Solver translation

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:

Import the Abaqus INP file.

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 allows you to set the parameters for importing the model. The example uses default parameters for importing the model.

Output:

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.

Export the CDB file.

export_cdb_result = file_io.export_mapdl_cdb(
    r"E:\test3\Abaqus_Input_multistep.cdb",
    prime.ExportMapdlCdbParams(model),
)
print(export_cdb_result)

ExportMapdlCdbParams allows setting parameters to control the export of MAPDL CDB files.

ExportMapdlCdbResults contains the summary result of the export process in json format. This writes the CDB file to the specified location.

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

HEADING None

NODE SYSTEM=R

ELEMENT TYPE=B31, C3D10, C3D4, C3D6, C3D6H, C3D8, C3D8H, C3D8R, C3D8RH, COH3D6, COH3D8, CONN3D2, DCOUP3D, M3D3, M3D4, MASS, R3D3, R3D4, ROTARYI, S3, S3R, S4, S4R, SPRINGA, STRI65

KINEMATIC COUPLING None

MPC None

ORIENTATION DEFINITION=COORDINATES, NODES; SYSTEM=RECTANGULAR

SOLID SECTION None

SHELL SECTION DENSITY=0; NODAL THICKNESS; OFFSET

COHESIVE SECTION RESPONSE=CONTINUUM, TRACTION SEPARATION; THICKNESS=SPECIFIED

BEAM SECTION SECTION=CIRC, PIPE

CONNECTOR SECTION [CARTESIAN–CARDAN], [AXIAL], [CARTESIAN–ROTATION], [WELD], [CARTESIAN–EULER], [JOIN–REVOLUTE], [SLOT–ALIGN]

NSET None

ELSET GENERATE

SURFACE TYPE=ELEMENT, NODE

MATERIAL None

DENSITY None

DAMPING STRUCTURAL=0

ELASTIC TYPE=ISOTROPIC, TRACTION

CONNECTOR BEHAVIOR None

CONNECTOR ELASTICITY NONLINEAR, RIGID

CONNECTOR DAMPING NONLINEAR; TYPE=VISCOUS

SPRING None

MASS None

ROTARY INERTIA None

SECTION CONTROLS ELEMENT DELETION=YES; HOURGLASS=ENHANCED

FASTENER PROPERTY None

NONSTRUCTURAL MASS DISTRIBUTION=MASS PROPORTIONAL; UNITS=TOTAL MASS

TIE ADJUST=NO, YES

FASTENER ADJUST ORIENTATION=NO

AMPLITUDE DEFINITION=EQUALLY SPACED, PERIODIC, TABULAR, periodic; FIXED INTERVAL=0,3; SMOOTH=0; TIME=STEP TIME, step time

