Difference between revisions of "SimpleFoam"
(→Step by step analysis of the pressure equation) 
(→Step by step analysis of the pressure equation) 

Line 1,008:  Line 1,008:  
We see that fixedFluxPressure boundary condition sets the pressure gradient to the provided value such that the flux on the boundary is that specified by the velocity boundary condition. The pressure gradient is not set directly by the boundaryPatch but is set by the function constrainPressure which is called within the pressure equation.  We see that fixedFluxPressure boundary condition sets the pressure gradient to the provided value such that the flux on the boundary is that specified by the velocity boundary condition. The pressure gradient is not set directly by the boundaryPatch but is set by the function constrainPressure which is called within the pressure equation.  
−  In the next code snippet the pressure equation is solved. Furthermore a face flux <math> \  +  In the next code snippet the pressure equation is solved. Furthermore a face flux <math> \phi_f </math> is generated which is consistent with the pressure equation solved. Note that a very good explanation of the flux operator in OF can be found in https://www.cfdonline.com/Forums/openfoam/114933descriptionfluxmethod.html and is therefore not explained in detail. 
+  
+  The dot product <math> \nabla p_f \cdot \bold{S}_f </math> can be decomposed in following manner: <math> \nabla p_f \cdot \bold{S}_f = \nabla p_f \cdot \bold{E}_f + \nabla p_f \cdot \bold{T}_f </math> where the vector <math> \bold{E}_f </math> is pointing in direction of the two nodes straddling the face and the other one is perpendicular to this direction. The first term in the sum can be computed as function of the two cell center straddling the face and hence can be solved implicitly. The other therm can be written down only in a explicit manner (i.e. it is cast in the source term of the equation). For this reason we need a few iteration if the grid is highly non orthogonal. For details see <ref> Moukalled, F., L. Mangani, and M. Darwish. "The finite volume method in computational fluid dynamics." An Advanced Introduction with OpenFOAM and Matlab (2016): </ref>.  
<br><cpp>  <br><cpp> 
Revision as of 12:39, 22 December 2020
SimpleFoam
SimpleFoam is a steadystate solver for incompressible, turbulent flow, using the SIMPLE (SemiImplicit Method for Pressure Linked Equations) algorithm. In the newer releases it also includes an option to use the SIMPLEC (SemiImplicit 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 nonlinearity 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) 20112018 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 Steadystate 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; //  Pressurevelocity 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
The equation of motion in simpleFoam are written for a moving frame of reference. They are however formulated for the absolute velocity (the derivation of the equations of motion can be found in https://openfoamwiki.net/index.php/See_the_MRF_development and also in https://diglib.tugraz.at/download.php?id=581303c7c91f9&location=browse. Some additional information can be found in https://pingpong.chalmers.se/public/pp/public_courses/course07056/published/1497955220499/resourceId/3711490/content/UploadedResources/HakanNilssonRotatingMachineryTrainingOFW111.pdf):

 (1) 
represent the absolute velocity, the relative veloicty, the angular velocity of the rotating fram of reference and and are the viscose and turbulent stresses. Not that in simpleFoam the momentum equation solve, is divided by the constant density . Note that since the relative velocity appears in the divergence term, the face flux appearing in the finite volume discretization of the momentum equation should be calculated with the relative velocity.
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); }
The source code of the acceleration resulting from the description in a moving frame of reference can be found in the following src/finiteVolume/cfdTools/general/MRF/MRFZoneList.C
Foam::tmp<Foam::volVectorField> Foam::MRFZoneList::DDt ( const volVectorField& U ) const { tmp<volVectorField> tacceleration ( new volVectorField ( IOobject ( "MRFZoneList:acceleration", U.mesh().time().timeName(), U.mesh() ), U.mesh(), dimensionedVector(U.dimensions()/dimTime, Zero) ) ); volVectorField& acceleration = tacceleration.ref(); forAll(*this, i) { operator[](i).addCoriolis(U, acceleration); } return tacceleration; }
The calculation of the Coriolis force is done in the file src/finiteVolume/cfdTools/general/MRF/MRFZone.C
void Foam::MRFZone::addCoriolis ( const volVectorField& U, volVectorField& ddtU ) const { if (cellZoneID_ == 1) { return; } const labelList& cells = mesh_.cellZones()[cellZoneID_]; vectorField& ddtUc = ddtU.primitiveFieldRef(); const vectorField& Uc = U; const vector Omega = this>Omega(); forAll(cells, i) { label celli = cells[i]; ddtUc[celli] += (Omega ^ Uc[celli]); } }
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 :
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 ^{[1]}. ):
 (2) 
are the matrix coefficient associated with the centre point P, the matrix coefficients associated with all neighbours influencing the computational stencil around point P and is the source therm. The sum is taken over all neighbours influencing the computational stencil around point P.
