How Thin is a Thin Plate? 4

[glenn11897]

In shell analysis (i.e. buckling, etc...), I've always wondered how thin is a thin plate. What is considered a thin plate? What is the definition of a thin plate? This is something I missed asking my profesors back in college. Thanks.

 

[corus]

A thin plate element can be used if you think that the stress distribution through the thickness will be linear.

corus

http://www.corusresearch.com

 

[fsi]

Acording to the criterion often applied to define a thin plate (for purposes of technical calculations) the ratio of the thickness to the smaller span length should be less than 1/20.
fsi

 

[EnglishMuffin]

corus:
Your recommended practice neatly demonstrates that FEA is an art as much as a science: those who wished to be uncharitable might criticise such a "modus operandi" on the grounds that it requires precognition of the correct result. Perhaps the substitution of "is" for "will be" might at least go some way to avoiding the suspicion of "circularity".

 

[Drej]

In "thick" plates, shear deformation and rotary inertia effects are included in the element formulation. See:

http://www.me.mtu.edu/~bettig/MEEM4405/Lecture12.pdf

It is very difficult nowadays to actually use elements based on thin plate theory. Moreover, many FE packages do not even offer pure plate elements for use in FE analyses, offering only the more general shells instead. I'm not sure the earlier statement suggesting that "A thin plate element can be used if you think that the stress distribution through the thickness will be linear" is entirely accurate, since if this were true you would be able to use it for all linear analyses!

A couple of points about plates:

* Generally speaking, plates are designed only to take transverse loading (loading perpendicular to the plane of the element). Think of a bookshelf: this would be a plate structure.
* A plate structure is one in which curvilinear geometry cannot be accurately captured i.e. use these elements for "flat" structures only.
* Curved geometry would look massively faceted using plates.
* If you're using something like ABAQUS, you wont get the choice of using plates, so just go for something like the S4R (say) which doesn't really care (up to a point) whether your structure is "thin" or "thick", as it will adapt as required.

The best of luck,

-- drej --

 

[corus]

There are always assumptions and to a certain extent a presumption of the result before a model is started. Generally such assumptions have to be justified on the grounds that the difference between the simpler shell/plate model and a more rigorous analysis is negligible. To that extent it is an art, or more likely experience that tells you that the results you get will be 'good enough'.
Unfortunately the design codes which people ultimately refer to don't address the problems of finite element analyses or the correct procedures to be taken. Fortunately those who wrote the design codes recognized the limitations of human ability and built-in sufficient safety margins to make FE results, and the even more dodgey hand calculations with their wild assumptions, safe (we hope).
Thin shell/plates could also be used where the non-linear results (referring to the stress gradient through the thickness) aren't required for assessment. In the latter case I'm thinking of nozzle to shell models which typically use shell elements where the user isn't interested in the peak stresses at the juncture. In general though the 1/20th rule is commonly adopted.
For curved geometry the 8 noded shell elements do capture curvilinear geometry as far as I'm aware.

corus

http://www.corusresearch.com

 

[Whe]

You mentioned thin plates but also buckling - big topic.

Can depend on mode of failure - elastic vs plastic buckling for example.

For flat plates, NiDI have a free Structural Design Manual for stainless steel (probably similar to Aluminium, but somewhat different to most carbon steels that have a defined yield point). For cylindrical shells, have you looked at books with diamond vs elephant's foot buckling (ie elastic vs plastic)?

Be aware that 'perfect' geometries (as modelled by FEA usually ) can have a much higher load for onset of buckling than is observed experimentally.

If this is what you are looking for, let us know and I can probably post some specifics.

Q

 

[glenn11897]

Thanks for all the replies. I just got back from vacation. I didn't expect a reply that quick and that many.

I gather 1/20 is a good rule of thumb (thanks fsi). I agree with corus about the shell in that ‘stress distribution through the thickness (roughly) linear’ (with good engineering judgment-of course). Yes, I believe that in FEA packages, there is always a certain amount of assumption and compromise. I think, FEM’s are here to aid us in analysis not the substitute. With good engineering judgment, and probably some conservatism (especially in the field of aerospace) a sound engineering analysis can be attained. And there is more to improve in FEA to assess real structures or models.

Drej, thanks for the FEM link. I downloaded some of the lessons to take a look at.

Hope everyone had a good Thanksgiving…

 

[labosonic]

I'll reply with my own university lectures souvenirs :
- U can assume that a thin shell is thin when thickness is 1/20 of length (i was learned 1/10 but i'ld rather use 1/20). This notion is geometric and not linked to your element size.
- U must check that your problem is linear i-e :
- a normal section of your shell will stay normal after deformation.
- a normal section of your shell will have the same dimension at the end of your analysis

 

[LesT]

Not being a FEA user myself, I often questioned the applicability of FEA with thin structures.

