the previous naming tan1, tan2, normal was non-intuitive and very confusing.
It was not practical to maintain backward compatibility but all tutorials and
example refineMeshDict files have been updated to provide examples of the
change.
The inside or outside region refinement level is now specified using the simple
"level <level>" entry in refinementRegions e.g.
refinementRegions
{
refinementBox
{
mode inside;
level 5;
}
}
rather than
refinementRegions
{
refinementBox
{
mode inside;
levels ((1E15 5));
}
}
where the spurious "1E15" number is not used and the '((...))' is unnecessary clutter.
The pressure work term for total internal energy is div(U p) which can be
discretised is various ways, given a mass flux field phi it seems logical to
implement it in the form div(phi/interpolate(rho), p) but this is not exactly
consistent with the relationship between enthalpy and internal energy (h = e +
p/rho) and the transport of enthalpy, it would be more consistent to implement
it in the form div(phi, p/rho). A further improvement in consistency can be
gained by using the same convection scheme for this work term and the convection
term div(phi, e) and for reacting solvers this is easily achieved by using the
multi-variate limiter mvConvection provided for energy and specie convection.
This more consistent total internal energy work term has now been implemented in
all the compressible and reacting flow solvers and provides more accurate
solutions when running with internal energy, particularly for variable density
mixing cases with small pressure variation.
For non-reacting compressible solvers this improvement requires a change to the
corresponding divScheme in fvSchemes:
"div\(alphaPhi.*,p\)" -> "div\(alphaRhoPhi.*,\(p\|thermo:rho.*\)\)"
and all the tutorials have been updated accordingly.
The themo tables used in wallBoiling have had their Cp/Cv values
corrected, and have been coarsened and reduced in size to bound only the
operating point of the wallBoiling tutorials. They have also been moved
to $FOAM_TUTORIALS/resources/thermoData.
The correction to thermophysical properties has improved the stability
of these cases. As a result it has been possible to reduce the amount of
under-relaxation used in the wall modelling.
The phase-fraction filtering of the compressibility terms is present to avoid
spurious phase-change due to numerical noise. The fvModels contribution may
cause physical phase-change due to cavitation, boiling, transfer from film or
VoF even where none of the phase is present and hence must be added after the
compressibility filtering.
With VoFClouds and VoFSurfaceFilm compressibleInterFoam supports Lagrangian
clouds which can impinge on walls forming a film which in turn can transfer to
the VoF when the film is thick enough to resolve. The new tutorial case
tutorials/multiphase/compressibleInterFoam/laminar/cylinder
is provided to demonstrate this functionality.
Direct transfer of droplets to the VoF phase is not yet supported but will be
added later.
Now the VoFSurfaceFilm library is optionally loaded at run-time for cases that
require surface film by adding the optional "libs" entry in controlDict:
libs ("libVoFSurfaceFilm.so");
See tutorials/multiphase/compressibleInterFoam/laminar/plateFilm
To provide more flexibility, extensibility, run-time modifiability and
consistency the handling of optional pressure limits has been moved from
pressureControl (settings in system/fvSolution) to the new limitPressure
fvConstraint (settings in system/fvConstraints).
All tutorials have been updated which provides guidance when upgrading cases but
also helpful error messages are generated for cases using the old settings
providing specific details as to how the case should be updated, e.g. for the
tutorials/compressible/rhoSimpleFoam/squareBend case which has the pressure
limit specification:
SIMPLE
{
...
pMinFactor 0.1;
pMaxFactor 2;
...
generates the error message
--> FOAM FATAL IO ERROR:
Pressure limits should now be specified in fvConstraints:
limitp
{
type limitPressure;
minFactor 0.1;
maxFactor 2;
}
file: /home/dm2/henry/OpenFOAM/OpenFOAM-dev/tutorials/compressible/rhoSimpleFoam/squareBend/system/fvSolution/SIMPLE from line 41 to line 54.
