11.2.2 Setting Up the Sliding Mesh Problem

The steps for setting up a sliding mesh problem are listed below. (Note that this procedure includes only those steps necessary for the sliding mesh model itself; you will need to set up other models, boundary conditions, etc. as usual.)

1.   Enable the appropriate option for modeling transient flow in the General task page. (See Section  26.12 for details about the transient modeling capabilities in ANSYS FLUENT.)

General

2.   Set the cell zone conditions for the sliding action:

Cell Zones Conditions

In the Solid or Fluid dialog box of each moving fluid or solid zone, select Moving Mesh in the Motion Type drop-down list and set the translational and/or rotational velocity. (Note that a solid zone cannot move at a different speed than an adjacent fluid zone.)

Note that simultaneous translation and rotation can be modeled only if the rotation axis and the translation direction are the same (i.e., the origin is fixed).

3.   Set the boundary conditions for the sliding action:

Boundary Conditions

Change the zone type of the interface zones of adjacent cell zones to interface in the Boundary Conditions task page.

By default, the velocity of a wall is set to zero relative to the motion of the adjacent mesh. For walls bounding a moving mesh this results in a "no-slip'' condition in the reference frame of the mesh. Therefore, you need not modify the wall velocity boundary conditions unless the wall is stationary in the absolute frame, and therefore moving in the relative frame. See Section  7.3.14 for details about wall motion.

See Chapter  7 for details about input of cell zone and boundary conditions.

4.   Define the mesh interfaces in the Mesh Interfaces dialog box (Figure  11.2.1).

Mesh Interfaces Create/Edit...

Figure 11.2.1: The Create/Edit Mesh Interfaces Dialog Box

(a)   Enter a name for the interface in the Mesh Interface field.

(b)   Specify the two interface zones that comprise the mesh interface by selecting one or more zones in the Interface Zone 1 list and one or more zones in the Interface Zone 2 list. (The order does not matter.)

(c)   Enable the desired Interface Options, if appropriate. There are two options relevant for sliding meshes:

• Enable Periodic Repeats when each of the two cell zones has a single pair of conformal periodics adjacent to the interface (see Figure  6.4.6). This option is typically used when simulating the interface between a rotor and stator. See Section  6.4 for further details.

  Periodic Repeats is not a valid option when more than one zone is selected in each Interface Zone.

• Enable Coupled Wall if you would like to model a thermally coupled wall between two fluid zones that share a sliding mesh interface.

  Note that the following interfaces are coupled by default: the interface between a solid zone and fluid zone the interface between a solid zone and solid zone Therefore, no action is required in the Mesh Interfaces dialog box to set up such interfaces.

(d)   Click Create to create a new mesh interface.

For all types of interfaces, ANSYS FLUENT will create boundary zones for the interface, which will appear under Boundary Zone 1 and Boundary Zone 2. You can use the Boundary Conditions task page to change them to another zone type (e.g., pressure far-field, symmetry, pressure outlet).

If you have enabled the Coupled Wall option, ANSYS FLUENT will also create wall interface zones, which will appear under Interface Wall Zone 1 and Interface Wall Zone 2.

If you create an incorrect mesh interface, you can select it in the Mesh Interface list and click the Delete button to delete it. (Any boundary zones that were created when the interface was created will also be deleted.)

When you have completed the problem setup, you should save an initial case file so that you can easily return to the original mesh position (i.e., the positions before any sliding occurs). The mesh position is stored in the case file, so case files that you save at different times during the transient calculation will contain meshes at different positions.

For cases with strong impeller-baffle interactions, it is recommended that you switch from an MRF model setup to a sliding mesh setup using the following text command: mesh $\rightarrow$ modify-zones $\rightarrow$ mrf-to-sliding-mesh To successfully switch from an MRF to a sliding mesh, you must provide the ID of the fluid zone. ANSYS FLUENT identifies all the zones belonging to this fluid zone as well as fluid zones shared in the domain. ANSYS FLUENT then splits these zones into walls, after which the walls are slit converted to interfaces. ANSYS FLUENT then changes the cell zone condition of the fluid zone to Moving Mesh in the Fluid dialog box. The sliding mesh solution tends to be more robust than the MRF solution.