The Discrete Phase Model uses a Lagrangian approach to derive the equations for the underlying physics, which are solved transiently. Transient numerical procedures in the Discrete Phase Model can be applied to resolve steady flow simulations as well as transient flows.
In the Discrete Phase Model Dialog Box you have the option of choosing whether you want to treat the particles in an unsteady or a steady fashion. This option can be chosen independent of the settings for the solver. Thus, you can perform steady-state trajectory simulations even when selecting a transient solver for numerical reasons. You can also specify unsteady particle tracking when solving the steady continuous phase equations. This can be used to improve numerical stability for very large particle source terms or simply for postprocessing purposes. Whenever you enable a breakup or collision model to simulate sprays, the Unsteady Particle Tracking will be switched on automatically.
When Unsteady Particle Tracking is enabled, several new options appear. If steady-state equations are solved for the continuous phase, you simply enter the Particle Time Step Size and the Number of Time Steps, thus tracking particles every time a DPM iteration is conducted. When you increase the Number of Time Steps, the droplets penetrate the domain faster.
When solving unsteady equations for the continuous phase, you must decide whether you want to use Fluid Flow Time Step to inject the particles, or you prefer a Particle Time Step Size independent of the Fluid Flow Time Step. With the latter option, you can use the Discrete Phase Model in combination with changes in the time step for the continuous equations, as it is done when using adaptive flow time stepping.
If you do not use Fluid Flow Time Step, you must decide when to inject the particles for a new time step. You can either Inject Particles at Particle Time Step or at the Fluid Flow Time Step. In any case, the particles will always be tracked in such a way that they coincide with the flow time of the continuous flow solver, as long as the maximum number of time steps used to compute a single trajectory is sufficient (see Tracking Parameters for the Discrete Phase Model for details).
You can use a user-defined function (DEFINE_DPM_TIMESTEP) to change the time step for DPM particle tracking. The time step
can be prescribed for special applications where a certain time step
is needed. For more information about changing the time step size
for DPM particle tracking, see DEFINE_DPM_TIMESTEP in the Fluent Customization Manual.
Important: When the density-based solver is used with the explicit unsteady formulation, the particles are advanced once per time step and are calculated at the start of the time step (before the flow is updated).
Additional inputs are required for each injection in the Set Injection Properties Dialog Box, as detailed in Defining Injection Properties. For Unsteady
Particle Tracking, the injection Start Time and Stop Time must be specified under Point Properties. Injections with start and stop times
set to zero will be injected only at the start of the calculation
(). If the In-Cylinder mesh motion
is enabled, the start and stop times are replaced by Start
Crank Angle and Stop Crank Angle,
respectively. The injection specified in this way will be repeated
at the starting and stopping crank angle if the simulation is run
through more than one cycle. Changing injection settings during a
transient simulation will not affect particles currently released
in the domain. At any point during a simulation, you can clear particles
that are currently in the domain by clicking the button in the Discrete Phase Model Dialog Box.
You can choose the Parcel Release Method to determine how ANSYS Fluent creates parcels. For an overview of the concept of parcels, see Parcels. The methods available are:
injects a single parcel per injection stream per time
step. The number of particles in the parcel, , is determined as
follows:
(23–1) |
| where, | |
|
| |
|
| |
|
| |
|
|
This is the default method.
injects parcels with a user-specified number of particles per parcel. The number of parcels is determined to satisfy the specified mass-flow rate and particle size distribution for the injection.
injects parcels with a user-specified parcel mass. The number of parcels is determined to satisfy the specified mass-flow rate and particle size distribution for the injection.
injects parcels with a user-specified parcel diameter. The number of parcels is determined to satisfy the specified mass-flow rate and particle size distribution for the injection.
Note that for atomizer injections, file injections, or injections that use the DEFINE_DPM_INJECTION_INIT user defined function, the Fluent solver automatically uses the default standard parcel release method. Other parcel release methods are not available.
For cases involving sprays and particle size distributions in general, the recommended setting for Parcel Release Method is constant-number. For DEM simulations, you can use constant-diameter or constant-mass to ensure that the parcel diameter does not exceed the size of the smallest cells in the computational mesh.
Note that a lower value specified for constant-number, constant-mass, or constant-diameter will result in a larger number of parcels injected and a finer discretization of the DPM phase. This may be beneficial for accuracy and stability of the calculation, at the expense of additional computational cost.
