Translating Abaqus files to Nastran bulk data files

The translator from Abaqus to Nastran converts certain entities in an Abaqus file into equivalent entities in Nastran. Only “flat” Abaqus files can be translated; i.e., the Abaqus file cannot contain parts and assemblies.

The following topics are discussed:

Using the translator
Summary of Abaqus keywords translated
Command summary
Command line options

Using the translator

The Abaqus input data must be in a file with the extension .inp or .sim. If you specify an .inp file, the execution procedure translates selected keywords and creates a Nastran bulk data file with the extension .bdf. If you use the substructure option and specify a substructure .sim file, the execution procedure translates the substructure 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, SECTION=GENERAL	PBAR
BOUNDARY	SPC
CLOAD	FORCE
COUPLING, DISTRIBUTING	RBE3
COUPLING, KINEMATIC	RBE2
ELEMENT, B31	CBAR (for BEAM GENERAL SECTION, SECTION=GENERAL)
ELEMENT, B33	CBAR (for BEAM GENERAL SECTION, SECTION=GENERAL)
ELEMENT, C3D4x	CTETRA
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, 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
NODE	GRID
ORIENTATION, DEFINITION=COORDINATES	CORD2R, CORD2C, or CORD2S
SHELL GENERAL SECTION (Non-composite)	PSHELL
SHELL SECTION (Non-composite)	PSHELL
SHELL SECTION (Composite)	PCOMP
SHELL GENERAL SECTION (Composite)	PCOMP
SOLID SECTION	PSOLID
SOLID SECTION (Trusses)	PROD
STATIC	SOL 101
SYSTEM	CORD2R, CORD2C, or CORD2S
TRANSFORM	CORD2R, CORD2C, or CORD2S

Command summary

abaqus tonastranjobjob-nameinputinput-filesubstructurecomplex{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.
substructure: This option is used to translate a substructure within an Abaqus .sim file into 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.