[Situla]

Hi!

I have been working with SU2 for a few weeks now and managed to get decent results for my aerofoils when solving Euler problems. Since my main goal is to obtain the pressure coefficient distribution at Mach numbers up to about 0.8 or 0.9, I started looking into the Navier Stokes problem, but I cannot seem to get the solution to converge. I am also struggling to interpret the residuals, because the default output shows me "Res[Rho]" and "Res[nu]", but there seems to be no correlation of those to the "log10[maximum residual]" in the intermediate reports. Also, some of my Euler problems which did converge exited after reaching the convergence criteria (reduction of residuals), but the "Res[RhoE]" of the last iteration was sometimes as high as 2.

As for my attempts with NS, I have tried high and low

• CFL numbers
• Mach numbers
• AOA
• JST dissipation coefficients

for both the SST and the SA model, as well as varying some other settings, all relative to the configuration file of the transonic turbulent aerofoil tutorial.

I do not know too much about most of the CFD settings, so it could very well be that some silly mistake is causing these problems.
In general, what confuses me and what might very well be the main error in my setup are the geometry markers. For example, I do not see how SU2 can know about the flow direction if I do not give an "inlet" marker (only far-field), but exactly these simulations were the ones that looked most promising. With regards to markers in the NS problem, I have tried the following combinations for my square domain.

• inlet left and far-field on all four sides
• only far-field left
• far-field everywhere

...and maybe some others I have forgot.

I attached my current configuration file, but it is a mess because I am varying parameters everywhere and trying various combinations.
Any information to shine light upon my ignorance will be greatly appreciated.

@SU2 team: you're doing great work! Very impressive.

EDIT: I am getting a much more steady iteration behaviour after reducing the CFL to 0.2 (using a threefold multi-grid right now), judging by the residuals. Despite that, however, there does not seem to be a converged solution in sight (after 16k iterations) - again, judging by the residuals. The intermediate flow results qualitatively look somewhat reasonable in Paraview, but that seems to be the case regardless of what SU2 tells me about the residuals in the console.

[wallym]

Hi Situla!


Thanks for using SU2 and posting on the forum!


You are indeed running with a low CFL, which suggests something is going on. Your config looks good, and JST should be able to converge this.



My two main thoughts are that boundary marker behind the airfoil needs to be BC_OUTLET or the problem is actually unsteady. Lastly, it could be mesh dependent. These could prevent convergence in your case.



What were your residuals in your last run?


I hope this helps.


Wally

[Situla]

Hello!

Thank you very much for your reply.
It is interesting that you say this, because I have used several different configuration files from tutorials and they do not seem to have any markers other than the body and the far-field.
I will of course try it.

Well, in the very last run, which I did now with a modified configuration file, were -4.4 for Res[Rho], -6.9 for Res[kine], and -1.1 for Res[omega], which was achieved by only thirty iterations, but then it auto-exited, telling me that it diverged. I really cannot make sense of what those residuals mean.

[wallym]

Your residuals are good, but it seems something got set or was divided by zero. This could possibly be an incorrect config option, but it may be a code issue.



What version of SU2 are you using?
Would you mind uploading the mesh file so I can take a look (hopefully later today)? Also the config file, if is not the same as the one you posted earlier?

[Situla]

I am using release 6.2.0. Here is a set of data from a few hours ago. Unfortunately, I cannot seem to upload an su2 mesh file, and the mesh is about 7 MB large. If you happen to have gmsh, I uploaded the geometry file I used to generate the mesh.

Thank you very much for your time!

EDIT: FYI, the config file is similar to the previous one. The main difference is that it was ROE instead of JST.

[wallym]

I was unable to generate your mesh unfortunately. However, running on the NACA0012, I did not run into any issues with your config, I was able to bump up the CFL to 10. My guess is there is something in your mesh that SU2 doesnt like. It could be that the there isn't enough refinement in the boundary layer, or some cells are a bit wonky.



