Extracting stress in intersecting points of bodies 1

[BTHS]

Hi

I've setup this model in Ansys workbench. It's a 2D model, and it has been sliced and combined in Designmodeler to make the mesh comply to the specified lines. I would like to extract the stress in this intersection (Marked by the two green dots), but i'm getting an error: "You have a result that is attached to an entity shared by more than one body. The solution cannot proceed until this is fixed.". I could choose to select the nodes and that works, but as this is a parametric model where the geometry changes this method breaks down. See photo below:

Best Regards

 

[scheah]

Hi BTHS,

Would this work for you?...

Step1: Create name selection 'line1' and 'line2' in DesignModeler/SpaceClaim. These lines share that one node of interest.
Step2: Add Post Command Snippet below:

! Find node of interest
cmsel, s, line1
cmsel, r, line2
*get, nodenum, node, 0, num, min

! Use your *get function. An example below. 
/post1
set, last
*get, my_sout, node, nodenum, s, eqv

Step3: Create parametric results argument in "Details of Command Snippet": my_sout


Best regards,
Jason

 

[BTHS]

Hi Jason

Thank you for a fast and accurate response.

I modded the code to exactly fit my purpose:

! Find first node of interest 0.4*t from the weld
cmsel, s, line1
cmsel, r, line2
*get, nodenum1, node, 0, num, min

! Find second node of interest 1*t from the weld
cmsel, s, line2
cmsel, r, line3
*get, nodenum2, node, 0, num, min

! Use *get function to acquire 1st principal stress in selected nodes
/post1
set, last
*get, HS_04, node, nodenum1, s, 1
*get, HS_10, node, nodenum2, s, 1

It is working very well. One thing i noticed was when i wanted to edit the "Par" name in "*get, HS_10, node, nodenum2, s, 1" i had to also change the output search prefix to HS_ .

 

[BTHS]

One problem i have is if i have to change the code and rerun the analysis i get this error:

"The solution was executed using only post commands information. Check the Post Output on the Solution Information object for more details"
​

My it can be fixed by clearing all result data and rerun analysis, but the method seems a little rough. Is there a more smooth solution to this?

Best,
BTHS

 

[scheah]

BTHS,

The problem could be due to the DB file not automatically saved so it's complaining no named selection exist.

Try the following:
Step1: Set "Analysis Settings>Analysis Data Management>Save MAPDL db" as "Yes".

Step2: Modify your Post Command Snippet:

finish
resume,file,db
/post1
set,last

! Find first node of interest 0.4*t from the weld
cmsel, s, line1
cmsel, r, line2
*get, nodenum1, node, 0, num, min

! Find second node of interest 1*t from the weld
cmsel, s, line2
cmsel, r, line3
*get, nodenum2, node, 0, num, min

! Use *get function to acquire 1st principal stress in selected nodes
set, last
*get, HS_04, node, nodenum1, s, 1
*get, HS_10, node, nodenum2, s, 1

Step3: Clear Generated Data for your Solution and solve again.

After the above steps, the Post commands should run with any new snippet changes.


Best regards,
Jason

 

[BTHS]

Hi Jason

That worked. Thank you so much for your help!

Best,
BTHS