CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   k-omega SST and wall functions in OpenFOAM-1.5-dev (http://www.cfd-online.com/Forums/openfoam-solving/84266-k-omega-sst-wall-functions-openfoam-1-5-dev.html)

vaina74 January 25, 2011 04:13

k-omega SST and wall functions in OpenFOAM-1.5-dev
 
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 January 25, 2011 22:54

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 January 26, 2011 04:06

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

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:
Code:

[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 January 26, 2011 04:50

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 January 26, 2011 05:09

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 January 26, 2011 09:50

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
Code:

#  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 January 26, 2011 10:48

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 January 26, 2011 11:45

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
Code:

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 January 26, 2011 12:14

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 February 16, 2011 05:30

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 February 24, 2011 19:58

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 February 7, 2012 08:57

SST kw and wall functions
 
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 July 11, 2013 04:29

Hi,

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

Thank you

Filankes February 7, 2014 03:48

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


All times are GMT -4. The time now is 07:32.