Warped Elements 1

[jball1]

Can anyone point me to a resource which explains specifically how warped quad elements affect FEM results? I have been doing some searching online, but haven't had much success finding specifics.

One powerpoint I have found seems to suggest that warped elements underestimate bending strains because forces in the plane of the element do not cause bending strains, even though they should. For example, a force on node 4 in the below image that is parallel to the element plane should cause bending in the element, but does not. If I understood that correctly, it makes sense to me. However, I have also heard that warped elements can produce artificially high stresses, so it seems like there is more going on here than just underestimating bending strains.

I will keep looking, but if anyone knows of a resource that breaks down the effects of warped elements, I would appreciate it.

Also, I understand that these details aren't necessary to understand in many cases. However, I am currently modeling a complex surface and warp is going to be unavoidable. I would like to have a more in-depth, (hopefully at least somewhat at the mathematical level) understanding of the effects of warp to help me navigate this particular job.

 

[rb1957]

warp with rectangular elements is generally unavoidable. It is as undesirable as any other distortion from flat square elements. I would pay more attention to element aspect ratio.

this is usually code and element dependent. The user manual for your s/ware will have preferred limits.

Usual QA checks on a FEM will highlight poor elements.

You should investigate this for yourself, doing single element patch tests. This is a typical approach to validate how elements perform under different loads, and with different distortions.

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

 

[IceBreakerSours]

I can't recall a resource right off the top of my mind but, usually when I have questions that go into the weeds, I pick out Klaus-Jurgen Bathe's book and find a satisfactory explanation in there.

Take this with a healthy dose of skepticism because I haven't looked at this in a long time and I am going by memory (which sucks!): It comes down to the Jacobian, which pops in many analytical equations of continuum mechanics. If the element is crooked, the Jacobian terms will overwhelm the actual quantities of interest. Or, something like that ..

The reason I wanted to post a response is because what gets lost in the structural/solid mechanics community is discussion about gradients and how the elements need to capture those gradients well - it is not about how good looking (cube-like) the element is supposed to look, how well the mesh "flows", etc. On the fluids side, poor aspect ratio elements are used all the time - in the boundary layer - and they are aligned in such a way that the gradients are captured very well. Now, what helps the fluids folks is that the elements do not deform and this is where the discussion on the structural side gets interesting (assuming large deformation/distortion occurs). Element quality evolves over the period of the structural simulation AND we tend to run various load cases with the same mesh. Can you come up with a mesh quality that works reasonably well for the entire duration of the simulation and the variety of use cases in a reasonable time frame? How much time can you invest in meshing vs. analyzing (which is what you get paid to do)? Some of the most serious modelers are arguing that automation with tetrahedrals is more valuable than great meshes with just a few use cases - man-hours are expensive; compute time is cheap.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[rb1957]

absolutely, stress gradients are critical to mesh density. However the element is distorted away from the ideal flat square it's performance is degraded. Codes usually limits wherein their elements are reliable.

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

 

[IceBreakerSours]

Yes, some codes will simply quit running the analysis if the element quality is deemed to be below a threshold. I suppose this too seems to suggest perhaps, as awful as they are, tetrahedrals are okay - as long as you have enough of them!

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[IceBreakerSours]

Jonathan Shewchuk from Berkeley has looked into this issue in great detail. Look up this publication or some recent ones that might cite it. Warning: The content can go into the deep end of the pool pretty quickly so skimming the introductory sections might be a reasonable strategy.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[nlgyro]

Well...

There is a standard patch test which checks the stability of finite elements shells under extremely warped conditions. Its the McNeal's twisted beam problem as shown below:

(Note: The deflections are measured in the direction of the loading at the tip.)

For the mesh density that this patch test is checked against(12x2), each element along the length of the beam is twisted by 7.5deg and the peak warpage is in excess of 10deg which occurs at the mid-span of the beam. There is a special variation to this patch test mentioned in R.D Cook's text of FEA (Cook, et.al. "Concepts and Applications of Finite Element Analysis" 4th edition) where if the thickness is reduced by an order of magnitude (say 100) the test then check membrane locking of shells in addition to the twist and warpage. The text also contains the theoretical results for this variation of the problem.

I have no idea what kind of a structure you're modeling, how severe is the warpage and how coarse your mesh size is going to be, but as other posters have mentioned if you stick to the limits in your solver then you should be okay. But before you take a stab at your problem I would suggest you to model these patch tests on the elements that you are supposed to use and see for yourself where they stand against benchmark results.