zhyang-dev/openfoam
1
0
Fork 0
mirror of https://develop.openfoam.com/Development/openfoam.git synced 2025-11-28 03:28:01 +00:00
Code Issues Actions Packages Projects Releases Wiki Activity

simpleFoam/SRFSimpleFoam: Added support for SIMPLEC

Browse Source 
SIMPLEC (SIMPLE-consistent) is selected by setting "consistent" option true/yes:

SIMPLE
{
    nNonOrthogonalCorrectors 0;
    consistent yes;
}

which relaxes the pressure in a "consistent" manner and additional
relaxation of the pressure is not generally necessary.  In addition
convergence of the p-U system is better and reliable with less
aggressive relaxation of the momentum equation, e.g. for the motorbike
tutorial:

relaxationFactors
{
    equations
    {
        U               0.9;
        k               0.7;
        omega           0.7;
    }
}

The cost per iteration is marginally higher but the convergence rate is
better so the number of iterations can be reduced.

The SIMPLEC algorithm also provides benefit for cases with large
body-forces, e.g. SRF, see tutorials/incompressible/SRFSimpleFoam/mixer
and feature request http://www.openfoam.org/mantisbt/view.php?id=1714
This commit is contained in:
Henry
2015-05-29 11:30:40 +01:00
parent 1971c1eb88
commit 38177526ff
8 changed files with 60 additions and 61 deletions
Download Patch File Download Diff File Expand all files Collapse all files

17
applications/solvers/incompressible/simpleFoam/SRFSimpleFoam/pEqn.H
View File

@ -2,17 +2,28 @@
volScalarField rAUrel(1.0/UrelEqn().A());
volVectorField HbyA("HbyA", Urel);
HbyA = rAUrel*UrelEqn().H();
UrelEqn.clear();
surfaceScalarField phiHbyA("phiHbyA", fvc::interpolate(HbyA) & mesh.Sf());
adjustPhi(phiHbyA, Urel, p);
tmp<volScalarField> rAtUrel(rAUrel);
if (simple.consistent())
{
rAtUrel = 1.0/(1.0/rAUrel - UrelEqn().H1());
phiHbyA +=
fvc::interpolate(rAtUrel() - rAUrel)*fvc::snGrad(p)*mesh.magSf();
HbyA -= (rAUrel - rAtUrel())*fvc::grad(p);
}
UrelEqn.clear();
// Non-orthogonal pressure corrector loop
while (simple.correctNonOrthogonal())
{
fvScalarMatrix pEqn
(
fvm::laplacian(rAUrel, p) == fvc::div(phiHbyA)
fvm::laplacian(rAtUrel(), p) == fvc::div(phiHbyA)
);
pEqn.setReference(pRefCell, pRefValue);
@ -31,7 +42,7 @@
p.relax();
// Momentum corrector
Urel = HbyA - rAUrel*fvc::grad(p);
Urel = HbyA - rAtUrel()*fvc::grad(p);
Urel.correctBoundaryConditions();
fvOptions.correct(Urel);
}

19
applications/solvers/incompressible/simpleFoam/pEqn.H
View File

@ -2,20 +2,29 @@
volScalarField rAU(1.0/UEqn().A());
volVectorField HbyA("HbyA", U);
HbyA = rAU*UEqn().H();
UEqn.clear();
surfaceScalarField phiHbyA("phiHbyA", fvc::interpolate(HbyA) & mesh.Sf());
fvOptions.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);
}
UEqn.clear();
// Non-orthogonal pressure corrector loop
while (simple.correctNonOrthogonal())
{
fvScalarMatrix pEqn
(
fvm::laplacian(rAU, p) == fvc::div(phiHbyA)
fvm::laplacian(rAtU(), p) == fvc::div(phiHbyA)
);
pEqn.setReference(pRefCell, pRefValue);
@ -34,7 +43,7 @@
p.relax();
// Momentum corrector
U = HbyA - rAU*fvc::grad(p);
U = HbyA - rAtU()*fvc::grad(p);
U.correctBoundaryConditions();
fvOptions.correct(U);
}

18
src/finiteVolume/cfdTools/general/solutionControl/solutionControl/solutionControl.C
View File

