This makes usage of transformPoints the same as for
surfaceTransformPoints. Transformations are supplied as a string and are
applied in sequence.
Usage
transformPoints "\<transformations\>" [OPTION]
Supported transformations:
- "translate=<translation vector>"
Translational transformation by given vector
- "rotate=(<n1 vector> <n2 vector>)"
Rotational transformation from unit vector n1 to n2
- "Rx=<angle [deg] about x-axis>"
Rotational transformation by given angle about x-axis
- "Ry=<angle [deg] about y-axis>"
Rotational transformation by given angle about y-axis
- "Rz=<angle [deg] about z-axis>"
Rotational transformation by given angle about z-axis
- "Ra=<axis vector> <angle [deg] about axis>"
Rotational transformation by given angle about given axis
- "scale=<x-y-z scaling vector>"
Anisotropic scaling by the given vector in the x, y, z
coordinate directions
Example usage:
transformPoints \
"translate=(-0.05 -0.05 0), \
Rz=45, \
translate=(0.05 0.05 0)"
The MomentumTransportModels library now builds of a standard set of
phase-incompressible and phase-compressible models. This replaces most
solver-specific builds of these models.
This has been made possible by the addition of a new
"dynamicTransportModel" interface, from which all transport classes used
by the momentum transport models now derive. For the purpose of
disambiguation, the old "transportModel" has also been renamed
"kinematicTransportModel".
This change has been made in order to create a consistent definition of
phase-incompressible and phase-compressible MomentumTransportModels,
which can then be looked up by functionObjects, fvModels, and similar.
Some solvers still build specific momentum transport models, but these
are now in addition to the standard set. The solver does not build all
the models it uses.
There are also corresponding centralised builds of phase dependent
ThermophysicalTransportModels.
The new fvModels is a general interface to optional physical models in the
finite volume framework, providing sources to the governing conservation
equations, thus ensuring consistency and conservation. This structure is used
not only for simple sources and forces but also provides a general run-time
selection interface for more complex models such as radiation and film, in the
future this will be extended to Lagrangian, reaction, combustion etc. For such
complex models the 'correct()' function is provided to update the state of these
models at the beginning of the PIMPLE loop.
fvModels are specified in the optional constant/fvModels dictionary and
backward-compatibility with fvOption is provided by reading the
constant/fvOptions or system/fvOptions dictionary if present.
The new fvConstraints is a general interface to optional numerical constraints
applied to the matrices of the governing equations after construction and/or to
the resulting field after solution. This system allows arbitrary changes to
either the matrix or solution to ensure numerical or other constraints and hence
violates consistency with the governing equations and conservation but it often
useful to ensure numerical stability, particularly during the initial start-up
period of a run. Complex manipulations can be achieved with fvConstraints, for
example 'meanVelocityForce' used to maintain a specified mean velocity in a
cyclic channel by manipulating the momentum matrix and the velocity solution.
fvConstraints are specified in the optional system/fvConstraints dictionary and
backward-compatibility with fvOption is provided by reading the
constant/fvOptions or system/fvOptions dictionary if present.
The separation of fvOptions into fvModels and fvConstraints provides a rational
and consistent separation between physical and numerical models which is easier
to understand and reason about, avoids the confusing issue of location of the
controlling dictionary file, improves maintainability and easier to extend to
handle current and future requirements for optional complex physical models and
numerical constraints.
This function gives a value of one during a user-specified duration, and
zero at all other times. It is useful for defining the time range in
which an injection or ignition heat source or similar operates.
Example usage, scaling a value:
<name>
{
type scale;
scale squarePulse;
start 0;
duration 1;
value 100;
}
This function has been utilised in a number of tutorial fvOption
configurations to provide a specific window in which the fvOption is
applied. This was previously achieved by "timeStart" and "duration"
controls hard coded into the fvOptions themselves.
A number of fvOptions that apply to a user-derined field can now
automatically work what primitive type they apply to. These options can
apply to any field type, and in some cases even multiple fields of
differing type. Example usage of the options to which this change
applies are shown below:
codedSource1
{
type codedSource;
name codedSource1;
field h;
...
