# Solver Showing Element Violation

Member Posts: 1

Hello all,

Been trying to get this simulation to solve for several days, but I keep running into "element formulation" errors.

Much of the research I've found so far mention using Newton-Raphson residual forces or to solve for element violations find the problematic areas, and then refining the mesh around that area (for example: Error in Element Formulation — Ansys Learning Forum) However, I'm still running into issues of convergence, and my solver times are through the roof.

I've attached the Solver Output as a PDF.

Any ideas on how to resolve?

Tagged:

• Posts: 11,372Member

This 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.

```AUTOMATIC TIME STEPPING . . . . . . . . . . . . ON
INITIAL NUMBER OF SUBSTEPS . . . . . . . . . 5
MAXIMUM NUMBER OF SUBSTEPS . . . . . . . . . 20
MINIMUM NUMBER OF SUBSTEPS . . . . . . . . . 1
```

Try this setting:﻿

```INITIAL NUMBER OF SUBSTEPS . . . . . . . . . 20
MAXIMUM NUMBER OF SUBSTEPS . . . . . . . . . 200
MINIMUM NUMBER OF SUBSTEPS . . . . . . . . . 20
```

This is a big model:

```...Number of elements: 1,043,980
...Number of nodes: 1,472,525﻿
```

Your 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.

You 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.

• Posts: 11,372Member

It would help if you inserted an image of the Newton-Raphson Force Convergence Plot in your reply.

• Posts: 4Member

@

• Posts: 11,372Member

That is a Force Residual plot, not a force convergence plot.

https://forum.ansys.com/discussion/6808/force-convergence-plot

• Posts: 4Member

Apologies.

• Posts: 4Member

@peteroznewman 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.