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!

[Roland.Kalamar]

Any ideas? If I'm really off track with this, just give me a few tips or general direction, please.

Thanks in advance!

[TheCADWhisperer]

File>Export and then Attach your *.f3d file here.

What do you want to know from the analysis (be as specific as possible on desired information outcomes).

[Roland.Kalamar]

Thanks for trying to help, i attached the file.

For now i just want to simulate the clamping - for the lack of a better word, I am not a native speaker - of the pipe.

If i can set it up, i would eventually use this to determine the permissible forces and torques along all 3 axis, that i can apply to the pipe, without breaking the pipe support.

Assumption is that the base structure, where the whole support would be located, is totally rigid, hence the fixed constraint for the lower plate.

Thank you in advance!

[TheCADWhisperer]

I have a couple of concerns here.

You have relatively thin features for some of the components.

Linear elastic static stress does not return a measure of fracture - only indicates if component is with elastic range of stress/strain graph.

Can the assembly be simplified to a single component that you are interested in analyzing?

Which component is most important to you?  The pipe?

or

"without breaking the pipe support", the pipe support?

[Roland.Kalamar]

It may look thin, to be honest the loads that would occur would not be too large either. The forces i have so far applied stand for M8 bolt tightening forces, for example. I do know that the simulation assumes elastic behaviour even beyond the yield strength.

Further simplifying might be a good idea. I am basically interested in the support structure, as indicated in the line quoted by you. But that includes both the upper and lower part.

Also, i don't really know, how could i eliminate or replace the pipe itself, because that's what the support is holding, and that is the part where i should eventually apply further loads. So the shape, friction etc. of the pipe itself is important if I want to get a somewhat realistic result.

I hoped that it could work with just correcting some of the contact setups.

Thanks in advance!

[Roland.Kalamar]

Anyway, it seems to me, that the rod part that is pulled down is showing some unrealistic behaviour (and i mean both unrealistic compared to my expectations based on how i tried to setup the simulation and also to my expectations on the actual real behaviour). It is "sticking" to the lower part (?).

Could you maybe give some more help on this? I would have to proceed with this somehow but I'm really don't know what's wrong.

Thanks in advance!

[Roland.Kalamar]

Bump?

I am still stuck with this, please help 🙂

This doesn't seem to be a very complex problem, i just don't have experience with the setup of such simluations.

[Roland.Kalamar]

Another bump, (I still can't figure it out on my own)

[TheCADWhisperer]

Are you familiar with splitting faces for the purpose of applying loads/constraints?

[Roland.Kalamar]

I did raise a part of an otherwise flat surface sometimes in the past, to get the force act on a limited area only.

I am not sure if you meant something like that, or a more specific and effective method?

Also, how would i use this here? I am open to any idea you have.

[Roland.Kalamar]

Any more detail on what you meant with this? I have been working on some other stuff, but coming back to this problem, I am still stuck on this one.

[Roland.Kalamar]

Bump

[John_Holtz]

Hi @Roland.Kalamar 

What looks unreasonable to you?

I have not done any hand calculations to verify the results, but the pipe is behaving as I would expect.

I added constraints to the front face of the pipe and the bottom of the U-bolts (where the force is applied) to restrain motion in X and Y. Without these constraints, the model may be too unstable and go flying off into space. In fact, you can eliminate the separation contact between the U-bolt and the holes in the lower part. The constraints will simulate the contact between the bolt and the sides of the hole.

I also suggest that you delete the coefficient of friction. There is circumstantial evidence that friction is not supported in a static analysis, so I want to eliminate that as a possible factor in the analysis. If you need to include friction, you should use a nonlinear static analysis.

I will let you know if I see anything else.

[Roland.Kalamar]

@John_Holtz Thank you very much for your help!

I need to investigate the permissible loads for the clamp itself (I would add different loads to the short pipe later to determine what forces/torques coming from the piping are permissible for a certain type of clamp) so the important bit is not (just) the pipe but the clamp.

(What looked unreasonable to me was the high stress/displacement on the bolts lower parts, while nothing serious above the holes).

About the constraints:

Is the pipe constraint still usable in your opinion, if i want to later add loads to the pipe as well (as described above)?

What type of contraints are those applied to the bolts? For these it seems a little unintuitive to me to add constraint to a part that I am trying "pull" in this case, but i may be wrong...?

