2.2.1.1. LinearAdvectionDiffusionFoam

\[\frac{\partial U}{\partial t}+ c \nabla U = \nu \nabla^2 U\]

Where U is Vector velocity field in 3D i.e. (u v w) & c is constant dimensioned velocity.

2.2.1.1.2. Family of equations.

Name

Equation

Name

Equation

1D First-order Linear Advection
\[\frac{\partial u}{\partial t} + c \frac{\partial u}{\partial x} = 0\]

1D Second-order Linear Diffusion
\[\frac{\partial u}{\partial t} = \nu \frac{\partial^2 u}{\partial x^2}\]

2D First-order Linear Advection
\[ \begin{align}\begin{aligned}\frac{\partial u}{\partial t}+c \frac{\partial u}{\partial x} + c \frac{\partial u}{\partial y} = 0\\\frac{\partial v}{\partial t}+c \frac{\partial v}{\partial x} + c \frac{\partial v}{\partial y} = 0\end{aligned}\end{align} \]

2D Second-order Linear Diffusion
\[ \begin{align}\begin{aligned}\frac{\partial u}{\partial t} = \nu ( \frac{\partial^2 u}{\partial x^2} + \frac{\partial^2 u}{\partial y^2} )\\\frac{\partial v}{\partial t} = \nu ( \frac{\partial^2 v}{\partial x^2} + \frac{\partial^2 v}{\partial y^2} )\end{aligned}\end{align} \]

2.2.1.1.3. Step 1: Understanding modified advection term.

\[\frac{\partial U}{\partial t}+ \nabla c U = \nabla \bullet (\nu \nabla U)= \nu \nabla^2 U\]

In OpenFOAM advection is represented as div(phi,U) where phi = c * face area of cell = flux

2.2.1.1.4. Step 2: Create a base directory for solver.

foamNewApp is script to create template for a new application in easiest way which Creates a directory containing source .C file and Make directory rather than copying/modifying exiting solver code.

For more details

mkdir -p $FOAM_RUN                          // Creates directory "/home/user/OpenFOAM/user-foamVerion/run"
cd $FOAM_RUN                                // Enter into directory
foamNewApp LinearAdvectionDiffusionFoam     // Creates base directory for solver
cd LinearAdvectionDiffusionFoam             // Enter into directory
ls */*                                      // List the contents

In LinearAdvectionDiffusionFoam directory there are files i.e. Make/files, Make/options, LinearAdvectionDiffusionFoam.C

2.2.1.1.5. Step 3: Contents of LinearAdvectionDiffusionFoam.C .

Open file with any text editor or use nano in terminal. Basic header declarations are already present. Add following lines and create a createFields.H file (mind the extension .H).

 1
 2
 3
 4
 5
 6
 7
 8
 9
10
11
12
13
14
15
16
17
18
19
20
 #include "fvCFD.H"
 // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 int main(int argc, char *argv[])
 {
     #include "setRootCase.H"
     #include "createTime.H"
     #include "createMesh.H"    //<----

     #include "createFields.H"  //<----

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

     Info<< nl << "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
         << "  ClockTime = " << runTime.elapsedClockTime() << " s"
         << nl << endl;

     Info<< "End\n" << endl;

     return 0;
 }

2.2.1.1.6. Step 4: Create field and variables (U,c,nu) in createFields.H

Insert the following code in createFields.H file. ‘c’ is defined vector to generalized code.

Note the last line createPhi.H is included and this file is currently not present in base directory.

 1
 2
 3
 4
 5
 6
 7
 8
 9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
 Info<< "Reading transportProperties\n" << endl;

 IOdictionary transportProperties
 (
     IOobject
     (
         "transportProperties",
         runTime.constant(),
         mesh,
         IOobject::MUST_READ_IF_MODIFIED,
         IOobject::NO_WRITE
     )
 );

 dimensionedScalar nu
 (

     transportProperties.lookup("nu")
 );
     // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 dimensionedVector c           // This Block of code just added to code
 (                      // Rest is template in any solver folder i.e. icoFoam

     transportProperties.lookup("c")
 );

 Info<< "Reading field U\n" << endl;

 volVectorField U
 (
     IOobject
     (
         "U",
         runTime.timeName(),
         mesh,
         IOobject::MUST_READ,
         IOobject::AUTO_WRITE
     ),
     mesh
 );


 #include "createPhi.H"               //<------ Note here

2.2.1.1.7. Step 5: About createPhi.H

Copy createPhi.H file to current directory and modified as follows.

cp /opt/openfoam5/src/finiteVolume/cfdTools/incompressible/createPhi.H .

 1
 2
 3
 4
 5
 6
 7
 8
 9
10
11
12
13
14
15
 Info<< "Reading/calculating face flux field phi\n" << endl;

 surfaceScalarField phi
 (
     IOobject
     (
         "phi",
         runTime.timeName(),
         mesh,
         IOobject::READ_IF_PRESENT,
         IOobject::AUTO_WRITE
     ),
     //fvc::flux(U)                           //<--- comment or delete this line
     c & mesh.Sf()                            //<--- modifying definition 'phi'
 );

2.2.1.1.8. Step 6: Adding main code.

Again open LinearAdvectionDiffusionFoam.C file and add/edit following code snippet.

 1
 2
 3
 4
 5
 6
 7
 8
 9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
 Info<< "\nStarting time loop\n" << endl;

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

     #include "CourantNo.H"

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

     fvVectorMatrix UEqn
     (
         fvm::ddt(U)
       + fvm::div(phi, U)
       - fvm::laplacian(nu, U)
     );

     UEqn.solve();

      runTime.write();

      Info<< nl << "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
          << "  ClockTime = " << runTime.elapsedClockTime() << " s"
          << nl << endl;

 }

2.2.1.1.9. Step 7: Compiling code.

OpenFOAM provides wmake system to build a project or application to avoid complex compilation process. Run following command in terminal.

wmake

2.2.1.1.10. Step 8: Testing

Finally solver is ready and time to build a cases for validation. See Test cases