ChannelOodles initial conditions

nzy102 · May 1, 2007, 20:20

Hi Eugene:

A quick question: what does "pressure gradient" in log file stand for? Is it the streamwise pressure gradient after each step? If this is the case, it should be negative for channelOodles. For my case, Retau = 180. Channel dimension is pi*1*pi/2. No matter which perturbU code I used, pressure gradient always converged to a certain value between 1 and 2. Did I misunderstood something?

Ning

eugene · May 2, 2007, 06:12

gradp is the magnitude of the externally applied pressure gradient needed to maintain Ubar.

It is applied to the momentum equation as:

== flowDirection*gradp

Check channelOodles.C for details.

Certainly, its sign has no bearing on perturbU, which only sets initial conditions.

rex · May 2, 2007, 20:13

Thanks Euqene for providing the new version of pertubU, I am testing it now!

Ning, I think you get the meaning for gradP now from Euqene. For my case, the pressure gradient is about (1.21e-5), and the normalized value is 1.8. I think it is in the reasonable range.

nzy102 · May 2, 2007, 20:42

Somehow I still can't get pressure gradient right. Anyhow, thank you for letting me know.

Eugene: thank you for your explanation. It is now pretty clear to me.

Ning

marhamat · May 5, 2007, 02:53

Hi Ning and Rex

What is your idea about new version of perurbU?
Did you see turbulance structures in your case after
running?

Best Regards
Marhamat

marhamat · May 8, 2007, 07:20

Hello Eugene
For initialization of LES cases we are testing a new method.
You can see application of this method for turbulent flat plate in http://www.cfd-online.com/OpenFOAM_D...tml?1178524227
what is your idea after a first general view ?
Best Regards
Marhamt

eugene · May 8, 2007, 08:28

Are you seriously trying to run a LES flat plate in 2D?

marhamat · May 8, 2007, 09:02

I'm trying LES flat plate in 2D only for time serving.So i don't sure in 2D simulation of this case.

Thanks alot
Marhamat

marhamat · May 9, 2007, 17:04

Hello Eugene
Can i expect good result from 2D simulation of LES flat plate?
In oodles step flow simulated in 2D.
Best Regards
Marhamat

eugene · May 10, 2007, 05:36

No, 2D LES generally has no meaning and certainly wont work for channel flows. If it is done for a tutorial case, then it is simply a demonstration of model and solver settings.

Unless you have a prominent turbulence production mechanism like a free shear layer or shedding, 2D LES wont produce any resolved motion at all.

marhamat · May 21, 2007, 02:54

Hi Eugene

I tried on 3D LES cases by noted code(Tuesday, May 08, 2007 - 05:20 am) but i didn't see turbulent structures in 3D turbulent flat plate.
I add that in duct flow i got good result by that.
I'm compeletly wondering.
Essentially what is the difference between these cases?
What is your idea?

Best Regards
Marhamat

hadi · July 9, 2007, 03:36

Hi to all,

I am simulating a LES turbulent channelflow using channelOodles, i fixed the value of Ubar and i ran the case for few iterations, i would like to get the values of u_tau in order to estimate the corresponding Re_tau.
Does openFoam print out these values?
u_tau=(nu*(du_x/dy+du_z/dy))^0.5

Thanks in advance
hadi

hadi · July 17, 2007, 04:10

Hello,

Can u please answer my question posted above?
I also tried to extract wallShearStress but i got the following message error : "keyword turbulenceModel is undefined in dictionary".
Can anyone tell me how to get a converged value of U_tau?

Cheers
Hadi

hadi · August 9, 2007, 04:45

Hi to all,
I ran a LES channel flow simulation using channelOodles , and after 40 flows through time the mean fields are not symmetric.
Could u please tell me what might be wrong in my simulation?
dimensions 3.2x1x1.2
mesh:64x64x64
Ubar=1
Re_tau=180
y+=1

Uinitial

Umean

R

hjasak · August 9, 2007, 04:59

Nothing wrong here, as far as I can tell: either do averaging across homogenous planes (in z-direction?) or keep running.

Hrv

hadi · August 9, 2007, 05:19

Thank you so much for your reply!

I will keep running the simulation.
Over how many flows through time should i run the simulation, to get the right mean fields?
(i checked the velocity profile is good, rms of u, v and w did not converge yet)

cheers
Hadi

eugene · August 9, 2007, 07:45

We recently had to run such a case and it took around 200 flow-through times to converge the mean profiles. Normally a figure of around 100 is quoted in literature.

Making the duct longer can reduce the overall cost a bit since you have less artificial periodicity.

hadi · August 10, 2007, 04:01

Thank you Eugene for your reply, hopefully i will get good results at the end.

