Products: Abaqus/Standard Abaqus/Explicit
The translator from ANSYS to Abaqus converts certain entities in an ANSYS input file into their equivalent in an Abaqus input file.
The abaqus fromansys translator can convert ANSYS archived model files (.cdb) into Abaqus input file format.
Note: abaqus fromansys is certified against Version 11.0 of the ANSYS Workbench, but you can translate ANSYS data created by earlier versions of ANSYS.
The ANSYS data entries that are translated are listed in the tables below. Other valid ANSYS data are skipped over and noted in the log file. Unless the key option for a particular ANSYS element is specifically cited, the translator uses the default value for that key option during translation.
Table 3.2.25–1 Nodal data mapping for ANSYS keywords.
| ANSYS syntax | Abaqus equivalent |
|---|---|
| NBLOCK, 6, SOLID (3i8,6e16.9) 1 0 0    2 0 0    . . . Node n 0 0    | *NODE 1, , , 2, , , . . . Node n, , , |
| NBLOCK, 6, SOLID (3i8,6e16.9) 1 0 0    2 0 0 3 0 0    | *NSET, NSET=_Pick4, INSTANCE=PART1, INTERNAL 2, 3, 1 *NSET, NSET=Datum-csys-1, INTERNAL _Pick4 *TRANSFORM, NSET=Datum-csys-1  ,  ,  ,  ,  ,  |
Table 3.2.25–2 Element data mapping for ANSYS structural lines.1
| ANSYS element | Abaqus equivalent |
|---|---|
| LINK1 | *ELEMENT, TYPE=T2D2 |
| LINK8 | *ELEMENT, TYPE=T3D2 |
| LINK10 | *ELEMENT, TYPE=T3D2 |
| LINK11 | *ELEMENT, TYPE=T3D2 |
| LINK180 | *ELEMENT, TYPE=T3D2 |
| 1 Only element data are translated for structural line components in ANSYS. Translation of related physics is not supported. | |
Table 3.2.25–3 Element data mapping for ANSYS structural beams.
| ANSYS element | Abaqus equivalent |
|---|---|
| BEAM3 | *ELEMENT, TYPE=B21 Abaqus translates element data only; beam section data, real constant block data, and any other related physical data are not translated. |
| BEAM4 | *ELEMENT, TYPE=B31 Abaqus translates element data only; beam section data, real constant block data, and any other related physical data are not translated. |
| BEAM23 | *ELEMENT, TYPE=B21 Abaqus translates element data only; beam section data, real constant block data, and any other related physics are not translated. |
| BEAM24 | *ELEMENT, TYPE=B31 Abaqus translates element data only; beam section data, real constant block data, and any other related physical data are not translated. |
| BEAM188 | *ELEMENT, TYPE=B31 or B32 Abaqus does not translate cross-sectional data for beam general sections. |
| BEAM189 | *ELEMENT, TYPE=B32 Abaqus does not translate cross-sectional data for beam general sections. |
Table 3.2.25–4 Element data mapping for ANSYS structural shells.
| ANSYS element | Supported ANSYS key options | Abaqus equivalent |
|---|---|---|
| SHELL28 | None. | *ELEMENT, TYPE=S4 |
| SHELL43 | None. | *ELEMENT, TYPE=S4 or S3 |
| SHELL63 | Key option 1=0 | *ELEMENT, TYPE=S4 or S3 |
| Key option 1=1 | *ELEMENT, TYPE=M3D4 or M3D3 | |
| Key option 1=2 | *ELEMENT, TYPE=S4 or S3 | |
| SHELL93 | None. | *ELEMENT, TYPE=S8 or S6 |
| SHELL181 | Key option 3=0 Key option 1=0 | *ELEMENT, TYPE=S4R or S3R |
| Key option 3=0 Key option 1=1 | *ELEMENT, TYPE=M3D4R or M3D3 | |
| Key option 3=0 Key option 1=2 | *ELEMENT, TYPE=S4R or S3R | |
| Key option 3=0 Key option 1=0 | *ELEMENT, TYPE=S4 or S3 | |
| Key option 3=0 Key option 1=1 | *ELEMENT, TYPE=M3D4 or M3D3 | |
| Key option 3=0 Key option 1=2 | *ELEMENT, TYPE=S4 or S3 |
Table 3.2.25–5 Element data mapping for ANSYS structural pipes.2
| ANSYS element | Abaqus equivalent |
|---|---|
| PIPE16 | *ELEMENT, TYPE=PIPE32 |
| PIPE20 | *ELEMENT, TYPE=PIPE31 |
| PIPE59 | *ELEMENT, TYPE=PIPE31 |
| 2 Only element data are translated for structural pipe components in ANSYS. Translation of related physics is not supported. | |
Table 3.2.25–6 Element data mapping for ANSYS planar elements.
