to provide smoother behavior on start-up when an acceleration impulse is
applied, e.g. if the body is suddenly released. e.g.
dynamicFvMesh dynamicMotionSolverFvMesh;
motionSolverLibs ("librigidBodyMeshMotion.so");
solver rigidBodyMotion;
rigidBodyMotionCoeffs
{
report on;
solver
{
type Newmark;
}
ramp
{
type quadratic;
start 0;
duration 10;
}
.
.
.
will quadratically ramp the forces from 0 to their full values over the first
10s of the run starting from 0. If the 'ramp' entry is omitted no force ramping
is applied.
Description
Ramp function base class for the set of scalar functions starting from 0 and
increasing monotonically to 1 from \c start over the \c duration and
remaining at 1 thereafter.
Usage:
\verbatim
<entryName> <rampFunction>;
<entryName>Coeffs
{
start 10;
duration 20;
}
\endverbatim
or
\verbatim
<entryName>
{
type <rampFunction>;
start 10;
duration 20;
}
\endverbatim
Where:
\table
Property | Description | Required | Default value
start | Start time | no | 0
duration | Duration | yes |
\endtable
The following common ramp functions are provided: linear, quadratic, halfCosine,
quarterCosine and quaterSine, others can easily be added and registered to the run-time
selection system.
e.g.
ramp
{
type quadratic;
start 200;
duration 1.6;
}
but the old format is supported for backward compatibility:
ramp linear;
rampCoeffs
{
start 200;
duration 1.6;
}
Formally this is equivalent to the previous formulation but more convenient to
use given that for compressible flow the mass flux rather than the volume flux
is available.
These legacy boundary conditions are no longer needed and have been superseded
by the more flexible sixDoFRigidBodyMotion and rigidBodyMotion solvers. See tutorials:
incompressible/pimpleDyMFoam/wingMotion/wingMotion2D_pimpleDyMFoam
multiphase/interDyMFoam/RAS/DTCHull
multiphase/interDyMFoam/RAS/floatingObject
Resolves bug-report https://bugs.openfoam.org/view.php?id=2487
Using
decomposePar -copyZero
The mesh is decomposed as usual but the '0' directory is recursively copied to
the 'processor.*' directories rather than decomposing the fields. This is a
convenient option to handle cases where the initial field files are generic and
can be used for serial or parallel running. See for example the
incompressible/simpleFoam/motorBike tutorial case.
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 a1c8cde310
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.
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;
}
}
This allows single, multi-phase and VoF compressible simulations to be performed
with the accurate thermophysical property functions for liquids provided by the
liquidProperty classes. e.g. in the
multiphase/compressibleInterFoam/laminar/depthCharge2D tutorial water can now be
specified by
thermoType
{
type heRhoThermo;
mixture pureMixture;
properties liquid;
energy sensibleInternalEnergy;
}
mixture
{
H2O;
}
as an alternative to the previous less accurate representation defined by
thermoType
{
type heRhoThermo;
mixture pureMixture;
transport const;
thermo hConst;
equationOfState perfectFluid;
specie specie;
energy sensibleInternalEnergy;
}
mixture
{
specie
{
molWeight 18.0;
}
equationOfState
{
R 3000;
rho0 1027;
}
thermodynamics
{
Cp 4195;
Hf 0;
}
transport
{
mu 3.645e-4;
Pr 2.289;
}
}
However the increase in accuracy of the new simpler and more convenient
specification and representation comes at a cost: the NSRDS functions used by
the liquidProperties classes are relatively expensive to evaluate and the
depthCharge2D case takes ~14% longer to run.
Description
Base-class for thermophysical properties of solids, liquids and gases
providing an interface compatible with the templated thermodynamics
packages.
liquidProperties, solidProperties and thermophysicalFunction libraries have been
combined with the new thermophysicalProperties class into a single
thermophysicalProperties library to simplify compilation and linkage of models,
libraries and applications dependent on these classes.
The entries for liquid and solid species can now be simply be the name unless
property coefficients are overridden in which are specified in a dictionary as
before e.g. in the tutorials/lagrangian/coalChemistryFoam/simplifiedSiwek case
the water is simply specified
liquids
{
H2O;
}
and solid ash uses standard coefficients but the coefficients for carbon are
overridden thus
solids
{
C
{
rho 2010;
Cp 710;
kappa 0.04;
Hf 0;
emissivity 1.0;
}
ash;
}
