[ANSYS, Inc. Logo] return to home search
next up previous contents index

29.1.1 Displaying the Mesh

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 display the outline of all or part of the domain, as shown in Figure  29.1.1; draw the mesh lines (edges), as shown in Figure  29.1.2; draw the solid surfaces (filled meshes) for a 3D domain, as shown in Figure  29.1.3; and/or draw the nodes on the domain surfaces, as shown in Figure  29.1.4.

See also Section  29.1.5 for information about displaying the mesh on a surface that sweeps through the domain.

Figure 29.1.1: Outline Display

Figure 29.1.2: Mesh Edge Display

Figure 29.1.3: Mesh Face (Filled Mesh) Display

Figure 29.1.4: Node Display

Steps for Generating Mesh or Outline Plots

You can draw the mesh or outline for all or part of your domain using the Mesh Display dialog box (Figure  29.1.5).

figure General figure Display...

Figure 29.1.5: The Mesh Display Dialog Box

The basic steps for generating a mesh or outline plot are as follows:

1.   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, 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).

To choose all "outline'' surfaces (i.e., surfaces on the outer boundary of the domain), click the Outline button below the Surface Types list. If all outline surfaces are already selected, this will deselect them. To choose all "interior'' surfaces, click the Interior button. If all interior surfaces are already selected, this will deselect them.

2.   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  29.1.1), 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  29.1.2), select Edges under Options and All under Edge Type.

  • To generate a filled-mesh display (as in Figure  29.1.3), select Faces under Options.

  • To draw the nodes on the selected surfaces (as in Figure  29.1.4), select Nodes under Options.

3.   Set any of the mesh and outline display options described below.

4.   Click the Display button to draw the specified mesh or outline in the active graphics window.

If you choose to display filled meshes, and you want a smoothly shaded display, you should turn on 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 Section  29.2.7 for details.

Mesh and Outline Display Options

The options mentioned in the procedure above 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.

Modifying the Mesh Colors

ANSYS FLUENT allows 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  29.1.6) by clicking on the Colors... button in the Mesh Display dialog box.

Figure 29.1.6: The Mesh Colors Dialog Box

(Note that 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, allowing 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 (i.e., meshes that are drawn for surfaces created using the dialog boxes opened from the Surface menu) 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.

Adding Features to an Outline Display

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 (i.e., those that are used by only one face on the boundary) are drawn. In Figure  29.1.7, which shows the outline display for a complicated duct geometry, only the inlet and outlet are visible.

Figure 29.1.7: Standard Outline of Complex Duct

Figure 29.1.8: Feature Outline of Complex Duct

You can capture additional features using the Feature option in the Mesh Display dialog box. (See Figure  29.1.8.) Turn on 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 $^\circ$, the edge between those faces will be drawn. Decreasing the Feature Angle will result in more edge lines (i.e., 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.

Drawing Partition Boundaries

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.

Shrinking Faces and Cells in the Display

If you need to distinguish individual faces or cells in the display, you may want to 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 allow you to distinguish one face or cell from its neighbor. Displays with different Shrink Factor values are shown in Figures  29.1.9 and  29.1.10. Remember that you must click Display to see the effect of the change in Shrink Factor.

Figure 29.1.9: Mesh Display with Shrink Factor = 0

Figure 29.1.10: Mesh Display with Shrink Factor = 0.01

next up previous contents index Previous: 29.1 Basic Graphics Generation
Up: 29.1 Basic Graphics Generation
Next: 29.1.2 Displaying Contours and
Release 12.0 © ANSYS, Inc. 2009-01-29