The Parcel Release Method is specified in the Parcel tab of the Set Injection Properties dialog box.
You can also choose one of several methods to control when the particles are tracked.
In steady-state simulations, particles are tracked at the user-specified intervals (DPM Iteration Interval). Individual particles are tracked from their injection position until either they escape the domain or certain termination criteria are met. Particle tracking is performed only if the global Number of Iterations is equal to or exceeds DPM Iteration Interval. The particle sources are updated during tracking, and then applied to the gas phase in subsequent flow iterations.
In transient flow simulations, particle tracking always occurs at the beginning of each flow time step, irrespective of DPM Iteration Interval. The particles are advanced in time based on the current continuous-phase solution, and DPM sources are updated. The DPM sources prevail up to the next time the particle tracker is run.
(transient flow) If the DPM Iteration Interval is larger than or equal to Max Iterations/Time Step, then particles are tracked only once per time step. If the DPM Iteration Interval is less than Max Iterations/Time Step, then the particle tracker is run multiple times during the time step. Each time the particle tracker is used, particles are returned to their original state at the beginning of the time step. Then particles are advanced in time based on the current continuous-phase solution, and DPM sources are updated. If Particle Time Step is larger than Fluid Flow Time Step (to allow injection of particles at a different time scale than the fluid), then particles are advanced only for the fluid flow time step.
(transient flow) If you specify a value of zero as the DPM Iteration Interval, the particles are advanced at the end of the time step. Note that if you have previously enabled the resetting of DPM source terms at the beginning of every time step using the TUI command define/models/dpm/interaction/reset-sources-at-timestep?, ANSYS Fluent will disable this option once you set the DPM Iteration Interval to zero, because this feature combination is not advisable.
In cases where Interaction with Continuous Phase is enabled, you must provide a sufficient number of particle source term updates to ensure that particle source terms reach their final values (see Figure 23.36: Effect of Number of Source Term Updates on Source Term Applied to Flow Equations). This can be achieved either by setting the DPM under-relaxation factor to 1 or in other cases by enabling Update DPM Sources Every Flow Iteration. If the latter is disabled and the DPM under-relaxation factor is less than 1, then the value you specify for DPM Iteration Interval must be small compared to Max Iterations/Time Step.
In steady-state discrete phase modeling, particles do not interact with each other and are tracked one at a time in the domain.
If the collision model is used, you will not be able to set the DPM Iteration Interval. Refer to Collision and Droplet Coalescence Model Theory in the Fluent Theory Guide for details about this limitation.
Note: As explained in Setting Initial Conditions for the Discrete Phase, the injection flow rate is defined per unit meter of depth in
2D problems. In such cases, each injected parcel is considered to
be a solid cylinder of diameter and depth 1 meter. The parcel volume is then expressed
as:
However, the particles that are dense-packed in the parcel are assumed to be spheres rather than pucks (ice-hockey). The volume of each particle is the same as in 3D cases:
Consider next the theoretical atomic packing factor of spherical particles
in a cylinder of one meter depth, also expressed as the volume ratio
of all particles to all injected parcels.
In 2D, the particles of diameter are
stacked on top of one another in a cylinder of diameter
and depth 1 meter. The total number of particles that can be stacked
in the cylinder in such a way is
. The total volume occupied by
these particles is
The volume of the surrounding parcel cylinder of depth 1 m is
The atomic packing factor will have a constant value of 2/3 when
expressed as:
In order to use the same parameters (spring constant and coefficient of restitution
) for the DEM spring
dashpot models in both 3D and 2D simulations, parcels of the same
mass must be injected in 3D and 2D.
In 3D, the injected parcel is a sphere with diameter and mass
. The number of spherical particles
in a spherical parcel is calculated by
In 2D, the parcel is a cylinder of 1 m depth. This cylinder
has the same mass as the spherical parcel in 3D (), but its
volume differs and is calculated as:
The number of particles per cylindrical parcel NP and the volume they occupy is the same as in 3D, that is
Since the ratio of these two volumes must be equal to the theoretical
atomic packing factor , we obtain
The parcel diameter in 2D can then be calculated as:
Note that in 2D, the parcel diameter is used as a collision range and it is
different than the parcel diameter
in 3D.
For each parcel release method, the input values for the parcel
mass and parcel diameter ( and
, respectively) are the same in both 3D and 2D, while
the output values for parcel diameters are different:
in 2D simulations and
in 3D simulations.