3.2.20 Execution procedure for translating NASTRAN bulk data files to ABAQUS input files

Products: ABAQUS/Standard  ABAQUS/Explicit  

Reference

Overview

The translator from NASTRAN to ABAQUS converts certain entities in a NASTRAN input file into their equivalent in ABAQUS.

Using the translator

The NASTRAN data must be in a file with the extension .bdf. The NASTRAN data entries that are translated are listed in the tables below. Other valid NASTRAN data are skipped over and noted in the log file.

The translator is designed to translate a complete NASTRAN input file. If only bulk data are present, the first two lines in the file should be the terminators for the executive control and case control sections, namely:

CEND 
BEGIN BULK
For normal termination, end the NASTRAN input data with the line
ENDDATA
NASTRAN solution sequences are translated to the ABAQUS procedures listed in Table 3.2.20–1. The translator attempts to create a history section based on the contents of the case control data in the NASTRAN file.

The INCLUDE command is not supported.

Summary of NASTRAN entities translated

Table 3.2.20–1 Executive control data.

NASTRAN StatementABAQUS Equivalent
SOL 
1 (STATICS1)*STATIC
24 (STATICS)
101 (SESTATIC) 
106 (NLSTATIC)
3 (MODES)*FREQUENCY
25 (OLDMODES)
103 (SEMODES)
5 (BUCKLING)*BUCKLE
105 (SEBUCKL)
26 (DFREQ)*STEADY STATE DYNAMICS, DIRECT
108 (SEDFREQ)
27 (DTRAN)*DYNAMIC
109 (SEDTRAN)
107(SEDCEIG)*COMPLEX FREQUENCY
110 (SEMCEIG)
30 (DFREQ)*FREQUENCY and *STEADY STATE DYNAMICS
111 (SEMFREQ)
31 (MTRAN)*FREQUENCY and *MODAL DYNAMIC
112 (SEMTRAN)

Table 3.2.20–2 Case control data.

NASTRAN CommandComment
SPCSelects SPC sets alone or in combinations
LOADSelects individual loads and load combinations
METHODSelects EIGRL, EIGR, or EIGB from bulk data for eigenfrequency extraction and eigenvalue buckling prediction procedures
SUBCASEDelimiter for steps or load cases; optional if there is only one step
TITLEEchoed as comment at top of input file and for each step
SUBTITLEEchoed as comment for the step to which it applies
LABELUsed as text following the *STEP option
DLOADSelects dynamic loads from bulk data
LOADSET
FREQUENCYSelects forcing frequencies from bulk data
MPCSelects MPCADD and MPC from bulk data if referenced in the first SUBCASE
SUPORT1Selects SUPORT1 from bulk data
TSTEPSelects TSTEP from bulk data
K2GGSelects DMIG from bulk data using the matrix name from the first SUBCASE
K2PP
M2GG
M2PP
TEMPERATURESelects nodal temperatures from bulk data

Table 3.2.20–3 Bulk data.

NASTRAN Data EntryComment
PARAMIgnored except for:
1. WTMASS, which can be used to modify density, mass, and rotary inertia values if the wtmass_fixup command line parameter is used
2. INREL, which if equal to –1 or –2 will create inertia relief loads
CDAMP1DASHPOT1/DASHPOT2 and *DASHPOT
CDAMP2
PDAMP
CELAS1SPRING1/SPRING2 and *SPRING
CELAS2
PELAS
CBUSHCONN3D2 and *CONNECTOR SECTION
PBUSH
PBUSHT
CONM1MASS and/or ROTARY INERTIA and/or UEL
CONM2MASS and/or ROTARY INERTIA
CHEXAC3D8I/C3D20R/C3D6/C3D15/C3D4/C3D10 and *SOLID SECTION
CPENTA
CTETRA
PSOLID
CQUAD4S4/S3R/S8R/STRI65, and *SHELL SECTION, *SHELL GENERAL SECTION, or *MEMBRANE SECTION.
CTRIA3
CQUAD8
CTRIA6
CQUADR
CTRIAR
PSHELL
PCOMP
PCOMPG
CSHEARM3D4 and *MEMBRANE SECTION; T3D2 and *SOLID SECTION
PSHEAR
CBARB31 and *BEAM SECTION or *BEAM GENERAL SECTION
CBEAM
PBAR
PBARL
PBEAM
PBEAML
CRODT3D2 and *SOLID SECTION
CONROD
PROD
CGAPGAPUNI and *GAP
PGAP
RBAR*COUPLING or *MPC, TYPE=BEAM
MAT1*ELASTIC, TYPE=ISO; *EXPANSION, TYPE=ISO; and *DENSITY (G is used only for *BEAM GENERAL SECTION)
MAT2When used alone in a PSHELL, MAT2 is translated to *ELASTIC, TYPE=LAMINA or *ELASTIC, TYPE=ANISOTROPIC. When used in combination with other materials, the coefficients relating midsurface strains and curvatures to section forces and moments are computed and entered following the *SHELL GENERAL SECTION option.
MAT8*ELASTIC, TYPE=LAMINA; *EXPANSION, TYPE=ORTHO; and *DENSITY
MAT9*ELASTIC, TYPE=ANISOTROPIC unless the data are found to be orthotropic, in which case the data are analyzed to create *ELASTIC, TYPE=ENGINEERING CONSTANTS. Also *DENSITY; and *EXPANSION, TYPE=ANISO or ORTHO.
NSM*NONSTRUCTURAL MASS
NSM1
NSML
NSML1
NSMADD
GRID*NODE and *SYSTEM
CORD1R*SYSTEM for nodes; *TRANSFORM if referred to on GRID; *ORIENTATION for some elements
CORD1C
CORD1S
CORD2R
CORD2C
CORD2S
RBE2*COUPLING and *KINEMATIC; or *KINEMATIC COUPLING
RBE3*COUPLING and *DISTRIBUTING; or DCOUP3D and *DISTRIBUTING COUPLING
SPCADDUsed to combine SPC/SPC1/SPCD data into a new set
SPC*BOUNDARY
SPC1
SPCD
LOADUsed to combine FORCE, MOMENT, etc. data into a new set
FORCE*CLOAD
FORCE1
FORCE2
MOMENT
MOMENT1
MOMENT2
PLOAD*DLOAD
PLOAD1
PLOAD2
PLOAD4
RFORCE
DLOADDynamic loads as functions of time or frequency
DAREA
LSEQ
RLOAD1
RLOAD2
TLOAD1
TABLED1
TABLED2
TABLED4
DELAY
DPHASE
TEMP*INITIAL CONDITIONS, TYPE=TEMPERATURE and *TEMPERATURE
TEMPD
TSTEPTime step size for dynamic and modal dynamic procedures
EIGB*BUCKLE
EIGR*FREQUENCY
EIGRL
EIGC*COMPLEX FREQUENCY
TABDMP1*MODAL DAMPING
FREQForcing frequencies for steady-state dynamic procedures
FREQ1
FREQ2
MPCADD*EQUATION
MPC
SUPORT*INERTIA RELIEF and *BOUNDARY
SUPORT1
DMIG*MATRIX INPUT and *MATRIX ASSEMBLE
GENEL *USER ELEMENT, LINEAR and *MATRIX, TYPE=STIFFNESS