Friction:

I guess i will have to use friction' anyway later, when i will try to simulate longitudinal piping forces (as friction is the only thing keeping the pipe in place in that case.

Is it advisable to just switch to nonlinear? I am honestly not familiar with that, and don't know the main differences compared to static?

[John_Holtz]

Hi @Roland.Kalamar 

Here are the results of a linear static analysis without friction. These results are not as smooth as they should be, probably because the mesh is too large (and the warnings that indicated that it did not converge). It would be nice to have 2 elements through the thickness of the pipe wall.

My understanding is that you want to apply loads and see the pipe slip. The problem with that approach is that a static analysis cannot calculate a solution when the pipe slips! So the best that you can hope for is run an analysis with a load of A. If it solves, it did not slip. You increase the load to B, then C, then D. Once it fails to solve, you hope the reason is because it slipped at some load between the load that succeeded and the load that failed.

I think it would be as accurate and faster to do a hand calculation of whether the friction will hold the pipe. But this assumes that Fusion will give you the result that you want (the contact forces acting on the pipe), and I think that Fusion does not give that result.

If you want to proceed and find a philosophy that will give the answer you want, then these are the things that I would do:

1. Model the U-bolt and the strap that is bonded to the U-bolt as 1 piece. (This avoids using bonded contact between the two pieces.)
2. Setup a nonlinear analysis with friction. Constrain one end of the pipe in Ux and Uy (the horizontal directions). The load that is not restrained by the friction will be resisted by the constraints. (So you should be able to see when the reaction force changes as the indication that the pipe has "slipped".)
3. Cut the U-bolt short of the bottom bar.
4. Use a Bolt Connector between the end of the U-bolt and the hole in the bottom bar, and give it the correct preload. (Applying a force to the U-bolt is not correct because it ignores the increasing load in the U-bolt when the pipe loads try to move the pipe.)

Let us know what you find out.

[Roland.Kalamar]

Again, thank you very much!

I don't understand everything you wrote at first glance, but i will probably just try to follow your ideas anyway, as my own approaches have failed so far.

I will definitely get back to you with the results, maybe there will still be more questions than asnwers, but at least i have some new directions.

BTW i would use a finer mesh but it generally causes slow calculations rather quickly.

[Roland.Kalamar]

@John_Holtz 

I still can not get any result other than 'fail' with the setup you advised. The only difference that I am aware of is that i have not included the axial force yet, just the bolt connectors.

One thing is that the DOF view still shows the pipe as unconstrained, but i guess it is normal because Uz is not fixed?

The other warning shows that something about the material (steel) properties for nonlinear simulation is missing, this can be one reason why it is not working. Any idea on getting this out of the way?

(On a side note: nonlinear requires cloud solving, and it says i have 100 tickets left. Does it mean that if I were to  actually start doing successful simulations, i would have to buy tickets after that?)

Thank you for your time, again, i really appreciate it.

[John_Holtz]

Hi @Roland.Kalamar 

Can you provide the current version of your model?

You are correct that the DOF view is showing a potential problem because it only checks the constraints. It (probably) does not know about the contact, or at least not enough to know for a fact that the parts will be constrained by contact. (Even the solver does not know that the pipe is constrained by the contact until it performs the analysis and determines if all of the input parameters are sufficient to constrain the pipe.)

The material properties are not the problem. That is just an "FYI" that you are doing a nonlinear analysis, why are you not using nonlinear material? Maybe it's because you don't need nonlinear material. There are other reasons to perform a nonlinear analysis (like friction, large displacement, neither of which are related to nonlinear material properties.)

Yes, you will need to cloud credits to perform nonlinear solves.

[Roland.Kalamar]

So, red parts in DOF view should not be a problem in itself generally?

I attached the pipe support, it's basically a new file built using your recommendations.

But before you jump right into it: maybe the fact that there is no actual load yet (i have not included the axial force yet), just the bolt connectors, could cause a problem? I thought that the bolt connector can be seen as a load but maybe Fusion thinks otherwise.

(Otherwise, i see that nonlinear simulation uses 25 tickets (?) and i get that it's 100 USD per 100 ticket? If that's right this might turn into a costly endeavour very soon 🙂   )

Thank you again!