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.
To see the different behavior of flow through and around the blockage
change D in constant/fvOptions:
// D 100; // Very little blockage
// D 200; // Some blockage but steady flow
// D 500; // Slight waviness in the far wake
D 1000; // Fully shedding behavior
in decomposeParDict.
This default number of processors may be overridden by the new "-np"
option to runParallel which must be specified before the application
name e.g.:
runParallel -np 4 pisoFoam
Adding boundary file from our dev to incompressible/simpleFoam/airFoil2D
Adding missing boundaryRadiationProperties combustion/fireFoam/les/flameSpreadWaterSuppressionPanel
The built-in explicit symplectic integrator has been replaced by a
general framework supporting run-time selectable integrators. Currently
the explicit symplectic, implicit Crank-Nicolson and implicit Newmark
methods are provided, all of which are 2nd-order in time:
Symplectic 2nd-order explicit time-integrator for 6DoF solid-body motion:
Reference:
Dullweber, A., Leimkuhler, B., & McLachlan, R. (1997).
Symplectic splitting methods for rigid body molecular dynamics.
The Journal of chemical physics, 107(15), 5840-5851.
Can only be used for explicit integration of the motion of the body,
i.e. may only be called once per time-step, no outer-correctors may be
applied. For implicit integration with outer-correctors choose either
CrankNicolson or Newmark schemes.
Example specification in dynamicMeshDict:
solver
{
type symplectic;
}
Newmark 2nd-order time-integrator for 6DoF solid-body motion:
Reference:
Newmark, N. M. (1959).
A method of computation for structural dynamics.
Journal of the Engineering Mechanics Division, 85(3), 67-94.
Example specification in dynamicMeshDict:
solver
{
type Newmark;
gamma 0.5; // Velocity integration coefficient
beta 0.25; // Position integration coefficient
}
Crank-Nicolson 2nd-order time-integrator for 6DoF solid-body motion:
The off-centering coefficients for acceleration (velocity integration) and
velocity (position/orientation integration) may be specified but default
values of 0.5 for each are used if they are not specified. With the default
off-centering this scheme is equivalent to the Newmark scheme with default
coefficients.
Example specification in dynamicMeshDict:
solver
{
type CrankNicolson;
aoc 0.5; // Acceleration off-centering coefficient
voc 0.5; // Velocity off-centering coefficient
}
Both the Newmark and Crank-Nicolson are proving more robust and reliable
than the symplectic method for solving complex coupled problems and the
tutorial cases have been updated to utilize this.
In this new framework it would be straight forward to add other methods
should the need arise.
Henry G. Weller
CFD Direct
so that the specification of the name and dimensions are optional in property dictionaries.
Update tutorials so that the name of the dimensionedScalar property is
no longer duplicated but optional dimensions are still provided and are
checked on read.
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.
With the SIMPLE "consistent" option and optimized relaxation factors
this tutorial now converges in 210 iterations, previously with SIMPLE it
took 950. Despite the increase in cost per time-step due to the
increase in relaxation factors and number of solver iterations the
speed-up is 3.5x.
by introducing rational base-classes rather than using the hideous
'switch' statement. Further rationalization of the cell-selection
mechanism will be implemented via an appropriate class hierarchy to
replace the remaining 'switch' statement.
Mesh-motion is currently handled very inefficiently for cellSets and not
at all for inter-region coupling. The former will be improved when the
cell-selection classes are written and the latter by making the
meshToMesh class a MeshObject after it has been corrected for mapFields.
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.
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
Disadvantage is that the BC values have to be specified in terms of hU
rather than U. The alternative would be to add complex code to map h
and U BCs into the equivalent for hU.
Resolves bug-report http://www.openfoam.org/mantisbt/view.php?id=1566
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.
The standard/previous general symmetry type is now named symmetry
both in class and lookup name for consistency. The rigorous
symmetryPlane type is needed for moving-mesh cases in which the
motion it constrained by one or two planes.
