[airwarriorg91]

Hello Everyone !
I am new to SU2 for CFD simulations. I trying RANS simulation for NACA 64(1)-412 airfoil at Re=20000. I have conducted DNS simulation using NEK5000 for the same case and obtained satisfactory results.

The domain is 30c x 12c with airfoil centered at (10c,0). It has velocity inlet with (1,0,0) and pressure outlet (P=0). The top and bottom wall are periodic whereas the airfoil is wall is no-slip and adiabatic wall. The case is non-dimensionalized such that the Re=20000. The mesh is such that y^+<1.

I used the numerical settings from the turbulent NACA 0012 tutorial case.

The problem is flow converges and looks correct. But the lift coefficient is very off from the expected value whereas the drag coefficient is closer to the actual value.

+------------+------------+------------+
| Case | CD | CL |
+------------+------------+------------+
| Experiment | 0.036663 | -0.03036 |
| DNS | 0.03518 | -0.03245 |
| RANS | 0.03253 | 0.13866 |
+------------+------------+-------------+

I have attached the config file and mesh file for your reference. I am getting similar results using both SA and SST models. Can anyone help me in this ?

Thanks,
Gaurav

Files Link: https://drive.google.com/file/d/1D_V...ew?usp=sharing

[bigfootedrockmidget]

First thing that comes to mind is that the values used to nondimensionalize CL do not correspond, but then CD would probably also not be correct.

Then there is the issue of the mesh quality. If you look here:

https://turbmodels.larc.nasa.gov/naca0012_val.html

The meshes used for the final CL/CD curve are quite fine, also the far-field boundaries are quite far away. I would also change the periodic boundaries to far-field boundaries.
I had a quick look at your mesh and it is better to use a completely structured mesh like on the nasa website. It is easy to make with gmsh.

[airwarriorg91]

Hey !
Happy New Year !!

Non-dimensionalization is not an issue because I am getting the correct Re output in the SU2 screen output.

I am using a hybrid domain instead of the a structured domain since this is a validation case for the actual simulation (which has a complex geometry), hence structured grid is not possible in that case.

Also, I am trying to use the same mesh type and b.c. from DNS but the RANS mesh is 3x times the DNS mesh. I will try with a larger mesh. Although the current mesh is fine enough with y+<1. Is there some issue with periodic boundary conditions in SU2 (in comparison with farfield) ?

Thanks,
Gaurav

[airwarriorg91]

Hey @bigfoot !
I solved the issue by setting the turbulence_intensity and mach number to the experimental value. I didn't had to set these during DNS so I didn't notice these parameters. Now, I am getting the almost accurate values with the coarse (original) mesh itself.

[bigfootedrockmidget]

Happy new Year!


That's great to hear that results are closer to measurements/DNS.
If you want, we can add your case to the validation test cases on the website. We can then also document that the results are quite sensitive to the turbulent boundary conditions.

[airwarriorg91]

Hey @bigfoot !
Sure, I am okay with the addition of the validation test cases on the website.

Right now, I was working on grid convergence. The initial mesh was coarse (66k elements), the current mesh comparatively fine (180k elements). Absurdly, the CL for fine mesh is converging to -0.08. I tried lower CFL values (25, 10, 7.5) but the no change. Do you know why this could happen ?

I have attached the updated cfg and mesh file along with the history file.

Link: https://drive.google.com/drive/folde...v_?usp=sharing

[bigfootedrockmidget]

The history file shows that the case has not converged yet. The residuals, especially pressure, should converge to -12 at least (the convergence event horizon). It looks like your case is still converging, but much slower (as is often observed for larger meshes and finer cells).


So the first thing to do is to let it converge.


Then: CL is not guaranteed to converge monotonously with increasing mesh size. Some of the cell refinement will not impact your results. It might be that you need an even finer mesh.

And finally: RANS might simply not be super accurate - you could check in the literature on RANS results for this testcase. Although, for a NACA profile at zero angle of attack I expect decent results.

[airwarriorg91]

The case actually stalls at about -7 to -8 depending on the CFL number (See the attached image). For coarser mesh, the case converged to -14 at CFL of 25. Since it is zero AoA, I am also expecting some good results with RANS.

So, what should I do to improve the convergence and in regards to grid convergence ?