[kaszt]

I recently installed OpenFOAM-v1706 released from ESI, and I am having trouble running a test case that I had previously ran without problems when I was using OpenFOAM version 3.0.1.

I discovered this problem when using the pimpleFoam solver in solving for incompressible, laminar flow over a 2D cylinder. I used the same setup as I had previously used in OpenFOAM 3.0.1., but when I ran the case using OpenFOAM-v1706, the pressure and velocity do not converge and there is very strange behavior in the residuals as compared to the working case ran with my previous build of OpenFOAM 3.0.1.

The picture I attached are the residuals I have from running the case using pimpleFoam for 0.1 simulation seconds. To me, there is weird behavior in everything here - they do not behavior like I expect from using pimpleFoam (like the final graph shown here).

My fvSolution file is as follows:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    p                                  
    {
        solver          GAMG;           
        tolerance       1e-04;          
        relTol          0.01;  
        smoother        DICGaussSeidel;        
    }
    
    pFinal
    {
        solver          GAMG;
        tolerance       1e-04;
        relTol          0.0;
        smoother        DICGaussSeidel; 
    }

    U
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-4; 
        relTol          0.01; 
    }
    
    UFinal
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-04; 
        relTol          0.0;
    }
}

PIMPLE 
{
    nNonOrthogonalCorrectors 0;
    nCorrectors     1;  
    nOuterCorrectors 50;    
    
    //pRefCell        0; 
    //pRefValue       0;
    
    residualControl 
    {
        U
        {
            tolerance   1e-4;
            relTol      0.0;
        }
        p
        {
            tolerance   1e-4;
            relTol      0.0;
        }
    }
}

relaxationFactors // 0 < relaxationFactors <= 1
{
    fields
    {
        p       0.3; 
        pFinal  1;
    }
    equations
    {
        U       0.3; 
        UFinal  1;    
    }
}



// ************************************************************************* //

and my controlDict file is as follows:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     pimpleFoam;

startFrom       startTime;

startTime       0;

stopAt          endTime;

endTime         1; 

deltaT          0.01; 

writeControl   	runTime;

writeInterval   1;

purgeWrite      0;

writeFormat     ascii;

writePrecision  8; 

writeCompression off;

timeFormat      general;

timePrecision   6;

runTimeModifiable true;

adjustTimeStep  yes;

maxCo           5;

functions
{
    forces
    {
        type        forces;
        functionObjectLibs  ("libforces.so");
        writeControl   runTime;
        writeInterval  1;
        patches     (fixedWalls);
        
        pName       p;
        UName       U;
        
	rho         rhoInf;
	rhoInf      1;
        log         true;
        CofR        (0 0 0); // origin for moment calculation
        
        writeFields yes;
        
        binData
        {
            nBin    90; //output data into 20 bins
            direction   (1 0 0); // bin direction
            format  gnuplot;
            cumulative  yes;
        }
    }


    forceCoefficients
    {
        type        forceCoeffs;
        functionObjectLibs  ("libforces.so");
        writeControl   runTime;
        writeInterval  1;
        patches     (fixedWalls);
        
        writeFields yes;
        
        log         true;
        patches     (fixedWalls); // on cyl only
        pName       p;
        UName       U;
        dragDir     (1 0 0);
        liftDir     (0 1 0);
        pitchAxis   (0 0 1);
        CofR        (0 0 0);
        magUInf     10; // free stream velocity
        lRef        1;
        Aref        0.79; // cross sectional area
    
	rho         rhoInf;
	rhoInf      1;
        origin      (0 0 0);
    
        coordinateRotation
        {
            type        EulerRotation
            degrees     true;
            rotation    (0 0 0);
        }
        
        binData
        {
            nBin    90; //output data into 20 bins
            direction   (1 0 0); // bin direction
            format  gnuplot;
            cumulative  yes;
        }
    }
}
// ************************************************************************* //

And for anyone curious, here is where you can download the case I am talking about.

I'd like to ask if anyone has ran into similar problems with using pimpleFoam and OpenFOAM-v1706, or if there is anything that I am just missing that is included in the new release. I know that the residual behavior of this test case is strange, and I would appreciate any and all tips for uncovering what the problem is!

[kaszt]

Sorry to answer my own question here but after some more debugging I found the source of my problem; using pure Crank Nicolson for the time derivatives was causing the blow-up in pressure residuals after the first time step. I switched to a backward scheme and I am much happier with the use of pimpleFoam - it behaves in a way that I understand