Translating LS-DYNA data files to Abaqus input files | ||||
|
| |||
ProductsAbaqus/Explicit
Using the translator
The translator supports translation of input files created by LS-DYNA Version 971 Rev 5 or earlier. The input file can have any name and an optional extension.
The LS-DYNA keywords that are supported are listed in the tables below. Other LS-DYNA keywords and data are skipped over and noted in the log file.
The translator creates an Abaqus input file that contains both the model data and history data. However, the translator does not create exact Abaqus equivalents for specific output quantities for nodal output, element output, and contact output; it uses preselected variables instead. You can provide additional output entities to complete the requests.
Element numbering and grouping
All elements in the generated Abaqus input file have unique element numbers. New element numbers are assigned automatically to elements with non-unique element numbers in the LS-DYNA input; all element number reassignments are noted in the log file.
Elements that are assigned the same PART identification number are grouped together in an element set. Elements that have different material or properties must be given different PART identification numbers; that is, the same material and properties must be applicable to all elements grouped in the same element set.
When a PART references a rigid material, the part is considered rigid. The element set that corresponds to the part is used in the rigid body definition.
Material models
The translator supports only the material models shown in Table 1. All unsupported material models are translated as linear elastic if a stress-strain law definition is required. In these cases the translator provides nominal values for the material properties.
Mapping LS-DYNA elements that end in _ID or _TITLE
Many LS-DYNA keywords include the options _ID, _TITLE, or both of these options. Unless the LS-DYNA keyword with _ID or _TITLE is specified in the mapping tables in this document, the translator maps data from these options to the same Abaqus keywords specified for the main LS-DYNA keyword.
Summary of LS-DYNA entities translated
The translator from LS-DYNA to Abaqus supports the mappings shown in the tables below.
| LS-DYNA Keyword | Abaqus Equivalent |
|---|---|
| *MAT_BLATZ-KO_RUBBER | HYPERELASTIC, NEO HOOKE |
| *MAT_CABLE_DISCRETE_BEAM | ELASTIC |
| *MAT_DAMPER_NONLINEAR_VISCOUS | CONNECTOR DAMPING, NONLINEAR |
| *MAT_DAMPER_VISCOUS | CONNECTOR DAMPING |
| *MAT_ELASTIC | ELASTIC |
| *MAT_ELASTIC_PLASTIC_THERMAL | ELASTIC |
| PLASTIC | |
| EXPANSION | |
| *MAT_FU_CHANG_FOAM | LOW DENSITY FOAM and UNIAXIAL TEST DATA |
| *MAT_HONEYCOMB | Built-in VUMAT user material model ABQ_HONEYCOMB1 |
| *MAT_JOHNSON_COOK | PLASTIC, HARDENING=JOHNSON COOK |
| RATE DEPENDENT, TYPE=JOHNSON COOK | |
| SHEAR FAILURE, TYPE=JOHNSON COOK | |
| TENSILE FAILURE, TYPE=JOHNSON COOK | |
| *MAT_LINEAR_ELASTIC_DISCRETE_BEAM | CONNECTOR ELASTICITY and CONNECTOR DAMPING |
| *MAT_LOW_DENSITY_FOAM | HYPERFOAM and UNIAXIAL TEST DATA |
| *MAT_NULL | ELASTIC |
| Shell elements that reference a null material are translated as surface elements | |
| *MAT_OGDEN_RUBBER | HYPERELASTIC, OGDEN |
| *MAT_PIECEWISE_LINEAR_PLASTICITY | PLASTIC |
| *MAT_PLASTIC_KINEMATIC | PLASTIC, HARDENING=KINEMATIC |
