tree on creep bearings

[tele5palla]

Hello everyone,
I'm trying in a static analysis of a tree on bronzine, using the static structural module of ansys workbench.
since I am particularly interested in the distribution of pressure on bronzines I am using non-linear formulations of contacts between these and the tree.

the problem is that on one of the bronzine the distribution of pressure is uneven.. you can see an image in the annex.


on the other, however, everything as I expected. What could be the problem? is the famous chattering?


I'll tell you how I set the contacts.
are both frictional, coeff 0.2
asymmetrical
as formulation I used augmented lagrange,
I gave the update stiffness each iteration command


from the initial contact tool there was a gap in one of the two bronzines (the one that works well) that I closed with "adjust to touch"

I strongly hope to receive your help.
Thank you.

 

[stefano.garbin]

Step by step.

0. make sure that the mesh is made as a god commands (preferably mapped or with regular tetrahedra)

1. eliminate bronzine and contact surfaces between tree and bronzine put a compression only bond. launch the solution and see what happens. this would be the case of infinitely rigid bronzes.

2. after point 1 you can do another analysis with the bronzine as you have already tried to do but be careful to:
-shows contacts as "symmetric". asymmetric contact only makes sense if you have two bodies in contact with very different stiffnesses of which the most rigid is always the target.
"augmented lagrange" is fine.
-0.2 is a coefficient of friction that but adapts to a bronze. I would put "fricionless" or a coefficient of type 0.04-0.05
"update stiffness at each iteration" is fine.
- "adjust to touch" is fine.

3. ah I forgot after you created contacts and mesh go to the tree where you are contacts and enter the "contact tool", so you can verify the accuracy of the contacts you have defined before you solve all the analysis.

 

[tele5palla]

Thanks stefano for the answer!
I think I solved it... and you caught in the sign, in the sense that most likely the problem is that mesh is not fit enough to describe the contact well. even because almost all the other evidence that I recommend doing I have already done.

I had already done the test using compression only as a constraint, and everything went wonder.
the problem has arisen at the time when I substituted the bronzes with the contacts.
I initially tried symmetrical contacts, and then modified them in asymmetric to try to solve the problem but nothing changed. in the latter case I tried both with contact on the bronzine and the tree.


I have not yet launched the analysis with a mesh quite dense, but I have changed the value of contact stiffness using a 0.01 factor and now everything seems to work perfectly.
using the contact tool in the postprocessing phase I have a very low interconnection and even pressure distribution.

I believe that everything is due to the fact that not having a mesh thick enough the small initial compenetrations are almost enough to balance the applied force. I expect very low pressures.

anyway I think that in the next few days I will do the analysis improving mesh (using contact sizing) and setting contacts as you recommended me.


ps in version 14 in autometic contact is autoasymnmetric... I think you'll know better than me. basically makes contact asymmetrically choosing appropriately contact and tag.

Thank you again!