### 2.2.3. Pull-Down Menu - Import - LS-DYNA

Import Options

After browsing for an LS-DYNA keyword file, select import options in this dialog.

Retain LS-DYNA part definitions

  Names the important parts from definitions within the LS-DYNA file. Otherwise, generic names are automatically generated for the parts.

Merge duplicate materials

  Merges duplicate materials

Check shell orientation

  Checks for inconsistent or non-manifold shell meshes. If the mesh is inconsistent and manifold, you should re-orient the mesh to have consistent normals.

LS-DYNA Keyword File Format

Both formatted and free formatted (comma delimited) LS-DYNA keyword files can be imported into Autodyn. The standard used is based on version 970 of LS-DYNA.

The primary use of the LS-DYNA reader is to allow you to define a mesh to be used with the unstructured solvers. In addition, other information regarding material definitions, boundary conditions and initial conditions can be imported and stored in Autodyn.

An overview of the information that can be imported into Autodyn from an LS-DYNA keyword file is given below.

Mesh

  The mesh, represented as nodal positions and element connectivity, is read into Autodyn and sorted to produce Parts and Components. A Part is a collection of connected elements of the same classification (for example, volume elements, shell elements and beam elements). A Component is a collection of all connected elements regardless of their topology. By default, the defined Parts in Autodyn will not necessarily be equivalent to those defined in the LS-DYNA keyword file.

  An option to retain the Part definitions in the LS-DYNA file is also available.

Materials

  Each element defined in the keyword file will have an associated material definition. Corresponding materials will be automatically generated during the import of the keyword file into Autodyn. In general (except for the materials identified below), the actual material parameters will not be read into Autodyn and you should ensure that all materials are properly defined after the import.

  At present, a subset of the material definitions and parameters are automatically read into Autodyn. These include materials of type rigid, elastic, piecewise linear plasticity and spring elastic material models.

Initial and Boundary Conditions

  Fixed and prescribed boundary conditions are imported from the LS-DYNA keyword file into Autodyn. These are converted into the equivalent Autodyn boundary conditions including parameters, where possible.

  Initial velocities defined on nodes and sets of nodes in the keyword file are read into Autodyn and converted into Initial Conditions. The initial condition is also automatically applied to the identified nodes.

Shell and Beam Sections

  Shell sections defined in the keyword file are automatically transformed into Autodyn initial conditions. The local direction for layered shells is not currently translated.

  Beam cross-sections and directions are read from the keyword file and these and the relevant data are converted to be compatible with beam types used in Autodyn.

Keyword Compatibility

The current capabilities of the Autodyn import capability for LS-DYNA (.k) keyword files is summarized below:

Keyword | Compatibility
--- | ---
*BOUNDARY_SPC_NODE | Translational velocities only. DORFX, DORFY, DORFZ not recognized
*BOUNDARY_SPC_SET | Translational velocities only. DORFX, DORFY, DORFZ not recognized
*DEFINE_CURVE | Full
*ELEMENT_SOLID | Full
*ELEMENT_SHELL | Full
*ELEMENT_BEAM | Full
*INITIAL_VELOCITY | BOXID and IRIGID are not recognized
*INITIAL_VELOCITY_NODE | Translational velocities only. VXR, VYR and VZR are not recognized.
*INITIAL_VELOCITY_GENERATION | Translational velocities only. OMEGA, XC, YC, ZC, NX, NY, NZ and PHASE not recognized.
*MAT_PIECEWISE_LINEAR _PLASTICITY | Full
*MAT_ELASTIC | Full
*MAT_RIGID | Full
*MAT_SPRING_ELASTIC | Full
*NODE | Full
*PART | Full
*SECTION_BEAM | Beam types 1-5 supported. QR/IRID, SCOOR, NSM, NSLOC, NTLOC and IRR are not recognized.
*SECTION_SHELL | Shell thickness at first node is read in and set a shell thickness in initial condition.
*SET_NODE_LIST | Full
*SET_PART_LIST | Full
*SET_SHELL_LIST | Full
*SET_BEAM | Full
*SET_DISCRETE | Full
*SET_SOLID | Full
*SET_TSHELL | Full
*SET_NODE_LIST_GENERATE | Full
*SET_NODE_PART_GENERATE | Full
*SET_NODE_SHELL_GENERATE | Full
*SET_BEAM_GENERATE | Full
*SET_DISCRETE_GENERATE | Full
*SET_SOLID_GENERATE | Full
*SET_TSHELL_GENERATE | Full

Release 18.2 - © ANSYS, Inc. All rights reserved.