CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   whats the cause of error? (http://www.cfd-online.com/Forums/openfoam-solving/114133-whats-cause-error.html)

immortality March 5, 2013 17:54

whats the cause of error?
 
i have written three pressure BC.and then tried to do by groovyBC.although it seems equivalent to others it don't work.
if this problem resolve i think the trouble is removed.
fixedValue p:OK
Code:

type fixedValue;
        value uniform 1023382.5;

totalPressure:OK
Code:

type totalPressure;
        rho none;
        psi psi;
        phi phi;
        p0 1023382.5;
        gamma 1.4;

but groovyBC:
Code:

type groovyBC;
        fractionExpression "1";
        valueExpression "1023382.5/pow(1+(1.4-1)*magSqr(U)/(2*1.4*287.14*T),3.5)";
        value uniform 3523382.5;

results in:
Code:

Create time

Create mesh for time = 0


PIMPLE: no residual control data found. Calculations will employ 3 corrector loops

Reading thermophysical properties

Selecting thermodynamics package hPsiThermo<pureMixture<sutherlandTransport<specieThermo<janafThermo<perfectGas>>>>>
Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting turbulence model type laminar
Creating field dpdt

Creating field kinetic energy K


Starting time loop

Courant Number mean: 0 max: 0
deltaT = 1e-06
Time = 1e-06

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
PIMPLE: iteration 1
DILUPBiCG:  Solving for Ux, Initial residual = 0.9999620096, Final residual = 4.199402748e-15, No Iterations 2
DILUPBiCG:  Solving for Uy, Initial residual = 1.005998662e-08, Final residual = 7.973709578e-16, No Iterations 1
DILUPBiCG:  Solving for h, Initial residual = 0.0001693584029, Final residual = 4.837750541e-11, No Iterations 1
#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2  in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4  void Foam::divide<Foam::fvsPatchField, Foam::surfaceMesh>(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#5  Foam::tmp<Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> > Foam::operator/<Foam::fvsPatchField, Foam::surfaceMesh>(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::tmp<Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> > const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#6  Foam::fv::backwardDdtScheme<Foam::Vector<double> >::fvcDdtPhiCorr(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#7
at rhoPimpleFoam.C:0
#8
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/rhoPimpleFoam"
#9  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/rhoPimpleFoam"
Floating point exception

why?
thanks for quick helps.

immortality March 5, 2013 17:57

the whole p is:
Code:

FoamFile
{
    version    2.0;
    format      ascii;
    class      volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -2 0 0 0 0];

internalField  uniform 3523382.5;//1823382.5

boundaryField
{
    right
    {
       
        /*type fixedValue;
        value uniform 1023382.5;*/
        /*type totalPressure;
        rho none;
        psi psi;
        phi phi;
        p0 1023382.5;
        gamma 1.4;*/
        type groovyBC;
        fractionExpression "1";
        valueExpression "1023382.5/pow(1+(1.4-1)*magSqr(U)/(2*1.4*287.14*T),3.5)";
        value uniform 3523382.5;
       
    }

    left
    {
      type zeroGradient; 
    }

    walls
    {
        type zeroGradient;
       
    }

    empty
    {
        type empty;
       
    }
}

the problem is in p(other variables are ok as i tested)
I have to write BC in groovyBC form because of more complicated main case I have to solve.
thanks very much.please answer rapidly.;)

chegdan March 5, 2013 19:50

There are several issues:
  • Divide by Zero Error I am taking a guess that there is a divide by zero in there
    Code:

    Floating point exception
    If I were to start to track that one down, I would look where a divide by zero might be. Looking at what you have provided...I would say its near
    Code:

    valueExpression "1023382.5/pow(1+(1.41)*magSqr(U)/(2*1.4*287.14*T),3.5)";
    which is equivalent to

    \frac{1023382.5}{\left(1+\frac{1.41*||\vec{U}||}{2*1.4*287.14*T}\right)^{3.5}}

    I see a T in the denominator, and if there is a zero there....one will have a divide by zero issue....this could be the problem
  • OpenFOAM Protip
    Using things like "please answer rapidly" will most likely do exactly the opposite of what you want. In my experience, people answer questions here for several reasons:
    • They have experienced the same problem in their own work want to save the questioner some head ache
    • They are genuinely interested in the problem and want to take the time out of their schedule and learn something for themselves and also help the person posing the questions
    • They are interested in helping future questioners that may thoroughly search the issue and stumble upon the solution to their current problem
    • The questioner has helped them in the past and they want to return the favor.
    • Fame, fortune, and super moderator status :D

Your BC may be giving the error when a boundary condition is corrected and has a T == zero for some reason. Honestly, without more information this is the best i can do with solving your issue...but its an educated guess at this point.