}
fixedValueConstraint1
{
type fixedValueConstraint;
fieldValues
{
R (1 0 0 1 0 1);
epsilon 150;
}
...
}
phaseLimitStabilization11
{
type phaseLimitStabilization;
field sigma.liquid;
...
}
Previously to apply to a given type, these options had to be selected
with the name of the type prepended to the option name (e.g., "type
symmTensorPhaseLimitStabilization;") and those that operated on multiple
fields were restricted to those fields being of the same type.
A number of other options have had improvements made to their handling
of user specification of fields. Where possible, the option will now
attempt to work out what field the option applies to automatically. The
following options, therefore, no longer require "field" or "fields"
entries:
actuationDiskSource
buoyancyEnergy
buoyancyForce
meanVelocityForce
rotorDiskSource
volumeFractionSource
constantHeatTransfer
function2HeatTransfer
variableHeatTransfer
Non-standard field names can be overridden in the same way as in
boundary conditions; e.g., the velocity name can be overridden with a "U
<UName>;" entry if it does not have the default name, "U". The name of
the energy field is now always determined from the thermodynamics
model and should always be correct. Some options that can be applied to
an individual phase also support a "phase <phaseName>;" entry;
fvOptions field-name handling has been rewritten to increase its
flexibility and to improve warning messages. The flexibility now allows
for options that apply to all fields, or all fields of a given phase,
rather than being limited to a specific list of field names. Messages
warning about options that have not been applied now always print just
once per time-step.
Originally the only supported geometry specification were triangulated surfaces,
hence the name of the directory: constant/triSurface, however now that other
surface specifications are supported and provided it is much more logical that
the directory is named accordingly: constant/geometry. All tutorial and
template cases have been updated.
Note that backward compatibility is provided such that if the constant/geometry
directory does not exist but constant/triSurface does then the geometry files
are read from there.
The phase-change functionality in interPhaseChangeFoam has been generalised and
moved into the run-time selectable twoPhaseChange library included into
interFoam providing optional phase-change. The three cavitation models provided
in interPhaseChangeFoam are now included in the twoPhaseChange library and the
two interPhaseChangeFoam cavitation tutorials updated for interFoam.
interPhaseChangeFoam has been replaced by a user redirection script which prints
the following message:
The interPhaseChangeFoam solver has solver has been replaced by the more general
interFoam solver, which now supports phase-change using the new twoPhaseChange
models library.
To run with with phase-change create a constant/phaseChangeProperties dictionary
containing the phase-change model specification, e.g.
phaseChangeModel SchnerrSauer;
pSat 2300; // Saturation pressure
See the following cases for an example converted from interPhaseChangeFoam:
$FOAM_TUTORIALS/multiphase/interFoam/laminar/cavitatingBullet
$FOAM_TUTORIALS/multiphase/interFoam/RAS/propeller
A volumetric flow rate through a tri-surface can now be obtained using
the volumetricFlowRateTriSurface preconfigured function object, using
the following entry in system/controlDict:
fuctions
{
#includeFunc "volumetricFlowRateTriSurface(name=surface.stl)"
}
Where "surface.stl" is a tri-surface file in the constant/triSurface
directory. An example of this has been added to the
incompressible/pimpleFoam/RAS/impeller tutorial case.
Note that when possible, it is preferable to use the flowRatePatch or
flowRateFaceZone functions, as these make direct use of the flux and
therefore report a value that is exactly that computed by the solver.
volumetricFlowRateTriSurface, by contrast, does interpolation of the
velocity field which introduces error.
In addition, a minor fix has been made to the underlying
surfaceFieldValue function object so that it does not need a zone/set
name when values on a searchable surface are requested.
Description
Transforms the specified velocity field into a
cylindrical polar coordinate system or back to Cartesian.
