Reply To: How to extract running loads and moments from SHELL181 elements in workbench?

[peteroznewman]

I struggle to get the FreeBody tool to work in FEMAP and it seems to have about as many steps as the Ansys process.  As a point of reference, I made a little 4 linear element model with a bending force on one side.  

Here is the Moment Result using the method I described above.  You can see that it is 5 in-lb about the local Y axis.

Thanks for the link to that post. I can now give you the steps for plotting the Element Moments you want.

 

1. Right click on Geometry and Insert Element Orientation, pick the body and define by the Global Coordinate System.
2. Right click on Analysis Settings, Output Controls, and set General Miscellaneous to Yes.
3. Solve (you might have to right click on Solution and Clear Generated Data first).
4. Right click on Solution and Insert a User Defined Result and type SMISC1 to get the Force11.
5. Right click on that User Defined Result and Duplicate Without Results, edit the Expression to SMISC2
6. Repeat four more times to get up to SMISC6.

 

Here it is with smaller elements.