[Andris]

Hi all,
I have managed to generate a 3d Octree mesh with 3 layers of prisms on the wall. The geometry is a blood artery bifurcation that I constructed on AutoCad. Doing some mesh checks, I found that my expansion ratio and max angle indicate a poor quality mesh despite smoothing. I tried to fix this by increasing the number of elements (by lowering the global element scale factor) yet this seems to make the problem worse.
Could anyone please tell me how I could increase my mesh quality?
Any help would be greatly appreciated,
Andris

[diamondx]

here is a small pdf made by Simon on how to deal with quality in if you have tetra/prism.
https://dl.dropbox.com/u/35161486/Prism_NoPyramids.pdf
I assume you did a geometry repair when you imported your geometry in icem. delete unwanted curves and points. if you don't icem will be force to put nodes there. sometimes unwanted. sometime i see others creating just one layer of prism, then they divide it in the edit mesh section.
Dig more into this forum, use the search button for quation tetra i'm sure you will find a lot.
hope it can help

[Andris]

Hi,
Thank you very much for your help. The document has helped alot.
I didn't do any geometry repair, I simply labelled all the parts to my model and extracted curves from the wall surface, a method not too unlike the meshing of the Aorta in the ICEM tutorial.
I was wondering what exactly is geometry repair? Is it to cover up holes in the model and extract curves from the surfaces?
Thank you very much for your help,
Andris

[diamondx]

sometime when you import your geometry in icem, you will see useless curves and points, geometry repair let you fix that by deleting them, sometimes you can see holes in your surfaces, you can fix that by patching the surfaces...etc
If you have an account in ansys's website, there are training material and workshops, one section is dedicated to geometry repair, you can learn a lot there...

[Andris]

Hi,
Thanks a million for your help. I will check it out.
Regards,
Andris

[Andris]

Hi, just to say thanks for the information, the document has helped alot and my mesh is looking good,
I was just wondering what would be a good enough quality for a mesh?
Do ALL the elements have to be below a certain threshold value? I realise that different applications demand different qualities, so mine is for a simple fluid dynamics simulation.
Andris

[diamondx]

About quality, an expert once said

This is definitely a solver based question… Look at your solver manual (or ask on that portion of the CFD-Online site) and find out what the requirements are. Some solvers are fine with 179 degree internal angles, others are very sensitive to angle quality. Some solvers are sensitive to pyramids but don’t mind really skewed prisms instead…

One thing to keep in mind is that most solvers are going to sneak in a factor of safety, so you may read that they need an internal angle of at least 18 degrees. In reality, 9 degrees would probably be fine and you may even be able to get away with >0 degrees. By publishing higher requirements, the solver tech support can blame any convergence issues on the mesh ;^).

I check a few usual suspects. ICEM CFD “Quality” (circumsphere ratio) should usually be above 0.1 for tetras and hexas, and above 0.01 for prisms. Determinant (1/jacobian) should be greater than 0.1. Angle should be greater than 9 or 18 degrees. Often I will have a few cells of lower quality. As long as they are above zero and not in a critical region, I may still try to run the model and see if it will converge.

oh yea, two more quick thoughts about ICEM CFD quality...

First, prism quality in ICEM CFD is calculated harshly. They divide the prism into 3 tetras and report the quality of the worst one (circumsphere ratio) as the prism quality. This makes the ICEM CFD prisms look much worse than they are, so keep that in mind when comparing qualities between softwares.

Second, at 12.0, ICEM CFD added a TGrid Skew metric to make it easier for Fluent users to check their quality against the Fluent manual. At 12.1, ICEM CFD added an Expansion rate metric for CFX users. (12.1 is not due out until the end of 2009, but the check is already in the Beta version.)

By SIMON

[Andris]

Amazing thanks a million