CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Native Meshers: snappyHexMesh and Others (http://www.cfd-online.com/Forums/openfoam-meshing-snappyhexmesh/)
-   -   Refinement edges (http://www.cfd-online.com/Forums/openfoam-meshing-snappyhexmesh/104298-refinement-edges.html)

vinezio July 6, 2012 06:28

Refinement edges
 
5 Attachment(s)
Hi Foamers,
the figure shows the inlet and outlet of my cooler. I would to ask you how i can obtain the similar result in proximity of edges. The concentric layers are important to study turbulence model. This geometry comes from fluent export. Any ideas??

SirWombat July 7, 2012 06:04

Hi Vincenzo,

your "snappyHexMeshDict" looks good. If your layer cells don't get filtered by the quality settings, then this should be fine. (You could switch off all quality controls and check what it looks like then. Then carefully raise quality controls until "checkMesh" gives you an OK ... << see this post)

So why are there no layer cells?:

Assuming, that the images you posted are the full geometry, then here is a possible answer: snappyHexMesh cannot make layer cells orthogonal to a boundary. They will always start growing at a boundary edge. So unless you will cut your geometry in half in paraview/parFoam you will not see, whether there are any layers and what they look like. You could use a cutting plane for that, or better "extractedCellsByRegion".

SOLUTION:

AFAIK there is no solution for that problem. Though it might be possible to extend the geometry at the boundary, then snappyHexMesh the extended version of your mesh and afterwards cut the extended part off. But this is only a idea ... I never tried it.

Greets,
Jan

vinezio July 10, 2012 19:14

Thanks so much Jan!! I'm tried several options. We'll inform about the progress.

Greets,
vinezio

SirWombat July 13, 2012 13:58

Hi Vincenzo,

I just came across a possible solution:

If you set your "inlet"-patch to patch type "empty" in your blockMeshDict then snappyHexMesh will give you orthogonal cell layers. No need for cutting!

e.g.

Code:

...
    inlet
    {
        type empty;
        faces
        (
            (0 4 7 3)
        );
    }
...

then run blockMesh and SHM.

Afterwards you will need to change the patch type in the "boundary"-file located under "constant/polyMesh/" to type "patch".

Here's the link for reference: https://sites.google.com/site/snappy.../cylinder-case


Greets, Jan


All times are GMT -4. The time now is 22:11.