[mjavrincon]

Hi everyone,

I'm trying to set up a custom source term for the enthalpy field h in my OpenFOAM-v2212 simulation with buoyantSimpleFoam and using the scalarCodedSource functionality within fvOptions. To troubleshoot, I created an fvOptions file with no custom code, just the basic structure. However, I am consistently encountering the following error:

--> FOAM FATAL ERROR: (openfoam-2212 patch=230110)
Not implemented

    From virtual void Foam::fv::energySourceFvOptionscalarSource::addSup(const volScalarField&, Foam::fvMatrix<double>&, Foam::label)
    in file codedFvOptionTemplate.C at line 178.

Here's the dummy fvOptions file I'm using:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2212                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvOptions;
}

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

codedSource
{
    type            scalarCodedSource;
    selectionMode   all;
    active          true;
    fields          ( h );
    name            exampleCodedSource;

    codeInclude
    #{
        // Empty block
    #};

    codeCorrect
    #{
        // Empty block
    #};

    codeConstrain
    #{
        // Empty block
    #};

    codeAddSup
    #{
        // Empty block
    #};
}

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

Even with this minimal setup that doesn't include any operational code, I am still encountering the "not implemented" error. It seems like the addSup function might not be fully implemented for scalarCodedSource.

Has anyone experienced a similar issue or could provide guidance on how to correctly implement a custom source term for the enthalpy field in OpenFOAM? Any insights or examples would be greatly appreciated!

Thank you!

[olesen]

Originally Posted by mjavrincon

Hi everyone,

I'm trying to set up a custom source term for the enthalpy field h in my OpenFOAM-v2212 simulation with buoyantSimpleFoam and using the scalarCodedSource functionality within fvOptions. To troubleshoot, I created an fvOptions file with no custom code, just the basic structure. However, I am consistently encountering the following error:

There is indeed a bit of confusion there. As well as codeAddSup there is also a coddAddSupRho too. It looks like this is where your "not implemented" is coming from.
Unfortunately no way to template and define just a single code block for compressible/incompressible, thus the two different code chunks are needed.

[mjavrincon]

Thanks a lot That was actually what I needed.

It seems like you know quite a bit about coded source terms. Perhaps you can help me with another problem I have encountered: I am trying to retrieve the value of Cp in each cell and calculate its mean, but I cannot retrieve this data from the thermophysical properties. So far, this is what I have achieved (with errors):

enthalpySource
{
    type            scalarCodedSource;
    selectionMode   all;
    active          true;
    fields          ( h );  // Applying the source term to the temperature field
    name            enthalpySource;

    codeInclude
    #{
        #include "fvCFD.H"
        #include "$FOAM_SRC/thermophysicalModels/basic/basicThermo/basicThermo.H"
    #};

    codeCorrect
    #{
        // Ensure this block is present but empty
    #};

    codeConstrain
    #{
        // Ensure this block is present but empty
    #};

    codeAddSupRho
    #{
        const scalar temperatureTarget = 323.15;  // Target temperature provided by the user in Kelvin

        // Get the temperature and enthalpy fields
        const volScalarField& T = mesh().lookupObject<volScalarField>("T");
        const volScalarField& h = mesh().lookupObject<volScalarField>("h");

        const scalarField& V = mesh_.V();

        scalarField& heSource = eqn.source();

        // Calculate the volumetric mean value of temperature
        scalar meanT = 0.0;
        scalar Vtotal = 0.0;

        forAll(T, celli)
        {
            meanT += T[celli] * V[celli];
            Vtotal += V[celli];
        }
        meanT /= Vtotal;

        // Get the specific heat capacity (Cp) for each cell
        const volScalarField& Cp = basicThermo.Cp();  // ERROR ENCOUNTERED

        // Calculate the mean Cp across all cells
        scalar Cp_mean = 0.0;
        scalar Vtotal = 0.0;
        forAll(Cp, celli)
        {
            Cp_mean += Cp[celli] * V[celli];
            Vtotal += V[celli];
        }
        Cp_mean /= Vtotal;       

        const scalar delta_h = Cp_mean * (temperatureTarget - meanT);  // Change in enthalpy
        // Apply the enthalpy source term        
        forAll(h, celli)
        {
            // cell volume specific source
            heSource[celli] += delta_h * V[celli];
        }
    #};

}

I am using buoyantSimpleFoam and I get an error each time I try and get the Cp values. I have tried pretty much everything... Any clues?

