[vaina74]

Hi everybody,

I always used OpenFOAM-1.6 and 1.7 so far, but I just started to work with OpenFOAM-1.5-dev because I have to set up a propeller case. I wonder how k-omega SST turbulence model is implemented, I'm afraid it's different from OpenFOAM-1.7 one. I took a look at the fora, but I can't get a univocal answer. I think the implementation has often changed and developed through years. Which is the actual 'state of the art'?
I use the MRFSimpleFoam, I mean to apply a high Re model, I have no resources to resolve the b.l.. Are wall functions automatically included? In other words, have I to set just zeroGradient for omega and k as boundary condition? Another trivial question: are only p, U, k, omega and not nut need in 0 folder? I hope someone can answer to me.

[tcarrigan]

Hi,

If you look, you'll notice that OF-1.5-dev includes both a high and low Re k-omega SST model (kOmegaSST and kOmegaSST-LowRe).

From my testing it seems that the kOmegaSST model will actually work for wall functions and boundary layer resolved flows.

Wall functions are not automatically included. If you would like to use wall functions, omega should be set to type 'omegaWallFunction', and k should be 'kqRwallFunction'.

For the kOmegaSST model: p, U, k, omega need to be in the 0 directory. nut isn't required, however, if you'd like to record nut for postprocessing you will need to put it in the 0 directory. Also, if you use nut, type should be set to 'nutWallFunction'.

Hope this helps.

[vaina74]

Thanks for your reply.
So, as in OpenFOAM-1.7, I must set on the wall patches e.g.:

k
{
    type            kqRWallFunction;
    value           uniform 0.1;
}
omega
{
    type            omegaWallFunction;
    value           uniform 100;
}
p
{
    type            zeroGradient;
}
U
{
    type            fixddValue;
    value           uniform (0 0 0);
}

If I want to resolve the b.l. I have to set:

[COLOR]k[/COLOR]
{
    type        zeroGradient;
}
omega
{
    type        zeroGradient;
}
p
{
    type        zeroGradient;
}
U
{
    type         fixddValue;
    value        uniform (0 0 0);
}

Anyway, is the turbulent model called kOmegaSST in both cases? I mean into the RASProperties file.

[Chris Lucas]

Hi,

if you need the ggi interface from openFoam 1.5 dev and have worked with openFoam 1.6 (1.7) before, you should use the "new" dev version OpenFoam 1.6-ext .

In this case, the sst model is the same or at least you can use the sst model from openFoam 1.7

Regards,
Christian

[vaina74]

Hi, Chris.

I know OpenFOAM 1.6-ext, but I use OF at work and cannot choose the release. I need ggi interfaces, so I must use OF-1.5-dev. Anyway, I'd like to be sure about boundary settings close to the wall surfaces. I can't get a univocal information. I read somewhere I have to set k and omega as zeroGradient, if I apply a high Re k-omega SST turbulence model, but someone else, as tcarrigan, doesn't agree.

[vaina74]

Maybe I solved my doubt. I look at the kOmegaSST.C file in both OpenFOAM releases. Unlike in OF-1.7, in OF-1.5-dev I read

#   include "kOmegaWallViscosityI.H"
#   include "kOmegaWallFunctionsI.H"

So I think I must set k and omega as zeroGradient on wall patches, with high-Re k-w SST model.
Please, if you're expert about this, confirm or correct.

[tcarrigan]

If you want to resolve the boundary layer, then U and p should be set to 'zeroGradient'. However, k and omega should be set as follows:

k
---------
type fixedValue;
value uniform 0;

omega
-----------
type omegaWallFunction;
value uniform (some value);


This is because turbulent kinetic energy is zero on the wall, so it should be specified as such. However, omega is usually large and must be specified. You can use 'omegaWallFunction' as I have indicated above and it will calculate omega on the wall, or you can simple use the equation below and set type to 'fixedValue' with the value you get from the equation. I believe 'omegaWallFunction' uses this equation.

omega_wall = 10 * 6 * nu / ( 0.075 * y^2 )

[vaina74]

