When you have defined discrete phase particle injections, as described in Setting Initial Conditions for the Discrete Phase, you can display the trajectories of these discrete particles using the Particle Tracks Dialog Box (Figure 23.37: The Particle Tracks Dialog Box).
You can create named particle track definitions and save them for later use. See Creating and Using Contour Plot Definitions for additional information on graphics object definitions.
Note that particle track definitions can be included in scenes as long as the XY Plot option is not enabled. See Displaying a Scene for additional information on scenes.
Results → Graphics →
Particle Tracks
New...
The procedure for drawing trajectories for particle injections is as follows:
Select the particle injection(s) you want to track in the Release from Injections list. (You can choose to track a specific particle, instead, as described below.)
Set the length scale and the maximum number of steps in the Discrete Phase Model Dialog Box, as described in Numerics of the Discrete Phase Model.
Setup → Models → Discrete Phase
Edit...
If stochastic and/or cloud tracking is desired, set the related parameters in the Set Injection Properties dialog box, as described in Stochastic Tracking.
Note: Displaying tracks multiple times at the same solution state will result in identical random tracks. This is because the same random seeds are used enabling you to postprocess different variables on the same particle tracks.
Set any of the display options described below.
Click the button to draw the trajectories or click the button to animate the particle positions. The button will become the button during the animation, and you must click to stop the pulsing.
Important: For unsteady particle tracking simulations, clicking will show only the current location of the particles. Typically, you should select point in the Track Style drop-down list when displaying transient particle locations since individual positions will be displayed. The button option is not available for unsteady tracking.
You can display the trajectory for an individual particle stream instead of for all the streams in a given injection. Additionally, you can visualize the trajectories for the wall film particles (if they are present in the simulation) and/or free stream particles. To do so, you must first determine which particle is of interest. Use the Injections Dialog Box to list the particle streams in the desired injection, as described in Creating and Modifying Injections.
Setup → Models → Discrete Phase → Injections
Edit...
Note the ID numbers listed in the first column of the listing printed in the ANSYS Fluent console. Then perform the following steps after step 1 above. In the Particle Tracks Dialog Box:
Enable Free Stream Particles if you want to display those types of particles. Note that this option is available only when the Lagrangian wall film model is enabled in the wall boundary conditions dialog box, under the DPM tab.
Enable Wall Film Particles if you want to display those types of particles. Note that this option is available only when the Lagrangian wall film model is enabled in the wall boundary conditions dialog box, under the DPM tab.
Enable the Track Single Particle Stream to display those types of particles.
In the Stream ID field, specify the ID number of the particle stream for which you want to plot the trajectory.
Particle tracking 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, ribbon, triangle, coarse-cylinder, medium-cylinder, or fine-cylinder in the Track Style drop-down list in the Particle Tracks dialog box. Pulsing can be done only on point, sphere, or line styles.
Once you have selected the track style, click the button to specify how you would like to display the particle tracks.
Note: The Track Style options that will appear depend on whether you are running a transient or steady-state simulation. For a transient case, the only Track Style options available are the point and sphere styles.
If you are using the line or line-arrows style, set the Line Width in the Track Style Attributes dialog box (Figure 23.38: The Track Style Attributes Dialog Box) that appears when you click the button. For line-arrows you will also set the Spacing Factor, which controls the spacing between the particles tracks. The size of the arrow heads can be adjusted by entering a value in the Scale text-entry box.
If you are using the point style, you will set the Marker Size in the Track Style Attributes dialog box. The thickness of the particle track will be the thickness of the marker.
If you are using the sphere style, you will set the Diameter, scale, and Detail in the Particle Sphere Style Attributes dialog box (Figure 23.39: The Particle Sphere Style Attributes Dialog Box). You have the option of specifying a constant diameter if you enable Constant under Options and you will then specify the Diameter. If you enable Variable, you can select a particle variable to estimate the size of the spheres. The spheres are scaled by the factor entered in the Scale entry box.
The best constant diameter to use will depend on the dimensions of the domain, the view, and the particle density. However, an adequate starting point would be a diameter on the order of 1/4 of the average cell size or 1/4 step size. Units for the Diameter field correspond to the mesh dimensional units.
The level of detail applied to the graphical rendering of the spheres can be controlled using the Detail field. The level of detail uses integer values ranging from 4 to 50. Note that the performance of the graphical rendering as well as the memory consumption will be better when using a small level of detail, that is, very coarse spheres, such as 6 or 8. The rendering performance significantly decreases with higher levels of detail. You should gradually increase the detail to determine the best-case scenario between performance and quality.
Whenever Auto Range is disabled, the spheres are displayed only if they have values between Min and Max.
Also note that to take full advantage of spherical rendering, lighting should be turned on in the view. The Gouraud setting provides much smoother looking spheres than the Flat setting and better performance than the Phong setting. For more information on lighting, see Adding Lights.
If you are using the triangle or any of the cylinder styles, you will set the Width in the Track Style Attributes dialog box. For triangles, the specified value will be half the width of the triangle’s base, and for cylinders, the value will be the cylinder’s radius.
If you are using the ribbon style, clicking on the button will open the Ribbon Attributes Dialog Box, in which you can set the ribbon’s Width. You can also specify parameters for twisting the ribbon tracks. In the Twist By drop-down list, you can select a scalar field on which the tracks twisting is based (for example, helicity). Select the desired category in the upper list and then select a related quantity in the lower list. The twisting may not be displayed smoothly because the scalar field by which you are twisting the tracks is calculated at cell centers only (and not interpolated to a particle’s position). The Twist Scale sets the amount of twist for the selected scalar field. To magnify the twist for a field with very little change, increase this factor; to display less twist for a field with dramatic changes, decrease this factor.