Example of function object specification to convert the velocity field U
into cylindrical polar coordinates before averaging and returning the
average to Cartesian coordinates:
\verbatim
cartesianToCylindrical
{
type cylindrical;
libs ("libfieldFunctionObjects.so");
origin (0 0 0);
axis (0 0 1);
field U;
writeControl outputTime;
writeInterval 1;
}
#includeFunc fieldAverage(cylindrical(U))
cylindricalToCartesian
{
type cylindrical;
libs ("libfieldFunctionObjects.so");
origin (0 0 0);
axis (0 0 1);
field cylindrical(U)Mean;
toCartesian true;
result UMean;
writeControl outputTime;
writeInterval 1;
}
\endverbatim
This is particularly useful for cases with rotating regions, e.g. mixer
vessels with AMI.
See tutorials/incompressible/pimpleFoam/laminar/mixerVesselAMI2D
This tutorial now serves as an example of how to compute flow-rates
through zones defined by triangulated surfaces.
A small fix has also been added to searchableSurfaceToFaceZone to
improve robustness on ambiguous cases.
Most fvOptions change the state of the fields and equations they are applied to
but do not change internal state so it makes more sense that the interface is
const, consistent with MeshObjects. For the few fvOptions which do maintain a
changing state the member data is now mutable.
foamDictionary executions are now wrapped by runApplication like any
other execution so that they do not print during a test loop.
foamDictionary does not produce a conforming log, however, so
log.foamDictionary has been filtered out of the formation of the test
loop report so that false failures are not reported.
providing the shear-stress term in the momentum equation for incompressible and
compressible Newtonian, non-Newtonian and visco-elastic laminar flow as well as
Reynolds averaged and large-eddy simulation of turbulent flow.
The general deviatoric shear-stress term provided by the MomentumTransportModels
library is named divDevTau for compressible flow and divDevSigma (sigma =
tau/rho) for incompressible flow, the spherical part of the shear-stress is
assumed to be either included in the pressure or handled separately. The
corresponding stress function sigma is also provided which in the case of
Reynolds stress closure returns the effective Reynolds stress (including the
laminar contribution) or for other Reynolds averaged or large-eddy turbulence
closures returns the modelled Reynolds stress or sub-grid stress respectively.
For visco-elastic flow the sigma function returns the effective total stress
including the visco-elastic and Newtonian contributions.
For thermal flow the heat-flux generated by thermal diffusion is now handled by
the separate ThermophysicalTransportModels library allowing independent run-time
selection of the heat-flux model.
During the development of the MomentumTransportModels library significant effort
has been put into rationalising the components and supporting libraries,
removing redundant code, updating names to provide a more logical, consistent
and extensible interface and aid further development and maintenance. All
solvers and tutorials have been updated correspondingly and backward
compatibility of the input dictionaries provided.
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.
This significant improvement is flexibility of SemiImplicitSource required a
generalisation of the source specification syntax and all tutorials have been
updated accordingly.
Description
Semi-implicit source, described using an input dictionary. The injection
rate coefficients are specified as pairs of Su-Sp coefficients, i.e.
\f[
S(x) = S_u + S_p x
\f]
where
\vartable
S(x) | net source for field 'x'
S_u | explicit source contribution
S_p | linearised implicit contribution
\endvartable
Example tabulated heat source specification for internal energy:
\verbatim
volumeMode absolute; // specific
sources
{
e
{
explicit table ((0 0) (1.5 $power));
implicit 0;
}
}
\endverbatim
Example coded heat source specification for enthalpy:
\verbatim
volumeMode absolute; // specific
sources
{
h
{
explicit
{
type coded;
name heatInjection;
code
#{
// Power amplitude
const scalar powerAmplitude = 1000;
// x is the current time
return mag(powerAmplitude*sin(x));
#};
}
implicit 0;
}
}
\endverbatim
Rather than specifying the controls per field it is simpler to use a single set
of controls for all the fields in the list and use separate instances of the
fieldAverage functionObject for different control sets:
Example of function object specification setting all the optional parameters:
fieldAverage1
{
type fieldAverage;
libs ("libfieldFunctionObjects.so");
writeControl writeTime;
restartOnRestart false;
restartOnOutput false;
periodicRestart false;
restartPeriod 0.002;
base time;
window 10.0;
windowName w1;
mean yes;
prime2Mean yes;
fields (U p);
}
This allows for a simple specification with the optional prime2Mean entry using
#includeFunc fieldAverage(U, p, prime2Mean = yes)
or if the prime2Mean is not needed just
#includeFunc fieldAverage(U, p)
Description
PTT model for viscoelasticity using the upper-convected time
derivative of the stress tensor with support for multiple modes.
