김경종
14 KiB
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 Statement | Abaqus Equivalent |
| SOL |
| Nastran Statement | Abaqus 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 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 |
| Nastran Command | Comment |
| 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 |
| DLOADLOADSET | Selects dynamic loads from bulk data |
| 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 |
| K2GGK2PPM2GGM2PPB2GGB2PPK42GG | Selects DMIG from bulk data using the matrix name from the first SUBCASE |
| TEMPERATURE | Selects nodal temperatures from bulk data |
| SETDISPLACEMENTVELOCITYACCELERATIONSPCFORCESPRESSURE | Selects nodal quantities for output |
Table 3.2.30–3 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 |
| Nastran Data Entry | Comment |
| 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 |
| 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 |
| Nastran Data Entry | Comment |
| 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 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 Entry | Comment |
| 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 |
| SPCADD | Used to combine SPC/SPC1/SPCD data into a new set |
| SPCSPC1SPCD | *BOUNDARY |
| LOAD | Used to combine FORCE, MOMENT, etc. data into a new set |
| FORCEFORCE1FORCE2MOMENTMOMENT1MOMENT2 | *CLOAD |
| PLOADPLOAD1PLOAD2PLOAD4RFORCE | *DLOAD |
| Nastran Data Entry | Comment |
| DLOAD | Dynamic loads as functions of time or frequency |
| DAREALSEQ | |
| 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 |
| EIGREIGRL | *FREQUENCY |
| EIGC | *COMPLEX FREQUENCY |
| TABDMP1 | *MODAL DAMPING |
| FREQ | Forcing frequencies for steady-state dynamic procedures |
| FREQ1 | |
| FREQ2 | |
| FREQ3 | |
| FREQ4 | |
| FREQ5 | |
| MPCADD | *EQUATION |
| MPC |
| Nastran Data Entry | Comment |
| 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]
[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:
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, 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:
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.
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}