SimScale CAE Forum

Nut Staking Tool


#1

Can I please get some help with the project below? I keep getting a “The solution matrix is not factorizable” error. I don’t know what else is needed to eliminate the rigid body motion.

Nut Staking


#2

Hi @cschmidt!

Will have a look at your project later on. I am tagging my colleagues from the @PowerUsers_FEA here who might help you in the meantime.

Best,

Jousef


#3

Hi @cschmidt,

I think your problem is coming from the fact that you have a gap between your parts in combination with a force driven boundary condition. The solver is not able to find a solution because there is nothing resisting the load (at least in the initial state).

There are a few things you can try:

  • Add an elastic support to the moving part. This will give the load something to push against until contact is made with the other body. You want the spring stiffness to be high enough to allow the solver to find a solution but low enough that it does not have a significant influence on the results.
  • Add a fictitious clearance between the parts to artificially close the gap. This option can be found under the physical contact definition.
  • Modify the geometry so that there is an initial contact (or slight overlap) .
  • Change the force driven boundary condition to a displacement driven boundary condition. The displacement driven boundary condition does not need a resistance to solve.

General tips:

  • In general I think you will find it difficult to solve this simulation because of the nature of your physical contact. You have two very sharp edges coming into contact with each other. I expect it will be much easier to solve with a small landing on both parts.
  • With non-linear simulations it is best to define your loads (force or displacement) as a function time. This way the solver can ramp the load gradually for a more robust solution.

Here is one example of a first pass approach.

I hope this helps.


#4

Thanks Ben for the suggestions. I really appreciate your help with this. You gave me some great observations that I never knew had an impact on the solver reaching a solution. The only concern is the 10000 lbf/in elastic support. This seems almost as high as the 2000 lbf at the given deflection. How can I trust the results with this much support?


#5

Hi @cschmidt,

You are right that the elastic support load (1,300 lb) is quite high compared to the applied load (2,000 lb). You can substantially reduce the elastic support load by reducing the gap between the two parts.

You could also try increasing the size of the applied load (1300 +2000 lb) to overcome the elastic support load so that the load transferred to the nut is the 2000 lb you require.


#6

Okay, now I understand thank you.