NACA0012 airfoil at high angle of attack field inversion

[uttamcadambi07]

Hi,

I am trying to use field inversion for NACA0012 airfoil at 16 degree angle of attack

I got a working mesh, use the SA model (wall resolved completely) and with empty boundary condition for front and back faces, I manage to get convergence.

But when I switch to symmetry boundary condition, I do not get convergence despite trying all settings i.e. changing the discretizatio nschemes, the solution methods and the boundary conditions.

presumably, by setting the symmetry boundary condition, we are telling OpenFOAM that the problem is 3D when in reality, in my case it is only 2D. And at a high angle of attack such as 16 degrees, the flow separation and physics are 3D in nature which becomes hard to solve with just one cell in the z direction.

Is there no way around the empty boundary condition? What is the reason anyway for not having it?

The only solution that I can think of at the moment is to provide a few cells in the z direction and make it 3D. Perhaps then there would be sufficient domain in the z direction to account for the 3D nature of setting the symmetry boundary condition.

Would you happen to have any other suggestions that I can try?

[friedenhe]

Can you share the case? I am curious why the DASimpleFoam did not work with the sym BC. We do not support empty because it will give seg fault. We don't have time to dig into this....

[uttamcadambi07]

Sure. Here it is: airfoil_naca0012_16deg.zip
I have implemented my own turbulence model in SpalartAllmarasFieldInversion (it is the same SpalartAllmaras turbulence model from native OF but implemented the same way SpalartAllmarasFv3FieldInversion in DAFoam has been implemented). This is done because Fv3 version resulted in baseline design failing.

[friedenhe]

I can reproduce your issue. I suggest: 1. Update your mesh. Please try to use pyHyp to generate high-quality airfoil meshes. Your mesh has a very large non-ortho near the wall, which is bad for y+1 meshes. 2. Please try to use the upwind scheme to converge the flow, and then use it as the initial condition to run the linearUpwind scheme.

[lnhang0618]

I alse found the same question in S809 .When the frontAndback set to empty,it is really easy to converge.But when I switch to symmtery boundary,the residual in Uz is really high(more the 1e-3), and the pressure residual will not converge.
S809_predict_xiaoh.zip

[lnhang0618]

@friedenhe I'm not sure why changing the boundary condition from empty to symmetry would cause such changes, but adjusting the fvSolution doesn't make it converge. When it converges to a certain extent, there will be significant oscillations.

[uttamcadambi07]

I am going to check my case to see what I did. I’ll keep you posted.

[friedenhe]

@lnhang0618, have you tried to converge the simulation with a lower angle of attack and then use it as the initial condition to start a high angle of attack simulation? I managed to use this trick to converge other high angle of attack cases.

[uttamcadambi07]

Relaxation factor of 0.3 is very low for velocity. It is not good practice to have it so low, the results will be unreliable in this case. But thanks for the update

[lnhang0618]

I believe that the non-physical fluctuations in the Uz direction are the reason for the lack of convergence. I tried reducing the relaxation factor for U to control the magnitude of this part, but perhaps reducing the tolerance for U could achieve a similar effect?

[uttamcadambi07]

Ah i see what the issue is now. Yes you have to set Uz tolerance to be high, Typically, although the tolerance in the Z direction is high and you have a high magnitude of Uz, continuity equation will still be enforced since continuity equation requires you to satisfy dw/dz. So long as that is satisfied, you need not worry about the absolute value of the out of plane component of velocity. In DAFoam if i remember correctly, it checks for the tolerance of Ux and p and then proceeds to the next optimization step.

[lnhang0618]

It sounds like you recommend setting the tolerance in the z-direction very large? I understand that either an empty-like approach should be used to eliminate the z-direction velocity, or the z-direction velocity should not be updated (such as setting a very large tolerance limit). But I'm not sure if v1812 supports setting tolerance for a specific direction.

[uttamcadambi07]

It does! Just set Uz 0.01 or something like that and Ux 1e-5 and Uy 1e-5