Modeling Two-Phase Thermodynamic Equilibrium Flow

The Two-phase Thermodynamic Equilibrium model is a multiphase mixture approach that is restricted to modeling two phases. The two phases—liquid and vapour—must be of the same substance and single-component, for example, water and steam. The two phases are assumed to be in thermodynamic equilibrium.

When planning the simulation domain, set the inflow boundary in a location where a pure phase enters the domain—not in a location where phase transfer occurs.

To set up a Two-Phase Thermodynamic Equilibrium 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

    		Implicit Unsteady

    Material

    Multiphase

    Multiphase Interaction
    Multiphase Model
    • Two-Phase Thermodynamic Equilibrium
    Viscous Regime Select one of:

    • Laminar

    • Turbulent
    Flow Select one of:
    • Segregated Flow

    • Coupled Flow
    Energy Two-Phase Thermodynamic Equilibrium requires an energy solver.
    • If you have selected the Segregated Flow solver, Segregated Fluid Enthalpy is automatically activated.
    • If you have selected the Coupled Flow solver, Coupled Energy is automatically activated.
    Optional Models

    If you want to model wall boiling, select Gravity.

    The Wall Boiling model becomes available in the phase interaction.

    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.

  2. Create two Eulerian phases, typically one gas phase and one liquid phase. For each phase:
    1. Right-click the Multiphase > Eulerian Phases node and select New.
    2. Right-click [phase] > Models and click Select Models.
    3. In the Phase Model Selection dialog, select the following models:

      Group Box

      Model

      Material Select one of the following:
      • Gas
      • Liquid
      Equation of State

      Any

      See General Equation of State Models.

      Energy

      		Depending on the chosen solver, select one of the following:
      • Segregated Fluid Enthalpy
      • Coupled Energy
      Optional Models Wall Distance

      See Wall Distance.

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.

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
    • Thermal Conductivity
    • Turbulent Prandtl Number
  2. Set the initial volume fraction of each phase.
    See Setting Initial Conditions.
  3. (Optional) Set up any porous regions.

    Simcenter STAR-CCM+ provides the porous region modelling with Two-Phase Thermodynamic Equilibrium, which introduces source terms into the momentum transport equations to approximate the pressure losses. 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.

Define the phase interactions between 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 Two-Phase Equilibrium Interaction

    Optional Models

    The following phase interaction models are available:

    • If you want to obtain a better estimate of the distribution of void fraction and mixture density than the default Two-Phase Thermodynamic Equilibrium multiphase mixture model, select Algebraic Slip.

      This option is available for segregated flow only.

    • If you want to account for the kinematic effects of relative motion between the phases, select Drift Flux.

      This option is available for both coupled flow and segregated flow.

    • If you want to model boiling, select Wall Boiling.

      This model is available when the Gravity model is activated in the physics continuum.

      When the Wall Boiling model is activated, the Rohsenow Boiling and Transition Boiling models become available for selection in the Wall Boiling Models group box.

  4. Set the appropriate phase interaction model properties.
    See Rohsenow Boiling Model Properties, and Transition Boiling Model Properties.
  5. Set up any monitors, plots, and scenes that you require.
  6. Run the simulation.