zhyang-dev/OpenFOAM-12
1
0
Fork 0
Code Issues Pull Requests Actions Packages Projects Releases Wiki Activity

fvModels: Specify source property values in field files

Browse Source 
When an fvModel source introduces fluid into a simulation it should also
create a corresponding source term for all properties transported into
the domain by that injection. The source is, effectively, an alternative
form of inlet boundary, on which all transported properties need an
inlet value specified.

These values are now specified in the property field files. The
following is an example of a 0/U file in which the velocity of fluid
introduced by a fvModel source called "injection1" is set to a fixed
value of (-1 0 0):

    dimensions      [0 1 -1 0 0 0 0];

    internalField   uniform (0 0 0);

    boundaryField
    {
        #includeEtc "caseDicts/setConstraintTypes"

        wall
        {
            type            noSlip;
        }

        atmosphere
        {
            type            pressureInletOutletVelocity;
            value           $internalField;
        }
    }

    // *** NEW ***
    sources
    {
        injection1
        {
            type            uniformFixedValue;
            uniformValue    (-1 0 0);
        }
    }

And the following entry in the 0/k file specifies the turbulent kinetic
energy introduced as a fraction of the mean flow kinetic energy:

    sources
    {
        injection1
        {
            type            turbulentIntensityKineticEnergy;
            intensity       0.05;
        }
    }

The specification is directly analogous to boundary conditions. The
conditions are run-time selectable and can be concisely implemented.
They can access each other and be inter-dependent (e.g., the above,
where turbulent kinetic energy depends on velocity). The syntax keeps
field data localised and makes the source model (e.g., massSource,
volumeSource, ...) specification independent from what other models and
fields are present in the simulation. The 'fieldValues' entry previously
required by source models is now no longer required.

If source values need specifying and no source condition has been
supplied in the relevant field file then an error will be generated.
This error is similar to that generated for missing boundary conditions.
This replaces the behaviour where sources such as these would introduce
a value of zero, either silently or with a warning. This is now
considered unacceptable. Zero might be a tolerable default for certain
fields (U, k), but is wholly inappropriate for others (T, epsilon, rho).

This change additionally makes it possible to inject fluid into a
multicomponent solver with a specified temperature. Previously, it was
not possible to do this as there was no means of evaluating the energy
of fluid with the injected composition.
This commit is contained in:
Will Bainbridge
2023-10-12 10:04:40 +01:00
parent 5e03874bbb
commit 171101d1e5
160 changed files with 7453 additions and 1612 deletions
Download Patch File Download Diff File Expand all files Collapse all files

17
tutorials/incompressibleVoF/damBreak/0/U
View File

@ -20,17 +20,9 @@ internalField uniform (0 0 0);
boundaryField
{
leftWall
{
type noSlip;
}
#includeEtc "caseDicts/setConstraintTypes"
rightWall
{
type noSlip;
}
lowerWall
wall
{
type noSlip;
}
@ -40,11 +32,6 @@ boundaryField
type pressureInletOutletVelocity;
value $internalField;
}
defaultFaces
{
type empty;
}
}

17
tutorials/incompressibleVoF/damBreak/0/alpha.water.orig
View File

@ -20,17 +20,9 @@ internalField uniform 0;
boundaryField
{
leftWall
{
type zeroGradient;
}
#includeEtc "caseDicts/setConstraintTypes"
rightWall
{
type zeroGradient;
}
lowerWall
wall
{
type zeroGradient;
}
@ -41,11 +33,6 @@ boundaryField
inletValue $internalField;
value $internalField;
}
defaultFaces
{
type empty;
}
}

19
tutorials/incompressibleVoF/damBreak/0/epsilon
View File

@ -20,19 +20,9 @@ internalField uniform 0.1;
boundaryField
{
leftWall
{
type epsilonWallFunction;
value $internalField;
}
#includeEtc "caseDicts/setConstraintTypes"
rightWall
{
type epsilonWallFunction;
value $internalField;
}
lowerWall
wall
{
type epsilonWallFunction;
value $internalField;
@ -44,11 +34,6 @@ boundaryField
inletValue $internalField;
value $internalField;
}
defaultFaces
{
type empty;
}
}

19
tutorials/incompressibleVoF/damBreak/0/k
View File

@ -20,19 +20,9 @@ internalField uniform 0.1;
boundaryField
{
leftWall
{
type kqRWallFunction;
value $internalField;
}
#includeEtc "caseDicts/setConstraintTypes"
rightWall
{
type kqRWallFunction;
value $internalField;
}
lowerWall
wall
{
type kqRWallFunction;
value $internalField;
@ -44,11 +34,6 @@ boundaryField
inletValue $internalField;
value $internalField;
}
defaultFaces
{
type empty;
}
}

17
tutorials/incompressibleVoF/damBreak/0/nuTilda
View File

@ -20,17 +20,9 @@ internalField uniform 0;
boundaryField
{
leftWall
{
type zeroGradient;
}
#includeEtc "caseDicts/setConstraintTypes"
rightWall
{
type zeroGradient;
}
lowerWall
wall
{
type zeroGradient;
}
@ -41,11 +33,6 @@ boundaryField
inletValue $internalField;
value $internalField;
}
defaultFaces
{
type empty;
}
}