[zapp.branigan]

The cell-index is not correct I think.


see problems creating a sink term with scalarCodedSource

[mjavrincon]

Thank you! You are right, the cellIDs were wrong. Now is corrected as shown below, however, I am still unable to obtain the Cp values at each cell. Any ideas?

enthalpySource
{
    type            scalarCodedSource;
    selectionMode   all;
    active          false;
    fields          ( h );  // Applying the source term to the enthalpy field
    name            enthalpySource;

    codeInclude
    #{
        #include "fvCFD.H"
        #include "$FOAM_SRC/thermophysicalModels/basic/basicThermo/basicThermo.H"
    #};

    codeCorrect
    #{
        // Ensure this block is present but empty
    #};

    codeConstrain
    #{
        // Ensure this block is present but empty
    #};

    codeAddSupRho
    #{
        const scalar temperatureTarget = 323.15;  // Target temperature provided by the user in Kelvin

        // Get the temperature, enthalpy, and static pressure fields
        const volScalarField& T = mesh().lookupObject<volScalarField>("T");
        const volScalarField& h = mesh().lookupObject<volScalarField>("h");

        // Get the mesh volume and cell IDs
        const scalarField& V = mesh_.V();
        const labelList& cellIDs = cells();

        scalarField& heSource = eqn.source();

        // Calculate the volumetric mean value of temperature
        scalar meanT = 0.0;
        scalar Vtotal = 0.0;

        forAll(T, i)
        {
            label celli = cellIDs[i];

            meanT += T[celli] * V[celli];
            Vtotal += V[celli];
        }
        meanT /= Vtotal;

        // Get the specific heat capacity (Cp) for each cell
        const volScalarField& Cp = basicThermo.Cp();  // ERROR ENCOUNTERED

    #};

}

[dlahaye]

Not sure.

Cp(), however, is merely a virtual member function of the basisThermo class, see e.g. (depending on the version you are using) L436 of https://www.openfoam.com/documentati...8H_source.html

This implies that the implementation of the Cp() member function is postponed to a child class of the basisThermo parent class.

heThermo is an example of such a child class. See e.g. L372 of https://www.openfoam.com/documentati...8C_source.html

This implies that in your code block you might (emphasis on "might") be required to

1/ extract your thermo object from the object registry (not sure whether thermo object is stored in object registry - should check)

2/ cast your thermo object to a type that has a Cp() member function explicitly defined (most likely the thermo type used in your simulation);

I appreciate learning how it goes.

[olesen]

Originally Posted by mjavrincon

Thanks a lot That was actually what I needed.

It seems like you know quite a bit about coded source terms.

Thanks. I really enjoyed that comment (unironically)!

[arunkl]

I am new to these user defined terms in Openfoam so I am trying to implement the degassing boundary condition using Fvoptions and getting the error of not implemented
can you please help me debug the code
degassing bc.txt


/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 3.0.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object fvOptions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

degassingMassSource
{
type scalarCodedSource;
active yes;
selectionMode all;

name degassingMassSource;
patches (outlet);
rhoName thermo:rho.air;
alphaName alpha.air;

scalarCodedSourceCoeffs
{
selectionMode all;

fields (thermo:rho.air);

codeInclude
#{
#include "fvm.H"
#};

codeCorrect
#{

#};

codeAddSup
#{
// Get the names of the patches on which to apply the degassing forces
DynamicList<word, 1, 0> patches;
coeffs().lookup("patches") >> patches;

// Get the required fields
const word rhoName = coeffs().lookup("rhoName");
const volScalarField& rhoAir = mesh().lookupObject<volScalarField>(rhoName);
const word alphaName = coeffs().lookup("alphaName");
const volScalarField& alphaAir = mesh().lookupObject<volScalarField>(alphaName);

// Get the timestep
const scalar deltaT = mesh().time().deltaT().value();

// Create degassing mass source coefficient and initialize to zero
volScalarField degassingMassSourceCoeff
(
IOobject
(
"degassingMassSourceCoeff",
mesh().time().timeName(),
mesh(),
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
mesh(),
dimensionedScalar("degassingMassSourceCoeff", dimless/dimTime, 0.0)
);

// Compute the degassing mass source coefficient for each cell adjacent to the selected patches
forAll(patches, iPatch)
{
// Get the boundary patch
const fvPatch& patch = mesh().boundary()[patches[iPatch]];

// Loop through each boundary face and compute degassing force coefficient in adjacent cell
forAll(patch, iFace)
{
label iCell = patch.faceCells()[iFace];
degassingMassSourceCoeff[iCell] = -alphaAir[iCell]/deltaT;
}
}

// Add the degassing force term
eqn += fvm::Sp(degassingMassSourceCoeff, rhoAir);
#};

codeSetValue
#{

#};

