sixDoFRigidBodyDisplacementPointPatchVectorField, uncoupledSixDoFRigidBodyDisplacementPointPatchVectorField: removed

These legacy boundary conditions are no longer needed and have been superseded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

Resolves bug-report https://bugs.openfoam.org/view.php?id=2459

Resolves bug-report https://bugs.openfoam.org/view.php?id=2489

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.

Patch contributed by Mattijs Janssens

Fewer limiter iterations are now required to obtain sufficient boundedness and
restart is more consistent.

PBiCGStab has proved more reliable than PCG for solving the pressure equation in
compressible systems.

Resolves bug-report https://bugs.openfoam.org/view.php?id=2475

Both stardard SIMPLE and the SIMPLEC (using the 'consistent' option in
fvSolution) are now supported for both subsonic and transonic flow of all
fluid types.

rhoPimpleFoam now instantiates the lower-level fluidThermo which instantiates
either a psiThermo or rhoThermo according to the 'type' specification in
thermophysicalProperties, see also commit a1c8cde3

Resolves bug-report https://bugs.openfoam.org/view.php?id=2477

Both stardard SIMPLE and the SIMPLEC (using the 'consistent' option in
fvSolution) are now supported for both subsonic and transonic flow of all
fluid types.

rhoSimpleFoam now instantiates the lower-level fluidThermo which instantiates
either a psiThermo or rhoThermo according to the 'type' specification in
thermophysicalProperties, e.g.

thermoType
{
    type            hePsiThermo;
    mixture         pureMixture;
    transport       sutherland;
    thermo          janaf;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleInternalEnergy;
}

instantiates a psiThermo for a perfect gas with JANAF thermodynamics, whereas

thermoType
{
    type            heRhoThermo;
    mixture         pureMixture;
    properties      liquid;
    energy          sensibleInternalEnergy;
}

mixture
{
    H2O;
}

instantiates a rhoThermo for water, see new tutorial
compressible/rhoSimpleFoam/squareBendLiq.

In order to support complex equations of state the pressure can no longer be
unlimited and rhoSimpleFoam now limits the pressure rather than the density to
handle start-up more robustly.

For backward compatibility 'rhoMin' and 'rhoMax' can still be used in the SIMPLE
sub-dictionary of fvSolution which are converted into 'pMax' and 'pMin' but it
is better to set either 'pMax' and 'pMin' directly or use the more convenient
'pMinFactor' and 'pMinFactor' from which 'pMax' and 'pMin' are calculated using
the fixed boundary pressure or reference pressure e.g.

SIMPLE
{
    nNonOrthogonalCorrectors 0;

    pMinFactor      0.1;
    pMaxFactor      1.5;

    transonic       yes;
    consistent      yes;

    residualControl
    {
        p               1e-3;
        U               1e-4;
        e               1e-3;
        "(k|epsilon|omega)" 1e-3;
    }
}

Resolves bug-report https://bugs.openfoam.org/view.php?id=2470

Resolves bug-report https://bugs.openfoam.org/view.php?id=2470

functionObjects::fieldCoordinateSystemTransform: added coordinateSystem sub-dict and updated the description

Patch contributed by Bruno Santos
Resolves bug-report https://bugs.openfoam.org/view.php?id=2454

This allows single, multi-phase and VoF compressible simulations to be performed
with the accurate thermophysical property functions for liquids provided by the
liquidProperty classes.  e.g. in the
multiphase/compressibleInterFoam/laminar/depthCharge2D tutorial water can now be
specified by

thermoType
{
    type            heRhoThermo;
    mixture         pureMixture;
    properties      liquid;
    energy          sensibleInternalEnergy;
}

mixture
{
    H2O;
}

as an alternative to the previous less accurate representation defined by

thermoType
{
    type            heRhoThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState perfectFluid;
    specie          specie;
    energy          sensibleInternalEnergy;
}

mixture
{
    specie
    {
        molWeight   18.0;
    }
    equationOfState
    {
        R           3000;
        rho0        1027;
    }
    thermodynamics
    {
        Cp          4195;
        Hf          0;
    }
    transport
    {
        mu          3.645e-4;
        Pr          2.289;
    }
}

However the increase in accuracy of the new simpler and more convenient
specification and representation comes at a cost: the NSRDS functions used by
the liquidProperties classes are relatively expensive to evaluate and the
depthCharge2D case takes ~14% longer to run.

Description
    Base-class for thermophysical properties of solids, liquids and gases
    providing an interface compatible with the templated thermodynamics
    packages.

liquidProperties, solidProperties and thermophysicalFunction libraries have been
combined with the new thermophysicalProperties class into a single
thermophysicalProperties library to simplify compilation and linkage of models,
libraries and applications dependent on these classes.

