
[Sponsors] 
April 12, 2007, 16:17 
Hi:
I am a new user. I've b

#1 
Member
Ning Yang
Join Date: Mar 2009
Location: University Park, PA, USA
Posts: 85
Rep Power: 10 
Hi:
I am a new user. I've being testing channel les lately. My case is similar to channel395 in channelOodles folder. I used perturbUDict to initialize velocity field. The problem is after several thousands steps, the results are still converging. Is there other way I can accelerate this? In FLUENT, I know to accerate the convergence, kepsilon model can be solved first then the solution for velocity field can be used as initial condition for les. Can I do the same thing in OpenFOAM? I am alos wondering what kind of initial perturbation conditions are applied to channel395? It seems that every variable has an initial field except nuTilda. Thank you. Ning 

April 23, 2007, 10:56 
Hi Ning
I think the initial

#2 
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 10 
Hi Ning
I think the initial condition in channel395 is a result of another solution of this case. It might be DNS or LES of turbulent channel flow. So it has specification of turbulent flow. Did you get right result after convergence? What is your criterion for convergence? How long it take? And what is your reference for validation? Best Regards Marhamat 

April 23, 2007, 19:56 
Hi Marhamat:
Somehow I coul

#3 
Member
Ning Yang
Join Date: Mar 2009
Location: University Park, PA, USA
Posts: 85
Rep Power: 10 
Hi Marhamat:
Somehow I couldn't get converged results. The calcuated pressure gradient is way off from the analytical solution. I am trying to compare my results with kim's dns data and moser's les data. My setup is exactly same as channel395 except that I used different computational domain. The initial condition for u is generated using perturbU. I've be running this case for more than 20 flow through times. Do you have similar experience? Regarding perturbU, do I need to turn on bulk flow? Ning 

April 24, 2007, 04:45 
Hi Ning
It seems that some

#4 
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 10 
Hi Ning
It seems that some Fomers got right result using perturbU.But up to now i didn't get turbulence structure using this code . I am completely wondering for that. Marhamat 

April 24, 2007, 10:09 
HI Marhamat:
I am just curi

#5 
Member
Ning Yang
Join Date: Mar 2009
Location: University Park, PA, USA
Posts: 85
Rep Power: 10 
HI Marhamat:
I am just curious if you got converged results, even though the results have no turbulence structure. Ning 

April 27, 2007, 17:40 
Hi Ning
Sorry for this late a

#6 
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 10 
Hi Ning
Sorry for this late answer ): What is your criterion for convergence? Regards Marhamat 

April 27, 2007, 17:48 
Hi, Ning and Marhamat
I am

#7 
New Member
lijian sun
Join Date: Mar 2009
Posts: 7
Rep Power: 10 
Hi, Ning and Marhamat
I am also working on channelOodles now, to the tutorial case, although it fits well with the log law, but I think that more grid points are needed in the boundary layer: (at least 15 points needed across the boundary layer and with the first grid point at a position of approximately y+=1) So, I refine the mesh, and get initial condition by using perturbU, after 6000 time steps, the results still have no turbulence structure and the mean velocity profile is not right either, more like that for the laminar flow case. I am wondering that whether or not more iteration steps needed to let the turbulent to develop. anyway, the code is still running and I hope that nice result could be made. Rex. 

April 27, 2007, 18:12 
Marhamat:
I used the same c

#8 
Member
Ning Yang
Join Date: Mar 2009
Location: University Park, PA, USA
Posts: 85
Rep Power: 10 
Marhamat:
I used the same criteria as tutorial channel395. As I said before, all the setups are as the same as tutorial. Ning 

April 27, 2007, 18:24 
Hello Rex:
I don't quite un

#9 
Member
Ning Yang
Join Date: Mar 2009
Location: University Park, PA, USA
Posts: 85
Rep Power: 10 
Hello Rex:
I don't quite understand what you posted. Are you saying that in the coarse grid you got good results in log region? Did you see any turbulent structure in the instantaneous flow under the coarse grid? To be honest, I have the similar problem with channeloodles( check my post for details). About iteration number, 20 flow through time should be enough for flow to be fully developed. What is the Reynolds number (Retau) for your case? I am not sure if this is because Reynolds number is too low so that turbulent flow structure are damped out as time advances. My another curiosity is how you specified streamwise and spanwise perturbation spacing in perturbDict. Do you know any source for that? Ning 

April 27, 2007, 19:47 
Ning
I am running the same

#10 
New Member
lijian sun
Join Date: Mar 2009
Posts: 7
Rep Power: 10 
Ning
I am running the same case as the one in the tutorial, only the mesh is refined. yes, I can see the turbulent structure in the instantaneous flow under the original settingup in the tutorial, the turbulent structure wouldn't be damped out even after very long time stpes ( 6000 time steps to me now) To the one with refined grid, all the discretisation and solution schemes are keeped. My concern is: as the resolved grid scale has been changed, do I need to change other parameters as well, like time scale, and also those you mentioned, streamwise and spanwise perturbation spacing in perturbDict. the utility, perturbU, will accelerate the convergence process, and shouldn't affect the final result. by using long enough time steps, same result should be get even without using perturbU. Am I right? At the same time, I am setting up the same case by fluent. Any commons and hints will be highly appreciated! Rex. 