19
tutorials/incompressibleVoF/damBreak/0/nut
View File

@ -20,19 +20,9 @@ internalField uniform 0;
boundaryField
{
leftWall
{
type nutkWallFunction;
value $internalField;
}
#includeEtc "caseDicts/setConstraintTypes"
rightWall
{
type nutkWallFunction;
value $internalField;
}
lowerWall
wall
{
type nutkWallFunction;
value $internalField;
@ -43,11 +33,6 @@ boundaryField
type calculated;
value $internalField;
}
defaultFaces
{
type empty;
}
}

19
tutorials/incompressibleVoF/damBreak/0/omega
View File

@ -20,19 +20,9 @@ internalField uniform 11.1;
boundaryField
{
leftWall
{
type omegaWallFunction;
value $internalField;
}
#includeEtc "caseDicts/setConstraintTypes"
rightWall
{
type omegaWallFunction;
value $internalField;
}
lowerWall
wall
{
type omegaWallFunction;
value $internalField;
@ -44,11 +34,6 @@ boundaryField
inletValue $internalField;
value $internalField;
}
defaultFaces
{
type empty;
}
}

19
tutorials/incompressibleVoF/damBreak/0/p_rgh
View File

@ -20,19 +20,9 @@ internalField uniform 0;
boundaryField
{
leftWall
{
type fixedFluxPressure;
value $internalField;
}
#includeEtc "caseDicts/setConstraintTypes"
rightWall
{
type fixedFluxPressure;
value $internalField;
}
lowerWall
wall
{
type fixedFluxPressure;
value $internalField;
@ -43,11 +33,6 @@ boundaryField
type prghTotalPressure;
p0 $internalField;
}
defaultFaces
{
type empty;
}
}

47
tutorials/incompressibleVoF/damBreakInjection/0/U Normal file
View File

@ -0,0 +1,47 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class volVectorField;
location "0";
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
#includeEtc "caseDicts/setConstraintTypes"
wall
{
type noSlip;
}
atmosphere
{
type pressureInletOutletVelocity;
value $internalField;
}
}
sources
{
injection
{
type uniformFixedValue;
uniformValue (-1 0 0);
}
}
// ************************************************************************* //

49
tutorials/incompressibleVoF/damBreakInjection/0/epsilon Normal file
View File

@ -0,0 +1,49 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class volScalarField;
location "0";
object epsilon;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -3 0 0 0 0];
internalField uniform 0.1;
boundaryField
{
#includeEtc "caseDicts/setConstraintTypes"
wall
{
type epsilonWallFunction;
value $internalField;
}
atmosphere
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
}
sources
{
injection
{
type turbulentMixingLengthDissipationRate;
mixingLength 0.0146;
}
}
// ************************************************************************* //

49
tutorials/incompressibleVoF/damBreakInjection/0/k Normal file
View File

@ -0,0 +1,49 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class volScalarField;
location "0";
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 0.1;
boundaryField
{
#includeEtc "caseDicts/setConstraintTypes"
wall
{
type kqRWallFunction;
value $internalField;
}
atmosphere
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
}
sources
{
injection
{
type turbulentIntensityKineticEnergy;
intensity 0.05;
}
}
// ************************************************************************* //

10
tutorials/incompressibleVoF/damBreakInjection/Allclean
View File

@ -4,8 +4,14 @@ cd ${0%/*} || exit 1 # Run from this directory
# Source tutorial clean functions
. $WM_PROJECT_DIR/bin/tools/CleanFunctions
cleanVoFCase && rm -rf 0 system
cleanVoFCase
find constant -type f -not -name fvModels.injection -delete
find 0 -type f -not \( \
-name epsilon -or -name k -or -name U \
\) -delete
find constant -type f -not -name fvModels -delete
rm -rf system
#------------------------------------------------------------------------------

5
tutorials/incompressibleVoF/damBreakInjection/Allrun
View File

@ -4,11 +4,10 @@ cd ${0%/*} || exit 1 # Run from this directory
# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions
# Copy the source case and add the volume source model
# Copy the source case
isTest "$@" && path=.. || path=$FOAM_TUTORIALS/incompressibleVoF
cp -rn $path/damBreak/0 $path/damBreak/constant $path/damBreak/system .
runApplication foamDictionary constant/fvModels \
-entry injection -dict -merge constant/fvModels.injection
rm -f 0/alpha.water
# Run
runApplication blockMesh

20
tutorials/incompressibleVoF/damBreakInjection/constant/fvModels.injection → tutorials/incompressibleVoF/damBreakInjection/constant/fvModels
View File

@ -10,26 +10,26 @@ FoamFile
format ascii;
class dictionary;
location "constant";
object fvModels.injection;
object fvModels;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
turbulenceDamping
{
type VoFTurbulenceDamping;
delta 1e-4;
}
injection
{
type volumeSource;
phase water;
points ((0.438 0.438 0.0073));
volumetricFlowRate 0.0003;
phase water;
fieldValues
{
U (-1 0 0);
k 0.1;
epsilon 0.1;
}
}