General Mechanical

General Mechanical

Solution failed to converge – loss of convergence

    • rmknox
      Subscriber

      Hi everyone,


      I'm running a compression-shear analysis on a spinal fusion device and am unable to get the solution to converge long-term. What I mean by that is an individual substep will converge, then the solution loses convergence on the first iteration of the next substep. I've included an image below to show what I mean.



      I've run this simulation many times using different parameters with similar results. In several cases, multiple substeps will converge, but the solution will always lose convergence in the iteration immediately following the converged iteration.


      Is this a problem that can be fixed simply by adding more substeps? More generally, does this pattern (converged substep followed by immediate loss of convergence) indicate a particular solution?


      I am happy to provide any further information as necessary. Thank you in advance for your help.

    • Sandeep Medikonda
      Ansys Employee

      Hi, Can you explain what kind of analysis you are doing? and provide details on the materials in use, the Analysis and Contact settings?


      Regards,
      Sandeep

    • rmknox
      Subscriber

      Hi Sandeep,


      I'm running a Transient Structural analysis of a spinal fusion device under compression and shear. I'm defining by substeps, minimum = 200, initial = 400, maximum = 500. Large deflection is turned on.


      All contacts are frictional with COF = 0.3 and Adjust to Touch interface treatment. I've also performed local Contact Sizing mesh refinements at all frictional contact areas.


      I'm using custom permutations of Ti6%Al4%V for my materials.


      I hope this helps!


       

    • Sandeep Medikonda
      Ansys Employee

      What is the exact error you are seeing? Are you seeing pivoting error or errors related to a certain degree of freedom (DOF) exceeding limits? If so, please see this post. You 


      Any reason why you aren't using Static Structural?


      Lastly, have you checked for the Newton-Raphson residuals and checked if the contact is causing the problem? Also, use the initial contact tool and check for the pinball radius, make sure it is large enough to enclose the contact gaps.


      If you are still having problems, Can you post images and explain when you reply?


      Regards,
      Sandeep

    • peteroznewman
      Subscriber

      Have a look at these videos to see how to use the information in a Newton-Raphson residual plot to aid in convergence.


      Regards,
      Peter

    • rmknox
      Subscriber

      Hi Sandeep,


      I've posted the error message I receive here:



      Unfortunately, it doesn't reference DOF errors or any other problems I've seen elsewhere online.


      Regarding contacts, the initial status for each contact pair is Closed. It seems like the Pinball for each region is large enough to enclose any penetrations or gaps, I've included a picture of the initial information screen below:



      We tend to use Transient Structural over Static Structural because we've had more success using it for our applications in the past. I can try to redo everything using Static Structural to see if that helps at all.


      I have several Newton-Raphson residual plots active. The frictional contact areas are definitely where the trouble is arising. I'll be sure to use Peter's video suggestions to look deeper into this.


      Thank you!

    • Sandeep Medikonda
      Ansys Employee

      Have you tried these suggestions from the manual:



      • Check for sufficient supports to prevent rigid body motion or that contact with other parts will prevent rigid motion.

      • Check that the loading is of a reasonable nature. Unlike linear problems whose results will scale linearly with the loading, advanced contact is nonlinear and convergence problems may arise if the loading is too big or small in a real world setting.

      • If the contact type is frictionless, try setting the type to rough. This may help some problems to converge if any possible sliding is not constrained.

      • Check that the mesh is sufficiently fine on faces that may be in contact. Too coarse a mesh may cause inaccurate answers and convergence difficulties.

      • Consider softening the normal contact stiffness KN to a value of .1. The default value is 1 and may be changed by setting the Normal Stiffness. Smaller KN multipliers will allow more contact penetration which may cause inaccuracies but may allow problems to converge that would not otherwise.

      • If symmetric contact is being used (by default the contact is symmetric), consider using asymmetric contact pairs. This may help problems that experience oscillating convergence patterns due to contact chattering. The program can be directed to automatically use asymmetric contact in the Details view of the Contact Folder.

    • rmknox
      Subscriber

      Hi Sandeep,


      I was able to get the simulation to solve by running it in Static Structural. Thank you for your suggestions, I will be sure to keep them in mind in the future.

    • marsicano1
      Subscriber

      Hi everyone!!


      I am running a bulge test simulation.


      My problem is that the solution does not converges and a warning about  the solver pivoting  appears.


      Could you give me a hand pleace?


      I attach my file.


      Thanks in advance


       

    • peteroznewman
      Subscriber

      Hi Marsicano,


      Thank you for deleting your post out of the discussion that had nothing to do with your question.


      This discussion is relevant to your question. Did you read all the advice in this discussion?


      It is still better for you to start a New Discussion using the big green button at the top right of this page. I have put an image of that below.



      The reason is that the member who starts a discussion gets automatic email notification of new posts, if they check that box.  So in this discussion, that is rmknox and not you.


      In your New Discussion, you can put a link in your post that you have read this relevant discussion and it didn't help you to solve your problem. You do that by right mouse click on a #Permalink on any post in this discussion and Copy link address (if using Chrome).  Then you can paste that link in your post by clicking on any word in your post and using the Link button to insert a link. Then you paste.



       

    • peteroznewman
      Subscriber

      Hi Marsicano,


      I made some changes to your model. I reduced the element size on the part being bent.  I turned on Large Deflection. I put a command to force the solver to keep going. I edited the Contact details. Now it solves. Please open a New Discussion to ask further questions.


    • marsicano1
      Subscriber

      Hi Peter!!!


      Many Thanks for your help!!!!


      Unfortunately when I open your file, the software gives me a message.


      As you suggested me I opened a new discussion.


      Could you help me?

    • pravallikalikith
      Subscriber
      Hai peter,n I am doing transient structural analysis for my piezoelectric model. When I run the simulation, solution is converging very slowly and sometimes failed to converge. I have tried the possibilities what you have posted earlier. please suggest me how to resolve.n
    • peteroznewman
      Subscriber
      nIf your solution is converging, that is good. Some solutions take a long time. There are ways to speed them up.nIf your solution fails to converge, use the things you have read about to get them to converge.nI have no suggestions, you have not provided me with anything to look at.nn
    • pravallikalikith
      Subscriber
      Hi peter,n My solution is converging successfully but it is taking a lot of time (2-3) days. How to speed up the simulation? My model is having 4,57,238 mesh elements and 19,313,248 nodes. Apart from reducing the number of elements, please suggest me how to do?nthank you.nWith regards.n
Viewing 14 reply threads
  • You must be logged in to reply to this topic.