### 2.2.4. Pull-Down Menu - Import - Nastran

Import Options

After browsing a NASTRAN input file, select import options in this dialog.

Convert Properties to Autodyn parts

  Names the imported parts from definitions within the NASTRAN file. Otherwise, generic names are automatically generated for the parts.

Merge duplicate materials

  Merges duplicate materials.

Check shell orientation is consistent

  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.

Input File Format

Autodyn can import MSC.NASTRAN™ input files in both free and fixed format. In free format, the entries can appear anywhere on the line and are separated by commas. With fixed format, a field must be located in a set part of the line. The fixed format field can be small (8 characters) or large (16 characters).

In addition to the MSC.NASTRAN™ bulk data input, Autodyn can recognize the expanded input data set for explicit transient dynamics, as given by MSC.DYTRAN™ version 4.7.

The primary use of the MSC.NASTRAN™ 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, which can be imported into Autodyn from an MSC.NASTRAN™ bulk data 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 e.g. volume elements, shell elements and beam elements. A component is a collection of all connected elements regardless of their topology.

Materials

Each element, imported from the bulk data file will have the material name as defined on the property field for the element (PSOLID, PSHELL). 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

Every element property is translated into an Initial Condition in Autodyn and allocated to the appropriate elements.

Fixed and prescribed boundary conditions are imported from the bulk data 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 bulk data file are read into Autodyn and converted into Initial Conditions. The initial condition is also automatically applied to the identified nodes.

Bulk Data Compatibility

The current capabilities of the Autodyn import capability for MSC.NASTRAN™ bulk data files is summarized below:

Keyword | Compatibility
--- | ---
BEGIN BULKDATA | Full
CBAR | Only grid numbers to define local x-y plane
CBEAM | Only grid numbers to define local x-y plane
CHEXA | Full
CPENTA | Full
CQUAD4 | No material direction
CTETRA | Full
CTRIA3 | No material direction
JOIN | Full
FORCE | Full
GRID | No coordinate system; no SPC
PBAR | Full
PBEAM | Only constant cross-section
PBEAM1 | Only as PBEAM
PCOMP | Full
PLOAD | Full
PSHELL | No thickness
PSHELL1 | Up to field 7
PSOLID | Full
SET1 | Full 1
SPC | Full
SPC1 | No ranges
TABLED1 | Full
TLOAD1 | Only FORCE

Any keyword not mentioned in the table above will be ignored.

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