#OFProtip

immortality March 5, 2013 20:03

thanks.T isn't zero and also its same for all three tests.but only in groovy it occurs.

chegdan March 5, 2013 20:23

did you try another time integration scheme? I see a backwardDdtScheme in your error message and there may be something happening there. Also, just to prove that its not the T in the denominator, change your value expression to

Code:

valueExpression "1023382.5/pow(1+(1.41)*magSqr(U)/(2*1.4*287.14*T + 1e-8),3.5)";
and give it a try.

immortality March 6, 2013 06:07

i changed time scheme to Euler and changed T but error persists.initial U is zero and i changed it but the error didn't change
these are variable BC's:
p:
Code:

FoamFile
{
    version    2.0;
    format      ascii;
    class      volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -2 0 0 0 0];

internalField  uniform 3523382.5;//1823382.5

boundaryField
{
    right
    {
       
        /*type fixedValue;
        value uniform 1023382.5;*/
        /*type totalPressure;
        rho none;
        psi psi;
        phi phi;
        p0 1023382.5;
        gamma 1.4;*/
        type groovyBC;
        fractionExpression "1";
        valueExpression "1023382.5/pow(1+(1.4-1)*magSqr(U)/(2*1.4*287.14*T+1e-8),3.5)";
        value uniform 3523382.5;
       
    }

    left
    {
      type zeroGradient; 
    }

    walls
    {
        type zeroGradient;
       
    }

    empty
    {
        type empty;
       
    }
}

U:
Code:

dimensions      [0 1 -1 0 0 0 0];

internalField  uniform (1 0 0);

boundaryField
{
    right
    {
    type zeroGradient;
    }

    left
    {
     
        type fixedValue;
      value uniform (0 0 0);
        /*type groovyBC;

        variables (
);
        fractionExpression "1";
        valueExpression "vector(internalField(U).x,0,0)";
        value uniform (0 0 0);*/
    }
walls
    {
        type fixedValue;
        value uniform (0 0 0);
       
    }

    empty
    {
        type empty;
       
    }
}

T:
Code:

FoamFile
{
    version    2.0;
    format      ascii;
    class      volScalarField;
    object      T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 1 0 0 0];

internalField  uniform 973;

boundaryField
{
  right
    {
        type zeroGradient;
        /*type            groovyBC;
        value          uniform 973;
      // valueExpression "907";//T0_2-(1.4-1)*magSqr(internalField(U))/(2*1.4*287.14)
        gradientExpression "0";
        fractionExpression "0";*/

    }

    left
    {
     
      type zeroGradient;
 
     
    }

    walls
    {
        type zeroGradient;
       
    }

    empty
    {
        type empty;
       
    }
}

fvSolution is:
Code:

solvers
{
    p
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance      1e-11;
        relTol          0;
    }

    pFinal
    {
        $p;
        relTol          0;
    }

    "rho.*"
    {
        $p;
        tolerance      1e-10;
        relTol          0;
    }

    "(U|e|h|R|k|epsilon|omega)"
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance      1e-10;
        relTol          0;
        maxIter 25000;
    }

    "(U|h|R|k|epsilon|omega)Final"
    {
        $U;
        relTol          0;
    }
}

PIMPLE
{
    momentumPredictor yes;
    nOuterCorrectors 3;
    nCorrectors    5;
    nNonOrthogonalCorrectors 0;
    rhoMin          rhoMin [ 1 -3 0 0 0 ] 0.01;
    rhoMax          rhoMax [ 1 -3 0 0 0 ] 100.0;
}

fvScheme:
Code:

ddtSchemes
{
    default        Euler;//backward
}

gradSchemes
{
    default        faceMDLimited Gauss midPoint 1;
    grad(p)        faceMDLimited Gauss midPoint 1;
    grad(U)        faceMDLimited Gauss cubic 1; //faceMDLimited Gauss GammaV 1
}

divSchemes
{
    default        none;
    div(phi,U)      Gauss SFCDV grad(U);//SFCDV-linearUpwind
    div(phi,K)      Gauss SuperBee;//Minmod
    div(phi,h)      Gauss SuperBee;
    div(phi,k)      Gauss SuperBee;
    div(phi,omega)  Gauss SuperBee;
    div(U)          Gauss SuperBeeV;//Gauss limitedLimitedLinear 1 0 1
    div((muEff*dev2(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default      Gauss midPoint limited .5;//limited .5
    /*laplacian(muEff,U) Gauss linear corrected;
    laplacian(mut,U) Gauss linear corrected;
    laplacian(DkEff,k) Gauss linear corrected;
    laplacian(DomegaEff,omega) Gauss linear corrected;
    laplacian((rho*(1|A(U))),p) Gauss linear corrected;
    laplacian(alphaEff,h) Gauss linear corrected;
    laplacian(k,T)  Gauss linear corrected; 
    laplacian(alpha,e) Gauss linear corrected;
    laplacian(alphaEff,e)  Gauss linear corrected;*/
}

interpolationSchemes
{
    default        midPoint;// cubicCorrection
}

snGradSchemes
{
    default      limited .5;//corrected
}

fluxRequired
{
    default        no;
    p              ;
}

and at last controlDict:
Code:

