
[Sponsors] 
October 12, 2010, 20:05 
komega SST OpenFOAM 1.7

#1 
Senior Member
Join Date: Mar 2009
Posts: 225
Rep Power: 9 
Good day to everyone!
I'm having a little trouble setting up the case in OpenFOAM 1.7 using komega SST turbulence model. My question is, could anyone of you post/send a sample, simple test case with all the initial files set up for the run. Whatever I'm and was trying to do, it is not running and I'm not getting any meaningful results. Thank you very much in advance and I hope someone can help. All the best! K 

October 12, 2010, 20:07 

#2 
Senior Member
Join Date: Mar 2009
Posts: 225
Rep Power: 9 
I should have mentioned I'm planing to use interFoam for twophase flow simulation.
Thanks, K 

October 13, 2010, 02:19 

#3 
Member
Join Date: Nov 2009
Location: Germany
Posts: 96
Rep Power: 7 
Hi,
what problems exactly do you have? Have you tried the dambreak tutorial yet? It uses the kepsilon model but I think it is a good start. You can also modify this case for the komega modell. Regards, Toni 

October 13, 2010, 03:15 

#4 
Senior Member
Join Date: Mar 2009
Posts: 225
Rep Power: 9 
Hi there,
I'm well familiar with damBreak problem, I managed to run it without trouble and I'm aware and able to set up kepsilon model without trouble. I tried to repeat my results with komega SST model, however, I cannot succeed. That's why I'm asking if anyone, for example damBreak problem, could set up just a very initial state with the boundary conditions suitable to run the same case with komega SST model. I cannot succeed with my case. Thanks a lot, K 

October 13, 2010, 17:28 

#5 
Senior Member
Join Date: Mar 2009
Posts: 225
Rep Power: 9 
OK. Problem solved, I guess..
There is tutorial case using omega... incompressible/simpleFoam/motorBike. Lots of web browsing to get there. Regards, K 

October 13, 2010, 19:26 

#6 
Senior Member
Ziad Boutanios
Join Date: Mar 2009
Location: Montréal, Canada
Posts: 113
Rep Power: 8 
Is the komega model even available with the multiphase solvers? The twoPhaseEulerFoam model has its own kepsilon model and does not allow using the other RAS models as far as I know. I haven't used them all but I think the multiphase models might be like that.
The motorbike problem uses simpleFoam, a steadystate singlephase RAS model which allows loading the RAS turbulence models that come with Foam. 

October 13, 2010, 20:22 

#7 
Senior Member
Join Date: Mar 2009
Posts: 225
Rep Power: 9 
interFoam uses RASProperties library, I assume it is possible to use different turbulence models. VoF works with kepsilon, I think it should also work with komega and komega SST.
At the moment, I'm running some tests and I'm getting "some" output. Gamma field doesn't look very pretty, but it is understandable since at that point I'm using very coarse mesh and timestep and just want to see if I can run different models. Can anyone comment on that? I'm still at the learning stage of OpenFOAM, just testing its capability. Thanks, K 

October 13, 2010, 22:19 

#8 
Senior Member
Ziad Boutanios
Join Date: Mar 2009
Location: Montréal, Canada
Posts: 113
Rep Power: 8 
simpleFoam.dep has the following header files in it:
Code:
simpleFoam.dep: $(WM_PROJECT_DIR)/src/turbulenceModels/incompressible/RAS/RASModel/RASModel.H simpleFoam.dep: $(WM_PROJECT_DIR)/src/turbulenceModels/incompressible/turbulenceModel/turbulenceModel.H The multiphase models in openFOAM are mostly based on Henrik Rusche's PhD thesis and he uses the Gosman kepsilon model which is hardcoded with bubbleFoam and co. I am not even aware of any applications of komega in multiphase flow solvers yet. Of course I hope I am wrong cause I would love to use SST in multiphase. In Fluent 6 you are restricted to the various flavours of kepsilon offered (standard, RNG, realizable). Don't know how it is in 12 but I'd be very surprised if it was any different. Redefining the RAS model constants for multiphase is not a simple task and most people have only looked at kepsilon so far. 

