OverPimpleDyMFoam

OverPimpleDyMFoam

Transient solver for incompressible flow of Newtonian fluids on a moving mesh using the PIMPLE (merged PISO-SIMPLE) algorithm. Turbulence modelling is generic, i.e. laminar, RAS or LES may be selected.

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 overset method allows to solve the governing equaiton on a set of disjoint meshes, i.e., the meshes are not connected over faces. The coupling between the differnt meshes is done over an implicit interpolation.

The source code can be found in overPimpleDyMFoam.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) 2016-2018 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
    overPimpleDyMFoam
 
Group
    grpIncompressibleSolvers grpMovingMeshSolvers
 
Description
    Transient solver for incompressible flow of Newtonian fluids
    on a moving mesh using the PIMPLE (merged PISO-SIMPLE) algorithm.
 
    Turbulence modelling is generic, i.e. laminar, RAS or LES may be selected.
 
\*---------------------------------------------------------------------------*/
 
#include "fvCFD.H"
#include "dynamicFvMesh.H"
#include "singlePhaseTransportModel.H"
#include "turbulentTransportModel.H"
#include "pimpleControl.H"
#include "fvOptions.H"
 
#include "cellCellStencilObject.H"
#include "zeroGradientFvPatchFields.H"
#include "localMin.H"
#include "interpolationCellPoint.H"
#include "transform.H"
#include "fvMeshSubset.H"
#include "oversetAdjustPhi.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
int main(int argc, char *argv[])
{
    argList::addNote
    (
        "Transient solver for incompressible, turbulent flow"
        " on a moving mesh."
    );
 
    #include "postProcess.H"
 
    #include "setRootCaseLists.H"
    #include "createTime.H"
    #include "createDynamicFvMesh.H"
    #include "initContinuityErrs.H"
 
    pimpleControl pimple(mesh);
 
    #include "createFields.H"
    #include "createUf.H"
    #include "createMRF.H"
    #include "createFvOptions.H"
    #include "createControls.H"
    #include "CourantNo.H"
    #include "setInitialDeltaT.H"
 
    turbulence->validate();
 
    // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
    Info<< "\nStarting time loop\n" << endl;
 
    while (runTime.run())
    {
        #include "readControls.H"
        #include "CourantNo.H"
 
        #include "setDeltaT.H"
 
        ++runTime;
 
        Info<< "Time = " << runTime.timeName() << nl << endl;
 
        bool changed = mesh.update();
 
        if (changed)
        {
            #include "setCellMask.H"
            #include "setInterpolatedCells.H"
 
            surfaceScalarField faceMaskOld
            (
                localMin<scalar>(mesh).interpolate(cellMask.oldTime())
            );
 
            // Zero Uf on old faceMask (H-I)
            Uf *= faceMaskOld;
            // Update Uf and phi on new C-I faces
            Uf += (1-faceMaskOld)*fvc::interpolate(U);
            phi = mesh.Sf() & Uf;
 
            // Zero phi on current H-I
            surfaceScalarField faceMask
            (
                localMin<scalar>(mesh).interpolate(cellMask)
            );
            phi *= faceMask;
        }
 
 
        if (mesh.changing() && correctPhi)
        {
            // Calculate absolute flux from the mapped surface velocity
            #include "correctPhi.H"
        }
 
        // Make the flux relative to the mesh motion
        fvc::makeRelative(phi, U);
 
        if (mesh.changing() && checkMeshCourantNo)
        {
            #include "meshCourantNo.H"
        }
 
        // --- Pressure-velocity PIMPLE corrector loop
        while (pimple.loop())
        {
            #include "UEqn.H"
 
            // --- Pressure corrector loop
            while (pimple.correct())
            {
                #include "pEqn.H"
            }
 
            if (pimple.turbCorr())
            {
                laminarTransport.correct();
                turbulence->correct();
            }
        }
 
        runTime.write();
 
        runTime.printExecutionTime(Info);
    }
 
    Info<< "End\n" << endl;
 
    return 0;
}
 
 
// ************************************************************************* //
 

2 Equations

The equation of motion used in OpenFOAM for moving meshes are written in the Arbitrary-Euler-Lagrange (ALE) formulation. This formulation is one of the most popular if morphing meshes are used to describe the solid body deformation or displacement . If the overset method is used, this formulation avoids to formulate the equation of motion in multiple frames of references \cite{horne2019}. For the derivation of the equation see . The continuity and momentum equation read in this form:

- $\frac{d}{dt}\int\rho dV + \oint\rho \mathbf{n} \cdot (\mathbf{U} - \mathbf{U_g} ) dS = 0.$

(1)

- $\frac{d}{dt}\int\rho \mathbf{U} dV + \oint\rho \bold{n} \cdot (\mathbf{U} - \mathbf{U_g} ) \mathbf{U} dS - \oint \rho \nu \bold{n} \cdot \nabla \mathbf{U} dS + \oint p \bold{n} dS = 0.$

(1)

In the above equations $\U$ is the fluid velocity, $p$ the pressure, $\nu$ the molecular viscosity and $\rho$ the density. The only difference to the equation of motion in a fixed mesh is the introduction of a new variable, i.e. the grid velocity $\mathbf{U_g}$. In order to determine the grid velocity the space conservation law (SCL) has to be solved (see also )

- $\frac{d}{dt}\int dV - \oint \bold{n} \cdot \mathbf{U_g} dS = 0.$

(1)

In order to not introduce additional mass conservation errors, the temporal discretisation of the SCL should be the same as used in the other conservation equation (see also