
[Sponsors] 
December 17, 2012, 11:23 

#81 
Senior Member
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 185
Rep Power: 9 
Hi Errico,
have a look on the channelFoam tutorials. That's a good starting point. OpenFOAM2.1.x / tutorials / incompressible / channelFoam / channel395 / Then, this forum page should be interesting too. Cédric 

December 17, 2012, 23:29 

#82 
New Member
j.t.
Join Date: Nov 2012
Posts: 11
Rep Power: 5 
dear cedric,
I read posts in this thread and I facing problems in convergence. It would be nice if you give tips on the fvSchemes and fvSolutions settings for cases involving flow separation like backward facing step, periodic hill etc. I use periodic BCs for inflow/outflow and spanwise boundaries. my fvSchemes and fvSolutions settings are same to channel395 tutorial, and use smagorinsky model,vanDriest damping with default coefficient.but my simulation residual diverge after few hundred iters. time step is sufficiently less. Any idea you can give? As to the schemes which can use for cases having separated flow ? thanking you... 

December 18, 2012, 09:27 

#83 
Senior Member
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 185
Rep Power: 9 
Dear j.t.
I used a quite old version of OF for these calculations. Details of my numerics can be found on a previous message (July 30, 2008, 11:17) I did a periodic hill calculation with the same numerics without any problems. Could you give me more details of your case: What's your configuration? your mesh ? and you initial fields ? Cédric 

December 18, 2012, 22:33 

#84  
New Member
j.t.
Join Date: Nov 2012
Posts: 11
Rep Power: 5 
Quote:
I read ur previous post. I want to simulate periodic hill and backward facing step flow. first, im focus on periodic hill., OF 2.1., channelFoam solver. My mesh is the same as used by Temmerman et. al. in "Highly resolved largeeddy simulation of separated ﬂow in a channel with streamwise periodic constrictions",2004. Its 198 X 128 X 186 cells, and 4.7 million cells total. I'm want to reproduce their results, atleast get reasonable flow field converged solution. I have attached initial fields "0" folder. (in .zip) below is LES properties file.I use Euler backward time stepping.nOrthoCorrector=2. Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.1.1   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "constant"; object LESProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // LESModel Smagorinsky; delta vanDriest; printCoeffs on; SmagorinskyCoeffs { ce 1.05; ck 0.07; } cubeRootVolCoeffs { deltaCoeff 1; } PrandtlCoeffs { delta cubeRootVol; cubeRootVolCoeffs { deltaCoeff 1; } smoothCoeffs { delta cubeRootVol; cubeRootVolCoeffs { deltaCoeff 1; } maxDeltaRatio 1.1; } Cdelta 0.158; } vanDriestCoeffs { delta cubeRootVol; cubeRootVolCoeffs { deltaCoeff 1; } smoothCoeffs { delta cubeRootVol; cubeRootVolCoeffs { deltaCoeff 1; } maxDeltaRatio 1.1; } Aplus 26; Cdelta 0.158; } smoothCoeffs { delta cubeRootVol; cubeRootVolCoeffs { deltaCoeff 1; } maxDeltaRatio 1.1; } I calculate yplus value of bottom wall by yplusLES utility, and it shows very high yplus values. Im sure grid is good, so problem is with 'U', I think due to gradients in flow separation. Where am I making mistake? Thanks very much for interest and help. 

December 19, 2012, 05:42 

#85 
Senior Member
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 185
Rep Power: 9 
Dear j.t.,
I think your initial field is too far from reality. Uniform velocity is not enough to run a LES calculation. Even if your calculation is running, you will spend days to get converged statistics. You should improve your initial condition. First, run on a coarse grid (very coarse), and use perturbU tool to initialize the velocity field. When you get a turbulent flows, even if it is not physically correct, use mapField tool to initialise your fine grid quantities. I think this will help you. If you have more questions, create a new thread, to keep this one on channel flow calculation only. Cédric 

December 20, 2012, 03:31 

#86 
New Member
j.t.
Join Date: Nov 2012
Posts: 11
Rep Power: 5 
dear Cedric,
I understand the meaning. The flow is not very turbulent enough to be used for LES or any turbulence modeling technique. I will do the same, and will create new thread if I need help. Thanks so much for your help. J.T. 