I was recently confronted with a honeycomb type structure that was modeled with FEA. The 304 Stainless Steel walls of the structure are only 0.08mm(0.003in) thick. Modelled 10 elements across thickness, indicating a localised over stressed area about two elements deep.

Certainly from a practical point with these thin structures, the stresses, induced, raised etc are started to be driven by physical phenomena ie metallic grain structure, surface affects, surface tension, residual stresses, surface roughness, means of attachment, manufacture inconsistencies etc. These side issues becomes dominant and lessens the practical application of FEM.

Does anybody have some reference or rule of thumb(like the 1/20 of above) as up to what point the FEA and practical test results are still comparable.

 

[fsi]

LesT
It is not possible to model 10 elements across the thickness of thin plate elements in FEA. Only 1 element is formulated, used and possible. You could be referring to solid elements which do not apply to this thread.
In reference to your other question about FEA being practical, if all the side effects that you mentioned are modelled in FEA which is possible using nonlinear FEA, practical test results and FEA results are comparable within 1% of each other.

 

[jagad5]

One more general rule of thumb: If the deflection of the "thin" plate exceeds the thickness, it becomes a non-linear, large deflection problem. This means you must turn some more knobs in your software. The answers can change dramatically.

Doug

 

[jetmaker]

Just wanted to add that jagad5's comment is spot on. Having just gotten back from a course presented by MSC... they recommend that anytime the out-of-plane linear static deflection of a shell or beam element exceeds the thickness of the element, then a non-linear large deflection analysis needs to be performed due to the membrane behaviour contributing to the out-of-plane stiffeness. The difference in out-of-plane deflection is staggering.

regards,

jetmaker

 

[glenn11897]

yes. we are currently studying a structure that was giving us some weird numbers (bending and deformation) when ran using SOL 101 (Nastran). were now runnig it using SOL 106 (nonlinear-MSC.Nastran) due to the membrane effect that jetmaker & jagad5 brought up. so far were not converging only up to 20% but were already seeing that the difference between 101 & 106 as far as the large displacement runs.

 

[pja]

With regards to when geometric nonlinearities are important
for thin plates the rule of thumb of 1 plate thickness is a safe one. However the boundary conditions of the model play a factor here as well. A cantilever plate will display linear behavior for deflections up to 15-20 thicknesses. A plate which is fixed on all 4 sides on the otherhand will display nonlinear behavior for deflections on the order of a 1 plate thickness or so. However when in doubt one should always(time permitting of course) run both a linear and nonlinear analysis just be sure.

 

[analyzer]

What is a penalty factor when it comes to thin plate element formulation?

 

[Breezer]

Thin shell elements (ie. Bending stiffness included but shear stiffness infinite): thickness < 5% of other dimensions
Thick shell elements (ie. Bending and shear stiffness included): Thickness between 5% and 10% of the other dimensions.

Using the shear stiffness on elements < 5% thick will not give worse answers. The answers will actually improve. The influence of the shear on the deformation is just small, so that's why you can drop it. If you refine a shell mesh (on a part that shell theory is valid) to the point where the thickness of the element is > 10% of it's other dimensions, then shear stiffness will dominate (or at least be significant) for the element even if it's not dominating the total plate's response. For this reason, add the shear stiffness to help "stabilize" the global stiffness matrix. (you can use much more elements (getting better accuracy) before the solver will have big round-off errors)

 

[feadude]

"pja" wrote:
"A cantilever plate will display linear behavior for deflections up to 15-20 thicknesses."
Is this correct? I thought it will be less than 15-20

 

[jhardy1]

feadude,

Consider a steel plate 1 metre long, 100 mm wide, 10 mm thick, fully fixed at one end only. Assume it has a transverse pressure load, so it bends like a cantilever beam. Because this arrangement generates no significant membrane stresses until you get very large deflections, it will behave linearly (or very nearly so), up to quite large deflections. (When I ran this check, it stays effectively linear well beyond 200 mm defelction, or 20 plate thicknesses, if you ignore material yielding and plasticity effects.)

The same plate held at both ends will start to act non-linearly at much smaller deflections, as the membrane stresses can develop at much smaller deflection. (When I ran this model, significant non-linear behaviour was apparent when the deflection reached just 3 mm, or about 0.3 times plate thickness.)

 

[feadude]

Julian:
I agree . The plate held at both ends, was it also fixed at both ends?
If not will it still show nonlinearity at about .3 times plate thickness or it will be higher?
Thank You