Help: Non-Linear Static Stress Simulation Error

[2203270EZLLQ]

Hi all I've been trying for days to do a non-linear static stress simulation, I'm not sure if it's because of my set-up or mesh size, would like to hear your opinions!

Project Purpose: Evaluating clamp plastic deformation over a period with a constant torque.

Constraints:

I have constrained only the rail as the fishplate which is the structure beside it is free moving and I would like the clamp itself to be able to deform.

DOF:

Load:

I have only applied a torque load to simulate a screwing force which would tighten the bolt, and over time cause plastic deformation in the clamp's base.

Contacts:

I used auto contact with separation contact type as separation to allow realistic sliding or separation under load.

Error: 

[henderh]

Hi @2203270EZLLQ,

Although the setup is in accordance to 'real life' I see a few issues with this approach, which is likely causing headaches for the solver. Simulation setups aren't necessarily always going to be 1:1 with real-life when we have to consider limitations inherent in the finite element method for any FEA simulation software.

1. It appears that it's expected the moment load will turn the shaft, and the threads will cause the shaft to advance to apply the force required to stress the structure. Unfortunately, this is asking the static stress solver to try to solve a dynamic problem (the shaft both rotating and translating with rigid body motion).
2. Often times, physically modeled threads could cause headaches for the mesher. In general, modeled threads should be removed, also (in most cases) they don't add significant stiffness to the structure.
3. If all contact types are changed to Separation, there's likely open degrees of freedom acting along the axis of the rail for all of the non-rail bodies. FEA solvers cannot handle open degrees of freedom since structure is not locked down, and 'statically stable' enough.
4. Having fixed constrains applied to all faces on the rail will cause the faces to be fully fixed in 3D space. Any compliance that body had is now essentially removed (i.e. now it has an infinite stiffness). Fixing only a cut end face should be sufficient.

What I'd try first is to get reasonable results using the linear static stress study type. Once you're happy with the results you can move on to the (sometimes more finicky) Nonlinear static stress study type to examine the plastic deformation.

The setup can be altered to remove the threads (in the Simplify workspace, to not affect the model in the Design workspace) by using the Remove Faces, or Remove Features commands. Instead of using a moment load, use a different 'load type' instead. You can cut a chunk out of the shaft and add Prescribed Displacements (equal in magnitude and opposite in direction) to the cut faces. Calculate the advancement using the formula:

• Thread Advancement = Torque / (π * Mean Thread Radius * Friction Coefficient)

I offer no guarantees this approach will work, they're just my 'hand waving ideas' from the images of the setup.

Hope this helps! Please let us know if you have any additional questions, comments, or suggestions.

[henderh]

I forgot to include a symmetry technique that will both constrain the model in the open DOF, and cut the computation time in half.

1. In the Simplify workspace, create a construction plane along the model's plane of symmetry
2. Use Modify > Split Body to cut through all bodies using the construction plane
3. Window select one symmetric half of the bodies > Right-click in the canvas > Remove > Finish Simplify
4. Add a Frictionless constraint to all faces created by the cut

Best regards,