Modeling Mixture Multiphase Flow

The Mixture Multiphase (MMP) model is used if the mixture of phases can be modeled by a single set of weighted physical properties. This model treats mass, momentum, and energy as mixture quantities rather than phase quantities, and is computationally more efficient than models that simulate each phase separately. Simcenter STAR-CCM+ solves transport equations for the mixture as a whole, and not for each phase separately.

The Mixture Multiphase (MMP) model can be used for an arbitrary combination of phases where the phase interactions can be of any kind.

To set up a Mixture Multiphase (MMP) simulation for a physics continuum:

  1. Right-click the Continua > [physics continuum] > Models node and select the following models:

    Group Box

    Model

    Space

    		Select one of :

    • Axisymmetric

    • Three Dimensional (required for Adaptive Mesh)

    • Two Dimensional

    Time

    		Select one of :

    • Steady

    • Implicit Unsteady

    Material

    Multiphase

    Multiphase Interaction (selected automatically)

    Multiphase Model

    Mixture Multiphase (MMP)

    See Mixture Multiphase (MMP) Model Reference

    Gradients (Selected automatically)

    Viscous Regime Select one of :

    • Laminar

    • Turbulent
    Flow
    Optional Models

    Segregated Multiphase Temperature

    If you want to apply automated time-step control, select Adaptive Time-Step and set the Adaptive Time-Step solver properties.

    See Setting Up Adaptive Time-Stepping.

    If you want to refine the mesh locally based on user-defined refinement criteria that query the flow solution as the simulation runs to reduce the computation time, select the Adaptive Mesh model. An example application is modeling the shock wave in a steam turbine rotor.

    Activate the User-Defined Mesh Refinement criteria and specify the appropriate properties.

    See Adaptive Mesh Refinement.

    If you want to model porous media, select Porous Media.

    This model is appropriate when you want to model the physical velocity inside a porous medium instead of the superficial velocity, or when the solid and the fluid inside porous media are not in thermal equilibrium.

    See Porous Media Models.

  2. Define the Eulerian phases and select the appropriate phase models.
    A typical case would have one liquid phase and one vapor phase. If you are modeling interphase reactions each phase should be multi-component.

    • To model evaporation and condensation, set up all of the phases as multi-component phases and activate the Spalding Evaporation/Condensation model in each phase.

      Single-component phases are not supported. However, to model single-component phases, you can use multi-component phases that have only one component.

    • To model particle hydrodynamics and to account for the particle size and its distribution in dispersed multiphase flows, activate Discrete Quadrature S-Gamma.

      Selecting this model automatically restricts the flow regime to dispersed/continuous, where the phase for which you select the model is set as the dispersed phase.

    See Defining Eulerian Phases.

Specify the material properties of each phase.
  1. For each phase, expand the [phase] > Models > [phase material] > Material Properties node, select the individual material property nodes, and modify the property values to suit your requirements.

    You can specify the following phase properties:

Specify the material properties of the mixture.

  1. Expand the Multiphase > Mixture > Material Properties node, select the individual material property nodes, and modify the property values to suit your requirements.

    You can specify the following mixture properties:

    • Dynamic Viscosity
    • Specific Heat (when an energy model is activated)
    • Thermal Conductivity (when an energy model is activated)
  2. Set the initial volume fraction of each phase.
    See Setting Initial Conditions.
  3. If you expect free surface flows with sharp phase interfaces to co-exist with dispersed mixtures between the same pair of phases in your simulation, select the Mixture Multiphase (MMP) node and set Convection to Adaptive Interface Sharpening.

    This method models the interface between phases, when such an interface exists, and handles the volume fraction transport accordingly.

    The Adaptive Interface Sharpening and Large-Scale Interface Detection child nodes are added, where you set the appropriate properties.

    See Adaptive Interface Sharpening (ADIS) Scheme for Volume Fraction and Large Scale Interface Detection.

  4. For compressible MMP simulations (that is, where the Mach number exceeds about 0.3), set Face Density Reconstruction to 2nd-Order.

    This option is computationally more expensive, but offers a higher level of consistency between all transport equations.

    See Mixture Multiphase (MMP) Properties.

  5. (Optional) Set up any porous regions.

    Simcenter STAR-CCM+ provides two approaches to model the effects of the porous medium on the flow. One approach, porous region modelling, introduces source terms into the momentum transport equations to approximate the pressure losses. The other approach, porous media modeling using a solid phase, is more general in that it accounts for the increase in physical velocity when the flow enters the porous medium.

    In both approaches, you specify the porosity of the region, the porous inertial resistance and the porous viscous resistance for each phase, and any volume fraction sources that are required.

    See Porous Regions Workflow and Porous Media Model Workflow.

Define a phase interaction, specify the two interacting phases, and select the appropriate phase interaction models.
  1. Right-click the Multiphase Interaction > Phase Interactions node and select New > [primary phase] > [secondary phase].
    The Phase Interaction 1 node is added under Phase Interactions.
  2. Right-click the [phase interaction] > Models node and click Select Models.
  3. In the model selection dialog, activate the following models in order:

    Group Box

    Model

    Enabled Models

    The appropriate Phase Interaction Topology selection is selected automatically, corresponding to the model that is activated in the physics continuum and the phase pair chosen for the interaction:

    Optional Models
    For an MMP-MMP Phase Interaction, the following phase interaction models are available:
    • Interaction Length Scale

      See Interaction Length Scale Model Reference.

