Translating LS-DYNA Data Files to Abaqus Input Files

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.

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.

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.

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-01

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

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.