
[Sponsors] 
July 19, 2005, 16:14 
Hi,
I was thinking of using t

#41 
New Member
Akshay Gowardhan
Join Date: Mar 2009
Posts: 1
Rep Power: 0 
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 

July 20, 2005, 05:48 
0] Use a public domain mesh ge

#42 
Super Moderator
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 17 
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. 

August 10, 2005, 12:23 
Eugene,
The channelflow per

#43 
Member
Ali Heidari
Join Date: Mar 2009
Location: Surrey, London, United Kingdom
Posts: 39
Rep Power: 9 
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? 

August 10, 2005, 18:35 
The tutorial flow is a previou

#44 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 13 
The tutorial flow is a previous result. The perturbation code only creates preturbulent 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. 

August 10, 2005, 18:40 
So, what would be the best cho

#45 
Member
Ali Heidari
Join Date: Mar 2009
Location: Surrey, London, United Kingdom
Posts: 39
Rep Power: 9 
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. :) 

August 10, 2005, 18:50 
np.
p=0 and small k is fine

#46 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 13 
np.
p=0 and small k is fine. nuSgs doesn't matter because it is calculated from k and delta. 

November 3, 2006, 08:52 
Compiling perturbU in OpenFOAM

#47 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
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
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

November 22, 2006, 04:54 
Hi everyone
I used oodles f

#48 
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 9 
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¶meter changing in pitzDaily. Please help me. regards marhamat 

November 26, 2006, 03:20 
Hi
In lesmodels some paramet

#49 
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 9 
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 

November 27, 2006, 05:09 
Hello,
you're right, the impl

#50 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
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/OpenFOAM1.3/src/LESmodels/incompressible and OpenFOAM/OpenFOAM1.3/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
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

November 27, 2006, 05:16 
Thanks a lot Alberto
marhamat

#51 
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 9 
Thanks a lot Alberto
marhamat 

November 27, 2006, 08:04 
You also can find more informa

#52 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
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
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

November 27, 2006, 08:56 
Dear Alberto
Thanks for your

#53 
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 9 
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 

November 30, 2006, 09:13 
I don't have the paper in elec

#54 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
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, StratocumulusCapped mixed layers derived from a threedimensional model", oundaryLayer Metereology, 18:495527, 1980. C. H. Moeng, J. C. Wyangaard, Spectral analysis of large eddy simulation of the convective boundary layer, J. Atmos. Sci., 45:35753587, 1984. P. P. Sullivan, J. C. McWilliams, C.H. Moeng, A subgridscale model for large eddy simulation of planetaryboundary layer flows, BoundaryLayer Metereology, 71:247276, 1994. Regards, Alberto
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

December 1, 2006, 11:32 
Thanks a lot Alberto
Your ex

#55 
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 9 
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 

December 1, 2006, 13:23 
The results you obtain depends

#56 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
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
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

December 1, 2006, 18:47 
Hi Alberto
I think my mesh si

#57 
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 9 
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 

December 3, 2006, 09:41 
Hello marhamat,
if the grid a

#58 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
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
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

December 3, 2006, 22:52 
Hi everyone:
I am working

#59 
Member
Bobby
Join Date: Mar 2009
Location: wuhan, hubei, China
Posts: 33
Rep Power: 9 
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 

December 11, 2006, 02:44 
Hi Alberto
In your last expla

#60 
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 9 
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 

Thread Tools  
Display Modes  

