zhyang-dev/OpenFOAM-6
1
0
Fork 0
mirror of https://github.com/OpenFOAM/OpenFOAM-6.git synced 2025-12-08 06:57:46 +00:00
Code Issues Actions Packages Projects Releases Wiki Activity

rhoSimpleFoam: added support for compressible liquid flows

Browse Source 
rhoSimpleFoam now instantiates the lower-level fluidThermo which instantiates
either a psiThermo or rhoThermo according to the 'type' specification in
thermophysicalProperties, e.g.

thermoType
{
    type            hePsiThermo;
    mixture         pureMixture;
    transport       sutherland;
    thermo          janaf;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleInternalEnergy;
}

instantiates a psiThermo for a perfect gas with JANAF thermodynamics, whereas

thermoType
{
    type            heRhoThermo;
    mixture         pureMixture;
    properties      liquid;
    energy          sensibleInternalEnergy;
}

mixture
{
    H2O;
}

instantiates a rhoThermo for water, see new tutorial
compressible/rhoSimpleFoam/squareBendLiq.

In order to support complex equations of state the pressure can no longer be
unlimited and rhoSimpleFoam now limits the pressure rather than the density to
handle start-up more robustly.

For backward compatibility 'rhoMin' and 'rhoMax' can still be used in the SIMPLE
sub-dictionary of fvSolution which are converted into 'pMax' and 'pMin' but it
is better to set either 'pMax' and 'pMin' directly or use the more convenient
'pMinFactor' and 'pMinFactor' from which 'pMax' and 'pMin' are calculated using
the fixed boundary pressure or reference pressure e.g.

SIMPLE
{
    nNonOrthogonalCorrectors 0;

    pMinFactor      0.1;
    pMaxFactor      1.5;

    transonic       yes;
    consistent      yes;

    residualControl
    {
        p               1e-3;
        U               1e-4;
        e               1e-3;
        "(k|epsilon|omega)" 1e-3;
    }
}
This commit is contained in:
Henry Weller
2017-02-24 11:18:01 +00:00
parent cb2bc60fa5
commit 655fc78748
35 changed files with 1115 additions and 123 deletions
Download Patch File Download Diff File Expand all files Collapse all files

4
tutorials/compressible/rhoPorousSimpleFoam/angledDuctExplicit/system/fvSolution
View File

@ -54,8 +54,8 @@ solvers
SIMPLE
{
nNonOrthogonalCorrectors 0;
rhoMin 0.5;
rhoMax 1.5;
pMinFactor 0.5;
pMaxFactor 1.5;
residualControl
{

4
tutorials/compressible/rhoPorousSimpleFoam/angledDuctImplicit/system/fvSolution
View File

@ -48,8 +48,8 @@ SIMPLE
{
nUCorrectors 2;
nNonOrthogonalCorrectors 0;
rhoMin 0.5;
rhoMax 2.0;
pMinFactor 0.5;
pMaxFactor 2.0;
residualControl
{

4
tutorials/compressible/rhoSimpleFoam/angledDuctExplicitFixedCoeff/system/fvSolution
View File

@ -54,8 +54,8 @@ solvers
SIMPLE
{
nNonOrthogonalCorrectors 0;
rhoMin 0.4;
rhoMax 1.5;
pMinFactor 0.4;
pMaxFactor 1.5;
residualControl
{

5
tutorials/compressible/rhoSimpleFoam/squareBend/system/fvSolution
View File

@ -39,8 +39,8 @@ solvers
SIMPLE
{
nNonOrthogonalCorrectors 0;
rhoMin 0.1;
rhoMax 1.0;
pMinFactor 0.1;
pMaxFactor 1.5;
transonic yes;
consistent yes;
@ -60,7 +60,6 @@ relaxationFactors
fields
{
p 1;
rho 1;
}
equations
{

42
tutorials/compressible/rhoSimpleFoam/squareBendLiq/0/T Normal file
View File

@ -0,0 +1,42 @@
/*--------------------------------*- 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 volScalarField;
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 1 0 0 0];
internalField uniform 300;
boundaryField
{
Default_Boundary_Region
{
type fixedValue;
value uniform 350;
}
inlet
{
type fixedValue;
value $internalField;
}
outlet
{
type inletOutlet;
inletValue $internalField;
}
}
// ************************************************************************* //

42
tutorials/compressible/rhoSimpleFoam/squareBendLiq/0/U Normal file
View File

@ -0,0 +1,42 @@
/*--------------------------------*- 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 volVectorField;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
Default_Boundary_Region
{
type noSlip;
}
inlet
{
type flowRateInletVelocity;
massFlowRate constant 5;
rhoInlet 1000; // Guess for rho
}
outlet
{
type inletOutlet;
value uniform (0 0 0);
inletValue uniform (0 0 0);
}
}
// ************************************************************************* //

