
[Sponsors] 
June 13, 2010, 06:55 
Atmospheric boundary layer

#1 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 15 
Hi
I try to simulate an atmospheric boundary layer, on bottom I use wall function, but if i use nutRoughWallFunction, epsilon has a overshooting in last cells why? Best Regards 

June 14, 2010, 05:57 

#2 
Member
Michael
Join Date: Mar 2009
Posts: 48
Rep Power: 16 
Hi,
the overshooting is a known problem! Look for example here: http://www.openfoamworkshop.org/2009...ner_slides.pdf What Version of OpenFOAM are you using? I think, there have been some problems with the nutRoughWallCondition in OpenFOAM 1.6! So, you should use OpenFOAM 1.6.x!! Hope, that helps! 

June 14, 2010, 06:05 

#3 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 15 
Hi
I read this paper, useful. But the problem is openfoam 1.6! I use now wall function of 1.6.x and I haven't overshooting problem,thanks you 

June 14, 2010, 11:58 

#4 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 15 
using openfoam 1.6.x the overshooting there isn't; but I Have another problem: in atmospheric boundary layer simulation, th wall value of epsilon and k would be costant? In my simulation these value are constant only after some cells along x axis Why?
Last edited by Daniele111; June 15, 2010 at 05:16. 

June 15, 2010, 05:04 

#5 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 15 
Hi
What are the correct boundary conditions for p field in these simulation? Thanks 

June 15, 2010, 05:05 

#6 
Member
Michael
Join Date: Mar 2009
Posts: 48
Rep Power: 16 
What is x?? Is it the height of your domain or the main flow direction??


June 15, 2010, 05:13 

#7 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 15 
Main flow direction, change inlet p condition:


June 15, 2010, 05:29 

#8 
Member
Michael
Join Date: Mar 2009
Posts: 48
Rep Power: 16 
Sorry, I don't understand what Wss means...
I've chosen a "zeroGradient"condition for my ABLSimulations at the inlet for p! To achieve a homogenous ABL (constant values in flow direction), you have to calculate the right Ks (and Cs) in subject to your z0 (conversion of z0 to Ks due to your roughWallBC)! Hope, that helps... 

June 15, 2010, 05:32 

#9 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 15 
Wss, is wall shear stress, my z0 is 0.001, Ks=0.02, Cs=0.5 it's wrong?
Thanks you! 

June 15, 2010, 05:36 

#10 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 15 
My Bc. Thanks you again


June 15, 2010, 05:42 

#11 
Member
Michael
Join Date: Mar 2009
Posts: 48
Rep Power: 16 
I'm getting a value of 0.019586! Almost the same...
I've used the formula: Ks = E*z0/Cs where E=9.793 is a constant of the wall function! 

June 15, 2010, 05:47 

#12 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 15 
My Ks=20*y0, but where is th mistake? Your Cs=0.5? E in your simulation epsilon, k are constant in the first cell along main flow direction, my xaxis?


June 15, 2010, 05:52 

#13 
Member
Michael
Join Date: Mar 2009
Posts: 48
Rep Power: 16 
I think, the velocity at the bottom should be zero (no slip condition)!
Unfortunately, I don't have any experiences with the timeVaryingMappedFixedValueBC! So, I can't help with this! I used the GroovyBC for the analytical profiles! Maybe, you should define the constants of the wall function in the nutfile! Just to be sure, you use the same like in your conversion from z0 to Ks! Actually, Cs is 0.327 in your BC's and not 0.5 like you mentioned before! 

June 15, 2010, 06:01 

#14 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 15 
I just use groovyBc, timeVaryingMappedFixedValueBC is not the problem, it's the same thing. I don't understand when you say that I would define the constants of the wall function in the nutfile. What do i do this? The velocity at the bottom has a value becouse I use like reference a paper that imposed it, but I pose it 0 and the problem there is. The p bc is the same that you have?


June 15, 2010, 06:48 

#15 
Member
Michael
Join Date: Mar 2009
Posts: 48
Rep Power: 16 
Yes, p BC is the same!!


June 15, 2010, 15:02 

#16 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 15 
Hi
Bah I try to use absurd values of Ks and Cs, but the result is always the same; I copied the turbulenceModels folder of OpenFOAM 1.6.x and I copy it in src folder of OpenFOAM 1.6 and the I compile it. It's wrong? Because if I change ks and cs not change the result? 

June 15, 2010, 16:01 

#17 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 15 
Can i see your bc?


June 15, 2010, 17:36 

#18 
Member
Michael
Join Date: Mar 2009
Posts: 48
Rep Power: 16 
Hi,
sure! Here are my BC's! I definitely get a change when I use different values for Ks (see the picture)! Hope that helps! Why do you want to simulate an ABL? What is the topic of your project?? 

June 15, 2010, 17:53 

#19 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 15 
Thank you! I must simulate sand dune evolution. So I would calculate shear stress at bottom. Thank you again
What are these fields in your groovy bc? refValue uniform 0; refGradient uniform 0; valueFraction uniform 1; value uniform 0.1; valueExpression "para"; gradientExpression "0"; fractionExpression "1"; Last edited by Daniele111; June 15, 2010 at 18:18. 

June 16, 2010, 05:08 

#20 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 15 
I try to use your bc setup, but the velocity field along main flow is these. It's correct? What is your first cell higth? My domain is higth 100m
Last edited by Daniele111; June 16, 2010 at 07:20. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Wind turbine simulation  Saturn  CFX  58  July 3, 2020 01:13 
Turbulent Boundary Layer on a Flat Plate  Hoshang Garda  FLUENT  1  November 27, 2013 10:24 
RPM in Wind Turbine  Pankaj  CFX  9  November 23, 2009 04:05 
Combining BCs: wall  outlet. Boundary layer disappears  MartinaF  OpenFOAM Running, Solving & CFD  1  July 20, 2009 18:14 
Convective Heat Transfer  Heat Exchanger  Mark  CFX  6  November 15, 2004 15:55 