Display Nastran Editor Results in Simulation Mechanical

You can export models that originate in Simulation Mechanical to the Autodesk Nastran Editor for solving. Click here for more information. After solving a model, you can merge the Nastran Editor results into your original Simulation Mechanical model. Then, you can review the results using the full capabilities of the Simulation Mechanical Results environment. This functionality is supported for the following six analysis types:

• Static Stress with Linear Material Models
• Natural Frequency (Modal)
• Natural Frequency (Modal) with Load Stiffening
• Critical Buckling Load
• Static Stress with Nonlinear Material Models
• Steady-State Heat Transfer

Note: You can also export Dynamic Design Analysis Method (DDAM) models from Simulation Mechanical to the Nastran Editor. However, merging DDAM results into the original Simulation Mechanical model is not currently supported. Use the Nastran Editor to evaluate the results of DDAM analyses that you choose to run within the Nastran Editor. You can also set up, run, and post-process DDAM analyses entirely within Simulation Mechanical using the native SimMech processor.

Caution: Results for composite elements are generated differently between Nastran and Simulation Mechanical. The Nastran Editor calculates results at the middle of elements. Simulation Mechanical calculates results at the element corners. During results translation, the element-middle Nastran results are replicated at the element corners, introducing some error. For the greatest accuracy, models containing composite elements that are solved in the Nastran Editor should also be post-processed in the Nastran Editor.

Procedure

After a model has been solved successfully within the Nastran Editor, perform the following steps to review the results within Simulation Mechanical:

1. Return to the Simulation Mechanical user interface. If you have closed the original model, reopen it now.
2. From the FEA Editor, click Application Menu Merge.
3. Choose the Nastran results (*.fno, *.op2) option from the Files of type drop-down menu.
4. Navigate to the model folder and select the appropriate *.fno or *.op2 file.
5. Click Open to merge the results into the current Simulation Mechanical model.
6. Go to the Results environment. The Nastran solution results should be available for viewing.

Important: You, the analyst, are responsible for ensuring that the appropriate results are merged into your Simulation Mechanical model. Otherwise, errors will occur and you will corrupt the active Simulation Mechanical design scenario:

• Ensure that the correct *.fno or *.op2 file is merged. The file must result from running a Nastran deck that you previously exported from the currently loaded Simulation Mechanical model.
• Do not modify the node or element geometry of the model within the Nastran Editor after exporting it from Simulation Mechanical.
• Ensure that the analysis type matches between the currently loaded Simulation Mechanical design scenario and the incoming Nastran *.fno or *.op2 file.

Note: Simulation Mechanical expects merged results in the *.fno or *.op2 file to have the following characteristics:

• Volume (solid) element results are in the global coordinate system.
• Results for all other elements (planer, 2D, and line type) are in the element local coordinate system.

When a model is exported from Simulation Mechanical to the Nastran Editor, the necessary directive cards are added to the Nastran deck automatically. Appropriate comments accompany these directive cards. Do not modify or delete these directives if you plan on merging the results into the original Simulation Mechanical model.

Merged File Format Considerations (*.fno versus *.op2)

Generally, *.fno files produce more accurately translated results, and they are preferred for this reason. For example, avoid merging *.op2 files in the following situations. (These limitations do not apply to merged *.fno results):

• When shell elements are present: The translated *.op2 results do not account for shell element orientation differences between Nastran and Simulation Mechanical. ¹
• When plate elements are present: For translated *.op2 results, the coordinate systems upon which plate result calculations are based do not always agree between Nastran and Simulation Mechanical. ¹
• When beam element shear and moment diagrams are needed: Translated beam shear and moment diagrams from *.op2 files are not correct. Otherwise, beam element results are all right.

¹ Note: Orientation differences for planar elements (plates and shells) affect stress and strain tensor results, which are direction-specific. Calculated equivalent stresses and strains (such as von Mises and Tresca*2) are unaffected. Additionally, quadrilateral elements are the least affected, and triangular elements the most affected, by local coordinate system inconsistencies.

Result translations for volume (solid) elements are comparable whether *.fno or *.op2 files are merged into Simulation Mechanical.