
[Sponsors] 
May 7, 2013, 07:22 
convergence of QUICK scheme  simpleFoam

#1 
New Member
Luis Batista
Join Date: Mar 2013
Location: Lisboa / Setúbal
Posts: 17
Rep Power: 6 
Hello,
I am using SimpleFoam for a Laminar cavity flow model. I am doing a grid refinement study and to improve my convergence, I want to use a higher order convection scheme QUICK. The plotted residuals are not looking very nice and after I have changed the relaxation parameters, it seems that this is not being sensitive to my changes. I here post my controlDict; fvSchemes and fvSolution and send plot the residuals in attachment. Please help! controlDict: /** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.2.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object controlDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // application simpleFoam; startFrom latestTime; startTime 0; stopAt endTime; endTime 1000; deltaT 1; writeControl timeStep; writeInterval 50; purgeWrite 1; writeFormat ascii; writePrecision 12; writeCompression off; timeFormat general; timePrecision 6; runTimeModifiable true; } // ************************************************** *********************** // fvSchemes: /** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.2.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; grad(p) Gauss linear; grad(U) Gauss linear; } divSchemes { default none; div(phi,U) bounded Gauss QUICK; div(phi,k) bounded Gauss upwind; div(phi,epsilon) bounded Gauss upwind; div(phi,R) bounded Gauss upwind; div(R) Gauss linear; div(phi,nuTilda) bounded Gauss upwind; div((nuEff*dev(T(grad(U))))) Gauss linear; } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear corrected; laplacian((1A(U)),p) Gauss linear corrected; laplacian(DkEff,k) Gauss linear corrected; laplacian(DepsilonEff,epsilon) Gauss linear corrected; laplacian(DREff,R) Gauss linear corrected; laplacian(DnuTildaEff,nuTilda) Gauss linear corrected; } interpolationSchemes { default linear; interpolate(U) linear; } snGradSchemes { default corrected; } fluxRequired { default no; p ; } // ************************************************** *********************** // fvSolution: /** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.2.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { p { solver PCG; preconditioner DIC; tolerance 1e6; relTol 0.01; } U { solver PBiCG; preconditioner DILU; tolerance 1e5; relTol 0.1; } } SIMPLE { nNonOrthogonalCorrectors 0; pRefCell 0; pRefValue 0; residualControl { p 1e2; U 1e3; } } relaxationFactors { fields { p 0.3; } equations { U 0.7; } } // ************************************************** *********************** // Regards, Luis Batista 

May 7, 2013, 08:30 

#2  
Senior Member

Quote:
It seems, your pressure is not converging after some time iterations. Well, for your particular problem case why don't you go for icoFoam (laminar). simpleFoam is Steadystate solver for incompressible, turbulent flow. As for the files are concerned it seems all OK to me. I think you are using the already available case files with OF. 

May 7, 2013, 08:59 

#3  
New Member
Luis Batista
Join Date: Mar 2013
Location: Lisboa / Setúbal
Posts: 17
Rep Power: 6 
Quote:
thanks for your support. I share the same impression as you, that it, the pressure is not converging (and the velocities are also not converging monotonically). About IcoFoam: I am using SimpleFoam since from my previous experience with IcoFoam, I have not managed to use underrelaxation factors for p and U. I have tried to use them previously and the solution was not reacting at all. I concluded that the convergence cannot be controled in IcoFoam thry this. (please correct me if I am wrong). From my POV, icoFoam is meant to produce a timeaccurate solution and the only way to control the algorithm convergence is by the local linear system residual (there is no outer loop convergence criteria). (correct me if I am wrong). Additionally, I also inform that the convergence problem herefound was also happening in Icofoam. About simpleFoam: With respect to the problem here reported, it seems that the QUICK scheme is always trying to solve the algorithm for a source term (maybe coming from deferration´from previous time step)...I don´t know. Did I add any further information that you find helpful to understand my problem? thanks, Luis 

May 8, 2013, 01:48 

#4  
Senior Member

Quote:
You are correct, about both the IcoFoam & SimpleFoam solvers. Since, you are using QUICK scheme then why don't you check with coarse mesh first, as the convergence depends on source term (deffered correction). If you are successful then try with fine mesh. I would suggest you to try with different solver, may be it will be beneficial in getting convergence. 