The next step performed is the under relax the equation:
UEqn.relax();
The under relaxation is required in order to prevent the solution to diverge. Even though the discrete equation of the momentum
equation is linear, the non linearity is resolve by using the solution of the previous iteration. This causes a large change of the new velocity leading often to divergence ^{[2]}. Using Patankar's implicit under relaxation the new semi discrete momentum equation can be written as:
 (3) 
Here denotes the under relaxation factor and denotes the solution at the previous iteration step. The source code for the under relaxation can be found in fvMatrix.C (see also https://www.openfoam.com/documentation/cppguide/html/fvMatrix_8C_source.html):
template<class Type> void Foam::fvMatrix<Type>::relax(const scalar alpha) { if (alpha <= 0) { return; } if (debug) { InfoInFunction << "Relaxing " << psi_.name() << " by " << alpha << endl; } Field<Type>& S = source(); scalarField& D = diag(); // Store the current unrelaxed diagonal for use in updating the source scalarField D0(D); // Calculate the summag offdiagonal from the interior faces scalarField sumOff(D.size(), 0.0); sumMagOffDiag(sumOff); // Handle the boundary contributions to the diagonal forAll(psi_.boundaryField(), patchi) { const fvPatchField<Type>& ptf = psi_.boundaryField()[patchi]; if (ptf.size()) { const labelUList& pa = lduAddr().patchAddr(patchi); Field<Type>& iCoeffs = internalCoeffs_[patchi]; if (ptf.coupled()) { const Field<Type>& pCoeffs = boundaryCoeffs_[patchi]; // For coupled boundaries add the diagonal and // offdiagonal contributions forAll(pa, face) { D[pa[face]] += component(iCoeffs[face], 0); sumOff[pa[face]] += mag(component(pCoeffs[face], 0)); } } else { // For noncoupled boundaries add the maximum magnitude diagonal // contribution to ensure stability forAll(pa, face) { D[pa[face]] += cmptMax(cmptMag(iCoeffs[face])); } } } } if (debug) { // Calculate amount of nondominance. label nNon = 0; scalar maxNon = 0.0; scalar sumNon = 0.0; forAll(D, celli) { scalar d = (sumOff[celli]  D[celli])/mag(D[celli]); if (d > 0) { nNon++; maxNon = max(maxNon, d); sumNon += d; } } reduce(nNon, sumOp<label>(), UPstream::msgType(), psi_.mesh().comm()); reduce ( maxNon, maxOp<scalar>(), UPstream::msgType(), psi_.mesh().comm() ); reduce ( sumNon, sumOp<scalar>(), UPstream::msgType(), psi_.mesh().comm() ); sumNon /= returnReduce ( D.size(), sumOp<label>(), UPstream::msgType(), psi_.mesh().comm() ); InfoInFunction << "Matrix dominance test for " << psi_.name() << nl << " number of nondominant cells : " << nNon << nl << " maximum relative nondominance : " << maxNon << nl << " average relative nondominance : " << sumNon << nl << endl; } // Ensure the matrix is diagonally dominant... // Assumes that the central coefficient is positive and ensures it is forAll(D, celli) { D[celli] = max(mag(D[celli]), sumOff[celli]); } // ... then relax D /= alpha; // Now remove the diagonal contribution from coupled boundaries forAll(psi_.boundaryField(), patchi) { const fvPatchField<Type>& ptf = psi_.boundaryField()[patchi]; if (ptf.size()) { const labelUList& pa = lduAddr().patchAddr(patchi); Field<Type>& iCoeffs = internalCoeffs_[patchi]; if (ptf.coupled()) { forAll(pa, face) { D[pa[face]] = component(iCoeffs[face], 0); } } else { forAll(pa, face) { D[pa[face]] = cmptMin(iCoeffs[face]); } } } } // Finally add the relaxation contribution to the source. S += (D  D0)*psi_.primitiveField(); }
After the under relaxation the contribution of the pressure gradient is added to the right hand side of the matrix and the system is solve:
solve(UEqn == fvc::grad(p));
The equation in semi discrete form looks as follows:
 (4) 
denotes the contribution of the pressure gradient to the equation of the cell centre p. It depends on the scheme chosen to discretize the gradient operator.
