Project 3- Adding a temperature dictionary to the incompressible icoFoam case to solve the energy equation
Adding a temperature dictionary to the incompressible icoFoam case to solve the energy equation
A pdf file is attached that contains the code in LATEX.
In this project, we are adding a temperature dictionary to the incompressible icoFoam solver to solve for the energy equation.
The following changes are done:
First, copy the icoFoam solver from the solver folder and paste it in the run directory. Rename the icoFoam.C file to icoTempFoam.C .
Next, the following changes are made in the icoTempFoam.C file-we add a fvScalarMatrix(T) to the code to solve for temperature.
icoTempFoam.C
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | www.openfoam.com
\\/ M anipulation |
-------------------------------------------------------------------------------
Copyright (C) 2011-2016 OpenFOAM Foundation
Copyright (C) 2019 OpenCFD Ltd.
-------------------------------------------------------------------------------
License
This file is part of OpenFOAM.
OpenFOAM is free software: you can redistribute it and/or modify it
under the terms of the GNU General Public License as published by
the Free Software Foundation, either version 3 of the License, or
(at your option) any later version.
OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
FITNESS FOR A PARTICULAR PURPOSE. See the GNU General Public License
for more details.
You should have received a copy of the GNU General Public License
along with OpenFOAM. If not, see <http://www.gnu.org/licenses/>.
Application
icoFoam
Group
grpIncompressibleSolvers
Description
Transient solver for incompressible, laminar flow of Newtonian fluids.
\heading Solver details
The solver uses the PISO algorithm to solve the continuity equation:
\f[
\div \vec{U} = 0
\f]
and momentum equation:
\f[
\ddt{\vec{U}}
+ \div \left( \vec{U} \vec{U} \right)
- \div \left(\nu \grad \vec{U} \right)
= - \grad p
\f]
Where:
\vartable
\vec{U} | Velocity
p | Pressure
\endvartable
\heading Required fields
\plaintable
U | Velocity [m/s]
p | Kinematic pressure, p/rho [m2/s2]
\endplaintable
\*---------------------------------------------------------------------------*/
#include "fvCFD.H"
#include "pisoControl.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
int main(int argc, char *argv[])
{
argList::addNote
(
"Transient solver for incompressible, laminar flow"
" of Newtonian fluids."
);
#include "postProcess.H"
#include "addCheckCaseOptions.H"
#include "setRootCaseLists.H"
#include "createTime.H"
#include "createMesh.H"
pisoControl piso(mesh);
#include "createFields.H"
#include "initContinuityErrs.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Info<< "\nStarting time loop\n" << endl;
while (runTime.loop())
{
Info<< "Time = " << runTime.timeName() << nl << endl;
#include "CourantNo.H"
// Momentum predictor
fvVectorMatrix UEqn
(
fvm::ddt(U)
+ fvm::div(phi, U)
- fvm::laplacian(nu, U)
);
if (piso.momentumPredictor())
{
solve(UEqn == -fvc::grad(p));
}
// --- PISO loop
while (piso.correct())
{
volScalarField rAU(1.0/UEqn.A());
volVectorField HbyA(constrainHbyA(rAU*UEqn.H(), U, p));
surfaceScalarField phiHbyA
(
"phiHbyA",
fvc::flux(HbyA)
+ fvc::interpolate(rAU)*fvc::ddtCorr(U, phi)
);
adjustPhi(phiHbyA, U, p);
// Update the pressure BCs to ensure flux consistency
constrainPressure(p, U, phiHbyA, rAU);
// Non-orthogonal pressure corrector loop
while (piso.correctNonOrthogonal())
{
// Pressure corrector
fvScalarMatrix pEqn
(
fvm::laplacian(rAU, p) == fvc::div(phiHbyA)
);
pEqn.setReference(pRefCell, pRefValue);
pEqn.solve(mesh.solver(p.select(piso.finalInnerIter())));
if (piso.finalNonOrthogonalIter())
{
phi = phiHbyA - pEqn.flux();
}
}
#include "continuityErrs.H"
U = HbyA - rAU*fvc::grad(p);
U.correctBoundaryConditions();
}
fvScalarMatrix TEqn
(
fvm::ddt(T)
+ fvm::div(phi, T)
- fvm::laplacian(kappa, T)
);
TEqn.solve();
runTime.write();
runTime.printExecutionTime(Info);
}
Info<< "End\n" << endl;
return 0;
}
// ************************************************************************* //
Next, we add an IOobject for temperature in createFields.H file. We also add dictionary reader for kappa(some scalar)
createFields.H
