[adkar]

Could someone please tell me what "false" means in IOobject?
This is found in so many places inside OpenFOAM.
The following is an example piece of code.

Thank you in advance.

***************************************
location: /src/thermophysicalModels/radiationModels/radiationModel/viewFactor/viewFactor.C
***************************************
Foam::tmp<Foam::volScalarField> Foam::radiation::viewFactor::Rp() const
{
return tmp<volScalarField>
(
new volScalarField
(
IOobject
(
"Rp",
mesh_.time().timeName(),
mesh_,
IOobject::NO_READ,
IOobject::NO_WRITE,
false
),
mesh_,
dimensionedScalar
(
"zero",
dimMass/pow3(dimTime)/dimLength/pow4(dimTemperature),
0.0
)
)
);
}
*******************************

[TobM]

In: http://foam.sourceforge.net/docs/cpp/a01169.html
you see, that "false" says, that the field Rp is not a registered object. For default it is set to true.

[adkar]

Firstly,thank you so much for taking your time and answering my question.

I am pretty new to OpenFOAM. But I think the above 'false' is cpp syntax.
I will do my homework in searching what registered object means

This might be wrong but, does the above "false" mean that when Rp() is called inside another class (radiationModel.C) there will not be any values sent inside the function Rp() since it is declared as "false" ?
Ru() is defined in in ViewFactors.C (the above piece of code) and called in another file called radiationModel.C


http://openfoam.com/documentation/cp...ml/a02143.html

Thank you once again.

[floquation]

You can compare it with local and global variables.

In principle every variable is local: it lives within the scope it was defined.

However, OpenFOAM holds a database of IOobjects. From the mesh-variable you can get any of the IOobjects stored inside that database.
Therefore, those stored IOobjects are in essence global variables: As long as you have access to a reference to the mesh instance, you can access all of those stored IOobjects.

In your code snippet it means that the only reference to the IOobject is the return value of the Rp()-function.
If it was set to true, there would be another reference to that IOobject inside OpenFOAM's "global IOobject variables" database.

[fluidmobil]

thanks so far,

can someone explain the meaning of the last three lines before the closing parenthesis in the following code snippet?

lambda_
    (
        IOobject
        (
            "lambdaTemp"
            U.time().timeName(),
            U_.db()
        ),
        U_.mesh(),
        dimensionedScalar("lambdaTemp", dimensionSet(1, 1, -3, -1, 0),0),
        calculatedFvPatchScalarField::typeName
    ),

so what means U_.mesh(), dimensionedScalar and calculatedFvPatchScalarField::typeName

is a file "lambdaTemp" created somewhere?

thanks in advance

Mathi

[Zeppo]

Originally Posted by fluidmobil

thanks so far,

can someone explain the meaning of the last three lines before the closing parenthesis in the following code snippet?

lambda_
    (
        IOobject
        (
            "lambdaTemp"
            U.time().timeName(),
            U_.db()
        ),
        U_.mesh(),
        dimensionedScalar("lambdaTemp", dimensionSet(1, 1, -3, -1, 0),0),
        calculatedFvPatchScalarField::typeName
    ),

so what means U_.mesh(), dimensionedScalar and calculatedFvPatchScalarField::typeName

is a file "lambdaTemp" created somewhere?

thanks in advance

Mathi

The type of your object lambda_ is volScalarField which is essentially:

//--- volFieldsFwd.H ---
typedef GeometricField<scalar, fvPatchField, volMesh> volScalarField;

Now look at the constructor of GeometricField:

//--- GeometricField.c ---
//- Constructor given IOobject, mesh, dimensioned<Type> and patch type.
template<class Type, template<class> class PatchField, class GeoMesh>
Foam::GeometricField<Type, PatchField, GeoMesh>::GeometricField
(
    const IOobject& io,
    const Mesh& mesh,
    const dimensioned<Type>& dt,
    const word& patchFieldType
)
:
    Internal(io, mesh, dt, false),
    timeIndex_(this->time().timeIndex()),
    field0Ptr_(NULL),
    fieldPrevIterPtr_(NULL),
    boundaryField_(mesh.boundary(), *this, patchFieldType)
{
    if (debug)
    {
        InfoInFunction << "Creating temporary" << endl << this->info() << endl;
    }

    boundaryField_ == dt.value();

    readIfPresent();
}

The last 3 parameters unknown to you are:
U_.mesh() - a reference to mesh (as a set of finite volumes with boundaries) your field is defind on;
dimensionedScalar("lambdaTemp", dimensionSet(1, 1, -3, -1, 0),0) - a scalar zero value to initialize your field;
calculatedFvPatchScalarField::typeName - a type (expressed as a string) of boundary patches