| ANSYS element | Supported ANSYS key options | Abaqus equivalent3 |
|---|---|---|
| PLANE42 | Key option 2=0 Key option 3=0 | *ELEMENT, TYPE=CPSn(I) |
| Key option 2=0 Key option 3=1 | *ELEMENT, TYPE=CAXn(I) | |
| Key option 2=0 Key option 3=2 | *ELEMENT, TYPE=CPEn(I) | |
| Key option 2=0 Key option 3=3 | *ELEMENT, TYPE=CPSn(I) | |
| Key option 2=1 Key option 3=0 | *ELEMENT, TYPE=CPSn | |
| Key option 2=1 Key option 3=1 | *ELEMENT, TYPE=CAXn | |
| Key option 2=1 Key option 3=2 | *ELEMENT, TYPE=CPEn | |
| Key option 2=1 Key option 3=3 | *ELEMENT, TYPE=CPSn | |
| PLANE82 | Key option 3=0 | *ELEMENT, TYPE=CPSn |
| Key option 3=1 | *ELEMENT, TYPE=CAXn | |
| Key option 3=2 | *ELEMENT, TYPE=CPEn | |
| Key option 3=3 | *ELEMENT, TYPE=CPSn | |
| PLANE182 | Key option 1=0, 2, or 3 Key option 3=0 | *ELEMENT, TYPE=CPSn |
| Key option 1=0, 2, or 3 Key option 3=1 | *ELEMENT, TYPE=CAXn | |
| Key option 1=0, 2, or 3 Key option 3=2 | *ELEMENT, TYPE=CPEn | |
| Key option 1=0, 2, or 3 Key option 3=3 | *ELEMENT, TYPE=CPSn | |
| Key option 1=0, 2, or 3 Key option 3=5 | *ELEMENT, TYPE=CPEGn | |
| Key option 1=1 Key option 3=0 | *ELEMENT, TYPE=CPSn(R) | |
| Key option 1=1 Key option 3=1 | *ELEMENT, TYPE=CAXn(R) | |
| Key option 1=1 Key option 3=2 | *ELEMENT, TYPE=CPEn(R) | |
| Key option 1=1 Key option 3=3 | *ELEMENT, TYPE=CPSn(R) | |
| Key option 1=1 Key option 3=5 | *ELEMENT, TYPE=CPEGn | |
| PLANE183 | Key option 3=0 | *ELEMENT, TYPE=CPSn |
| Key option 3=1 | *ELEMENT, TYPE=CAXn | |
| Key option 3=2 | *ELEMENT, TYPE=CPEn | |
| Key option 3=3 | *ELEMENT, TYPE=CPSn | |
| Key option 3=5 | *ELEMENT, TYPE=CPEGn | |
| 3 The translation creates Abaqus elements where n is the number of nodes in the resulting Abaqus element. The supported values are 3, 4, 6, and 8. If (I) is included in the mapping, incompatible modes are supported for 4-noded elements. If (R) is included in the mapping, reduced integration modes are supported for 4- and 8-noded elements. | ||
Table 3.2.25–7 Element data mapping for ANSYS solid elements.4
| ANSYS element | Supported ANSYS key options | Abaqus equivalent |
|---|---|---|
| SOLID45 | Key option 1=0 Key option 2=0 | *ELEMENT, TYPE=C3D8I, C3D4, or C3D6 |
| Key option 1=0 Key option 2=1 | *ELEMENT, TYPE=C3D8R, C3D4, or C3D6 | |
| Key option 1=1 Key option 2=0 | *ELEMENT, TYPE=C3D8, C3D4, or C3D6 | |
| Key option 1=1 Key option 2=1 | *ELEMENT, TYPE=C3D8R, C3D4, or C3D6 | |
