<!-- source-page: 471 -->

# 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 
```

<!-- source-page: 472 -->

# 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.

<!-- source-page: 473 -->

# 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. 

<table><tr><td>Abaqus Keyword</td><td>Nastran Complement</td></tr><tr><td>*BEAM GENERAL SECTION,SECTION=GENERAL</td><td>PBAR</td></tr><tr><td>*BOUNDARY</td><td>SPC</td></tr><tr><td>*CLOAD</td><td>FORCE</td></tr><tr><td>*COUPLING, DISTRIBUTING</td><td>RBE3</td></tr><tr><td>*COUPLING, KINEMATIC</td><td>RBE2</td></tr></table>

<!-- source-page: 474 -->

<table><tr><td>Abaqus Keyword</td><td>Nastran Complement</td></tr><tr><td>*ELEMENT, B31</td><td>CBAR (for *BEAM GENERAL SECTION, SECTION=GENERAL)</td></tr><tr><td>*ELEMENT, B33</td><td>CBAR (for *BEAM GENERAL SECTION, SECTION=GENERAL)</td></tr><tr><td>*ELEMENT, C3D4x</td><td>CTETRA</td></tr><tr><td>*ELEMENT, C3D10x</td><td>CTETRA</td></tr><tr><td>*ELEMENT, C3D6x</td><td>CPENTA</td></tr><tr><td>*ELEMENT, C3D15x</td><td>CPENTA</td></tr><tr><td>*ELEMENT, C3D8x</td><td>CHEXA</td></tr><tr><td>*ELEMENT, C3D20x</td><td>CHEXA</td></tr><tr><td>*ELEMENT, MASS</td><td>CONM2</td></tr><tr><td>*ELEMENT, ROTARYI</td><td>CONM2</td></tr><tr><td>*ELEMENT, S3x</td><td>CTRIA3</td></tr><tr><td>*ELEMENT, S4x</td><td>CQUAD4</td></tr><tr><td>*ELEMENT, S8x</td><td>CQUAD8</td></tr><tr><td>*ELEMENT, SPRING1 or SPRING2</td><td>CELAS</td></tr><tr><td>*ELEMENT, SPRINGA</td><td>CROD</td></tr><tr><td>*ELEMENT, STRI65</td><td>CTRIA6</td></tr><tr><td>*ELEMENT, T3D2</td><td>CROD</td></tr><tr><td>*FREQUENCY</td><td>SOL 103</td></tr><tr><td>*HEADING</td><td>TITLE</td></tr><tr><td>*MATERIAL, DENSITY</td><td>MAT1</td></tr><tr><td>*MATERIAL, ELASTIC, TYPE=ISO</td><td>MAT1</td></tr><tr><td>*MATERIAL, ELASTIC, TYPE=LAMINA</td><td>MAT8</td></tr><tr><td>*MATERIAL, EXPANSION, TYPE=ISO</td><td>MAT1</td></tr><tr><td>*MATERIAL, EXPANSION, TYPE=ORTHO</td><td>MAT8</td></tr><tr><td>*NODE</td><td>GRID</td></tr><tr><td>*ORIENTATION, DEFINITION=COORDINATES</td><td>CORD2R, CORD2C, or CORD2S</td></tr></table>

<!-- source-page: 475 -->

<table><tr><td>Abaqus Keyword</td><td>Nastran Complement</td></tr><tr><td>*SHELL GENERAL SECTION (Non-composite)</td><td rowspan="2">PSHELL</td></tr><tr><td>*SHELL SECTION (Non-composite)</td></tr><tr><td>*SHELL SECTION (Composite)</td><td rowspan="2">PCOMP</td></tr><tr><td>*SHELL GENERAL SECTION (Composite)</td></tr><tr><td>*SOLID SECTION</td><td>PSOLID</td></tr><tr><td>*SOLID SECTION (Trusses)</td><td>PROD</td></tr><tr><td>*STATIC</td><td>SOL 101</td></tr><tr><td>*SYSTEM</td><td rowspan="2">CORD2R, CORD2C, or CORD2S</td></tr><tr><td>*TRANSFORM</td></tr></table>

# 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.

<!-- source-page: 476 -->

<!-- source-page: 477 -->

# 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 , , <jobname>, 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. 

