How to run Nastran with Hypermesh

Basically, the preparation and postprocessing of a Nastran model in Hypermesh is the same as preparing a model for Optistruct. In fact the format of the input decks are nearly identically. There are a few few significant differences.
  1. The Nastran model is not solved in Hypermesh but either in the command line using the Nastran line command or in Windows using Nastran 2005.1 GUI.
  2. There are a few lines that need to be manually added to the Nastran input file (*.dat file)
  3. The results from Nastran (*.pch ASCII punch card file) must be translated to the Hypermesh results format (*.res) using the hmnast translator before postprocessing in Hypermesh.
Here are the basic steps that need to be taken to prepare, run and postprocess a Nastran model in Hypermesh
  1. Start Hypermesh
  2. In the Geometry panel select User Profile and pick Nastran.
  3. Prepare a finite element model in hypermesh just as you would normally.
  4. Before exporting the Nastran *.dat file in the BC panel select the Control Cards subpanel and choose the SOL card. This is a card which specifies what solver Nastran will use to solve your model. For linear static analysis use SOL=101. If this is not set the *.pch file will not be written and you will not be able to postprocess your results.
  5. Now you need to export your model to be solved in Nastran. To do this under the Files subpanel select export and choose the name for your Nastran input file (a *.dat file) and select the other parameters appropriately to your model and write.
  6. Open the *.dat file in a text editor like emacs or notepad (not Word) and add the follwoing lines imediatly after the SUBCASE card (after LOAD=xxx)

    DISPLACEMENT(PUNCH)=ALL
    SPCFORCES(PUNCH)=ALL
    STRESS(PUNCH)=ALL

    So, you should have something that looks as follows

    SUBCASE
      SPC=1
      LOAD=1
    DISPLACEMENT(PUNCH)=ALL
    SPCFORCES(PUNCH)=ALL
    STRESS(PUNCH)=ALL

    and save.

  1. Next you must solve your model using Nastran. In Windows use the file manager that pops up when you start Nastran 2005.1 either from the desktop icon or from the Start menu, select your *.dat model file. Then in the next panel hit run and hopefully there are no errors in your model and then you have a solution. In Unix or Linux you need to run Nastran from the command line. Either way, you should have a *.pch file and a *.f06 file. If not then something went wrong and you will not be able to translate your results (if you have any) into Hypermesh. If there was some problem look at the *.log file to get some insight into what went wrong.
  2. Finally, we need to translate the Nastran results into a Hypermesh *.res, results file. To do this go back to Hypermesh and in the BCs panel select the Solver subpanel. In the Solver subpanel set the button in the top left corner to hmnast (usually it is set to Optistruct). This is the command that will translate the Nastran *.pch file to a *.res file. Select the input to your *.pch file and the output file to an appropriately named *.res file and hit Solve.
  3. Now you are done! Load the *.res file in the File subpanel using the Results option and then you can go to the Post panel and view your results just as you would if you solved your model using Optistruct.
  4. Have fun!
In general Nastran has greater capabilities than Optistruct. It can perform nonlinear analysis with large deformation, nonlinear materials, contact .etc as well as dynamic analysis implicit or explicit. To learn more about using Nastran see some of the other tutorials or look at the Nastran Documentation.