Using Streamlines and Streaklines to Identify Recirculation Zones
One of the benefits of flow simulation is that it provides an enormous amount of detailed information about the flow but at the same time, the amount of information can be challenging to digest. Recirculation regions in the flow field are of particular interest in many applications since their presence can have a significant impact. For example, a recirculation zone upstream of a power plant intake can reduce the efficiency of the turbines by a few percent, resulting in millions of dollars in lost revenue. In casting processes, a recirculation zone may trap oxides inside of the casting rather than allow the oxides to flow to the overflows where they won’t impact the quality of the casting.
In this article, two FLOW-3D flow field analysis tools—streamlines and streaklines—will be discussed. To demonstrate these tools, a simulation of flow into a power plant intake, shown above, will be analyzed. Ideally, the flow would enter the intake without significant rotational motion, since this can induce an air core in the intake reducing turbine efficiency. Streamlines and streaklines will be used to identify the flow structure near the inlet.
Streamlines represent lines in the flow which are tangent to the instantaneous velocity field. A streamline is generated by defining a starting point, commonly referred to as a seed point, and then integrating a line through the flow field which is tangent to the velocity field at that instant in time. If the flow field is steady, a streamline is a good indicator of flow characteristics such as recirculation zones. If the flow is highly unsteady (e.g., a filling simulation), streamlines provide more of an approximate location of flow features since the flow field is actually changing in time as the streamline moves through the flow field.
Generating Streamline Seeds
Streamlines seeds can be easily generated interactively in FLOW-3D Version 9.4. Open the simulation results file on the Analyze tab and then select the 3D tab. In the Options dropdown list, select “Activate Plain Streamline Seeding.” Then click Render. The view will change to the Display tab and the flow field will be displayed with a seed plane shown in green. Select the orientation and location of the plane on which streamline seed points will be defined using the Streamline Edit dialog box. In this case, the flow enters from the Y-max boundary so the seeding plane should be located there. Select the radio button next to the Y-direction slider and move the slider to the right.
Creating Seed Points
To create the seed points on the seed plane, rotate and zoom the image so that the plane is clearly visible, hold the Shift key, and then click on the plane where you would like the streamlines to start from. In this case, the flow nearest to the inlet will be most likely to be pulled into the inlet so the seed points will be located on a vertical line just inside the channel.
Click Render on the Streamline Edit dialog to generate the streamlines.
The streamlines clearly indicate that the flow exhibits a strong rotation once it enters the intake box and turbine performance will likely be hampered.
Streaklines are also called dye lines since they can be generated by releasing dye in the flow at a particular location. A snapshot of the dye trace at some point in time represents a streakline. The advantage of a streakline over a streamline is that a streakline is more meaningful in unsteady flows since the motion of the flow is tracked continuously in time.
Streaklines can be generated in FLOW-3D using tracer particles released at regular intervals from point sources. Tracer particles are massless particles which can be used to represent dye released in the flow. They move with the flow and do not change the flow patterns. In order to give the illusion of a continuous line, the tracer particles must be released at a sufficiently high rate so that the distance between them is almost unnoticeable.
Whereas streamlines can be computed after the simulation has completed, streaklines must be generated before the simulation has been run. Therefore, the release points for the tracer particles and release rates must be defined in the simulation setup. The first step will be to define particle sources and then define the rate of release for each source.
Defining Particle Sources
To define a particle source, select the Model Setup/Physics tab. Click the Particles button to display the Particles dialog.
Click the Add Source button to display the Particles dialog. For comparison purposes, the locations of the particle sources will be defined roughly at the same locations as the seed locations for the streamlines defined previously. The only other parameter which needs to be defined for the particle sources is the rate. The rate needs to be defined so that the particles are close enough together so that they appear continuous. A rule of thumb is that roughly 5 particles in each computational cell will achieve this.
Determing Particle Generation Rate
In order to determine a particle generation rate which distributes 5 particles per computation cell, a representative velocity needs to be determined. In this simulation, the velocity of water in the channel is 1 m/s and the computational cells are 0.05 m. The particle spacing should then be:
Particle spacing = 5 particles/0.05m = 100 particles/m
The particle generation rate is then:
Particle generation rate = Particle spacing/flow velocity = (100 particles/m)/1.0m/s = 100 particles/s
The same rate is applied to all particle sources. By default, particles will be generated at random times resulting in irregular gaps in the streaklines. Select the “Regularized in Time at Sources” radio button under Initialization to create uniform streaklines.
After the simulation has completed, the particles are displayed on the Analyze/3D tab by selecting Add Plain Particles under the Options dropdown. The particle display at 10.0 seconds is shown below.
In the image above, notice how the particles form well-defined streaklines initially but become much less defined as the flow approaches the inlet. A closer examination of the velocity near the inlet indicates that the velocity is about 2.0 m/s so the particle release rate should be double the original estimate. However, the flow near the inlet is highly turbulent so the particle release rate would need to be increased significantly to produce a continuous line. Nevertheless, the streaklines clearly indicate the rotational nature of the flow in the inlet.
The maximum number of particles in a simulation is set on the Particles dialog and defaults to 10000. If this maximum is exceeded during the simulation, new particles cannot enter the simulation until particles leave the simulation. An alternative to this is to set the maximum number of particles higher but it can be difficult to know how large to set it due to the unsteady nature of the flow.
Streamlines are convenient for identifying flow structures since they can be generated after the simulation has been completed. However they may not give the most accurate indication of the flow path since they are computed assuming the flow field is steady. Particles sources can be used to generate streaklines if particles are released rapidly enough to produce a solid line.