Actually i am new to LES and openFOAM, but i found that it is important to calculate u_tau, when u fix U_bar, me i calculate u_tau=(nu*(du_x/dy+du_z/dy))^0.5 by modifying wallGradU utility without doing time average, but i dont know if it is the right way to do it.(does openFoam calculate this value?)
My concern is when u simulate a new case that does not exist in literature, do you run the simulation to get a converged value of u_tau, and then u change the mesh with the adequate y+?
(Sorry if my question seems a bit stupid or unclear)
Thanks in advance
Cheers
Hadi

eugene · August 10, 2007, 05:46

You should not use u_tau=(nu*(du_x/dy+du_z/dy))^0.5 to calculate utau since this will only be accurate if your y+ < ~2. channelOodles provides you with a driving pressure gradient. Since wall shear is the only force balancing this gradient it is simple to compute utau from the pressure gradient. Thus if you want a fixed utau, it is better to prescribe a fixed pressure gradient than to adjust Ubar for instance.

hadi · August 10, 2007, 06:09

Thank you eugene for your answer, actually in my case y+=1.
I know that i can calculate utau using :
U_tau=[(gradp/rho)*2delta]^0.5
But i thought it is only valid for DNS.
Is it the right way to do it?

Cheers
Hadi

May 1, 2007, 20:20	Hi Eugene: A quick question	#21
nzy102 Member Ning Yang Join Date: Mar 2009 Location: University Park, PA, USA Posts: 84 Rep Power: 17	Hi Eugene: A quick question: what does "pressure gradient" in log file stand for? Is it the streamwise pressure gradient after each step? If this is the case, it should be negative for channelOodles. For my case, Retau = 180. Channel dimension is pi1pi/2. No matter which perturbU code I used, pressure gradient always converged to a certain value between 1 and 2. Did I misunderstood something? Ning

May 2, 2007, 06:12	gradp is the magnitude of the	#22
eugene Senior Member Eugene de Villiers Join Date: Mar 2009 Posts: 725 Rep Power: 21	gradp is the magnitude of the externally applied pressure gradient needed to maintain Ubar. It is applied to the momentum equation as: == flowDirection*gradp Check channelOodles.C for details. Certainly, its sign has no bearing on perturbU, which only sets initial conditions.

May 2, 2007, 20:13	Thanks Euqene for providing th	#23
rex New Member lijian sun Join Date: Mar 2009 Posts: 7 Rep Power: 17	Thanks Euqene for providing the new version of pertubU, I am testing it now! Ning, I think you get the meaning for gradP now from Euqene. For my case, the pressure gradient is about (1.21e-5), and the normalized value is 1.8. I think it is in the reasonable range.

May 2, 2007, 20:42	Somehow I still can't get pres	#24
nzy102 Member Ning Yang Join Date: Mar 2009 Location: University Park, PA, USA Posts: 84 Rep Power: 17	Somehow I still can't get pressure gradient right. Anyhow, thank you for letting me know. Eugene: thank you for your explanation. It is now pretty clear to me. Ning

May 5, 2007, 02:53	Hi Ning and Rex What is yo	#25
marhamat Senior Member Marhamat Zeinali Join Date: Mar 2009 Location: Tehran, Tehran, iran Posts: 107 Rep Power: 17	Hi Ning and Rex What is your idea about new version of perurbU? Did you see turbulance structures in your case after running? Best Regards Marhamat

May 8, 2007, 07:20	Hello Eugene For initializati	#26
marhamat Senior Member Marhamat Zeinali Join Date: Mar 2009 Location: Tehran, Tehran, iran Posts: 107 Rep Power: 17	Hello Eugene For initialization of LES cases we are testing a new method. You can see application of this method for turbulent flat plate in http://www.cfd-online.com/OpenFOAM_D...tml?1178524227 what is your idea after a first general view ? Best Regards Marhamt

May 8, 2007, 08:28	Are you seriously trying to ru	#27
eugene Senior Member Eugene de Villiers Join Date: Mar 2009 Posts: 725 Rep Power: 21	Are you seriously trying to run a LES flat plate in 2D? atmcfd likes this.

May 8, 2007, 09:02	I'm trying LES flat plate in 2	#28
marhamat Senior Member Marhamat Zeinali Join Date: Mar 2009 Location: Tehran, Tehran, iran Posts: 107 Rep Power: 17	I'm trying LES flat plate in 2D only for time serving.So i don't sure in 2D simulation of this case. Thanks alot Marhamat

May 9, 2007, 17:04	Hello Eugene Can i expect goo	#29
marhamat Senior Member Marhamat Zeinali Join Date: Mar 2009 Location: Tehran, Tehran, iran Posts: 107 Rep Power: 17	Hello Eugene Can i expect good result from 2D simulation of LES flat plate? In oodles step flow simulated in 2D. Best Regards Marhamat

May 10, 2007, 05:36	No, 2D LES generally has no me	#30
eugene Senior Member Eugene de Villiers Join Date: Mar 2009 Posts: 725 Rep Power: 21	No, 2D LES generally has no meaning and certainly wont work for channel flows. If it is done for a tutorial case, then it is simply a demonstration of model and solver settings. Unless you have a prominent turbulence production mechanism like a free shear layer or shedding, 2D LES wont produce any resolved motion at all.

