Coating Solid Mesh with plates for Stress Recovery. 2

[SeatrendSam]

I was having a discussion with some collegues concerning caoting a brick or tet mesh with plate elements. Their opinion was that it was the only way to get accurate surface stresses. In my opinion, coating the model with plates (even if very, very thin) would not result in correct stresses. What are your opinions? Has anyone done something like this before? Was it successful?

Thanks in advance.

 

[corus]

I can't see why this would work. Plate elements assume a linear stress distribution through them which would probably be incorrect for a solid body where the surface stresses are required. In addition the plates need a thickness which would obviously add material and stiffness to the body and thus give incorrect results. I have seen beams added to the surface of a 2D body before in a dynamic analysis but why, I have no idea. It'd be interesting if anyone knew the advantages.

 

[mloew]

Actually, when using shell elements this is a somewhat standard technique when the surface stresses will be used for a subsequent fatigue study. I saw this technique demonstrated by engineers at nCode (

http://www.nCode.com)

for this purpose. The fatigue analysis was only concerned with the stresses at the surface of the component, so it was convenient (and computationally efficient) to use only the stresses from the shell elements. The shell elements used were very thin and the stress results did not differ greatly when compared to the same model run without the surface shells (solid elements only).

I would look for some additional resources to confirm this practice (try Google.com and the FAQ for this forum.).
Best regards,

Matthew Ian Loew

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips Fora.

 

[tld23]

SeatrendSam
Unless there is a specific requirement like that described by Mloew above I cannot see the logic in this technique.

The accuracy depends on a number of factors, but I will limit discussion to mesh density issues. As the mesh is refined the solution variables should converge to the true values. In reality one has to use a computationally managable mesh which means there will be an error. Now numerically the stresses are calculated at the element integration points and extrapolated to the nodes. If the elements are small enough the error will be small and hopefully accecptable too. If the elements are too large because of computational restrictions the errors would just be passed-on to the shell elements but with the advantage that the displacement function would dictate deformations of the shells. However these displacement functions would also be in error because of the lack of mesh convergence. In addition the extra stiffness of the shells (even if thin) would introduce a further error. So why not use the extra computational load that the shells would use and just refine the solid mesh?

Else please explain the logic.

TERRY

 

[brad]

This is actually a fairly common procedure. The "plate" coating is most accurately accomplished using very thin membrane elements (not shell elements). There is a clear rationale for this:
1) In "blocky" structures the peak stresses will be on the free surface (barring any defects--which of course FEA can't account for).
2) On the free surface the stress tensor devolves to two normal components and one shear (which the membrane element captures nicely).

By coating the continuum elements with membrane elements (at coincident nodes), the membrane elements go along for the ride (if they are sufficiently thin) and the membrane element shape function is then used to calculate the surface stresses at the membrane integration points (which of course are at the free surface, as opposed to the integration points of the continuum elements which reside beneath the surface).

The membrane elements can be made VERY thin (as they introduce no near-singularity problems since their connectivity mimics that of the much stiffer continuum elements). Therefore the error due to increased stiffness is VERY small. And the increased accuracy due to integration point calculations at the surface is better than for the continuum elements which must extrapolate to the surface.

As Matthew pointed out, this is very common for fatigue. It was also much more common back in the "old days" (which is actually not that long ago) when computer size limited the mesh density for cast components (hence the error due to stress extrapolation was nontrivial).

Brad

 

[mloew]

Brad,

Great post. Thanks for getting me back up to date!

Best regards,

Matthew Ian Loew

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips Fora.

 

[izax1]

This method is also quite convinient when trying to map analysis results to strain gauge measurements. Also in MSC/PATRAN Random Vibration utility it is a must to coat the solids with thin membrane elements to get the correct stress value.

 

[garymostyn]

Hi Gents,

I today experienced the benefit of adding shell elements to the surface nodes of a solid mesh for Fatigue analysis purposes. I am currently investigating the fatigue life of a machined fitting which I meshed using Tet10 elements. Obviously I am only interested in the magnitude of the max principal surface stresses for fatigue. The mesh density is relatively fine in the fitting resulting in 250000 dof and as a result I do not wish to go any finer. I meshed the surface of the Tet10 elements using very thin (1000x thinner than the plate thickness) Tria6 (parabolic) elements and a comparison of the max principal stresses revealed an increase in stress of 10% greater than that predicted by the solid elements which is not insignificant for fatigue problems. I think it is important to remember that for 99% of fatigue problems we are interested in the surface stresses only, which is where the surface flaws are. I obviously agree that you would converge upon the 'correct' answer by increasing the density of Tet10 elements but this results in an exponential increase in nodal dof. Whereas the Tria6 elements share the same nodes as the Tet10 elements. Also when looking at a contour plot of the principal stresses you are sure you are looking in plane of interest.

Cheers,

Gary Mostyn
Aerospace Stress Engineer.

 

[SeatrendSam]

garymostyn,
Thanks for the reply.
When you have the strains/stresses from your FEA model, did you happen to have a chance to compare the values to physical test data? If so, how did the values compare? Was there any correlation?

Thanks in advance.