Modeling Lagrangian Multiphase Flow

To use the Lagrangian Multiphase model, you define the properties of the continuous and dispersed phases, their boundary conditions, their interactions, and their mode of injection.

You can model particles that are distributed and carried freely in the continuous phase by defining a free-stream Lagrangian phase. For droplets that stick to or slide on solid surfaces, that is, they are bound to the wall, you use the Lagrangian wall-bound phase. The wall-bound phase requires you to set up a fluid film phase and a shell region.

To model Lagrangian multiphase flow:

  1. Create a physics continuum that represents the continuous phase.
    1. Right-click the Continua node and select New Physics Continuum.
    2. Right-click the [continuous phase physics continuum] > Models node and select the following models:
      Group Box Model
      Space Any
      Material Any
      Flow Any
      Equation of State Any
      Energy Any
      Time Any
      Viscous Regime Any
      Optional Models Lagrangian Multiphase
      • Fluid Film—if you want to model wall-bound droplets, you are required to set up a fluid film.
      • Multiphase Interaction—select this model if you want to model interactions between Lagrangian phases and other phases such as the continuous phase or the fluid film phase.
  2. Define the Lagrangian phase.
    1. Right-click the [continuous phase physics continuum] > Lagrangian Multiphase > Lagrangian Phases node and select New, then choose one of the following:
      • Free-stream Phase—select this phase type if you want to model particles that are carried freely by the continuous phase. Free-stream particles are injected and tracked in fluid regions.
      • Wall-bound Phase—select this phase type if you want to model single or multi-component droplets that slide on a surface. Wall-bound droplets are injected and tracked in shell regions.
    2. Depending on your choice of Lagrangian phase type, do one of the following:
      Lagrangian Phase Type Steps
      Free-stream Phase
      1. Right-click the Lagrangian Phases > [free-stream phase] node and select the free-stream phase models.
      2. Define boundary conditions for each Lagrangian free-stream phase.

        How particles respond on impact with a solid boundary greatly depends on the properties of the particle. For this reason, each Lagrangian phase contains a Boundary Conditions node that defines the default response at solid boundaries for particles belonging to that phase. Further information on specifying impact behavior is given in Lagrangian Phase Boundary Conditions.

      Wall-bound Phase
      1. Right-click the Lagrangian Phases > [wall-bound phase] node and select the wall-bound phase models.
      2. To define the shell region on the wall boundary where the sliding droplet is to be tracked, right-click the Regions > [region] > Boundaries > [wall boundary] node and select Create Shell Region.
      3. Select the Regions > [shell region] node and set Continuum to [fluid film phase].
      4. Select the [continuous phase physics continuum] > Models > Lagrangian Multiphase > Lagrangian Phases > [Lagrangian wall-bound phase] node and set Regions to [shell region].

        You can associate multiple wall-bound phases with the same shell region. One wall-bound phase can be tracked in multiple shell regions.

      5. Specify the phase-specific wall boundary conditions:
        • For the wall boundaries that a wall-bound droplet crosses, such as wall edges in shell regions, select the [Lagrangian wall-bound phase] > Boundary Conditions > Wall > Physics Conditions > Mode node and set Active Mode to one of the following:
          • Composite
          • Escape
          • Rebound
        • For the wall boundaries that a wall-bound droplet slides on, which are wall boundaries in shell regions except the edges, expand the Wall > Physics Values node and specify the Contact Angle.

          The contact angle is used by the Spherical Cap model.

        • To configure the adhesion force, select the Physics Values > Contact Angle Hysteresis > Advancing/Receding node and specify Advancing Contact Angle and Receding Contact Angle.

          These contact angle values are used by the Adhesion model.
  3. Define material properties for each Lagrangian phase.
    If a Material Particle model is chosen in the Phase Model Selection dialog, set the material properties, using the corresponding material node in the Lagrangian phase object tree. Further information on the material models available for a Lagrangian phase is given in Modeling Lagrangian Phase Materials.
  4. To define interactions with other multiphase model phase types and model a change of flow regime, or to model the transition of free-stream droplets to wall-bound droplets, right-click the Continua > [physics continuum] > Models > Multiphase Interaction > Phase Interactions node and select New > [phase 1] > [phase 2]. The interactions take place between [phase 1] and [phase 2].
    The following phase interactions are available:
  5. Create and define injectors.
    The locations at which particles enter the fluid continuum, and the manner in which they enter, are defined using injectors. Each injector generates new parcels for a given Lagrangian phase. Any number of injectors can be associated with the same Lagrangian phase.
    For the generation of wall-bound droplets, only four types of injector are available: Part, Point, Surface, and Table. Select the Injectors > [injector] > Conditions > Project to Boundary node and activate Enabled.
    Full information on creating and defining injectors is given in Working with Injectors.
  6. Set parameters for the Lagrangian Multiphase solver.
    The default settings of the solver are a good compromise between accuracy, CPU time, and stability.
    When you are modeling Two-Way Coupling on a fine mesh, set the Volume Source Smoothing Method of the Two-Way Coupling solver to Cell Cluster (or Shell Source Smoothing Method if Lagragrangian particles impinge on a fluid film in a shell region). This ensures that two-way coupling assumptions are valid when particle sizes are comparable to cell sizes.
    Use the Method property of the Cell Cluster > Cluster Length node to control the size of the cell clusters. The cells of the large-scale grid are not always convex, but are approximately cubical in most cases. See Volume and Shell Source Smoothing Methods.
    If the Two-Way Coupling model is active, source terms that the Lagrangian phase models compute are stored for subsequent application in their respective transport equations. If the Two-Way Coupling model is not active, it is possible to freeze the Lagrangian Multiphase Solver until convergence is reached, using its Solver Frozen property. Freezing can save significant CPU time. The Lagrangian Multiphase solution can then be obtained by unfreezing the solver and stepping the solution. Even when the Two-Way Coupling model is active, an economic route to a steady solution can be to update the Lagrangian Multiphase solution less frequently than the other solvers. Use the Update Frequency property of the Lagrangian Steady solver. However, do not use the Solver Frozen feature as your first choice in other situations, since it is primarily a “debugging” tool and not supported for normal simulation work.
    See the section Lagrangian Multiphase Solver Reference for more detail on how accuracy and stability can be increased when necessary.
  7. Prepare for post-processing. Define scenes, reports, monitors, and plots for output such as:
  8. Run the simulation and view the results.