Assigning bolt connectors in a Nastran analysis

Bolt connectors

If you happen to work with products that require bolts, it is worth taking a moment to consider how the analysis will be approached. 

One concern with performing a simulation that incorporates bolts would be the number of elements required to do so. Recall that every surface in a CAD model gets meshed. Due to the fine threads and other details of a bolt, they require a large number of elements. This can add significantly to the solve time. In most finite element analyses, the stress on individual bolts is not as critical as the stress on the assembly as a whole. Bolts can be reduced to simple connector elements, so long as their contribution to the stiffness of the assembly is accounted for. 

If a CAD representation of the bolt is required, it’s generally recommended to use a simplified version by removing details, as shown in the image below. Even the simplified version on the far right contains approximately 1,000 elements.



In cases where it is suitable to use a simplified connection, the bolt connector will save drastically on elements, requiring, roughly, fewer than 100 elements. 

Beyond making a simplified CAD model of the bolt, another option to consider is forgoing any sort of bolt model and using bonded contact between the (normally) bolted parts. Before making that assumption, please consider the implications of that simplification on your results. 

If it is decided some type of bolt is required, but doesn’t need to be a CAD part, the connector type of bolt allows you to easily add bolt or cap screw representations. You will choose where the bolt starts and ends, the diameter, whether to add washers, the material, and a preload.



Note that this connector can be used to model bolts or cap screws. 

The bolt connector type is a useful finite element simplification of a fastener, and a good middle ground between ignoring all bolts and CAD modeling the bolts.

Results

It is possible to determine how much force and moment there is in a bolt connector in Inventor Nastran. Prior to running the analysis, be sure to edit the analysis and check Output Set>Force.

When reviewing the results, edit the contour and choose Result Data>Beam Diagram and set the Type according to the table shown below to view the beam result of interest.

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

Assign bolt connectors – Exercise

  1. Open the Fender Assembly 2.iam file from your working folder. 
  2. In the Environments tab>Begin panel, click Autodesk Inventor Nastran. 
  3. In the Nastran Model Tree, expand the nodes for Solid 1 and Solid 2 and note that you have two materials being used in this model (Alloy Steel and Aluminum 6061).



  4. In the Autodesk Inventor Nastran tab>Mesh panel, click Generate Mesh. This will allow you to see where the materials are being used on the model, as shown below.



  5. In the Prepare panel, click Connectors. 
  6. With the Connector dialog box open, do the following: 
    • Change the Type to Bolt. 
    • Pan around the model and zoom in to one of the bolt holes to see the edge. Select it so it appears in the Bearing surface/edge for bold head box. 
    • Turn the model around to see the opposite side’s edge. Select it so it appears in the Bearing surface/edge for nut box. 
    • Enter 10 for Bolt Diameter(mm).
    • Change Materials to Alloy Steel. 
    • In the PreLoad area, confirm Axial is selected, then set the PreLoad (N) to 50.  
    • In the Connector Element area, click Next. 
    • Select the edge of the second bolt hole for the bold head, then turn the model and select the edge for the nut. 
    • Repeat the process for the remaining 4 bolt holes. When finished, you should have five bold elements defined. 
    • Click OK.



  7. Pan and zoom in to the tubes on the side of the model. 
  8. In the Setup panel, click Constraints. 
  9. In the Constraint dialog box, change the Name to Fixed. For the Selected Entities, select the end faces of the two tubes, as shown below, and click OK.



  10. Pan and zoom to the bottom edge of the aluminum flap. 
  11. In the Setup panel, click Loads. 
  12. With the Load dialog box open, select the bottom edge so it is added to the Selected Entities box. For the Magnitude (N), change Fx to (negative) -200. Click OK.




  13. In the Contacts panel, click Auto. 
  14. In the Nastran Model Tree, expand Surface Contacts and select one of the contacts to view it in the model.



  15. In the Nastran Model Tree, right-click on Contact (6) and select Edit.  
  16. In the Surface Contact Dialog box, change the Contact Type to Separation and click OK. 
  17. Repeat the process to change Contact (7) to Separation. 
  18. In the Nastran Model Tree, right-click on Analysis 1 and select Edit. 
  19. In the Analysis dialog box, in the Elemental section, select the Force output and click OK.



  20. In the Autodesk Inventor Nastran tab>Solve panel, click Run. 
  21. This will take approximately 5 minutes to solve. 
  22. When the analysis is complete, the Nastran Solution Complete message will display. Click OK. 
  23. In the results window, change the drop-down list in the top-left corner to Displacement. In the model, note that the max. displacement for the flap is 1.707 mm.



  24. Change the drop-down list to Stress, then select SOLID VON MISES STRESS from the next drop-down list. Note the load is being transmitted from one part to the other through the bolts, which is what you want to see.
  25. Change the drop-down list to Beam Diagram. 
  26. Change the sub-type to Beam Force End A-X. 
  27. This result type will plot the Axial force in the bolt connectors. The Maximum should be approximately 722 N.



  28. Save and close the model.