[agowardhan]

Hi,
I was thinking of using this code to simulate flow around buildings in an urban boundary layer.
I was wonderrring how dificult it would be to incorporqte building geometery as it works on unstructured mesh.

Akshay

[mattijs]

0] Use a public domain mesh generator. Netgen, GMSH etc. can do automatic tet mesh generation (however do not try to run LES on tets)

1] A simple way would be to
- generate a big block of cells (blockMesh)
- select the cells that represent your building with the cellSet utility and 'boxToCell' source (have a look at the cellSetDict sample in the cellSet directory)
- invert the set
- subsetMesh <root> <case> <cellsetname>

2] If you have the buildings as an e.g. STL file you could use the selectCells utility which selects based on surface normal. Again this writes a cellSet you can use with subsetMesh.

Just some ideas.

[ali]

Eugene,

The channelflow perturbation code you provided just intiates the velocity. Is the initial velocity field in "0" directory of channelOodles tutorial created with this perturbation method or they are result of a previous run to accelerate the solution to the statistically steady situation?

I'm asking this because k,nuSgs,and p all have initial values? Is it also possible to create initial values for these variables from the linear perturbation or they are results of previous runs?

[eugene]

The tutorial flow is a previous result. The perturbation code only creates pre-turbulent sinuous waves of raised low speed fluid. These give rise to true turbulence over a period of around 20 flowthrough times, which is more than enough to produce the proper k, nuSgs and p distributions.

It is important to realise that the perturbation code does not produce turbulence, it only initiates the wall turbulence production cycle.

[ali]

So, what would be the best choice of initial "k" and "nuSgs" (I assume initial value for "p" is zero)? Any estimate? Or just setting them to a small value is ok?

Thank you Eugene. :-)

[eugene]

np.

p=0 and small k is fine.
nuSgs doesn't matter because it is calculated from k and delta.

[alberto]

Compiling perturbU in OpenFOAM 1.3 gives this error:

Making dependency list for source file perturbU.C
could not open file fvCFD.H for source file perturbU.C

due to incomplete options file. Correcting it gives:

perturbU.C: In function 'int main(int, char**)':
perturbU.C:162: error: 'physicalConstant' has not been declared
perturbU.C:165: error: 'physicalConstant' has not been declared

because physicalConstant has been renamed to mathematicalConstant.

I attach the corrected version of the tool.

Best regards,
Alberto

perturbU.tar.gz

[marhamat]

Hi everyone

I used oodles for turbulent pipe flow modeling
but the results are not as I expected from LES.

I do this with mesh&parameter changing in pitzDaily.

Please help me.

regards
marhamat

[marhamat]

Hi
In lesmodels some parameters&cofficients identified(for example:ck,cI,ce,...) that are strange for me.
How i can reach to basic knowledge about them.
Are any usefull reference in this field?

Thanks
marhamat

[alberto]

Hello,
you're right, the implementation of some LES models in OpenFOAM differs a bit from the usual formulation.

However, you can find a short description of each LES model in the header files in OpenFOAM/OpenFOAM-1.3/src/LESmodels/incompressible and OpenFOAM/OpenFOAM-1.3/src/LESmodels/compressible

For example, for the incompressible Smagorinsky model, you have:
<pre>
The Isochoric Smagorinsky Model
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
Algebraic eddy viscosity SGS model founded on the assumption that
local equilibrium prevails, hence

B = 2/3*k*I - 2*nuEff*dev(D)

where

D = symm(grad(U));
k = (2*ck/ce)*delta^2*||D||^2
nuSgs = ck*sqrt(k)*delta
nuEff = nuSgs + nu
</pre>
From these expressions you should be able to relate the usual Smagorinsky constan c_s to ck and ce.

Regards,
Alberto

[marhamat]

Thanks a lot Alberto
marhamat

[alberto]

You also can find more information on this paper:

C.Fureby, G.Tabor, H.Weller and A.D.Gosman, A Comparative Study of Sub Grid Scale Models in Homogeneous Isotropic Turbulence, Physics of Fluids, 9/5, pp. 1416 - 1429, 1997.

