Export a Model to the Autodesk Nastran Editor

Using a new command in the Application menu (Export Autodesk Nastran Editor), you can transfer supported models from Simulation Mechanical 2015 R1 directly into the Nastran Editor. You can use this export function when the following conditions are satisfied:

• The analysis type must be one of the seven types listed in the Additional Autodesk Nastran Solvers page.
• Mesh and setup the model so that it is ready to solve. Define the element types, element definitions, materials, loads, constraints, contact options, and analysis parameters.
• Do not include element types or material models that are unsupported for models exported to Nastran. Refer to the Nastran page of the FEA Model Import and Export Functionality documentation for the legacy Nastran support capabilities. Also, refer to the Additional Material Models page of this addendum for the latest additions to the material export capabilities.

Important: When exporting a nonlinear structural analysis model to the Nastran Editor, multiple event intervals with differing capture rates are not supported. Also, custom load curves are not supported. Only the specified Number of time steps is used from the Event tab of the Analysis Parameters dialog box. So you can change the number of requested steps. The default load curve is always used for transferred models. The load multiplier ramps up from 0 to 1 in 1 time unit.

Notes:

• When exporting a solid model to the Nastran Editor, each pyramid elements is automatically split into a pair of tetrahedra. The Nastran Editor does not support pyramid (5-node) solid elements. This pyramid-splitting operation differs from the behavior of the Export Third-Party FEA Nastran function, which retains pyramid elements.
• The Output results of all time steps option in the Output tab of the Analysis Parameters dialog box is supported for nonlinear models exported to the Nastran Editor. This option is mapped to an equivalent Nastran Editor option.
• The Nastran Stress/Strain option in the Output tab is also supported for nonlinear analyses.
• For DDAM analyses, there is no Nastran Stress/Strain option in the analysis parameters. When exporting a DDAM model to the Nastran Editor, stress output is assumed by default, and the appropriate card is included in the exported Nastran deck. If you wish to output strain instead of stress, manually edit the exported deck within the Nastran Editor. In addition, when exporting a DDAM model to the Nastran Editor, only declassified DDAM codes are exported. When necessary, change the DDAM codes within the Nastran Editor after the model is transferred.

Procedure

1. After satisfying the requirements detailed above, click Application Menu Export Autodesk Nastran Editor.
2. Specify a name for the Nastran file. If you do not include an extension, the .nas filename extension is applied by default. The file location is in the same folder as the Simulation Mechanical model, but you can browse to a different folder if desired.
3. Click Save and the model will be solid meshed (if required), checked, and will appear within the Autodesk Nastran Editor.
4. You may wish to adjust the model setup or adjust advanced, Nastran-specific options.
   Caution: If you wish to merge the model results into the original Simulation Mechanical model after running the solution in the Nastran Editor, do not change the model geometry. Make no changes that affect the element count, node numbering, or nodal coordinates. (See the Display Nastran Editor Results in Simulation Mechanical page for more information.)
5. If you wish to review the simulation results within the Nastran Editor, perform the following change:
   • Expand the Output Control Directives group in the browser.
   • Use the RSLTFILETYPE drop-down box to select the FEMAPBINARY option.

   Alternatively, if you wish to merge the Nastran Editor results into the original Simulation Mechanical model and do your post-processing there, then keep the default NASTRANBINARY option.

   Note: Use the FEMAPBINARY setting for all exported DDAM analyses. Nastran DDAM results cannot be merged back into the original Simulation Mechanical model, so you must evaluate the results within the Nastran Editor.
6. Click Analysis Run, or press the F5 key to run the analysis.

For more information, consult the Autodesk Nastran Editor Help.