Setting Up a Film Casting Simulation

Film casting is modeled as a free-surface flow with a two-dimensional mesh, for a thin film of one or more layers of viscoelastic fluids extruded into free space.

The figure below shows a typical case. The film flows into the simulated area at the top and out at the bottom. The edge is a free surface. Only half of the film between the die and the roller needs to be simulated, through the use of a symmetry plane running down the middle.

The thickness of the film is negligible, allowing for use of a two-dimensional mesh. The shape of the film is modeled, but the shapes of the die and roller are not included in the simulation.



To set up a film-casting simulation.

  1. Create a two-dimensional mesh of the film, with edges designated as inlet, outflow and walls or symmetry planes. Use relatively small cells where velocity gradients will be steep, such as the free surface and the outflow. The following figure shows the film before deformation.


  2. In the physics continuum, select the following models:
    Group Box Model
    Time Steady or Implicit Unsteady
    Flow Viscous Flow
    Optional Models Two Dimensional
    Polymer Displacement Free Surface
    Optional Models Film Casting
  3. Edit the Models > Free Surface node and set the Free Surface Properties to specify the direction of flow.
  4. If the film consists of multiple layers, create a Layer node for each layer:
    1. Right-click Film Casting > Extra Layers and select New.
      This creates a Layer n node with Material Properties sub-nodes.
    2. Expand the Layer n > Material Properties node and set the material properties for the layer.
  5. Edit the Regions > [viscous film region] > Boundaries > [inlet boundary] node and set Type to Velocity Inlet.
  6. Edit the Regions > [viscous film region] > Boundaries > [free surface boundary] node and set Type to Free Surface.
  7. Edit the other nodes under Regions > [viscous film region] > Boundaries node and set Type for each to Free Stream or Symmetry Plane. The boundary for the outlet must be Free Stream.
  8. Edit the Boundaries > [inlet boundary] > Physics Values node and set the values for Velocity and Film Thickness. If the film consists of multiple layers, specify the thickness for each layer:
    1. Edit the [inlet boundary] > Physics Values > Film Thickness node and set Method to Constant or (for space- or time-varying film thickness) Composite.
      Selecting Composite creates a Composite node with a ScalarProfile node for each layer in the film, one for the original layer and one for each Layer n node.
    2. Edit each ScalarProfile node and set the Method property for determining the layer thickness.
    See Boundary Settings.
  9. Edit the Boundaries > [outlet boundary] > Physics Condition > Traction node and the value for Method to Traction Velocity or Normal Velocity.
    For Traction Velocity, the velocity component normal to flow is set to zero; for Normal Velocity, the force component normal to flow is set to zero.
    With either method, the Physics Values > Traction Velocity node appears.
  10. Edit the Physics Values > Traction Velocity node and select the value for Method.
  11. Edit the Physics Condition nodes for the free surface and set the following:
    Node Property Setting
    Morpher Specification Specification Displacement
    Morpher Displacement Specification Specification Internal
If the case is non-isothermal, use the following steps:
  1. In the physics continuum, select Viscous Energy from the Optional Models box .
  2. Edit the [inlet boundary] > Physics Values > Static Temperature node and set the Value property.
  3. For the side boundaries, edit the [side boundary] > Physics Conditions > Thermal Specification node and set Condition property. In most cases, since the film thickness is small, use Adiabatic.
  4. Edit the Regions > [viscous film region] > Physics Conditions > Flux Option node and set Option, most commonly to Convection & Radiation.
  5. Edit the Regions > [viscous film region] > Physics Values node and set the values for Ambient Temperature, Heat Flux, Heat Transfer Coefficient, and Surface Emissivity.
  6. Run the simulation.

    The mesh morphs in response to the difference between inflow and outflow velocities:



    The simulation calculates film thickness, temperature, velocity, and stress profiles over the film.