The available materials include:

You can use the Material Editor dialog box to create custom materials for realistic rendering.

To create a custom material:

Once a new material is created, it is available for selection in the relevant dialog boxes (Surface Rendering Properties Dialog Box, Zone Type Color and Material Assignment Dialog Box, and Mesh Display Dialog Box). Refer to Realistic Rendering of Materials for guidance on how to use these dialog boxes to achieve your rendering goals.

The following limitations exist for the rendering of realistic materials in Fluent:

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 40.21: Standard Outline of Complex Duct, which shows the outline display for a complicated duct geometry, only the inlet and outlet are visible.

Figure 40.21: Standard Outline of Complex Duct

Figure 40.22: Feature Outline of Complex Duct

You can capture additional features using the Feature option in the Mesh Display Dialog Box. (See Figure 40.22: 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 40.23: Mesh Display with Shrink Factor = 0 and Figure 40.24: Mesh Display with Shrink Factor = 0.01. Click Display to see the effect of the change in Shrink Factor.

Figure 40.23: Mesh Display with Shrink Factor = 0

Figure 40.24: Mesh Display with Shrink Factor = 0.01

Color-filled contour or profile plots show a contour or profile display containing a continuous color display (see Figure 40.30: 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.

Figure 40.30: Filled Contours of Static Pressure

To display smoothly shaded filled contours, ensure the lighting interpolation method is not set to 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.

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.

Figure 40.31: Filled Contours with Clip to Range On

Figure 40.32: Filled Contours with Clip to Range Off

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 Display 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.

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.

Enabling Boundary Values in addition to Node Values, displays interpolated boundary face values, when available. If Boundary Values are enabled with Node Values disabled, then the displayed values are boundary face values (not interpolated), if available. Variables that have explicit node values available at boundaries are indicated by "bnv" in Table 42.2: Pressure and Density Categories – Table 42.21: Acoustics Category . Note that when Boundary Values is enabled and velocity contours are selected for postprocessing, Fluent reports the user-specified wall velocity values for wall zones.

The displayed values are derived as follows:

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:

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:

You can save up to 10 different setups.

By default, vectors are scaled automatically so that the arrows overlap minimally when no vectors are skipped. For instructions on thinning the vector display, see “Thinning” Pathlines. With the Auto Scale option, you can modify the Scale factor (which is set to 1 by default) to increase or decrease the vector scale from the default “auto scale”. The main advantage of autoscaling is that the vector display with a scale factor of 1 will always be appropriate, regardless of the size of the domain, giving you a better starting point for fine-tuning the vector scale.

If you turn off the Auto Scale option, the vectors will be drawn at their actual sizes scaled by the scale factor (Scale, which is set to 1 by default). The “actual” size of a vector is the magnitude of the vector variable (velocity, by default) at the point where it is drawn. A vector drawn at a point where the velocity magnitude is 100 m/s is drawn 100 m long, whether the domain is 0.1 m or 1000 m. You can modify the vector scale by changing the value of Scale in the Vectors Dialog Box until the size of the vectors (that is, the actual size multiplied by Scale) is satisfactory.

If your vector display is difficult to understand because there are too many arrows displayed, you can “thin out” the vectors by changing the Skip value in the Vectors Dialog Box. By default, Skip is set to 0, indicating that a vector will be drawn for each cell in the domain or for each face on the selected surface (for example, vectors). If you increase Skip to 1, every other vector will be displayed, yielding vectors. If you increase Skip to 2, every third vector will be displayed, yielding vectors, and so on. The order of faces on the selected surface (or cells in the domain) will determine which vectors are skipped or drawn; therefore adaption will change the appearance of the vector display when a nonzero Skip value is used.

For some problems, you may be interested in visualizing velocity (or other vector) components that are normal to the flow. These “secondary flow” components are usually much smaller than the components in the flow direction and are difficult to see when the flow direction components are also visible. To easily view the normal flow components, you can enable the In Plane option in the Vector Options Dialog Box. When this option is on, Ansys Fluent will display only the vector components in the plane of the surface selected for display. If the selected surface is a cross-section of the flow domain, you will be displaying the components normal to the flow.

Figure 40.40: Velocity Vectors Generated Using the In Plane Option shows velocity vectors generated using the In Plane option. Note that these vectors have been translated outside the domain, as described in Transforming Geometric Objects in a Scene, so that they can be seen more easily.

Figure 40.40: Velocity Vectors Generated Using the In Plane Option

By default, the length of a vector is proportional to its velocity magnitude. If you want all of the vectors to be displayed with the same length, you can enable the Fixed Length option in the Vector Options Dialog Box. To modify the vector length, adjust the value of the Scale factor in the Vectors Dialog Box.

