The floatingObject tutorial has been update to demonstrate this functionality by
adding the following topoChanger entry to dynamicMeshDict:
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)
(ghf none)
);
// Write the refinement level as a volScalarField
dumpLevel true;
}
Note that currently only single rigid body motion is supported (but multi-body
support will be added shortly) and the Crank-Nicolson scheme is not supported.
Description
Evolves a passive scalar transport equation.
- To specify the field name set the \c field entry
- To employ the same numerical schemes as another field set
the \c schemesField entry,
- The \c diffusivity entry can be set to \c none, \c constant, \c viscosity
- A constant diffusivity is specified with the \c D entry,
- If a momentum transport model is available and the \c viscosity
diffusivety option specified an effective diffusivity may be constructed
from the laminar and turbulent viscosities using the diffusivity
coefficients \c alphal and \c alphat:
\verbatim
D = alphal*nu + alphat*nut
\endverbatim
Example:
\verbatim
#includeFunc scalarTransport(T, alphaD=1, alphaDt=1)
\endverbatim
For incompressible flow the passive scalar may optionally be solved with the
MULES limiter and sub-cycling or semi-implicit in order to maintain
boundedness, particularly if a compressive, PLIC or MPLIC convection
scheme is used.
Example:
\verbatim
#includeFunc scalarTransport(tracer, diffusion=none)
with scheme specification:
div(phi,tracer) Gauss interfaceCompression vanLeer 1;
and solver specification:
tracer
{
nCorr 1;
nSubCycles 3;
MULESCorr no;
nLimiterIter 5;
applyPrevCorr yes;
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-8;
relTol 0;
diffusion
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-8;
relTol 0;
}
}
\endverbatim
replacing the virtual functions overridden in engineTime.
Now the userTime conversion function in Time is specified in system/controlDict
such that the solver as well as all pre- and post-processing tools also operate
correctly with the chosen user-time.
For example the user-time and rpm in the tutorials/combustion/XiEngineFoam/kivaTest case are
now specified in system/controlDict:
userTime
{
type engine;
rpm 1500;
}
The default specification is real-time:
userTime
{
type real;
}
but this entry can be omitted as the real-time class is instantiated
automatically if the userTime entry is not present in system/controlDict.
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.
for consistency with the regionToCell topo set source and splitMeshRegions and
provides more logical extension to the multiple and outside point variants insidePoints,
outsidePoint and outsidePoints.
This required standardisation of the mapping between the class and selection
names of the solid transport models:
constIso -> constIsoSolid
exponential -> exponentialSolid
polynomial -> polynomialSolid
To simplify maintenance and further development of chemistry solution the
standardChemistryModel and TDACChemistryModel have been merged into the single
chemistryModel class. Now the TDAC mechanism reduction and tabulation
components can be individually selected or set to "none" or the corresponding
entries in the chemistryProperties dictionary omitted to switch them off thus
reproducing the behaviour of the standardChemistryModel.
For example the following chemistryProperties includes TDAC:
#includeEtc "caseDicts/solvers/chemistry/TDAC/chemistryProperties.cfg"
chemistryType
{
solver ode;
}
chemistry on;
initialChemicalTimeStep 1e-7;
odeCoeffs
{
solver seulex;
absTol 1e-8;
relTol 1e-1;
}
reduction
{
tolerance 1e-4;
}
tabulation
{
tolerance 3e-3;
}
#include "reactionsGRI"
and to run without TDAC the following is sufficient:
chemistryType
{
solver ode;
}
chemistry on;
initialChemicalTimeStep 1e-7;
odeCoeffs
{
solver seulex;
absTol 1e-8;
relTol 1e-1;
}
#include "reactionsGRI"
or the "reduction" and "tabulation" entries can be disabled explicitly:
#includeEtc "caseDicts/solvers/chemistry/TDAC/chemistryProperties.cfg"
chemistryType
{
solver ode;
}
chemistry on;
initialChemicalTimeStep 1e-7;
odeCoeffs
{
solver seulex;
absTol 1e-8;
relTol 1e-1;
}
reduction
{
method none;
tolerance 1e-4;
}
tabulation
{
method none;
tolerance 3e-3;
}
#include "reactionsGRI"
The mesh in the upstream region of this case has been refined back to
its original density. This restores the wave propagation behaviour
through this region.
It is now possible to use waveVelocity and waveAlpha boundary conditions
in cases in which the waves generate localised flow reversals along the
boundary. This means waves can be speficied at arbitrary directions and
with zero mean flow. Previously and integral approach, similar to
flowRateOutlet, was used, which was only correct when the direction of
wave propagation was aligned with the boundary normal.
This improvement has been achieved by reformulating the waveVelocity and
waveAlpha boundary conditions in terms of a new fixedValueInletOutlet
boundary condition type. This condition enforces a fixed value in all
cases except that of advection terms in the presence of outflow. In this
configuration a gradient condition is applied that will relax towards
the desired fixed value.
