3.2.32 Translating ANSYS input files to partial Abaqus input files
Products: Abaqus/Standard Abaqus/Explicit
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.
| ANSYS command | Abaqus equivalent |
|---|---|
| NBLOCK | *NODE *TRANSFORM |
Table 3.2.32–2 Element data mapping for ANSYS structural lines.
| ANSYS command | Abaqus equivalent |
|---|---|
| LINK1 | *ELEMENT, TYPE=T2D2 |
| LINK8 | *ELEMENT, TYPE=T3D2 |
| LINK10 | *ELEMENT, TYPE=T3D2 |
| LINK11 | *ELEMENT, TYPE=T3D2 |
| LINK180 | *ELEMENT, TYPE=T3D2 |
Table 3.2.32–3 Element data mapping for ANSYS structural beams.
| ANSYS command | Abaqus 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 command | Abaqus 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 command | Abaqus 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 command | Abaqus equivalent |
|---|---|
| PLANE42 PLANE82 PLANE182 PLANE183 | *ELEMENT, TYPE=CPSn, CAXn, or CPEn |
Table 3.2.32–7 Element data mapping for ANSYS solid elements.
| ANSYS command | Abaqus 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 command | Abaqus 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 |
| 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 command | Abaqus equivalent |
|---|---|
| MPTEMP, … MPDATA, … , EX MPDATA, … , NUXY or PRXY | *MATERIAL and *ELASTIC Minor Poisson's ratios (such as NUXY), if present, are automatically converted to major Poisson's ratios (such as PRXY). |
| MPTEMP, …. MPDATA, … , EX MPDATA, … , EY MPDATA, … , EZ MPDATA, … , NUXY or PRXY MPDATA, … , NUXZ or PRXZ MPDATA, … , NUYZ or PRYZ MPDATA, … , GXY MPDATA, … , GXZ MPDATA, … , GYZ | *MATERIAL and *ELASTIC, TYPE=ENGINEERING CONSTANTS Minor 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 |
Command line options
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 input file containing the ANSYS data. Diagnostics created by the translator will be written to a file named job-name.log.
This option is used to specify the name of the file containing the ANSYS data if it is different from job-name.