
[Sponsors] 
February 14, 2005, 05:49 
Dear all,
Which kind of bo

#1 
Guest
Posts: n/a

Dear all,
Which kind of boundary conditions should I apply for k and epsilon at the wall when I am using a low Re kepsilon model? The same as the high renolds number model? zerogradient? 

February 14, 2005, 05:51 
fixedValue of 0 for k and zer

#2 
Guest
Posts: n/a

fixedValue of 0 for k and zeroGradient for epsilon although with most low Re models it will work perfectly well with zeroGradient on k.


February 15, 2005, 09:56 
How can we change the value o

#3 
Guest
Posts: n/a

How can we change the value of k at inlet to zero gradient? I choose inlet and k is automatically made fixed value.


February 15, 2005, 10:00 
A zeroGradient inlet conditio

#4 
Guest
Posts: n/a

A zeroGradient inlet condition is effectively an upstream extrapolation from inside the domain and is therfore unstable for a convectiondominated property.


February 16, 2005, 03:55 
From my experience (although

#5 
Guest
Posts: n/a

From my experience (although short) from spray calculations in Foam using the Launder Sharma kepsilon model, choosing k to have a zero gradient on walls, can cause the timestep to become very small (of the order of nanoseconds). If k is set to zero, this behaviour seems to go away.


February 16, 2005, 09:26 
Surely, the original paper wi

#6 
Guest
Posts: n/a

Surely, the original paper will tell you what boundary conditions you should use.


June 20, 2005, 09:47 
Hi all!
I have a question a

#7 
Member
Tommaso Lucchini
Join Date: Mar 2009
Posts: 83
Rep Power: 10 
Hi all!
I have a question about turbulence models and mesh motion. Usually the function turbulence>correct() is calculated after the PISO loop. In the case of a moving mesh, the flux phi is calculated according to: phi = fvc::interpolate(rho) *((fvc::interpolate(U) & mesh.Sf())  mesh.phi()); In the correct() function of the turbulenceModel divU is corrected by: if (mesh_.moving()) { divU += fvc::div(mesh_.phi()); } why? Shouldn't be divU = fvc::div(mesh_.phi()); Could someone explain this? thanks a lot Regards Tommaso 

June 20, 2005, 10:12 
in
phi = fvc::interpolate(r

#8 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 15 
in
phi = fvc::interpolate(rho) *((fvc::interpolate(U) & mesh.Sf())  mesh.phi()); the  mesh.phi() converts the absolute fluxes obtained from the absolute U into relative fluxes. if (mesh_.moving()) { divU += fvc::div(mesh_.phi()); } adds the contribution from the mesh motion to the divergence calculated from the relative fluxes. 

January 24, 2006, 08:12 
Hi FOAMers,
I´ve just looked

#9 
Member
Ralph
Join Date: Mar 2009
Posts: 40
Rep Power: 10 
Hi FOAMers,
I´ve just looked at the implementation of some of the turbulence models for incompressible flows in Open FOAM and there I is one thing I did´t get so far. Maybe someone can help me out. For the calculation of the Reynoldstensor there´s obviously used the BoussinesqApproximation, where k is used to avoid a traceless stress tensor: n<sub>t</sub>(¶u<sub>i</sub>/¶x<sub>j</sub>+¶u<sub>j</sub>/¶x<sub>i</sub>)2/3kd<sub>ij</sub>. This is done in the method: turbulenceModel::R(). In the method turbulenceModel::divR(), which calculates the divergence of this part in combination with the laminar part, the correction by 2/3kd<sub>ij</sub> is omitted, which should actually be of the form: 2/3*grad(k). Is this regular or do I omit a part of the normal stresses (which is added to the pressuregradient term and falsify the static pressure)? Thanks in advance, Ralph 

January 24, 2006, 09:27 
Yes, or "well, yes". All you

#10 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,790
Rep Power: 23 
Yes, or "well, yes". All you need to do is subtrack k from the pressure field and you'll get the static pressure.
Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

January 24, 2006, 10:04 
Thanks Hrvoje
for your quick

#11 
Member
Ralph
Join Date: Mar 2009
Posts: 40
Rep Power: 10 
Thanks Hrvoje
for your quick reply. By the way: In turbulenceModel::divR() for incompressible cases, the deviatoric part of grad(U).T() is used (in an explicit manner). Is this done for stabilisation reasons, as the trace of the tensor should be zero anyway (incompressible)? Ralph 

January 24, 2006, 11:40 
Ralph,
dev(grad(U).T()) is

#12 
Member
E. David Huckaby
Join Date: Mar 2009
Posts: 57
Rep Power: 10 
Ralph,
dev(grad(U).T()) is the second term and the missing divergence term in the Boussinesq approximation as written above. I beleive the reason this is treated explitly is that the term is a crosscoupling term between the different components of the velocity vector. Treating this term implicitly is not possible with a segregated solver. Dave 

