Exporting Meshes to Nastran

You can export meshes from a finite element model to a Nastran bulk data file (.nas).

Before you begin:
  • You must have the appropriate role to export meshes to Nastran.
  • Switch to Model or Mesh ; FEM export is not available from Scenario .
  • From the standard area of the action bar, select Update to update the FEM. The FEM must be up-to-date.
See Also
Importing Nastran Meshes
  1. From the top bar, select Share > Export > Export FEM.
    The Export FEM dialog box appears.
  2. Select .
    The Save As dialog box appears.
  3. Browse to the location where you want to save the bulk data file.

    Note: The folder name cannot contain Unicode characters, such as accents and other diacritical marks.

  4. Enter a name in the File name field, or select an existing file to overwrite that file.

    Change the Save as type to include the proper file extension.

    Note: You can also type the extension as part of the File name.

  5. Select Save.
    The Export FEM dialog box displays the selected path and file name.
  6. Optional: Toggle on Create a log file, select , and select a location to save a log file of the export operation.

    The log file is saved using the same name as the export file and a .log extension. The file contains information about the exported mesh data. The log file might be empty if no potential issues occur during export, or it might contain warnings and errors from the export process.

  7. Expand Units to change units for length, mass, time, temperature, amount of substance, and angle.
  8. Expand Granularity to select a subset of features to export. You can select one or more of the following options:
    OptionDescription
    Group Nastran groups are used primarily as postprocessing filters. Nastran does not distinguish element sets from node sets, but the exported file contains comments specifying the exported group types. Only node and element groups are supported. Edge and face groups are not supported.
    Materials Nastran does not use material names. The exported file contains comments specifying the exported material types.
    Properties Nastran cannot embed a property name. The exported file contains comments specifying what property name is being exported.
    Special elements Element connectivity and element specifications are exported according to hard-coded translation from special elements to Nastran element cards.
  9. Expand Options to select a subset of options that configure individual 3DEXPERIENCE-to-Nastran mappings. You can select one or more of the following options:
    OptionDescription
    OP2/XDB generation Instructs Nastran to generate files consisting of input model data and output results data.
    • PARAM,POST,-2 $ general OP2 (default): Writes PARAM, POST, -2 to the exported Nastran file. This instruction generates an OP2 results and model data file with additional and alternative datablocks used by other postprocessors.
    • PARAM,POST,-1 $ original OP2: Writes PARAM, POST, -1 to the exported Nastran file. This instruction generates an OP2 results and model data file with fundamental Nastran default datablocks.
    • PARAM,POST,0 $ XDB: Writes PARAM, POST, 0 to the exported Nastran file. This instruction generates an interactive XDB results and model data file for attached Nastran postprocessing (not imported).
    • PARAM,POST,1 $ implicit OP2: Writes PARAM, POST, 1 to the exported Nastran file. This instruction generates an OP2 results and model data file with datablocks updated for Nastran SOL 400.
    • Not Enabled: Disables OP2 generation.

    For more information, see Parameter POST in the Nastran quick-reference guides for more details on the differences between these postprocessing options.
    Force the beam properties to export with CBEAM and PBEAM
    • NO (default): Exports beam properties into a mix of BAR and BEAM data cards based on whether the beam property is applied on Euler-Bernoulli or Timoshenko beam elements in Abaqus.
      • For Euler-Bernoulli beam elements, beam properties are exported as PBEAM/PBEAML (taper beams) and PBAR/PBARL (all other cases). For PBEAM, the shear factor fields, K1 and K2, are set to 0.0. For PBAR, the shear factor fields, K1 and K2, are set blank so that the transverse shear flexibility is set to zero.
      • For Timoshenko beam elements, beam properties are exported as PBAR/PBARL (polar symmetric profiles, bi-symmetric profiles, and general profiles with I12=0) and PBEAM/PBEAML (all other cases). For PBAR and PBEAM, the shear factors, K1 and K2, are computed from the Abaqus transverse shear values, K13 and K23. If the computed K1 and K2 values are ≥1000, the corresponding field is left blank for PBAR and set to 0.0 for PBEAM.
    • YES: Exports beam properties into CBEAM and PBEAM/PBEAML data cards only.
    Nastran card used for the axial spring
    • CELAS1/PELAS (default): Exports axial connectors and springs into CELAS1 elements and PELAS properties.
    • CELAS2: Exports axial connectors and springs into elements without reference to a property entry.
    Nastran card used for the composite
    • PCOMP (default): Exports the composite properties into PCOMP.
    • PCOMPG: Exports the composite properties into PCOMPG.
    Failure theory for the composite
    • Blank (default): Indicates Nastran does not perform a composite failure calculation. This option is available when you select PCOMP or PCOMPG as the Nastran card used for the composite.
    • Hill: Sets the Hill theory for the FT field in PCOMP or PCOMPG.
    • Hoffman: Sets the Hoffman theory for the FT field in PCOMP or PCOMPG.
    • Tsai-Wu: Sets the Tsai-Wu theory for the FT field in PCOMP or PCOMPG.
    • Maximum Strain: Sets the Maximum Strain theory for the FT field in PCOMP or PCOMG.
    Stress or strain output request for individual plies
    • NO (default): Sets the stress/strain output request field for all the plies in all the PCOMP/PCOMPG data cards to NO. This option yields total stress and strain for the composite element rather than for individual plies. If you select this option and the general output requests contain stress and strain output requests for elements, the app writes PARAM, NOCOMPS, -1 to the exported file.
    • YES: Sets the stress/strain output request field for all the plies in all the PCOMP/PCOMPG cards to YES. This option yields the stress and strain for individual plies.
    Tension and compression allowable type Instructs Nastran to populate the allowable failure stress or strain fields in the MAT8 bulk data entry as either STRESS (default) or STRAIN. The entries determine the composite failure index by Nastran.
    Nastran card used for the truss element
    • CROD/PROD (default): Exports the truss section in Abaqus into a CROD element and an associated PROD property in Nastran.
    • CONROD: Exports the truss section in Abaqus to a CONROD entry in Nastran.
    Nastran card used for the beam connector
    • CBUSH/PBUSH (default): Exports the beam connector features to CBUSH/PBUSH data cards. When you export to CBUSH/PBUSH data cards, you can specify the Translational stiffness and Rotational stiffness of the beam connector features. The default calculated stiffness values are 50 times the highest modulus found between all materials in the model.
    • RBE2: Exports the beam connector features to RBE2 data cards if at least one node is independent. If all nodes of a beam connector feature are dependent, the 3DEXPERIENCE platform exports this feature to a CBUSH/PUSH data card with the default stiffness values.
  10. Click Export.
    The Export FEM dialog box is closed, the meshes are exported into the selected file, and the report is displayed.
  11. Optional: In the Export Report dialog box, expand the Execution section to details of the export operation.

    If desired, click Save to save a copy of the report.

The 3DEXPERIENCE platform exports all element types in the Mesh Creation app.