The defaultPatch type currently defaults to empty which is appropriate for 1D
and 2D cases but not when creating the initial blockMesh for snappyHexMesh as
the presence of empty patches triggers the inappropriate application of 2D point
constraint corrections following snapping and morphing. To avoid this hidden
problem a warning is now generated from blockMesh when the defaultPatch is not
explicitly set for cases which generate a default patch, i.e. for which the
boundary is not entirely defined. e.g.
.
.
.
Creating block mesh topology
--> FOAM FATAL IO ERROR:
The 'defaultPatch' type must be specified for the 'defaultFaces' patch, e.g. for snappyHexMesh
defaultPatch
{
name default; // optional
type patch;
}
or for 2D meshes
defaultPatch
{
name frontAndBack; // optional
type empty;
}
.
.
.
All the tutorials have been update to include the defaultPatch specification as
appropriate.
to limit the time-step by comparing the film Courant number with the maximum
Courant number obtain from the optional maxCo entry in the system/<film
region>/fvSolution file. If maxCo is not provided the film model does not limit
the time-step.
See tutorials/multiphase/compressibleInterFoam/laminar/cylinder as an example
demonstrating this functionality.
For most multiphase flows it is more appropriate to evaluate the total pressure
from the static pressure obtained from p_rgh rather than from p_rgh directly.
Now that Cp and Cv are cached it is more convenient and consistent and slightly
more efficient to cache thermal conductivity kappa rather than thermal
diffusivity alpha which is not a fundamental property, the appropriate form
depending on the energy solved for. kappa is converted into the appropriate
thermal diffusivity for the energy form solved for by dividing by the
corresponding cached heat capacity when required, which is efficient.
There is no longer any need for the surfaceFilmModel abstract base class and
"New" selection method as surface films are now handled within the fvModel
framework. This makes the surfaceFilmModel entry in the surfaceFilmProperties
dictionary redundant.
The surfaceFilm and VoFSurfaceFilm fvModels now instantiate a thermoSingleLayer
providing direct access to all the film functions, simplifying the
implementation better ensuring consistency between the film and primary region
equations.
Mesh motion and topology change are now combinable run-time selectable options
within fvMesh, replacing the restrictive dynamicFvMesh which supported only
motion OR topology change.
All solvers which instantiated a dynamicFvMesh now instantiate an fvMesh which
reads the optional constant/dynamicFvMeshDict to construct an fvMeshMover and/or
an fvMeshTopoChanger. These two are specified within the optional mover and
topoChanger sub-dictionaries of dynamicFvMeshDict.
When the fvMesh is updated the fvMeshTopoChanger is first executed which can
change the mesh topology in anyway, adding or removing points as required, for
example for automatic mesh refinement/unrefinement, and all registered fields
are mapped onto the updated mesh. The fvMeshMover is then executed which moved
the points only and calculates the cell volume change and corresponding
mesh-fluxes for conservative moving mesh transport. If multiple topological
changes or movements are required these would be combined into special
fvMeshMovers and fvMeshTopoChangers which handle the processing of a list of
changes, e.g. solidBodyMotionFunctions:multiMotion.
The tutorials/multiphase/interFoam/laminar/sloshingTank3D3DoF case has been
updated to demonstrate this new functionality by combining solid-body motion
with mesh refinement/unrefinement:
/*--------------------------------*- 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 dictionary;
location "constant";
object dynamicMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
mover
{
type motionSolver;
libs ("libfvMeshMovers.so" "libfvMotionSolvers.so");
motionSolver solidBody;
solidBodyMotionFunction SDA;
CofG (0 0 0);
lamda 50;
rollAmax 0.2;
rollAmin 0.1;
heaveA 4;
swayA 2.4;
Q 2;
Tp 14;
Tpn 12;
dTi 0.06;
dTp -0.001;
}
topoChanger
{
type refiner;
libs ("libfvMeshTopoChangers.so");
// How often to refine
refineInterval 1;
// Field to be refinement on
field alpha.water;
// Refine field in between lower..upper
lowerRefineLevel 0.001;
upperRefineLevel 0.999;
// Have slower than 2:1 refinement
nBufferLayers 1;
// Refine cells only up to maxRefinement levels
maxRefinement 1;
// Stop refinement if maxCells reached
maxCells 200000;
// Flux field and corresponding velocity field. Fluxes on changed
// faces get recalculated by interpolating the velocity. Use 'none'
// on surfaceScalarFields that do not need to be reinterpolated.
