Bolted Joint modeling

keithmcarthur

I had a couple of questions about modeling bolted joints and am looking for input on advice/experience.

There is one thread that discusses pre-load on bolted joints by applying a thermal stress on the bolt which is cleaver and works quite well. My questions are around the solvers and constraints.

For modeling the contact between the two bolted surfaces it appears that using the nonlinear static 3D CCX solver and using a contact constrain between the surfaces is one way. This requires and input for the the "Normal stiffness per unit area", does this automatically populate based on the materials assigned to each of the faces? I am just curious about normal values and their influence on the results.

The other question I have is using the internal solver Static 3D. When nodes are used for multiple named face selections and the each of the named selections are used in different constraints I get a node error in when running the solver. Does the internal solver just have a limitation that the a node can only be used in a single constraint?

I was attempting to model a bolted joint with using the internal solver static 3D and applying a compression only support to the two faces that would be clamped in the bolted assembly. I run into issues with node errors but what would the anticipated result be? Would it be similar to using a the nonlinear CCX solver with a contact constraint.

Presently only looking at static 3D but also need to look at Dynamic Response 3D and need to include the pre-loaded bolts influence the stiffness of the assembly.

Thanks.

Victor

Yes, the default value is based on the materials of the face(s) at the time. It's just a rough estimate that will often get a solution, but you may need to adjust it again. I usually adjust it by an order of magnitude or two at a time. The theoretically correct value is infinity, but you have to choose something low enough for the solver to converge and high enough to avoid excess penetration, which you can see by looking at the solution. A rule of thumb is 10*E/t where E is Young's modulus and t is thickness of the thinnest part in contact.

bonded contact doesn't allow some nodes to be shared with other constraints with the internal solver. Some workarounds are:

• Exclude those nodes' faces
  
• Extrude a thin layer from one surface to carry the constraint separately from its adjacent surface
  
• Combine multiple adjacent bonded contacts into one
  
• Use the CCX solver and the Elastic option in the bonded contact.
  
• Replace the other constrain with elastic support having a high stiffness (same meaning as the stiffness used in contact).
  

Cyclic symmetry is another constraint that has this limitation. Other constraint types can typically be mixed arbitrarily on the same nodes as long as they don't physically conflict with each other.

Compression-only support is a contact with ground, so it may not be suitable for a bolted joint. Its meaning is equivalent to contact with an invisible fully constrained high-stiffness object. It's also generally slower and less stable than contact with CCX. Usually, prefer contact over compression-only support.