Important for the understanding of the later described pressure equation is that the contribution of the pressure equation is not added to the source therm of the
matrix object UEqn. Rather a new fvMatrix object is returned by the call of the overloaded operator == to the function solve:
UEqn == fvc::grad(p)
The function solve is then executed, which solves the new fvMatrix object in order to obtain the estimate by also considering the contribution of the pressure equation. Note that the the volVectorField U is modified by solving the matrix since the solution vector of the matrix is a reference to U. An explanation of the the implementation can be found also in https://www.cfdonline.com/Forums/openfoam/213566whysolveueqnfvcgradpueqnsourcenotmodifiedueqnhchang.html.
2.2 Pressure Equation
In this section the pressure equation solved in simpleFoam in order to ensure the mass conservation is derived. A good explanation of the derivation of the SIMPLE and also SIMPLEC method in simpleFoam can be found also in http://hobbyfoam.blogspot.com/2016/01/simplecalgorithmofopenfoam.html.
Starting point for the derivation of the pressure equation is the momentum equation in semi discrete form after the solution of the momentum equation:
 (5) 
After dividing the above equation by we obtain:
 (6) 
Note that according to https://openfoamwiki.net/index.php/See_the_MRF_development and also in https://diglib.tugraz.at/download.php?id=581303c7c91f9&location=browse the continuity equation is the same for the relative velocity described in a reference frame subject to a rigid body motion and the velocity described in an inertial frame of reference. For that reason the following equation are valid for the relative velocity and also the absolute velocity . is the vector from the center of rotation to the position of interest. For this reason we get the equations solve in the case of a moving reference frame simply by adding the term on both sides of equation (6) and continue with the same procedure as described in the following.
are the modified diagonal coefficients of the matrix after the under relaxation.
The scope of the next step is to find a correction for the velocity and for the pressure in order to find a velocity which satisfies the continuum equation:
 (7) 
The equation for the velocity correction can be written as:
 (8) 
Note that here it is assumed that the diagonal coefficients of the corrector equation are the same as in the momentum equation previously solved. Taking the divergence of the above equation and setting it to zero (we want to obtain a velocity field which satisfies the continuity equation) we get an equation for the pressure :
 (9) 
denotes the values evaluated at the face.