correctFluxes
(
(phi none)
(nHatf none)
(rhoPhi none)
(alphaPhi.water none)
(meshPhi none)
(meshPhi_0 none)
(ghf none)
);
// Write the refinement level as a volScalarField
dumpLevel true;
}
// ************************************************************************* //
Note that currently this is the only working combination of mesh-motion with
topology change within the new framework and further development is required to
update the set of topology changers so that topology changes with mapping are
separated from the mesh-motion so that they can be combined with any of the
other movements or topology changes in any manner.
All of the solvers and tutorials have been updated to use the new form of
dynamicMeshDict but backward-compatibility was not practical due to the complete
reorganisation of the mesh change structure.
to provide a single consistent code and user interface to the specification of
physical properties in both single-phase and multi-phase solvers. This redesign
simplifies usage and reduces code duplication in run-time selectable solver
options such as 'functionObjects' and 'fvModels'.
* physicalProperties
Single abstract base-class for all fluid and solid physical property classes.
Physical properties for a single fluid or solid within a region are now read
from the 'constant/<region>/physicalProperties' dictionary.
Physical properties for a phase fluid or solid within a region are now read
from the 'constant/<region>/physicalProperties.<phase>' dictionary.
This replaces the previous inconsistent naming convention of
'transportProperties' for incompressible solvers and
'thermophysicalProperties' for compressible solvers.
Backward-compatibility is provided by the solvers reading
'thermophysicalProperties' or 'transportProperties' if the
'physicalProperties' dictionary does not exist.
* phaseProperties
All multi-phase solvers (VoF and Euler-Euler) now read the list of phases and
interfacial models and coefficients from the
'constant/<region>/phaseProperties' dictionary.
Backward-compatibility is provided by the solvers reading
'thermophysicalProperties' or 'transportProperties' if the 'phaseProperties'
dictionary does not exist. For incompressible VoF solvers the
'transportProperties' is automatically upgraded to 'phaseProperties' and the
two 'physicalProperties.<phase>' dictionary for the phase properties.
* viscosity
Abstract base-class (interface) for all fluids.
Having a single interface for the viscosity of all types of fluids facilitated
a substantial simplification of the 'momentumTransport' library, avoiding the
need for a layer of templating and providing total consistency between
incompressible/compressible and single-phase/multi-phase laminar, RAS and LES
momentum transport models. This allows the generalised Newtonian viscosity
models to be used in the same form within laminar as well as RAS and LES
momentum transport closures in any solver. Strain-rate dependent viscosity
modelling is particularly useful with low-Reynolds number turbulence closures
for non-Newtonian fluids where the effect of bulk shear near the walls on the
viscosity is a dominant effect. Within this framework it would also be
possible to implement generalised Newtonian models dependent on turbulent as
well as mean strain-rate if suitable model formulations are available.
* visosityModel
Run-time selectable Newtonian viscosity model for incompressible fluids
providing the 'viscosity' interface for 'momentumTransport' models.
Currently a 'constant' Newtonian viscosity model is provided but the structure
supports more complex functions of time, space and fields registered to the
region database.
Strain-rate dependent non-Newtonian viscosity models have been removed from
this level and handled in a more general way within the 'momentumTransport'
library, see section 'viscosity' above.
The 'constant' viscosity model is selected in the 'physicalProperties'
dictionary by
viscosityModel constant;
which is equivalent to the previous entry in the 'transportProperties'
dictionary
transportModel Newtonian;
but backward-compatibility is provided for both the keyword and model
type.
* thermophysicalModels
To avoid propagating the unnecessary constructors from 'dictionary' into the
new 'physicalProperties' abstract base-class this entire structure has been
removed from the 'thermophysicalModels' library. The only use for this
constructor was in 'thermalBaffle' which now reads the 'physicalProperties'
dictionary from the baffle region directory which is far simpler and more
consistent and significantly reduces the amount of constructor code in the
'thermophysicalModels' library.
