Need connection forces

[trainguy]

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

 

[inertia4u]

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

 

[stresscalcs]

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.

 

[palomc]

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.