2.2.1 Simple
If we neglect the contribution of the neighbours of the velocity correction (i.e. we set ) we get the pressure equation solved in the simplec algorithm:
 (10) 
The source code can be found in pEqn.H:
{ volScalarField rAU(1.0/UEqn.A()); volVectorField HbyA(constrainHbyA(rAU*UEqn.H(), U, p)); surfaceScalarField phiHbyA("phiHbyA", fvc::flux(HbyA)); MRF.makeRelative(phiHbyA); adjustPhi(phiHbyA, U, p); tmp<volScalarField> rAtU(rAU); if (simple.consistent()) { rAtU = 1.0/(1.0/rAU  UEqn.H1()); phiHbyA += fvc::interpolate(rAtU()  rAU)*fvc::snGrad(p)*mesh.magSf(); HbyA = (rAU  rAtU())*fvc::grad(p); } tUEqn.clear(); // Update the pressure BCs to ensure flux consistency constrainPressure(p, U, phiHbyA, rAtU(), MRF); // Nonorthogonal pressure corrector loop while (simple.correctNonOrthogonal()) { fvScalarMatrix pEqn ( fvm::laplacian(rAtU(), p) == fvc::div(phiHbyA) ); pEqn.setReference(pRefCell, pRefValue); pEqn.solve(); if (simple.finalNonOrthogonalIter()) { phi = phiHbyA  pEqn.flux(); } } #include "continuityErrs.H" // Explicitly relax pressure for momentum corrector p.relax(); // Momentum corrector U = HbyA  rAtU()*fvc::grad(p); U.correctBoundaryConditions(); fvOptions.correct(U); }
2.2.2 Simplec
The starting point for the simplec algorithm is the equation for the velocity correction. The goal is the obtain a simplification to get an explicit relation for the velocity correction and hence avoiding to solve a matrix equation:
 (11) 
Inserting the above approximation into the equation for the velocity correction we get:
 (12) 
Solving for the velocity correction:
 (13) 
The above equation formulates an explicit relation between velocity correction and pressure correction. In the next step we write down:
 (14) 
By taking the divergence of the above equation and setting it to zero we obtain the pressure equation for the simplec algorithm:
 (15) 
The difference between the pressure equation in the SIMPLE and SIMPLEC consists only in one term.
The source code for the pressure equation can be seen here:
volScalarField rAU(1.0/UEqn.A()); volVectorField HbyA(constrainHbyA(rAU*UEqn.H(), U, p)); surfaceScalarField phiHbyA("phiHbyA", fvc::flux(HbyA)); MRF.makeRelative(phiHbyA); adjustPhi(phiHbyA, U, p); tmp<volScalarField> rAtU(rAU); if (simple.consistent()) { rAtU = 1.0/(1.0/rAU  UEqn.H1()); phiHbyA += fvc::interpolate(rAtU()  rAU)*fvc::snGrad(p)*mesh.magSf(); HbyA = (rAU  rAtU())*fvc::grad(p); } tUEqn.clear(); // Update the pressure BCs to ensure flux consistency constrainPressure(p, U, phiHbyA, rAtU(), MRF); // Nonorthogonal pressure corrector loop while (simple.correctNonOrthogonal()) { fvScalarMatrix pEqn ( fvm::laplacian(rAtU(), p) == fvc::div(phiHbyA) ); pEqn.setReference(pRefCell, pRefValue); pEqn.solve(); if (simple.finalNonOrthogonalIter()) { phi = phiHbyA  pEqn.flux(); } } #include "continuityErrs.H" // Explicitly relax pressure for momentum corrector p.relax(); // Momentum corrector U = HbyA  rAtU()*fvc::grad(p); U.correctBoundaryConditions(); fvOptions.correct(U); }
2.2.3 Step by step analysis of the pressure equation
In this section we will analyze step by step the pressure equation since this source code does not solve only the pressure equation but executes also the corrector step for the velocity (which is used as initial guess for the solution of the momentum equation in the next iteration step) and for the face flux which is used to discretize the convective terms in the momentum equation.
volScalarField rAU(1.0/UEqn.A());
This line computes the field of diagonal entries of the momentum equation required later on to solve the pressure equation:
Since the reciprocal of the diagonal is required a few times, the division is done once and then it is multiplied where required. This is done since the multiplication are computationally cheaper than the division.
volVectorField HbyA(constrainHbyA(rAU*UEqn.H(), U, p));
The source code can be found in the file $FOAM_SCR/finiteVolume/cfdTools/general/constrainHbyA/constrainHbyA.C
Foam::tmp<Foam::volVectorField> Foam::constrainHbyA ( const tmp<volVectorField>& tHbyA, const volVectorField& U, const volScalarField& p ) { tmp<volVectorField> tHbyANew; if (tHbyA.isTmp()) { tHbyANew = tHbyA; tHbyANew.ref().rename("HbyA"); } else { tHbyANew = new volVectorField("HbyA", tHbyA); } volVectorField& HbyA = tHbyANew.ref(); volVectorField::Boundary& HbyAbf = HbyA.boundaryFieldRef(); forAll(U.boundaryField(), patchi) { if ( !U.boundaryField()[patchi].assignable() && !isA<fixedFluxExtrapolatedPressureFvPatchScalarField> ( p.boundaryField()[patchi] ) ) { HbyAbf[patchi] = U.boundaryField()[patchi]; } } return tHbyANew; }
The velocity at the boundary face should satisfy following equation:

The subscript bf denoted that the quantity is evaluated at the boundary face. The function constrainHbyA ensures that the field does not violate the above equation. The boundary condition fixedFluxExtrapolatedPressure sets the pressure gradient in order that the above equation is satisfied. If we cannot modify the velocity, the function sets the field \frac{\bold {H[u] }}{a_P }_{bf} = \bold{u}_{bf} </math> in order that the field does not contradict the zero gradient boundary condition which should be applied for the pressure if the velocity is fixed.
