Separation Contact during Linear Static with Pre Load Analysis

[Anonymous]

Hello everyone,

I'm currently performing a linear static analysis with preload. What I found out was that, in the second subcase, the separation contacts became bonded. Is this how the algorithm is written or have I made an error in setting up the contact. 

Thanks for the help,

Prasanna

FEM model showing the contactsLinear static Analysis - Deformation of the body in red. Where it sepatates from the body in yellowLinear Static Analysis with Preload. The body in red does not separate from the body in yellow even when the boundary conditions remain constant.FEM Model with the Bolt in place

[shigeaki.k]

Hello @Anonymous ,

could you provide further information such as which version of Nastran In-CAD or Inventor Nastran you are using, the workflow, and the type of analysis you are conducting. You mentioned that you are running linear static but I am not clear on how you are setting up a preload with multiple subcases.

Regards,

Shigeaki K.

[John_Holtz]

I assume the preload is coming from the bolt.

I just did a simple test with version 2020. Two parts, one bolt, separation contact between them, and two subcases. The parts were able to separate in both subcases. If you open the log file with Notepad, you should see lines that indicate the analysis is performing iterations during both subcases, such as this:

• LINEAR CONTACT SOLUTION FOR SUBCASE 1 ITERATION 1
• LINEAR CONTACT SOLUTION FOR SUBCASE 1 ITERATION 2
• ...
• LINEAR CONTACT SOLUTION FOR SUBCASE 1 ITERATION M
• LINEAR CONTACT SOLUTION FOR SUBCASE 2 ITERATION 1
• LINEAR CONTACT SOLUTION FOR SUBCASE 2 ITERATION 2
• ...
• LINEAR CONTACT SOLUTION FOR SUBCASE 2 ITERATION N

The iteration number will increase for the first subcase until it converges, and then it repeats for the second subcase.

Also, check to make sure there are no warnings such as "failed to converge". It could be that the second subcase did not get to the final result and is outputting an invalid solution. (Invalid as in some points are in tension instead of converging so that no points are in tension.)

[Anonymous]

Hi @shigeaki.k ,

thanks for the reply. Unfortunately last Thursday was a bank holiday here in Germany and hence we were off for the whole week. 

I'm using Nastran In-CAD 2019 2.0.288

Autodesk Nastran 2019 13.2.0.168

I performed the linear static analysis with preload.

I gave the bolt details in the connectors part.

In the first subcase, I gave the boundary conditions such as the frictionless contacts and pin contacts. 

In the second subcase, I used the same boundary conditions and to that, I gave an additional rotational speed.

I hope I've answered your question.

Regards

Prasanna

[Anonymous]

Hello @John_Holtz ,

thanks for your support.

Sorry for the delayed reply. We had a long weekend in Germany last week. 

I checked the warning messages as you suggested, and I received the following warnings

WARNING AND ERROR MESSAGE SUMMARY

WARNING G3012: - ELEMENT - HAS A SKEW ANGLE GREATER THAN - (165)
WARNING G3015: - ELEMENT - HAS AN INTERIOR ANGLE LESS THAN - (855)
WARNING G3016: - ELEMENT - HAS AN EDGE POINT RATIO GREATER THAN - (18)
WARNING G3051: MODIFYING POSITION OF SLAVE GRID - ON CONTACT ELEMENT - (7594)
WARNING G3057: PART PROPERTY - HAS ZERO MASS (2)
WARNING E5009: - ELEMENT - IS NON-POSITIVE DEFINITE (2)
WARNING E5016: LOAD SET - DOES NOT EXIST (1)

 And I did not get any FAILED TO CONVERGE error

I've also attached the Log file!!

Regards,

Prasanna

[shigeaki.k]

Hello @Anonymous ,

hard to say without looking at the model... Are you able to share the model?

Regards,

Shigeaki K.

[John_Holtz]

Hi @Anonymous 

The log file that you attached indicates that there is only 1 subcase in the analysis. Perhaps you attached the wrong log file? Or is In-CAD somehow showing results for a second subcase that doesn't exist? 

[Anonymous]

Hi @John_Holtz 

sorry my mistake, I sent you the LOG file for the analysis where I just performed a one-step analysis.

I'm sending you the correct LOG file now.

Regards,

Prasanna

[John_Holtz]

Hi @Anonymous 

You have a few warnings that I am not familiar with: E5009 Element is non-positive and E5016 Load set does not exist. (Maybe I need to start checking my log files more closely .)

Can you provide the model to us? Zip/rar/compress the part files (.ipt) and assembly files (.iam) is what we need. If there is more than one assembly, please indicate which file we should open.

[Anonymous]

Hello @John_Holtz ,

we had a long weekend here in Germany. Couldn't provide you with the model earlier. Can you provide me your E-Mail so that I can send it to you? I'm not sure if I'm allowed to post the link publically.

Regards,

Prasannna

[John_Holtz]

Sorry @Anonymous. I missed the fact that the analysis type is Prestress Static. I just did a test model using a prestress static analysis with a bolt and separation contact, and both subcases show that the separation contact was treated as bonded contact.

My suspicion is that prestress static does not handle separation contact, just like a direct transient analysis does not handle separation contact. (Faces with separation contact held together in a linear analysis in Nastran) I think that only "linear static" supports separation contact.

I will check with development to see if this is true.