CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Tetra boundary layer (http://www.cfd-online.com/Forums/ansys-meshing/112205-tetra-boundary-layer.html)

mario1701 January 23, 2013 16:52

Tetra boundary layer
 
Hi,

I have to create a tetra boundary layer around a high-speed train in ICEM and I wondering what is the best way to do it - so far, I have read just about hybrid meshes or prism boundary layers (as I have mentioned before - it has to be tetra mesh). I would be very grateful for any smart methods.

Mario

Far January 23, 2013 17:24

1. tetra size ratio

2. tetra width


http://imageshack.us/a/img267/8161/51943058.jpg

diamondx January 23, 2013 19:39

sorry for jumping in, i have a question in the surface mesh tab, what does tetra width useful for ???

diamondx January 23, 2013 19:51

i have chaging it but nothing change ??

Far January 23, 2013 23:42

Quote:

Originally Posted by diamondx (Post 403658)
i have a question in the surface mesh tab, what does tetra width useful for ???

Quote:

Originally Posted by diamondx (Post 403661)
i have chaging it but nothing change ??

It is working when you define the tet width and ratio for the volume meshing. It applies these settings on volume and surface. But only for surface meshing, I dont think they have any effect.

PSYMN January 24, 2013 09:12

Tetra width specifies the number of elements into the volume before the tetra ratio starts to expand the mesh. It only works with Octree Tetra.

If I had a surface size of 2 and a max size of 64 and a tetra width of 3, I would get at least 3 layers of size 2 volume mesh before the mesh started to expand up to the max size.

It is like putting a mesh density region near the surface, and in fact, works the same way in the back ground.

mario1701 January 26, 2013 11:04

Thank you very much for reply, but in case of using wall functions, it doesn't influence the results (y+ is not decreasing). I thought rather about characteristic "elongated" shape, which can be obtained with use of the prism mesh. Maybe I should create such a prism mesh and then convert it into a tetra mesh?

Far January 26, 2013 11:09

Are you using scalable wall functions? What is the minimum wall Yplus in your simulations?

I think prisms are better than tetras

mario1701 January 26, 2013 18:11

I was using standard wall functions. Unfortunately, I have to use tetras (I use some special applications developed at my university that need tetra meshes). Y+ is still huge - on mesh of 126k nodes I have minimal y+ on the surface of locomotive equal approximately 2e3.

Far January 27, 2013 02:23

are you sure about units of your model?

Another option is to use the T-Rex type algorithm!!!

mario1701 January 27, 2013 13:04

When it comes to the units - everything seems to be correct. The mesh was created in [mm] and is correctly read by fluent (the main dimensions are presented in meters, but are for sure correct). I tried to create a prism boundary layer and then converted it to tetra - y+ decreased signifficantly, but the quality of the worst element is quite low (I am not sure if 0.05 - 0.1 for 15% of elements is a reasonable level - but maybe for boundary layer it does not matter (large pressure changes just in normal direction)?). ICEM does not support T-Rex, does it?

PSYMN February 6, 2013 10:54

Sure, use prisms to get the Y+ you want and then use the Edit mesh option to change mesh type and covert all to Tetra...

Roberto Meloni September 12, 2014 09:56

Transition between finer and coarse mesh zones
 
1 Attachment(s)
Hi All.
I have a problem with a mesh Iím trying to build and I wonder if you can help me to solve it.
My problem is that I canít define a proper transition between finer zones of the model and the coarse ones. I set up specific part size for the surfaces as well as for tetra size ratio, but it seems not to work fine. I believe that the system doesnít respect the mesh size of the mesh I specify on the surface, but it builds a very finer mesh.
Iíam meshing with the following setting:
- Robust(Octree);
- Patch Independent
- In the Global Mesh Size panel, I enable the Curve/proximity based refinement
The high density zones you can see from the picture refer to small holes. I have to mesh them with a very fine mesh (0.17 mm). The red zone refer to the core region of the model.

Could you please help me?
Best regards,
Roberto.


All times are GMT -4. The time now is 05:09.