May 31, 2013, 18:25 
LES open channel

#87 
Member
Pedro Ramos
Join Date: Mar 2012
Location: Portugal
Posts: 61
Rep Power: 6 
Hello...!
I'm a newbie in OF... ANy of you have a tutorial/example for LES open channel? I want to simulate a open channel flow around a pille to study the scour around it. Best regards. Pedro. 

May 31, 2013, 18:48 
Inlet error

#88 
Member
Pedro Ramos
Join Date: Mar 2012
Location: Portugal
Posts: 61
Rep Power: 6 
Hi!
I'm doing the open channel flow simulation around a pile (LES) and I find an error in the inlet section (too much velocity) wich causes a increment of pressure in the bed of the channel (right up corner of the image: http://d.pr/i/vIcS) See the video also: http://www.youtube.com/watch?v=G_dtwb8JFD0 Any tips? 

October 21, 2013, 04:38 
LES Channel in Openfoam

#89 
New Member
subhendu
Join Date: May 2012
Posts: 10
Rep Power: 6 
Hello
I am to run channel flow with dynSmagorinsky(channel395), but my statistics are not in good agreement with Moser DNS(Retau=395) Dimesion of my domain is : 4*2*2,80*50*60 I generate initial condition using perturbU utility and run the simulation for long time . After the initial peaks in turbulent kinetic energy the energy fluctuates around a value. After that I run a long simulation and perform average. using post channel utility 1. vrms , wrms are underestimated. 2. urms is overestimated . 3. Umean is also not matching far from the wall. the schemes of my channel: ddtSchemes { default backward; } gradSchemes { default Gauss linear; grad Gauss linear; grad Gauss linear; } divSchemes { default none; div(phi,U) Gauss linear; div(phi,k) Gauss limitedLinear 1; div(phi,B) Gauss limitedLinear 1; div Gauss linear; div(phi,nuTilda) Gauss limitedLinear 1; div((nuEff*dev(grad .T()))) Gauss linear; } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear corrected; laplacian((1A ),p) Gauss linear corrected; laplacian(DkEff,k) Gauss linear corrected; laplacian(DBEff,B) Gauss linear corrected; laplacian(DnuTildaEff,nuTilda) Gauss linear corrected; } interpolationSchemes { default linear; interpolate linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; } I use delta cubeRootVol; Same issue I have with static Smagorinsky model also. Please see my results Thankyou Subhendu 

February 23, 2014, 18:20 

#90 
Member
Tony
Join Date: Nov 2013
Posts: 35
Rep Power: 4 
Dear Cedric,
I find your posts on LES channel flow very useful. Just one question, how did you deal with the data, in other words, how did you perform the field averaging like getting mean velocity profile and rms plots? It would be great if you can give me some hints on that. Thank you very much. Best regards, Tony 

March 5, 2014, 10:34 

#91 
New Member
Arne Eggers
Join Date: Oct 2013
Posts: 5
Rep Power: 5 
Hi,
im trying to simulate the Moser channel with LES Turbulence Modelling. Im using a university code . Its possible to define a pressure gradient to generate a flow in the channel. Im trying to implement a dynamic pressure gradient to define a fixed mass flow through the channel, as Moser et al. and others did. Atm im using a function delta_pressure_gradient = (u_soll  uist ) / 10. Where delta_pressure_gradient is the change in pressure gradient. u_soll is the velocity calculated by the mass flow of the DNS data and u_ist the current velocity averaged in space (over the whole channel) and in time over 1000 time steps. My problem is that this pressure gradient adjustment need a lot of time unil it get into some kind of stationary status. Does anybody know a better function to calculate the pressure gradient for the next time steps ? Arne 

March 9, 2014, 02:02 

#92 
Senior Member
Huang Xianbei
Join Date: Sep 2013
Location: CAU,China
Posts: 277
Rep Power: 6 
Hi:
By the way, I'd like to ask a question about the initial fileds. Yes, perturbU is the best utility to generate a velocity filed, while how about the other fields such as p, nusgs? As we can see from channel395 tutorial, the 0 folder contains 6 files of the initial fields which are all nonuniform list values. How can we generate as these? Huang Xianbei 

March 10, 2014, 09:39 

#93  
Senior Member
Huang Xianbei
Join Date: Sep 2013
Location: CAU,China
Posts: 277
Rep Power: 6 
Quote:
I have the same problem as you posted here. Whether the geometry is changed or not , the u_tau is underestimated through the whole calculation, I think it's due to the gradP adjustment during the calculation. However, as you mentioned, the u_tau=0.073 which is only 92.4% of the expected value. This will lead to a lower Re_tau. Have you ever found any solutions up to now? Xianbei 