| *MAT_RIGID | ELASTIC |
| RIGID BODY (for LS-DYNA parts that refer to a rigid material) | |
| *MAT_SEATBELT | CONNECTOR ELASTICITY, NONLINEAR |
| *MAT_SPOTWELD | CONNECTOR ELASTICITY, RIGID |
| *MAT_SPRING_ELASTIC | CONNECTOR ELASTICITY |
| *MAT_SPRING_NONLINEAR_ELASTIC | CONNECTOR ELASTICITY, NONLINEAR |
| *MAT_VISCOELASTIC | VISCOELASTIC, TIME=PRONY |
| 1 For more information about using ABQ_HONEYCOMB, refer to “Abaqus/Explicit honeycomb material model,” which is available in the Dassault Systèmes Knowledge Base at http://www.3ds.com/support/knowledge-base. | |
| LS-DYNA Keyword | Abaqus Equivalent |
|---|---|
| *PART*PART_PRINT | ELSET and the corresponding type of element section |
| *PART_CONTACT | SURFACE INTERACTION properties |
| *PART_INERTIA | ELEMENT, TYPE=MASS |
| ELEMENT, TYPE=ROTARYI |
| LS-DYNA Keyword | Abaqus Equivalent |
|---|---|
| *DEFINE_COORDINATE_NODES | ORIENTATION, DEFINITION=NODES |
| *DEFINE_COORDINATE_SYSTEM | ORIENTATION, DEFINITION=COORDINATES |
| *DEFINE_COORDINATE_VECTOR | ORIENTATION, DEFINITION=COORDINATES |
| *DEFINE_CURVE | Data from a single curve used in the following keywords: |
| AMPLITUDE | |
| CONNECTOR DAMPING (nonlinear) | |
| CONNECTOR ELASTICITY (nonlinear) | |
| SURFACE BEHAVIOR | |
| UNIAXIAL TEST DATA | |
| *DEFINE_SD_ORIENTATION | ORIENTATION |
| *DEFINE_TABLE | Multi-curve data used in conjunction with PLASTIC and LOW DENSITY FOAM in which the stress-strain relationship is defined for various strain rates |
| LS-DYNA Keyword | Abaqus Equivalent |
|---|---|
| *SECTION_BEAM | Beam elements: BEAM SECTION or BEAM GENERAL SECTION |
| Truss elements: SOLID SECTION | |
| *SECTION_DISCRETE | CONNECTOR SECTION |
| *SECTION_SEATBELT | CONNECTOR SECTION |
| *SECTION_SHELL | Shell elements: SHELL SECTION |
| Membrane elements: MEMBRANE SECTION | |
| Surface elements: SURFACE SECTION | |
| *SECTION_SOLID | SOLID SECTION |
| *SECTION_TSHELL | SHELL SECTION |
| LS-DYNA Keyword | Abaqus Equivalent |
|---|---|
| *NODE | NODE |
| LS-DYNA Keyword | Abaqus Equivalent |
|---|---|
| *DATABASE_BINARY_D3PLOT | OUTPUT, FIELD and ELEMENT OUTPUT |
| *DATABASE_BINARY_D3THDT | OUTPUT, FIELD and ELEMENT OUTPUT |
| *DATABASE_DEFORC | OUTPUT, FIELD and ELEMENT OUTPUT |
| *DATABASE_ELOUT | OUTPUT, FIELD and ELEMENT OUTPUT |
| *DATABASE_NODOUT | OUTPUT, FIELD and NODE OUTPUT |
| *DATABASE_HISTORY_BEAM | OUTPUT, HISTORY and ENERGY OUTPUT |
| *DATABASE_HISTORY_BEAM_ID | |
| *DATABASE_HISTORY_BEAM_SET | |
| *DATABASE_HISTORY_NODE | OUTPUT, HISTORY and ENERGY OUTPUT |
| *DATABASE_HISTORY_NODE_ID | |
| *DATABASE_HISTORY_NODE_SET | |
| *DATABASE_HISTORY_SHELL | OUTPUT, HISTORY and ENERGY OUTPUT |
| *DATABASE_HISTORY_SHELL_ID | |
| *DATABASE_HISTORY_SHELL_SET | |
| *DATABASE_HISTORY_SOLID | OUTPUT, HISTORY and ENERGY OUTPUT |
| *DATABASE_HISTORY_SOLID_ID | |
| *DATABASE_HISTORY_SOLID_SET |
| LS-DYNA Keyword | Abaqus Equivalent |
|---|---|
| *ELEMENT_BEAM | Beam elements: ELEMENT, TYPE=B31 |
| Truss elements: ELEMENT, TYPE=T3D2 | |
| *ELEMENT_BEAM_PID | ELEMENT, TYPE=CONN3D2 and FASTENER |
| *ELEMENT_DISCRETE | ELEMENT, TYPE=CONN3D2 |
| *ELEMENT_MASS | ELEMENT, TYPE=MASS and MASS |
| *ELEMENT_SEATBELT | ELEMENT, TYPE=CONN3D2 |
| *ELEMENT_SHELL | Shell elements: ELEMENT, TYPE=S3R or S4R |
