you are here:   / News & Insights / Engineering Advantage Blog / Obtaining Solution Convergence for Nonlinear FEA

Engineering Advantage

Obtaining Solution Convergence for Nonlinear FEA

Nonlinear FEA Convergence
June 20, 2014 By: George Bauer

Many times, finite element simulations require us to consider problems that exhibit some form of nonlinear behavior.  Whether it is large scale deformation, plasticity, or contact between bodies, we generally classify these nonlinear problems as containing some form of varying stiffness in the model.  Sometimes, this change in flexibility can be abrupt - like bodies coming into contact with each other, or smooth - like creep or low levels of plasticity.  With all of these problems, a representative force-deflection curve is not linear and your stiffness changes with deformation.  
Finite element programs have taken on the task of solving nonlinear static structural problems in a number of ways.  In all cases, the algorithms have to iterate to achieve equilibrium for static structural problems.  The solver will apply some portion of the external forces to the model, then calculate the resultant internal forces to balance the applied load.  There will initially be some out of balance residual force so the solver will improve the stiffness to narrow down the imbalance difference toward zero. (Or a value acceptably close: the "criteria" or "tolerance")

Obtaining final convergence and equilibrium when running these iterative problems can be very challenging.  Some of my FEA consulting colleagues may believe I'm crazy when I jump out of my chair and start my end zone dance because my complicated problem converged!

I've listed some tips below that may help to jump-start convergence improvement with your analysis.  Of course, every situation is different but, try some of these tips and perform sanity checks on the results.  Some of these tips will be handy when employing the technique of preloaded fastener structural analyses, as discussed in my earlier post.

General Nonlinear Convergence Tips

  • Break your finite element analysis into multiple load steps.

- Some of your problem may exhibit a well behaved linear response.  Get through this efficiently and concentrate computing time and accuracy around nonlinear regions with a more incremental approach with more substeps.

- Bolt pretension.  The first load step in the analysis is typically used to "tighten" fasteners in the particular installation/torque sequence.  (As manufactured)  Then, in subsequent load steps, lock the fasteners in place and ramp up mechanical & thermal loads.

  • Employ a displacement controlled load step vs. applied forces, if possible.  
  • Is your default convergence tolerance way too small?  This may indicate no applied loads or a free thermal expansion problem.  Double check loads and constraints.
  • Problems with abrupt stiffness degradation (Snap-through buckling, plastic hinge, delamination, damage modeling, etc... ) may need some artificial damping.  Use some local or system level damping to stabilize the behavior but keep track on the artificial energy levels used.
  • Run a modal analysis to identify rigid body motion issues and regions with local instabilities.

Contact and Body Interaction Tips

Many times,  bodies in your static analysis that are only restrained by contact exhibit rigid body motion problems which impair convergence. To help, try these:

  • Use a tool to check contact pairs before starting the analysis.  Doing so will often identify what bodies are in initial contact and those parts that inadvertently do not detect each other.  Also, turn on contact results trackers and iteration force residuals while the problem is solving to monitor potential problems.
  • One of the biggest ways to help with penalty based contact methods is to reduce the default normal stiffness value.  This can play a big role in improving convergence.  Just make sure that you still have a minimal level of penetration.  Also, consider other contact methods - like projection-based contact.
  • Another trick used to prevent movement instabilities is to constrain the large parts susceptible to rigid body motion while others are "seated" in the first load step.  Then, in the second step, release the unnecessary constraints while applying the final loads. 
  • Review mesh density for contact pairs.  The faceting of flat element faces representing curved surfaces can wreak havoc.  It's like putting a square peg in a round hole, so use a fine mesh. Using higher order elements will also minimize this issue.  
  • Utilize automated contact adjustment to account for unrealistic gaps and penetration, if applicable.
  • Add friction to contact behavior.  A small amount of friction can help with convergence instability and is often a mechanism present in actual load transfer.
  • For troubleshooting, you may want to bond certain contact pairs together just to isolate other problem areas for further investigation.

While every analysis problem involving nonlinearities has its own nuances, many of these approaches noted above are useful in achieving success.  Have you found other useful "tricks" to get nonlinear models to converge?