Selecting the Physics Models

Physics models define the primary variables of the simulation, including pressure, temperature, velocity, and what mathematical formulation is used to generate the solution.

In this simulation, the flow is turbulent and the problem involves multiphase flow and cavitation. Three fluids (air, water, and water vapor) are required for the analysis. However, since these fluids occupy the same domain, only one continuum and one region are required to set up the simulation. By default, a continuum that is called Physics 1 2D is created when the mesh is converted to two-dimensional.

To select the physics models:

  1. Rename the Physics 1 2D continuum node to Injector.
  2. For the physics continuum, Continua > Injector, select the following models in order:
    Group Box Model
    Enabled Models Two Dimensional (Pre-selected)
    Time Implicit Unsteady
    Material Multiphase

    Multiphase Interaction (selected automatically)

    Multiphase Model Volume of Fluid (VOF)

    Gradients (selected automatically)

    Segregated Flow (selected automatically)

    Viscous Regime Turbulent

    Reynolds-Averaged Navier-Stokes (selected automatically)

    Reynolds-Averaged Turbulence K-Epsilon Turbulence

    Realizable K-Epsilon Two-Layer (selected automatically)

    Wall Distance (selected automatically)

    Two-Layer All y+ Wall Treatment (selected automatically)

  3. Click Close.
  4. To review the models, open the Injector > Models node.


  5. Save the simulation.