MYSTRAN Users Manual

User Manual:

Open the PDF directly: View PDF .
Page Count: 283

Download
Open PDF In Browser	View PDF

Users Reference Manual
For the

MYSTRAN General Purpose Finite Element
Structural Analysis Computer Program
(Nov 2011)

Table of Contents

1 INTRODUCTION

2 GENERAL DESCRIPTION OF INPUT DATA

3 THE FINITE ELEMENT MODEL

3.1 Grid points
3.1.1 Grid point and coordinate system definition
3.1.2 Grid point sequencing
3.1.2.1 Automatic grid point sequencing
3.1.2.2 Manual grid point sequencing

6
6
7
7
7

3.2 Elements
3.2.1 Element connection, property, and material definition
3.2.2 Elastic elements
3.2.2.1 Scalar spring
3.2.2.2 Rod element
3.2.2.3 Bar element
3.2.2.4 Plate elements
3.2.2.5 Solid elements
3.2.3 Rigid elements
3.2.3.1 RBE2 rigid element
3.2.4 RBE3 element
3.2.5 RSPLINE element

8
8
9
9
9
10
11
13
13
13
14
14

3.3 Applied loads
3.3.1 Forces and moments directly applied to grids
3.3.2 Pressure loads on plate elements
3.3.3 Gravity loads
3.3.4 Equivalent loads due to thermal expansion
3.3.5 Equivalent loads due to enforced displacements
3.3.6 Loads due to rigid body rotation about a specified grid (RFORCE)
3.3.7 LOAD Bulk Data entry – combining loads

15
15
15
16
16
16
17
17

17
3.4 Constraints
17
3.4.1 Single point constraints
3.4.1.1 AUTOSPC feature…………………………………………………………………….18
19
3.4.2 Multi point constraints
19
3.4.3 Boundary degrees of freedom in Craig-Bampton analyses
3.5 Mass
3.5.1 Mass density on material entries
3.5.2 Mass per unit length or area of finite elements
3.5.3 Concentrated masses at grids
3.5.4 Model total mass
3.5.5 Mass units

19
19
20
19
20
21

3.6 Displacement set notation

4 MYSTRAN SOLUTION TYPES

4.1 Statics

4.2 Eigenvalues

4.3 Craig-Bampton model generation

Figures

5 REFERENCES

6 DETAILED DESCRIPTION OF INPUT DATA

6.1 File Management

6.2 Executive Control
6.2.1 IN4 Exec Control command
6.2.2 OUTPUT4 Exec Control command

34
35
35

6.3 Case Control
6.3.1 Detailed Description of Case Control Entries
6.3.1.1 BEGIN BULK
6.3.1.2 ACCELERATION
6.3.1.3 DISPLACEMENT
6.3.1.4 ECHO
6.3.1.5 ELDATA
6.3.1.6 ELFORCE
6.3.1.7 ENFORCED
6.3.1.8 ELSTRAIN
6.3.1.9 ELSTRESS
6.3.1.10 FORCE
6.3.1.11 GPFORCES
6.3.1.12 LABEL
6.3.1.13 LOAD
6.3.1.14 MEFFMASS
6.3.1.15 METHOD
6.3.1.16 MPC
6.3.1.17 MPCFORCES
6.3.1.18 MPFACTOR
6.3.1.19 OLOAD
6.3.1.20 SET
6.3.1.21 SPC
6.3.1.22 SPCFORCES
6.3.1.23 STRAIN
6.3.1.24 STRESS
6.3.1.25 SUBCASE
6.3.1.26 SUBTITLE
6.3.1.27 TEMPERATURE
6.3.1.28 TITLE
6.3.1.29 VECTOR

40
41
42
43
44
45
46
48
49
50
51
52
53
54
55
56
57
58
59
60
61
62
63
64
65
66
67
68
69
70
71

6.4 Bulk Data
6.4.1 Detailed Description of Bulk Data Entries
6.4.1.1 ASET

72
81
82

iii

6.4.1.2
6.4.1.3
6.4.1.4
6.4.1.5
6.4.1.6
6.4.1.7
6.4.1.8
6.4.1.9
6.4.1.10
6.4.1.11
6.4.1.12
6.4.1.13
6.4.1.14
6.4.1.15
6.4.1.16
6.4.1.17
6.4.1.18
6.4.1.19
6.4.1.20
6.4.1.21
6.4.1.22
6.4.1.23
6.4.1.24
6.4.1.25
6.4.1.26
6.4.1.27
6.4.1.28
6.4.1.29
6.4.1.30
6.4.1.31
6.4.1.32
6.4.1.33
6.4.1.34
6.4.1.35
6.4.1.36
6.4.1.37
6.4.1.38
6.4.1.39
6.4.1.40
6.4.1.41
6.4.1.42
6.4.1.43
6.4.1.44
6.4.1.45
6.4.1.46
6.4.1.47
6.4.1.48
6.4.1.49
6.4.1.50
6.4.1.51
6.4.1.52
6.4.1.53
6.4.1.54
6.4.1.55
6.4.1.56
6.4.1.57

ASET1
BAROR….
CBAR
CBUSH
CELAS1
CELAS2
CELAS3
CELAS4
CHEXA
CMASS1
CMASS2
CMASS3
CMASS4
CONM2
CONROD
CORD1C
CORD1R
CORD1S
CORD2C
CORD2R
CORD2S
CPENTA
CQUAD4
CQUAD4K
CROD
CSHEAR
CTETRA
CTRIA3
CTRIA3K
CUSERIN
DEBUG
EIGR
EIGRL
FORCE
GRAV
GRDSET
GRID
LOAD
MAT1
MAT2
MAT8
MAT9
MOMENT
MPC
MPCADD
OMIT
OMIT1
PARAM
PARVEC
PARVEC1
PBAR
PBARL
PBUSH
PCOMP
PCOMP1
PELAS

83
84
85
87
89
90
91
92
93
94
95
96
97
98
99
100
101
102
103
104
105
106
107
108
109
110
111
112
113
114
116
121
123
124
125
126
127
128
129
131
133
135
136
137
138
139
140
141
149
150
151
153
157
159
160
161

6.4.1.58
6.4.1.59
6.4.1.60
6.4.1.61
6.4.1.62
6.4.1.63
6.4.1.64
6.4.1.65
6.4.1.66
6.4.1.67
6.4.1.68
6.4.1.69
6.4.1.70
6.4.1.71
6.4.1.72
6.4.1.73
6.4.1.74
6.4.1.75
6.4.1.76
6.4.1.49
6.4.1.78
6.4.1.79
6.4.1.80
6.4.1.81
6.4.1.82

PLOAD2
PLOAD4
PLOTEL
PROD
PSHEAR
PSHELL
PSOLID
PUSERIN
RBE2
RBE3
RFORCE.
RSPLINE
SEQGP
SLOAD
SPC
SPC1
SPCADD
SPOINT
SUPORT
PARAM
TEMPD
TEMPP1
TEMPRB
USET
USET1

162
163
165
166
167
168
170
172
173
174
175
177
178
179
180
181
182
183
184
185
186
187
189
191
192

7 APPENDIX A: MYSTRAN SAMPLE PROBLEM NO. 1

193

8 APPENDIX B: EQUATIONS FOR REDUCTION OF THE G-SET TO THE A-SET

210

8.1 Introduction

211

8.2 Reduction of the G-set to the N-set

211

8.3 Reduction of the N-set to the F-set

213

8.4 Reduction of the F-set to the A-set

214

8.5 Reduction of the A-set to the L-set

216

8.6 Solution for constraint forces

216

9 APPENDIX C: EQUATIONS FOR ELEMENT STRESS RECOVERY MATRICES

220

9.1 General discussion

221

9.2 Rod element

221

9.3 Bar element

222

9.4 Plate elements
9.4.1 Membrane stresses
9.4.2 Bending stresses
9.4.3 Combined membrane and bending stresses
9.4.4 Transverse shear stresses

224
224
225
225
225

227

APPENDIX D: CRAIG-BAMPTON MODEL GENERATION

10.1 Craig-Bampton equations of motion for substructures

228

10.2 Development of displacement output transformation matrices

233

10.3 Development of load output transformation matrices
10.3.1 LTM terms for substructure interface forces
10.3.2 LTM terms for net c.g. loads
10.3.3 LTM terms for element forces and stresses
10.3.4 LTM terms for grid point forces due to MPC’s

236
236
236
238
238

10.4 Development of acceleration output transformation matrices

241

10.5 Correspondence between matrix names and CB Equation Variables

242

10.6 Craig-Bampton model generation example problem
10.6.1 CB-EXAMPLE-12b.F06
10.6.2 OUTPUT4 matrices written to CB-EXAMPLE-12-b.OP1 and OP2
10.6.3 Displ, Elem force/stress OTM’s written to CB-EXAMPLE-12-b.OP8 and OP9

244
245
246
246

265

APPENDIX E: DERIVATION OF RBE3 CONSTRAINT EQUATIONS

11.1 Introduction

266

11.2 Equations for translational force components

268

11.4 Summary of equations for the RBE3

275

List of Figures
Figure 3 1: Rectangular, Cylindrical and Spherical Coordinate Systems

Figure 3 2: Rod Element Geometry, Coordinate System and Forces

Figure 3 3: Bar Element Geometry and Coordinate System

Figure 3 4: Bar Element Forces

Figure 3 5: Plate Element Geometry and Coordinate Systems

Figure 3 6: Plate Element Force Resultants

Figure 3 7: Example of MYSTRAN Development of Equations for a Rigid Element

vii

List of Tables
Table 6-1: Matrices that can be written to OUTPUT4 files

viii

1 Introduction
MYSTRAN is a general purpose finite element analysis computer program for structures that can be
modeled as linear (i.e. displacements, forces and stresses proportional to applied load). MYSTRAN is an
acronym for “My Structural Analysis”, to indicate it’s usefulness in solving a wide variety of finite element
analysis problems on a personal computer (although there is no reason that it could not be used on
mainframe computers as well). For anyone familiar with the popular NASTRAN computer program
developed by NASA (National Aeronautics and Space Administration) in the 1970’s and popularized in
several commercial versions since, the input to MYSTRAN will look quite familiar. Indeed, many
structural analyses modeled for execution in NASTRAN will execute in MYSTRAN with little, or no,
modification. MYSTRAN, however, is not NASTRAN. All of the finite element processing to obtain the
global stiffness matrix (including the finite element matrix generation routines themselves), the reduction
of the stiffness matrix to the solution set, as well as all of the input/output routines are written in
independent, modern, Fortran 90/95 code. The major solution algorithms (e.g., triangular decomposition
of matrices and forward/backward substitution to obtain solutions of linear equations) as well as the
Givens method of eigenvalue extraction, however, were obtained from the popular LAPACK code,
Reference 1, available to the general public on the World Wide Web. The code for the Lanczos method
of eigenvalue extraction, Reference 2, was obtained from the ARPACK library, also available to the
general public on the World Wide Web. The code for the grid point sequencing algorithm (used to insure
a minimum bandwidth for the stiffness matrix) was obtained from the author of Reference 3.
Besides the LAPACK linear equation solver, there is an optional sparse matrix solver from the Intel Math
kernel Library (MKL) that is necessary for extremely large problems (hundreds of thousands of degrees of
freedom). In addition, there is another solver that uses sparse matrix technology and is described in
Reference 13. The choice of solver (LAPACK, Intel MKL or Yale) is chosen by the user via parameter
SOLLIB in the MYSTRAN input data section.
There is no inherent limitation to problem size, or number of degrees of freedom, for the version of
MYSTRAN distributed with an ”Unlock” key. Rather, the users’ personal computer memory (RAM and
disk) limitations will dictate what size problems can be effectively solved using MYSTRAN on their
computer.
Major features of the program are:


NASTRAN style input. NASTRAN model files will run in MYSTRAN with little or no
modification for static and eigenvalue analyses



3D structures with arbitrary geometry.



Linear static analysis.



Eigenvalue analysis via Lanczos, Givens and modified Givens methods. In addition, for the
fundamental mode there is also an Inverse Power method.


Optional calculation of modal mass and/or modal participation factors (Reference 8)



Craig-Bampton model generation.



Interface to the popular FEMAP pre/post processor program.



Grid points (3 translations and 3 rotations per grid) that define the finite element model mesh:



Locations can be defined in rectangular, cylindrical or spherical coordinate systems
that can be different for each grid



Global stiffness matrix can be formulated in rectangular, cylindrical or spherical
coordinate systems that can be different for each grid



Scalar points (SPOINT’) that have no defined geometry (one degree of freedom)



A finite element library consisting of the following elastic and rigid elements.
Elastic Elements (1, 2 and 3D):




1D and scalar elements.


BAR element with two grids and stiffness for up to six degrees of freedom
per grid (axial, two planes of bending, torsion) for beams that have their
shear center and elastic axis coincident



BUSH element (spring connecting two grids)



ELAS1,2,3,4 elements (scalar spring connecting two degrees of freedom)



ROD element (axial load and torsion element connected to two grid points)

Triangular and quadrilateral plate elements for thick (Mindlin plate theory) and thin
(Kirchoff plate theory) plates. The plates can include membrane and/or bending
stiffness and can be either single or multi ply composite elements:


QUAD4 quadrilateral plate element with plate membrane and bending
stiffness, as well as transverse shear flexibility, based on Mindlin thick plate
theory (References 5 and 9). This is essentially a flat element, however
small distortion out of plane is accommodated. Version 2.06 of MYSTRAN
introduced the QUAD4 element described in Reference 9 to correct the
deficiency in the prior QUAD4 that had diminished accuracy for elements that
were not rectangular



TRIA3 flat triangular plate element with plate membrane and bending
stiffness, as well as transverse shear flexibility, based on Mindlin thick plate
theory (Reference 4)



QUAD4K quadrilateral plate element with plate membrane and bending
stiffness based on Kirchoff thin plate theory (Reference 7). This is essentially
a flat element, however small distortion out of plane is accommodated.



TRIA3K flat triangular plate element with plate membrane and bending
stiffness based on Kirchoff thin plate theory (Reference 6)



SHEAR element that carries in-plane shear stresses

3D solid elements


TETRA 4 and 10 node solid elements. See Reference 10



PENTA 6 and 15 node elements with selective substitution reduction for
shear (if desired). See Reference 10



HEXA 8 and 20 node elements with selective substitution reduction for shear
(if desired). See Reference 10

R-elements:
 RBE2 rigid element specifying a relationship for one or more degrees of
freedom (DOF's) of one or more grids being rigidly dependent on the DOF's
of another grid.
 RBE3 element for distributing loads or mass from one grid to other grids.
 RSPLINE element for interpolating displacements between elements



User defined elements:


CUSERIN element where the user inputs the stiffness and mass matrices
and specifies the connection of the element to defined grids and scalar points



Single point constraints (SPC’s) wherein some degrees of freedom are grounded (e.g. for
specifying boundary conditions).



Other SPC’s wherein specified degrees of freedom have a specified motion (enforced
displacements).



Multi point constraints (MPC’s), wherein specified degrees of freedom are linearly dependent
on other degrees of freedom.



Loads on the finite element model via:


Forces and/or moments applied directly to grid points



Pressure loading on plate element surfaces



Gravity loads on the whole model (in conjunction with mass defined by the user)



Equivalent loads due to thermal expansion



Equivalent loads due to enforced displacements



Inertia Loads due to rigid body angular velocity and acceleration about some
specified grid (RFORCE)



Loads on scalar SPOINT’s (via SLOAD)



Linear isotropic, orthotropic and anisotropic material properties.



Mass defined via:


Density on material entries



Mass per unit length, or per unit area, for finite elements



Concentrated masses at grids (CONM2) with possible offsets and moments of inertia.



Scalar masses (CMASS1,2,3,4)



Multiple subcases to allow for solution for more than one loading condition in one execution.



Output of


Displacements (six degrees of freedom per grid) for any defined set of grids desired



Applied loads for any defined set of grids



Single point forces of constraint for any defined set of grids



Multi point forces of constraint for any defined set of grids (includes forces of
constraint due to MPC’s as well as rigid elements)



Grid point force balance for any defined set of grids



Element engineering and/or nodal forces for any defined set of elements



Element stresses for any defined set of elements



Element strains for 2D and 3D elements (including ply strains in composite elements)



Effective modal mass and/or modal participation factors in eigenvalue analyses



Output transformation matrices (OTM's) in Craig-Bampton analyses for displacement,
acceleration, force, and stress quantities



Interface to FEMAP post processing program for display of model and results (see Bulk Data
entry PARAM with parameter name POST)



Guyan reduction to statically reduce the stiffness and mass matrices. This is needed if the
Givens method of eigenvalue analyses is used to remove degrees of freedom that have no
mass (however, LANCZOS is the preferred method of eigenvalue extraction)



Limited CHKPNT/RESTART feature that allows a previous job to be restarted to obtain new
or different outputs (displacements, etc). The finite element model and solution (SOL in Exec
Control) must remain the same.



General:


AUTOSPC (automatic SPC generation based on used control)



Stiffness matrix equilibrium checks on request (Bulk Data PARAM entry EQCHECK)



Automatic grid point resequencing to reduce matrix bandwidth (Bulk Data PARAM
entry GRIDSEQ with value BANDIT – default).

2 General description of input data
A general description of MYSTRAN input data (referred to as a data section) is given in this section. A
more detailed description of each of the three parts of the data section will be given in Section 5.
Appendix A contains a sample MYSTRAN input and may be of help when reviewing this section.
The MYSTRAN data section consists of three distinct parts:


The Executive Control section



The Case Control section



The Bulk Data section

The Executive Control section is an overall identification of the job and the solution type to be performed
1
(e.g. statics, eigenvalues). It usually consists of a very few entries . It begins with an ID entry and ends
with a mandatory CEND entry. All Executive Control section entries are described in Section 5.1.
The Case Control section defines the job title that is printed out with the output, the loading for each of the
different subcases, the constraint boundary conditions and the sets that define the grids and elements for
displacement, load and stress output. The Case Control section begins with the entry following the
Executive Control CEND entry and ends with the mandatory BEGIN BULK entry. The only requirement
on the order of entries in the Case Control section is that the order makes sense when there are multiple
subcases. The details of each of the Case Control section entries are given in Section 5.2
The Bulk Data section defines the finite element model in detail. It begins with the entry immediately
following the BEGIN BULK entry and ends with the mandatory ENDDATA entry. Grid points form the
“mesh” of the finite element model and are defined with their locations (in any of several coordinate
systems). The elements that make up the finite element model are defined by the grid points to which
they are connected, by their physical properties and by their material properties. Loads and boundary
conditions are also defined in the Bulk Data section. In the case of eigenvalue analysis, the eigenvalue
extraction method is also defined here.
All physical Bulk Data entries are broken down into 10 fields of 8 columns each with field 1 being a
mnemonic that defines the type of entry (e.g. GRID for a grid point definition, PBAR for a bar element
property definition, etc.). Since 10 fields may not be enough for some of the entries, provision is made to
include “continuation” entries. For example, the PBAR Bulk Data entry that defines geometric properties
for a bar element has three physical entries necessary to define all of the properties. These three
physical entries comprise the one logical PBAR entry. This is explained in detail in the description of Bulk
Data entries in Section 5.3. Suffice it to say here that a logical Bulk data entry in MYSTRAN may consist
of several physical entries with the initial entry being called the “parent” entry and subsequent
continuation entries (if necessary) called “child” entries. Since all logical Bulk Data entries have a
mnemonic that defines which type of input it describes, there is no requirement on the order of logical
entries in the Bulk Data section. Physical entries that make up a given logical entry must, however, be in
order and grouped together.

“entry” is used to mean a single line of entry in the data section. It is a holdover from the familiar 80
column punched entries used to enter data into computers long ago. The MYSTRAN data section does
consist of lines of entry that can contain data in columns 1 through, possibly, column 80 (each denoted as
a physical entry). A logical entry can, in some instances, consist of more than one physical entry.

3 The finite element model
The finite element model is specified by defining:


Grid points that locate the frame to which elements are connected



Finite elements (connection, property and material definitions)



Applied loads



Constraints



Mass at grid points and or of elements

The following sub-sections discuss each of these.

3.1

Grid points

3.1.1 Grid point and coordinate system definition
Grid points are defined on GRID Bulk Data section entries. The GRID entry gives the grid point number
and the coordinates of the grid point in any of several types of coordinate systems. The grid point
numbers can be any arbitrary integers containing from 1 to 8 digits as long as the numbers are unique
among all grids. The GRID entry can also be used to specify constraint information. A “basic” coordinate
system is implicitly defined and is rectangular. Grid coordinates are either defined in the basic system or
in other rectangular, cylindrical or spherical coordinate systems whose location can be traced back to the
basic system. If coordinate systems other than the implicitly defined basic system are used, their
locations are defined using the CORD2R, CORD2C and CORD2S Bulk Data entries (for rectangular,
cylindrical and spherical coordinate systems). These entries give the location of three points in some
other coordinate system that is previously defined. This is cascaded until the last coordinate system is
defined relative to the basic system.
In addition to locating grid points, the GRID entry references another coordinate system, known as the
global coordinate system for that grid point. This global coordinate system is the system in which the
overall (global) stiffness matrix is generated for each grid and in which constraints are applied and
solution for displacements is obtained. Again, the basic system is the default for the global system at any
grid but can be overridden on the GRID entry for the grid in question. It is important to realize that when
reference is made to the “global” coordinate system, what is really meant is a collection of coordinate
systems that may be different for each grid point. Alternatively, the global coordinate system for a grid
point is also referred to as its displacement coordinate system.
Each grid point has six degrees of freedom: translations along three orthogonal axes and the orthogonal
rotations about these three axes. The six degrees of freedom will be collectively referred to as the
displacements of the grid point in question and are denoted as:
u1g ,u2g ,u3g , 1g , 2g , 3g

3-1

where g designates a grid point. In the case of a rectangular displacement coordinate system for a grid
point, the three orthogonal translations are positive along axes that are at the grid and parallel to the three
coordinate axes directions defined by a CORD2R entry. The three rotations are positive for right hand
rule rotation (in radians) about these three axes. For a cylindrical displacement coordinate system for a

grid point, the translations are along the radial, tangential and axial directions at the grid and the rotations
are again positive for right hand rule rotation about these three axes. For a spherical displacement
coordinate system the three translations are in the radial, meridional and azimuthal directions with the
rotations about these axes. Figure 3-1 shows these three coordinate systems.
The GRID entry also has a field that can be used to denote constraints that are for zero displacement for
any of the six degrees of freedom for that grid point. These constraints are known as permanent single
point constraints (or PSPC’s).

3.1.2 Grid point sequencing
It is important to include provision for internally rearranging the order of the grids in order to obtain a
global stiffness matrix that has a minimal bandwidth. The CPU time to perform linear equation solutions
is directly dependent on the stiffness matrix bandwidth. In addition, several matrices have to be put into
“banded” form for the LAPACK algorithms used in MYSTRAN. Thus, bandwidth is extremely important in
determining the disk storage requirements for those matrices.
The sequencing method used in any execution of MYSTRAN is controlled via the Bulk Data PARAM
GRIDSEQ entry. The user has several options for specifying sequencing that are basically manual or
automatic, as explained below.
3.1.2.1

Automatic grid point sequencing

Automatic grid point sequencing to achieve a minimal stiffness matrix bandwidth is accomplished using
an algorithm called BANDIT which is described in Reference 3. The code for accomplishing this was
obtained from that author and is imbedded in MYSTRAN. BANDIT, when originally written, was a standalone program that generated SEQGP Bulk Data entries (see section on the Bulk Data section) which
defined the sequence order for each grid. Within MYSTRAN, BANDIT is a subroutine which generates
these SEQGP entries and MYSTRAN uses these to define the grid sequencing. BANDIT is the default
sequencing method in MYSTRAN and is equivalent to including a Bulk Data PARAM GRIDSEQ entry with
BANDIT specified in field 3 of the PARAM entry. When BANDIT sequencing is used, any user supplied
SEQGP Bulk Data entries are ignored and a warning message is given.
3.1.2.2

Manual grid point sequencing

In manual grid sequencing, the user supplies the Bulk Data section SEQGP entries which are used to
sequence the grids. However, only those grids which are to be re-sequenced from their initial order need
to have their sequence number specified on SEQGP entries. In order to facilitate this MYSTRAN starts
out with a predefined sequence order that can then be modified with the user supplied SEQGP entries.
The predefined sequence order can be one of two possibilities (and is defined on the PARAM GRIDSEQ
Bulk Data entry):
 Grid numerical order (PARAM GRIDSEQ GRID)
 Order of the grids as they appear in the Bulk Data section (PARAM GRIDSEQ INPUT)
The following beam model with seven grid points illustrates this:

201

301

401

101

501

601

701

Assuming that the user has the initial order set with PARAM GRIDSEQ GRID then grid 101 would be
sequenced 1st initially. However, for a minimum stiffness matrix bandwidth, it should be sequenced so
that it is 4th. Using the SEQGP entry, grid 101 can be re-sequenced to be 4th by giving it a sequence
number between where grids 401 and 501 are sequenced. Since the sequence number can be a decimal
value then grid 101’s sequence number should be a number that is greater than 4 but less than 5 (say
4.1)

3.2

Elements

3.2.1 Element connection, property, and material definition
Elastic elements are defined by their connectivity (the grids to which they attach), by their geometric
properties and, in all but the ELAS1 element, by their material properties. The mnemonic in field 1 of all
elastic element connection entries begins with a “C” followed by the element name. The mnemonic in
field 1 of a bar element connection entry, for example, is CBAR (in columns 1-4). Field 2 of a connection
entry gives the element ID, which is an arbitrary integer (although elements must have unique IDs among
the set of all elements). Field 3 of the connection entry for all one and two dimensional elements gives
the ID of an element property Bulk Data entry that is used to specify geometric properties of the element.
Following this on the element connection entry, the grid points to which the element connect are
specified. With the exception of the scalar spring element, all elements have a local element coordinate
system. This local element coordinate system is defined by the order of the grids on the element
connection entry and by, for some elements, an orientation vector that is also defined on the element
connection entry. This will be discussed in detail in each of the separate element sections below.
Element property entries define the geometric properties of the elements (e.g. cross-sectional areas,
moments of inertia of bars, thickness of plates, etc.). The mnemonic in field 1 for all property entries
begins with a “P” followed by the element name. The property entry for a bar element, for example, has
PBAR in field 1 and has, in field 2, the property ID that was referenced on the connection entry. Field 3
specifies an ID of a material Bulk Data entry. The remaining fields define the geometric properties of the
bar element and can take up to three physical entries for the complete description. For example, the
PBAR entry has the following properties:


Cross-sectional area



Moments of inertia and product of inertia



Torsional constant



Mass per unit length



Up to four locations, on the cross-section, where stresses are to be calculated



Area factors for shear flexibility

Material properties are specified on the MAT1 Bulk Data entry for linear isotropic materials and on the
MAT8 entry for linear orthotropic materials (plate elements only). Field 2 contains the material ID and the
remaining fields contain material constants (such as Young’s modulus, Poisson’s ratio, mass density,
thermal expansion coefficients, etc.).
The reason for the connection entries pointing to property entries which, in turn, point to material entries
is the following: every element must have a connection entry but many of them may be for elements that
have the same physical properties and there may be even fewer material entries needed. Also, in this

manner, it is not required that the entries in the Bulk Data section be in any specific order with the
exception that, for continuation entries, the child entries must follow the parent entry in order.

3.2.2 Elastic elements
3.2.2.1

Scalar spring (ELAS and BUSH elements)

The ELAS1 scalar spring element connects between two degrees of freedom. The CELAS1 Bulk Data
entry defines the connection information, which consists of a pair of grid points and the displacement
components at those grid points that the spring is to be connected between. In addition, the CELAS1
entry references a PELAS property entry that will define the spring rate, K, and a stress recovery
coefficient, S, such that S times the elongation of the spring gives the stress that is output for the element.
No material entry is needed for the CELAS1 element.
Care must be taken when using scalar spring elements that rigid body motion of the model is not
constrained. For example, if the spring is connected between two non-coincident grids then rigid body
motion of the model may be constrained if the degrees of freedom that the spring is connected to are not
along a line between the grids.
Output for a spring element can include any, or all, of the following:


Element nodal forces:




Output in either global or basic coordinates at all grids for selected elements

Element stress (positive for positive engineering forces):


Stress calculated as the spring stress recovery coefficient (specified on the PELAS
Bulk Data entry) times the spring elongation.

The BUSH element is a spring connecting two grid points. It can have up to 6 stiffness values (one for
each displacement degree of freedom). The element connection can take into consideration that the two
grid points are not coincident. It is a better choice for a scalar spring than the ELAS elements if the grids
are not coincident. The BUSH can have the following element outputs:


Element nodal forces:


Output in either global or basic coordinates at all grids for selected elements



Element engineering forces:



Element stress (positive for positive engineering forces):


Stress calculated as the spring stress recovery coefficient (specified on the PELAS
Bulk Data entry) times the spring elongation.

3.2.2.2

Rod element

The rod is a one-dimensional element that is connected between two grid points (G1 and G2) and which
has stiffness for axial and torsional motion. The CROD entry specifies the element connection for the rod
and the PROD entry defines the area, torsional constant, torsional stress recovery coefficient and mass
per unit length for the rod. The local element coordinate system only requires the definition of one axis;
namely along the axis from grid point G1 through grid point G2 as shown in Figure 3-2.
Output for a rod element can include any, or all, of the following:




Element engineering forces:


Axial force (positive is tension)



Torsion (positive as shown on Figure 3-2)

Element nodal forces:




3.2.2.3

Output in either local, global, or basic coordinates at all grids for selected elements

Element stresses (positive for positive engineering forces):


Axial stress and margin of safety



Torsional stress and margin of safety

Bar element

The bar element is a simple beam that has its shear center coincident with its neutral axis. It is defined
using the CBAR connection entry and the PBAR property entry. It can carry bending and shear in two
planes, axial force and torque. Shear flexibility can also be included. Figures 3-3 and 3-4 show the
element coordinate system and element engineering forces.
The ends of the bar element can be offset from the grids G1 and G2 as indicated on Figure 3-3. This is a
rigid offset and can have components in up to three orthogonal directions. The components of the offset
vectors are specified on the CBAR entry in the global coordinate systems of grids G1 and G2,
respectively.
The v vector in Figure 3-3 is used to determine Plane 1 and Plane 2 of the bar as indicated in the figure.
This is necessary so that the moments of inertia (I1, I2, I12) on the PBAR entry can be interpreted
correctly. The v vector is specified on the CBAR entry as either three components of a vector measured
from end “a” in the global coordinate system of grid G1, or by a grid point, G0, along the v vector (which,
together with end “a”, defines v). The moment of inertia, I1, on the PBAR entry is the moment of inertia
about the element ze axis. Moment of inertia, I2, on the PBAR entry is about the element ye axis. Planes
1 and 2 need not be principal planes. If they are not, then the product of inertia, I12, must be specified on
the PBAR entry.
The bar can be disconnected from a grid point in any of the six degrees of freedom, resulting in the
corresponding force(s) in the bar being zero. This is referred to as a “pin flag” feature for the bar. Either
end of the bar can be pin flagged. However, the pin flags specified cannot result in the bar being
completely disconnected from the grid mesh in any rigid body degree of freedom. For example, degree of
freedom 1 (axial) cannot be pin flagged at both ends. This would result in the bar being disconnected
from the grid mesh along its xe axis.

The following output is available for the bar element:
 Element engineering forces:



Axial force



Torque



Bending moments at both ends in each of the two planes



Shear in the two planes

Element nodal forces




Output in either local, global, or basic coordinates at all grids for selected elements

Element stresses (positive for positive engineering forces):


Stresses due to bending in the two planes at up to four points defined by the user on
the PBAR entry



Stress due to axial force



Maximum, and minimum, combined bending and axial stress at each end of the bar



Margins of safety for tension and compression stresses, flagged when they are less
than zero



Torsional stress (if SCOEFF is input on the Bulk data PBAR entry)

Maximums and minimums are determined from the stress due to axial force and the bending stresses at
the four points, at each end, if the user specified those points on the PBAR entry. Otherwise the
maximums and minimums are based on the stress due to axial force.
3.2.2.4

Plate elements

MYSTRAN provides for both triangular and quadrilateral plate elements that include membrane and/or
bending stiffness, several of which may be used to model thick plates consistent with Mindlin plate theory.
All of the plate element formulations have constant thickness. The separate connection entries available
for this modeling are given below (in all cases the mid-plane of the plate can be offset from the grids) :




Combination Membrane-Bending Elements:


CTRIA3: triangular element for modeling thick plates and shells



CTRIA3K: triangular element for modeling thin plates and shells



CQUAD4: quadrilateral element for modeling thick plates and shells



CQUAD4K: quadrilateral element for modeling thin plates and shells

In-plane shear element Elements:



CSHEAR: quadrilateral element for modeling thin shear plates

The property entry used for the combination membrane-bending elements is either the PSHELL or
PCOMP/PCOMP1 entry. The SHEAR element properties are specified via the PSHELL entry. The
PSHELL entry has provision for specifying membrane, bending and transverse shear properties
(CTRIA3K, CQUAD4K do not have transverse shear flexibility). As with other property entries, the
PSHELL entry has the property ID in field 2 and up to three material IDs (fields 3, 5 and 7); one each for
membrane, bending and transverse shear. In addition, the membrane, bending and transverse shear
properties themselves are input (fields 4, 6 and 8). A mass per unit area can also be input (field 9). The
membrane, bending and transverse shear properties and material IDs are discussed in detail below.


PSHELL Property Values and Material IDs:




Membrane


Field 3 specifies MID1, the ID of a material entry for the membrane portion of
the plate. If this field is left blank, no membrane stiffness will be computed.



Field 4 specifies TM, the membrane thickness. This is required, even if the
MID1 field is left blank, since it is used in the computation of bending and
transverse shear properties.

Bending


Field 5 specifies MID2, the ID of a material entry for the bending portion of
the plate. If this field is left blank, no bending stiffness or transverse shear
flexibility will be computed.



Field 6 specifies 12(I/TM**3), a normalized bending property where I is the
moment of inertia per unit width of the plate and TM is the membrane
thickness discussed above. This normalized bending property has a default
value of 1.0. If field 6 is left blank, it signifies a homogeneous plate.

Transverse Shear


Field 7 specifies MID3, the ID of a material entry for the transverse shear
portion of the plate. If this field is left blank, no transverse shear flexibility will
be calculated. Only the CTRIA3 and CQUAD4 thick plate elements have the
capability for transverse shear flexibility.



Field 8 specifies TS/TM, the ratio of shear to membrane thickness. This has
a default value of 5/6 = 0.833333, if field 8 is left blank. This is an historic
value that is based on the shear stress distribution in a solid cross-section
beam. A more realistic value for plates is based on Mindlin plate theory and
2
(or 0.822467), which is only a few percent different than the historic
is 
12
value. The default value for all PSHELL property entries can be reset on the
Bulk Data entry PARAM (with name TSTM_DEF in field 2 and the new value
in field 3).

The PCOMP or PCOMP1 property entry is for defining the plies, or lamina, of composite elements
(laminates). Each ply can have a distinct material property that can be isotropic, orthotropic or
anisotropic. The assumption is made that each ply, is in a state of plane stress, the bonding material
between the plies is perfect, and two dimensional plate theory can be used for the laminate.

Figure 3-5 shows the triangular and quadrilateral element coordinate systems. Figure 3-6 shows the
convention for plate force resultants which are the basis for calculating element stresses. These are
standard definitions of plate force resultants that can be found in texts on the theory of plates and shells.
The quadrilateral elements can accommodate some out of plane warping, but they are generally intended
for use as flat elements. When the quadrilateral element has out of plane distortion, the xe – ye plane for
the element (as shown in Figure 3-5) is the mean plane between the grids. Instead of allowing significant
warp of quadrilateral elements, triangular elements should be used.
Output for the plate elements includes:




Element engineering forces:


Membrane force resultants (force/length) as shown on Figure 3-6



Bending moment resultants (moment/length) as shown on Figure 3-6



Transverse shear force resultants (force/length) for the QUAD4 and TRIA3 as shown
on Figure 3-6

Element nodal forces




Output in either global or basic coordinates at all grids for selected elements

In plane element stresses at fiber distances Z1 and Z2 (on the PSHELL entry, with +/-TM/2
as default) that are derived from the above force and moment resultants


Normal stress in the xe direction



Normal stress in the ye direction



In-plane shear stress



Major and minor principal stress and the associated angle



Max in-plane shear stress



von Mises or max shear stress



Transverse shear stresses (for the QUAD4 and TRIA3)

For the QUAD4 stresses can be output at the element center as well as at the corner nodes of the
element. The TRIA3 element has constant stress so only one output per element is provided.

3.2.2.5

3D Solid elements

MYSTRAN has hexahedra, pentahedra and tetrahedra elements for modeling of 3D structures. The
CHEXA hex element comes in 8 node and 20 node versions. The CPENTA element comes in 6 node
and 15 node versions. The CTETRA is available in 4 node and 10 node versions. Properties for these
solid elements are specified on the PSOLID Bulk Data entry, with several choices for integration order
and integration scheme. Material properties are specified on the MAT1 entry. Outputs for the solid
elements are in the form of stresses at the element center and can include von Mises and max shear
results.

3.2.3 Rigid elements
In addition to the elastic elements discussed above, MYSTRAN also has a capability for specifying a rigid
relationship among specified degrees of freedom. These elements are suited for situations where a
portion of a model is so much stiffer than the remainder that it could cause ill conditioning of the stiffness
matrix if it were modeled with elastic elements. When rigid elements are used, selected degrees of
freedom are eliminated from the solution set using equations (automatically generated in MYSTRAN) that
represent rigid body notion of the “dependent” degrees of freedom based on rigid motion of a selected set
of “independent” degrees of freedom. Specification of rigid elements in MYSTRAN is accomplished with
Bulk Data entries similar to elastic element connection entries (however, no property ID is needed). Field
1 of the rigid element connection entry, like elastic elements, has a mnemonic describing the rigid
element type
Care must be taken when using rigid elements in thermal distortion analyses. The rigid elements do not
expand with temperature and can otherwise constrain a model that the user expects to expand in a stress
free manner.

3.2.3.1

RBE2 rigid element

The RBE2 element specifies that the motion of a set of grid points (all having the same set of dependent
degree of freedom numbers) are dependent on the six degrees of freedom at another grid point.
An example of the equations developed by MYSTRAN to eliminate the dependent degrees of freedom is
shown in Figure 3-7 (for a simple one-dimensional problem). In this example, degrees of freedom 1, 2
and 6 at grid 103 will be eliminated from the solution set of degrees of freedom using the equations
shown. The user does not have to input these equations; only the Bulk Data RBE2 field entries.

3.2.4 RBE3 element
The RBE3 element is not a rigid element but is used to distribute loads and mass from some central grid
point to other grids in the model. It is defined by a dependent, central, point at which the load or mass is
defined along with grids to which the load or mass are to be distributed along with weighting factors at
these distributed grids. The dependent point on the RBE3 should never be connected to other elastic
elements in the model to avoid stiffening of the structure by the RBE3 element. Appendix E gives a
mathematical derivation of the RBE3 equations which reduce the dependent grid point out of the model
equations of motion.

3.2.5 RSPLINE element
The RSPLINE element is generally used to model transitions from a coarse to a fine mesh. In
MYSTRAN, the RSPLINE element connects to 2 independent end points. Displacements along and
perpendicular to the line between the end points is interpolated using the 6 displacements of the end
points as follows:


Displacenents along the line and rotations about the line are linear



Displacements perpendicular to the line are cubic



Rotations normal to the line are quadratic

3.3

Applied loads

MYSTRAN provides several methods of specifying applied loads:


Forces and/or moments applied directly to grids



Pressure loading on plate elements



Gravity loads



Equivalent loads due to thermal expansion



Equivalent loads due to enforced displacements



Loads on scalar points (SLOAD)

All of the Bulk Data entries defining these loads have a set ID which is used to control whether they are
used in a particular subcase. Thus, the user is free to include load entries in the Bulk Data that may not
be used in a particular execution of the program (that might be used in a subsequent run, for example).

3.3.1 Forces and moments directly applied to grids
Bulk Data entries FORCE and MOMENT are used to define forces and/or moments applied directly to a
grid point. Both of these entries have, in field 2, a set ID.
Field 3 of both the FORCE and MOMENT entry specifies the grid point where the load is to be applied.
Field 5 specifies an overall scale factor and fields 6 – 8 specify the vector components of the load. The
load applied in a component direction is the product of the overall scale factor times the vector
component in that direction. The vector components are in a coordinate system whose ID is specified in
field 4.
FORCE and MOMENT entries to be used in a particular subcase must be requested in Case Control with
a LOAD = SID Case Control entry. The SID is either the set ID from the FORCE and/or MOMENT entries
or is the set ID of a Bulk Data LOAD entry (see below) that has the FORCE and/or MOMENT set IDs
specified.

3.3.2 Pressure loads on plate elements
Pressure loads normal to the surface of plate elements can be specified on PLOAD2 and PLOAD4 Bulk
Data entries. As with the grid point load entries discussed above, the PLOAD entries have a set ID in
field 2 that must be referenced (directly or indirectly) in Case Control in order to be used for a particular
subcase. The pressure value is specified in field 3. The remainder of the entry presents two options for
specifying what plate elements are to have this pressure value. One option is to list the element IDs
using in fields 4 through 9 of the parent entry and, if necessary, fields 2 through 9 of continuation entries.
The other option allows the elements to be specified using a THRU option, in which case any element
whose ID is in the range of EID1 (field 4) through EID2 (field 6) will receive the pressure value in field 3.
Pressure loads are requested in Case Control the same as was described for the FORCE and MOMENT
entries (either directly or by use of the LOAD Bulk Data entry).

3.3.3 Gravity loads
Gravity loads for the model are specified using the GRAV Bulk Data entry. The GRAV entry specifies an
acceleration vector that, in conjunction with the mass at the grid points (discussed later), allows
MYSTRAN to calculate static forces at all of the grid points due to the specified acceleration using the
inertia properties of the model (grid point masses, etc., discussed later). As with other loads, the GRAV
entry has a set ID in field 2. Fields 4 through 7 specify the magnitude and vector components of the
acceleration in a coordinate system whose ID is given in field 3. The magnitude and/or vector
components must be given in units consistent with model mass, discussed in a later section.
Gravity loads are requested in Case Control the same as was described for the FORCE and MOMENT
entries (either directly or by use of the LOAD Bulk Data entry).

3.3.4 Equivalent loads due to thermal expansion
The equivalent loads due to thermal expansion are calculated automatically in MYSTRAN based on grid
and/or element temperature data supplied by the user on a variety of Bulk Data entries, listed below, all of
which have a set ID in field 2 of the entry:




Grid temperature definition Bulk Data entries:


TEMPD specifies a default temperature for all grids



TEMP specifies a temperature for grids listed on this entry. These temperatures
override any default values on TEMPD entries.

Element temperature Bulk Data entries:


TEMPRB specifies average element temperatures for ROD and BAR elements as
well as temperature gradients through the depth for BAR elements



TEMPP1 specifies average element temperatures and gradients through the
thickness for plate elements

When a temperature load is to be used, all of the elements in the model must have a temperature
defined. This may be done either indirectly using a TEMPD or TEMP entry that defines the temperatures
of the grids to which the element connects, or directly by specification on a TEMPRB or TEMPP1 element
temperature entry. Thermal expansion coefficients and reference temperatures, needed in the calculation
of equivalent loads due to thermal expansion, must be specified on material Bulk Data entries.
The user must request temperatures in Case Control with the Case Control entry TEMP = SID where SID
is the set ID on the above Bulk Data temperature entries which define the temperatures for the model.

3.3.5 Equivalent loads due to enforced displacements
If the user knows, a priori, the displacement (translation or rotation) of some degrees of freedom,
MYSTRAN handles this by what is referred to as “enforced displacements”. The user specifies the known
displacement on a Bulk Data SPC entry (in the global directions for the grid) and MYSTRAN uses this as
a constraint. The Bulk Data SPC entries’ set ID must be selected in Case Control with the Case Control
entry SPC = SID, where SID is the set ID of the Bulk Data SPC entries defining the enforced
displacements.

The program calculates loads necessary to enforce this constraint and applies them to the structure in
combination with all other loads specified. When forces of constraint are calculated in the program, the
forces listed (in the output, if Case Control entry SPCFORCES is included) are those necessary to make
the degrees of freedom displace the amounts that were specified as enforced displacements.

3.3.6 Loads due to rigid body rotation about a specified grid (RFORCE)
The finite element model can have loads calculated due to a rigid body angular velocity and/or angular
acceleration. The loads are calculated as if the body were rotating when, in actuality, it is fixed. The
equivalent loads due to this angular velocity and acceleration are applied to the fixed body. In this
fashion, situations such as rotating turbines with centripetal forces can be simulated. This force is
calculated via the Bulk data entry RFORCE.

3.3.7 LOAD Bulk Data entry – combining loads
Loads defined via the FORCE, MOMENT, GRAV and PLOAD2 entries that have different set IDs can be
combined into one set for use in a subcase using the LOAD Bulk Data entry (not to be confused with the
LOAD Case Control entry). The LOAD Bulk Data entry has a set ID in field 2. The following fields
(including possible continuation entries) specify which of the individual load sets to use. This is specified
as pairs of set IDs (of FORCE, MOMENT, GRAV or PLOAD2 loads) and scale factors for each of the
separate loads. In addition, an overall scale factor for the combination of the loads on the LOAD Bulk
Data entry is defined in field 3.

3.4

Constraints

3.4.1 Single point constraints
Single point constraints (SPC’s) are needed for the following reasons:


To specify boundary conditions where the model is to be grounded. These constraints will
result in those degrees of freedom being zero and will also result in, generally, non-zero
forces of constraint at the specified degrees of freedom.



To remove singularities in the model. The global stiffness matrix is built on the basis of six
degrees of freedom (3 translations and 3 rotations) per grid point which, for some models,
means that some degrees of freedom may not have any stiffness. For example, a 2D model
of a plate for bending and membrane action would have, at most, five degrees of freedom per
grid since the plate elements have no stiffness for rotation about the normal to the plate.
Thus, this plate model will have a singular global stiffness matrix for the degrees of freedom
representing rotation about the normal to the plate. The user has a choice of identifying
these explicitly or by having MYSTRAN constrain degrees of freedom that are singular
through the use of an AUTOSPC feature (see Bulk Data PARAM entry for parameter
AUTOSPC). In either event, these degrees of freedom are constrained to zero prior to
solving for the displacements. If there is no stiffness for these degrees of freedom, the
forces of constraint for them will be zero



To specify enforced displacements at degrees of freedom where the user knows, a priori, the
nonzero value of those displacements.

For the user defined SPC’s the constraints are specified on SPC or SPC1 Bulk Data entries (or as
“permanent” single point constraints in field 8 of the GRID Bulk Data entry). Both the SPC and SPC1
entries have a set ID in field 2. In addition, there is a SPCADD Bulk Data entry that can be used to
combine requests made by the SPC and/or the SPC1 entries. The constraints specified on the SPC,

SPC1 or SPCADD entries must be selected in Case Control with the SPC = SID Case Control entry,
where SID is the set ID of either a SPCADD or of one or more SPC and/or SPC1 Bulk Data entries.
The SPC Bulk Data entry must be used for nonzero enforced displacements. Either the SPC or SPC1
entry (two different methods of specifying zero constraints of selected degrees of freedom) can be used
for the other types of SPC’s.
There can be only one SPC request in Case Control for any one MYSTRAN execution.

3.4.1.1

AUTOSPC Feature

The AUTOSPC feature mentioned above is done automatically in MYSTRAN unless the user includes a
Bulk data PARAM AUTOSPC entry with an N in field 3 to request that MYSTRAN do not perform an
AUTOSPC calculation. The explanation of the AUTOSPC feature that follows assumes the user is
familiar with the displacement set notation defined in Section 3.6.
In order to identify singular degrees of freedom when the G-set singularity processor is run, MYSTRAN
uses a comparison of stiffness terms to a small number and constrains the degree of freedom if this
criterion is met. The specific procedure is explained below:


For each grid of the G-set stiffness matrix, the two 3x3 stiffness matrices (one for translation
and one for rotation) are obtained for one grid.



The three eigenvalues and eigenvectors of the two 3x3 matrix are determined.



The ratio of each of the three eigenvalues to the eigenvalue that is the max among the three
is determined. A comparison of the ratio to AUTOSPC_RAT (see PARAM AUTOSPC Bulk
Data entry field 4) is made.