October 13, 2010, 22:40 

#9 
Senior Member
Join Date: Mar 2009
Posts: 225
Rep Power: 9 
Ziad,
Thanks a lot for you reply. Regarding the Fluent package, I'm pretty sure you can also run twophase flow simulations using VoF using komega and komega SST models. The question is how reliable is their application. I heard many people not trusting Fluent, on the other hand it still provides "some" results. Actually, I try to compare numerical results to the experimental data. Right now I was unsuccessful getting some good measures using Fluent's kepsilon model. On the other hand komega SST gives some possibly acceptable results. Now I would like to get some results using OpenFOAM. Krystian 

October 13, 2010, 23:38 

#10 
Senior Member
Ziad Boutanios
Join Date: Mar 2009
Location: Montréal, Canada
Posts: 113
Rep Power: 8 
Right, VoF not Eulerian model! You're right VoF does allow use of komega in Fluent. Guess you don't have to redefine the constants then cause the fluids are not interpenetrating. Would be curious to see where they load the turbulence model in interFoam cause it looks very similar to bubbleFoam.
Did a quick search on VoF and komega and it seems to be give better results than kepsilon in most hits. Komega was originally developed for enclosed flows anyway and works better with boundaries. Did you try your SST testcase with Fluent or OpenFoam? 

October 14, 2010, 03:13 

#11 
Senior Member
Join Date: Mar 2009
Posts: 225
Rep Power: 9 
I don't understand something. "interFoam" solver incorporates VoF. How come otherwise would you want to solve multiphase (two phase) problem?
I'm a little bit confused. Eulerian, generally means incompressible model, right? So incompressible solver would be still called Eulerian, is it right? What you mean by Eulerian vs. VoF? Sorry, but I'm not fluids specialist, just a civil engineer Yes, I ran some tests. First using Fluent. kepsilon for some reason brings some not very good looking results. komega SST gave some more expected results. I don't care much about accurate result at that point, I just want to verify those results with OpenFOAM. Now I'm testing kepsilon with OpenFOAM. I also wanted to test komega SST for twophase flow. However, now I hear from you it is not possible to use it with interFoam solver for multiphase flows. If it is not possible, how come I am able to set up the model and define it in the OpenFOAM dictionary... and yes... I'm getting some results. Again, so far my mesh is very coarse, but the whole simulation works. Can anyone provide some input on that? 

October 14, 2010, 10:22 

#12 
Senior Member
Ziad Boutanios
Join Date: Mar 2009
Location: Montréal, Canada
Posts: 113
Rep Power: 8 
Anything more than one fluid is multiphase. VoF is a multiphase approach used when the different fluids are completely separated (immiscible) so you solve one set of equations for one fluid in the region where it flows and the other set for the other fluid where it flows. The interface cells are the only ones where you can have both fluids and this is tracked with the volume fraction alpha1 having values between 0 and 1. Everywhere else in the domain it is either 0 or 1 since you only have one of the fluids at a time.
The Eulerian solver in Fluent is a dispersed flow multiphase solver and the equivalent of bubbleFoam and twoPhaseEulerFoam. The word Eulerian refers to the formulation of the equations, in that it uses an Eulerian frame of reference which is fixed in space as opposed the Lagrangian formulation which uses a Lagrangian frame of reference which moves with the individual particle being tracked. To make things simple, the NavierStokes equations as you usually solve them in most CFD codes are in Eulerian form. Solvers like icoFoam, simpleFoam, pisoFoam etc. all use the Eulerian formulation. Actually even interFoam uses the Eulerian formulation because it does not track individual particles, and yes it is multiphase. You say you already set up interFoam with SST. Can you run just one iteration and redirect the output in a log file and post it? Just do Code:
interFoam > output.log Last edited by ziad; October 14, 2010 at 13:12. 

October 14, 2010, 16:17 

#13 
Senior Member
Join Date: Mar 2009
Posts: 225
Rep Power: 9 
I thought bubbleFoam and twoPhaseEulerFoam also use VoF (btw. what's the difference between them and interFoam? I tried to search for it, but so far I didn't find much information).
Here the code comes: Code:
kOmegaSSTCoeffs { alphaK1 0.85034; alphaK2 1; alphaOmega1 0.5; alphaOmega2 0.85616; gamma1 0.5532; gamma2 0.4403; beta1 0.075; beta2 0.0828; betaStar 0.09; a1 0.31; c1 10; } Reading g Calculating field g.h time step continuity errors : sum local = 2.73224e06, global = 2.73224e06, cumulative = 2.73224e06 DICPCG: Solving for pcorr, Initial residual = 1, Final residual = 9.39572e11, No Iterations 285 time step continuity errors : sum local = 2.56822e16, global = 1.91542e18, cumulative = 2.73224e06 Courant Number mean: 4.46994e05 max: 0.0593157 Starting time loop Courant Number mean: 4.46994e05 max: 0.0593157 Interface Courant Number mean: 0 max: 0 Time = 0.0001 MULES: Solving for alpha1 Liquid phase volume fraction = 6.8306e07 Min(alpha1) = 0 Max(alpha1) = 1 MULES: Solving for alpha1 Liquid phase volume fraction = 1.36612e06 Min(alpha1) = 0 Max(alpha1) = 1 MULES: Solving for alpha1 Liquid phase volume fraction = 2.04918e06 Min(alpha1) = 0 Max(alpha1) = 1 MULES: Solving for alpha1 Liquid phase volume fraction = 2.73222e06 Min(alpha1) = 0 Max(alpha1) = 1 DICPCG: Solving for p_rgh, Initial residual = 1, Final residual = 0.0487633, No Iterations 93 time step continuity errors : sum local = 1.33644e07, global = 1.24748e08, cumulative = 2.74472e06 DICPCG: Solving for p_rgh, Initial residual = 0.0264555, Final residual = 0.00130094, No Iterations 68 time step continuity errors : sum local = 1.06971e07, global = 8.80192e09, cumulative = 2.73591e06 DICPCG: Solving for p_rgh, Initial residual = 0.00530873, Final residual = 9.45304e08, No Iterations 185 time step continuity errors : sum local = 5.89045e12, global = 1.4112e13, cumulative = 2.73591e06 DILUPBiCG: Solving for omega, Initial residual = 1, Final residual = 1.34868e10, No Iterations 5 DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 1.37486e09, No Iterations 5 ExecutionTime = 2.98 s ClockTime = 3 s 