All Cartesian components of the vectors are drawn by default, so that the arrow points along the resultant vector in physical space. However, sometimes one of the components, say, the component, is relatively large. In such cases, you may want to suppress the component and scale up the vectors, in order to visualize the smaller and components. To suppress one or more of the vector components, turn off the appropriate button(s) (X, Y, or Z Component) in the Vector Options Dialog Box.

By default, the minimum and maximum vectors included in the vector display are set based on the range of vector-variable (velocity, by default) magnitudes in the entire domain. If you want to focus in on a smaller range of values, you can restrict the range to be displayed. The color scale for the vector display will change to reflect the new range of values. (You can also use the minimum and maximum values on the selected surfaces—rather than on the entire domain—to determine the range, or change the scalar field by which the vectors are colored from velocity magnitude to any other scalar, as described below.)

To manually set the range of velocity magnitudes (or the range of whatever scalar field is selected in the Color by drop-down list), turn off the Auto Range option in the Vectors Dialog Box. The Min and Max fields will become editable, and you can enter the new range of values to be displayed. For example, if you want to display velocity vectors only in regions where the velocity magnitude exceeds 150 m/s but is less than 300 m/s, you will change the value of Min to 150 and the value of Max to 300. Similarly, if you are coloring the vectors by static pressure, you can choose to display velocity vectors only in regions where the pressure is within a specified range. To show the default range at any time, click Compute and the Min and Max fields will be updated.

When you restrict the range of vectors displayed, you can also 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 vectors), 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. This feature is the same as the one available for displaying filled contours (see Figure 40.31: Filled Contours with Clip to Range On and Figure 40.32: Filled Contours with Clip to Range Off).

You can also choose to base the minimum and maximum values on the range of values on the selected surfaces, rather than the entire domain. To do this, turn off the Global Range option in the Vectors Dialog Box. The Min and Max values will be updated when you next click Compute or Display.

If you want to color the vectors by a scalar field other than velocity magnitude (the default), you can select a different variable or function in the Color by drop-down list. Select the desired category in the upper list, and then choose one of the related quantities from the lower list. If you choose static pressure, for example, the length of the vectors will still correspond to the velocity magnitude, but the color of the vectors will correspond to the value of pressure at each point where a vector is drawn.

You can adjust the tessellation of the 3d arrow and 3d arrowhead vector plot Styles. This control has a valid range of 0-74.

Tessellation is accessed by clicking Vector Options... in the Vectors dialog box. Tessellation affects how round the edges of the cylinder and arrowhead appear. Lower values appear less round, which comes with some performance benefit in rendering the vector plot.

Figure 40.41: 3D Arrow Vectors with Tessellation of 24

Figure 40.42: 3D Arrow Vectors with Tessellation of 6

If you want all of the vectors to be the same color, you can select the color to be used in the Color drop-down list in the Vector Options Dialog Box. If no color is selected (that is, if you choose the empty space at the top of the drop-down list—the default selection), the vector color will be determined by the Color by field specified in the Vectors Dialog Box. Single color vectors are useful in displays that overlay contours and vectors.

For some problems, especially complex 3D geometries, you may want to include portions of the mesh in your vector plot as spatial reference points. For example, you may want to show the location of an inlet and an outlet along with the vectors. This is accomplished by turning on the Draw Mesh option in the Vectors 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 Display in the Vectors Dialog Box, the mesh display, as defined in the Mesh Display Dialog Box, will be included in the vector plot.

There are seven different vector arrow styles available. Choose 3d arrow, 3d arrowhead, cone, filled-arrow, arrow, harpoon, or headless in the Style drop-down list in the Vectors Dialog Box.

If you choose a vector arrow style that includes heads, you can control the size of the arrowhead by modifying the Scale Head value in the Vector Options Dialog Box.

To create your own custom vector, you will use the Custom Vectors Dialog Box (Figure 40.43: The Custom Vectors Dialog Box). This dialog box enables you to define custom vectors based on existing quantities. Any vectors that you define will be added to the Vectors of list in the Vectors Dialog Box.

To open the Custom Vectors Dialog Box, click Custom Vectors... in the Vectors Dialog Box.

Figure 40.43: The Custom Vectors Dialog Box

The steps for creating a custom vector are as follows:

Once you have defined your vectors, you can manipulate them using the Vector Definitions Dialog Box (Figure 40.44: The Vector Definitions Dialog Box). You can display a vector definition to be sure that it is correct, delete the vector if you decide that it is incorrect and must be redefined, or give the vector a new name. You can also save custom vectors to a file or read them from a file. The custom vector file enables you to transfer custom vectors between case files.

To open the Vector Definitions Dialog Box, click Manage... in the Custom Vectors Dialog Box.

