Radiative heat transfer may now be added to any solver in which an energy
equation is solved at run-time rather than having to change the solver code.
For example, radiative heat transfer is now enabled in the SandiaD_LTS
reactingFoam tutorial by providing a constant/fvOptions file containing
radiation
{
type radiation;
libs ("libradiationModels.so");
}
and appropriate settings in the constant/radiationProperties file.
For example the porosity coefficients may now be specified thus:
porosity1
{
type DarcyForchheimer;
cellZone porosity;
d (5e7 -1000 -1000);
f (0 0 0);
coordinateSystem
{
type cartesian;
origin (0 0 0);
coordinateRotation
{
type axesRotation;
e1 (0.70710678 0.70710678 0);
e2 (0 0 1);
}
}
}
rather than
porosity1
{
type DarcyForchheimer;
active yes;
cellZone porosity;
DarcyForchheimerCoeffs
{
d (5e7 -1000 -1000);
f (0 0 0);
coordinateSystem
{
type cartesian;
origin (0 0 0);
coordinateRotation
{
type axesRotation;
e1 (0.70710678 0.70710678 0);
e2 (0 0 1);
}
}
}
}
support for which is maintained for backward compatibility.
For example the actuationDiskSource fvOption may now be specified
disk1
{
type actuationDiskSource;
fields (U);
selectionMode cellSet;
cellSet actuationDisk1;
diskDir (1 0 0); // Orientation of the disk
Cp 0.386;
Ct 0.58;
diskArea 40;
upstreamPoint (581849 4785810 1065);
}
rather than
disk1
{
type actuationDiskSource;
active on;
actuationDiskSourceCoeffs
{
fields (U);
selectionMode cellSet;
cellSet actuationDisk1;
diskDir (1 0 0); // Orientation of the disk
Cp 0.386;
Ct 0.58;
diskArea 40;
upstreamPoint (581849 4785810 1065);
}
}
but this form is supported for backward compatibility.
The standard naming convention for heat flux is "q" and this is used for the
conductive and convective heat fluxes is OpenFOAM. The use of "Qr" for
radiative heat flux is an anomaly which causes confusion, particularly for
boundary conditions in which "Q" is used to denote power in Watts. The name of
the radiative heat flux has now been corrected to "qr" and all models, boundary
conditions and tutorials updated.
by combining with and rationalizing functionality from
turbulentHeatFluxTemperatureFvPatchScalarField.
externalWallHeatFluxTemperatureFvPatchScalarField now replaces
turbulentHeatFluxTemperatureFvPatchScalarField which is no longer needed and has
been removed.
Description
This boundary condition applies a heat flux condition to temperature
on an external wall in one of three modes:
- fixed power: supply Q
- fixed heat flux: supply q
- fixed heat transfer coefficient: supply h and Ta
where:
\vartable
Q | Power [W]
q | Heat flux [W/m^2]
h | Heat transfer coefficient [W/m^2/K]
Ta | Ambient temperature [K]
\endvartable
For heat transfer coefficient mode optional thin thermal layer resistances
can be specified through thicknessLayers and kappaLayers entries.
The thermal conductivity \c kappa can either be retrieved from various
possible sources, as detailed in the class temperatureCoupledBase.
Usage
\table
Property | Description | Required | Default value
mode | 'power', 'flux' or 'coefficient' | yes |
Q | Power [W] | for mode 'power' |
q | Heat flux [W/m^2] | for mode 'flux' |
h | Heat transfer coefficient [W/m^2/K] | for mode 'coefficent' |
Ta | Ambient temperature [K] | for mode 'coefficient' |
thicknessLayers | Layer thicknesses [m] | no |
kappaLayers | Layer thermal conductivities [W/m/K] | no |
qr | Name of the radiative field | no | none
qrRelaxation | Relaxation factor for radiative field | no | 1
kappaMethod | Inherited from temperatureCoupledBase | inherited |
kappa | Inherited from temperatureCoupledBase | inherited |
\endtable
Example of the boundary condition specification:
\verbatim
<patchName>
{
type externalWallHeatFluxTemperature;
mode coefficient;
Ta uniform 300.0;
h uniform 10.0;
thicknessLayers (0.1 0.2 0.3 0.4);
kappaLayers (1 2 3 4);
kappaMethod fluidThermo;
value $internalField;
}
\endverbatim
Description
Temperature-dependent surface tension model in which the surface tension
function provided by the phase Foam::liquidProperties class is used.
