The Set Injection Properties dialog box allows you to define the properties of an existing discrete-phase injection (which was created in the Injections Dialog Box). See Defining Injection Properties for details about the items listed in this section.
The Set Injection Properties dialog box is opened from the Injections Dialog Box.

Controls
sets the name of the injection.
contains a drop-down list of the available injection types: single, group, cone, surface, plain-orifice-atomizer, pressure-swirl-atomizer, air-blast-atomizer, flat-fan-atomizer, effervescent-atomizer, and file. (cone is not available in 2D.) These choices are described in Injection Types.
indicates the number of particle streams in a group, cone, or any of the atomizer injections. (This item will not appear for single, surface, or file injections.)
indicates the surface from which the particles in a surface injection will be released. (This item will appear only for a surface injection.)
specifies the particle type as Massless, Inert, Droplet, Combusting, or Multicomponent. These types are described in Particle Types.
(not for massless particles) contains inputs for customized particle laws.
enables the specification of customized particle laws and opens the Custom Laws Dialog Box.
(not for massless particles) indicates the material for the particles. If this is the first time you have created a particle of this type, you can choose from all of the materials by copying them from the database or creating them from scratch, as discussed in Setting Discrete-Phase Physical Properties and described in detail in Using the Create/Edit Materials Dialog Box.
(not for massless particles) allows you to change from the default linear interpolation method used to determine the size of the particles in a group injection, or the default uniform method used to determine the size of the particles in a surface injection, to the rosin-rammler or rosin-rammler-logarithmic method. The Rosin-Rammler method for determining the range of diameters is described in Using the Rosin-Rammler Diameter Distribution Method.
(for droplet particles) specifies the gas-phase species created by the vaporization and boiling laws (laws 2 and 3).
(for combusting particles) specifies the gas-phase species created by the devolatilization law (law 4).
This item will not appear for two-mixture-fraction non-premixed combustion calculations.
(for combusting particles) specifies the destination stream for the gas-phase species created by the devolatilization law (law 4).
This item will appear only for two-mixture-fraction non-premixed combustion calculations.
(for combusting particles) specifies the gas phase species that participates in the surface char combustion reaction (law 5).
(for combusting particles) specifies the gas-phase species created by the surface char combustion reaction (law 5).
This item will not appear for two-mixture-fraction non-premixed combustion calculations.
(for combusting particles) specifies the destination stream for the gas-phase species created by the surface char combustion reaction (law 5).
This item will appear only for two-mixture-fraction non-premixed combustion calculations.
is available when using the Dense Discrete Phase Model, described in Including the Dense Discrete Phase Model.
is available when using the DEM Collision model, described in Modeling Collision Using the DEM Model.
displays the inputs for the point properties for the injection (for example, position, velocity, diameter, temperature, and mass flow rate). These inputs are described for each injection type in Point Properties for Single Injections – Point Properties for Effervescent Atomizer Injections.
specifies the first point properties for the injection.
specifies the last point properties for the injection.
displays the inputs for injection-specific physics models.
allows the setting of the drag law used in calculating the force balance on the particles. See Particle Force Balance in the Theory Guide for details on the items below.
is a drop-down list containing the available choices for the drag law:
assumes that the particles are smooth spheres.
assumes that the particles are not spheres, but are all identically shaped. The shape is specified by the Shape Factor.
is for use with sub-micron particles. A Cunningham Correction is added to Stokes’ drag law to determine the drag.
is similar to the spherical law with corrections to account for a particle Mach number greater than 0.4 or a particle Reynolds number greater than 20.
is used in gas-liquid flows. This drag law is only available if the magnitude and direction of the gravity vector are specified in the Operating Conditions dialog box. See Ishii-Zuber Drag Model in the Fluent Theory Guide for details.
is used in gas-liquid flows. This drag law is only available if the magnitude and direction of the gravity vector are specified in the Operating Conditions dialog box. See Grace Drag Model in the Fluent Theory Guide for details.
accounts for the effects of droplet distortion. This drag law is available only when one of the droplet breakup models is used in conjunction with unsteady tracking. See Dynamic Drag Model Theory in the Theory Guide for details.
specifies the shape of the particles when nonspherical is selected as the Drag Law ( in Equation 16–75 in the Theory Guide). It is
the ratio of the surface area of a sphere having the same volume as
the particle to the actual surface area of the particle. The shape
factor value cannot be greater than
1.
( in Equation 16–77 in the Theory Guide) is used
with Stokes’ drag law to determine the force acting on the particles
when the particles are sub-micron size. It appears when Stokes-Cunningham is selected as the Drag Law.
contains settings for the modeling of particle rotation when the Enable Rotation check box is selected (see Wall-Particle Reflection Model Theory in the Fluent Theory Guide).
is a drop-down list of available rotational drag law models:
uses Equation 16–4 in the Fluent Theory Guide to calculate the rotational drag
coefficient .
implies zero torque, that is, it excludes the influence of the fluid on the rotational particle motion.
is a drop-down list of available Magnus lift law models:
uses Oesterle and Bui Dinh’s formulation (Equation 16–18 in the Fluent Theory Guide).
