code_saturne User's Forum

Hello everybody,

One of my test case involving the turbomachinery module is on case with two meshes (generated with ICEM ) which I coupled in CS 5.2 (please see the setup.xml attached). One mesh consists on a cylindrical domain including a horizontal axis tidal turbine) the other the rest of the tank.

Unfortunately the few jobs I launched with this testcase have not even started to iterate. An error pointing a divergence solving for wall distance occured in all my attempts.

Please find attached .xml error and listing files.

Best regards.
FA

Hello,

Did you run a mesh quality check (and visualize the output) ?

The issue you describe can occur mainly when there are very thin and warped cells near the boundary, which can occur in hex-block meshes mainly when the mesh is highly refined normal to the wall (fro viscous layers) but not refined enough in other directions. In this case we could recommend some "bad cell" settings, but in general, it probably means there s more refinement than needed at the boundary.

A view of the mesh (especially a zoom near the boundary where it is most refined) would help confirm this.

Regards,

Yvan

Hi Yvan,

Thank you!
just one thing ids not very clear: What do you mean with "running a mesh quality check"?.. it is about selecting "Mesh quality criteria" in Calculation script parameters?...

Anyway I think may mesh may be too refined around blade's wall (link to the mesh file https://www.dropbox.com/s/06kgirwdnit2g ... .cgns?dl=0 )

Regards.
FA

Hi everybody,

I am trying to face this issue by simplifying my mesh! In this regard I am going to increase the minimum wall distance from the blades. I would like to ask you a couple of questions:
-I would like to know what values of y+ from wall are ideal to use the wall functions provided with the k-w SST?
-What about if I do not use any turbulent model and try to solve euler(for the blades: Do I have to impose Symmetry as BC instead of wall)?

Best regards.

FA

Hello.
what values of y+ from wall are ideal to use the wall functions provided with the k-w SST?
It's usually desired to have an Y+ value for the SST model in range 1...3 or so. One cannot obtain an ideal Y+ distribution along the wall so we can try to approach this range but, in practice, you may have too low or too big Y+ in some locations. I tried Saturne with SST not paying very much attention to Y+ (because it was just test) and it worked well.

At the same time, it' very sensitive to the growth ratio and the cell shape, not like Fluent or CFX that will "eat" even very bad (although not any) mesh without divergence. When you have the inflation layers you also have the transition from prisms to your "main" volume mesh. If the growth ration at this transition boundary is too high Saturn is likely to diverge (I made the test, didn't manage, with various settings, to run it without divergence on the mesh where this transition growth ratio was quite high).

One "funny thing" is that Fluent diverges on the gas turbine swirled-outlet case with high velocities up to ~250m/s while Saturne works Turbulence models was SST, mesh was made with Salome NetGen mesher.

Hello,

I'll just add that last week, an "all y+" wall function option was added to the EBRST and SST turbulence models (If I remember correctly, some of the progress on the "all-y+" work was presented at the 2016 user meeting). In any case, it is still better to avoid having too much "very thin" wall layer cells, especially on curved surfaces, because they degrade mesh quality.

I hope to release version 5.3 later this week, so these options may be available then.

It would be interesting to see how the model mentioned which diverged on FLUENT works with the new options, as we now use more "standard" boundary conditions for k-omega (but an option allows reverting to the previous behavior).

Best regards,

Yvan

Hello,

Thank you both of you for your answers!
I will be more careful on the quality of the mesh that I am going to do with ICEM. In these last few days though I have worked on doing a coarser and less refined mesh next to the walls (blades in my case) in order to perform an inviscid simulation. (I want to test "the coupling" option in the turbomachinery module before running a "full NS"; I need more time to further adjust my mesh.).


This morning I launched my case (inviscid) with the version 5.2 and the following error was given:
Invalid turbulence model: off.

For the BC in Code Saturne I tried both Symmetry and wall. The error aforementioned appeared in both cases.

I think this it may be due to the nature of BC given when I saved the mesh in a cgns file in ICEM.

The following BC were given:
1) BCtype general for the surface meshes to be "coupled" with the second mesh in code saturne
2)BCtype wall for blades and hub

Please find attached setup.xml and listing file.

Best regards.

FA

Hello,

This actually seems like there is an inconsistency in the setup (or a bug in the GUI). Could you check that you have a turbulence model activated under the GUI ? Upgrading to version 5.2.1 might help.

The issue is probably not related to ICEM export options, as Code_Saturne only reads the names of the boundary conditions, not their natures.

Best regards,

Yvan

HI Yvan,

What do you mean with: Could you check that you have a turbulence model activated under the GUI?

Under Turbulence model I selected the following: No model(i.e. laminar flow)
which is the option I guess I should adopt to run an inviscid case.

Best regards,

FA

Hello everybody,

By updating to the version 5.2.1 as Yvan suggested, I did not face this issue anymore. I am trying a frozen rotor with mesh coupling. No turbulence model is used.
The job started to iterate, but it looks very unstable although the the CFL number seems to be within the "stable range" (below 10) when the velocity starts diverging.


What is weird this time is that no error file was written. The only information regarding this error is written in the file attached script_parallel.o2066175.txt
Please find also listing and setup.xml.

Best regards.
FA