Your Partner in Simulation Technology

Create Flexible Bodies for Adams Using Patran

Published 2013-05-15

This document describes how to generate an MNF for use as a flexible body in ADAMS or Vi-Rail using Patran

In Patran, create the FEM of the part required for the problem:

  • In the material properties, density has to be specified in order to run a “normal modes” analysis.
  • Identify all the nodes that will be the interface points to the rest of the system in Adams/Vi-Rail via connections or springs and dampers.
  • Create a “Degrees of freedom” List as shown below; this will define the interface nodes of the component. (Under “Meshing”, select “Create” and for “Object” select “DOF List”). 
Interface points on FE part

Interface points on FE part

  • Enter a name for the DOF List to be created.
  • Under “Define Terms”, for “Node List”, select the nodes where attachments will be made in the Adams/VI-Rail model.
        • NB: The selected nodes in the FEM have to be able to transfer all forces and moments in the 6 degree of freedom (DOF) directions. i.e: Do not only select a single node of a solid element since it does not transfer moments. On solid elements a number of nodes need to be connected to the single interface node using RBE2’s. The supported elements of which nodes may thus be selected as the interface nodes include CBEAM, CQUADR, CTRIAR, RBAR and RBE2's).
  • Select all of the Degrees of freedom.
  • Ensure that no constraints are present in the model as this will affect the stiffness of the part. Any  applied loads will be ignored.

Setup the Analysis

Analysis set

Analysis set

Analysis setup

Analysis setup

  • Create a new analysis job
  • Select “Analyze”, “Entire Model” and “Full Run”.
  • For solution type select normal modes
  • Open “Select ASET/QSET”. Select the DOF List created and click ok
  • Open “Solution Parameters”.
    • Select “ADAMS Preparation”
    • For “ADAMS Output” select “MNF Only”.

      Analysis settings for Adams preparation

      Analysis settings for Adams preparation

    • NB: Open Units and select the appropriate units for the job.
    • Enter the “Num. Shapes to Adams” (e.g. 10 or 26 etc).
      • This determines the amount of mode shapes that will be calculated in addition to the stiffness modes between interface points. The possible amount of mode shapes that will be present in the MNF file, will now be: 10+(num. of interface nodes)x(6 for degrees of freedom of each). In the case of the model above: 26+(23x6)=164.
    • Under Output requests, Select all of the options and select OK.

Select OK to close solution parameters

  • Open subcases:
    • Select the load case that has no loads or boundary conditions applied.
    • Select “Output Requests”
      • Under “Select Result Type, select “Grid Point Stresses.
        • This will allow stresses to be calculated in ADAMS/VI-Rail.
      • “GPSTRESSES=…” will now appear under the Output Requests list.
      • Select “Apply” and “Cancel” to close “Output requests”.
    • Open “Subcase Parameters”
      • Under “Number of Desired roots”, enter the “Num. shapes to Adams” minus 6:

In this case 26 – 6 = 20

Subcase Paramaters

  • Select Apply to run the Analysis.
  • A “.mnf” file is then created that can now be used in ADAMS or VI-Rail to use as a flexible body.

See Using flexible bodies in Adams or Vi-Rail how to use the created MNF in Adams or Vi-Rail.

I think this is...

4 comments on “Create Flexible Bodies for Adams Using Patran”

  1. Thank you very much. Why I cannot find the mnf file in the working directory? There are a few other files created but non of them has .mnf as its format.

    1. The MNF will be created in the working folder of the Patran model, where Nastran creates its output. If there is no MNF file, it was either not requested correctly or the analysis did not complete successfully. Check the .F06 file for the words "fatal error". If present, the cause must be found and corrected first.

  2. Have you ever experienced a case where the number of requested modes is not what shows up in the solve? For example, I have asked for 152 modes (roots) in the subcase parameter form based on 6 rigid, 6*21 DOF nodes , and 20 structural. I ask for 26 in the ADAMS prep form. But, then only 149 modes are generated.

    1. Can you maybe just clarify what your 2 values were regarding the modes that you entered on the two forms to get your result?

linkedin facebook pinterest youtube rss twitter instagram facebook-blank rss-blank linkedin-blank pinterest youtube twitter instagram