The procedure to incorporate the sliding mesh technique is as follows:
Define a sub-task to model the flow domain that contains the surrounding and sliding domains.
Define the flow and/or thermal boundary conditions.
Select the relevant boundaries of the surrounding domain to impose Source of connected condition.
Source of connected condition
Impose Target of connected condition on relevant boundaries of the sliding domains. In this menu, select the corresponding source boundary to create a pair of connected boundaries.
Target of connected condition
Note: The panel presents numerical parameters used by Ansys Polyflow when connecting the boundaries. You should not revise these numerical values unless you have been requested to do so by the Ansys Polyflow support team. For additional information about the non-conformal method, see Non-Conformal Boundaries.
Define other boundary conditions, Inflow, wall, Cartesian velocity imposed (vx, vy, [vz]), Temperature imposed, Heat Fluxes, symmetry.
Select the Define Sliding meshes menu item.
Define Sliding meshes
Click Creation of a new sliding mesh.
Creation of a new sliding mesh
This creates a new menu, sliding mesh #1. Then Ansys Polydata will present further options in a new menu:
-
Define the moving part domain
Specify the list of subdomains corresponding to the sliding mesh domain.
-
Define the motion
Specify the parameters of the rigid rotation of the sliding mesh. You can specify an initial translation vector and/or an initial rotation to position the sliding mesh domain in the surrounding domain correctly.
Note: Specify the angular velocity in radians per time units, and the initial angle of rotation in radians.
-
Modification of title
You can modify the default name of the sliding mesh.
Select the Define Sliding meshes menu to define another sliding mesh or to delete an existing one.
Click Upper level menu repeatedly to return to the task menu.