so that they operate in the conventional manner in a right-handed coordinate
system:
//- Rotational transformation tensor about the x-axis by omega radians
// The rotation is defined in a right-handed coordinate system
// i.e. clockwise with respect to the axis from -ve to +ve
// (looking along the axis).
inline tensor Rx(const scalar& omega)
//- Rotational transformation tensor about the y-axis by omega radians
// The rotation is defined in a right-handed coordinate system
// i.e. clockwise with respect to the axis from -ve to +ve
// (looking along the axis).
inline tensor Ry(const scalar& omega)
//- Rotational transformation tensor about the z-axis by omega radians
// The rotation is defined in a right-handed coordinate system
// i.e. clockwise with respect to the axis from -ve to +ve
// (looking along the axis).
inline tensor Rz(const scalar& omega)
//- Rotational transformation tensor about axis a by omega radians
// The rotation is defined in a right-handed coordinate system
// i.e. clockwise with respect to the axis from -ve to +ve
// (looking along the axis).
inline tensor Ra(const vector& a, const scalar omega)
Description
Transform (translate, rotate, scale) a surface.
Usage
\b surfaceTransformPoints "\<transformations\>" \<input\> \<output\>
Supported transformations:
- \par translate=<translation vector>
Translational transformation by given vector
- \par rotate=(\<n1 vector\> \<n2 vector\>)
Rotational transformation from unit vector n1 to n2
- \par Rx=\<angle [deg] about x-axis\>
Rotational transformation by given angle about x-axis
- \par Ry=\<angle [deg] about y-axis\>
Rotational transformation by given angle about y-axis
- \par Rz=\<angle [deg] about z-axis\>
Rotational transformation by given angle about z-axis
- \par Ra=\<axis vector\> \<angle [deg] about axis\>
Rotational transformation by given angle about given axis
- \par scale=\<x-y-z scaling vector\>
Anisotropic scaling by the given vector in the x, y, z
coordinate directions
Example usage:
surfaceTransformPoints \
"translate=(-0.586 0 -0.156), \
Ry=3.485, \
translate=(0.586 0 0.156)" \
constant/geometry/w3_orig.stl constant/geometry/w3.stl
The transformation sequence is specified like a substitution string used by
Description
Transform (translate, rotate, scale) a surface.
The rollPitchYaw option takes three angles (degrees):
- roll (rotation about x) followed by
- pitch (rotation about y) followed by
- yaw (rotation about z)
The yawPitchRoll does yaw followed by pitch followed by roll.
Usage
\b surfaceTransformPoints "\<transformations\>" \<input\> \<output\>
Example usage:
surfaceTransformPoints \
"translate=(-0.586 0 -0.156), \
rollPitchYaw=(0 -3.485 0), \
translate=(0.586 0 0.156)" \
constant/geometry/w3_orig.stl constant/geometry/w3.stl
The constant heat capacity hacked thermo in surfaceFilmModels and the
corresponding transfer terms in Lagrangian have been replaced by the standard
OpenFOAM rhoThermo which provides a general handling of thermo-physical
properties, in particular non-constant heat capacity. Further rationalisation
of liquid and solid properties has also been undertaken in support of this work
to provide a completely consistent interface to sensible and absolute enthalpy.
Now for surfaceFilmModels the thermo-physical model and properties are specified
in a constant/<region>/thermophysicalProperties dictionary consistent with all
other types of continuum simulation.
This significantly rationalises, simplifies and generalises the handling of
thermo-physical properties for film simulations and is a start at doing the same
for Lagrangian.
pMin and pMax settings are now available in multiphaseEulerFoam in the
PIMPLE section of the system/fvOptions file. This is consistent with
other compressible solvers. The pMin setting in system/phaseProperties
is no longer read, and it's presence will result in a warning.
SLGThermo has been moved to lagrangian, which still depends on it, pending
complete removal and replacement with a more rational interface to the carrier
phase thermodynamics.
