
[Sponsors] 
February 27, 2013, 01:32 
kepsilon boundary condition in openFoam

#1 
New Member
Amitabh
Join Date: Feb 2013
Posts: 7
Rep Power: 10 
I am trying to validate kepsilon model on openFoam for a simple turbulent channel via the pisoFoam solver. The boundary condition being used for k and epsilon is the kqRWallFunction. While the previous forum posts suggest that kqRWallFunction simply applies a zero gradient condition for k at the wall, I'm not seeing dk/dy=0 at the wall for the solutions I am getting. In fact, for the converged solution, there seems to be a very steep gradient in k at the wall, and k(y=0) seems to be nonzero. My first grid point at the wall is at around y^+=1.
I am still not very good at reading the source code, and I found scare documentation for this. So does anyone know what exactly the kqRWallFunction wall BC means ? I'm guessing it is some sort of loglaw based wallfunction, and maybe my first grid point needs to be outside the viscous region. Any insight on this would be great. Amitabh 

February 27, 2013, 02:48 

#2 
Senior Member
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 18 
You are right about your first grid cell. If you got y+ around wall, you should not use wall functions. How did you calculate y+? (See this thread: http://www.cfdonline.com/Forums/ope...testcase.html )
You can find the wall functions here: src/turbulenceModels/incompressible/RAS/derivedFvPatchFields/wallFunctions Of special interest is the epsilonWallFunction, have a look at epsilonWallFunctionFvPatchScalarField.C , the member function updateCoeffs (line 175 and further). Here you can see what is actually being calculated (G is the production term). 

February 27, 2013, 03:40 

#3 
New Member
Amitabh
Join Date: Feb 2013
Posts: 7
Rep Power: 10 
Thanks Bernhard, this was very helpful. The source code seems to indeed use a loglaw based wall function for epsilon. I clearly need to use a larger grid size near the wall.
I am basically imposing pressure gradient in the flow, so it is then easy to calculate u_tau from dP/dx and channel halfwidth H. I calculate l^+ as nu/u_tau. Let me know if this does not sound right. thanks ! Amitabh 

February 27, 2013, 03:52 

#4 
Senior Member
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 18 
You could also choose to switch to a LowRe RANSmodel, but than you may have to do some implementation yourself. It depends a bit on your needs.
I am not 100% sure about your way of calculating y+, but you can easily check it afterwards with the utilities provided in the thread I linked above. You may want to just calculate y* if you decide to coarsen your mesh. 

February 27, 2013, 08:51 

#5 
New Member
Amitabh
Join Date: Feb 2013
Posts: 7
Rep Power: 10 
I had a followup question. It seems to me that (for highRe RANS) there should be a slip velocity at the wall if y+ of the first grid point is large. The slip velocity can be obtained from the loglaw, i.e. U=u_tau*(log(y+)/kappa+B_i). Alternatively dU/dy=u_tau/(kappa*y) can be imposed.
For all the example problems I have seen, U=0 is imposed at the wall, which seems wrong. Again, any insight on this would be great. regards Amitabh p.s.: seems like I'll need to start writing my own boundary condition routines soon 

January 9, 2014, 10:47 

#6 
Member
Kapa Lilla
Join Date: Mar 2009
Location: Bruxelles, Belgium
Posts: 57
Rep Power: 13 
Dear Amitabh,
did you finally managed with kepsilon? I did a periodic channel flow simulation with different turbulence models. I tried low Re kepsilon model, but did not manage to get the right velocity gradient at the wall, no matter what wall treatment I'm using. My wall+ is around 0.8. In any case my wall gradient is under estimated, it is around 2/3 of the DNS database I'm using. If I use v2f instead, everything is fine. Thanks, Lilla 

January 9, 2014, 11:37 

#7 
New Member
Amitabh
Join Date: Feb 2013
Posts: 7
Rep Power: 10 
I did indeed manage to figure out the low Re kepsilon last year  it seemed to be working ok. I can send you the files if you can somehow send me your email, since there are upload limits here.


January 9, 2014, 11:50 

#8 
Member
Kapa Lilla
Join Date: Mar 2009
Location: Bruxelles, Belgium
Posts: 57
Rep Power: 13 
Thank you very much! My email is kapalilla@gmail.com


January 17, 2014, 05:50 

#9 
Member
Manan
Join Date: Oct 2013
Location: Göteborg
Posts: 37
Rep Power: 9 
Hi
Is it possible for you to send me the low Re k epsilon model files too? I am trying a similar exercise in validating the model for channel flow with periodic inlet and outlet. My email id is manan.lalit@gmail.com. Thanks. Last edited by MaLa; February 14, 2014 at 12:13. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
domain imbalance for enrgy equation  happy  CFX  14  September 6, 2012 02:54 
A general openfoam development question about boundary condition  kaifu  OpenFOAM  11  August 15, 2012 13:51 
Problem occurs in Boundary condition of pressure in openFOAM  jignesh_thaker2007  OpenFOAM  0  February 6, 2012 14:05 
How to transfer boundary condition from Openfoam to fluent  sachinlb  OpenFOAM PostProcessing  1  January 6, 2012 02:41 
[Commercial meshers] Trimmed cell and embedded refinement mesh conversion issues  michele  OpenFOAM Meshing & Mesh Conversion  2  July 15, 2005 05:15 