
[Sponsors] 
June 9, 2009, 05:34 
Perturbation dissapears after many iterations.

#1 
New Member
Quentin
Join Date: May 2009
Posts: 22
Rep Power: 10 
Hi OpenFoamers
I've a problem with the preprocessing 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 

June 10, 2009, 05:24 

#2 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 14 
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.


June 11, 2009, 04:39 

#3 
New Member
Quentin
Join Date: May 2009
Posts: 22
Rep Power: 10 
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. 

June 11, 2009, 06:30 

#4 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 14 
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.


June 11, 2009, 08:50 

#5 
New Member
Quentin
Join Date: May 2009
Posts: 22
Rep Power: 10 
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((1A(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; } // ************************************************** *********************** // 

June 11, 2009, 09:14 

#6 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 14 
Well there is nothing overly diffusive that I can see. Have you tried different SGS models?


June 16, 2009, 04:43 

#7 
New Member
Quentin
Join Date: May 2009
Posts: 22
Rep Power: 10 
In my case I use the Smagorinsky model. Do you think there is a more adapted SGS for a turbulent couette flow?


June 16, 2009, 05:35 

#8 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 14 
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 nearwall length scale and thus SGS dissipation will be too high.


June 16, 2009, 09:45 

#9 
New Member
Quentin
Join Date: May 2009
Posts: 22
Rep Power: 10 
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. 

June 17, 2009, 04:56 

#10 
New Member
Quentin
Join Date: May 2009
Posts: 22
Rep Power: 10 
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. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Moving mesh  Niklas Wikstrom (Wikstrom)  OpenFOAM Running, Solving & CFD  122  June 15, 2014 06:20 
How to write k and epsilon before the abnormal end  xiuying  OpenFOAM Running, Solving & CFD  8  August 27, 2013 15:33 
Low Mach number Compressible jet flow using LES  ankgupta8um  OpenFOAM Running, Solving & CFD  7  January 15, 2011 14:38 
Differences between serial and parallel runs  carsten  OpenFOAM Bugs  11  September 12, 2008 11:16 
Unknown error  sivakumar  OpenFOAM PreProcessing  9  September 9, 2008 12:53 