme (1 * 1). Should be small enough
to ensure the stability and the precision of the integration scheme.
p Excitation (nDof * N). p(:,k) corresponds to time point t(k).
u1 Displacements at time point t(1) (nDof * 1). Defaults to zero.
v1 Velocities at time point t(1) (nDof * 1). Defaults to zero.
u Displacements (nDof * N). u(:,k) corresponds to time point t(k).
t Time axis (1 * N), defined as t = [0:N-1] * dt.
Bibliography

[1] K.J. Bathe. Finite Element Procedures. Prentice-Hall, Englewood Cliffs, NJ, second edition, 1996.
[2] A.K. Chopra. Dynamics of structures: theory and applications to earthquake engineering. Prentice-Hall,
Englewood Cliffs, New Jersey, 1995.
[3] R.D. Cook. Finite element modelling for stress analysis. John Wiley and Sons, 1995.

[4] R.D. Cook, D.S. Malkus, M.E. Plesha, and R.J. Witt. Concepts and applications of finite element analysis.
John Wiley and Sons, fourth edition, 2002.
[5] J.S. Przemieniecki. Theory of matrix structural analysis. Dover Publications, New York, NY, 1985.
[6] O.C. Zienkiewicz and R.L. Taylor. The finite element method, Volume 1: the basis. Butterworth-Heinemann,
Oxford, United Kingdom, fifth edition, 2000.
[7] O.C. Zienkiewicz and R.L. Taylor. The finite element method, Volume 2: solid mechanics. Butterworth-
Heinemann, Oxford, United Kingdom, fifth edition, 2000.
[8] O.C. Zienkiewicz and R.L. Taylor. The finite element method, Volume 3: fluid dynamics. Butterworth-
Heinemann, Oxford, United Kingdom, fifth edition, 2000.

[9] O.C. Zienkiewicz, R.L. Taylor, and J.Z. Zhu. The finite element method: its basis and fundamentals. Elsevier
Butterworth-Heinemann, sixth edition, 2005.