
[Sponsors] 
July 29, 2008, 12:06 
Hi OpenFOAM, in particular LES

#1 
Senior Member
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 187
Rep Power: 10 
Hi OpenFOAM, in particular LES players,
I want to start a new thread about LES channel flow. There is already one but in OpenFOAMBugs and here there are no bugs. The problem here is that I can't get "good" results for a channel flow with OpenFOAM. statistics are not so good and the same for the mean flow. configuration : I want to validate OpenFOAM from Moser DNS (Retau = 395). This test case was used prveviously by Eugene in his Ph'D and Henry and Gavin in the conference (LES of turbulent channel flows). OpenFOAM "has been" validated in LES with this litterature. the size of my channel is 2Pi*2*Pi with 96*196*69 node (which is huge). I'm using the one transport equation for the turbulent kinetic energy (like Eugene's calculation) and it's refered to the B1 models in the paper from Gavin and Henry. Here are the plots, the mean flow in normal scale then in log scale and then rms values: You can see from the second picture the mesh which is correct (y+ = 0.11) and I've more than 10 nodes in the viscous area. So in normal scale, I thing I've the same as the paper (for statistic also) but, in log scale there is a "big" difference when we compared to the DNS calculation. The rms value are also not realy efficient. Are these differences due to second order scheme ? Are these differences due to SGS model ? (I didn't find in the litterature validations for this model in channel flow) In Gavin and Henry's paper, dynamic models do not improve the results. So my question are:  Can I have better results in LES with OpenFOAM ?  Someone has results for a such case? Thank you for giving your point of view about these calculations. Cedric 

July 29, 2008, 17:11 
Not sure about the symbols in

#2 
New Member
Luca Liberti
Join Date: Mar 2009
Location: Rome, Italy
Posts: 22
Rep Power: 10 
Not sure about the symbols in your plots Uf_0, Uf_2 etc.
If you calculate the Reynolds stresses from the resolved field you are missing the sgs part so my guess would be that you are not going to match DNS values even if everything works fine. Could you give more details on the B1 model? Luca 

July 29, 2008, 18:02 
Hi Cedric,
The difference b

#3 
Senior Member
kumar
Join Date: Mar 2009
Posts: 112
Rep Power: 10 
Hi Cedric,
The difference between the DNS and OpenFOAM result is "big" in the near wall region or the region where the viscosity plays an important role. (y+ < 10). I also got similar results in this region. But in the region where it matters (y+ 100  1000), your results are very good. your slope is (1/0.41) and your constant appears to be very close to what you would get from the DNS calculation. I see that you have indeed used a large number of cells , 1.3 million. how many cells have Moser et.al used ? for example kim et al used 3.2 million cells in their 1987 smooth wall computation for a Re_tau of 180! . so i think your result is different in the laminar region because it is still unresolved. what is the time that you take for one flow time in your openfoam LES calculation. ( if flow time is [half of depth of channel/u_tau ] )? I also did the smooth wall case with my LES solver. if you want i can post it. Thanks Kumar 

July 30, 2008, 03:07 
Thank you for your answers,

#4 
Senior Member
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 187
Rep Power: 10 
Thank you for your answers,
@Luca : the only difference between Uf_0 and Uf_2 is the mesh repartition normal to the wall. one is linear and the other is a tanh. But, because in the plots only Uf_2 is symboled (by cross) you won't see the mesh. And in fact, as you can see, the results is the same. then, you have the classic log law and the linear law close to the wall. These last 2 law are the "asymptotic solution" in visous and inertial layer. for B1 model, I can write you here all the theory but, I think it's better for you to find the reference LES paper in OpenFOAM. For exemple, "Large Eddy Simulation of Turbulent Channel Flows" from C. Fureby, A.D. Grosman, G. Tabor, H.G.Weller . You can find it for free from google. Eugene Ph'D is also very well written and explained the SGS models very clearly. Then you can have a look about Tabor (Gavin) and Fureby who did lot's of work on LES model (in particular OF's LES model). About your comments, I calculated Re stresses from the resolved field but, the SGS model play as a viscosity in this field (and in the NS equations) so I'm suppose to see it there. don't I ? @Kumar: I can't find Moser's paper now but, you are right, he probably used more cells but .... he did a DNS :). And I wall normal direction, plots show us (from y+) that ... it's resolved at the wall, doesn't it ? Then, conference paper (where the results are "better") obtained good results if delta x+ = 35 delta z+ = 20 delta y+ between (2,20) without any wall model ... In my case, utau = 0.0079 yes, I'll be gratefull if you can post here or send by mail your LES results with some description. Thanks for giving idea, I'll keep looking for .... something :o) Cedric 

