Dear Friends,

I am trying to incorporate S-A turbulence model into an existing NS solver. I am faced with the problem of code blowing up on very strectched meshes, typical of turbulent flows. In this context, I plan to go for wall functions, so as to obtain accurate solutions at expense of less stretched grid(or correspondingly a higher y+). Could anyone point out some references that explain S-A model with wall functions in detail ?

Thanks in advance

Regards,

Ganesh

Are you getting negative turbulent viscosity ? Is that what is causing blow-up ?

Dear Praveen,

Yes, I have problems with negative turbuelnt viscosity, which leads to code blow up. I have improved the convergence a bit using a limit on the lower bound of turbulent viscosity, but from the solution point of view doesnot seem to be helping much.

Any comments/suggestions are most welcome

Regards,

Ganesh

I've implemented the S-A model too.

here are some suggestions based on my experience.

If the eddy viscosity is negative in the wake--> it is normal for S-A model. the problem can be overcame reducing the stretching

Another way, which is not so clean, is to perform something like DES using for the parameter d (distance) a mix between the wall-distance and the cell dimension

If the eddy viscosity is negative in the wall region --> you have a problem..

In this last case try to inizialize the eddy viscosity with a value different from zero but low.

If the problem is still present it can be due to the fact that the flow is laminar in this place and this can be overcame using the tripping function of the turbulent model.

Good luck

I have found that if you use an explicit scheme, then the destruction term causes the eddy viscosity to become negative. Try switching off the destruction term to see if this is the case with you. I treat the destruction term in a semi-implicit way: ν² in the destruction term is replaced with ν⁽ⁿ⁾ ν⁽ⁿ⁺¹⁾. Note that without the destruction term, SA model satisfies a maximum principle; so negative values should not arise if you have a proper descretization.

Also, it is recommended to use only a first order upwind scheme for the SA model. Together with a Galerkin discretization of the elliptic terms, you should get a stable scheme.

Dear Mar and Praveen,

I do make use of a first order upwind for SA model. The source terms are linearised, and the destruction terms are treated implcitly. I make use of a diamond path reconstruction procedure for the viscous fluxes. On finer grids, I still end up with a negative viscosity in the vicinity of the leading edge. I am not using the trip term of the model. Could neglecting the trip term lead to such a catastrophic failure of the code as Mar pointed out ?

Thanks for your comments

Regards,

Ganesh

In stationary cases I succeed to a stable solution even if for small Reynolds number involving separation bubbles (Re=50000) but in instationary simulations involving relaminarization of the flow-field i have many problems in the leading edge region.

If you are performing stationary cases I suggest to properly inizialize the turbulent variables. It MUST works.

[cfdman_aero]

Dear friends,

I have also problem with the SA model where the destruction term increases abruptly. I checked the code ans saw that it is because of the negative eddy viscosity nu. I applied it in backward facing and external flows. I neglect the transient terms ft1 and ft2. If the problem is with transient condition please let me know about the trip point and how we should set that term.

Thanks