Reference:
\verbatim
Thien, N. P., & Tanner, R. I. (1977).
A new constitutive equation derived from network theory.
Journal of Non-Newtonian Fluid Mechanics, 2(4), 353-365.
\endverbatim
Currently the common exponential form of the PTT model is provided but it could
easily be extended to also support the linear and quadratic forms if the need
arises.
By specifying a list of coefficients in turbulenceProperties, e.g. for the
generalised Maxwell model:
modes
(
{
lambda 0.01;
}
{
lambda 0.04;
}
);
of for the generalised Giesekus model:
modes
(
{
lambda 0.01;
alphaG 0.05;
}
{
lambda 0.04;
alphaG 0.2;
}
);
Visco-elasticity stress tensors (sigma0, sigma1...) are solved for each mode and
summed to create the effective stress of the complex fluid:
Any number of modes can be specified and if only one mode is required the
'modes' entry is not read and the coefficients are obtained as before.
The mode sigma? fields are read if present otherwise are constructed and
initialised from the sigma field but all of the mode sigma? fields are written
for restart and the sigma field contains the sum.
References:
http://en.wikipedia.org/wiki/Generalized_Maxwell_model
Wiechert, E. (1889). Ueber elastische Nachwirkung.
(Doctoral dissertation, Hartungsche buchdr.).
Wiechert, E. (1893).
Gesetze der elastischen Nachwirkung für constante Temperatur.
Annalen der Physik, 286(11), 546-570.
The mean, prime2Mean and base now have default values:
{
mean on; // (default = on)
prime2Mean on; // (default = off)
base time; // time or iteration (default = time)
window 200; // optional averaging window
windowName w1; // optional window name (default = "")
}
so for the majority of cases for which these defaults are appropriate the
fieldAverage functionObject can now be specified in the functions entry in
controlDict thus:
functions
{
fieldAverage1
{
#includeEtc "caseDicts/postProcessing/fields/fieldAverage.cfg"
fields
(
U.air
U.water
alpha.air
p
);
}
}
also utilising the new fieldAverage.cfg file.
For cases in which these defaults are not appropriate, e.g. the prime2Mean is
also required the optional entries can be specified within sub-dictionaries for
each field, e.g.
fieldAverage1
{
#includeEtc "caseDicts/postProcessing/fields/fieldAverage.cfg"
fields
(
U
{
prime2Mean yes;
}
p
{
prime2Mean yes;
}
);
}
For example in the new tutorial case:
tutorials/incompressible/pimpleFoam/laminar/pitzDailyPulse
a cosine bell velocity pulse is specified at the inlet by directly defining the
code for it:
inlet
{
type uniformFixedValue;
uniformValue coded;
name pulse;
codeInclude
#{
#include "mathematicalConstants.H"
#};
code
#{
return vector
(
0.5*(1 - cos(constant::mathematical::twoPi*min(x/0.3, 1))),
0,
0
);
#};
}
which is then compiled automatically and linked into the running pimpleFoam
dynamically and executed to set the inlet velocity.
e.g. in tutorials/incompressible/pisoFoam/LES/motorBike/motorBike/system/cuttingPlane
surfaceFormat vtk;
writeFormat binary;
fields (p U);
selects writing the VTK surface files in binary format which significantly
speeds-up reading of the files in paraview.
Currently binary writing is supported in VTK and EnSight formats.
These cases now check for a mesh in geometrically identical cases and
copy rather than re-generate if possible. This reduces the run-time of
the test loop by about 20 minutes.
A surface geometry file should be stored in
$FOAM_TUTORIALS/resources/geometry if it is used in multiple cases,
otherwise it should be stored locally to the case. This change enforces
that across all tutorials.
