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 further in this section, along with details about the boundary types.
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.
Important: 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 Specifying the Rotation Axis).
To define the turbomachinery topology in ANSYS Fluent, you will use the Turbo Topology Dialog Box (Figure 31.79: The Turbo Topology Dialog Box).
Setting Up Domain → Mesh Models → Turbo Topology...
The procedure for defining topology for your turbomachinery application are as follows:
Select a boundary type under Boundaries (for example, Hub in Figure 31.79: The Turbo Topology Dialog Box). The boundary types are described in detail in Boundary Types.
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, click
and select Surface Type under
Group By, which organizes the surfaces in a tree
view that is grouped by surface type.
Another shortcut is to use the Filter Text entry box to filter the Surfaces list to show only the surfaces that match the pattern you enter. For additional information on using the Filter Text entry box, see Filter Text Entry Boxes.
Repeat the steps 1 and 2 for all the boundary types that are relevant for your model.
Important: 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.
Enter a name in the Turbo Topology Name field or keep the default name.
Click Define to complete the definition of the boundaries.
ANSYS Fluent will inform you that the turbomachinery postprocessing functions have been activated.
Specify a position vector that is defined as . This position vector should be outside the domain,
for example, if your domain lies in the first and second quadrant,
specify negative
-axis as the zero
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 line is
-axis. If this axis passes through
the domain, you should define the zero
line, so as to satisfy
above criteria.
To view a defined topology, select the topology from the Turbo Topology Name drop-down list and click . The defined topology is shown in the active graphics window. This enables you to visually check the boundaries to ensure that you have defined them correctly.
To edit a defined topology, select the topology from the Turbo Topology Name drop-down list, make the appropriate changes and click Modify.
To remove a defined topology, select the topology from the Turbo Topology Name drop-down list and click Delete.
Important: 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.
The boundaries for the turbomachinery topology are as follows (see Figure 31.80: Turbomachinery Boundary Types):
is the wall zone(s) forming the lower boundary of the flow passage (generally toward the axis of rotation of the machine).
is the wall zone(s) forming the upper boundary of the flow passage (away from the axis of rotation of the machine).
is the periodic boundary zone(s) on the circumferential boundaries of the flow passage.
and Theta Max are the wall zones
at the minimum and maximum angular () positions on a circumferential
boundary.
is the inlet zone(s) through which the flow enters the passage.
is the outlet zone(s) through which the flow exits the passage.
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.