ANSYS Fluent enables you to plot contour lines or profiles superimposed on the physical domain. Contour lines are lines of constant magnitude for a selected variable (isotherms, isobars, and so on). A profile plot draws these contours projected off the surface along a reference vector by an amount proportional to the value of the plotted variable at each point on the surface. Sample plots are shown in Figure 31.11: Contours of Static Pressure and Figure 31.12: Profile Plot of y Velocity.
For information about displaying contours or profiles on a surface that sweeps through the domain, see Displaying Results on a Sweep Surface.
You can plot contours or profiles using the Contours Dialog Box (Figure 31.13: The Contours Dialog Box).
Results → Graphics → Contours
Edit...
The basic steps for generating a contour or profile plot are as follows:
Select the variable or function to be contoured or profiled 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 Field Function Definitions for an explanation of the variables in the list.)
Choose the surface or surfaces on which to draw the contours or profiles in the Surfaces list. For 2D cases, if no surface is selected, contouring or profiling is done on the entire domain. For 3D cases, you must always select at least one surface.
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.
Specify the number of contours or profiles in the Levels field. The maximum number of levels allowed is 100.
If you are generating a profile plot, enable the Draw Profiles option. In the resulting Profile Options Dialog Box (Figure 31.14: The Profile Options Dialog Box) you will define the profiles.
Set the “zero height” reference value for the profile (Reference Value) and the length scale factor for projection (Scale Factor). Any point on the profile with a value equal to the Reference Value will be plotted exactly on the defining surface. Values greater than the Reference Value will be projected ahead of the surface (in the direction of Projection Dir.) and scaled by Scale Factor), and values less than the Reference Value will be projected behind the surface and scaled.
These parameters can be used to create fuller profiles when you need to display the variation in a variable that is small compared to the absolute value of the variable. Consider, for example, the display of temperature profiles when the temperature range in the domain is from 300 K to 310 K. The 10 K range in the temperature will be hard to detect when profiles are drawn using the default scaling (which will be based on the absolute magnitude of 310 K). To create a fuller profile, you can set the Reference Value to 300 and the profile Scaling Factor to 5 (for example) to magnify the display of the remaining 10 K range. In subsequent display of the profiles, the reference value of 300 will be effectively subtracted from the data before display so that the temperatures of 300 K will not be offset from the baselines. The profiles will then reflect only the variation of temperature from 300 K.
Set the direction in which profiles are projected (Projection Dir.). In 2D, for example, a contour plot of
pressure on the entire domain can be projected in the direction to form a carpet
plot, or a contour plot of
velocity on a sequence of
-coordinate slice lines can be
projected in the
direction to form a series of velocity profiles
(as shown in Figure 31.12: Profile Plot of y Velocity).
Click and close the Profile Options Dialog Box.
Set any of the contour and profile plot options described below.
Click to draw the specified contours or profiles in the active graphics window.
The resulting display will include the specified number of contours or profiles of the selected variable, with the magnitude on each one determined by equally incrementing between the values shown in the Min and Max fields.
The options mentioned in the procedure above include drawing color-filled contours/profiles (instead of the default line contours/profiles), specifying a range of values to be contoured or profiled, including portions of the mesh in the contour or profile display, choosing node or cell values for display, and storing the contour or profile plot settings.
Color-filled contour or profile plots show a contour or profile display containing a continuous color display (see Figure 31.15: Filled Contours of Static Pressure), instead of just drawing lines representing specific values. Note that a color-filled profile display is often referred to as a “carpet plot”. To generate a filled contour or profile plot, enable the Filled option in the Contours Dialog Box during step 5 in the previous section.
To display smoothly shaded filled contours, you must enable lighting and select a lighting interpolation method other than Flat in the Display Options Dialog Box or the Lights Dialog Box. You will not get smooth shading of filled contours if the Clip to Range option is turned on. Smooth shading of filled profiles is not available.
Note: The Draw Profile option settings are not saved with the contour plot definition. Once the dialog box is closed these options will revert to being disabled.
By default, the minimum and maximum values contoured or profiled are set based on the range of values in the entire domain. This means that the color scale will start at the smallest value in the domain (shown in the Min field) and end at the largest value (shown in the Max field). If you are plotting contours or profiles on a subset of the domain (that is, on a surface), your plot may cover only the midrange of the color scale. For example, if blue corresponds to 0 and red corresponds to 10, and the values on your surface range only from 4 to 6, your plot will contain mostly green contours or profiles, since green is the color at the middle of the default color scale.
To focus in on a smaller range of values, so that blue corresponds to 4 and red to 6, manually reset the range to be displayed. You can also use the minimum and maximum values on the selected surfaces—rather than in the entire domain—to determine the range. Another reason to manually set the range is if you are interested only in certain values. For example, if you want to determine the region where pressure exceeds a certain value, you can increase the minimum value for display so that the lower pressure values are not displayed.
To manually set the contour/profile range, turn off the Auto Range option in the Contours Dialog Box. The Min and Max fields will become editable, and you can enter the new range of values to be displayed.
