This section provides instructions for using the optional discrete phase models available in ANSYS Fluent. All of them can be enabled in the Physical Models tab of the Discrete Phase Model dialog box (Figure 23.2: The Discrete Phase Model Dialog Box and the Physical Models).
Setup → Models → Discrete Phase
Edit...
If you want to include the effect of radiation heat transfer to the particles (Equation 5–34 in the Theory Guide), you must enable the Particle Radiation Interaction option under the Physical Models tab, in the Discrete Phase Model Dialog Box (Figure 23.2: The Discrete Phase Model Dialog Box and the Physical Models). You also must define additional properties for the particle materials (emissivity and scattering factor), as described in Description of the Properties. This option is available only when the P-1 or discrete ordinates radiation model is used.
If you want to include the effect of the thermophoretic force on the particle trajectories (Equation 16–11 in the Theory Guide), enable the Thermophoretic Force option under the Physical Models tab, in the Discrete Phase Model Dialog Box. You also must define the thermophoretic coefficient for the particle material, as described in Description of the Properties.
For sub-micron particles, you can also model the lift due to shear (the Saffman lift force, described in Saffman’s Lift Force in the Theory Guide) in the particle trajectory. To do this, enable the Saffman Lift Force option under the Physical Models tab, in the Discrete Phase Model Dialog Box.
In cases where the density of the fluid approaches or exceeds the density of the particles (for example liquid flow with gaseous bubbles), it is recommended that you include the Virtual Mass and Pressure Gradient forces in the particle force balance. To do this, enable Virtual Mass Force and Pressure Gradient Force under the Physical Models tab in the Discrete Phase Model Dialog Box. See Other Forces in Fluent Theory Guide for information on the Virtual Mass and Pressure Gradient forces.
To monitor particle erosion and accretion rates at wall boundaries:
Enable Erosion/Accretion in the Physical Models tab of the Discrete Phase Model Dialog Box.
Enabling the Erosion/Accretion option will cause the erosion and accretion rates to be calculated at wall boundary faces when particle tracks are updated.
For each wall zone, select erosion models and specify erosion model parameters as described in Setting Particle Erosion and Accretion Parameters.
With this option you can modify the condition for switching
from droplet vaporization (Law 2) to boiling (Law 3). By default ANSYS Fluent will
switch from the vaporization to the boiling law when the particle
temperature has reached the boiling point defined for the droplet
material (Equation 16–120 in the Theory Guide). When the Pressure Dependent Boiling option
is enabled, the switching condition will change to , where
is the saturation vapor
pressure at the droplet temperature and
is the domain pressure. If
while in the boiling law, the model will switch
back to the vaporization law. If this option is enabled it is essential
to enter the appropriate droplet saturation vapor pressure data to
cover the complete pressure/temperature range in your model.
When Pressure Dependent Boiling is enabled, then the Temperature Dependent Latent Heat model automatically applies (see Including the Effect of Droplet Temperature on Latent Heat).
Setting the Pressure Dependent Boiling option has no effect on the multicomponent particles, where switching from the vaporization to the boiling regime is always based on the component saturation vapor pressures (see Multicomponent Particle Definition (Law 7) in the Theory Guide) Finally, selection of the Pressure Dependent Boiling option is not available with the real-gas models, as the pressure dependence always applies. See Using the Cubic Equation of State Models with the Lagrangian Dispersed Phase Models for more information.
For pressures higher than the critical pressure of the droplet material (), a boiling point
, defined as the temperature at the saturation vapor pressure (
), cannot be determined as the vapor pressure curve is defined only up to the critical point. Under supercritical pressure conditions (
), the vaporization models are applicable at droplet temperatures below the critical point (
), and the switching condition from vaporization to boiling is never met. For supercritical pressure conditions, you must enter the droplet saturation vapor pressure data for the complete pressure/temperature range up to the critical point
.
When is enabled, you can use the text user interface command
/define/models/dpm/options/allow-supercritical-pressure-vaporization?
to enforce the switching from vaporization to boiling even if the boiling point is not calculated from the vapor pressure data.
If the pressure in your model is above critical (), you must retain the default setting (
yes) for allow-supercritical-pressure-vaporization?.
For subcritical pressure conditions (), the setting for
allow-supercritical-pressure-vaporization? will have no effect unless the boiling point calculation fails, which usually indicates that either the vapor pressure data do not cover the complete temperature/pressure range for your model, or inaccurate data have been entered. In that case, if allow-supercritical-pressure-vaporization? is set to no, the normal boiling point defined for the droplet material will be imposed as a switching condition from vaporization to boiling.
To include the droplet temperature effects on the latent heat as described in Equation 16–113 in the Theory Guide, enable Temperature Dependent Latent Heat under the Physical Models tab. If you enable this option you must provide accurate temperature-dependent specific heat data for both the droplet and the evaporating species materials.
Particles can damp or produce turbulent eddies [76]. In ANSYS Fluent, the formulation described in [29] and [6] is used to compute turbulence modulation. Damping occurs when the particle diameter is less than one tenth of the turbulent length scale. For larger particle diameters turbulence kinetic energy is produced [37].
If you want to consider these effects in the chosen turbulence model, you can enable this using Two-Way Turbulence Coupling, under the Physical Models tab.
