Assigning rod connectors in a Nastran analysis

Rod connectors

With rod connectors, you select two points that define the end points of the rod. These two points can be vertices of existing CAD geometry (to create the rod between them), between a vertex of the CAD model and a work point, or between two work points. 

The rod is a good way to connect two points with a member that can carry tension or compression. Functionally, the rod element can carry tension and compression, but not bending. 

As can be seen from the image below, the rod type of connector requires, at a minimum, input for the end points, the material, and a cross-sectional area. A polar moment of inertia (J), torsional stress coefficient, and nonstructural mass (NSM) may also be entered.



Example

In the video, we’ll take a look at this simple truss system, modeled using the rod type connectors in Inventor Nastran.



Given:

  • F = 10,000 lbf 
  • L = 120 in 
  • A = 2 in2 
  • E = 30x106 psi 
  • [degree icon.jpg] = 45°


Anticipated results: 

  • Deflection 
    • X direction = 0.004 in 
    • Y direction = -0.0159 in 
  • Member Force 
    • Vertical = 7929 lbf 
    • Diagonal = 2929 lbf 
    • Horizontal 2071 lbf 
  • Member Stress 
    • Vertical = 3965 psi 
    • Diagonal = 1465 psi 
    • Horizontal = 1036 psi

Assign rod connectors - Exercise

  1. Start Autodesk Inventor if not already open. 
  2. On the Inventor home page, click Part. 
  3. In the 3D Model tab>Sketch panel, click Start 2D Sketch. 
  4. In the drawing, select the XY Plane. 
  5. In the Sketch tab>Create panel, click Point. 
  6. Click to add a point at the origin, then click again to add a second point to the right on the horizontal axis. 
  7. In the Sketch tab>Constrain panel, click Dimension. 
  8. Click the two points to dimension between them, then change the dimension to 120.



  9. In the Sketch tab>Create panel, click Point. 
  10. Click to add a point on the vertical axis. 
  11. In the Sketch tab>Constrain panel, click Dimension. 
  12. Click the two points on the vertical axis to dimension between them, then change the dimension to 120.



  13. Add a final point in the top-right quadrant, dimensioning it to 120 both horizontally and vertically, as shown below.



  14. Click Finish Sketch. 
  15. In the Model Tree, right-click on the sketch and select Dimension Visibility to turn it off. 
  16. On the ViewCube, click FRONT. 
  17. In the Environments tab>Begin panel, click Autodesk Inventor Nastran. 
  18. In the Autodesk Inventor Nastran tab>Prepare panel, click Connectors. 
  19. In the Connector dialog box, do the following:
    • Change the Type to Rod. 
    • Click in the End point of connector box and select the top-left work point, then the bottom-left work point. 
    • In the Rod area, set A to 2. 
    • In the Connector Element area, click Next. 
    • Select the bottom-left work point, then the top-right work point. 
    • Click Next. 
    • Select the bottom-left work point, then the bottom-right work point. 
    • Click OK.



  20. In the Nastran Model Tree, right-click on the Generic material under Connector 1 and select Edit. 
  21. In the Material dialog box, in the Structural area, set E to 30e6 and click OK.



  22. In the Setup panel, click Constraints. 
  23. In the Constraint dialog box, do the following: 
    • Change the Name to Fixed. 
    • Select the locations of the fully fixed boundary conditions. 
    • Click OK.



  24. In the Setup panel, click Loads. 
  25. With the Load dialog box open, select the point at the origin. In the Magnitude (lbf) area, set Fy to (negative) 10000. Click OK.



  26. In the Nastran Model Tree, right-click on Analysis 1 and select Edit. 
  27. In the Analysis dialog box, select Force and click OK.



  28. In the Solve panel, click Run. 
  29. In the Save As dialog box, name the part Truss and click Save. 
  30. When the Nastran Solution Complete message displays, click OK. 
  31. Review the results. Note that you have displacements, the values range from 0 to .016, and the geometry all looks blue.  
  32. In the Display panel, expand Object Visibility and uncheck Connectors. Now the connectors will display as line representations, as shown below.



  33. In the top-left corner of the results window, expand the TOTAL drop-down list and change it to ALONG X-AXIS. The X displacement value should be about 0.004. 
  34. Change the drop-down list to ALONG Y-AXIS. The Y displacement value should be around 0.0159. 
  35. Expand the Displacement drop-down list and select Other. 
  36. In the Results panel, click Probe. Hover your cursor over each member and confirm you have results similar to the following: 
    • Vertical = 7929 
    • Diagonal = 2929 
    • Horizontal = 2071



  37. Expand the Other drop-down list and select Stress. 
  38. Still using the Probe tool, hover your cursor over each member and confirm you have results similar to the following: 
    • Vertical = 3965 
    • Diagonal = 1465 
    • Horizontal = 1036



  39. Save and close the model.
Was this information helpful?