Translating Nastran Data to Abaqus Files

The translator from Nastran to Abaqus converts finite element entities in a Nastran text input file into their equivalent in an Abaqus text input file. It can also convert matrix data (DMIGs) to their equivalent in an Abaqus binary SIM file.

This page discusses:

Converting Nastran Bulk Data in Text Files to Abaqus Input Files

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 1. The translator attempts to create a history section based on the contents of the case control data in the Nastran file.

Converting Nastran DMIG Matrix Data in Bulk Data Text Files to an Abaqus Binary SIM File

You can specify that the translator create a SIM file of matrix data in addition to a text input file. The matrix data can be translated to

  • a SIM file structured as if it were created from a MATRIX GENERATE step in an Abaqus input file or
  • a SIM file equivalent to that resulting from an Abaqus analysis with a SUBSTRUCTURE GENERATE step.

Converting Nastran DMIG Matrix Data in Output2 Binary Files to an Abaqus Binary SIM File

The Nastran matrix data can be in one or more binary Output2 files. The DMIG matrix data are assumed to be written to an Output2 file using a command as follows:

ASSIGN OUTPUT2='jobname_matrixdata.op2',UNIT=30
…
EXTSEOUT(STIFFNESS,
         MASS,
         DAMPING,
         K4DAMP,
         LOADS,
         ASMBULK,
         EXTBULK,
         EXTID=10,
         DMIGOP2=30)

The nodal coordinate data may be in a second Output2 file, created with a command as follows:

ASSIGN OUTPUT2='jobname.op2',UNIT=12
…
DISP(PLOT) = ALL
…
PARAM,POST,-2

These Output2 files are referenced by the op2file1 and op2file2 options. The use of op2file2 is optional. Using the file names from the example above, you specify the command line options as follows:

op2file1=jobname_matrixdata.op2 op2file2=jobname.op2

The op2target option determines the type of matrix data to create. The matrix data can be translated to

  • a partial Abaqus input file with a MATRIX INPUT representation of the matrix data,
  • a SIM file structured as if it were created from a MATRIX GENERATE step in an Abaqus input file, or
  • a SIM file equivalent to that resulting from an Abaqus analysis with a SUBSTRUCTURE GENERATE step.

Summary of Nastran Entities Translated

Table 1. Executive control data.
Nastran Statement Abaqus 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 2. Case control data.
Nastran Command Comment
SPC Selects SPC sets alone or in combinations
LOAD Selects individual loads and load combinations
METHOD Selects EIGRL, EIGR, or EIGB from bulk data for eigenfrequency extraction and eigenvalue buckling prediction procedures
SUBCASE Delimiter for steps or load cases; optional if there is only one step
TITLE Echoed as comment at top of input file and for each step
SUBTITLE Echoed as comment for the step to which it applies
LABEL Used as text following the STEP option
DLOAD Selects dynamic loads from bulk data
LOADSET
FREQUENCY Selects forcing frequencies from bulk data
MPC Selects MPCADD and MPC from bulk data if referenced in the first SUBCASE
SUPORT1 Selects SUPORT1 from bulk data
TSTEP Selects TSTEP from bulk data
K2GG Selects DMIG from bulk data using the matrix name from the first SUBCASE
K2PP
M2GG
M2PP
B2GG
B2PP
K42GG
TEMPERATURE Selects nodal temperatures from bulk data
SET Selects nodal quantities for output
DISPLACEMENT
VELOCITY
ACCELERATION
SPCFORCES
PRESSURE
Table 3. Bulk data.
Nastran Data Entry Comment
PARAM Ignored 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
CDAMP1 DASHPOT1/DASHPOT2 and DASHPOT
CDAMP2
PDAMP
PDAMPT
CELAS1 SPRING1/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
CBUSH CONN3D2 and CONNECTOR SECTION
PBUSH
PBUSHT
CWELD FASTENER and FASTENER PROPERTY
PWELD
CONM1 MASS and/or ROTARY INERTIA and/or UEL
CONM2 MASS and/or ROTARY INERTIA
CHEXA C3D8I/C3D20R/C3D6/C3D15/C3D4/C3D10 and SOLID SECTION
CPENTA
CTETRA
PSOLID
PLSOLID
CQUAD4 S4/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, or SHEAR4 and SHELL GENERAL SECTION
PSHEAR
CBAR B31 and BEAM SECTION or BEAM GENERAL SECTION
CBEAM
PBAR
PBARL
PBEAM
PBEAML
CROD T3D2 and SOLID SECTION
CONROD
PROD
CGAP GAPUNI and GAP
PGAP
RBAR COUPLING or MPC, type BEAM
MAT1 ELASTIC, TYPE=ISO; EXPANSION, TYPE=ISO; DENSITY; and DAMPING (G is used only for BEAM GENERAL SECTION)
MAT2 When 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; DENSITY and DAMPING
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
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(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
SPCADD Used to combine SPC/SPC1/SPCD data into a new set
SPC BOUNDARY
SPC1
SPCD
LOAD Used to combine FORCE, MOMENT, etc. data into a new set
FORCE CLOAD
FORCE1
FORCE2
MOMENT
MOMENT1
MOMENT2
PLOAD DLOAD
PLOAD1
PLOAD2
PLOAD4
RFORCE
DLOAD Dynamic 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
TSTEP Time step size for dynamic and modal dynamic procedures
EIGB BUCKLE
EIGR FREQUENCY
EIGRL
EIGC COMPLEX FREQUENCY
TABDMP1 MODAL DAMPING
FREQ Forcing frequencies for steady-state dynamic procedures
FREQ1
FREQ2
FREQ3
FREQ4
FREQ5
MPCADD EQUATION
MPC
SUPORT INERTIA RELIEF and BOUNDARY
SUPORT1
DMIG MATRIX INPUT and MATRIX ASSEMBLE
GENEL USER ELEMENT, LINEAR and MATRIX, TYPE=STIFFNESS
PLOTEL T3D2 (Ignored unless the command line option plotel=ON.)

