[ycui]

Dear All,

I'm implementing a new particle force with two input parameters. And I want these two parameters can be read from input file (/constant), then I do not need to compile for every runs. The way I did as following:

IOdictionary environmentalProperties
(
IOobject
(
"environmentalProperties",
runTime.constant(),
mesh,
IOobject::MUST_READ,
IOobject::NO_WRITE
)
);

scalar a(readScalar(environmentalProperties.lookup("a"))) ;
scalar b(readScalar(environmentalProperties.lookup("b"))) ;

However, during compiling, errors occurs:

error: ‘runTime’ was not declared in this scope
error: ‘mesh’ was not declared in this scope

I need your help!

Greetings,

ycui

[floquation]

(Please use code-tags, not quote-tags for code.)

The error is quite clear: the variables 'runTime' and 'mesh' do not exist at the position where you inserted your code.

So where exactly did you insert this piece of code?

[ycui]

Originally Posted by floquation

(Please use code-tags, not quote-tags for code.)

The error is quite clear: the variables 'runTime' and 'mesh' do not exist at the position where you inserted your code.

So where exactly did you insert this piece of code?

In: /home/ycui/OpenFOAM/ycui-2.3.1/src/lagrangian/intermediate/submodels/Kinematic/ParticleForces/

I try to use this->mesh().time() and this->mesh(), but doesn't works.

[floquation]

The mesh and runTime variables are part of the solver. The thing you are changing is a library used by the solver - but it has no knowledge of what is going on inside your solver. It is just doing its own thing.

To find out how to do this, use search commands:

cd ${FOAM_SRC}/lagrangian/intermediate/submodels/Kinematic/ParticleForces/
grep -rn "IOobject" .

This will teach you that OpenFoam has no example for you specifically related to ParticleForces. Going up one directory:

cd ${FOAM_SRC}/lagrangian/intermediate/submodels/Kinematic/
grep -rn "IOobject" .

Will give you (amongst other examples) the file:

vi ./PatchInteractionModel/LocalInteraction/LocalInteraction.C +122

where the following may be seen:

template<class CloudType>
Foam::volScalarField& Foam::LocalInteraction<CloudType>::massEscape()
{
    if (!massEscapePtr_.valid())
    {
        const fvMesh& mesh = this->owner().mesh();

        massEscapePtr_.reset
        (
            new volScalarField
            (
                IOobject
                (
                    this->owner().name() + ":massEscape",
                    mesh.time().timeName(),
                    mesh,
                    IOobject::READ_IF_PRESENT,
                    IOobject::AUTO_WRITE
                ),
                mesh,
                dimensionedScalar("zero", dimMass, 0.0)
            )
        );
    }

    return massEscapePtr_();
}

Can you try and see if that compiles for a ParticleForce?

[ycui]

Dear floquation,

Thank you very much for the answer.

I found a simple way to do this, just add

myParameter_(readScalar(this->coeffs().lookup("myParameter")))

in the constructor. Then the code can read from the input file.

However, your method would be very helpful when one reads a time dependent parameter.

Thank you again,

Best regards,

ycui

[sy2516]

Hey,

Can you help me to implement a new force to OpenFOAM? I really appreciate it. Thank you in advance.