[Combas]

I am doing some validation cases in Euler and Navier-Stokes with the naca0012 airfoil.

The Navier-Stokes solver seems to give good results compared to the ones provided by NASA (http://turbmodels.larc.nasa.gov/naca0012_val_sa.html)

In my opinion, at low Mach number, the Euler solver should give zero drag (in 2D). Unfortunately, it is not what I get with the naca0012 airfoil. For example, at zero angle of attack, I get Cd = 0.0004 (even if it is not huge, it is not negligible). When I zoom on the flow around the airfoil, there is a loss of speed near the airfoil, and so a loss of total pressure, which could explain the drag I get.
My question is: is it a problem of numerical scheme, or a problem of mesh (it is the same mesh as the one used for Navier-Stokes, so with very thin cells near the boundary), or a problem in the Euler solver?

I put the some files in attachment to illustrate what I said.

Thank you for your answers
Laurent

[hlk]

Yes, for a 2-D body in inviscid flow there should be zero drag (d'Alembert's paradox).
The small finite drag is likely due to numerical dissipation, which is the same mechanism that enforces the Kutta condition here. Most if not all CFD codes have this effect to some extent. Mesh refinement can reduce the magnitude, as would reduced numerical error within the scheme.

[Combas]

Thank you for your answer, but what seems strange to me is that with the same mesh and the same scheme but in Navier-Stokes, results are much better (I get exactly the drag given by NASA on http://turbmodels.larc.nasa.gov/naca0012_val_sa.html so a numerical error on Cd below 0.0001)

And the loss of velocity near the wall should not happen: it looks like a boundary layer with a very low friction coefficient... That is why I am wondering if the Euler solver does not have a problem...

Laurent

[fpalacios]

Originally Posted by Combas

Thank you for your answer, but what seems strange to me is that with the same mesh and the same scheme but in Navier-Stokes, results are much better (I get exactly the drag given by NASA on http://turbmodels.larc.nasa.gov/naca0012_val_sa.html so a numerical error on Cd below 0.0001)

And the loss of velocity near the wall should not happen: it looks like a boundary layer with a very low friction coefficient... That is why I am wondering if the Euler solver does not have a problem...

Laurent

Hi,

My answer is related with Heather's reply. The key is the artificial dissipation introduced by the numerical scheme.

Navier-Stokes grids have been created to simulate problems with boundary layers, in other words they have an a-priori grid adaptation that has beneficial effect when you run a Navier-Stokes problems. But these grids are a very bad choice when you try to run an Euler problem (completely different behavior on the wall: hyperbolic vs. elliptic).

So… with high-stretching grids, the convective scheme is not adding the optimal dissipation (in the normal direction the wall) and you detect that strange effect. Obviously, if you solve a NS problem, the viscous effects are dominant close to the wall and the solution is correct.

Conclusion, the a-priori adaptation should be done based on the equation that you are solving. Otherwise it will deteriorate the convergence and the solution quality because you are adapting some features that are not present in your continuous model.

Thanks for using SU2,

Best,
Francisco

[Combas]

Thank you very much for this answer that solves my problem. So I am going to try better meshes for Euler cases.

Thank you for your great work!
Best regards,
Laurent