# Turbulence models and wall boundary conditions

 Register Blogs Members List Search Today's Posts Mark Forums Read

 February 14, 2005, 05:49 Dear all, Which kind of bo #1 Daniele Panara (Panara) Guest   Posts: n/a Sponsored Links Dear all, Which kind of boundary conditions should I apply for k and epsilon at the wall when I am using a low Re k-epsilon model? The same as the high renolds number model? zerogradient?

 February 14, 2005, 05:51 fixedValue of 0 for k and zer #2 Henry Weller (Henry) 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 Kaushik Balakrishnan (Balakrishnan) 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 Henry Weller (Henry) Guest   Posts: n/a A zeroGradient inlet condition is effectively an upstream extrapolation from inside the domain and is therfore unstable for a convection-dominated property.

 February 16, 2005, 03:55 From my experience (although #5 Fabian Peng Kärrholm (Kärrholm) Guest   Posts: n/a From my experience (although short) from spray calculations in Foam using the Launder Sharma k-epsilon 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 Hrvoje Jasak (Hjasak) 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 Boussinesq-Approximation, where k is used to avoid a traceless stress tensor: nt(¶ui/¶xj+¶uj/¶xi)-2/3kdij. 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 2/3kdij 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 pressure-gradient 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: 1,802 Rep Power: 24 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 cross-coupling 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: 1,802 Rep Power: 24 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 diego_n 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 Launder-Sharma 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 high-Re turbulence model which uses wall-functions. 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 log-law region! In the case of low-Re models with special near-wall modelling you have to come up with highly resolved mesh near-wall region.

 July 18, 2006, 05:46 I am using Launder-Sharma comp #17 diego_n Guest   Posts: n/a I am using Launder-Sharma compressible lo-Re 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 low-Re model #18 Member   Christian Lindbäck Join Date: Mar 2009 Posts: 55 Rep Power: 10 When I'm using a low-Re 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 1e-20 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: 649 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 (OF-1.5): 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 wall-normal 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 Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post jposunz OpenFOAM Running, Solving & CFD 2 October 23, 2009 04:02 sivaramakrishnaiah CFX 2 August 21, 2008 10:25 Stanislav Kraev FLUENT 1 March 14, 2006 06:55 vishwas FLUENT 1 January 31, 2006 17:59 Mohamed Sofiane KHELLADI Main CFD Forum 1 April 25, 2000 20:10