If the ratio is less than the criteria, one degree of freedom will be constrained. The degree of
freedom that is constrained is the one whose eigenvector absolute value is largest (using the
eigenvector corresponding to the eigenvalue for that ratio).

If the eigenvalues of the 3x3 matrices are exactly zero, then no forces of constraint will result from the
AUTOSPC’s. There are instances in problems with near singularities in which the eigenvalue ratios are
not exactly zero and in those cases some small force of constraint will result. These should be generally
negligible, but the user should always request output of the forces of constraint, especially when using the
AUTOSPC feature. An example of a case where these small ratios can be nonzero is in the case of
modeling a curved surface with only plate elements. If the user makes several models and continually
refines the mesh, then at some point two contiguous elements will become nearly parallel. At this point
there will be negligible stiffness at a common node for rotation about the normal to the plate. When this
stiffness gets small enough, MYSTRAN will constrain it if the AUTOSPC feature is turned on.
Through this procedure, the AUTOSPC feature can identify many, but perhaps not all, singular degrees of
freedom. In the case where the model has either rigid elements or multi-point constraints (MPC’s) a
situation can arise where the G-set stiffness matrix is singular. When the G-set singularity processor is
called for each grid, any grid that is specified as independent on an MPC or rigid element is skipped. This
is done since these grids may not have any stiffness (they may have no elastic element connected to all
six grid components) in the G-set stiffness matrix but may get stiffness when the MPC and rigid element
degrees of freedom are eliminated. Thus they must be ignored until after the reduction from the G-set to
the N-set. After this reduction, the N-set stiffness matrix will be scanned (if AUTOSPC_NSET on the
PARAM AUTOSPC entry is equal to 1) to see if any rows are null. There may be null rows if some of the
independent degrees of freedom on MPC’s and rigid elements do not have stiffness at this point. If any
rows are null, the degrees of freedom corresponding to these rows are AUTOSPC’d also.

AUTOSPC_NSET can also be set to 2 or 3 also. If equal to 2, then MYSTRAN will remove any N-set
degrees of freedom whose diagonal stiffness ratio (to max diagonal stiffness) is less than
AUTOSPC_RAT. If it is equal to 3, then both actions for AUTOSPC_NSET = 1 and 2 are applied. In
general AUTOSPC_NSET = 1 (default) is recommended.

3.4.2 Multi point constraints
Multi point constraints (MPC’s) may be needed for the following reason:


To specify linear dependence of some degrees of freedom on other degrees of freedom. The
equation relating the linear dependence is specified on MPC Bulk Data entries. Rigid
elements are really automated multi point constraints that represent rigid motion of an
“element” and are a subset of the more general MPC relationship. MPC’s are a more general
way of specifying linear dependence of some degrees of freedom on other degrees of
freedom.

There can be only one MPC request in Case Control for any one MYSTRAN execution.

3.4.3 Boundary degrees of freedom in Craig-Bampton analyses (SUPORT)
This feature is primarily included for Craig-Bampton (CB) model generation. It provides a set of degrees
of freedom (DOF’s) that are to be boundary DOF’s used in calculating modal properties of a substructure.
Reference 11 and Appendix D describe the Craig-Bampton method as it is currently implemented in
MYSTRAN. The boundary DOF’s are identified on Bulk Data SUPORT entries and define the R-set of
degrees of freedom (see later discussion on displacement set notation). For CB analyses the modal
properties of the substructure are determined with fixed boundaries so that the R-set is constrained to
zero for the purposes of calculating modal properties of the substructure. The SUPORT feature is not
intended for use in any of the other MYSTRAN solutions (e.g. statics, eigenvalues). If the SUPORT
feature is used in any solution method other than Craig-Bampton, the result is the same as if the
SUPORT DOF’s were identified as constrained to zero motion on SPC or SPC1 Bulk Data entries.

3.5

Mass

Mass for the finite element model can be specified in several ways:


Mass density for finite elements (specified on property Bulk Data material entries)



Mass per unit length, or per unit area, for finite elements (specified on element property Bulk
Data entries)



Concentrated masses at grids (using CONM2 Bulk Data entry) with possible offsets and
moments of inertia.

Any of the above can be used in combination, or separately, in defining the mass for any finite element
(or grid point in the case of CONM2’s) in the model.

3.5.1 Mass density on material entries
The MAT1 Bulk data entry used to define material properties, discussed earlier, has a field to specify the
mass density of the material. This mass density, together with the volume of each finite element, can be

used by MYSTRAN to calculate a mass for each element. For example, plate elements have a surface
area defined by the grid locations of the three or four grids that the plate element is connected to. The
plate element thickness (membrane thickness on the property entry PSHELL) along with the surface area
defines a volume for the element. The mass density on the MAT1 entry times this volume defines the
mass for this element. Similarly, a beam element (BAR) has a length defined by the two grids that the
element connects to and has a cross-sectional area specified on the PBAR entry. The element volume is
calculated from this area and length.

3.5.2 Mass per unit length or area of finite elements
Mass can also be defined using data entered on the element property Bulk Data entries. The PBAR
entry, for example, has a provision for specifying mass per unit length of the bar. The plate element
property entries have a field in which a mass per unit area can be defined. These can be used in
conjunction with the other two methods of defining mass, or can be used independently to completely
define the mass for an element.

3.5.3 Concentrated masses at grids
Concentrated masses can be placed directly at grid points using the CONM2 Bulk Data entry. This entry
provides the user with the option of specifying a mass value with possible offsets from the grid point and
mass moments of inertia, including products of inertia. The offsets and inertia’s can be specified in a
coordinate system referenced on the CONM2 entry. Use of the CONM2 presents a convenient method
for including “rigid masses” at grid points. The CONM2 entry has an “element” ID in field 2, the ID for the
grid to which the mass is attached in field 3, the coordinate system in which the mass properties are
specified in field 4 and the mass value in field 5. The remainder of the logical entry (which can span two
physical entries) is used to specify possible offsets and moments and products of inertia. The offsets are
the relative coordinates of the c.g of the mass with respect to the grid and are specified in the coordinate
system whose ID is in field 3. The inertia values are the moments and products of inertia of the mass
about it’s own c.g., also with respect to the coordinate system specified in field 3. Moments of inertia
about any of the three axes of this coordinate system can be specified. There are, possibly, six products
of inertia but only the three independent ones need be specified. The offsets and inertia values are
optional.
A 6 x 6 symmetric mass matrix, M, (at the c.g. of the mass) is created by MYSTRAN as given by:
0
0
0
m

m
0 md3

0
m md2
M
I11


SYM



md3
0
md1
I12
I22

md2 

md1 
0 

I13 
I23 

I33 

3-2

In the above, m denotes the mass value on the CONM2 entry and d1, d2 and d3 denote the offsets of m
from the grid and Iij are the six independent moments and products of inertia. The 1,2 and 3 subscripts
refer to the 3 axes of the coordinate system whose ID is in field 4 of the CONM2 entry.

3.5.4 Model total mass
MYSTRAN can calculate the rigid body mass properties (total mass, overall c.g. and moments of inertia)
of the finite element model if the user desires. The calculation is done in the basic coordinate system and
can be done relative to any user specified grid point. The Bulk Data entry PARAM with a parameter
name of GRDPNT in field 2 is used to request output of the rigid body mass properties of the model. If

field 3 of this PARAM entry contains a grid point ID, the calculation will give the mass properties relative
to that grid point. If field 3 is blank (or zero), the calculation will be done relative to the origin of the basic
coordinate system.

3.5.5 Mass units
All units of mass input in the Bulk data must be consistent. However, the user can input these in terms of
mass or weight. If weight units are used, the finite element mass matrix must be converted back to mass
units prior to performing eigenvalue analyses. This is accomplished using the Bulk Data PARAM entry
with a parameter name of WTMASS in field 2. The value of the WTMASS parameter is used to multiply
the mass matrix prior to eigenvalue analyses. Thus, if the user has input weight units instead of mass
units a WTMASS value of 1.0/gravity (e.g. 1.0/386 if gravity is 386 in/sec2) must be used. The units of the
output for the rigid body mass properties of the whole model (discussed above) are the same as the input
units (mass or weight).
If the user has specified a gravity loading (see section on Applied Loads) the units of the acceleration on
the GRAV entry must also be consistent with the units of mass. For example, if mass units are used then
the GRAV entry should specify the gravity loading in acceleration units. However, if weight units are used
the gravity loading should be specified in terms of g’s.

3.6

Displacement set notation

As was mentioned in an earlier section, MYSTRAN originally constructs stiffness and mass matrices for
the model based on all grid points having six degrees of freedom. These matrices are referred to as the
G-set matrices such that if there are n grid points, the original stiffness and mass matrices will have 6n
rows and columns (i.e., the G-set consists of 6n degrees of freedom). The stiffness matrix for these G-set
degrees of freedom must, therefore, be singular since no constraints of any kind will have been imposed
on it; either through specification of boundary constraints or through rigid elements (which cause
constraints as well). In order to reduce this matrix to the independent degrees of freedom, MYSTRAN
partitions and reduces the G-set to the independent degrees of freedom, denoted as the L-set. This
section describes the various sets as MYSTRAN reduces from the G-set to the L-set.
The G set is initially constructed in a degree of freedom (DOF) order that is discussed in the section on
Grid point sequencing. The G-set is then partitioned into two sets; one of which consists of all degrees of
freedom denoted as dependent on rigid elements or multi-point constraints (M-set) plus all others
(denoted as the N-set). In displacement set notation, then:
U 
UG   N 
UM 

3-3

The M-set degrees of freedom are eliminated using the multi point constraint equations as well as
equations developed in MYSTRAN based on the rigid element geometry and the dependent degrees of
freedom in the N-set. Following this reduction, the stiffness and mass matrices are in terms of the N-set
degrees of freedom. This N-set is further partitioned into two sets; those that are constrained via single
point constraints (denoted as the S-set) plus all other degrees of freedom from the N-set (denoted as the
F-set). The displacement set notation for this is:
U 
UN   F 
US 

3-4

The S-set degrees of freedom are eliminated using the single point constraints (both zero constraints and
enforced displacements). Following this reduction, the stiffness and mass matrices are in terms of the Fset degrees of freedom. At this point, the F-set may well be an independent set of degrees of freedom.
However, MYSTRAN allows for a further reduction of the F-set based on Guyan reduction (static
condensation). A Guyan reduction is necessary, for real eigenvalue analysis by the Givens method, if
there are any zeros on the diagonal of the mass matrix. Zero diagonal terms would occur, for example, if
the mass matrix had mass terms only for the translation degrees of freedom and not for the rotation
degrees of freedom. Other situations could also result in zero diagonal terms in the mass matrix. The
degrees of freedom to be eliminated by static condensation are denoted as the O-set. The O-set is
defined using the Bulk Data entry OMIT or OMIT1 (or alternately via the ASET or ASET1 entry). In
general, there is no reason to specify an O-set for static analysis. At any rate, the F-set is partitioned into
these 0-set degrees of freedom plus all remaining degrees of freedom in the F-set (denoted as the A-set).
The displacement set notation for this is:
U 
UF   A 
UO 

3-5

The O-set degrees of freedom are eliminated via Guyan reduction (static condensation). Following this
reduction, the stiffness and mass matrices are in terms of the A-set degrees of freedom. In the static and
eigenvalue analysis solutions, the A-set is the final, independent, set of degrees of freedom. However,
for Craig-Bampton (CB) model generation the A-set is comprised of the L and R-sets. The displacement
set notation for this is:
U 
UA   L 
UR 

3-6

The R-set are the degrees of freedom at the boundary of the substructure where it connects to other
substructures. The R-set is defined by the user via the SUPORT Bulk Data entry. In CB analysis, the Rset are constrained to zero for the purposes of calculating the fixed interface modal properties of the
substructure and the R-set is used in determining the boundary stiffness and mass. As shown in
Reference 11, these matrices provide the overall properties of the substructure in terms of modal and
boundary degrees of freedom which are typically a much smaller subset of the physical degrees of
freedom in the R and L-sets combined.
Following elimination of the R-set degrees of freedom, MYSTRAN is set to solve for the displacements of
the L-set.
If there is no R-set defined by the user, then the L-set is equivalent to the A-set. If there is no O-set
defined by the user, then the A-set is equivalent to the F-set. If there is no S-set, the F-set is equivalent
to the N-set (although the stiffness matrix for this would be singular since no boundary constraints would
exist). If there is no M-set then the N-set is equivalent to the G-set.
The mutually exclusive sets are the M-set, the S-set, the O-set and the R-set and the L-set. The G-set
consists of all of these.
Appendix B has a complete mathematical discussion on the details of how the G-set is reduced to the Aset

When the degree of freedom (DOF) tables are printed out (if requested by the user through the PARAM
PRTSET and PARAM PRTDOF Bulk Data entries), the S-set is broken down into the several sub-sets.
Below is a summary of all of the columns of the DOF table:
 G: All DOF’s in the model
 M: All DOF's multi-point constrained
 N: G – M ( or F + S)
 SA: DOF’s SPC’d when AUTOSPC = Y
 SB: DOF’s SPC’d to zero via Bulk Data SPC, SPC1 Bulk Data entries (requested in CaseControl)
 SE: DOF’s SPC’d to nonzero values (enforced displacements) (requested in Case Control)
 SG: DOF’s SPC’d to zero values that are identified in field 8 of the Bulk data GRID entry
 SZ: SA + SB + SG (all zero value SPC’s)
 S: All DOF’s single-point constrained (S = SA + SB + SG + SE)
 F: N – S ( or A + O)
 O: All DOF’s statically omitted
 A: F – O (or L + R)
 R: All DOF's defined via Bulk Data SUPORT entries
 L: A – R

4 MYSTRAN solution types
MYSTRAN currently has 3 solution types: SOL = 1 for statics, SOL = 3 for eigenvaluse and SOL = 31 for
Craig-Bampton (CB) model generation. The first two of these are very similar to the static and eigenvalue
solution types in NASTRAN and will not be elaborated upon. The third, CB model generation is a new
analysis type and is discussed in more detail

4.1

Statics

SOL 1 or, alternately, SOL STATICS is for static solution of a model with constant loads. It is the same
as statics for NASTRAN and uses all of the features described above for model description, load
definition, etc. Output for displacements, applied loads, constraint forces, grid point force balance,
element forces and stresses are available. In addition output of matrices and debug information is
available

4.2

Eigenvalues

SOL 3 or, alternately, SOL MODES, or SOL MODAL or SOL NORMAL MODES is for eigenvalue
analyses of a model. It is the same as the eigenvalue analysis type of solution in NASTRAN. All of the
model features in statics (with a few exceptions such as loads and enforced displacements) are available.
Besides the eigenvalues themselves, output for displacements, constraint forces, element forces and
stresses are available. Also, output of modal participation factors and modal effective mass is available.
In addition output of matrices and debug information is available

4.3

Craig-Bampton model generation

SOL 31 or SOL GEN CB MODEL is for Craig-Bampton (CB) model generation and is a new feature in
MYSTRAN that is not a direct solution type available in NASTRAN. It involves reduction of a large model,
originally in terms of physical degrees of freedom (DOF’s) at all grid locations, to one in which the DOF’s
are a smaller subset using modal DOF’s for fixed base modes to describe the vibration characteristics of
the model and physical DOF’s for the boundaries between substructures. Appendix D gives a detailed
description of CB analyses including references to the original work by those that pioneered the technique
and also includes an example problem. Using NASTRAN to get CB models is a more cumbersome
technique than the direct one in MYSTRAN in that it employs a rather complicated (and in some areas
arcane) DMAP (or Direct Matrix Abstraction Programming) program.
Sometimes called dynamic substructure analysis, CB analysis is often used in cases where a very large
model is broken into smaller pieces each of which is generally a defined substructure. An example would
be a spacecraft with several scientific instrument and appendages. Each of these individual pieces may
come from different analytical groups and may be needed in a combined analysis. Each of the groups
developing models of their substructure would deliver an analytical CB model of their hardware and the
systems contractor would assemble these for a combined structural dynamic analysis.
The input to a SOL 31 CB model generation analysis for a single substructure is the same as that for a
standard eigenvalue analysis with a few additions. The biggest difference is in defining the boundary
DOF’s for the substructure where it connects to other substructures. The boundaries are defined using
Bulk Data SUPORT entries which key MYSTRAN to put these DOF’s into the R-set. The fixed base
modes of the substructure are those for which the R-set is constrained to zero. However, the model
delivered to the system contractor for integration cannot be grounded at these DOF’s since they will be

active in the combined analysis. Thus, the CB solution takes into account that these boundary DOF’s are
free in the matrices that define the CB model even though they were temporarily grounded to obtain the
fixed mode properties of the substructure. It should be mentioned that the boundary DOF’s defined via
the SUPORT Bulk Data entry must be the only DOF’s constrained to zero motion except for those
removed to avoid singularities.
The output from the CB analysis of a single substructure is quite different than those from a normal
eigenvalue analysis except that the fixed base modal frequencies and mode shapes can be output and
are the same as those that would result from a SOL 3 eigenvalue analysis with the R-set constrained to
zero motion. The rest of the available outputs are generally for Output Transformation Matrices (OTM’s)
and other CB model matrices needed by the systems contractor in performing the combined analysis.
Appendix D discusses all of the available OTM’s from a SOL 31 CB model generation analysis. However,
the following is a general idea of how to obtain CB model data from MYSTRAN:


For any of the matrices listed in Table 9.5 of Appendix B (including Net C.G. loads and Interface
Force LTM) use the OUTPUT4 entry in Executive Control. Theses are written to disk files with the
names filename.ext where ext (file extension) is OPi with i=1,2,3,4,5,6,7 as defined by the user in
the OUTPUT4 command.



For displacement, acceleration, element force, element stress, MPC forces, use normal Case
Control requests (including defining sets of grids/elements for output). These OTM’s are output in
the normal F06 output file and also onto disk files with the extension OP8 (for grid related OTM’s)
and extension OP9 (for element related OTM’s. Text files (extensions OT8 and OT9) have
explanations of the rows of the OTM’s written to the OP8 and OP9 files.

In addition to creating CB models, MYSTRAN can synthesize CB models, along with an optional finite
element model, into a systems model for eigenvalue analyses. This feature is demonstrated in

Figures
Figure 4-1: Rectangular, Cylindrical and Spherical Coordinate Systems

Z
u3g (Z direction)

G.P. g

u2g (Y direction)

u1g (X direction)

Rectangular

Z
u3g (z direction)

u2g ( direction)

r
G.P. g

u1g (r direction)

Cylindrical
Y



(G.P. = Grid Point)

u1g (r direction)
u3g ( direction)

G.P. g

u2g ( direction)

r


Spherical
Y



X
26

Figure 4-2: Rod Element Geometry, Coordinate System and Forces

Mt
Fa

Fa
Mt

Fa  Axial Load
Mt  Torque
x e  Rod axis (positive from grid G1 through grid G2)

Figure 4-3: Bar Element Geometry and Coordinate System

Bar end b
ye


wb


v

Plane 1
G2
Plane 1 is xe , y e
Plane 2 is xe , ze

Plane 2


wa

Bar end a
G1

xe  Neutral axis of the bar (positive direction goes from end a toward end b)

v  Vector specified on the CBAR card that is used in defining Plane 1.

ze  Axis in the plane defined by xe and the vector cross product xe  v
ye  Axis in the direction of the vector cross product ze  xe

wa  Vector from grid G1 on the CBAR card to end a of the bar (the offset at end a)

wb  Vector from grid G2 on the CBAR card to end b of the bar (the offset at end b)

Figure 4-4: Bar Element Forces

ye
V1

M1a

a
Mt

M1b
xe

Plane 1

ze
V2

M2 a

a
Mt

xe
P

P
V2

M2b

Plane 2

P  Axial Load
Mt  Torque
V1  Shear in Plane 1
V2  Shear in Plane 2
M1a  Bending Moment in Plane 1 at end a
M1b  Bending Moment in Plane 1 at end b
M2a  Bending Moment in Plane 2 at end a
M2b  Bending Moment in Plane 2 at end b

Figure 4-5: Plate Element Geometry and Coordinate Systems
ye

Triangular Plate Element

Gi is a grid point

G3
G4




Quadrilateral Plate Element

G1
G2

Figure 4-6: Plate Element Force Resultants

Mxy

Myy

Mxx

Mxy
Vy

Mxy

Mxx

Myy

Mxy

Plate Bending Moment and Transverse Shear Force Resultants

Ny
Nxy

Nxy
Nx

Nx
Nxy

Nxy

Plate Membrane Force Resultants

Figure 4-7: Example of MYSTRAN Development of Equations for a Rigid Element

Y (global degree of freedom
numbers 2, 5)

12
101

13
102

14
103

104

X ( global degree of
freedom numbers 1, 4)

Z (global degree of
freedom numbers 3, 6)

Grid ID's are: 101 - 106
Element ID's are: 12 - 14 (12 and 14 elastic and 13 rigid)
Global displacement system is the X, Y, Z basic system shown
Define:
ui  displ of grid i in the X direction,  xi  rotation of grid i about X axis
v i  displ of grid i in the Y direction,

 yi  rotation of grid i about Y axis

w i  displ of grid i in the Z direction,  zi  rotation of grid i about Z axis
X i  X coordinate of grid i
Assume that rigid element 13 is rigid only in the X - Y plane.
Take grid 103, degrees of freedom 1,2,6 as dependent. Use grid 102 as independent.
The linear equations that specify the dependence of grid 103 on grid 102 in the X - Y plane are:
u103  u102
v103  v102  ( X 103  X 102 ) z102
 z103   z102

5 References
1. LAPACK Users’ Guide, 3rd edition, SIAM, 1999 (see website at http://www.netlib.org/lapack)
2. ARPACK Users’ Guide, 3rd edition, SIAM, 1998 (see website at
http://www.caam.rice.edu/software/ARPACK/)
3. Everstine, G. C., “Recent improvements to Bandit”, NASTRAN: Users’ Experiences, Volume NASA
TM X-3278 pages 511-521, Washington, DC, 1975. National Aeronautics and Space Administration.
4. Tessler, A. and Hughes, T.J.R., “A three-node Mindlin plate element with improved transverse shear”,
Computer Methods In Applied Mechanics And Engineering 50 (1985) 71-101
5. Tessler, A. and Hughes, T.J.R., “An improved treatment of transverse shear in the Mindlin-type fournode quadrilateral element”, Computer Methods In Applied Mechanics And Engineering 39 (1983)
311-335
6. Batoz, J., “An explicit formulation for an efficient triangular plate-bending element”, International
Journal For Numerical Methods In Engineering, Vol. 18 (1982), 1077-1089
7. Batoz, J. and Tahar, M.B., “Evaluation of a new quadrilateral thin plate”, International Journal For
Numerical Methods In Engineering, Vol. 18 (1982), 1655-1677
8. Case, William R., “A NASTRAN DMAP procedure for calculation of base excitation modal
th
participation factors”, 11 NASTRAN User’s Colloquium, May 5-6, 1983
9. Liu,, J, Riggs, H.R. and Tessler, A. , “A four-node, shear-deformable shell element developed via
explicit Kirchoff constraints”, International Journal For Numerical Methods In Engineering, Vol. 2000,
49, pp 1065-1086
10. MacNeal, Richard H., “Finite Elements. Their Design and Performance”, Marcel Dekker, 1993
11. Case, William R., DMAP for generating Craig-Bampton Models, notes from a course given at the
Goddard Space Flight Center (contact author for copy of paper)
12. MYSTRAN-Demo-Problem-Manual (contained in the MYSTRAN setup file downloaded from
www.MYSTRAN.com along with this manual.
13. S. C. Eisenstat, M. C. Gursky, M. H. Schultz and A. H. Sherman. “Yale Sparse Package. The
Symmetric Codes,” Yale University of Computer Science Research Report #112

6. Detailed description of input data
The input entries for the Executive Control, Case Control and Bulk Data Sections are described in detail
in the next three sections. In all of the sections, an entry with a $ sign in column 1 is considered as a
comment and is ignored. In addition, any blank entry is ignored. All other entries must be in upper case.
Appendix A contains a sample problem input/output.

6.1

File Management

As mentioned earlier, the input data file consists of 3 sections: Executive Control, Case Control and Bulk
Data. In order to make the most efficient use of resources, each of these can contain requests to include
some defined file to be part (or all) of that portion of the input data file. This is accomplished through the
use of an INCLUDE entry whose format is:
INCLUDE ‘filename’
Where filename is the name of a file to include at the location where the INCLUDE entry exists. The
INCLUDE entries can be used in any or all of the 3 sections of the input data file. In addition, multiple
INCLUDE entries in any section are permitted. The quotes around filename are recommended but not
required.

6.2

Executive Control

The Executive Control Section consists of only a few entries. Most are free field; that is they can begin in
any column and the parts of an entry may be separated by any amount of columns within the confines of
the 80 column physical entry. In addition, the fields of an entry may be delimited by tabs, as well as a
white space. Some of the entries are required and some are not required but are recognized. Other
entries are ignored with a warning message printed in the output. Any requirements on the order of the
entries in the Executive Control Section are noted.
With the CHKPNT/RESTART feature, users may restart a previously run job to get additional outputs. In
a restart the Bulk Data must remain the same except for a few PARAM and DEBUG entries. Case
Control requests for additional displacements, element forces, stresses, etc will be processed.

Executive Control Entries required and/or recognized by MYSTRAN
Entry
ID
IN4

Required
(Y/N)
N
N

Format

Description

Free Field

If input, it is generally the first entry in the Exec Control Section.
Defines a file containing element stiffness, mass and other data for
a CUSERIN element
An entry of APP DISP is common if this entry is included
Required if the user expects to restart the current job, at a later
date, to obtain additional outputs
These are the same as the Bulk Data DEBUG entries and are
allowed here since some DEBUG values need to be used prior to
reading the Bulk Data
Requests for CB matrices to be written to unformatted files in the
same format as NASTRAN uses. An example is shown below
along with the allowable matrices that can be output
Requests to partition a previously defined OUTPUT4 matrix
Required only if the current job is a restart of an earlier job in
which the CHKPNT entry was present. The file name (w/ ext) of
the CHKPNT’d original run must follow the command RESTART
SOL entry must have a value that designates what kind of problem
this is:
(1) SOL 1 or SOL STATICS designates the job as a statics
problem
(2) SOL 3 or SOL = MODAL or SOL MODES or SOL NORMAL
MODES for eigenvalues
(3) SOL 31 or SOL GEN CB MODEL for Craig-Bampton (CB)
model generation
TIME n, where n is the job estimated time in minutes, is a typical
input
The CEND entry has no other input required. It must be the last
entry in the Exec Control Section

APP
CHKPNT

N
Y/N

Free Field
Free Field

DEBUG

OUTPUT4

Fields of 8
chars like
Bulk Data
Free Field

PARTN
RESTART

N
Y/N

Free Field
Free Field

SOL

Free Field

TIME

Free Field

CEND

Free Field

6.2.1 IN4 Exec Control command
The Exec Control command IN4 specifies binary files (NASTRAN INPUTT4 format) which contain the
element matrices needed for CUSERIN Bulk Data element definition. The IN4 command has the
following format:
IN4 i filename
Where i is the ID of the file and is what must appear in field 3 of the Bulk Data PUSERIN property entry
for the CUSERIN element. filename is the name of the file that contains the matrices specified on the
PUSERIN entry for the element. filename must contain the full path unless the file is in the current path
where the program is being executed. An example is:
IN4 100 cb1_example1.OP1

6.2.2 OUTPUT4 and PARTN Exec Control commands
MYSTRAN allows output of selected matrices to binary files in the OUTPUT4 format that is the same as
that currently used by NASTRAN. The form of the OUTPUT4 command is:
OUTPUT4 MAT1,MAT2,MAT3,MAT4,MAT5//ITAPE/IUNIT $
From 1 to 5 matrices can be output per OUTPUT4 command. All 4 commas must be present even if
fewer than 5 matrices are requested. The // followed by ITAPE value (must be 0 to -3 but is currently not
used) must also be present. The final / followed by a file unit number (can be 21-27) is also required. A
trailing $ can exist but is not required. If present, it signifies the end of data read for the OUTPUT4
command.
These OUTPUT4 matrices can be partitioned, in some cases, using an Exec Control PARTN command.
The resulting partitioned matrix will be the one output to the OUTPUT4 binary file. The partitioning
vectors that define which columns and rows to partition from the original OUTPUT4 matrix are defined on
Bulk Data PARVEC and PARVEC1 entries. These Bulk Data partitioning vector entries give the grid and
component pairs of the columns and rows to partition. As such, the partitioning can only be done on
OUTPUT4 matrices that have columns and/or rows that are part of a normal displacement set (the G-set,
M-set, etc.). See section 3.6, “Displacement set notation”, for a definition of all of the displacement sets.
The general form for the PARTN command for MYSTRAN is:
PARTN MAT, CP, RP /

where MAT is an OUTPUT4 matrix previously requested for OUTPUT4 output and CP and RP are
column and row partitioning vectors defined in the Bulk data using PARVEC and/or PARVEC1 Bulk Data
entries.
If the input file for a MYSTRAN run is filename.DAT, the binary OUTPUT4 file names are filename.OPi
where i=1,7 (corresponding to units 21-27 used as values for UNIT in the OUTPUT4 command). The
format in which these files are written is the same as that for the NASTRAN OUTPUT4 matrices.
The table on the following page shows the matrices that are currently eligible for OUTPUT4 output. Note
that there is a correspondence between MYSTRAN and NASTRAN matrix names. The OUTPUT4
commands can use either name as desired by the user. All matrix names must be no more than16
characters long. An example of the use of the Exec Control commands OUTPUT4 and PARTN is given
following the table.

Table 6-1
Matrices that can be written to OUTPUT4 files
(and the correspondence between MYSTRAN matrix names, NASTRAN names
and CB Equation Variables)
MYSTRAN NASTRAN
Matrix Name
DMAP
(OUTPUT4
Name
matrices)

CB equation variable in Appendix D
(where applicable)

LTM116r

LTM126N 0 

Matrix size1

CG_LTM

DLR

LxR

EIGEN_VAL

LAMA

 2NN

NxN

EIGEN_VEC

PHIG

 GN , (LN with rows expanded to G-set)

GxN

GEN_MASS

mNN

Nx1 vector of
diag. terms

IF_LTM

KAA

K AA

AxA

KGG

K GG

GxG

KLL

K LL

LxL

KRL

KLR(t)

K LR

LxR

KRR

K RR

RxR

KRRcb

KBB

T
k RR  K RR  K LR
DLR

RxR

KXX

KRRGN

K XX

(R+N)x(R+N)

LTM

CG_LTM and IF_LTM merged

(6+R)x(2R+N)

MCG

RBMCG

mcg

6x6

Modal effective mass
Modal participation factors

Nx6
Nx6 or NxR

LTM21RR

16 MEFFMASS
17 MPFACTOR

LTM22RN LTM23RR 

Partition
rows
and/or
cols

6x(2R+N)

Rx(2R+N)

rows and
cols

rows

rows
rows and
cols
rows and
cols
rows and
cols
rows and
cols
rows and
cols
rows and
cols

rows and
cols
rows and
cols
rows and
cols
rows and
cols

MAA

AxA

MGG

GxG

MLL

LxL

MRL

RxL

MRN

T
mRN  mNR

RxN

rows

MRR

RxR

rows and
cols

MRR

Table 6-1 (con’t)
MYSTRAN NASTRAN
Matrix
DMAP
Name
Name
(OUTPUT4
matrices)
24

MRRcb

MXX

26
27
28
29

PA
PG
PL
PHIXG

MBB

TR6_CG

MXX

m
  RR
mNR

T

mNR

mNN 

Matrix size 1

RxR

PHIXG

RBR

RBRCG

 AX , (  AX with rows expanded to G-set)
The G-set displacement transformation matrix is
written out in the F06 file under
“C B D I S P L A C E M E N T O T M”
Rigid body mass matrix relative to the basic origin
TR6 : rigid body displacement matrix for R-set
relative to the model basic coordinate system
TR6 : rigid body displacement matrix for R-set
relative to the model CG

Partition
rows
and/or
cols
rows and
cols

(R+N)x(R+N)

(A-set static reduced loads - only used in statics)
(G-set static loads - only used in statics)
(L-set static reduced loads - only used in statics)

PHIZG
RBM0
TR6_0

T
T
T
mRR  MRR  MLR
DLR  (MLR
DLR )T  DLR
MLLDLR

MRRGN

31
32

CB equation variable in Appendix D
(where applicable)

Rows
Rows
rows
Gx(R+N)

rows

Gx(2R+N)

rows

6x6
Rx6

rows

Rx6

rows

Note: (t) indicates matrix transposition

Matrix size given in rows x columns where R means the size of the R-set, L is the size of the L-set, A is
the size of the A-set, G is the size of the G-set and N is the number of eigenvectors. See section 3.6 for
definition of the complete displacement set notation

Example of OUTPUT4 request in Exec Control
Format:
OUTPUT4 MAT1, MAT2, MAT3, MAT4, MAT5 // ITAPE / IUNIT $
Example:
OUTPUT4 PHIZG, KRRcb,,, // -1 / 22

a) The OUTPUT4 entry is free-field (except that there can be no blank characters in any of the
names, including OUTPUT4).
b) MATi can be any of the matrix names in the OUTPUT4 table above. There can be 1 to 5 matrices
in any OUTPUT4 request but all 4 commas must be present.. If there is a name for the matrix in
the column “NASTRAN DMAP Name”, that name can be used in place of the MYSTRAN Matrix
Name for OUTPUT4 purposes
c)

ITAPE (using NASTRAN notation) should be: - 3  ITAPE  0 (but is currently not used in
MYSTRAN),

d) IUNIT must be: 21  IUNIT  28 . Any number of the OUTPUT4 matrices can be sent to one
IUNIT and more than one IUNIT can be used in one Exec Control section,
e) The / characters must be present,
f)

Anything after the $ character (if present) is ignored.

Example of PARTN request in Exec Control

Format:
PARTN MAT, CP, RP/

CP is the column partitioning vector and RP is the row partitioning vector
Example:
OUTPUT4 PHIZG,, RVEC1 /

a) The PARTN entry is free-field (except that there can be no blank characters in any of the names,
including PARTN).
b) MAT is the name of the matrix to partition (with restrictions noted in Table 6-1 regarding whether
rows and or column of this matrix are available for partitioning).
c) RP (RVEC1 in the example) is the row partition vector which must be specified using either the
PARVEC or PARVEC1 Bulk Data entry.
d) The PARTN entry must have 2 and only 2 commas. Note that in the example above that CP is
not specified (since PHIZG is only available for row partitioning) but the 2nd comma is present.
e) The PARTN entry for MAT must follow (but not necessarily immediately) the mandatory
OUTPUT4 request for it.

6.3

Case Control

The Case Control Section performs several functions outlined below. The entries for each of the major
purposes are enumerated below. A detailed explanation of each is contained in the following section. A
BEGIN BULK entry is considered as the last, and mandatory, entry in the Case Control Section. In
addition, the fields of an entry may be delimited by tabs, as well as a white space.




The following entries specify the titles that will be printed in the output file, none of which are
required:
TITLE

Specifies a line of text to be printed in the output file

SUBTITLE

Specifies a 2nd line of text to be printed in the output file

LABEL

Specifies a 3rd line of text to be printed in the output file

The following entries select items from the Bulk data to be used in the current job (loads,
constraints, temperature sets, eigenvalue extraction ID):
ENFORCED

Specifies a file containing all grid displacements (all translations and
rotations for all grids). With this command, users can run cases in which
all displacements are known (as for example from test data) and can
request any outputs based on these displacements.

LOAD

Selects FORCE, MOMENT, GRAV, PLOAD2, PLOAD4, RFORCE and
LOAD sets from the Bulk Data Section that define loads for a statics
solution.

METH

Selects an eigenvalue extraction set from the Bulk Data for a eigenvalue
solution.

SPC

Selects SPC, SPC1 from the Bulk Data Section that define single point
constraints (including enforced displacements) for the current job.

MPC

Selects MPC entries from the Bulk Data Section that define multi-point
constraints for the current job.

TEMP

Selects TEMP, TEMPD and TEMPP1 sets from the Bulk Data Section
that define temperature loads for a statics solution.

The following entries define output requests:
ACCEL

Requests output of accelerations.

DISPL

Requests output of displacements.

ECHO

Requests form of the input file echoed to the output file.

ELDATA

Requests element matrix generation output to the BUG file 2 .

ELFORCE

Requests output of element engineering and/or node forces.

The various files (output and scratch) generated by MYSTRAN are described in a later section. BUG is
the extension of one of those files.



GPFORCE

Requests output of grid point force balance showing all of the forces
acting on a grid point and checking equilibrium of those forces.

MEFFMASS

Requests output of modal effective masses in eigenvalue analyses.

MPCFORCE

Requests output of multi point forces of constraint (due to MPC’s as well
as rigid elements).

MPFACTOR

Requests output of modal participation factors in eigenvalue analyses.

OLOAD

Requests output of applied loads.

SET

Specifies sets that define grid points and elements for which output is
desired.

SPCFORCE

Requests output of single point forces of constraint.

STRESS

Requests output of element stresses.

STRAIN

Requests output of element strains for shell and solid elements

The following entry defines subcases for which solutions will be calculated in static analyses
(SOL 1):
SUBCASE

A entry that indicates that the following entries (until another SUBCASE
entry is encountered) define the conditions for one solution in the current
job. A separate subcase must be used for each loading condition for
which a solution is desired.

6.3.1 Detailed Description of Case Control Entries
The following pages give the details for each of the Case Control Section entries listed above. The
format of each is free field with the following conventions:


Upper case letters must be entered as shown.



Lower case letters indicate that a substitution must be made.



Parentheses shown must be entered.



Braces { } indicate that a choice, from the items listed, must be made.



Brackets [ ] indicate that the terms enclosed may be omitted, if desired. Braces within
brackets indicate that if terms within the brackets are input a choice must be made of the
portion within the braces.



Underlined values are the default values.

In addition, some of the entries have an acceptable abbreviation of the entry name. For example, the
entry requesting displacement output can be DISPLACEMENT or at least the first four letters of the
name. This is noted in the detailed description with brackets. Thus DISP[LACEMENT] indicates the
acceptable forms of this Case Control entry.

BEGIN BULK
6.3.1.1 BEGIN BULK
Description:
Indicates the end of the Case Control section

Format:
BEGIN BULK

ACCELERATION
6.3.1.2 ACCELERATION
Description:
Requests output of grid point accelerations in the global coordinate system for selected grids. For CraigBampton model generation, the output is of the columns of the acceleration transfer matrix (ATM).

Format:
 ALL 


ACCE[LERATION] =  n 
NONE 



Examples:
ACCELERATION = ALL (requests output of accelerations for all grid points)
ACCE = 45 (requests output of accelerations for grid points included in Case Control entry SET 45)

Options:
Option
ALL
n
NONE

Meaning
Accelerations for all grid points in the model will be output.
ID of a SET Case Control entry previously defined. Accelerations for the grid points
defined by SET n will be output. Integer > 0, no default value.
No accelerations will be output.

Remarks:
1. NONE is used to override an overall output request made above the SUBCASE level.

DISPLACEMENT
6.3.1.3 DISPLACEMENT
Description:
Requests output of grid point displacements in the global coordinate system for selected grids. For
eigenvalue analyses, the output is of eigenvectors.

Format:
 ALL 


DISP[LACEMENT] =  n 
NONE 



Examples:
DISPLACEMENT = ALL (requests output of displacements for all grid points)
DISP = 45 (requests output of displacements for grid points included in Case Control entry SET 45)

Options:
Option
ALL
n
NONE

Meaning
Displacements for all grid points in the model will be output.
ID of a SET Case Control entry previously defined. Displacements for the grid points
defined by SET n will be output. Integer > 0, no default value.
No displacements will be output.

Remarks:
1. NONE is used to override an overall output request made above the SUBCASE level.

ECHO
6.3.1.4 ECHO
Description:
Requests that the input data file be echoed in the output file

Format:
 NONE 
ECHO= 

UNSORT 

Examples:
ECHO = NONE

Options:
Option

Meaning

NONE

No echo of the input data file will be in the output file.

UNSORT

The echo of the data file in the output will be in the same entry order that the input data
file is in.

ELDATA
6.3.1.5 ELDATA
Description:
Requests output of element data from the element matrix generation subroutines for selected elements.
The data is written to files separate from the standard output file. Description of the data items that can
be output is given in the table below. The output files that the data is written to are described in the
MYSTRAN Installation and Run Manual.

Format:
   ,PRINT    ALL 
 
  

ELDA[TA] (m  ,PUNCH ) =  n 
   ,BOTH   NONE 
  

 

Examples:
ELDATA(1,BOTH) = 2 (print and punch output of elem data item 1 for elems in SET 2).
ELDATA(3) = 3 (print output of elem data item 3 for elems included in SET 3).
ELDATA(2,PUNCH) = ALL (punch output of elem data item 2 for all elems).

Options:
Option
m
ALL
n
NONE

Meaning
Defines which element data items are to be output (see table below)
Data items m for all elements will be output.
ID of a SET Case Control entry previously defined. Element data for item m defined by
SET n will be output. Integer > 0, no default value.
No element data items will be output.

Remarks:
1. NONE is used to override an overall output request made above the SUBCASE level.
2. See table below for a description of the data items that can be output

Element Data Items Output for ELDATA Case Control Entry

Data Item(s) Output

Actual and internal grid points and basic coordinates.
Array of element property data.
Array of element material data.
Array of element temperature data.
Bar element v vector in basic coordinates.
Bar pin flag data.
Bar offsets.
TE coord transform matrix (transforms a vector from basic to local elem coords).
Actual and internal grid points and local element coordinates.
Element mass matrix in local element coordinates.
Element thermal and pressure loads in local element coordinates.
Element stiffness matrix in local element coordinates.
Element stress recovery matrices in local element coordinates.
Element grid point displacements and loads. The coordinate system will be the
one defined by Bulk data PARAM ELFORCEN.
Data on isoparametric element shape functions and Jacobian matrices
Isoparametric element shape functions
Check isoparametric element strain-displ matrices for rigid body motion and
constant strain

1
2
3
4
5
6
7
8

Printed
to
Text
File
With
Extension
BUG

Written
To
Unformatted
File
With
Extension

BUG
BUG
BUG
BUG
BUG

F21
F22
F23
F24
F25

BUG
BUG
BUG

Notes:
1) The filename will be the same as the input data file but with the extension given in the table.
2) See Appendix B for a description of some of these matrices that can be output.

ELFORCE
6.3.1.6 ELFORCE
Description:
Requests output of nodal or engineering forces for selected elements.

Format:
 ENGR   ALL 


 
ELFO[RCE] (NODE) =  n 
 (BOTH)  NONE 

Examples:
ELFORCE = ALL (requests output of element engineering forces for all elements)
ELFO(NODE) = 125 (requests output of element nodal forces for elements included in SET 125)

Options:
Option
ALL
n
NONE

Meaning
Element forces for all elements in the model will be output.
ID of a SET Case Control entry previously defined. Element forces for the elements
defined by SET n will be output. Integer > 0, no default value.
No element forces will be output.

Remarks:
1. NONE is used to override an overall output request made above the SUBCASE level
2. The forces can be output in local element, basic, or global coordinates. See Bulk Data PARAM
ELFORCEN entry

ENFORCED
6.3.1.7 ENFORCED
Description:
Requests a run in which the displacements (all 3 translations and rotations) are specified in a file whose
name is given as part of this command. The situation in which this might be useful is one in which all grid
displacements are known from test data and the user would like to get other outputs (e.g. stresses) due to
these displacements.

Format:
ENFORCED = filename

Examples:
ENFORCED = Case1-displacements-rotations.txt

Remarks:
1. filename is a text file with NGRID+1 records (where NGRID are the number of grids in the model)
a) Record 1 is a comment line
b) Records 2 through NGRID+1 have the following in CSV format for each grid:
grid ID, T1, T2, T3, R1, R2, R3
2. An example of the ENFORCED file for 2 grids is:
Displacements and rotations for model A with 3 grids (101, 102)
101, 1.23456D-02, 2.34567D-02, 3.45678D-03, 0.00000D+00, 4.56789D-04, 3.67890D-05
102, 6.54321D-02, 7.65432D-03, 8.76543D-03, 9.87654D-05, 5.43210D-06, 0.00000D-05

3. All grids must have all 6 components specified in the file (i.e. all DOF’s must be in the S-set)
4. Any Case Control requests for SPC’s or MPC’s will result in an error
5. Any Bulk Data ASET or OMIT entries will result in an error

ELSTRAIN
6.3.1.8 ELSTRAIN
Description:
Requests output of strains for selected elements. See STRAIN entry for description

ELSTRESS
6.3.1.9 ELSTRESS
Description:
Requests output of stresses for selected elements. See STRESS entry for description

FORCE
6.3.1.10 FORCE
Description:
Requests element engineering and/or node forces. See ELFORCE entry.

GPFORCES
6.3.1.11 GPFORCES
Description:
Requests output of grid point force balance in the global coordinate system for selected grids.

Format:
 ALL 


GPFO[RCES] =  n 
NONE 



Examples:
GPFO = ALL (requests output of grid point force balance for all grid points)
GPFO = 45 (requests output of grid point force balance for grid points included in SET 45)

Options:
Option
ALL
n
NONE

Meaning
Grid point force balance for all grid points in the model will be output
ID of a SET Case Control entry. Grid point force balance for the grid points defined by
this set will be output. Integer > 0, no default value.
No grid point force balance will be output

Remarks:
1. NONE is used to override an overall output request made above the SUBCASE level.

LABEL
6.3.1.12 LABEL
Description:
Specifies a third text line to be printed in the output file.

Format:

LABE[L] = [optional text material up to, and including, column 80]

Remarks:
1. This line of text will be printed in the output file and can be different for each subcase

LOAD
6.3.1.13 LOAD
Description:
Indicates what applied loads (identified in the Bulk Data) are to be used for a solution.

Format:
LOAD = n

Examples:
LOAD = 98 (requests load set 98 be used)

Options:
Option
n

Meaning
Set ID of a load (must be the ID of at least one of the following Bulk data entries: LOAD,
FORCE, GRAV, MOMENT, PLOAD2). Integer > 0, no default value.

Remarks:
1. If the Case Control LOAD entry identifies a Bulk Data LOAD entry (load combining entry), then n must
not appear as a set ID on any of the Bulk Data FORCE, GRAV, MOMENT or PLOAD2 entries that
are in the input data file.
2. The Case Control LOAD entry must be present if a static loading is desired in a solution.

MEFFMASS
6.3.1.14 MEFFMASS
Description:
Requests calculation and output of modal effective masses in an eigenvalue solution.

Format:
MEFFMASS

Remarks:
1. This entry may appear in the Case Control section for eigenvalue extraction solutions.
2. See Bulk Data PARAM MEFMLOC for the reference point to use in calculating effective masses
in Craig-Bampton (SOL 31) analyses

METHOD
6.3.1.15 METHOD
Description:
Indicates what eigenvalue extraction method (identified in the Bulk Data on an EIGR or EIGRL entry) is to
be used for an eigenvalue solution.

Format:
METH[OD] = n

Examples:
METHOD = 18 (requests that eigenvalue extraction method 18 be used)

Options:
Option
n

Meaning
Set ID of a Bulk data EIGR entry. Integer > 0, no default value.

Remarks:
1. This entry must appear in the Case Control section for all eigenvalue extraction solutions.

MPC
6.3.1.16 MPC
Description:
Indicates what multipoint constraints (identified in the Bulk Data) are to be used for a solution.

Format:
MPC = n

Examples:
MPC = 47 (requests multi point constraint set 47, defined in Bulk Data, be used)

Options:
Option
n

Meaning
Set ID of an MPC and/or MPCADD Bulk data entry. Integer > 0, no default value.

Remarks:
1. There can be only one Case Control MPC entry per solution. It should appear in the Case Control
section above any SUBCASE definitions.

MPCFORCES
6.3.1.17 MPCFORCES
Description:
Requests output of multi point constraint forces in the global coordinate system for selected grids. Multi
point constraint forces consist of forces due to directly defined MPC’s and also due to rigid elements
(which are automated, internally in MYSTRAN, as MPC’s)

Format:
 ALL 


MPCF[ORCES] =  n 
NONE 



Examples:
MPCF = ALL (requests output of multi point constraint forces for all grid points)
MPCF = 45 (requests output of multi point constraint forces for grid points included in SET 45)

Options:
Option
ALL
n
NONE

Meaning
Multi point constraint forces for all grid points in the model will be output
ID of a SET Case Control entry. Multi point constraint forces for the grid points defined by
this set will be output. Integer > 0, no default value.
No Multi point constraint forces will be output

Remarks:
1. NONE is used to override an overall output request made above the SUBCASE level.

