'Thermomechanics' simulation project by potyka_csaba


I created a new simulation project called 'Thermomechanics':

Thermomechanical problem

More of my public projects can be found here.


Hi @potyka_csaba,

Very interesting simulation. I have noticed your run time for the simulation is exceeding. I would suggest you to do the following which will decrease your computation time without compromising on the accuracy.

  1. Since your model and boundary conditions are symmetric, you can use quarter of your original model and apply symmetry boundary conditions on the cut faces.This will decrease your number nodes to 1/4th of your current model.

  2. Merge all the solids that are in bonded contact as their material is same.

  3. Use Tetrahedral with local refinements to refine only in the curved surface and the faces that are in contact(physical contact). This will further reduce the size of your problem.

If you are still facing any other problem in your simulation, feel free to comment below.



Hello @nava!

Thanks for you r suggestions!
I don’t want to create symmetric model where contacts are defined in the symmetry plane thus there the solver will have fatal problems in the contact formulations.
On the other hand I need the contacts, because I am interested in the contact behaviour, basically this is one of the goals by this simulation.
Yes I use the Tetrahedral with local refinements, and I will try to reduce somehow the model size!
Nevertheless further ideas are very welcome!



Hi @potyka_csaba,

I noticed you are still having some issues with your simulation. I did a simulation on your model by using symmetry along YZ and ZX symmetry(manually restricting displacement normal to the symmetry plane) and for meshing I used Tetrahedral automatic with Coarse setting.


I hope this helps.



Thanks @nava!

I try the model you have built. It seems to be working! Great!



Hello @nava!

I’ve got no idea how do you managed it, but the quarter model works well. It is great!
My experience until now was that when symmetry constrains were applied at nodes which were in contact, then the solver did’nt worked at all.
But it is maybe different for Bonded or Sliding contacts.
I have one further question. Why the bolt pretension drops after the first load step? Shouldn’t it remain constant based on the “fictitious clearance” setting? Could you check it in my project? I have results about it there…

Thanks in advance:


Hi @potyka_csaba,

I looked at your project and found only one problem. There is a small mistake in the simulation set up that I gave you earlier; the bolt in y and z direction was fixed, which won’t happen in real life. Sorry for that.Nevertheless, it won’t effect the overall result except for bending in the bolt.

In the simulation set up (without temperature) given here, I have made the following correction.

  • The contact between the bolt and clamp face is specified as penalty with friction.
  • The bolt is supported by elastic support. This is needed for first timestep as there is no friction initially to hold the bolt in y and z direction.

Now, regarding your question on decreasing bolt load after pressure application, I think the reason might be due to pivoting of the two flange faces about the seal. You can clearly see this in the animation(t=10 to t+20)

The graph here show the average X and Y displacement of the clamp face( the face which has bolt hole).

In the normal case. the clamp face should retract after pressure application resulting in increase in the bolt load, but here due to rotation of flange faces, the clamp keeps on moving in -ve x direction and the bolt follows it to maintain the gap which results in decreases in the bolt load. This situation is similar to the case where plates are preloaded with a bolt and then the plates are compressed.

I hope this answers your question.