Quad4 vs. Quad8 and Quad8 vs. Tet10 in Bending

VMH

For solid elements subjected to primarily bending, a few layers through the thickness are usually recommended for linear solid elements. Solid elements have only 3 degrees of freedoms at their nodes (3 displacements) compared to shell elements that have all 6 degrees of freedoms at their nodes (3 displacements and 3 rotations) which are good for bending.

From the attachments, comparisons of linear vs. quadratic quadrilateral shell elements (Quad4 vs. Quad8, respectively) and quadratic quadrilateral shell elements vs quadratic tetrahedral solid elements (Quad8 vs. Tet10, respectively) were performed. For the comparison, max. element size of 1in was used. Quad4 model has 2,953 nodes, Quad8 model has 8,737 nodes, and Tet10 model has 38,603 nodes. The downside of using Tet10 is having alot more nodes which result in much larger model and require more time to solve. However, if the model was created from solid model and has alot of complex geometric, it is difficult or sometime impossible to model using all shell elements or extracting the midsurface from the solid model to obtain a shell model for the analysis. From this comparison, we can see that even a single layer through the thickness using quadratic tetrahedral solid elements yielded very similar results as the quadratic quadrilateral shell elements. All meshing and analysis performed in Mecway FEA.

Also see the following link for more information:
http://www.ansys.com/staticassets/ANSYS/staticassets/resourcelibrary/confpaper/2004-Int-ANSYS-Conf-9.PDF

All files are also attached.

rhoka

38.603 vs 2.953 nodes with different element models

look interested, when a small model (<1/10) yield nearest same result

so the analyst can start to think not a part but a whole models using effective elements representation

VMH

rhoka, my intention was to show that Tet10 elements can also be used in thin wall components (also discussed in the referenced paper). Sometime we don't have a choice to choose to use all shell elements especially in complex geometry. Tet10 is a good alternative.

rhoka

yes, Tet10 is quadratic element. i usually get reliable result even for thin/long element.

about large nodes/dof. i think maybe different for me, in civil/structural engineering problems are large and complex it can be imagine a steel building with bolt contact etc., become impossible to complete modeling. how much nodes/dof would be?

last day i just simple run a model (attached) of single colum with considering bolt holes, fillet profile and chamfer weld. analysis are elastic linear, nodes about 300k, the solver fails to run. i didn't know is MECWAY capable.

so, FE modeling in structural areas much engineers stuck in beam+shell element to model complete building. spring connection and rigid links play a role.

VMH

Thanks for your comments. I wouldn't attempt to build a mesh model using solid elements of the entire building. I have solved 300,000 nodes in Mecway with my 5 years old i7 intel quad core without any issue. It took about 20min to 30min to solve on my old computer.

You can refine area of interest with finer mesh and other areas with coarser to reduce the number of nodes. If you not too interested in the radius at the flange and web of your attached image/model plot, you can reduce the number of element per curve and apply local refinements in areas of interest in the meshing option.

VMH

rhoka, can you provide the step file that you were using that failed to solve after meshed with 300k nodes? Thanks

VMH

Correction to my previous post: it took about 45min to solve 325,000 nodes with 4 bonded contacts using linear static analysis on my 2nd generation i7 quad core.

rhoka

thanks for suggesting, these mesh generate automatically by program. looking good to study torsion stress distribution.

but it's too much nodes created. yes, mesh around fillet should be reduced.

attached step files,

rhoka

well, about CPU. i still using my old laptop with 4gb ram running on 32bit win7. at the time my decision is based on graphics card since SAP required huge amount of memory, it's frequently lags and freeze before.

in this case MECWAY graphics performance challenging SAP, i don't know why even both programs using DirectX technologies (AFAIK).

your CPU is great class, look from benchmark is far away compare to my specs.

barrti

Thanks for this guys. I read the paper and then tried using one 10 node tet thru the thickness. The steel plate was 1000mm by1000mm by 2mm thick. I placed a single 10N load in the centre and used simple supports on two opposite sides.

With an element size of 10mm it compared well with an 8 node shell element of the same size. Deflection was the same(1.58mm) and stress was within 7-8 percent (7.5 MPa)
It was a short test but I was impressed and surprised.

Does anyone know of more work where ten node tets are used for thin shells (1 element thru thickness)?

Does this hold when long thin elements are use?. I was a little unsure of what the paper was suggesting when it spoke of a 2000:1 ratio. We're they talking about very long thin elements or that the plate itself had a 2000:1 length to thickness ratio?

[Deleted User]

i didn't read the paper, however, i'm sure they meant the plate itself being 2000:1. Usually you want a cube as the perfect element shape.

VMH

The maximum element size that I specified for a coarse mesh was 6 to 8 times the thickness. And then I did a refinement at the max stress locations. If the stress changes about 5%, the previous mesh density is okay to use without further refinement. I have not tried or wouldn't use 2000:1

barrti

Yes i thought the ratios were crazy. This means that the paper is recommending various tet element sizes depending on the ratio of plate length to plate thickness eg for 50:1, an element size of 3 times the plate thickness is recommended. For 2000:1, an element size of 25 times the plate thickness is used. I reran my models above with just gravity and a uniform load. With a 2mm plate, I used a 6mm mesh. It gave stress and deflection results within 5 percent of the theoretical hand calculation. I have not repeated it for a 2000:1 ratio.

Note that the paper makes these recommendations for thin plates in the context of finding the natural frequencies within 2% of the theoretical. It does not discuss stress and deflection. From what VMH has said and my very limited tests, it seems like one element thru thickness for 10 node tets are a viable way of meshing many cases of thin plate models. As is pointed out, mid planing some models and then plate meshing is a whole lot of work.

VMH

barrti,

There's another paper called "A Comparison of All Hexagonal and All Tetrahedral Finite
Element Meshes for Elastic and Elasto-plastic Analysis" by Steven E. Benzley, Ernest Perry, Karl Merkley, Brett Clark from Brigham Young University, Provo, Utah.

http://www.csimsoft.com/download?file=Documents/hex_tet_comparison.pdf

barrti

VMH thanks for this. The 10 node tet still looks like a great alternative except perhaps non linear.

[Deleted User]

There are a few other FEA technologies that may be of interest to you. AMPS Tech uses what they call strain-enriched FEA or Sefea, to allow accurate results using low order tets. It is available in IronCAD and KeyCreator as well. So you can solve a model with much lower node counts. They also seem to say it is more tolerant of poor mesh quality. Of course, it costs way more than Mecway. It doesn't look like AMPS currently supports composites. I have not personally used AMPS to know that much about it however.

Another option may be Scan & Solve, which is a Rhino plugin. It doesn't use a mesh at all, just a rectangular grid of points. I believe Scan & Solve is reasonably affordable, but I have not personally used it either. The reason being, Scan & Solve does not yet have pre-stressed modal analysis with spin softening like Mecway does. But if you just want stress and displacement, and are having issues with meshing, Scan & Solve may be of interest to you.

Otherwise, for traditional FEA, using elements with mid-side nodes is always a good idea. You can view stress and/or displacement contours to see if the model contains enough elements to provide the desired amount of detail. I find modal analysis results to be helpful in this regard. Solid elements are not always appropriate. Beam and shell elements have their places.