Inventor 2013 - Stress Analysis: Thin Bodies

[dhankin]

I am having a problem with moments applied to my stress analysis model when using the thin wall bodies feature. See attached file. When I use solid elements I get sensible results, but if I use the thin bodies feature I get nonsense results. If I remove the applied moments then the thin walled results are OK, so it seems the applied moments are causing a problem. I'm sure I have applied the moments correctly since I use the same moments in the solid model.

Any help would be much appreciated.

Regards,

Dave

[raviburla]

Hi,

I looked into the model. The results for solid and shell are very close to each other. Were you seeing something different?

Thanks,

Ravi Burla

[dhankin]

Hi Ravi,

Yes, the maximum displacement is quite similar, but the distribution of displacement is very different. However, I'm mainly interested in the von Mises stresses. For the shell model the max VM stress is 997MPa at the tip of one of the legs, in the solid model it is 153MPa at the joint between the leg and the main can. The solid model result is what I expected, the shell model result doesn't make sense to me. See images below.

Thanks,

Dave

SHELL MODEL

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

SOLID MODEL

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

[raviburla]

Hi Dave,

Thanks for the details. I now understand the issue you are concerned about. I was also able to create a simplified model which reproduces the behavior. We will log this issue in our system for tracking purposes.

Thanks,
Ravi Burla

[dhankin]

Thanks.

In my company we are just starting to use the stress analysis module, as an alternative to Ansys which is much more expensive. This problem has shaken our confidence in the accuracy of the results. Can you notify me when this problem is resolved? Should I accept your last reply as the solution?

For the time being it appears I can use the solid model rather than the shell model. Can you confirm that the solid model will give valid results? I used the shell model because it was recommended by Inventor - is the purpose of the shell model only to reduce computing time, or is there a problem using solid elements for thin bodies?

Regards,

Dave

[raviburla]

Hi Dave,

I have experiemented with Autodesk Nastran In-CAD our other offering for stress analysis with Inventor. I am getting similar results as was obtained with the Stress-Analysis Addin. So I am thinking that this behavior is specific to shell model in this example.

Autodesk Nastran In-CAD is based on the Nastran solver and provides lot more capabilities than Inventor Stress Analysis. You might want to consider this package as well.

We have performed several benchmarks and we believe that the solutions provided by the Stress Analysis Addin are accurate. 

Thanks,
Ravi Burla

[Anonymous]

I am also struggling with thin bodies in Stress Analysis, but discovered a characteristic that seems to me a bug. I am also very curious about possible differences between solid bodies and shells. Could you send me your both your solid part and you shell part as a zip-files with the stress analysis files included. Regards, Wim.

[Anonymous]

It looks to me like FEA is doing what you and the original poster are asking.

In the 3d model the moment is applied to the end face of the tube.

The thin plate model is treating each linear element at the end of the tube so is applying a moment to each element individually.

Richard

[raviburla · Accepted solution]

Hi Dave,

Our internal experts have looked into this in detail and here is the explanation for the observed behavior:

The solid and shell results are identical as originally modeled. Need to change the stress legend to Max=100 MPa to see it.

The only difference is localized effects on the edges of the shells where the moment was applied because these are applied as nodal moments. These effects dissipate a few elements in and produce results in the main body that match expectations.  

Stress Analysis is converting the moment load into a more distributed load since solids don’t understand nodal moments. This is done by transformation of moment load into a linearly distributed load which is equivalent to the applied moment. 

An important point is that the loaded tubes show large sectional distortion. This is unlikely to be real. I’d expect these moments represent loads from pipes that should be attached.  They would reinforce the local shape. Rigids in In-CAD would produce a much better local result.

I am also attaching the ppt with the details.

Thanks,
Ravi Burla

[dhankin]

Sorry, but I'm out of the office now for 2 weeks for Christmas, and I don't have access to the files. The original ipt file that I posted should have everything you need, to convert to solid you just need to delete the mid-surfaces.

[dhankin]

Thanks, I understand now what's going on. I think I need to modify the model and come up with a better way of applying the moment.