CFD Online Discussion Forums - Error when I try a case with pimple instead of simple solver

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM (https://www.cfd-online.com/Forums/openfoam/)

- - Error when I try a case with pimple instead of simple solver (https://www.cfd-online.com/Forums/openfoam/118796-error-when-i-try-case-pimple-instead-simple-solver.html)

Error when I try a case with pimple instead of simple solver

Dear All,

I have a problem with a transient simulation. Actually, I do have a case with a steady solution and I have calculated it.
I am now trying to calculate the same solution as the limit of the unsteady counterpart.

But as soos as I run

Code:

buoyanPimpleFoam

instead of

Code:

buoyanSimpleFoam

I get this error message:

Code:

lab@lab-laptop:~/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/NOPCM/pseudoTransient$ buoyantPimpleFoam

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2.1.0                                 |

|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

Build  : 2.1.0-0bc225064152

Exec   : buoyantPimpleFoam

Date   : Jun 04 2013

Time   : 16:30:09

Host   : "lab-laptop"

PID    : 4178

Case   : /home/lab/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/NOPCM/pseudoTransient

nProcs : 1

sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

fileModificationChecking : Monitoring run-time modified files using timeStampMaster

allowSystemOperations : Disallowing user-supplied system call operations



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

Create time



Create mesh for time = 0





Reading g

Reading thermophysical properties



Selecting thermodynamics package hRhoThermo<pureMixture<constTransport<specieThermo<hConstThermo<perfectGas>>>>>

Reading field U



Reading/calculating face flux field phi



Creating turbulence model



Selecting turbulence model type RASModel

Selecting RAS turbulence model kEpsilon

--> Upgrading k to employ run-time selectable wall functions

    Backup original k to k.old

    Writing updated k

--> Upgrading epsilon to employ run-time selectable wall functions

    Backup original epsilon to epsilon.old

    Writing updated epsilon

--> Creating mut to employ run-time selectable wall functions

    Writing new mut

--> Creating alphat to employ run-time selectable wall functions

    Writing new alphat

kEpsilonCoeffs

{

    Cmu             0.09;

    C1              1.44;

    C2              1.92;

    C3              -0.33;

    sigmak          1;

    sigmaEps        1.3;

    Prt             1;

}



Calculating field g.h



Reading field p_rgh



Creating field dpdt



Creating field kinetic energy K



Courant Number mean: 0 max: 0





--> FOAM FATAL ERROR: 

Residual data for p_rgh must be specified as a dictionary



    From function bool Foam::solutionControl::read()

    in file cfdTools/general/solutionControl/solutionControl/solutionControl.C at line 79.



FOAM exiting



lab@lab-laptop:~/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/NOPCM/pseudoTransient$

Could you please help?

Thanks a lot,
Samuele

I forgot my fvSolution file. Here it is:

Code:

/*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2.1.0                                 |

|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

FoamFile

{

    version     2.0;

    format      ascii;

    class       dictionary;

    location    "system";

    object      fvSolution;

}

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



solvers

{

    p_rgh

    {

        solver          PCG;

        preconditioner  DIC;

        tolerance       1e-06;

        relTol          0.01;

    }



    "(U|h|k|epsilon)"

    {

        solver          PBiCG;

        preconditioner  DILU;

        tolerance       1e-05;

        relTol          0.1;

    }



    G

    {

        $p_rgh;

        tolerance       1e-05;

        relTol          0.1;

    }

}



PIMPLE

{

    nNonOrthogonalCorrectors 0;

    pRefCell        0;

    pRefValue       0;



    residualControl

    {

        p_rgh           1e-2;

        U               1e-3;

        h               1e-3;

        G               1e-3;

    }

}



relaxationFactors

{

    fields

    {

        rho             1.0;

        p_rgh           0.7;

    }

    equations

    {

        U               0.2;

        h               0.2;

        "(k|epsilon|R)" 0.5;

        G               0.7;

    }

}





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

Hey

I did not understand the problem completely but you can make a small change in your fvSolution by this
PIMPLE
{
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;

residualControl
{
p_rgh 1e-2;
U 1e-3;
h 1e-3;
G 1e-3;
}
}

replace it by this

PIMPLE
{
momentumPredictor no;
nOuterCorrectors 1;
nCorrectors 2;
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
}
relaxationFactors
{
p 0.7;
U 0.3;
T 0.5;
k 0.5;
omega 0.5;
nut 0.5;
R 0.5;
nuTilda 0.5;
}

see if it works.

