WIP Enh/add non zero bc

[greole]

This PR adds some non-zero initial fields for T and U for the scalarAdvection case. Below are some screenshots of the initial fields of T and U. I'm open to use a different method to generate the fields in order to decrease the file size and make it easier to scale the mesh.

[happyKitesurfer]

I set the T field by the setFields utility: The dictionary looks like this:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2406                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      setFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

defaultFieldValues
(
    volScalarFieldValue T 300
);

regions
(
    boxToCell
    {
        box (0.25 0.75 -1) (0.75 1. 1);
        fieldValues
        (
            volScalarFieldValue T 273
        );
    }
);


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

[greole]

Is there something similar for U though?

[happyKitesurfer]

you can specify a custom inlet profile like this:

boundaryField
{
    #includeEtc "caseDicts/setConstraintTypes"
    
    inlet
    {
        
        name    parabolicInlet;
        type    codedFixedValue;

        code
        #{
            // Uncomment for testing on non-windows systems [fragile]
            // IOobject::scopeSeparator = '_';

            const scalar Q(4.17e-08);
            const scalar maxR(gMax(this->patch().Cf().component(0)));
            scalar vMax;
            vMax = 2.*Q/(M_PI*pow(maxR,2));
            scalarField vz(vMax*(1. -  pow(this->patch().Cf().component(0),2)/pow(maxR,2)));
            

            vectorField v(this->patch().size(), vector(0, 0, 0));
            v.replace(vector::Z, vz);
            operator==(v);
        #};

        value           $internalField;
        
        
    }

Is this what you are looking for? Or do you want to specify the velocity in the whole domain?

[greole]

That looks good. I don't think we have specific needs for the velocity profile, just something that moves the temperature blob.

[happyKitesurfer]

I think then specifying an internal field which is not zero will do the job

[HenningScheufler]

You can also do this with setexprfield

https://www.cfd-online.com/Forums/openfoam-pre-processing/239290-setexprfields.html

[greole]

So here are the expressions used inititially:
for U

Foam::scalarField X(mesh.C().component(0));
Foam::scalarField Y(mesh.C().component(1));
Foam::scalarField u(-Foam::sin(2.0 * pi * Y) * Foam::pow(Foam::sin(pi * X), 2.0));
Foam::scalarField w(Foam::sin(2.0 * pi * X) * Foam::pow(Foam::sin(pi * Y), 2.0));
forAll(U0, celli)
{
       U0[celli].x() = u[celli];
       U0[celli].y() = w[celli];
       U0[celli].z() = 0.0;
}

for T

Foam::scalar spread = 0.05;
forAll(T, celli)
       {
           T[celli] = std::exp(
               -0.5
               * (std::pow((mesh.C()[celli].x() - 0.5) / spread, 2.0)
                  + std::pow((mesh.C()[celli].y() - 0.75) / spread, 2.0))
           );
       }