Rather than defining patches for all external block faces to provide name and
type use the defaultPatch entry to collect undefined faces into a single named
and typed patch, e.g.
defaultPatch
{
name walls;
type wall;
}
Both the functionObject call context (the command line for postProcess, and the
controlDict path for run-time post-precessing) and the configuration file
context where the arguments are substituted are now printed in the error
message, e.g.
postProcess -func 'patchAverage(name=inlet, ields=(p U))'
generates the message
--> FOAM FATAL IO ERROR:
Essential value for keyword 'fields' not set in function entry
patchAverage(name=inlet, ields=(p U))
in command line postProcess -func patchAverage(name=inlet, ields=(p U))
Placeholder value is <field_names>
file: /home/dm2/henry/OpenFOAM/OpenFOAM-dev/etc/caseDicts/postProcessing/surfaceFieldValue/patchAverage from line 13 to line 17.
and with the following in controlDict
functions
{
#includeFunc patchAverage(name=inlet, ields=(p U))
}
generates the message
--> FOAM FATAL IO ERROR:
Essential value for keyword 'fields' not set in function entry
patchAverage(name=inlet, ields=(p U))
in file /home/dm2/henry/OpenFOAM/OpenFOAM-dev/tutorials/incompressible/pimpleFoam/RAS/pitzDaily/system/controlDict at line 55
Placeholder value is <field_names>
file: /home/dm2/henry/OpenFOAM/OpenFOAM-dev/etc/caseDicts/postProcessing/surfaceFieldValue/patchAverage from line 13 to line 17.
The volumeFractionSource represents the effect of a reduction in the
volume of the domain due to the presence of a stationary phase, most
likely a solid porous media. It only represents the dynamic effects
associated with the reduction in volume; it does not does not model
loss, drag or heat transfer. Separate models (e.g., the existing
porosity models) will be necessary to represent these effects. An
example usage, in system/fvOptions, is as follows:
volumeFraction
{
type volumeFractionSource;
phase solid;
phi phi;
rho rho;
U U;
fields (rho U e);
}
The volume fraction will be read from constant/alpha.<phase>, and must
be generated in advance using setFields or a function object. Note that
the names of the flux, density (if compressible) and velocity must all
be specified. Every field for which a transport equation is solved
should also be specified in the "fields" entry.
The solidEquilibriumEnergySource adds the thermal inertia and diffusive
characteristics of a stationary solid phase to the energy equation of
the fluid, assuming that the two phases are in thermal equilibrium. An
example usage is as follows:
solidEqulibriumEnergy
{
type solidEqulibriumEnergySource;
phase solid;
field e;
}
This will read the volume fraction in the same way as the
volumeFractionSource option. In addition, thermal properties of the
solid will be constructed from settings in
system/thermophysicalProperties.<phase>.
Two tutorials have been added, demonstrating use of these options in
both incompressible and compressible simulations. These are
incompressible/pimpleFoam/laminar/blockedChannel and
compressible/rhoPimpleFoam/laminar/blockedChannel.
Implementation of the Giesekus model for visco-elasticity, derived from the new
generalised form of the Maxwell model which now support additional sources.
Giesekus, H., 1982.
A simple constitutive equation for polymer fluids based on the
concept of deformation-dependent tensional mobility.
J. Non-Newton. Fluid. 11, 69–109.
This implementation is instantiated for incompressible, compressible and VoF
two-phase flow.
For most steady cases simpleFoam is likely to converge faster than pimpleFoam
with LTS but this capability may be useful for testing meshes, BCs etc. for more
complex solver for which SIMPLE is not stable and LTS is provided instead.
Now for transient simulations "Final" solver settings are required for ALL
equations providing consistency between the solution of velocity, energy,
composition and radiation properties.
However "Final" relaxation factors are no longer required for fields or
equations and if not present the standard value for the variable will be
applied. Given that relaxation factors other than 1 are rarely required for
transient runs and hence the same for all iterations including the final one
this approach provide simpler input while still providing the flexibility to
specify a different value for the final iteration if required. For steady cases
it is usual to execute just 1 outer iteration per time-step for which the
standard relaxation factors are appropriate, and if more than one iteration is
executed it is common to use the same factors for both. In the unlikely event
of requiring different relaxation factors for the final iteration this is still
possible to specify via the now optional "Final" specification.
