Contributed by Bruno Santos
Resolves patch report http://www.openfoam.org/mantisbt/view.php?id=2023

Update online documentation http://openfoam.github.io/Documentation-dev/html/

The deprecated non-const tmp functionality is now on the compiler switch
NON_CONST_TMP which can be enabled by adding -DNON_CONST_TMP to EXE_INC
in the Make/options file.  However, it is recommended to upgrade all
code to the new safer tmp by using the '.ref()' member function rather
than the non-const '()' dereference operator when non-const access to
the temporary object is required.

Please report any problems on Mantis.

Henry G. Weller
CFD Direct.

To be used instead of zeroGradientFvPatchField for temporary fields for
which zero-gradient extrapolation is use to evaluate the boundary field
but avoiding fields derived from temporary field using field algebra
inheriting the zeroGradient boundary condition by the reuse of the
temporary field storage.

zeroGradientFvPatchField should not be used as the default patch field
for any temporary fields and should be avoided for non-temporary fields
except where it is clearly appropriate;
extrapolatedCalculatedFvPatchField and calculatedFvPatchField are
generally more suitable defaults depending on the manner in which the
boundary values are specified or evaluated.

The entire OpenFOAM-dev code-base has been updated following the above
recommendations.

Henry G. Weller
CFD Direct

The boundary conditions of HbyA are now constrained by the new "constrainHbyA"
function which applies the velocity boundary values for patches for which the
velocity cannot be modified by assignment and pressure extrapolation is
not specified via the new
"fixedFluxExtrapolatedPressureFvPatchScalarField".

The new function "constrainPressure" sets the pressure gradient
appropriately for "fixedFluxPressureFvPatchScalarField" and
"fixedFluxExtrapolatedPressureFvPatchScalarField" boundary conditions to
ensure the evaluated flux corresponds to the known velocity values at
the boundary.

The "fixedFluxPressureFvPatchScalarField" boundary condition operates
exactly as before, ensuring the correct flux at fixed-flux boundaries by
compensating for the body forces (gravity in particular) with the
pressure gradient.

The new "fixedFluxExtrapolatedPressureFvPatchScalarField" boundary
condition may be used for cases with or without body-forces to set the
pressure gradient to compensate not only for the body-force but also the
extrapolated "HbyA" which provides a second-order boundary condition for
pressure.  This is useful for a range a problems including impinging
flow, extrapolated inlet conditions with body-forces or for highly
viscous flows, pressure-induced separation etc.  To test this boundary
condition at walls in the motorBike tutorial case set

    lowerWall
    {
        type            fixedFluxExtrapolatedPressure;
    }

    motorBikeGroup
    {
        type            fixedFluxExtrapolatedPressure;
    }

Currently the new extrapolated pressure boundary condition is supported
for all incompressible and sub-sonic compressible solvers except those
providing implicit and tensorial porosity support.  The approach will be
extended to cover these solvers and options in the future.

Note: the extrapolated pressure boundary condition is experimental and
requires further testing to assess the range of applicability,
stability, accuracy etc.

Henry G. Weller
CFD Direct Ltd.

Provides support for running laminar.

It is better to declare the namespace of each function in the C file
rather than "open" the namespace as this may lead to inconsistencies
between the declaration in the H files and definition in the C file.

fvOptions are transferred to the database on construction using
fv::options::New which returns a reference.  The same function can be
use for construction and lookup so that fvOptions are now entirely
demand-driven.

The abstract base-classes for fvOptions now reside in the finiteVolume
library simplifying compilation and linkage.  The concrete
implementations of fvOptions are still in the single monolithic
fvOptions library but in the future this will be separated into smaller
libraries based on application area which may be linked at run-time in
the same manner as functionObjects.

See also commit 82ccde32

Simplifies lookup of RAS or LES models

Avoids the clutter and maintenance effort associated with providing the
function signature string.

Now consistent with constructors.

