Step 3: Defining the Turbomachinery Topology

  You will define the topologies of the flow domain in order to establish a turbomachinery-specific coordinate system. This coordinate system is used in subsequent postprocessing functions. Specifically, you will select the boundary zones that comprise the hub, shroud, inlet, outlet, and periodics. The boundaries may consist of more than one zone. The topologies that you define will be saved to the case file when you save the current model. Thus, if you read the saved case back into ANSYS FLUENT, you do not need to set up the topology again.

For more information on defining turbomachinery topologies, see this section in the separate User's Guide.

Define $\rightarrow$ Turbo Topology...

1.   Specify the surfaces representing the hub.

(a)   Retain the default selection of Hub in the Boundaries group box.

(b)   Select the surface that represent the hub ( rotor-hub) in the Surfaces selection list.

2.   Specify the surfaces representing the casing.

(a)   Select Casing in the Boundaries group box.

(b)   Select rotor-shroud in the Surfaces selection list.

3.   Specify the surfaces representing theta periodic.

  Theta periodic are all rotationally periodic boundary conditions surfaces (periodic boundary condition type) which border the turbo topology on the lateral (pitchwise) boundaries.

(a)   Select Theta Periodic in the Boundaries group box.

(b)   Select rotor-periodic-wall-1 and rotor-periodic-wall-2 in the Surfaces selection list.

4.   Specify the surfaces representing theta min.

(a)   Select Theta Min in the Boundaries group box.

(b)   Select rotor-blade-suction

in the Surfaces selection list.

   Theta Min and Theta Max are all walls which may border the turbo topology on the lateral (pitchwise) boundaries. The "min'' and "max'' are determined by the right hand rule about the axis of rotation. Specifically, using the right hand rule, the min surfaces would have the minimum pitchwise coordinate and the max surfaces would have the maximum pitchwise coordinate.

5.   Specify the surfaces representing theta max.

(a)   Select Theta Max in the Boundaries group box.

(b)   Select rotor-blade-pressure in the Surfaces selection list.

6.   Specify the surface representing the inlet.

(a)   Select Inlet in the Boundaries group box.

(b)   Select rotor-inlet in the Surfaces selection list.

7.   Specify the surface representing the outlet.

(a)   Select Outlet in the Boundaries group box.

(b)   Select rotor-outlet in the Surfaces selection list.

8.   Retain the default name of new-topology-1 for the Turbo Topology Name.

9.   Click Define to set all the turbomachinery boundaries.

  Create a second topology to represent the stator.

10.   Specify the surfaces representing the hub.

(a)   Select Hub in the Boundaries group box.

(b)   Select the surface that represent the hub ( stator-hub) in the Surfaces selection list.

Hint:   Scroll down the Surfaces list to locate the surfaces representing the hub.

11.   Specify the surfaces representing the casing.

(a)   Select Casing in the Boundaries group box.

(b)   Select stator-shroud in the Surfaces selection list.

12.   Specify the surfaces representing theta periodic.

(a)   Select Theta Periodic in the Boundaries group box.

(b)   Select stator-periodic-wall-1 and stator-periodic-wall-2 in the Surfaces selection list.

13.   Specify the surfaces representing theta min.

(a)   Select Theta Min in the Boundaries group box.

(b)   Select stator-blade-suction

in the Surfaces selection list.

14.   Specify the surfaces representing theta max.

(a)   Select Theta Max in the Boundaries group box.

(b)   Select stator-blade-pressure in the Surfaces selection list.

15.   Specify the surface representing the inlet.

(a)   Select Inlet in the Boundaries group box.

(b)   Select stator-inlet in the Surfaces selection list.

16.   Specify the surface representing the outlet.

(a)   Select Outlet in the Boundaries group box.

(b)   Select stator-outlet in the Surfaces selection list.

17.   Retain the default name of new-topology-2 for the Turbo Topology Name.

18.   Click Define to set all the turbomachinery boundaries.

19.   Close the Turbo Topology dialog box.

   ANSYS FLUENT will inform you that the turbomachinery postprocessing functions have been enabled, and the Turbo menu will appear in ANSYS FLUENT menu bar at the top of the console. You can define any number of turbo topologies in the Turbo Topology dialog box. This is especially useful when you have a model comprising multiple blade rows and you need to define more than one blade row simultaneously. Each topology can be assigned a specific name and accessed using the drop-down list in the Turbo Topology dialog box.

For more information on defining turbomachinery topologies, see this section in the separate User's Guide.

Note:   You can display the selected surfaces by clicking the Display button in the Turbo Topology dialog box. This is useful as a graphical check to ensure that all relevant surfaces have been selected.