MPFACTOR
6.3.1.18 MPFACTOR
Description:
Requests calculation and output of modal participation factors in an eigenvalue solution.

Format:
MPFACTOR

Remarks:
1. This entry may appear in the Case Control section for eigenvalue extraction solutions.

OLOAD
6.3.1.19 OLOAD
Description:
Requests output of applied loads in the global coordinate system for selected grids.

Format:
 ALL 


OLOA[D] =  n 
NONE 



Examples:
OLOAD = ALL (requests output of applied loads for all grid points)
OLOAD = 45 (requests output of applied loads for grid points included in SET 45)

Options:
Option
ALL
n
NONE

Meaning
Applied loads for all grid points in the model will be output
ID of a SET Case Control entry previously defined. Applied loads for the grid points
defined by this set will be output. Integer > 0, no default value.
No applied loads will be output

Remarks:
1. NONE is used to override an overall output request made above the SUBCASE level.

SET
6.3.1.20 SET
Description:
Defines sets of grid points or elements for which output is desired.

Format:
SET n = {i1[, i 2 , i 3 , i 4 THRU i 5 , EXCEPT i 6 , i 7 , i 8 THRU i 9 ]}

Examples:
SET 39 = 2998
SET 57 = 101 THRU 298
SET 12 = 301, 305, 491 THRU 672 EXCEPT 501

Options:
Option
n

Meaning
Set ID number. Integer > 0, no default.

i1, i2, i3, etc.

Individual grid point or element numbers.

i4 THRU i5

Inclusive group of grid or element numbers.

EXCEPT

Grid or element numbers following EXCEPT (but before next THRU) will be excluded from
the previous THRU group.

Remarks:
1. Any number of SETs can be defined as long as the ID numbers are unique integers. The SET logical
entry can consist of multiple physical entries, each of 80 columns max. If a SET definition requires
more than one physical entry each entry (except the last) must end with a “,”
2. Ranges in THRU statements must be increasing (that is, i4 must be less than i5 in the above
example). It is acceptable that some grid or element numbers in the THRU range do not exist.
However, all grids or elements that are in the THRU range will be included in the SET.
3. Whether the set indicates grids or elements is dependent on the context in which the SET is used. If
DISP = 39 output is requested, then the integers in SET 39 will be interpreted as grid point numbers.
If ELFORCE = 39 output is requested, then the integers in SET 39 will be interpreted as element
numbers.

SPC
6.3.1.21 SPC
Description:
Indicates what single point constraints (identified in the Bulk Data) are to be used for a solution.

Format:
SPC = n

Examples:
SPC = 74 (requests single point constraint set 74 be used)

Options:
Option
n

Meaning
Set ID of at least one SPC, SPC1 and/or SPCADD Bulk data entries. Integer > 0, no
default value.

Remarks:
1. There can be only one Case Control SPC entry per solution. It should appear in the Case Control
section above any SUBCASE definitions.

SPCFORCES
6.3.1.22 SPCFORCES
Description:
Requests output of single point constraint (SPC) forces in the global coordinate system for selected grids.

Format:
 ALL 


SPCF[ORCES] =  n 
NONE 



Examples:
SPCF = ALL (requests output of SPC forces for all grid points)
SPCFORCES = 45 (requests output of SPC forces for grid points included in SET 45)

Options:
Option
ALL
n
NONE

Meaning
SPC forces for all grid points in the model will be output.
ID of a SET Case Control entry previously defined. SPC forces for the grid points defined
by this set will be output. Integer > 0, no default value.
No SPC forces will be output.

Remarks:
1, NONE is used to override an overall output request made above the SUBCASE level

STRAIN
6.3.1.23 STRAIN
Description:
Requests output of stresses for selected elements.

Format:
 ALL 
 VONMISES   CENTER  

STRA IN 

=  n 
MAXS or SHEAR  CORNER  NONE 



Examples:

Options:
Option
VONMISES

Meaning
Requests von Miises strain (default)

MAXS or
SHEAR

Requests maximum shear strain for shell elements and octrahedral strain for solid
elements

CENTER

Requests strains at the center of shell and solid elements (default)

CORNER

Requests strains at the element corners for the QUAD4 and QUAD4K elements, in
addition to strains at the element center

ALL
n
NONE

Strains for all elements in the model will be output.
ID of a SET Case Control entry previously defined. Strains for the elements defined by
SET n will be output. Integer > 0, no default value.
No displacements will be output.

Remarks:
1. NONE is used to override an overall output request made above the SUBCASE level
2. ELSTRAIN is an alternate form of this Case Control command
3. The options VONMISES, MASS (or SHEAR), CENTER and CORNER will apply for all subcases

STRESS
6.3.1.24 STRESS
Description:
Requests output of stresses for selected elements.

Format:
 ALL 
 VONMISES   CENTER  

STRE SS  

=  n 
MAXS or SHEAR  CORNER  NONE 



Examples:

Options:
Option
VONMISES

Meaning
Requests von Miises stress (default)

MAXS or
SHEAR

Requests maximum shear stress for shell elements and octrahedral stress for solid
elements

CENTER

Requests stresses at the center of shell and solid elements (default)

CORNER

Requests stresses at the element corners for the QUAD4 and QUAD4K elements, in
addition to stresses at the element center

ALL
n
NONE

Stresses for all elements in the model will be output.
ID of a SET Case Control entry previously defined. Stresses for the elements defined by
SET n will be output. Integer > 0, no default value.
No displacements will be output.

Remarks:
1. NONE is used to override an overall output request made above the SUBCASE level
2. ELSTRESS is an alternate form of this Case Control command
3. The options VONMISES, MASS (or SHEAR), CENTER and CORNER will apply for all subcases

SUBCASE
6.3.1.25 SUBCASE
Description:
Beginning of the portion of the Case Control section that defines the options to be used in one subcase.
Multiple subcases must be used when solution with separate static loads in one run is desired.

Format:
SUBC[ASE] = n

Examples:
SUBCASE = 361

Options:
Option
n

Meaning
Set ID of a subcase. Integer > 0, no default value.

Remarks:
1. There can be multiple subcases and there is no restriction on the integer numbers used for subcase
IDs
2. All Case Control entries following a SUBCASE entry (up to the next SUBCASE Case Control entry)
identify the conditions for solution (loads and output) for this subcase. Case Control entries “above”
the SUBCASE level will be used for all subcases unless specifically overridden in the subcase
definition.

SUBTITLE
6.3.1.26 SUBTITLE
Description:
Specifies a second text line to be printed in the output file.

Format:

SUBT[ITLE] = [optional text material up to, and including, column 80]

Remarks:
1. This line of text will be printed in the output file and can be different for each subcase.

TEMPERATURE
6.3.1.27 TEMPERATURE
Description:
Indicates temperature distributions (identified in the Bulk Data) that are to be used for a statics solution.

Format:
TEMP[ERATURE] = n

Examples:
TEMP = 174 (requests temperature set 174 be used)
TEMPERATURE = 13 (requests temperature set 13 be used)

Options:
Option
n

Meaning
Set ID of Bulk Data TEMP, TEMPD, TEMPRB and/or TEMPP1 cards. Integer > 0, no
default value.

Remarks:
1. Thermal loads can be used in combination with other static loads in any subcase but must be
selected in Case Control with the TEMPERATURE = n card.

TITLE
6.3.1.28 TITLE
Description:
Specifies a text line to be printed in the output file.

Format:

TITLE = [optional text material up to, and including, column 80]
Remarks:
1. This line of text will be printed in the output file and can be different for each subcase

VECTOR
6.3.1.29 VECTOR
Description:
Requests eigenvector output. See DISPLACEMENT entry.

6.4

Bulk Data

The major function of the Bulk Data Section is to define the finite element model and the loading and
constraints. In the case of loading and constraints, the Bulk Data entries have a set ID which must be
chosen in Case Control for the particular load or constraint to be applied.
The entries for each of the major purposes are enumerated below. A detailed explanation of each is
contained in the following section. An ENDDATA entry is considered as the last, and mandatory, entry in
the Bulk data Section.
 Geometry/scalar point definition



GRID

Defines grid point ID and location, coordinate systems for the grid
location and for the global coordinate system, and permanent single
point constraints.

GRDSET

Defines default values for coordinate systems and permanent SPC’s for
GRID entries whose corresponding fields are blank.

SPOINT

Defines a scalar point to which elastic and mass elements may be
attached.

Grid point sequencing
SEQGP

Used to define the internal sequence order for grid points so as to obtain
a banded stiffness matrix. If not input, then the grid order is set to, either:
grid numerical order (default) or grid input order (using PARAM
SEQUENCE)

 Coordinate system definition (i = 1 or 2)

CORDiR

Defines a rectangular coordinate system.

CORDiC

Defines a cylindrical coordinate system.

CORDiS

Defines a spherical coordinate system.

 Element connection definition

Scalar and bushing elastic elements
CBUSH

Spring element with geometry definition

CELAS1

Defines a spring element ID, property ID and the grid/degrees of freedom
to which the spring element is connected.

CELAS2

Defines a spring element ID, stiffness and the grid/degrees of freedom to
which the spring element is connected.

CELAS3

Defines a spring element ID, property ID and the scalar points to which
the spring element is connected.

CELAS4

Defines a spring element ID, stiffness and the scalar points to which the
spring element is connected.

1D elastic elements
CBAR

Defines a bar (axial load, bending, torsion) element ID, property ID and
the grid connections and v vector (which, together with the bar axis,
defines the orientation of the bar cross-section in the model).

BAROR

Defines default values of property ID and v vector for the CBAR entry.

CROD,

Defines a rod (axial load and torsion) element ID, property ID and the
grid connections. The bar element can be used to describe 1D element
extension, as well.

CONROD

Alternate form of CROD

2D elastic elements
CQUAD4K

Defines a thin quadrilateral plate (membrane, bending, twist) element ID,
property ID and the grid points to which the quad element is connected.

CQUAD4

Defines a thick quadrilateral plate (membrane, bending, twist) element
ID, property ID and the grid points to which the quad element is
connected.

CTRIA3K

Defines a thin triangular plate (membrane, bending, twist) element ID,
property ID and the grid points to which the triangular element is
connected.

CTRIA3

Defines a thick triangular plate (membrane, bending, twist) element ID,
property ID and the grid points to which the triangular element is
connected.

CSHEAR

Defines a thin quadrilateral element that carries only in-plane shear

3D elastic elements
CHEXA

Defines a hexahedron element with either 8 or 20 nodes.

CPENTA

Defines a pentahedron element with either 6 or 15 nodes.

CTETRA

Defines a tetrahedron element with either 4 or 10 nodes.

R- elements
The R-elements (currently RBE2 and RBE3) are used to generate internal multi-point
constraint equations (MPC’s) that define a dependence of some degrees of freedom of
the model with respect to the other degrees of freedom in the model.
RBE2

Defines a rigid portion of the finite element model by specifying an
element ID plus a number of dependent grid points that will behave in a
rigid fashion relative to the six components of motion at a specified
independent grid point. The degrees of freedom for the dependent grids
are also specified. In its most simplistic form, the RBE2 can be used to
define, for instance, a rigid 1-D bar or a rigid 2-D element.

RBE3

Defines one dependent grid point (and the dependent degrees of
freedom at that grid point) and one or more grids (and their degrees of
freedom) that the dependent degrees of freedom depend on. The most
common use of this element is to distribute loads or mass specified at
the dependent grid to ones at the independent grid. This is very different
than the RBE3 which is a rigid element. In general, the dependent grid
on the RBE3 should not be connected via elastic or rigid elements to the
rest of the structure except via the RBE3 element on which it is defined.
There is also a provision for specifying weighting factors at the
independent grids (which in many cases are just 1.0).

RSPLINE

Constraint element that defines interpolations of displacements between
it’s 2 ends. Displacements and rotations avout a line between the 2 ends
are interpolated linearly. Displacements perpendicular to the line are
interpolated cubically. Rotations perpendicular to the line are
interpolated quadrically.

Scalar mass elements
CMASS1

Defines a mass element ID, property ID and the grid/degrees of freedom
to which the mass element is connected.

CMASS2

Defines a mass element ID, stiffness and the grid/degrees of freedom to
which the mass element is connected.

CMASS3

Defines a mass element ID, property ID and the scalar points to which
the mass element is connected.

CMASS4

Defines a mass element ID, stiffness and the scalar points to which the
mass element is connected.

User defined elements
CUSERIN

Elements whose elastic properties will be defined via stiffness and mass
matrices on disk files. The CUSERIN entry defines the degrees of
freedom that the element is connected to. These elements are used in
substructure analyses (primarily Craig-Bampton dynamic analyses).

 Element property definition

Scalar elastic element
PELAS

Defines a spring element property ID and the stiffness, damping and
stress recovery values for a ELAS1 scalar spring element

PBUSH

Defines the elastic properties of a CBUSH element

1D elastic elements
PBAR, PBARL Defines a bar property ID and material ID and the bar properties,
including: cross-sectional area, area moments, and cross-products, of
inertia, torsional constant, mass per unit length, stress recovery locations
on the cross-section and area factors for shear flexibility.
PROD

Defines a rod property ID and material ID and the rod properties,
including: cross-sectional area, torsional constant, torsion stress
recovery coefficient and mass per unit length

2D elastic elements
PSHEAR

Defines the elastic properties of a CSHEAR element

PSHELL

Defines a 2D plate element property ID and material IDs and the plate
properties, including: thickness, .bending moment of inertia ratio, shear
thickness ratio, fiber distances for stress calculation, mass per unit
length.

PCOMP, 1

Defines the properties of a 2D composite plate element with n plies.

3D elastic elements
PSOLID

Defines a 3D solid element property ID and material ID and integration
parameters.

User elements
PUSERIN

Defines information needed to locate the matrices (specified on disk
files) for CUSERIN elements.

 Element material definition

MAT1

Defines a material ID and the material properties, including: Young’s
modulus, shear modulus, Poisson’s ratio, material mass density, thermal
expansion coefficient, reference temperature, and a damping coefficient.

MAT2

Defines a 2D anisotropic material.

MAT8

Defines an orthotropic material.

MAT9

Defines an anisotropic material.

PMASS

Defines scalar mass for elements defined on CMASS2,4 entries.

 Grid point mass

CONM2

Defines a concentrated mass at a grid point, including: mass ID, grid
where mass is located, the mass value, the offsets from the grid to the
mass center of gravity (c.g.), the six independent moments and products
of inertia of the mass about its c.g., and the coordinate system in which
the offsets and moments of inertia are specified.

 Applied loads

FORCE

Defines a concentrated force at a grid point, including: load ID, grid ID at
which the force acts, coordinate system in which the force is specified,
and the magnitude and direction of the force.

MOMENT

Defines a concentrated moment at a grid point, including: load ID, grid ID
at which the moment acts, coordinate system in which the moment is
specified, and the magnitude and direction of the moment.

GRAV

Defines an acceleration vector for the finite element model, including:
load ID, coordinate system in which the acceleration vector is specified,
and magnitude and direction of the acceleration vector. MYSTRAN
creates a static load that is applied to a model to simulate a gravity type
of loading but with rigid body motion restrained.

PLOAD2

Defines a pressure load for 2D elements, including: load ID, pressure
magnitude, and element IDs for the elements that are to have the
pressure load.

PLOAD4

Defines a pressure load for 2D elements, including: load ID, pressure
magnitudes at up to 4 grids, and element IDs for the elements that are to
have the pressure load.

LOAD

Defines a static load for the finite element model that is a linear
combination of loads that are defined on FORCE, MOMENT, GRAV and
PLOAD2 entries, including: ID of this load combination, a scale factor to
be applied to all loads being combined, and load set IDs and magnitudes
of the various load sets being combined.

RFORCE

Defines an angular velocity and optional angular acceleration of the finite
element model about some defined grid point and in some defined
coordinate system.

SLOAD

Defines a.

 Thermal loads (all are used by MYSTRAN to calculate loads on the model)

TEMPD

Defines an overall constant temperature for the finite element model
including: temperature set ID and the temperature value.

TEMP

Defines a temperature for a grid point including: temperature set ID, the
grid ID, and the temperature value

TEMPRB

Defines a temperature field for the bar element including: temperature
set ID, the average temperature of the cross-section at the two bar ends,
the two temperature gradients through the bar cross-section at each of
the two ends.

TEMPP1

Defines a temperature field for 2D elements including: temperature set
ID, the average temperature of the element at its mid-plane, the
temperature gradient through the element.

 Single point constraints (SPC)

SPC

Defines a constraint for a single degree of freedom including: SPC set
ID, the grid and degree of freedom component number, and the
constraint value. If the constraint value is nonzero (that is, an enforced
displacement), MYSTRAN calculates equivalent grid forces and applies
them to the model.

SPC1

Defines degrees of freedom where displacement is zero. The definition
Includes: the SPC set ID, the degree of freedom component number and
the grids that are to be constrained.

SPCADD

Defines an SPC as a union of SPC’s defined via SPC and/or SPC1 Bulk
data entries.

 Multi point constraints (MPC)

MPC

Defines a dependence of one degree of frrrdom on one or more other
degrees of freedom.

MPCADD

Defines an MPC as a union of MPC’s defined via MPC Bulk data entries.

 Boundary degrees of freedom for Craig-Bampton (CB) analyses

SUPORT

Defines degrees of freedom at the boundary of a CB model.

 Analysis degrees of freedom (only needed when Guyan reduction is employed)

ASET

Defines degrees of freedom that are to be included in the A-set by
specifying pairs of component/grid IDs

ASET1

Defines degrees of freedom that are to be included in the A-set by
specifying a component number and a list of grid IDs

OMIT

Defines degrees of freedom that are to be included in the O-set by
specifying pairs of component/grid IDs

OMIT1

Defines degrees of freedom that are to be included in the O-set by
specifying a component number and a list of grid IDs

 Eigenvalue extraction

EIGR

Defines the data needed during eigenvalue extraction by the Givens
(GIV), modified Givens( MGIV) or Inverse Power (INV) method,
including: eigenvalue extraction set ID, extraction method, frequency
range to search, number of estimated and desired eigenvalues, the
eigenvector orthogonality criteria, and method of eigenvector
renormalization.

EIGRL

Defines the data needed during eigenvalue extraction by the Lanczos
method, including: eigenvalue extraction set ID, desired eigenvalues,
and method of eigenvector renormalization. Either ARPACK or TRLan
(Thick Restart Lanczos) can be requested. Use of TRLan requires
converting the eigenproblem from generalized format to standard which
can be quite time and resource consuming. On the other hand,
ARPACK K and M matrices must be stored in banded form which can
require a considerable amount of memory.

 Partitioning vectors (used in conjunction with the OUTPUT4 and PARTN Exec Control entries)

PARVEC

The format for this entry is similar to the Bulk Data SPC entry and gives
the grid/component pairs of the degrees of freedom (in any of the
allowable displacement sets 3 ) that define the rows or columns to be
partitioned from the OUTPUT4 matrix.

PARVEC1

The format for this entry is similar to the Bulk Data SPC1 entry and gives
the same information as for the PARVEC entry, only in a different format

 Degree of freedom set definition (requests output in a row format of a displacement set)

USET

The format for this entry is similar to the Bulk Data SPC entry and
requests a tabular output of selected grid/component pairs, in internal
sort, that are members of a named displacement set (e.g. the A-set).

USET1

The format for this entry is similar to the Bulk Data SPC1 entry and gives
the same information as for the USET entry, only in a different format.

 PARVEC The format for this entry is the same as that for the Bulk Data SPC entry PARAM
Field 2 identifies the parameter name and subsequent fields define the Parameters (used
to control solution options during execution)

PARAM

Field 2 identifies the parameter name and subsequent fields define the
parts of the parameter either as character, integer or real data.

 Debug (used to control debug options during execution)

DEBUG

The word DEBUG must be in field 1. The DEBUG number (I) goes in
field 2 and the value of DEBUG(I) goes in field 3.

 Plot elements (only for compatibility with NASTRAN input data files)

PLOTEL
3

see section 3.6 for a definition of displacement sets

A Bulk Data physical entry contains 80 columns of data in up to 10 fields of 8 columns each. As
discussed in an earlier section, some Bulk data entries require more than the 10 fields in order to specify
all of its data. Thus, a logical entry exists to describe all of the data required for one Bulk data entry. This
logical entry can consist of more than one physical entry with the initial entry of 10 fields being called the
“parent” and subsequent continuation entries called “child” entries. Whenever a logical entry requires
continuation entries, or is capable of having continuation entries, this is noted.
Each of the Bulk Data entries is described with:
 Name of the entry and a brief sentence describing its function.
 Format of the entry with names of the data items that go in each of the (up to) 10 fields.
 Numerical example(s).
 Description of each fields’ contents, data type (i.e. character, integer, real) and default values.
 Remarks regarding the entry.

An example of the format section for the PBAR Bulk Data entry is shown below with some explanation of
the format. The data can be entered in the traditional way as shown with 10 fields of 8 columns each.
Alternatively, the 10 fields can be separated by either commas (referred to as comma separated values,
or CSV) or tabs (TSV)

Format (small field entry with 8 columns for each of the 10 fields):
1
PBAR
+CONT1
+CONT2

2
PID
Y1
K1

3
MID
Z1
K2

4
A
Y2
I12

5
I1
Z2

6
I2
Y3

7
J
Z3

8
MPL
Y4

9
Z4

10
+CONT1
+CONT2

The format section for the PBAR has four rows of text. Note the following:


Row 1 of the format section (for all Bulk Data entry descriptions) is only to show the field number
of the Bulk Data entry and is not part of the input for the Bulk Data entry. Each of the 10 fields is
8 columns wide.



Row 2 is the “parent” entry for the entry illustrated here (PBAR) and is always required.


The entry in field 1 is the name of the Bulk Data entry and must be entered exactly as
shown, starting in column 1 of field 1.



Fields 2-9 in general (2-8 in the PBAR above), show names of the data items (in row 1)
for the Bulk Data entry (e.g. PID is the property ID for this PBAR). The data names are to
be replaced by actual data that can be placed anywhere in the field. The data for a
specific field might call for a character or integer or real value and this requirement is
noted for each field. The entry in field 10 is only required if there is a continuation entry.
If no continuation entry will be used, field 10 could contain comments.



If continuation entries are required or optional for the parent entry, they will be shown in rows 3
and on as in the example above.


The entry in field 1 of a continuation must be the same as that in field 10 of the previous
continuation (or parent, in the case of the first continuation).



The entry in fields 2-9, like those on the parent are to contain data that can be placed
anywhere in the field.



The entry in field 10 is only required if there is to be another continuation entry to follow.



Continuation entries must contain a “+” sign in column 1 of field 10 of one entry and field
1 of the following entry and be the same otherwise. They do not have to be as shown in
the example above (e.g. +CONT1 in field 10 of the parent and in field 1 of the first
continuation entry)



Shaded fields (like field 9 of the parent entry, above, and fields 5-9 of the second continuation
entry), must be left blank.



Data can be character, integer or real but must be of the type specified and with the following
conventions:


Character data can be alphanumeric but must begin with an alpha character. No
quotation marks are to be included. Character data that can go in fields 2-9 are always
spelled out as to what the options are and must be entered exactly as shown (except that
they may be placed anywhere in the field).



Integer data must contain no decimal point or imbedded blanks.



Real data must contain a decimal point and no imbedded blanks. Some examples of
valid real entries are:


1.234567



2.57E-4 or 2.57-4 (i.e. 2.57x10-4)



Each of the Bulk Data entries are described in detail on the following pages

There is also a large field Bulk data entry capability where data fields 2 through 9 of a Bulk Data entry can
be 16 characters long, instead of just 8 characters. This is done in order to allow more precision in the
input for real data fields. Recall that each small field physical entry has 10 fields of 8 characters each. In
the large field entry, there are 2 physical entries required to specify all of the data from a small field entry.
The following shows the correspondence between small and large field entries:
Small field PBAR parent entry (1 physical entry for the 10 fields of data):
1
PBAR

2
PID

3
MID

4
A

5
I1

6
I2

7
J

8
MPL

10
+CONT1

Format (large field entry with 16 columns for each of fields 2 through 9):
Large field PBAR parent entry (2 physical entries needed to specify the 10 fields of data)
1
PBAR*
link
*

2
PID

3
MID

4
A

5
I1

6
I2

7
J

8
MPL

link
*

Note that an * is used after PBAR to indicate that this is a large field entry. In addition, in order to link the
2 halves of the physical entry, an * is placed in column 73 of the 1st part of the entry and in column 1 of
the 2nd part of the entry. Fields 1 and 10, as well as the last field of the 1st part and the 1st field of the 2nd
part, are 8 columns each. Fields 2 through 9 are 16 columns each.

6.4.1 Detailed Description of Bulk Data Entries
The following sections describe the input required for each of the different Bulk Data entries.

ASET
6.4.1.1 ASET
Description:
Define degrees of freedom to go into the analysis set (A-set)

Format:
ASET

2345

124

134

Example:
ASET

Data Description:
Field

Contents

Type

Default

ID numbers of grids

Integer > 0

None

Displacement component numbers

Integers 1-6

None

Remarks:
1. The degrees of freedom defined by grids Gi, components Ci will be placed in the mutually exclusive
A-set. These degrees of freedom cannot have been defined to be in any other mutually exclusive set
(i.e.. M, S or O-sets).
2. If there are no ASET (or ASET1) and no OMIT (or OMIT1) entries, all degrees of freedom not in the M
or S-set will be placed in the A-set
3. If ASET (or ASET1) entries are present in the input data file, then all degrees of freedom not specified
on these entries and also not in the M or S-sets will be placed in the O-set.
4. If both ASET (or ASET1) and OMIT (or OMIT1) are present, then all degrees of freedom not in the M
and S-sets must be explicitly defined on these ASET (or ASET1) and OMIT (or OMIT1) entries.
5. Up to four pairs of Gi, Ci can be specified on one ASET entry. For more pairs, use additional ASET
entries (i.e. there is no continuation entry for ASET).

ASET1
6.4.1.2 ASET1
Description:
Define degrees of freedom to go into the analysis set (A-set)

Format No. 1:
ASET1
+Q001

C
G8

G1
G9

G2
(etc)

THRU

135

17934

THRU

19012

+Q001

Format No. 2:
ASET1

Example:
ASET1

Data Description:
Field

Contents

Type

Default

ID numbers of grids. G2 > G1

Integer > 0

None

Displacement component numbers

Integers 1-6

None

Remarks:

1. In Format No. 2, any grid whose ID is in the range G1 through G2 will have component C defined in
the A-set.
2. The degrees of freedom defined by grids GI, components Ci will be placed in the mutually exclusive
A-set. These degrees of freedom cannot have been defined to be in any other mutually exclusive set
(i.e.. M, S or O-sets).
3. If there are no ASET (or ASET1) and no OMIT (or OMIT1) entries, all degrees of freedom not in the
M or S-set will be placed in the A-set
4. If ASET (or ASET1) entries are present in the input data file, then all degrees of freedom not specified
on these entries and also not in the M or S-sets will be placed in the O-set.
5. If both ASET (or ASET1) and OMIT (or OMIT1) are present, then all degrees of freedom not in the M
and S sets must be explicitly defined on these ASET (or ASET1) and OMIT (or OMIT1) entries.
6. Up to four pairs of Gi, Ci can be specified on one ASET entry. For more pairs, use additional ASET
entries (i.e. there is no continuation entry for ASET).

BAROR
6.4.1.3 BAROR
Description:
Define default values for the CBAR entry.

Format No.1:
PID

PID

BAROR

1.3

BAROR

1563

BAROR

3.5

0.7

Format No.2:
BAROR

Examples:

Data Description:
Field

Contents

Type

Default

PID

ID number of a PBAR Bulk data entry

Integer > 0
or blank

None

ID of a grid used to define the orientation v vector

Integer > 0
or blank

None

The three components of the orientation v vector specified in the
global coordinate system for grid G1 on the CBAR entry.

Real or blank

None

Remarks:
1. Only one BAROR entry is allowed in the input data file. Any data entered on a BAROR entry will be
used unless overridden on a CBAR entry. If format 1 is used, all three components of the v vector
must be entered.
2. The orientation v vector can be specified using either a grid point (G0) or the components Vi. Either
one of these, in conjunction with the grid G1 on the CBAR entry, defines the orientation vector.
3. See CBAR entry for remarks concerning the v vector.

CBAR
6.4.1.4 CBAR
Description:
1D bar element for axial load, bending and torsion

Format No. 1:
1
CBAR
+CONT

2
EID
P1

3
PID
P2

4
G1
W11

5
G2
W12

6
G0
W13

W21

W22

W23

EID
P1

PID
P2

GA
W11

GB
W12

V1
W13

V2
W21

V3
W22

W23

CBAR
+BAR98

98
456

43
13

1234
0.0

56
0.2

78
0.3

0.1

0.05

0.10

CBAR

1234

0.5

1.5

3.2

10
+CONT

Format No. 2:
CBAR
+CONT

+CONT

Examples:
+BAR98

Data Description:
Field

Contents

Type

Default

EID

Element ID number

Integer > 0

None

PID

ID number of a PBAR Bulk data entry

Integer > 0

EID

ID numbers of the grids to which the element is attached

Integer > 0

None

ID of a grid used to define the orientation v vector

Integer > 0

None

Components of the orientation v vector

Real

None

G1, G2

P1, P2

Pin flags for bar ends 1 and 2 respectively

Integers 1-6

None

W1j

Components of the bar offset from grid G1

Real

None

W2j

Components of the bar offset from grid G2

Real

None

Remarks:
1. No other element in the model may have the same element ID
2. The v vector is a vector from either: (a) grid G1 to grid G0, or (b) from grid G1 in the direction of the
vector defined by V1, V2, V3. These components are measured in the global coordinate system of
grid G1 (see GRID entry for definition of the global coordinate system for a grid). If format 1 is used,
all three components of the v vector must be entered.

3. The local x axis of the element is a vector from G1 through G2 (see Figure 4-3)
4. The x axis and the v vector define a plane. On the PBAR entry, I1 is the bending moment of inertia in
this plane.

CBUSH
6.4.1.5 CBUSH
Description:
Spring element

Format No. 1:
1
CBUSH
+CONT

2
EID
S

3
PID
OCID

4
G1
S1

5
G2
S2

6
G0
S3

9
CID

10
+CONT

EID
S

PID
OCID

GA
S1

GB
S2

V1
S3

CID

+CONT

CBUSH
+BAR98

98
456

43
13

1234
0.0

56
0.2

78
0.3

CBAR

1234

0.5

Format No. 2:
CBUSH
+CONT

Examples:
+BAR98

1.5

3.2

Data Description:
Field

Contents

Type

Default

EID

Element ID number

Integer > 0

None

PID

ID number of a PBAR Bulk data entry

Integer > 0

EID

ID numbers of the grids to which the element is attached

Integer > 0

None

ID of a grid used to define the orientation v vector

Integer > 0

None

Components of the orientation v vector

Real

None

Element coordinate system identification (0 is basic system) If blank,
the element system is defined by G0 or Vi

Integer >= 0
or blank

None

Location of spring

0.< Real < 1.

0.5

ID of coordinate system used in defining the offstes. OCID = -1
indicates that the offsets are specified in the element coordinate
system

Integer >= -1

-1

Real

G1, G2

CID
S
OCID

Components of spring offset

Remarks:
1. No other element in the model may have the same element ID

2. If CID >= 0 the element x axis is along the x axis of coordinate system CID, etc.
3. A V vector must be specified. That is, fields 6-9 cannot all br blank
4. GB cannot be blank
5. The following pertains to OCID:
(a) OCID = -1 (or blank) means S is used and Si are ignored
(b) OCID >= 0 menas S is ignored and Si are used

Ze
V
G0
G1
Ye
G2
Figure 1: BUSH element
Xe

Ze
Ye

(S1,S2,S3)

Xe
G2

Figure 2: Offsets Si

CELAS1
6.4.1.6 CELAS1
Description:
Scalar spring element connected to 2 grid points (GRID’s) with reference to a PELAS entry to define the
real values for the element

Format:
1
CELAS1

2
EID

3
PID

4
G1

5
C1

6
G2

7
C2

789

3731

Example:
CELAS1

Data Description:
Field

Contents

Type

Default

EID

Unique element identification (ID) number

Integer > 0

None

PID

ID number of a PROD Bulk data entry

Integer > 0

EID

ID numbers of the grids to which the element is attached

Integer > 0

None

Component number (1-6) of the degree of freedom, at Gi, to which the
spring element is connected

Integer 1-6

None

Remarks:
1. No other element in the model may have the same element ID
2. The degrees of freedom specified by Gi/Ci must be global degrees of freedom
3. Care must be exercised that rigid body motion of the model is not restrained when using scalar
springs For example, connecting a scalar spring between two translational degrees of freedom that
are not colinear may restrain rigid body motion and give erroneous results

CELAS2
6.4.1.7 CELAS2
Description:
Scalar spring element connected to 2 grid points (GRID’s) with the element stiffness defined

Format:
1
CELAS2

2
EID

3
K

4
G1

5
C1

6
G2

7
C2

789

1.234+06

3731

Example:
CELAS2

Data Description:
Field

Contents

EID

Unique element identification (ID) number

Type

Default

Integer > 0

None

Real

Stiffness value

ID numbers of the grids to which the element is attached

Integer > 0

None

Component number (1-6) of the degree of freedom, at Gi, to which the
spring element is connected

Integer 1-6

None

CELAS3
6.4.1.8 CELAS3
Description:
Scalar spring element connected to 2 scalar points (SPOINT’s) with reference to a PELAS entry to define
the real values for the element

Format:
1
CELAS3

2
EID

3
PID

4
S1

5
S2

789

3731

Example:
CELAS3

Data Description:
Field

Contents

EID
PID
Si

Type

Default

Unique element identification (ID) number

Integer > 0

None

ID number of a PROD Bulk data entry

Integer > 0

EID

ID numbers of the SPOINT’s to which the element is attached

Integer > 0

None

Remarks:
1. No other element in the model may have the same element ID
2. The degrees of freedom specified by Si must be global degrees of freedom
3. Care must be exercised that rigid body motion of the model is not restrained when using scalar
springs For example, connecting a scalar spring between two translational degrees of freedom that
are not colinear may restrain rigid body motion and give erroneous results

CELAS4
6.4.1.9 CELAS4
Description:
Scalar spring element connected to 2 scalar points (SPOINT’s) with the element stiffness defined

Format:
1
CELAS4

2
EID

3
K

4
S1

5
S2

789

3731

Example:
CELAS4

Data Description:
Field

Contents

EID

Unique element identification (ID) number

Stiffness value

ID numbers of the SPOINT’s to which the element is attached

Type

Default

Integer > 0

None

Real

Integer > 0

None

CHEXA
6.4.1.10 CHEXA
Description:
3D solid tetrahedron element

Format No. 1:
1
CHEXA
+CH1
+CH2

2
EID
G7
G15

3
PID
G8
G16

4
G1
G9
G17

5
G2
G10
G18

6
G3
G11
G19

7
G4
G12
G20

8
G5
G13

9
G6
G14

10
+CH1
+CH2

98
43

43
998

101

123

254

621

8945

+CH1

Example:
CHEXA
+CH1

Data Description:
Field

Contents

EID
PID
G1-G20

Type

Default

Unique element identification (ID) number

Integer > 0

None

ID number of a PSOLID Bulk data entry

Integer > 0

None

ID numbers of the grids to which the element is attached. Specify G1G8 for a 4 node HEXA and all 20 for a 20 node HEXA

Integer > 0

None

Remarks:
1. No other element in the model may have the same element ID
2. The first continuation entry is required. The second is only needed for the 20 node element

CMASS1
6.4.1.11 CMASS1
Description:
Scalar mass element connected to 2 grid points (GRID’s) with reference to a PMASS entry to define the
real values for the element

Format:
1
CMASS1

2
EID

3
PID

4
G1

5
C1

789

3731

Example:
CMASS1

Data Description:
Field

Contents

Type

Default

EID

Unique element identification (ID) number

Integer > 0

None

PID

ID number of a PMASS Bulk data entry

Integer > 0

EID

ID number of the grid to which the element is attached

Integer > 0

None

Component number (1-6) of the degree of freedom, at G1, to which
the mass element is connected

Integer 1-6

None

Remarks:
1. No other element in the model may have the same element ID
2. The degrees of freedom specified by Gi/Ci must be global degrees of freedom.
3. For MYSTRAN, the mass can only be connected to 1 grid (not 2 as is allowed in NASTRAN)

CMASS2
6.4.1.12 CMASS2
Description:
Scalar mass element connected to 2 grid points (GRID’s) with the element stiffness defined

Format:
1
CMASS2

2
EID

3
K

4
G1

5
C1

789

1.234+06

3731

Example:
CMASS2

Data Description:
Field

Contents

EID

Unique element identification (ID) number

Type

Default

Integer > 0

None

Real

Stiffness value

ID numbers of the grids to which the element is attached

Integer > 0

None

Component number (1-6) of the degree of freedom, at Gi, to which the
mass element is connected

Integer 1-6

None

CMASS3
6.4.1.13 CMASS3
Description:
Scalar mass element connected to 2 scalar points (SPOINT’s) with reference to a PMASS entry to define
the real values for the element

Format:
1
CMASS3

2
EID

3
PID

4
S1

789

3731

Example:
CMASS3

Data Description:
Field

Contents

EID
PID
Si

Type

Default

Unique element identification (ID) number

Integer > 0

None

ID number of a PMASS Bulk data entry

Integer > 0

EID

ID numbers of the SPOINT’s to which the element is attached

Integer > 0

None

Remarks:
1. No other element in the model may have the same element ID
2. The degrees of freedom specified by Si must be global degrees of freedom.
3. For MYSTRAN, the mass can only be connected to 1 scalar point (not 2 as is allowed in NASTRAN)

CMASS4
6.4.1.14 CMASS4
Description:
Scalar mass element connected to 2 scalar points (SPOINT’s) with the element stiffness defined

Format:
1
CMASS4

2
EID

3
K

4
S1

789

3731

Example:
CMASS4

Data Description:
Field

Contents

EID

Unique element identification (ID) number

Stiffness value

ID numbers of the SPOINT’s to which the element is attached

Type

Default

Integer > 0

None

Real

Integer > 0

None

CONM2
6.4.1.15 CONM2
Description:
Concentrated mass at a grid point

Format:
1
CONM2
+CONT

2
EID
I11

3
G
I21

4
CID
I22

5
M
I31

6
X1
I32

7
X2
I33

8
X3

98
123.

354
-45.

29
321.

0.5
12.

0.3
-43.

1.2
567.

0.65

10
+CONT

Example:
CONM2
+1002

+1002

Data Description:
Field

Contents

EID
G
CID

Type

Default

Element identification (ID) number

Integer > 0

None

ID number of the grid to which the mass is attached

Integer > 0

None

ID number of a coordinate system defined on a CORD2C, CORD2R or
CORD2S Bulk Data entry

Integer > 0

Mass value

Real

Offset distances from grid G to the center of gravity of M in coordinate
system CID

Real

Iij

The 6 independent moments of inertia of M about its center of gravity
measured in coordinate system CID.

Real

Remarks:
1. EID must be unique among all CONM2 entries
2. The continuation entry is optional.
3. The moments of inertia I11, I22 and I33 (if entered) must be > 0.
4. A blank entry for CID implies the basic coordinate system.

CONROD
6.4.1.16 CONROD
Description:
1D elastic rod element for axial load and torsion with properties

Format:
1
CROD

2
EID

3
PID

4
G1

5
G2

1234

6
A

7
J

8
C

9
NSM

Example:
CROD

Data Description:
Field

Contents

EID
PID
G1, G2

Type

Default

Unique element identification (ID) number

Integer > 0

None

ID number of a PROD Bulk data entry

Integer > 0

EID

ID numbers of the grids to which the element is attached

Integer > 0

None

Bar cross-sectional area

Real

Torsional constant

Real

Torsional stress recovery coefficient

Real

Mass per unit length

Real

MPL

Remarks:
1. No other element in the model may have the same element ID
2. The local xe axis of the element is a vector from G1 through G2 (see Figure 4-2)

CORD1C
6.4.1.17 CORD1C
Description:
Cylindrical coordinate system definition defined via 3 grid points. Two separate coordinate systems may
be defined on one physical CORD1C entry.

Format:
1
CORD1C

2
CIDA

3
G1A

4
G2A

5
G3A

6
CIDB

7
G1A

8
G2A

9
G3A

Example:
CORD1C

Data Description:
Field

Contents

Type

Default

CID

Coordinate system ID number

Integer > 0

None

G1A, G1B

ID’s of grid points at the origin of systems A, B respectively

Integer > 0

None

G2A, G2B

ID’s of grid points along the z axis of systems A, B respectively

Integer > 0

None

G1C, G2C

ID’s of grid points in the x-z plane of systems A, B respectively

Integer > 0

None

Remarks:
1. See Figure 4-1 for the cylindrical coordinate system notation and the “defining” rectangular system
2. CIDA, CIDB must be unique over all coordinate systems defined in the model.
3. One or 2 coordinate systems may be defined on a single CORD1S entry.
4. The grid points on this entry must be defined in a system that does not involve the system being
defined.
5. See Figure 4-1 for a definition of the various coordinate systems and the directions of the
displacements in those systems.
6. The location of a grid point using this coordinate system is defined by the r, θ , z coordinates of a
cylindrical coordinate system (see Figure 4-1).

100

CORD1R
6.4.1.18 CORD1R
Description:
Rectangular coordinate system definition defined via 3 grid points. Two separate coordinate systems
may be defined on one physical CORD1C entry.

Format:
1
CORD1C

2
CIDA

3
G1A

4
G2A

5
G3A

6
CIDB

7
G1A

8
G2A

9
G3A

Example:
CORD1C

Data Description:
Field

Contents

Type

Default

CID

Coordinate system ID number

Integer > 0

None

G1A, G1B

ID’s of grid points at the origin of systems A, B respectively

Integer > 0

None

G2A, G2B

ID’s of grid points along the z axis of systems A, B respectively

Integer > 0

None

G1C, G2C

ID’s of grid points in the x-z plane of systems A, B respectively

Integer > 0

None

Remarks:
1. See Figure 4-1 for the cylindrical coordinate system notation and the “defining” rectangular system
2. CIDA, CIDB must be unique over all coordinate systems defined in the model.
3. One or 2 coordinate systems may be defined on a single CORD1S entry.
4. The grid points on this entry must be defined in a system that does not involve the system being
defined.
5. See Figure 4-1 for a definition of the various coordinate systems and the directions of the
displacements in those systems.
6. The location of a grid point using this coordinate system is defined by the x, y, z coordinates of a
rectangular coordinate system (see Figure 4-1).

101

CORD1S
6.4.1.19 CORD1S
Description:
Spherical coordinate system definition defined via 3 grid points. Two separate coordinate systems may
be defined on one physical CORD1C entry.

Format:
1
CORD1C

2
CIDA

3
G1A

4
G2A

5
G3A

6
CIDB

7
G1A

8
G2A

9
G3A

Example:
CORD1C

Data Description:
Field

Contents

Type

Default

CID

Coordinate system ID number

Integer > 0

None

G1A, G1B

ID’s of grid points at the origin of systems A, B respectively

Integer > 0

None

G2A, G2B

ID’s of grid points along the z axis of systems A, B respectively

Integer > 0

None

G1C, G2C

ID’s of grid points in the x-z plane of systems A, B respectively

Integer > 0

None

Remarks:
1. See Figure 4-1 for the cylindrical coordinate system notation and the “defining” rectangular system
2. CIDA, CIDB must be unique over all coordinate systems defined in the model.
3. One or 2 coordinate systems may be defined on a single CORD1S entry.
4. The grid points on this entry must be defined in a system that does not involve the system being
defined.
5. See Figure 4-1 for a definition of the various coordinate systems and the directions of the
displacements in those systems.
6. The location of a grid point using this coordinate system is defined by the r, θ,  coordinates of a
spherical coordinate system (see Figure 4-1).

102

CORD2C
6.4.1.20 CORD2C
Description:
Cylindrical coordinate system definition

Format:
1
CORD2R
+CONT

2
CID
C1

3
RID
C2

4
A1
C3

5
A2

6
A3

7
B1

8
B2

9
B3

10
+CONT

26
4.9

41
26.2

4.6
3.4

1.9

13.89

5.76

11.3

2.7

+01A

Example:
CORD2R
+01A

Data Description:
Field

Contents

Type

Default

CID

Coordinate system ID number

Integer > 0

None

RID

ID number of the reference coordinate system in which the points Ai, Bi,
Ci are specified

Integer >= 0
or blank

Coordinates of the origin of CID (specified in RID coordinate system)

Real

None

Coordinates of a point on the z axis of the defining rectangular system
of CID (specified in RID coordinate system)

Real

None

Coordinates of a point in the x-z plane of the defining rectangular
system of CID (specified in RID coordinate system)

Real

None

Remarks:
1. See Figure 4-1 for the rectangular coordinate system notation and the “defining” rectangular system.
2. CID must be unique over all coordinate systems defined in the model.
3. The continuation entry is required.
4. RID = 0 or blank means that the reference coordinate system is the basic coordinate system.
5. CID must be able to be traced, through a chain of coordinate references, back th the basic system.
For example, in the example above CID 26 is defined using system 46. Coordinate system 46 can be
defined using some other coordinate system, and so on, until the final RID is 0 (basic).
6. The basic system need not be defined explicitly. Its axes are implied from the model (grid point
coordinates on GRID entries and coordinate system definitions of all other systems)

103

CORD2R
6.4.1.21 CORD2R
Description:
Rectangular coordinate system definition

Format:
1
CORD2R
+CONT

2
CID
C1

3
RID
C2

4
A1
C3

5
A2

6
A3

7
B1

8
B2

9
B3

10
+CONT

26
4.9

41
26.2

4.6
3.4

1.9

13.89

5.76

11.3

2.7

+01A

Example:
CORD2R
+01A

Data Description:
Field

Contents

Type

Default

CID

Coordinate system ID number

Integer > 0

None

RID

ID number of the reference coordinate system in which the points Ai, Bi,
Ci are specified

Integer >= 0
or blank

Coordinates of the origin of CID (specified in RID coordinate system)

Real

None

Coordinates of a point on the z axis of the defining rectangular system
of CID (specified in RID coordinate system)

Real

None

Coordinates of a point in the x-z plane of the defining rectangular
system of CID (specified in RID coordinate system)

Real

None

104

CORD2S
6.4.1.22 CORD2S
Description:
Spherical coordinate system definition

Format:
1
CORD2S
+CONT

2
CID
C1

3
RID
C2

4
A1
C3

5
A2

6
A3

7
B1

8
B2

9
B3

10
+CONT

26
4.9

41
26.2

4.6
3.4

1.9

13.89

5.76

11.3

2.7

+01A

Example:
CORD2S
+01A

Data Description:
Field

Contents

Type

Default

CID

Coordinate system ID number

Integer > 0

None

RID

ID number of the reference coordinate system in which the points Ai, Bi,
Ci are specified

Integer >= 0
or blank

Coordinates of the origin of CID (specified in RID coordinate system)

Real

None

Coordinates of a point on the z axis of the defining rectangular system
of CID (specified in RID coordinate system)

Real

None

Coordinates of a point in the x-z plane of the defining rectangular
system of CID (specified in RID coordinate system)

Real

None

105

CPENTA
6.4.1.23 CPENTA
Description:
3D solid pentahedron element

Format No. 1:
1
CPENTA
+CP1
+CP2

2
EID
G7
G15

3
PID
G8

4
G1
G9

5
G2
G10

6
G3
G11

7
G4
G12

8
G5
G13

9
G6
G14

101

123

254

1002

10
+CP1
+CP2

Example:
CPENTA

Data Description:
Field

Contents

EID
PID
G1-G15

Type

Default

Unique element identification (ID) number

Integer > 0

None

ID number of a PSOLID Bulk data entry

Integer > 0

None

ID numbers of the grids to which the element is attached. Specify G1G6 for a 6 node PENTA and all 15 for a 15 node PENTA

Integer > 0

None

Remarks:
1. No other element in the model may have the same element ID
2. Continuation entries are only needed for the 15 node element

106

CQUAD4
6.4.1.24 CQUAD4
Description:
Thick quadrilateral plate element. This element has membrane and bending stiffness and can

include flexibility for transverse shear deformations.
Format:
1
CQUAD4

2
EID

3
PID

4
G1

5
G2

6
G3

7
G4

123

935

1357

8
THETA

9
ZOFFS

Example:
CQUAD4

Data Description:
Field

Contents

EID
PID
Gi

Type

Default

Unique element identification (ID) number

Integer > 0

None

ID number of a PSHELL Bulk data entry

Integer > 0

EID

ID numbers of the grids to which the element is attached

Integer > 0

None

THETA

Material property orientation angle in degtees measured from axis
connectiong grids 1 and 2

Real

ZOFFS

Offset of the grid plane to element reference plane

Real

Remarks:
1. No other element in the model may have the same element ID
2. The grids must be numbered in a clockwise or counter clockwise direction around the quadrilateral
element.
3. The local ze axis of the element is in the direction of the cross-product of the diagonal from G1 to G3
with the diagonal from G2 to G4. If the element is rectangular, the local xe axis is the projection of the
vector from G1 to G2 onto the mean plane. If not rectangular, this is rotated to split the angle
between the diagonals. The local ye axis is in the direction of ze cross xe. See Figure 4-5

107

CQUAD4K
6.4.1.25 CQUAD4K
Description:
Thin quadrilateral plate element . This element has membrane and bending stiffness but does not
include flexibility for transverse shear deformations.

