×
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!
  • Students Click Here

*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.

Students Click Here

Jobs

ANSYS Workbench-scripting

ANSYS Workbench-scripting

ANSYS Workbench-scripting

(OP)
Hello everyone,

I have a question regarding Ansys workbench. I have a model in WB and I am doing a parametric study. I have an input parameter which is a radius which I have parametarized (by checking the box next to it). Now my radius is in the table of design points. I am trying to run the simulation by giving a range of values of radius in the table of design points. In output, I want the coordinates of the node with the maximum von mises stress. I know that I can export the von mises stress results (by right clicking von mises stress) into excel and get the x,y,z coordinates of the node with maximum stress. But, I was wondering if there was a way to these coordinates automatically for all the radius values that I specify in the table of design points by writing a code or some other way.
Also, if it is possible to get the coordinates in the table of design points.

Any help is appreciated!!

Thanks,
Sameer Jade
MIE Dept., UMass Amherst

RE: ANSYS Workbench-scripting

Hi Sameer

Try inserting the following APDL commands in the solution area of your simulation:

SET,LAST
NSORT,S,EQV,0
*GET,my_n_seqv_max,SORT,0,IMAX
my_nx=nx(my_n_seqv_max)
my_ny=ny(my_n_seqv_max)
my_nz=nz(my_n_seqv_max)

once you have pasted them, click on the Search Parameters button and the values of the variables that start with my_ (you can change this prefix in the Details/Definition/Output Search Prefix of the command object) in your code will be created in the Details/Results of the command object.
Check them and you should be able to get the results in the table of design points.

I hope it helps!

RE: ANSYS Workbench-scripting

(OP)
Hi Carles,

Firstly, thanks a lot for your reply. It worked. I am trying to see the equivalent stress in a portion of my total model (because of some stress concentrations that I want to avoid). Therefore, I created an Equivalent stress 2 for the small portion of the model in the solution window. However, when I use EQV in the NSORT line of the snippet, it considers the entire model. Is there a way that, it only considers the Equivalent stress 2. I have attached a snapshot of my window.

Thanks!

Sameer Jade

RE: ANSYS Workbench-scripting

(OP)
I tried using named selection by selecting the face where I want to monitor the maximum stress. But I am not sure how to put the named selection in the code. Any help?

Thanks,
Sameer Jade
MIE Dept., UMass Amherst

RE: ANSYS Workbench-scripting

Sameer,

have a look at the command CMSEL

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