×
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: How to get SEPC?

ANSYS Workbench: How to get SEPC?

ANSYS Workbench: How to get SEPC?

(OP)
Hi,

I've been trying without success to obtain the structural error (global) in Ansys Workbench for a very simple model. Using the APDL command for the SEPC doesn't work as it says that SEPC is not available.

Any ideas?

Many thanks,

RE: ANSYS Workbench: How to get SEPC?

Hi

Either in the analysis settings branch or in the solution branch, there is an option to set your requested output items, play with those settings and see if it helps. I'm not at the computer now so can't give any closer details.
Hope this helps
/petb

RE: ANSYS Workbench: How to get SEPC?

(OP)
Hi,

Thanks for your interest but I can't find that option in the GUI. As far as I understand, the only way is to run the APDL command PRERR using an object, but it gives me the error I mentioned before.

Best,

RE: ANSYS Workbench: How to get SEPC?

Hi,

I had another look at this. Make sure to unselect non-structural elements like surface-elements before trying to get the PRERR-item, also this command need the graphics from an element-plot to work. This will work in the /graphics,full-mode only. The command snippet below will work for a shell model with 181-type elements. It's likely easy to adjust for your needs, depending on your APDL-knowledge of course.

/post1 
! enter the post processor
set,first
! first result set
esel,S,ename,,181
! select only your structural elements
/GRAPHICS, FULL
! Turn on full graphics
eplot ! plot elements[/indent] *get,U,PRERR,0,SENSM
! get the error energy of the selected elements
*get,e,PRERR,0,SERSM
! get the strain energy of the selected energy
MY_SEPC=100*SQRT(e/(e+U))
! normalize the energy error against the strain energy
! N.B keep the MY_-prefix to force Mechanical to put the
! result in the Results cell of the Details view of your Command-snippet
PRERR
! Put the SEPC in the output-file, now compare the calculated MY_SEPC to this to check that our calculated value is correct.
allsel
! Select everything so you don't F*** up subsequent results in the Solution branch
finish
! Exit /post1 nicely

Hope this helps

/petb

RE: ANSYS Workbench: How to get SEPC?

Forgot to mention something, the reason i used /graphics, full and eplot was to be able to use PRERR. Now as you see if you run the snippet above, you can calculate it yourself using the errror energy and the strain energy. So the snippen can be shortened to (comments removed):

/post1 
set,first 
esel,s,ename,,181 
*get,U,PRERR,0,SENSM 
*get,e,PRERR,0,SERSM 
MY_SEPC=100*SQRT(e/(e+U)) 
allsel 
finish 
 

HTH

/Petb

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