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/)
-   -   BCbs for high Renumbers (http://www.cfd-online.com/Forums/openfoam-solving/60228-bcbs-high-renumbers.html)

gjesing April 20, 2005 05:04

Hi all, Which b.c. should b
 
Hi all,

Which b.c. should be used at a wall with a flow with high Re-number?

I searched the forum and think the answer for my question is zeroGradient for both k and epsilon, is that right?

But, when is it then best to use the wall-functions?

Thanks,
Rasmus

henry April 20, 2005 05:55

You should use zeroGradient fo
 
You should use zeroGradient for k and epsilon at walls when using wall-functions.

It is best to use wall-functions when there is no choice, i.e. when you cannot afford the resolution required for running a low-Re model.

gjesing April 20, 2005 06:05

Ok, but for HIGH-Re flows, sho
 
Ok, but for HIGH-Re flows, should both k and epsilon have zeroGradient b.c.?

And are wall-functions valid for HIGH-Re flows?

/Rasmus

henry April 20, 2005 06:09

You should use zeroGradient fo
 
You should use zeroGradient for k and epsilon at walls when using wall-functions.

Yes wall-functions are valid for high-Re flows.

mattos May 22, 2005 21:31

Hi All I have looked for tr
 
Hi All

I have looked for trough this board message about boundary conditions for High Re flows. I have a doubt: I'm trying to use the sonicTurbFoam solver to calculate an external flow (3d NACA profile). I read that the tutorial NACA case use a low-Re turb. Model, thus is adequate to define no-slip condition for U componentes. Otherwive, the prism tutorial test case uses High-Re turbulence model and the boundary conditions for U is also no-slip.

Now I have a question: Should be more correct, in the High-Re cases, that the boundary conditions for U componentes imposed as slip conditions? In that case, is the OpenFoam correctly implemented to define K and epsilon as function of wall stress provides by the wall function?

At glance, what I must to do to define correctly the boundary conditionf for high-Re turb/models with wall functions? Which conditions must I impose for all variables?


Many Tanks in advance

Wladimyr Dourado

henry May 23, 2005 03:39

Why do you think the BC for U
 
Why do you think the BC for U should be slip when using wall-functions? The OpenFOAM implementtation of wall-functions requires the U BC to be no-slip with zero-gradient on p, k and epsilon.

mattos May 23, 2005 09:54

Hi Weller In my investigati
 
Hi Weller

In my investigation in the literature, the wall laws requires the folowing setups:
1) The velocities componentes, Ui, are imposed in such way that is a slip boundary condition with zero flux trough the wall or imposed, for transpirant wall type.
2) The effective stress tensor (or friction velocity) is given by the wall function, by the distance of the boundary elements upto the wall and the velocity magnitude found at 1). The distance can be defined either by the user or by the code using standart y+ limits. This value is found often by an interactive procedure such as Newton-Rapson. This found effective stress is imposed in the boundary patch (nodes and or faces).
3) The equilibrium condition and the friction velocity are used to calculate the k and epsilon values.
I have implemented this procedure in my codes and I find right valus for U, K and epsilon.

The imposition of no-slip BC for U I guest that it provoques a condition completely wrong BC for k and epsilon once that this value of U is over the wall and then k and epsilon is also zero (if I'm not wrong). The problem lies the fact that High-Re turbulence models are unable to treat the viscous and buffer layers. Thus, is necessary a wall function to impose valid values outside these first two regions such that the turbulence model begin to be valid.

Am I wrong to thing that is necessary a slip condition for U? In the case of OpenFoam, is it imposing U BC with the wall function in such way? If not, why and please let me know as much as possible. In this case, have some reference which can I read about?

Many tanks in advance

Wladimyr Mattos Dourado

henry May 23, 2005 10:51

I do not agree with your asses
 
I do not agree with your assessment of the need for a slip BC for U, in fact I think this is wrong because it's a non-slip wall thus U should have a zero value. No one has found anything wrong with the implementation or results from the wall-functions in OpenFOAM and they have been extensively tested over very many years.

If you are unhappy with the current implementation and would prefer one based on a slip condition for U please feel free to implement it, you have complete source access to do so.

mattos May 23, 2005 11:32

Hi Weller May be I don't un
 
Hi Weller

May be I don't understand well how wall function is implemented in OpenFoam. I agree with you completely about the no-slip condition at wall where the velocity must be zero. I think that I have not written clear enought. In the implementations that I know up to now, the condition in the wall is no-slip and the wall function is used to give the value of friction velocity at the first boundary point located over the wall at a given distance such that y+ is greater then a value suitable for the turbulence model. The boundary of the mesh is displaced by this distance from the actual wall.
But seeing your position I have a question: where and how the information coming from wall function is introduced in the flowfield? In opemfoam, Is the first point really over the wall?

I can't be unhappy with current implementation because I not tested it yet. May be I will intoduce in the future the Reichardt wall law but I will necesary to use as base the actual implementation.

Anyway, tank you in advance for your answer

henry May 23, 2005 11:40

Yes the BC for U does coincide
 
Yes the BC for U does coincide with the wall and that is why it is the physical BC of no-slip. I cannot see the point of moving the mesh around to correspond to a particular y+ particularly for unsteady flows where this approach would require the mesh to move every timestep just for the wall-function!

Take a look at the implementation and you will see how it is done in OpenFOAM.

frank May 7, 2006 09:51

when I read David Hill's thesi
 
when I read David Hill's thesis,It was writen that, Eqn. (4.36)
for y+ > 11.6, G=pow(Cmu,3/4)*rho*pow(k,3/2)*y+/yP
and
Eqn. (4.35)
for y+ < 11.6, G=alpha*pow(Cmu,3/4)*rho*pow(k,3/2)*ln(E*y+)/kappa*yP

but for wallFuctions.H in bubbleFoam solver, It was writen

if (yPlus > 11.6)
{
G[faceCelli]+=
nuw[facei}*magFaceGradU[facei]*Cmu25*::sqrt(k[faceCelli]
/(kappa.value()*y[patchi][facei]);
}

Hill's and implementatoin of Foam are inconsistent. why?
would anyone given me some hints?

Best regards
Q.Li


All times are GMT -4. The time now is 02:58.