Max Mises inconsistent when opening .odb or reading with script 1

[SteffenB]

I'm doing a simulation combining Beam and Shell sections, using the script provided in the following link (I've also seen it in this forum before) to find the maximum value of von Mises stress.

http://130.149.89.49:2080/v6.7/books/cmd/default.htm?startat=pt04ch08s10.html

However, the result this script outputs differs from the information I'm getting when opening the .odb manually, viewing the results. In my case, when opening it manually in the Abaqus GUI I'm getting roughly 229MPa, while the script outputs about 241MPa.

The step and frame displayed in the GUI are the same in which the script finds the maximum stress value.

Does anybody have an idea what could cause this difference in output?

I've attached an example .odb in which this occurs. If any files or code would actually help, I'm happy to provide.

 

[Mustaine3]

The script uses that data in the elements. The contour plot in A/CAE extrapolates the values and averages them at the nodes. This could introduce a difference. Look first at the unaveraged data. See Results -> Options -> Averaging

But I think in your case it's coming from the section points of beams an shells. The contour plot uses a default section, but the max result could be in a different section. So switch the sections. Results -> Section Points. Or use the Envelope plot in this menu.

 

[SteffenB]

Hello Mustaine3,

thanks for your great input, I learned something new.

I had to change to the "Envelope" section to see the actual max stress, you were on point.