Project 1- Creating your own openFOAM solver
step1:- at first we have copied a icoFoam solver from the appication folder to run folder by running thye command
cp -r incompressible/icoFoam/
step2:- we have renamed the solver as scalarFoam.
in that we have files called createFields.H/make/and we have renamed the icofoam.c file as scalarFoam.c
step3:- in above mentioned files at first we need to open an file called createFields.H file added in a scalar term to it (its an temperature parameter)
here how it looks after adding an parameter 's' to it the 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.lookup("nu")
);
Info<< "Reading field p\n" << endl;
volScalarField p
(
IOobject
(
"p",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);
Info<< "Reading field s\n" << endl;
volScalarField s
(
IOobject
(
"s",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);
dimensionedScalar su
(
"su",
dimViscosity,
transportProperties.lookup("su")
);
Info<< "Reading field U\n" << endl;
volVectorField U
(
IOobject
(
"U",
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())step4:- after this above steos we need to add an main scalaer equation in a scalarFoam.C file this were all the test equatuon present.
here how its looks aftwer adding the scalar equation to slover
/---------------------------------------------------------------------------\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Copyright (C) 2011-2018 OpenFOAM Foundation
\\/ M anipulation |
-------------------------------------------------------------------------------
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
scalarFoam
Description
Transient solver for incompressible, laminar flow of Newtonian fluids.
\---------------------------------------------------------------------------/
#include "fvCFD.H"
#include "pisoControl.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
int main(int argc, char *argv[])
{
#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();
if (piso.finalNonOrthogonalIter())
{
phi = phiHbyA - pEqn.flux();
}
}
#include "continuityErrs.H"
U = HbyA - rAU*fvc::grad(p);
U.correctBoundaryConditions();
}
//scalar transport equation
fvScalarMatrix sEqn
(
fvm::ddt(s)
+ fvm::div(phi, s)
- fvm::laplacian(su, s)
);
sEqn.relax();
sEqn.solve();
runTime.write();
Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
<< " ClockTime = " << runTime.elapsedClockTime() << " s"
<< nl << endl;
}
Info<< "End\n" << endl;
return 0;
}
// ************************* //step 5:- after adding a slover to the scalarFoam.C file we need to save this solver in an USER_APPBIN folder my makeing changes in 'Make' file that to in Files folder by writing the EXE file like this
scalarFoam.C
EXE = $(FOAM_USER_APPBIN)/scalarFoam.
step6:- after make changes in the all required files we need to run a command called wmake.by this means our own solver is created and its ready to use in any case
step7:- in this stage we need to copy a case from tutoriouls folder to run folder and rename it as scalarcavity.after copying the file to run folder we need to create a 's' file in '0' folder
below code shows the 's' file in zero folder its been adited as per required
/--------------------------------- C++ -----------------------------------\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 9
\\/ M anipulation |
\---------------------------------------------------------------------------/
FoamFile
{
format ascii;
class volScalarField;
object s;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 1 0 0 0];
internalField uniform 300;
boundaryField
{
movingWall
{
type fixedValue;
value uniform 350.0;
}
fixedWalls
{
type fixedValue;
value uniform 300.0;
}
frontAndBack
{
type empty;
}
}
// ************************* //step8:- in this we need to go to the system folder and look for fvschemes to add up our parameter after adding the required parameters in to the fvschemes file.. this is how it looks
/--------------------------------- C++ -----------------------------------\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 9
\\/ M anipulation |
\---------------------------------------------------------------------------/
FoamFile
{
format ascii;
class dictionary;
location "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default Euler;
}
gradSchemes
{
default Gauss linear;
grad(p) Gauss linear;
}
divSchemes
{
default none;
div(phi,U) Gauss linear;
div(phi,s) Gauss linear;
}
laplacianSchemes
{
default Gauss linear orthogonal;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default orthogonal;
}
// ************************* //step9:- below file shows the fvsolution after adding needed parameter in to that to file
/--------------------------------- C++ -----------------------------------\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 9
\\/ M anipulation |
\---------------------------------------------------------------------------/
FoamFile
{
format ascii;
class dictionary;
location "system";
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;
}
s
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-07;
relTol 0.0;
}
}
PISO
{
nCorrectors 2;
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
}
// ************************* //setp10:- in this steps we are editing the contolDict file for requirement.. here how it looks after editing
/--------------------------------- C++ -----------------------------------\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 9
\\/ M anipulation |
\---------------------------------------------------------------------------/
FoamFile
{
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application scalarFoam;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 0.5;
deltaT 0.005;
writeControl timeStep;
writeInterval 20;
purgeWrite 0;
writeFormat ascii;
writePrecision 6;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
// ************************* //transportproperties file:-
/--------------------------------- C++ -----------------------------------\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 9
\\/ M anipulation |
\---------------------------------------------------------------------------/
FoamFile
{
format ascii;
class dictionary;
location "constant";
object transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
nu [0 2 -1 0 0 0 0] 0.01;
su [0 2 -1 0 0 0 0] 0.002;
// ************************* //step11:- in this step after doing all the required changes into the files we need to run the command of the solver name that is scalarFoam in the terminal window. after that be nned to run a command called blockMesh to create a blockmesh file.
we can check visualy by running a command called paraFoam
below figure shows the result of scalar quantity 's'
above figure show the variable 's' at its intial conditions
figure2:- this is the figure in which the variable 's' in its last time step
figure3:- out put of variable 's' and its graph here 's' is considered as temperature
