Hybrid Grid

[rbecker]

Hello,

I try to calculate the flow in a hybrid grid, where one zone is built from hexahedral and a second zone is built from tetrahedral elements. Both zones are connected by pyramids, so that the mesh is conformal.
I have found that the code calculates unreliable results, whatever time stepping (IDTVAR), Gradient Reconstruction scheme (IMRGRA), spatial resolution scheme I use. It seems CS has problems handling the pyramids. Do I have to make special provision to handle such a hybrid grid?

Thank you in advance.
Kind regards,
Ralf Becker

[Brian Angel]

Hello Ralf,

Can you attach a couple of images of the mesh and the results so that I can take a look? When you say that the results are unrealiable, in what sense are they unrealiable; visually, when comparing with experimental data? Also, where are the results unreliable; next to the walls, in the zone where there are the pyramid cells, other zones of the mesh?

Best regards,

Brian Angel.

[Yvan Fournier]

Hello Ralf,

Could you also tell us what mesh format the mesh was saved in ?

Best regards,

Yvan

[rbecker]

Hello Brian, hello Yvan,

mesh format is "CGNS".
I repeated the calculations with a much simpler geometry. The conclusions are more or less the same.
The geometry is a 50mmx50mm square duct, with inflow at x=0, v = 10m/s.
Parameters for both calculations are: IDTVAR=0; DTREF=1e-6, IMRGRA03, ITURB=0, NTMABS=10000.
I have attached the head of the listing and the CGNS files (ICEM), displayed are the solutions (magnitude of velocity) in the last step.

Kind regards,
Ralf

[Yvan Fournier]

Hello Ralf,

Could you also post your flow conditions (or xml file) ?

Otherwise, could you show a cut plane of the flow inside the mesh ? As the view of the "outside" of the mesh shows values at cell centers, with tetrahedra and hexahedra of less regular thicknesses near the boundary, you might be visualizing the flow at various y+ values. This could be a good part of the explanation depending on your boundary layer thickness. In this case, visualizing the flow at vertices (Cell data to point data filter under ParaView, Cell to Node under EnSight) would provide a smoother visualization.

Otherwise, increasing the number of "sweeps" for the resolution of pressure and velocity may help. With versions 3.x, velocity components are solved in a coupled manner, leading to better impliciting of certain terms for the boundary layer (no guarantee it would make a difference for your case, but it might help). Options such as number of sweeps are also accessible using the GUI in 3.x, while you need user subroutines to adjust them with version 2.0.

In any case, a layer of prisms at the boundary, allowing for a more regular "cell center to wall" distance should help if you can build it easily (as you seem to be using ICEM, this should be relatively easy for you).

Best regards,

Yvan

[Brian Angel]

Hello Ralf,

I've just imported your mesh into the Code_Saturne GUI and ran the mesh check. All seems to be okay with the mesh but I cannot see any boundary conditions defined. Can you let us know where or how you are specifying your boundary conditions? Also, as Yvan has asked, can you upload your xml file and images showing internal slices of the volume mesh?

Another thought, can you confirm that each mesh type has common vertices (or nodes) at the interface between the two meshes for all cells?

Best regards,

Brian Angel.

[rbecker]

Hello Brian, hello Yvan,

thank you for the help and the suggestions.
I tried a grid with a prism layer, but this does not change the situation. A calculation with an increased numbers of sweeps (NTERUP) is just running.
Could it be an ill-conditioned LS? This might result in a flow field, where the calculated values in the hex elements are more or less constant and the flow develops in the tet-region.

Nevertheless, I have bundled the result-files (Tecplot-Format), the fortran source codes (BC and solver options) and
some slices displaying the internal flow in a tar-archive.
As, I couldn't attached it to the post, please download it from: http://www.akk.org/~ralf/hybrid.tbz2.
Sorry for the inconvenience.

Kind regards,
Ralf

[Brian Angel]

Hello Ralf,

I generated via SALOME a square duct with dimensions of (x,y,z) 1000mm x 50mm x 50mm. The first half of the duct (0mm to 500mm) is meshed using hex cells and the second half (500mm to 1000mm) using tet cells. Two meshes were generated. The first mesh is relatively coarse, please see the images Mesh_Hex_1, Mesh_Tet_1 and Mesh_Hex_Tet_1_ClipZ=0.5. The second mesh is finer and an extrusion layer is used for the tet mesh, pls see the images Mesh_Hex_2, Mesh_Tet_2 and Mesh_Hex_Tet_2_ClipZ=0.5.

I ran a CS simulation for 500 iterations using V3.0. An interface was used to connect the two meshes. The first mesh gives results very similar to yours, i.e. a smooth velocity field in the hex mesh but a bizarre looking velocity field in the tet mesh. Please see image Vmag_MeshHexTet_1. However, the second mesh gives reasonable looking results and the velocity field is very smooth and continuous in the tet mesh. Please see the image Vmag_MeshHexTet_2.

I see that you are using CS V2.0, can you update to V3.0 which is available for download on the Code_Saturne website? Can you also regenerate the ICEM mesh using the second mesh as a possible template? This second mesh has the following specs:

Hex cell size : 5mm cubes everywhere
Tet cell size : max size = 5mm, min size = 2mm
Extrusion layer : 5mm thick, 3 cell layers with an expansion ratio of 1.2

Best regards,

Brian.