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:
- Rename the Physics 1 2D node to Chambers.
-
For the physics continuum,
, 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
- Click Close.
-
To review the models, open the
node.
- Save the simulation.