To show the default range at any time, click and the Min and Max fields will be updated.
If you are drawing filled contours or profiles you can control whether or not values outside the prescribed Min/ Max range are displayed.
To leave areas in which the value is outside the specified range empty (that is, draw no contours or profiles), enable the Clip to Range option. This is the default setting. If you turn Clip to Range off, values below the Min value will be colored with the lowest color on the color scale, and values above the Max value will be colored with the highest color on the color scale. Figure 31.16: Filled Contours with Clip to Range On and Figure 31.17: Filled Contours with Clip to Range Off show the results of enabling/disabling the Clip to Range option.
To base the minimum and maximum values on the range of values on the selected surfaces, rather than in the entire domain, turn off the Global Range option in the Contours Dialog Box. The Min and Max values will be updated when you next click Compute or .
For some problems, especially complex 3D geometries, you may want to include portions of the mesh in your contour or profile plot as spatial reference points. For example, you may want to show the location of an inlet and an outlet along with the contours. This is accomplished by turning on the Draw Mesh option in the Contours Dialog Box. The Mesh Display Dialog Box will appear automatically when you enable the Draw Mesh option, and you can set the mesh display parameters there. When you click in the Contours Dialog Box, the mesh display, as defined in the Mesh Display Dialog Box, will be included in the contour or profile plot.
Note: The Draw Mesh option settings are not saved with the contour plot definition. Once the dialog box is closed these options will revert to being disabled.
To include the mesh with a contour plot that will be persisted with the case file, you can create a mesh plot definition and include both the mesh and contour plots in a scene. See Displaying a Scene for more details.
In ANSYS Fluent you can choose to display the computed cell-center values or values that have been interpolated to the nodes. By default, the Node Values option is turned on, and the interpolated values are displayed. For line contours or profiles, node values are always used. To display filled contours or profiles and to display the cell values, turn off the Node Values option. Filled contours/profiles of node values will show a smooth gradation of color, while filled contours/profiles of cell values may show sharp changes in color from one cell to the next.
For face-only functions (for example, Wall Shear Stress), the cell values that are displayed for boundary zone surfaces will actually be the face values. This is only true in the case of boundary zone surfaces created for postprocessing, where the actual cell values are used for the part of the surface that lies in the interior. These face values are more accurate, as face-only functions are computed on the faces and not on the cells. For more information about cell values, see Cell Values.
If you are plotting contours to show the effect of a porous medium or 2D fan boundary, to depict a shock wave, or to show any other discontinuities or jumps in the plotted variable, you should use cell values; if you use node values in such cases, the discontinuity will be smeared by the node averaging for graphics and will not be shown clearly in the plot.
For frequently used combinations of contour variables and options, you can store the information needed to generate the contour plot as follows:
In the Contours Dialog Box, specify a Setup number.
Set up the desired information in the Contours Dialog Box.
Click .
The settings for Options, Contours of, Min, Max, and Surfaces will be saved.
You can then change the Setup number to an unused value (that is, an ID for which no information has been saved) and generate a different contour plot.
To generate a plot using the saved setup information:
Change the Setup number back to the value for which you saved contour information.
Click .
You can save up to 10 different setups.
Important: Note that the number of contour Levels, the surfaces selected for display in the Mesh Display Dialog Box (when the Draw Mesh option is activated), and the settings for profiles in the Profile Options Dialog Box (when the Draw Profiles option is activated) will not be saved in the Setup, nor will the Setup be saved in the case file.
You can create named contour plot definitions and save them for later use. This could be useful for demonstration purposes, scene creation, or for postprocessing the results of your simulation when varying the settings between runs (to name a few examples).
The number of contour plot definitions is not limited.
To create a contour plot definition:
Results → Graphics → Contours
New...
In the Contours Dialog Box, in the Contour Name text entry
box, enter the name for your contour plot definition (or accept the
default name
contour-).id
Important: Contour and vector plot definitions must have unique names.
Set contour parameters and options.
The Draw Mesh and Draw Profile option settings are not saved with the contour plot definition. Once the dialog box is closed these options will revert to being disabled.
Click .
The specified contour will be displayed in the active graphics window, and the new contour plot definition with the name you have entered will appear in the tree under Contours.
Once the contour plot definition is created, you can perform the following actions using the right-click menu commands:

Edit the existing contour plot definition.
Copy the contour plot definition.
When creating a copy of the existing contour, you can modify contour settings in the Contours dialog box that will open.
Delete the selected contour plot definition.
Display the contour in the graphics window.
Add the selected contour to the plot in the graphics window.
Note that while Display replaces the current contents of the graphics window, Add to graphics preserves the current graphics window contents.
You can move the colormap of contour plot definitions by left-clicking and dragging it to the desired location. The colormap can also be resized by dragging the corners of the box that appears when you hover over the colormap. The colormap location is not saved with the contour plot definition.
For 2D cases, Fluent automatically creates a new surface when you click in the Contours dialog box, if you have not selected any surfaces for display. New surfaces are only created for fluid zones that do not already have a surface defined.
These commands are also available through the text user interface
(display/objects).