(Shell) element size vs. its thickness?

[JBlack68]

To all

Before I "dive" back into my book on the FE method I thought I ask the question

Assuming a model made of 2D elements (shell) with a thickness 't' (let's say t=5mm) and the surface of interest being much larger that 't' (assumes a square 1000mmx10000mm) if one keeps refining the elements and end up with a very small size (let's say 0.25mm or even smaller if you want) is there a point when one "violates" the theoretical assumptions of a shell element? I am thinking about the fact that the element is much thicker than its size

Any thoughts?

Thanks
Regards

 

[rb1957]

I think you are pretty free to model with elements sized irrespective of the thickness. The bigger question is when to move to 3D elements.

be aware of out-of-plane deflections, typical 2D shell elements work like a plate and are quickly inaccurate if there are out-of-plane displacements.

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

 

[aerostress82]

What you describe looks like a beam from here.
For SOL101, if you read through Nastran books, you will come up with a 3t (t=thickness) ideal element size there. But if you work on designs with complex surfaces, you will come to see that 3t is actually not the best size that suits all your needs. After sometime, the term "mesh convergence" will strike from another research. So, all hand in hand really comes down to your model and assumptions (always).

With your beam like plate structure, it would probably undergo buckling/linear static/modal analysis all at once. So, a mesh size of your element thicknesses would do. If you would happen to check the stresses around your fastener regions "in detail", then you would need to create a "flexible fastener modeling" & nice finemesh regions for your plate modeling for those fastener surroundings.

As long as you are SOL101 (or other linear solvers), then your "finemeshed fastener area and element size equal to the thickness" should be adequate for that plate. If your stresses are still high, you have a weird mechanism going on there which is either stiffening your structure infinitely, or as less of a chance: some of your loadpaths are broken. But from your other post, I don't think you would be at a level to face this as of yet. Just keep in the back of your mind. Broken loadpaths are weird and cause peaks out of nowhere. Have seen some examples of them in other people's models but never had one myself. So, not everybody causes them really. Just some people.

Spaceship!!
Aerospace Engineer, M.Sc. / Aircraft Stress Engineer

 

[ShellsPlatesMeshes]

Brief answer (at least for linear static analysis) is: its OK to refine the mesh as much as you need, to obtain more accurate results.For example, the following analysis of a statically (wind-) loaded perforated panel, based on quadrilaterals using the Mindlin approach, works just fine:

http://members.ozemail.com.au/~comecau/perforated_panel.htm

 

[JBlack68]

Thanks for the link. Will have a look at it a bit later

 

[gravityandinertia]

By my estimation, something like this isn't probable anyway. Using a second order shell element on the sizes that you are talking about yields 5.76 BILLION Degrees-of-Freedom. I certainly don't have a computer capable of handling anything like that in any reasonable timeframe.

Avoiding this is one of the reasons for starting with a coarse mesh, refining, then checking for convergence. That process is essentially hunting for the largest size that can accurately represent the "infinitesimal" used in analytic calculations. It avoids problems like incredibly fine meshes when they don't provide much additional accuracy.

 

[Shu Jiang PEng SE]

Reducing shell element size does not violate shell element formation. Shape function used to form shell element stiffness matrix is applicable if the two dimensions of plate is far larger than plate thickness. The fine size of the element will not introduce error in theory. However, too small element may bring two problems in real calculation: 1, taking more computation time; 2, possible element or global stiffness matrixes ill-condition