Smart questions
Smart answers
Smart people
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Member Login




Remember Me
Forgot Password?
Join Us!

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips now!
  • 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!

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

Donate Today!

Do you enjoy these
technical forums?
Donate Today! Click Here

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.
Jobs from Indeed

Link To This Forum!

Partner Button
Add Stickiness To Your Site By Linking To This Professionally Managed Technical Forum.
Just copy and paste the
code below into your site.

davidnoc (Structural)
20 Jan 09 22:49
Hi All,
How to output the element forces(CBAR)in F06 file. I requested for element forces in "output request" in PATRAN, but  F06 file didn't output element forces.I can see element stresses, forces at SPC but NOT element forces for all the elements.

Please some body spread some light on how to output the element forces in F06 file.

 
truckcab (Automotive)
25 Jan 09 4:50
Use the CASE command:

ELFORCE(PRINT, SORTX)=Y

Where X is 1 or 2 depending on output format. Y is the number of the SET including your bar(s).

Hope this helps



Live Long and Prosper !

fl11 (Aeronautics)
28 Jan 09 7:47
Hi, with Patran sometimes, it might be just that you forgot to click on an apply botton somewhere.

First thing to do is to go in Analysis - Subcases

There you can create subcases and associate them with load cases that you previously define, otherwise you just use the default load case and subcase.

Anyhow, to get the element force, you need to click on a subcase (first box at the top: Available subcases) NOT on a load case (second box: available subcase). This is very important. Once you click on a subcase, the associated load cases should highlight as well. If you want to change the load case, then you can click on another one. Once the subcase has been selected and the appropriate load case selected as well, then click on output request.

By default, you have displacement, stress and SPCForce. If you don't want one of them, then click on it and click on delete. To add results, Element force in your case, CLick on it and it goes directly in the Output requests box.

Here, it is important to click ok and then, click Apply on the next form (Subcases) so you can create a subcase with those output requests. If you are using the default subcase, it will replace what was created in it by default. If you dont click apply on that form, the subcase with output request will not be taken into account!

After clicking apply, on the analysis menu form, click on Subcases select to make sure that you have selected the right subcase to run. Then run the analysis. If a BDF file is created, go in it and make sure that you have in the case control deck something like:

FORCE(SORT1,REAL,BILIN)=ALL

You can also just do Analysis - Entire Model - Analysis deck and that way you will only create the bdf file without running the entire model.


You should now have the element force you requested.  

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!

Back To Forum

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