<table><tr><td>ANSYS command</td><td>Abaqus equivalent</td></tr><tr><td>NBLOCK</td><td>*NODE*TRANSFORM</td></tr></table>

Table 3.2.32–2 Element data mapping for ANSYS structural lines. 

<table><tr><td>ANSYS command</td><td>Abaqus equivalent</td></tr><tr><td>LINK1</td><td>*ELEMENT, TYPE=T2D2</td></tr><tr><td>LINK8</td><td>*ELEMENT, TYPE=T3D2</td></tr><tr><td>LINK10</td><td>*ELEMENT, TYPE=T3D2</td></tr></table>

<!-- source-page: 478 -->

<table><tr><td>ANSYS command</td><td>Abaqus equivalent</td></tr><tr><td>LINK11</td><td>*ELEMENT, TYPE=T3D2</td></tr><tr><td>LINK180</td><td>*ELEMENT, TYPE=T3D2</td></tr></table>

Table 3.2.32–3 Element data mapping for ANSYS structural beams. 

<table><tr><td>ANSYS command</td><td>Abaqus equivalent</td></tr><tr><td>BEAM3</td><td>*ELEMENT, TYPE=B21</td></tr><tr><td>BEAM4</td><td>*ELEMENT, TYPE=B31</td></tr><tr><td>BEAM23</td><td>*ELEMENT, TYPE=B21</td></tr><tr><td>BEAM24</td><td>*ELEMENT, TYPE=B31</td></tr><tr><td>BEAM188</td><td>*ELEMENT, TYPE=B31 or B32</td></tr><tr><td>BEAM189</td><td>*ELEMENT, TYPE=B32</td></tr></table>

Table 3.2.32–4 Element data mapping for ANSYS structural shells. 

<table><tr><td>ANSYS command</td><td>Abaqus equivalent</td></tr><tr><td>SHELL43</td><td>*ELEMENT, TYPE=S4 or S3</td></tr><tr><td>SHELL63</td><td>*ELEMENT, TYPE=S4, S3, M3D4, or M3D3</td></tr><tr><td>SHELL93</td><td>*ELEMENT, TYPE=S8R or STRI65</td></tr><tr><td>SHELL181</td><td>*ELEMENT, TYPE=S4R or S3R</td></tr></table>

Table 3.2.32–5 Element data mapping for ANSYS structural pipes. 

<table><tr><td>ANSYS command</td><td>Abaqus equivalent</td></tr><tr><td>PIPE16</td><td>*ELEMENT, TYPE=PIPE32</td></tr><tr><td>PIPE20</td><td>*ELEMENT, TYPE=PIPE31</td></tr><tr><td>PIPE59</td><td>*ELEMENT, TYPE=PIPE31</td></tr></table>

<!-- source-page: 479 -->

Table 3.2.32–6 Element data mapping for ANSYS planar elements. 

<table><tr><td>ANSYS command</td><td>Abaqus equivalent</td></tr><tr><td>PLANE42</td><td>*ELEMENT, TYPE=CPSn, CAXn, or CPEn</td></tr><tr><td>PLANE82</td><td></td></tr><tr><td>PLANE182</td><td></td></tr><tr><td>PLANE183</td><td></td></tr></table>

Table 3.2.32–7 Element data mapping for ANSYS solid elements. 

