29.10.4 Displaying Turbomachinery 2D Contours

In postprocessing a turbomachinery solution, it is often desirable to display contours on surfaces of constant spanwise coordinate, and then project these contours onto a plane. This permits easier evaluation of the contours, especially for surfaces that are highly three-dimensional.

Steps for Generating Turbo 2D Contour Plots

You can display contours using the Turbo 2D Contours dialog box (Figure  29.10.8).

Turbo $\rightarrow$ 2D Contours...

Figure 29.10.8: The Turbo 2D Contours Dialog Box

The basic steps for generating a turbo 2D contour plot are as follows:

1.   Specify a specific predefined turbomachinery topology using the Turbo Topology drop-down list.

2.   Enter a value for the Normalized Spanwise Coordinates (0 to 1) for the spanwise surface you want to create.

If shroud and hub are the curved surfaces, the iso-surface very close to them may contain void spaces as ANSYS FLUENT displays only a plane cut surface.

3.   Select the variable or function to be displayed in the Contours of drop-down list.

First select the desired category in the upper list; you may then select a related quantity in the lower list. (See Section  29.10.7 for a list of turbomachinery-specific variables, and see Chapter  31 for an explanation of the variables in the list.)

4.   Specify the number of contours in the Levels field. The maximum number of levels allowed is 100.

5.   Click the Display button to draw the specified contours in the active graphics window.

The resulting display will include the specified number of contours of the selected variable, with the magnitude on each one determined by equally incrementing between the values shown in the Min and Max fields.

Contour Plot Options

Depending on the type of contour plot you want to display, select appropriate choice under Options. These options are the same as those in the standard Contours dialog box. See Section  29.1.2 for details about using them.