43
tutorials/compressible/rhoSimpleFoam/squareBendLiq/0/alphat Normal file
View File

@ -0,0 +1,43 @@
/*--------------------------------*- 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 volScalarField;
location "0";
object alphat;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
Default_Boundary_Region
{
type compressible::alphatWallFunction;
Prt 0.85;
value uniform 0;
}
inlet
{
type calculated;
value uniform 0;
}
outlet
{
type calculated;
value uniform 0;
}
}
// ************************************************************************* //

47
tutorials/compressible/rhoSimpleFoam/squareBendLiq/0/epsilon Normal file
View File

@ -0,0 +1,47 @@
/*--------------------------------*- 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 volScalarField;
location "0";
object epsilon;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -3 0 0 0 0];
internalField uniform 200;
boundaryField
{
Default_Boundary_Region
{
type epsilonWallFunction;
Cmu 0.09;
kappa 0.41;
E 9.8;
value uniform 200;
}
inlet
{
type turbulentMixingLengthDissipationRateInlet;
mixingLength 0.005;
value uniform 200;
}
outlet
{
type inletOutlet;
inletValue uniform 200;
value uniform 200;
}
}
// ************************************************************************* //

44
tutorials/compressible/rhoSimpleFoam/squareBendLiq/0/k Normal file
View File

@ -0,0 +1,44 @@
/*--------------------------------*- 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 volScalarField;
location "0";
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 1;
boundaryField
{
Default_Boundary_Region
{
type kqRWallFunction;
value uniform 1;
}
inlet
{
type turbulentIntensityKineticEnergyInlet;
intensity 0.05;
value uniform 1;
}
outlet
{
type inletOutlet;
inletValue uniform 1;
value uniform 1;
}
}
// ************************************************************************* //

45
tutorials/compressible/rhoSimpleFoam/squareBendLiq/0/nut Normal file
View File

@ -0,0 +1,45 @@
/*--------------------------------*- 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 volScalarField;
location "0";
object nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
Default_Boundary_Region
{
type nutkWallFunction;
Cmu 0.09;
kappa 0.41;
E 9.8;
value uniform 0;
}
inlet
{
type calculated;
value uniform 0;
}
outlet
{
type calculated;
value uniform 0;
}
}
// ************************************************************************* //

39
tutorials/compressible/rhoSimpleFoam/squareBendLiq/0/p Normal file
View File

@ -0,0 +1,39 @@
/*--------------------------------*- 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 volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
internalField uniform 1e5;
boundaryField
{
Default_Boundary_Region
{
type zeroGradient;
}
inlet
{
type zeroGradient;
}
outlet
{
type fixedValue;
value $internalField;
}
}
// ************************************************************************* //

31
tutorials/compressible/rhoSimpleFoam/squareBendLiq/constant/thermophysicalProperties Normal file
View File

@ -0,0 +1,31 @@
/*--------------------------------*- 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 thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
thermoType
{
type heRhoThermo;
mixture pureMixture;
properties liquid;
energy sensibleInternalEnergy;
}
mixture
{
H2O;
}
// ************************************************************************* //

30
tutorials/compressible/rhoSimpleFoam/squareBendLiq/constant/turbulenceProperties Normal file
View File

@ -0,0 +1,30 @@
/*--------------------------------*- 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 kEpsilon;
turbulence on;
printCoeffs on;
}
// ************************************************************************* //

127
tutorials/compressible/rhoSimpleFoam/squareBendLiq/system/blockMeshDict Normal file
View File

