Can't get membrane only stress

[rlkillian]

I've modeled a large flat plate with a thickness of 0.1875". It's loaded with a uniform pressure normal to the surface and I used nonlinear static analysis with large deflection. I want to know the membrane only stress. I set EQVSTRESSTYPE to 2 and I also set DIRSTRESSTYPE to 2 separately and at the same time. The stress results are the same regardless of how they are set. How do I get this to show only membrane stress? I'm using Inventor Nastran 2023.0.0.23.

[dreierWTK29]

I have the same issue. Is there a solution?

[John_Holtz]

I think a nonlinear analysis only calculates the total stress since the stress through the thickness does not need to be linear (like in a linear analysis). Any portion of the thickness can yield which makes the stress distribution nonlinear.

If you want to create the equivalent of a membrane stress and bending stress, you can calculate it from two equations, two unknowns (applied to each of the stress results: X-Normal, Y-Normal, and I don't know about the XY-Shear Stress)

• Stress on top = membrane + bending
• Stress on bottom = membrane - bending

Those lead to membrane = (stress on top + stress on bottom)/2 and bending = stress on top - membrane. Once you have the membrane or bending stresses, you can then calculate the other stress results (von Mises, principal, etc) if it makes sense.

John

[dreierWTK29]

Thank you! The manual shows EQVSTRESSTYPE is only applicable in linear anaysis.

https://help.autodesk.com/view/NINCAD/2024/CHT/?guid=GUID-6D511A27-6CA5-46DF-91FF-73F5A1D6959A

For DIRSTRESSTYPE there is no hint.

Unfortunately I need to evaluate the membran stress of a complete cylinder / vessel and I cannot use your calculation for each element.

[John_Holtz]

Hi @dreierWTK29 

One question that comes to mind is can you use a linear analysis, at least as an approximation to get the membrane and bending stress? Why are you using a nonlinear analysis?

The calculations can be done for the entire model, but the question is whether it is worth the effort to do this. (Since it is nonlinear, you probably have multiple increments also, so the volume for the entire model, all steps could be huge, but fairly straight forward.) The steps are as follows:

1. Download the third-party app FNO Reader
2. Output the stress on the top and bottom of the shells to a text file. Use the workflow FNO to Table so that the top and bottom stresses are side by side. (To simplify the volume, perhaps you can limit the calculation to the centroid of the elements.)
3. Open the text file with Excel.
4. Do the two calculations per element to get the membrane and bending stress.
5. At this step, you can decide whether to just use the list of results in Excel, or if you want to write the results back to the results file (.FNO) so that you can view the results in Inventor. That can be done with the workflow List to FNO but takes a little more work. Since you are altering the results file, you want to use some caution so that it does not get corrupted. (Or create a new FNO file so that the original is not changed.) 

John

[Dr_Nastran]

So DIRSTRESSTYPE does not work in nonlinear analysis.  Whatever you set it to it will be ignored.   If DIRSTRESSTYPE is specified, EQVSTRESSTYPE will be set to DIRSTRESSTYPE.  These parameters were created for the Naval Maritime community using DDAM analysis.  Now there is a simple solution.  if you only want membrane stress in large displacement nonlinear analysis you can set the stress recovery points to zero.  

In Nastran plate/shell elements, if you want membrane-only stresses, set the stress recovery location through the thickness to the mid-plane / neutral surface.

In practical terms:

Set stress recovery points to:

z1 = 0.0, z2 = 0.0

So for membrane-only plate stresses, recover stresses at the middle surface, not at the top and bottom fibers.

[dreierWTK29]

Thank you! That sounds very promising. I would like to try this solution. Can you describe how to set the stress recovery points? Is it it done in the advanced option under stress recovery?

[dweinberg8290]

Yes.  You need to use the advanced options.  Just put in 0.0 for the Stress Recovery...Top Fiber box and Bottom Fiber Box.