Create Mesh with viscous layer

Hi,

My name is Matthias and I am working for a small hydropower company in Austria. I use Salome for FEM Meshing together with code aster. Right now I am trying to do a CFD analysis with code saturne and I am trying to create a mesh. 

I am trying now for quit a long time and I fail to create a mesh with and without viscous layer.

I was wondering if maybe one of you could try out if he/she is able to get a mesh easily. Maybe if you know the right algorithm it is not so hard. Attached is the geometry and also the salome file. In the salome file the faces for the boundary conditions are created.

It is a distributor for a pelton turbine. The first cell for the boundary layer should be 0.009m. But for the beginning also a mesh without viscous layer would be enough.

Thanks for any help.

Best Regards

Matthias

Hi Matthias

I would try if you attached your geometry.

St.Michael

Hi,

Thanks you very much. That would be great.

Link:

https://www.file2send.eu/de/download/bEcW49MLQ.AWB.kgNt1PWYSBret7.iofsJHnJA15X4JfKsD.dn-7U3VgaWPD4vk2TEo7

BG

New Link:

https://www.file2send.eu/en/download/cq3sCpiyTM3FZrR1c1.g.5J5hWuIbaVK9KsY2WrssypGFre48OfTUVOKW9Q0Chu5c1K6

New Link:

https://www.file2send.eu/en/download/cq3sCpiyTM3FZrR1c1.g.5J5hWuIbaVK9KsY2WrssypGFre48OfTUVOKW9Q0Chu5c1K6

I manged to make a 3D mesh at least. My steps were:

1) I created a mesh with NETGEN 1D-2D w/o a hypothesis and compute it.
2) Meshing failed on 18 faces. I published them in the study tree by clicking [Publish Sub-shape] in Computation report dialog.
3) I checked the mesh that NETGEN generated on these problematic faces to see what caused the failure. It was too dense 1D mesh generated on boundaries of these faces.
4) To fix this, I created a sub-mesh on these 18 faces with Wire Discretization and Local Length = 0.5. Then 2D meshing succeeded.
5) I added Tetrahedron (Netgen) algorithm and finally, in a couple of hours, got a 3D mesh.

St.Michael

Thank you very much. I tried it out and i also get a mesh now but i guess with viscous layer it is not so easy ? Right now code saturn does not accept the mesh. Do you know do I need special mesh for saturne?

I added Viscous Layers hyp ( 5 layers per 0.009 ) and the mesh computed OK.

I don't know requirements of Saturne. What it complains about?

St.Michael

hello St. Michael

I am working on a turbine and the mesh process ends successfully with "viscous layer". My problem arises when I import the mesh to openFoam, the mesh is getting errors if I run "checkMesh". If I do not include "viscous layers", "checkMesh" does not report errors in the mesh. Could you help me?.

Thank you.

Hi

I can try but usually if viscous layers are incorrect, there is nothing the user can do. You can post you model here so that the salome developers could fix a bug.

St.Michael

Hi St. Michael.

this is my .hdf file. As I said before, Salome does the mesh without problem. If I don't use "viscous layers", checkMesh does not report errors. with "viscous layers" checkMesh fails in the geometry check

https://www.mediafire.com/file/2gypatyp17ytcnq/malla_3.hdf/file

Hi

Alas! There are intersecting prisms.

St.Michael

Hello,

If you are using code_saturne, you can also add viscous layers inside code_saturne itself.

Compared to doing this in Salome, cell elements may be a bit "flattened", and bulging may occur in some "free" sides in some cases if not enough faces are constrained (due to an incomplete feature). On the other hand, intersecting elements are mostly detected and avoided by reducing the number of layers where this is overconstrained, as shown here : https://github.com/code-saturne/code_saturne/issues/7.

So for many industrial cases with complex geometries, we generate meshes with Salome without boundary layers, and add those in the code_saturne preprocessing. This is not infallible, but generally more robust.

Best regards,

  Yvan