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/)
-   -   Perturbation dissapears after many iterations. (http://www.cfd-online.com/Forums/openfoam-solving/65223-perturbation-dissapears-after-many-iterations.html)

Bedotto June 9, 2009 05:34

Perturbation dissapears after many iterations.
 
Hi OpenFoamers

I've a problem with the pre-processing utility perturbU. I study a turbulent couette flow in a channel with the solver Oodles and I've implmented the energy equation in this solver.

Before launching the calculation I apply perturbU on my initial velocity field. I've checked with paraFoam that it pertubs the velocity field. My problem is that after many iterations, the velocity field is laminar and there's no perturbations in my flow. I've searched in previous threads and I've checked if that was due to my time step (its value is 0.01) but I don't think that's the origin of the problem.

The dimensions' box are (64,2,12) (x,y,z), the Reynolds number is 8600 and Re_tau=1280. (and Ubar=0.5, it's required for perturbU but not for the solver Oodles).

Is the amplitude of my perturbation is too weak and it dissapears after a certain number of iterations? In this case what I should modify? I think Re_tau is high enough...

I hope you will have some hints.

My regards.

Quentin

eugene June 10, 2009 05:24

perturbU is only for use with channelOodles. If you are running oodles it means you have a fixed value inlet which will eventually flush all the perturbations from the system. To maintain perturbations in a ducted system, you either need to recycle turbulence via a mapped inlet or channelOodles, or you need some kind of vortex generator.

Bedotto June 11, 2009 04:39

Indeed I use Oodles but I've imposed periodic conditions on the inlet and on the outlet of the channel. I don't use U_bulk (here its value is zero). In order to make move my stream I've imposed the velocity field (1 0 0) on the TopWall and thus the stream moves by viscosity.
So in these conditions I think perturbU is relevant here. What's your opinion about this point?


P.S: I've tried to use a 'trick' in order to avoid this problem:
*I just launch a perturbU and solve my problem in the case of a simple channel (I mean that the Topwall doesn't move) .

* Then when I am in a fully develloped turbulent flow, I stop the iterations. Next I impose the velocity field (1 0 0) on the Topwall and resume the calcul.
* After many iterations my turbulent flow becomes laminar.... It seems that's my moving TopWall is the origin of the problem.

In these conditions is there an other way to simulate a turbulent couette flow?

My regards
Quentin.

eugene June 11, 2009 06:30

In that case, please post the contents of your fvSchemes dictionary. Perhaps one of your schemes is too diffusive to maintain smooth wall generated turbulence.

Bedotto June 11, 2009 08:50

Here is the fvSchemes file I'm using:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
default backward;
}

gradSchemes
{
default Gauss linear;
grad(p) Gauss linear;
grad(U) Gauss linear;
}

divSchemes
{
default none;
div(phi,U) Gauss linear;
div(phi,k) Gauss limitedLinear 1;
div(phi,B) Gauss limitedLinear 1;
div(B) Gauss linear;
div(phi,nuTilda) Gauss limitedLinear 1;
div((nuEff*dev(grad(U).T()))) Gauss linear;
div(phi,T) Gauss linear;
}

laplacianSchemes
{
default none;
laplacian(nuEff,U) Gauss linear corrected;
laplacian((1|A(U)),p) Gauss linear corrected;
laplacian(DkEff,k) Gauss linear corrected;
laplacian(DBEff,B) Gauss linear corrected;
laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
laplacian(DT,T) Gauss linear corrected;
}

interpolationSchemes
{
default linear;
interpolate(U) linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}


// ************************************************** *********************** //

eugene June 11, 2009 09:14

Well there is nothing overly diffusive that I can see. Have you tried different SGS models?

Bedotto June 16, 2009 04:43

In my case I use the Smagorinsky model. Do you think there is a more adapted SGS for a turbulent couette flow?

eugene June 16, 2009 05:35

The Smagorinsky model should be fine provided you are using vanDriest damping for the length scale. If you do not use the damping function, your near-wall length scale and thus SGS dissipation will be too high.

Bedotto June 16, 2009 09:45

I've checked in turbulentProperties file and I use the VanDriest damping function.

The trick I talked about in my previous post (June 11, 2009 10:39) seem to work. Indeed I''ve awaited for a longer time before imposing my velocity field (1 0 0) on the TopWall and my Couette flow seems being turbulent now but I have to make more iterations before confirming that works really.

I'm going to post soon some pictures to show you.

Bedotto June 17, 2009 04:56

2 Attachment(s)
X corresponds to the direction of the flow Y coresponds to the altitude and Z corresponds to the width of the channel.

On these two pictures I'v plotted the velocity field. On the first one we can see that the velocity field is being perturbed (finally!) but on the other side of the channel (pic2) there's still no perturbations. I think (and I hope) this part of the channel will be perturbed after many iterations.

However I would like to know why it doesn't work without this trick? (Did I make a mistake?)
If anyone has an idea concerning this point, go ahead.

Quentin.


All times are GMT -4. The time now is 13:29.