// Dummy entry. Make dependent on above to trigger recompilation
code
#{
$codeInclude
$codeCorrect
$codeAddSup
$codeSetValue
#};
}
}

degassingForce
{
type vectorCodedSource;
active yes;
selectionMode all;

name degassingForce;
patches (outlet);
rhoName thermo:rho.air;
alphaName alpha.air;
UName U.air;

vectorCodedSourceCoeffs
{
selectionMode all;

fields (U.air);

codeInclude
#{
#include "fvm.H"
#};

codeCorrect
#{

#};

codeAddSup
#{
// Get the names of the patches on which to apply the degassing forces
DynamicList<word, 1, 0> patches;
coeffs().lookup("patches") >> patches;

// Get the required fields
const word rhoName = coeffs().lookup("rhoName");
const volScalarField& rhoAir = mesh().lookupObject<volScalarField>(rhoName);
const word alphaName = coeffs().lookup("alphaName");
const volScalarField& alphaAir = mesh().lookupObject<volScalarField>(alphaName);
const word UName = coeffs().lookup("UName");
const volVectorField& UAir = mesh().lookupObject<volVectorField>(UName);

// Get the timestep
const scalar deltaT = mesh().time().deltaT().value();

// Create degassing force coefficient and initialize to zero
volScalarField degassingForceCoeff
(
IOobject
(
"degassingForceCoeff",
mesh().time().timeName(),
mesh(),
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
mesh(),
dimensionedScalar("degassingForceCoeff", dimDensity/dimTime, 0.0)
);

// Compute the degassing force coefficient for each cell adjacent to the selected patches
forAll(patches, iPatch)
{
// Get the boundary patch
const fvPatch& patch = mesh().boundary()[patches[iPatch]];

// Loop through each boundary face and compute degassing force coefficient in adjacent cell
forAll(patch, iFace)
{
label iCell = patch.faceCells()[iFace];
degassingForceCoeff[iCell] = -rhoAir[iCell]*alphaAir[iCell]/deltaT;
}
}

// Add the degassing force term
eqn += fvm::Sp(degassingForceCoeff, UAir);
#};

codeSetValue
#{

#};

// Dummy entry. Make dependent on above to trigger recompilation
code
#{
$codeInclude
$codeCorrect
$codeAddSup
$codeSetValue
#};
}
}


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




i am also getting varies errors like type conversion and number of variables

thankyou in advance please help me

[arunkl]

PIMPLE: iteration 1
MULES: Solving for alpha.air
MULES: Solving for alpha.air
alpha.air volume fraction = 0.40003 Min(alpha1) = 0.4 Max(alpha1) = 0.5
Using dynamicCode for fvOption::degassingMassSource at line 31 in "/home/arunkl/openFoamFiles/bubbleColumn/constant/fvOptions/degassingMassSource/scalarCodedSourceCoeffs"
Selecting finite volume options type degassingMassSource
Source: degassingMassSource
- selecting all cells
- selected 1875 cell(s) with volume 0.015


--> FOAM FATAL ERROR: (openfoam-2312)
Not implemented

From virtual void Foam::fv::degassingMassSourceFvOptionscalarSource: :addSup(const volScalarField&, Foam::fvMatrix<double>&, Foam::label)
in file /home/arunkl/openFoamFiles/bubbleColumn/constant/fvOptions/degassingMassSource/scalarCodedSourceCoeffs at line 109.

FOAM aborting

[stack trace]
=============
#1 Foam::error::simpleExit(int, bool) in /usr/lib/openfoam/openfoam2312/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so
#2 ? in /usr/lib/openfoam/openfoam2312/platforms/linux64GccDPInt32Opt/lib/libreactingMultiphaseSystem.so
#3 ? in /usr/lib/openfoam/openfoam2312/platforms/linux64GccDPInt32Opt/lib/libreactingMultiphaseSystem.so
#4 Foam:haseSystem::correct() in /usr/lib/openfoam/openfoam2312/platforms/linux64GccDPInt32Opt/lib/libreactingMultiphaseSystem.so
#5 ? in /usr/lib/openfoam/openfoam2312/platforms/linux64GccDPInt32Opt/lib/libreactingTwoPhaseSystem.so
#6 ? in /usr/lib/openfoam/openfoam2312/platforms/linux64GccDPInt32Opt/bin/reactingTwoPhaseEulerFoam
#7 ? in /lib/x86_64-linux-gnu/libc.so.6
#8 __libc_start_main in /lib/x86_64-linux-gnu/libc.so.6
#9 ? in /usr/lib/openfoam/openfoam2312/platforms/linux64GccDPInt32Opt/bin/reactingTwoPhaseEulerFoam
=============
Aborted