July 30, 2008, 04:18 
Cedric,
I see now you are und

#5 
New Member
Luca Liberti
Join Date: Mar 2009
Location: Rome, Italy
Posts: 22
Rep Power: 10 
Cedric,
I see now you are underpredicting U mean in the viscous and transition layer and on the other hand overpredicting Urms. If you calculate the Urms on a resolved LES field it should be less than the corresponding DNS value since you are missing the small scale motions whose dissipation is taken into account by the SGS model. However this is not your case since you are actually overpredicting Urms. I'll try to look at the paper to get more info on the SGS model. One thing you can try is to run a different geometry and compare to more data. I would try the Lid Driven cavity flow. Best 

July 30, 2008, 04:52 
I assume all your configuratio

#6 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 14 
I assume all your configuration settings are identical to those in the channel395 channelOodles tutorial case?


July 30, 2008, 05:17 
Hi Eugene,
euh ....not real

#7 
Senior Member
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 187
Rep Power: 10 
Hi Eugene,
euh ....not really :o) As I told, the geometry and the grid are different. it's the same geometry as the DNS calculation. So streaks are shorter than the box and there is (should be) no effect from the outlet on the inlet. the time discretisation is CrankNicholson. (I think it's backward in the tutorial). For the numerical scheme I using only central diffential scheme (to keep second order accurate). so there is no limitedLinear 1 for these terms (div(phi,k), div(phi,B)) Then, the time step is different to keep Co number less than 0.4. For the solver, I'm using ICCG to solve the pressure (and the same PISO as the tutorial) and BICCG for the other quantities, which is quite different from the tutorial also. Can these settings bring me some over diffusive terms, because, it should not, contrary to the tutorial (convective scheme view). Thank you for giving advise,... I hope it's not a stupid question. But, because the results are not so "bad" (but also not so good :o) ), I think it's just a small things. Cedric 

July 30, 2008, 05:30 
The settings you reported are

#8 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 14 
The settings you reported are ok.
What are your turbulenceProperties settings? 

July 30, 2008, 05:55 
@Luca: I don't agree with you,

#9 
Senior Member
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 187
Rep Power: 10 
@Luca: I don't agree with you, I think for both Umean and rms I underpredicted the value. In the rms, I overpredicted the pic of rms and, the maximum is shift to bigger y+ .... which is not good also.
@Eugene: Here are the turbulentProperties: I'm now running a dynOneEqEddy channel flow to check if the result is really not better if we compare to a nondynamic procedure ( like the paper ). But the plot I put was from a oneEqEddy model. I didn't change the constant value in the properties and I'm using the cubeRootVol for delta. Thanks for your interrest. Cedric 

July 30, 2008, 06:23 
Try vanDriest for delta with o

#10 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 14 
Try vanDriest for delta with oneEqEddy. Check the channel395 tutorial turbulenceProperties.


July 30, 2008, 07:02 
Hi
I did LES of Turbulent Ch

#11 
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 10 
Hi
I did LES of Turbulent Channel Flow using with OpenFOAM.Unlike my imagination the result for rms component isn't good.I attached the file that containes my results and computational details.What's your idea about it? With Kind Regards Marhamat 

July 30, 2008, 07:57 
@Eugene Thank you for you com

#12 
Senior Member
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 187
Rep Power: 10 
@Eugene Thank you for you comment, I'll try that.
I thought about that point before and that is the reason why I'm doing a calculation with the dynamic procedure. I'm not supposed to need Van Driest damping function for this run so I'll try both and compare the calculation. I'll upload my resluts after because I'm sure I'm not the only one who tryed such calculation in LES. Cedric. 

July 30, 2008, 08:42 
Hi
I did LES of Turbulent Ch

#13 
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 10 
Hi
I did LES of Turbulent Channel Flow using with OpenFOAM.Unlike my imagination the result for rms component isn't good.I attached the file that containes my results and computational details.What's your idea about it? Fully developed turbulent channel flow11_Page_1.tif Fully developed turbulent channel flow1_Page_2.rar With Kind Regards Marhamat 

July 30, 2008, 09:07 
Sorry alot
The attached file

#14 
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 10 
Sorry alot
The attached file was very big ): 