| SOLID65 | Key option 1=0 | *ELEMENT, TYPE=C3D8I, C3D4, or C3D6 |
| Key option 1=1 | *ELEMENT, TYPE=C3D8R, C3D4, or C3D6 | |
| SOLID92 | None. | *ELEMENT, TYPE=C3D10 |
| SOLID95 | Key option 11=0 | *ELEMENT, TYPE=C3D20, C3D10, or C3D15 |
| Key option 11=1 | *ELEMENT, TYPE=C3D20, C3D10, or C3D15 | |
| SOLID147 | None. | *ELEMENT, TYPE=C3D20, C3D10, or C3D15 |
| SOLID148 | None. | *ELEMENT, TYPE=C3D10 |
| SOLID185 | Key option 2=0 or 3 Key option 6=0 | *ELEMENT, TYPE=C3D8, C3D4, or C3D6 |
| Key option 2=0 or 3 Key option 6=1 | *ELEMENT, TYPE=C3D8H, C3D4H, or C3D6H | |
| Key option 2=2 Key option 6=0 | *ELEMENT, TYPE=C3D8I, C3D4, or C3D6 | |
| Key option 2=2 Key option 6=1 | *ELEMENT, TYPE=C3D8IH, C3D4H, or C3D6H | |
| Key option 2=1 Key option 6=0 | *ELEMENT, TYPE=C3D8R, C3D4, or C3D6 | |
| Key option 2=1 Key option 6=1 | *ELEMENT, TYPE=C3D8RH, C3D4H, or C3D6H | |
| SOLID186 | Key option 2=0 Key option 6=0 | *ELEMENT, TYPE=C3D20R, C3D10, or C3D15 |
| Key option 2=0 Key option 6=1 | *ELEMENT, TYPE=C3D20RH, C3D10H, or C3D15H | |
| Key option 2=1 Key option 6=0 | *ELEMENT, TYPE=C3D20, C3D10, or C3D15 | |
| Key option 2=1 Key option 6=1 | *ELEMENT, TYPE=C3D20H, C3D10H, or C3D15H | |
| SOLID187 | Key option 6=0 | *ELEMENT, TYPE=C3D10 |
| Key option 6=1 | *ELEMENT, TYPE=C3D10H | |
| 4 Only element data are translated for solid elements in ANSYS. Translation of related physics is not supported. | ||
Table 3.2.25–8 Solid section data mapping.
| ANSYS solid section parameter | Abaqus equivalent |
|---|---|
| None. (ANSYS does not write any keywords for solid section data.) | *SOLID SECTION |
Table 3.2.25–9 Homogeneous shell section data mapping.
| ANSYS shell section parameter | Abaqus equivalent |
|---|---|
| SECTYPE, 1, SHELL | *SHELL SECTION |
| SECOFFSET, MID | *SHELL SECTION, OFFSET=0.0 (default) |
| SECOFFSET, TOP | *SHELL SECTION, OFFSET=0.5 |
| SECOFFSET, BOT | *SHELL SECTION, OFFSET=-0.5 |
| SECOFFSET, USER | *SHELL SECTION, OFFSET= , where is a user-specified value between  and  |
| SECBLOCK, MATERIAL ID | *SHELL SECTION, MATERIAL=material_name |
| SECBLOCK, GAUSS INTEGRATION POINT | *SHELL SECTION, SECTION INTEGRATION=GAUSS |
| SECCONTROL, E11 | *TRANSVERSE SHEAR STIFFNESS |
| SECCONTROL, E22 | *TRANSVERSE SHEAR STIFFNESS |
| SECCONTROL, E12 | *TRANSVERSE SHEAR STIFFNESS |
| SECCONTROL, ADDMAS | *SHELL SECTION, DENSITY=n |
Table 3.2.25–10 Shell section data mapping.
