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.


«1

Comments

  • 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 2020

    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!

  • Hi

    When I ran my full Simulation I got the result with some warning and no error. In result I have equivalent stress (Von mises stress) around 3 times more than Yield and Ulimate strength but still there is no fracture seen in the model. How do I get to know the model I created in transient structural is correct.

  • peteroznewmanpeteroznewman Member
    edited October 2020

    @Jasmin

    Please read this discussion and come back with any follow up questions.

    https://forum.ansys.com/discussion/1373/i-want-to-see-the-failure/p1

  • Hi Peter

    I have gone through the attached link. I got the point explained.

  • I have doubt when I tried to create model in the static structural I was not able to get the converge solution I used to get error solver was unable to converge the nonlinear problem . When I shifted to Transient Structural module I got the Converged solution even though my problem was static. Is it because the Transient Structural uses Full newton Raphson Method? like how do we decide the Static or Transient module to be used. Can you please give some tips/ example.

  • peteroznewmanpeteroznewman Member
    edited November 2020

    @Jasmin

    One type of problem that is difficult to solve with Static Structural analysis that is easier to solve in Transient Structural (or Explicit Dynamics) is snap-through behavior. This occurs when a structure buckles into a new shape. It is difficult for the Static solver to increment the load gradually and remain in static equilibrium to get to the buckled state. But a Transient solver can solve the dynamic equilibrium by including the inertial forces that arise from accelerating the mass to snap-through to the buckled state.

    So the key difference is what type of equilibrium is the solver trying to converge on, static equilibrium or dynamic equilibrium.

  • Thanks for Explanation.

  • Can you please suggest what and all condition can lead to sudden drop in contact pressure as seen in attached image in 3rd step. In 3rd step differential pressure is applied on the C component between the plate. I have been changing the numerical damping value in Analysis setting to check Impact load issue while differential pressure is applied. Also tried by varying stabilization damping factor in contact controls it didn't help much.

  • @Jasmin

    Numerical damping stabilizes the numerical integration scheme by damping out the unwanted high frequency modes. You should not need to change this value. You need Structural Damping. Structural damping refers to physical damping present in the system. For more information, see Damping in the Structural Analysis Guide. 

    The contact pressure could make a sudden reduction if the deformation in the C changes from one node in contact at the tip to several nodes in contact on the side.

  • Thanks for the explanation.

  • In 2D Axisymmetric analysis I'm not able to define rigid-deformable contact. In geometry when I try to define stiffness behavior as flexible to C and rigid to the 2 side plates. It does'nt take. So I'm able to define only deformable-deformable contact with flexible stiffness behavior. Is there any other way to change the contact definition.


  • @Jasmin

    You can't define the Stiffness Behavior of the body to be Rigid in a 2D Axisymmetric model.

    But you can pick that face/body, and assign a Displacement BC to both X and Y coordinates, which makes the body behave like a rigid body.

Sign In or Register to comment.