Figure 40.44: The Vector Definitions Dialog Box

The following actions can be performed in the Vector Definitions Dialog Box:

For some problems, especially complex 3D geometries, you may want to include portions of the mesh in your pathline display as spatial reference points. For example, you may want to show the location of an inlet and an outlet along with the pathlines (as in Figure 40.45: Pathline Plot). This is accomplished by turning on the Draw Mesh option in the Pathlines Dialog Box. The Mesh Display Dialog Box will appear when you enable the Draw Mesh option, where you can set the mesh display parameters. When you click Display in the Pathlines Dialog Box, the mesh display, as defined in the Mesh Display Dialog Box, will be included in the plot of pathlines.

Pathlines can be displayed as lines (with or without arrows), ribbons, cylinders (coarse, medium, or fine), triangles, spheres, or a set of points. You can choose line, line-arrows, point, sphere, refined-sphere, ribbon, triangle, coarse-cylinder, medium-cylinder, or fine-cylinder in the Style drop-down list in the Pathlines Dialog Box. Pulsing can be done only on point, sphere, refined-sphere, or line styles.

Once you have selected the pathline style, click Style Attributes... to set the pathline thickness and other parameters related to the selected Style:

By default, the pathlines are colored by the particle ID number. That is, each particle’s path will be a different color. You can also choose the color based on the surface from where the pathlines were released from using the surface ID as the particle variable. You can choose to color the pathlines by any of the scalar fields in the Color by drop-down list. Select the desired category in the upper list and then select a related quantity in the lower list. If you color the pathlines by velocity magnitude, for example, each particle’s path will be colored depending on the speed of the particle at each point in the path.

The range of values of the selected scalar field will, by default, be the upper and lower limits of that field in the entire domain. The color scale will map to these values accordingly. If you prefer to restrict the range of the scalar field, turn off the Auto Range option (under Options) and set the Min and Max values manually beneath the Color by list. If you color the pathlines by velocity, and you limit the range to values between 30 and 60 m/s, for example, the “lowest” color will be used when the particle speed falls below 30 m/s and the “highest” color will be used when the particle speed exceeds 60 m/s. To show the default range at any time, click Compute and the Min and Max fields will be updated.

If your pathline plot is difficult to understand because there are too many paths displayed, you can “thin out” the pathlines by changing the Path Skip value in the Pathlines Dialog Box. By default, Path Skip is set to 0, indicating that a pathline will be drawn from each face on the selected surface (for example, pathlines). If you increase Path Skip to 1, every other pathline will be displayed, yielding pathlines. If you increase Path Skip to 2, every third pathline will be displayed, yielding , and so on. The order of faces on the selected surface will determine which pathlines are skipped or drawn; therefore adaption will change the appearance of the pathline display when a nonzero Path Skip value is used.

To further simplify pathline plots, and reduce plotting time, a coarsening factor can be used to reduce the number of points that are plotted. Providing a coarsening factor of , will result in each ^th point being plotted for a given pathline in any cell. This coarsening factor is specified in the Pathlines Dialog Box, in the Path Coarsen field. For example, if the coarsening factor is set to 2, then Ansys Fluent will plot alternate points.

If you are interested in determining the source of a particle for which you know the final destination (for example, a particle that leaves the domain through an exit boundary), you can reverse the pathlines and follow them from their destination back to their source. To do this, enable the Reverse option in the Pathlines Dialog Box. All other inputs for defining the pathlines will be exactly the same as for forward pathlines; the only difference is that the surface(s) selected in the Release From Surfaces list will be the final destination of the particles instead of their source.

If you want to display “oil-flow” pathlines (that is, pathlines that are constrained to lie on a particular boundary), enable the Oil Flow option in the Pathlines Dialog Box. You will then need to select one or more boundary zones in the On Zone list. The selected zone(s) are the boundaries on which the oil-flow pathlines will lie.

If you are going to use the Pulse button in the Pathlines Dialog Box to animate the pathlines, you can choose one of two pulse modes for the release of particles that follow the pathlines. To release a single wave of particles, select the Single option under Pulse Mode. To release particles continuously from the initial positions, select the Continuous option.

You can save an animation of the pathline pulse by enabling Save Pulse Animation under Options. This creates an additional Write/Record Format drop-down to appear below the display state. You can specify whether you write a video file or picture files. Click Video Options... to open the Video Options Dialog Box, which controls additional settings for the Video File option. Click Picture Options... to open the Save Picture Dialog Box, which controls additional settings for the Picture Files option.

A Continuous pulse video file will be 5 seconds long, while a Single pulse video will be one full cycle.

If you are using large time step size for the calculation, there might be significant error introduced while calculating the pathlines. To control this error, select Accuracy Control and specify the value of Tolerance. The tolerance value will be taken in to consideration while calculating the pathlines for each time step.

