General Mechanical

General Mechanical

Convergence problem-hip implant

    • Goddy
      Subscriber

       I am having problem doing analysis on this hip implant. I get the error of a highly distorted element. I have done many things turning off pilot solver, using the ncnv command changing the magnitude of my force, checking my contacts, refining the mesh, checking to  make sure my fixed constraint on the cylinder is right but i still get the highly distorted element problem and failure of solution to converge.


      Can you help me please. 

    • Sandeep Medikonda
      Ansys Employee

      Goddy,


        What materials are you using? Can post snapshots of your force convergence plot, analysis settings etc?


      Regards,
      Sandeep


       

    • Goddy
      Subscriber

      I am using titanium (E=114 GPa) for the implant and epoxy resin (E=3.7 GPa) for the cylinder. I also use poisson ratio of 0.3 for both. I thought you could see all the information in the file of my project i attached above. I'll post the snapshots you requested.


      Thanks

    • Sandeep Medikonda
      Ansys Employee

      We are not allowed to open those files. Your initial force is extremely high and you don't have even one substep convergence. How are you loading this and what do you have in the command snippets?


      Regards,
      Sandeep

    • Goddy
      Subscriber

      I am loading it with a constant force. I thought the 10 substeps in the analysis settings means the force is ramped up slowly(a minimum of 10 steps) to the maximum force of 500N i defined? Even when i used a tabular force started with a force of about 100N and increased gradually, i got the same error so i don't know if the problem is an initial high force.


      There is nothing but ncnv, ,1e30 in the command snippet which i think means the solution should continue even if it doesn't converge.

    • Sandeep Medikonda
      Ansys Employee

      I would recommend you to remove that command, it just sets the key to terminate an analysis.



      Terminates program execution if the largest nodal DOF solution value (displacement, temperature, etc.) exceeds this limit. Defaults to 1.0E6 for all DOF except MAG and A. Defaults to 1.0E10 for MAG and A.



      Look at the contact settings. Something is putting a high force initially if your materials and mesh are fine (I'll take your word here) and your model is properly constrained. It should be coming from contact as you have fairly straightforward boundary conditions. 


      So, what contacts are you using?


      Regards,
      Sandeep

    • Bhargava Sista
      Ansys Employee

      Goddy,


      Is the applied force the actual imposed load or is it an estimated force that you're working with? For gaining better insight into the system, I'd recommend you to replace the force loading with a displacement loading and measure the reaction force on the displacement boundary condition (drag and drop the displacement condition on Solution and that'll create a force probe on the displacement condition). This will give you a better control over the element distortion issues.


      Also, for a problem like this, I'd recommend turning on auto-time stepping and issue an initial, min. and a max. num. of steps Stat with something like: 



      • initial of 20 steps

      • min. of 10 steps

      • max. of 1000 steps.

    • peteroznewman
      Subscriber

      Goddy, I opened your archive (I don't work for ANSYS) and think I see your problem.


      You have an implant in a cylinder of epoxy.



      If I turn off the cylinder, I see the length of the implant.



      But if I turn off the implant and turn on the cylinder, I don't see a hole in the epoxy for the implant.



      You have to subtract the solid implant from the epoxy cylinder and leave a hole and fill that hole with the implant. Then you can bond those two parts together.


      I can't do that for you as the geometry is not in the archive, it is in SolidWorks.  Do that subtraction and let's see what you get. Also, all the advice the ANSYS members gave should be rolled into your next attempt.


      Regards,
      Peter

    • Goddy
      Subscriber

      Thank you. Will do that and let you know

    • Goddy
      Subscriber

      Thank you will do that and let you Know.


       

    • KCPUTREVU
      Subscriber
      hi peter, I am getting an error internal magnitude limit was exceeded.nplease help me out with this.n
Viewing 10 reply threads
  • You must be logged in to reply to this topic.