FoamFile
{
    version    2.0;
    format      ascii;
    class      dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
libs (
      "libOpenFOAM.so"
      "libsimpleSwakFunctionObjects.so"
      "libswakFunctionObjects.so"
      "libgroovyBC.so"
    );

application    rhoPimpleFoam;

startFrom      latestTime;

startTime      0;

stopAt          endTime;

endTime        2000e-6;//0.020708089;

deltaT          1e-6;

writeControl    adjustableRunTime;

writeInterval  .000001;

purgeWrite      0;

writeFormat    ascii;

writePrecision  10;

writeCompression off;

timeFormat      general;

timePrecision  6;

runTimeModifiable true;

adjustTimeStep  yes;

maxCo          0.1;

maxDeltaT      1;


immortality March 6, 2013 11:21

thanks for your effort to help dear Daniel.
It was because of new groovyBC.I changed to old version and it answer now.

chegdan March 6, 2013 11:22

OK, it is indeed your BC setup. I don't have the time to set this up for you, but i have some suggestions.
  • go and look through the groovyBC examples, they will cover what you want. If you dont have them, google for them...they are out there :D
  • Start with a simpler groovyBC that will be easier to debug.

Good luck

EDIT: read your new post that just mystically appeared....glad you figured it out :)

immortality March 6, 2013 12:41

a question occur to me that I'm curious about.
when I set BC for U to zeroGradient or:
Code:

right
    {
    type groovyBC;
    fractionExpression "0";
    gradientExpression "vector(0,0,0)";
    }

it answers without any error
but when I set it to:
Code:

right
    {
    type groovyBC;
    fractionExpression "1";
    valueExpression "internalField(U)";//vector(internalField(U).x,0,0)
    }

it falls to an error on T(energy equation probably) as so:
Code:

From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -3333091.721
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 4080511.561
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -7124696.499
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 5774453.414
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -6575768.989
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 5981361.409
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 1404258.482
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -17090209.16
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 36020792.5
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -94818398.64
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 40233402.34
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -106376680.8
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 37389446.51
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -76115211.3
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -24650104.63
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -26951665.22
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 471535.4463
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 465677.0027
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 277204.4414
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -145721.0621
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 15779.92442
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 112883.4828
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -3083.273126
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 43.52495911
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 4976486.257
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 3178348.937
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -32897237.32
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -44825686.95
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -22612.51171
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -1870.615087
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 9690.272357
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -39521.73991
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 93265.31041
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -340838.0148
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 610015.5259
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -1813983.217
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 2650248.864
--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = -6558287.943

I thought that internalField(U) or vector(internalField(U).x,0,0) do the same way as zeroGradient(or in groovyBC gradientExpression"0" does).
why?

CFDUser_ April 21, 2014 01:14

Quote:

Code:

--> FOAM Warning :
From function janafThermo<EquationOfState>::limit(const scalar T) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 4080511.561


Hi Ehsan,

Did you find any clue for above warning to fix?

Regards,
CFDUser_

immortality April 21, 2014 10:45

Quote:

Originally Posted by CFDUser_ (Post 487211)
Hi Ehsan,

Did you find any clue for above warning to fix?

Regards,
CFDUser_

Hi, yes I did it ! if I remember truely, it was because of the BC. when we use zeroGradient BC it solves the equations implicitly but when use internalField the equations are solved explicitly and may be unstable although in both cases the values on the boundary and internal value is the same but in zeroGradient case we say to OpenFOAM that solve these equations so that the values on the boundary be at last equal as the value on neighbor cells but in internalField case we say put the value on the neighbor cells on the boundaries now and then solve the equations!
besides that, the velocity on outward flow should be read from inside implicitly and only pressure should be set there as a known value otherwise error will arise due to instability.
I hope these explanations be what you asked about.

CFDUser_ April 22, 2014 12:32

Quote:

Originally Posted by immortality (Post 487324)
Hi, yes I did it ! if I remember truely, it was because of the BC. when we use zeroGradient BC it solves the equations implicitly but when use internalField the equations are solved explicitly and may be unstable although in both cases the values on the boundary and internal value is the same but in zeroGradient case we say to OpenFOAM that solve these equations so that the values on the boundary be at last equal as the value on neighbor cells but in internalField case we say put the value on the neighbor cells on the boundaries now and then solve the equations!
besides that, the velocity on outward flow should be read from inside implicitly and only pressure should be set there as a known value otherwise error will arise due to instability.
I hope these explanations be what you asked about.

Wow, This is more than expected. Thanks a lot Ehsan. :)

Regards,
CFDUser_


All times are GMT -4. The time now is 08:09.