[libe]

Hello guys,
I am new in OpenFoam and I face several difficulties. I have followed the advice of Henrik for new openfoamers _ http://www.cfd-online.com/Forums/ope...gramming.html_ but still i cant find how to add in my model a new source term! I want to add the term
Source = A * cos(f * t)
I tried the following

while (runTime.loop())
{
Info<< "Time = " << runTime.timeName() << nl << endl;

Source = A* Foam::cos(f * runTime.time().value());

but nothing

and after the

At creatFields.H

volScalarField Source
(
"Source",
A* Foam::cos(f * runTime.time().value())
);

but nothing again...
I know its something very simple but I cant understand what I am missing!
Please help!
Thanks

[akidess]

It sounds like you managed to create a source field, but you didn't include it in any equation.

[libe]

Hello akidess for ur interest,
the system of equations that i try to solve is the following

while (runTime.loop())
{
Info<< "Time = " << runTime.timeName() << nl << endl;

// #include "readPISOControls.H"
// #include "CourantNo.H"

Source = A* Foam::cos(f * runTime.time().value());

tmp<fvVectorMatrix> EEqn
(
epsilon0*fvm::ddt(E)==fvc::curl(H)

);
// EEqn().relax();
EEqn().solve();


tmp<fvVectorMatrix> HEqn
(
mu*fvm::ddt(H)== -fvc::curl(E)+Source


);
// HEqn().relax();
HEqn().solve();

The transient form of Maxwell equations. When I put the Source term there are compiler's error. Is there any manual or something for general treatment of source terms?

[akidess]

Originally Posted by libe

...
volScalarField Source = A* Foam::cos(f * runTime.time().value());
...

What errors do you get?

[libe]

When I am using the lines that you mentioned at the creatField.H i take the following message

createFields.H:50: error: no matching function for call to ‘Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricField(const char [7], Foam::doubleScalar)’
/home/stagiere/OpenFOAM/OpenFOAM-1.7.1/src/OpenFOAM/lnInclude/GeometricField.C:652: note: candidates are: Foam::GeometricField<Type, PatchField, GeoMesh>::GeometricField(const Foam::IOobject&, const Foam::GeometricField<Type, PatchField, GeoMesh>&, const Foam::wordList&) [with Type = double, PatchField = Foam::fvPatchField, GeoMesh = Foam::volMesh]
/home/stagiere/OpenFOAM/OpenFOAM-1.7.1/src/OpenFOAM/lnInclude/GeometricField.C:617: note: Foam::GeometricField<Type, PatchField, GeoMesh>::GeometricField(const Foam::IOobject&, const Foam::GeometricField<Type, PatchField, GeoMesh>&, const Foam::word&) [with Type = double, PatchField = Foam::fvPatchField, GeoMesh = Foam::volMesh]
/home/stagiere/OpenFOAM/OpenFOAM-1.7.1/src/OpenFOAM/lnInclude/GeometricField.C:587: note: Foam::GeometricField<Type, PatchField, GeoMesh>::GeometricField(const Foam::word&, const Foam::tmp<Foam::GeometricField<Type, PatchField, GeoMesh> >&) [with Type = double, PatchField = Foam::fvPatchField, GeoMesh = Foam::volMesh]

[libe]

when i am using the code u mentioned at the solver file myMycro.C I take:

myMicro.C:57: error: conversion from ‘Foam::doubleScalar’ to non-scalar type ‘Foam::volScalarField’ requested
/home/stagiere/OpenFOAM/OpenFOAM-1.7.1/src/finiteVolume/lnInclude/initContinuityErrs.H:37: warning: unused variable ‘cumulativeContErr’
make: *** [Make/linux64GccDPOpt/myMicro.o] Error 1

[akidess]

How are A and f defined? Is f a scalar and A a volScalarField?

[libe]

for the moment i remove A and f i let only the cos(t) in order to avoid athor problems.i just examine a very simple form

[akidess]

It can't work like that for two reasons:
1. You are trying to assign a scalar value to a matrix. This is giving you the compiler error. Use

volScalarField Source
    (
        IOobject
        (
            "Source",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::NO_WRITE
        ),
        mesh,
        dimensionedScalar("Source", dimensionSet(0,0,0,0,0,0,0), cos(runTime.time().value()))
    );

2. Using this will probably give you a run time error because the dimensions are not correct. Fill in the proper dimensions in the dimensionSet above and all should be well.

- Anton

[libe]

Thank u Anton very much

[herbert]

Hi,

correct me if I'm wrong, but shouldn't Source be of type volVectorField? Just because it is a source term inside a vector equation.

Regards,
Stefan

[rieuk]

I was thinking the same thing (volVectorField). Also, could someone explain what the difference between runtime.value() and runtime.time().value() is?

[akidess]

Stefan: Yes, I overlooked that this is a vector equation, so I guess the source should be a volVectorField.

Rieuk: If I remember correct former will give you a dimensionedScalar, while the latter expression will give you a raw number.

[rieuk]

Thanks Anton. I've been using runTime.value() all this time assuming it was dimensionless. However wmake gives no dimension errors when compiling...could this be giving me bad solutions?