If you want to display the pathlines relative to the moving reference frame, enable the Relative Pathlines option in the Pathlines Dialog Box. You will then need to select the surfaces from the Release from Surfaces list.

If you want to generate an XY plot along the trajectories of the pathlines you have defined, enable the XY Plot option in the Pathlines Dialog Box. The Color by drop-down list will be replaced by Y Axis Function and X Axis Function lists. Select the variable to be plotted on the -axis in the Y Axis Function list, and specify whether you want to plot this quantity as a function of the Time elapsed along the trajectory, or the Path Length along the trajectory by selecting the appropriate item in the X Axis Function drop-down list. Specify the Step Size, number of Steps, and other parameters as usual for a standard pathline display. Then click Plot to display the XY plot.

Once you have generated an XY plot, you may want to save the plot data to a file. You can read this file into Ansys Fluent at a later time and plot it alone using the Plot Data Sources Dialog Box, as described in Creating an XY Plot From Multiple Data Sources (Including Files), or add it to a plot of solution data, as described in Including External Data in the Solution XY Plot.

To save the plot data to a file, enable the Write to File option in the Pathlines Dialog Box. The Plot button changes to a Write... button. Clicking Write... opens The Select File Dialog Box, in which you can specify a name and save a file containing the plot data. The format of this file is described in XY Plot File Format.

To save pathline data to a file, perform the following steps:

To initiate saving pathline data through the text command interface enter the following TUI command:

display/path-lines/write-to-files

In addition to pathline data, you can also export particle data in either Standard, EnSight or Geometry type. For information on exporting particle data in FIELDVIEW (standard), EnSight or .ibl (geometry) format, refer to Exporting Steady-State Particle History Data.

FVPARTICLES 2 1 
Tag Names 
0 
Variable Names 
2 
time 
particle_id 
3 
0.2 0.8 1.3 0.2 0 
0.3 0.9 1.3 0.4 0 
0.5 1.1 1.3 0.6 0 

Closed	Index	Arclength
Begin section ! 1
	Begin curve ! 1
	1                  185.61 	    0                 23.26
  	2       88.90000000000001 	    0                -89.67

  	Begin curve ! 2
  	1       88.89999999999569 	    0      -89.6699999999997
  	2       76.90221619148909 	    0     -101.2290490001453
  	3       62.92208239159677 	    0     -110.2907424975297
  	4       47.47166726362848 	    0     -116.5231659809653
  	5       31.11689338997181 	    0     -119.6980363161113
  	6       14.45680848476821 	    0     -119.6990633707006
  	7      -1.898356710978934 	    0     -116.5262095254603
  	8      -17.34954014966171 	    0     -110.2956910520416
  	9      -31.33079110697006 	    0     -101.2357213074894
  	10       -43.330000000007 	    0     -89.67815166483965

  	Begin curve ! 3
  	1                  -43.33 	    0     -89.67815166485001
  	2                 -175.56 	    0         64.69066040289 

File is written from fluent in ensight measured particle format for
t = 2.42813e-04
particle coordinates
		9
		1-7.27734e-05 1.91710e-03 4.69093e-03
		2-1.75772e-04 1.97040e-03 3.92842e-03
		3-2.26051e-04 2.10134e-03 5.63228e-03
		4-1.16390e-04 2.32442e-03 5.23423e-03
		5-6.32735e-04 2.53326e-03 5.70791e-03
		6-9.69431e-04 2.37006e-03 5.27602e-03
		7-6.77868e-04 2.92054e-03 4.11570e-03
		8-9.78029e-04 2.75717e-03 4.13314e-03
		9-8.54859e-04 3.73727e-03 2.23796e-03

particle id
	0.00000e+00 6.00000e+00 1.20000e+01 1.80000e+01 2.40000e+01 3.00000e+01
	3.60000e+01 4.20000e+01 4.80000e+01

FORMAT
type: ensight gold
GEOMETRY
model: spray2-unsteady.geo
measured: 1 particle.mpg****
VARIABLE
scalar per measured node: 1 particle-id particle.mscl****
scalar per node: pressure                     spray2-unsteady.scl1
scalar per node: pressure-coefficient         spray2-unsteady.scl2
vector per node: velocity                     spray2-unsteady.vel
TIME
time set: 1 Model
number of steps: 10
filename start number:   1
filename increment:      1
time values: 0.00000e+00 1.21406e-04 2.42813e-04 3.64219e-04 4.85626e-04
6.07032e-04 7.28438e-04 8.49845e-04 9.71251e-04 1.09266e-03

In Ansys Fluent you can determine the scalar field value at a particle location using 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 used. If you prefer to use the cell values, turn the Node Values option off. Note that for face-only functions like Wall Shear Stress, the cell value is the area-weighted average from the face values that define that cell as c0.

If you are plotting pathlines 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.