Thin Plate Model in STAAD

[JedClampett]

I'm trying to check the behavior of a perforated plate. It's 10 ft. by 10 ft. by 1/8 inch thick. I put a 20 psf wind load on it. I ran it on STAAD with each side simply supported in all three directions. I thought it would deflect a few inches and put a lateral load (in the plane of the plate) at the supports, like a catenary.
The analysis results showed 23 inches of deflection and no lateral forces at the supports. (Side note; when you animate it it's like a trampoline!) Is there a way to get STAAD to analyze this more realistically? I know I might have to add some stiffening members, but I'd feel better about it if my first try would come out more as I expect.

 

[dig1]

Jed,

I did a quick Roark analysis on a 1/8" thick solid plate (I did neglect diaphragm action) and came up with 22.6" of deflection for the geometry and loading you indicated. I don't know if the deflection makes you feel any better or not as a starting point.

If i get some more time tonight I'll take a another look at it.

Patrick

 

[JoshPlumSE]

A first order analysis of the plates will not include any stiffening effects brought on by membrane tension in the elements. Instead, the plates resist the load entirely through flexure.

If you want to get membrane tensions to resist the load, this would require a true 2nd order analysis of the plates. I do not know if STAAD has that capability or not.

To validate this line of thinking you might try the following:
Apply 10% of the applied load and record the deflected shape. Change the geometry of the model so that the starting shape is approximately equal to this 10% deflected shape.

Then apply the remaining 90% of the load and see what you get for the deflected shape. The structure should be a lot stiffer and the axial stiffness of the plates should start resisting a good amount of the total applied load.

 

[JStephen]

The choice of elements selected could enter into it also- I'm not a STAAD user so don't know if it's possible to go wrong there or not.

 

[SAIL3]

Did not understand JoshPlum's explanation at all, so I decided to check RISA's pl elements and got a big surprise when I read their supporting literature. They note that the plate elements they use in RISA will not develop membrane forces if the only loading on the pl is out of plane loading. To activate the membrane forces there must be some in-plane forces as an input to begin with. This sounds like some hybrid type pl element and may be the same in STAAD. So you could input some insignificant in-plane loads in combination with your wind loading to see if this kicks off the membrane capacity of the pl. Also check your boundary condition to ensure the plate is "held" in the in-plane direction.

 

[Gumpmaster]

Jed,

Like Josh said, this requires a 2nd order analysis. In effect it's a non-linear analysis because the materials behavior changes as the deflection changes.

I don't think that STAAD can do this.

SAP2000 may be able to if you specify a non-linear analysis. I haven't tried it. You may have to use a staged construction analysis to work your way to the final deflected shape per Josh's recommendation. The good thing is that's very simple in SAP.

Josh, can RISA do this (in a single analysis, not a two stage one as you described)?

 

[JoshPlumSE]

RISA does not consider 2nd order effects like this for plate elements. My belief is that none of the major structural programs (STAAD, SAP, RAM et cetera) do this either.... at least not for plates. Obviously, I cannot be sure of that.

You could contact SAP or GTStrudl to see if they added it without my knowing. If not, then it probably gets more expensive than is worthwhile unless your business plan depends heavily on these types of projects.

 

[SethGuthrie]

I had one suggestion from a colleague who does some of he finite element programming at Bentley, but he admits he hasn't tested the idea:

...our shell element includes two stiffness matrices, one for membrane and one for plate action and they are not coupled. Hence, you can't get any membrane action while loading the shell in out of plane direction.

One modeling approach could be creating a dense grid of cables and between them inserting shells with only membrane stiffness. So the shells do load transfer between cables through their membrane action while cables do catenary action.

 

[JedClampett]

Thank all of you for your answers. Meanwhile, I put some stiffening elements in the grid and have come to an understanding with the thin plate.
I was just a little surprised that STAAD didn't consider this in the first place. When a plate is deflecting to the magnitude I got, it seemed that some of the load has to go into tension.

 

[TehMightyEngineer]

Yes, this really shows the limits of STAAD vs a true FEA program as STAAD will not do 2nd order effects such as membrane forces, post-buckling strengths, or inelastic effects. We run into this all the time at the office with all the weird industrial stuff we get into.

Maine EIT, Civil/Structural.