| Membrane elements: ELEMENT, TYPE=M3D3 or M3D4R | |
| Surface elements (with *MAT_NULL): ELEMENT, TYPE=SFM3D3 or SFM3D4R | |
| *ELEMENT_SOLID | ELEMENT, TYPE=C3D4, C3D6, C3D8R, or C3D10M |
| *ELEMENT_TSHELL | ELEMENT, TYPE=SC6R or SC8R |
| LS-DYNA Keyword | Abaqus Equivalent |
|---|---|
| *BOUNDARY_PRESCRIBED_MOTION_NODE | BOUNDARY, TYPE=DISPLACEMENT, VELOCITY, or ACCELERATION |
| *BOUNDARY_PRESCRIBED_MOTION_SET | BOUNDARY, TYPE=DISPLACEMENT, VELOCITY, or ACCELERATION |
| *BOUNDARY_PRESCRIBED_MOTION_RIGID | BOUNDARY for reference node of rigid body |
| *BOUNDARY_PRESCRIBED_MOTION_RIGID_LOCAL | BOUNDARY for reference node of rigid body |
| *BOUNDARY_SPC_NODE | BOUNDARY |
| *BOUNDARY_SPC_SET | BOUNDARY |
| *INITIAL_VELOCITY_GENERATION | INITIAL CONDITIONS,TYPE=ROTATING VELOCITY |
| *INITIAL_VELOCITY_NODE | INITIAL CONDITIONS,TYPE=VELOCITY |
| LS-DYNA Keyword | Abaqus Equivalent |
|---|---|
| *CONSTRAINED_NODE_SET | EQUATION |
| *CONSTRAINED_NODAL_RIGID_BODY | MPC type BEAM |
| *CONSTRAINED_EXTRA_NODES_NODE | Node set used as TIE NSET in the definition of RIGID BODY |
| *CONSTRAINED_EXTRA_NODES_SET | Node set used as TIE NSET in the definition of RIGID BODY |
| *CONSTRAINED_JOINT_CYLINDRICAL | ELEMENT, TYPE=CONN3D2 |
| *CONSTRAINED_JOINT_REVOLUTE | ELEMENT, TYPE=CONN3D2 |
| *CONSTRAINED_JOINT_SPHERICAL | ELEMENT, TYPE=CONN3D2 |
| *CONSTRAINED_JOINT_STIFFNESS_GENERALIZED | ELEMENT, TYPE=CONN3D2 |
| CONNECTOR SECTION, BEHAVIOR | |
| *CONSTRAINED_JOINT_TRANSLATIONAL | ELEMENT, TYPE=CONN3D2 |
| *CONSTRAINED_JOINT_UNIVERSAL | ELEMENT, TYPE=CONN3D2 |
| *CONSTRAINED_RIGID_BODIES | Merged element set used in the definition of RIGID BODY |
| *CONSTRAINED_SPOTWELD | MPC type BEAM |
| LS-DYNA Keyword | Abaqus Equivalent |
|---|---|
| *LOAD_BODY_PARTS | ELSET for DLOAD |
| *LOAD_BODY_X | DLOAD |
| *LOAD_BODY_Y | DLOAD |
| *LOAD_BODY_Z | DLOAD |
| *LOAD_NODE_POINT | CLOAD with node data |
| *LOAD_NODE_SET | CLOAD with node set data |
| LS-DYNA Keyword | Abaqus Equivalent |
|---|---|
| *SET_NODE_LIST | NSET with node data |
| *SET_NODE_LIST_GENERATE | NSET with node data |
| *SET_PART | ELSET with element set data |
| *SET_PART_LIST | ELSET with element set data |
| *SET_PART_LIST_GENERATE | ELSET with element set data |
| *SET_SEGMENT | ELSET with element data |
| *SET_SHELL_LIST | ELSET with element data |
| *SET_SHELL_LIST_GENERATE | ELSET with element data |
| *SET_SOLID_LIST | ELSET with element data |
Command summary
Command line options
- job
-
This option is used to specify the name of the Abaqus input file to be output by the translator. The name of the Abaqus input file must be given without the .inp extension. Diagnostics created by the translator are written to a file named job-name.log.
- input
-
This option is used to specify the name of the file containing the LS-DYNA keyword data. The LS-DYNA input file can have an extension.
- splitFile
-
This option specifies whether the Abaqus input file is to be split into multiple files. If splitFile=ON, the following files are output:
-
job-name_nodes.inc: include file that contains the nodal data
-
job-name_elements.inc: include file that contains the element data
-
job-name_model.inc: include file that contains the remaining model data
-
job-name.inp: Abaqus input file that includes all of the above include files and the history data
-