| ANSYS shell section real constant | Abaqus equivalent |
|---|---|
| THICK | *SHELL SECTION shell thickness |
| TK(I), TK(J), TK(K), or TK(L) | *SHELL SECTION shell thickness Note: Abaqus translates shell thickness data only when the shell sections at nodes I, J, K, and L are of a constant thickness. |
Table 3.2.25–11 Beam section data mapping.
| ANSYS beam section parameter | Abaqus equivalent |
|---|---|
| SECTYPE, 1, BEAM, HREC | *BEAM SECTION, SECTION=BOX |
| SECTYPE, 1, BEAM, CSOL | *BEAM SECTION, SECTION=CIRC |
| SECTYPE, 1, BEAM, RECT | *BEAM SECTION, SECTION=RECT |
| SECTYPE, 1, BEAM, I | *BEAM SECTION, SECTION=I |
| SECTYPE, 1, BEAM, L | *BEAM SECTION, SECTION=L |
| SECTYPE, 1, BEAM, CTUB | *BEAM SECTION, SECTION=PIPE |
| SECDATA | Beam-related data are mapped to the data lines for *BEAM SECTION. |
Table 3.2.25–12 Load and boundary condition data mapping.
| Load or boundary condition classification | ANSYS keyword | Abaqus equivalent |
|---|---|---|
| Surface loads on elements | SFE, ELEM, LKEY, PROC, KVAL, VAL1, VAL2, VAL3, VAL4, where VAL1=VAL2=VAL3=VAL4=n. | *ELEMENT, ELSET=pickedsurf2 *SURFACE, TYPE=ELEMENT, NAME=pickedset3 pickedsurf2, S4 *DSLOAD pickedset3, P, n |
| SFE, ELEM, LKEY, HFLU, KVAL, VAL1, VAL2, VAL3, VAL4, where VAL1=VAL2=VAL3=VAL4=n. | *ELEMENT, ELSET=pickedsurf2 *SURFACE, TYPE=ELEMENT, NAME=pickedset3 pickedsurf2, S6 *DSFLUX pickedset3, P, n | |
| SFE, ELEM, LKEY, CONV, KVAL, VAL1, VAL2, VAL3, VAL4, where VAL1=VAL2=VAL3=VAL4=n. | *ELEMENT, ELSET=pickedsurf2 *SFILM element-based surface name, F, reference sink temperature value (  ), film coefficient value (h) | |
| Nodal body force load | BF, NODE, Lab, VAL1, VAL2, VAL3, VAL4 | Ignored except for Lab=TEMP, which is translated as *TEMPERATURE; and for Lab=HGEN, which is translated as *CFLUX. |
| Element body force load | BFE, NODE, Lab, STLOCVAL1, VAL2, VAL3, VAL4 | Ignored except for Lab=HGEN, which is translated as *DFLUX. |
| Linear acceleration of structure | ACEL, 1-component, 2-component, 3-component | *DLOAD GRAV, 1-component, 2-component, 3-component |
| Load at a node | F, NODE, Lab, VALUE, VALUE2, NEND, NINC, where Lab=FX, FY, or FZ | *NSET, NSET=nset1 1, ... *CLOAD pickset1, 1, 1020 |
| DOF constraints at nodes | D, NODE, Lab, VALUE, VALUE2, NEND, NINC, where Lab=UX ,UY, UZ, ROTX, ROTY, or ROTZ | *NSET, NSET=nset1 1, ... *BOUNDARY pickset1, 1, 1020 |
| CMBLOCK, XYMMP, NODE, 50 CMGRP, XSYMM, XSYMMP, XSYMMB CMSEL,, XSYMM D, ALL, UX, 0,, | *NSET, NSET=pickset1 (node in CMBLOCK) *BOUNDARY pickset1, 1, 0.00 | |
| D, CMGRP, UX, 0,,, | *NSET, NSET=pickset1 (node in CMBLOCK) *BOUNDARY | |
| D, CMBLOCK, UY, 0,,, | *NSET, NSET=pickset1 (node in CMBLOCK) *BOUNDARY pickset1, 2, 0.00 |
Table 3.2.25–13 Interaction data mapping.
