This change changes the point-tetIndices-face interpolation function
method to take barycentric-tetIndices-face arguments instead. This
function is, at present, only used for interpolating Eulerian data to
Lagrangian particles.
This change prevents an inefficiency in cellPointInterpolation whereby
the position of the particle is calculated from it's barycentric
coordinates, before immediately being converted back to barycentric
coordinates to perform the interpolation.
Updated the tetrahedron and triangle classes to use the barycentric
primitives. Removed duplicate code for generating random positions in
tets and tris, and fixed bug in tri random position.
"pos" now returns 1 if the argument is greater than 0, otherwise it returns 0.
This is consistent with the common mathematical definition of the "pos" function:
https://en.wikipedia.org/wiki/Sign_(mathematics)
However the previous implementation in which 1 was also returned for a 0
argument is useful in many situations so the "pos0" has been added which returns
1 if the argument is greater or equal to 0. Additionally the "neg0" has been
added which returns 1 if if the argument is less than or equal to 0.
The calculation of the max and min limits are now only performed if required,
i.e. specified in fvSolution.
Also resolves bug-report https://bugs.openfoam.org/view.php?id=2566
This addition allows for theoretical wave models to be utilised for
initialisation and as boundary conditions. Multiple models can be used
simultaneously, each with differing phases and orientations. If multiple
models are used the shapes and velocities are superimposed.
The wave models are specified in the velocity boundary condition. The
phase fraction boundary condition and the set utility both look up the
velocity condition in order to access the wave model. A velocity
boundary may be specified as follows:
inlet
{
type waveVelocity;
origin (0 0 0);
direction (1 0 0);
speed 2;
waves
(
Airy
{
length 300;
amplitude 2.5;
depth 150;
phase 0;
angle 0;
}
);
scale table ((1200 1) (1800 0));
crossScale constant 1;
}
The alpha boundary only requires the type, unless the name of the
velocity field is non-standard, in which case a "U" entry will also be
needed. The setWaves utility does not require a dictionary file; non-
standard field names can be specified as command-line arguments.
Wave models currently available are Airy (1st order) and Stokes2 (second
order). If a depth is specified, and it is not too large, then shallow
terms will be included, otherwise the models assume that the liquid is
deep.
This work was supported by Jan Kaufmann and Jan Oberhagemann at DNV GL.
Now the "localEuler" ddt scheme does not apply any corrections due to
mesh-motion; the old-time volumes are not used and the mesh-motion flux is set
to zero. A consequence of these changes is that boundedness of transported
scalars is ensured but mesh-motion causes a conservation error which will
reduces to zero as steady-state is approached and the mesh becomes stationary.
discontinuous fields, with the discontinuity defined by a level set. The
functions do a proper integration of the discontinuous fields by tet-
and tri-cutting along the plane of the level set.
See tutorials/compressible/rhoPimpleFoam/RAS/squareBendLiq for exapmle
pimpleControl: Added SIMPLErho option for running in SIMPLE mode
with large time-step/Courant number and relaxation. With this option the
density is updated from thermodynamics rather than continuity after the pressure
equation which is better behaved if pressure is relaxed and/or solved to a
loose relative tolerance. The need for this option is demonstrated in the
tutorials/compressible/rhoPimpleFoam/RAS/angledDuct tutorial which is unstable
without the option.
Provides the additional compression necessary to ensure interface integrity
adjacent to a boundary at a low angle of incidence to the interface. This is
particularly important when simulating planing hulls.
except turbulence and lagrangian which will also be updated shortly.
For example in the nonNewtonianIcoFoam offsetCylinder tutorial the viscosity
model coefficients may be specified in the corresponding "<type>Coeffs"
sub-dictionary:
transportModel CrossPowerLaw;
CrossPowerLawCoeffs
{
nu0 [0 2 -1 0 0 0 0] 0.01;
nuInf [0 2 -1 0 0 0 0] 10;
m [0 0 1 0 0 0 0] 0.4;
n [0 0 0 0 0 0 0] 3;
}
BirdCarreauCoeffs
{
nu0 [0 2 -1 0 0 0 0] 1e-06;
nuInf [0 2 -1 0 0 0 0] 1e-06;
k [0 0 1 0 0 0 0] 0;
n [0 0 0 0 0 0 0] 1;
}
which allows a quick change between models, or using the simpler
transportModel CrossPowerLaw;
nu0 [0 2 -1 0 0 0 0] 0.01;
nuInf [0 2 -1 0 0 0 0] 10;
m [0 0 1 0 0 0 0] 0.4;
n [0 0 0 0 0 0 0] 3;
if quick switching between models is not required.