Info<< "Reading transportProperties\n" << endl;
IOdictionary transportProperties
(
IOobject
(
"transportProperties",
runTime.constant(),
mesh,
IOobject::MUST_READ_IF_MODIFIED,
IOobject::NO_WRITE
)
);
dimensionedScalar nu
(
"nu",
dimViscosity,
transportProperties
);
dimensionedScalar kappa
(
"kappa",
dimViscosity,
transportProperties
);
Info<< "Reading field p\n" << endl;
volScalarField p
(
IOobject
(
"p",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);
Info<< "Reading field U\n" << endl;
volVectorField U
(
IOobject
(
"U",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);
Info<< "Reading field T\n" << endl;
volScalarField T
(
IOobject
(
"T",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);
#include "createPhi.H"
label pRefCell = 0;
scalar pRefValue = 0.0;
setRefCell(p, mesh.solutionDict().subDict("PISO"), pRefCell, pRefValue);
mesh.setFluxRequired(p.name());
Once done, the next step is to change contents in Make/files . Rename thhe solver to icoTempFoam.C and with exe being created to $(FOAM_USER_APPBIN) icoTempFoam
Once done, compile using wmake. The solver is ready to be used.
Test Case
Copy the folder cavity from incompressible/icoFoam tutorial and in the controlDict file, rename the solver to icoTempFoam .
controlDict
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2206 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application icoTempFoam;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 0.5;
deltaT 0.005;
writeControl timeStep;
writeInterval 10;
purgeWrite 0;
writeFormat ascii;
writePrecision 6;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
// ************************************************************************* //In fvSchemes file,Add a div(phi,T) in divSchemes and laplacian(kappa,T) in laplacianSchemes
fvSchemes
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2206 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default Euler;
}
gradSchemes
{
default Gauss linear;
grad(p) Gauss linear;
}
divSchemes
{
default none;
div(phi,U) Gauss linear;
div(phi,T) Gauss linear;
}
laplacianSchemes
{
default Gauss linear orthogonal;
laplacian(kappa,T) Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default orthogonal;
}
// ************************************************************************* //In transport properties file, add the value of kappa, as shown below:
transportProperties
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2206 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
nu 0.01;
kappa [0 2 -1 0 0 0 0] 0.001;
// ************************************************************************* //
In fvSolution, add a smoothSolver linear solver for temperature in fvSolution. Use a tolerance of 1e-07 and a relTol of 0 .
fvSolution
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2206 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
p
{
solver PCG;
preconditioner DIC;
tolerance 1e-06;
relTol 0.05;
}
pFinal
{
$p;
relTol 0;
}
U
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-05;
relTol 0;
}
T
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-07;
relTol 0;
}
}
PISO
{
nCorrectors 2;
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
}
// ************************************************************************* //
Create a new file for temperature so that our solver could read the contents.
T file
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2206 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 1 0 0 0];
internalField uniform 300;
boundaryField
{
movingWall
{
type fixedValue;
value uniform 400;
}
fixedWalls
{
type zeroGradient;
}
frontAndBack
{
type empty;
}
}
Once done, run blockMesh followed by icoTempFoam. Then type foamToVTK to postprocess results and view in paraView.
Temperature animation
Velocity animation
Code in LATEX
\documentclass[12pt]{report}
\usepackage{graphicx} % Required for inserting images
\usepackage{amsfonts,amsmath,amssymb}
\usepackage[margin=1in]{geometry}
\usepackage[inline]{enumitem}
\date{May 2023}
\begin{document}
\begin{center}
\section*{Adding a temperature dictionary to the Incompressible icoFoam solver}
\end{center}
In this project, we are adding a temperature dictionary to the incompressible icoFoam solver to solve for the energy equation.