I hope this helps,
Wally

[Situla]

Okay, I will try refining the mesh.
Quite honestly, I think it could be explained by the boundary conditions. I am not sure how to set them. For a square domain, do I use far-field top, left, and bottom, and a pressure outlet on the right? What pressure should I prescribe at the outlet? My simulation 'converges' (log(res) < -4) best if I use a lower pressure, but should it not just be the free-stream pressure (e.g. 101325 Pa)? If I use that - or anything close to it - , the residuals immediately diverge.
I can observe a phenomenon as shown in the attached image, which leads me to believe that something is definitely wrong with by boundary settings, but of course that does not exclude the possibility of errors in any other settings.

[Situla]

For future reference, I managed to achieve convergence after consulting a professor at my university.

I went back to a mesh without a pressure outlet (far-field and only far-field everywhere) and used the FREESTREAM_VELOCITY parameter to prescribe the direction of the flow. This is what threw me off, because several tutorial configuration files (mostly those which somewhat resemble my case) do not contain that, and I could not figure out how the solver knows the direction of the flow if only a far-field is prescribed.
For the free-stream velocity parameter I used the vector (1.0 0.0 0.0) and then used FREESTREAM_VEL_EQ_ONE for the (non-)dimensionalisation ("REF_DIMENSIONALIZATION"). Having done that, the setup converged after less than 2000 iterations because high CFL numbers did not lead to immediate divergence using the SA turbulence model. I am currently running the same case with SST to see what I get.

Thank you for your time and help.

[wallym]

That is interesting. The image of the outlet, is indeed concerning. Ill look into in the coming days.

I am glad you were able to reach convergence with non-dimensional flow parameters. I hope SST works!

[ari003]

Originally Posted by Situla

Hi!

I have been working with SU2 for a few weeks now and managed to get decent results for my aerofoils when solving Euler problems. Since my main goal is to obtain the pressure coefficient distribution at Mach numbers up to about 0.8 or 0.9, I started looking into the Navier Stokes problem, but I cannot seem to get the solution to converge. I am also struggling to interpret the residuals, because the default output shows me "Res[Rho]" and "Res[nu]", but there seems to be no correlation of those to the "log10[maximum residual]" in the intermediate reports. Also, some of my Euler problems which did converge exited after reaching the convergence criteria (reduction of residuals), but the "Res[RhoE]" of the last iteration was sometimes as high as 2.

As for my attempts with NS, I have tried high and low

• CFL numbers
• Mach numbers
• AOA
• JST dissipation coefficients

for both the SST and the SA model, as well as varying some other settings, all relative to the configuration file of the transonic turbulent aerofoil tutorial.

I do not know too much about most of the CFD settings, so it could very well be that some silly mistake is causing these problems.
In general, what confuses me and what might very well be the main error in my setup are the geometry markers. For example, I do not see how SU2 can know about the flow direction if I do not give an "inlet" marker (only far-field), but exactly these simulations were the ones that looked most promising. With regards to markers in the NS problem, I have tried the following combinations for my square domain.

• inlet left and far-field on all four sides
• only far-field left
• far-field everywhere

...and maybe some others I have forgot.

I attached my current configuration file, but it is a mess because I am varying parameters everywhere and trying various combinations.
Any information to shine light upon my ignorance will be greatly appreciated.

@SU2 team: you're doing great work! Very impressive.

EDIT: I am getting a much more steady iteration behaviour after reducing the CFL to 0.2 (using a threefold multi-grid right now), judging by the residuals. Despite that, however, there does not seem to be a converged solution in sight (after 16k iterations) - again, judging by the residuals. The intermediate flow results qualitatively look somewhat reasonable in Paraview, but that seems to be the case regardless of what SU2 tells me about the residuals in the console.

Hi Martin, I m a new user in SU2 and I would like to know how did you plot the coef of pressure along the upper and lower surface. Would be really helpful if you respond.

[bigfootedrockmidget]

I don't know the solution approach of the other users, but my preferred approach is to save output results as PARAVIEW_MULTIBLOCK. In paraview, you then have the surfaces available as separate entities and if it is a 2d geometry you can plot directly over the 1D contour.