Command summary

abaqus fromnastran
job=job-name
 
[input=input-file]
[wtmass_fixup={OFF |  ON}]
[loadcases={OFF |  ON}]
[pbar_zero_reset=[small_real_number]]
[distribution={OFF |  ON}]
[cbar=2_node_beam_element]
[cquad4=4_node_shell_element]
[chexa=8_node_brick_element]
[ctetra=10_node_tetrahedron_element]

Command line options

job

This option is used to specify the name of the ABAQUS input file to be output by the translator. It is also the default name of the file containing the NASTRAN data. Diagnostics created by the translator will be written to a file named job-name.log.

input

This option is used to specify the name of the file containing the NASTRAN data if it is different from job-name.

wtmass_fixup

If wtmass_fixup=ON, the value on the NASTRAN data line PARAM, WTMASS, value is used as a multiplier for all density, mass, and rotary inertia values created in the ABAQUS input file.

This option can be defined in the ABAQUS environment file as follows:

fromnastran_wtmass_fixup={OFF | ON}

loadcases

By default, each SUBCASE is translated to a *STEP option in ABAQUS. If loadcases=ON, this behavior is altered for linear static analyses: each SUBCASE is translated to a *LOAD CASE option, and all such *LOAD CASE options are grouped in a single *STEP option.

This option can be defined in the ABAQUS environment file as follows:

fromnastran_loadcases={OFF | ON}

pbar_zero_reset

NASTRAN allows beams to have zero values for cross-sectional area or moments of inertia; ABAQUS does not. Set this option equal to a small real number to reset any zero values for A, , , or J to the specified small real number. If this option is omitted or present without a value, the default value of 1.0 10–20 is used in place of the zeros. To retain the zeros in the translated ABAQUS input file, set pbar_zero_reset=0.

This option can be defined in the ABAQUS environment file as follows:

fromnastran_pbar_zero_reset=small_real_number

distribution

NASTRAN shell elements may have their orientations and offsets defined on the element connectivity. By default, all elements that reference a single PSHELL translate to a single *SHELL SECTION or *SHELL GENERAL SECTION in ABAQUS and the variation in their properties will be defined using the *ELEMENT PROPERTIES and *DISTRIBUTION keywords. If distribution=OFF, a separate *SHELL SECTION or *SHELL GENERAL SECTION is created for each element set that has a unique combination of orientation, offset, and/or thickness.

This option can be defined in the ABAQUS environment file as follows:

fromnastran_distribution={OFF | ON}

surface_based_coupling

Certain NASTRAN rigid elements have more than one equivalent in ABAQUS. If surface_based_coupling=ON, RBE2 and RBE3 elements translate to *COUPLING with the appropriate parameters. Otherwise, RBE2 elements translate to *KINEMATIC COUPLING and RBE3 elements translate to *DISTRIBUTING COUPLING. This translation behavior also applies to “implied” RBE2-type rigid elements used for offsets on CBAR, CBEAM, and CONM2 elements.

For input files created with surface_based_coupling=ON, the translated elements can be visualized and manipulated in ABAQUS/CAE. However, large numbers of these elements may cause slower performance.

This option can be defined in the ABAQUS environment file as follows:

fromnastran_surface_based_coupling={OFF | ON}

cbar

This option is used to define the 2-node beam that is created from CBAR and CBEAM elements. The default is B31.

This option can be defined in the ABAQUS environment file as follows:

fromnastran_cbar=2_node_beam_element

cquad4

This option is used to define the 4-node shell that is created from CQUAD4 elements. The default is S4. If a reduced-integration element is chosen, the enhanced hourglass formulation is applied automatically.

This option can be defined in the ABAQUS environment file as follows:

fromnastran_cquad4=4_node_shell_element

chexa

This option is used to define the 8-node brick that is created from CHEXA elements. The default is C3D8I. If a reduced-integration element is chosen, the enhanced hourglass formulation is applied automatically.

This option can be defined in the ABAQUS environment file as follows:

fromnastran_chexa=8_node_brick_element

ctetra

This option is used to define the 10-node tetrahedron that is created from CTETRA elements. The default is C3D10.

This option can be defined in the ABAQUS environment file as follows:

fromnastran_ctetra=10_node_tetrahedron_element