topic Re: Mesh convergence DOES NOT CONVERGE in Inventor Nastran Forum

Mesh convergence DOES NOT CONVERGE

Anonymous — Tue, 16 Nov 2021 17:37:08 GMT

So, I am inputting different element sizes and the smaller the element size, the larger the max stress value. Not only that, ALL stress values increase and I have no clue as to why. No one I have spoken to has had this issue happen to them. The max stress value is meant to be converging with a decreasing element size (or an increasing number of elements, same thing) but mine doesn't, it basically linearly increases when I put the results in MATLAB and plotted them out. Someone please help asap. Thanks.

Re: Mesh convergence DOES NOT CONVERGE

John_Holtz — Tue, 16 Nov 2021 19:11:14 GMT

Hi @Anonymous

I agree that it should converge.

In fact, it does converge when I sketch around your outline and create my own shell model.

Convergence Plot

The stresses from the coarse mesh and fine mesh also agree in my situation. Other than the discontinuity in the center of the hook, all the other contours line-up to within a pixel or two. (Here is a composite image where I overlaid the 0.35 mesh size result on the 0.1 mesh size result. The contour range was set to the same range for both plots.)

Contour plot comparison

I suggest that you check your log file for warning messages. Also, check the reaction forces to confirm the different meshes have the same load. (Right-click on the constraint > SPC Summation.) If you do not find a reason, feel free to attach your model (the .ipt file).

Re: Mesh convergence DOES NOT CONVERGE

Anonymous — Tue, 16 Nov 2021 20:29:48 GMT

Here is my model. My lecturer suggested to just do Mesh Control on the edge where the max stress is located and do the convergence that way, but it still does not converge. I have everything at 1mm and that edge at smaller values of like 0.1mm and even 0.05mm, but it gets extremely distorted and the elements do not represent the model accurately in my opinion because they are distorted so much.

Re: Mesh convergence DOES NOT CONVERGE

Anonymous — Tue, 16 Nov 2021 20:38:06 GMT

By the way, I am using Inventor and Nastran 2022

Re: Mesh convergence DOES NOT CONVERGE

John_Holtz — Tue, 16 Nov 2021 21:15:36 GMT

Hi @Anonymous

Your convergence graph appears to be based on the centroidal stress. Why are you using the stress at the center of the elements?

You have the equivalent of a beam in bending. The bending stress is linear from the neutral axis to the surface. By measuring the result at the center of the element, and by changing the size of the elements, you are measuring the stress at different distances from the neutral axis. You do not want to do that!

You should be using the corner stress since the corners are on the surface of the model and therefore at a "consistent" location. When you use the corner stress results, the convergence is very tight.

Technically, this graph may not be accurate either. I used the "maximum" value from each mesh size. If the location of the maximum result changes, then you have the same problem as before. (However, the variation of the stress over a small area of the surface surrounding the maximum point is very small.) In order to do a proper graph, you should split the model near the area of maximum stress, and then plot the stress at the node that is always at the split versus element size.

Hope this helps and you pass your test. 🙂

Re: Mesh convergence DOES NOT CONVERGE

Anonymous — Tue, 16 Nov 2021 21:25:55 GMT

Thanks a lot, this is just a coursework and EVERYONE I spoke to got results of like 2mm and our models are similar, I don't know why mine is doing this, we are all using the same method, just taking the max von Mises stress and we don't care where it is because eventually two results will be identical and at basically the same location.

However, my results differ from yours, I am getting 172.3 for 0.3mm and 173.6 for 0.2mm, which clearly won't match your graph if you extrapolate, I don't know how your values converge, mine keep going up and up and up. I don't know how to not take the measurement from the centre, we weren't told how to do this. All I'm doing is taking the max stress, I don't really care where it comes from, this is not meant to be that in-depth. How did you get those values???

Re: Mesh convergence DOES NOT CONVERGE

John_Holtz — Tue, 16 Nov 2021 21:26:07 GMT

Good question. You edit the contour plot -- "Results > Options > Data Type > Corner" instead of "Centroid".

I think one of your friends secretly changed the setting on your computer. 😁

Re: Mesh convergence DOES NOT CONVERGE

Anonymous — Tue, 16 Nov 2021 21:30:18 GMT

Wait WHAT?!? Is this the default setting?? How tf did my PC have it as centroidal????? I just watched my lecturer's vid and it's corner on there as well WTFFF I've been here about 7 hours trying to fix this... So what exactly is the difference between the two?? And why was mine set as centroidal?

Re: Mesh convergence DOES NOT CONVERGE

benoit.neu-faber — Wed, 17 Nov 2021 07:01:39 GMT

Hi Christos,

Here you can find information about this topic

Hope this Help.

Please accept solution and give likes if applicable

Benoit Neu-Faber

INNOSIM https://servicesmarketplace.autodesk.com/provider/public/innosim

Autodesk Service Provider / Simulation Expert

https://www.linkedin.com/in/benoit-neu-faber/