surfaceScalarField phiHbyA("phiHbyA", fvc::flux(HbyA));
The above function performs the following operation:
It interpolates the field at the cell faces and makes than the scalar product of the interpolated field with the surface vector . The source can be found in $FOAM_SCR/finiteVolume/finiteVolume/fvc/fvcFlux.C
Foam::tmp<Foam::surfaceScalarField> Foam::fvc::flux ( const volVectorField& vvf ) { return scheme<vector> ( vvf.mesh(), "flux(" + vvf.name() + ')' )().dotInterpolate(vvf.mesh().Sf(), vvf); }
In a grid which is not deforming and moves with a moving frame of reference the continuity equation has to be satisfied within this grid. This means that the sum of the relative fluxes over the control volumes have to be zero:
is the vector pointing from the origin of the rotation to the face center.
MRF.makeRelative(phiHbyA);
The source code can be found in $FOAM_SCR/cfdTools/general/MRF/MRFZoneTemplates.C and $FOAM_SCR/cfdTools/general/MRF/MRFZone.C
void Foam::MRFZone::makeRelative(surfaceScalarField& phi) const { makeRelativeRhoFlux(geometricOneField(), phi); } template<class RhoFieldType> void Foam::MRFZone::makeRelativeRhoFlux ( const RhoFieldType& rho, surfaceScalarField& phi ) const { if (!active_) { return; } const surfaceVectorField& Cf = mesh_.Cf(); const surfaceVectorField& Sf = mesh_.Sf(); const vector Omega = omega_>value(mesh_.time().timeOutputValue())*axis_; const vectorField& Cfi = Cf; const vectorField& Sfi = Sf; scalarField& phii = phi.primitiveFieldRef(); // Internal faces forAll(internalFaces_, i) { label facei = internalFaces_[i]; phii[facei] = rho[facei]*(Omega ^ (Cfi[facei]  origin_)) & Sfi[facei]; } makeRelativeRhoFlux(rho.boundaryField(), phi.boundaryFieldRef()); }
This call ensures that the global mass balance is satisfied if one sets a refence pressure. For more details see the thread https://www.cfdonline.com/Forums/openfoamprogrammingdevelopment/83876prefadjustphi.html.
adjustPhi(phiHbyA, U, p);
tmp<volScalarField> rAtU(rAU);
This if condition computes the fields required for the simplec method.
Furthermore it already adds the velocity correction to the field HbyA.
This field is later used to compute the corrected velocity to be used as initial condition for the next iteration of the momentum equation.
