Post-processing issue

General Questions
1

Good morning,

I am doing a certain analysis that requires to export stress values.
I created an element set where the max Von Mises is. After the analysis I see in PrePoMax the location of the max value VON MISES, which is 820 MPa. It is located on the surface.

Then, I exported the stress values of the element sets where the max value point is. I exported the stress tensor in Excel and then I added a column where I wrote the general Von Mises formula. But, when I use the MAX function, it finds 927 MPa.

image
image1157×103 29.6 KB

Assuming that the von mises formula is written correctly, what could be the issue?

Thanks

2

Don’t assume this, double-check the formula used in Exel, especially the brackets.

3

I checked and rewrote the formula,but it seems to be correct.

image
image932×205 13.4 KB

4

Can you share this Excel file ? It will be easier to help.

5

A+B_12_28_22 - Copia.zip (1.8 MB)

Here it is the Excel file.
Thank you

6

Those are the stresses from history output save to .dat file, they are taken directly from integration points. Field output displayed as contour plots in PrePoMax is obtained differently - those are averaged nodal stresses and hence the difference.

7

How can this problem can be solved? I Mean, it’s a big difference in values.

8

It’s a standard problem in FEA. In fact, we usually look at both average and unaveraged stresses and check values directly at integration points to check the correctness of results. Such differences may indicate erroneous stress peaks. Check this region (around element number 78300) and see if there is any suspicious behavior there. Local mesh refinement in this area may help.

2 Likes
9

Thank you. So, what is ‘‘more correct’’ to take into account? For example for a fatigue analysis?

10

Fatigue analysis software typically uses nodal stresses from the surface of the component.

11

So, the one displayed on PrePoMax

12

@FEAnalyst
Hi Jakub, i think in PrePoMax it is Not possible to show averaged and unaveraged Stress, or isn’t it?
Maybe this would be a nice tool in Future?

Because often a huge difference between averaged and unaveraged stress indicates a to coarse mesh. Therefore the comparison is useful for mesh validation.

13

See CalculiX-Examples/Linear/Separate at master · calculix/CalculiX-Examples · GitHub for a way to obtain non-averaged solutions. It actually duplicates nodes such that no node is shared by more than one element. Mesh continuity is enforced by appropriate equations.

The helper script CalculiX-Examples/separate.py at master · calculix/CalculiX-Examples · GitHub is the key element in the workflow. Integration in PrePoMax would imply;

  • export input file with nodes and elements
  • run separate.py
  • replace the original mesh by the generated files (nodes, elements, equations)

This can be done as the last operation before actually running the input file.

It might be worth the effort to restrict the separation to certain regions (node or element sets) to mitigate increase of output file size.

1 Like
14

Hey,

I had a similar issue not too long ago. I did a simple analysis with a material model with complete yielding at yield stress. The model showed stresses above yield stress, which i found odd, but i then created a history output of the stresses and saw that no value went above yield stress.

See my post: Load variation in non-linear material problem - #15 by mkraska

1 Like