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 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 cshear { UEL SHEAR4 } plotel { OFF ON } cdh_weld { OFF RIGID COMPLIANT } dmig2sim { GENERIC SUBSTRUCTURE } op2file1 op2-filename-1 op2file2 op2-filename-2 op2target { INPUT GENERIC SUBSTRUCTURE }

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, I1, I2, 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

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:

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.

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

fromnastran_surface_based_coupling={OFF | ON}
beam_offset_coupling

If beam_offset_coupling=ON, beam element offsets are translated by creating new nodes at the offset locations, changing the beam connectivity to the new nodes, and rigidly coupling the new and original nodes.

If beam_offset_coupling=OFF, beam element offsets are translated to the CENTROID and SHEAR CENTER options, which are suboptions of the BEAM GENERAL SECTION option.

The setting for this parameter is ignored if the beam element references a PBARL or PBEAML property or if the beam offset has a significant component in the direction of the beam axis. In these situations the beam offsets are always translated as if beam_offset_coupling=ON.

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

fromnastran_beam_offset_coupling={OFF | ON}
beam_orientation_vector

If beam_orientation_vector=OFF, beam cross-section orientations are translated by creating new nodes at the tips of vectors defining the first principal direction of the cross-section and changing the beam connectivity to the new nodes.

If beam_orientation_vector=ON, beam cross-sections are translated by defining vectors on the BEAM SECTION and BEAM GENERAL SECTION options.

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

fromnastran_beam_orientation_vector={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 S4R. 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
cshear

By default, CSHEAR elements are translated to user elements, as described in Table 3. If cshear=SHEAR4, CSHEAR elements are translated to SHEAR4 elements.

plotel

By default, PLOTEL elements are not translated. If plotel=ON, PLOTEL elements are translated to T3D2 truss elements in an element set named PLOTEL_TRUSSES. The cross-sectional area of the trusses is 1.0 × 10−20, and the material has a Young's modulus, E, equal to 1.0.

cdh_weld

By default, CHEXA elements with RBE3 elements at all eight corner nodes are translated to the type of 8-node element specified in the chexa parameter. If cdh_weld=RIGID, CHEXA elements with RBE3 elements at all eight corner nodes are translated to rigid fasteners in Abaqus. If cdh_weld=COMPLIANT, CHEXA elements with RBE3 elements at all eight corner nodes are translated to compliant fasteners in Abaqus.

dmig2sim

This option is used to write DMIG matrix data to a binary SIM file for further processing by Abaqus.

If dmig2sim=GENERIC, a SIM file with a generic matrix system equivalent to that produced by a MATRIX GENERATE step is created.

If dmig2sim=SUBSTRUCTURE, a SIM file with a substructure matrix system equivalent to that produced by a SUBSTRUCTURE GENERATE step is created.

op2file1
This option is used only in a workflow that reads DMIG matrix data in an Output2 file. It specifies the name of an Output2 file containing DMIG matrix data. The complete file name with the extension must be given.
op2file2
This option is used to give the name of a second Output2 file containing nodal coordinate data associated with DMIG entries. If the op2file1 option is present, specifying op2file2 is optional. If specified, the complete file name with the extension must be given.
op2target

This option controls the translation behavior for the DMIG matrix data in an Output2 file.

If op2target=INPUT, a partial Abaqus input file containing a MATRIX INPUT option is created.

If op2target=GENERIC, a SIM file with a generic matrix system equivalent to that produced by a MATRIX GENERATE step is created.

If op2target=SUBSTRUCTURE, a SIM file with a substructure matrix system equivalent to that produced by a SUBSTRUCTURE GENERATE step is created.