The new fvModels is a general interface to optional physical models in the
finite volume framework, providing sources to the governing conservation
equations, thus ensuring consistency and conservation. This structure is used
not only for simple sources and forces but also provides a general run-time
selection interface for more complex models such as radiation and film, in the
future this will be extended to Lagrangian, reaction, combustion etc. For such
complex models the 'correct()' function is provided to update the state of these
models at the beginning of the PIMPLE loop.
fvModels are specified in the optional constant/fvModels dictionary and
backward-compatibility with fvOption is provided by reading the
constant/fvOptions or system/fvOptions dictionary if present.
The new fvConstraints is a general interface to optional numerical constraints
applied to the matrices of the governing equations after construction and/or to
the resulting field after solution. This system allows arbitrary changes to
either the matrix or solution to ensure numerical or other constraints and hence
violates consistency with the governing equations and conservation but it often
useful to ensure numerical stability, particularly during the initial start-up
period of a run. Complex manipulations can be achieved with fvConstraints, for
example 'meanVelocityForce' used to maintain a specified mean velocity in a
cyclic channel by manipulating the momentum matrix and the velocity solution.
fvConstraints are specified in the optional system/fvConstraints dictionary and
backward-compatibility with fvOption is provided by reading the
constant/fvOptions or system/fvOptions dictionary if present.
The separation of fvOptions into fvModels and fvConstraints provides a rational
and consistent separation between physical and numerical models which is easier
to understand and reason about, avoids the confusing issue of location of the
controlling dictionary file, improves maintainability and easier to extend to
handle current and future requirements for optional complex physical models and
numerical constraints.
A population balance suffix after the phase suffix makes determining the
phase for a given name more complex. The additional suffix is also
unnecessary as a phase can only ever belong to one population balance,
so the phase name alone uniquely idetifies the grouping.
Patch contributed by Institute of Fluid Dynamics,
Helmholtz-Zentrum Dresden - Rossendorf (HZDR)
A modified Arrhenius reaction rate given by:
k = (A * T^beta * exp(-Ta/T))*a
Where a is the phase surface area per unit volume. The name of the phase is
specified by the user.
Example usage:
oxidationAtSurface
{
type irreversiblePhaseSurfaceArrhenius;
reaction "O2^0 + TiCl4 = TiO2_s + 2Cl2";
A 4.9e1; // The pre-exponential factor is in units
// equal to that in the usual volumetric
// reaction rate **divided by length**, as
// the Arrhenius expression is taken to give
// rate per unit area, not per unit volume
beta 0.0;
Ta 8993;
phase particles;
}
This reaction has been applied to the titaniaSynthesisSurface tutorial,
which avoids the need for explicit caching of the surface area density
field.
This function gives a value of one during a user-specified duration, and
zero at all other times. It is useful for defining the time range in
which an injection or ignition heat source or similar operates.
Example usage, scaling a value:
<name>
{
type scale;
scale squarePulse;
start 0;
duration 1;
value 100;
}
This function has been utilised in a number of tutorial fvOption
configurations to provide a specific window in which the fvOption is
applied. This was previously achieved by "timeStart" and "duration"
controls hard coded into the fvOptions themselves.
This fvOption applies a mass source to the continuity equation and to
all field equations.
Example usage:
massSource
{
type massSource;
selectionMode cellSet;
cellSet massSource;
massFlowRate 1e-4;
fieldValues
{
U (10 0 0);
T 350;
k 0.375;
epsilon 14.855;
}
}
Values should be provided for all solved for fields. Warnings will be
issued if values are not provided for fields for which transport equations
are solved. Warnings will also be issued if values are provided for fields
which are not solved for.
A number of fvOptions that apply to a user-derined field can now
automatically work what primitive type they apply to. These options can
apply to any field type, and in some cases even multiple fields of
differing type. Example usage of the options to which this change
applies are shown below:
codedSource1
{
type codedSource;
name codedSource1;
field h;
...