is based on the particle spin rate (Equation 16–19 in the Fluent Theory Guide).
uses a linear dependence of the rotational lift coefficient on the spin
rate (Equation 16–21 in the Fluent Theory Guide).
implies that the Magnus lift will not be included in your simulation.
enables the incorporation of the effects of Brownian motion. This option is available only when the Stokes-Cunningham drag law is selected from the Drag Law drop-down list. See Brownian Force in the Theory Guide for details.
contains parameters that control droplet breakup and collision. (This section of the dialog box appears only if Unsteady Tracking is enabled in the Discrete Phase Model Dialog Box.)
enables breakup for this injection.
is a drop-down list containing parameters that control droplet breakup. (This item appears only if Enable Breakup is selected.)
enables the Taylor Analogy Breakup (TAB) model, which is applicable to many engineering sprays. This method is based upon Taylor’s analogy between an oscillating and distorting droplet and a spring mass system. See Taylor Analogy Breakup (TAB) Model in the Theory Guide for details.
For the TAB model, you must specify the following constants:
is the constant in Equation 16–374 in the Theory Guide.
is the number of child parcels the droplet is split into, as described in Velocity of Child Droplets in the Theory Guide.
enables the Wave breakup model, which considers the breakup of the injected liquid to be induced by the relative velocity between the gas and liquid phases. See Wave Breakup Model for details.
For the Wave model, you must specify the following constants:
is the constant in Equation 16–401 in the Theory Guide.
is the constant in Equation 16–403 in the Theory Guide.
enables the Kelvin-Helmholtz Rayleigh-Taylor breakup model, which considers the two competing effects of aerodynamic breakup and instabilities due to droplet acceleration. See KHRT Breakup Model in the Theory Guide for details.
For the KHRT model, you must specify the following constants:
is the constant in Equation 16–401 in the Theory Guide.
is the constant in Equation 16–403 in the Theory Guide.
is the constant in Equation 16–408 in the Theory Guide.
is the constant in Equation 16–409 in the Theory Guide.
is the constant in Equation 16–404 in the Theory Guide.
enables the stochastic secondary droplet breakup model, where the probability of breakup is independent of the parent droplet size and the secondary droplet size is sampled from an analytical solution of the Fokker-Planck equation for the probability distribution. See Stochastic Secondary Droplet (SSD) Model in the Theory Guide for details.
For the SSD model, you must specify the following constants:
is the critical Weber number in Equation 16–410 in the Theory Guide.
is B in Equation 16–411 in the Theory Guide.
is the average number in parcels for daughter parcels.
is in Equation 16–412 in the Theory Guide.
displays the inputs for stochastic tracking and cloud tracking.
controls the stochastic tracking for turbulent flows. Stochastic tracking includes the effect of turbulent velocity fluctuations on the particle trajectories using the DRW model described in Stochastic Tracking in the Theory Guide. See Stochastic Tracking for details about the items below.
includes the effect of instantaneous turbulent velocity formulations on the particle trajectories through stochastic method.
specifies that the characteristic lifetime of the eddy is to be random.
controls the inclusion of turbulent velocity fluctuations.
An input of 1 or greater tells ANSYS Fluent to include turbulent velocity fluctuations in the particle force balance.
is in Equation 16–24 in the Theory Guide. The default
is 0.15; if you use the RSM, a value of 0.3 is recommended.
incorporates the effects of turbulent dispersion on the injection. For details on the following items, see Particle Cloud Tracking in the Theory Guide and Cloud Tracking.
enables particle cloud tracking.
specifies the diameter of the cloud in which the particles enter the domain.
specifies the maximum allowed cloud diameter.
displays the inputs for controlling the discrete phase parcels.
contains settings for how parcels are defined
specifies the method for releasing parcels. Available settings are standard, constant-number, constant-mass, and constant-diameter. See Steady/Transient Treatment of Particles for details about these settings.
displays the inputs for the wet combustion model.
allows the combusting particles to include an evaporating/boiling material.
contains a drop-down list of liquid materials that can be chosen as the evaporating/boiling material to be included with the combusting particles.
sets the volume fraction of the liquid present in the particle.
displays the inputs for Multicomponent for use in the definition of the particle injection. For details on the following items, see Vapor Liquid Equilibrium Theory in the Theory Guide.
contains the multicomponent injections.
specifies the component that is a part of the multicomponent species.
specifies the mass fraction of the component in a multicomponent species.
specifies the gas-phase species to be evaporated.
specifies the source stream from which the species will be evaporated.
displays the inputs for User-Defined Functions for use in the definition of the particle injection. For details about user-defined functions, see the separate Fluent Customization Manual.
contains a drop-down list of available user-defined functions. The UDF that you choose will be used to modify the injection properties at the time the particles are injected into the domain.
allows you to select the user-defined function that defines the heat or mass transfer.
displays the inputs for Multiple Surface Reactions. See Particle Surface Reactions for details about this model.
specify the combustible fraction of the combusting particle if you have defined more than one particle surface species. See Using the Multiple Surface Reactions Model for Discrete-Phase Particle Combustion for details.
opens The Select File Dialog Box, in which you can select a file containing the injection definition (when file is selected as the Injection Type).