Format:
1
CQUAD4K

2
EID

3
PID

4
G1

5
G2

6
G3

7
G4

123

935

1357

Example:
CQUAD4K

Data Description:
Field

Contents

EID
PID
Gi

Type

Default

Unique element identification (ID) number

Integer > 0

None

ID number of a PSHELL Bulk data entry

Integer > 0

EID

ID numbers of the grids to which the element is attached

Integer > 0

None

108

CROD
6.4.1.26 CROD
Description:
1D elastic rod element for axial load and torsion

Format:
1
CROD

2
EID

3
PID

4
G1

5
G2

1234

Example:
CROD

Data Description:
Field

Contents

EID
PID
G1, G2

Type

Default

Unique element identification (ID) number

Integer > 0

None

ID number of a PROD Bulk data entry

Integer > 0

EID

ID numbers of the grids to which the element is attached

Integer > 0

None

Remarks:
1. No other element in the model may have the same element ID
2. The local xe axis of the element is a vector from G1 through G2 (see Figure 4-2)

109

CSHEAR
6.4.1.27 CSHEAR
Description:
Defines a quadrilateral shell element that carries only in-plane shear

Format:
1
CSHEAR

2
EID

3
PID

4
G1

5
G2

6
G3

7
G4

978

564

465

Example:
CSHEAR

Data Description:
Field

Contents

EID
PID
Gi

Type

Default

Unique element identification (ID) number

Integer > 0

None

ID number of a PROD Bulk data entry

Integer > 0

EID

ID numbers of the grids to which the element is attached

Integer > 0

None

Remarks:
1. No other element in the model may have the same element ID
2. The local xe axis of the element is defined the same as for the QUAD4 element

110

CTETRA
6.4.1.28 CTETRA
Description:
3D solid tetrahedron element

Format No. 1:
1
CTETRA
+CT1

2
EID
G7

3
PID
G8

4
G1
G9

5
G2
G10

6
G3

7
G4

101

123

254

8
G5

9
G6

10
+CT1

Example:
CTETRA

Data Description:
Field

Contents

EID
PID
G1-G10

Type

Default

Unique element identification (ID) number

Integer > 0

None

ID number of a PSOLID Bulk data entry

Integer > 0

None

ID numbers of the grids to which the element is attached. Specify G1G4 for a 4 node TETRA and all 10 for a 10 node TETRA

Integer > 0

None

Remarks:
1. No other element in the model may have the same element ID
2. Continuation entries are only needed for the 15 node element

111

CTRIA3
6.4.1.29 CTRIA3
Description:
Thick triangular plate element . This element has membrane and bending stiffness and can

include flexibility for transverse shear deformations
Format:
1
CTRIA3

2
EID

3
PID

4
G1

5
G2

6
G3

123

935

1357

7
THETA

8
ZOFFS

Example:
CTRIA3

Data Description:
Field

Contents

EID
PID
Gi

Type

Default

Unique element identification (ID) number

Integer > 0

None

ID number of a PSHELL Bulk data entry

Integer > 0

EID

ID numbers of the grids to which the element is attached

Integer > 0

None

THETA

Material property orientation angle in degtees measured from axis
connectiong grids 1 and 2

Real

ZOFFS

Offset of the grid plane to element reference plane

Real

Remarks:
1. No other element in the model may have the same element ID
2. The local xe axis of the element is in the direction from G1 to G2. The local ze axis is in the direction
of the cross product of the vector from G1 to G2 with the vector from G1 to G3. The local ye axis is in
the direction of ze cross xe. See Figure 4-5.

112

CTRIA3K
6.4.1.30 CTRIA3K
Description:
Thin triangular plate element . This element has membrane and bending stiffness but does not
include flexibility for transverse shear deformations.

Format:
1
CTRIA3K

2
EID

3
PID

4
G1

5
G2

6
G3

123

935

1357

Example:
CTRIA3K

Data Description:
Field

Contents

EID
PID
Gi

Type

Default

Element identification (ID) number

Integer > 0

None

ID number of a PSHELL Bulk data entry

Integer > 0

EID

ID numbers of the grids to which the element is attached

Integer > 0

None

113

CUSERIN
6.4.1.31 CUSERIN
Description:
User defined element for which the user will supply the mass and stiffness matrices via NASTRAN
formatted INPUTT4 files.

Format 1:
1
CUSERIN
+CU01
+CU11

2
EID
G1
S1

3
PID
C1
S2

4
NG
G2
S3

5
NS
C2
etc

6
CID0
etc

10
+CU01
+CU11

2
EID
G1
S1

3
PID
C1
THRU

4
NG
G2
S2

5
NS
C2

6
CID0
etc

10
+CU01
+CU11

32
201
20001

123
123
THRU

3
202
20008

8
13

198
203

Format 2:
1
CUSERIN
+CU01
+CU11

Example:
CUSERIN
+CU01
+CU02

+CU01
+CU02

Data Description:
Field

Contents

Type

Default

EID

Element identification (ID) number

Integer > 0

None

PID

ID number of a PUSERIN Bulk Data entry

Integer > 0

EID

Number of grid points (GRID’s) that the element is attached to

Integer >= 0

Number of scalar points (SPOINT’s) that the element is attached to

Integer >= 0

CID0

ID of the coordinate system that defines the basic coord system of this
element relative to the basic coord system of the overall model

Integer >= 0

Gi, Ci

NG grid/component numbers for the grids and components that the
element connects to (Ci have to be integers 1,2,3,4,5 and/or 6)

Integer > 0

None

NS scalar points (Bulk Data SPOINT) that the element connects to

Integer > 0

None

Remarks:
1. No other element in the model may have the same element ID
2. An example of how this element is used is in Craig-Bampton analyses where a system model is made
up of one or more substructures (generated in CB model generation solution sequence, SOL 31).

114

Each CB model’s connection information is described by a CUSERIN element. The PUSERIN Bulk
Data entry is required.

115

DEBUG
6.4.1.32 DEBUG
Description:
Define debug parameters

Format:
1
DEBUG

2
i

3
VALUE

Example:
DEBUG

Data Description:
Field
i
VALUE

Contents
Debug number (index in DEBUG array)
The value for DEBUG(i)

Type

Default

0 < Integer < 100

None

Integer

Remarks:
1. No other element in the model may have the same element ID
2. See table below for actions taken based on the various debug values. Unless otherwise stated,
DEBUG(i) = 0 is the default and, for the “print” parameters, no printing is done.

116

Action Taken For DEBUG(I) Values
I
1
2
3
4
5
6
7
8
9

11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26

31
32
33
34
35
36

DEBUG(I)
1
1
1
1
1
1
2
1
1
2
3
>0
11 or 33
12 or 32
13 or 33
21 or 33
22 or 32

Action (NOTE: default values are zero)
Print KIND parameters defined in module PENTIUM_II_KIND to F06 file
Print constants (parameters) defined in module CONSTANTS_1
Print machine parameters as determined by LAPACK function DLAMCH
Do not use BMEAN when calculating membrane quad element stiffness for warped elements
Print Gauss quadrature abscissas and weight s for plate elements
Print some quad elem data to BUG file (over and above what is printed with Case Control ELDATA)
Print some hexa elem data to BUG file (over and above what is printed with Case Control ELDATA)
Print arrays ESORT1, ESORT2, EPNT, ETYPE in subr ELESORT before/after sorting elems
Print grid temperature data in subr TEMPERATURE_DATA_PROC
Print elem temperature data in subr TEMPERATURE_DATA_PROC
Print both grid and elem temperature data in subr TEMPERATURE_DATA_PROC
Prints debug info on BAR pin flag processing
Print data on algorithm to create STF stiffness arrays in subr ESP
Print detailed data on algorithm to create STF arrays in subr SPARSE
Print template of nonzero terms in KGG if PARAM SETLKTK = 1 or 2
Print data on algorithm to create EMS mass arrays in subr ESP
Print detailed data on algorithm to create EMS mass arrays in subr SPARSE

1
2
3
1
1
1
1
1
>0
>1
>0
1
0
1
0
1
1
>0
1 or 3
2 or 3
1 or 3
2 or 3
1

Print individual 6x6 rigid body. displacement matrices in basic and global coordinates for each grid
Print NGRID by 6 rigid body displacement matrix in global coordinates for the model
Print both
Use area shear factors in computing BAR stiffness matrix regardless of I12 value
Print grid sequence tables in subr SEQ
Print matrices generated in the rigid element generation subr's
Print concentrated mass data in subr CONM2_PROC_1
Use static equivalent instead of work equivalent pressure loads for the QUAD4, TRIA3
Print some info in subr KGG_SINGULARITY_PROC for grids that have AUTOSPC'd components
Do above for all grids (not just ones that have AUTOSPC's)
Print diagnostics in subr QMEM1 regarding checks on the BMEAN matrix satisfying R.B. motion
Print debug output from subr STOKEN
Use simple solution for GMN if RMM is diagonal.
Bypass the simple solution for GMN if RMM is diagonal and use subr SOLVE_GMN instead
Use MATMULT_SFF to multiply stiffness matrix times rigid body displs in STIFF_MAT_EQUIL_CHK
Use LAPACK subroutine DSBMV
Print RBMAT in subr STIFF_MAT_EQUIL_CHK
Do equilibrium checks on stiffness matrix even though model has SPOINT's
Print KFSe matrix in subr REDUCE_KNN_TO_KFF
Print KSSe matrix in subr REDUCE_KNN_TO_KFF
Print PFYS matrix in subr REDUCE_N_FS
Print QSYS matrix in subr REDUCE_N_FS
Print YS matrix (S-set enforcorced displs) in LINK2 (LAPACK)

1
1
1
1 or 3
2 or 3
1
1

Print KLL stiff matrix in LINK3-LAPACK
Print PL load matrix in LINK3-LAPACK
Print UL displacement matrix before refining sulotion in LINK3_LAPACK
Print ABAND matrix (KLL in band form) before equilibrating it in LINK3 (LAPACK
Print ABAND matrix after equilibrating it in LINK3 (LAPACK)
Print ABAND’s decomp matrix (KLL triangular factor) in LINK3 (LAPACK)
Print grid 6x6 mass for every grid in LINK2

117

Action (NOTE: default values are zero)

41
42
43

DEBUG(I)
1 or 3
2 or 3
1
1
1
1
1

46
47
48
49

1
1
1
1

Print debug info for Inverse Power eigenvalue extraction
Print eigenvalue estimates at each iteration in Lanczos
Do not calculate off-diag terms in generalized mass matrix
Print diagnostics in ARPACK subroutine DSBAND

1
2
3

Print PHIXG in full format in EXPAND_PHIXA_TO_PHIXG
Print PHIZG in full format in LINK5
Do both

Print banded stiffness matrix ABAND in subr EIG_GIV_MGIV
Print banded mass matrix ABAND in subr EIG_GIV_MGIV
print RFAC = KLL - sigma*MLL in subr EIG_INV
print RFAC = KLL - sigma*MLL in subr EIG_LANCZOS
Print KLL stiffness matrix in LINK4
Print MLL stiffness matrix in LINK4
Print eigenvectors in LINK4 (normally not printed until LINK9)

118

I
80
81
82
83

84
85
86

DEBUG(I)
>0
1
2
3
1
1
2
3
1
2
3
1
1
2
3

88
89

1
1

91
92

1
1

102
103
104
105

>0
>1
>0
>1
>0
>0
>0
>0

106

107
108
109
110
111
112
113
114
115
116

>0
>0
>0
>0
>0
>0
>0
>0
>0
=1
=2
=3

100
101

Action (NOTE: default values are zero)
Print LAPACK_S scale factors, in subr EQUILIBRATE, used to equilibrate the stiffness matrices
Print data on how subr MATADD_SSS_NTERM determines no. terms to allocate for matrix add
Print data on progress of matrix add in subr MATADD_SSS
Print data from both subroutines
Print data on progress of matrix multiply in subr MATMULT_SFF
Print data on how subr MATMULT_SFS_NTERM determines no. terms to allocate for matrix multiply
Print data on progress of matrix multiply in subr MATMULT_SFS
Print data from both subroutines
Print data on how subr MATMULT_SSS_NTERM determines no. terms to allocate for matrix multiply
Print data on progress of matrix multiply in subr MATMULT_SSS
Print data from both subroutines
Print data on matrix transposition in subr MATTRNSP_SS
Print data on how subr PARTITION_SS_NTERM determines no. terms to allocate for matrix partition
Print data on progress of matrix partition in subr PARTITION_SS
Print data from both subroutines
Print data on algorithm to convert sparse CRS matrix to sparse CCS in subr
SPARSE_CRS_SPARSE_CCS
Do not write separator line between grids several places(matrix diagonal output, equil check)
Write row numbers where there are zero diag terms in subroutine SPARSE_MAT_DIAG_ZEROS
Print Information on how the maximum number of requests for grid or element related outputs is
determined. This controls the allocation of memory in LINK9
Print OLOAD, SPCF, MPCF totals even if global coordinate systems for all grids are not the same

Check allocation status of allocatable arrays.
Also write memory allocated to all arrays to F06 file.
Write sparse I_MATOUT array in subroutine READ_MATRIX_1.
Call subroutine to check I_MATOUT array to make sure that terms are nondecreasing
Print debug info in subroutine MERGE_MAT_COLS_SSS
Do not use MRL (or MLR) in calc of modal participation factors and effective mass
Check if KRRcb is singular
write KLLs matrix to unformatted file
write info on all files in subr WRITE_ALLOC_MEM_TABLE (if 0 only write for those arrays that have
memory allocated to them
Write allocated memory in F04 file with 6 decimal points (3 if DEBUG(107) = 0)
Write EDAT table
Write debug info in subr ELMDIS
Write debug info for BUSH elem in subrs ELMDAT1, ELMGM1
Write some debug info on RSPLINE
Write THETAM (plate element material angle) and the location in subr EMG where it was calculated
Write PBARL entries in a special format that has 1 line per PBAR entry
Write debug info in subr OU4_PARTVEC_PROC
Write debug info in subr READ_INCLUDE_FILNAM
Write debug info in Yale subr SFAC
Write debug info in Yale subr NFAC
Do both

119

DEBUG(I)

Action (NOTE: default values are zero)

172
173
174

>0
=1
=2
>0

175

176

177
178
179
180
181
182
183
184

>0
=1
=1
>0
=1
=1
=1
>0

185

186
187
188

197
198
199

>0
>0
>0
1
2
3
>0
=0
>0
=1
=2
=3
=4
=5
=6
=9
= 100
= 999
1 or 3
2 or 3
3
>0
0
>0
>0
>0
>0

200

Calc PHI_SQ for the MIN4T based on area weighting of the TRIA3's. Otherwise, use simple average
Write some debug info in subr PARSE_CSV_STRING
Write some more detailed data
Print MPFACTOR, MEFFMASS values with 2 decimal places of accuracy rather than 6
Write debug output from subroutine SURFACE_FIT regarding the polynomial fit to obtain element
corner stresses from Gauss point stresses
Calculate stresses using element SEi, STEi matrices and displacements rather than from BEi matrices
and strains
Print BAR, ROD margins of safety whether or not they would otherwise be
Print info on user key if PROTECTED = 'N'
Print blank space at beg of lines of output for CUSERIN entries in the F06 file
Write debug info to F06 for USERIN elements
Include USERIN RB mass in subr GPWG even though user did not input 3rd matrix (RBM0) on IN4FIL
Print debug data in subr MGGS_MASS_MATRIX for scalar mass matrix
Write some debug data for generating TDOF array
Write L1M data to F06
Let eigen routines find and process all eigenval, vecs found even if NVEC > NDOFL NUM_MLL_DIAG_ZEROS
Print debug info for pressure loads on faces of solid elements
Write list ao the number of various elastic elements in the DAT file to the F06 file
Do not abort in QPLT3 if KOO is reported to be singular
Print messages in subroutine ESP for KE in local coords if element diagonal stiffness < 0
Print these messages in subroutine ESP after transformation to global
Do both
Do not round off FAILURE_INDEX to 0 in subr POLY_FAILURE_INDEX
Use temperatures at Gauss points for thermal loads in solid elements
Print some summary info for max abs value of GP force balance for each solution vector
call FILE_INQUIRE at end of LINK1
call FILE_INQUIRE at end of LINK2
call FILE_INQUIRE at end of LINK3
call FILE_INQUIRE at end of LINK4
call FILE_INQUIRE at end of LINK5
call FILE_INQUIRE at end of LINK6
call FILE_INQUIRE at end of LINK9
call FILE_INQUIRE at end of MAIN
do all of the above
skip check on CW/CCW numbering of QUAD's
2 or 3 skip check on QUAD interior angles < 180 deg
skip both
Print CB OTM matrices to F06 at end of LINK9
Matrix output filter SMALL = EPSIL(1)
Matrix output filter SMALL = TINY (param defined by user with default = 0.D0)
Print debug info in subr EC_ENTRY_OUTPUT4 which reads Exec Control OUTPUT4 entries
Write debug info in subroutine QPLT3 (for QUAD4 element)
Check matrix times its inverse = identity matrix in several subroutines
Write problem answers (displs, etc) to filename.ANS as well as to filename.F06 (where filename is the
name of the DAT data file submitted to MYSTRAN. This feature is generally only useful to the author
when performing checkout of test problem answers

189
190
191
192

193

194
195
196

120

EIGR
6.4.1.33 EIGR
Description:
Eigenvalue extraction data

Format:
1
EIGR
+CONT

2
SID
NORM

3
METH
G

4
F1
C

5
F2

EIGR
+ZZ02

98
MAX

GIV

0.1

EIGR
+ZZ02

25
POINT

GIV
471

15.
3

6
NE

7
ND

9
CRIT

10
+CONT

20.

1.E-4

+ZZ02

20.

1.E-4

+ZZ02

Examples:

Data Description:
Field

Contents

Type

Default

SID

Eigenvalue extraction set number

Integer > 0

None

METH

Method for eigenvalue extraction: (GIV, MGIV, INV)

Character

None

F1, F2

Frequency range of interest

Real

Number of estimated eigenvalues in range (not used for GIV)

Integer

Number of desired eigenvalues in range (not used for GIV)

Integer

Real

Method of eigenvector renormalization (POINT, MAX, MASS)

Character

None

If NORM = POINT, the grid to be used in normalizing eigenvector to
1.0

Integer > 0
or blank

If NORM = POINT, the component (1-6) at G to be used in normalizing
the eigenvector = 1.0

Integer 1-6
or blank

CRIT
NORM

Orthogonality criteria

Remarks:
1. Givens (GIV) or Modified Givens (MGIV) methods of eigenvalue extraction are available. In addition,
an Inverse Power (INV) method is also available, but only for the fundamental mode.
2. The EIGR set ID, SID, must be selected in Case Control with the entry METHOD = SID

121

3. The three methods of eigenvector renormalization are:
MASS: eigenvectors are normalized to unit generalized mass (1.0)
MAX: eigenvectors are normalized to 1.0 for the largest term
POINT: eigenvectors are normalized such that the value at grid G, component C is 1.0
4. For the GIV method the mass matrix must be positive definite (thus the mass matrix can have no
zeros on its diagonal). For the MGIV method, the model must have the stiffness matrix positive
definite (thus modes of a model that is not restrained from rigid body motion cannot be obtained)

122

EIGRL
6.4.1.34 EIGRL
Description:
Eigenvalue extraction data for Lanczos method

Format:
1
EIGR
+CONT

2
SID
MODE

3
F1
TYPE

4
F2

50.

5
N

6
7
MSGLVL NCVFACL

8
SIGMA

9
NORM

10
+CONT

Examples:
EIGRL

Data Description:
Field

Contents

Type

Default

SID

Eigenvalue extraction set number

Integer > 0

None

Real

Number of desired eigenvalues

Integer

MSGLVL

Output message level (0 for none, or 1 or 2 for some messaging)

Integer

NCVFAC

Used to dimension several arrays in the Lanczos method. Must be > 1

Integer

Real

-10.

Character

None

Integer

Character

DPB

F1, F2
N

Frequency range of interest

SIGMA

Shift eigenvalue

NORM

Method of eigenvector renormalization (MAX, MASS)

Mode

Lanczos mode for calculating eigenvalues

Type

Lanczos matrix type (DPB, DGB)

Remarks:
1. The EIGRL set ID, SID, must be selected in Case Control with the entry METHOD = SID
2. Either F1 (and F2) or N must be specified. If both are specified, N will be used.
3. Mode refers to the Lanczos mode type to be used in the solution. In mode 3 the mass matrix,
Maa,must be nonsingular whereas in mode 2 the matrix K aa  Maa must be nonsingular (where  =
SIGMA). See Bulk Data PARAM ART_MASS for use if the mass matrix is singular.
4. TYPE = DPB uses sym storage of the matrices (preferred) whereas DGB stores all nonzero terms.
5. SIGMA is the shift eigenvalue. It should generally be a small negative real number.

123

FORCE
6.4.1.35 FORCE
Description:
Static concentrated force at a grid point

Format:
1
FORCE

2
SID

3
GID

4
CID

5
F

6
N1

7
N2

8
N3

1234

567

1000.

1.5

2.5

3.5

Example:
FORCE

Data Description:
Field

Contents

Type

Default

SID

Load set ID number

Integer > 0

None

GID

ID of the grid at which this concentrated force acts

Integer >0

None

CID

ID of the coordinate system in which the Ni are specified

Integer >= 0

An overall scale factor for the force

Real

Components of a vector in the direction of the force

Real

Remarks:
1. The static concentrated force applied to the grid is the vector:



P  FN

with Ni in fields 6-8 the components of the vector N

2. In order for this load to be used in a static analysis the load set ID must either be selected in Case
Control by LOAD = SID, or this load set ID must be referenced on a LOAD Bulk Data entry which
itself is selected in Case Control.
3. A blank entry for CID implies the basic coordinate system.

124

GRAV
6.4.1.36 GRAV
Description:
Gravity load definition

Format:
1
GRAV

2
SID

3
CID

4
A

5
N1

6
N2

7
N3

975

246

386.

Example:
GRAV

Data Description:
Field

Contents

Type

Default

SID

Load set ID number

Integer > 0

None

CID

ID of the coordinate system in which the Ni are specified

Integer >= 0

Acceleration value

Real

Components of a vector in the direction of the force

Real

Remarks:
1. GRAV causes a static load to be applied to the complete model that is calculated based on the
acceleration vector on the GRAV entry and the mass properties of the model.
2. The acceleration vector applied to the model is the vector:



a  AN

with Ni in fields 5-7 the components of the vector N
3. In order for this load to be used in a static analysis the load set ID must either be selected in Case
Control by LOAD = SID, or this load set ID must be referenced on a LOAD Bulk Data entry which
itself is selected in Case Control.
4. A blank entry for CID implies the basic coordinate system.

125

GRDSET
6.4.1.37 GRDSET
Description:
Default values for the GRID entry

Format:
1
GRDSET

3
CID1

7
CID2

8
PSPC

245

Example:
GRDSET

Data Description:
Field

Contents

Type

Default

CID1

Default value for the coordinate system ID in which grids will be
located for GRID entries which have a blank in this field

Integer >= 0

CID2

Default value for the global coordinate system for GRID entries which
have a blank in this field

Integer >= 0

PSPC

Default value for permanent single point constraints for GRID entries
which have a blank in this field

Integers 1-6

Remarks:
1. Only one GRDSET entry is allowed in the data file. Any data entered on a GRDSET entry will be
used for the corresponding field of any GRID entry that has that field blank. Thus, if the user desires
to have CIDi be the basic system on a GRID entry, and a GRDSET entry is present with nonzero
value for CIDi, the GRID entry in question must have 0 (not blank) for CIDi.
2. See the GRID entry for remarks on the above fields of this entry.
3. A blank entry for CIDi implies the basic coordinate system.

126

GRID
6.4.1.38 GRID
Description:
Grid point definition

Format:
1
GRID

2
GID

3
CID1

4
X1

5
X2

6
X3

7
CID2

8
PSPC

10.

20.

245

Example:
GRID

Data Description:
Field

Contents

GID
CID1
Xi

Type

Default

Grid point ID number

Integer > 0

None

ID of the coordinate system that the Xi are defined in

Integer >= 0

Real

Coordinates of the grid defined in coordinate system CID1

CID2

ID of the global coordinate system for this grid point

Integer >= 0

PSPC

Permanent single point constraints at this grid point

Integers 1-6

Blank

Remarks:
1. Grid IDs must be unique among all GRID entries.
2. The word “permanent” in regards to the single point constraints (SPC’s) defined on the GRID entry is
merely a designation given to SPC’s defined on GRID entries. The PSPC field does not have to be
used. Any, or all, of the zero value (i.e., not enforced displacement) single point constraints used in a
model can be specified on Bulk Data SPC or SPC1 entries or as PSPC’s on the GRID entry.
3. A blank entry for CIDi implies the basic coordinate system.

127

LOAD
6.4.1.39 LOAD
Description:
This entry combines loads defined on FORCE, MOMENT, PLOAD2, GRAV entries
Format:
1
LOAD
+CONT

2
SID
S4

3
S
L4

4
S1
(etc)

5
L1

6
S2

7
L2

8
S3

9
L3

10
+CONT

12345
2450.1

1500.
12

151.5

290.2

780.3

+L002

Example:
LOAD
+L002

Data Description:
Field

Contents

SID

Load set ID number

Type

Default

Integer > 0

None

An overall scale factor for the load combination

Real

Scale factor for load set Li

Real

Load set ID number for loads defined on FORCE, MOMENT,
PLOAD2, GRAV entries

Integer > 0

None

Remarks:
1. The static load applied to the model is the vector:



P  SiSP
i Li
where PLi is the load defined on the FORCE, MOMENT, PLOAD2 or GRAV that has Li load set ID.
2. In order for this load to be used in a static analysis the load set ID must be selected in Case Control
by the command LOAD = SID.
3. Any number of continuation entries may be included.

128

MAT1
6.4.1.40 MAT1
Description:
Linear isotropic material definition

Format:
1
MAT1
+CONT

2
MID
TA

3
E
CA

4
G
SA

10
10000.

1.E7
20000.

15000.

5
NU

6
RHO

7
ALPHA

8
TREF

0.33

0.1

2.E-5

21.

9
GE

10
+CONT

Example:
MAT1
+MATL01

+MATL01

Data Description:
Field

Contents

MID

Material ID number

Type

Default

Integer > 0

None

Young’s modulus

Real > 0. or blank

See remarks

Shear modulus

Real > 0. or blank

See remarks

Poisson’s ratio

Real > 0. or blank

See remarks

Material mass density

Real > 0. or blank

Coefficient of thermal expansion

Real > 0. or blank

Reference temperature

Real > 0. or blank

Damping coefficient

Real > 0. or blank

Tension allowable for the material

Real > 0. or blank

Compression allowable for the material

Real > 0. or blank

Shear allowable for the material

Real > 0. or blank

RHO
ALPHA
TREF

Remarks:
1. MID must be unique among all material property entries.
2. The continuation entry is not required.
3.

The following action is taken if one or more of the fields E, G and NU are blank:
a)

If one of E, G or NU is blank it will be calculated using the relationship E = 2(1 + NU)G

If E and NU are blank or if G and NU are blank, these two are set to 0.

If E and G are blank (or zero) a fatal error occurs

129

4. A warning is given if:

.5 < NU < 0.

A warning is given if if E, G and NU are all input and do not satisfy the relationship:
1

E
 0.01
2(1  NU)G

130

MAT2
6.4.1.41 MAT2
Description:
Linear anisothotropic material definition for 2D plate elements

Format:
1
MAT2
+CONT

2
MID
A1

3
G11
A2

4
G12
A3

5
G13
TREF

6
G22
GE

7
G23
ST

8
G33
SC

9
RHO
SS

10
+CONT1

10
2.-5

9.9+6
3.-5

3.+6
1.5-5

2.+6
21.

10.1+6
.001

3.2+6
30000.

8.9+6
20000.

.00025
25000

+MAT21

Example:
MAT2
+MAT21

Data Description:
Field

Contents

Type

Default

MID

Material ID number

Integer > 0

None

Terms in the 3x3 material property matrix

Real

Material mass density

Real

Thermal expansion coefficients

Real

Reference temperature

Real

Structural damping coefficient

Real

Tension stress limit

Real

Compression stress limit

Real

Shear stress limit

Real

Gij
RHO
Ai
TREF

Remarks:
1. MID must be unique among all material property entries.
2. The continuation entry is not required.
3. If this entry is used for the transverse shear properties (MID3 on PSHELL) then G13, G23 and G33
are ignored .

131

4. The stress strain relationship for an element using the MAT2 is:
.
 1   G11 G12 G13   1 
 1 
  
 
 

2   G12 G22 G23  2   (T  Tref )  2 
  G
 
 
 3   13 G23 G33  3 
 3
and
xz 
 
yz 

 G11 G12    xz 
G
 
 12 G22    yz 

132

MAT8
6.4.1.42 MAT8
Description:
Linear orthotropic material definition for plate elements

Format:
1
MAT8
+CONT1
+CONT2

2
MID
A1
GE

3
E1
A2
F12

4
E2
TREF
STRN

5
NU12
Xt

6
G12
Yc

7
G1Z
Yt

8
G2Z
Yc

9
RHO
S

10
+CONT1
+CONT2

10
20.-5

9.+6
22.-5

11.+6
21.0

0.29

4.+6

3.+6

5.+6

.00258

+MATL01
+MATL02

Example:
MAT8
+MATL01
+MATL02

Data Description:
Field

Contents

MID

Material ID number

Type

Default

Integer > 0

None

Elastic modulus in longitudinal direction

Real > 0.

Elastic modulus in lateral direction

Real > 0.

G12

In-plane shear modulus

Real >= 0.

G1Z

Transverse shear modulus in the 1-Z plane

Real >= 0.

G2Z

Transverse shear modulus in the 2-Z plane

Real >= 0.

NU12

Poisson’s ratio

Real >= 0.

RHO

Material mass density

Real >= 0.

Coefficient of thermal expansion in the longitudinal direction

Real >= 0.

Coefficient of thermal expansion in the lateral direction

Real >= 0.

Real

Real > 0.

TREF

Reference temperature

Damping coefficient

F12
STRN

Compression allowable for the material

133

Remarks:
1. MID must be unique among all material property entries.
2. The continuation entries are not required.
3. If G1Z and G2Z are zero (or blank) transverse shear flexibility is zero (infinite transverse shear
stiffness).

134

MAT9
6.4.1.43 MAT9
Description:
Linear anisotropic material definition for 3D solid elements

Format:
1
MAT9
+CONT1
+CONT2
+CONT3

2
MID
G23
G44
A2

3
G11
G24
G45
A3

4
G12
G25
G46
A4

5
G13
G26
G55
A5

6
G14
G33
G56
A6

8.+6

4.+4

3.2+6

2.5+6
10.+6

4.+6
22.-5

18.-5

7
G15
G34
G66
TREF

8
G16
G35
RHO
GE

9
G22
G36
A1

10
+CONT1
+CONT2
+CONT3

9.+6

+MATL01
+MATL02
+MATL03

Example:
MAT8
+MATL01
+MATL02
+MATL03

5.+6

3.+6

.003

20.-5

Data Description:
Field

Contents

MID

Material ID number

Gij
RHO
AI
TREF
GE

Type

Default

Integer > 0

None

Elements of the 6x6 material matrix

Real > 0.

Material mass density

Real >= 0.

Coefficients of thermal expansion

Real >= 0.

Real

Real > 0.

Reference temperature
Damping coefficient

Remarks:
1. MID must be unique among all material property entries.
2. The first two continuation entries are required but the third continuation entry is not required.
3. The Gij are the transformation of strains to stresses as in:
 x 
 
 y
 
 z
  
 xy 
 
 yz 
zx 

G11 G12 G13

G22 G23


G33



sym



135

G14

G15

G24
G34
G44

G25
G35
G45
G55

G16    x 
 
G26    y 
G36    z 
 
G46    xy 
G56    yz 
 
G66    
 zx 

MOMENT
6.4.1.44 MOMENT
Description:
Static concentrated moment at a grid point

Format:
1
MOMENT

2
SID

3
GID

4
CID

5
M

6
N1

7
N2

8
N3

1234

567

1000.

1.5

2.5

3.5

Example:
MOMENT

Data Description:
Field

Contents

Type

Default

SID

Load set ID number

Integer > 0

None

GID

ID of the grid at which this concentrated moment acts

Integer >0

None

CID

ID of the coordinate system in which the Ni are specified

Integer >= 0

An overall scale factor for the moment

Real

Components of a vector in the direction of the moment

Real

Remarks:
1. The static concentrated moment applied to the grid is the vector:



P  MN

with Ni in fields 6-8 the components of the vector N
2. In order for this load to be used in a static analysis the load set ID must either be selected in Case
Control by LOAD = SID, or this load set ID must be referenced on a LOAD Bulk Data entry which
itself is selected in Case Control.
3. A blank entry for CID implies the basic coordinate system.

136

MPC
6.4.1.45 MPC
Description:
Multi point constraints define a linear dependence of one degree of freedom (that becomes a
member of the M-set) on other degrees of freedom.
Format:
1
MPC
+MPC1
+MPC2

2
SID

3
G1
G3
G6

4
C1
C3
C5

5
D1
S3
D6

6
G2
G4
etc…

7
C2
C4

8
D2
D4

10
+MPC1
+MPC2

Example:
As an example consider the following equation relating several degrees of freedom (in global
coordinates):
1.2w101  4.5v 201  0.63y623  12.7z76  0

where w101 is the the displacement in the global z direction at grid 101, v201 is the displacement in the
global y direction at grid 201, and the remaining two terms are the rotation about the global y and z
directions at grids 623 and 76 respectively. Assuming that w101 has been chosen as the M-set degree of
freedom for this MPC equation, the input would be:
MPC
+M01

101
623

3
5

1.2
-.63

201
76

2
6

4.5
12.7

+M01

Data Description:
Field

Contents

Type

Default

SID

ID number of the multi point constraint set

Integer > 0

None

ID numbers of the grids involved in the constraint. Grid G1, componrnt
C1 is, by definition, the dependent (M-set) degree of freedom

Integer > 0

None

Component numbers at grids Gi involved in the MPC equation

Integers 1-6

None

The value for coefficient D for grid Gi, component Ci

Real

Remarks:
1. Multi point constraint sets must be selected in Case Control with the entry MPC = SID in order for
them to be applied.
2. Degrees of freedom defined as dependent on MPC entries will be members of the M-set and cannot
be defined as being members of any other mutually exclusive set.
3. G1/C1 is the degree of freedom eliminated (M-set) due to the MPC equation and the remaining terms
in the MPC equation can be for degrees of freedom belonging to any displacement set.

137

MPCADD
6.4.1.46 MPCADD
Description:
Combine multi-point constraint sets defined on MPC entries
Format:
1
MPCADD
+CONT

2
SID
S8

3
S1
S9

4
S2
(etc)

5
S3

6
S4

283

123

564

7
S5

8
S6

9
S7

10
+CONT

Example:
SPCADD

Data Description:
Field

Contents

SID
Si

Type

Default

Multi-point constraint set ID number

Integer > 0

None

Set IDs of MPC Bulk Data entries

Integer > 0

None

Remarks:
1. Multi-point constraint sets must be selected in Case Control with the entry MPC = SID in order for
them to be applied.
2. All multi-point constraints specified on MPC entries whose set IDs are the Si on the MPCADD will be
applied to the model if MPC = SID is in Case Control.

138

OMIT
6.4.1.47 OMIT
Description:
Define degrees of freedom to go into the omit set (O-set)

Format:
1
OMIT

2
G1

3
C1

4
G2

5
C2

6
G3

7
C3

8
G4

9
C4

2345

124

134

Example:
OMIT

Data Description:
Field

Contents

Type

Default

ID numbers of grids

Integer > 0

None

Displacement component numbers

Integers 1-6

None

Remarks:
1. The degrees of freedom defined by grids GI, components Ci will be placed in the mutually exclusive
O-set. These degrees of freedom cannot have been defined to be in any other mutually exclusive set
(i.e.. M, S or A sets).
2. If OMIT or OMIT1 are present in the data file, then all degrees of freedom not specified on these
entries and also not in the M or S sets will be placed in the A-set. If both ASET (or ASET1) and OMIT
(or OMIT1) are present, then all degrees of freedom not in the M and S sets must be explicitly defined
on ASET (or ASET1) and OMIT (or OMIT1)
3. Up to four pairs of Gi, Si can be specified on one OMIT entry. For more pairs, use additional OMIT
entries (i.e. there is no continuation entry for OMIT).

139

OMIT1
6.4.1.48 OMIT1
Description:
Define degrees of freedom to go into the omit set (O-set)

Format No. 1:
OMIT1
+Q001

C
G8

G1
G9

G2
(etc)

THRU

135

17934

THRU

19012

+Q001

Format No. 2:
OMIT1

Example:
OMIT1

Data Description:
Field

Contents

Type

Default

ID numbers of grids. G2 > G1

Integer > 0

None

Displacement component numbers

Integers 1-6

None

Remarks:
1. In Format No. 2, all grids in the range G1 through G2 will have component C defined in the O-set.
2. The degrees of freedom defined by grids GI, components C will be placed in the mutually exclusive
O-set. These degrees of freedom cannot have been defined to be in any other mutually exclusive set
(i.e.. M, S or A sets).
3. If OMIT or OMIT1 are present in the data file, then all degrees of freedom not specified on these
entries and also not in the M or S sets will be placed in the A-set. If both ASET (or ASET1) and OMIT
(or OMIT1) are present, then all degrees of freedom not in the M and S sets must be explicitly defined
on ASET (or ASET1) and OMIT (or OMIT1)

140

PARAM
6.4.1.49 PARAM
Description:
Provide values, other than default values, for parameters that control options during execution.
Format:
1
PARAM

2
NAME

3
V1

PRTDOF

4
V2

5
V3

6
V4

Example:
PARAM

Data Description:
Field
NAME
Vi

Contents

Type

Default

Parameter name

Char

None

Char, Integer or real

Various

Values for the parts of the parameter

Remarks:
1. See table below for a list of the various parameters and what action is taken based on their values.
Unless otherwise stated, only value V1 is used. The parameter name always goes in field 2 and V1
always goes in field 3. When there is more than one Vi, the table explicitly states in what fields the Vi
go.

141

Parameters
Parameter
Name
ARP_TOL

Data
Type
Real

ART_KED

Char

(for diff stiffness
– not fully
implemented)

ART_MASS

Char

AUTOSPC

BAILOUT

Char
Real
Int
Char
Char
Int

CBMIN3

Real

CBMIN4

Real

CBMIN4T

Real

CHKGRDS
CUSERIN

Char
Char
Int
Int
Int
Int
Char
Int

DARPACK

Int

EIGESTL

Int

EIGNORM2

Char

Function of Parameter
NOTE: Default values of parameters are: N for Char, 0 for Int and 0.0 for real
Default = 1x10-6
Tolerance to use in Lanczos eigenvalue extraction method for convergence
Field 3: ART_KED, default = N. If Y add artificial stiff to diag of KED stiff matrix
Field 4: ART_TRAN_MASS: value for translation degrees of freedom, default 1x10-6
Field 5: ART_ROT_MASS: value for translation degrees of freedom, default 1x10-6
Field 3: ART_MASS, default = N. If Y add artificial mass to diag of MGG mass matrix
Field 4: ART_TRAN_MASS: value for translation degrees of freedom, default 1x10-6
Field 5: ART_ROT_MASS: value for translation degrees of freedom, default 1x10-6
Field 3: AUTOSPC value, default = Y (AUTOSPC), N turns AUTOSPC off.
Field 4: AUTOSPC_RAT, default = 1x10-6 (see Section 3.4.1.1)
Field 5: AUTOSPC_NSET, default = 1 (see Section 3.4.1.1)
Field 6: AUTOSPC_INFO, default = N. If Y then print messages about the AUTOSPC’s
Field 7: AUTOSPC_SPCF, default = N. If Y print AUTOSPC forces of constraint
Default = 1
If > 0 quit if a singularity in decomposing a matrix is detected.
If <= 0 do not quit
Default = 2.0
CBMIN3 is the constant CB used in tuning the shear correction factor in Ref 3 for the
TRIA3 plate element. The default 2.0 is the value suggested by the author.
Default = 3.6
CBMIN4 is the constant CB used in tuning the shear correction factor in Ref 4 for the
QUAD4 plate element (QUAD4TYP = ‘MIN4 ‘). See Ref 4
Default = 3.6
CBMIN4T is the constant CB used in tuning the shear correction factor in Ref 4 for the
QUAD4 plate element (QUAD4TYP = ‘MIN4T’).
Default = Y. If N do not check that all grids for all elements exist
If this parameter is present, Bulk Data entries for Craig-Bampton (CB) reduced models
will be written to the F06 file as a CUSERIN element (including grids, coordinate
systems, etc)
Field 3: element ID, default = 9999999
Field 4: property ID default = 9999999
Field 5: starting index for the SPOINT’s to represent modes of the CB model, default =
1001
Field 6: IN4 file number that goes on the PUSERIN entry for this CUSERIN element,
default = 9999999
Field 7: Set-ID for the CUSERIN element (typically the “R”, or boundary, set), default is
blank field
Field 8: Format for how to write the component numbers (1 thru 6) for each grid of the
CUSERIN element. If 0, write them in compact form (e.g. 1356). If > 0 write them in
expanded form (1 3 56), default = 0
Default = 2
how many extra modes to find above EIG_N2 on the EIGRL entry. These few highest
mode are not used due to difficulty with getting good GP force balance.
Defaule 5000
For eigenvalue problems by the Lanczos method, if the number of L-set DOF’s exceed
EIGESTL the method for specifying the search range will be changed from F1 to F2 to N
(see EIGRL Bulk Data entry) to avoid excessive run times (since the code to estimate
the number of eigens in the F1 to F2 range can be excessive).
Default = N. if 'Y' then eigenvectors will be renormalized a last time by multiplying by a
set of scale factors (1 per eigenvector) supplied in a file with the same name as the
input file and extension 'EIN' (if it exists)

142

Parameters (continued)
Parameter
Name
ELFORCEN

Data
Type
Char

EPSERR
EPSIL

Char
Real

EQCHECK

Int
Int
Int
Int
Int
Int

GRDPNT

Real
Char
Int

GRIDSEQ

Char

Char
Char

Function of Parameter
NOTE: Default values of parameters are: N for Char, 0 for Int and 0.0 for real
Default = GLOBAL
If ELFORCEN = GLOBAL, and nodal forces have been requested in Case Control, they
will be output in the global coordinate system.
If ELFORCEN = BASIC, and nodal forces have been requested in Case Control, they
will be output in the basic coordinate systeml.
If ELFORCEN = LOCAL, and nodal forces have been requested in Case Control, they
will be output in the local element coordinate system.
Default = Y. If N, do not calculate the NASTRAN like “epsilon error estimate”
There are 3 EPSIL(i) values each of which requires a separate PAPAM EPSIL Bulk
Data entry with the index (i) in field 3 and EPSIL(i) value in field 4.
These are small numbers used in MYSTRAN for the purposes indicated below:
1) EPSIL(1) (default = 1x10-15) is used in MYSTRAN such that, in any real number
comparisons, any real number whose absolute magnitude is less than EPSIL(1) is
considered to be zero. If no PARAM EPSIL 1 entry is in the data file then this value
is reset (from the default) in LINK1 to a value based on machine precision
calculated using LAPACK BLAS function DLAMCH. If the user has a PARAM
EPSIL 1 entry, this value will be used for EPSIL(1) instead of the LAPACK machine
precision.
2) Currently not used
3) EPSIL(3) is used in the Inverse Power method of eigenvalue extraction to test
convergence of an eigenvalue. The default value (% change) is 1x10-5 %
4) EPSIL(4) is used to calculate the maximum warp for quadrilateral plate elements,
above which a warning message will be written. This maximum warp is EPSIL(2)
times the average length of the quadrilateral’s two diagonals. The default for
EPSIL(2) is 1.x10-1.
5) EPSIL(5) (default 1.x10-6) is used in BAR and ROD margin of safety calculations. If
a stress magnitude is less than EPSIL(5) a 1.x1010 margin of safety will printed out
for that stress (in other words, an infinite margin of safety)
6) EPSIL(6) (default 1.x10-15) is used in BAR margin of safety calculations
Field 3: Default = 0 (basic origin) or reference grid to use in calculating the rigid body
displacement matrix for the equilibrium check
Field 4: If nonzero, do equilibrium check on the G-set
Field 5: If nonzero, do equilibrium check on the N-set
Field 6: If nonzero, do equilibrium check on the F-set
Field 7: If nonzero, do equilibrium check on the A-set
Field 8: If nonzero, do equilibrium check on the L-set
The value in fields 4-8 can be:
1: print loads due to rigid body displacements
2: print strain energy due to rigid body displacements
3: print both
Field 9: EQCHK_TINY, default = 1x10-5. I Do not print grid forces smaller than this
Field 10: Default = N. If Y, normalize the grid forces on diagonal stiffness
Default = -1. If not -1 then the value is interpreted as a grid number
If GRDPNT /= 0, calculate total mass properties of the model relative to the basic
coordinate system origin or relative to the specified grid.
Field 3: GRIDSEQ value (default = BANDIT). Other values are GRID and INPUT.
BANDIT is automatic grid sequencing. GRID is sequencing in grid ID numerical order.
INPUT is sequencing in the grid input order.
Field 4: SEQQUIT, default = N. If Y, then quit in the sequence processor if BANDIT did
not run correctly.
Field 5: SEQPRT, default = N. If Y, print SEQGP card images generated by BANDIT to
the F06 output file

143

Parameters (continued)
Parameter
Name
HEXAXIS

Data
Type
Char

IORQ1M

Int

IORQ1S

Int

IORQ1B

Int

IORQ2B

Int

IORQ2T

Int

ITMAX

Int

KLLRAT
KOORAT
LANCMETH
MATSPARS

Char
Char
Char
Char

MAXRATIO

Real

MEFMCORD

Int

MEFMLOC

Char

MEMAFAC

Int

MIN4TRED

Char

MKLFACij

Char

MKLMATST

Char

Function of Parameter
NOTE: Default values of parameters are: N for Char, 0 for Int and 0.0 for real
'SIDE12', use side 1-2 as the local elem x axis.
'SPLITD' (default), use angle that splits the 2 diags to define the elem x axis
Default = 2
Gaussian integration order for membrane direct stress terms for the QUAD4, QUAD4K
quadrilateral elements
Default = 1
Gaussian integration order for membrane shear stress terms for all quad elements
Default = 2
Gaussian integration order for bending stress terms for the QUAD4K element
Default = 2
Gaussian integration order for bending stress terms for the QUAD4 element
Default = 3
Gaussian integration order for transverse shear stress terms for the QUAD4 element
Default = 5
Max number of iterations in refining the solution when parameter UREFINE = Y
Default = Y to tell whether to calc ratio of max/min KLL diagonal terms
Default = Y to tell whether to calc ratio of max/min KOO diagonal terms
Procedure to use for Lanczos eigenvalue extraction (ARPACK or TRLan)
If = Y (default), use sparse matrix routines for add/multiply in all matrix operations. If N,
use full matrix add/multiply (not recommended)
Default =1X107
Max value of matrix diagonal to factor diagonal before messages are written and
BAILOUT tested for aborting run
Default = 0. The coordinate system in which to calculate modal mass and participation
factors
Reference location for calculating modal effective mass in Craig-Bampton (SOL 31)
analyses. This only affects the rotational modal effective masses. Field 3 can be
GRDPNT, GRID or CG:
If field 3 = GRDPNT (default): ref point is the same as the one for PARAM GRDPNT
If field 3 = CG: use the model center of gravity as the reference point
If field 3 = GRID: use the grid point number in field 4 as the reference point
Field 4: MEFMGRID (grid to use when field 3 is GRID)
Default = 0.9. Factor to multiply the size request of memory to be allocated when
looping to find an allowable amount of memory to allocate. Used when the initial request
for memory (in subrs ESP or EMP) cannot be met and we know that the request is
conservative.
Default = STC. Defines the method for how the 5th node of the MIN4T element is
reduced out (to get a 4 node quad element). STC (default) is static condensation. B%$
(not implemented as of Version 3.0) uses a method developed by the element author
(see Users Reference manual)
Default = INDEF. Matrix type for use in decomposing matrices in various subroutines in
MYSTRAN when PARAM SOLLIB is IntMKL’
MKLFAC21 is for use in subr REDUCE_KAA_TO_KFF
MKLFAC31 is for use in subr LINK3
MKLFAC41 is for use in subr EIG_INV_PWR
MKLFAC42 is for use in subr EIG_LANCZOS_ARPACK
MKLFAC61 is for use in subr CALC_KRRcb
MKLFAC62 is for use in subr SOLVE_DLR
MKLFAC63 is for use in subr SOLVE_PHIZL1
Default = NONSYM. Matrix structure to use when PARAM SOLLIB = IntMKL. Values
can be NONSYM or SYM

