# 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: ```python 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: ```python 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: ```python 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: ```python 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: ```python 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 # 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 $1 . 0 \times 1 0 ^ { - 2 0 }$ , 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. # 3.2.31 TRANSLATING Abaqus FILES TO NASTRAN BULK DATA FILES Products: Abaqus/Standard Abaqus/Explicit # References • “Execution procedure for Abaqus: overview,” Section 3.1.1 • “Translating Nastran bulk data files to Abaqus input files,” Section 3.2.30 # Overview 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. # 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 3.2.31–1 Abaqus keyword–to–Nastran mapping.
Abaqus KeywordNastran Complement
*BEAM GENERAL SECTION,SECTION=GENERALPBAR
*BOUNDARYSPC
*CLOADFORCE
*COUPLING, DISTRIBUTINGRBE3
*COUPLING, KINEMATICRBE2
Abaqus KeywordNastran Complement
*ELEMENT, B31CBAR (for *BEAM GENERAL SECTION, SECTION=GENERAL)
*ELEMENT, B33CBAR (for *BEAM GENERAL SECTION, SECTION=GENERAL)
*ELEMENT, C3D4xCTETRA
*ELEMENT, C3D10xCTETRA
*ELEMENT, C3D6xCPENTA
*ELEMENT, C3D15xCPENTA
*ELEMENT, C3D8xCHEXA
*ELEMENT, C3D20xCHEXA
*ELEMENT, MASSCONM2
*ELEMENT, ROTARYICONM2
*ELEMENT, S3xCTRIA3
*ELEMENT, S4xCQUAD4
*ELEMENT, S8xCQUAD8
*ELEMENT, SPRING1 or SPRING2CELAS
*ELEMENT, SPRINGACROD
*ELEMENT, STRI65CTRIA6
*ELEMENT, T3D2CROD
*FREQUENCYSOL 103
*HEADINGTITLE
*MATERIAL, DENSITYMAT1
*MATERIAL, ELASTIC, TYPE=ISOMAT1
*MATERIAL, ELASTIC, TYPE=LAMINAMAT8
*MATERIAL, EXPANSION, TYPE=ISOMAT1
*MATERIAL, EXPANSION, TYPE=ORTHOMAT8
*NODEGRID
*ORIENTATION, DEFINITION=COORDINATESCORD2R, CORD2C, or CORD2S
Abaqus KeywordNastran Complement
*SHELL GENERAL SECTION (Non-composite)PSHELL
*SHELL SECTION (Non-composite)
*SHELL SECTION (Composite)PCOMP
*SHELL GENERAL SECTION (Composite)
*SOLID SECTIONPSOLID
*SOLID SECTION (Trusses)PROD
*STATICSOL 101
*SYSTEMCORD2R, CORD2C, or CORD2S
*TRANSFORM
# Command summary abaqus tonastran job=job-name [input=input-file] [substructure] [complex={YES | NO}] # 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. # 3.2.32 TRANSLATING ANSYS INPUT FILES TO PARTIAL Abaqus INPUT FILES Products: Abaqus/Standard Abaqus/Explicit # Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 # Overview The translator from ANSYS to Abaqus converts certain entities in an ANSYS blocked coded database file into their equivalent in an Abaqus input file. # Using the translator The abaqus fromansys translator can convert ANSYS blocked coded database files (.cdb) into a “flat” Abaqus input file; that is, an Abaqus input file that is not written in terms of parts and assemblies. The .cdb file must be created in ANSYS using the following command: CDWRITE , , , cdb The second field of the CDWRITE command may contain ALL or DB. The eighth field may contain BLOCKED. Any other use of the CDWRITE command will create problems for the translator. # Summary of ANSYS entities translated The translator from ANSYS to Abaqus supports the mappings shown in the tables below. Table 3.2.32–1 Nodal data mapping for ANSYS commands.
ANSYS commandAbaqus equivalent
NBLOCK*NODE*TRANSFORM
Table 3.2.32–2 Element data mapping for ANSYS structural lines.
ANSYS commandAbaqus equivalent
LINK1*ELEMENT, TYPE=T2D2
LINK8*ELEMENT, TYPE=T3D2
LINK10*ELEMENT, TYPE=T3D2
ANSYS commandAbaqus equivalent
LINK11*ELEMENT, TYPE=T3D2
LINK180*ELEMENT, TYPE=T3D2
Table 3.2.32–3 Element data mapping for ANSYS structural beams.