July 30, 2008, 11:37 
Cedric, your experiments and c

#15 
Member
Philippe B. Vincent
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 32
Rep Power: 10 
Cedric, your experiments and concerns are of great interest so please keep us posted with your results. I haven't look at the test case "LES of turbulent channel flows" yet, but I'm running DES in the ERCOFTAC conical diffuser and I saw that you presented on the subject in Milan. Unfortunatly I wasn't there.
We could start another thread on the subject of LES in the diffuser, but for now I have some general questions I hope you can help me with. I guess you use the solver channelOodles for the LES of turbulent channel flow, but do you use oodles or channelOodles for the diffuser? What fundamental difference there is between the two? I see, in your presentation, that you perturbed the Poiseuille flow for turbulent inlet boundary conditions, but how do you initialize the diffuser? Do you start from a perturbed RANS solution? While I'm at it, do add initial perturbation to your LES of turbulent channel flow to initiate the turbulence cycle? Well, that would be it for today. I hope you can take the time to answer. As I said before, we could start a thread on LES in the ERCOFTAC diffuser. I have some results that suggest separation and recirculation and I will be very interested in your time averaged solutions. Best regards and merci! Philippe 

August 2, 2008, 02:28 
Hi FOAMers
I require to obtio

#16 
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 10 
Hi FOAMers
I require to obtion a solution for fully developed turbulent channel flow with inlet B.C!. I want to study the effect of adding a particular source term to N.S equation,in one section of domain.(with periodic B.C the source term effect on inlet flow.). Can i ask your idea? Can i get good result If i use the obtioned result, in one section of a channel with periodic B.C as a inlet condition for a long channel(L2/L1=10) with inlet B.C? @ Eugene and Cedric : What's your idea about my obtioned result in Turbulent Channel Flow? Best Regards Marhamat 

August 29, 2008, 03:39 
Hi LES FOAMers
Sorry for th

#17 
Senior Member
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 187
Rep Power: 10 
Hi LES FOAMers
Sorry for the delay but, the august month is very quiet and vacation was there ..... well, I came back :) I'm running 3 jobs now with the same mesh :  static oneEqEddy  static oneEqEddy + Van Driest  dynamic oneEqEddy and .... it working better for the mean flow (picture below) (thank you Eugene) here is a premilinary conclusion, with the help of a paper (JCP 2008 Desjardin et al. "High order conservative finite difference scheme for 3 variable density low Mach number turbulent flows") "with a second order accurate code, we can't get the same mean flow in log scale as a DNS. Plot should be below (like the previous plot)" I think it answers also to Marhamat previous message. In the article they plot result in a periodic pipe mean velocity in log scale from second and higher order scheme. The question now is what is the minimum error we can get. And I feel my runs can be better .... let's check. Any comments ? regards, Cedric PS: Hi Philippe, nice to meet you. please feel free to open a new thread on this topic or to send me a mail about your work. I'll be happy to discuss with you as much as I can. 

December 1, 2008, 13:17 
Good morning everyone,
I ha

#18 
Member
Philippe B. Vincent
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 32
Rep Power: 10 
Good morning everyone,
I have a technical question about the turbulent channel flow : How exactly do you get the drinving pressure gradient to calculate utau? Thank you Philippe 

December 1, 2008, 14:45 
Hi Philippe,
the pressure g

#19 
Senior Member
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 187
Rep Power: 10 
Hi Philippe,
the pressure gradient is calculated eatch time step from these lines (in channelOodles.C): // Extract the velocity in the flow direction dimensionedScalar magUbarStar = (flowDirection & U)().weightedAverage(mesh.V()); // Calculate the pressure gradient increment needed to // adjust the average flowrate to the correct value dimensionedScalar gradPplus = (magUbar  magUbarStar)/rUA.weightedAverage(mesh.V()); first, you get the volume average of the streamwise velocity sum(mesh.V()*Ustreamwise)/sum(mesh.V()) then, you calculate a "streamwise body force" by the difference of magUbar (you imposed in transportProperties files) and the average you just calculated. In OpenFOAM, you don't calculate both utau and mass flow rate but, the mean velocity "Ubulk" you imposed. I hope it helps, Cedric 

December 2, 2008, 12:09 
Hi Cedric,
thank you for yo

#20 
Member
Philippe B. Vincent
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 32
Rep Power: 10 
Hi Cedric,
thank you for your answer. I get the idea for the adjustment of gradP at each timestep in channelOodle. So correct me if I'm wrong, but to plot U+ vs y+, you use the final pressure gradient in the channel to get Tau_w and then U_tau? Philippe 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Pressure inlet boundary conditions for open channel flows  jack2000  OpenFOAM Running, Solving & CFD  4  October 6, 2016 08:51 
LES In Turbulent in channel flow  pankaj saha  Main CFD Forum  18  November 20, 2014 06:49 
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 