quad - size and thickness

[40818]

I was always taught that its good modelling practice when using shell type elements to have a reasonable relation between the element side lengths to the proposed material property thickness. For example if the material being modelled was 1mm thick then a typical minimum element size would be 1mm x 1mm square. Today i thought i test it, and set up a simple beam under pressure load fixed at both ends and compared FE results against hand calcs, and it didn't make a blind bit of difference to the deflection/stresses if the Quad4 element was 0.1mm x 0.1mm by 10mm deep (i used a 25mm x 10mm deep beam).
I suppose my question is two-fold, firstly why doesn't it make a difference and secondly, how does the old number cruncher calculate the extreme fibre stresses.
Oh, using MSC nastran & patran.
Cheers.

 

[Denial]

As I understand shell elements (ie hardly at all), one of the key assumptions in their underlying mathematics is that they are infinitely thin. If so, then they are equally thin relative to a 1000mm element side length as they are relative to a 1mm side length.

 

[Stringmaker]

What really matters when using shell elements is not so much the relative element dimensions (length and width) compared to it's thickness; but rather the thickness of the shell to the radius of curvature contained in the geometry. Large r/t ratios typically lend to an almost purely membrane response of the shell (inplane stresses). When a model has a high rate of curvature associated with its geometry the stresses will be predominantly due to bending.

To answer your questions, the reason you do not see any sort of difference is probably due to the model you're considering. Typically, plate structures tend to act about 10% stiffer than beams with identical geometry.

If you want to understand how stresses are computed I'd recommend a good FE or Plate/Shell theory text book. In the end everything is calculated based on elasticity and the principle of virtual work. No short answer exists to your question.

 

[40818]

I understand how plates and shells theory works. And have a fairly decent FE knowledge, but i dont know how Nastran calculated the bending stresses. Your right about the radius of curvature being the critical factor when determining whether it can be defined within the small displacement theory that is the backbone of classical engineering theory and also applies to FE. But i suppose what i thought of as "not as expected" was if you were to take an element in isolation with all its applied translational and rotational forces at its nodes, if the element has a small planar size compared to a very deep thickness, i would have expected some degradation of results.

 

[EdR]

40818:

While not true for all cases typically for shells (and plates) the stress computations simplify to (P/A +/- M y/I) i.e. a membrane and a bending stress component.....I'm not familiar with the specific element formulation of the Nastran elements but it's probably much as I have said.....If this is the case then the membrane stresses decrease with thickness (linearly) and the bending portion varies as (t/I). Thus to compute the extreme fiber stress I would take stresses at any 2 points through the thickness and linearly extrapolate them in the thickness direction...From your post I'm not sure I have said anything you didn't already know so maybe I don't fully understand the question......

Ed.R.

 

[rb1957]

a couple of clarifications please ...

you had the same mesh and only varied the element thickness ?

the thickness direction is transverse (sort of like a web thickness, rather than a flange thickness) ?

my recollection is that CQUAD4s assume a constant stress state and that the output is truly correct at the element centroid. so if you've got several elements thru the depth of the web, plotting the element results at their centroid and extrapolating should yield the classic bending distribution.

lastly, i thought the rule of thumb was to make the element size > the thickness (2, 4, 10*)

 

[40818]

Just to clarify, i chose to do a simple rectangular beam with fixed ends, with a single layer of quad4's. The beam was 25mm wide x 10mm deep, the beam was 100mm long, and i think i had 10000N applied as a UDl pressure.
I started off with a coarse mesh, and ran it for varying thickness, from 1mm to 25mm deep (i.e a square CSA)then subseuently finished at a mesh size of 0.1mm x 0.1mm by 10mm deep(250000 elems), and the results always stacked up to be the same (and within a gnats c*ck to results by hand).

Your right about the quad4 being a constant stress element.

I suppose my rule of thumb might have been hit with a hammer once or twice!! But from my very limited test, it seems to be a meaningless rule of thumb, as it doesn't matter if you greatly exceed it, it seems.

 

[40818]

Had a read through some nastran files, and the quad4 membrane and bending stresses are computed by Mc/I +-P/A as you would think. So it must just do the numbers asis for the element stresses regardless of the thickness chosen as the associated property with whatever element size given.
Hmmm.