**SimpleFoam**

SimpleFoam is a steady-state solver for incompressible, turbulent flow, using the SIMPLE (Semi-Implicit Method for Pressure Linked Equations) algorithm. In the newer releases it also includes an option to use the SIMPLEC (Semi-Implicit Method for Pressure Linked Equations Consistent) algorithm.

## Contents

## 1 Solution Strategy

The solver follows a segregated solution strategy. This means that the equations for each variable characterizing the system (the velocity , the pressure and the variables characterizing turbulence) is solved sequentially and the solution of the preceding equations is inserted in the subsequent equation. The non-linearity appearing in the momentum equation (the face flux which is a function of the velocity) is resolved by computing it from the velocity and pressure values of the preceding iteration. The dependence from the pressure is introduced to avoid a decoupling between the momentum and pressure equations and hence the appearance of high frequency oscillation in the solution (check board effect). The first equation to be solve is the momentum equation. It delivers a velocity field which is in general not divergence free, i.e. it does not satisfy the continuity equation. After that the momentum and the continuity equations are used to construct an equation for the pressure. The aim is to obtain a pressure field , which, if inserted in the momentum equation, delivers a divergence free velocity field . After correcting the velocity field, the equations for turbulence are solved. The above iterative solution procedure is repeated until convergence.

The source code can be found in simpleFoam.C

/*---------------------------------------------------------------------------*\ ========= | \\ / 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 simpleFoam Description Steady-state solver for incompressible, turbulent flow, using the SIMPLE algorithm. \*---------------------------------------------------------------------------*/ #include "fvCFD.H" #include "singlePhaseTransportModel.H" #include "turbulentTransportModel.H" #include "simpleControl.H" #include "fvOptions.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // int main(int argc, char *argv[]) { #include "postProcess.H" #include "setRootCaseLists.H" #include "createTime.H" #include "createMesh.H" #include "createControl.H" #include "createFields.H" #include "initContinuityErrs.H" turbulence->validate(); // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Info<< "\nStarting time loop\n" << endl; while (simple.loop(runTime)) { Info<< "Time = " << runTime.timeName() << nl << endl; // --- Pressure-velocity SIMPLE corrector { #include "UEqn.H" #include "pEqn.H" } laminarTransport.correct(); turbulence->correct(); runTime.write(); Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s" << " ClockTime = " << runTime.elapsedClockTime() << " s" << nl << endl; } Info<< "End\n" << endl; return 0; } // ************************************************************************* //

## 2 Equations

### 2.1 Momentum Equation

| (1) |

represent the velocity and and are the viscose and turbulent stresses. Not that in simpleFoam the momentum equation solve, is divided by the constant density .

The source code can be found in UEqn.H:

// Momentum predictor MRF.correctBoundaryVelocity(U); tmp<fvVectorMatrix> tUEqn ( fvm::div(phi, U) + MRF.DDt(U) + turbulence->divDevReff(U) == fvOptions(U) ); fvVectorMatrix& UEqn = tUEqn.ref(); UEqn.relax(); fvOptions.constrain(UEqn); if (simple.momentumPredictor()) { solve(UEqn == -fvc::grad(p)); fvOptions.correct(U); }