if (simple.consistent()) { rAtU = 1.0/(1.0/rAU  UEqn.H1()); phiHbyA += fvc::interpolate(rAtU()  rAU)*fvc::snGrad(p)*mesh.magSf(); HbyA = (rAU  rAtU())*fvc::grad(p); } tUEqn.clear();
This function updates the pressure gradient for the patches where a fixedFluxPressure boundary condition is chosen
// Update the pressure BCs to ensure flux consistency constrainPressure(p, U, phiHbyA, rAtU(), MRF);
For the simple method the velocity at point P con be written:
For the simplec method the velocity obtains following expression:
If we add to the above expression and make the dot product with the surface are vector we get for the simple method
and for the simplec method
Finally we rearrange for the pressure gradient, divide by the magnitude of the surface are vector and evaluate at the boundary we get (see also https://caefn.com/openfoam/solversrecentchanges):
The source code can be found in $FOAM_SRC/finiteVolume/cfdTools/general/constrainPressure/constrainPressure.C:
template<class RAUType, class MRFType> void Foam::constrainPressure ( volScalarField& p, const volVectorField& U, const surfaceScalarField& phiHbyA, const RAUType& rAU, const MRFType& MRF ) { constrainPressure(p, geometricOneField(), U, phiHbyA, rAU, MRF); } template<class RhoType, class RAUType, class MRFType> void Foam::constrainPressure ( volScalarField& p, const RhoType& rho, const volVectorField& U, const surfaceScalarField& phiHbyA, const RAUType& rhorAU, const MRFType& MRF ) { const fvMesh& mesh = p.mesh(); volScalarField::Boundary& pBf = p.boundaryFieldRef(); const volVectorField::Boundary& UBf = U.boundaryField(); const surfaceScalarField::Boundary& phiHbyABf = phiHbyA.boundaryField(); const typename RAUType::Boundary& rhorAUBf = rhorAU.boundaryField(); const surfaceVectorField::Boundary& SfBf = mesh.Sf().boundaryField(); const surfaceScalarField::Boundary& magSfBf = mesh.magSf().boundaryField(); forAll(pBf, patchi) { if (isA<fixedFluxPressureFvPatchScalarField>(pBf[patchi])) { refCast<fixedFluxPressureFvPatchScalarField> ( pBf[patchi] ).updateSnGrad ( ( phiHbyABf[patchi]  rho.boundaryField()[patchi] *MRF.relative(SfBf[patchi] & UBf[patchi], patchi) ) /(magSfBf[patchi]*rhorAUBf[patchi]) ); } } }
We see that fixedFluxPressure boundary condition sets the pressure gradient to the provided value such that the flux on the boundary is that specified by the velocity boundary condition. The pressure gradient is not set directly by the boundaryPatch but is set by the function constrainPressure which is called within the pressure equation.
In the next code snippet the pressure equation is solved. Furthermore a face flux is generated which is consistent with the pressure equation solved. Note that a very good explanation of the flux operator in OF can be found in https://www.cfdonline.com/Forums/openfoam/114933descriptionfluxmethod.html and is therefore not explained in detail.
The dot product can be decomposed in following manner: where the vector is pointing in direction of the two nodes straddling the face and the other one is perpendicular to this direction. The first term in the sum can be computed as function of the two cell center straddling the face and hence can be solved implicitly. The other therm can be written down only in a explicit manner (i.e. it is cast in the source term of the equation). For this reason we need a few iteration if the grid is highly non orthogonal. For details see ^{[3]}.
// Nonorthogonal pressure corrector loop while (simple.correctNonOrthogonal()) { fvScalarMatrix pEqn ( fvm::laplacian(rAtU(), p) == fvc::div(phiHbyA) ); pEqn.setReference(pRefCell, pRefValue); pEqn.solve(); if (simple.finalNonOrthogonalIter()) { phi = phiHbyA  pEqn.flux(); } }
This file writes the continuity error on the screen.
#include "continuityErrs.H"
// Explicitly relax pressure for momentum corrector p.relax();
// Momentum corrector U = HbyA  rAtU()*fvc::grad(p); U.correctBoundaryConditions(); fvOptions.correct(U); }
2.3 Avoiding checker boarder effects
The usual way to avoid the so called "checker board" effect is to interpolate the velocities at the faces by means of the Rhie and Chow interpolation (see e.g. ^{[4]} or ^{[5]}. ) . The checker board effect has its origin in the absence of neighbouring pressure terms in the momentum equation due to the discretization of the pressure gradient term in the frame of the finite volume method using a collocated variable arrangement. The same absence of neighbouring pressure terms is obtained when the Laplacian term is discretized by linear interpolation of the pressure gradient on the face centres. In the implementation of the simpleFoam solver, the Rhie and Chow interpolation is not done in an explicit way. The introduction of neighbour pressure terms in the momentum and pressure equation is done in the spirit of Rhie and Chow ^{[6]} . It is achieved by two contribution: The first one is the way the Laplacian term is disretized (see also http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2007/rhiechow.pdf). The second contribution is achieved by the flux() operator after the solution of the pressure equation:
if (simple.finalNonOrthogonalIter()) { phi = phiHbyA  pEqn.flux(); }
The principle of how the pressure oscillations are avoided in simpleFoam are explained by means of a simple 1D convection equation:
 (16) 
The above equation is to be discretized on a equidistant grid:
              WW ww W w P e E ee  EE              
The usual geographic notation is adoped to describe the discretization stencil around the point P for which the solution has to be obtained.