| ANSYS keyword | ANSYS key option | Abaqus equivalent |
|---|---|---|
| CONTA173 or CONTA174 (Surface-to-surface contact) | Key option 12=1 (for rough contact) | *SURFACE BEHAVIOR, AUGMENTED LAGRANGE *CONTACT PAIR, ADJUST=node_set, TIED *FRICTION, ROUGH |
| Key option 12=2 (for no separation) | *SURFACE BEHAVIOR, NO SEPARATION *CONTACT PAIR *FRICTION 0 | |
| Key option 12=3 (for bonded contact) | *SURFACE BEHAVIOR, AUGMENTED LAGRANGE *CONTACT PAIR, ADJUST=node_set, TIED | |
| Key option 12=5 (for always bonded contact) | ||
| Key option 12=6 (for initially bonded contact) | ||
| Key option 2=0 (augmented Lagrangian, default) | *SURFACE BEHAVIOR, AUGMENTED LAGRANGE | |
| Key option 2=1 (penalty function) | *SURFACE BEHAVIOR, PENALTY | |
| RLBLOCK | FTOLN (penetration tolerance factor) | *CONTACT CONTROLS |
| TCC (thermal contact conductance) | *GAP CONDUCTANCE | |
| FACT (static/ dynamic ratio) | *FRICTION, EXPONENTIAL DECAY static friction coefficient (  ), kinetic friction coefficient ( ), decay coefficient ( ) | |
| DC (exponential decay coefficient) | *FRICTION, EXPONENTIAL DECAY | |
| SLTO (allowable elastic slip) | *FRICTION, SLIP TOLERANCE= | |
| FKN | *SURFACE BEHAVIOR, PENALTY |
Table 3.2.25–14 Material data mapping.
| Material property classification | ANSYS keyword | Abaqus equivalent |
|---|---|---|
| Isotropic elasticity | MP, EX, 1, E, MP, PRXY, 1,  , | *MATERIAL, NAME=default_name *ELASTIC E, |
| Isotropic elasticity with temperature dependency | MPTEMP, R5.0, 2, 1,  ,  , ...,  MPDATA, R5.0, 2, EX, 1, 1,  ,  , ...,  MPTEMP, R5.0, 2, 1, , , ..., MPDATA, R5.0, 1, PRXY, 1, 1,  ,  , ...,  | *MATERIAL, NAME=default_name *ELASTIC , , , , |
| Orthotropic elasticity | MP, EX, 1, , MP, EY, 1, , MP, EZ, 1,  , MP, PRXY, 1,  ,MP, PRYZ, 1,  ,MP, PRXZ, 1,  ,MP, GXY, 1,  , MP, GYZ, 1,  , MP, GXZ, 1,  , | *ELASTIC, TYPE=ENGINEERING CONSTANTS, , , , , , , |
| Thermal conductivity | MPTEMP, R5.0, 2, 1,  ,MPDATA, R5.0, 2, KXX, 1, 1,  | *CONDUCTIVITY, |
| Density | MPTEMP, R5.0, 2, 1, , MPDATA, R5.0, 2, DENS, 1, 1, mass density (Mass density is expressed in units of ML–3.) | *DENSITY mass density, |
| Specific heat | MPTEMP, R5.0, 2, 1, , MPDATA, R5.0, 2, C, 1, 1, specific heat per unit mass (Specific heat per unit mass is expressed in units of JM–1 –1.) | *SPECIFIC HEAT specific heat per unit mass, |
| Instantaneous coefficients of thermal expansion | MPTEMP, R5.0, 2, 1, , MPDATA, R5.0, 2, CTEX, 1, 1,  , | *EXPANSION, |
Table 3.2.25–16 Output data mapping.
| ANSYS syntax | Abaqus equivalent |
|---|---|
| By default, the ANSYS input file does not include output requests. | *OUTPUT, VARIABLE=PRESELECT |
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.