[rahul_ju]

Have anyone used Spalart Allmaras turbulence model in SU2 in deforming grid?
I am running SU2 test case of pitching airfoil (NACA64A010) in deforming grid at Mach number 0.796 and Reynolds Number 10000000.
Results in Rigid motion is coming quite different form Deforming grid.Specially in case of plunge motion results are coming completely different in Rigid Motion and Deforming case.
Please let me know if anyone has used SU2 code in viscous transonic regime using deforming grid.

[hlk]

For pitching and plunging motion, rigid motion will be more appropriate, since the shape of the airfoil does not change.
When the mesh is deformed, the quality of the mesh is not always preserved and the resulting solution may be less accurate. You can check the mesh manually by setting VISUALIZE_DEFORMATION = YES. There is a set of options associated with mesh deformation that you can find in the config_template file. I think this may be especially important in the transonic case since you may be dealing with a shock that will change locations on the airfoil - if the shock is moving from a region of the mesh that is highly refined to a coarser region of the mesh in one or both of these simulations, that could explain the difference, since the shock being in a coarse region of the mesh would not produce an accurate solution.

You should also make sure that the solutions are fully converged.
Based on what you describe I think that they should match, but if they are not fully converged or there is a problem with the mesh the results could easily be different.

Originally Posted by rahul_ju

Have anyone used Spalart Allmaras turbulence model in SU2 in deforming grid?
I am running SU2 test case of pitching airfoil (NACA64A010) in deforming grid at Mach number 0.796 and Reynolds Number 10000000.
Results in Rigid motion is coming quite different form Deforming grid.Specially in case of plunge motion results are coming completely different in Rigid Motion and Deforming case.
Please let me know if anyone has used SU2 code in viscous transonic regime using deforming grid.

[rahul_ju]

Thanks For your reply. I have checked with low Reynolds number flow
at Re = 50000 , where with or without any turbulence model results should be identical.

In case of Rigid Plunge Motion I have obtained desired results-With and Without SA equation results are quite identical. In case of Deforming Grid they are not identical.

If I don't call SA solver or in Inviscid cases Rigid Motion and Deforming results are identical.

Hence I have concluded there might be some problem occurring when SA equation is called.I have checked in the numerics_direct_turbulent.cpp and solver_direct_turbulent.cpp but both the cases have been treated equally.
My .cfg file is attached and mesh file used is same as SU2 test case .su2 file
mesh_NACA64A010_turb.su2.

Thanks,
Rahul

[hlk]

Sorry, I didn't realize from your initial question that this problem was only occurring with SA, and that in other situations it works as you expected.

I'm a little bit surprised that with and without turbulence you get identical results (with rigid motion) - I think that the inclusion of turbulence should change at least some part of the solution, especially on a pitching/plunging airfoil that, if I recall correctly, would be expected to produce some separated flow.

I'm not sure what's happening there, but a couple of follow up questions may help narrow it down:
- Have you tried other turbulence models, and how are the results? This could narrow down whether it is a problem of just the SA model or turbulence in general.
- When you output the deformed mesh, did it look reasonable at the most extremely deformed point?
- How many orders of magnitude is the residual reduced? I note that your config file uses a residual reduction of only 4, and minimum residual of -8. Have you tried moving these limits/checking which limit is stopping the solution? The convergence behavior may change depending on whether or not turbulence is included.
- Is the low reynolds number case also transonic? Do you see similar behavior on a subsonic case?
- What is the y+ value of the mesh? (Checking if the boundary layer is resolved) This should be output in the surface solution file. Note that most of the meshes in the test cases are coarser than would be used normally in order to reduce the time of regression testing and the size of the repositories.

If these suggestions don't reveal something that leads to either matching solutions, or another explanation for the problem, I would suggest reporting this as a bug under the 'issues' tab on github. When doing so, I recommend mentioning the details included in your most recent post, and including plots illustrating the discrepancies you describe as well as your convergence history.