144

Parameters (continued)
Parameter
Name
MKLSTATS
MPFOUT

Data
Type
Char
Char

MXALLOCA

Int

MXITERI

Int

MXITERL

Int

OTMSKIP
PBARLDEC

Int
Int

PBARLSHR
PCHSPC1

Char
Char
Int
Char

PCMPTSTM
PCOMPEQ

Real
Int

POST
PRTBASIC
PRTCGLTM
PRTCONN
PRTCORD
PRTDISP

Int
Int
Int
Int
Int
Int

PRTDLR
PRTDOF

Int
Int

PRTFOR

Int

PRTGMN
PRTGOA

Int
Int

Function of Parameter
NOTE: Default values of parameters are: N for Char, 0 for Int and 0.0 for real
Default = N. If Y write stats on matrix decomposition when PARAM SOLLIB = IntMKL
(1) ‘6’ (default) indicates to output modal participation factors (MPF) relative to the 6
DOF’s at grid MEFMGRID (see PARAM MEFMLOC)
(2) ‘R’ indicates to output MPF’s for all of the R-set DOF’s individually
Default = 10. Max number of attempts to allow when trying to allocate memory in
subroutine ALLOCATE_STF_ARRAYS
Default = 50. Max number of iterations to use in the Inverse Power eigenvalue
extraction method
Default = 50. Max number of iterations to use in the Lanczos eigenvalue extraction
method
Number of lines to skip between segments of OTM text file descriptors
Default = 5. Number of decimal digits when writing PBAR equivalents for PBARL entry
real data
Default = Y. Include K1, K2 for PBAR equiv to PBARL BAR properties
Field 3: PCHSPC1 value (default = N, do not punch SPC1 card images for constraints
generated by the AUTOSPC feature, use Y to punch these)
Field 4: SPC1SID value (default = 9999999, the set ID to put on the SPC1 card images)
Field 5: SPC1QUIT value (default = N, do not stop after SPC!’s are punched, or Y to
stop processing)
Factor to multiply composite ply thickness for effective shear thickness
Default = 0. Indicator to write equiv PSHELL, MAT2 to F06 for PCOMP's. If > 0, write
the equivalent PSHELL amd MAT2 Bulk Data entries for the PCOMP. If > 1 also write
the data in a format with a greater number of digits of accuracy.
If = -1 then write FEMAP neutral file for post processing of MYSTRAN outputs
If = 1 print grid coordinates in the basic coordinate system
If = 1 print CB matrix for C.G. LTM loads
If = 1, print table of elements connected to each grid
If PRTCORD = 1 print coordinate system transformation data
PRTDISP(I), I=1-4 go in fields 3-6 of the PARAM PRTDISP entry that prints
displacement matrices for G, N, F, and/or A-sets:
V1 = PRTDISP(1) = 1 print UG
V2 = PRTDISP(2) = 1 or 3 print UN, 2 or 3 print UM
V3 = PRTDISP(3) = 1 or 3 print UF, 2 or 3 print US
V4 = PRTDISP(4) = 1 or 3 print UA, 2 or 3 print UO
V5 = PRTDISP(5) = 1 or 3 print UL, 2 or 3 print UR
If = 1, the DLR matrix will be printed
If PRTDOF = 1 or 3 print TDOF table, in grid point ID numerical order, which gives a list
of the degree of freedom numbers for each displacement set (size is number of degrees
of freedom x number of displacement sets)
If PRTDOF = 2 or 3 print TDOF table, in degree of freedom numerical order, which
gives a list of the degree of freedom numbers for each displacement set (size is number
of degrees of freedom x number of displacement sets)
PRTFOR(I), I=1-4 go in fields 3-6 of the PARAM PRTFOR entry that prints sparse force
matrices for G, N, F, and/or A-sets:
V1 = PRTFOR(1) = 1 print sparse PG
V2 = PRTFOR(2) = 1 or 3 print sparse PN, 2 or 3 print PM
V3 = PRTFOR(3) = 1 or 3 print sparse PF, 2 or 3 print PS
V4 = PRTFOR(4) = 1 or 3 print sparse PA, 2 or 3 print PO
V5 = PRTFOR(5) = 1 or 3 print sparse PL, 2 or 3 print PR
If PRTGMN = 1, print GMN matrix
If PRTGOA = 1, print GOA matrix

145

Parameters (continued)
Parameter
Name
PRTHMN
PRTIFLTM
PRTKXX
PRTMASSD
PRTMASS

Data
Type
Int
Int
Int
Int
Int

PRTMXX
PRTOU4
PRTPHIXA
PRTPHIZL
PRTPSET
PRTQSYS
PRTRMG

Int
Int
Int
Int
Int
Int
Int

PRTSCP
PRTSTIFD
PRTSTIFF

Int
Int
Int

PRTTSET

Int

PRTUO0
PRTUSET
PRTYS
Q4SURFIT

Int
Int
Int
Int

QUAD4TYP

Char

QUADAXIS

Char

Function of Parameter
NOTE: Default values of parameters are: N for Char, 0 for Int and 0.0 for real
If = 1 print HMN constraint matrix
If = 1 print CB matrix for Interface Forces LTM
If = 1 print CB matrix KXX
Same as PRTMASS, except only print diagonal terms
PRTMASS(I), I=1-4 go in fields 3-6 of the PARAM PRTMASS entry that prints sparse
mass matrices for G, N, F, and/or A-sets:
V1 = PRTMASS(1) = 1 print sparse MGG
V2 = PRTMASS(2) = 1 or 3 print sparse MNN, 2 or 3 print MNM, MMM
V3 = PRTMASS(3) = 1 or 3 print sparse MFF, 2 or 3 print MFS, MSS
V4 = PRTMASS(4) = 1 or 3 print sparse MAA, 2 or 3 print MAO, MOO
V5 = PRTMASS(5) = 1 or 3 print sparse MLL, 2 or 3 print MLR, MRR
If = 1 print CB matrix MXX
If > 0 write all OU4 (OUTPUT4) matrices to F06 file
If = 1 print CB matrix PHIXA
If = 1 print CB matrix PHIZL
If > 0 print the OUTPUT4 matrix partitioning vector sets
If = 1 print matrix QSYS
If PRTRMG = 1 or 3, print constraint matrix RMG
If PRTRMG = 2 or 3, print partitions RMN and RMM of constraint matrix RMG
If PRTSCP = 1 print data generated in the subcase processor
Same as PRTSTIFF, except only print diagonal terms
Defaults = 0 for PRTSTIFF(I), I=1-4 which go in fields 3-6 of the PARAM PRTSTIFF
entry that prints sparse stiffness matrices for G, N, F, and/or A-sets:
V1 = PRTSTIFF(1) = 1 print sparse KGG
V2 = PRTSTIFF(2) = 1 or 3 print sparse KNN, 2 or 3 print KNM, KMM
V3 = PRTSTIFF(3) = 1 or 3 print sparse KFF, 2 or 3 print KFS, KSS
V4 = PRTSTIFF(4) = 1 or 3 print sparse KAA, 2 or 3 print KAO, KOO
V5 = PRTSTIFF(5) = 1 or 3 print sparse KLL, 2 or 3 print KLR, KRR
If PRTSET = 1 print TSET table which gives the character name of the displacement
sets that each degree of freedom belongs to (size is number of grids x 6)
If = 1 print UO0
If > 0 print the user defined set (U1 or U2) definitions
If = 1 print matrix YS
Default = 6. Polynomial order for the surface fit of QUAD4 stress/strain when stresses
are requested for other than corner locations
'MIN4T' ! Which element to use in MYSTRAN as the QUAD4 element
'MIN4T (default)': Use Tessler's MIN4T element made up of 4 MIN3 triangles
'MIN4 ': Use Tessler's MIN4 element
Default = ‘SIDE12’
This determines how the quad element local x axis is defined. ‘SIDE12’ means that the
axis between grids 1 and 2 of the quad define the local x axis. ‘SPLITD’ means that the
axis is defined as the direction that splits the angle between the quad diagonals

146

Parameters (continued)
Parameter
Name
RCONDK

Data
Type
Char

RELINK3
SETLKTK

Char
Int

Char
Int
SETLKTM
SHRFXFAC

Real

SKIPMKGG

Char

SOLLIB

Char

SORT_MAX

Int

SPARSTOR

Char

STR_CID

Int

SUPINFO

Char

SUPWARN

Char

THRESHK

Real

Function of Parameter
NOTE: Default values of parameters are: N for Char, 0 for Int and 0.0 for real
If RCONDK = Y, then LAPACK calculates the condition number of the A-set stiffness
matrix. This is required if LAPACK error bounds on the A-set displacement solution are
desired. This can require significant solution time.
‘Y’ or ‘N’ to specify whether to rerun LINK3 and also LINK5 in a restart
Field 3: SETLKTK value. Default = 0. Method to estimate number of nonzeros in G-set
stiffness matrix so array can be allocated.
(1) If SETLKTK = 0, estimate LTERM_KGG based on full element stiffness matrices
unconnected (most conservative but not time consuming).
(2) If SETLKTK = 1, estimate LTERM_KGG based on KGG bandwidth.
(3) If SETLKTK = 2, estimate LTERM_KGG based on KGG density of nonzero terms
(4) If SETLKTK = 3, estimate LTERM_KGG based on actual element stiffness matrices
unconnected.
(5) f SETLKTK = 4, estimate LTERM_KGG on value input by user in field 5 of the
PARAM SETLKT entry (PARAM USR_LTERM_KGG).
Field 4: ESP0_PAUSE value (default = N, do not pause after subr ESP0 to let user input
LTERM_KGG, or pause if = Y
Field 5: User input value of LTERM_KGG
Same as SETLKTK but for the G-set mass matrix. Only the values for SETLKTM = 1, 3,
4 are available
Default = 1x106. Factor used to adjust transverse shear stiffness when user has
indicated zero shear flexibility for shell elements. The shear stiffness will be reset from
infinite (zero flexibility) to SHRFXFAC times the average of the bending stiffnesses in
the 2 planes
Default = N. 'Y', 'N' indicator to say whether to skip calculation of MGG, KGG in which
case MGG, KGG will be read from previously generated, and saved, files (LINK1L for
KGG, LINK1R for MGG)
Default = IntMKL. Denotes which library to use for matrix decomposition and equation
solution. Options are:
IntMKL: Intel Math Kernel Library (matrices stored in sparse form)
LAPACK (matrices stored in band form)
YaleSMP: (matrices stored in sparse form) – not fully implemented in MYSTRAN
Default = 5
Max number of times to run algorithm when sorting arrays before fatal message.
Default = SYM
If SYM, symmetric matrices are stored with only the terms on and above the diagonal. If
NONSYM all terms are stored. SYM requires less disk storage but NONSYM can save
significant time in sparse matrix partitioning and multiply operations.
Default = -1. Indicator for the coordinate system to use ID for elem stress, strain and
emgineering force output:
-1 is local element coordinate system (default)
0 is basic coordinate system
j (any other integer) is a defined coordinate system for output
Default = Y
Indicator of whether some information messages should be suppressed in the F06
output file. N indicates to suppress, Y indicates to not suppress messages in the file.
Default = Y
Indicator of whether warning messages should be suppressed in the F06 output file.
N indicates to suppress, Y indicates to not suppress messages in the file.
Default = 0.1
User defined value for the threshold in deciding whether to equilibrate the A-set stiffness
matrix in LAPACK subroutine DLAQSB. Default value 0.1, LAPACK suggests

147

Parameters (continued)
Parameter
Name
TINY
TRLLOHI

Data
Type
Real
Int

TRLMXLAN

Int

TRLMXMV

Int

TRLREST
TRLTOL

Int
Real

TRLVERB
TSTM_DEF

Int
Real

USETSTR

Char

USR_JCT

Int

WINAMEM

Real

WTMASS

Real

Function of Parameter
NOTE: Default values of parameters are: N for Char, 0 for Int and 0.0 for real
Do not print matrix values whose absolute value is less than this parameter value
For TRLan eigen extraction (default = -1) - which end of spectrum to compute:
< 0, the smallest eigenvalues
= 0. whichever converges first
> 0, the largest eigenvalues
For TRLan eigen extraction (default = 7) - Max num Lanczos basis vectors to be used
(If user enters a Bulk Data PARAM TRLMXLAN then internal parameter
USER_TRLMXLAN is set to ‘Y’)
For TRLan eigen extraction (default = -2000) - Max number of matrix-vector
multiplications allowed
For TRLan eigen extraction (default = 1) - Index of restarting schemes
For TRLan eigen extraction (default = 1.4901D-8) - Eigenpair is declared converged if
its residual norm is < tol*||OP||
For TRLan eigen extraction (default = 0) - Level of output data written by TRLan
Default = 5/6 = 0.833333
Value for TS/TM on PSHELL Bulk data entry when that field on the PSHELL is blank
Requests output of the internal sequence order for displacement sets (e.g. G-set, etc).
See section 3.6 for a discussion of displacement sets. In addition to the sets in section
3.7, the user displacement sets U1 and U2 (see Bulk Data entry USET and USET1) can
also have the internal sort order output to the F06 file. As an example, to obtain a row
oriented tabular output of the internal sort order for the R-set, include the Bulk data
entry:
PARAM, USETSTR, R
User supplied value for JCT - used in shell sort subroutines. If USR_JCT = 0, internal
values for JCT will be used in the shell sort.
Default = 2.0 GB. Max memory Windows allows for any array. If it is exceeded, a
message is printed out and execution is aborted. This is used to avoid a failure which
aborts MYSTRAN catastrophically (due to a system fault).
Default = 1.0
Multiplier for mass matrix after the model total mass is output in the Grid Point Weight
Generator (GPWG). This allows user to input mass terms as weight to get model mass
properties in weight units and then to convert back to mass units after the GPWG has
run. For example, if the model units are lb-sec2/inch for mass and inches for length and
the input data file has lb for “mass” (read weight), then 1/386, or 0.002591 would be the
value for WTMASS needed to convert the “mass” matrix from weight units to mass
units.

148

PARVEC
6.4.1.50 PARVEC
Description:
Defines a partitioning vector to be used in partitioning an OUTPUT4 matrix. See the Exec
Control statements OUTPUT4 and PARTN.
Format:
1
PARVEC

2
NAME

3
G1

4
C1

5
G2

6
C2

COLVEC

101

201

7
G3

8
C3

Example:
PARVEC

Data Description:
Field
NAME

Contents

Type

Default

Name of a row or column partitioning vector specified in a PARTN
Exec Control command

Char

None

ID numbers of the grids that will be partitioned

Integer > 0

None

Component numbers at grids Gi that will be partitioned

Integers 1-6

None

Remarks:
1. The Gi, Ci must be members of the displacement set for the matrix being partitioned. For example, if
the OUTPUT4 matrix being partitioned is K RL the row partitioning vector grid/component values must
be members of the R-set and the column partitioning vector must be a member of the L-set.

149

PARVEC1
6.4.1.51 PARVEC1
Description:
Defines a partitioning vector to be used in partitioning an OUTPUT4 matrix. See the Exec
Control statements OUTPUT4 and PARTN.
Format No. 1:
1
PARVEC1
+CONT

2
NAME
G7

3
C
G8

4
G1
G9

5
G2
(etc)

6
G3

7
G4

8
G5

9
G6

2
U1

3
C

4
G1

5
THRU

6
G2

PARVEC1
+SZA

52
2003

135
2004

1001

1002

103

1004

2001

2002

PARVEC1

135

1001

THRU

1004

10
+CONT

Format No. 2:
1
PARVEC1

Examples:
+SZA

Data Description:
Field
NAME

Contents

Type

Default

Name of a row or column partitioning vector specified in a PARTN
Exec Control command

Char

None

ID numbers of the grids that will be partitioned

Integers 1-6

None

Component numbers at grids Gi that will be partitioned

Integer > 0

None

Remarks:
1. The Gi, Ci must be members of the displacement set for the matrix being partitioned. For example, if
the OUTPUT4 matrix being partitioned is K RL the row partitioning vector grid/component values must be
members of the R-set and the column partitioning vector must be a member of the L-set.
.

150

PBAR
6.4.1.52 PBAR
Description:
Property definition for BAR element

Format:
1
PBAR
+CONT1
+CONT2

2
PID
Y1
K1

3
MID
Z1
K2

4
A
Y2
I12

5
I1
Z2
CT

6
I2
Y3

7
J
Z3

8
MPL
Y4

9
Z4

10
+CONT1
+CONT2

5
0.5
.833

2
0.6
.833

1.44
-0.5

.144
0.6

.1
-0.5

.005
-0.6

0.1
0.5

-0.6

+P01
+P02

Example:
PBAR
+P01
+P02

Data Description:
Field

Contents

Type

Default

PID

Property ID number

Integer > 0

None

MID

Material ID number

Integer > 0

None

Bar cross-sectional area

Real

Section moment of inertia about the element z axis

Real

Section moment of inertia about the element y axis

Real

Torsional constant

Real

MPL

Mass per unit length

Real

Yi, Zi

Element y, z coordinates, in the bar cross-section, of four points at
which to recover stresses

Real

Area factors for shear

Real

I12

Section cross-product of inertia

Real

Torsional stress recovery coefficient

Real

K1, K2

Remarks:
1. PID must be unique among all PBAR, PBARL property ID’s
2. Neither continuation entry is required
3. The shear center and neutral axis of the beam coincide.
4. See Figure 4-3 for bar element axes
5. Torsional stress is CT/J times the torsion load in the CBAR

151

4. K1 and K2 are used to calculate the transverse shear flexibility of the bar. For infinite shear stiffness
(zero shear flexibility), K1 and K2 must be infinite by beam element theory. In order to implement
this, and avoid dealing with very large numerical values for K1 and K2, MYSTRAN interprets zero K1
and K2 to indicate zero transverse shear flexibility

152

PBARL
6.4.1.53 PBARL
Description:
Property definition for a CBAR element via reference to a cross-section shape (whose dimensions are
specified)

Format:
1
PBAR
+CONT1
+CONT2

2
PID
DIM1
DIM9

3
MID
DIM2
etc

4
DIM3
NSM

5
0.5

2
1.6

0.2

5
TYPE
DIM4

DIM5

DIM6

DIM7

DIM8

10
+CONT1
+CONT2

Example:
PBAR
+P01

CHAN
0.1

+P01

Data Description:
Field

Contents

Type

Default

PID

Property ID number

Integer > 0

None

MID

Material ID number

Integer > 0

None

TYPE

Cross section type

Real

DIMi

Cross-section dimensions

Real

NSM

Nonstructural mass per unit length

Real

Remarks:
1.

PID must be unique among all PBAR, PBARL property ID’s

If ECHO /= NONE the equivalent PBAR entries will be printed in the F06 file

Allowable cross-section types are:
BAR
CROSS
ROD

BOX
H
T

BOX1
HAT
T1

CHAN
HEXA
T2

CHAN1
I
TUBE

CHAN2
I1
Z

The figures on the following 3 pages show the above cross-section types along with the dimension
variables (DIMi) and the cross-section axes. The axes are centered on the cross-section shear
center. Points C, D E F are where stresses will be recovered.

153

Ye
C

DIM4
C

DIM3

DIM2

Ze
E

DIM1

TYPE = BAR

TYPE = BOX

DIM4

DIM6

DIM5
C

DIM3

DIM2

DIM3
E

DIM4

DIM1

TYPE = CHAN

TYPE = BOX1

DIM2

DIM4

DIM1
F

DIM4

DIM1

DIM3

DIM2
TYPE = CHAN2

TYPE = CHAN1

PBARL cross-section types – Fig 1 of 3

154

DIM3

DIM1

Ye
Ye

0.5*DIM1

0.5*DIM2

0.5*DIM2
C

0.5*DIM1
DIM4
D

DIM4

DIM3

DIM3
DIM1

DIM2

TYPE = H

TYPE = CROSS

DIM1
Ze

DIM2

DIM3

DIM1

DIM3

DIM4

E
D

DIM2
TYPE = HEX

TYPE = HAT

Ye
DIM3
F

0.5*DIM1

0.5*DIM1
C

DIM6
DIM1
DIM5

DIM3

DIM4

Ze
DIM2

DIM2
TYPE = I

TYPE = I1

PBARL cross-section types – Fig 2 of 3

155

Ye
DIM1

DIM1

DIM3

DIM2
DIM4

TYPE = ROD

TYPE = T

Ye
Ye
F

DIM1
DIM4
DIM4

DIM2

DIM

Ze
DIM3
D

DIM3

DIM1

TYPE = T1

TYPE = T2

Ye
DIM1
C

DIM2

DIM1

DIM3
D

DIM4

DIM2
E

TYPE = TUBE

TYPE = Z

PBARL cross-section types – Fig 3 of 3

156

PBUSH
6.4.1.54 PBUSH
Description:
Property definition for a spring element defined by a CBUSH entry

Format:
1
PBUSH
+CONT1

2
PID

3
“K”
“RCV”

4
K1
SA

5
K2
ST

6
K3
EA

7
K4
ET

8
K5

9
K6

136

K
RCV

10000.
30.

20000.
40.

30000.
.01

4000.
.02

50000.

60000.

10
+CONT1

Example:
PBUSH
+PB1

+PB1

Data Description:
Field

Contents

Type

Default

PID

Property ID number

Integer > 0

None

“K”

Indicates that the next 6 foelds are stiffness values

Char

None

Stiffness values

Real

“RCV”

Indicates that the next 4 values are stress/strain recovery
coefficients

Real

Stress recovery coefficient in the 3 translational directions

Stress recovery coefficient in the 3 rotational directions

Strain recovery coefficient in the 3 translational directions

Strain recovery coefficient in the 3 rotational directions

Remarks:
1.

Element stresses and are calculated by multiplying element engineering forces times the RCV
coefficients

157

PCOMP
6.4.1.55 PCOMP
Description:
Property definition for a composite 2D plate/shell element made up of one or more plies

Format:
1
PCOMP
+CONT1
+CONT2

2
PID
MID1
MID3

3
Z0
T1
(etc)

4
NSM
THETA1

5
SB
SOUT1

6
FT
MID2

7
TREF
T2

8
GE
THETA2

136
91

-1.02
.02

.0003
30.

30000

TSAI

21.

.002

9
10
LAM
+CONT1
SOUT2 +CONT2

Example:
PCOMP
+PC1

SYM

+PC1

Data Description:
Field

Contents

Type

Default

PID

Property ID number

Integer > 0

None

Distance from reference plane to bottom surface of the element

Real

Remark 2

Non structural mass

Real

Allowable interlaminar shear stress

Real

Failure theory

Char

None

Reference temperature

Real

Structural damping coefficient

Real

LAM

Symmetric lamination option

Char

NONSYM

MIDi

Ply material ID (MID1 must be specified)

Integer

Last one

Ply thickness (T1 must be specified)

Real

Last one

THETAi

Material angle of ply relative to element material axis

Real

SOUTi

Not currently used in MYSTRAN

NSM

TREF
GE

158

5. If LAM = SYM only plies on one side of the laminate are to be specified. If an odd number of plies are
desired with LAM = SYM then the center ply should have a thickness equal to one-half the actual
thickness.
6. The default for MIDi is the previous defined MID. The same holds true for Ti.
7. In order for a ply to be defined, at least one of the 4 ply fields on continuation entries must be present.

159

PCOMP1
6.4.1.56 PCOMP1
Description:
Property definition for a composite 2D plate/shell element made up of one or more plies where all plies
are the same thickness and same material

Format:
1
PCOMP1
+CONT1

2
PID
THETA1

3
Z0
THETA2

4
NSM
THETA3

5
SB
etc

6
FT

7
MID

8
T

9
LAM

10
+CONT1

136
91

-1.02
.02

.0003
30.

30000

TSAI

21.

.002

SYM

+PC1

Example:
PCOMP
+PC1

Data Description:
Field

Contents

Type

Default

PID

Property ID number

Integer > 0

None

Distance from reference plane to bottom surface of the element

Real

Remark 2

Non structural mass

Real

Allowable interlaminar shear stress

Real

Failure theory

Char

None

NSM

MID

Material ID for all plies

Integer > 0

None

Thickness for all plies

Real

Symmetric lamination option

Char

NONSYM

Material angle of ply relative to element material axis

Real

LAM
THETAi

Remarks:
1. PID must be unique among all PCOMP/PSHELL property entries
2. The default for Z0 is 0.5 times the laminate thickness
3. The failure index for the interlaminar shear is the maximum transverse shear stress divided by SB
4. The allowable failure theories are FT = HILL, HOFF, TSAI or STRN
5. If LAM = SYM only plies on one side of the laminate are to be specified. If an odd number of plies are
desired with LAM = SYM then the center ply should have a thickness equal to one-half the actual
thickness.

160

PELAS
6.4.1.57 PELAS
Description:
Stiffness definition for CELAS spring elements

Format:
1
PELAS

2
PID

3
K

1.55E6

4
GE

5
S

Example:
PELAS

.015

Data Description:
Field

Contents

PID

Property ID number

K
GE
S

Type

Default

Integer > 0

None

Spring stiffness

Real

Damping coefficient

Real

Stress recovery coefficient

Real

Remarks:
1. PID must be unique among all PELAS property entries
2. Stress is output for this element as S times the elongation of the spring.

161

PLOAD2
6.4.1.58 PLOAD2
Description:
Uniform pressure load for 2D bending plate elements

Format No. 1:
1
PLOAD2

2
SID

3
P

4
EID1

5
EID2

6
EID3

7
EID4

8
EID5

9
EID6

2
SID

3
P

4
EID1

5
THRU

6
EID2

PLOAD2

267

.05

124

9789

PLOAD2

345

.167

269

THRU

9823

Format No. 2:
1
PLOAD2

Examples:

Data Description:
Field

Contents

SID

Load set ID number

P
EIDi

Pressure value
ID numbers of elements that are to have this pressure as a load

Type

Default

Integer > 0

None

Real

Integer > 0

None

Remarks:
1. A positive value of P will result in a pressure being applied in the positive direction of the local z axis
for the element (perpendicular to the elements’ average midplane)
2. If the THRU option is used EID2 must be greater than EID1. All elements whose ID’s are in the range
EID1 through EID2 will have the pressure load (if SID selected in Case Control directly or via the load
combining LOAD Bulk Data entry).
3. In order for this load to be used in a static analysis the load set ID must either be selected in Case
Control by LOAD = SID, or this load set ID must be referenced on a LOAD Bulk Data entry which
itself is selected in Case Control.
4. Up to six elements can have their pressure specified on one PLOAD2 entry in Format No 1. For more
elements, use additional PLOAD2 entries (i.e. there is no continuation entry for PLOAD2).

162

PLOAD4
6.4.1.59 PLOAD4
Description:
Pressure load on the face of 2D bending plate elements, CTRIA3, CTRIA3K, CQUAD4, CQUAD4K

Format No. 1:
1
PLOAD4

2
SID

3
EID

4
P1

5
P2

6
P3

7
P4

2
SID

3
EID1

4
P1

5
P2

6
P3

7
P4

8
THRU

9
EID2

PLOAD4

267

987

1.1

1.5

1.25

1.4

PLOAD4

345

101

2.4

2.25

2.1

2.0

THRU

200

Format No. 2:
1
PLOAD4

Examples:

Data Description:
Field

Contents

SID

Load set ID number

Pi
EIDi

Pressure value at up to 4 grid locations
ID numbers of elements that are to have this pressure as a load

Type

Default

Integer > 0

None

Real

Integer > 0

None

Remarks:
1. A positive value of P will result in a pressure being applied in the positive direction of the local z axis
for the element (perpendicular to the elements’ average midplane)
2. If the THRU option is used EID2 must be greater than EID1. All elements whose ID’s are in the range
EID1 through EID2 will have the pressure load (if SID selected in Case Control directly or via the load
combining LOAD Bulk Data entry).
3. In order for this load to be used in a static analysis the load set ID must either be selected in Case
Control by LOAD = SID, or this load set ID must be referenced on a LOAD Bulk Data entry which
itself is selected in Case Control.
4. If the fields for P2, P3 and/or P4 are blank that pressure is set equal to P1. P4 has no meaning for
triangular elements.

163

164

PLOTEL
6.4.1.60 PLOTEL
Description:
1 dimensional dummy element that only serves the purpose of plotting a line. It has no elastic properties

Format No. 1:
1
PLOTEL

2
EID

3
G1

4
G2

1001

2365

Example:
PLOTEL

Data Description:
Field

Contents

EID
Gi

Type

Default

Element ID number

Integer > 0

None

Grid point ID’s

Integer > 0

None

Remarks:
1. EID must be unique among all element ID’s
2. This element does not result in any stiffness or mass. It’s purpose is only to plot a line between 2
grids

165

PROD
6.4.1.61 PROD
Description:
Property definition for ROD element

Format:
1
PROD

2
PID

3
MID

4
A

5
J

6
C

7
MPL

.175

.093

1.5

0.0175

Example:
PROD

Data Description:
Field

Contents

Type

Default

PID

Property ID number

Integer > 0

None

MID

Material ID number

Integer > 0

None

Bar cross-sectional area

Real

Torsional constant

Real

Torsional stress recovery coefficient

Real

Mass per unit length

Real

MPL

Remarks:
1. PID must be unique among all PROD property entries
2. The torsional stress is calculated as:
C

Mt
J

where Mt is the torsional moment in the rod element.

166

PSHEAR
6.4.1.62 PSHEAR
Description:
Property definition for SHEAR element

Format:
1
PSHEAR

2
PID

3
MID

4
T

5
NSM

.175

.093

Example:
PSHEAR

Data Description:
Field

Contents

PID
MID
T
NSM

Type

Default

Property ID number

Integer > 0

None

Material ID number

Integer > 0

None

Real > 0.

None

Real

Shear panel thickness
Nonstructural mass per unit area

Remarks:
1. PID must be unique among all PROD property entries

167

PSHELL
6.4.1.63 PSHELL
Description:
Property definition for 2D plate elements

Format:
1
PSHELL
+CONT

2
PID
Z1

3
MID1
Z2

4
TM

5
MID2

6
12I/TM**3

7
MID3

8
TS/TM

9
MPA

10
+CONT

PSHELL
+ABC

987
0.5

234
-0.5

0.10

123

125.

20.

.005

+ABC

PSHELL

234

0.10

234

Examples:

+ABC

Data Description:
Field

Contents

Type

Default

PID

Property ID number

Integer > 0

None

Material ID number for membrane material properties

Integer > 0 or
blank

None

Membrane thickness

Real or blank

Material ID number for bending material properties

Integer > 0 or
blank

None

Ratio of actual bending moment inertia (I) to bending inertia of a solid
plate of thickness TM

Real or blank

1.0

MID3

Material ID number for transverse shear material properties

Integer > 0 or
blank

None

TS/TM

Ratio of shear to membrane thickness

Real or blank

Remark 3

Mass per unit area

Real

Distances from the neutral plane of the plate to locations where
stress is calcilated

Real

Remark 4

MID1
TM
MID2
12I/TM**3

MPA
Z1, Z2

Remarks:
1. PID must be unique among all PSHELL property entries
2. Continuation entry is not required. If Z1 and Z2 are not input, then stresses are calculated at +/-TM/2.
3. Default value for TS/TM is 5/6 = 0.83333 unless a PARAM Bulk data entry with parameter name
TSTM_DEF is in the data file, in which case the TSTM_DEF value on the PARAM entry is used.

168

4. The following holds for the cases of MIDi blank:
If MID1 is blank, no membrane stiffness is calculated
If MID2 is blank, no bending or transverse shear stiffness is calculated
If MID3 is blank, no transverse shear flexibility is included (Kirchoff plate theory: plate is assumed
infinitely stiff in transverse shear) so that normals to the mid-plane remain normal after bending)

169

PSOLID
6.4.1.64 PSOLID
Description:
Property definition for 3D solid elements

Format:
1
PSOLID

2
PID

3
MID

4
CID

5
IN

987

234

7
ISOP

Examples:
PSOLID

FULL

Data Description:
Field

Contents

PID

Property ID number

MID1
CID
IN
ISOP

Material ID number for membrane material properties
Material coordinate system ID
Indicator for integration order (see table below)
Integration scheme (whether to use FULL or REDUCED integration

Remarks:
1. See table below for values of IN and ISOP to use

170

Type

Default

Integer > 0

None

Integer > 0 or
blank

None

Integer or
blank

Integer = 2,3

Character

REDUCED

PSOLID entries IN and ISOP for solid elements – only use ones that have comment: OK
(based on test runs by the author)
(bold, underline indicates default which can also be blank)
HEXA

8 node

20 node

PENTA

6 node

15 node

TETRA

4 node

10 node

Integration

ISOP

Comments

2x2x2 reduced shear

REDUCED

2x2x2 standard isopar.

FULL or 1

(1)

3x3x3 reduced shear

REDUCED

(1)

3x3x3 standard isopar

FULL or 1

(1)

2x2x2 reduced shear

REDUCED

(2)

2x2x2 standard isopar.

FULL or 1

3x3x3 reduced shear

REDUCED

3x3x3 standard isopar

FULL or 1

Integration

ISOP

Comments

2x3 reduced shear

REDUCED

2x3 standard isopar.

FULL or 1

(1)

3x7 reduced Shear

REDUCED

(1)

3x7 standard isopar

FULL or 1

(1)

2x3 reduced shear

REDUCED

(2)

2x3 standard isopar.

FULL or 1

3x7 reduced shear

REDUCED

3x7 standard isopar

FULL or 1

Integration

ISOP

Comments

1 point standard isopar

FULL

(1)

4 point standard isopar

FULL

(1)

FULL

(2)

FULL

1 point standard isopar
4 point standard isopar

Notes: (1) Answers degrade for aspect ratio (AR) above AR =1
(2) Answers are nonsense
OK means answers are good
Reduced integration is used for shear strains to avoid shear locking. For HEXA 2x2x2 and PENTA 2x3
integration it uses selective substitution. For HEXA 3x3x3 reduced integration it uses 2x2x2 for shear. For
PENTA 3x7 reduced integration it uses 2x3 for shear

171

PUSERIN
6.4.1.65 PUSERIN
Description:
Property definition for CUSERIN elements

Format:
1
PUSERIN

2
PID

3
IN4_ID

4
KNAME

5
MNAME

101

KRRGN

MRRGN

6
RBNAME

7
PNAME

Examples:
PUSERIN

Data Description:
Field

Contents

PID

Property ID number

Type

Default

Integer > 0

None

IN4_ID

ID of an Exec Control IN4 entry that specifies the NASTRAN
formatted INPUTT4 file containing the stiffness and mass matrices
(whose name are KNAME, MNAME)

Integer > 0 or
blank

None

KNAME

Name of the stiffness matrix which was written to the INPUTT4 file
when it was created. This can be up to 8 characters long

Char

None

MNAME

Name of the mass matrix which was written to the INPUTT4 file
when it was created. This can be up to 8 characters long

Char

None

RBNAME

Name of a 6x6 rigid body mass matrix which specifies the rigid body
mass relative to the C.G. of the CUSERIN element in its basic
coordinate system. This can be up to 8 characters long

Char

None

PNAME

Name of the load matrix which was written to the INPUTT4 file when
it was created. This can be up to 8 characters long.

Char

None

Remarks:
1. PID must be unique among all PUSERIN property entries
2. IN4_ID is required. In the example above, an Exec Control entri IN4 with ID = 234 is required
3. The matrix whose name is RBNAME is not required. However, the rigid body mass properties
(PARAM GRDPNT) for the overall model will be in error unless the element has the same basic
coordinate system as the overall model.
4. The matrix whose name is PNAME is only used for statics solutions.

172

RBE2
6.4.1.66 RBE2
Description:
Rigid element that has specified components at a number of grids dependent on the six degrees
of freedom at one other grid.
Format:
1
RBE2
+CONT

2
EID
GM6

3
GN
GM7

4
CM
(etc)

5
GM1

6
GM2

7
GM3

8
GM4

9
GM5

10
+CONT

43
1045

1021

346

1031

1033

1035

1041

1043

+REL01

Example:
RBE2
+REL01

Data Description:
Field

Contents

Type

Default

EID

Element ID number

Integer > 0

None

ID number of the grid that will have all 6 components as the 6
independent degrees of freedom for this rigid element

Integer > 0

None

The component numbers of the dependent degrees of freedom at grid
points GMi

Integers 1-6

None

GMi

The components CM at grids GMi are the dependent degrees of
freedom that will be eliminated due to this rigid element

Integer > 0

None

Remarks:
1. No other element in the model may have the same element ID
2. All of the degrees of freedom defined by components CM at each of the grids GMi are made
members of the M-set and their displacements will be rigidly dependent on the six degrees of
freedom at grid GN.
3. Dependent degrees of freedom defined by RBE2 elements can not be defined as members of any
other mutually exclusive set (i.e., cannot appear on SPC, SPC1, OMIT, OMIT1, ASET or ASET1
entries, nor can they appear as dependent degrees of freedom on other rigid elements)

173

RBE3
6.4.1.67 RBE3
Description:
Element used to distribute loads or mass from one grid point (denoted as the dependent grid) to
other grids in the model. The element is defined based on the grids/components that it
connects. The resulting multi-point constraints (MPC’s) generated internally in MYSTRAN, will
eliminate the dependent degrees of freedom and will distribute any loads or mass from the
dependent grid to the remaining grids defined on the RBE3. Unlike the NASTRAN RBE3, the
MYSTRAN RBE3 does not support the “UM” option at the current time
Format:
1
RBE3
+1
+2

2
EID
G1,3
C3

3
WT2
G3,1

43
1003

1004

4
REFGRID
C2
G3,2

5
REFC
G2,1
etc

6
WT1
G2,2

7
C1
G2,3

8
G1,1
G2,4

9
G1,2
WT3

+1
+2

9001

123456

1.0

123

1001

1002

+R1

Example:
RBE3
+R1

Data Description:
Field

Contents

EID
REFGRID
REFC
WTi
Ci
Gi,j

Type

Default

Element ID number

Integer > 0

None

Grid that will be the dependent (or reference) grid

Integer > 0

None

The component numbers of the dependent degrees of freedom at grid
point REFGRID

Integers 1-6

None

Weighting factors for the grids/components that follow
Displacement components at the following Gi,j that have weighting
factor WTi
Grids that REFGRID depend on

Real
Integers 1-6

None
None

Integer > 0

None

Remarks:
1. No other element in the model may have the same element ID
2. Fpr most applications only the translation displacement components (1,2,3) should be defined for the
Ci. If REFGRID and a Gi,j are coincident then rotation components (4,5,6) can be defined for Ci.
3. Dependent degrees of freedom defined by RBE3 elements can not be defined as members of any
other mutually exclusive set (i.e., cannot appear on SPC, SPC1, OMIT, OMIT1, ASET or ASET1
entries, nor can they appear as dependent degrees of freedom on other rigid elements)

174

RFORCE
6.4.1.68 RFORCE
Description:
Defines rigid body rotational velocity, and optional rotational acceleration, of the model about some
specified grid for the purpose of generating inertia forces on the finite element model.

Format:
1
RFORCE
+RF1

2
SID
A

3
GID

4
CID

5
V

6
N1

7
N2

8
N3

10
+RF1

Example:

Data Description:
Field

Contents

Type

Default

SID

Load set ID number (must be selected in Case Control)

Integer > 0

None

GID

ID of the grid at which this concentrated moment acts

Integer >0

None

CID

ID of the coordinate system in which the Ni are specified

Integer >= 0

An overall scale factor for the angular velocity in revolutions per unit
time

Real

Components of a vector in the direction of the angular velocity and
angular acceleration

Real

An overall scale factor for the angular acceleration in revolutions per
unit time squared

Real

Remarks:
1. The force at grid i due to the angular velocity and acceleration is:

Fi   M i   (  (ri  ra )  a  (ri  ra ) 
where
i = grid point
M i  6x6 mass matrix at grid i

 = rigid body angular velocity of the model
a = rigid body angular acceleration of the model
ri = distance from basic system origin to grid i
ra = distance from basic system origin to reference grid about which the model rotates

175

2. The load set ID (SID) is selected by the Case Control entry LOAD:
3. GID = 0 signifies that the rotation vector acts through the basic system origin.
4. CID = 0 indicates that the rotation vector is defined in the basic coordinate system

176

RSPLINE
6.4.1.69 RSPLINE
Description:
Interpolation element. A spline fit using the 2 independent end points (GI1, GI2) is applied to
the locations of the dependent points (defined by GDi/CDi) to rigidly constrain the GDi/CDi
Format:
1
RSPLINE
+CONT

2
EID
CD3

43
123456

5
GD1
etc

6
CD1
GI2

7
GD2

8
CD2

9
GD3

10
+CONT

GD4

4
GI1
CD4

1001
123456

2001
2005

123456
123456

2002
1002

123456

2003

+REL01

2004

Example:
RBE2
+REL01

Data Description:
Field

Contents

Type

Default

EID

Element ID number

Integer > 0

None

GIi

Grid numbers of the 2 independent end points

Integer > 0

None

GDi

Grid numbers of the dependent grtids

Integers > 0

None

CDi

Displacement component numbers at the GDi

Integer 1-6

None

Remarks:
1. No other element in the model may have the same element ID
2. Displacements at the GDi are interpolated using the following rules applied to the line between the 2
end ponts:


Displacenents along the line and rotations about the line are linear



Displacements perpendicular to the line are cubic



Rotations normal to the line are quadratic

177

SEQGP
6.4.1.70 SEQGP
Description:
Manual re-sequencing of grids

Format:
1
SEQGP

2
G1

3
S1

4
G2

5
S2

6
G3

7
S3

8
G4

9
S4

1001

1.5

1011

1021

1031

3.5

Example:
SEQGP

Data Description:
Field

Contents

ID number of a grid point

The sequence number for Gi

Type

Default

Integer > 0

None

Integer or Real > 0

None

Remarks:
1. The SEQGP entry is used to manually re-sequence grids. See the Bulk Data PARAM GRIDSEQ
entry for the starting sequence MYSTRAN uses in manual grid sequencing.
2. Either integer or real sequence numbers are allowed but all are converted to real internally. Thus, if
the user has two grids sequenced consecutively, say with integer sequence numbers 10 and 11, then
some other grid can be inserted in the sequence between the two with a real sequence number
anywhere in the range:
10. < Si < 11.
3. Up to four pairs of Gi, Si can be specified on one SEQGP entry. For more pairs, use additional
SEQGP entries (i.e. there is no continuation entry for SEQGP).
4. If automatic grid point sequencing by BANDIT, any used defined SEQGP entries are ignored.

178

SLOAD
6.4.1.71 SLOAD
Description:
Defines the existence of a scalar load on a scalar point
Format:
1
SLOAD

2
SID

3
Si

4
FMAG

101

125.6

Example:
SPOINT

Data Description:
Field

Contents

SID
Si
FMAG

Type

Default

Load set ID number

Integer > 0

None

Scalar point ID

Integer > 0

None

Real

Magnitude of the orce on scalar point Si

Remarks:
1. In order for this load to be used in a static analysis the load set ID must either be selected in Case
Control by LOAD = SID, or this load set ID must be referenced on a LOAD Bulk Data entry which
itself is selected in Case Control.

179

SPC
6.4.1.72 SPC
Description:
Single point constraints that are defined by specifying the degree of freedom and its
displacement (either zero or some enforced nonzero value)
Format:
1
SPC

2
SID

3
G1

4
C1

5
D1

6
G2

7
C2

8
D2

101

1.2E-3

201

0.0

Example:
SPC

Data Description:
Field

Contents

Type

Default

SID

ID number of the single point constraint set

Integer > 0

None

ID numbers of the grids that will have component number Ci
constrained

Integer > 0

None

Component numbers at grids Gi that will be constrined

Integers 1-6

None

The value for the displacement at grid Gi, component Ci

Real

Remarks:
1. Single point constraint sets must be selected in Case Control with the entry SPC = SID in order for
them to be applied.
2. Degrees of freedom defined on SPC entries will be members of the S-set and cannot be defined as
being members of any other mutually exclusive set.
2. Up to two gid/component pairs can be specified as being single point constrained on one SPC entry
(i.e. continuation entries are not allowed). Additional SPC entries can have the same SID.
3. If a Gi/Ci pair is constrained more than once (with the same SID), the last value read for Di will be
used.
4. A degree of freedom may be specified redundantly as a permanent single point constraint on a GRID
Bulk Data entry and on an SPC or SPC1 Bulk Data entry. If it is defined on the GRID entry and on an
SPC Bulk Data entry, Di must be zero on the SPC entry or a fatal error will occur.

180

SPC1
6.4.1.73 SPC1
Description:
Single point constraints that are defined by specifying the degree of freedom to be constrained
to zero displacement.
Format No. 1:
1
SPC1
+CONT

2
SID
G7

3
C
G8

4
G1
G9

5
G2
(etc)

6
G3

7
G4

8
G5

9
G6

2
SID

3
C

4
G1

5
THRU

6
G2

SPC1
+SZA

52
2003

135
2004

1001

1002

103

1004

2001

2002

SPC1
SPC1

52
52

135
135

1001
2001

THRU
THRU

1004
2004

10
+CONT

Format No. 2:
1
SPC1

Examples:
+SZA

Data Description:
Field

Contents

Type

Default

SID

ID number of the single point constraint set

Integer > 0

None

Component numbers at grids Gi that will be constrained

Integers 1-6

None

ID numbers of the grids that will have component number Ci
constrained

Integer > 0

None

The value for the displacement at grid Gi, component Ci

Real

181

SPCADD
6.4.1.74 SPCADD
Description:
Combine single point constraint sets defined on SPC, SPC1 entries
Format:
1
SPCADD
+CONT

2
SID
S8

3
S1
S9

4
S2
(etc)

5
S3

6
S4

283

123

564

7
S5

8
S6

9
S7

10
+CONT

Example:
SPCADD

Data Description:
Field

Contents

SID
Si

Type

Default

Single point constraint set ID number

Integer > 0

None

Set IDs of SPC and/or SPC1 Bulk Data entries

Integer > 0

None

Remarks:
1. Single point constraint sets must be selected in Case Control with the entry SPC = SID in order for
them to be applied.
4. All single point constraints specified on the SPC and/or SPC1 entries whose set IDs are the Si on the
SPCADD will be applied to the model if SPC = SID is in Case Control.

182

SPOINT
6.4.1.75 SPOINT
Description:
Defines the existence of a scalar point (1 component of displacement) in the model
Format 1:
1
SPOINT
+S01

2
ID1
ID9

3
ID2
etc

4
ID3

5
ID4

6
ID5

7
ID6

8
ID7

9
ID8

10
+S01

2
ID1

3
THRU

4
ID2

101

1.2E-3

201

0.0

Format 2:
1
SPOINT

Example:
SPOINT

Data Description:
Field
IDi

Contents
ID of an SPOINT

Type

Default

Integer > 0

None

Remarks:
1. SPOINT ID’s must be unique among all other SPOINT’s and among all GRID’s
2. SPOINT’s are like GRID’s but have only 1 component of displacement and their outputs are scalar, not
vector, quantities. In the F06 output file, however, the output quantities are reported under the T1
headings.