Regards,
Alberto

[marhamat]

Dear Alberto
Thanks for your kindness.
But this paper is not avaiable for me.If it is possible to you please mail it to my Email
Regard
Marhamat

[alberto]

I don't have the paper in electronic format.

However, if you write the SGS stress tensor as:

tau_ij = -2 * nu_t * S_ij

you can define the eddy viscosity as:

nu_t = Ck * l * sqrt(e)

where e is the SGS kinetic energy.

If you write the transport equation for the SGS energy e:

de/dt + u_j de/dx_j = P + B - epsilon + D

where:

P = production = -tau_ij * S_ij
B = buoyancy
epsilon = dissipation = C_e * e^(3/2) / l
D = diffusion = d/dxi(2 nu_t de/dx_i)

If in the equation for e you put the shear production equal to the dissipation, you get:

nu_t = (C_s*Delta)^2 sqrt(2 S_ij S_ij)

The Smagorinsky constant C_s can consequently be calculated as a function of C_e and C_k:

C_s = sqrt(C_k * sqrt(C_k/C_e))

You can found the details here:

J. W. Deardoff, Stratocumulus-Capped mixed layers derived from a three-dimensional model", oundary-Layer Metereology, 18:495-527, 1980.

C. H. Moeng, J. C. Wyangaard, Spectral analysis of large eddy simulation of the convective boundary layer, J. Atmos. Sci., 45:3575-3587, 1984.

P. P. Sullivan, J. C. McWilliams, C.H. Moeng, A subgrid-scale model for large eddy simulation of planetary-boundary layer flows, Boundary-Layer Metereology, 71:247-276, 1994.

Regards,
Alberto

[marhamat]

Thanks a lot Alberto
Your explanation are very usefull.
For Openfoam examination when we use LES for turbulence modelein i used oodles for turbulent pipe flow . I do this by changing in mesh and parameters in pitzDaily .
But result are not as I expected from LES in comparison whit experimental results.
What do you propse to me for exmanition of OPenFOAM.

Best regards
marhamat

[alberto]

The results you obtain depends on many factors:

- What's your domain size?
- What's the Reynolds number of your flow?
- What discretisation are you using? I mean what grid density and what interpolation schemes are you using?
- How do you initialize the flow field?
- Why are your results different from experimental data? Are you comparing velocity profiles? Or considering statistics?

Regards,
Alberto

[marhamat]

Hi Alberto
I think my mesh size are fine enough(65,40,60).
Re=4000 &inlet velocity is uniform =2m/s
I used Turbinlet for inlet boundry condition &
inletOutlet for output boundry condition.
i comparing velocity profile.
In my obtioned profile near the wall the velosity gradient is not sharp enough .
Discretisation sheme is same as used in pitzDaily.

Thanks
marhamat

[alberto]

Hello marhamat,
if the grid and the BC's settings are OK, probably it's just a question of time averaging.

Check if your turbulent flow is fully developed and start averaging from that point on.

Regards,
Alberto

[aderliner]

Hi everyone:

I am working on my project about fuel spray using lesinterFoam, but it seems that it does not break up at all. I wonder if it is right to choose lesinterFoam, or, I need to creat the solver myself?

By the way, is the lesinterFoam using LES theory and VOF method?

Thx~!
Best regards~!

Bobby
12.2

[marhamat]

Hi Alberto
In your last explanation(Thursday, November 30, 2006 )we have:
C_s = sqrt(C_k * sqrt(C_k/C_e))
In many of OpenFOAM LES models for example in one equation eddy model C_k=0.07,C_e=1.005.
So the value of C_s for different problems is constan.
we know that the value of C_s in different problems is varriable:
in pipe flow :C_s=0.1
in Channel flow C_s =0.065 ...
Am i in wrong?

Regards
Marhamat