# 3.2.30 TRANSLATING NASTRAN BULK DATA FILES TO Abaqus INPUT FILES Products: Abaqus/Standard Abaqus/Explicit # References • “Execution procedure for Abaqus: overview,” Section 3.1.1 • “Translating Abaqus files to Nastran bulk data files,” Section 3.2.31 • “Importing a model from a Nastran input file,” Section 10.5.4 of the Abaqus/CAE User’s Guide # 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, .dat, .nas, .nastran, .blk, or .bulk. 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 3.2.30–1. The translator attempts to create a history section based on the contents of the case control data in the Nastran file. # Summary of Nastran entities translated Table 3.2.30–1 Executive control data.
Nastran StatementAbaqus Equivalent
SOL
Nastran StatementAbaqus Equivalent
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 3.2.30–2 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
Nastran CommandComment
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
DLOADLOADSETSelects dynamic loads from bulk data
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
K2GGK2PPM2GGM2PPB2GGB2PPK42GGSelects DMIG from bulk data using the matrix name from the first SUBCASE
TEMPERATURESelects nodal temperatures from bulk data
SETDISPLACEMENTVELOCITYACCELERATIONSPCFORCESPRESSURESelects nodal quantities for output
Table 3.2.30–3 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 used2. INREL, which if equal to -1 or -2 will create inertia relief loads3. G, which is translated to *GLOBAL DAMPING, STRUCTURAL, FIELD=MECHANICAL4. GFL, which is translated to *GLOBAL DAMPING, STRUCTURAL, FIELD=ACOUSTIC
CDAMP1DASHPOT1/DASHPOT2 and *DASHPOT
CDAMP2
PDAMP
PDAMPT
CELAS1SPRING1/SPRING2 and *SPRING(CELAS2 at SPOINTs are translated to *MATRIX INPUT, stiffness, and/or structural damping terms.)
CELAS2
PELAS
PELAST
CMASS2*MATRIX INPUT mass terms
CBUSHCONN3D2 and *CONNECTOR SECTION
PBUSH
PBUSHT
CWELD*FASTENER and *FASTENER PROPERTY
PWELD
CONM1MASS and/or ROTARY INERTIA and/or UEL
CONM2MASS and/or ROTARY INERTIA
Nastran Data EntryComment
CHEXAC3D8I/C3D20R/C3D6/C3D15/C3D4/C3D10 and *SOLID SECTION
CPENTA
CTETRA
PSOLID
PLSOLID
CQUAD4S4/S3R/S8R/STRI65, and *SHELL SECTION, *SHELL GENERAL SECTION, or *MEMBRANE SECTION.
CTRIA3
CQUAD8
CTRIA6
CQUADR
CTRIAR
PSHELL
PCOMP
PCOMPG
CSHEAR*USER ELEMENT, LINEAR and *MATRIX, TYPE=STIFFNESS and TYPE=MASS
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
Nastran Data EntryComment
MAT1*ELASTIC, TYPE=ISO; *EXPANSION, TYPE=ISO; *DENSITY; and *DAMPING (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; *DENSITY; and *DAMPING
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; *EXPANSION, TYPE=ANISO or ORTHO; and *DAMPING.
MAT10*ACOUSTIC MEDIUM and *DENSITY
ACMODL*TIE between a *SURFACE, TYPE=ELEMENT defining the exterior surfaces of all acoustic solid elements and a *SURFACE, TYPE=NODE defined by the SET1 referenced by the SSID.
NSM*NONSTRUCTURAL MASS
NSM1
NSML
NSML1
NSMADD
GRID*NODE and *SYSTEM
Nastran Data EntryComment
CORD1RCORD1CCORD1SCORD2RCORD2CCORD2S*SYSTEM for nodes; *TRANSFORM if referred to on GRID; *ORIENTATION for some elements
RBE2*COUPLING and *KINEMATIC; or *KINEMATIC COUPLING(If the RBE2 has only two nodes and neither node has rotational stiffness, the RBE2 is translated to *MPC, type LINK)
RBE3*COUPLING and *DISTRIBUTING; or DCOUP3D and *DISTRIBUTING COUPLING
SPCADDUsed to combine SPC/SPC1/SPCD data into a new set
SPCSPC1SPCD*BOUNDARY
LOADUsed to combine FORCE, MOMENT, etc. data into a new set
FORCEFORCE1FORCE2MOMENTMOMENT1MOMENT2*CLOAD
PLOADPLOAD1PLOAD2PLOAD4RFORCE*DLOAD
Nastran Data EntryComment
DLOADDynamic loads as functions of time or frequency
DAREALSEQ
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
EIGREIGRL*FREQUENCY
EIGC*COMPLEX FREQUENCY
TABDMP1*MODAL DAMPING
FREQForcing frequencies for steady-state dynamic procedures
FREQ1
FREQ2
FREQ3
FREQ4
FREQ5
MPCADD*EQUATION
MPC
Nastran Data EntryComment
SUPORT*INERTIA RELIEF and *BOUNDARY
SUPORT1
DMIG*MATRIX INPUT and *MATRIX ASSEMBLE
GENEL*USER ELEMENT, LINEAR and *MATRIX, TYPE=STIFFNESS
PLOTELT3D2 (Ignored unless the command line option plotel=ON.)
Command summary ```ini abaqus fromnastran job=job-name [input=input-file] [wtmass_fixup={OFF | ON}] [loadcases={OFF | ON}] [pbar_zero_reset=[small-real-number]] [distribution={OFF | preservePID | ON}] [surface_based_coupling={OFF | ON}] [beam_offset_coupling={OFF | ON}] [beam_orientation_vector={OFF | ON}] [cbar=2-node-beam-element] [cquad4=4-node-shell-element] [chexa=8-node-brick-element] [ctetra=10-node-tetrahedron-element] [plotel={OFF | ON}] [cdh_weld={OFF | RIGID | COMPLIANT}] ``` 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: ```python 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: ```python 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, $I _ { 1 } , I _ { 2 }$ , or J to the specified small real number. If this option is omitted or present without a value, the default value of $1 . 0 \times 1 0 ^ { - 2 0 }$ 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: ```python fromnastran_pbar_zero_reset=small-real-number ``` # distribution This option determines how shell and membrane sections in Nastran data are translated to Abaqus. If distribution=OFF, a separate section is created for each combination of orientation, material offset, and/or thickness. If distribution=preservePID or ON, element orientations and offsets are written using the \*DISTRIBUTION option. If distribution=preservePID, an Abaqus section is created corresponding to each PSHELL or PCOMP property ID. If distribution=ON, a single Abaqus section is created for all homogeneous elements referencing the same material. This option can be defined in the Abaqus environment file as follows: ```txt fromnastran_distribution={OFF | preservePID | 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: ```python fromnastran_surface_based_coupling={OFF | ON} ```