183

SUPORT
6.4.1.76 SUPORT
Description:
Defines degrees of freedom that are to be in the R-set (for Craig-Bampton model generation)
Format:
1
SUPORT

2
GID

3
C

4
GID

5
C

6
GID

7
C

4981

695

123

5647

456

8
GID

9
C

Example:
SUPORT

Data Description:
Field

Contents

GID
C

Type

Default

ID of a grid whose components in the next field will be put into the
R-set

Integer > 0

None

Displacement component numbers (digits 1 through 6)

Integer > 0

None

Remarks:
1. This Bulk Data entry is meant for use in Craig-Bampton analyses. The degrees of freedom specified
on this entry will be treated the same as Single Point Constraints (SPC’s) in all other analyses

184

TEMP
6.4.1.77 TEMP
Description:
Grid point temperature definition for purposes of calculating thermal loads on the model.

Format:
1
TEMP

2
SID

3
G1

4
T1

5
G2

6
T2

7
G3

8
T3

1011

25.

1012

32.

1013

28.

Example:
TEMP

Data Description:
Field

Contents

Type

Default

SID

ID number of the temperature set

Integer > 0

None

ID numbers of the grids whose temperature is being defined

Integer > 0

None

Temperature of grid Gi

Real

Remarks:
1. Temperature sets must be selected in Case Control with the entry TEMP = SID in order for them to
be used in calculating thermal loads
2. Every element in the model must have its temperature defined for set SID, either explicitly through an
element temperature entry on TEMPRB, TEMPP1 Bulk Data entry or implicitly using grid
temperatures on TEMP, TEMPD Bulk Data entries. Element temperatures defined on element
TEMPRB, TEMPP1 entries take precedence over any that might be defined using grid temperatures.
If no element temperature is explicitly defined, the element temperature is taken to be the average of
the temperatures of the grids to which the element is connected.
3. Thermal loads for the model are calculated using element temperatures defined via TEMP, TEMPD,
TEMPRB, TEMPP1 Bulk data entries, the element properties and the material properties (including
coefficient of thermal expansion and reference temperature). The thermal loads calculated are based
on element temperatures that are the difference between those defined on TEMP, TEMPD, TEMPRB,
TEMPP1 and the reference temperature defined on the material entry for the element.
4. Only three grids may have their temperature defined for set SID in one TEMP entry. Additional grid
temperatures can be specified using more TEMP Bulk Data entries with the same SID.

185

TEMPD
6.4.1.78 TEMPD
Description:
Default grid point temperature definition for purposes of calculating thermal loads on the model.

Format:
1
TEMP

2
SID1

3
T1

4
SID2

5
T2

46.2

52.1

6
SID3

7
T3

8
SID4

9
T4

Example:
TEMP

Data Description:
Field

Contents

SIDi

ID number of a temperature set

The default temperature for grids for set SIDi

Type

Default

Integer > 0

None

Real

Remarks:
1. Temperature sets must be selected in Case Control with the entry TEMP = SID in order for them to
be used in calculating thermal loads
2. All grids whose temperature is not defined on a TEMP Bulk Data entry will have the default
temperature T, if there is one defined on a TEMPD for set SID.
3. Every element in the model must have its temperature defined for set SID, either explicitly through an
element temperature entry on TEMPRB, TEMPP1 Bulk Data entry or implicitly using grid
temperatures on TEMP, TEMPD Bulk Data entries. Element temperatures defined on element
TEMPRB, TEMPP1 entries take precedence over any that might be defined using grid temperatures.
If no element temperature is explicitly defined, the element temperature is taken to be the average of
the temperatures of the grids to which the element is connected.
4. Thermal loads for the model are calculated using element temperatures defined via TEMP, TEMPD,
TEMPRB, TEMPP1 Bulk data entries, the element properties and the material properties (including
coefficient of thermal expansion and reference temperature). The thermal loads calculated are based
on element temperatures that are the difference between those defined on TEMP, TEMPD, TEMPRB,
TEMPP1 and the reference temperature defined on the material entry for the element.
5. Only four pairs of SIDi/Ti may be defined on one TEMPD entry. Additional pairs can be specified
using more TEMPD Bulk Data entries.

186

TEMPP1
6.4.1.79 TEMPP1
Description:
Defines temperatures and temperature gradients for 2D plate elements.

Format No. 1:
1
TEMPP1
+CONT

2
SID
EID2

3
EID1
EID3

4
TBAR
EID4

5
TPRIME
EID5

10
+CONT

2
SID
EID2

3
EID1
THRU

4
TBAR
EID3

5
TPRIME
EID4

10
+CONT

THRU

EID5

TEMPP1
+TP1

13
2679

2101
3201

35.7
1104

10.1
32

5555

TEMPP1
+TP1

13
2304

2101
THRU

35.7
6789

10.1
12

THRU

(etc)

Format No. 2:
1
TEMPP1
+CONT

Examples:
+TP1

+TP1
46

Data Description:
Field

Contents

SID
EIDi
TBAR
TPRIME

Type

Default

ID number of the temperature set

Integer > 0

None

Element ID numbers

Integer > 0

None

Average temperature of the element

Real

Linear thermal gradient through the thickness of the element

Real

Remarks:
1. Any number of continuation entries can be used
2. For format number 2, the THRU ranges must have the second element ID greater than the first.
3. Temperature sets must be selected in Case Control with the entry TEMP = SID in order for them to
be used in calculating thermal loads.
4. Every element in the model must have its temperature defined for set SID, either explicitly through an
element temperature entry on TEMPRB, TEMPP1 Bulk Data entry or implicitly using grid
temperatures on TEMP, TEMPD Bulk Data entries. Element temperatures defined on element
TEMPRB, TEMPP1 entries take precedence over any that might be defined using grid temperatures.

187

If no element temperature is explicitly defined, the element temperature is taken to be the average of
the temperatures of the grids to which the element is connected.
5. Thermal loads for the model are calculated using element temperatures defined via TEMP, TEMPD,
TEMPRB, TEMPP1 Bulk data entries, the element properties and the material properties (including
coefficient of thermal expansion and reference temperature). The thermal loads calculated are based
on element temperatures that are the difference between those defined on TEMP, TEMPD, TEMPRB,
TEMPP1 and the reference temperature defined on the material entry for the element.

188

TEMPRB
6.4.1.80 TEMPRB
Description:
Defines temperatures and temperature gradients for 1D bar elements.

Format No. 1:
1
TEMPRB
+CONT

2
SID
EID2

3
EID1
EID3

4
TA
EID4

5
TB
EID5

6
TP1A
(etc)

7
TP1B

8
TP2A

9
TP2B

10
+CONT

2
SID
EID2

3
EID1
THRU

4
TA
EID3

5
TB
EID4

6
TP1A
THRU

7
TP1B
EID5

8
TP2A

9
TP2B

10
+CONT

TEMPRB
+TP1

13
67

2101
89

35.7
2

10.1
13

789

TEMPRB
+TP1

13
68

2101
THRU

35.7
97

10.1
2101

THRU

4009

Format No. 2:
1
TEMPRB
+CONT

Examples:
+TP1

+TP1

Data Description:
Field

Contents

Type

Default

SID

ID number of the temperature set

Integer > 0

None

EIDi

Element ID numbers

Integer > 0

None

Average temperature of the element at end a

Real > 0.

Average temperature of the element at end b

Real > 0.

TP1A

Linear temperature gradient in element y axis at end a

Real

TP1B

Linear temperature gradient in element y axis at end b

Real

TP2A

Linear temperature gradient in element z axis at end a

Real

TP2B

Linear temperature gradient in element z axis at end b

Real

Remarks:
1. Any number of continuation entries can be used
2. For format number 2, the THRU ranges must have the second element ID greater than the first
3. Temperature sets must be selected in Case Control with the entry TEMP = SID in order for them to
be used in calculating thermal loads

189

4. Every element in the model must have its temperature defined for set SID, either explicitly through an
element temperature entry on TEMPRB, TEMPP1 Bulk Data entry or implicitly using grid
temperatures on TEMP, TEMPD Bulk Data entries. Element temperatures defined on element
TEMPRB, TEMPP1 entries take precedence over any that might be defined using grid temperatures.
If no element temperature is explicitly defined, the element temperature is taken to be the average of
the temperatures of the grids to which the element is connected.
5. Thermal loads for the model are calculated using element temperatures defined via TEMP, TEMPD,
TEMPRB, TEMPP1 Bulk data entries, the element properties and the material properties (including
coefficient of thermal expansion and reference temperature). The thermal loads calculated are based
on element temperatures that are the difference between those defined on TEMP, TEMPD, TEMPRB,
TEMPP1 and the reference temperature defined on the material entry for the element.

6. The average temperatures TA and TB at ends a and b respectively are:
TA=

1
Ta (y,z)dA
A


A

TB=

1
Tb (y,z)dA
A


A

where A is the cross-sectional area and Ta(y,z) and Tb(y,z) are the temperature distributions at ends a
and b respectively.
7. The linear gradients through the thickness, TP1A, TP1B, TP2A and TP2B, are:

TP1A=

1
Ta (y,z)ydA
I1


A

TP1B=

1
Tb (y,z)ydA
I1


A

TP2A=

1
Ta (y,z)zdA
I2


A

TP2B=

1
Tb (y,z)zdA
I2


A

where I1 and I2 are the bending moments of inertia for the bar (on the PBAR entry) and Ta(y,z) and
Tb(y,z) are the temperature distributions at ends a and b respectively.

190

USET
6.4.1.81 USET
Description:
Defines a set of degrees of freedom that belong to a user defined set (named either “U1” or
“U2”). The purpose is for the user to get an output listing that defines the internal degree of
freedom order for the members of the set.
Format:
1
USET

2
NAME

3
G1

4
C1

5
G2

6
C2

101

201

7
G3

8
C3

Example:
USET

Data Description:
Field
NAME

Contents

Type

Default

A user defined set. The name must be either “U1” or “U2”

Char

None

ID numbers of the grids that the user wants to be members of the set

Integer > 0

None

Component numbers at grid Gi that will be members of the set

Integers 1-6

None

Remarks:
1. The Gi, Ci are defined as members of the displacement set named SNAME.
2. A row oriented tabular output showing the internal sort order of the members of the set (named
SNAME) can be output if a PARAM, USETSTR, Ui Bulk Data entry is present (I = 1 or 2).
3. In order to get a listing of the internal sort order, a Bulk Data PARAM, USETSTR, Ui (i=1 or 2) must
be included

191

USET1
6.4.1.82 USET1
Description:
Defines a set of degrees of freedom that belong to a user defined set (named either “U1” or
“U2”). The purpose is for the user to get an output listing that defines the internal degree of
freedom order for the members of the set.
Format No. 1:
1
USET1
+CONT

2
SNAME
G7

3
C
G8

4
G1
G9

5
G2
(etc)

6
G3

7
G4

8
G5

9
G6

2
SNAME

3
C

4
G1

5
THRU

6
G2

USET1
+SZA

U2
2003

135
2004

1001

1002

103

1004

2001

2002

USET1

135

1001

THRU

1004

10
+CONT

Format No. 2:
1
USET1

Examples:
+SZA

Data Description:
Field
SNAME

Contents

Type

Default

A user defined set. The name must be either “U1” or “U2”

Char

None

ID numbers of the grids that are members of the user defined set

Integers 1-6

None

Component numbers at grids Gi that are part of the user defined set

Integer > 0

None

Remarks:
1. The Gi, C are defined as members of the displacement set named SNAME.
2. A row oriented tabular output showing the internal sort order of the members of the set (named
SNAME) can be output if a PARAM, USETSTR, Ui Bulk Data entry is present (I = 1 or 2).
3. In order to get a listing of the internal sort order, a Bulk Data PARAM, USETSTR, Ui (i=1 or 2) must
be included

192

7 Appendix A: MYSTRAN Sample Problem

193

This example problem shows the input and output for a simple rod with 7 grids and 6 elements. The rod
is subjected to loads in two subcases as described below:

Z0, X13

201

101
1

401

301
2

501
4

701

601
5

Yo, Z13

The basic coordinate system is the X0, Y0, Z0 system shown (with X0 in the direction of Yo cross Z0). In
addition, rectangular coordinate system X13, Y13, Z13 (with X13 in the same direction as Z0) is also shown
and will be used in the input data in order to help explain the use of coordinate systems. The basic
system does not have to be defined explicitly. It is implied through the model grid coordinates and any
other coordinate systems (other than basic) which might be referenced in field 3 of the Bulk Data GRID
entry. Coordinate system 13 must be defined via a CORD2R Bulk data entry.
The grid point IDs are 101-701 and the rod element IDs are 1-6. The total length is 60 inches consisting
of 6 elements of 10 inches each. All of the rods have the same cross-sectional area of 0.6 inch2. The
material is aluminum with a Young’s modulus of 1x107. The model is constrained at the left end. Several
loads are applied in two subcases.
Subcase 35 consists of a 120 lb load at grid 701
P101   0. 

 

P201   0. 
P301   0. 


 
P  P401    0. 
P   0. 

 501  
P601   0. 


 
P701  120.

Subcase 8 consists of a 240 lb load at grid 201, a 150. Lb load at grid 301 and a 200 lb load at grid 401
P101   0. 

 

P201  240.
P301  150. 


 
P  P401   200.
P   0. 

 501  
P601   0. 


 
P701   0. 

194

The output, which includes an echo of the input data deck, is shown on the following pages. Note the
following about the OUTPUT:


The input data consists of everything from the ID entry through the ENDDATA entry, and
consists of the Executive Control, Case Control and Bulk Data Decks. Entries that begin with
a $ sign (and have anything after $ in the entry) are commentary and are ignored.


The Executive Control Deck begins with the optional ID entry, has the mandatory
SOL entry (1 for statics) and ends with the mandatory CEND entry. All Executive
Control entries are free field in that they may be anywhere within the 80 columns of
an entry.



The Case Control Deck begins with the entry following CEND (which in this case is a
TITLE Case Control entry) and ends with the mandatory BEGIN BULK entry. The
entries in between can be in any order that makes sense. That is, if there are no
subcases, the data can be in any order. When there are subcases, as is the case for
this example, the entries between one SUBCASE entry and another apply only to
that subcase. Anything “above” the subcase level pertains to all subcases, unless
overridden in a subcase. All Case Control entries are free field.



The SPC = 19 entry requests that a Bulk Data SPC (or SPC1, SPCADD) with
set ID = 19 be used in defining the single point constraints for the model.



The following three entries request various outputs (displacements, etc) with
ALL meaning that displacements for all grids (DISP = ALL), applied loads for
all grids (OLOAD = ALL) and forces of single point constraint (SPCF = ALL).
As these are “above” the subcase ;evel, they apply to all subcases (unless a
subcase requests output of the same type for a different set of grids or
elements)



Subcase 35 (the first subcase in Case Control) is defined with its own subtitle
and with LOAD = 191 requesting that a Bulk Data entry with set ID of 191
define the loads for this subcase (which requires that the load be defined on
a LOAD, FORCE, MOMENT, GRAV od PLOAD2 Bulk Data entry). In this
case, Bulk Data entry FORCE with a set ID od 191 contains the load
definition for this subcase. Element engineering force and stress output is
requested for this subcase (in addition to the requests above the subcase
level). .



Subcase 8 (the second subcase in Case Control) is defined with its own
subtitle (notice the order doesn’t matter) and requesting load set 26 in Bulk
Data to define the load. There is also another output request (for nodal
element forces) for set 98. Set 98 is defined as 2,5. Since set 98 output is
requested as element forces, the 2,5 is interpreted as the element numbers
for which nodal element forces will be output in this subcase only. If the
request had been above the subcase level (as DISP = ALL, etc) the request
would have been honored for both subcases.

The Bulk Data Deck begins with the entry immediately following BEGIN BULK and
ends with the mandatory ENDDATA entry. The logical entries in between can be in
any order with the exception that any one logical entry must be in order. Thus the
MAT1 logical entry, which has one parent entry and one continuation entry must be
entered together and in the order shown.

195



Coordinate system 13 is defined on the CORD2R Bulk Data entry with 13 as
the coordinate system ID in field 2. The reference system in field 3 is, in this
case, the basic system. It does not have to be. Coordinate system 13 could
use some other coordinate system as its reference, and so on. However, the
last system in the chain would have to have the basic system as its
reference. The nine real numbers on the remainder of the CORD2R logical
entry describe three points in coordinates of the reference (basic) system.
The first three numbers are the coordinates of the origin of coordinate system
13, which is at the origin of the basic system. The next three numbers are
the coordinates of a point on the Z13 axis, which is in the direction of the Y0.
The next three numbers (on the continuation entry) are the coordinates of a
point in the X13 – Z13 plane. Thus it is seen that this CORD2R entry
describes coordinate system 13 as seen on the figure above.



The seven grid points of the model are defined on the GRID entries. Note
that field 3 (coordinate systems for grid coordinates) is blank indicating the
basic coordinate system for grid locations for all seven grids. Field 7, the
global coordinate system for each grid is also the basic system for grids 101
through 601. Grid 701, however uses coordinate system 13 as its global
system. Field 8 of the GRID entries is for “permanent” single point
constraints. Note that 13456 are the permanent single point constraints for
grids 101 - 601. Since the rod can only take axial load and torque, only
global degrees of freedom that are for displacement along the rod, or rotation
about its axis can possibly have stiffness. Since grids 101 - 601, have the
basic system as global, degrees of freedom 1346 will be singular and must
therefore be removed via single point constraints at these grids. In addition,
since the PROD entry has zero torsional constant (field 4 of PROD is blank),
there will be no stiffness for global degree of freedom 5 at grids 101 - 601.
Thus, field 7 of the grid 101 - 601 entries have 13456 constrained. These
constraints do not have to appear on the GRID entry, they can be on SPC (or
SPC1) entries as well. Because they appear on the GRID entry these
constraints will be used regardless of whether an SPC = SID entry appears
in Case Control. Grid 701, on the other hand, uses coordinate system 13 as
its global coordinate system. Thus, by the same reasoning as above, global
degrees of freedom 12456 are taken as permanent single point constraints.



The connection entries for the rod elements are the six CROD’s whose
element IDs are indicated in field 2. Field 3 (with 16 in it) is the property ID
and points to the PROD, ID = 16) for the rod elements properties, which are
all the same in this example. Fields 4 and 5 give the grids to which the
elements are attached.



The PROD 16 entry points to a material entry (ID = 20) in field 3 and gives
the rod cross-sectional area in field 4.



The material properties are defined on the MAT1 with ID = 20. Only Young’s
modulus is needed for this example but a material density of 0.1 is also
entered in field 6.



Case Control had a request for single point constraint set. The SPC entry,
with set ID 19, specifies the remaining constraint of zero displacement in
global degree of freedom 2 at grid 101. This could have been included with
the constraints specified in field 7 of the GRID 101 entry, in which case the
SPC = 19 would not have been needed in Case Control.

196



Case Control had a request for load set 191 for subcase 35. The FORCE
Bulk Data entry with ID = 191 is the ID requested for this subcase and
defines a 120 lb load at grid 701. The coordinate system for this load
definition is coordinate system 13 (indicated by the 13 in field 4). Since the
components of the load vector are 0., 0., 1. (fields6-8) this indicates a force in
the Z13 direction which is along the axis of the rod.



Case Control also had a request for load set 26 for subcase 8. As shown
above, this loading condition has axial loads on three grid points. As such,
these could have been defined using three FORCE Bulk Data entries, all with
set ID = 26. However, the LOAD (load combining) Bulk Data entry will be
used for illustrative purposes. The LOAD entry has set ID = 26 which is the
ID requested for this subcase. It defines a load that is a linear combination of
load sets 39, 5 and 178, where the loads for sets 39, 5 and 178 are specified
on the FORCE Bulk Data entries below the LOAD 26 entry. The linear
combination on LOAD 26 is:

Pset 26  2(4Pset 39  3Pset 5



 0. 


240.
150. 


 Pset178 )  200.
 0. 


 0. 


 0. 



The PARAM GRDPNT 101 requests that the Grid Point Weight Generator
calculate the total model mass properties relative to grid point 101.



The PARAM PRTDOF 1 requests printing of the degree of freedom table.



The ENDDATA signifies the end of the Bulk Data Deck.

The remainder of the output for the sample problem is shown on the pages following the
ENDDATA


The next of page lists some informational messages printed out as MYSTRAN
executes.



The degree of freedom table is printed as requested via the Bulk Data PARAM
PRTDOF entry. It shows the degree of freedom numbers for each of the
displacement sets and is in internal degree of freedom order. Note on this listing that
the A-set (analysis set) has six degrees of freedom and these are the axial degrees
of freedom of the rod at the “free” grids, namely 201 – 701. Note that for grids 201 –
601, the A-set degree of freedom is in the “2” direction. This is the global “2”
direction for these grids, which is the basic Y0 system. Note also that grid 701 has its
A-set degree of freedom as “3” which, since the global system for this grid is
coordinate system 13, is in the Z13 direction



The Grid Point Weight Generator (GPWG) calculates the model total mass properties
and prints them. In this example problem, 0.1 was the “mass” density on the MAT1
Bulk data entry. This happens to be the weight density of the aluminum material of
which the rod is made. Thus, the units for the GPWG output are lb.

197



The following couple of pages list some informational messages printed out as
MYSTRAN executes.



The remainder of the output shows the items requested in Case Control for each
subcase. The output shows the subcase number at the beginning of each subcases’
output. The output values are easily verified as being correct with some simple hand
calculations. Note the following:


Displacement, applied load and constraint force output are for grids and all
have headings “T1”, etc, where
T1 is translation in the global X direction of that grid
T2 is translation in the global Y direction of that grid
T3 is translation in the global Z direction of that grid
R1 is rotation about the global X axis
R2 is rotation about the global Y axis
R3 is rotation about the global Z axis



Grids 201 – 601 have T2 displacements since they use the basic system as
global and T2 is in the Y0 direction. Grid 701, however, uses coordinate
system 13 as global and has T3 displacement since T3 is in the Z13 direction



Element engineering forces and stresses are output in the local element
coordinate system for each element. See Figure 3-2 for the rod element
local axes.



Element node forces are output in the same format as grid point
displacements, that is, forces at the grids in global coordinate directions

198

119150503
MYSTRAN Version

2.06

>> MYSTRAN BEGIN:
>> LINK

Jan 19 2006 by Dr Bill Case

1/19/2006 at 15: 5: 3. 15 The input file is EXAMPLE1.DAT

1 BEGIN

ID ROD SAMPLE PROBLEM FOR USERS MANUAL
SOL 1
CEND
TITLE = ROD WITH AXIAL LOADS IN 2 SUBCASES
ECHO = UNSORT
SPC
= 19
DISP
= ALL
OLOAD
= ALL
SPCF
= ALL
SUBCASE 35
SUBTITLE = 120 LB LOAD ON GRID 701
ELFORCE = ALL
STRESS
= ALL
LOAD = 191
SUBCASE 8
SET 98 = 2,5
LOAD = 26
ELFORCE(NODE) = 98
SUBTITLE = 240 LB ON GRID 201 + 150 LB ON GRID 301 + 200 LB ON GRID 401
BEGIN BULK
$
CORD2R 13
0
0.
0.
0.
0.
1.
0.
+CORD13
+CORD13 0.
0.
1.
$
GRID
701
0.
60.
0.
13
12456
GRID
601
0.
50.
0.
13456
GRID
501
0.
40.
0.
13456
GRID
401
0.
30.
0.
13456
GRID
301
0.
20.
0.
13456
GRID
201
0.
10.
0.
13456
GRID
101
0.
0.
0.
13456
$
CROD
1
16
101
201
CROD
2
16
201
301
CROD
3
16
301
401
CROD
4
16
401
501
CROD
5
16
501
601
CROD
6
16
601
701
$
PROD
16
20
.6
$
MAT1
20
1.+7
.33
.1
1.
+MAT1
*INFORMATION: MAT1 ENTRY
20 HAD FIELD FOR G BLANK. MYSTRAN CALCULATED G

199

3.759398E+06

+MAT1
$
SPC1
$
FORCE
$
LOAD
FORCE
FORCE
FORCE
$
PARAM
PARAM
DEBUG
$
ENDDATA

10000.

101

191

701

120.

26
39
5
178

2.0
201
301
401

4.0
0
13
0

39
30.
25.
100.

3.0
0.
0.
0.

5
1.
0.
1.

1.0
0.
1.
0.

GRDPNT
PRTDOF
200

101
1
1

178

200

*INFORMATION: SPARSE MATRICES ARE STORED IN SYM

FORMAT

*INFORMATION: BANDIT WAS CALLED TO RESEQUENCE THE GRIDS AND HAS RETURNED WITH ERROR

*INFORMATION: FILE EXAMPLE1.SEQ
CONTAINING THE BULK DATA SEQGP CARD IMAGES (NEEDED FOR AUTO GRID POINT SEQUENCING REQUESTED BY
THE USER VIA PARAM GRIDSEQ BANDIT ), DOES NOT EXIST
IT MAY BE THAT BANDIT FOUND THAT NO RESEQUENCING WAS NEEDED OR DUE TO ERROR IN RUNNING BANDIT.
MAKE SURE BANDIT HAS RUN SUCCESSFULLY (CHECK FILE BANDIT.OUT IN THE DIRECTORY WHERE MYSTRAN.EXE RESIDES).
*INFORMATION: SUBR AUTO_SEQ_PROC DID NOT SEQUENCE ALL OF THE
7 GRIDS. ONLY
MYSTRAN WILL DEFAULT TO A SEQUENCE THAT IS IN GRID NUMERICAL ORDER

201

0 GRIDS WERE SEQUENCED.

EXTERNAL
GRD-COMP
NUMBER
101-1
-2
-3
-4
-5
-6
201-1
-2
-3
-4
-5
-6
301-1
-2
-3
-4
-5
-6
401-1
-2
-3
-4
-5
-6
501-1
-2
-3
-4
-5
-6
601-1
-2
-3
-4
-5
-6
701-1
-2
-3
-4
-5
-6

DEGREE OF FREEDOM TABLE SORTED ON GRID POINT (TDOF)
(Before any AUTOSPC)
INTERNAL
DOF NUMBER FOR DISPLACEMENT SET:
GRD-COMP ---------------------------------------------------------------------------------------------------------------|
NUMBER
G
M
N
SA
SB
SG
SZ
SE
S
F
O
A
R
L
1-1
-2
-3
-4
-5
-6
2-1
-2
-3
-4
-5
-6
3-1
-2
-3
-4
-5
-6
4-1
-2
-3
-4
-5
-6
5-1
-2
-3
-4
-5
-6
6-1
-2
-3
-4
-5
-6
7-1
-2
-3
-4
-5
-6

TOTAL NUMBER OF DOF:

1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42

0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0

1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42

0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0

0
1
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0

1
0
2
3
4
5
6
0
7
8
9
10
11
0
12
13
14
15
16
0
17
18
19
20
21
0
22
23
24
25
26
0
27
28
29
30
31
32
0
33
34
35

1
2
3
4
5
6
7
0
8
9
10
11
12
0
13
14
15
16
17
0
18
19
20
21
22
0
23
24
25
26
27
0
28
29
30
31
32
33
0
34
35
36

0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0

1
2
3
4
5
6
7
0
8
9
10
11
12
0
13
14
15
16
17
0
18
19
20
21
22
0
23
24
25
26
27
0
28
29
30
31
32
33
0
34
35
36

0
0
0
0
0
0
0
1
0
0
0
0
0
2
0
0
0
0
0
3
0
0
0
0
0
4
0
0
0
0
0
5
0
0
0
0
0
0
6
0
0
0

0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0

0
0
0
0
0
0
0
1
0
0
0
0
0
2
0
0
0
0
0
3
0
0
0
0
0
4
0
0
0
0
0
5
0
0
0
0
0
0
6
0
0
0

0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0

0
0
0
0
0
0
0
1
0
0
0
0
0
2
0
0
0
0
0
3
0
0
0
0
0
4
0
0
0
0
0
5
0
0
0
0
0
0
6
0
0
0

------- ------- ------- ------- ------- ------- ------- ------- ------- ------- ------- ------- ------- ------42
0
42
0
1
35
36
0
36
6
0
6

202

O U T P U T

F R O M
G R I D
P O I N T
W E I G H T
REFERENCE POINT IS GRID POINT
101

TOTAL MASS =

G E N E R A T O R

3.600000E+00

X
Y
Z
C.G. LOCATION : 0.000000E+00 3.000000E+01 0.000000E+00
(RELATIVE TO REFERENCE POINT IN BASIC COORDINATE SYSTEM)

M.O.I. MATRIX - ABOUT REFERENCE POINT IN BASIC COORDINATE SYSTEM
***
***
* 4.380000E+03 0.000000E+00 0.000000E+00 *
* 0.000000E+00 0.000000E+00 0.000000E+00 *
* 0.000000E+00 0.000000E+00 4.380000E+03 *
***
***

M.O.I. MATRIX - ABOUT C.G. IN BASIC COORDINATE SYSTEM
***
***
* 1.140000E+03 0.000000E+00 0.000000E+00 *
* 0.000000E+00 0.000000E+00 0.000000E+00 *
* 0.000000E+00 0.000000E+00 1.140000E+03 *
***
***

M.O.I. MATRIX - ABOUT C.G. IN PRINCIPAL DIRECTIONS
***
***
* 0.000000E+00 0.000000E+00 0.000000E+00 *
* 0.000000E+00 1.140000E+03 0.000000E+00 *
* 0.000000E+00 0.000000E+00 1.140000E+03 *
***
***

TRANSFORMATION FROM BASIC COORDINATES TO PRINCIPAL DIRECTIONS
***
***
* 0.000000E+00 1.000000E+00 0.000000E+00 *
* 1.000000E+00 0.000000E+00 0.000000E+00 *
* 0.000000E+00 0.000000E+00 1.000000E+00 *
***
***

203

*INFORMATION: LTERM_MGGE ESTIMATE OF THE NUMBER OF NONZEROS IN MASS MATRIX MGGE IS

468

*INFORMATION: NUMBER OF NONZERO TERMS IN THE MGG MASS MATRIX IS

*INFORMATION: MAX NUMBER OF NONZERO TERMS IN A ROW OF THE G-SET MASS MATRIX

*INFORMATION: LTERM_KGG ESTIMATE OF THE NUMBER OF NONZEROS IN STIFF MATRIX KGG IS

468

*INFORMATION: NUMBER OF NONZERO TERMS IN THE KGG STIFFNESS MATRIX IS

*INFORMATION: MAX NUMBER OF NONZERO TERMS IN A ROW OF THE G-SET STIFFNESS MATRIX

*INFORMATION: NUMBER OF GRID POINTS
*INFORMATION: NUMBER OF G SET DEGREES OF FREEDOM (NDOFG)

=
=

7
42

>> LINK

1 END

>> LINK

2 BEGIN

*INFORMATION: BASED ON PARAMETER AUTOSPC_NSET =

1 MYSTRAN IS CHECKING KNN TO SEE IF THERE ARE NULL ROWS THAT SHOULD BE AUTOSPC'd

*INFORMATION: MYSTRAN FOUND NO N-SET DOF's THAT WERE SINGULAR AND THAT WERE NOT ALREADY MEMBERS OF THE S-SET

*INFORMATION: AUTOSPC Summary, Overall: after identification of all AUTOSPC's
AUTOSPC_RAT = 1.000000E-06
Number
Number
Number
Number
Number
Number

of
of
of
of
of
of

DOF's
DOF's
DOF's
DOF's
DOF's
DOF's

identified
identified
identified
identified
identified
identified

for
for
for
for
for
for

AUTOSPC
AUTOSPC
AUTOSPC
AUTOSPC
AUTOSPC
AUTOSPC

in
in
in
in
in
in

component
component
component
component
component
component

Total number of DOF's identified overall
*INFORMATION:
*INFORMATION:
*INFORMATION:
*INFORMATION:
*INFORMATION:
*INFORMATION:
*INFORMATION:
*INFORMATION:
*INFORMATION:

NUMBER
NUMBER
NUMBER
NUMBER
NUMBER
NUMBER
NUMBER
NUMBER
NUMBER

OF M SET DEGREES OF FREEDOM (NDOFM)
OF N SET DEGREES OF FREEDOM (NDOFN)
OF S SET DEGREES OF FREEDOM (NDOFS)
OF SA SET DEGREES OF FREEDOM (NDOFSA)
OF F SET DEGREES OF FREEDOM (NDOFF)
OF O SET DEGREES OF FREEDOM (NDOFO)
OF A SET DEGREES OF FREEDOM (NDOFA)
OF R SET DEGREES OF FREEDOM (NDOFR)
OF L SET DEGREES OF FREEDOM (NDOFL)

1
2
3
4
5
6

=
=
=
=
=
=

0
0
0
0
0
0
-----------=
0
=
=
=
=
=
=
=
=
=

204

0
42
36
0
6
0
6
0
6

>> LINK

2 END

>> LINK

3 BEGIN

*INFORMATION: NUMBER OF SUPERDIAGONALS IN THE UPPER TRIANGLE OF MATRIX
*INFORMATION: MAXIMUM DIAGONAL TERM IN MATRIX
KLL
*INFORMATION: MINIMUM DIAGONAL TERM IN MATRIX
KLL
*INFORMATION: RATIO OF MAX TO MIN DIAGONALS IN MATRIX

KLL

*INFORMATION: MAX RATIO OF MATRIX DIAGONAL TO FACTOR DIAGONAL FOR MATRIX

KLL

=
=
=

1.200000E+06 Occurs in row/col no.
6.000000E+05 Occurs in row/col no.
2.000000E+00

1
6

KLL =

1.897367E+03 Occurs in row/col no.

*INFORMATION: FOR INTERNAL SUBCASE NUMBER

1 EPSILON ERROR ESTIMATE

1.421085E-15 Based on U'*(K*U - P)/(U'*P)

*INFORMATION: FOR INTERNAL SUBCASE NUMBER

2 EPSILON ERROR ESTIMATE

1.104361E-15 Based on U'*(K*U - P)/(U'*P)

>> LINK

3 END

>> LINK

5 BEGIN

>> LINK

5 END

>> LINK

9 BEGIN

205

SUBCASE
35
ROD WITH AXIAL LOADS IN 2 SUBCASES
120 LB LOAD ON GRID 701
D I S P L A C E M E N T S
(in global coordinate system at each grid)
T2
T3
R1
R2

GRID

COORD
T1
R3
SYS
101
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
201
0 0.000000E+00 2.000000E-04 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
301
0 0.000000E+00 4.000000E-04 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
401
0 0.000000E+00 6.000000E-04 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
501
0 0.000000E+00 8.000000E-04 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
601
0 0.000000E+00 1.000000E-03 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
701
13 0.000000E+00 0.000000E+00 1.200000E-03 0.000000E+00 0.000000E+00 0.000000E+00
------------- ------------- ------------- ------------- ------------- ------------MAX (for output set):
0.000000E+00 1.000000E-03 1.200000E-03 0.000000E+00 0.000000E+00 0.000000E+00
MIN (for output set):
0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
ABS (for output set):

0.000000E+00

1.000000E-03

1.200000E-03

0.000000E+00

SUBCASE
35
ROD WITH AXIAL LOADS IN 2 SUBCASES
120 LB LOAD ON GRID 701

GRID

A P P L I E D
F O R C E S
(in global coordinate system at each grid)
T2
T3
R1
R2

COORD
T1
R3
SYS
101
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
201
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
301
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
401
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
501
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
601
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
701
13 0.000000E+00 0.000000E+00 1.200000E+02 0.000000E+00 0.000000E+00 0.000000E+00
------------- ------------- ------------- ------------- ------------- ------------MAX (for output set):
0.000000E+00 0.000000E+00 1.200000E+02 0.000000E+00 0.000000E+00 0.000000E+00
MIN (for output set):
0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
ABS (for output set):

0.000000E+00 0.000000E+00 1.200000E+02 0.000000E+00 0.000000E+00 0.000000E+00
------------- ------------- ------------- ------------- ------------- ------------APPLIED FORCE TOTALS: not printed since all grids do not have the same global coordinate system

206

SUBCASE
35
ROD WITH AXIAL LOADS IN 2 SUBCASES
120 LB LOAD ON GRID 701
S P C
F O R C E S
(in global coordinate system at each grid)
T2
T3
R1
R2

GRID

COORD
T1
R3
SYS
101
0 0.000000E+00 -1.200000E+02 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
201
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
301
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
401
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
501
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
601
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
701
13 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
------------- ------------- ------------- ------------- ------------- ------------MAX (for output set):
0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
MIN (for output set):
0.000000E+00 -1.200000E+02 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
ABS (for output set):

0.000000E+00 1.200000E+02 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
------------- ------------- ------------- ------------- ------------- ------------SPC FORCE TOTALS: not printed since all grids do not have the same global coordinate system

SUBCASE
35
ROD WITH AXIAL LOADS IN 2 SUBCASES
120 LB LOAD ON GRID 701

Element
Axial
ID
Force
1 1.200000E+02
4 1.200000E+02

Torque
0.000000E+00
0.000000E+00

E L E M E N T
E N G I N E E R I N G
F O R C E S
F O R
E L E M E N T
T Y P E
R O D
Element
Axial
Torque
Element
Axial
ID
Force
ID
Force
2 1.200000E+02 0.000000E+00
3 1.200000E+02
5 1.200000E+02 0.000000E+00
6 1.200000E+02

Torque
0.000000E+00
0.000000E+00

SUBCASE
35
ROD WITH AXIAL LOADS IN 2 SUBCASES
120 LB LOAD ON GRID 701
E L E M E N T
Element
ID
1
3
5

Axial
Stress
2.000000E+02
2.000000E+02
2.000000E+02

S T R E S S E S
I N
L O C A L
F O R
E L E M E N T
T
Safety
Torsional
Safety
Margin
Stress
Margin
4.90E+01
0.000000E+00
4.90E+01
0.000000E+00
4.90E+01
0.000000E+00

E L E M E N T
C O O R D I N A T E
S Y S T E M
Y P E
R O D
Element
Axial
Safety
Torsional
ID
Stress
Margin
Stress
2 2.000000E+02 4.90E+01
0.000000E+00
4 2.000000E+02 4.90E+01
0.000000E+00
6 2.000000E+02 4.90E+01
0.000000E+00

207

Safety
Margin

SUBCASE
8
ROD WITH AXIAL LOADS IN 2 SUBCASES
240 LB ON GRID 201 + 150 LB ON GRID 301 + 200 LB ON GRID 401
D I S P L A C E M E N T S
(in global coordinate system at each grid)
T2
T3
R1
R2

GRID

COORD
T1
R3
SYS
101
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
201
0 0.000000E+00 9.833333E-04 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
301
0 0.000000E+00 1.566667E-03 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
401
0 0.000000E+00 1.900000E-03 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
501
0 0.000000E+00 1.900000E-03 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
601
0 0.000000E+00 1.900000E-03 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
701
13 0.000000E+00 0.000000E+00 1.900000E-03 0.000000E+00 0.000000E+00 0.000000E+00
------------- ------------- ------------- ------------- ------------- ------------MAX (for output set):
0.000000E+00 1.900000E-03 1.900000E-03 0.000000E+00 0.000000E+00 0.000000E+00
MIN (for output set):
0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
ABS (for output set):

0.000000E+00

1.900000E-03

0.000000E+00

SUBCASE
8
ROD WITH AXIAL LOADS IN 2 SUBCASES
240 LB ON GRID 201 + 150 LB ON GRID 301 + 200 LB ON GRID 401

GRID

A P P L I E D
F O R C E S
(in global coordinate system at each grid)
T2
T3
R1
R2

COORD
T1
R3
SYS
101
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
201
0 0.000000E+00 2.400000E+02 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
301
0 0.000000E+00 1.500000E+02 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
401
0 0.000000E+00 2.000000E+02 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
501
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
601
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
701
13 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
------------- ------------- ------------- ------------- ------------- ------------MAX (for output set):
0.000000E+00 2.400000E+02 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
MIN (for output set):
0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
ABS (for output set):

0.000000E+00 2.400000E+02 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
------------- ------------- ------------- ------------- ------------- ------------APPLIED FORCE TOTALS: not printed since all grids do not have the same global coordinate system

208

SUBCASE
8
ROD WITH AXIAL LOADS IN 2 SUBCASES
240 LB ON GRID 201 + 150 LB ON GRID 301 + 200 LB ON GRID 401
S P C
F O R C E S
(in global coordinate system at each grid)
T2
T3
R1
R2

GRID

COORD
T1
R3
SYS
101
0 0.000000E+00 -5.900000E+02 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
201
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
301
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
401
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
501
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
601
0 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
701
13 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
------------- ------------- ------------- ------------- ------------- ------------MAX (for output set):
0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
MIN (for output set):
0.000000E+00 -5.900000E+02 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
ABS (for output set):

0.000000E+00 5.900000E+02 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
------------- ------------- ------------- ------------- ------------- ------------SPC FORCE TOTALS: not printed since all grids do not have the same global coordinate system

SUBCASE
8
ROD WITH AXIAL LOADS IN 2 SUBCASES
240 LB ON GRID 201 + 150 LB ON GRID 301 + 200 LB ON GRID 401
E L E M
Element
ID
2

Grid
Point
201
301
501
601

MAX (for output set):
MIN (for output set):

0.000000E+00
0.000000E+00
0.000000E+00
0.000000E+00
------------0.000000E+00
0.000000E+00

ABS (for output set):

0.000000E+00

>> LINK

N O D A L
F O R
T2

F O R C E S
E L E M E N T
T3

-3.500000E+02 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
3.500000E+02 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
-2.273737E-13 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
2.273737E-13 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
------------- ------------- ------------- ------------- ------------3.500000E+02 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
-3.500000E+02 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00
3.500000E+02

0.000000E+00

9 END

>> MYSTRAN END

I N
G L O B A L
C O O R D S
T Y P E
R O D
R1
R2
R3

1/19/2006 at 15: 5: 3.8

209

0.000000E+00

8 Appendix B: Equations for the reduction of the G-set to the Aset and solution for displacements and constraint forces

210

8.1

Introduction

As discussed in Section 3.6, MYSTRAN builds the original stiffness and mass matrices based on the
G-set, which has 6 degrees of freedom per grid specified in the Bulk Data deck. The stiffness matrix
is by definition singular as, at this point, there have been no constraints imposed. There are two type
of constraints MYSTRAN allows; single point constraints and multi-point constraints as discussed
earlier in this manual. In order to apply boundary conditions that restrain the model from rigid body
motion, single point constraints must be used. Multi-point constraints (using rigid elements or Bulk
Data MPC entries) are used to express some degrees of freedom (DOF’s) of the model as being
rigidly restrained to some other DOF’s. Thus, MYSTRAN must reduce the G-set stiffness, mass, and
loads to the independent A-set DOF’s
The discussion below shows the process that MYSTRAN uses to solve for the displacements and
constraint forces by going through a systematic reduction of the G-set to the N-set then to the F-set
and finally to the L-set which represent the independent DOF’s. These equations can then be solved
for the L-set DOF’s. The other DOF displacements, as well as constraint forces, can then be
recovered. Element forces and stresses are obtained from the displacements as discussed in
Appendix C. The process in this appendix uses the displacement set notation developed in Section
3.6 which should be reviewed prior to this section. In general, the matrix notation used in this
development is such that the matrix subscripts describe the matrix size. Thus, KGG is a matrix which
has G rows and columns, RCG is a matrix that has C rows and G columns and RTCG is the transpose
of RCG and has G rows and C columns. If a matrix has only one column, it would exhibit only one
subscript, as in YS which is an S x 1 matrix of single point constraint values

8.2

Reduction of the G-set to the N-set

In terms of this G-set, the equations of motion for the structure can be written as:
  K U  P  RT q
MGGU
G
GG G
G
CG C

(8-1)
RCGUG  YC

In the first of equations 8.1 MGG is the G-set mass matrix, KGG is the G-set stiffness matrix, UG are the
G-set displacements, PG are the applied loads on the G-set DOF’s and qC are the independent,
generalized, constraint forces (due to single and multi-point constraints). The second of 8.1
expresses the constraints (both single and multi-point constraints) wherein C is the number of
constraint equations, RCG is a constraint coefficient matrix and YC is a vector of constraint values. For
example, if all of the constraints were single point constraints, then all of the coefficients in any one
row of RCG would be zero except for one unity value. In addition, if all of these single point constraints
were for DOF’s that are grounded, then all of the YC values would be zero and these single point
constraints would all have the form of ui = 0.
The unknowns in 8.1 are the UG displacements and the qC generalized constraint forces and there
are G+C equations to solve for these unknowns. As will be explained later, direct solution of the qC
constraint forces will not be made.
The qC generalized forces of constraint do not necessarily have any physical meaning. Rather, the
G-set nodal forces of constraint are of interest and are expressed in terms of the qC as:
QG  RT CG qC

In order to reduce 8.1 the G-set is partitioned into the N and M-sets, where the M DOF’s are to be
eliminated using the multi-point constraints (from rigid elements as well as MPC Bulk Data entries
211

(8-2)

defined by the user in the input data deck). The UN are the remainder of the DOF’s in the G-set.
Thus, write UG as:
U 
UG   N 
UM 

(8-3)

The number of constraints is C which is equal to M+S (where S is the number of DOF’s in the S set).
Thus, partition qC and YC as:
q 
qC   S 
qM 

(8-4)
Y 
YC   S 
0M 

0M is a column vector of M zeros. That is, only the S-set can have nonzero constraint values.
With the second of 8.4 in mind, partition the second of equations 8.1 using 8.3 as:
 RSN 0SM  UN   YS 

    
RMN RMM  UM  0M 

(8-5)

The 0SM partition is an S x M matrix of zero’s. This is required by the form of the single point
constraint equations which are all of the form ui = Yi where Yi is a constant (zero or some enforced
displacement value).
Using 8.3, partition the first of equations 8.1 as:
T
T 
   K
 MNN MNM  U
KNM  UN  PN  RSN
RMN
 qS 
NN
N

 T
   T
      T


T

M NM MMM  UM  K NM K MM  UM  PM   0SM RMM  qM 

(8-6)

The bars over the N-set mass, stiffness and loads matrices are used for convenience to distinguish
these terms from those that will result from the reduction of the G-set to the N-set. From the second
of the constraint equations in 8.5 solve for UM in terms of UN:
UM  GMNUN

(8-7)

1
GMN  (RMM
RMN )

(8-8)

U   I 
UG   N    NN  UN
UM  GMN 

(8-9)

where

Using 8.7, equation 8.3 can be written as:

where INN is an identity matrix of size N.
Substitute 8.9 into 8.6 and premultiply the result by the transpose of the coefficient matrix in 8.9. The
result can be written as:

212

q 
T
T
T
  K U  P  RT
 GMN
MNNU
(RMN
RMM
)  S 
N
NN N
N
 SN
 q
 M

(8-10)

where:
T
KNN  KNN  KNMGMN  (KNMGMN )T  GMN
KMMGMN

T
MNN  MNN  MNMGMN  (MNMGMN )T  GMN
MMMGMN

(8-11)

T
PN  PN  GMN
PM

MNN , KNN and PN are the reduced N-set mass stiffness and loads. Note that PN is not the set of
applied loads on the N-set if there are applied loads on the M-set as expressed by the second of
equations 8.11 ( PN are the applied loads on the N set).
In addition, the second term in the square brackets in 8.10 is zero by the definition of GMN in 8.8 so
that 8.10 and 8.5 can be written as:
  K U  P  RT q
MNNU
N
NN N
N
SN S

8.3

(8-12)

Reduction of the N-set to the F-set

The N-set can now be partitioned into the F and S-sets where the S DOF’s are to be eliminated using
the single point constraints identified by the user in the input data deck. The F-set are the remainder
of the DOF’s in the N-set and are known as the “free” DOF’s (i.e. those that have no constraints
imposed on them). Thus, partition UN into UF and US:
U 
UN   F 
US 

(8-13)

Rewrite equation 8.5 in terms of the F, S and M-sets with the restriction that the single point
constraints are of the form ui = Yi where Yi is a constant (zero or some enforced displacement value),
using:
RSN  0SF ISS 
RMN  RMF RMS 

(8-14)

where OSF is an S x F matrix of zeros and ISS is an S size identity matrix. Equation 8.5 can be written
as:

 0SF ISS

RMF RMS

U 
OSM   F   YS 
 U    
RMM   S  0M 
UM 

Substitute 8.13 and the first of 8.14 into 8.12 and partition the mass, stiffness and load matrices into
the F and S-sets to get:

213

(8-15)

MFF
 T
MFS

  K
MFS  U
FF
F
      T
MSS  US  K FS

K FS  UF  PF  OFS 
     
 qS
K SS  US  PS   ISS 

(8-16)

Note that 0SF is the transpose of 0FS and is an S x F matrix of zero’s. From the first of 8.15 it is seen
that the single point constraints are of the form:
US  YS  constants

(8-17)

where YS is a column matrix of known constant displacement values (either zero or some enforced
displacement). This agrees with the single point constraint form discussed above; that is, single point
constraints express one DOF as being equal to a constant.
Substituting 8.17 into the first of 8.16 results in the equations for the F-set displacements:
  K U  P
MFFU
F
FF F
F

(8-18)

PF  PF  KFS YS

(8-19)

where

At this point the F-set equations in 8.18 can be solved for since there are F unknowns and F
equations with which to solve for them. However, MYSTRAN also allows for a Guyan reduction
which, although not generally used in static analysis, may be relevant for eigenvalue analysis. In
eigenvalue analyses by the GIV method (see EIGR Bulk Data entry), the mass matrix must be
nonsingular. In a situation where the model has no mass for the rotational DOF’s, the mass matrix
would be singular. Guyan reduction to statically condense massless DOF’s will result in a
nonsingular mass matrix. Thus, if the user identifies an O set, there is a further reduction; that from
the F-set to the A-set

8.4

Reduction of the F-set to the A-set

The F-set is partitioned into the A and O-sets where the O DOF’s are to be eliminated using Guyan
reduction identified by the user either through the use of ASET/ASET1 or OMIT/OMIT1 entries in the
input data deck. The A-set are the remainder of the DOF’s in the F-set and are known as the
“analysis” DOF’s. Thus, partition UF into UA and UO:
U 
UF   A 
UO 

(8-20)

Substitute 8.20 into 8.18 and partition the stiffness and load matrices into the A and O-sets to get:

MAA
 T
MAO

  K
MAO  U
K AO  UA  PA 
AA
A
   T
    
  K
MOO  U
 UO  PO 
O   AO K OO 

(8-21)

Guyan reduction is only exact, in general, for a statics problem. In a dynamic problem it is only exact
if there is no mass on the O-set. In order to explain the Guyan reduction, consider equation 8.21 for a
statics problem:
 =0) the second of 8.21 can be used to get:
In a static analysis ( U

214

K AA
 T
K AO

K AO  UA  PA 
    
K OO  UO  PO 

(8-22)

From the 2nd of 8.22 we can solve for UO in terms of UA . We can then write:
UA 
 
UO 
where

 0 
 IAA 

 UA   0 
GOA 
UO 

1 T
GOA  K OO
K AO

(8-23)

and
1
U0O  K OO
PO

The first part of the first equation in 8.23 suggests the possibility of using:
UA 
 
UO 

 IAA 

 UA
GOA 

(8-24)

Using 8.24 in 8.22 and premutiplying by the transpose of the coefficient matrix in 8.24 yields:
IAA

K
T
  TAA
GOA
K AO

K AO   IAA  UA 

    IAA
K OO  GOA  UO  

P 
T
  A 
GOA
PO 

or
K AA UA  PA

(8-25)

where
K AA  K AA  K AO GOA  (K AO GOA )  G K OO GOA  K AA  K AO GOA (by virtue of definition of GOA )
T

T
MN

and
T
PA  PA  GOA
PO

Which is exactly what would have been found if 8.23 had been substituted into 8.22 for UO .
Equation 8.24 to can be used as a way to eliminate the O-set degrees of freedom for the dynamic
system of equations in 8.21. This would be an approximation unless there was no mass associated
with the O-set degrees of freedom and is the classic Guyan reduction approximation made in
dynamic analyses in which the O-set is eliminated by static condensation (i.e. using the GOA in
equation 8.23). Using 8.24 in 8.21 yields
IAA

MAA
T
GOA
 MT
 AO

 
MAO   IAA  U
A
    IAA


MOO  GOA  UO 

K AA
T
GOA
 K T
 AO

where:

215

K AO   IAA  UA 

    IAA
K OO  GOA  UO  

PA 
T
GOA
 P  (8-26)
 O 

  K U  P
MAA U
A
AA A
A
where
T
MAA  MAA  MAO GOA  (MAO GOA )T  GOA
MOO GOA

(8-27)

K AA  K AA  K AO GOA
T
PA  PA  GOA
PO

Now, equation 8.27 can be solved for the A-set DOF displacements. The process of recovering the
displacements of the O, S and M-set displacements is accomplished by reversing the process we just
went through in the reduction. First, the O set displacements are recovered using 8.23. The
combination of the A and O-sets yields the F-set. The S-set is given by 8.17. The combination of the
F and S-sets yields the N-set. The M-set is recovered from the N-set by 8.7 and the combination of
the N and M-sets yield the complete model displacements in the G-set.

