Setting Up the Physics

As the simulation involves moving parts in real time the implicit unsteady solver is selected. The mixture of paint and air is solved as a multiphase flow applying the Volume of Fluid (VOF) model.

In the physics continuum you select the Adaptive Mesh model then activate free surface mesh refinement and overset mesh refinement. Additionally, you create a flat wave from the VOF waves model and use its field functions for initializing the VOF phases.

To select the physics models:

  1. For the physics continuum, Continua > Physics 1, select the following models in order:

    Group Box

    Model

    Space

    Three Dimensional

    Time

    Implicit Unsteady

    Material

    Multiphase

    Multiphase Interaction (Selected automatically)

    Volume of Fluid (VOF)

    Segregated Flow (Selected automatically)

    Gradients (Selected automatically)

    Viscous Regime

    Turbulent

    Reynolds-Averaged Navier-Stokes (Selected automatically)

    K-Epsilon Turbulence

    Realizable K-Epsilon Two-Layer (Selected automatically)

    Wall Distance (Selected automatically)

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

    Optional Models

    Gravity

    Adaptive Mesh

    VOF Waves

    VOF Wave Zone Distance (Selected automatically)
  2. Click Close.
  3. To specify the model driven adaptive mesh criteria:
    1. Right-click the Physics 1 > Models > Adaptive Mesh > Adaptive Mesh Criteria node and select New > Free Surface Mesh Refinement.
    2. Right-click the Adaptive Mesh Criteria node and select New > Overset Mesh Refinement.
    3. Use the default settings for the two refinement criteria.
  4. To add two Eulerian phases:
    1. Right-click the Multiphase > Phases node and select New
    2. Right-click the Phase 1 > Models node and choose Select models....
    3. Select the following models in order:

      Group Box

      Model

      Material

      Liquid

      Equation of State

      Constant Density

    4. Click Close.
    5. Rename Phase 1 to Paint.
    6. Right-click the Multiphase > Phases node and select New
    7. Right-click the Phase 1 > Models node and choose Select models....
    8. Select the following models in order:

      Group Box

      Model

      Material

      Gas

      Equation of State

      Constant Density

    9. Click Close.
    10. Rename the Phase 1 node to Air.
    NoteMaterial properties of H2O are set as default when the liquid material is selected. To simplify the tutorial set-up, the material properties of water are kept. In a realistic paint dipping simulation, the correct material properties of the paint should be applied in the physics continuum.
  5. To create a VOF flat wave:
    1. Right-click the VOF Waves > Waves node and select New > Flat.
    2. Select the Flat Vof Wave 1 node and set the Point On Water Level to [0,0,-1.92]m.
    You obtain the following field functions to use as initialization and boundary condition settings:
    • Vof Wave > Flat Vof Wave 1 > Hydrostatic Pressure of Heavy Fluid of Flat Vof Wave 1
    • Vof Wave > Flat Vof Wave 1 > Volume Fraction of Heavy Fluid of Flat Vof Wave 1
    • Vof Wave > Flat Vof Wave 1 > Volume Fraction of Light Fluid of Flat Vof Wave 1
    • Vof Wave > Flat Vof Wave 1 > Velocity of Flat Vof Wave 1
  6. To set initial conditions, in the Physics 1 continuum, edit the Initial Conditions node and set the following properties:
    Node Property Setting
    Pressure Method Field Function
    Scalar Function Vof Wave > Flat Vof Wave 1 > Hydrostatic Pressure of Heavy Fluid of Flat Vof Wave 1
    Velocity Method Field Function
    Vector Function Vof Wave > Flat Vof Wave 1 > Velocity of Flat Vof Wave 1
    Volume Fraction Method Composite
    Composite > Paint Method Field Function
    Scalar Function Vof Wave > Flat Vof Wave 1 > Volume Fraction of Heavy Fluid of Flat Vof Wave 1
    Composite > Air Method Field Function
    Scalar Function Vof Wave > Flat Vof Wave 1 > Volume Fraction of Light Fluid of Flat Vof Wave 1
    At the start of the simulation, the dipping tank is filled with paint to the depth of 2.08m.


  7. To set the correct volume fraction condition on the pressure outlets:
    1. Expand the Regions > Background > Boundaries node and multi-select the left, right and top nodes.
    2. Right-click one of the nodes and select Edit.
    3. For Physics Values > Volume Fraction, set Value to [0,1].
      NoteThe volume fraction value [0,1] indicates that only air can enter the simulation domain through the pressure outlets in case of backflow.
  8. Save the simulation.