Stress simulation contact setup

[Roland.Kalamar]

Dear all,

I am a beginner at Fusion 360 simulation. I have a little problem with contact setup:

What i want to simulate is a pipe support, that consists of an upper part, (made from a bent threaded rod and a bent flat steel) that is bolted to a lower part (basically a flat steel). The pipe is located between these components. See attached picture "Pipe_support".

First off i would like to just simulate this tightening of the assembly, (then, if i manage to do this, i would add some other loads on the short pipe section).

So far i have simplified the model to just the basic parts, and two downward forces acting directly on the upper part (I am interested in the behaviour of the upper part and pipe, not in the detailed results regarding the bolt connection itself). See attached "Pipe_support_simplified"

The lower plate is fixed, but all other contraints are the contacts set up between the components. These are bonded connections for the bodies that would be welded together (bent rod and bent flat steel) and separation for the other contacts.

I wonder if this is even the right approach to this at all, because - while it seems logical to me - the "DOF" view shows the pipe and upper part as "free", and just the fixed lower part as totally contrained (green). I don't know if this is an actual problem for the simulation?

So far it gives me a result that seems unrealistic (see "Pipe_support_result" . It's as if the holes in the lower part would really restrict the downward movement of the rod, even if there is a 0,5 mm clearance between them and the contact type is set up as separation, with 0,2 friction coeff..

I would really appreciate some help on finding the way to simulate this. I have either approached this in a wrong way, or maybe just couldn't set up the contacts to work properly?

Thank you very much in advance!

[John_Holtz]

Hi.

I have just downloaded the new model, so I will have some better answers later. But here are some replies to your comments.

"So, red parts in DOF view should not be a problem in itself generally?" That is correct as long as you know that contact will constrain the "free" parts. Of course, if you missed defining one of the contacts and a part becomes free to float off into space, that would be a problem.

"I thought that the bolt connector can be seen as a load but maybe Fusion thinks otherwise." I think there is a 50-50 chance that you are correct. 😊 It depends on what the error is and when it occurs. If my memory is correct, the solver does not require a load to be applied. It will happily calculate results of 0, or in this case, the constant result due to the bolt preload. If the error occurs before the solver starts the actual analysis, it could be because Fusion is detecting that no "live loads" have been applied. If the error occurs during the actual solving phase, then the problem is something else and needs to be determined from the error message.

"I see that nonlinear simulation uses 25 tickets (?) and i get that it's 100 USD per 100 ticket?". Yes, simulations on the cloud do require tickets. However, you should only be charged when the analysis succeeds. Failed analyses do not provide any results, so you do not get charged for those.

[John_Holtz]

Hi @Roland.Kalamar 

The initial problem is that there are too many contact elements being created. The model may "look small" (meaning the number of nodes and elements is not too large: 137k and 80k), but the contact elements are way over 11 million elements! To minimize the number of contact elements, the maximum activation distance should be specified. (In other words, you know what is needed in the analysis better than the software!) I am trying these settings:

• Pipe to plate: maximum activation distance = 4 mm 7 mm. (As the pipe compresses, some areas not initially in contact may come into contact. You need elements between these nodes to detect that contact.)
• 3 contact pairs between the pipe and Ubolt = 4 mm. (It looks like the mesh size is approximately 3 mm. When there is no relative sliding between the parts, the maximum activation distance only needs to be 10% to 20% larger than the mesh.)
• (new) I added gravity load just in case the solver wanted a load to be applied.
• (new) I changed the contact between the top of the Ubolt to the pipe from symmetric to unsymmetric. I did this just to reduce the number of contact elements to get the analysis to solver faster.
• (new) The analysis was still having problems converging just because the bolt preload is applied at time 0, so it takes a lot and lot of iterations to get the contact all figured out. There is not much that you can do in this situation other than let it run. Instead, I reduced the bolt preload from 1.05E4 N to 1.05E2 N. The analysis ran in 33 minutes.

I will edit this message as I make progress.