To support this more convenient parameter specification the inconsistent
specification of seedSampleSet in the streamLine and wallBoundedStreamLine
functionObjects had to be corrected from
// Seeding method.
seedSampleSet uniform; //cloud; //triSurfaceMeshPointSet;
uniformCoeffs
{
type uniform;
axis x; //distance;
// Note: tracks slightly offset so as not to be on a face
start (-1.001 -0.05 0.0011);
end (-1.001 -0.05 1.0011);
nPoints 20;
}
to the simpler
// Seeding method.
seedSampleSet
{
type uniform;
axis x; //distance;
// Note: tracks slightly offset so as not to be on a face
start (-1.001 -0.05 0.0011);
end (-1.001 -0.05 1.0011);
nPoints 20;
}
which also support the "<type>Coeffs" form
// Seeding method.
seedSampleSet
{
type uniform;
uniformCoeffs
{
axis x; //distance;
// Note: tracks slightly offset so as not to be on a face
start (-1.001 -0.05 0.0011);
end (-1.001 -0.05 1.0011);
nPoints 20;
}
}
For example the porosity coefficients may now be specified thus:
porosity1
{
type DarcyForchheimer;
cellZone porosity;
d (5e7 -1000 -1000);
f (0 0 0);
coordinateSystem
{
type cartesian;
origin (0 0 0);
coordinateRotation
{
type axesRotation;
e1 (0.70710678 0.70710678 0);
e2 (0 0 1);
}
}
}
rather than
porosity1
{
type DarcyForchheimer;
active yes;
cellZone porosity;
DarcyForchheimerCoeffs
{
d (5e7 -1000 -1000);
f (0 0 0);
coordinateSystem
{
type cartesian;
origin (0 0 0);
coordinateRotation
{
type axesRotation;
e1 (0.70710678 0.70710678 0);
e2 (0 0 1);
}
}
}
}
support for which is maintained for backward compatibility.
For example the actuationDiskSource fvOption may now be specified
disk1
{
type actuationDiskSource;
fields (U);
selectionMode cellSet;
cellSet actuationDisk1;
diskDir (1 0 0); // Orientation of the disk
Cp 0.386;
Ct 0.58;
diskArea 40;
upstreamPoint (581849 4785810 1065);
}
rather than
disk1
{
type actuationDiskSource;
active on;
actuationDiskSourceCoeffs
{
fields (U);
selectionMode cellSet;
cellSet actuationDisk1;
diskDir (1 0 0); // Orientation of the disk
Cp 0.386;
Ct 0.58;
diskArea 40;
upstreamPoint (581849 4785810 1065);
}
}
but this form is supported for backward compatibility.
Off-centering is specified via the mandatory coefficient \c ocCoeff in the
range [0,1] following the scheme name e.g.
\verbatim
ddtSchemes
{
default CrankNicolson 0.9;
}
\endverbatim
or with an optional "ramp" function to transition from the Euler scheme to
Crank-Nicolson over a initial period to avoid start-up problems, e.g.
\verbatim
ddtSchemes
{
default CrankNicolson
ocCoeff
{
type scale;
scale linearRamp;
duration 0.01;
value 0.9;
};
}
\endverbatim
Note this functionality is experimental and the specification and implementation
may change if issues arise.
Both stardard SIMPLE and the SIMPLEC (using the 'consistent' option in
fvSolution) are now supported for both subsonic and transonic flow of all
fluid types.
rhoPimpleFoam now instantiates the lower-level fluidThermo which instantiates
either a psiThermo or rhoThermo according to the 'type' specification in
thermophysicalProperties, see also commit 655fc78748
rhoSimpleFoam now instantiates the lower-level fluidThermo which instantiates
either a psiThermo or rhoThermo according to the 'type' specification in
thermophysicalProperties, e.g.
thermoType
{
type hePsiThermo;
mixture pureMixture;
transport sutherland;
thermo janaf;
equationOfState perfectGas;
specie specie;
energy sensibleInternalEnergy;
}
instantiates a psiThermo for a perfect gas with JANAF thermodynamics, whereas
thermoType
{
type heRhoThermo;
mixture pureMixture;
properties liquid;
energy sensibleInternalEnergy;
}
mixture
{
H2O;
}
instantiates a rhoThermo for water, see new tutorial
compressible/rhoSimpleFoam/squareBendLiq.