The following changes are done: First, copy the icoFoam solver from the solver folder and paste it in the run directory. Rename the \texttt{icoFoam.C} file to \texttt{icoTempFoam.C}.
Next, the following changes are made in the \texttt{icoTempFoam.C} file-we add a fvScalarMatrix(T) to the code to solve for temperature.\\
\texttt{icoTempFoam.C}
\begin{verbatim}
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | www.openfoam.com
\\/ M anipulation |
-------------------------------------------------------------------------------
Copyright (C) 2011-2016 OpenFOAM Foundation
Copyright (C) 2019 OpenCFD Ltd.
-------------------------------------------------------------------------------
License
This file is part of OpenFOAM.
OpenFOAM is free software: you can redistribute it and/or modify it
under the terms of the GNU General Public License as published by
the Free Software Foundation, either version 3 of the License, or
(at your option) any later version.
OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
FITNESS FOR A PARTICULAR PURPOSE. See the GNU General Public License
for more details.
You should have received a copy of the GNU General Public License
along with OpenFOAM. If not, see <http://www.gnu.org/licenses/>.
Application
icoFoam
Group
grpIncompressibleSolvers
Description
Transient solver for incompressible, laminar flow of Newtonian fluids.
\heading Solver details
The solver uses the PISO algorithm to solve the continuity equation:
\f[
\div \vec{U} = 0
\f]
and momentum equation:
\f[
\ddt{\vec{U}}
+ \div \left( \vec{U} \vec{U} \right)
- \div \left(\nu \grad \vec{U} \right)
= - \grad p
\f]
Where:
\vartable
\vec{U} | Velocity
p | Pressure
\endvartable
\heading Required fields
\plaintable
U | Velocity [m/s]
p | Kinematic pressure, p/rho [m2/s2]
\endplaintable
\*---------------------------------------------------------------------------*/
#include "fvCFD.H"
#include "pisoControl.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
int main(int argc, char *argv[])
{
argList::addNote
(
"Transient solver for incompressible, laminar flow"
" of Newtonian fluids."
);
#include "postProcess.H"
#include "addCheckCaseOptions.H"
#include "setRootCaseLists.H"
#include "createTime.H"
#include "createMesh.H"
pisoControl piso(mesh);
#include "createFields.H"
#include "initContinuityErrs.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Info<< "\nStarting time loop\n" << endl;
while (runTime.loop())
{
Info<< "Time = " << runTime.timeName() << nl << endl;
#include "CourantNo.H"
// Momentum predictor
fvVectorMatrix UEqn
(
fvm::ddt(U)
+ fvm::div(phi, U)
- fvm::laplacian(nu, U)
);
if (piso.momentumPredictor())
{
solve(UEqn == -fvc::grad(p));
}
// --- PISO loop
while (piso.correct())
{
volScalarField rAU(1.0/UEqn.A());
volVectorField HbyA(constrainHbyA(rAU*UEqn.H(), U, p));
surfaceScalarField phiHbyA
(
"phiHbyA",
fvc::flux(HbyA)
+ fvc::interpolate(rAU)*fvc::ddtCorr(U, phi)
);
adjustPhi(phiHbyA, U, p);
// Update the pressure BCs to ensure flux consistency
constrainPressure(p, U, phiHbyA, rAU);
// Non-orthogonal pressure corrector loop
while (piso.correctNonOrthogonal())
{
// Pressure corrector
fvScalarMatrix pEqn
(
fvm::laplacian(rAU, p) == fvc::div(phiHbyA)
);
pEqn.setReference(pRefCell, pRefValue);
pEqn.solve(mesh.solver(p.select(piso.finalInnerIter())));
if (piso.finalNonOrthogonalIter())
{
phi = phiHbyA - pEqn.flux();
}
}
#include "continuityErrs.H"
U = HbyA - rAU*fvc::grad(p);
U.correctBoundaryConditions();
}
fvScalarMatrix TEqn
(
fvm::ddt(T)
+ fvm::div(phi, T)
- fvm::laplacian(kappa, T)
);
TEqn.solve();
runTime.write();
runTime.printExecutionTime(Info);
}
Info<< "End\n" << endl;
return 0;
}
// ************************************************************************* //
\end{verbatim}
Next, we add an IOobject for temperature in createFields.H file. We also add dictionary reader for kappa(some scalar).\\
