CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

ChannelOodles initial conditions

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree3Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   April 12, 2007, 16:17
Default 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: 8
nzy102 is on a distinguished road
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, k-epsilon 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
nzy102 is offline   Reply With Quote

Old   April 23, 2007, 10:56
Default Hi Ning I think the initial
  #2
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
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
marhamat is offline   Reply With Quote

Old   April 23, 2007, 19:56
Default Hi Marhamat: Somehow I coul
  #3
Member
 
Ning Yang
Join Date: Mar 2009
Location: University Park, PA, USA
Posts: 85
Rep Power: 8
nzy102 is on a distinguished road
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
nzy102 is offline   Reply With Quote

Old   April 24, 2007, 04:45
Default Hi Ning It seems that some
  #4
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
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
marhamat is offline   Reply With Quote

Old   April 24, 2007, 10:09
Default HI Marhamat: I am just curi
  #5
Member
 
Ning Yang
Join Date: Mar 2009
Location: University Park, PA, USA
Posts: 85
Rep Power: 8
nzy102 is on a distinguished road
HI Marhamat:

I am just curious if you got converged results, even though the results have no turbulence structure.

Ning
nzy102 is offline   Reply With Quote

Old   April 27, 2007, 17:40
Default Hi Ning Sorry for this late a
  #6
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
Hi Ning
Sorry for this late answer )-:
What is your criterion for convergence?

Regards
Marhamat
marhamat is offline   Reply With Quote

Old   April 27, 2007, 17:48
Default Hi, Ning and Marhamat I am
  #7
rex
New Member
 
lijian sun
Join Date: Mar 2009
Posts: 7
Rep Power: 8
rex is on a distinguished road
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.
rex is offline   Reply With Quote

Old   April 27, 2007, 18:12
Default Marhamat: I used the same c
  #8
Member
 
Ning Yang
Join Date: Mar 2009
Location: University Park, PA, USA
Posts: 85
Rep Power: 8
nzy102 is on a distinguished road
Marhamat:

I used the same criteria as tutorial channel395. As I said before, all the setups are as the same as tutorial.

Ning
nzy102 is offline   Reply With Quote

Old   April 27, 2007, 18:24
Default Hello Rex: I don't quite un
  #9
Member
 
Ning Yang
Join Date: Mar 2009
Location: University Park, PA, USA
Posts: 85
Rep Power: 8
nzy102 is on a distinguished road
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
nzy102 is offline   Reply With Quote

Old   April 27, 2007, 19:47
Default Ning I am running the same
  #10
rex
New Member
 
lijian sun
Join Date: Mar 2009
Posts: 7
Rep Power: 8
rex is on a distinguished road
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 setting-up 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.
rex is offline   Reply With Quote

Old   April 27, 2007, 21:08
Default Rex: Thank you for your rep
  #11
Member
 
Ning Yang
Join Date: Mar 2009
Location: University Park, PA, USA
Posts: 85
Rep Power: 8
nzy102 is on a distinguished road
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.
nzy102 is offline   Reply With Quote

Old   April 30, 2007, 14:51
Default hi, Ning, for my Fluent simul
  #12
rex
New Member
 
lijian sun
Join Date: Mar 2009
Posts: 7
Rep Power: 8
rex is on a distinguished road
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.
rex is offline   Reply With Quote

Old   April 30, 2007, 15:31
Default hi, everyone: For my OpenFO
  #13
rex
New Member
 
lijian sun
Join Date: Mar 2009
Posts: 7
Rep Power: 8
rex is on a distinguished road
hi, everyone:

For my OpenFOAM simulation, after 10000 time steps(more than 50 flow-through-time), 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.
rex is offline   Reply With Quote

Old   April 30, 2007, 17:14
Default http://www.cfd-online.com/Open
  #14
rex
New Member
 
lijian sun
Join Date: Mar 2009
Posts: 7
Rep Power: 8
rex is on a distinguished road

rex is offline   Reply With Quote

Old   April 30, 2007, 17:15
Default Here is my result: http://w
  #15
rex
New Member
 
lijian sun
Join Date: Mar 2009
Posts: 7
Rep Power: 8
rex is on a distinguished road
Here is my result:



Rex.
rex is offline   Reply With Quote

Old   May 1, 2007, 05:38
Default If there are no tubulent struc
  #16
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
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.
eugene is offline   Reply With Quote

Old   May 1, 2007, 07:10
Default Hello Eugene How we can amp
  #17
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
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
marhamat is offline   Reply With Quote

Old   May 1, 2007, 07:45
Default Hmmm, that depends which versi
  #18
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
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
eugene is offline   Reply With Quote

Old   May 1, 2007, 11:46
Default Thanks, Eugene. I will try tha
  #19
Member
 
Ning Yang
Join Date: Mar 2009
Location: University Park, PA, USA
Posts: 85
Rep Power: 8
nzy102 is on a distinguished road
Thanks, Eugene. I will try that and see how it goes.

Ning
nzy102 is offline   Reply With Quote

Old   May 1, 2007, 11:52
Default Rex: Can you let me know wh
  #20
Member
 
Ning Yang
Join Date: Mar 2009
Location: University Park, PA, USA
Posts: 85
Rep Power: 8
nzy102 is on a distinguished road
Rex:

Can you let me know what is your pressure gradient value after 50 flow-through 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
nzy102 is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 02:39.