Assigning rigid body connectors in a Nastran analysis

Rigid body connectors

Rigid Body Connectors provide a method of connecting mesh nodes together for an FEA. Typically, this is used to connect a face or edge to a singular control point. A force, constraint, or lumped mass can be applied to the control point to influence the mesh. Some examples are shown below:



When choosing a Rigid Body Connector, you have two sub-types: Rigid and Interpolation. Rigid (RBE2) elements are perfectly stiff and can’t deform relative to the control point. When using Rigid elements, the dependent entities will move exactly how the independent entities move. Interpolation (RBE3) elements are typically used to distribute loads. When using Interpolation elements, the displacement of the reference nodes is the weighted average of the displacement of the "entities to average."



While creating a Rigid Body Connector, you must select the Dependent Entities and an Independent Vertex/Point. Multiple faces, edges, or points can be chosen as Dependent Entities. This allows you to transfer a load or mass across several surfaces or holes at once. The dialog box also contains Degrees of Freedom (DOF) checkboxes (TX, TY, TZ, RX, RY, RZ). These are the active DOF for the rigid elements. The boxes that are checked represent the translational and rotational directions in which they provide rigidity. Deactivate any DOF in which you want to allow relative motion between Independent / Reference Point and the Dependent entities.



Rigid Body Connectors can use a sketch point or a work point as the Independent vertex. These points can easily be constructed within Autodesk Inventor for the FEA. The “Point at Center” option will automatically create a work point at the center of all the selected entities. This can save you the hassle of creating the point manually.

Any referenced datasets can be downloaded from "Module downloads" in the module overview.

Assign bolt connectors - Exercise

  1. Open the Rigid-Connector.ipt file from your working folder. 
  2. In the Environments tab>Begin panel, click Autodesk Inventor Nastran. 
  3. In the Autodesk Inventor Nastran tab>Mesh panel, click Generate Mesh.



  4. In the Prepare panel, click the drop-down arrow beneath Idealizations and select Concentrated Masses. 
  5. In the graphics window, select the work point (work point <1>) as the selected entity. 
  6. Enter 200 lb in the Mass field. 
  7. Select OK. 
  8. In the Setup panel, click Loads. 
  9. Change the Name to Gravity. 
  10. Change the Type to Gravity. 
  11. Enter -386.4 in the Fz field. 
  12. Select OK.



  13. Select Connectors from the Prepare panel. 
  14. Change the Type to Rigid Body. 
  15. In the graphics window, select all 4 of the hole edges in the middle of the plate.



  16. Click once in the Independent Vertex/Point box so it turns blue. 
  17. Select the same work point as the concentrated mass (work point <1>). 
  18. Select OK.



  19. Select Run from the Solve panel. 
  20. Select OK once the solution is complete.
  21. View the results and toggle Object Visibility as necessary. 
  22. Save and Close the model.