# Attempt to understand icoFoam transientSimpleFoam on cavity testcase

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

 April 28, 2008, 09:06 Dear All Greetings. Conc #1 Senior Member   Join Date: Mar 2009 Posts: 248 Rep Power: 11 Dear All Greetings. Conceptually both SIMPLE and PISO formulations can be used to solve problems of transient nature. In the list of OpenFOAM solvers --> icoFoam is the transient solver for incompressible, laminar flow of Newtonian fluids. --> transientSimpleFoam is the transient solver for incompressible, turbulent flow of on-Newtonian fluids. In principle if one modifies the transientSimpleFoam solver by removing the turbulence calculation part then the two solvers should deliver the same result. As far my as understanding goes the transientSimpleFoam shall take more time to converge as it uses under-relaxation. The original icoFoam solver in its unmodified form is: int main(int argc, char *argv[]) { # include "setRootCase.H" # include "createTime.H" # include "createMesh.H" # include "createFields.H" # include "initContinuityErrs.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Info<< "\nStarting time loop\n" << endl; for (runTime++; !runTime.end(); runTime++) { Info<< "Time = " << runTime.timeName() << nl << endl; # include "readPISOControls.H" # include "CourantNo.H" fvVectorMatrix UEqn ( fvm::ddt(U) + fvm::div(phi, U) - fvm::laplacian(nu, U) ); solve(UEqn == -fvc::grad(p)); // --- PISO loop for (int corr=0; corr UEqn ( fvm::ddt(U) + fvm::div(phi, U) + fvm::laplacian(nu, U) ); UEqn().relax(); solve(UEqn() == -fvc::grad(p)); p.boundaryField().updateCoeffs(); volScalarField rUA = 1.0/UEqn().A(); U = rUA*UEqn().H(); UEqn.clear(); phi = fvc::interpolate(U) & mesh.Sf(); adjustPhi(phi, U, p); // Store pressure for under-relaxation p.storePrevIter(); // Non-orthogonal pressure corrector loop for (int nonOrth=0; nonOrth<=nNonOrthCorr; nonOrth++) { fvScalarMatrix pEqn ( fvm::laplacian(rUA, p) == fvc::div(phi) ); pEqn.setReference(pRefCell, pRefValue); pEqn.solve(); if (nonOrth == nNonOrthCorr) { phi -= pEqn.flux(); } } # include "continuityErrs.H" // Explicitly relax pressure for momentum corrector p.relax(); // Momentum corrector U -= rUA*fvc::grad(p); U.correctBoundaryConditions(); } runTime.write(); Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s\n\n" << endl; } Info<< "End\n" << endl; return(0); } I ran both solvers on the cavity with same settings in the controlDict, fvSchemes, fvSolution. the fvSolution has the subDict settings for both algorithms: PISO { nCorrectors 2; nNonOrthogonalCorrectors 0; pRefCell 0; pRefValue 0; } // Relaxation factors are used for transient SIMPLE relaxationFactors { p 0.5; U 0.8; } The results I get are completely different. I am posting here the pressure and velocity fields at t=0.5 for both solvers. IcoFoam results (all the settings are standard by which I mean the settings given in the UserGuide for the lid driven cavity tutorial) transientSimpleFoam results Note the difference in the direction of velocity vectors The difference in the results could be due to several reason. All I am trying here is to understand how to tune these two solvers which are solving the same physics but using different pressure-velocity coupling. Any inputs will be helpful With best regards Jaswi

 April 28, 2008, 10:47 Hi Jaswi Looking at the low #2 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,740 Rep Power: 29 Hi Jaswi Looking at the lowermost plot, which I suspect is the velocity field, I cannot see any boundary, where the velocity is not zero!?! Thus could it be that you have forgotten to set the boundary condition on U? Best regards, Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

 April 28, 2008, 19:04 Hi Niels Thank for the comm #3 Senior Member   Join Date: Mar 2009 Posts: 248 Rep Power: 11 Hi Niels Thank for the comment. Please take a notice of the comments in the post. I have mentioned above that the first two pictures, i.e. pressure and velocity plots are for the led driven cavity using icoFOAM Now icoFoam uses PISO pressure-velocity coupling algorithm. There is also another solver called transientSimpleFoam which uses the SIMPLE pressure-velocity coupling algorithm . The last two picture are pressure and velocity for the same led driven cavity but now using the modifeid transientSimpleFoam given above in the post. I again emphasize on the fact that the two solvers differing only in their pressure-velocity coupling algorithm were run on the same case i.e. lid driven cavity. Hope that clears the doubt. I am waiting eagerly for the comments :-) With Regards Jaswi

 April 29, 2008, 04:37 Any reason you're adding and n #4 Super Moderator   Mattijs Janssens Join Date: Mar 2009 Posts: 1,416 Rep Power: 18 Any reason you're adding and not subtracting the viscous contribution in your UEqn? + fvm::laplacian(nu, U)

 April 29, 2008, 05:40 Hi Mattijs Thanks a lot for #5 Senior Member   Join Date: Mar 2009 Posts: 248 Rep Power: 11 Hi Mattijs Thanks a lot for pointing out that mistake. I am really sorry for not cross checking my stuff and creating unnecessary trouble. With that correction , both SIMPLE and PISO deliver identical results , at first glance at least. I am thankful to you for help. If possible please point me to necessary routines on how I can compare the error for the two solvers and make a quantitative analysis. Just some pointers. In that way I can do the quantitative analysis for these two pres-velocity algorithms solving the same physical model and put the results on Wiki. It might be useful to somebody trying to understand the solution approach With Best Regards Jaswi

 April 29, 2008, 05:41 Hi Nice spotting Mattjis... #6 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,740 Rep Power: 29 Hi Nice spotting Mattjis... That could easily explain the lowermost picture, because the change in sign makes the diffusion term into an energy source. Thus if you put on a scale bar, you will probably experience that the maximum velocities in your transientSimpleFoam case is significantly larger than the lid velocity. - Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

 July 10, 2009, 05:01 #7 Member   Bernard Esterhuyse Join Date: Mar 2009 Location: Pretoria, South Africa Posts: 50 Rep Power: 10 Hi I'm looking for the transientSimpleFoam solver, but I cannot find it in the 1.5 distribution. Is there another location for it? Thanks

 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 unoder OpenFOAM Running, Solving & CFD 7 September 20, 2016 05:47 manuel OpenFOAM Running, Solving & CFD 8 September 22, 2010 04:10 skabilan OpenFOAM Running, Solving & CFD 2 June 4, 2008 20:39 Araz Main CFD Forum 0 August 5, 2004 08:36 Aldo Bonfiglioli Main CFD Forum 0 September 11, 1998 09:02

All times are GMT -4. The time now is 12:01.