29.10.1 Defining the Turbomachinery Topology

In order to establish the turbomachinery-specific coordinate system used in subsequent postprocessing functions, ANSYS FLUENT requires you to define the topology of the flow domain. The procedure for defining the topology is described below, along with details about the boundary types.

Note that the current implementation of the turbomachinery topology definition for postprocessing is no longer limited to one row of blades at a time. If your geometry contains multiple rows of blades, you can define all turbomachinery topologies simultaneously. You can name and/or manage all topologies and perform various turbomachinery postprocessing tasks on a single topology or on all topologies at once.

The turbo coordinates can only be generated properly if the correct rotation axis is specified in the boundary conditions dialog box for the fluid zone (see Section  7.2.1).

To define the turbomachinery topology in ANSYS FLUENT, you will use the Turbo Topology dialog box (Figure  29.10.1).

Define $\rightarrow$ Turbo Topology...

Figure 29.10.1: The Turbo Topology Dialog Box

The steps for defining topology for your turbomachinery application are as follows:

1.   Select a boundary type under Boundaries (e.g., Hub in Figure  29.10.1). The boundary types are described in detail below.

2.   In the Surfaces list, choose the surface(s) that represent the boundary type you selected in step 1.

If you want to select several surfaces of the same type, you can select that type in the Surface Types list instead. All of the surfaces of that type will be selected automatically in the Surfaces list (or deselected, if they are all selected already). Another shortcut is to specify a Surface Name Pattern and click Match to select surfaces with names that match the specified pattern. For example, if you specify wall*, all surfaces whose names begin with wall (e.g., wall-1, wall-top) will be selected automatically. If they are all selected already, they will be deselected. If you specify wall?, all surfaces whose names consist of wall followed by a single character will be selected (or deselected, if they are all selected already).

3.   Repeat the steps above for all the boundary types that are relevant for your model.

For a complete turbo topology definition the surfaces defined as inlet, outlet, hub, casing, periodic, theta min, and theta max (if available) should form a closed domain.

4.   Enter a name in the Turbo Topology Name field or keep the default name.

5.   Click Define to complete the definition of the boundaries.

ANSYS FLUENT will inform you that the turbomachinery postprocessing functions have been activated, and the Turbo menu will appear in ANSYS FLUENT's menu bar at the top of the console window.

6.   Specify a position vector that is defined as $\theta\ = 0$. This position vector should be outside the domain, e.g., if your domain lies in the first and second quadrant, specify negative $y$ axis as the zero $\theta$ line. This will ensure that there is no discontinuity in angular coordinates within the domain. This can be done using the display/set/zero-angle-dir command.

  Default zero $\theta$ line is $+y$ axis. If this axis passes through the domain, you should define the zero $\theta$ line, so as to satisfy above criteria.

7.   To view a defined topology, select the topology from the Turbo Topology Name drop-down list and click Display. The defined topology is shown in the active graphics window. This allows you to visually check the boundaries to ensure that you have defined them correctly.

8.   To edit a defined topology, select the topology from the Turbo Topology Name drop-down list, make the appropriate changes and click Modify.

9.   To remove a defined topology, select the topology from the Turbo Topology Name drop-down list and click Delete.

Note that the topology setup that you define will be saved to the case file when you save the current model. Thus, if you read this case back into ANSYS FLUENT, you do not need to set up the topology again.

However, use of a boundary condition file to set the turbo topology for two similar cases may not work properly. In that case you need to set the turbo topology manually.

Boundary Types

The boundaries for the turbomachinery topology are as follows (see Figure  29.10.2):

Hub   is the wall zone(s) forming the lower boundary of the flow passage (generally toward the axis of rotation of the machine).

Casing   is the wall zone(s) forming the upper boundary of the flow passage (away from the axis of rotation of the machine).

Theta Periodic   is the periodic boundary zone(s) on the circumferential boundaries of the flow passage.

Theta Min   and Theta Max are the wall zones at the minimum and maximum angular ( $\theta$) positions on a circumferential boundary.

Inlet   is the inlet zone(s) through which the flow enters the passage.

Outlet   is the outlet zone(s) through which the flow exits the passage.

Blade   is the wall zone(s) that defines the blade(s) (if any). Note that these zones cannot be attached to the circumferential boundaries. For this situation, use Theta Min and Theta Max to define the blade.

Figure 29.10.2: Turbomachinery Boundary Types