}
fixedValueConstraint1
{
type fixedValueConstraint;
fieldValues
{
R (1 0 0 1 0 1);
epsilon 150;
}
...
}
phaseLimitStabilization11
{
type phaseLimitStabilization;
field sigma.liquid;
...
}
Previously to apply to a given type, these options had to be selected
with the name of the type prepended to the option name (e.g., "type
symmTensorPhaseLimitStabilization;") and those that operated on multiple
fields were restricted to those fields being of the same type.
A number of other options have had improvements made to their handling
of user specification of fields. Where possible, the option will now
attempt to work out what field the option applies to automatically. The
following options, therefore, no longer require "field" or "fields"
entries:
actuationDiskSource
buoyancyEnergy
buoyancyForce
meanVelocityForce
rotorDiskSource
volumeFractionSource
constantHeatTransfer
function2HeatTransfer
variableHeatTransfer
Non-standard field names can be overridden in the same way as in
boundary conditions; e.g., the velocity name can be overridden with a "U
<UName>;" entry if it does not have the default name, "U". The name of
the energy field is now always determined from the thermodynamics
model and should always be correct. Some options that can be applied to
an individual phase also support a "phase <phaseName>;" entry;
fvOptions field-name handling has been rewritten to increase its
flexibility and to improve warning messages. The flexibility now allows
for options that apply to all fields, or all fields of a given phase,
rather than being limited to a specific list of field names. Messages
warning about options that have not been applied now always print just
once per time-step.
Vertices are generated using run time compilation functionality.
File duplication avoided by placement in:
tutorials/resources/blockMesh/sloshingTank2D
tutorials/resources/blockMesh/sloshingTank3D
Originally the only supported geometry specification were triangulated surfaces,
hence the name of the directory: constant/triSurface, however now that other
surface specifications are supported and provided it is much more logical that
the directory is named accordingly: constant/geometry. All tutorial and
template cases have been updated.
Note that backward compatibility is provided such that if the constant/geometry
directory does not exist but constant/triSurface does then the geometry files
are read from there.
Mesh-motion with or without topology change or AMI is now supported in
multiphaseEulerFoam for both cell- and face-momentum algorithms.
The new tutorial case mixerVesselAMI2D is provided which is the AMI version of
the 4-phase MRF mixerVessel2D case. It is setup with the cell-momentum
algorithm but also runs fine with the face-momentum algorithm although the
results are noticeably less accurate, particularly when the case is run
single-phase and compared directly with those from pimpleFoam.
Further testing is in progress.
I2D/constant/thermophysicalProperties.water
The phase-change functionality in interPhaseChangeFoam has been generalised and
moved into the run-time selectable twoPhaseChange library included into
interFoam providing optional phase-change. The three cavitation models provided
in interPhaseChangeFoam are now included in the twoPhaseChange library and the
two interPhaseChangeFoam cavitation tutorials updated for interFoam.
interPhaseChangeFoam has been replaced by a user redirection script which prints
the following message:
The interPhaseChangeFoam solver has solver has been replaced by the more general
interFoam solver, which now supports phase-change using the new twoPhaseChange
models library.
To run with with phase-change create a constant/phaseChangeProperties dictionary
containing the phase-change model specification, e.g.
phaseChangeModel SchnerrSauer;
pSat 2300; // Saturation pressure
See the following cases for an example converted from interPhaseChangeFoam:
$FOAM_TUTORIALS/multiphase/interFoam/laminar/cavitatingBullet
$FOAM_TUTORIALS/multiphase/interFoam/RAS/propeller
End points of topoSet cylinder sources should now be specified as
"point1" and "point2", which is consistent with other parts of the code.
The previous keywords, "p1" and "p2" have been retained for backwards
compatibility but may be removed in future.
