Solution failed to converge - loss of convergence

  • Last Post 17 September 2018
  • Topic Is Solved
rmknox posted this 07 September 2018

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.

Order By: Standard | Newest | Votes
SandeepMedikonda posted this 07 September 2018

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


rmknox posted this 07 September 2018

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!


SandeepMedikonda posted this 08 September 2018

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?


  • Liked by
  • peteroznewman
peteroznewman posted this 08 September 2018

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


rmknox posted this 10 September 2018

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!

SandeepMedikonda posted this 10 September 2018

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 posted this 17 September 2018

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.