Restart with new mesh

[StandardRANSUser001]

Hi Everyone,

I am having some trouble in resarting a case with a new mesh, and perhaps I am doing this incorrectly? I am working on a HPC system, and I am unable to use the GUI. I am currently using the cs_user_parameters.py script to load the exisiting results, the existing men_input.csm (14,043,600 cells), and the new preprocessed mesh_input.csm (32,971,890 cells). I think I have done this correctly, and the case begins, but there is an error with the wall distance calculation.

I have found that there are some flags available for reprocessing wall-distance (https://www.code-saturne.org/documentat ... tance.html), but I am unsure of how I activate one of these flags. Could anybody please provide advice on this? Both mesh are structured, and have been developed with the same script, the only difference is the cell density.

Hopefully this is a very easy fix!

Best regards,
Sean Hanrahan

=============================================
@
@ @@ WARNING: Wall distance calculation
@ =========
@ The laplacian solution does not respect the maximum
@ principle in 8787225 cells. We recompute the laplacien
@ without reconstructions.



cs_wall_distance.cpp:510: Fatal error.

Problem for the positivity of wall distance


Call stack:
1: 0x14fb0a0d6d1e <cs_wall_distance+0x131e> (libsaturne-8.2.so)
2: 0x14fb0a11fff4 <tridim_+0x62f4> (libsaturne-8.2.so)
3: 0x14fb09e71254 <caltri_+0x316e> (libsaturne-8.2.so)
4: 0x14fb0ae0780b <+0x580b> (libcs_solver-8.2.so)
5: 0x14fb0ae07b20 <main+0x157> (libcs_solver-8.2.so)
6: 0x14fb0001e24d <__libc_start_main+0xef> (libc.so.6)
7: 0x202e1a <> (cs_solver)
End of stack
==================================================

[Yvan Fournier]

Hello,

The issue seems to be that the mesh quality is bad, or for example you have very thin and warped or non-orthogonal cells at the boundary. This will cause convergence issues with all variables unless you deactivate flux reconstruction.

You may also try to use the mesh robustness options (check for cs_glob_mesh_quantities_flag in the cs_user_parameters-base examples), but this can be of limited help.

Best regards,

Yvan

[StandardRANSUser001]

Dear Yvon,

Yes I am studying something that vaguely resembles a pipe flow with a structured mesh, and I use grid stretching at the inlet and outlet. This means that I have a very refined boundary layer region, but very stretched elements near the domain inlet and outlet.

So is this an issue with interpolating a coarse solution mesh onto a more refined mesh? If I interpolate a refined mesh onto a coarse mesh, will I have the same problem? Just checking that this function works for the CS development team?

Perhaps this is a discussion for a new post, but perhaps this relates to the mesh quality as well. I am working with K-W SST and EBRSM models, and I have had success in deactivating flux reconstruction for the k and omega terms. I am having a lot of trouble working with the EBRSM model though, as a "checkerboard like effect" occurs for the epsilon and Rij fields, and this looks like clipping in regions where I would not expect this to occur. This occurs regardless of whether I am using coupled or uncoupled solving of Rij, and regardless of whether CS_TIME_STEP_LOCAL or CS_TIME_STEP_CONSTANT. This clipping does not seem to affect the velocity or pressure fields.

Is this issue also related to mesh quality?

Best regards,
Sean Hanrahan

[Yvan Fournier]

Hello,

Regarding the EBRSM model, I'll let Jean-François provide more details or recommendations.

Otherwise, regarding interpolation, the problems you will have or not have probably simply depends on the target mesh. Simply running a few iterations from start on that mesh should give you an idea of the expected behavior.
If you have already done this, all seems fine, and you have problems specific to the interpolation case, do let us know. Maybe some post-interpolation smoothing is necessary in this case, and I could explain how to add/test that in an additional loop in cs_user_initialization.

Otherwise, regarding mesh quality, just remember that high aspect ratios and curvature do not go well together when using reconstruction in our colocated finite volume schemes, though using gradient limiters might help.

Best regards,

Yvan

[StandardRANSUser001]

Dear Yvon,

Thanks for your comments on this.

If you could provide Jean-François' contact information, that would be very helpful. I have several more questions about the EBRSM, and his advice would be really helpful for my current project.

A little bit more information about the mesh. The geometry is complex and has considerable surface curvature, and the structured mesh has been developed with a target cell height of y^+<1.0. A consequence is that the cells do have a high aspect ratio near the wall. Both mesh run separately with the KW SST model, although I have been receiving a warningin the run_solver.log file that "Incoming flow detained for 621 out of 33200 outlet faces", and the number of detained values changes with each timestep. I have used an extended outlet with some grid stretching in the streamwise direction to prevent the outlet interfereing with the region of interest.

It would be great if you could provide recommendations on post interpolation smoothing, as well as any guidance on using the gradient limiters.

Best regards,
Sean Hanrahan