CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Running, Solving & CFD (
-   -   Atmospheric boundary layer (

Daniele111 June 13, 2010 06:55

Atmospheric boundary layer
1 Attachment(s)
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

farbfilm June 14, 2010 05:57


the overshooting is a known problem! Look for example here:

What Version of OpenFOAM are you using? I think, there have been some problems with the nutRoughWall-Condition in OpenFOAM 1.6! So, you should use OpenFOAM 1.6.x!!

Hope, that helps!

Daniele111 June 14, 2010 06:05

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

Daniele111 June 14, 2010 11:58

1 Attachment(s)
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?

Daniele111 June 15, 2010 05:04

What are the correct boundary conditions for p field in these simulation?


farbfilm June 15, 2010 05:05

What is x?? Is it the height of your domain or the main flow direction??

Daniele111 June 15, 2010 05:13

1 Attachment(s)
Main flow direction, change inlet p condition:

farbfilm June 15, 2010 05:29

Sorry, I don't understand what Wss means...
I've chosen a "zeroGradient"-condition for my ABL-Simulations 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...

Daniele111 June 15, 2010 05:32

Wss, is wall shear stress, my z0 is 0.001, Ks=0.02, Cs=0.5 it's wrong?

Thanks you!

Daniele111 June 15, 2010 05:36

1 Attachment(s)
My Bc. Thanks you again

farbfilm June 15, 2010 05:42

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!

Daniele111 June 15, 2010 05:47

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 x-axis?

farbfilm June 15, 2010 05:52

I think, the velocity at the bottom should be zero (no slip condition)!

Unfortunately, I don't have any experiences with the timeVaryingMappedFixedValue-BC! 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 nut-file! 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!

Daniele111 June 15, 2010 06:01

I just use groovyBc, timeVaryingMappedFixedValue-BC 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 nut-file. 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?

farbfilm June 15, 2010 06:48

Yes, p BC is the same!!

Daniele111 June 15, 2010 15:02

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?

Daniele111 June 15, 2010 16:01

Can i see your bc?

farbfilm June 15, 2010 17:36

2 Attachment(s)

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??

Daniele111 June 15, 2010 17:53

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";

Daniele111 June 16, 2010 05:08

1 Attachment(s)
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

All times are GMT -4. The time now is 17:14.