SimpleFoam

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.

1 Solution Strategy

The solver follows a segregated solution strategy. This means that the equations for each variable characterizing the system (the velocity $\bold u$, the pressure $p$ 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 $\phi_f$ 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 $\bold u^*$ 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 $p^{n}$, which, if inserted in the momentum equation, delivers a divergence free velocity field $\bold u$. 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

$\frac{\partial \left( {u}_j u_i \right) }{\partial x_j}= - \frac{1}{\rho}\frac{\partial p} {\partial{x_i}} + \frac{1}{\rho}\frac{\partial}{\partial x_j} \left( \tau_{ij} + \tau_{t_{ij}} \right)$

(1)

$u$ represent the velocity and $\tau_{ij}$ and $\tau_{t_{ij}}$ are the viscose and turbulent stresses. Not that in simpleFoam the momentum equation solve, is divided by the constant density $\rho$.

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);
    }
 

In the following the numeric used to solve the momentum equation are briefly explained. The first step performed is to assemble the matrix which is later solved to obtain the estimate of the velocity $\bold u^*$:

 
    tmp<fvVectorMatrix> tUEqn
    (
        fvm::div(phi, U)
      + MRF.DDt(U)
      + turbulence->divDevReff(U)
     ==
        fvOptions(U)
    );
 

In the usual semi discrete form it can be written as (see also . ):

$\bold{a_P u_P} + \sum_{N} \bold{a_N u_N} = \bold b_P$

(1)

$\bold a_P$ are the matrix coefficient associated with the centre point P, $\bold a_N$ the matrix coefficients associated with all neighbours influencing the computational stencil around point P and $\bold b_P$ is the source therm. The sum $\sum_N$ is taken over all neighbours influencing the computational stencil around point P.