linear static calculation with separate contacts

[Anonymous]

Hello everybody,

I am new here and have already done some calculations with Nastran In-CAD. 
In the past, I've calculated much of the software built into Inventor.
In Nastran In CAD, I would like to perform an assembly with only separate contacts a linear static calculation.
But I get wrong reaction forces and deflection.
A 1/4 assembly connected to separate contacts rests on a steel beam.
The assemblyy is loaded with a force (2943 N). Here I use symmetrical boundary conditions in two directions. The steel beam is fixed. The module is made of PP.
I want to determine the maximum deflection of the assembly (estimated 10-12 mm).
I discovered the problem. 
WARNING E5034: NO CONVERGENCE IN MAXIMUM NUMBER OF ITERATIONS PERMITTED
My model is not stable enough due to separate contacts. 
According to the nastran help, I am to use grounded springs to stabilize the model. 
I understood the theory, but I do not know how to implement it.

Can someone help me please? I attached the model.

In the Inventor integrated FEA program the spring will be added automatically.

Regards
V. Becker

[Anonymous]

Hi Becker,

I am currently working on a similar situation where I have to apply grounded springs to my assembly but I have not succeeded to do this either. 

I hope there is someone here that can help us!

SSC

[Anonymous]

Maybe this image will help:

Be sure you hit the "Advanced Options >>" button and add some stiffnes to the first three degrees of freedom for a solid model. K1, K2, K3 means translation in X, Y and Z.

[Anonymous]

Hi Michael,

thanks for your answer.

I found this option and tried it, but it did not do much.

I did not know exactly where these points shoulde be most meaningfully in my model.

What should I pay attention to when positioning the springs or points?

Thanks in advance.

Regards

[Roelof.Feijen]

I ran the analysis you attached without changing anything.

It solve without any problem. See displacement results below.

[Anonymous]

In your case there is no need for soft springs because of the symmetry constraints. I ran the analysis of your model and had no fatal error and the warnings are not critical. Displacement is about 1mm, max. Von Mises stress is about 35 MPa.

But there seems to be somthing wrong with one of the contacts though. I guess the plain face of the support should be the contact face and not the rounds.

[Anonymous]

Hello Roelof,

thank you for your answer.

The calculation works by me too. however, if you look at the reaction forces in y direction, you will find that they do not match the load.

In addition, symmetrical boundary conditions are set in both direction, so that the assembly must not bend in the middle as in your picture. Deflection must take place at the symmetry plane.

At a load of 300 kg i expect a deflection of 10 mm on a 1/4 plastic assembly.

This is because a plastic pallet is simulated in a rack.

I believe that I need something like soft springs as that is automatically used in Inventor stress analysis.

I also tried this option:

"I've found such a function in Nastran parameters called "INERTIALRELIEF".

When You select "Auto" then software will find and eliminate rigid body modes.

Obviously it's working only in Linear Static Analysis when applied loads are in balance."

but without success.

[Anonymous]

Hi Michael,

thanks for you answer.

I calculated another design using Inventor stress analysis (see Appendix). The design consists of the same components, material, connections, boundary conditions and load. There are only a few holes more on the top of the part to reduce the weight. And I get the right reaction forces and also an expected deflection.

I saw also that Inventor stress analysis used soft springs during the calculation.

Regards

V. Becker

[Anonymous]

Hello all,

does not have an idea? 😞

regards

[Anonymous]

Hi Becker,

I ran your example file and have seen that the reaction forces are different than the load (a lot smaller).

However, when I use glued contacts instead of separate contacts, the reaction forces seem to be OK. In this case, also the displacement results are as you describe (10-12mm).  

Unfortunately I was also not able to get these results using separate contacts 😞

CT

[John_Holtz]

Hi @Anonymous 

I am looking at your model. I added grounded springs to make sure that each part was statically stable, but that did not solve the discrepancy between the applied load and the reaction force.

I will let you know what I find out.

[Anonymous]

Hi @John_Holtz,

thanks.

I found this article and tried it. Until now still without success:

https://knowledge.autodesk.com/support/nastran/troubleshooting/caas/sfdcarticles/sfdcarticles/Nastra...

I hope you will have more success.

Thanks in advance.

Regards

Becker

[shigeaki.k · Accepted solution]

Hello @Anonymous ,

for now please could you use nonlinear static analysis. I am not sure if the issue is from the way contacts are behaving in linear static, from the fact that you are trying to run linear static analysis when the problem is nonlinear (i.e. large deformation) and changing contact status or any other reasons.

I go with the basic rule I learnt in my FEA courses. If the contact status is changing, treat it as nonlinear. This is albeit Nastran allowing for such behavior on a very small scale).

Below are the screenshots of the results. The Fy force and reaction are comparable. 

I will attach the nonlinear analysis model shortly. I removed all the local mesh and ran the analysis. 

Regards,

Shigeaki K.

-----------------

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[shigeaki.k]

Attached is the nonlinear static analysis model.

Regards,

Shigeaki K.

-----------------

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[Anonymous]

Hi @shigeaki.k ,

yes that works. many thanks.

I could use this method first as an alternative solution.

It would still be nice to know how to use "soft" spring in Nastran In-CAD.

Regards

Becker

[John_Holtz]

Hi @Anonymous 

The grounded springs are not the solution.

I do not know what the mathematics are doing, but the problem is somehow related to the gaps between the faces that are in contact. (Even if the CAD model is theoretically in perfect contact, the approximation due to the meshing can create gaps.) The solution so far is to change the Penetration Surface Offset on each of the contact pairs. This hypothetically creates an interference, but the solver removes it when creating the contact (and generates the G3051 warning about moving the slave nodes).

I tried it on your model using a coarse mesh (20 mm mesh size everywhere), so the analysis runs in a few minutes. The reaction force was 2927 compared to the applied load of 2943. (I still had the grounded springs on the model, so they should be absorbing the rest of the applied load.)

Please try increasing the Penetration Surface Offset on each of the contact pairs in your original model. I used a value of 1 mm.

Note that the mesh on the "support" does not need to be fine. You can use a really coarse mesh on it. (I assume you don't care about the stress in the support, so it does not need a fine mesh to give accurate results.) You may want to use a Maximum Activation Distance on the contacts of 10% to 20% larger than the largest mesh size on each contact pair.

[John_Holtz]

Hi @Anonymous 

I wanted to check if you have tried the suggestion of changing the Penetration Surface Offset in your original model. If so, what was the result?

[Anonymous]

Hi @John_Holtz ,

I am on a business trip this week.

I will post my results here at end of the week.

Thanks in advance.

Regards

Becker