Assigning spring connectors in a Nastran analysis

Spring connectors

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

Functionally, the spring element can behave like a physical spring (define K stiffness) or a damper (define GE damping coefficient) or both.  

As can be seen from the image below, the spring type of connector requires, at a minimum, input for the end points, and a stiffness or damping coefficient. A material definition or cross-section is not required as the damping value or stiffness input determines the mechanics of the spring.



Usage tips

The spring connector is a good way to add damping and/or stiffness into a model, either because the physical model contains a spring or damper or in the event you need to help stabilize a part. 

  • The spring element, as the name implies, will be useful in a finite element analysis model to represent just about any instance where there are springs or a damper in the physical product. 
  • Note that weak springs are also occasionally utilized in analyses when there is a body/part that is not fully constrained, and that instability is causing convergence failure or failure to solve. A weak spring (small stiffness) in the direction of the possible motion, applied to the part, can help to stabilize the geometry.  
  • You may want to consider attaching a rigid body connector to the CAD model and then a spring to the common node of the rigid body to help alleviate possible stress concentrations. 
  • When applying Stiffness, use the Advanced Options menu to input values for each direction. K1 (Tx), K2 (Ty), K3 (Tz), K4 (Rx), K5 (Ry), and K6 (Rz).

Example

Problem description:

A horizontal beam (length = 30 in, width = 0.5 in, and height = 0.75 in) is fixed on one end and supported by a spring (with stiffness k = 54 lb/in) at the other end. A distributed load (w = 5 lb/in) is applied on the top of the beam, as shown below.



The material properties of the beam include: 

  • Modulus of elasticity (E) = 30 x 106 psi 
  • Poisson’s ratio = 0.3 

Find the deflection at point A (the free end of the beam) and the force in the spring.

Anticipated results: 

  • Theoretical displacement (in.) = -0.499 
  • Force (lbf) = -26.95

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

Assign spring connectors – Exercise

  1. Start Autodesk Inventor if not already open.
  2. In the File menu, click New. 
  3. In the Create New File dialog box, select Spring.ipt and click Create. 
  4. In the 3D Model tab>Sketch panel, click Start 2D Sketch. 
  5. In the drawing, select the XY Plane. 
  6. In the Sketch tab>Create panel, click Line. 
  7. Draw a line from the origin point out to the right along the horizontal axis to represent the beam. 
  8. In the Sketch tab>Constrain panel, click Dimension and change the dimension to 30.



  9. In the Sketch tab>Create panel, click Point. 
  10. Add a point 5 inches below the right end of the beam, as shown below.



  11. Click Finish Sketch. 
  12. In the Model Tree, right-click on the sketch and select Dimension Visibility to turn it off. 
  13. On the ViewCube, click the Home view. 
  14. In the Environments tab>Begin panel, click Autodesk Inventor Nastran. 
  15. In the Autodesk Inventor Nastran tab>Prepare panel, click Idealizations. 
  16. In the Idealizations dialog box, do the following: 
    • Set the Type to Line Elements. 
    • Set the Line Element Type to Beam. 
    • Set the Input Type to Cross Section. 
    • Click the Cross Section Definition button. 
  17. In the Cross Section Definition dialog box, do the following: 
    • Change the Shape to BAR. 
    • For DIM 1 (in), enter .75. 
    • For DIM 2 (in), enter .5. 
    • Click Draw End A. 
    • Click OK.



  18. In the Idealizations dialog box, do the following: 
    • Select the Associated Geometry option. 
    • Click in the Selected Entities box, then select the sketch line. 
    • Click OK.



    • The sketch line can now be found under the Idealizations node in the Nastran Model Tree and is identified as Beam 1. 
  19. In the Mesh panel, click Generate Mesh. Once the mesh has been generated, note that it has 27 nodes and 26 elements, as displayed in the Nastran Model Tree.



  20. In the Nastran Model Tree, under the Idealizations>Beams>Beam 1 node, right-click on Generic and select Edit. 
  21. In the Material dialog box, in the Structural area, set E to 30e6 and v to 0.3, then click OK.



  22. In the Prepare panel, click Connectors. 
  23. In the Connector dialog box, do the following: 
    • Change the Type to Spring. 
    • For the first End point of connector, select the end of the beam. 
    • For the second End point of connector, select the point below it. 
    • Select the Stiffness checkbox. 
    •  Click on Advanced Options. 
    • For K2, enter 54. 
    • Click OK.



  24. In the Setup panel, click Constraints. 
  25. In the Constraint dialog box, do the following: 
    • Change the Name to Fixed. 
    • For the Selected Entities, select the free end of the beam and the free end of the spring. 
    • Click OK.



  26. In the Setup panel, click Loads. 
  27. In the Load dialog box, do the following: 
    • Change the Type to Distributed Load. 
    • For the Selected Entities, select the beam. 
    • In the Magnitude (lbf/in) area, set Fy to (negative) -5. 
    • Click OK.



  28. In the model, note that there are load indicators showing at either end of the beam. To change the visual display to better indicate that it is a distributed load, in the Nastran Model Tree, right-click on Load 1 and select Edit. In the Load dialog box, in the Display Options area, use the slide to increase the Density (select the Preview option to see the changes in the model as you move the slider) and click OK.



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



  31. In the Solve panel, click Run. 
  32. In the Save As dialog box, name the part Spring and click Save. 
  33. When the Nastran Solution Complete message displays, click OK. 
  34. In the Results window, expand the drop-down list in the top-left corner and select Displacement to review the results. Note that the result should be about 0.499.



  35. Expand the drop-down list again and select Other. Expand the second drop-down list and select BUSH FORCE-Y. Note that the result should be about -27.



    • If the spring results are obscured, in the Display panel, expand the Object Visibility drop-down list and uncheck Connectors. 
  36. Save the model.