8.5

Reduction of the A-set to the L-set

The A-set is partitioned into the L and R-sets where the R DOF’s are boundary DOF’s where one
substructure attaches to another in Craig-Bampton (CB) analyses. The modal properties of the
substructure in CB analysis are fixed boundary modes so that, for the modal portion of CB, the R-set
are constrained to zero. The development of the subsequent CB equations of motion in terms of the
modal and boundary DOF’s will not be presented here. See Appendix D and reference 11 for a
complete discussion of CB analyses. For other analyses there is no R-set so that the L set is the
same as the A set for solution of the independent degrees of freedom
U 
UA   L 
UR 

8.6

Solution for constraint forces

The constraint forces are recovered as follows. Rewrite 8.2 by partitioning QG into QF, QN and QM
and partitioning qC into qS and qM. Using the coefficient matrix in 8.15 for RCG we get, for QG:
 QF 
 
QG   QS  
Q 
 M

 0FS

 ISS

0MS

T 
RMF
 q 
T
RMS
 S
q
T  M
RMM


(8-28)

As discussed earlier, the distinction between the q and Q is that the former are generalized forces of
constraint and the later are physical constraint forces on the DOF’s of the model. It is the Q
constraint forces that are of interest.

216

Rewrite 8.28 as:
T
 0F   RMF 


 
T
QG   qS   RMS
 qM
0   T 
 M  RMM 

(8-29)

where 0F and 0M are null column matrices of size F and M.
Equation 8.29 can be written as:
QG  QGSPC  QGMPC

(8-30)

The first term in 8.30 represents the forces of single point constraint and the second the forces of
multi-point constraint. Comparing 8.29 and 8.30:

QGSPC

 0F 
 
  qS 
0 
 M

(8-31)
QGMPC 

T 
 RMF
 T 
RMS  qM
 T 
RMM 

From the first of 8.31 it is seen that the grid point SPC constraint forces are equal to the generalized
qS forces. Using 8.17 and the second of 8.16 (keeping in mind that the derivatives of the S-set
degrees of freedom are zero due to 8.17) the qS, or QS is:

QGSPC

0F
 0F  


 
T
  K U  K Y  P 
 QSSPC   MFFU
FF
FS F
SS S
S

 

0
M

 0M  

(8-32)

Thus, there are SPC forces only on the S-set DOF’s
From the second of 8.31 and using 8.14 it is seen that the MPC forces can be written as:
RT 
QGMPC   MN  qM
T
RMM


(8-33)

From 8.7 and the second of 8.6, solve for qM :
T
T
  (K T  K G )U  P ]
qM  RMM
[(MNM
 MMMGMN )U
N
NM
MM MN
N
M

(8-34)

Substituting 8.34 into 8.33 yields:
RT R  T 
T
  (K T  K G )U  P ]
 MMMGMN )U
QGMPC   MN MM  [(MNM
N
NM
MM MN N
M
 IMM 

217

(8-35)

Using 8.8 this becomes:
 QNMPC   GT 
T
MN
  (K T  K G )U  P ]
QGMPC  
 [(MNM  MMMGMN )U

N
NM
MM MN N
M
Q
I
 MMPC   MM 

(8-36)

This can also be written as:
QNMPC 
QGMPC  

QMMPC 
with
  H U  P
QMMPC  LMNU
N
mn n
m
T
QNMPC  Gmn
QMMPC

(8-37)

where
T
Hmn  (KNM
 K MMGMN )
T
LMN  (MNM
 MMMGMN )

There are MPC forces on the N-set (which includes the F and S-sets) as well as on the M-set.
Equations 8.32 and 8.36 (or 8.37) are used to determine the constraint forces once the UG are found.
This completes the derivation of the solution for the G-set displacements and the constraint forces.
However, it is of interest to demonstrate that the constraint forces satisfy the principal of virtual work
(that is, constraint forces do no virtual work).
Let WC be the work done by the constraint forces and WC the virtual work done by the constraint
forces. Write WC as:
WC  WSPC  WMPC  0
where
WSPC  virtaul work of the SPC single point constraint forces

(8-38)

and
WMPC  virtaul work of the MPC multi-point constraint forces

The virtual work of the constraint forces is equal to the constraint forces moving through a virtual
displacement, U . Thus:

WSPC  QSTSPC US
By virtue of 8.17:

218

(8-39)

US  YS  0S

(8-40)

That is, the virtual displacements of the S-set are zero since YS contains specified values (zero or
some enforced displacement). Therefore:
Wspc  0

(8-41)

Thus WMPC must also be zero by virtue of the first of 8.38. This virtual work of the MPC forces can
be written as a combination of the virtual work of the MPC forces on the N and M-sets as follows:
T
WMPC  QNTMPC UN  QM
UM
MPC

(8-42)

T
WMPC  (QNTMPC  QM
GMN )UN
MPC

(8-43)

T
WMPC  (QNMPC  GMN
QMMPC )T UN  0

(8-44)

Using 8.7 this can be written as:

using 8-41:

Since the virtual displacements of the N-set are not necessarily zero this requires that:
T
QNMPC  GMN
QMMPC

(8-45)

This agrees with 8.36. Thus, the constraint forces developed above are consistent with the principal
of virtual work.

219

9 Appendix C: Equations for element stress recovery

220

9.1

General discussion

The element internal forces and stresses are recovered using the element displacements. These
displacements, along with several matrices, are used to calculate element stresses (as well as
element forces which are stress resultants).
For each element, an array called STRESS is calculated that is based on the parameters of the
particular element. This STRESS array can contain up to 9 rows and there is one of these calculated
for each subcase. Rows 1-3 are referred to as array STRESS1, rows 4-6 as STRESS2 and rows 7-9
as STRESS3. Array STRESS doesn’t necessarily contain actual stress values in all cases. It does,
however, contain the basic information needed to determine stresses throughout the element. In all
cases, array STRESS is:
STRESS1 


STRESS  STRESS2 


STRESS3 

(9-1)

where STRESSi has 3 rows and is written as the sum of two terms:
STRESSi  (SEi)  Ue  (STEi)

(9-2)

Ue are the displacements of the nodes of the element in the local element coordinate system (see
Figures 3-2 through 3-6 in the main body of this manual) and are obtained from the G-set
displacements, the solution for which is discussed in Appendix B. These G-set displacements for the
nodes of an element are transformed to the local element coordinate system to obtain Ue which has
a number of rows equal to 6n where n is the number of nodes for the element (e.g. n=4 for a
quadrilateral plate element). There is one Ue for each subcase in the solution. The SEi arrays each
have 3 rows and 6n columns and are based on the strain-displacement relationships for individual
elements. The STEi arrays contain the thermal stress effects, if there are any, and have 3 rows and
as many columns as there are thermal subcases.. That is, if the input data deck has 5 subcases and
two of these have thermal loads, then STEi will have only 2 columns while Ue will have 5 columns. If
a user outputs the SEi and STEi arrays, it is their responsibility to keep track of which subcases the
columns of STEi belong. MYSTRAN does this internally for its stress output calculations.
The following sections show what is contained in arrays STRESSi for each of the element types. In
that manner, it will be obvious how MYSTRAN uses the SEi and STEi arrays, generated internally in
MYSTRAN, to obtain stresses. If desired, they are available to be output to a text or unformatted
binary file through use of the Case Control entry ELDATA. They need not be output for the user to
obtain element stresses, however, which are available in the normal text output file through use of the
Case Control entry STRESS.

9.2

Rod element

The rod geometry and loading is shown in Figure 3-2 in the main body of this manual. It is a very
simple element and has only two stresses that can be output: the axial stress and the torsional stress.
It only uses the first 2 rows of array STRESS1 with row 1 being the axial stress and row 2 the torsional
stress. Array STRESS1 is:
axial 


STRESS1    
 0 



221

(9-3)

As an example of what is in arrays SE1 and STE1 for a simple element, the arrays are shown below
for this rod element. More complicated elements won’t have a simple closed form for these matrices
and will not be shown.
Array SE1 for the rod element is:
0
0 0 E 0 0
0
0 0
 E 0 0
1

SE1   0 0 0 C  G 0 0 0 0 0 C  G 0 0 
L
 0 0 0
0
0 0 0 0 0
0
0 0 

(9-4)

E and G are Young’s modulus and shear modulus from the Bulk Data material entry for the element,
L is the element length and C is the torsional stress recovery coefficient from a PROD entry.
Array STE1 would have the following column for each subcase that has a thermal load:
 1
 
STE1  E(T  Tref ) 0 
 
0 

(9-5)

 and Tref are the coefficient of thermal expansion and reference temperature from the material Bulk
Data entry for the element and T is the average element temperature for the thermal subcase.

9.3

Bar element

The bar element geometry and loading is shown in Figures 3-3 and 3-4 in the main body of this
manual. For the bar element, array STRESS uses all 3 rows of STRESS1 and STRESS2. The first
row of STRESS1 contains the actual axial stress in the bar and the third row of STRESS2 contains the
actual torsional stress. The second and third rows of STRESS1 and the first two rows of STRESS2 are
not actual stress values. Rather, they are the four independent parameters needed to determine the
bending stresses at points in the bar cross-section. Thus:
axial 
 2a 




  , STRESS2   2b 
STRESS1   1a
  


 1b

 
where
M I  M2aI12
M I  M2bI12
  1a 2
  1b 2
1a
, 1b
2
2
I1I2  I12
I1I2  I12
2a 

M2aI1  M1aI12
2
I1I2  I12

2b 

(9-6)

M2bI1  M1bI12
2
I1I2  I12

and
axial  Axial stress at the neutral axis
  Torsional stress
I1 , I2 , I12  the moments of inertia of the bar on the PBAR entry for this bar element
M1a , M2a , M1b , M2b = the moments in planes 1 and 2 at ends a and b of the bar

This can be put into the form of equation 8.2 as:

222

(9-7)

STRESS1  SE1 Ue  STE1
STRESS2  SE2  Ue  STE2
where
SE1  B1K aa

, STE1  B1K aa AT 

B1K ab 

SE2  B2K aa

B2K ab  , STE1  B2K aa AT 

Kaa and Kab are 6x6 partitions from the 1st 6 rows of the bar element stiffness matrix and B1, B2 and
A
are matrices of element properties as shown below:
 1
0 0 0
0
 A
B1   0
0 0 0 12

0
0 0 0 2



0 

1 

12 


0  L  L
0
1
12

B2  0 12L  2L
0

C
0
0
0
J

0
1

0 L1I1
6


L12I1
0
6
A
0
0

12I1
0
2

I

11
0
2

and

0
L1I1

1 
12 

0 


12
2
0

3
L12I1
3
0
12I1
2
1I1
2

L12I2
L 2I2
0
 2I2
12I2

2
2

0
L12I2
L 2I2
0
 2I2
12I2

3
3

2
2















T  Tref   avg bulk temp above material ref temp 

 

  gradient through bar in plane 1 at end a 
 T1a


 
T    T1b
   gradient through bar in plane 1 at end b 
 T   gradient through bar in plane 2 at end a 

 2a  
  gradient through bar in plane 2 at end b 
 T2b

with the following bar properties:

223

L  bar length
A  cross-sectional area
I1  area moment of inertia in plane 1
I2  area moment of inertia in plane 1
I12  product of inertia
1 
2 
12 

I2
2
I1I2  I12

I1
2
I1I2  I12

I12
2
I1I2  I12

Stresses due to bending (i.e. not including axial stress at the neutral axis) at ends a and b of the bar
element are obtained from:
 y e  2a ze ) ,
a  ( 1a

 ye  2b ze )
b  ( 1b

(9-8)

where a , b are the bending stresses at ends a and b of the bar and y e , ze are the coordinates of
a point on the bar cross section as measured in the local element coordinate system (see Figure 3-3
in the main body of this manual). It should be noted that temperature distributions through the depth
of the bar that are higher order than linear are ignored

9.4

Plate elements

Triangular and quadrilateral plate element geometry, loading and stress conventions are shown in
Figures 3-5 and 3-6 in the main body of this manual. They can use all three of the STRESSi arrays.

9.4.1 Membrane stresses
STRESS1 contains the membrane stresses (at the plate mid-plane)
 
 x 
STRESS 1   y 
 
xy z 0

(9-9)

This can be put into the form of equation 8.2 as:
STRESS1  (SE1)  Ue  (STE1)
where
SE1  EmBm

(9-10)
and

STE1  Em (T  Tref )

Em is the 3x3 membrane material matrix, Bm is the element membrane strain-displacement matrix
(developed internally in MYSTRAN),  is the 3x1 vector of coefficients of thermal expansion for the
material, T is the element average bulk temperature and Tref is the reference temperature for the
element material.

224

9.4.2 Bending stresses
STRESS2, times a fiber distance, contains the stresses due to bending, where:
 
 x 
STRESS2    y 


  xy 

(9-11)

This can be put into the form of equation 8.2 as:
STRESS2  (SE2)  Ue  (STE2)

(9-12)

where
SE2  EbBb

and

STE2  Eb T 

Eb is the 3x3 bending material matrix, Bb is the element bending strain-displacement matrix
(developed internally in MYSTRAN),  is the 3x1 vector of coefficients of thermal expansion for the
material and T  is the temperature gradient through the thickness of the plate element.

9.4.3 Combined membrane and bending stresses
The total bending and in-plane shear stresses at a fiber distance z are obtained from STRESS1 and
STRESS2 as:
 
 x 
  y   STRESS1  z(STRESS2 )
 
xy 

(9-13)

9.4.4 Transverse shear stresses
The average transverse shear stresses through the thickness of the plate (for TRIA3 and QUAD4
elements only) are obtained from STRESS3:
zx 
 
STRESS3  zy 
 
0 

This can be put into the form of equation 8.2 as
STRESS3  SE3
where
SE3  EsBs

Es is the 3x3 transverse shear material matrix and Bs is the element transverse shear straindisplacement matrix (developed internally in MYSTRAN).
225

(9-14)

The transverse shear stresses are not output in the normal output file even if stress output is
requested in Case Control. However, the transverse shear stress resultants (integrals of shear stress
through thickness) are output if there is a request in Case Control for element engineering forces

226

10 Appendix D: Craig-Bampton Model Generation

227

10.1 Craig-Bampton Equations of Motion for Substructures
MYSTRAN has the capability to generate Craig-Bampton (CB) models via SOL 31 (or SOL GEN CB
MODEL). This solution sequence calculates the fixed-base modes of a substructure and generates
all of the matrices needed to couple the substructure to other CB models. This appendix describes
the Craig-Bampton method and its implementation in MYSTRAN and includes an example problem to
explain the input and output for SOL 31.
Craig and Bampton 1 are credited with the first unified approach to modal synthesis, or substructuring
for dynamic analysis, using fixed interface flexible modes augmented by boundary constraint modes
to describe each substructure. Their work was a simplification of earlier work by Hurty 2 who first
introduced the concept for substructures with redundant boundary degrees of freedom (DOF’s).
In order to explain the Craig-Bampton (CB) method, consider a structure represented by the picture
below that is comprised of several (in this case 5) substructures connected at an arbitrary number of
points:

III
II

Figure 10.1 - Overall Structure Composed of Several Substructures

Each substructure is joined to one or more other substructures at some number of interface, or
boundary, DOF’s (indicated by the hatched areas in the above picture. The complete structure,
consisting of the connected substructures, may or may not be restrained from free body motion. For
any one of the substructures ( j = I, II, III, etc.) the G-set equations of motion (ignoring damping for
the moment) are:

Craig, R.R. and Bampton, M.C.C. “Coupling of Substructures for Dynamic Analysis”, AIAA Journal,
Vol. 6, No. 7, July 1968, pp 1313-1319
2
Hurty, W.C. “Dynamic Analysis of Structural Systems Using Component Modes”, AIAA Journal, Vol.
3, No. 4, April 1965, pp 678-685
228

j
j
Gj  K GG
MGG
u
uGj  PGj  QGj

where

QGj QmG  QGs  QrjG
j

uAj  
 j  analysis DOF's
u 
omitted DOF's 
uGj   Oj   

SPC'd DOF's 
uS  

uMj   MPC'd DOF's 
10-1

and

PGj

= applied loads on the G-set
j

QmG  constraint forces due to multi-point constraints (MPC's)
j

QGs  constraint forces due to single point constraints (SPC's)
j

QrG  interface forces at boundaries between substructures
In MYSTRAN nomenclature, the G-set is reduced to the A-set by the elimination of the M-set multipoint constraints, the S-set single point constraints and the O-set omitted DOF’s (using OMIT’s or
ASET’s). The A-set DOF’s for this substructure must contain all DOF’s that will be connected to other
substructures The resulting A-set equations of motion (dropping the j superscript notation for each
substructure) are:

A  K AA uA  PA  QrA
MAA u

10-2

where the A set matrices are mathematical reductions from the G-set (see Appendix B for details)
Partition 2 into the R-set and L-set, where, the R-set represents the boundary DOF’s in which this
substructure connects with other substructures and the L-set are all free interior DOF’s in this
substructure
T
T
R  K RR K LR
MRR MLR
 u
 uR  PR  QRr 




 

     
L
 MLR MLL  u
K LR K LL  uL  PL   o 

Notice at this point that there remain forces of constraint only at the substructure attach points as the
L-set represents all free DOF’s for this substructure.
At this point we can introduce the transformation from the physical displacements in equation (3) to
what are known as the CB DOF’s; namely the flexible mode DOF’s and the boundary (R-set) DOF’s.
In order to show that this is not any further approximation to equation 3, consider the following
argument:

uR 
 DOF’s are clearly a complete set of DOF’s for the substructure in that,
uL 

1) the uA  

once they are known, the complete g-set DOF’s for this substructure can be determined.

229

10-3

2) similarly, a new set of DOF’s for the substructure,

u 
uX   R 
 N 

10-4

are a complete set of DOF’s if N are the generalized DOF’s for flexible modes when

uR  0
3) Thus we can take uL to be a linear combination of uR and N or:

uL  DLRuR  LNN

10-5

if we insist that:
a) LN are shapes when uR  0 and N are modal DOF’s. That is, the columns of

LN are the flexible modes, Li , when the boundary is fixed. The i-th column of the
modal matrix

LN is Li .

b) DLR are shapes when

N  0 . That is, the columns of DLR are the L-set shapes

for unit motions of the R-set when the flexible mode DOF’s are zero.

Li are easy to understand. They are the eigenvectors resulting from solving an eigenvalue
problem from equations 3 with uR  0 . This eigenvalue problem would be:

The

(K LL  2MLL )L  0

10-6

This requires that the determinant of the coefficient matrix on the left side of equation 6 be zero:

K LL  2MLL  0

which yields N eigenvalues

12 , 22 , N2  0

10-7

The i-th eigenvector, L , is then determined by solving the equation:
i

(K LL  i2MLL )Li  0

Solution of equation 8 requires that one element of

for

i  1, 2,,N

10-8

Li be arbitrarily set (the Li are shapes and their

amplitude does not matter). Once equation 8 is solved, the modal matrix is:

LN  1l l2  NL 

DLR can also be explained easily. As stated above, the DLR are shapes when the flexible mode
response is zero. We can see from equation 5 that a column of DLR represents the displacements at
The

the L-set DOF’s due to motion at one of the R-set DOF’s while all other R-set DOF’s are zero (as well
230

10-9

as all N  0 ). We can therefore solve for

DLR from equation 3 by taking all applied forces and

accelerations equal to zero and solving the statics problem:
T
K RR K LR
 uR  QRr 

 s   
 K LR K LL  uL   o 

10-10

uLs are static displacements of the L-set. From the second row of equation 10, solve for uLs in
terms of uR :

where

uLs  K LL1K LRuR  DLRuR
10-11

or
1
LL

DLR  K K LR
Thus, the CB DOF’s are contained in

uX (equation 4) and the transformation between uX and uA is:
uR   I
 
uL  DLR

0  uR 
 
LN   N 

10-12

where I is an R x R identity matrix. Equation 12 can be written as:

uA   AXuX
10-13

where

 I
 AX  
DLR

0 
u 
u 
, uA   R  , u X   R 

LN 
uL 
 N 

 AX is the CB transformation matrix and is of A-set size. In MYSTRAN this is called matrix PHIXA.
When expanded to G-set size, PHIXA becomes matrix PHIXG:

uG   GXuX
 GX  matrix data block PHIXG

10-14

PHIXG  PHIXA expanded to G-set
Note that when all flexible modes of the substructure are used in

uX equation 13 is exact. In

practice, all modes are never used since this would defeat the purpose of making the transformation
(which is to find a smaller set of DOF’s which are nonetheless an accurate representation of the Aset). Substituting equation 13 into equation 2 and premultiplying the result by the transpose of  AX
yields:

X  K XXuX  PX  QrX
MXXu
231

10-15

where:
T
T
 I DLR
 MRR MLR
 I
MXX   TAXMAA  AX  

T 
0 LN  MLR MLL  DLR

T
T
 I DLR
 K RR K LR
 I
K XX   TAXK AA  AX  



T
0 LN  K LR K LL  DLR

0  mRR

LN  mNR
0  k RR

LN   0

T

mNR

mNN 

0 
k NN 
10-16

T
 I DLR
 PR   PR 
T
PX   TAXPA  
    , PR  PR  DLRPL ,
T 

P

0
 N
LN   L 


T
N  LN
PL

T
 I DLR
 QRr  QRr 
QrX   TAXQrA  
 
T 
0

o
 0 
LN  


and:
T
T
T
mRR  MRR  MLR
DLR  (MLR
DLR )T  DLR
MLLDLR
T
mNR  LN
(MLR  MLLDLR )
T
mNN  LN
MLL LN

10-17

T
k RR  K RR  K LR
DLR
T
k NN  LN
K LL LN

mNN , k NN are diagonal matrices of generalized maesses and stiffnesses, respectively.

Equations 15 for the i-th substructure can be written as:

mRR

mNR

T
R  k RR
 u
mNR
    
mNN   N   0

0  uR   PR  QRr 
     
k NN   N  N   0 

The off-diagonal terms in the above stiffness matrix are zero due to the definition of

10-18

DLR in equation

k RR in equation 18 is null if the boundary is a determinant interface. Equations
14 and 18 are the Craig-Bampton equations of motion for the i-th substructure. The PR are due to

11. In addition, matrix

applied loads on the R and L-set DOF’s (see equation 16) and the

QRr are the interface forces where

substructures connect. Once the equations are developed for all substructures, the individual
substructures can be connected and the resulting equations solved for the combined R-set and N-set
DOF’s uR and N for all substructures. Once this is done, the forces of inter-connection, or
substructure interface forces, (that is, the

QRr ) can be solved from the individual substructure
232

equations in the top row of equation 18. Equation 14 is used to obtain displacements for all G-set
DOF’s.
Each organization that is developing a substructure in CB format would deliver the above coefficient
matrices in equations 14 and 18 to the organization that is doing the combined structure analysis. In
addition, Displacement and Load Transformation Matrices (DTM’s and LTM’s) collectively known as
Output Transformation Matrices, (OTM’s), described below, are also delivered as part of the CB
model.

10.2 Development of Displ Output Transformation Matrices (Displ OTM’s)
Typically, a set of displacement output transformation matrices (displ OTM’s, or DTM’s for short), is
delivered with a Craig-Bampton model to the organization that will couple all substructures and solve
for the primary unknowns ( uR and N and

QRr ) in order that desired displacements at some of the

substructure G-set DOF’s may be obtained along with the coupled solution.
Once the combined structure has been solved for the primary variables, the original

uL physical

DOF’s could be determined from equation 5 and then element forces and stresses could be
determined from the uR and uL displacements . This is called recovery of the uL DOF’s and
element forces and stresses using the Modal Displacement Method (MDM). However, as is often the
case, equations 18 are solved using a severely truncated set of modes for each substructure. While
this may not compromise the accuracy of the solutions for uR and N , it could compromise the
accuracy of element forces and stresses calculated using displacements determined from equation 5
with the truncated set of modes. In order to avoid this problem, the uL DOF’s can be found using the
Modal Acceleration Method (MAM), described below. It should be noted that the MAM described
below ignores damping forces so that it is only useful when the damping is small (e.g. less than 10%
or so).
From the bottom row of equation 3, solve for

uL in terms of the other variables in the equation:

1
1
1
R  MLLu
L )  K LL
uL  K LL
(MLRu
K LRuR  K LL
PL
1
1
R  MLLu
L )  DLRuR  K LL
 K LL
(MLRu
PL

10-19

L in equation 19, to get:
Differentiate equation 5 twice and use the result for u

1
1
uL   K LL
(MLR  MLLDLR ) K LL
MLL LN

The term

R 
u
 
DLR   N   K LL1P
u 
 R

10-20

1
K LL
MLL LN in equation 20. can be written in a form more convenient for calculation. From

equation 8 it can be seen that:
1
K LL
MLL Li 

so that
233

1 i
L
i2

1
K LL
MLL  1l l2  LN   1l l2

 12

N 
 L 




2
2








2 
N 

or
1
2
K LL
MLL LN  LNNN

10-21

where

2
NN

12






22







N2 

10-22

substitute equation 21 into equation 20 to get:

uL   K (MLR  MLLDLR ) LN
1
LL

2
NN

R 
u
 
1
DLR   N   K LL
PL
u 
 R

10-23

The various terms in the coefficient matrices in equation 23 are known as Displacement
Transformation Matrices (DTM’s). Equation 23 can be written as:

uL  DTM1LR DTM2LN

R 
u
 
DTM3LR   N   DTM4LL Pl
u 
 R

10-24

where
1
DTM1LR  K LL
(MLR  MLLDLT )
2
DTM2LN  LNNN

DTM3LR  DLR
1
DTM4LL  K LL

Equations 24 and 25 represent the MAM for recovering displacements for the L-set, for the i-th
substructure, once the assembled substructure equations have been solved for the uR and qN
DOF’s. Once the L-set displacements have been found, recovery of the remaining displacements in
234

10-25

the G-set is accomplished through the transformation matrices used in their elimination from equation
1 (for details see Appendix B). At the G-set level, equation 24 is:
uG  DTM1GR

DTM2GN

R 
u
 
DTM3GR   N   DTM4GL PL
u 
 R

uG  GZ uZ  DTM4GL PL

10-26

where

GZ  DTM1GR

DTM2GN DTM3GR   DTMGZ

and

R 
u
 
uZ   N  ,
u 
 R

where uZ are the Craig-Bampton Degrees of freedom (CB_DOF's)

.
where each of the G-set DTM’s in equation 26 is obtained from the L-set DTM’s in equation 25
through the normal recovery operations to build back up to the G-set from the L-set. The coefficient
matrix in equation 26 that has DTM’s 1 - 3 in it is called matrix PHIZG. The table below explains the
meaning of each of the DTM’s in equation 26:
Table 10.1
i-th col of:

DTM1GR

Represents:
displ’s of G-set due to a unit accel of the i-th interface DOF (all other R, N set DOF’s zero)

DTM2GN displ’s of G-set due to a unit accel of the i-th flex mode DOF (all other R, N set DOF’s
zero)

DTM3GR displ’s of G-set due to a unit displ of the i-th interface DOF (all other R, N set DOF’s zero)
DTM4GL displ’s of G-set due to a unit force on the i-th L-set DOF (all other L-set forces zero)

235

10.3 Development of Load Output Transformation Matrices (Load OTM’s)
Once the G-set displacements have been found, substructure element forces and stresses, as well as
grid point forces, can be recovered and assembled into a Loads Output Transformation Matrix, or
Load OTM (more commonly referred to as LTM). There are several types of quantities one may
desire in an LTM. Equations are developed, below, for several types of LTM quantities typically used
in CB analyses.

10.3.1 LTM Terms for Substructure Interface Forces
From the top row of equation 18, the interface forces can be determined once the substructures have
been coupled and the uR and N solved. The interface forces are:
T 
R  mNR
QRr  mRRu
N  k RRuR  PR

QRr  mRR

10-27

R 
u
 
N   IRRPR
k RR  
u 
 R

T
mNR

where IRR is an RxR identity matrix. Equation 27 can be written as:

Q  LTM21RR LTM22RN
r
R

R 
u
 
LTM23RR   N   LTM24RR PRr
u 
 R

or
QRr  JRZUZ  IRRPR
where
JRZ  LTM21RR LTM22RN LTM23RR   LTM2RZ
LTM21RR  mRR

10-28

T
LTM22RN  mNR

LTM23RR  k RR
LTM24RR  IRR

10.3.2 LTM Terms for Net cg Loads
Terms can also be included in the overall LTM that will recover what are known as “net” accelerations
at the center of gravity (cg) of the CB model. These are termed Net Load factors (NLF’s) and
r

represent rigid body accelerations of the cg due to the reaction (or interface) forces, QR . The
development below demonstrates how these are determined.
236

Define:

ucg  6 x 1 matrix of rigid body displacements of the cg of the substructure
uRrb  r x 1 vector of rigid body displacements at the r DOF
TR6  r x 6 matrix where each column represents rigid body displacements of

10-29

the r DOF due to a unit motion in one DOF at the cg

Qcg  6 x 1 vector of forces at the cg that are static equivalents of Qrr
Then:

uRrb  TR6ucg
10-30

and
T
Qcg  TR6
QRr

Substitute equation 27 into 30 for QR :
T
T 
R  mNR
Qcg  TR6
(mRRu
N  k RRuR  PR )

10-31

cg
Qcg  mcgu

10-32

For rigid body motion:

where mcg is the 6 x 6 rigid body mass matrix relative to the cg and is equal to:
T
mcg  TR6
mRR TR6

10-33

and mRR is given in equation 17. From equations 31 through 33 we can write the cg acceleration net
load factors (NLF’s) as:

1
1 T
cg  mcg
u
Qcg  mcg
TR6 mRR

T
mNR

R 
u
 
1 T
k RR   N   mcg
TR6PR
u 
 R

10-34

However, TR6k RR  0 since the columns of TR6 are rigid body modes. Therefore:
T

cg  m Qcg  m T mRR
u

1
cg

1 T
cg R6

237

T
NR

R 
u
 
1 T
0   N   mcg
TR6PR
u 
 R

10-35

which can be written as:

cg  LTM116R LTM126N
u

R 
u
 
0 6R  
N   LTM146R PR
u 
 R

where
1 T
LTM116R  mcg
TR6mRR

10-36

1 T
T
LTM126N  mcg
TR6mNR
1 T
LTM146R  mcg
TR6

LTM16Z  LTM116R LTM126N

0

10.3.3 LTM Terms for Element Forces and Stresses
In MYSTRAN, element forces and stresses are obtained from the G-set displacement vector and the
individual element stiffness matrices. Equation 26 is the G-set displacement vector:

uG  DTM1GR DTM2GN

R 
u
 
DTM3GR   N   DTM4GL PL   GZuZ  DTM4GL PL
u 
 R

Thus the columns of each of the DTM’s represents G-set displacements per unit value of one of the

R , 
N, uR , PL as described in Table 10.1. Therefore, each of the DTM’s can be used as if
variables u
they were a matrix of displacements in calculating element forces and stresses to give:

fe  LTM31eR LTM32eN

R 
u
 
LTM33eR   N   LTM34eL PL
u 
 R

where

fe  vector of element forces and stresses (e = number of finite elements )
LTM31eR  matrix of element forces and stresses due to G-set displ's DTM1GR

10-37

LTM32eN  matrix of element forces and stresses due to G-set displ's DTM2GN
LTM33eR  matrix of element forces and stresses due to G-set displ's DTM3GR
LTM34eL  matrix of element forces and stresses due to G-set displ's DTM4GL

LTM3eZ  LTM31eR LTM32eN LTM33eR 

10.3.4 LTM Terms for Grid Point Forces due to multi-point constraints (MPC’s)
There are cases in CB analyses in which the forces due to MPC’s are of interest. As an example, if a
user wishes to determine a load in a bolt at an interface between components, it is common to model
the bolt as an MPC where two coincident grids are constrained to have the same displacements.
This section develops the equations for determining an LTM for grid point MPC forces.
238

Equation 1 for the i-th substructure (dropping the superscript-j notation):

G  K GGuG  PG  QGs  QmG  QrG
MGGu

10-38

As described in section 10.1 the Q constraint forces on the right side of equation 38 are the constraint
forces on the S-set SPC DOF’s, the M-set MPC DOF’s and on the R-set boundary DOF’s
respectively. Since all of the boundary DOF’s are contained in the R-set there should be no
constraint forces on the S-set. That is, all S-set DOF’s should be the result of removing singularities
and not the result of grounding the model 3 . With this assumption, as well as the assumption that
there are no applied loads on the M-st degrees of freedom the following equation is valid for the MPC
forces on the M-set grids:

G  K GGuG  QrG
QmG  MGGu

10-39

We want to get 39 in a form like the other LTM’; that is, in terms of uZ .
From equation 26 with applied loads zero:

R 
u
 
uG  GZuZ , uZ   N 
u 
 R

10-40

The g-set DOF vector can also be written using equation 14:

u 
uG   GXuX , uX   R 
 N 

10-41

Differentiating twice:

G   GXu
X
u
This can also be written as:

G    GX
u

 
u
0  X 
uR 

10-42

Partition the x DOF’s into R and N as in equation 13. This will require partitioning  GX into submatrices for the R and N also, so that equation 42 can be written as:

This should be verified by the user by inspection of the forces of single point constraint in the output
from the analysis
239

G    GR
u

 GN

R 
u
 
0  N   GZuZ
u 
 R
10-43

where

 GZ    GR

 GN 0    GX

0

G respectively to get:
Substitute equations 40 and 43 into 39 for uG and u
QmG  MGG  GZuZ  K GGGZuZ  QrG

10-44

We need to express the boundary constraint forces in equation 44 in terms of the uZ vector as we did
for the inertia and stiffness terms. From 28:

QRr  JRZuZ  IRRPR
r

10-45
r

The QR boundary forces on the R-set can be expanded from the R-set to the G-set QG by adding
zero rows to 45 for the M, S, O-sets (all of the G-set but the R degrees of freedom) to give

QrG  JGZuZ  IGRPR

10-46

where JGZ is JRZ expanded to G-set size by addition of zero rows for M, S, O-sets and IGR is
expanded from IRR in the same fashion (recall IRR is an R size identity matrix). Substituting 46 into 44
we get::

QmG  (MGG  GZ  K GGGZ  JGZ )uZ
or

QmG  LTM4GZ uZ
where

LTM4GZ  (MGG  GZ  K GGGZ  JGZ )
LTM4GZ is the LTM for MPC forces at grids that have no applied load

240

10-47

10.4 Development of Acceleration Output Transfer Matrices (Accel OTM)
In addition to the displacement and load output transformation matrices (DTM’s and LTM’s) it is
common to supply acceleration output transformation matrices (accel OTM’s or ATM’s for short).
From equation 10-12 and differentiating twice we obtain:

R 
R 
u
u
     ATM  
uL 
 N 
where

10-48

 I
ATM  
DLR

0 
LN 

ATM is the acceleration transfer matrix. Notice that the “degrees of freedom” for the ATM are the
accelerations of the boundary and modal degrees of freedom whereas all of the other OTM’s have as
degrees of freedom: boundary accelerations, modal accelerations and boundary displacements.
This is due to the use of the modal acceleration method for recovery of displacements and element
forces.

241

10.5 Correspondence between matrix names and CB Equation Variables
The table below shows the correspondence between variables introduced in the above equations and
matrix data block names in the DMAP program in Section 10.5. Any of these may be output in a
MYSTRAN CB model generation analysis using the Executive Control entry OUTPUT4.

Table 10-2
Matrices that can be written to OUTPUT4 files
MYSTRAN NASTRAN
Matrix Name
DMAP
(OUTPUT4
Name
matrices)

CB equation variable in Appendix D
(where applicable)

LTM116r

LTM126N 0

Matrix size1

CG_LTM

DLR

LxR

EIGEN_VAL

LAMA

 2NN

NxN

EIGEN_VEC

PHIG

 GN , (LN with rows expanded to G-set)

GxN

GEN_MASS

mNN

Nx1 vector of
diag. terms

IF_LTM

KAA

K AA

AxA

KGG

K GG

GxG

KLL

K LL

LxL

KRL

KLR(t)

K LR

LxR

KRR

K RR

RxR

KRRcb

KBB

T
k RR  K RR  K LR
DLR

RxR

KXX

KRRGN

K XX

(R+N)x(R+N)

LTM

CG_LTM and IF_LTM merged

(6+R)x(2R+N)

RBMCG

mcg

6x6

Modal effective mass
Modal participation factors

Nx6
Nx6 or NxR

MCG

LTM21RR

16 MEFFMASS
17 MPFACTOR

LTM22RN LTM23RR 

Partition
rows
and/or
cols

6x(2R+N)

Rx(2R+N)

rows and
cols

rows

rows
rows and
cols
rows and
cols
rows and
cols
rows and
cols
rows and
cols
rows and
cols

rows and
cols
rows and
cols
rows and
cols
rows and
cols

MAA

AxA

MGG

GxG

MLL

LxL

MRL

RxL

MRN

T
mRN  mNR

RxN

rows

MRR

RxR

rows and
cols

MRR

242

Table 10-2 (con’t)
MYSTRAN NASTRAN
Matrix
DMAP
Name
Name
(OUTPUT4
matrices)
24

MRRcb

MBB

MXX

MRRGN

26
27
28
29

PA
PG
PL
PHIXG

30
PHIZG

T
T
T
mRR  MRR  MLR
DLR  (MLR
DLR )T  DLR
MLLDLR

m
MXX   RR
mNR

T

mNR

mNN 

Matrix size 4

RxR

Partition
rows
and/or
cols
rows and
cols

(R+N)x(R+N)

(A-set static reduced loads - only used in statics)
(G-set static loads - only used in statics)
(L-set static reduced loads - only used in statics)

PHIXG

31
32

CB equation variable in Appendix D
(where applicable)

RBM0
TR6_0

TR6_CG

RBR

RBRCG

Rows
Rows
rows
Gx(R+N)

rows

Gx(2R+N)

rows

6x6
Rx6

rows

Rx6

rows

Notes:
a. (t) indicates matrix transposition
b. Matrix mRR will be singular if there are rotational DOF’s but no rotational
inertia in the R-set, in which case small rotational inertias may have to be
added at these DOF’s.
c.

Matrix k RR is null if the boundary is a determinant set of DOF’s.

d. Matrix mRR is the rigid body mass matrix if the boundary is a determinant set
of DOF’s

Matrix size given in rows x columns where R means the size of the R-set, L is the size of the L-set,
A is the size of the A-set, G is the size of the G-set and N is the number of eigenvectors. See section
3.6 for definition of the complete displacement set notation
243

10.6 Craig-Bampton model generation example problem
The figure below shows a small example problem that is a frame made of CBAR’s that is a
substructure assumed to be attached to some other structure in DOF’s 1,2,3 at grids 11 and 13 and in
DOF’s 2,3 at grid 12. The example problem F06 file (with the input echo’d) is shown on the following
pages. This section will discuss the input and output in an effort to explain the Craig-Bampton model
generation process.
Equation 10.26 defines the Craig-Bampton degrees of freedom (CB-DOF’s) as Uz which, for this
example, consists of the 18 DOF’s:


R
8 boundary acceleration DOF’s, u



2 modal acceleration DOF’s, 
N (see EIGRL request for 2 modes to be extracted)



8 boundary displacement DOF’s, uR

Figure 10.2 – Example CB model: CB-EXAMPLE-12b.DAT

244

Notes on section 10.6.1: CB-EXAMPLE-12b.F06
The echo of the input shows the following salient points for a CB model generation (much like a SOL
3 eigenvalue analysis in terms of input data):




Executive Control:


SOL 31 indicates CB model generation



The OUTPUT4 commands show the matrices that will be written in a format the same as
NASTRAN OUTPUT4 files. These matrix data blocks are ones that are listed on Table
10.2 as allowable OUTPUT4 matrices. Notice that several are written to unit 21 while
others are written to unit 22. As explained in section 5.1 of the MYSTRAN Users
Reference Manual, unit numbers 21 through 27 are valid for writing OUTPUT4 matrices.

Case Control:


METHOD = 1 is to be used for a normal eigenvalue analysis (same as if SOL were 3)



Outputs (ACCE, DISP, ELFORCE, STRESS) are for Output Transformation Matrices
(OTM’s) for the specified sets. These will be written to the text F06 file. In addition they
will be written to binary files (same name, CB-EXAMPLE-12b) with extension OP8 for the
element related OTM;s (ELFORCE, STRESS in this case and OP9 for the grid related
OTM’s (ACCE, DISP in this case)

Bulk Data:


Shows the model for this example (notice it has mostly CBAR’s but there is also a RBE2)



Degrees of freedom at the boundary where this substructure attaches to other
substructures are defined with the SUPORT Bulk Data entry. This is the same procedure
that is used in CB analyses by the NASTRAN DMAP (Direct Matrix Abstraction Program)
method familiar to NASTRAN CB analysts.



Eigenvalue extraction, EIGRL requesting 2 modes to be extracted

The delineated F06 output begins on the page following the input model echo and shows the
following:


Eigenvalues extracted



Messages on the matrices requested to be written to OUTPUT4 files



For the first 3 of the 18 CB_DOF’s in this example the following output (requested in Case
Control) is shown (other 15 were left out for clarity):



Displacement OTM for the requested grids (see Case Control command DISP = 102)



Element engineering force OTM (see Case Control command ELFORCE = 201)



Element stress OTM (see Case Control command STRESS = 202)

R
Acceleration OTM. As shown in equation 10.48 the acceleration OTM has columns for u
and 
N but not uR . For this example, there are 10 columns in the acceleration OTM (8
boundary acceleration DOF’s and 2 modal acceleration DOF’s)

245

Notes on section 10.6.2: OUTPUT4 matrices written to CB-EXAMPLE-12b.OP1 and OP2
As shown in the Executive Control section of the F06 file in section 10.6.1, there were 3 matrices
requested to be written to unit 21 and 4 to unit 22. These binary files, translated to text, are shown in
section 10.6.2. The number of actual columns for each matrix is indicated in Table 10.2 but only the
first 5 of the columns are shown here for the sake of brevity. These are several of the important CB
matrices needed to couple this CB substructure to other substructures in a combined analysis. The
binary OUTPUT4 files are written in the same format as the NASTRAN OUTPUT4 binary files.
Notes on section 10.6.3: Displ and elem force/stress OTM’s written to CB-EXAMPLE-12b.OP1, OP2
Any output requests in Case Control for grid related outputs (e.g. DISPL, ACCEL) and element
force/stress outputs (e.g. ELFORCE, STRESS) are written to the text F06 file and also written to
OUTPUT4 binary files (automatically; that is, no formal OUTPUT4 request is needed). The element
related OTM’s are always written to a file with the same filename as the F06 file but with extension
OP8. The grid related OTM’s are written to a file with extension OP9.
The first page of section 10.6.3 is a text translation of the element related OTM’s written to file
CB-EXAMPLE-12b.OP8. The values are the same as was written to the F06 file for element forces
and stresses but are also written to binary files in OUTPUT4 format to be used in analyses that
couple the CB substructures. In order to explain the contents of the binary OP8 file, a text file with
extension OT8 is also automatically written (provided any Case Control requests are included for
element forces/stresses) describing the contents of the OP8 binary file. This OT8 text file gives an
overview of the OP8 binary file and then goes on to describe each row written to the OP8 file.
The next several pages show the same type of information on the grid related OTM’s written to binary
file with extension OP9 (with text description in OT9). Again, this is the grid related outputs requested
in Case Control and also written to the F06 text file.
*

246

10.6.1 CB-EXAMPLE-12-b.F06
(delineated – some output not included here for the sake of clarity)

247

1030180330
MYSTRAN Version 3.00
>> MYSTRAN BEGIN
>> LINK

Oct 20 2006 by Dr Bill Case (this TRIAL edition is SP protected)

: 10/30/2006 at 18: 3:30.640 The input file is CB-EXAMPLE-12-b.DAT

1 BEGIN

SOL 31
$
OUTPUT4
CG_LTM
, IF_LTM
,
OUTPUT4
KRRGN
, RBMCG
, MRRGN
OUTPUT4
MR
,
,
CEND
TITLE = TEST OF CRAIG-BAMPTON SOLUTION
SUBTI = FRAME USING CBAR's
SPC
= 1
METHOD = 1
ECHO
= UNSORT
$
SET 101 = 32
SET 102 = 22, 32
SET 201 = 211, 212
SET 202 = 201
$
ACCE
= 101
DISP
= 102
ELFORCE = 201
STRESS
= 202
MEFFMASS = ALL
MPFACTOR = ALL
$
BEGIN BULK
$
EIGRL
1
2
$
EIGR
2
MGIV
+E1
MASS
GRID
11
0.
0.
GRID
12
100.
0.
GRID
13
50.
0.
GRID
21
0.
100.
GRID
22
100.
100.
GRID
31
50.
50.
GRID
32
50.
50.
$
RBE2
401
31
123456 32

,
,
,

,
//-1/21 $
, RBRCG //-1/22 $
,
//-1/21 $

DPB

-1.

