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 1. Nodal data mapping for ANSYS commands.| ANSYS command | Abaqus equivalent |
|---|
| NBLOCK |
NODETRANSFORM |
Table 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. 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 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 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 6. Element data mapping for ANSYS planar elements.| ANSYS command | Abaqus equivalent |
|---|
| PLANE42PLANE82PLANE182PLANE183 |
ELEMENT, TYPE=CPSn, CAXn, or CPEn |
Table 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 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 9. Material data mapping.| ANSYS command | Abaqus equivalent |
|---|
| MPTEMP, …MPDATA, … , EXMPDATA, … , 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, … , EXMPDATA, … , EYMPDATA, … , EZMPDATA, … , NUXY or PRXYMPDATA, … , NUXZ or PRXZMPDATA, … , NUYZ or PRYZMPDATA, … , GXYMPDATA, … , GXZMPDATA, … , 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 Summary
abaqus fromansysjobjob-nameinputinput-file
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 input file containing the ANSYS 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 ANSYS data if it is different from job-name. |