Really thick shell elements

[trainguy]

To all,

I am reviewing an FE model where 2.5 inch thick plate is being modeled with shell elements. Some of the elements are 0.5 x 0.5 inches. Will this produce good results? The analysis types are linear and nonlinear static. Are there practical limits to adhere to as far as shell element size versus thickness?

Thanks.

tg

 

[SWComposites]

Maybe. Depends on:
a) what type of results: displacement, stress, ?
b) your definition of "good"
c) the overall size of the plate - if it is 20 ft x 20 ft, then the results may be acceptable; if it is 1 ft x 1 ft, then you don't have a thin shell and the results will not be correct.

The real question to ask is: does the "structure" behave like a thin shell?

 

[Denial]

I am in total agreement with SWComposites. If your structure (ie your overall plate) is "thin" and you are modelling it with thin-shell elements, then you will NOT introduce any errors by subdividing your plate into a ridiculously large number of ridiculously small elements.

(Even if you do have to wait a ridiculously long time for your answer.)

 

[GBor]

Denial,

Perhaps I didn't read SW[\b]'s post the same way, but I think you are making the same point. I understood SW's post as trying to define "thin". IF the plate is 1'x1', then a 2-1/2" thick plate hardly qualifies for shell elements. If, however, it is 20'x20', then 2.5" may still exhibit plate/shell behavior.

The question is, "Does the shell behave like a 'thin' shell?" This question really relates to the mathematics and which theoretical basis the software will use to calculate results: thin shell, thick shell, brick?

 

[EdR]

Gbor has it right.....It really depends on the particular element being used and its formulation....Some formulations will give poor results for the case described while others will give very good results......

The best way to make this kind of determination is to run a test case or two with the specific element and check the results against known solutions...(Look in text books, Roark, or other references)...

There are undoubtably practical limits, but again they will vary depending on the specific elements used and testing should be done to verify results......

Ed.R.

 

[truckcab]

Why not make a simple test? Compare stress results with different element sizes for a simple plate? My experience from such tests (Nastran/Abaqus) is that the danger of violating the theoretical thickness/side length ratio for shell elements are a little bit exaggerated. Of course, there are such occasions where you will get wrong results, however, in the light of other shortcomings/approximations in your analysis it might just not matter at all.



Live Long and Prosper !

 

[corus]

The shell element size will depend on how much of the stress variation along its length you want to capture. For the case of using shell elements then, in a similar fashion, it depends if you want to capture the non-linear variation of stress through the thickness. In addition for a thick shell you won't be capturing the localised stiffening effect of the thick shell where it abuts on to another structure. At worst, by using shell elements, you could say all you're calculating is the mean stress. For pressure vessels I think the rule is to use shell elements if the thickness is less than d/10, but I'd still consider a local 2D or 3D solid model to calculate the local stresses at joints if you're interested in the peak stresses.

corus