Admin here - moving this post to a new topic.
Hi Fischer sorry for interrupting in your post but I had to ask Blas something,
I see you always reccomend the use of HEX instead of TET, this is ofcourse true and the ideal situation is always using HEX mesh, but most of the geometries I encounter are way too complex for HEX meshing in 3D solid elements (different wall thickneses, crazy curved surfaces etc.), what I am trying to understan is how critical is it really? Today with advanced CAD tools, design engineers are creating crazy geometries since it is possible in the CAD tool and also in the advanced manufacturing methods and HEX meshing seems unfeasable in alot of cases.
Solved! Go to Solution.
The answer is in your hands: solve the same model using TET4 vs. HEX8 and compare results, you will see what a difference exist between both models, not only in quality of plot results, but also both convergence & the solution time is faster.
The price to pay: you will have to spend your time preparing the solid geometry, splitting and cutting in regular components where HEX meshing is available. You can split a BODY between HEX & TET mesh regions, and prescribing mesh mating conditions with GLUE COINCIDENT option this will make both parts to share common nodes.
Using 3D Swept Mesh to create HEXAEDRAL-TETRAHEDRAL interfaces
You can use 3D Swept Mesh command to create a mapped mesh of hexahedral or tetrahedral elements to link to a free mesh of tetrahedral elements on an adjacent body. To use this capability, you must create a Glue Coincident type of Mesh Mating Condition between the bodies. Then, you use 3D Swept Mesh to create the mapped mesh. Finally, you can create the tetrahedral mesh on the adjacent body. When you solve your model, the software uses multi-point constraint equations to automatically connect the nodes on the tetrahedral and hexahedral elements.
With FE flow model meshing, the basic rule is that fluid can only pass from one fluid body to another if the faces of the 3D flow elements are co-planar at the interface. For greatest accuracy and performance, the adjacent faces should have coincident nodes. The Mesh Mating Condition command ensures that nodes are coincident at the interface between two fluid bodies and the solver joins the two fluid volumes at the interface, and treats them as a single flow domain.
When you create a flow model for CFD analysis with either NX Thermal and Flow or NX Electronic Systems Cooling solver, you must define the 3D flow model. The fluid itself is modeled with different types of 3D elements, such as tetrahedral elements, hexahedral elements, wedge elements, and pyramid elements. You can also combine different 3D element types.
You can mesh with high-order TET10 or HEX20 solid elements, but the NX FLOW/THERMAL solver do not take advance of midside nodes, then is useless, so simply mesh with TET4 or better HEX8 solid elements.
The reason: both NX THERMAL/FLOW are based in a finite volume formulation.
Fischer - again, I am sorry for hijacking your post...
Since I am intending on purchasing of NX Flow and still not using it, it is very good information to know before getting the software, Thanks for this.
What about the use of TET10 Vs HEX8 in regular FEA (NX Nastran/Adina for stractural analysis)?
Do not mix things, the comparison is not between "finite element " and "volume element", each method use different approach to arrive to the same results, then the element behavior is different.
With finite element (FE) solvers, like NX NASTRAN, the use of TET4 elements are not recommended at all for production models, the FE model tends to be more stiff than in real life. Please do not confuse with NX FLOW where the use of TET4 elements is perfect to mesh complex geometries for CFD fluid flow analysis. Of course, HEX8 elements give superior quality results than TET4 in CFD analysis, with the same element size. If the geometry is simply, then surely you can take advance of HEX meshing, but in complex geometries the only resource available is TET meshing. In any case, to get accurate results you need to follow the meshing guidelines common to ALL CFD softwares (this could be matter of another post), here not any differences between NX/FLOW or other CFD software vendors exist.
Regarding TET10 vs. HEX8 (or HEX 20, or HEX27, see this link: http://www.iberisa.com/soporte/femap/nolinealavanz
Simply mesh a 3-D SOLID cube of say 100x100x100 mm with both 3-D solid TET10 and HEX8 elements using the same element size of say Esize= 5.0 mm and compare model size, you will have the following numbers:
As you can see from the above numbers the Model Size Ratio between TET10/HEX8 = 81363/9261 = 8.78 times bigger!!. In summary, not only the TET10 accuracy is worst than the HEX8 elements for the same element size, but also the resulting model size is near to 10 times bigger!!. And in real life nonlinear or advanced dynamic FE analysis the model size is critical, understood?.
Thanks for your reply, as I stated before - for structural analysis it is understood, and the "quality" of TET10 VS HEX8 is another big debate, but with today computer resources comparing to the time consuming process of HEX meshing TET10 elements even for nonlinear analysis seems to me as a good option. Ofcourse I always try to HEX mesh but when time is an essence with complex geometries HEX meshing seems too time consuming.
Thanks again for your informative replies!
And finally, another important key is the size of output results: as you say with modern computer resources we can run big problems with millions of nodes, yes, this is valid for linear static or steady state heat transfer problems, but when you run -for instance- modal frequency response dynamic problems or time history dynamic analysis (or nonlinear transient analysis with many time steps), then size matters!!. The size of the output results could be thousand of GIGAS!!, and probably you won't be available to postprocess results.
Then, you will remember my words, and will do your best since the very first moment when preparing geometry to use HEX meshing as much as possible. But you need to pass yourself to understand what I say.
Of course, everything is understood, these are things you always have to consider before starting an analysis, and this is what I always do, considering the time I have to invest in manual meshing Vs. the quality of the solution and the computer resources I have.
Hola Blas - Muchas gracias por tus explicaciones!
Actually, I was now able to solve the problem by changing the model in the locations where the mesh seemed weird/failed. Now it's converging again. (I am and was using 3D-Tet elements)
No problem for your hijacking. Also for me it's interesting to hear Blas' responses.
A practical experience I just had with Hex vs. Tet elements:
I was doing a simulation of a shell shrink fitted on a shaft. The goal was to calculate the stress in the shell caused by the shrink fit, with a surface-to-surface-contact between the two.
First I chose to mesh all the model with Tet elements.
Then I changed to Hex elements. But the Hex elements of the shell and the shaft didn't match on the contact surface.
Then I changed the mesh so that on the contact surface of the shell and the shaft the meshes matched.
Very striking was how much faster the contact analysis converged after I changed to the matching mesh!
Best regards, fischer_sh