code_saturne User's Forum

Hi everybody,

I'm trying to launch calculation with Saturne to obtain the flow around a NACA_0012 airfoil [V=5m/s, alpha = 0°].

By using Salome to mesh the volume, I did these steps :
 
Create group of edges [Inlet, Outlet, Extrados ...] in GEOM Module Mesh the 2D face which is a partitionned face with triangles. Create Submesh to create a quadratic mesh close to the airfoil to be able to see effects close to the airfoil Extrusion along a path in MESH Module Import group from geometry [With the extrusion, the group of edges changed into group of faces, Salome extends the name like this : Outlet_extruded for all groups.] I used Code_Saturne to start calculation and define boundary conditions

At the end, I obtain a result which apply "something" on the border between quadratic and triangle mesh ! Nevertheless, I would like to apply a free face on this border, as my real airfoil is behind. I don't know how to be able to apply something on an internal face and how to see this face in the "Group of faces" ?

I tried to define in GEOM the edge on the 2D face, but I didn't see it in the Group of faces after extrusion. I think it's due to its internal characteristic.
 
I attach screen shots of this results (pressure, velocity and tke), and also the mesh.
 
I would like to know if you have a solution, or some advices.
 
Regards.
 
Gauthier

Turbulent Kinetic Energy screen shot

Hello,

I am not sure I understand your question. Normally, the way your mesh was built, faces at boundaries between extruded triangles and extruded quadrangles are just interior faces, not distinguishable from any other, so if that is what you call "free faces", this is already the case.

It is otherwise not currently possible to apply specific treatments to interior faces (you could use a source term or a head loss on cells containing those faces, but nothing applies directly to interior faces).

If you want to do some post-processing on those faces, create a group of edges (faces once extruded) at the boundary between triangles and quadrangles, then use the usdpst user subroutine to define a post-processing sub-mesh by calling "getfac" for that group's name.

Best regards,

  Yvan

Hello,

I agree with you that normally, faces at boundaries between extruded triangles and quadrangles are just interior faces and nothing is applied in theory.

But, if you have a look on pressure results, you could see an excessive pressure on the leading edge before the physical airfoil; which is wrong. I applied wall boundary conditions and tick "sliding wall" with all coefficients equal to 0 on Extrados and Intrados.

Do you think this result is due to wrong boundary condition applied on the airfoil ? Or, due to a wrong mesh quadrangles_triangles ?

Thanks for your help.

Gauthier

Hello,

I checked my boundary conditions, and I didn't tick the sliding wall case for extrados. By correcting this error, I obtained better results as you can see, we can see Von Karman Vortex at the trailing edge.

Nevertheless, I would like to change the angle of attack. I tried to modify the inlet boundary conditions parameter with "direction" "user profile"
Dx = 5*cos(20°);
Dy=0;
Dz=-5*sin(20°);

Do you think that we can consider a wind direction equal to 20° on the leading edge with this hypothesis ? I can also have access to parameters in "Initialization tab" !
 
Thanks for your help.

Regards.
 
Gauthier

Hello,

I am not sure using a sliding wall for an airfoil is useful, as you already seem to work in the airfoil's frame of reference (though using a sliding wall with coefficients set to 0 should be the same as using a simple wall).

The results are strange, so the first thing to check would be that you do not have any "boundary" faces on the interior. use "code_saturne check_mesh" or activate visualization of boundary faces and use transparency in ParaView so as to check that boundary faces only include true boundary faces, and not some interior "construction" faces (though you probably would have an issue with boundary conditions in that case, it is always safe to check this).

Otherwise, it would be interesting to test the sensitivity of your calculation to gradient reconstruction options. The problem may be mesh-related, due to the rapid change in mesh refinement at the prisms/hexahedra interfaces.

Also, we have seen that in some cases leading to divergence due to mesh polarization issues, using a "relaxation of pressure increase" may help (a relaxation factor of 0.9 is enough). If you are using the steady calculation model, I believe this is already the default, but for unsteady calculations, the default value is 1.

Also, I am not sure (due to lack of zoom) how the trailing edge is meshed, but prolonging and merging the "intrados/extrados" sections after the trailing edge may be better.

If you still have issues, we are interested in having your mesh if that is possible.

Best regards,

  Yvan

I think you posted this comment before having time to read my comment with new results.
The mesh.med is too big to be attached, and I didn't write the script for the mesh in python. I have only the Geometry in python.
Regards,
 
Gauthier