INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Jobs

Extracting stress in intersecting points of bodies

Extracting stress in intersecting points of bodies

(OP)
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




RE: Extracting stress in intersecting points of bodies

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:

CODE --> ANSYS

! 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

RE: Extracting stress in intersecting points of bodies

(OP)
Hi Jason

Thank you for a fast and accurate response.

I modded the code to exactly fit my purpose:

CODE --> ANSYS

! 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_ .

RE: Extracting stress in intersecting points of bodies

(OP)
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

RE: Extracting stress in intersecting points of bodies

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:

CODE --> Ansys

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

RE: Extracting stress in intersecting points of bodies

(OP)
Hi Jason

That worked. Thank you so much for your help!

Best,
BTHS

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources


Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close