October 15, 2010, 09:12 

#14  
Senior Member
Ziad Boutanios
Join Date: Mar 2009
Location: Montréal, Canada
Posts: 113
Rep Power: 8 
Quote:
The inter*Foam family of multiphase solvers relies instead on a onefluid mixture formulation and solves only only one set of NS equations with a variable alpha. This is probably why it is possible to use komega with them since you are still solving for one fluid, the mixture. The interface is tracked based on alpha with the additional VoF equation. Not sure about the rest of the multiphase solvers. 

October 15, 2010, 09:35 

#15 
Senior Member
Join Date: Mar 2009
Posts: 225
Rep Power: 9 
Yeah, that's what it seems for me.
So bubbleFoam seems like it is EulerEuler type equation. Hmm... It's not what I need, I don't really care about bubble dispersion etc. Now I remember my past reading, VoF should make a trick. Coming back to interFoam, that's what it seems. I don't feel confident saying what interFoam does exactly, but as much as I learned and I can see, I think, any of the turbulence models should work with it, since all is coupled through VoF, which is kind of a weighting function. Anyways, thanks for your time and reply. 

October 15, 2010, 09:46 

#16 
Senior Member
Ziad Boutanios
Join Date: Mar 2009
Location: Montréal, Canada
Posts: 113
Rep Power: 8 
Actually they are all Eulerian formulations. They just treat the additional fluid differently. I usually use twoPhaseEulerFoam but soon I will need to compute film formation and this will require interFoam.
Enjoy! 

October 15, 2010, 15:29 

#17 
Senior Member
Join Date: Mar 2009
Posts: 225
Rep Power: 9 
Yes, yes, in Eulerian frame.
Film? Can you elaborate more about it? I would gladly hear why for that kind of case you would need interFoam and not twoPhase... solver. Thx! K 

October 23, 2010, 14:10 

#18  
Senior Member
Ziad Boutanios
Join Date: Mar 2009
Location: Montréal, Canada
Posts: 113
Rep Power: 8 
Quote:
Sorry for the late reply. I use twoPhaseEulerFoam to compute dispersed flows of solid particles in air and interFoam for a fully segregated film transport on pipe walls. Cheers, Ziad 

June 12, 2014, 09:01 
kwsst model

#19 
New Member
Lamia
Join Date: Feb 2013
Posts: 18
Rep Power: 4 
hello everybody
I am having a problem with boundary conditions of the model KW SST for turbulent Intensity KineticEnergy Inlet "k" = 0.05 or 5% and velocity U reference = 4.15, and Y reference 0.35 mm so what would be the value of Omega? please I need help I dont know what to put in: internalField uniform ?? and value uniform?? heeeeeelp 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
OpenFOAM 1.7 installation on Redhat linux  maxims  OpenFOAM Installation  2  November 30, 2012 05:29 
OpenFOAM 1.6 and 1.7 with interFoam, groovyBC give different strange results  Arnoldinho  OpenFOAM  7  December 9, 2010 17:29 
Crosscompiling OpenFOAM 1.7.0 on Linux for Windows 32 and 64bits with Mingww64  wyldckat  OpenFOAM Announcements from Other Sources  3  September 8, 2010 06:25 
k Omega SST SAS for OpenFOAM 1.5???  barath.ezhilan  OpenFOAM Running, Solving & CFD  3  June 2, 2010 07:41 
Wall function implementation K Omega SSt  cbarry  OpenFOAM  3  August 18, 2009 10:09 