[adambarfi]

hi everybody,

I defined a new solver that solve natural convection in a viscoelastic Fluid. it made successfully, but when I want to run my model the following error was appeared:

--> FOAM FATAL ERROR:

     gradientInternalCoeffs cannot be called for a calculatedFvPatchField
     on patch floor of field p in file "/home/mostafa/OpenFOAM/mostafa-2.1.0/run/tutorials/viscoelastic/viscoelasticFluidFoam/Hasan_Giesekus/0/p"
     You are probably trying to solve for a field with a default boundary condition.
     From function calculatedFvPatchField<Type>::gradientInternalCoeffs() const
     in file fields/fvPatchFields/basic/calculated/calculatedFvPatchField.C at line 186.

  FOAM exiting

do anybody know where is the problem?

Thanks

[nimasam]

DEAR mostafa
could you post your p file here?

[adambarfi]

the attachment contains the p, fvSolution and fvSchemes files.
I changed the floor boundary condition and even delete the p file but this problem didn't had been solve. I think the problem is somewhere in the fvSolution or fvSchemes.

[nimasam]

this solver reads p or p-rgh ?
it seems it reads p, if it reads p! then you should define BC for p, you can not use calculated BC, you should use (fixedValue or fixedGradient) for it

[adambarfi]

Originally Posted by nimasam

this solver reads p or p-rgh ?
it seems it reads p, if it reads p! then you should define BC for p, you can not use calculated BC, you should use (fixedValue or fixedGradient) for it

It reads p and calculate the p-rgh, such as bouyantbuossinesqsimplefoam. I change the bc to fixedValue and fixedGradient but this this error didn't had been omit.

[nimasam]

Dear mostafa let me ask another questions, which version of openfoam do you use?
could you run this test case before heat transfer implementation?
put the test case and solver here, then may other can help you

[ata]

Hi
Did you set p equal to another field in your solver during calculations? i.g.
p=....?

[adambarfi]

this is where I use the p in createFields.H:

    Info<< "Calculating field g.h\n" << endl;
    volScalarField gh("gh", g & mesh.C());
    surfaceScalarField ghf("ghf", g & mesh.Cf());

    volScalarField p
    (
        IOobject
        (
            "p",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        p_rgh + rhok*gh
    );

    label pRefCell = 0;
    scalar pRefValue = 0.0;
    setRefCell(p,p_rgh, mesh.solutionDict().subDict("PISO"), pRefCell, pRefValue);


    if (p_rgh.needReference())
    {
        p += dimensionedScalar
        (
            "p",
            p.dimensions(),
            pRefValue - getRefCellValue(p, pRefCell)
        );
    }

and in pEqn:

    p = p_rgh + rhok*gh;

    if (p_rgh.needReference())
    {
        p += dimensionedScalar
        (
            "p",
            p.dimensions(),
            pRefValue - getRefCellValue(p, pRefCell)
        );
        p_rgh = p - rhok*gh;
    }

what is wrong in my code?

[ata]

Hi
I think you have two options two solve the problem. Selection is your choice:
1:
volScalarField p ( IOobject ( "p", runTime.timeName(), mesh, IOobject::MUST_READ, IOobject::AUTO_WRITE ), mesh );
or
2:
p == p_rgh + rhok*gh;

[adambarfi]

Dear Ata
I applied what you offered me and what Nima said, that error was solved. but after some iterations (50) the following error appeared:

