Pin and universal joint between bodies

[Anonymous]

Hi,

I'm completely new to Autodesk Nastran in-cad. 

I need to model pinned and universal joints between bodies in an assembly. How do I go about to do this?

With a universal joint I mean that the bodies are connected by spherical bearings that allow rotation around all axis, but are fixed in translation, hence the joint can not transfer moments.

Thanks!

Roger

[John_Holtz]

Hi Roger (@Anonymous)

This post has some information about creating joints between parts of a model: Pinned connection in Autodesk Nastran

It also depends on whether you are performing a linear analysis (which uses small displacements) or nonlinear analysis (which uses large displacements and rotations), and whether you are simulating a joint between the model and the environment, or between two parts of the model. For joints between two parts of the model, one solution is to create separate rigid connectors in each part, and then connect the rigid connectors with beams or springs. use end releases on the beams or low spring stiffness to allow the free rotations about the desired directions. These two figures attempt to show the concept.

Figure 1: Sample JointFigure 2: Five Pieces to Create a Pin Joint

[Anonymous]

Hi John (@John_Holtz)

Thank you for the reply. It is a linear analysis with small rotations. The connections basically prevents moment transfer.

I made a test case to try what you suggested. It works fine as long as I use one spring to connect the rigid connector at the center of one of the fitting holes to the rigid connector at the center of the lug hole. But, when I add a second spring that connects the rigid connector in the center of the lug hole with the rigid connector in the center of the second fitting hole, it does not work anymore. Basically the lug is no longer free to rotate, which is quite obvious from the stress distribution and deformation. Both springs have high spring stiffness in all directions except from in rotation around the axis of the hole (where it is set to 0).

What am I doing wrong here?

Thanks

Roger

One springTwo springsSpring and rigid connector set-up for two springsSpring configuration

[John_Holtz]

Hi Roger,

Out of curiosity, what happens if you delete the first spring (the one that worked) and leave the second spring (the one that did not work).

• If the lug rotates properly, then there is something strange with the two springs connected together.
• If the lug does not rotate, then check to make sure the stiffness of the second spring are setup properly.

If you cannot find the problem and solution, please zip the assembly and part files (.iam and .ipt) and attach them to this post.

[Anonymous]

Hi,

One of a several solutions I already tried. It works with one spring (either spring), but not two. I've attached the assembly and part files to this reply. For boundary conditions I've used a fixed support at the base of the fitting and a rigid connector to a support with freedom to rotate around the hole axis (pinned support) at the other end of the beam with the lug.

[John_Holtz · Accepted solution]

Hi Roger,

This was an unexpected problem.

The generic material properties were causing the problem. Because they were so weak (E=0.0001), the analysis thought that the model was underconstrained, so it added some automatic constraints. However it decided to constrain the model, it acted as if the lug was constrained in Rz.

If you enter a more realistic modulus of elasticity (such as E=1E5), the analysis runs without warnings and gives the expected deformed shape.

______________________________________________________________

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[Anonymous]

John,

Unexpected and learning by doing 🙂

It works, thank you!

Would be nice to see an easier way to implement joints and similar boundary conditions in NASTRAN in-cad 🙂

Roger

[Anonymous]

@John_Holtz a follow up question to this.

Is it possible to extract the forces in a joint simulated using springs?

Thanks,

Roger

[John_Holtz · Accepted solution]

Yes, you can view the results in the spring connectors.

1. Before running the analysis, edit the analysis settings ("Analysis > Edit") and check the option to output force.
2. Run the analysis.
3. In the results, choose "Other > BUSH FORCE ..." or "Other > BUSH MOMENT ...". ("BUSH" is Nastran's name for a spring element. )

[Anonymous]

That's good to know.  I was hoping there would be an equivalent to the pin and universal joints that sim-mechanical has, but this will suffice for now.  I'm having trouble setting up the universal joint using the same techniques shown here.  Would you be able to show a similar set-up example for that case?

Thanks in advance,

Ben Scheele