Usage
\table
Property | Description | Required | Default value
phase | Phase name | yes |
\endtable
Example of the surface tension specification:
\verbatim
sigma
{
type liquidProperties;
phase water;
}
\endverbatim
for use with e.g. compressibleInterFoam, see
tutorials/multiphase/compressibleInterFoam/laminar/depthCharge2D
These models have been particularly designed for use in the VoF solvers, both
incompressible and compressible. Currently constant and temperature dependent
surface tension models are provided but it easy to write models in which the
surface tension is evaluated from any fields held by the mesh database.
Created a base-class from contactAngleForce from which the
distributionContactAngleForce (for backward compatibility) and the new
temperatureDependentContactAngleForce are derived:
Description
Temperature dependent contact angle force
The contact angle in degrees is specified as a \c Function1 type, to
enable the use of, e.g. contant, polynomial, table values.
See also
Foam::regionModels::surfaceFilmModels::contactAngleForce
Foam::Function1Types
SourceFiles
temperatureDependentContactAngleForce.C
Off-centering is specified via the mandatory coefficient \c ocCoeff in the
range [0,1] following the scheme name e.g.
\verbatim
ddtSchemes
{
default CrankNicolson 0.9;
}
\endverbatim
or with an optional "ramp" function to transition from the Euler scheme to
Crank-Nicolson over a initial period to avoid start-up problems, e.g.
\verbatim
ddtSchemes
{
default CrankNicolson
ocCoeff
{
type scale;
scale linearRamp;
duration 0.01;
value 0.9;
};
}
\endverbatim
Note this functionality is experimental and the specification and implementation
may change if issues arise.
For example in the potentialFreeSurfaceFoam/oscillatingBox tutorial it is
cleaner to apply the "linearRamp" function to the "sine" function rather than
using an amplitude table:
floatingObject
{
type fixedNormalInletOutletVelocity;
fixTangentialInflow false;
normalVelocity
{
type uniformFixedValue;
uniformValue
{
type scale;
value
{
type sine;
frequency 1;
amplitude 0.025;
scale (0 1 0);
level (0 0 0);
}
scale
{
type linearRamp;
duration 10;
}
}
}
value uniform (0 0 0);
}
coupled patches, to prevent rebound/stick/etc... on these patches. Also
added "none" interaction type to LocalInteraction, which reverts the
patch interaction to the fundamental behaviour. This is primarily useful
for non-coupled constraint types.
Resolves https://bugs.openfoam.org/view.php?id=2458
including support for TDAC and ISAT for efficient chemistry calculation.
Description
Eddy Dissipation Concept (EDC) turbulent combustion model.
This model considers that the reaction occurs in the regions of the flow
where the dissipation of turbulence kinetic energy takes place (fine
structures). The mass fraction of the fine structures and the mean residence
time are provided by an energy cascade model.
There are many versions and developments of the EDC model, 4 of which are
currently supported in this implementation: v1981, v1996, v2005 and
v2016. The model variant is selected using the optional \c version entry in
the \c EDCCoeffs dictionary, \eg
\verbatim
EDCCoeffs
{
version v2016;
}
\endverbatim
The default version is \c v2015 if the \c version entry is not specified.
Model versions and references:
\verbatim
Version v2005:
Cgamma = 2.1377
Ctau = 0.4083
kappa = gammaL^exp1 / (1 - gammaL^exp2),
where exp1 = 2, and exp2 = 2.
