
[Sponsors] 
June 16, 2009, 03:37 

#61 
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Copenhagen, Denmark
Posts: 1,898
Rep Power: 36 
Hi Daniel
As far as I can see, then your wallShearStress is actually U_tau, as you apply the "sqrt". Then you take the square root of the wSS (I assume it is the above mentioned wallShearStress), hence you have defined tau = rho U_tau^4 which obviously leads to erroneous results. Best regards, Niels 

June 16, 2009, 03:48 

#62 
Senior Member
Daniel WEI (老魏)
Join Date: Mar 2009
Location: Beijing, China
Posts: 689
Blog Entries: 9
Rep Power: 20 
O, yes, my mistake.
Thank you Niels! Another question, how did you get coefficient Cf? Using sum(wallShearStress) or using file gradP.raw, which is the easist way that you went?
__________________
~ Daniel WEI  Boeing Research & Technology  China Beijing, China 

June 26, 2009, 05:34 

#63 
New Member
Gabriela Bracho
Join Date: Mar 2009
Location: Valencia, Valencia, Spain
Posts: 14
Rep Power: 16 
Hi Daniel!
Do you use the "wallShearStress" utility for calculate U_tau in your LES cases? I've tried to use it in my LES, but that utility it is defined for RASproperties..... Am I missing something? Thanks Gaby 

June 26, 2009, 05:50 

#64 
Senior Member
Daniel WEI (老魏)
Join Date: Mar 2009
Location: Beijing, China
Posts: 689
Blog Entries: 9
Rep Power: 20 
from my post " June 16, 2009, 03:26", you will see how to get wallshearstress;
then I do an average of wallshearstress; then sqrt(wallshearstress);
__________________
~ Daniel WEI  Boeing Research & Technology  China Beijing, China 

June 26, 2009, 06:43 

#65 
Member
Leonardo Giampani Morita
Join Date: Apr 2009
Location: Paris, France
Posts: 58
Rep Power: 16 
Another option, as already suggested by Sebastian, is to get gradP and then:
Tau = (dP/dx)*h utau = (Tau/rho)^(1/2) Retau = utau*h/nu where h is the half channel width. Note that OpenFOAM gives us gradP already divided by rho, so you can just do: utau = (gradP*h)^(1/2) Retau = utau*h/nu Obs: these equations are valid for a flat plate; those presented by Sebastian are valid for a cylindrical tube. 

July 6, 2009, 11:19 

#66 
New Member
Gabriela Bracho
Join Date: Mar 2009
Location: Valencia, Valencia, Spain
Posts: 14
Rep Power: 16 
Hi
Daniel and Leonardo, thanks for your answers. The problem that I'm solving is about a flow with pressure gradient (from high P to low P). So, I have 2 questions: 1) In my case, some times gradP is > 0 , and the eq for calculate utau is: utau = sqrt( D/(4*rho) * gradP ), and numerically this is no possible: sqrt(a), if a<0. Am I doing something wrong? Can I solve with LES this kind of pressure gradient cases? 2) If I want to define the Ubar in transport properties, this is related to the U at the inlet or to the U at the Outlet? Thanks in advance Gaby 

July 6, 2009, 22:00 

#67 
Senior Member
Daniel WEI (老魏)
Join Date: Mar 2009
Location: Beijing, China
Posts: 689
Blog Entries: 9
Rep Power: 20 
Hi Gaby,
Sorry, I am not familiar with your case, so I cannot give much help. But are you sure channelOodles is suitable for your FPG case? I guess equations like "utau = sqrt( D/(4*rho) * gradP )" should be best understood in a averaging sense, so I think my approach, using wall shear stress is more universal. I believe LES (like oodles) is able to achieve your goal, so what's your b.c.? Ubar means U_bulk, but eventually, we need to get a desired Re_tau based on u_tau, this can be only done in LES with fine mesh. Ubar gives the mean value of the initial velocity profile, note inlet and outlet are but periodic conditions. I'm not sure this helped very much. Regards,
__________________
~ Daniel WEI  Boeing Research & Technology  China Beijing, China 

