The underlying physics of the Discrete Phase Model is described by ordinary differential equations (ODE) as opposed to the continuous flow which is expressed in the form of partial differential equations (PDE). Therefore, the Discrete Phase Model uses its own numerical mechanisms and discretization schemes, which are completely different from other numerics used in ANSYS Fluent.
The Numerics tab gives you control over the numerical schemes for particle tracking as well as solutions of heat and mass equations (Figure 23.8: The Discrete Phase Model Dialog Box and the Numerics).
To solve equations of motion for the particles, the following numerical schemes are available:
uses an implicit Euler integration of Equation 16–1 in the Theory Guide which is unconditionally stable for all particle relaxation times.
uses a semi-implicit trapezoidal integration.
uses an analytical integration of Equation 16–1 of the Theory Guide where the forces are held constant during the integration.
facilitates a 5th order Runge Kutta scheme derived by Cash and Karp [19].
For additional details, see Solution Strategies for the Discrete Phase.
You can either choose a single tracking scheme, or switch between higher order and lower order tracking schemes using an automated selection based on the accuracy to be achieved and the stability range of each scheme. In addition, you can control how accurately the equations need to be solved.
enables the solution of equations of motion within a specified tolerance. This is done by computing the error of the integration step and reducing the integration step if the error is too large. If the error is within the given tolerance, the integration step will also be increased in the next steps.
is the maximum relative error that has to be achieved by the tracking procedure. Based on the numerical scheme, different methods are used to estimate the relative error. The implemented Runge-Kutta scheme uses an embedded error control mechanism. The error of the other schemes is computed by comparing the result of the integration step with the outcome of a two step procedure with half the step size.
is the maximum number of step size refinements in one single integration step. If this number is exceeded the integration will be conducted with the last refined integration step size.
provides a mechanism to switch in an automated fashion between numerically stable lower order schemes and higher order schemes, which are stable only in a limited range. In situations where the particle is far from hydrodynamic equilibrium, an accurate solution can be achieved very quickly with a higher order scheme, since these schemes need less step refinements for a certain tolerance. When the particle reaches hydrodynamic equilibrium, the higher order schemes become inefficient since their step length is limited to a stable range. In this case, the mechanism switches to a stable lower order scheme and facilitates larger integration steps.
Important: This mechanism is only available when Accuracy Control is enabled.
can be chosen from the group consisting of trapezoidal and runge-kutta scheme.
consists of implicit and the exponential analytic integration scheme.
is selectable only if Automated is switched off. You can choose any of the tracking schemes. You also can combine each of the tracking schemes with Accuracy Control.
When DEM Collisions are enabled, ANSYS Fluent will automatically set Tracking Scheme to implicit and disable Accuracy Control.
The equation for rotating particle motion (Equation 16–214 in the Fluent Theory Guide) is solved using the Euler implicit discretization scheme.
By default, the particle heat and mass equations are solved in a segregated manner using an implicit Euler integration over the time step used for the trajectory calculation If you enable the Coupled Heat-Mass Solution option for the Droplet, Combusting, or Multicomponent particles, ANSYS Fluent will solve the corresponding equations using a coupled ODE solver with error tolerance control. The increased accuracy, however, comes at the expense of increased computational time.
To ensure solution accuracy for the Droplet and Multicomponent particles, ANSYS Fluent will
automatically switch to the coupled algorithm during the integration
time step when the evaporated mass is greater than the limiting mass
change (defined in Equation 23–4), or when the particle temperature
change is greater than the limiting temperature change
(defined in Equation 23–5).
(23–4) |
where is the particle mass (kg) and
is the vaporization limiting factor for the mass.
(23–5) |
where is the particle temperature (K),
is the bulk temperature (K), and
is the vaporization limiting factor for
the temperature.
You will enter the Vaporization Limiting Factors for Mass and Heat
. The defaults 0.3 and 0.1 are recommended.
Particle tracking is related to a coordinate system. With Track in Absolute Frame enabled, you can choose to track the particles in the absolute reference frame. All particle coordinates and velocities are then computed in this frame. The forces due to friction with the continuous phase are transformed to this frame automatically.
In rotating flows it might be appropriate for numerical reasons to track the particles in the relative reference frame. If several reference frames exist in one simulation, then the particle velocities are transformed to each reference frame when they enter the fluid zone associated with this reference frame.
When the impact of particles with walls in multiple rotating reference frames is important, as it is the case with a rotating impeller in a stationary baffled tank, it is necessary to model the flow as a sliding mesh simulation.
In general, the presence of DPM parcels may affect the continuous phase fluid flow meaning that discrete phase source terms and particle data such as fluid drag, temperature, volume fraction, and velocity can be integrated into the flow solver. By default in ANSYS Fluent, the effects of a particular DPM parcel are applied only to the cell containing that parcel. As an alternative, Node Based Averaging is offered which distributes the effects of a DPM parcel among neighboring nodes in the mesh. This allows a reduction of grid dependency of DPM simulations, since each parcel’s effects on the flow solver are distributed more smoothly across neighboring cells.
