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 nonunique 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.
Parameters and Parameter Expressions
In the translation of the LS-DYNA keyword
*PARAMETER, the value of the parameter is
used directly in the Abaqus input. For example, consider the following
LS-DYNA
input: *PARAMETER
R YM_STEEL 3.000E+07
*MAT_ELASTIC
3 7.000E-04 &YM_STEEL 3.000E-01The translated Abaqus input
is: MATERIAL, NAME=M3;MAT_ELASTIC
DENSITY
7.0000E-04
ELASTIC
3.000000E+07, 0.3
The LS-DYNA keyword
*PARAMETER_EXPRESSION is translated
similarly. In this case, the translator supports a new parameter defined by an
expression limited to two entities (either a parameter or a constant) and one
arithmetic operation: +, –, *, or /. For example: *PARAMETER
R YM_STEEL 3.000E+07
*PARAMETER_EXPRESSION
R YM_METAL YM_STEEL*1.25
Additional Information
The LS-DYNA keyword
*PART_CONTACT listed in Table 2 is always used in conjunction with the contact
keywords listed in Table 12. The translation of the contact keywords
results in CONTACT and CONTACT INCLUSIONS in
the Abaqus input, and these contact keywords are not listed in Table 2.
Summary of LS-DYNA Entities Translated
The translator from LS-DYNA to
Abaqus
supports the mappings shown in the tables below.
Table 1. Material data.
| LS-DYNA Keyword
|
Abaqus
Equivalent
|
| *MAT_ANISOTROPIC_VISCOPLASTIC
|
ELASTIC |
| PLASTIC |
| RATE DEPENDENT |
| *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_FABRIC
|
FABRIC
|
| UNIAXIAL
|
| LOADING DATA |
| *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_NONLINEAR_ELASTIC_DISCRETE_BEAM
|
CONNECTOR ELASTICITY
and CONNECTOR DAMPING
|
| *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_GENERAL_NONLINEAR
|
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 . |
Table 5. Nodal data.
| LS-DYNA Keyword
|
Abaqus
Equivalent
|
| *NODE
|
NODE
|
Table 6. Output options data.
| 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_HISTORY_BEAM
|
OUTPUT, HISTORY and
ENERGY OUTPUT
|
| *DATABASE_HISTORY_BEAM_ID
|
| *DATABASE_HISTORY_BEAM_SET
|
| *DATABASE_HISTORY_DISCRETE
|
OUTPUT,
HISTORY and ENERGY OUTPUT
|
| *DATABASE_HISTORY_DISCRETE_ID
|
| *DATABASE_HISTORY_DISCRETE_SET
|
| *DATABASE_HISTORY_NODE
|
OUTPUT,
HISTORY
|
| *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
|
| *DATABASE_HISTORY_TSHELL
|
OUTPUT,
HISTORY and ENERGY OUTPUT
|
| *DATABASE_HISTORY_TSHELL_ID
|
| *DATABASE_HISTORY_TSHELL_SET
|
| *DATABASE_NODOUT
|
OUTPUT,
FIELD and NODE OUTPUT
|
Table 7. Element data.
| 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_SEATBELT_ACCELEROMETER
|
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
|
Table 8. Prescribed conditions data.
| LS-DYNA Keyword
|
Abaqus
Equivalent
|
| *BOUNDARY_PRESCRIBED_MOTION_NODE
|
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_PRESCRIBED_MOTION_SET
|
BOUNDARY,
TYPE=DISPLACEMENT,
VELOCITY, or
ACCELERATION
|
| *BOUNDARY_SPC_NODE
|
BOUNDARY
|
| *BOUNDARY_SPC_SET
|
BOUNDARY
|
| *INITIAL_VELOCITY
|
INITIAL CONDITIONS,
TYPE=VELOCITY
|
| *INITIAL_VELOCITY_GENERATION
|
INITIAL CONDITIONS,
TYPE=ROTATING VELOCITY
|
| *INITIAL_VELOCITY_NODE
|
INITIAL CONDITIONS,
TYPE=VELOCITY
|
Table 9. Miscellaneous constraints data.
| LS-DYNA Keyword
|
Abaqus
Equivalent
|
| *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_SPHERICAL_LOCAL
|
ELEMENT,
TYPE=CONN3D2
|
| *CONSTRAINED_JOINT_STIFFNESS_GENERALIZED
|
ELEMENT, TYPE=CONN3D2
|
| CONNECTOR SECTION, BEHAVIOR
|
| *CONSTRAINED_JOINT_STIFFNESS_TRANSLATIONAL
|
ELEMENT,
TYPE=CONN3D2
|
| CONNECTOR SECTION,
BEHAVIOR
|
| *CONSTRAINED_JOINT_TRANSLATIONAL
|
ELEMENT, TYPE=CONN3D2
|
| *CONSTRAINED_JOINT_UNIVERSAL
|
ELEMENT, TYPE=CONN3D2
|
| *CONSTRAINED_NODAL_RIGID_BODY
|
RIGID BODY
with TIE NSET for
the case of no release of displacements or rotations |
| COUPLING
and KINEMATIC
for the case with release of displacements or rotations |
| *CONSTRAINED_NODE_SET
|
EQUATION
|
| *CONSTRAINED_RIGID_BODIES
|
Merged element set used in the
definition of
RIGID BODY
|
| *CONSTRAINED_SPOTWELD
|
MPC type BEAM
|
Table 10. Load data.
| 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
|
Table 11. 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
|
Table 13. Miscellaneous data.
| LS-DYNA Keyword
|
Abaqus
Equivalent
|
| *CONTROL_BULK_VISCOSITY
|
BULK VISCOSITY |
| *CONTROL_TERMINATION
|
Time period entered in
DYNAMIC, EXPLICIT
|
| *END STEP
|
END STEP
|
| *INCLUDE
|
Process multiple
LS-DYNA files |
| *KEYWORD
|
None |
| *TITLE
|
HEADING
|
Command Summary
abaqus
fromdyna jobjob-name
inputdyna-input-file
splitFile{OFFON}
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
|