May 8, 2013, 02:39 

#5 
Senior Member
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 237
Rep Power: 10 
Why don't you use a linearUpwind Scheme ? It's the second order of the upwind scheme You can also use the linearUpwindV that is the pure upwind scheme of linearUpwind (the difference is in the "V" at the end).
div(phi,U) bounded Gauss upwind; becomes div(phi,U) Gauss linearUpwind grad(U); You can also put all your other scheme to second order. Be careful, the gradient term must have the corresponding variable (= the second variable in the div() that correspond to the one solved). So div(phi,k) bounded Gauss upwind; becomes div(phi,k) Gauss linearUpwind grad(k); 

May 8, 2013, 04:55 

#6  
New Member
Luis Batista
Join Date: Mar 2013
Location: Lisboa / Setúbal
Posts: 17
Rep Power: 6 
Quote:
I have tried this scheme up to grid refinement ratios of 4, that is, from 50x50 up to 400x400. It is the same problem.... I believe I am going to try a different scheme for now, p.e., Linear Upwind and leave this issue for when I understand better how the deferred correction is working for QUICK scheme. If you now where I can find this type of information please let me know. Best Regards, Luis 

May 8, 2013, 05:08 

#7  
New Member
Luis Batista
Join Date: Mar 2013
Location: Lisboa / Setúbal
Posts: 17
Rep Power: 6 
Quote:
However, I have not implemented exactly as you wrote, let me recapitulate what I believe I now in order that you can give me a further push div(phi,U)  means the discretization of the convection term where phi is denominates as flux of the dependent variable U thru velocitycell faces and U is the dependent variable (unknown). so, I do no understand why you mention: " div(phi, U) Gauss linearUpwind grad(U); " 1) Isn´t it enough to write? " div(phi, U) Gauss linearUpwind " 

May 8, 2013, 05:16 

#8 
Senior Member
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 237
Rep Power: 10 
no it's not enough because the linearUpwind needs to know what is the direction of your "flow" or variable your study. The linearUpwind only consider the flow from where it comes and not from where it goes. Therefor you need to tell the scheme in which direction he needs to make the computation.
Originally you could write: "div(phi, U) Gauss linearUpwind phi" where phi tells the direction of the flow. But with the new versions of OpenFoam, people got use to write the gradient of the variable, which is the same as giving phi (the flux at the face). I'm not sure if the solver accept "div(phi, U) Gauss linearUpwind". Maybe the scheme takes a default value defined as "phi". However, this is only true for the velocity scheme. For the other, you need to specify the corresponding flux (by using the gradient). 

May 8, 2013, 05:28 

#9  
New Member
Luis Batista
Join Date: Mar 2013
Location: Lisboa / Setúbal
Posts: 17
Rep Power: 6 
Quote:


May 11, 2013, 17:35 

#11  
New Member
Luis Batista
Join Date: Mar 2013
Location: Lisboa / Setúbal
Posts: 17
Rep Power: 6 
Quote:
I am having success with LinearUpwind, however, I was expecting a better order of convergence... Anyhow, I will try to run tests and see what are the variables that I must use to have convergence with QUICK. Regards, Luis 

Tags 
simplefoam;quick 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
QUICK scheme paper by T. Hayase 1992  bouloumag  Main CFD Forum  1  July 7, 2011 15:07 
Implementation of QUICK scheme  Romuald Skoda  Main CFD Forum  10  August 3, 2010 12:23 
2nd order boundary condition for QUICK scheme  Jafarnia  Main CFD Forum  0  February 25, 2004 10:03 
Quick Scheme  Mikel A.  Main CFD Forum  2  February 23, 2004 13:58 
Quick Scheme  Ahmad Falahat Pisheh  Main CFD Forum  0  January 10, 2004 12:38 