Resolves bug-report http://www.openfoam.org/mantisbt/view.php?id=1816

to simplify construction of dimensionedScalar properties and avoid the
duplication of the name string in the constructor call.

Added calls to setFluxRequired for p, p_rgh etc. in all solvers which
avoids the need to add fluxRequired entries in fvSchemes dictionaries.

    Select LTS via the ddtScheme:

        ddtSchemes
        {
            default         localEuler rDeltaT;
        }

See tutorials/compressible/rhoSimpleFoam/squareBend

SIMPLE
{
    nNonOrthogonalCorrectors 0;
    rhoMin          0.1;
    rhoMax          1.0;
    transonic       yes;
    consistent      yes;

    residualControl
    {
        p               1e-3;
        U               1e-4;
        e               1e-3;

        // possibly check turbulence fields
        "(k|epsilon|omega)" 1e-3;
    }
}

relaxationFactors
{
    fields
    {
        p               1;
        rho             1;
    }
    equations
    {
        p               1;
        U               0.9;
        e               0.9;
        k               0.9;
        epsilon         0.9;
    }
}

e.g. in tutorials/compressible/rhoPimpleFoam/ras/angledDuctLTS

PIMPLE
{
    momentumPredictor   yes;
    transonic           no;
    nOuterCorrectors    50;
    nCorrectors         1;
    nNonOrthogonalCorrectors 0;
    consistent          yes;

    rhoMin          0.5;
    rhoMax          2.0;

    residualControl
    {
        "(U|k|epsilon)"
        {
            relTol          0;
            tolerance       0.0001;
        }
    }

    turbOnFinalIterOnly off;
}

relaxationFactors
{
    fields
    {
        "p.*"           0.9;
        "rho.*"         1;
    }
    equations
    {
        "U.*"           0.9;
        "h.*"           0.7;
        "(k|epsilon|omega).*" 0.8;
    }
}

LTS is selected by the ddt scheme e.g. in the
tutorials/multiphase/interFoam/ras/DTCHull case:

ddtSchemes
{
    default         localEuler rDeltaT;
}

LTSInterFoam is no longer needed now that interFoam includes LTS
support.

Select LTS via the ddtScheme:

ddtSchemes
{
    default         localEuler rDeltaT;
}

The LTS algorithm is controlled with the standard settings in
controlDict, e.g.:

maxCo           0.5;
maxDeltaT       2e-8;

with the addition of the optional rDeltaT smoothing coefficient:

rDeltaTSmoothingCoeff 0.02;

which defaults to 0.02.

For cases with reasonably uniform meshes like the forwardStep tutorial
LTS does not provide much benefit but for cases with large variation in
cell-size like the biconic25-55Run35 tutorial LTS provides significant
speed-up to convergence particularly if started from uniform conditions.

Reverted changes proposed in
http://openfoam.org/mantisbt/view.php?id=1548 as it adversely affects
fixed-value BCs and is formulated to fix an issue with an unphysical
case.  Further analysis of the handling of fixed pressure outlet
conditions as the Mach number approaches 1 is required.

Now consistent with the way the Courant number is calculated for other solvers

Resolves bug-report http://www.openfoam.org/mantisbt/view.php?id=1748

Resolves bug-report http://openfoam.org/mantisbt/view.php?id=1730

fvOptions does not have the appropriate structure to support MRF as it
is based on option selection by user-specified fields whereas MRF MUST
be applied to all velocity fields in the particular solver.  A
consequence of the particular design choices in fvOptions made it
difficult to support MRF for multiphase and it is easier to support
frame-related and field related options separately.

Currently the MRF functionality provided supports only rotations but
the structure will be generalized to support other frame motions
including linear acceleration, SRF rotation and 6DoF which will be
run-time selectable.

Resolves bug-report http://www.openfoam.org/mantisbt/view.php?id=1421

Resolves bug-report http://openfoam.org/mantisbt/view.php?id=1548

Resolves bug-report http://openfoam.org/mantisbt/view.php?id=1548

Needed to create generic compressible turbulence model library