Bolt connector Preload- Creating excessive unreal stress

[apatel4FM8K]

Analysis: Linear Static

Basics: Two members (L bracket and Plate) connected with bolt connecter with 4 holes, 9 mm clearance holes. 

Bolt connector: Picked edges of holes to create, Preload applied about 4500 lb. 

Constraints: One of a member has big surface, split a surface and added fixed constrain. (not near the load path)

Contact: Separation between two members. 

External Force: 1 lb., just for sake of running model.  (Adding external force increase stress more)

Meshing:  Generalized mesh and local control on bolt bearing surface area 0.08-inch mesh. 

Results: Max stress near the bolt surface area below bolt head, in the range of 300 KSI. 

Observed similar FEA on web running without any issues. 

https://www.youtube.com/watch?v=KpVdgtdCF68

https://www.youtube.com/watch?v=UAk9mUe9Ya4

Thanks for reviewing and your help. 

[apatel4FM8K]

@John_Holtz Hi John, noticed you have great knowledge in Nastran. Tagging you to refer to my query if you could help. Really appreciate it. 

[John_Holtz]

Hi @apatel4FM8K . Welcome to Inventor Nastran.

The answer is to ignore the high stress. It is not possible to get accurate results underneath a bolt head using a bolt connector. The bolt connector only gives accurate loads transferred so that other areas of the model are accurate.

Also see Why do stresses keep going up when the mesh is refined in Nastran. The issue with the bolt connector is similar.

John

[apatel4FM8K]

@John_Holtz Thank you for your quick response, John. 

The only thing I can't understand is why it's behaving normal for others as I attached in those videos?

We use Inventor Professional 2022.5.3, and Nastran version is 2022.3.0166. (Attached Screenshot)

[John_Holtz]

Hi @apatel4FM8K 

I so not have any experience with SolidWorks simulation, so I cannot comment on how they avoid high stresses where their bolt connector attached to the model in the Solidworks video.

For the Inventor Nastran video, I think it was created by frequent contributor @lucmartzz . To me, it looks like the legend scale was changed to cap the maximum value to 100.0 and 150.0 instead of showing the maximum stress of xxx.x. (From the ribbon, "Results > Options > Contour Options > Set Min/Max".) Also, the Min and Max markers are hidden to not show that the maximum result is xxx.x.

John

[apatel4FM8K]

@John_Holtz  Sounds good John. I'll neglect the stress below bolt heads in that case. Thank you for being responsive and providing information quickly, it does help a lot and saves my time. 

[lucmartzz]

@apatel4FM8K if you check closely my video you can see that I'm including a preload on the bolts setup, as mention by @John_Holtz  you can ignore those areas of stress. 

[apatel4FM8K]

Thanks for confirming @lucmartzz. Appreciate you all actively providing information here. 😊

[mpuckettXRFV8]

I have a follow up question that I think ties in with this.  I understand that the preload stresses can generally be ignored, but if I'm trying to do a non linear analysis with plastic deformation, I feel like this might be causing me issues.  Stresses that high are going to cause significant plastic deformation around the bolt head, which I think might be one of the reasons my analyses are failing to complete.  Is there a better way to model a bolted joint with preload in a non-linear analysis with materials that yield?

[apatel4FM8K]

Have you given try to any of these options. Just a suggestion, I haven't used them.

How to apply a bolt preload to a solid modeled bolt in Inventor Nastran

[mpuckettXRFV8]

Sort of.  I have tried using the "split bolt" (the third option on that link), but I ended up with so many contact surfaces and constraints that I had a different issue when trying to run the model.  I'm a bit worried that either of the other two options would have a similar problem.

Any my apologies, I meant to reply to the thread as a whole, not specifically to you, but I appreciate the response either way!

[lucmartzz]

@mpuckettXRFV8 

Are you expecting to see large deformation on your parts?

Best

Esteban.

[lucmartzz]

@mpuckettXRFV8 

For my tutorial I also ran nonlinear analysis to find out if the results was going to be different. (https://www.youtube.com/watch?v=UAk9mUe9Ya4) but I had no problems of convergence. 

[mpuckettXRFV8]

Guess that depends on what your definition of large. Maximum displacement should be less than an inch. Whole model is one corner of a chassis for a large truck though, so it's fairly small relative to the size of the model otherwise.

[mpuckettXRFV8]

I'll have to take a look and see. Maybe I can make a small simple model with just two plates bolted together to see what it does. Just seems like it would be really unhappy if I'm getting 600 ksi at the perimeter of the bolt holes and the material yields at 40k and full on fractures at 60k. Feels like Nastran would just keep stretching the material more and more, but I guess if it's compressive stresses and they are restrained by the plates opposite them that it could be less of an issue.

[John_Holtz]

Hi @mpuckettXRFV8 

I have never tried to reduce (or eliminate) the stress at the bolt connector. These may help or not help enough.

• Does refining the mesh around the bolt hole help? That would create more spokes around the perimeter of the hole which should help distribute the load better.
• Does splitting the face around the hole help? Kind of like creating an imprint of the washer on the face of the solid. Then when defining the bolt, select the "washer" face instead of the edge of the hole. Is the bolt load transferred better?
• The stress concentration may be detrimental for the convergence, but the degree of plasticity may be lower than you would think. If the high stress is at one corner of the element, the centroid and other corners may not have yielded. Even if the corner (or more nodes) do yield, the amount of plasticity depends on the stress-strain curve after yielding. Usually there is some slope to the stress-strain curve, so the stress and strain can continue out to infinity; that is, there is no fracture in a nonlinear analysis.

John

[mpuckettXRFV8]

I'll have to give those a shot and see, thanks for the tips! As a bit of a secondary question, how important is preload as far as analysis anyway? Could I just run the simulation without preload and check the forces in the bolt connections to see if they are higher than the preload I would typically put on the bolt? I got the impression the bolt connector effectively acts like a "bonded pin" or something to that effect, so wondering if maybe I could just run the simulation with to start with to see if that helps any.

[apatel4FM8K]

John can explain more, but my two cents, you want the bolt connectors with applied preload. Applied preload changes the stiffness of your Joint connection & assembly, allowing the load to transfer to your members and not fully pass the load on the bolts.

You can find the max preload to be applied by considering proof load of member/bolt and factor it for temp or permeant connection. That gives you max stiffness in the assembly without yielding anything, allowing the stress to distribute amongst members.