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:

  1. 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.

  1. 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

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.

    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.

  2. 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.