\texttt{createFields.H}
\begin{verbatim}
Info<< "Reading transportProperties\n" << endl;
IOdictionary transportProperties
(
IOobject
(
"transportProperties",
runTime.constant(),
mesh,
IOobject::MUST_READ_IF_MODIFIED,
IOobject::NO_WRITE
)
);
dimensionedScalar nu
(
"nu",
dimViscosity,
transportProperties
);
dimensionedScalar kappa
(
"kappa",
dimViscosity,
transportProperties
);
Info<< "Reading field p\n" << endl;
volScalarField p
(
IOobject
(
"p",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);
Info<< "Reading field U\n" << endl;
volVectorField U
(
IOobject
(
"U",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);
Info<< "Reading field T\n" << endl;
volScalarField T
(
IOobject
(
"T",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);
#include "createPhi.H"
label pRefCell = 0;
scalar pRefValue = 0.0;
setRefCell(p, mesh.solutionDict().subDict("PISO"), pRefCell, pRefValue);
mesh.setFluxRequired(p.name());
\end{verbatim}
Make necessary changes in Makefile.
Once done, compile using wmake. The solver is ready to be used.\\
\textbf{Test Case}\\
Copy the folder cavity from incompressible/icoFoam tutorial and in the \texttt{controlDict} file, rename the solver to icoTempFoam .
\begin{verbatim}
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2206 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application icoTempFoam;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 0.5;
deltaT 0.005;
writeControl timeStep;
writeInterval 10;
purgeWrite 0;
writeFormat ascii;
writePrecision 6;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
// ************************************************************************* //
\end{verbatim}
In fvSchemes file,Add a div(phi,T) in divSchemes and laplacian(kappa,T) in laplacianSchemes
\texttt{fvSchemes}
\begin{verbatim}
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2206 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default Euler;
}
gradSchemes
{
default Gauss linear;
grad(p) Gauss linear;
}
divSchemes
{
default none;
div(phi,U) Gauss linear;
div(phi,T) Gauss linear;
}
laplacianSchemes
{
default Gauss linear orthogonal;
laplacian(kappa,T) Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default orthogonal;
}
// ************************************************************************* //
\end{verbatim}
In transport properties file, add the value of kappa, as shown below
\begin{verbatim}
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2206 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
nu 0.01;
kappa [0 2 -1 0 0 0 0] 0.001;
// ************************************************************************* //
\end{verbatim}
In fvSolution, add a smoothSolver linear solver for temperature in fvSolution. Use a tolerance of 1e-07 and a relTol of 0 .
\begin{verbatim}
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2206 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
p
{
solver PCG;
preconditioner DIC;
tolerance 1e-06;
relTol 0.05;
}
pFinal
{
$p;
relTol 0;
}
U
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-05;
relTol 0;
}
T
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-07;
relTol 0;
}
}
PISO
{
nCorrectors 2;
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
}
// ************************************************************************* //
\end{verbatim}
Create a new file for temperature so that our solver could read the contents.
\begin{verbatim}
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2206 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 1 0 0 0];
internalField uniform 300;
boundaryField
{
movingWall
{
type fixedValue;
value uniform 400;
}
fixedWalls
{
type zeroGradient;
}
frontAndBack
{
type empty;
}
}
\end{verbatim}
Once done, run \texttt{blockMesh} followed by \texttt{icoTempFoam}. Then type \texttt{foamToVTK} to postprocess results and view in paraView.
\end{document}