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

LES of turbulent channel flows

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

Like Tree9Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   June 16, 2009, 03:37
Default
  #61
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,610
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
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
ngj is online now   Reply With Quote

Old   June 16, 2009, 03:48
Default
  #62
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to lakeat
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
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   June 26, 2009, 05:34
Cool
  #63
New Member
 
Gabriela Bracho
Join Date: Mar 2009
Location: Valencia, Valencia, Spain
Posts: 14
Rep Power: 8
gaby is on a distinguished road
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
gaby is offline   Reply With Quote

Old   June 26, 2009, 05:50
Default
  #64
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to lakeat
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
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   June 26, 2009, 06:43
Default
  #65
Member
 
Leonardo Giampani Morita
Join Date: Apr 2009
Location: Paris, France
Posts: 58
Rep Power: 8
leonardo.morita is on a distinguished road
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.
leonardo.morita is offline   Reply With Quote

Old   July 6, 2009, 11:19
Default
  #66
New Member
 
Gabriela Bracho
Join Date: Mar 2009
Location: Valencia, Valencia, Spain
Posts: 14
Rep Power: 8
gaby is on a distinguished road
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
gaby is offline   Reply With Quote

Old   July 6, 2009, 22:00
Default
  #67
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to lakeat
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
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   July 7, 2009, 04:46
Default
  #68
New Member
 
Gabriela Bracho
Join Date: Mar 2009
Location: Valencia, Valencia, Spain
Posts: 14
Rep Power: 8
gaby is on a distinguished road
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
gaby is offline   Reply With Quote

Old   July 23, 2009, 19:35
Default
  #69
Senior Member
 
Sandy Lee
Join Date: Mar 2009
Posts: 207
Rep Power: 9
sandy is on a distinguished road
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?
sandy is offline   Reply With Quote

Old   July 23, 2009, 21:35
Default
  #70
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to lakeat
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 test-case as starting point to taste it. For example, the turbulent channel flow.

Best,
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   July 24, 2009, 00:41
Default
  #71
Senior Member
 
Sandy Lee
Join Date: Mar 2009
Posts: 207
Rep Power: 9
sandy is on a distinguished road
Hi Daniel,

I am reading your past post (LES ), 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 2e-05; //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.
sandy is offline   Reply With Quote

Old   July 24, 2009, 00:49
Default
  #72
Senior Member
 
Sandy Lee
Join Date: Mar 2009
Posts: 207
Rep Power: 9
sandy is on a distinguished road
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?
sandy is offline   Reply With Quote

Old   July 24, 2009, 03:00
Default
  #73
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to lakeat
Quote:
Originally Posted by sandy View Post
You think, what is the Eugene's viewpoint: ' Unless your walls are well resolved, you should put nuSgsWallFunction on the nuSgs BCs for walls.' ?
Sorry, I don't quite understand your question.

Quote:
Originally Posted by sandy View Post
In addition, what is the defination of the boundary condition 'InletOutlet' ? When should we choose it as BC?
Are you refering to Channel Flow case?

Anyway, you can read these two posts:
  1. Questions about the inletOutlet and outletInlet boundary conditions
  2. Inletoutlet

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,
  1. Initial condition is different from boundary condition, I suggest the following link for a first view: Turbulence free-stream boundary conditions . Initial condition is transient. Eg., in my case, a small value is ok.
  2. Wall b.c., is a hard issue, it depends on your first grid height, (zero or zeroGradient).
  3. Inlet b.c. gives the information about inlet turbulence condition, some cases are very sensitive to the inlet b.c., others are not, so the inlet condition is different from one another. Sensitive in channel flow, diffuser, etc., but insensitive in most wind tunnel cases, ie. a small value is ok.
  4. If you are doing a case sensitive to the inlet b.c., please refer to some papers on that, it's a hot topic.
  5. Outflow, many wind tunnel cases set the out boundary in a distance far away, for example in a cylinder case, 6D or 10D or 15D, it depends on your interest, but the basic idea is by comparison to choose a sound distance to remove the undesired numerical influence. and then, zeroGradient (or zero for p) can be applied in most cases.

I'm not sure this helps...

Regards,
solefire likes this.
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog

Last edited by lakeat; July 24, 2009 at 04:56.
lakeat is offline   Reply With Quote

Old   July 24, 2009, 12:02
Default
  #74
Senior Member
 
Sandy Lee
Join Date: Mar 2009
Posts: 207
Rep Power: 9
sandy is on a distinguished road
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?

sandy is offline   Reply With Quote

Old   November 19, 2009, 05:18
Default Use of Crank Nicholson Scheme
  #75
And
New Member
 
Andrea Aprovitola
Join Date: Nov 2009
Posts: 16
Rep Power: 7
And is on a distinguished road
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 P-43 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
solefire likes this.
And is offline   Reply With Quote

Old   January 11, 2010, 06:20
Red face
  #76
Member
 
Join Date: Sep 2009
Posts: 45
Rep Power: 7
AirS is on a distinguished road
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,
AirS is offline   Reply With Quote

Old   January 12, 2010, 09:55
Default
  #77
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to lakeat
Easy, you just need to choose VanDriest

Regards,
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   January 12, 2010, 10:17
Default
  #78
Member
 
Join Date: Sep 2009
Posts: 45
Rep Power: 7
AirS is on a distinguished road
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!
AirS is offline   Reply With Quote

Old   January 12, 2010, 10:31
Default
  #79
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to lakeat
  1. Yes
  2. By ajusting Ck you can change Cs, I suggest you read some papers to get an idea about their detailed relationship.

Regards,
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   December 14, 2012, 13:15
Default Boundary conditions on a turbulent channel flow LES
  #80
New Member
 
Join Date: Mar 2012
Posts: 3
Rep Power: 5
operita is on a distinguished road
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
operita 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
LES In Turbulent in channel flow pankaj saha Main CFD Forum 18 November 20, 2014 06:49
Pressure inlet boundary conditions for open channel flows jack2000 OpenFOAM Running, Solving & CFD 3 October 21, 2012 14:10
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


All times are GMT -4. The time now is 08:37.