You can enable Node Based Averaging in the Numerics tab of the Discrete Phase Model dialog box, as shown in Figure 23.8: The Discrete Phase Model Dialog Box and the Numerics.
When enabled, Node Based Averaging is applied to particle velocity, particle temperature, particle volume fraction, and DPM concentration. By default, Average DPM Source Terms is also enabled, which applies node averaging to the source terms as well. When the Dense Discrete Phase Model is being used, the Average DDPM Variables option appears to provide node based averaging for the discrete phase specific variables, such as DDPM particle drag. When Contour Plots for DPM Variables is enabled (Reporting of Discrete Phase Variables), these quantities will also be node averaged.
Average in Each Integration Step should be enabled if you find that the flux report is showing discrepancies for mass flow rates of particles injected into and leaving the domain. This option increases computation time so it is not enabled by default.
Once you have enabled Node Based Averaging, you must also select the Averaging Kernel to accumulate the particle related data on the mesh nodes and to redistribute them back to the finite volume cells. The kernel and related settings are specified in the Kernel Settings section of the Discrete Phase Model dialog box. The following kernels are available:
nodes-per-cell
shortest-distance
inverse-distance
gaussian
If you use
the gaussian kernel, you must also specify the Gaussian Factor, which determines the width of the Gaussian
distribution. The default value is 1.
For details about the averaging and kernel equations, refer to Node Based Averaging in the Theory Guide.
Source terms for discrete phase momentum, energy, and species
can be linearized with respect to the cell variable, :
(23–6) |
This linearization strongly increases numerical stability for steady flows. For transient flows, it typically allows the use of larger time steps and larger under-relaxation factors for the DPM model.
You can enable source term linearization with the Linearize Source Terms option in the Numerics tab of the Discrete Phase Model dialog box.
The source term linearization can be combined with the Average DPM Source Terms (Node Based Averaging of Particle Data) and Update DPM Sources Every Flow Iteration (Options for Interaction with the Continuous Phase) options. However, you should disable Average DPM Source Terms when using linearized DPM source terms for vaporizing particles. Combination of these two features in vaporization cases may lead to numerical instabilities and unphysical results for the gas temperature.
In order to obtain a better representation of an injector, the particles can be staggered spatially and/or temporally. When particles are staggered spatially, ANSYS Fluent randomly samples from the region in which the spray is specified (for example, the sheet thickness in the pressure-swirl atomizer) so that as the calculation progresses, trajectories will originate from the entire region. This allows the entire geometry specified in the atomizer to be sampled while specifying fewer streams in the input dialog box, thus decreasing computational expense.
When spatial staggering is enabled for non-atomizer injections, a stagger radius must be specified to define the region from which particles are released. The stagger radius is specified in the text user interface (TUI), using the command:
/define/models/dpm/options/stagger-radius
You can also enable injection-specific spatial staggering of the particles by selecting the Stagger Positions option and specifying Stagger Radius in the Point Properties tab of the Set Injection Properties dialog box. For more information, see the appropriate sections for injection-specific point properties.
When injecting particles in a transient calculation using relatively large time steps in relation to the spray event, the particles can clump together in discrete bunches. The clumps do not look physically realistic, though ANSYS Fluent calculates the trajectory for each particle as it passes through a cell and the coupling to the gas phase is properly accounted for. To obtain a statistically smoother representation of the spray, the particles can be staggered in time. During the first time step, the particle is tracked for a random percentage of its initial step. This results in a sample of the initial volume swept out by the particle during the first time step and a smoother, more uniform spatial distribution at longer time intervals.
The setup commands for staggering are available in the text user interface (TUI), under
stagger-spatially-atomizer-injections?
stagger-spatially-standard-injections?
stagger-temporally?
staggering-factor
The “staggering factor” is applied to temporal staggering only. It is a constant that multiplies the time step size to give the random sampling interval. The staggering factor controls the percentage of every particle’s initial time step that will be sampled. For example, if the staggering factor is 0.5, then the parcels in the injection will be tracked between half and all of their full initial time step. If the staggering factor is 0.1, then the parcels will be tracked between ninety percent and all of their initial time step. If the staggering factor is set to 0.9, the parcels will be tracked between ten percent and all of their initial time step. This allows you to control the amount of smoothing between injections.
The default values for the options in the TUI are spatial staggering for atomizers (including the solid-cone), no temporal staggering and a temporal staggering factor of 1.0. The temporal staggering factor is inactive until the flag for temporal staggering is enabled.
As the wall film moves and spreads on the wall faces, under-relaxation is applied to the film height computation. The under-relaxation factor can be specified using the following text command:
define/models/dpm/numerics/underrelax-film-height
A lower under-relaxation factor results in a smoother film appearance, especially closer to the film edge. However, it may distort the film shape, especially for cases where high velocity droplets are impinging on the film. The recommended values range between 0.5 (default) and 0.9.