@ -2,7 +2,7 @@
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 2011 OpenFOAM Foundation
\\ / A nd | Copyright (C) 2011-2015 OpenFOAM Foundation
\\/ M anipulation |
-------------------------------------------------------------------------------
License
@ -37,16 +37,21 @@ namespace Foam
void Foam::solutionControl::read(const bool absTolOnly)
{
const dictionary& solnDict = this->dict();
const dictionary& solutionDict = this->dict();
// Read solution controls
nNonOrthCorr_ =
solnDict.lookupOrDefault<label>("nNonOrthogonalCorrectors", 0);
momentumPredictor_ = solnDict.lookupOrDefault("momentumPredictor", true);
transonic_ = solnDict.lookupOrDefault("transonic", false);
solutionDict.lookupOrDefault<label>("nNonOrthogonalCorrectors", 0);
momentumPredictor_ =
solutionDict.lookupOrDefault("momentumPredictor", true);
transonic_ = solutionDict.lookupOrDefault("transonic", false);
consistent_ = solutionDict.lookupOrDefault("consistent", false);
// Read residual information
const dictionary residualDict(solnDict.subOrEmptyDict("residualControl"));
const dictionary residualDict
(
solutionDict.subOrEmptyDict("residualControl")
);
DynamicList<fieldData> data(residualControl_);
@ -177,6 +182,7 @@ Foam::solutionControl::solutionControl(fvMesh& mesh, const word& algorithmName)
nNonOrthCorr_(0),
momentumPredictor_(true),
transonic_(false),
consistent_(false),
corr_(0),
corrNonOrtho_(0)
{}

10
src/finiteVolume/cfdTools/general/solutionControl/solutionControl/solutionControl.H
View File

@ -2,7 +2,7 @@
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 2011-2012 OpenFOAM Foundation
\\ / A nd | Copyright (C) 2011-2015 OpenFOAM Foundation
\\/ M anipulation |
-------------------------------------------------------------------------------
License
@ -83,6 +83,10 @@ protected:
//- Flag to indicate to solve using transonic algorithm
bool transonic_;
//- Flag to indicate to relax pressure using the
// "consistent" approach of SIMPLEC
bool consistent_;
// Evolution
@ -169,6 +173,10 @@ public:
//- Flag to indicate to solve using transonic algorithm
inline bool transonic() const;
//- Flag to indicate to relax pressure using the
// "consistent" approach of SIMPLEC
inline bool consistent() const;
// Evolution

8
src/finiteVolume/cfdTools/general/solutionControl/solutionControl/solutionControlI.H
View File

@ -2,7 +2,7 @@
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 2011 OpenFOAM Foundation
\\ / A nd | Copyright (C) 2011-2015 OpenFOAM Foundation
\\/ M anipulation |
-------------------------------------------------------------------------------
License
@ -67,6 +67,12 @@ inline bool Foam::solutionControl::transonic() const
}
inline bool Foam::solutionControl::consistent() const
{
return consistent_;
}
inline bool Foam::solutionControl::correctNonOrthogonal()
{
corrNonOrtho_++;

12
tutorials/incompressible/SRFSimpleFoam/mixer/system/fvSolution
View File

@ -37,22 +37,14 @@ solvers
SIMPLE
{
nNonOrthogonalCorrectors 0;
consistent yes;
}
relaxationFactors
{
fields
{
p 0.3;
}
equations
{
Urel 0.7;
k 0.7;
epsilon 0.7;
omega 0.7;
R 0.7;
nuTilda 0.7;
".*" 0.9;
}
}

30
tutorials/incompressible/SRFSimpleFoam/mixer/turbulenceProperties
View File

@ -1,30 +0,0 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
simulationType RAS;
RAS
{
RASModel kOmegaSST;
turbulence on;
printCoeffs on;
}
// ************************************************************************* //

7
tutorials/incompressible/simpleFoam/motorBike/system/fvSolution
View File

@ -66,6 +66,7 @@ solvers
SIMPLE
{
nNonOrthogonalCorrectors 0;
consistent yes;
}
potentialFlow
@ -75,13 +76,9 @@ potentialFlow
relaxationFactors
{
fields
{
p 0.3;
}
equations
{
U 0.7;
U 0.9;
k 0.7;
omega 0.7;
}