23.2.2. Steady/Transient Treatment of Particles

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 Clear Particles 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:

standard

injects a single parcel per injection stream per time step. The number of particles in the parcel, , is determined as follows:

(23–1)

where, 
  is the number of particles in a parcel
  is the mass flow rate of the particle stream
  is the time step
  is the particle mass

This is the default method.

constant-number

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.

constant-mass

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.

constant-diameter

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 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.


Important:


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.



Release 18.2 - © ANSYS, Inc. All rights reserved.