Solid "skinning"

[Zigmhount]

Hi all,

I'm currently testing the "skinning" of a 3D-finite elemente model to reduce the amount of data for a fatigue analysis (mentionned at the end of thread727-232206).

I modelled a complex (cast) part with Tet10 (10-nodes tetrahedal) volume elements, then meshed the surfaces with Tria6 (6-nodes surface elements) shell elements and merged the nodes of solid and surface meshes (including midside nodes).
The shell elements have a thickness of 0,001mm and the same material property as the volume elements.

I then compare the nodal output in solid and shell elements (unaveraged maximum value of strain and stress).

The max principal stress/strain distribution is the same in both solid and shell meshes, however the max stress value in the skin is slightly inferior to the max value at the corner of the solid elements (up to 1%, depending on mesh fineness)... Which one should I trust??...

Thanks for your help!
Simon

 

[GBor]

I got lost in the description. Can you post an image?

Also, 0.001mm sounds like a membrane, not a shell, but that's just a "gut feel".

 

[corus]

A 1% error sounds more like a rounding error than anything to be concerned about. But if you're so wworried, then why not compare the results to analytical values which are true, rather than to each other for which you have no certainty at all.

corus

 

[EdR]

Why would you believe either one over the other....the stresses at nodes are extrapolations of the stresses at integration points and will depend on the extrapolation method used....

If we have gotten to the point where we are concerned about 1% differences in results then someone is kidding themselves!!!!

Ed.R.

 

[Zigmhount]

Well, thanks for your answers.

GBor, there's a picture of an example with a simple plate, in green there are the volume elements and in orange the "skin".
For this model indeed I got the 1% error, which rose to about 10% with the complex geometry... but maybe I used a mesh that wasn't fine enough...

Still, do you have some advices for this "skinning"?

 

[johnhors]

"reduce the amount of data for a fatigue analysis" - can you not directly filter out the free surface nodes of the solid elements rather than resort to "skinning"?

Solid elements are incompatible with shell or membrane elements, they have different shape and displacement functions and different nodal degrees of freedom. Mixing element types invalidates the theoretical basis for FEA which abhors any form of discontinuity, yet by "skinning" you have introduced discontinuities over the free surfaces.

http://www.Roshaz.com

 

[GregLocock]

"an you not directly filter out the free surface nodes of the solid elements rather than resort to "skinning""

I think this is a Nastran workaround. And at that point I'll bow out gracefully.

Cheers

Greg Locock

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

 

[corus]

The idea of skinning is to give better results at the surface for fatigue analysis. Abaqus has a feature that enables skins to be applied to a solid model for this purpose I believe. I've yet to see a direct comparison with and without skins to show if there is greater accuracy or even if it allows an increase in mesh size for the 'solids', whlist retaining accuracy at the surface. A 10% error would be unacceptable though.

corus

 

[johnhors]

"The idea of skinning is to give better results at the surface for fatigue analysis"

If that is true then this is pure "magic" !!

http://www.Roshaz.com

 

[Zigmhount]

Yes, I use Nastran (NX), and I'm indeed trying to make this direct comparison. I'll check the stress values between coarse and fine meshes to get the accuracy...

I thought of filtering/extracting the nodes on surfaces, but the fatigue analysis software reads data directly from the f06 files, not from the postprocessor (Femap), and so it could import only the shell elements (I'm not sure how this works yet).

 

[gwolf2]

Skinning works fine in this context, 1% is very good, no need to go further. Skinning is of most help where the solid mesh is a bit too coarse and for some reason you can't refine it.

Skinning is a bit old fashioned. You can limit the results output in NASTRAN using the 'SET n' and 'STRESS(PLOT)=n' commands.

 

[Zigmhount]

Thanks gwolf, this NASTRAN command sounds interesting, I'll give it a try with the fatigue analysis software.

I tested my "complex" model with different mesh sizes. With the coarse mesh I got 10% difference between shell and tetra elements, with a finer mesh it fell to 1%, and with an even finer I got 3%.

In practical use though the calculation is non-linear, and I get convergence problems with the skin, whereas it was ok with tetras... I guess it's due to this discontinuities that johnhors mentionned.

Thanks all for your suggestions.