×
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

Need connection forces

Need connection forces

Need connection forces

(OP)
Hi guys.

I am re-posting after no replies in the UGS Femap forum.

I am assuming you AC stress guys do this often:

In a stressed skin structure (passenger railcar), I need to size welded connections of stiffeners to the skin they're welded to, using results from a beam/plate analysis done with Femap and NeiNastran.  The beam elements share nodes with the plate elements.

I suspect I need to use Grid Point Force balance, then only extract nodal forces applied by the shell elements to the beam elements.  How do I actually do this in FEMAP?  Any other ideas that would make this less painful?  Is there any output vector that does this?

Thanks,
tg  

RE: Need connection forces

Hi tg,

AC stress guys don't do any welding analysis, unless it is on secondary structure (like scuff plates near door openings), and then if necessary, the analysis is very simplistic.


Good Luck,

Nert


 

-----
Nert
 

RE: Need connection forces

Your thoughts are correct. The loads passing from beam to plate are found in the F06 file Grid Force Balance.
I cannot remember an output vector for this, as what you looking for is effectively a model internal force.

You can limit your nodes in the F06 GFB by using a set.

Have you considered what loads can be transmitted from your beam to plate? Unless you have done something special, a beam/plate connection at single nodes will have moments which perhaps you do not want or cannot cater for.

RE: Need connection forces

In Femap 10 at least you can create a freebody of the stiffener elements and nodes and display the forces that act on it.

When you do the run you have to request the grid point balance (Femap just calls it the Force Balance in the output requests of the analysis).

Then using layers show only the stiffener elements and nodes. In the "Select Postprocessing Data" form, click the "Freebody Display..." button, check off "Show Freebody Display", click the "Freebody" button to check off all the proper loads for a normal freebody analysis, then OK.

You can also create a coord system aligned with the stiffener and orient the vectors in that system so you can get the shear and normal components of the loads acting on the stiffener.

Most aerospace companies I have worked with/for have their own post-processing programs for this sort of thing and don't use Patran/Femap but there's no reason it shouldn't be correct. If I was you I'd do a double check of the Femap results vs a hand crank of the f06 numbers just to be sure. Patran/Femap don't document all that well exactly what their freebody results actually show.

Finally you will have to divide the nodal forces by the element middle-to-middle distances to get the running loads in the weld.

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