In order to support complex equations of state the pressure can no longer be
unlimited and rhoSimpleFoam now limits the pressure rather than the density to
handle start-up more robustly.
For backward compatibility 'rhoMin' and 'rhoMax' can still be used in the SIMPLE
sub-dictionary of fvSolution which are converted into 'pMax' and 'pMin' but it
is better to set either 'pMax' and 'pMin' directly or use the more convenient
'pMinFactor' and 'pMinFactor' from which 'pMax' and 'pMin' are calculated using
the fixed boundary pressure or reference pressure e.g.
SIMPLE
{
nNonOrthogonalCorrectors 0;
pMinFactor 0.1;
pMaxFactor 1.5;
transonic yes;
consistent yes;
residualControl
{
p 1e-3;
U 1e-4;
e 1e-3;
"(k|epsilon|omega)" 1e-3;
}
}
Description
Simple solidification porosity model
This is a simple approximation to solidification where the solid phase
is represented as a porous blockage with the drag-coefficient evaluated from
\f[
S = - \alpha \rho D(T) U
\f]
where
\vartable
\alpha | Optional phase-fraction of solidifying phase
D(T) | User-defined drag-coefficient as function of temperature
\endvartable
Note that the latent heat of solidification is not included and the
temperature is unchanged by the modelled change of phase.
Example of the solidification model specification:
\verbatim
type solidification;
solidificationCoeffs
{
// Solidify between 330K and 330.5K
D table
(
(330.0 10000) // Solid below 330K
(330.5 0) // Liquid above 330.5K
);
// Optional phase-fraction of solidifying phase
alpha alpha.liquid;
// Solidification porosity is isotropic
// use the global coordinate system
coordinateSystem
{
type cartesian;
origin (0 0 0);
coordinateRotation
{
type axesRotation;
e1 (1 0 0);
e2 (0 1 0);
}
}
}
\endverbatim
Description
Simple solidification porosity model
This is a simple approximation to solidification where the solid phase
is represented as a porous blockage with the drag-coefficient evaluated from
\f[
S = - \rho D(T) U
\f]
where
\vartable
D(T) | User-defined drag-coefficient as function of temperature
\endvartable
Note that the latent heat of solidification is not included and the
temperature is unchanged by the modelled change of phase.
Example of the solidification model specification:
\verbatim
type solidification;
solidificationCoeffs
{
// Solidify between 330K and 330.5K
D table
(
(330.0 10000) // Solid below 330K
(330.5 0) // Liquid above 330.5K
);
// Solidification porosity is isotropic
// use the global coordinate system
coordinateSystem
{
type cartesian;
origin (0 0 0);
coordinateRotation
{
type axesRotation;
e1 (1 0 0);
e2 (0 1 0);
}
}
}
\endverbatim
Avoids slight phase-fraction unboundedness at entertainment BCs and improved
robustness.
Additionally the phase-fractions in the multi-phase (rather than two-phase)
solvers are adjusted to avoid the slow growth of inconsistency ("drift") caused
by solving for all of the phase-fractions rather than deriving one from the
others.
e.g. in tutorials/heatTransfer/buoyantSimpleFoam/externalCoupledCavity/0/T
hot
{
type externalCoupledTemperature;
commsDir "${FOAM_CASE}/comms";
file "data";
initByExternal yes;
log true;
value uniform 307.75; // 34.6 degC
}
Previously both 'file' and 'fileName' were used inconsistently in different
classes and given that there is no confusion or ambiguity introduced by using
the simpler 'file' rather than 'fileName' this change simplifies the use and
maintenance of OpenFOAM.
which provided warning about backward-compatibility issue with setting div
schemes for steady-state. It caused confusion by generating incorrect warning
messages for compressible cases for which the 'bounded' should NOT be applied to
the 'div(phid,p)'.
