The Interior Wetted Wall, multiphysics coupling boundary feature can only be applied on interior boundaries.

It is similar to The Wetted Wall Coupling Feature available on exterior boundaries of the Laminar Two-Phase Flow, Level Set () and Turbulent Two-Phase Flow, Level Set () multiphysics interfaces, except that it applies on both sides of an interior boundary. It is an exclusive feature which overrides the Interior Wall feature in the Laminar or Turbulent Flow interface as well as the Thin Barrier feature in the Level Set interface. It is available for laminar flow and turbulent flow with wall functions or automatic wall treatment.

The Interior Wetted Wall coupling feature allows discontinuities (velocity, pressure, level set variable, and turbulence variables) across the boundary and can be used to avoid meshing thin structures in contact with the fluid-fluid interface. When this boundary condition is used, the fluid-fluid interface can move along the wall.

For laminar flow, this boundary condition enforces the no-penetration condition u ⋅ nwall = 0 on both sides of the wall, and adds a tangential stress on the form

where Knt = Kn − (Kn ⋅ nwall)nwall, Kn = Knwall, and K is the viscous stress tensor. β is the slip length. For numerical calculations, a suitable choice is β = h, where h is the mesh element size.

For turbulent flow, the wall is modeled using automatic wall treatment or wall functions depending on the Wall Treatment setting in the Turbulence section of the turbulent flow interface settings.

If the surface tension force is included in the momentum equation, the Interior Wetted Wall boundary condition also adds the following boundary force on both sides of the walls to enforce the contact angle:

Note that the contact angle is not enforced on boundaries adjacent to porous domains. For more information, see The Wetted Wall Coupling Feature.

The Label is the default multiphysics coupling feature name.

The default Name (for the first Interior Wetted Wall multiphysics coupling feature in the model) is iww1.

This section controls which individual interfaces are coupled by the current coupling feature. If a physics interface is deleted and then added to the model again, then in order to reestablish the coupling, you need to choose the correct physics interface again from the Fluid flow or Moving interfaces lists.

The Translational velocity setting controls the translational wall velocity, utr. The list is per default set to Automatic from frame. The physics automatically detects if the spatial frame moves. This can for example happen if an ALE interface is present in the model component. If there is no movement utr = 0. If the frame moves, utr becomes equal to the frame movement.

Select Manual from Translational velocity selection list in order to manually prescribe Velocity of moving wall, utr. This can for example be used to model an oscillating wall where the magnitude of the oscillations are very small compared to the rest of the model. Specifying translational velocity manually does not automatically cause the associated wall to move. An additional Moving Mesh interface needs to be added to physically track the wall movement in the spatial reference frame. For 2D axisymmetric components when Swirl flow is selected in the physics interface properties, the φ-component of utr can also be specified.

When using Navier Slip, the Slip Length setting is per default set to Factor of minimum element length. The slip length β is then defined as β = fhhmin, where hmin is the smallest element side (corresponds to the element size in the wall normal direction for boundary layer elements) and fh is a user input. Select User defined from Slip Length selection list in order to manually prescribe β (SI unit: m).

If the fluid physics interface includes porous domains, check Use porous slip wall treatment to use the porous slip wall treatment to provide tangential stresses and the slip velocity on boundaries adjacent to porous domains. If Use porous slip wall treatment is not checked, the condition selected in Wall condition is used for porous boundaries.

Select an option from the Specify contact angle list — Directly (the default) or Through Young’s equation. For Directly enter a Contact angle θw (SI unit: rad). The default is π/2 radians. For Through Young’s equation enter values or expressions for Phase 1-Solid surface energy density γs1 (SI unit: J/m2) and Phase 2-Solid surface energy density γs2 (SI unit: J/m2).