During the problem setup or when you are examining your solution, you may want to look at the mesh associated with certain surfaces. You can do the following:
Display the outline of all or part of the domain, as shown in Figure 31.1: Outline Display.
Draw the mesh lines (edges), as shown in Figure 31.2: Mesh Edge Display.
Draw the solid surfaces (filled meshes) for a 3D domain, as shown in Figure 31.3: Mesh Face (Filled Mesh) Display.
Draw the nodes on the domain surfaces, as shown in Figure 31.4: Node Display.
Note: The Post Processing option for mesh
display configuration is recommended when postprocessing your results
in ANSYS Fluent. This option is accessed by clicking
in the objects toolbar or by entering dislay/set/mesh-display-configuration in the console.
For information about displaying the mesh on a surface that sweeps through the domain, see Displaying Results on a Sweep Surface.
You can draw the mesh or outline for all or part of your domain using the Mesh Display Dialog Box (Figure 31.5: The Mesh Display Dialog Box).
Results → Graphics
→ Mesh
Edit...
The basic steps for generating a mesh or outline plot are as follows:
Choose the surfaces for which you want to display the mesh or outline in the Surfaces list.
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.
Depending on what you want to draw, do one or more of the following:
To draw an outline of the selected surfaces (as in Figure 31.1: Outline Display), select Edges under Options and Outline under Edge Type. If you need more detail in the outline display of a complex geometry, see the description of the Feature option, below.
To draw the mesh edges (as in Figure 31.2: Mesh Edge Display), select Edges under Options and All under Edge Type.
To generate a filled-mesh display (as in Figure 31.3: Mesh Face (Filled Mesh) Display), select Faces under Options.
To draw the nodes on the selected surfaces (as in Figure 31.4: Node Display), select Nodes under Options.
Set any of the mesh and outline display options described in the following section.
Click to draw the specified mesh or outline in the active graphics window.
To display filled meshes, with smoothly shaded display, enable lighting and select a lighting interpolation method other than Flat in the Display Options Dialog Box or the Lights Dialog Box.
If you display nodes, and you want to change the symbol representing the nodes, you can change the Point Symbol in the Display Options Dialog Box. See Modifying the Rendering Options for details.
The options mentioned in the procedure in the previous section include modifying the mesh colors, adding the outline of important features to an outline display, drawing partition boundaries, and shrinking the faces and/or cells in the display.
ANSYS Fluent enables you to control the colors that are used to render the meshes for each zone type or surface. This capability can help you to understand mesh plots quickly and easily. To modify the colors, open the Mesh Colors Dialog Box (Figure 31.6: The Mesh Colors Dialog Box) by clicking in the Mesh Display Dialog Box.
You can set colors individually for the meshes displayed on each surface, using the Scene Description Dialog Box.
By default, the Color by Type option is turned on, enabling you to assign colors based on zone type. To change the color used to draw the mesh for a particular zone type, select the zone type in the Types list and then select the new color in the Colors list. You will see the effect of your change when you next display the mesh. Note that the surface type in the Types list applies to all surface meshes (that is, meshes that are drawn for surfaces created using the dialog boxes opened from the button in the Surface group box of the Setting Up Domain ribbon tab) except zone surfaces.
If you prefer to use the colors ANSYS Fluent assigns by zone ID, then you can display the mesh using the Color by ID option.
For closed 3D geometries such as cylinders, the standard outline display often will not show enough detail to accurately depict the shape. This is because for each boundary, only those edges on the “outside” of the geometry (that is, those that are used by only one face on the boundary) are drawn. In Figure 31.7: Standard Outline of Complex Duct, which shows the outline display for a complicated duct geometry, only the inlet and outlet are visible.
You can capture additional features using the Feature option in the Mesh Display Dialog Box. (See Figure 31.8: Feature Outline of Complex Duct.) Enable Feature under Edge Type, and then set the Feature Angle. With the default Feature Angle of 20, if the difference between the normal directions of two adjacent faces is more than 20°, the edge between those faces will be drawn. Decreasing the Feature Angle will result in more edge lines (that is, more detail) being added to the outline display. The appropriate angle for your geometry will depend on its curvature and complexity. You can modify the Feature Angle until you find the value that yields the best outline display.
If you have partitioned your mesh for parallel processing, you can add the display of partition boundaries to the mesh display by turning on the Partitions option in the Mesh Display Dialog Box.
To distinguish individual faces or cells in the display, enlarge the space between adjacent faces or cells by increasing the Shrink Factor in the Mesh Display Dialog Box. The default value of zero produces a display in which the edges of adjacent faces or cells overlap. A value of 1 creates the opposite extreme: each face or cell is represented by a point and there is considerable space between each one. A small value such as 0.01 may be large enough to enable you to distinguish one face or cell from its neighbor. Displays with different Shrink Factor values are shown in Figure 31.9: Mesh Display with Shrink Factor = 0 and Figure 31.10: Mesh Display with Shrink Factor = 0.01. Click to see the effect of the change in Shrink Factor.
You can create named mesh plot definitions and save them for later use. See Creating and Using Contour Plot Definitions for additional information on graphics object definitions.
The steps for creating and using mesh plot definitions are similar to the steps for Generating Mesh or Outline Plots, with the addition of a field for naming the mesh plot definition.