The wavePressure boundary condition has been removed, as it is no longer
necessary or advisable to locally switch between velocity and pressure
formulations along a wave boundary. Wave boundaries should now have the
general fixedFluxPressure or fixedFluxExtrapolatedPressure conditions
applied to the pressure field.
Two new tutorial cases have been created to demonstrate the new
functionality. The multiphase/interFoam/laminar/wave3D case demonstrates
wave generation with zero mean flow and at arbitrary angles to the
boundaries, and incompressible/pimpleFoam/RAS/waveSubSurface
demonstrates usage for sub-surface problems.
Changed the laminar methane combustion cases to use the Wilke mixing rule for
the transport properties obtained from the Sutherland model but with coefficient
mixing for thermodynamic properties for efficient evaluation of reaction
equilibria.
This provides significantly more accurate results for laminar combustion,
producing a thinner flame and a 10K reduction in peak temperature.
to the <case>/<time>/uniform or <case>/<processor>/<time>/uniform directory.
Adding a new form of IOdictionary for this purpose allows significant
simplification and rationalisation of regIOobject::writeObject, removing the
need for explicit treatment of different file types.
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.
Removed the combustion/reactingFoam/Lagrangian/counterFlowFlame2DLTS
case as it was originally a consistency check between reactingFoam and
reactingParcelFoam. It is not necessary now these solvers have been
combined.
Removed an unused fvModels file in the
reactingFoam/Lagrangian/simplifiedSiwek tutorial.
A number of changes have been made to the surfaceFieldValue and
volFieldValue function objects to improve their usability and
performance, and to extend them so that similar duplicate functionality
elsewhere in OpenFOAM can be removed.
Weighted operations have been removed. Weighting for averages and sums
is now triggered simply by the existence of the "weightField" or
"weightFields" entry. Multiple weight fields are now supported in both
functions.
The distinction between oriented and non-oriented fields has been
removed from surfaceFieldValue. There is now just a single list of
fields which are operated on. Instead of oriented fields, an
"orientedSum" operation has been added, which should be used for
flowRate calculations and other similar operations on fluxes.
Operations minMag and maxMag have been added to both functions, to
calculate the minimum and maximum field magnitudes respectively. The min
and max operations are performed component-wise, as was the case
previously.
In volFieldValue, minMag and maxMag (and min and mag operations when
applied to scalar fields) will report the location, cell and processor
of the maximum or minimum value. There is also a "writeLocation" option
which if set will write this location information into the output file.
The fieldMinMax function has been made obsolete by this change, and has
therefore been removed.
surfaceFieldValue now operates in parallel without accumulating the
entire surface on the master processor for calculation of the operation.
Collecting the entire surface on the master processor is now only done
if the surface itself is to be written out.
With this change both of the following commands are equivalent:
topoSet -region air -dict topoSetDict1
topoSet -region air -dict system/air/topoSetDict1
I.e., if the system/<regionName> path is not specified then it is
assumed.
With this change both
blockMesh -dict fineBlockMeshDict
blockMesh -dict system/fineBlockMeshDict
are supported, if the system/ path is not specified it is assumed
Settings for the particleTracks utility are now specified in
system/particleTracksDict. Correspondingly, settings for
steadyParticleTracks are now specified in
system/steadyParticleTracksDict.
The -dict option is now handled correctly and consistently across all
applications with -dict options. The logic associated with doing so has
been centralised.
If a relative path is given to the -dict option, then it is assumed to
be relative to the case directory. If an absolute path is given, then it
is used without reference to the case directory. In both cases, if the
path is found to be a directory, then the standard dictionary name is
appended to the path.
Resolves bug report http://bugs.openfoam.org/view.php?id=3692
This is the 2006 version of Wilcox's k-omega RAS turbulence model which has some
similarities in formulation and behaviour to the k-omega-SST model but is much
simpler and cleaner. This model is likely to perform just as well as the
k-omega-SST model for a wide range of engineering cases.
Description
Standard (2006) high Reynolds-number k-omega turbulence model for
incompressible and compressible flows.
References:
\verbatim
Wilcox, D. C. (2006).
Turbulence modeling for CFD, 3rd edition
La Canada, CA: DCW industries, Inc.
Wilcox, D. C. (2008).
Formulation of the kw turbulence model revisited.
AIAA journal, 46(11), 2823-2838.
\endverbatim
The default model coefficients are
\verbatim
kOmega2006Coeffs
{
Cmu 0.09;
beta0 0.0708;
gamma 0.52;
Clim 0.875;
alphak 0.6;
alphaOmega 0.5;
}
\endverbatim
splitBaffles identifies baffle faces; i.e., faces on the mesh boundary
which share the exact same set of points as another boundary face. It
then splits the points to convert these faces into completely separate
boundary patches. This functionality was previously provided by calling
mergeOrSplitBaffles with the "-split" option.
mergeBaffles also identifes the duplicate baffle faces, but then merges
them, converting them into a single set of internal faces. This
functionality was previously provided by calling mergeOrSplitBaffles
without the "-split" option.
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.
Solving for enthalpy provides better convergence and stability than internal
energy. Also correctPhi is now off pending the addition of compressibility
effects to the pcorr equation.