Magnussen, B. F. (2005, June).
The Eddy Dissipation Concept -
A Bridge Between Science and Technology.
In ECCOMAS thematic conference on computational combustion
(pp. 21-24).
Version v1981:
Changes coefficients exp1 = 3 and exp2 = 3
Magnussen, B. (1981, January).
On the structure of turbulence and a generalized
eddy dissipation concept for chemical reaction in turbulent flow.
In 19th Aerospace Sciences Meeting (p. 42).
Version v1996:
Changes coefficients exp1 = 2 and exp2 = 3
Gran, I. R., & Magnussen, B. F. (1996).
A numerical study of a bluff-body stabilized diffusion flame.
Part 2. Influence of combustion modeling and finite-rate chemistry.
Combustion Science and Technology, 119(1-6), 191-217.
Version v2016:
Use local constants computed from the turbulent Da and Re numbers.
Parente, A., Malik, M. R., Contino, F., Cuoci, A., & Dally, B. B.
(2016).
Extension of the Eddy Dissipation Concept for
turbulence/chemistry interactions to MILD combustion.
Fuel, 163, 98-111.
\endverbatim
Tutorials cases provided: reactingFoam/RAS/DLR_A_LTS, reactingFoam/RAS/SandiaD_LTS.
This codes was developed and contributed by
Zhiyi Li
Alessandro Parente
Francesco Contino
from BURN Research Group
and updated and tested for release by
Henry G. Weller
CFD Direct Ltd.
to provide smoother behavior on start-up when an acceleration impulse is
applied, e.g. if the body is suddenly released. e.g.
dynamicFvMesh dynamicMotionSolverFvMesh;
motionSolverLibs ("librigidBodyMeshMotion.so");
solver rigidBodyMotion;
rigidBodyMotionCoeffs
{
report on;
solver
{
type Newmark;
}
ramp
{
type quadratic;
start 0;
duration 10;
}
.
.
.
will quadratically ramp the forces from 0 to their full values over the first
10s of the run starting from 0. If the 'ramp' entry is omitted no force ramping
is applied.
Description
Ramp function base class for the set of scalar functions starting from 0 and
increasing monotonically to 1 from \c start over the \c duration and
remaining at 1 thereafter.
Usage:
\verbatim
<entryName> <rampFunction>;
<entryName>Coeffs
{
start 10;
duration 20;
}
\endverbatim
or
\verbatim
<entryName>
{
type <rampFunction>;
start 10;
duration 20;
}
\endverbatim
Where:
\table
Property | Description | Required | Default value
start | Start time | no | 0
duration | Duration | yes |
\endtable
The following common ramp functions are provided: linear, quadratic, halfCosine,
quarterCosine and quaterSine, others can easily be added and registered to the run-time
selection system.
e.g.
ramp
{
type quadratic;
start 200;
duration 1.6;
}
but the old format is supported for backward compatibility:
ramp linear;
rampCoeffs
{
start 200;
duration 1.6;
}
Formally this is equivalent to the previous formulation but more convenient to
use given that for compressible flow the mass flux rather than the volume flux
is available.
These legacy boundary conditions are no longer needed and have been superseded
by the more flexible sixDoFRigidBodyMotion and rigidBodyMotion solvers. See tutorials:
incompressible/pimpleDyMFoam/wingMotion/wingMotion2D_pimpleDyMFoam
multiphase/interDyMFoam/RAS/DTCHull
multiphase/interDyMFoam/RAS/floatingObject
Resolves bug-report https://bugs.openfoam.org/view.php?id=2487
Using
decomposePar -copyZero
The mesh is decomposed as usual but the '0' directory is recursively copied to
the 'processor.*' directories rather than decomposing the fields. This is a
convenient option to handle cases where the initial field files are generic and
can be used for serial or parallel running. See for example the
incompressible/simpleFoam/motorBike tutorial case.