When you click , the Min and Max fields will be updated to show the range of the Twist By scalar field.
You can choose to have the particle tracks displayed as vectors. Choose the Vector Style from the drop-down list in the Particle Tracks dialog box:
If you select vector, the vector will be generated starting in the center of the particle, as shown in Figure 23.40: Particles with the Vector Style.
If you select centered-vector, the midpoint of the vector will appear in the center of the particle, as shown in Figure 23.41: Particles with the Centered Vector Style.
If you select centered-cylinder, the midpoint of the cylinder will appear in the center of the particle, as shown in Figure 23.42: Particles with the Centered Cylinder Style.
Click the button to specify how you would like to display the particle tracks. In the Particle Vector Style Attributes dialog box (Figure 23.43: The Particle Vector Style Attributes Dialog Box) you will set the Length, Scale, and Length to Head Ratio. The direction of the vectors is displayed for the selected variable under Vectors of. You have the option of specifying a Constant Length or a Variable Length, which is based on the variable selected under Length by. If Constant Color is enabled, then all vectors/cylinders are colored by the color selected in the Color drop-down list. Otherwise, it is the color selected in the Particle Tracks dialog box (seen in the Mesh Colors dialog box when Draw Mesh is enabled).
Vectors can be scaled by the factor given in the Scale entry box. The ratio of vector length to vector head size can be changed in the box Length to Head Ratio. In the case of a cylinder, the ratio of the length to the diameter is affected.
Use the Import Particle Data dialog box (Figure 23.44: The Import Particle Data Dialog Box) to import particle data to display in the graphics window.
Postprocessing → Model Specific → Discrete Phase → Import Particle Data...
Click to display a file selection dialog box where you can enter a file name and a directory that contains the imported data.
Choose from the available import options by selecting Auto Range and/or Draw Mesh under Options. If you prefer to restrict the range of the scalar field, disable the Auto Range option and set the Min and Max values manually beneath the Color by list.
Choose to color the particle pathlines by any of the scalar fields in the Color by list. If you select COLORBY, the pathlines will be colored by the quantity that was chosen when the particle data file was created. (See Exporting Steady-State Particle History Data)
Select a pathline style under Style. To set pathline style attributes, click the button. For more information about the pathline style types, see Controlling the Pathline Style.
The value of Steps sets the maximum number of steps a particle can advance. A particle will stop when it has traveled this number of steps or when it leaves the domain.
If your pathline plot is difficult to understand because there are too many paths displayed, you can “thin out” the pathlines by changing the Skip value.
Click the button to draw the pathlines, or click the button to animate the particle positions. The button will become the button during the animation, and you must click to stop the pulsing.
You can include the mesh in the trajectory display, control the style of the trajectories (including the twisting of ribbon-style trajectories), color them by different scalar fields and control the color scale, and coarsen trajectory plots. You can also choose node or cell values for display. If you are “pulsing” the trajectories, you can control the pulse mode. Finally, you can generate an XY plot of the particle trajectory data (for example, residence time) as a function of time or path length and save this XY plot data to a file.
Note: The Draw Mesh option settings are not saved with the particle track plot definition. Once the dialog box is closed these settings will revert to being disabled. If you want these settings persisted within the current session, you can use the non-persistent Particle Tracks dialog box.
Postprocessing → Graphics
→
Particle Tracks
→
Edit...
Plotting particle trajectories can be very time consuming, therefore,
to reduce the 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 trajectory in any cell. This coarsening
factor is specified in the Particle Tracks Dialog Box, in the Coarsen field and is only valid for
steady-state cases. For example, if the coarsening factor is set to
2, then ANSYS Fluent will plot alternate points.
Important: Note that if any particle or pathline enters a new cell, this point will always be plotted.
To reduce plotting time in transient cases, ANSYS Fluent has available
an option to skip plotting every particle
in an injection. Selecting this option is also done in the Particle Tracks Dialog Box by specifying a nonzero integer
in the Skip field. For example, if an individual
stream is selected and the skip option is set to 1, every other particle
will be plotted. If the entire injection is selected with a skip option
of 1, every other particle will be plotted for all streams in the
injection.
These options are controlled in exactly the same way that pathline-plotting options are controlled. See Options for Pathline Plots for details about setting the trajectory plotting options mentioned above.
Note that in addition to coloring the trajectories by continuous phase variables, you can also color them according to the following discrete phase variables: particle time, particle velocity, particle diameter, particle density, particle mass, particle temperature, particle law number, particle time step, and particle Reynolds number. If DEM Collisions is enabled in the Discrete Phase Model dialog box, you can also select the magnitude or components of the collisional force acting on the DEM parcel, total force acting on the DEM parcel, and total acceleration experienced by the particles in the parcel. These variables are included in the Particle Variables... category of the Color by list. To display the minimum and maximum values in the domain, click the button.
You can specify how you would like to filter the particles being displayed, by first enabling the Enable Filter option, then clicking the button. In the Particle Filter Attributes dialog box, select the field variable by which you want to filter, then specify whether you would like to display all the particle tracks Inside or Outside the Filter-Min and Filter-Max range, as shown in Figure 23.45: The Particle Filter Attributes Dialog Box.
Note: All particle variables as well as any field variable except for Custom Field Functions... can be used as a filter variable.
For axisymmetric problems in which the particle has a nonzero
circumferential velocity component, the trajectory of an individual
particle is often a spiral about the centerline of rotation. ANSYS Fluent displays
the and
components of the trajectory (but not the
component) projected
in the axisymmetric plane.