January 24, 2006, 11:43 
The term says
div(mu (grad

#13 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,790
Rep Power: 23 
The term says
div(mu (grad U)^T) and this can be rewritten as mu grad (div(U)) + grad mu . grad U The first one drops off because of the incompressibility constraint but the second one remains. However, after a lot of messing about it turns out that having the original form behaves better than grad mu . grad U and this is why it remains. Hope this is clear, Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

January 24, 2006, 12:11 
Thanks for your answers,
I th

#14 
Member
Ralph
Join Date: Mar 2009
Posts: 40
Rep Power: 10 
Thanks for your answers,
I think that´s clear. Maybe I expressed myself somewhat imprecise. My question was about the deviatoric part of (grad U)^T. Why is the the deviatoric part of the tensor and not the "whole" tensor used in the second term of "divR()"? Ralph 

July 17, 2006, 14:11 
First of all I have to say tha

#15 
Guest
Posts: n/a

First of all I have to say that being an undergraduated student I am very new with both Foam and CFD.
From literature I found that Launder Sharma model requires a zero value for epsilon at wall. But trying this boundary Foam produce a singularity error, as expected looking at model. Is Foam LaunderSharma model a particular one requiring zerogradient? 

July 18, 2006, 00:34 
I assume you want to use a hig

#16 
Member
chris book
Join Date: Mar 2009
Posts: 85
Rep Power: 10 
I assume you want to use a highRe turbulence model which uses wallfunctions. Therefore it is necessary to choose appropriate boundary conditions (i.e. zeroGradient for k and epsilon). Please note that wall functions are only valid if the y+ of your boundary cells is in the loglaw region!
In the case of lowRe models with special nearwall modelling you have to come up with highly resolved mesh nearwall region. 

July 18, 2006, 05:46 
I am using LaunderSharma comp

#17 
Guest
Posts: n/a

I am using LaunderSharma compressible loRe model and I have made an highly resolved mesh near wall to obtain an y+ value minor than 1.


May 15, 2007, 03:53 
When I'm using a lowRe model

#18 
Member
Christian Lindbäck
Join Date: Mar 2009
Posts: 55
Rep Power: 10 
When I'm using a lowRe model (e.g. LaunderSharma) my case crashes. I can attach the error message if someone is interested. When I instead change the k value of the walls from 0 to 1e20 it runs fine. Why is this?
Secondly, in FoamX, when setting a wall to "wall" or "wallFunctions" I can see that the k condition changes (fixedValue or zeroGradient). To what file is my choice to run with or without wall function written? I.e. how is the solver being aware of my wall function choice so that it computes the velocity at the first cell according to the wall function or not? Best regards, Christian Svensson 

May 15, 2007, 04:33 
It is just an intuitive guess:

#19 
Senior Member
Dragos
Join Date: Mar 2009
Posts: 648
Rep Power: 13 
It is just an intuitive guess:
in the file /constant/turbulenceProperties set: turbulenceModel laminar; turbulence on; So if I am wrong, please correct me! Dragos 

August 1, 2008, 06:01 
Hi Foamers,
I have a questi

#20 
Member
Stefan Radl
Join Date: Mar 2009
Location: Graz, Austria
Posts: 82
Rep Power: 11 
Hi Foamers,
I have a question regarding kEpsilon turbulence model and what it does near walls (the standard wall functions are implemented). Specifically, I'm interested in the production term "G" of k at the wall. In the file wallFunctionsI.H I found (OF1.5): G[faceCelli] += (nutw[facei] + nuw[facei]) *magFaceGradU[facei] *Cmu25*sqrt(k_[faceCelli]) /(kappa_.value()*RASModel::y_[patchi][facei]); which is a little confusing, as it should be: G=tau_wall*UP/yP (UP and yP is the velocity and the wallnormal distance to the first cell respectively and tau_wall is the wall shear stress) Has anybody an explanation where the term: Cmu25*sqrt(k_[faceCelli]) /(kappa_.value()*RASModel::y_[patchi][facei]) comes from? 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Wall functions and turbulence models implementations  jposunz  OpenFOAM Running, Solving & CFD  2  October 23, 2009 04:02 
wall boundary conditions  sivaramakrishnaiah  CFX  2  August 21, 2008 10:25 
Turbulence models and boundary layer  Stanislav Kraev  FLUENT  1  March 14, 2006 06:55 
Turbulence models integrable upto the wall  vishwas  FLUENT  1  January 31, 2006 17:59 
Turbulence : kepsilon boundary conditions  Mohamed Sofiane KHELLADI  Main CFD Forum  1  April 25, 2000 20:10 