To include the effect of collisions, as described in Collision and Droplet Coalescence Model Theory in the Theory Guide, select Stochastic Collision and Coalescence under Options.
Note: Coalescence will appear under Options after Stochastic Collision has been enabled.
The DEM collision model is suitable for simulating granular matter, where such simulations are characterized by a high volume fraction of particles, and the particle-particle interaction is important. See Modeling Collision Using the DEM Model for details about using this model.
To model droplet breakup in ANSYS Fluent, enable Breakup under Options. By default, this will enable breakup for all suitable injections. You can then specify the breakup models and parameters (or disable breakup) for each individual injection on the Physical Models tab in the Set Injection Properties dialog box as described in Breakup.
When either Breakup is enabled or wall-film is selected for Boundary Cond. Type in the DPM tab of the Wall dialog box, you can collect new generated child droplets and track them within the same time step by enabling Consider Children in the Same Tracking Step. This option provides higher accuracy and can lead to faster convergence within a transient flow time step.
To enable the DEM collision model, select DEM Collision under Options. A detailed description of this model can be found in Discrete Element Method Collision Model in the Theory Guide.
In the Physical Models tab of the Discrete Phase Model dialog box
Specify the settings your model requires under DEM Collision Model.
(Optional) By default, Adaptive Collision Mesh Width is enabled. This adjusts the width of the collision mesh to the largest parcel diameter multiplied by the Edge Scale Factor. If Adaptive Collision Mesh Width is disabled, a fixed Static Collision Mesh Width has to be given in the chosen units of length.
The Maximum Particle Velocity limits the maximum particle velocity to a physically plausible range.
Set up the injection.
Setup → Models → Discrete Phase → Injections
New...
In the Set Injection Properties dialog box, select a name from the DEM Collision Partner drop-down list that will serve as the collision partner. A default name using the particle material will be suggested.
Note: Selecting none from the drop-down list indicates that the particles released from this injection do not participate in the DEM collision computation.
If you want to use the rolling friction collision law (see step 4), under the Physical Models tab, enable Particle Rotation for those injections whose particles take part in collisions with rolling friction.
Set the boundary conditions for the discrete phase as you normally would. If the Boundary Cond. Type is reflect, select a name from the DEM Collision Partner drop-down list to designate the collision partner For example, in Figure 23.4: Wall Boundary Condition for the DEM Model, a wall boundary condition will suggest a wall material name, which will designate the collision partner. The name will have a dem- prefix However, if the DEM Collision Partner is none, the wall will reflect particles like any other DPM particles using the settings for the Discrete Phase Reflection Coefficients in the Normal and Tangent directions. These settings generally apply for particles that are not colliding according to DEM, such as massless particles.
Define the particle interaction between the pairs of the collision partners.
Click the button at the bottom of the Discrete Phase Model dialog box. The DEM Collisions dialog box (Figure 23.5: Collision Dialog Box) will appear where you can manage the collision partners. You can , , , , and collision partners. To define collision laws for a collision partner, select a collision partner from the Collision Partners list and click the button, or simply double-click the collision partner in the list.
In the DEM Collision Settings dialog box (Figure 23.6: DEM Collision Settings Dialog Box), a list of all the possible Collision Pairs will exist.
Select a pair of collision partners from the Collision Pairs list.
For this pair, select the Contact Force Laws that best describe the collision between these two partners.
The Normal contact force laws that exist are:
spring
spring-dashpot
hertzian
hertzian-dashpot
You can also choose to exclude the contact force law by selecting none.
For the Tangential contact force law (if considered), you can select form the following friction collision laws:
friction-dshf
friction-dshf-rolling (an extension of the friction-dshf friction collision law including rolling friction)
Each of the laws is described in the following sections:
Enter the Constants for the chosen Contact Force Laws. Refer to Theory in the Theory Guide for guidance on how to find reasonable values of the force-law constants.
Repeat for all other collision pairs.
Click or to apply these settings.
The choice of collision laws does not depend on the order in the pair of collision partners.
Failing to specify a force law for a collision pair implies that respective particles will not collide.
Rolling friction will only be factored in for a particular DEM particle injection if the Particle Rotation option is selected in the Set Injection Properties dialog box (Physical Properties tab).
Note: For parallel calculations, the DEM collision model can be optimized by enabling the hybrid optimization method for DPM. This method balances the load across machines, and, within each machine, the hybrid parallel DPM method is used to make sure the load is balanced by multi-threading. For more information, see the description of the Hybrid Optimization option in the Weighting tab discussion in Partitioning.
The following limitations currently apply when using the DEM collision model:
Axisymmetric geometry cannot be used.
Dynamic mesh motion cannot be used.
The Eulerian wall film model cannot be used.
Shear stress boundary conditions cannot be used at walls.
Marangoni stress boundary condition cannot be used at walls.
DEM particles do not transfer heat from particle to particle during contact.
To better preserve energy during particle collision, the following settings in the Numerics tab are recommended and will be automatically set when DEM Collisions are enabled.
Disable Accuracy Control to ensure that DEM time stepping remains small.
Disable Automated under Tracking Scheme Selection.
Select implicit from the Tracking Scheme drop-down list.
Refer to Numerics for Tracking of the Particles for more information about the settings in the Numerics tab.