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] Non-Conformal hexa mesh (http://www.cfd-online.com/Forums/ansys-meshing/110168-non-conformal-hexa-mesh.html)

RodriguezFatz December 5, 2012 06:06

Non-Conformal hexa mesh
 
1 Attachment(s)
Hi all,

I would like to try a non conformal mesh for a case, where one part is solid and the other one is fluid. Heat-conduction via the non conformal boundary couples the two domains:
Attachment 17478
I want to use ICEM blocking (hexa meshing) and later Fluent.
Now, as far as I understood it correctly, what I could do is:
Pre-meshing one part - convert it to unstructured mesh. Then pre-meshing the other part and convert (merge) to unstructured mesh. But then, during pre-meshing of the second part, all edge parameters of the first part get lost. This doesn't seem to be the best way to me.

If someone advises me against doing this at all, feel free to post :cool:

diamondx December 5, 2012 11:49

hmmm don't know why this happens, if it's non-conformal, why do you care about same edge parameter ?
Try isolating the block, topology - substract block... see if it can fix the problem...

RodriguezFatz December 5, 2012 11:58

Quote:

Originally Posted by diamondx (Post 395954)
hmmm don't know why this happens, if it's non-conformal, why do you care about same edge parameter ?

No, I do not care at all, but I never did this. :D I just don't know how to
a) tell ICEM that two neighboring blocks have a non-conformal surface between them and
b) tell the adjaced edges (to both blocks) that they have different numbers of cells in direction of block one than in direction of block two.

This is where I struggle.

diamondx December 5, 2012 12:19

This is how i usually do it... most of the setting is done in fluent
i create the mesh for the first part, i call the interface "interface-1"
I create the mesh for the second part, i call the interface "interface-2"
I joined them in fluent... (different msh file)

Far December 5, 2012 14:06

Use two fluids. First turn-off solid and output mesh for the Fluid and then repeat it for the Fluid and output mesh for the solid. Read both meshes in Fluent and create interface

RodriguezFatz December 6, 2012 02:53

Alright that sounds much more handy, thanks a lot.
What do you think in general about the idea of a non conformal interface at a fluid / solid boundary? Is it critical?

energy382 December 6, 2012 07:42

Quote:

Originally Posted by RodriguezFatz (Post 396052)
Alright that sounds much more handy, thanks a lot.
What do you think in general about the idea of a non conformal interface at a fluid / solid boundary? Is it critical?

no, it's recommended! you don't use a 1:1 connection at a fluid-solid interface. But make sure, that both sides have ~ similar mesh (edge paramters).

Even if both meshes are alsmost identical, use mesh match tolerance to make sure, interface is treated as GGI instead of 1:1 (if you use automatic interface)

RodriguezFatz December 6, 2012 08:50

By means of performance - what do I win, when the edge parameters of both meshes are similar anyway? I want to make the faces of the fluid mesh at the solid boundary much larger than the faces of the solid mesh to reduce the amount of fluid cells of the setup.

energy382 December 7, 2012 07:51

The GGI intersection algorithm seeks for overlapping cells from the corresponding interface partner side within a certain tolerance. Thus, in highly bended parts of the mesh, always some cells in the neighborhood might be found which do not really touch or overlap with the cell face currently under consideration.

This tolerance can be reduced with an expert parameter:

ggi separation factor (default = 1)

NOTE: In a 1:1 interface such a reduction is uncritical. In a non-matching interface with different mesh resolution on corresponding interface sides, this can lead to a situation where not any cell at all is detected on the other partner side.

Some best practice hints:

1.) Try to avoid two sides of an interface separated by a gap larger than the local mesh resolution.
2.) In highly curved parts of an interface, mesh resolution should be fine enough so that neighbouring cell face normals have "similar" directions (e.g. angle < 10 deg)
3.) Mesh resolution on both sides of the interface should be of similar size.


Not written by me, but good explanation. I always achieve bad convergence if I don't make the meshes on both interface sides fairly similar (on critical areas).

But hey.....just trial by error :D


I can also recommend this sheets (for a clearer understanding):

https://unihub.ru/tools/unicfdc2/svn...e/TurboGGI.pdf


All times are GMT -4. The time now is 14:45.