The entries for liquid and solid species can now be simply be the name unless
property coefficients are overridden in which are specified in a dictionary as
before e.g. in the tutorials/lagrangian/coalChemistryFoam/simplifiedSiwek case
the water is simply specified

liquids
{
    H2O;
}

and solid ash uses standard coefficients but the coefficients for carbon are
overridden thus

solids
{
    C
    {
        rho             2010;
        Cp              710;
        kappa           0.04;
        Hf              0;
        emissivity      1.0;
    }

    ash;
}

The defaultCoeffs entry is now redundant and supported only for backward
compatibility.  To specify a liquid with default coefficients simply leave the
coefficients dictionary empty:

    liquids
    {
        H2O {}
    }

Any or all of the coefficients may be overridden by specifying the properties in
the coefficients dictionary, e.g.

    liquids
    {
        H2O
        {
            rho
            {
                a 1000;
                b 0;
                c 0;
                d 0;
            }
        }
    }

When liquids are constructed from dictionary the coefficients are now first
initialized to their standard values and overridden by the now optional entries
provided in the dictionary.  For example to specify water with all the standard
temperature varying properties but override only the density with a constant
value of 1000 specify in thermophysicalProperties

liquids
{
    H2O
    {
        defaultCoeffs   no;

        H2OCoeffs
        {
            rho
            {
                a 1000;
                b 0;
                c 0;
                d 0;
            }
        }
    }
}

The fundamental properties provided by the specie class hierarchy were
mole-based, i.e. provide the properties per mole whereas the fundamental
properties provided by the liquidProperties and solidProperties classes are
mass-based, i.e. per unit mass.  This inconsistency made it impossible to
instantiate the thermodynamics packages (rhoThermo, psiThermo) used by the FV
transport solvers on liquidProperties.  In order to combine VoF with film and/or
Lagrangian models it is essential that the physical propertied of the three
representations of the liquid are consistent which means that it is necessary to
instantiate the thermodynamics packages on liquidProperties.  This requires
either liquidProperties to be rewritten mole-based or the specie classes to be
rewritten mass-based.  Given that most of OpenFOAM solvers operate
mass-based (solve for mass-fractions and provide mass-fractions to sub-models it
is more consistent and efficient if the low-level thermodynamics is also
mass-based.

This commit includes all of the changes necessary for all of the thermodynamics
in OpenFOAM to operate mass-based and supports the instantiation of
thermodynamics packages on liquidProperties.

Note that most users, developers and contributors to OpenFOAM will not notice
any difference in the operation of the code except that the confusing

    nMoles     1;

entries in the thermophysicalProperties files are no longer needed or used and
have been removed in this commet.  The only substantial change to the internals
is that species thermodynamics are now "mixed" with mass rather than mole
fractions.  This is more convenient except for defining reaction equilibrium
thermodynamics for which the molar rather than mass composition is usually know.
The consequence of this can be seen in the adiabaticFlameT, equilibriumCO and
equilibriumFlameT utilities in which the species thermodynamics are
pre-multiplied by their molecular mass to effectively convert them to mole-basis
to simplify the definition of the reaction equilibrium thermodynamics, e.g. in
equilibriumCO

    // Reactants (mole-based)
    thermo FUEL(thermoData.subDict(fuelName)); FUEL *= FUEL.W();

    // Oxidant (mole-based)
    thermo O2(thermoData.subDict("O2")); O2 *= O2.W();
    thermo N2(thermoData.subDict("N2")); N2 *= N2.W();

    // Intermediates (mole-based)
    thermo H2(thermoData.subDict("H2")); H2 *= H2.W();

    // Products (mole-based)
    thermo CO2(thermoData.subDict("CO2")); CO2 *= CO2.W();
    thermo H2O(thermoData.subDict("H2O")); H2O *= H2O.W();
    thermo CO(thermoData.subDict("CO")); CO *= CO.W();

    // Product dissociation reactions

    thermo CO2BreakUp
    (
        CO2 == CO + 0.5*O2
    );

    thermo H2OBreakUp
    (
        H2O == H2 + 0.5*O2
    );

Please report any problems with this substantial but necessary rewrite of the
thermodynamic at https://bugs.openfoam.org

Henry G. Weller
CFD Direct Ltd.

functionObjects::scalarTransport: Added support for optional laminar and turbulent diffusion coefficients

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,
    - A constant diffusivity may be specified with the \c D entry,

    - Alternatively if a turbulence model is available a turbulent diffusivity
      may be constructed from the laminar and turbulent viscosities using the
      optional diffusivity coefficients \c alphaD and \c alphaDt (which default
      to 1):
      \verbatim
          D = alphaD*nu + alphaDt*nut
      \endverbatim

Resolves feature request https://bugs.openfoam.org/view.php?id=2453

Resolves bug-report https://bugs.openfoam.org/view.php?id=2455

Now the interFoam and compressibleInterFoam families of solvers use the same
alphaEqn formulation and supporting all of the MULES options without
code-duplication.

The semi-implicit MULES support allows running with significantly larger
time-steps but this does reduce the interface sharpness.