Convergence issue in non linear problem

I'm solving 2D axis-symmetric problem when I apply required differential pressure on inside and outside surface. I get error solver unable to converge nonlinear problem. Due to elements getting distorted at contact region which I found from newton Raphon residual force. I have tried with finer mesh and changing contact parameter. If anyone with some suggestion will be really helpful.


  • It will be much easier to give a helpful suggestion if you show an image of the geometry.

  • I want to compress the C shape structure between 2 plates in LS1 and apply temperature and differential pressure in LS2. In order to ramp load I have created 5 steps as there was convergence issue. I'm doing this in Ansys workbench. Also I was trying to set convergence criteria as mesh so that remeshing will be done to get to convergence but I was not able to do that setting.

  • If the temperature load is symmetric, one suggestion is to use a horizontal plane of symmetry, then you can have just one plane moving toward that plane.

    Don't try to use automatic remeshing. Is the C shaped piece a hyperelastic material?

  • No C shaped component is metal. I have been doing entire model in static structural in workbench and applied thermal condition by setting reference temperature of component as 'by body' which is uniform. I will try making the horizontal plane of symmetry. In error file it says too much penetration of contact element into target and also some element are getting highly distorted near contact region. Main problem arises when differential pressure load is applied on inside and outside surface of C at that point only convergence issue is coming. If you see force convergence image it's the step5 where full differential pressure load is applied solver is unable to converge.

  • Convergence issues are often helped by taking many Initial or Minimum substeps under the Analysis Settings.

  • Thanks for the useful suggestion. Simulation moved 10% further but still there is nonconvergence due to some elements at contact region are getting highly distorted and too much penetration of contact element related to target element.

  • peteroznewmanpeteroznewman Member
    edited September 23

    The solution may be helped by softening the contact. Under the Contact Details, there is a line called Normal Contact Stiffness. Change that from Program Controlled to Factor and change the Factor from 1 to 0.1 or 0.001 and see if that helps.

    Another suggestion is the remove the sharp corner where contact is made and put a small blend radius on that corner. That way you can have many small elements around the contact point.

  • Thanks alot for all the suggestion. Solution got converged!

Sign In or Register to comment.