Ansys Products

Ansys Products

Discuss installation & licensing of our Ansys Teaching and Research products

Ansys Mechanical – Problem Using Frictional Contact Instead of Bonded

    • tortju


      I am modelling a pump clamp in Ansys Mechanical. The clamp itself consists of two solid parts: one upper and one lower part. These parts are held together by six preloaded bolts. Furthermore, the lower part is connected to two foot brackets via four more bolts. The underside of these bolts have a fixed support boundary condition. The inner surface of the upper part of the clamp are also fixed in the vertical direction in order to make the pretensioning of the first six bolts possible (the clamp is supposed to clamp around a cylinder-like pump):

      I have manually created all the contacts in the model. Between each of the two foot brackets and the plates extending from the lower part of the clamp, there are four bolt spacers on each side. These are connected to both the foot brackets and the plates using asymmetric frictional contact with a friction coefficient of 0,2:

      This seems to be the problem: I get solver pivot errors when using this contact type here (but the same frictional contact definition is no problem elsewhere in the model). Despite the pivot error the solver continues to solve the problem, but it will not converge. However, if I change the contact definition to bonded everything is ok, but this is to unphysical.

      What am I doing wrong here? I have generated initial contact information results, but I can't find anything problematic in those results.

      I am attaching a link to the workbench archive file here:


    • mjmiddle
      Ansys Employee

      I supressed the gravity since that can make convergence harder, being applied in the first load step. And it converged for me, but not without lots of pivot complaining and time bisections. It had to go down to 0.02 sec before it started converging, still with lots of pivot warnings. A deformation result showed 2 of these bolt sleeves moved off into the distance. You can manually set smaller time steps since the model is potentially unstable, because they are all frictional contacts, and some have significant gaps, which relies more on the other frictional contacts working right. I set 500 initial substeps, 20 mininum, and 1e5 max substeps in the first loadstep, with a bit less substeps in the second load step. Now only one sleeve has rigid body motion. If you hide the sleeve bodies, you will see the problem. For the sleeves that move away from the model, there is one element along the bolt for the sleeve contact (red arrow). For a sleeve that stays put, there is 2 elements along the contact length on the bolt (blue arrow):

      This is still very coarse. You really need to set much smaller mesh sizes on all these bolts:

    • tortju

      Your explanation makes sense!

      First I tried to only reduce the element size for the four bolts down to 5 mm. This seemed to work fine - the analysis converged to a solution without any warnings. However, I noticed that two of the bolt sleeves still "flew away" when looking at the deformation animation. This seems a bit strange, considering that the analysis did not show any warnings indicating rigid body motion.

      I also tried using your suggestion for the number of substeps for both the load steps, in addition to the now reduced bolt element size. This resulted in many pivot warnings and the analysis not converging to a solution.

      Before I got your answer I also tried using "adjust to touch" for the interface treatment in the contact definition. Doing this, the analysis converged to a solution. However, I am not quite sure what this setting does so I'm not fully confident that these results are valid. I think this setting closes the gaps between the bolts and the bolt holes. Is this correct?

      Am I doing something wrong here?

Viewing 2 reply threads
  • You must be logged in to reply to this topic.