* compressibleInterFoam
The creation of the 'viscosity' interface for the 'momentumTransport' models
allows the complex 'twoPhaseMixtureThermo' derived from 'rhoThermo' to be
replaced with the much simpler 'compressibleTwoPhaseMixture' derived from the
'viscosity' interface, avoiding the myriad of unused thermodynamic functions
required by 'rhoThermo' to be defined for the mixture.
Same for 'compressibleMultiphaseMixture' in 'compressibleMultiphaseInterFoam'.
This is a significant improvement in code and input consistency, simplifying
maintenance and further development as well as enhancing usability.
Henry G. Weller
CFD Direct Ltd.
For a set to zone conversion the name of the zone is now specified with the
'zone' keyword.
For a patch to set conversion the name of the patch is now specified with the
'patch' keyword.
Backward-compatibility is supported for both these changes.
Additionally the file name of a searchableSurface file is specified with the
'file' keyword. This should be 'surface' but that keyword is currently and
confusingly used for the surface type rather than name and this cannot be
changed conveniently while maintaining backward compatibility.
and only needed if there is a name clash between entries in the source
specification and the set specification, e.g. "name":
{
name rotorCells;
type cellSet;
action new;
source zoneToCell;
sourceInfo
{
name cylinder;
}
}
topoSet is a more flexible and extensible replacement for setSet using standard
OpenFOAM dictionary input format rather than the limited command-line input
format developed specifically for setSet. This replacement allows for the
removal of a significant amount of code simplifying maintenance and the addition
of more topoSet sources.
When using 'simple' or 'hierarchical' decomposition it is useful to slightly rotate a
coordinate-aligned block-mesh to improve the processor boundaries by avoiding
irregular cell distribution at those boundaries. The degree of slight rotation
is controlled by the 'delta' coefficient and a value of 0.001 is generally
suitable so to avoid unnecessary clutter in 'decomposeParDict' 'delta' now
defaults to this value.
The FOAM file format has not changed from version 2.0 in many years and so there
is no longer a need for the 'version' entry in the FoamFile header to be
required and to reduce unnecessary clutter it is now optional, defaulting to the
current file format 2.0.
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
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.
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 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
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
A new run-time selectable interface compression scheme framework has been added
to the two-phase VoF solvers to provide greater flexibility, extensibility and
more consistent user-interface. The previously built-in interface compression
is now in the standard run-time selectable surfaceInterpolationScheme
interfaceCompression:
Class
Foam::interfaceCompression
Description
Interface compression corrected scheme, based on counter-gradient
transport, to maintain sharp interfaces during VoF simulations.
The interface compression is applied to the face interpolated field from a
suitable 2nd-order shape-preserving NVD or TVD scheme, e.g. vanLeer or
vanAlbada. A coefficient is supplied to control the degree of compression,
with a value of 1 suitable for most VoF cases to ensure interface integrity.
A value larger than 1 can be used but the additional compression can bias
the interface to follow the mesh more closely while a value smaller than 1
can lead to interface smearing.
Example:
\verbatim
divSchemes
{
.
.
div(phi,alpha) Gauss interfaceCompression vanLeer 1;
.
.
}
\endverbatim
The separate scheme for the interface compression term "div(phirb,alpha)" is no
longer required or used nor is the compression coefficient cAlpha in fvSolution
as this is now part of the "div(phi,alpha)" scheme specification as shown above.
Backward-compatibility is provided by checking the specified "div(phi,alpha)"
scheme against the known interface compression schemes and if it is not one of
those the new interfaceCompression scheme is used with the cAlpha value
specified in fvSolution.
More details can be found here:
https://cfd.direct/openfoam/free-software/multiphase-interface-capturing
Henry G. Weller
CFD Direct Ltd.
Following the generalisation of the TurbulenceModels library to support
non-Newtonian laminar flow including visco-elasticity and extensible to other
form of non-Newtonian behaviour the name TurbulenceModels is misleading and does
not properly represent how general the OpenFOAM solvers now are. The
TurbulenceModels now provides an interface to momentum transport modelling in
general and the plan is to rename it MomentumTransportModels and in preparation
for this the turbulenceProperties dictionary has been renamed momentumTransport
to properly reflect its new more general purpose.