#0  Foam::error::printStack(Foam::Ostream&) in "/home/mostafa/OpenFOAM/OpenFOAM-2.1.0/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/home/mostafa/OpenFOAM/OpenFOAM-2.1.0/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#2  Uninterpreted: 
#3  Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/mostafa/OpenFOAM/OpenFOAM-2.1.0/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#4  Foam::fvMatrix<Foam::SymmTensor<double> >::solve(Foam::dictionary const&) in "/home/mostafa/OpenFOAM/OpenFOAM-2.1.0/platforms/linuxGccDPOpt/lib/libviscoelasticTransportModels.so"
#5  Foam::fvMatrix<Foam::SymmTensor<double> >::solve() in "/home/mostafa/OpenFOAM/OpenFOAM-2.1.0/platforms/linuxGccDPOpt/lib/libviscoelasticTransportModels.so"
#6  Foam::Giesekus::correct() in "/home/mostafa/OpenFOAM/OpenFOAM-2.1.0/platforms/linuxGccDPOpt/lib/libviscoelasticTransportModels.so"
#7  Foam::multiMode::correct() in "/home/mostafa/OpenFOAM/OpenFOAM-2.1.0/platforms/linuxGccDPOpt/lib/libviscoelasticTransportModels.so"
#8  Foam::viscoelasticModel::correct() in "/home/mostafa/OpenFOAM/OpenFOAM-2.1.0/platforms/linuxGccDPOpt/lib/libviscoelasticTransportModels.so"
#9  
 in "/home/mostafa/OpenFOAM/OpenFOAM-2.1.0/platforms/linuxGccDPOpt/bin/BuoyantBoussinesqViscoelasticFluidFoam"
#10  __libc_start_main in "/lib/i386-linux-gnu/libc.so.6"
#11  
 in "/home/mostafa/OpenFOAM/OpenFOAM-2.1.0/platforms/linuxGccDPOpt/bin/BuoyantBoussinesqViscoelasticFluidFoam"
Floating point exception

what is your opinion about this error?

again thank you so much

[nimasam]

it seems somewhere in your code something divide on zero or going to result indefinite value

[Tushar@cfd]

Are you able to resolve your error?

[adambarfi]

Originally Posted by Tushar@cfd

Are you able to resolve your error?

Dear Tushar,
yes, after some day hard working, finally I could solve it.

[Sasy]

Originally Posted by adambarfi

Dear Tushar,
yes, after some day hard working, finally I could solve it.

Dear Mostafa
how do you solved this problem?? I have some problem like this,but my problem dont solve by ata or nima offers...
I use interPhasechangeFoam solver and modified this solver for my simulation...
you can see my creatFields and Peqn

[adambarfi]

hi Sasan,

I get your attached files and I couldn't find any thing that made error!

so, attach your log file + the errors expression

[Sasy]

Originally Posted by adambarfi

hi Sasan,

I get your attached files and I couldn't find any thing that made error!

so, attach your log file + the errors expression

Hi Mostafa
Thank you for reply..
my error:
FOAM FATAL ERROR:

gradientInternalCoeffs cannot be called for a calculatedFvPatchField
on patch left of field p in file "/home/Sasan/Desktop/HardtMix/stephanProblem/0/p"
You are probably trying to solve for a field with a default boundary condition.
and attach the log file

[adambarfi]

You have to specify correct boundary conditions for p otherwise you cannot solve the pEqn!

The error message gave you already a hint what you have to do:

on patch left of field p in file "/home/Sasan/Desktop/HardtMix/stephanProblem/0/p"
    You are probably trying to solve for a field with a default boundary condition.

so, you are using a wrong BC for pEqn. I guess you used calculated type!
try other boundary conditions that are compatible with your solution.

[Sasy]

Originally Posted by adambarfi

You have to specify correct boundary conditions for p otherwise you cannot solve the pEqn!

The error message gave you already a hint what you have to do:

on patch left of field p in file "/home/Sasan/Desktop/HardtMix/stephanProblem/0/p"
    You are probably trying to solve for a field with a default boundary condition.

so, you are using a wrong BC for pEqn. I guess you used calculated type!
try other boundary conditions that are compatible with your solution.

Hi Mostafa
I used this test case with another solver and dont have problem,But for new solver,I have this problem.
my BC is not calculated....!!
you can see:

[Sasy]

Originally Posted by Sasy

Hi Mostafa
I used this test case with another solver and dont have problem,But for new solver,I have this problem.
my BC is not calculated....!!
you can see:

sorry.I forgot attach my file...

[adambarfi]

mhmm, I think there are problems with p BCs.
the userGuide says:

At all wall boundaries, the buoyantPressure boundary condition is applied to the pressure
field, which calculates the normal gradient from the local density gradient.

buoyantPressure: Sets fixedGradient pressure based on the atmospheric pressure gradient

I think such same BCs for p and p_rgh is wrong, let the solver calculate the pressure based upon potential function. try "calculated" type for p BCs.

Also, I can't understand these conditions you used for p_rgh:

        type            buoyantPressure;
        gradient        uniform 0;
        value           uniform 0;

try this one:

        type            buoyantPressure;
        rho             rhok;
        value           uniform 0;

see the buoyantBoussinesqPimpleFoam and buoyantBoussinesqSimpleFoam solvers. they have tips that may help you.