@ -0,0 +1,127 @@
/*--------------------------------*- 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;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 0.001;
vertices
(
// front-plane: z = +25mm
// inlet region
( -50 25 25) // pt 0
( 0 25 25) // pt 1
( -50 75 25) // pt 2
( 0 75 25) // pt 3
// outlet region
( -500 -75 25) // pt 4
( 0 -75 25) // pt 5
( -500 -25 25) // pt 6
( 0 -25 25) // pt 7
// bend mid-points
( 25 0 25) // pt 8
( 75 0 25) // pt 9
// back-plane: z = -25mm
// inlet region
( -50 25 -25) // pt 0 + 10
( 0 25 -25) // pt 1 + 10
( -50 75 -25) // pt 2 + 10
( 0 75 -25) // pt 3 + 10
// outlet region
( -500 -75 -25) // pt 4 + 10
( 0 -75 -25) // pt 5 + 10
( -500 -25 -25) // pt 7 + 10
( 0 -25 -25) // pt 8 + 10
// bend mid-points
( 25 0 -25) // pt 8 + 10
( 75 0 -25) // pt 9 + 10
);
blocks
(
hex (0 1 11 10 2 3 13 12) inlet ( 20 20 20) simpleGrading (1 1 1)
hex (4 5 15 14 6 7 17 16) outlet (200 20 20) simpleGrading (1 1 1)
hex (1 8 18 11 3 9 19 13) bend1 ( 30 20 20) simpleGrading (1 1 1)
hex (5 9 19 15 7 8 18 17) bend2 ( 30 20 20) simpleGrading (1 1 1)
);
edges
(
// block 2
arc 1 8 ( 17.678 17.678 25)
arc 11 18 ( 17.678 17.678 -25)
arc 3 9 ( 53.033 53.033 25)
arc 13 19 ( 53.033 53.033 -25)
// block 3
arc 7 8 ( 17.678 -17.678 25)
arc 17 18 ( 17.678 -17.678 -25)
arc 5 9 ( 53.033 -53.033 25)
arc 15 19 ( 53.033 -53.033 -25)
);
boundary
(
// is there no way of defining all my 'defaultFaces' to be 'wall'?
Default_Boundary_Region
{
type wall;
faces
(
// block0
( 0 1 3 2 )
( 11 10 12 13 )
( 0 10 11 1 )
( 2 3 13 12 )
// block1
( 4 5 7 6 )
( 15 14 16 17 )
( 4 14 15 5 )
( 6 7 17 16 )
// block2
( 1 8 9 3 )
( 18 11 13 19 )
( 3 9 19 13 )
( 1 11 18 8 )
// block3
( 5 9 8 7 )
( 19 15 17 18 )
( 5 15 19 9 )
( 7 8 18 17 )
);
}
inlet
{
type patch;
faces
(
(0 2 12 10)
);
}
outlet
{
type patch;
faces
(
(4 6 16 14)
);
}
);
mergePatchPairs
(
);
// ************************************************************************* //

51
tutorials/compressible/rhoSimpleFoam/squareBendLiq/system/controlDict Normal file
View File

@ -0,0 +1,51 @@
/*--------------------------------*- 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 "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application rhoSimpleFoam;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 500;
deltaT 1;
writeControl timeStep;
writeInterval 100;
purgeWrite 0;
writeFormat ascii;
writePrecision 6;
writeCompression off;
timeFormat general;
timePrecision 6;
graphFormat raw;
runTimeModifiable true;
// ************************************************************************* //

45
tutorials/compressible/rhoSimpleFoam/squareBendLiq/system/decomposeParDict Normal file
View File

@ -0,0 +1,45 @@
/*--------------------------------*- 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 "system";
object decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
numberOfSubdomains 8;
method hierarchical;
simpleCoeffs
{
n (8 1 1);
delta 0.001;
}
hierarchicalCoeffs
{
n (4 2 1);
delta 0.001;
order xyz;
}
manualCoeffs
{
dataFile "";
}
distributed no;
roots ( );
// ************************************************************************* //

59
tutorials/compressible/rhoSimpleFoam/squareBendLiq/system/fvSchemes Normal file
View File

@ -0,0 +1,59 @@
/*--------------------------------*- 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 "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default steadyState;
}
gradSchemes
{
default Gauss linear;
limited cellLimited Gauss linear 1;
}
divSchemes
{
default none;
div(phi,U) bounded Gauss linearUpwind limited;
div(phi,e) bounded Gauss linearUpwind limited;
div(phi,epsilon) bounded Gauss linearUpwind limited;
div(phi,k) bounded Gauss linearUpwind limited;
div(phi,Ekp) bounded Gauss linearUpwind limited;
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
// ************************************************************************* //

71
tutorials/compressible/rhoSimpleFoam/squareBendLiq/system/fvSolution Normal file
View File

@ -0,0 +1,71 @@
/*--------------------------------*- 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 "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
p
{
solver GAMG;
smoother GaussSeidel;
tolerance 1e-7;
relTol 0.1;
}
"(U|e|k|epsilon)"
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-7;
relTol 0.1;
}
}
SIMPLE
{
nNonOrthogonalCorrectors 0;
pMinFactor 0.1;
pMaxFactor 1.5;
transonic no;
consistent no;
residualControl
{
p 1e-4;
U 1e-4;
"(k|omega|epsilon|e|h)" 1e-3;
}
}
relaxationFactors
{
fields
{
p 0.3;
}
equations
{
U 0.7;
e 0.7;
k 0.7;
epsilon 0.7;
}
}
// ************************************************************************* //