    • Multiphase Material
    • Slip Velocity

      See Slip Velocity Model.

      The Slip Velocity model can be unstable in some situations, especially for a large interaction length scale. Two ways that you can resolve the problem are outlined below.

      • Set the Phase Slip Velocity solver Under-Relaxation Factor.

        Smaller under-relaxation values provide more stability, but also give slower convergence.

      • Set the Phase Slip Velocity solver Body Force Smoothing Iterations.

        Higher values provide a more uniform distribution of specific body forces and therefore more stability, but also decrease the local resolution of body forces.

      See Phase Slip Velocity Solver Properties.

    • If you want to model the rate of bulk boiling or condensation between phases, select Boiling/Condensation.

      See Modeling Boiling.

      If you want to model evaporation or condensation, select Spalding Evaporation/Condensation.

      This model is available for multi-component phases only.

      See Spalding Evaporation/Condensation Model.

    • If you want to account for the effects of breakup and coalescence on the predicted particle size distribution, select S-Gamma Breakup and S-Gamma Coalescence, respectively.

      See Discrete Quadrature S-Gamma Phase Interaction Models Reference.

    • If you want to model surface tension, select Surface Tension Force.

      See Surface Tension Force Model Reference.

    • If you want to model interphase reactions, select Interphase Reaction.

      Both of the phases must be multi-component.

      See Interphase Reaction Model Reference.

    For a Film-MMP Phase Interaction, the following phase interaction model is available: For an MMP-Lagrangian Phase Interaction, the following phase interaction models are available:
    • Resolved Transition—identifies large blobs that moving through an MMP-LSI field with significant momentum and velocity (also known as ballistic blobs) and transitions them to computationally more efficient Lagrangian parcels.

      See Resolved Transition.

    • Subgrid Transition—identifies small Lagrangian parcels (mists) and transitions them to a computationally more efficient MMP mixture.

      See Transitioning Lagrangian Particles to Mixture Multiphase (MMP).

    • Impingement—models the impingement of a Lagrangian phase on to an MMP continuous phase.

      See Modeling Impingement.

An MMP-MMP Phase Interaction allows multiple flow regimes (first dispersed regime, second dispersed regime, intermediate regime) by default. Values such as drag are calculated with a weighted sum of the interaction of each flow topology regime. You specify the blending function that is used in the transition between flow regimes. Alternatively, you can restrict the flow regime to a first dispersed regime only or a second dispersed regime only.

  1. Specify the flow regime:
    Flow Regime Procedure
    Unrestricted

    (multiple flow regimes)
    1. Select the [phase interaction] > Models > MMP-MMP Phase Interaction node and make sure that Flow Regime is set to Unrestricted.
    2. Select the MMP-MMP Phase Interaction > Flow Regime Weight Function node and set Method to one of the following options:
      • Gradient Corrected Standard
      • Standard
      • User Specified

      See Flow Regime Weight Function Properties.
    Restricted

    (first dispersed regime only

    or

    second dispersed regime only )

    		 Select the [phase interaction] > Models > MMP-MMP Phase Interaction node and set Flow Regime to First Dispersed Regime only or Second Dispersed Regime only, respectively.
    See MMP-MMP Phase Interaction Properties.
If any of the selected mass transfer models have multi-component phases, you must map the components in one phase to their corresponding components in the other phase.
  1. Expand the [phase interaction] > Models node and select the mass transfer model node. Click (Custom Editor) for the Connectivity property.
  2. In the Component Mapping - Connectivity dialog, match each pair of components.
  3. Set the appropriate phase interaction model properties.
    See Spalding Evaporation/Condensation Model, Discrete Quadrature S-Gamma Phase Interaction Models, Modeling Boiling.
If you want to simulate effects such as diffusion due to capillary effects or osmotic pressure, specify the appropriate momentum sources for each phase.
  1. Select the Regions > [physics continuum] > Phase Conditions > [phase] > Physics Conditions > Momentum Source Option node and set Momentum Source Option to Specified.

    See Region Settings.

If you want to reduce the run-time of your simulation without affecting quality, you can use Multi-Stepping and/or Adaptive Time-Stepping. By sub-stepping the volume fraction transport equation with a reduced time-step, Multi-Stepping allows you to increase the global time-step to reduce computational costs. Adaptive Time-Stepping allows you to control the time-step based on physics or numerical conditions.

  1. If you want to use multi-stepping to improve the interface resolution without increasing the global time-step:
    1. Select the Solvers > Segregated MMP node and set Solution Strategy to Implicit Multi-Step.

      When this option is selected, the Segregated MMP solver performs multiple steps per time-step.

    2. Select the Implicit Multi-Step node and specify the 隐式多步求解器属性.
  2. If you want to apply automated time-step control, select the Adaptive Time-Step model and set the Adaptive Time-Step solver properties.

    See Setting Up Adaptive Time-Stepping.