Added calls to setFluxRequired for p in all incompressible solvers which
avoids the need to add fluxRequired entries in fvSchemes dictionary.
Will add calls to setFluxRequired to the rest of the solvers.
SIMPLEC (SIMPLE-consistent) is selected by setting "consistent" option true/yes:
SIMPLE
{
nNonOrthogonalCorrectors 0;
consistent yes;
}
which relaxes the pressure in a "consistent" manner and additional
relaxation of the pressure is not generally necessary. In addition
convergence of the p-U system is better and reliable with less
aggressive relaxation of the momentum equation, e.g. for the motorbike
tutorial:
relaxationFactors
{
equations
{
U 0.9;
k 0.7;
omega 0.7;
}
}
The cost per iteration is marginally higher but the convergence rate is
better so the number of iterations can be reduced.
The SIMPLEC algorithm also provides benefit for cases with large
body-forces, e.g. SRF, see tutorials/incompressible/SRFSimpleFoam/mixer
and feature request http://www.openfoam.org/mantisbt/view.php?id=1714
Description
Specify an etc file to include when reading dictionaries, expects a
single string to follow.
Searches for files from user/group/shipped directories.
The search scheme allows for version-specific and
version-independent files using the following hierarchy:
- \b user settings:
- ~/.OpenFOAM/\<VERSION\>
- ~/.OpenFOAM/
- \b group (site) settings (when $WM_PROJECT_SITE is set):
- $WM_PROJECT_SITE/\<VERSION\>
- $WM_PROJECT_SITE
- \b group (site) settings (when $WM_PROJECT_SITE is not set):
- $WM_PROJECT_INST_DIR/site/\<VERSION\>
- $WM_PROJECT_INST_DIR/site/
- \b other (shipped) settings:
- $WM_PROJECT_DIR/etc/
An example of the \c \#includeEtc directive:
\verbatim
#includeEtc "etcFile"
\endverbatim
The usual expansion of environment variables and other constructs is
retained.
For multi-region cases the default location of blockMeshDict is now system/<region name>
If the blockMeshDict is not found in system then the constant directory
is also checked providing backward-compatibility
The Phi field is read if available otherwise created automatically with
boundary conditions obtained automatically from the pressure field if
available (with optional name) otherwise inferred from the velocity
field. Phi Laplacian scheme and solver specification are required. See
tutorials for examples.
The old separate incompressible and compressible libraries have been removed.
Most of the commonly used RANS and LES models have been upgraded to the
new framework but there are a few missing which will be added over the
next few days, in particular the realizable k-epsilon model. Some of
the less common incompressible RANS models have been introduced into the
new library instantiated for incompressible flow only. If they prove to
be generally useful they can be templated for compressible and
multiphase application.
The Spalart-Allmaras DDES and IDDES models have been thoroughly
debugged, removing serious errors concerning the use of S rather than
Omega.
The compressible instances of the models have been augmented by a simple
backward-compatible eddyDiffusivity model for thermal transport based on
alphat and alphaEff. This will be replaced with a separate run-time
selectable thermal transport model framework in a few weeks.
For simplicity and ease of maintenance and further development the
turbulent transport and wall modeling is based on nut/nuEff rather than
mut/muEff for compressible models so that all forms of turbulence models
can use the same wall-functions and other BCs.
All turbulence model selection made in the constant/turbulenceProperties
dictionary with RAS and LES as sub-dictionaries rather than in separate
files which added huge complexity for multiphase.
All tutorials have been updated so study the changes and update your own
cases by comparison with similar cases provided.
Sorry for the inconvenience in the break in backward-compatibility but
this update to the turbulence modeling is an essential step in the
future of OpenFOAM to allow more models to be added and maintained for a
wider range of cases and physics. Over the next weeks and months more
turbulence models will be added of single and multiphase flow, more
additional sub-models and further development and testing of existing
models. I hope this brings benefits to all OpenFOAM users.
Henry G. Weller
When using models which require the wallDist e.g. kOmegaSST it will
request the method to be used from the wallDist sub-dictionary in
fvSchemes e.g.
wallDist
{
method meshWave;
}
specifies the mesh-wave method as hard-coded in previous OpenFOAM versions.