July 7, 2009, 04:46 

#68 
New Member
Gabriela Bracho
Join Date: Mar 2009
Location: Valencia, Valencia, Spain
Posts: 14
Rep Power: 16 
Hi! Thnx for the answer again!
Now, I get the idea about Ubar… And after running the solver during the night I’m getting gradP<0 … In my case I have a channel with high pressure at the inlet and low pressure at the outlet, also the channel has a decreasing diameter (like a nozzle). Now, I think that I should use the oodles solver in spite of the channelOodles, like in the example of the diffuser (in Eungene’s thesis). Do you have any suggestion?? Cheers! Gaby 

July 23, 2009, 19:35 

#69 
Senior Member
Sandy Lee
Join Date: Mar 2009
Posts: 213
Rep Power: 17 
I know nothing about LES method, however, I want to use it as the tubulence model. What is the key I need to pay attention to? How to set the BC about it, for example k file. Could you give some advice?


July 23, 2009, 21:35 

#70 
Senior Member
Daniel WEI (老魏)
Join Date: Mar 2009
Location: Beijing, China
Posts: 689
Blog Entries: 9
Rep Power: 20 
Hi Gaby!
I am not familiar with that case, but I think it's not that hard, you can figure it out, at least you can find reference from his paper. And to Sandy, I think your question is too big to answer, if you are sure LES is really what you want, then pick a small standard testcase as starting point to taste it. For example, the turbulent channel flow. Best,
__________________
~ Daniel WEI  Boeing Research & Technology  China Beijing, China 

July 24, 2009, 00:41 

#71 
Senior Member
Sandy Lee
Join Date: Mar 2009
Posts: 213
Rep Power: 17 
Hi Daniel,
I am reading your past post (http://www.cfdonline.com/Forums/ope...043les7.html ), you gave the boudary conditions about k and nuSgs as follows: <pre>*******************initial k*********************************start internalField uniform 0; boundaryField { cylinder { type fixedValue; //zeroGradient???? value uniform 0; } lateral1 { type symmetryPlane; } lateral2 { type symmetryPlane; } inlet { type fixedValue; value uniform 2e05; //zero or zeroGradient or a small value?? } outlet { type inletOutlet; //zeroGradient or what..?? Why inletOutlet is preferred? inletValue uniform 0; //If inletOutlet, then how to set these 2 value properly? value uniform 0; } slip { type slip; } } *******************initial k***********************************end *******************initial nuSgs*****************************start internalField uniform 0; boundaryField { cylinder { type zeroGradient; } lateral1 { type symmetryPlane; } lateral2 { type symmetryPlane; } inlet { type zeroGradient; } outlet { type zeroGradient; } slip { type slip; } } *******************initial nuSgs*******************************end</pre> Then, finally how did you change them? I also have some difficulties to specify those BCs, and I don't know the relationship between the U and P's boudary condition with the k and nuSgs' BC. Could you talk about them? Thanks. 

July 24, 2009, 00:49 

#72 
Senior Member
Sandy Lee
Join Date: Mar 2009
Posts: 213
Rep Power: 17 
You think, what is the Eugene's viewpoint: ' Unless your walls are well resolved, you should put nuSgsWallFunction on the nuSgs BCs for walls.' ?
In addition, what is the defination of the boundary condition 'InletOutlet' ? When should we choose it as BC? 

July 24, 2009, 03:00 

#73  
Senior Member
Daniel WEI (老魏)
Join Date: Mar 2009
Location: Beijing, China
Posts: 689
Blog Entries: 9
Rep Power: 20 
Quote:
Quote:
Anyway, you can read these two posts:
As for Channel flow, the inlet and outlet b.c. are cyclic. If you are simulating the other cases, I suggest your question should be submitted in another post. But as for now, here are what I think,
I'm not sure this helps... Regards,
__________________
~ Daniel WEI  Boeing Research & Technology  China Beijing, China Last edited by lakeat; July 24, 2009 at 04:56. 

