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 example, the flow is turbulent. Use the default K-Epsilon Turbulence model, and apply a gravitational force in the -y direction. As the problem also involves multiphase flow, two fluids (air and water) are required for the analysis. However, since these fluids occupy the same domain, only one continuum and one mesh 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 node to Chambers.
  2. For the physics continuum, Continua > Chambers, 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

    Wall Distance (selected automatically)

    Realizable K-Epsilon Two-Layer (selected automatically)

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

    Optional Models

    Gravity

    Segregated Fluid Isothermal

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


  5. Save the simulation.