T-Junction CHT Internal Coupling Simulation not working with Fillet

[saintlyknighted]

Hi, I have been trying to set up a CHT internal coupling simulation of a T-Junction in code saturne to measure the temperature gradients in the pipe wall. I have this working in a T-Junction geometry where there is no fillet i.e a 90 degree corner. However when i add a fillet and carry out the same workflow in SALOME of partitioning, assigning a fluid and solid region and meshing the full geometry as I did on the geometry with the 90 degree corner, the simulation no longer works. Below are the error logs:
field minimum maximum set mean spatial mean
- -------------------- -------------- -------------- -------------- --------------
v boundary_stress[X] -15438 15516 -5.3207 0.63226
v boundary_stress[Y] -15682 15682 -3.7718 26.518
v boundary_stress[Z] -12335 8541.6 -139.42 -54.865
v ǁboundary_stressǁ 0.063707 15682 2953.3 2058
v Yplus 0 189.29 6.8319 9.4802
v Boundary temperature 20 60 -nan -nan
v Boundary Density 1000 7850 5187.2 5050.6


/home/saimmateen/Documents/code_saturne-9.0.0/src/base/cs_log_iteration.cpp Fatal error.

Invalid (not-a-number) values detected for a field. I have also seen that the number of fluid faces is not equal to that of the solid faces for the coupling interface: "auto:internal_coupling_0"
boundary faces: 15424
"auto:internal_coupling_0_fluid"
boundary faces: 8522
"auto:internal_coupling_0_solid"
boundary faces: 6902 The simulation with the 90 degree corner has 37k boundary faces. I would expect it to be less for the fillet, but not half as much. Does anyone know how to get this simulation working with a fillet and overcome this error? I have attached mesh and simulation files. Thanks.

[Yvan Fournier]

Hello,

There may be several issues here. Looking at the mesh, it seems that only the fluid portion is extruded, not the solid portion. Is this desired ? In any case, the code separates the fluid and solid parts before extrusion, which explains why y have more auto:internal_coupling_0_fluid than auto:internal_coupling_0_solid faces.

In the future, it will be be possible to choose the order of preprocessing operations, but thi is not the case today. And for thermal internal coupling, we should separate the fluid and solid faces last, but this is not the case here (a special test would be needed to change the order, so I'll see if doing the fix is easy or not).

In any case, it could be safe do do the extrusions in a separate preprocessing step, then run the computation with internal coupling starting from the first step's mesh_output (and without additional extrusion on that run). This would avoid having a discrepancy between auto:internal_coupling_0_fluid than auto:internal_coupling_0_solid faces, and might fix the issue.

If you still have the crash, you may need to change numerical options for robustness, but if the code ran well with the original mesh with no fillet and mesh quality is similar, I suspect the issue is more "topological" and can be fixed by the suggestion above.

Although in any case, you mesh is quite coarse, and using an orthogonal boundary layer mesh (such as that obtained using code_saturne's boundary layer insertion, available through user-defined functions, or building a viscous boundary layer mesh zone in Salome) would be better numerically.

Best regards,

Yvan