The new multiphaseEulerFoam is based on reactingMultiphaseEulerFoam with some
improvements and rationalisation to assist maintenance and further development.
The phase system solution has been enhanced to handle two phases more
effectively and all two-phase specific models updated for compatibility so that
multiphaseEulerFoam can also replace reactingTwoPhaseEulerFoam.
When running multiphaseEulerFoam with only two-phases the default behaviour is
to solve for both phase-fractions but optionally a reference phase can be
specified so that only the other phase-fraction is solved, providing better
compatibility with the behaviour of reactingTwoPhaseEulerFoam.
All reactingMultiphaseEulerFoam and reactingTwoPhaseEulerFoam tutorials have
been updated for multiphaseEulerFoam.
The base phaseSystem now provides all the functionality needed for
reactingMultiphaseEulerFoam and twoPhaseSystem is a specialisation, simplifying
maintenance.
Description
This functionObject writes the phase-fraction map field alpha.map with
incremental value ranges for each phase
e.g., with values 0-1 for water, 1-2 for air, 2-3 for oil etc.
Example of function object specification:
\verbatim
phaseMap
{
type phaseMap;
libs ("libreactingEulerFoamFunctionObjects.so");
writeControl writeTime;
}
\endverbatim
Usage
\table
Property | Description | Required | Default value
type | type name: phaseMap | yes |
\endtable
This replaces the alphas functionality previously built-in to
reactingMultiphaseEulerFoam so that the storage, calculation and writing of the
phase map field is now under user control.
The optional reference phase fraction field is not read even if the file is
present, it is constructed with "calculated" BCs as it is a derived field. All
other phase fraction field files are read and now must be present.
for compatibility with reactingMultiphaseEulerFoam when run with two-phases.
Some of these two-phase models could be enhanced to operate with multiple
dispersed phases in the future.
In order to update these models for reactingMultiphaseEulerFoam it has been
necessary to break compatibility with the now redundant twoPhaseEulerFoam solver
which has been superseded by the much more capable reactingEulerFoam solvers and
now removed.
to ensure the velocity and flux of the phases sum the conservative mixture
values obtained from the pressure solution.
Also corrected handling of MRF and updated to work with partial elimination.
The cellZoneInjection now correctly fills all tets of a given cell with
a random distribution of particles. Previously an error in the
calculation of the cumulative tet volume fractions for a cell meant that
one tet never had any particles injected into it.
Added optional pressure reference pRef to p_rgh in buoyantPimpleFoam,
buoyantSimpleFoam and chtMultiRegionFoam which handles cases in which the
pressure variation is small compared to the pressure level more accurately.
The pRef value is provided in the optional constant/pRef file.
All tutorials and templates have been updated to use pRef as appropriate.
This change protects the lookup of the drag model so that if it is not
found then the drag terms in the Theta equation are set to zero. This is
not likely to be correct usage in physical cases, but is useful for
doing uncoupled simulations for the purpose of model verification.
A new family of interface compression interpolation schemes based on
piecewise-linear interface calculation (PLIC). PLIC represents an interface by
surface-cuts which split each cell to match the volume fraction of the phase in
that cell. The surface-cuts are oriented according to the point field of the
local phase fraction. The phase fraction on each cell face — the interpolated
value — is then calculated from the amount submerged below the surface-cut.
The basic PLIC method generates a single cut so cannot handle cells in which
there are multiple interfaces or where the interface is not fully resolved. In
those cells, the interpolation reverts to an alternative scheme, typically
standard interface compression. PLIC, with a fallback to interface compression,
produces robust solutions for real engineering cases. It can run with large time
steps so can solve problems like hydrodynamics of a planing hull, with rigid
body motion of the hull (above). The user selects PLIC by the following setting
in fvSchemes:
div(phi,alpha) Gauss PLIC interfaceCompression vanLeer 1;
The multicut PLIC (MPLIC) scheme extends PLIC to handle multiple
surface-cuts. Where a single cut is insufficient, MPLIC performs a topological
face-edge-face walk to produce multiple splits of a cell. If that is still
insufficient, MPLIC decomposes the cell into tetrahedrons on which the cuts are
applied. The extra cutting carries an additional computational cost but requires
no fallback. The user selects MPLIC by the following setting in the fvSchemes
file:
div(phi,alpha) Gauss MPLIC;
Variants of the PLIC and MPLIC schemes are also available which use velocities
at the face points to calculate the face flux. These PLICU and MPLICU schemes
are likely to be more accurate in regions of interface under high shear.
More details can be found here:
https://cfd.direct/openfoam/free-software/multiphase-interface-capturing
Jakub Knir
CFD Direct Ltd.
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.
Only perfectGas and real-gas equations of state are consistent with standard
Janaf thermo data based on Cp. Using other equations of state is possible but
the Janaf Cp data would have to be modified for consistency.
The term "departure function" relates to difference between real and ideal gas
thermodynamic properties but the implementation is more general than that and
handles all contributions from the equations of state to the thermodynamic
properties. To reflect this the term "departure" has been replaced with
"contribution".
This change means that fields that are solved for by function objects
(e.g., a scalar transport field) can now be included in time/iteration
loop convergence tests.
Resolves bug report https://bugs.openfoam.org/view.php?id=3510
The entropy contribution from the equation of state corrects the integral of the
heat capacity divided by temperature for changes in pressure in the case of Cp
named Sp or changes in volume in the case of Cv, named Sv. This for enthalpy
based thermodynamics Sp is needed and for internal energy Sv is needed.
