## On this page
# Solver translation
Last update: 29.04.2026
Solver translation (FE2Ansys) translates Abaqus INP files to Ansys CDB and K files (MAPDL and LS-DYNA). The translation ensures that the Abaqus model can be used in Ansys without recreating from scratch. It helps to save time and effort even though minor manual adjustments may be required. The manual adjustments like redefining boundary conditions, loads, and material properties, ensures that the model behaves as expected in Ansys solver deck.
## Abaqus to Ansys MAPDL Conversion
The following example shows the translation of Abaqus INP file to CDB file format:
1. Import the Abaqus INP file.
> ```python
> file_io = prime.FileIO(model=model)
> import_results = file_io.import_abaqus_inp(
> r"E:/test2/Abaqus_Input_multistep.inp",
> prime.ImportAbaqusParams(model),
> )
> print(import_results)
>
> ```
> The import\_abaqus\_inp imports the INP file as mesh, extracts simulation specific information from the INP file and stores the information internally as a JSON document. [`ImportAbaqusParams`](../api/_autosummary/ansys.meshing.prime.ImportAbaqusParams.md#ansys.meshing.prime.ImportAbaqusParams)allows you to set the parameters for importing the model. The example uses default parameters for importing the model.
> **Output**:
> > ```pycon
> > summary_log : {"Counts": {"beam": 1,"connector": 3,"element": 6944,"elsets": 7,"errors": 0,"node": 6523,
> > "nsets": 2, "physical": 1,"shell": 5375,"skipped": 0,"solid": 1564,"translated": 65,"warnings": 0},"Ids":
> > {"beam": {"max": 7928,"min": 7928},"connector": {"max": 10001,"min": 7929},"element": {"max": 100000,"min": 1},
> > "node": {"max": 100002,"min": 13},"physical": {"max": 100000,"min": 100000},"shell": {"max": 5783,"min": 243},
> > "solid": {"max": 7287,"min": 13}},"Keywords": {"Counts": {"total_keywords_found": 96,"total_keywords_processed": 96,
> > "total_keywords_skipped": 0,"total_keywords_unprocessed": 0},"processed_keywords": {"BEAM SECTION": 1,"BOUNDARY": 1,
> > "CLOAD": 1,"COHESIVE SECTION": 1,"CONNECTOR BEHAVIOR": 1,"CONNECTOR ELASTICITY": 6,"CONNECTOR SECTION": 1,
> > "COUPLING": 1,"DENSITY": 3,"DLOAD": 1,"ELASTIC": 3,"ELEMENT": 13,"ELEMENT OUTPUT": 3,"ELSET": 7,"END STEP": 1,
> > "FASTENER": 1,"FASTENER PROPERTY": 1,"HEADING": 1,"KINEMATIC": 1,"KINEMATIC COUPLING": 1,"MASS": 1,"MATERIAL": 3,
> > "MPC": 3,"NODE": 6,"NODE OUTPUT": 1,"NONSTRUCTURAL MASS": 1,"NSET": 2,"ORIENTATION": 2,"OUTPUT": 2,"PLASTIC": 1,
> > "RIGID BODY": 1,"SECTION CONTROLS": 1,"SHELL SECTION": 2,"SOLID SECTION": 2,"SPRING": 1,"STATIC": 1,"STEP": 1,
> > "SURFACE": 12,"TIE": 4},"skipped_keywords": null,"unprocessed_keywords": null}}
> > error_code : ErrorCode.NOERROR
> > warning_codes : []
> >
> > ```
> Here, the import summary provides information on the following:
> - Total number of keywords in the imported file.
> - Total number of processed keywords.
> - Total number of skipped or unprocessed keywords.
> - Number of imported nodes.
> - Number of imported elements(solid, shell, beam and more).
> - Number and type of skipped elements.
> - Ids of imported nodes and elements.
> - Number of errors and warnings that occurred while importing the file.
1. Export the CDB file.
> ```python
> export_cdb_result = file_io.export_mapdl_cdb(
> r"E:\test3\Abaqus_Input_multistep.cdb",
> prime.ExportMapdlCdbParams(model),
> )
> print(export_cdb_result)
>
> ```
> [`ExportMapdlCdbParams`](../api/_autosummary/ansys.meshing.prime.ExportMapdlCdbParams.md#ansys.meshing.prime.ExportMapdlCdbParams) allows setting parameters to control the export of MAPDL CDB files.
> [`ExportMapdlCdbResults`](../api/_autosummary/ansys.meshing.prime.ExportMapdlCdbResults.md#ansys.meshing.prime.ExportMapdlCdbResults) contains the summary result of the export process in json format. This writes the CDB file to the specified location.
