[FernandoSoares]

Hi Foamers,

I was attempting to run simpleFoam using Spalart-Allmaras model for incompressible flow over a backward facing step in current OF240. The simulation starts normally, but I get the following warning:

--> FOAM Warning : 
    From function tmp<volScalarField> SpalartAllmaras::k() const
    in file SpalartAllmaras/SpalartAllmaras.C at line 280
    Turbulence kinetic energy not defined for Spalart-Allmaras model. 
    Returning zero field

As far as I knew, SA model variables were actually only nut and nuTilda (am I right?). And for the matter my original directory was mapped from a kOmegaSST solution obtained earlier and I used createTurbulenceFields to generate the remaining fields of interest. So my starting directory actually contains a k file.

I tried to find out why I was getting such a message by taking a look in the code. A similar message would also be displayed for the epsilon field, which does not happen in my simulation.

Has anyone ever had such issue with incompressible SA? Is it really meaningful in terms of solution for the model to get always zero field for k and epsilon? I'm asking this because I'm getting ~steady residuals way above the accuracy desired.

[dappe]

Hi Fernando
I'm having the same issue while simulating an Impinging Jet with a compressible solver. Also in my case I already have k folder because I ran the same case with kOmegaSSt. It is very strange and I d like to know if this affects the results: in fact I have oscillating residuals, the solution does not converge and I m trying to find out which could be the problem.
Let me know if you will solve this problem.
Alessandro

[ndev]

In my experience, a "Foam Warning" can be taken as an informational, but not significant, message about your simulation...though there could be some exceptions. In this case it is true that the SA equations cannot return a turbulent kinetic energy field...but having k in your zero directory shouldn't do anything. Alessandro, this in no way should produce oscillating results, or affect the solution in any way, so you can definitely start looking elsewhere for issues!

[dappe]

Thank you ndev!

[aerogt3]

Does anyone know where this could come from? I am getting the error despite not having k in any of the timesteps (or constant) folders in any of my processor folders. I have scoured controlDict and the function objects (like fieldaverage, etc.) looking for k but cannot find anything.

Really curious where this message comes from and eager to get rid of it!

[ndev]

You want to be looking for things that will call the k() method in Spalart-Allmaras. What boundary condition are you using on nut? I ask because if you are using "nutkWallFunction" you're calling in the BC:

const tmp<volScalarField> tk = turbModel.k();

If so, you may want to switch to "nutUSpaldingWallFunction" or "nutUWallFunction" as these really only use the velocity gradients and viscosity.

[aerogt3]

Originally Posted by ndev

You want to be looking for things that will call the k() method in Spalart-Allmaras. What boundary condition are you using on nut? I ask because if you are using "nutkWallFunction" you're calling in the BC:

const tmp<volScalarField> tk = turbModel.k();

If so, you may want to switch to "nutUSpaldingWallFunction" or "nutUWallFunction" as these really only use the velocity gradients and viscosity.

Good catch! That was the issue. I had been looking at my BCs, and all my wall functions were nutUSpalding wall function. BUT, on one zone, which had a roughness, I was using nutkRoughWallFunction. I've switched that out for nutURoughWallFunction. Thanks a lot!

[Leslie Lee]

Originally Posted by ndev

You want to be looking for things that will call the k() method in Spalart-Allmaras. What boundary condition are you using on nut? I ask because if you are using "nutkWallFunction" you're calling in the BC:

const tmp<volScalarField> tk = turbModel.k();

If so, you may want to switch to "nutUSpaldingWallFunction" or "nutUWallFunction" as these really only use the velocity gradients and viscosity.

Hi foamers,

I have the same issues while simulating an Impinging Jet with BuoyantBoussinesqSimpleFoam. So I try to use "nutUSpaldingWallFunction" and "nutUWallFunction", as you suggested. But, it didn't work out. Please let me know if you have other solutions to fix this. Thanks~

Lee