<table><tr><td>ANSYS command</td><td>Abaqus equivalent</td></tr><tr><td>SOLID45</td><td>*ELEMENT, TYPE=C3D8I, C3D4, or C3D6</td></tr><tr><td>SOLID65</td><td>*ELEMENT, TYPE=C3D8I, C3D4, or C3D6</td></tr><tr><td>SOLID92</td><td>*ELEMENT, TYPE=C3D10</td></tr><tr><td>SOLID95</td><td>*ELEMENT, TYPE=C3D20, C3D10, or C3D15</td></tr><tr><td>SOLID147</td><td>*ELEMENT, TYPE=C3D20, C3D10, or C3D15</td></tr><tr><td>SOLID148</td><td>*ELEMENT, TYPE=C3D10</td></tr><tr><td>SOLID185</td><td>*ELEMENT, TYPE=C3D8, C3D4, or C3D6</td></tr><tr><td>SOLID186</td><td>*ELEMENT, TYPE=C3D20R, C3D10, or C3D15</td></tr><tr><td>SOLID187</td><td>*ELEMENT, TYPE=C3D10</td></tr></table>

Table 3.2.32–8 Load and boundary condition data mapping. 

<table><tr><td>ANSYS command</td><td>Abaqus equivalent</td></tr><tr><td>SFE, ELEM, LKEY, PRES, KVAL, VAL1, VAL2, VAL3, VAL4, where VAL1=VAL2=VAL3=VAL4=n</td><td>*SURFACE and *DSLOAD</td></tr><tr><td>SFE, ELEM, LKEY, HFLU, KVAL, VAL1, VAL2, VAL3, VAL4, where VAL1=VAL2=VAL3=VAL4=n</td><td>*SURFACE and *DSFLUX</td></tr><tr><td>BF, NODE, TEMP, VAL1, VAL2, VAL3, VAL4</td><td>*TEMPERATURE and *CFLUX</td></tr></table>

<!-- source-page: 480 -->

<table><tr><td>ANSYS command</td><td>Abaqus equivalent</td></tr><tr><td>BFE, NODE, HGEN, STLOCVAL1, VAL2, VAL3, VAL4</td><td>*DFLUX</td></tr><tr><td>ACEL, 1-component, 2-component, 3-component</td><td>*DLOAD</td></tr><tr><td>F, NODE, Lab, VALUE, VALUE2, NEND, NINC, where Lab=FX, FY, or FZ</td><td>*CLOAD</td></tr><tr><td>D, NODE, Lab, VALUE, VALUE2, NEND, NINC, where Lab=UX,UY, UZ, ROTX, ROTY, or ROTZ</td><td>*BOUNDARY</td></tr></table>

Table 3.2.32–9 Material data mapping. 

<table><tr><td>ANSYS command</td><td>Abaqus equivalent</td></tr><tr><td>MPTEMP, ...MPDATA, ... , EXMPDATA, ... , NUXY or PRXY</td><td>*MATERIAL and *ELASTICMinor Poisson&#x27;s ratios (such as NUXY), if present, are automatically converted to major Poisson&#x27;s ratios (such as PRXY).</td></tr><tr><td>MPTEMP, ....MPDATA, ... , EXMPDATA, ... , EYMPDATA, ... , EZMPDATA, ... , NUXY or PRXYMPDATA, ... , NUXZ or PRXZMPDATA, ... , NUYZ or PRYZMPDATA, ... , GXYMPDATA, ... , GXZMPDATA, ... , GYZ</td><td>*MATERIAL and *ELASTIC, TYPE=ENGINEERING CONSTANTSMinor Poisson&#x27;s ratios (such as NUXY), if present, are automatically converted to major Poisson&#x27;s ratios (such as PRXY).</td></tr><tr><td>MPTEMP, ...MPDATA, ... , KXX</td><td>*MATERIAL and *CONDUCTIVITY</td></tr><tr><td>MPTEMP, ...MPDATA, ... , DENS</td><td>*DENSITY</td></tr><tr><td>MPTEMP, ...MPDATA, ... , C</td><td>*SPECIFIC HEAT</td></tr><tr><td>MPTEMP, ...MPDATA, ... , CTEX or ALPX</td><td>*EXPANSION</td></tr></table>