April 27, 2007, 21:08 
Rex:
Thank you for your rep

#11 
Member
Ning Yang
Join Date: Mar 2009
Location: University Park, PA, USA
Posts: 85
Rep Power: 10 
Rex:
Thank you for your reply. I think time scale has to be decreased to keep Courant number less than 1. Since you use the same computational geometry, I don't think you need to adjust perturbation spacing. Can you give me some details of your simulation? How high is Retau? What streamwise and spanwise spacing did you use for your initial run? Here is some information about my case: Retau = 180 domain size: pi*1*(pi/2) (x*y*z) grid: 72*72*72 I also ran the les smagrinsky model in fluent for the same case. The results are about 10% off from Kim's DNS data and Moser's LES data in term of mean and rms. I am interested in seeing how it goes with your fluent running. 

April 30, 2007, 14:51 
hi, Ning,
for my Fluent simul

#12 
New Member
lijian sun
Join Date: Mar 2009
Posts: 7
Rep Power: 10 
hi, Ning,
for my Fluent simulation case: Retau=395 domain size: (2pi,2, pi) grid: (64,65,96) my fluent simualation is still on going. I think you get very close LES result with Fluent. Rex. 

April 30, 2007, 15:31 
hi, everyone:
For my OpenFO

#13 
New Member
lijian sun
Join Date: Mar 2009
Posts: 7
Rep Power: 10 
hi, everyone:
For my OpenFOAM simulation, after 10000 time steps(more than 50 flowthroughtime), still there is no turbulent structure, anyone can tell me what is wrong with it!! My Simulation Case: Everything else are keeped the same as the tutorial case, channel395, except that the mesh is refined, initial value is given by perturbU. Thank you very much! Rex. 

April 30, 2007, 17:14 
http://www.cfdonline.com/Open

#14 
New Member
lijian sun
Join Date: Mar 2009
Posts: 7
Rep Power: 10 


April 30, 2007, 17:15 
Here is my result:
http://w

#15 
New Member
lijian sun
Join Date: Mar 2009
Posts: 7
Rep Power: 10 
Here is my result:
Rex. 

May 1, 2007, 05:38 
If there are no tubulent struc

#16 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 14 
If there are no tubulent structures after a few flowthrough times, you have applied perturbU incorrectly somehow.
Try using mapFields to map the results from the tutorial case to your new case. 

May 1, 2007, 07:10 
Hello Eugene
How we can amp

#17 
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 10 
Hello Eugene
How we can amplify the strength of initial perturbation that made by perturbU package? Which parameters must be change in this code? Best regards Marhamat 

May 1, 2007, 07:45 
Hmmm, that depends which versi

#18 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 14 
Hmmm, that depends which version of perturbU you are using. I have attached the latest one. It requires only that you set Ubar and Retau in the transportProperties dictionary. Obviously, making Retau bigger will increase the perturbation magnitude.
This perturbU should work for all periodic ducts (cylindrical and otherwise) and uses wall distance and Ubar to determine the coordinate system (so the duct can be aligned in any direction). A laminar profile is always used as the starting velcoity field since I found that an initial turbulent profile damps the perturbations very quickly due to the motion of fluid away from the wall. perturbU.tgz 

May 1, 2007, 11:46 
Thanks, Eugene. I will try tha

#19 
Member
Ning Yang
Join Date: Mar 2009
Location: University Park, PA, USA
Posts: 85
Rep Power: 10 
Thanks, Eugene. I will try that and see how it goes.
Ning 

May 1, 2007, 11:52 
Rex:
Can you let me know wh

#20 
Member
Ning Yang
Join Date: Mar 2009
Location: University Park, PA, USA
Posts: 85
Rep Power: 10 
Rex:
Can you let me know what is your pressure gradient value after 50 flowthrough times? Is it close to the value you expect? For my case, when I used the old perturbU code, even after 50 flow through times, my pressure gradient was still positive. Since my Retau is 180, I expect that pressure gradient is around negative 2 (nordimensionalized value by density*utau^2). I am testing the new perturbU code now. Ning 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Burgerbs equation non constant Boundary Conditions Initial Conditions  arkangel  OpenFOAM Running, Solving & CFD  1  October 2, 2008 14:48 
Initial conditions  Shuo  Main CFD Forum  2  July 27, 2007 08:57 
Initial conditions = final conditions  Chucho  CFX  5  December 16, 2005 18:14 
Initial conditions  Allan  CFX  5  April 23, 2002 08:54 
Initial conditions in CFX 5.5  Astrid  CFX  3  December 19, 2001 00:24 