30.1.1. Zone Surfaces

Zone surfaces are useful for displaying results on boundaries. For example, you may want to plot contours of velocity magnitude at the inlet and outlet of the problem domain, or temperature contours on the domain’s walls. To do so, you need to have a surface that contains the same faces (or cells) as an existing face (or cell) zone. Zone surfaces are created automatically for all boundary face zones in the domain, so you will generally not need to create any zone surfaces unless you accidentally delete one.

Use the text command: surface/reset-zone-surfaces to recreate any missing surface zones by resetting the case surface list.

To create a zone surface, you will use the Zone Surface Dialog Box (Figure 30.1: The Zone Surface Dialog Box).

 Setting Up Domain → Surface → Create → Zone...

Figure 30.1:  The Zone Surface Dialog Box

The Zone Surface Dialog Box

The steps for creating the zone surface are as follows:

  1. Select the zone(s) in the Zone list.

  2. Enter a name in New Surface Name if you do not want ANSYS Fluent to assign a default name to the newly created surface. By default, Fluent assigns each surface the same name as the zone that it corresponds to. If a surface already exists with that name, Fluent assigns the surface a unique name using the zone-surface prefix (for example, zone-surface-6).

    If you do not want to use the default name, enter a new name in New Surface Name. If the New Surface Name that you enter is the same as a surface that already exists, Fluent assigns the new surface a unique name using the zone-surface prefix (for example, zone-surface-7).


    Important:
    • The surface name that you enter must begin with an alphabetical letter. If your surface name begins with any other character or number, Fluent  rejects the entry.

    • If you are selecting multiple zones, you do not have the option to choose the surface names. ANSYS Fluent automatically give the surfaces the same names as their corresponding zone.


  3. Click Create. The new surface name is added to the Surfaces list in the dialog box.

If you want to delete or otherwise manipulate any surfaces, click Manage... to open the Surfaces Dialog Box. For details, see Grouping, Renaming, and Deleting Surfaces.


Release 18.2 - © ANSYS, Inc. All rights reserved.