Solver Showing Element Violation

- January 15, 2021 at 9:59 pm
  
  kevin_madsen
  Subscriber
  
  Hello all,
  Been trying to get this simulation to solve for several days, but I keep running into "element formulation" errors.
- January 15, 2021 at 11:50 pm
  
  peteroznewman
  Subscriber
  
  nIt would help if you inserted an image of the Newton-Raphson Force Convergence Plot in your reply.n
- January 16, 2021 at 4:54 am
  
  kevin_madsen
  Subscriber
  
  @nLet me know if this helps. Thanks for your reply!n
- January 16, 2021 at 5:04 am
  
  peteroznewman
  Subscriber
  
  nThat is a Force Residual plot, not a force convergence plot.n/forum/discussion/6808/force-convergence-plotn
- January 16, 2021 at 5:21 am
  
  kevin_madsen
  Subscriber
  
  Apologies.nn
- January 16, 2021 at 12:39 pm
  
  peteroznewman
  Subscriber
  
  nThis model has a Cast Iron material which uses plasticity equations. The solver must take many small steps to avoid the element shape changing too quickly. Each of the bisections is because the shape change was too large. Here are your step settings: You can see that 5 was too small to get started since it did a bisection.nAUTOMATIC TIME STEPPING . . . . . . . . . . . . ON nINITIAL NUMBER OF SUBSTEPS . . . . . . . . . 5 nMAXIMUM NUMBER OF SUBSTEPS . . . . . . . . . 20 nMINIMUM NUMBER OF SUBSTEPS . . . . . . . . . 1nTry this setting:?nINITIAL NUMBER OF SUBSTEPS . . . . . . . . . 20 nMAXIMUM NUMBER OF SUBSTEPS . . . . . . . . . 200 nMINIMUM NUMBER OF SUBSTEPS . . . . . . . . . 20nThis is a big model:n...Number of elements: 1,043,980n...Number of nodes: 1,472,525?nYour computer took 7.3 minutes per iteration, so 43 iterations took 5.3 hours. You are going to need more iterations than that to finish the model.nYou could reduce the wait time by reducing the number of nodes. You could cut away part of the model. Is the geometry and load symmetric? If so you could cut the model in half and use a symmetry boundary condition. Are there parts of the model that are of less concern? You could cut those away and use a Remote Force or Remote Displacement on the cut boundary. You could use a coarser mesh in places where the stress gradient is low and reserve nodes to make a fine mesh in places where the stress gradient is high. You could carve up the geometry into sweepable bodies and replace the tet mesh with a hex mesh, which is more efficient at filling the volume with fewer nodes.n
- January 18, 2021 at 4:50 pm
  
  kevin_madsen
  Subscriber
  
  That did the trick! Thank you so much for your help. The solver only took 2-ish hours to converge, even without truncating the models. I appreciate you taking your time to help out and teaching me some new techniques.n