May 21, 2007, 02:54	Hi Eugene I tried on 3D LES	#31
marhamat Senior Member Marhamat Zeinali Join Date: Mar 2009 Location: Tehran, Tehran, iran Posts: 107 Rep Power: 17	Hi Eugene I tried on 3D LES cases by noted code(Tuesday, May 08, 2007 - 05:20 am) but i didn't see turbulent structures in 3D turbulent flat plate. I add that in duct flow i got good result by that. I'm compeletly wondering. Essentially what is the difference between these cases? What is your idea? Best Regards Marhamat

July 9, 2007, 03:36	Hi to all, I am simulating	#32
hadi Member hadi tartoussi Join Date: Mar 2009 Location: paris Posts: 48 Rep Power: 17	Hi to all, I am simulating a LES turbulent channelflow using channelOodles, i fixed the value of Ubar and i ran the case for few iterations, i would like to get the values of u_tau in order to estimate the corresponding Re_tau. Does openFoam print out these values? u_tau=(nu*(du_x/dy+du_z/dy))^0.5 Thanks in advance hadi

July 17, 2007, 04:10	Hello, Can u please answer	#33
hadi Member hadi tartoussi Join Date: Mar 2009 Location: paris Posts: 48 Rep Power: 17	Hello, Can u please answer my question posted above? I also tried to extract wallShearStress but i got the following message error : "keyword turbulenceModel is undefined in dictionary". Can anyone tell me how to get a converged value of U_tau? Cheers Hadi

August 9, 2007, 04:45	Hi to all, I ran a LES channe	#34
hadi Member hadi tartoussi Join Date: Mar 2009 Location: paris Posts: 48 Rep Power: 17	Hi to all, I ran a LES channel flow simulation using channelOodles , and after 40 flows through time the mean fields are not symmetric. Could u please tell me what might be wrong in my simulation? dimensions 3.2x1x1.2 mesh:64x64x64 Ubar=1 Re_tau=180 y+=1 Uinitial Umean R

August 9, 2007, 04:59	Nothing wrong here, as far as	#35
hjasak Senior Member Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,905 Rep Power: 33	Nothing wrong here, as far as I can tell: either do averaging across homogenous planes (in z-direction?) or keep running. Hrv __________________ Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk

August 9, 2007, 05:19	Thank you so much for your rep	#36
hadi Member hadi tartoussi Join Date: Mar 2009 Location: paris Posts: 48 Rep Power: 17	Thank you so much for your reply! I will keep running the simulation. Over how many flows through time should i run the simulation, to get the right mean fields? (i checked the velocity profile is good, rms of u, v and w did not converge yet) cheers Hadi

August 9, 2007, 07:45	We recently had to run such a	#37
eugene Senior Member Eugene de Villiers Join Date: Mar 2009 Posts: 725 Rep Power: 21	We recently had to run such a case and it took around 200 flow-through times to converge the mean profiles. Normally a figure of around 100 is quoted in literature. Making the duct longer can reduce the overall cost a bit since you have less artificial periodicity.

August 10, 2007, 04:01	Thank you Eugene for your repl	#38
hadi Member hadi tartoussi Join Date: Mar 2009 Location: paris Posts: 48 Rep Power: 17	Thank you Eugene for your reply, hopefully i will get good results at the end. Actually i am new to LES and openFOAM, but i found that it is important to calculate u_tau, when u fix U_bar, me i calculate u_tau=(nu*(du_x/dy+du_z/dy))^0.5 by modifying wallGradU utility without doing time average, but i dont know if it is the right way to do it.(does openFoam calculate this value?) My concern is when u simulate a new case that does not exist in literature, do you run the simulation to get a converged value of u_tau, and then u change the mesh with the adequate y+? (Sorry if my question seems a bit stupid or unclear) Thanks in advance Cheers Hadi

August 10, 2007, 05:46	*You should not use u_tau=(nu(**	#39
eugene Senior Member Eugene de Villiers Join Date: Mar 2009 Posts: 725 Rep Power: 21	You should not use u_tau=(nu*(du_x/dy+du_z/dy))^0.5 to calculate utau since this will only be accurate if your y+ < ~2. channelOodles provides you with a driving pressure gradient. Since wall shear is the only force balancing this gradient it is simple to compute utau from the pressure gradient. Thus if you want a fixed utau, it is better to prescribe a fixed pressure gradient than to adjust Ubar for instance.

August 10, 2007, 06:09	Thank you eugene for your answ	#40
hadi Member hadi tartoussi Join Date: Mar 2009 Location: paris Posts: 48 Rep Power: 17	Thank you eugene for your answer, actually in my case y+=1. I know that i can calculate utau using : U_tau=[(gradp/rho)*2delta]^0.5 But i thought it is only valid for DNS. Is it the right way to do it? Cheers Hadi

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 17:14
Initial conditions	Allan	CFX	5	April 23, 2002 08:54
Initial conditions in CFX 5.5	Astrid	CFX	3	December 18, 2001 23:24