March 21, 2014, 13:47 
Reynolds number

#94 
New Member
Giulio S
Join Date: Oct 2013
Location: Italy
Posts: 4
Rep Power: 4 
I want to report a question concerned the U_bar used by OpenFoam in the channel flow tutorial, where:
U_bar=0.1335. If you calculate the Reynolds number as well as Re=2δU_bar/ν you get Re=13350. But if you want to compare the LES results with the DNS ones (computed at friction Reynolds number 395), as well as Pope suggested, the Reynolds number corresponding to the friction Reynolds number 395 is 13750, where U_bar_new=0.1375. That could be a cause of the misleading results. 

May 17, 2014, 16:52 

#95 
New Member
Hans Barósz
Join Date: May 2014
Posts: 22
Rep Power: 4 
Hello OFers,
can someone give me a hint concerning the channel395 tutorial with the oneEqEddy LESturbulence model? When I run the tutorial without any changes, i get a totally wrong velocity profile. I use the postChannel utility for the latest Times (1000) to get U over y. It gives me the following 25 values due to the symmetry of the geometry with 50 element layers in ydirection: 0.00480001 0.00827117 0.0148983 0.023951 0.026045 0.0374098 0.0383488 0.047655 0.05193 0.0558505 0.066921 0.0635531 0.0834683 0.0714288 0.101734 0.0794559 0.121895 0.0875807 0.144149 0.095728 0.168714 0.103805 0.195829 0.111702 0.225758 0.119296 0.258795 0.126453 0.295262 0.133031 0.335514 0.138891 0.379945 0.143905 0.428988 0.147972 0.483123 0.151042 0.542878 0.153137 0.608836 0.154375 0.681641 0.154972 0.762005 0.155195 0.850711 0.155256 0.948626 0.155269 Then I want to calculate ReTau, which should be around 395, but I only recieve 293. What I do: dU/dy @ y=0 : 0,00827117/0,00480001 = 1,72312 which sould be 3,1205 uTau = sqrt(2E5* 1,72312) = 0,00587 which should be 0,0079 ReTau = uTau/2E5 = 293 which should be 395 With these wrong values, the dimensionless velocity profile uPlus over yPlus is wrong indeed. I already refined the mesh, i also tried different SGS Model, but without improvement. I doubt my calculation of dU/dy is wrong, but I have clue why it is so atm. Probably its just a stupid mistake but I cant find it. Hopefully someone can help me with this issue. I am using OF2.3.0 with pimpleFoam solver and standard settings from the /tutorials/incompressible/pimpleFoam/channel395/ dict. PS: in this thread it was mentioned to calculate uTau with the pressure gradient, but in my case it is zero from x=0 to x=4m. Dont know how I can handle with this information. 

May 19, 2014, 04:02 

#96  
New Member
Giulio S
Join Date: Oct 2013
Location: Italy
Posts: 4
Rep Power: 4 
I think you have wrong to calculate du/dy. However, how many iterations have you done?
Quote:


August 21, 2014, 08:13 
Twopoint correlation scaling in Moser's et als data

#97 
Member
Timofey Mukha
Join Date: Mar 2012
Location: Uppsala, Sweden
Posts: 57
Rep Power: 6 
Dear Foamers, I'm also doing some channel flow computations, using the DNS data from Moser et al as reference. I am currently trying to compare the twopoint correlations and I can't figure out how they are scaled in the DNS data.
I mean, the correlations are already normalized by definition, so why the need for a new scale? It says in the files that it is scaled by U_tau and h, but I can't figure out how . Maybe those that worked with this data could give me a hint? 

November 12, 2014, 11:54 

#98  
Member
Timofey Mukha
Join Date: Mar 2012
Location: Uppsala, Sweden
Posts: 57
Rep Power: 6 
Quote:


November 19, 2014, 07:35 

#99 
New Member
Zhiwei Zheng
Join Date: May 2014
Posts: 23
Rep Power: 4 

March 29, 2015, 10:45 
initial condition

#100 
New Member
Amir
Join Date: Jul 2011
Location: Shiraz
Posts: 15
Rep Power: 7 
Hi
Im trying to validate results for OneEquation LES model and I also used MapField utility for grid study purpose but getting unacceptable results after mapping. How should I initialize the flow to get correct answers in channel flow case? 

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 