RIGID BODY None

STEP NLGEOM=NO, YES; PERTURBATION; UNSYMM=YES

STATIC STABILIZE=0

BOUNDARY BASE NAME=LOAD_FR, LOAD_RR; OP=NEW; TYPE=DISPLACEMENT

CLOAD FOLLOWER; LOADCASE=1; OP=NEW; REAL

DLOAD OP=NEW

OUTPUT FIELD, HISTORY, TIME INTERVAL=0

NODE OUTPUT None

END STEP None

DYNAMIC APPLICATION=MODERATE DISSIPATION, QUASI

ELEMENT OUTPUT POSITION=CENTROIDAL

SYSTEM None

TRANSFORM TYPE=R

PLASTIC None

HYPERELASTIC MODULI=LONG TERM; N=3; NEO HOOKE; REDUCED POLYNOMIAL; YEOH

SURFACE INTERACTION None

FRICTION SLIP TOLERANCE=0

CONTACT PAIR ADJUST=0; SMALL SLIDING; SMOOTH=0; TYPE=NODE TO SURFACE, SURFACE TO SURFACE

MONITOR DOF=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, node

NODE PRINT None

MEMBRANE SECTION None

TIME POINT None

CONTACT None

CONTACT INCLUSIONS ALL EXTERIOR

CONTACT EXCLUSIONS None

CONTACT PROPERTY ASSIGNMENT None

DAMAGE INITIATION CRITERION=DUCTILE

DAMAGE EVOLUTION TYPE=DISPLACEMENT

FREQUENCY DAMPING PROJECTION=ON; EIGENSOLVER=AMS; NORMALIZATION=MASS; RESIDUAL MODES; SIMULATION=STEADY STATE

Keyword	Options
HEADING	None
NODE	SYSTEM=R
ELEMENT	TYPE=B31, C3D10, C3D4, C3D6, C3D6H, C3D8, C3D8H, C3D8R, C3D8RH, COH3D6, COH3D8, CONN3D2, DCOUP3D, M3D3, M3D4, MASS, R3D3, R3D4, ROTARYI, S3, S3R, S4, S4R, SPRINGA, STRI65
KINEMATIC COUPLING	None
MPC	None
ORIENTATION	DEFINITION=COORDINATES, NODES; SYSTEM=RECTANGULAR
SOLID SECTION	None
SHELL SECTION	DENSITY=0; NODAL THICKNESS; OFFSET
COHESIVE SECTION	RESPONSE=CONTINUUM, TRACTION SEPARATION; THICKNESS=SPECIFIED
BEAM SECTION	SECTION=CIRC, PIPE
CONNECTOR SECTION	[CARTESIAN–CARDAN], [AXIAL], [CARTESIAN–ROTATION], [WELD], [CARTESIAN–EULER], [JOIN–REVOLUTE], [SLOT–ALIGN]
NSET	None
ELSET	GENERATE
SURFACE	TYPE=ELEMENT, NODE
MATERIAL	None
DENSITY	None
DAMPING	STRUCTURAL=0
ELASTIC	TYPE=ISOTROPIC, TRACTION
CONNECTOR BEHAVIOR	None
CONNECTOR ELASTICITY	NONLINEAR, RIGID
CONNECTOR DAMPING	NONLINEAR; TYPE=VISCOUS
SPRING	None
MASS	None
ROTARY INERTIA	None
SECTION CONTROLS	ELEMENT DELETION=YES; HOURGLASS=ENHANCED
FASTENER PROPERTY	None
NONSTRUCTURAL MASS	DISTRIBUTION=MASS PROPORTIONAL; UNITS=TOTAL MASS
TIE	ADJUST=NO, YES
FASTENER	ADJUST ORIENTATION=NO
AMPLITUDE	DEFINITION=EQUALLY SPACED, PERIODIC, TABULAR, periodic; FIXED INTERVAL=0,3; SMOOTH=0; TIME=STEP TIME, step time
RIGID BODY	None
STEP	NLGEOM=NO, YES; PERTURBATION; UNSYMM=YES
STATIC	STABILIZE=0
BOUNDARY	BASE NAME=LOAD_FR, LOAD_RR; OP=NEW; TYPE=DISPLACEMENT
CLOAD	FOLLOWER; LOADCASE=1; OP=NEW; REAL
DLOAD	OP=NEW
OUTPUT	FIELD, HISTORY, TIME INTERVAL=0
NODE OUTPUT	None
END STEP	None
DYNAMIC	APPLICATION=MODERATE DISSIPATION, QUASI
ELEMENT OUTPUT	POSITION=CENTROIDAL
SYSTEM	None
TRANSFORM	TYPE=R
PLASTIC	None
HYPERELASTIC	MODULI=LONG TERM; N=3; NEO HOOKE; REDUCED POLYNOMIAL; YEOH
SURFACE INTERACTION	None
FRICTION	SLIP TOLERANCE=0
CONTACT PAIR	ADJUST=0; SMALL SLIDING; SMOOTH=0; TYPE=NODE TO SURFACE, SURFACE TO SURFACE
MONITOR	DOF=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, node
NODE PRINT	None
MEMBRANE SECTION	None
TIME POINT	None
CONTACT	None
CONTACT INCLUSIONS	ALL EXTERIOR
CONTACT EXCLUSIONS	None
CONTACT PROPERTY ASSIGNMENT	None
DAMAGE INITIATION	CRITERION=DUCTILE
DAMAGE EVOLUTION	TYPE=DISPLACEMENT
FREQUENCY	DAMPING 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:

Import the Abaqus INP file.

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 allows you to set the parameters for importing the model. The example uses default parameters for importing the model.

Output

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.

Export the K file.

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 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 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

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.

Prime Mesh Python client library 2026 R1 SP01

Abaqus to Ansys MAPDL Conversion

Supported Abaqus Keywords

Abaqus to LS-DYNA Conversion

Connect with Ansys