I get this error

Code:

lab@lab-laptop:~/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/NOPCM/pseudoTransient$ buoyantPimpleFoam

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2.1.0                                 |

|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

Build  : 2.1.0-0bc225064152

Exec   : buoyantPimpleFoam

Date   : Jun 05 2013

Time   : 08:44:24

Host   : "lab-laptop"

PID    : 2367

Case   : /home/lab/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/NOPCM/pseudoTransient

nProcs : 1

sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

fileModificationChecking : Monitoring run-time modified files using timeStampMaster

allowSystemOperations : Disallowing user-supplied system call operations



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

Create time



Create mesh for time = 0





Reading g

Reading thermophysical properties



Selecting thermodynamics package hRhoThermo<pureMixture<constTransport<specieThermo<hConstThermo<perfectGas>>>>>

Reading field U



Reading/calculating face flux field phi



Creating turbulence model



Selecting turbulence model type RASModel

Selecting RAS turbulence model kEpsilon

kEpsilonCoeffs

{

    Cmu             0.09;

    C1              1.44;

    C2              1.92;

    C3              -0.33;

    sigmak          1;

    sigmaEps        1.3;

    Prt             1;

}



Calculating field g.h



Reading field p_rgh



Creating field dpdt



Creating field kinetic energy K



Courant Number mean: 0 max: 0



PIMPLE: Operating solver in PISO mode





Starting time loop



Courant Number mean: 0 max: 0

Time = 0.1



#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"

#1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"

#2   in "/lib/libc.so.6"

#3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"

#4  Foam::operator/(Foam::UList<double> const&, Foam::UList<double> const&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"

#5  Foam::diagonalSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"

#6  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"

#7  Foam::fvMatrix<double>::solve() in "/opt/openfoam210/platforms/linux64GccDPOpt/bin/buoyantPimpleFoam"

#8  

 in "/opt/openfoam210/platforms/linux64GccDPOpt/bin/buoyantPimpleFoam"

#9  __libc_start_main in "/lib/libc.so.6"

#10  

 in "/opt/openfoam210/platforms/linux64GccDPOpt/bin/buoyantPimpleFoam"

Floating point exception

lab@lab-laptop:~/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/NOPCM/pseudoTransient$

It is probably due to the BC. But using the steady solver it works fine and I can not und why.

Can you describe your case a little bit? and the boundary conditions as welll

Sure. I can share it, if you agree. Please, send an email to samuele.zampini@gmail.com and I'll send the case back to you.

Hi,

I got the same error message as you and was able to fix it by adding this to my fvSolution file:

Code:

    residualControl

    {

        p_rgh           

        {

            relTol          0;

            tolerance       0.0001;

        }

        U

        {

            relTol          0;

            tolerance       0.0001;

        }

        h

        {

            relTol          0;

            tolerance       0.0001;

        }

        // possibly check turbulence fields

        "(k|epsilon|omega)"        {

            relTol          0;

            tolerance       0.0001;

        }

        

    }

I guess that buoyantPimpleFoam expects the residual control information in this way "as a dictionary", i.e. inside braces with the two entries relTol and tolerance (the latter is probably the absolute value of the residual whereas the first one is the change between two time steps). buoyantSimpleFoam does not need the relTol as there are no time steps.

Joachim

Quote:

Originally Posted by samiam1000 (Post 431960)

Code:

buoyantSimpleFoam

I get this error message:

Code:

...



Courant Number mean: 0 max: 0





--> FOAM FATAL ERROR: 

Residual data for p_rgh must be specified as a dictionary



    From function bool Foam::solutionControl::read()

    in file cfdTools/general/solutionControl/solutionControl/solutionControl.C at line 79.



FOAM exiting