The old turbulenceProperties name is supported for backward-compatibility.
renaming the legacy keywords
RASModel -> model
LESModel -> model
laminarModel -> model
which is simpler and clear within the context in which they are specified, e.g.
RAS
{
model kOmegaSST;
turbulence on;
printCoeffs on;
}
rather than
RAS
{
RASModel kOmegaSST;
turbulence on;
printCoeffs on;
}
The old keywords are supported for backward compatibility.
Description
Reciprocal polynomial equation of state for liquids and solids
\f[
1/\rho = C_0 + C_1 T + C_2 T^2 - C_3 p - C_4 p T
\f]
This polynomial for the reciprocal of the density provides a much better fit
than the equivalent polynomial for the density and has the advantage that it
support coefficient mixing to support liquid and solid mixtures in an
efficient manner.
Usage
\table
Property | Description
C | Density polynomial coefficients
\endtable
Example of the specification of the equation of state for pure water:
\verbatim
equationOfState
{
C (0.001278 -2.1055e-06 3.9689e-09 4.3772e-13 -2.0225e-16);
}
\endverbatim
Note: This fit is based on the small amount of data which is freely
available for the range 20-65degC and 1-100bar.
This equation of state is a much better fit for water and other liquids than
perfectFluid and in general polynomials for the reciprocal of the density
converge much faster than polynomials of the density. Currently rPolynomial is
quadratic in the temperature and linear in the pressure which is sufficient for
modest ranges of pressure typically encountered in CFD but could be extended to
higher order in pressure and/temperature if necessary. The other huge advantage
in formulating the equation of state in terms of the reciprocal of the density
is that coefficient mixing is simple.
Given these advantages over the perfectFluid equation of state the libraries and
tutorial cases have all been updated to us rPolynomial rather than perfectFluid
for liquids and water in particular.
Implementation of the Giesekus model for visco-elasticity, derived from the new
generalised form of the Maxwell model which now support additional sources.
Giesekus, H., 1982.
A simple constitutive equation for polymer fluids based on the
concept of deformation-dependent tensional mobility.
J. Non-Newton. Fluid. 11, 69–109.
This implementation is instantiated for incompressible, compressible and VoF
two-phase flow.
Now for transient simulations "Final" solver settings are required for ALL
equations providing consistency between the solution of velocity, energy,
composition and radiation properties.
However "Final" relaxation factors are no longer required for fields or
equations and if not present the standard value for the variable will be
applied. Given that relaxation factors other than 1 are rarely required for
transient runs and hence the same for all iterations including the final one
this approach provide simpler input while still providing the flexibility to
specify a different value for the final iteration if required. For steady cases
it is usual to execute just 1 outer iteration per time-step for which the
standard relaxation factors are appropriate, and if more than one iteration is
executed it is common to use the same factors for both. In the unlikely event
of requiring different relaxation factors for the final iteration this is still
possible to specify via the now optional "Final" specification.
to avoid the need to evaluate departure functions and simplify evaluation of the
temperature. In general it makes more sense to use and e/Cv based
thermodynamics when solving for internal energy rather than h/Cp and have
convert between the energy forms.
All related tutorials and test cases have also been updated.
The new momentum stress model selector class
compressibleInterPhaseTransportModel is now used to select between the options:
Description
Transport model selection class for the compressibleInterFoam family of
solvers.
By default the standard mixture transport modelling approach is used in
which a single momentum stress model (laminar, non-Newtonian, LES or RAS) is
constructed for the mixture. However if the \c simulationType in
constant/turbulenceProperties is set to \c twoPhaseTransport the alternative
Euler-Euler two-phase transport modelling approach is used in which separate
stress models (laminar, non-Newtonian, LES or RAS) are instantiated for each
of the two phases allowing for different modeling for the phases.
Mixture and two-phase momentum stress modelling is now supported in
compressibleInterFoam, compressibleInterDyMFoam and compressibleInterFilmFoam.
The prototype compressibleInterPhaseTransportFoam solver is no longer needed and
has been removed.
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.