I think we're all a little confused
I think you're right, if you are talking about OpenFOAM-1.7 (anyway U is 0 and not zeroGradient on the wall). Indeed at low-RE (in order to solve the b.l.) I must set

k
{
    type            fixedValue;
    value           1e-11; // non-zero value
}
omega
{
    type            omegaWallFunction;
    value           uniform 100; // some value
}

Anyway, I refer to OpenFOAM-1.5-dev and high-Re. I read a lot of posts and there are no univocal answers, but I guess I must set k and omega as zeroGradient. In OpenFOAM-1.5-dev there is a specific low-Re k-omega SST model (kOmegaSST_LowRe)

[alberto]

Hi, I think you are correct. OF 1.5 did not have the new wall-function implementation, so your setup (zeroGradient) should work.

Best,

[Anne Lincke]

Dear Foamers,

I am currently computing kOmegaSST with OF 1.7.0 on a lowRe mesh.
Is there an alternative for omegaWallFunction as boundary condition?
I always get bounding omega and omega increases to values approx. e+07
When I was computing with zeroGradient for Omega at the wall, I did not observe those problems.

So would it be ok to set on the wall

Omega zeroGradient
k fixedValue e-11

?

In this thread you were talking about OF1.5-dev and you stated that zeroGradient is a working boundary condition for Omega. So I was wondering if this could work for OF1.7.0, too.

Looking forward to reading your answers!

Anne

[alex_rubel]

Hi Foamers,
I get the same question than Anne but for High Re model and OpenFoam 1.6
After several try I still have issues to solve the b.l for my low Y+ model (KomegaSST).
I'm still wondering how to set nut, k, omega at the wall ?
Thanks
Alex

[mehrdad_kbg]

Based on the concepts of the low Reynolds and high Reynolds number flows, if some one is using low Reynolds number option of the SST kw it means that the flow has different layers and a very fine resolution of the mesh is required close to the wall. this needs a mesh with a y-plus less than at least 5. Therefore in this case no wall function can be used.
For High Reynolds number flows, it is possible to apply the wall functions in the simulation.
So, if I want to summarize, for low Reynolds cases do use fine mesh with no wall function and in high Reynolds cases you have both two option but be careful about the y plus!!

[Dadou]

Hi,

If I use high Reynolds what's the condition on my y-plus ?

Thank you

[Filankes]

y + with 30-300 range , if u turn on wallfunction high re

[cleoo]

Originally Posted by Filankes

y + with 30-300 range , if u turn on wallfunction high re

what if you have low y+ value and high RE can you still use the wall function?

[Anne Lincke]

You should not use a wall function then. Set the turbulent properties k, omega (and epsilon) to appropriate boundary conditions in this case.
As far as I know, the omegaWallFunction can be used for both, highRe and lowRe. k has to be set to a small, non-zero value. nut to calculated, meaning that it is computed from the ratio of k and omega.

[cleoo]

Hi Anne, thanks for replying, I will try that, also do you know what to set alphat then?

[Anne Lincke]

Assuming that alphat corresponds to kappat in the earlier OpenFoam-versions, it should be set to "calculated" as well, meaning that it is computed from nut and Prt.

[cleoo]

Originally Posted by Anne Lincke

Assuming that alphat corresponds to kappat in the earlier OpenFoam-versions, it should be set to "calculated" as well, meaning that it is computed from nut and Prt.

should it be set to calculated even at the wall? do you mean for all boundary feilds? if it set to calculated where does it get the Prt number from as we specify it?

also do you know by any chance where the implemetation of how these values are calculated are in the code for the kOmegaSST model?

[Anne Lincke]

Yes, calculated at the wall and I also set it to calculated at the other boundaries.
The Prt number is specified in constant/transportProperties.
I would have a look at the file omegaWallFunctionFvPatchScalarField.C , in my old version it is saved in this folder

vi ~/OpenFOAM/OpenFOAM-2.1.1/src/turbulenceModels/incompressible/RAS/derivedFvPatchFields/wallFunctions/omegaWallFunctions/omegaWallFunction/omegaWallFunctionFvPatchScalarField.C

Some properties (for example kappat) are computed directly in the solver so you may have a look at the corresponding file.