|
Converting an Abaqus Input File to a Nastran Bulk Data Text File
The Abaqus input data must be in a file with the extension .inp. The
execution procedure translates selected keywords and creates a Nastran bulk data
file with the extension .bdf.
Converting Matrix Data in an Abaqus SIM File to a Nastran Bulk Data Text File
The Abaqus input data must be in a file with the extension .sim and
must have been created with either a matrix generation or a substructure generation
procedure. When you use the sim2dmig option,
the execution procedure translates the matrix data to Nastran
DMIG coefficients and creates a Nastran bulk
data file with the extension .bdf.
Summary of Abaqus Keywords Translated
In the
ELEMENT usages listed below, an italicized
x indicates that all
Abaqus
elements beginning with the preceding label will be mapped to the Nastran
entity shown. For example, the statement
ELEMENT, C3D4x indicates that the selected
Abaqus-to-Nastran
translation applies to the
Abaqus
elements C3D4, C3D4H, and C3D4T.
Table 1. Abaqus
keyword–to–Nastran mapping.
| Abaqus
Keyword
|
Nastran Complement
|
| BEAM GENERAL SECTION |
PBEAM or
PBEAML |
| BEAM SECTION |
PBEAML |
| BOUNDARY
|
SPC
|
| CLOAD
|
FORCE
|
| COUPLING, DISTRIBUTING
|
RBE3
|
| COUPLING, KINEMATIC
|
RBE2
|
| ELEMENT, B31
|
CBEAM
|
| ELEMENT, B33
|
CBEAM
|
| ELEMENT, C3D4x
|
CTETRA
|
| ELEMENT,
C3D5 |
CPYRAM |
| ELEMENT, C3D10x
|
CTETRA
|
| ELEMENT, C3D6x
|
CPENTA
|
| ELEMENT, C3D15x
|
CPENTA
|
| ELEMENT, C3D8x
|
CHEXA
|
| ELEMENT, C3D20x
|
CHEXA
|
| ELEMENT, MASS
|
CONM2
|
| ELEMENT, ROTARYI
|
CONM2
|
| ELEMENT, S3x
|
CTRIA3
|
| ELEMENT, S4x
|
CQUAD4
|
| ELEMENT, S8x
|
CQUAD8
|
| ELEMENT,
SHEAR4 |
CSHEAR |
| ELEMENT, SPRING1 or SPRING2
|
CELAS
|
| ELEMENT, SPRINGA
|
CROD
|
| ELEMENT, STRI65
|
CTRIA6
|
| ELEMENT, T3D2
|
CROD
|
| FREQUENCY
|
SOL 103
|
| HEADING
|
TITLE
|
| MATERIAL, DENSITY
|
MAT1
|
| MATERIAL, ELASTIC, TYPE=ISO
|
MAT1
|
| MATERIAL, ELASTIC, TYPE=LAMINA
|
MAT8
|
| MATERIAL, EXPANSION, TYPE=ISO
|
MAT1
|
| MATERIAL, EXPANSION, TYPE=ORTHO
|
MAT8
|
| MATRIX INPUT |
DMIG |
| NODE
|
GRID
|
| ORIENTATION, DEFINITION=COORDINATES
|
CORD2R,
CORD2C, or
CORD2S
|
| SHELL GENERAL SECTION (Non-composite)
|
PSHELL
|
| SHELL SECTION (Non-composite)
|
| SHELL SECTION (Composite)
|
PCOMP
|
| SHELL GENERAL SECTION (Composite)
|
| SOLID SECTION
|
PSOLID
|
| SOLID SECTION (Trusses)
|
PROD
|
| STATIC
|
SOL 101
|
| SYSTEM
|
CORD2R,
CORD2C, or
CORD2S
|
| TRANSFORM
|
Command Summary
abaqus
tonastranjobjob-name
inputinput-file
sim2dmig
complex{YESNO}
Command Line Options
- job
-
This option is used to specify the name of the Nastran bulk data file to be
output by the translator. It is also the default name of the
Abaqus
file. Diagnostics created by the translator are written to a file named
job-name.log.
- input
-
This option is used to specify the name of the file containing the
Abaqus
data if it is different from job-name.
- sim2dmig
-
This option is used to translate matrix data in an
Abaqus
.sim file into the Nastran bulk data file
(.bdf) format.
- complex
-
This option is used to determine how structural damping terms are
represented. If
complex=YES
(default), structural damping terms are written as the imaginary part of the
stiffness matrix; if
complex=NO,
structural damping terms are written as a separate real matrix.
|