Free Surface
The Free Surface node is used to define the free surface separating an interior modeled fluid from the outer fluid. The free surface follows the fluid motion, in the normal direction, and is governed by the fluid motion in the free surface domain and the surface tension of the fluid-fluid interface. The Free Surface node can only be applied to outer boundaries of a Deforming Domain that do not have any boundary condition assigned under Moving Mesh.
To control the attachment angle between the free surface and adjacent walls, a Contact Angle node is by default added under the Free Surface node.
The Free Surface feature is supported by laminar flow and by turbulence models using wall functions or automatic wall treatment, but not low-Reynolds number wall treatment. It also requires the study to be time dependent. The node is inactive for Frozen Rotor studies.
Free Surface
Enter an External pressure pext (SI unit: Pa) corresponding to the pressure level in the external fluid phase.
Surface Tension
The Surface tension coefficient σ (SI unit: N/m) can be specified from predefined libraries, by selecting Library coefficient, liquid/gas interface (the default) or Library coefficient, liquid/liquid interface, or set to User defined.
•
For Library coefficient, liquid/gas interface select an option from the list — Water/Air (the default), Acetone/Air, Acetic acid/Air, Ethanol/Air, Ethylene glycol/Ethylene glycol vapor, Diethyl ether/Air, Glycerol/Air, Heptane/Nitrogen, Mercury/Mercury vapor, or Toluene/Air.
•
For Library coefficient, liquid/liquid interface select an option from the list — Benzene/Water, 20°C, Corn oil/Water, 20°C, Ether/Water, 20°C, Hexane/Water, 20°C, Mercury/Water, 20°C, or Olive oil/Water, 20°C.
Dispersed Phase Boundary Condition
Select an option from the Dispersed phase boundary condition list — No dispersed phase flux (the default), Dispersed phase concentration, Dispersed phase outlet, Dispersed phase flux, or Symmetry.
•
For Dispersed phase concentration enter a Dispersed phase volume fraction ϕd0 (dimensionless). The default is 0. When Solve for interfacial area is selected under the Physical Model section, select either the Dispersed phase number density n0 (SI unit: 1/m3) or Diameter of particles/droplets dd (SI unit: m) button and enter a value or expression for n0 (the default is 5·106 1/m3) or dd (the default is 1 mm).
•
For Dispersed phase flux enter values or expression for the Dispersed phase flux Nϕd (SI unit: m/s) and, if Solve for interfacial area is selected under the Physical Model section, the Number density flux Νn (SI unit: 1/(m2⋅s)). The defaults are 0 m/s and 0 1/(m2⋅s), respectively.
Dispersed Phase Boundary Condition Equations in the CFD Module User’s Guide
The Free Surface feature imposes a mesh deformation in the normal direction. On adjacent boundaries, the mesh displacement parallel to those boundaries cannot be fixed if the contact point is moving. In this case a Mesh Slip, Symmetry/Roller, Prescribed Normal Mesh Displacement, or Prescribed Normal Mesh Velocity boundary condition under Moving Mesh should be selected. A Mesh Slip condition is automatically used on the boundaries that are adjacent to the Free Surface and dot not have a prescribed Moving Mesh boundary condition.
If a Free Surface feature is in contact with a solid boundary, the movement of the contact point is not compatible with the no slip condition. For laminar flow the Wall feature with the Navier Slip option should be selected. For turbulence models with wall functions or automatic wall treatment the Wall feature with the No Slip option can be selected.