[thiagopl]

Hi,

I'm using the chtMultiRegionSimpleFoam to simulate the problem of a enclosure vertically heated and cooled with an internal solid.
As I show bellow, even after all the convergence criteria is achieved (10^-6) the Simple algorithm doesn't stop.
I can't see the rho residuals, but I've changed it to 10^-3 and the results are the same. Why doesn't it stop?

Log showing all the residuals bellow the criteria convergence:

Time = 2216

Solving for fluid region air
DILUPBiCG:  Solving for Ux, Initial residual = 4.163122729918927e-09, Final residual = 4.163122729918927e-09, No Iterations 0
DILUPBiCG:  Solving for Uy, Initial residual = 4.59032787455036e-09, Final residual = 4.59032787455036e-09, No Iterations 0
DILUPBiCG:  Solving for h, Initial residual = 9.416101596905256e-07, Final residual = 9.416101596905256e-07, No Iterations 0
Min/max T:300 310
DICPCG:  Solving for p_rgh, Initial residual = 9.343214257414049e-07, Final residual = 9.343214257414049e-07, No Iterations 0
time step continuity errors : sum local = 2.758594777251156e-07, global = -1.499279134027018e-17, cumulative = 1.340309069704447e-15
Min/max rho:1.123451097280091 1.160905661033402

Solving for solid region body
DICPCG:  Solving for h, Initial residual = 8.686132203851212e-07, Final residual = 8.686132203851212e-07, No Iterations 0
Min/max T:min(T) [0 0 0 1 0 0 0] 303.7710276494997 max(T) [0 0 0 1 0 0 0] 306.1953321209988
ExecutionTime = 75.23 s  ClockTime = 75 s

Here is the fvSoltuion for the air region:

solvers
{
    rho
    {
       solver          PCG
       preconditioner  DIC;
       tolerance       1e-4;
       relTol          0.1;
    }

    p_rgh
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-6;
        relTol          0.1; //0.01
    }

    "(U|h|k|epsilon)"
    {
        solver           PBiCG;
        preconditioner   DILU;
        tolerance        1e-6;
        relTol           0; //0.1
    }
}

SIMPLE
{
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       1e5;
    rhoMin          rhoMin [1 -3 0 0 0] 0.2;
    rhoMax          rhoMax [1 -3 0 0 0] 2;

    residualControl
    {
    	p_rgh           1e-6;
    	U               1e-6;
    	h               1e-6;
	rho		1e-4;
    }
}

Here is the fvSoltuion for the solid region:

solvers
{
    h
    {
        solver           PCG;
        preconditioner   DIC;
        tolerance        1e-06;
        relTol           0;	//0.1
    }
}
SIMPLE
{
    nNonOrthogonalCorrectors 0;

    residualControl
    {
       h               1e-6;
   }
}
relaxationFactors
{
    fields
    {
    }
    equations
    {
        h               1;
    }
}

[alexeym]

Hi,

If you check source code of the solver, it does not check for convergence. runTime.loop() (loop method of Time class) just checks if time reached endTime.

    while (runTime.loop())
    {
        Info<< "Time = " << runTime.timeName() << nl << endl;

        forAll(fluidRegions, i)
        {
            Info<< "\nSolving for fluid region "
                << fluidRegions[i].name() << endl;
            #include "setRegionFluidFields.H"
            #include "readFluidMultiRegionSIMPLEControls.H"
            #include "solveFluid.H"
        }

        forAll(solidRegions, i)
        {
            Info<< "\nSolving for solid region "
                << solidRegions[i].name() << endl;
            #include "setRegionSolidFields.H"
            #include "readSolidMultiRegionSIMPLEControls.H"
            #include "solveSolid.H"
        }

        runTime.write();

        Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
            << "  ClockTime = " << runTime.elapsedClockTime() << " s"
            << nl << endl;
    }

[thiagopl]

Hmm... so it was a dumb question.
I believe that there is a way to modify it, but I still can't read the codes of the solvers.

Thank you.

PS: Why not check for convergence?

[alexeym]

Well, it was correct question though it was not a question about OpenFOAM but a question of OpenFOAM's consistency. It is quite obvious that user expects similar behavior from SIMPLE family of solvers.

And, in fact, modification of the solver would be rather simple.

Unfortunately simpleControl has only loop public method that does a little bit more than just checking convergence. And there is criteriaSatisfied method which is protected but does just what is necessary to check convergence. So you can create myOwnSimpleControl class, which is simpleControl child. In this class you create public converged method. It just returns result criteriaSatisfied method.

Then in addition to creation of the meshes for all regions you create myOwnSimpleControl objects for every mesh. Finally you create boolean allRegionsConverged and check convergence of the regions in forAll loops.