ANSYS commandAbaqus equivalent
BEAM3*ELEMENT, TYPE=B21
BEAM4*ELEMENT, TYPE=B31
BEAM23*ELEMENT, TYPE=B21
BEAM24*ELEMENT, TYPE=B31
BEAM188*ELEMENT, TYPE=B31 or B32
BEAM189*ELEMENT, TYPE=B32
Table 3.2.32–4 Element data mapping for ANSYS structural shells.
ANSYS commandAbaqus equivalent
SHELL43*ELEMENT, TYPE=S4 or S3
SHELL63*ELEMENT, TYPE=S4, S3, M3D4, or M3D3
SHELL93*ELEMENT, TYPE=S8R or STRI65
SHELL181*ELEMENT, TYPE=S4R or S3R
Table 3.2.32–5 Element data mapping for ANSYS structural pipes.
ANSYS commandAbaqus equivalent
PIPE16*ELEMENT, TYPE=PIPE32
PIPE20*ELEMENT, TYPE=PIPE31
PIPE59*ELEMENT, TYPE=PIPE31
Table 3.2.32–6 Element data mapping for ANSYS planar elements.
ANSYS commandAbaqus equivalent
PLANE42*ELEMENT, TYPE=CPSn, CAXn, or CPEn
PLANE82
PLANE182
PLANE183
Table 3.2.32–7 Element data mapping for ANSYS solid elements.
ANSYS commandAbaqus equivalent
SOLID45*ELEMENT, TYPE=C3D8I, C3D4, or C3D6
SOLID65*ELEMENT, TYPE=C3D8I, C3D4, or C3D6
SOLID92*ELEMENT, TYPE=C3D10
SOLID95*ELEMENT, TYPE=C3D20, C3D10, or C3D15
SOLID147*ELEMENT, TYPE=C3D20, C3D10, or C3D15
SOLID148*ELEMENT, TYPE=C3D10
SOLID185*ELEMENT, TYPE=C3D8, C3D4, or C3D6
SOLID186*ELEMENT, TYPE=C3D20R, C3D10, or C3D15
SOLID187*ELEMENT, TYPE=C3D10
Table 3.2.32–8 Load and boundary condition data mapping.
ANSYS commandAbaqus equivalent
SFE, ELEM, LKEY, PRES, KVAL, VAL1, VAL2, VAL3, VAL4, where VAL1=VAL2=VAL3=VAL4=n*SURFACE and *DSLOAD
SFE, ELEM, LKEY, HFLU, KVAL, VAL1, VAL2, VAL3, VAL4, where VAL1=VAL2=VAL3=VAL4=n*SURFACE and *DSFLUX
BF, NODE, TEMP, VAL1, VAL2, VAL3, VAL4*TEMPERATURE and *CFLUX
ANSYS commandAbaqus equivalent
BFE, NODE, HGEN, STLOCVAL1, VAL2, VAL3, VAL4*DFLUX
ACEL, 1-component, 2-component, 3-component*DLOAD
F, NODE, Lab, VALUE, VALUE2, NEND, NINC, where Lab=FX, FY, or FZ*CLOAD
D, NODE, Lab, VALUE, VALUE2, NEND, NINC, where Lab=UX,UY, UZ, ROTX, ROTY, or ROTZ*BOUNDARY
Table 3.2.32–9 Material data mapping.
ANSYS commandAbaqus equivalent
MPTEMP, ...MPDATA, ... , EXMPDATA, ... , NUXY or PRXY*MATERIAL and *ELASTICMinor Poisson's ratios (such as NUXY), if present, are automatically converted to major Poisson's ratios (such as PRXY).
MPTEMP, ....MPDATA, ... , EXMPDATA, ... , EYMPDATA, ... , EZMPDATA, ... , NUXY or PRXYMPDATA, ... , NUXZ or PRXZMPDATA, ... , NUYZ or PRYZMPDATA, ... , GXYMPDATA, ... , GXZMPDATA, ... , GYZ*MATERIAL and *ELASTIC, TYPE=ENGINEERING CONSTANTSMinor Poisson's ratios (such as NUXY), if present, are automatically converted to major Poisson's ratios (such as PRXY).
MPTEMP, ...MPDATA, ... , KXX*MATERIAL and *CONDUCTIVITY
MPTEMP, ...MPDATA, ... , DENS*DENSITY
MPTEMP, ...MPDATA, ... , C*SPECIFIC HEAT
MPTEMP, ...MPDATA, ... , CTEX or ALPX*EXPANSION