> ```pycon
> summary_log : {"Counts": {"errors": 0,"skipped": 1,"translated": 40,"warnings": 0},"Ids": {"beam":
> {"max": 7928},"constant": {"max": 44},"csys": {"max": 2},"element": {"max": 100117},"et": {"max": 28},
> "material": {"max": 114},"node": {"max": 100002},"section": {"max": 114},"shell": {"max": 100088},
> "solid": {"max": 7287}}}
> zone_mesh_results : []
> error_code : ErrorCode.NOERROR
> warning_codes : []
>
> ```
> CDB Export summary provides information about:
> - Number of error and warnings that occurred while exporting the CDB file.
> - Maximum number of node ids and elements ids that are exported.
> The following table provides a reference for Abaqus input file keywords supported. It serves as a translation reference for converting Abaqus INP format to APDL cdb format.
> #### **Supported Abaqus Keywords**
> **Keyword****Options**HEADINGNoneNODESYSTEM=RELEMENTTYPE=B31, C3D10, C3D4, C3D6, C3D6H, C3D8, C3D8H, C3D8R, C3D8RH, COH3D6, COH3D8, CONN3D2, DCOUP3D, M3D3, M3D4, MASS, R3D3, R3D4, ROTARYI, S3, S3R, S4, S4R, SPRINGA, STRI65KINEMATIC COUPLINGNoneMPCNoneORIENTATIONDEFINITION=COORDINATES, NODES; SYSTEM=RECTANGULARSOLID SECTIONNoneSHELL SECTIONDENSITY=0; NODAL THICKNESS; OFFSETCOHESIVE SECTIONRESPONSE=CONTINUUM, TRACTION SEPARATION; THICKNESS=SPECIFIEDBEAM SECTIONSECTION=CIRC, PIPECONNECTOR SECTION\[CARTESIAN–CARDAN\], \[AXIAL\], \[CARTESIAN–ROTATION\], \[WELD\], \[CARTESIAN–EULER\], \[JOIN–REVOLUTE\], \[SLOT–ALIGN\]NSETNoneELSETGENERATESURFACETYPE=ELEMENT, NODEMATERIALNoneDENSITYNoneDAMPINGSTRUCTURAL=0ELASTICTYPE=ISOTROPIC, TRACTIONCONNECTOR BEHAVIORNoneCONNECTOR ELASTICITYNONLINEAR, RIGIDCONNECTOR DAMPINGNONLINEAR; TYPE=VISCOUSSPRINGNoneMASSNoneROTARY INERTIANoneSECTION CONTROLSELEMENT DELETION=YES; HOURGLASS=ENHANCEDFASTENER PROPERTYNoneNONSTRUCTURAL MASSDISTRIBUTION=MASS PROPORTIONAL; UNITS=TOTAL MASSTIEADJUST=NO, YESFASTENERADJUST ORIENTATION=NOAMPLITUDEDEFINITION=EQUALLY SPACED, PERIODIC, TABULAR, periodic; FIXED INTERVAL=0,3; SMOOTH=0; TIME=STEP TIME, step timeRIGID BODYNoneSTEPNLGEOM=NO, YES; PERTURBATION; UNSYMM=YESSTATICSTABILIZE=0BOUNDARYBASE NAME=LOAD\_FR, LOAD\_RR; OP=NEW; TYPE=DISPLACEMENTCLOADFOLLOWER; LOADCASE=1; OP=NEW; REALDLOADOP=NEWOUTPUTFIELD, HISTORY, TIME INTERVAL=0NODE OUTPUTNoneEND STEPNoneDYNAMICAPPLICATION=MODERATE DISSIPATION, QUASIELEMENT OUTPUTPOSITION=CENTROIDALSYSTEMNoneTRANSFORMTYPE=RPLASTICNoneHYPERELASTICMODULI=LONG TERM; N=3; NEO HOOKE; REDUCED POLYNOMIAL; YEOHSURFACE INTERACTIONNoneFRICTIONSLIP TOLERANCE=0CONTACT PAIRADJUST=0; SMALL SLIDING; SMOOTH=0; TYPE=NODE TO SURFACE, SURFACE TO SURFACEMONITORDOF=1,2,3; NODE=FR\_DR\_JIG\_PT, FR\_DR\_RH\_JIG\_PT, JIG\_OS\_CENTER, RR\_DR\_JIG\_PT, RR\_DR\_RH\_JIG\_PT, nodeNODE PRINTNoneMEMBRANE SECTIONNoneTIME POINTNoneCONTACTNoneCONTACT INCLUSIONSALL EXTERIORCONTACT EXCLUSIONSNoneCONTACT PROPERTY ASSIGNMENTNoneDAMAGE INITIATIONCRITERION=DUCTILEDAMAGE EVOLUTIONTYPE=DISPLACEMENTFREQUENCYDAMPING PROJECTION=ON; EIGENSOLVER=AMS; NORMALIZATION=MASS; RESIDUAL MODES; SIMULATION=STEADY STATE
## Abaqus to LS-DYNA Conversion
Abaqus to LS-DYNA conversion helps you migrate models between solvers for different types of analysis. It avoids rebuilding the model from scratch and saves time and effort.
