[aerosjc]

Hi,

I have a question on the turbulence BC.

For example, https://su2code.github.io/tutorials/...lent_NACA0012/ gives a turbulent NACA0012 case. Normally we know that at the farfield the SA model uses Dirichlet BC nu_tilde = 3~5 nu_tilde_freestream. For refenrence, check NASA TMR page.

Using a CFD solver like SU2, we could obtain a converged solution.

The contour of nu_tilde (check the attached figure) shows that at the outflow boundary the calculated turbulence deviates from the pre-specified value (3 nu_tilde_freestream). The pre-specified nu_tilde at the outflow boundary is in the BLUE color while the calculated nu_tilde at the outflow boundary is in the white color.
So my question is: the calculated turbulence at the outflow boundary is different from the pre-specified turbulence, which means that we force a solution at the outflow boundary different from the calculated solution distribution. I think they are incompatible with each other. We force an incompatible BC but the solver still gets converged. Why?

[sbaffini]

Originally Posted by aerosjc

Hi,

I have a question on the turbulence BC.

For example, https://su2code.github.io/tutorials/...lent_NACA0012/ gives a turbulent NACA0012 case. Normally we know that at the farfield the SA model uses Dirichlet BC nu_tilde = 3~5 nu_tilde_freestream. For refenrence, check NASA TMR page.

Using a CFD solver like SU2, we could obtain a converged solution.

The contour of nu_tilde (check the attached figure) shows that at the outflow boundary the calculated turbulence deviates from the pre-specified value (3 nu_tilde_freestream). The pre-specified nu_tilde at the outflow boundary is in the BLUE color while the calculated nu_tilde at the outflow boundary is in the white color.
So my question is: the calculated turbulence at the outflow boundary is different from the pre-specified turbulence, which means that we force a solution at the outflow boundary different from the calculated solution distribution. I think they are incompatible with each other. We force an incompatible BC but the solver still gets converged. Why?

At an outflow, by definition, you get what comes from inside the domain. So it means that you get wake values in the wake and inlet values away from the wake.

It would be a problem if this was happening at an inlet but, in that case, you would indeed experience difficulties in convergence (unless a more complex inlet method is used)

[aerosjc]

After some numerical experiments, I confirm that the outflow boundary location would not affect the convergence only if the outflow boundary is placed 2 chord length away from the airfoil trailing edge. If the outflow boundary is placed at the wake region, the simulation blows up. The simulation is by SU2. This behavior seems reasonable to me. The PDE system adjusts its solution to different BC. For example, a simple equation f''=4 has the analytic solution f = 2 x^2 + a x + b. The coef a and b depend on BC. {f(1)=1, f(-1)=1} results in different solution from {f(1000)=1, f(-1000)=1}. But both allow a converged solution. In the cell-centered finite volume CFD solver, the BC is weakly coupled by a Riemann solver. A Dirichlet BC specifies the value in the ghost cell while the interior value is still calculated by the simulation. The real working value is the Riemann flux calculated based on both the interior value and the BC value.

[FMDenaro]

Originally Posted by aerosjc

After some numerical experiments, I confirm that the outflow boundary location would not affect the convergence only if the outflow boundary is placed 2 chord length away from the airfoil trailing edge. If the outflow boundary is placed at the wake region, the simulation blows up. The simulation is by SU2. This behavior seems reasonable to me. The PDE system adjusts its solution to different BC. For example, a simple equation f''=4 has the analytic solution f = 2 x^2 + a x + b. The coef a and b depend on BC. {f(1)=1, f(-1)=1} results in different solution from {f(1000)=1, f(-1000)=1}. But both allow a converged solution. In the cell-centered finite volume CFD solver, the BC is weakly coupled by a Riemann solver. A Dirichlet BC specifies the value in the ghost cell while the interior value is still calculated by the simulation. The real working value is the Riemann flux calculated based on both the interior value and the BC value.

That depends on the mathematical character of the PDE, you must differentiate the correct BCs for elliptic, parabolic, hyperbolic PDEs

[aerosjc]

Sure. I use the simple example of f''=4 because it takes a lot to discuss NS equation. We could have some feelings about how BCs of NS equation behave but it is hard to strictly give math descriptions of the behaviors.