July 24, 2009, 12:02 

#74 
Senior Member
Sandy Lee
Join Date: Mar 2009
Posts: 213
Rep Power: 17 
Hi Daniel,
Your advice is very very useful to me. Thank you a lot. By the way, if I specify the inlet velocity (fixValue), can I use the expression k = (2*ck/ce)*delta^2*D^2 to estimate the inlet k as BC. My LES model is oneEqEddy. Could you understand my question? 

November 19, 2009, 04:18 
Use of Crank Nicholson Scheme

#75 
New Member
Andrea Aprovitola
Join Date: Nov 2009
Posts: 16
Rep Power: 15 
Hi OpenFOAM channel flow community,
I'm working on LES of turbulent channel flow and so I'm deeply interested in your discussions and in particular on the validation on the OpenFOAM results. As I'm concerned in the study of both spatial than temporal discretizations OpenFOAM schemes for LES, my doubt is if selecting the flag CrankNicholson in ddt schemes would mean the correct use of such scheme as in the FOAM ProgrammersGuide P43 it is said that: "The Crank Nicholson scheme can be implemented by the mean of implicit and explicit terms: solve ( fvm::ddt(phi) == kappa*0.5*(fvm::laplacian(phi) + fvc::laplacian(phi)) ) ". If is this so, I'have to rewrite the left hand side of the corresponding UEqn.H exploiting both fvm and fvc operator in order to implement the Crank Nicholson scheme. Otherwise I would not have an effective Crank Nicholson time integration schemes and consequently losing the second order time accuracy. Any hints about that Regards Andrea 

January 11, 2010, 05:20 

#76 
Member
Join Date: Sep 2009
Posts: 45
Rep Power: 16 
Hi Foamers,
My simulation uses the LES Smagorinsky turbulent model. I would like to use cubRootVol for delta and the VanDriest damping function with it. Is that possible? How can I do that? Here is my LESProperties file: LESModel Smagorinsky; delta cubeRootVol; printCoeffs on; ... Thanks for your help, 

January 12, 2010, 09:17 

#78 
Member
Join Date: Sep 2009
Posts: 45
Rep Power: 16 
So the choice of vanDriest for delta permits to use cubeRootVol for delta along with the Van Driest damping function ?
Another question: Do you know where I can change the Cs coefficient ? I read somewhere it is equal to 0.13, but I'd like to change it to 0.1. Thanks! 

January 12, 2010, 09:31 

#79 
Senior Member
Daniel WEI (老魏)
Join Date: Mar 2009
Location: Beijing, China
Posts: 689
Blog Entries: 9
Rep Power: 20 
Regards,
__________________
~ Daniel WEI  Boeing Research & Technology  China Beijing, China 

December 14, 2012, 12:15 
Boundary conditions on a turbulent channel flow LES

#80 
New Member
Join Date: Mar 2012
Posts: 3
Rep Power: 13 
Dear Cedric, I want to run a LES of a turbulent channel flow and would need to figure out how the boundary conditions should be set to correctly represent the periodicity in x and the homogeneous span wise direction. Could you suggest where I can find info specifically about boundary conditions to be set in periodic channel flow? The version I use of OpenFOAM is 2.1.0. Regards


Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Pressure inlet boundary conditions for open channel flows  jack2000  OpenFOAM Running, Solving & CFD  5  December 6, 2018 11:00 
LES In Turbulent in channel flow  pankaj saha  Main CFD Forum  18  November 20, 2014 05:49 
LES In Turbulent in channel flow  pankaj saha  Main CFD Forum  8  April 15, 2009 11:34 
Turbulent channel flow  roberthino  OpenFOAM Running, Solving & CFD  5  August 15, 2007 08:35 
Bc for turbulent channel flow  roberthino  OpenFOAM Running, Solving & CFD  0  August 13, 2007 08:12 