The following example shows the translation of Abaqus INP file to K file format:
1. Import the Abaqus INP file.
> ```python
> fileio = prime.FileIO(model=model)
> import_results = fileio.import_abaqus_inp(
> r"E:\test3\spot_weld_test.inp",
> prime.ImportAbaqusParams(model),
> )
>
> ```
> The import\_abaqus\_inp imports the INP file as mesh, extracts simulation specific information from the INP file and stores the information internally as a JSON document. [`ImportAbaqusParams`](../api/_autosummary/ansys.meshing.prime.ImportAbaqusParams.md#ansys.meshing.prime.ImportAbaqusParams) allows you to set the parameters for importing the model. The example uses default parameters for importing the model.
> **Output**
>
> ```pycon
> summary_log : {"Counts": {"connector": 4,"element": 1420,"elsets": 5,"errors": 0,"node": 1708,"nsets": 19,
> "shell": 1416,"skipped": 0,"translated": 47,"warnings": 0},"Ids": {"connector": {"max": 900004,"min": 900001},
> "element": {"max": 900004,"min": 19},"node": {"max": 300424,"min": 47},"shell": {"max": 14186,"min": 19}},
> "Keywords": {"Counts": {"total_keywords_found": 65,"total_keywords_processed": 65,"total_keywords_skipped": 0,
> "total_keywords_unprocessed": 0},"processed_keywords": {"AMPLITUDE": 1,"BOUNDARY": 2,"CONNECTOR BEHAVIOR": 1,
> "CONNECTOR ELASTICITY": 6,"CONNECTOR SECTION": 1,"DENSITY": 2,"DYNAMIC": 1,"ELASTIC": 2,"ELEMENT": 3,
> "ELEMENT OUTPUT": 1,"ELSET": 5,"END STEP": 1,"ENERGY OUTPUT": 1,"FASTENER": 1,"FASTENER PROPERTY": 1,
> "FIXED MASS SCALING": 1,"HEADING": 1,"MATERIAL": 2,"NODE": 1,"NODE OUTPUT": 1,"NSET": 19,"ORIENTATION": 1,
> "OUTPUT": 2,"PLASTIC": 2,"SHELL SECTION": 2,"STEP": 1,"SURFACE": 2,"VARIABLE MASS SCALING": 1},
> "skipped_keywords": null,"unprocessed_keywords": null}}
> formatted_summary_log : None
> error_code : 0
> warning_codes : []
>
> ```
> Here, the import summary provides information on the following:
>
>
> - Total number of keywords in the imported file.
> - Total number of processed keywords.
> - Total number of skipped or unprocessed keywords.
> - Number of imported nodes.
> - Number of imported elements (solid, shell, beam and more).
> - Number and type of skipped elements.
> - Ids of imported nodes and elements.
> - Number of errors and warnings that occurred while importing the file.
2. Export the K file.
> ```python
> main_k_file = os.path.join(file_name.split(".")[0] + ".k")
> k_params = prime.ExportLSDynaKeywordFileParams(model=model)
> export_K_result = prime.FileIO(model).export_lsdyna_keyword_file(main_k_file, k_params)
> print(export_K_result)
>
> ```
[`FileIO.export_lsdyna_keyword_file`](../api/_autosummary/ansys.meshing.prime.FileIO.export_lsdyna_keyword_file.md#ansys.meshing.prime.FileIO.export_lsdyna_keyword_file) allows you to write out an LS-DYNA Keyword (\*.k) file that contains the mesh definition and other necessary information to carry out the analysis run using the LS-DYNA solver.
[`ExportLSDynaKeywordFileParams`](../api/_autosummary/ansys.meshing.prime.FileIO.export_lsdyna_keyword_file.md#ansys.meshing.prime.FileIO.export_lsdyna_keyword_file) allows you to specify the application type (SEATBELT, DOORSLAM), indicate whether to compute the spot weld thickness, append the material cards in the K file, provide the database cards to append in the K file, and specify the LS-DYNA data field format. You should specify the material properties card and the database keywords card in LS-DYNA format.
**Output**
> ```pycon
> summary_log : {"Counts": {"errors": 0,"skipped": 0,"translated": 16,"warnings": 0},
> "Ids": {"beam": {"max": 0},"csys": {"max": 1},"element": {"max": 900004},"friction": {"max": 0},
> "hour_glass": {"max": 6},"joint": {"max": 0},"load_curve": {"max": 4},"material": {"max": 67},
> "node": {"max": 300425},"part": {"max": 68},"section": {"max": 67},"set": {"max": 17},
> "shell": {"max": 14186},"solid": {"max": 0}},"Settings": {"analysis_type": "LSDynaAnalysisType_Doorslam",
> "compute_spotweld_thickness": "true","output_format": "LSDynaFormat_i10"}}
> zone_mesh_results : []
> error_code : 0
> warning_codes : []
>
> ```
> Export summary provides information about:
> > - Number of error and warnings that occurred while exporting the K file.
> > - Maximum number of node ids and elements ids that are exported.