MASS
+E1

0.
0.
50.
0.
0.
0.
0.

248

$
$ Frame support bars
$
CBAR
101
1
13
+C1
56
456
CBAR
102
1
13
+C2
56
456
$
$ Edge bars
$
CBAR
201
2
11
CBAR
202
2
12
CBAR
203
2
11
CBAR
204
2
21
$
$ Diag bars
$
CBAR
211
3
11
CBAR
212
3
12
CBAR
213
3
21
CBAR
214
3
22
$
PBAR
1
1
0.36
PBAR
2
1
0.10
PBAR
3
1
6.0
$
MAT1
1
10.+6
*INFORMATION: MAT1 ENTRY
$
CONM2
901
11
CONM2
902
12
CONM2
903
21
CONM2
904
22
CONM2
905
32
$
SPC1
1
456
13
$
$ BOUNDARY DOF'S
$
SUPORT 11
123
12
$
PARAM
WTMASS
.002591
$
ENDDATA

0.0

0.5

1.0

+C1

0.0

0.5

1.0

+C2

21
22
12
22

0.0
0.0
0.0
0.0

1.0
1.0
1.0
1.0

31
31
31
31

0.0
0.0
0.0
0.0

1.0
1.0
1.0
1.0

0.09
10.0
6.0

0.18
20.0
12.0

0.3
0.1
1 HAD FIELD FOR G
150.0
150.0
150.0
150.0
150.0

0.0
0.0
0.0
0.0
0.0

123

BLANK. MYSTRAN CALCULATED G
-5.0
-5.0
-5.0
-5.0
-5.0

249

3.846154E+06

E I G E N V A L U E

A N A L Y S I S

S U M M A R Y

NUMBER OF EIGENVALUES EXTRACTED

. . . . . .

LARGEST OFF-DIAGONAL GENERALIZED MASS TERM
. . .
MODE PAIR . . . . . . . . . .
. . .
NUMBER OF OFF DIAGONAL GENERALIZED MASS
TERMS FAILING CRITERION OF 1.0E-04. . . . .

MODE EXTRACTION
NUMBER
ORDER
1
2

1
2

>> LINK

4 END

>> LINK

6 BEGIN

EIGENVALUE

3.895211E+03
7.011163E+03

R E A L
E I G E N V A L U E S
RADIANS
CYCLES

6.241163E+01
8.373269E+01

9.933119E+00
1.332647E+01

250

(LANCZOS

Mode 2 DPB

Shift eigen = -1.00E+00)

2
-2.7E-13 (Vecs renormed to 1.0 for gen masses)
2
1

GENERALIZED
MASS

GENERALIZED
STIFFNESS

1.000000E+00
1.000000E+00

3.895211E+03
7.011163E+03

*INFORMATION: THE FOLLOWING

7 MATRICES WILL BE WRITTEN TO

2 OUTPUT4 FILES IN THE ORDER LISTED BELOW:

OUTPUT4 file
( 1)
( 2)
( 3)

on unit
CG_LTM
IF_LTM
MR

21 has been created as: CB-EXAMPLE-12-b.OP1 and
:
6 rows and
18 cols
This
:
8 rows and
18 cols
This
:
8 rows and
8 cols
This

will contain the matrices:
is MYSTRAN matrix CG_LTM
is MYSTRAN matrix IF_LTM
is MYSTRAN matrix MRRcb

OUTPUT4 file
( 1)
( 2)
( 3)
( 4)

on unit
KRRGN
RBMCG
MRRGN
RBRCG

22 has been created as: CB-EXAMPLE-12-b.OP2 and
:
10 rows and
10 cols
This
:
6 rows and
6 cols
This
:
10 rows and
10 cols
This
:
8 rows and
6 cols
This

will contain the matrices:
is MYSTRAN matrix KXX
is MYSTRAN matrix MCG
is MYSTRAN matrix MXX
is MYSTRAN matrix TR6

>> LINK

6 END

>> LINK

5 BEGIN

>> LINK

5 END

>> LINK

9 BEGIN

251

OUTPUT FOR CRAIG-BAMPTON DOF

1 OF

18
C B
D I S P L A C E M E N T
O T M
(in global coordinate system at each grid)
T2
T3
R1
R2

GRID

COORD
T1
SYS
0 -1.412939E-05 1.622140E-05 8.242222E-05 5.883709E-07 -1.667433E-06
0 1.051041E-05 -9.465944E-06 -3.182887E-06 -1.086181E-07 -9.450720E-07

22
32

R3
5.125151E-07
2.106009E-07

C B

E L E M E N T
E N G I N E E R I N G
F O R C E
O T M
F O R
E L E M E N T
T Y P E
B A R
Element
Bend-Moment End A
Bend-Moment End B
- Shear Axial
Torque
ID
Plane 1
Plane 2
Plane 1
Plane 2
Plane 1
Plane 2
Force
211 2.091876E-01 7.894539E-01 1.515607E+00 -1.439344E+00 -1.847556E-02 3.151997E-02 6.266800E-01 9.672846E-03
212 -1.133151E-01 -1.008960E-02 -1.725401E+00 -6.166148E-02 2.279833E-02 7.293366E-04 -2.953611E-01 -4.720428E-03

C B
Element
ID
201

E L E M E N T

S T R E S S
O T M
I N
L O C A L
E L E M E N T
C O O R D I N A T E
F O R
E L E M E N T
T Y P E
B A R
SA2
SA3
SA4
Axial
SA-Max
SA-Min
SB2
SB3
SB4
Stress
SB-Max
SB-Min

SA1
SB1
0.000000E+00
0.000000E+00

0.000000E+00
0.000000E+00

OUTPUT FOR CRAIG-BAMPTON DOF

GRID

2 OF

COORD
T1
SYS
0 -7.600290E-05
0 -5.990878E-05

22
32

0.000000E+00
0.000000E+00

S Y S T E M
M.S.-T
M.S.-C

0.000000E+00 -2.748670E+00 -2.748670E+00 -2.748670E+00
0.000000E+00
-2.748670E+00 -2.748670E+00

18
C B
D I S P L A C E M E N T
O T M
(in global coordinate system at each grid)
T2
T3
R1
R2

8.243595E-05
6.308617E-05

3.128787E-04
3.224179E-04

1.925291E-06
3.643362E-06

2.220055E-06
4.904270E-07

R3
1.292053E-07
3.218612E-08

C B

E L E M E N T
E N G I N E E R I N G
F O R C E
O T M
F O R
E L E M E N T
T Y P E
B A R
Element
Bend-Moment End A
Bend-Moment End B
- Shear Axial
Torque
ID
Plane 1
Plane 2
Plane 1
Plane 2
Plane 1
Plane 2
Force
211 3.640634E+00 -2.875040E+00 -7.752079E+00 4.486528E+00 1.611173E-01 -1.041083E-01 1.906435E+00 -5.333935E-03
212 3.789705E+00 2.992877E+00 -6.061077E+00 -4.713484E+00 1.393111E-01 1.089844E-01 1.808077E+00 5.333935E-03

C B
Element
ID
201

E L E M E N T
SA1
SB1

0.000000E+00
0.000000E+00

S T R E S S
O T M
I N
L O C A L
E L E M E N T
C O O R D I N A T E
F O R
E L E M E N T
T Y P E
B A R
SA2
SA3
SA4
Axial
SA-Max
SA-Min
SB2
SB3
SB4
Stress
SB-Max
SB-Min

0.000000E+00
0.000000E+00

7.582667E+00

252

7.582667E+00
7.582667E+00

S Y S T E M
M.S.-T
M.S.-C

OUTPUT FOR CRAIG-BAMPTON DOF

3 OF

C B
D I S P L A C E M E N T
O T M
(in global coordinate system at each grid)
T2
T3
R1
R2

GRID

COORD
T1
R3
SYS
0 3.800145E-05 -4.121798E-05 -1.564393E-04 -9.626456E-07 -1.110028E-06 -6.460267E-08
0 2.995439E-05 -3.154308E-05 -1.612090E-04 -1.821681E-06 -2.452135E-07 -1.609306E-08

22
32

C B
Element
Bend-Moment End A
ID
Plane 1
Plane 2
211 -1.820317E+00 1.437520E+00
212 -1.894852E+00 -1.496438E+00

C B
Element
ID
201

E L E M E N T
E N G I N E E R I N G
F O R C E
O T M
F O R
E L E M E N T
T Y P E
B A R
Bend-Moment End B
- Shear Axial
Torque
Plane 1
Plane 2
Plane 1
Plane 2
Force
3.876039E+00 -2.243264E+00 -8.055864E-02 5.205414E-02 -9.532175E-01 2.666968E-03
3.030538E+00 2.356742E+00 -6.965554E-02 -5.449220E-02 -9.040385E-01 -2.666968E-03

E L E M E N T
SA1
SB1

0.000000E+00
0.000000E+00

S T R E S S
O T M
I N
L O C A L
E L E M E N T
C O O R D I N A T E
F O R
E L E M E N T
T Y P E
B A R
SA2
SA3
SA4
Axial
SA-Max
SA-Min
SB2
SB3
SB4
Stress
SB-Max
SB-Min

0.000000E+00
0.000000E+00

0.000000E+00 -3.791334E+00 -3.791334E+00 -3.791334E+00
0.000000E+00
-3.791334E+00 -3.791334E+00

.
.
.
.
.
.
.
.
.

(output for the 4th – 18th CB DOF deleted)

253

S Y S T E M
M.S.-T
M.S.-C

OUTPUT FOR CRAIG-BAMPTON ACCEL OTM COL

GRID
32

COORD
T1
SYS
0 2.199853E-02 -2.028331E-02 -1.681579E-02 -3.363157E-04

COORD
T1
SYS
0 0.000000E+00

OUTPUT FOR CRAIG-BAMPTON ACCEL OTM COL

GRID
32

C B
A C C E L E R A T I O N
O T M
(in global coordinate system at each grid)
T2
T3
R1
R2

OUTPUT FOR CRAIG-BAMPTON ACCEL OTM COL

GRID

1 OF

COORD
T1
SYS
0 0.000000E+00

2 OF

8.006145E-03

0.000000E+00 -1.000000E+00 -2.000000E-02

0.000000E+00

R3
0.000000E+00

C B
A C C E L E R A T I O N
O T M
(in global coordinate system at each grid)
T2
T3
R1
R2
0.000000E+00

5.254334E-04

C B
A C C E L E R A T I O N
O T M
(in global coordinate system at each grid)
T2
T3
R1
R2

3 OF

5.000000E-01

1.000000E-02

0.000000E+00

.
.
.
.
.
.
.
.
.

(output for the 4th – 10th Accel OTM columns deleted)

254

R3
0.000000E+00

MODE
NUM
1
2

M O D A L
P A R T I C I P A T I O N
(dimensionless, in coordinate sys
T2
T3
R1

F A C T O R S
0)
R2

1.227574E-01 -1.758352E+00 8.791759E-01 1.259087E+00 6.535370E-02 -5.341716E-01
6.061630E-01 1.829524E-01 -9.147622E-02 -4.910542E-01 -1.366914E-01 -4.626569E-01

------------------------------------------------------------------------------------------------------------------------------------

E F F E C T I V E
M O D A L
M A S S E S
O R
W E I G H T S
(in coordinate system
0)
Units are same as units for mass input in the Bulk Data Deck
T1
T2
T3
R1
R2

MODE
R3
NUM
1 6.532677E+01 4.179096E+01 4.694259E+02 3.836785E+05 3.287406E+04 3.611917E+02
2 7.948285E+00 9.016521E-01 1.363070E+01 1.674257E+00 6.082279E+05 4.781873E+05
------------- ------------- ------------- ------------- ------------- ------------Sum all modes: 7.327506E+01 4.269261E+01 4.830566E+02 3.836801E+05 6.411019E+05 4.785485E+05
Total model mass: 9.325238E+02 9.325238E+02 9.325238E+02 4.105260E+06 4.094237E+06 8.139951E+06
Modes % of total mass*:
7.86
4.58
51.80
9.35
15.66
5.88
*If all modes are calculated the % of total mass should be 100% of the free mass (i.e. not counting mass at constrained DOF's).
Percentages are only printed for components that have finite model mass.
---->> LINK

9 END

>> MYSTRAN END

: 10/30/2006 at 18: 3:31.562

255

10.6.2 OUTPUT4 matrices written to CB-EXAMPLE-12-b.OP1 and OP2
(OUTPUT4 matrices requested in Exec Control)

256

OUTPUT4 matrices requested in Exec Control to be written to file CB-EXAMPLE-12-b.OP1 (on unit 21)
(note: only 1st 5 columns written here for the sake of clarity)
CG_LTM
1
2
3
4
5
6

1
-6.65821789802521E-05
-2.99785601343913E-05
-4.35697030582909E-05
-3.33844454038618E-04
8.13687816036514E-03
5.63393757592496E-04
IF_LTM

1
2
3
4
5
6
7
8

1
6.02957424769077E-01
7.32039059471623E-02
-3.66019529735811E-02
3.35492666170908E-02
-7.19015457719424E-02
-6.65046890695409E-01
-1.34708893096271E-01
6.78737140960850E-02
MR

1
2
3
4
5
6
7
8

1
6.02957424769077E-01
7.32039059471623E-02
-3.66019529735811E-02
3.35492666170908E-02
-7.19015457719424E-02
-6.65046890695409E-01
-1.34708893096271E-01
6.78737140960850E-02

NCOLS =

18
2
1.29562159612018E-17
-1.96135553418977E-04
-2.59100000000000E-03
-2.00000000000000E-02
1.47885176327023E-16
8.55130582230051E-17
NCOLS =

18
2
7.32039059471622E-02
4.25469107253153E+00
-2.12163357113457E+00
-2.21879607113459E+00
-1.10665832128050E-01
-7.32039059471504E-02
-2.21879607113459E+00
-1.83869738075211E-01
NCOLS =

8
2
7.32039059471622E-02
4.25469107253153E+00
-2.12163357113457E+00
-2.21879607113459E+00
-1.10665832128050E-01
-7.32039059471504E-02
-2.21879607113459E+00
-1.83869738075211E-01

NROWS =

6
3
-6.47810798060089E-18
1.04193052213477E-04
1.30775055100798E-03
9.80743672854175E-03
-7.39425881635114E-17
-4.27565291115026E-17
NROWS =

8
3
-3.66019529735811E-02
-2.12163357113457E+00
1.07224071582968E+00
1.10939803556729E+00
5.53329160640251E-02
3.66019529735752E-02
1.10939803556729E+00
9.19348690376054E-02
NROWS =

8
3
-3.66019529735811E-02
-2.12163357113457E+00
1.07224071582968E+00
1.10939803556729E+00
5.53329160640251E-02
3.66019529735752E-02
1.10939803556729E+00
9.19348690376054E-02

257

FORM

2
4
-1.29549999999999E-03
1.39356777670951E-03
1.29550000000001E-03
1.00000000000000E-02
-7.78457159844592E-17
9.99999999999996E-03
FORM

2
4
3.35492666170908E-02
-2.21879607113459E+00
1.10939803556729E+00
3.26418464157067E+00
1.75366508593570E-02
-1.24163383728600E+00
2.54146535101691E-01
8.11498842422746E-02
FORM

1
4
3.35492666170908E-02
-2.21879607113459E+00
1.10939803556729E+00
3.26418464157067E+00
1.75366508593570E-02
-1.24163383728600E+00
2.54146535101691E-01
8.11498842422746E-02

PREC

2
5
6.47766872193621E-05
-6.70858061739371E-05
6.19839872966866E-04
-5.07064059129018E-03
-5.93156091981744E-03
2.81696878796245E-04
PREC

2
5
-7.19015457719424E-02
-1.10665832128050E-01
5.53329160640251E-02
1.75366508593570E-02
4.96481812094837E-01
1.32307347677584E-01
3.05700710026811E-02
2.62006997196796E-02
PREC

.......
.......
.......
.......
.......
.......

2
5
-7.19015457719424E-02
-1.10665832128050E-01
5.53329160640251E-02
1.75366508593570E-02
4.96481812094837E-01
1.32307347677584E-01
3.05700710026811E-02
2.62006997196796E-02

.......
.......
.......
.......
.......
.......
.......
.......

OUTPUT4 matrices requested in Exec Control to be written to file CB-EXAMPLE-12-b.OP2 (on unit 22)
(note: only 1st 5 columns written here the sake of clarity)
KRRGN
1
2
3
4
5
6
7
8
9
10

1
1.19504240447136E+03
-5.45696821063757E-12
2.72848410531878E-12
2.08011385893769E-11
5.97521202235677E+02
-1.19504240447137E+03
-2.98427949019242E-13
-5.97521202235677E+02
0.00000000000000E+00
0.00000000000000E+00
RBMCG

1
2
3
4
5
6

1
2.41616914133782E+00
-3.30846461338297E-14
-6.52256026967279E-15
-1.35891298214119E-13
-3.92130772297605E-13
1.99662508748588E-12
MRRGN

1
2
3
4
5
6
7
8
9
10

1
6.02957424769077E-01
7.32039059471623E-02
-3.66019529735811E-02
3.35492666170908E-02
-7.19015457719424E-02
-6.65046890695409E-01
-1.34708893096271E-01
6.78737140960850E-02
1.22757372107055E-01
6.06162990294928E-01
RBRCG

1
2
3
4
5
6
7
8

1
1.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
1.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00

NCOLS =

10
2
-3.63797880709171E-12
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
-1.13686837721616E-13
0.00000000000000E+00
0.00000000000000E+00
-1.81898940354586E-12
0.00000000000000E+00
0.00000000000000E+00
NCOLS =

6
2
-3.35287353436797E-14
2.41616914133786E+00
2.27734497926235E-14
7.81374964731185E-13
2.88435941797616E-13
4.26325641456060E-14
NCOLS =

10
2
7.32039059471622E-02
4.25469107253153E+00
-2.12163357113457E+00
-2.21879607113459E+00
-1.10665832128050E-01
-7.32039059471504E-02
-2.21879607113459E+00
-1.83869738075211E-01
-1.75835189695839E+00
1.82952442095713E-01
NCOLS =

6
2
0.00000000000000E+00
1.00000000000000E+00
0.00000000000000E+00
1.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
1.00000000000000E+00
0.00000000000000E+00

NROWS =

10
3
1.81898940354586E-12
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
5.68434188608080E-14
0.00000000000000E+00
0.00000000000000E+00
9.09494701772928E-13
0.00000000000000E+00
0.00000000000000E+00
NROWS =

6
3
-6.52256026967279E-15
2.33146835171283E-14
2.41616914133783E+00
-1.24344978758018E-13
-6.75015598972095E-14
-3.62376795237651E-13
NROWS =

10
3
-3.66019529735811E-02
-2.12163357113457E+00
1.07224071582968E+00
1.10939803556729E+00
5.53329160640251E-02
3.66019529735752E-02
1.10939803556729E+00
9.19348690376054E-02
8.79175948479194E-01
-9.14762210478567E-02
NROWS =

8
3
0.00000000000000E+00
0.00000000000000E+00
1.00000000000000E+00
0.00000000000000E+00
1.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
1.00000000000000E+00

258

FORM

1
4
1.54614099301398E-11
1.81898940354586E-12
-9.09494701772928E-13
-1.16415321826935E-10
-1.59161572810262E-12
-1.79397829924710E-10
-4.31782609666698E-10
1.36424205265939E-12
0.00000000000000E+00
0.00000000000000E+00
FORM

2
4
-1.34114941374719E-13
7.74491581978509E-13
-9.59232693276135E-14
4.56169135583651E+03
-4.09272615797818E-12
-1.36424205265939E-11
FORM

1
4
3.35492666170908E-02
-2.21879607113459E+00
1.10939803556729E+00
3.26418464157067E+00
1.75366508593570E-02
-1.24163383728600E+00
2.54146535101691E-01
8.11498842422746E-02
1.25908689725916E+00
-4.91054200271590E-01
FORM

2
4
0.00000000000000E+00
-5.37849392786371E+01
-5.00000000000000E+01
-3.78493927863709E+00
-5.00000000000000E+01
0.00000000000000E+00
-3.78493927863709E+00
-5.00000000000000E+01

PREC

2
5
5.97521202235677E+02
0.00000000000000E+00
0.00000000000000E+00
9.43778388773353E-12
2.98760601117838E+02
-5.97521202235685E+02
-2.76401124210679E-12
-2.98760601117839E+02
0.00000000000000E+00
0.00000000000000E+00
PREC

2
5
-3.97903932025656E-13
2.89102075612391E-13
-7.10542735760100E-14
-3.86535248253495E-12
4.53313153018053E+03
2.85598256559946E+01
PREC

2
5
-7.19015457719424E-02
-1.10665832128050E-01
5.53329160640251E-02
1.75366508593570E-02
4.96481812094837E-01
1.32307347677584E-01
3.05700710026811E-02
2.62006997196796E-02
6.53537005701318E-02
-1.36691428775775E-01
PREC

.......
.......
.......
.......
.......
.......
.......
.......
.......
.......

.......
.......
.......
.......
.......
.......

2
5
5.37849392786371E+01
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
-5.00000000000000E+01
3.78493927863709E+00
0.00000000000000E+00
5.00000000000000E+01

.......
.......
.......
.......
.......
.......
.......
.......
.......
.......

.......
.......
.......
.......
.......
.......
.......
.......

10.6.3 Displ and Element force/stress OTM’s written to CB-EXAMPLE-12-b.OP8 and OP9
(OTM’s requested in Case Control)

259

CB-EXAMPLE-12-b.OP8 binary file of element force/stress OTM’s requested in Case Control
(note: only 1st 5 columns written here the sake of clarity)
OTM_ELFE
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16

1
2.09187572390564E-01
7.89453912890167E-01
1.51560714339846E+00
-1.43934432738336E+00
-1.84755627546901E-02
3.15199669918811E-02
6.26679968599842E-01
9.67284596743351E-03
-1.13315069892136E-01
-1.00896004659258E-02
-1.72540058669802E+00
-6.16614847670031E-02
2.27983320157212E-02
7.29336582157196E-04
-2.95361107284698E-01
-4.72042770150405E-03
OTM_STRE

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

1
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
-2.74867035744303E+00
-2.74867035744303E+00
-2.74867035744303E+00
-1.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
-2.74867035744303E+00
-2.74867035744303E+00
-2.74867035744303E+00
-1.00000000000000E+00
1.00000000000000E+10

NCOLS =

18
2
3.64063384390388E+00
-2.87503976462738E+00
-7.75207867487571E+00
4.48652751792572E+00
1.61117285562758E-01
-1.04108282913086E-01
1.90643492900070E+00
-5.33393540270422E-03
3.78970456518829E+00
2.99287680850590E+00
-6.06107677196644E+00
-4.71348398353008E+00
1.39311085669760E-01
1.08984399486375E-01
1.80807707871691E+00
5.33393540270377E-03
NCOLS =

18
2
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
7.58266712433821E+00
7.58266712433821E+00
7.58266712433821E+00
-1.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
7.58266712433821E+00
7.58266712433821E+00
7.58266712433821E+00
-1.00000000000000E+00
1.00000000000000E+10

NROWS =

16
3
-1.82031692195194E+00
1.43751988231369E+00
3.87603933743785E+00
-2.24326375896286E+00
-8.05586427813792E-02
5.20541414565432E-02
-9.53217464500349E-01
2.66696770135211E-03
-1.89485228259414E+00
-1.49643840425295E+00
3.03053838598322E+00
2.35674199176504E+00
-6.96555428348799E-02
-5.44921997431877E-02
-9.04038539358453E-01
-2.66696770135189E-03
NROWS =

18
3
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
-3.79133356216910E+00
-3.79133356216910E+00
-3.79133356216910E+00
-1.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
-3.79133356216910E+00
-3.79133356216910E+00
-3.79133356216910E+00
-1.00000000000000E+00
1.00000000000000E+10

260

FORM

2
4
-1.84227921264778E+00
1.92080844772306E+00
3.62690741509324E+00
-2.73874759882899E+00
-7.73459790410093E-02
6.58960735567147E-02
-1.19040949990613E-01
-5.34876839175438E-02
-1.26147862482940E+00
-4.03697533588189E+00
2.53928832803047E+00
6.82365970711492E+00
-5.37509617215390E-02
-1.53592573737906E-01
-1.95832712226347E+00
-1.12160973347287E-01
FORM

2
4
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
-1.07520478850513E+00
-1.07520478850513E+00
-1.07520478850513E+00
-1.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
-1.07520478850513E+00
-1.07520478850513E+00
-1.07520478850513E+00
-1.00000000000000E+00
1.00000000000000E+10

PREC

2
5
-9.14925412689932E-01
-1.26234542491864E-01
1.45527637571713E+00
2.35906653084923E-01
-3.35197151472623E-02
-5.12144990278700E-03
-1.14791218537626E-01
8.35971431688627E-04
-9.55864075040792E-01
-1.41398274167766E-02
1.96715396237338E+00
3.39064169416761E-02
-4.13377175157231E-02
-6.79476503928156E-04
3.00896480121837E-03
-3.69369770142806E-03
PREC

2
5
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
4.30045958649968E-01
4.30045958649968E-01
4.30045958649968E-01
-1.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
0.00000000000000E+00
4.30045958649968E-01
4.30045958649968E-01
4.30045958649968E-01
-1.00000000000000E+00
1.00000000000000E+10

.......
.......
.......
.......
.......
.......
.......
.......
.......
.......
.......
.......
.......
.......
.......
.......

.......
.......
.......
.......
.......
.......
.......
.......
.......
.......
.......
.......
.......
.......
.......
.......
.......
.......

CB-EXAMPLE-12-b.OT8 text file descriptor of rows in above binary file for element related OTM’s
This text file describes the rows of the elem related OTM matrices written to unformatted file: CB-EXAMPLE-12-b.OP8
---------------------------------------------------------------------------------------------The description for each of the matrices has the headers:
ROW
: row number in the individual OTM described
DESCRIPTION: what OTM is this
TYPE
: element type
EID
: element ID
Then, for the element nodal force OTM:
GRID
: grid number of the element that the OTM is for
COMP
: displacement component number (1,2,3 translations and 4,5,6 rotations)
and for element engineering force and element stress OTMs:
ITEM
: element force or stress item (axial force, torque, etc)
The number of rows for each OTM depends on the output requests, by the user, in Case Control
The number of cols for each OTM depends on the number of support DOFs (NDOFR) and the number of eigenvecors (NVEC)where:
NDOFR =
8
NVEC =
2
This text file has descriptions for the following element related OTMs from CB-EXAMPLE-12-b.OP8
Element engr force OTM (matrix OTM_ELFE) with 2*NDOFR + NVEC =
18 cols
Element stress
OTM (matrix OTM_STRE) with 2*NDOFR + NVEC =
18 cols
--------------------------------------------------------------------------------Explanation of rows of
16 row by
18 col matrix OTM_ELFE
ROW
------1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16

DESCRIPTION
-----------------------------Element engineering force
Element engineering force
Element engineering force
Element engineering force
Element engineering force
Element engineering force
Element engineering force
Element engineering force

TYPE
EID
-------- ------BAR
211
BAR
211
BAR
211
BAR
211
BAR
211
BAR
211
BAR
211
BAR
211

ITEM
-------------------M1a: Mom Plane1 EndA
M1b: Mom Plane2 EndA
M2a: Mom Plane1 EndB
M2b: Mom Plane2 EndB
V1 : Shear Plane1
V2 : Shear Plane2
FX : Axial force
T : Torque

Element
Element
Element
Element
Element
Element
Element
Element

BAR
BAR
BAR
BAR
BAR
BAR
BAR
BAR

M1a:
M1b:
M2a:
M2b:
V1 :
V2 :
FX :
T :

engineering
engineering
engineering
engineering
engineering
engineering
engineering
engineering

force
force
force
force
force
force
force
force

212
212
212
212
212
212
212
212

Mom Plane1 EndA
Mom Plane2 EndA
Mom Plane1 EndB
Mom Plane2 EndB
Shear Plane1
Shear Plane2
Axial force
Torque

261

--------------------------------------------------------------------------------Explanation of rows of
18 row by
18 col matrix OTM_STRE
ROW
------1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18

DESCRIPTION
-----------------------------Element stress
Element stress
Element stress
Element stress
Element stress
Element stress
Element stress
Element stress
Element stress
Element stress
Element stress
Element stress
Element stress
Element stress
Element stress
Element stress
Element stress
Element stress

TYPE
EID
-------- ------BAR
201
BAR
201
BAR
201
BAR
201
BAR
201
BAR
201
BAR
201
BAR
201
BAR
201
BAR
201
BAR
201
BAR
201
BAR
201
BAR
201
BAR
201
BAR
201
BAR
201
BAR
201

ITEM
-------------------SA1: Stress Pt1 EndA
SA2: Stress Pt2 EndA
SA3: Stress Pt3 EndA
SA4: Stress Pt4 EndA
Axial Stress
SA-Max
SA-Min
MS-Tension
Torsional Stress
SB1: Stress Pt1 EndB
SB2: Stress Pt2 EndB
SB3: Stress Pt3 EndB
SB4: Stress Pt4 EndB
Axial stress
SB-Max
SB-Min
MS-Compression
MS-Torsion

262

CB-EXAMPLE-12-b.OP9 binary file of displacement OTM’s requested in Case Control
(note: only 1st 5 columns written here the sake of clarity)
OTM_ACCE
1
2
3
4
5
6

1
2.19985250269592E-02
-2.02833087802606E-02
-1.68157865913898E-02
-3.36315731827796E-04
8.00614495648658E-03
5.25433423070610E-04
OTM_DISP

1
2
3
4
5
6
7
8
9
10
11
12

1
-1.41293911043985E-05
1.62214021120513E-05
8.24222187730972E-05
5.88370868696758E-07
-1.66743323917105E-06
5.12515138397389E-07
1.05104109813473E-05
-9.46594436701425E-06
-3.18288681491121E-06
-1.08618067423320E-07
-9.45071958677177E-07
2.10600905814006E-07

NCOLS =

10
2
0.00000000000000E+00
0.00000000000000E+00
-1.00000000000000E+00
-2.00000000000000E-02
0.00000000000000E+00
0.00000000000000E+00
NCOLS =

18
2
-7.60029025912968E-05
8.24359519633505E-05
3.12878663301563E-04
1.92529119983460E-06
2.22005501168008E-06
1.29205343624621E-07
-5.99087762260462E-05
6.30861677743807E-05
3.22417925611894E-04
3.64336233382231E-06
4.90427017653186E-07
3.21861205426993E-08

NROWS =

6
3
0.00000000000000E+00
0.00000000000000E+00
5.00000000000000E-01
1.00000000000000E-02
0.00000000000000E+00
0.00000000000000E+00
NROWS =

12
3
3.80014512956484E-05
-4.12179759816752E-05
-1.56439331650781E-04
-9.62645599917302E-07
-1.11002750584004E-06
-6.46026718123106E-08
2.99543881130231E-05
-3.15430838871904E-05
-1.61208962805947E-04
-1.82168116691115E-06
-2.45213508826593E-07
-1.60930602713497E-08

263

FORM

2
4
-5.00000000000004E-01
5.00000000000004E-01
5.00000000000005E-01
1.00000000000001E-02
0.00000000000000E+00
9.99999999999992E-03
FORM

2
4
1.29492635368416E-04
-1.30161832591346E-04
-2.40634384994669E-04
-2.07019101770705E-06
-1.14971054599053E-06
-1.07589130445167E-06
6.53233961326989E-05
-6.55217977160166E-05
-1.96081126486432E-04
-2.63986785628832E-06
-2.21449664764883E-07
-6.09852683088454E-07

PREC

2
5
1.09992625134795E-02
-1.01416543901302E-02
2.41592106704306E-01
-5.16815786591390E-03
-5.99692752175671E-03
2.62716711535305E-04
PREC

2
5
3.14571590643487E-06
-3.52963231517632E-06
-1.68993616070736E-05
1.88916538580397E-07
-8.88454144573320E-08
-9.61720937623318E-08
-1.57813540011406E-06
1.38681670255135E-06
-3.61627931263323E-05
-3.24126419085498E-08
1.36502293189118E-07
-3.82285587596693E-08

.......
.......
.......
.......
.......
.......

.......
.......
.......
.......
.......
.......
.......
.......
.......
.......
.......
.......

CB-EXAMPLE-12-b.OT9 text file descriptor of rows in above binary file for grid related OTM’s
This text file describes the rows of the grid related OTM matrices written to unformatted file: CB-EXAMPLE-12-b.OP9
---------------------------------------------------------------------------------------------The description for
ROW
:
DESCRIPTION:
GRID
:
COMP
:

each of the matrices has the headers:
row number in the individual OTM described
what OTM is this
grid number for this row of the OTM
displacement component number (1,2,3 translations and 4,5,6 rotations)

The number of rows for each OTM depends on the output requests, by the user, in Case Control
The number of cols for each OTM depends on the number of support DOFs (NDOFR) and the number of eigenvecors (NVEC)where:
NDOFR =
8
NVEC =
2
This text file has descriptions for the following grid relatad OTMs from CB-EXAMPLE-12-b.OP9
Acceleration OTM (matrix OTM_ACCE) with
NDOFR + NVEC =
10 cols
Displacement OTM (matrix OTM_DISP) with 2*NDOFR + NVEC =
18 cols
--------------------------------------------------------------------------------Explanation of rows of
6 row by
10 col matrix OTM_ACCE
ROW
------1
2
3
4
5
6

DESCRIPTION
-----------------------------Acceleration
Acceleration
Acceleration
Acceleration
Acceleration
Acceleration

GRID
------32
32
32
32
32
32

COMP
---1
2
3
4
5
6

--------------------------------------------------------------------------------Explanation of rows of
12 row by
18 col matrix OTM_DISP
ROW
------1
2
3
4
5
6
7
8
9
10
11
12

DESCRIPTION
-----------------------------Displacement
Displacement
Displacement
Displacement
Displacement
Displacement
Displacement
Displacement
Displacement
Displacement
Displacement
Displacement

GRID
------22
22
22
22
22
22

COMP
---1
2
3
4
5
6

32
32
32
32
32
32

1
2
3
4
5
6

264

11. Appendix E: Derivation of the RBE3 element constraint
equations

265

11.1 Introduction
The RBE3 element is used for distributing applied loads and mass from a reference point to other
points in the finite element model. The geometry and loads for a RBE3 are shown in Figure 1. Point
d in the figure is the RBE3 reference (or dependent) point and is the grid where loads will be applied
by the user. The RBE3 element will distribute these loads to other, independent, points i = 1,…,N, in
the model, where N is the total number of independent grid points defined on the RBE3 Bulk Data
entry. The RBE3 is not intended to add stiffness to the model as does a RBE2 element. As such, the
RBE3 reference point should not be a grid that is attached to other elements in the model – it should
be a stand alone grid only connected to other grids through the REB3 element definition. The
following describes the nomenclature used in this appendix in deriving the “constraint” equations used
in MYSTRAN for the RBE3 element.
Superscripts denote the location of a quantity:
“d” refers to the reference (or dependent) grid on the RBE3
“i” refers to the independent grids, the locations where the loads on point d will be distributed

X,Y,Z  coordinate system axes
ux , uy ,uz  displacements in the x, y, z directions
x , y , z  rotations about the x, y, z axes
Fx ,Fy ,Fz  forces in the x, y, z directions
Mx ,My ,Mz  moments about the x, y, z axes
dix , diy , diz  position of point i relative to the RBE3 reference point, d
For the sake of simplicity and clarity, the following derivation of the RBE3 equations is done for
conditions where the global coordinate systems of all grid points involved in the RBE3 are the same
and are rectangular. The code in the MYSTRAN program is written for general conditions where the
global system of all points may be different and non-rectangular.

266

Z, uz , z

Fzi

Point i (1 to N) is a typical point to
which loads will be transferred from
the reference point d via the RBE3

Fyi

Fxi

Point d is the RBE3 reference
point shown with the loads
applied. The loads will be
transferred to the points i (typical
point i shown above)
d
y

Mdx

Fyd

diz
Y, uy , y

Fxd

Fzd
dix

d
z

diy

X, ux , x
Fig 1: RBE3 geometry and loads

267

11.2 Equations for translational force components
In this section 3 equations will be developed that relate the forces applied at the RBE3 reference
point to those where the loads will be distributed (points i = 1,…,N).
The sum of the forces on the points i = 1,…,N must equal the forces on the reference point d. Thus:
N

 Fxi  Fxd

 Fyi  Fyd

i1

F

i1

i
z

 Fzd

11-1

The moments at reference point due to the forces at the points i are:
N

 (Fzi diy  Fyi diz )  Mdx

 (Fxi diz  Fzi dix )  Mdy

i1

 (F d
i
y

i1

i
x

 Fxi diy )  Mdz

11-2

Write the Fx , etc, as:

Fxi 

i d
Fx
WT

Fyi 

i d
Fy
WT

Fzi 

i d
Fz
WT

11-3

where i is the weighting factor (the WTi on the RBE3 Bulk Data entry) for the ith force and:
N

WT   i

11-4

i1

Equations 3 and 4 are sufficient for equations 1. Substitute equations 3 and 4 into 2 to get the
following 3 equations:

Fyd

Fzd
WT

d 

Fxd
WT

Fzd
d 

WT
i1

Fyd
WT

i1

i
i y

i
i z

 idix 
i1

Fxd
WT

d
i1

i
i z

d
i1

i
x

d
i1

i
y

 Mdx

11-5

 Mdy

11-6

 Mdz

11-7

Define:

dx 

1
WT

 idix

i1

dy 

1
WT

 idiy
i1

dz 

1
WT

d
i 1

i
i z

11-8

Using equation 8, equations 5-7 become:

Fzd d y Fyd dz  Mdx
268

11-9

Fxd d z Fzd dz  Mdy
Fyd d x Fxd dy  Mdz

11-10
11-11

The work done by the forces and moments at the reference point, d, is  d :

 d  Fxdudx  Fydudy  Fzdudz  Mdx dx  Mdy dy  Mdz dz

11-12

where u,  are the displacements and rotations of the reference point in the x, y, z directions.
Similarly, the work done by the forces on the points I = 1,…,N is:
N

N   (Fxi uix  Fyi uiy  Fzi uiz )

11-13

i1

The ux , ec, are the displacements in the x, y and z directions at point I. Substitute equation 3 into 12
and 9, 10 and 11 into 12 and equate the work done by the two systems of forces:

Fxdudx  Fydudy  Fzdudz  (Fzd d y Fyd dz )dx  (Fxd d z Fzd dz )dy  (Fyd d x Fxd dy )dz 
N

i

( W
i1

Fxduix 

i d i

Fy uy  i Fzduiz )
WT
WT

Rearrange:
N

(udx  d z dy  d y dz  
i1
N

(u  d z   d x   
d
y

d
x

d
z

i1
N

(udz  d y dx  d x dy  
i1

d
x ,

Since the F

d
y

d
z are

F and F

i i d
ux )Fx 
WT
i i d
uy )Fy 
WT

11-14

i i d
uz )Fz  0
WT

independent and, in general, not zero, equation 14 requires that:
N

(udx  d z dy  d y dz  
i1
N

(udy  d z dx  d x dz  
i1
N

(udz  d y dx  d x dy  
i1

i i
ux )  0
WT
i i
uy )  0
WT

11-15

i i
uz )  0
WT

Equation 15 represents 3 constraint equations for the RBE3. However, there are only 3 equations and
6 unknowns. This will be resolved in the next section where we develop 3 more equations based on
the moments at the reference point.

269

11.3 Equations for rotational moment components
In addition to the 3 equations developed in the last section there are also 3 equations that relate the
moments applied at the RBE3 reference point to those where the loads will be distributed (points i =
1,…,N).
Figure 2 shows how the forces in the y-z plane relate to the RBE3 reference point moment about the
x axis:

Z
Friyz ,Fφi yz are components of forces
Fxi , Fyi expressed in an r -  coord system.
i
d
u are displacements with (uy  uy ) the y
relative displ between points i and d, etc

Fzi , (uiz  udz )

Friyz ,uiryz
Fi yz ,uiyz
i

diy

Fyi , (uiy  udy )

diz
ryzi radius to point i from ref
point d in the y-z plane

M ,
d
x

Mdx , dx

d
x

iyz

are the moment and
rotation about the x axis.
iyz =angle in y-z plane to point i

Figure 2: Relationship of moments and forces in the y-z plane

270

Using the r- components of the forces, the moments about the x axis of the forces at the i = 1,..,N
points is:
N

F

r  Mdx

i
i
yz yz

i 1

11-16

As before, express the forces at the i points using the weighting factors, i :

i
yz

iryzi



 r
i 1

i i2
yz

Mdx

11-17

Note that if equation 17 were substituted into 16 it would be seen that 17 is a valid representation of
the tangential force components.
The work done by Mx must equal that due to all of the Fyz , or:
d

F

i
yz

uiyz  Mdx dx

11-18

where uyz is the tangential component of displacement at independent grid i in the y-z plane.
i

Substitute equation 17 into 18:

iryzi


i 1

Mdxuiyz  Mdx dx

 r
i 1

i i2
yz

or:
n

dx 

 r

i i
yz

i 1

uiyz

11-19

 r
i 1

i i2
yz

From Figure 2 it can be seen that:

uiyz  (uiz  udz )cos iyz  (uiy  udy )sin iyz
 (uiz  udz )

diy
ryzi

 (uiy  udy )

diz
ryzi

Therefore:

ryzi uiyz  (uiz  udz )diy  (uiy  udy )diz

11-20

Define:

eiyz 

1
WT

 r
i1

i i2
yz



271

1
WT

  (d
i1

i2
y

 diz )

11-21

Substitute equations 20 and 21 into 19

dx 

N
1 N i i

d
i



i (uiy  udy )diz 
(u
u
)d


z
z
y
i 
WT eyz  i1
i 1




1
WT eiyz



1
eiyz

N
N
N
 N i i d

i i
d
i i i







idizuiy 
(
d
)u
(
d
)u
d
u



y
z
z
y
y z
 
i 1
i 1
i 1
i 1



1
d
d
  dyuz  dzuy 
WT


 idiyuiz 
i 1

1
WT

11-22



d u 
i

i
z

i 1

i
y



In reference to Figures 3 and 4, define:

eizx 

1
WT

 iri zx 
2

i1

1
WT

  (d
i

i1

i2
z

 dix )

and
eixy 

11-23

1
WT

 r
i1

i i2
 xy



1
WT

  (d
i

i1

i2
x

 diy )

Then, y and z , by similar reasoning for x in equation 22 are:
d

dy 

N
1 N i i

d
i
(u
u
)d



i (uiz  udz )dix 

x
x
z
i 
WT ezx  i1
i 1


1
 i
ezx


1
d
d
  dzux  dxuz 
WT


1
d u 

WT
i 1
N

i
z

i
x


d u 

i 1

N

i
x

11-24

i
z

and

dz 

N
1 N i i

d
i



i (uix  uax )diy 
(u
u
)d

y
y
x
i 
WT exy  i1
i 1


1
 i
e xy


1
d
d
  dxuy  dyux 
WT


1
idixuiy 

WT
i 1
N


idiyuix 

i 1

N

11-25

Thus, for the rotations:

eyz dx  dzudy  dyudz 

1
WT

 idizuiy 

ezx dy  dzudx  dxudz 

1
WT

d u

exy dz  dyudx  dxudy 

1
WT

i 1

i
z

i
x



 idiyuix 
i 1

1
WT

d u

1
WT

d u

1
WT

i 1

i
y

i
x

i
z

d u
i 1

i
x

i
y

0

11-26

0

Equations 15 and 26 constitute 6 equations in the 6 unknown displacements and rotations at point a.
They are summarized in matrix notation below at the end of this appendix.
272

X
Frizx ,Fφi zx are components of forces
Fzi , Fxi expressed in an r -  coord system.
i
d
u are displacements with (uz  uz ) the z

relative displ between points i and d, etc

Fxi , (uix  udx )
Frizx ,uirzx
Fi zx ,uizx
i

diz

Fzi , (uiz  udz )

dix
rzxi radius to point i from ref
point d in the z-x plane

Mdy , dy

Mdy , dy
d

izx

are the moment and

rotation about the y axis.
izx =angle in z-x plane to point i

Figure 3: Relationship of moments and forces in the z-x plane

273

Y
Frixy ,Fφi xy are components of forces
Fxi , Fyi expressed in an r -  coord system.
i
d
u are displacements with (ux  ux ) the x

relative displ between points i and d, etc

Fyi , (uiy  udy )
Frixy ,uirxy
Fi xy ,uixy
i

dix

Fxi , (uix  udx )

diy
i
radius to point i from ref
rxy

point a in the x-y plane

M ,
d
z

Mdz , dz

d
z

izx

are the moment and
rotation about the z axis.
ixy =angle in x-y plane to point i

Figure 4: Relationship of moments and forces in the x-y plane

274

11.4 Summary of equations for the RBE3
In general, the equations for one RBE3 can be represented in matrix notation as:

RddUd  R dNUN  0

11-27

Rdd is the square, d x d, matrix of coefficients for the dependent (or reference) grid denoted as
REFGRID in field 4 of the RBE3 Bulk Data entry. It can have up to d = 6 dependent components
(REFC in field 5). For all 6 components, R dd and Ud are:

Rdd

 1

 0
 0

 

 0
d
 z
  d y

1
0

0
1

| d z
| dy


d z


dy

|
|


eyz


0

0
dx

d x |
0 |

0
0

ezx
0

0
d x

d y 

dx 
0 

 

0 
0 

exy 

 uax 
 a
 uy 
ua 
 z 
Ud    
 a 
 x
 ay 
 a
 z 

11-28

RdN is a rectangular, d x N, matrix of coefficients for the N independent grids on the RBE3

RdN 

1
Rd1 Rd2 . . . RdN 
WT

 U1 
U 
 2
 . 
UN   
 . 
 . 
 
UN 

11-29

uix 
 
Ui  uiy 
 i
uz 

11-30

A typical sub-matrix in Rai is of size d by 3 with Rai and Ui . For d = 6:

 i

 0
 0
1 
Rdi 
 
WT 
0

 idiz
 i i
  dy

0

0


idiz
0
idix

0 

0 
i 

 
idiy 

idix 

0 

A RBE3 is processed by solving equation 27 for the dependent degrees of freedom, Ud , in terms of
the independent degrees of freedom, UN .

275

Source Exif Data:

File Type                       : PDF
File Type Extension             : pdf
MIME Type                       : application/pdf
PDF Version                     : 1.6
Linearized                      : No
Author                          : Bill Case
Comments                        : 
Company                         : 
Create Date                     : 2011:11:07 16:53:39-05:00
MT Defer Field Update           : 1
MT Equation Number 2            : #S1-#E1
MT Equation Section             : 1
MT Win Eqns                     : 1
Modify Date                     : 2011:11:10 18:40:13-05:00
Source Modified                 : D:20111107215320
Subject                         : 
Has XFA                         : No
Tagged PDF                      : Yes
XMP Toolkit                     : Adobe XMP Core 4.2.1-c043 52.372728, 2009/01/18-15:08:04
Creator Tool                    : Acrobat PDFMaker 9.1 for Word
Metadata Date                   : 2011:11:10 18:40:13-05:00
Producer                        : Acrobat Distiller 9.4.6 (Windows)
Keywords                        : 
Format                          : application/pdf
Creator                         : Bill Case
Title                           : MYSTRAN
Description                     : 
Document ID                     : uuid:ce618df4-19fb-46fd-ae3b-6b8dc1905452
Instance ID                     : uuid:1d6543ef-4784-4311-a794-3914aa696a33
Page Layout                     : SinglePage
Page Mode                       : UseOutlines
Page Count                      : 283

EXIF Metadata provided by EXIF.tools

MYSTRAN Users Manual

Navigation menu

Versions of this User Manual:

Views

Navigation