Translating ANSYS input files to partial Abaqus input files

The translator from ANSYS to Abaqus converts certain entities in an ANSYS blocked coded database file into their equivalent in an Abaqus input file.

The following topics are discussed:

Using the translator
Summary of ANSYS entities translated
Command summary
Command line options

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.