The discretization with a finite volume method leads to the following equation:
 (17) 
is the phase flux and is computed from the previous iteration in order to resolve the nonlinearity in the momentum equation. Evaluating the above sum for the central point P we get:
 (18) 
With a central discretization of the velocity and pressure at the faces we obtain:
 (19) 
And finally:
 (20) 
It is evident that if no spatial care is taken and the face flux is obtained by linear interpolation of the velocities the velocity at the cell center P is not coupled with the pressure at P but only at the neighboring points E and W. The diagonal coefficient are in this case and the contributions of the neighbor cells are .
In order to understand how the pressure at the cell centre P is cast into the momentum equation it is important to understand how the flux() operator is defined in the fvMatrix class. Note that a very good description can be found in https://www.cfdonline.com/Forums/openfoam/114933descriptionfluxmethod.html. Using the implementation of the flux operator we get the new fluxes at the faces for this example:
 (21) 
 (22) 
Note that the quantities denoted with denote the quantities at the previous iteration and in this illustriously example. Note also that the pressure used to correct the face fluxes come from the solution of the pressure equation. After inserting the two above relations for the phase fluxes on the east and west side of the cell centre in the momentum equation we get:
 (23) 
It evident that by correcting the face fluxes with the flux() operator of the fvMatrix class we obtain a dependency of the velocity at the centre point P from the pressure at the centre point P. Furthermore also the pressure and velocities at the neighbouring points E and W enter the momentum equation.
The second measure undertaken to avoid a decoupling of the pressure at neighbouring points is achieved by the way the Laplacian operator is discretized: It computes the gradient at the cell faces by computing the difference between neighbour and owner cell centre and dividing this difference by the distance between this two points. In this way when the sum of all gradients is taken over the faces of a cell, the computational stencil is much smaller compared with the procedure to interpolated the gradient computed at the cell centre on the faces. Furthermore it involves direct neighbours without alternately skipping neighbours. In this way we obtain the following pressure equation for our simple example:
 (24) 
After interpolating the H operator we get:
 (25) 
and finally:
 (26) 
From the above relation we can clearly see, that with a discretization of the Laplacian operator by interpolating the pressure gradients to the cell centre we would have a pressure stencil involving the points P, WW and EE. Since in the computation of the source term of the pressure equation we have the velocities stored at the points P, WW and EE we would have a complete decoupling of the neighbouring points in the pressure equation. This allows the existence of oscillatory solutions in the discrete case which are not part of the continuous solutions.
2.4 Equations for the turbulence
The way the turbulent stresses enter into the momentum equation is well described here: https://www.openfoam.com/documentation/guides/latest/doc/guideturbulenceras.html.
3 References
 ↑ Moukalled, F., L. Mangani, and M. Darwish. "The finite volume method in computational fluid dynamics." An Advanced Introduction with OpenFOAM and Matlab (2016):
 ↑ Moukalled, F., L. Mangani, and M. Darwish. "The finite volume method in computational fluid dynamics." An Advanced Introduction with OpenFOAM and Matlab (2016):
 ↑ Moukalled, F., L. Mangani, and M. Darwish. "The finite volume method in computational fluid dynamics." An Advanced Introduction with OpenFOAM and Matlab (2016):
 ↑ Moukalled, F., L. Mangani, and M. Darwish. "The finite volume method in computational fluid dynamics." An Advanced Introduction with OpenFOAM and Matlab (2016):
 ↑ Ferziger, Joel H., and Milovan Peric. Computational methods for fluid dynamics. Springer Science & Business Media, 2012.
 ↑ Jasak, Hrvoje. "Error analysis and estimation for the finite volume method with applications to fluid flows." (1996).