The defaultPatch type currently defaults to empty which is appropriate for 1D
and 2D cases but not when creating the initial blockMesh for snappyHexMesh as
the presence of empty patches triggers the inappropriate application of 2D point
constraint corrections following snapping and morphing. To avoid this hidden
problem a warning is now generated from blockMesh when the defaultPatch is not
explicitly set for cases which generate a default patch, i.e. for which the
boundary is not entirely defined. e.g.
.
.
.
Creating block mesh topology
--> FOAM FATAL IO ERROR:
The 'defaultPatch' type must be specified for the 'defaultFaces' patch, e.g. for snappyHexMesh
defaultPatch
{
name default; // optional
type patch;
}
or for 2D meshes
defaultPatch
{
name frontAndBack; // optional
type empty;
}
.
.
.
All the tutorials have been update to include the defaultPatch specification as
appropriate.
For most multiphase flows it is more appropriate to evaluate the total pressure
from the static pressure obtained from p_rgh rather than from p_rgh directly.
Alpha contact angle boundaries are now specified in the following way
for multiphase solvers (i.e., multiphaseInterFoam,
compressibleMultiphaseInterFoam, and multiphaseEulerFoam):
boundaryField
{
wall
{
type alphaContactAngle;
contactAngleProperties
{
water
{
// Constant contact angle
theta0 90;
}
oil
{
// Dynamic contact angle
theta0 90;
uTheta 1;
thetaA 125;
thetaR 85;
}
}
value uniform 0;
}
}
All solvers now share the same implementation of the alphaContactAngle
boundary condition and the contact angle correction algorithm.
If alpha contact angle boundary conditions are used they must be
specified for all phases or an error will result. The consistency of the
input will also be checked. The angles given for water in the alpha.air
file must be 180 degrees minus the angles given for air in the
alpha.water file.
to provide a single consistent code and user interface to the specification of
physical properties in both single-phase and multi-phase solvers. This redesign
simplifies usage and reduces code duplication in run-time selectable solver
options such as 'functionObjects' and 'fvModels'.
* physicalProperties
Single abstract base-class for all fluid and solid physical property classes.
Physical properties for a single fluid or solid within a region are now read
from the 'constant/<region>/physicalProperties' dictionary.
Physical properties for a phase fluid or solid within a region are now read
from the 'constant/<region>/physicalProperties.<phase>' dictionary.
This replaces the previous inconsistent naming convention of
'transportProperties' for incompressible solvers and
'thermophysicalProperties' for compressible solvers.
Backward-compatibility is provided by the solvers reading
'thermophysicalProperties' or 'transportProperties' if the
'physicalProperties' dictionary does not exist.
* phaseProperties
All multi-phase solvers (VoF and Euler-Euler) now read the list of phases and
interfacial models and coefficients from the
'constant/<region>/phaseProperties' dictionary.
Backward-compatibility is provided by the solvers reading
'thermophysicalProperties' or 'transportProperties' if the 'phaseProperties'
dictionary does not exist. For incompressible VoF solvers the
'transportProperties' is automatically upgraded to 'phaseProperties' and the
two 'physicalProperties.<phase>' dictionary for the phase properties.
* viscosity
Abstract base-class (interface) for all fluids.
Having a single interface for the viscosity of all types of fluids facilitated
a substantial simplification of the 'momentumTransport' library, avoiding the
need for a layer of templating and providing total consistency between
incompressible/compressible and single-phase/multi-phase laminar, RAS and LES
momentum transport models. This allows the generalised Newtonian viscosity
models to be used in the same form within laminar as well as RAS and LES
momentum transport closures in any solver. Strain-rate dependent viscosity
modelling is particularly useful with low-Reynolds number turbulence closures
for non-Newtonian fluids where the effect of bulk shear near the walls on the
viscosity is a dominant effect. Within this framework it would also be
possible to implement generalised Newtonian models dependent on turbulent as
well as mean strain-rate if suitable model formulations are available.
* visosityModel
Run-time selectable Newtonian viscosity model for incompressible fluids
providing the 'viscosity' interface for 'momentumTransport' models.
Currently a 'constant' Newtonian viscosity model is provided but the structure
supports more complex functions of time, space and fields registered to the
region database.
Strain-rate dependent non-Newtonian viscosity models have been removed from
this level and handled in a more general way within the 'momentumTransport'
library, see section 'viscosity' above.
The 'constant' viscosity model is selected in the 'physicalProperties'
dictionary by
viscosityModel constant;
which is equivalent to the previous entry in the 'transportProperties'
dictionary
transportModel Newtonian;
but backward-compatibility is provided for both the keyword and model
type.
* thermophysicalModels
To avoid propagating the unnecessary constructors from 'dictionary' into the
new 'physicalProperties' abstract base-class this entire structure has been
removed from the 'thermophysicalModels' library. The only use for this
constructor was in 'thermalBaffle' which now reads the 'physicalProperties'
dictionary from the baffle region directory which is far simpler and more
consistent and significantly reduces the amount of constructor code in the
'thermophysicalModels' library.
* compressibleInterFoam
The creation of the 'viscosity' interface for the 'momentumTransport' models
allows the complex 'twoPhaseMixtureThermo' derived from 'rhoThermo' to be
replaced with the much simpler 'compressibleTwoPhaseMixture' derived from the
'viscosity' interface, avoiding the myriad of unused thermodynamic functions
required by 'rhoThermo' to be defined for the mixture.
Same for 'compressibleMultiphaseMixture' in 'compressibleMultiphaseInterFoam'.
This is a significant improvement in code and input consistency, simplifying
maintenance and further development as well as enhancing usability.
Henry G. Weller
CFD Direct Ltd.
When using 'simple' or 'hierarchical' decomposition it is useful to slightly rotate a
coordinate-aligned block-mesh to improve the processor boundaries by avoiding
irregular cell distribution at those boundaries. The degree of slight rotation
is controlled by the 'delta' coefficient and a value of 0.001 is generally
suitable so to avoid unnecessary clutter in 'decomposeParDict' 'delta' now
defaults to this value.
The FOAM file format has not changed from version 2.0 in many years and so there
is no longer a need for the 'version' entry in the FoamFile header to be
required and to reduce unnecessary clutter it is now optional, defaulting to the
current file format 2.0.
