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
Time-dependent external force restraint using Function1.
Usage
Example applying a constant force to the floatingObject:
restraints
{
force
{
type externalForce;
body floatingObject;
location (0 0 0);
force (100 0 0);
}
}
Based on code contributed by SeongMo Yeon
Resolves contribution request https://bugs.openfoam.org/view.php?id=3358
With the -noFields option the mesh is subset but the fields are not changed.
This is useful when the field fields have been created to correspond to the mesh
after the mesh subset.
and replaced interDyMFoam with a script which reports this change.
The interDyMFoam tutorials have been moved into the interFoam directory.
This change is one of a set of developments to merge dynamic mesh functionality
into the standard solvers to improve consistency, usability, flexibility and
maintainability of these solvers.
Henry G. Weller
CFD Direct Ltd.
