
[Sponsors] 
February 13, 2014, 21:58 
Initialize the field using another simpler turbolence model

#1 
Member
ArathoN
Join Date: Jul 2011
Posts: 86
Rep Power: 5 
hi foamers,
My friend told me that in Fluent there is an option to initialize the flow properties then run the desired the simulation. I searched for such an option on openfoam but i found nothing. So i was thinking if i use a 1ep.model like spalartallmaras to initialize the flow then i swith to my desired RAS model, Does this improve my solution? and more importantly does the solution converge faster? 

February 20, 2014, 14:51 

#2 
Member
ArathoN
Join Date: Jul 2011
Posts: 86
Rep Power: 5 
Resolved.
First before running any simulation use: Code:
refineMesh Then if you use kEpsilon, it's better to run potentialFoam to initialize the U & p fields, you need to add this in the fvsolution file Code:
potentialFlow { nNonOrthogonalCorrectors 10; } Code:
potentialFoam That's all i learned. If some one has more advice i'll gladly hear him. Last edited by ArathoN; February 21, 2014 at 10:08. Reason: fix a typo 

February 21, 2014, 05:47 

#3 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 891
Rep Power: 14 
Hi, i think this is exactly what Fluent does when using "Hybrid Initialization".
__________________
The skeleton ran out of shampoo in the shower. 

February 21, 2014, 10:07 

#4 
Member
ArathoN
Join Date: Jul 2011
Posts: 86
Rep Power: 5 
Exactly I have a friend using fluent and old me about this initialization so after some test and research i found out how to do it in openFoam. In the case of kEpsilon running potentialFoam before the main solver has little effect (at least for the cases i studied), but in case of different models (LaunderSharmaLowRe, kOmegaSST,....) the initialization with kEpsilon helps really in reducing the time needed for the convergence.


February 24, 2014, 02:41 

#5 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 891
Rep Power: 14 
Aditionally to the speedup, I also had a case that diverged with a simple constant initialization but not with the potentialFoam init.
__________________
The skeleton ran out of shampoo in the shower. 

February 27, 2014, 10:22 

#6 
Member
ArathoN
Join Date: Jul 2011
Posts: 86
Rep Power: 5 
If you use very accurate schemes, sometimes the case will diverge. It's better to start the simulation with a diffusive scheme but robust, then after some iterations switch to the accurate one. That's what i do when i need to simulate complex cases.


March 2, 2014, 21:55 

#7 
Member
Baris (Heewa)
Join Date: Jan 2013
Location: Japan
Posts: 86
Rep Power: 3 
Dear Arathon,
I also try to initialize my flow field using potentialflow before running my multiphase calculation according to your above explanation, but i couldnt succeed. in multiphase pressure dimension is kgm/s^2 however in potetialflow it is m^2/s^2. i set my cases as follows and but giving following error (is it error or not no idea). also how can i initialize the value of k and epsilon?? could you help to me pls...thanks ==>0/U Code:
dimensions [0 1 1 0 0]; internalField uniform (0 0 0); boundaryField { inlet { type fixedValue; value uniform (0 3.104 0); } outlet { type zeroGradient; } wall { type fixedValue; value uniform (0 0 0); } dimensions [0 2 2 0 0 0 0]; Code:
internalField uniform 0; boundaryField { inlet { type zeroGradient; } outlet { type fixedValue; value $internalField;; } wall { type zeroGradient; } Code:
ddtSchemes { default steadyState; } interpolationSchemes { default linear; interpolate(U) linear; } divSchemes { default none; div(phi,U) Gauss upwind; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; div(phi,nuTilda) Gauss upwind; div((nuEff*dev(T(grad(U))))) Gauss linear; } gradSchemes { default Gauss linear; grad(p) Gauss linear; grad(U) Gauss linear; } laplacianSchemes { default Gauss linear corrected; laplacian(nuEff,U) Gauss linear corrected; laplacian(1,p) Gauss linear corrected; laplacian(DkEff,k) Gauss linear corrected; laplacian(DepsilonEff,epsilon) Gauss linear corrected; laplacian(DnuTildaEff,nuTilda) Gauss linear corrected; } snGradSchemes { default corrected; } fluxRequired { default no; p ; } Code:
solvers { "(Ukomega)" { solver PBiCG; preconditioner DILU; tolerance 1e06; relTol 0; } p { solver PCG; preconditioner DIC; tolerance 1e06; relTol 0; } } potentialFlow { nNonOrthogonalCorrectors 10; } DICPCG: Solving for p, Initial residual = 1, Final residual = 8.80882e07, No Iterations 180 DICPCG: Solving for p, Initial residual = 0.168621, Final residual = 9.37342e07, No Iterations 131 DICPCG: Solving for p, Initial residual = 0.00789625, Final residual = 9.67837e07, No Iterations 115 DICPCG: Solving for p, Initial residual = 0.000384399, Final residual = 8.94174e07, No Iterations 101 DICPCG: Solving for p, Initial residual = 2.60676e05, Final residual = 8.91063e07, No Iterations 3 DICPCG: Solving for p, Initial residual = 1.92316e06, Final residual = 5.88908e07, No Iterations 1 DICPCG: Solving for p, Initial residual = 7.12976e07, Final residual = 7.12976e07, No Iterations 0 DICPCG: Solving for p, Initial residual = 7.12976e07, Final residual = 7.12976e07, No Iterations 0 DICPCG: Solving for p, Initial residual = 7.12976e07, Final residual = 7.12976e07, No Iterations 0 DICPCG: Solving for p, Initial residual = 7.12976e07, Final residual = 7.12976e07, No Iterations 0 DICPCG: Solving for p, Initial residual = 7.12976e07, Final residual = 7.12976e07, No Iterations 0 continuity error = 0.0244929 Interpolated U error = 0.000203337 ExecutionTime = 6.04 s ClockTime = 6 s 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
How to implement compressibility correction factor in kepsilon model  neeraj  OpenFOAM Programming & Development  3  October 15, 2012 00:53 
how to model a movable droplet sourse in electirc field  Chande  FLOW3D  1  March 12, 2011 17:49 
DPM model w/ Wave model  errors in documentation  HS  FLUENT  0  April 12, 2006 04:37 
just a question about airfoil (Turbolence model and Cd)  Maria Teresa Milesi  FLUENT  3  April 7, 2000 09:56 
I wish to find the proper model to validate the temperature field.  G.H.Lee  Main CFD Forum  1  May 6, 1999 02:05 