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.
Mesh convergence DOES NOT CONVERGE
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.
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.)
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).
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. 🙂
