# buoyantBoussinesqSimpleFoam and kappat

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

 November 16, 2011, 05:28 buoyantBoussinesqSimpleFoam and kappat #1 Senior Member   Join Date: Mar 2009 Posts: 138 Rep Power: 10 HI OF Users, I am simulating the flow over a hot board. I have done various Simulations with rhoSimpleFoam and buoyantSimpleFoam. Now I want to start a Simulation with the solver buoyantBoussinesqSimpleFoam. For that I have to specify the kappat, the 'kinematic turbulent thermal conductivity'. But I can´t find any information of how to calculate the initial values and which BC to set. Is there any Information for that? Thanks __________________ OF - 2.0.0

 November 16, 2011, 08:27 #2 New Member   Alex Join Date: Apr 2011 Location: München Posts: 13 Rep Power: 8 Hello camoesas, I found the following definition for the turbulent heat conductivity. It is the product of the heat capacity and the turbulent kinematic viscosity of your considered fluid. I found that in the following book (you can find it in google books): Innovative Food Processing Technologies: Advances in Multiphysics Simulation( Kai Knoerzer,Pablo Juliano,Peter Roupas). But I think you don't need to specify it exactly. For the walls you have a wall function and for the "Inlet" you can use the "calculated" boundary conditon. For the "Outlet" it is zeroGradient. I hope this helps. Best regards

November 16, 2011, 10:40
#3
Senior Member

Join Date: Mar 2009
Posts: 138
Rep Power: 10
HI Alex,

Thanks for the hint. I have now for kappat:

Inlet: calculated,
All Walls: kappatJayatillekeWallFunction;
and some empty and symmetry patches.

But my solition is aborting in the first iteration giving me this message:

Quote:
 Create time Create mesh for time = 0 Reading g Reading thermophysical properties Reading field T Reading field p_rgh Reading field U Reading/calculating face flux field phi Selecting incompressible transport model Newtonian Creating turbulence model Selecting RAS turbulence model kOmegaSST 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 field kappat Calculating field g.h SIMPLE: convergence criteria field p_rgh tolerance 1e-05 field U tolerance 1e-06 field h tolerance 1e-06 field "(k|epsilon|omega)" tolerance 1e-06 Starting time loop Time = 1 DILUPBiCG: Solving for Ux, Initial residual = 0.0002433629501, Final residual = 1.756349447e-07, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.002939968679, Final residual = 2.378267403e-06, No Iterations 1 DILUPBiCG: Solving for T, Initial residual = 1, Final residual = 0.03016392268, No Iterations 1 --> FOAM FATAL ERROR: request for volScalarField rho from objectRegistry region0 failed available objects of type volScalarField are 14 ( div(phi) rhok nut rAU k p_rgh nu gh p T omega p_rghPrevIter y kappat ) From function objectRegistry::lookupObject(const word&) const in file /home/camoesas/OpenFOAM/OpenFOAM-2.0.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 131. FOAM aborting #0 Foam::error:rintStack(Foam::Ostream&) in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::error::abort() in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 Foam::GeometricField const& Foam:bjectRegistry::lookupObject >(Foam::word const&) const in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so" #3 Foam::buoyantPressureFvPatchScalarField::updateCoe ffs() in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so" #4 Foam::fvMatrix::fvMatrix(Foam::GeometricFi eld const&, Foam::dimensionSet const&) in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/bin/buoyantBoussinesqSimpleFoam" #5 Foam::fv::gaussLaplacianScheme::fvmLaplacianUncorrected(Foam::GeometricFi eld const&, Foam::GeometricField const&) in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so" #6 Foam::fv::gaussLaplacianScheme::fvmLaplacian(Foam::GeometricField const&, Foam::GeometricField const&) in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so" #7 in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/bin/buoyantBoussinesqSimpleFoam" #8 in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/bin/buoyantBoussinesqSimpleFoam" #9 in "/home/camoesas/OpenFOAM/OpenFOAM-2.0.0/platforms/linux64GccDPOpt/bin/buoyantBoussinesqSimpleFoam" #10 __libc_start_main in "/lib64/libc.so.6" #11 at /usr/src/packages/BUILD/glibc-2.11.3/csu/../sysdeps/x86_64/elf/start.S:116
What does this mean? Is this an error of my BC or of the numerical setup?
Thanks for any hints

I have uploaded the whole case but I had to delete U p files. I have adopted them for initialization from another simulation so they are to large...
Attached Files
 setup_buoyantBoussinesqSimpleFoam.zip (40.0 KB, 192 views)
__________________
OF - 2.0.0

 November 16, 2011, 13:24 #4 New Member   Alex Join Date: Apr 2011 Location: München Posts: 13 Rep Power: 8 You have to define a reference for the density for the buoyantpressure boundary conditions. ... HOT { type buoyantPressure; rho rhok; value \$internalField; } ... By the way, for the inlet it is better to define the pressure as zerogradient. Otherwise your problem is overdetermined. I hope this will fix the problem. Good luck for your simulation! Regards, Alex camoesas, blake, klio and 1 others like this.

 November 17, 2011, 09:18 #5 Senior Member   Join Date: Mar 2009 Posts: 138 Rep Power: 10 HI Alex, thank you very much for going throw my case! And for this valuable solution. Indeed it fixed my simulation. But my pressure inlet is already zeroGradient. Do you mean the inlet for p_rgh? __________________ OF - 2.0.0

February 26, 2014, 08:39
Les
#6
Member

Peter
Join Date: Nov 2011
Posts: 46
Rep Power: 7
Quote:
 Originally Posted by al_pr Hello camoesas, I found the following definition for the turbulent heat conductivity. It is the product of the heat capacity and the turbulent kinematic viscosity of your considered fluid. I found that in the following book (you can find it in google books): Innovative Food Processing Technologies: Advances in Multiphysics Simulation( Kai Knoerzer,Pablo Juliano,Peter Roupas). But I think you don't need to specify it exactly. For the walls you have a wall function and for the "Inlet" you can use the "calculated" boundary conditon. For the "Outlet" it is zeroGradient. I hope this helps. Best regards
Hi, Alex!

What about LES? Is it still the same way to set up boundary condition for kappat as you said? Or should I do it the way as nuSgs in tutorial cases, that is, to set all boundaries zeroGradient?

Best regards
Peter

 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 makaveli_lcf OpenFOAM Running, Solving & CFD 21 February 28, 2014 03:50 jignesh_thaker2007 OpenFOAM 0 October 2, 2011 05:45 maysmech OpenFOAM 5 February 11, 2011 05:41 cbritan OpenFOAM 1 December 12, 2010 22:57

All times are GMT -4. The time now is 19:00.