Which constraints should I set to simulate stiffened panel under pure shear?

[Eugene Pavlov]

I have a stiffened panel that looks like this:

This panel is under shear:

All sides of the panel are pinned. Txy - is distributed shear load.
Which constraints should I set to simulate stiffened panel under pure shear?

[pre]
As for me I did this (but don't know is it good approach):
Constraints:
Tx Ty Tz Rx Ry Rz
Left: - - x - - x
Right: - - x - - x
Top: - - x - - x
Bottom: - - x - - x
A: x x - - - -
D: - x - - - -

Where: Tx, Ty, Tz - translational degrees of freedom
Rx, Ry, Rz - rotational degrees of freedom
'-' denotes free degree of freedom
'x' denotes fixed degree of freedom
A - left bottom node // B ---- C
D - right bottom node // | |
// A ---- D

Then I set distributed load on each side in appropriate direction.
[/pre]
So which kind of constraints would you advice?

 

[FEA way]

Generally those boundary conditions seem correct apart from unnecessary constraint Rz=0 for all edges.

If you are not sure about BCs, run a simple test analysis of a rectangular plate (without stiffeners) subjected to in-plane shear. Its results should show you whether the constraints are correct or not.

 

[rb1957]

ok, you've constrained the plate for shear, now how are you going to load it ? Replace constraints on a long side and a short side with UDL. Well a "proper" UDL ... 1/2 the QUAD load at each node (so that the extreme end nodes see only 1/2 the typical node load, yes?)

another day in paradise, or is paradise one day closer ?

 

[FEA way]

Some FEA programs offer special load called shell edge load and one of its types is shear. But of course it depends which software is used.

 

[rb1957]

another thing ... are the stiffeners 1D elements (rods) or 2D elements (cap and web) ? what constraint for the non-shear_web node ? I'd suggest axial load.

another day in paradise, or is paradise one day closer ?

 

[SWComposites]

EP - do you want the edges to remain straight? Your bc’s will not enforce that.

Start with an unstiffened plate model and work out loads and bc’s to get a state of pure shear stress. Then move to the stiffened panel.

And remesh with quad elements. If you are using 4 noded tet elements the results will be rubbish (at best).

 

[ESPcomposites]

You can have a look here under the INDIVIDUAL DOCUMENTS section. For the Basic Manual, Page 7 discusses the boundary conditions and some specifics about it. The Validation Cases PDF shows that this approach is accurate for in-plane loading (Nxy loading).

https://www.structuralfea.com/PlateMesh/download.html

Brian

http://www.espcomposites.com

 

[rb1957]

yeah, but "straight" edges is like "fixed constraint" ... a theoretical "construct" rather than a true reality.

I agree with the approach of starting with a simpler model and loading, and get that right (or "right") and adding complication.
One thing to think about is "what's beyond the model?" is it a rigid body or a theoretically infinite shear panel ? Possibly model as a cylinder if infinite ? Possibly model as "super-element" and combine 9 (16?, 25 ??) pieces together to see what happens.

For edges, maybe add a beam with very low area but very high I

yeah, avoid TET4s like they were some "red-haired orphan". But meshing this with TETs would take a lot of elements ! (but so what if it takes 5 minutes to run ...)

another day in paradise, or is paradise one day closer ?