Difference between revisions of "How to add transport of N solutes to icoFoam"

Latest revision as of 11:18, 21 October 2013

Before reading this tutorial, you should first understand how to add temperature to icoFoam. The idea here is the analogous, but in the case of solutions one can have an indefinite number of solutes dissolved in a solvent. The dissolution of different phases is not modelled here, therefore solute concentrations may not increase above solubility saturation (under saturation hypothesis).

1 solutionProperties dictionary

Cavity example of transportIcoFoamN solver.

The solute list containing Fick's Law diffusion coefficients is defined in

case/constant/solutionProperties

Check the example below

sugar
{
    diffusionModel  constant;
    D           D           [0 2 -1 0 0 0 0] 5.2e-10;
}
    
ethanol
{
    diffusionModel  constant;
    D           D           [0 2 -1 0 0 0 0] 1.6e-9;
}
 
N2
{
    diffusionModel  constant;
    D           D           [0 2 -1 0 0 0 0] 3.6e-9;
}

(Obs.: diffusionModel is not used here, but as an exercise you could model a temperature sensitive diffusion or a diffusivity model for turbulent flow, etc.)

2 Time mesh dictionaries

You will have to create field dictionaries for each solute (e.g. sugar, ethanol, etc.). Because each solute field has dimensions of molar concentration (kmol/m³), the field names are defined as "C_{solute}" (e.g. 0/C_sugar).

3 setFields

I used setFields utility to set different concentrations in the internal field. Check

cavity/system/setFieldsDict

4 Container class solute

Now it is a good opportunity learn a little bit of class inheritance. Let's create a container class for each solute, where the diffusivity constants (D) are stored together with the volScalarFields (C_solute). The solute class inherits all properties of volScalarFields -- and was based on the "phase" class used in multiphase solvers.

The inheritance is defined in solute.H by declaring

 
class solute
:
    public volScalarField

The solute is constructed entering the solute dictionary (sub-dictionary in solutionProperties-file) and the mesh.

 
Foam::solute::solute
(
    const dictionary& soluteDict,
    const fvMesh& mesh
)
:
    volScalarField
    (
        IOobject
        (
            "C_" + soluteDict.dictName(),
            mesh.time().timeName(),
            mesh,
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
        ),
        mesh
    ),
    name_("C_" + soluteDict.dictName()),
    soluteDict_(soluteDict),
    D_(soluteDict_.lookup("D")),
    diffusionModel_(soluteDict_.lookup("diffusionModel"))
{
    Info<< "Reading field " << name_ <<"\n" << endl;
}

We are going to dynamically allocate memory to each solute. Therefore we will be using pointers, which makes it interesting to have an instances solute::clone() and solute::iNew.

Finally, don't forget to declare solute in the main solver header.

 
#include "solute.H"

5 createFields.H

First, let's have a look into createFields.H to understand how solutionProperties dictionary and the C_-fields are read.

 
// * * * * * * * * * * * * * Properties fields * * * * * * * * * * * * * * * //
 
Info<< "Reading solutionProperties\n" << endl;
 
IOdictionary solutionProperties
(
    IOobject
    (
        "solutionProperties",
        runTime.constant(),
        mesh,
        IOobject::MUST_READ_IF_MODIFIED,
        IOobject::NO_WRITE
    )
);
 
const wordList soluteNameList(solutionProperties.toc());
 
PtrList<solute> soluteList(soluteNameList.size());
 
forAll(soluteNameList, i)
{
    const word& soluteName = soluteNameList[i];
    const dictionary& soluteDict = solutionProperties.subDict(soluteName);
 
    soluteList.set
    (
        i,
        new solute
        (
            soluteDict,
            mesh
        )
    );
}

IOdictionary::toc() returns a wordList containing the table of contents (toc) of solutionProperties.

Next, a list of pointers to solute class having the size of the number of entries in the solutionProperties dictionary is defined, before dynamically allocating solutes in the list by the "new" operator.

6 Groups for discretization schemes and solution options

We want to play with an indefinite number of N solutes, so it would be very troublesome to handle the solution options of those N solutes in fvSolution and fvSchemes dictionaries. To avoid that we can define the solver group

 
C_solutes 
    {
        solver           BICCG;
        preconditioner   DILU;
        tolerance        1e-7;
        relTol           0;
    };

and the divergent and laplacian schemes:

 
div(phi,C_solutes)      Gauss upwind;

and

 
laplacian(D,C_solutes)    Gauss linear corrected;

The group's dictionaries can be called by the fvm::div and fvm::laplacian and the solver dictionary must be given to fvScalarMatrix::solver (see below).

 
// ---  Mass transport
 
dictionary soluteSolveDict = mesh.solutionDict().subDict("solvers").subDict("C_solutes");
forAll(soluteNameList, i)
{
    fvScalarMatrix MassTransport
    (
          fvm::ddt(soluteList[i])
        + fvm::div(phi, soluteList[i], "div(phi,C_solutes)")
        - fvm::laplacian(soluteList[i].D(), soluteList[i], "laplacian(D,C_solutes)")
    );
 
    MassTransport.solve(soluteSolveDict);
}

6.1 Using POSIX regular expressions

You may also find it useful that OpenFOAM uses regular expressions, for example you can specify:

 
"C_solute1|C_solute2"
{
    solver            BICCG;
    preconditioner   DILU;
    tolerance        1e-7;
    relTol           0;
};

7 Files

Source files and example case: File:TransportIcoFoamN.tar.gz

8 References

• CFD Online forum: Read properties per component from an input file dictionary
• CFD Online forum: lookup non included scalars from a list