PDF
Turbulent Mixing of a Trace Species
Introduction
This tutorial demonstrates how mixing can be simulated in a stirred vessel by seeding a trace species from a point. The flow is modeled using the Rotating Machinery, Fluid Flow interface, which solves the Navier-Stokes equations on geometries with rotating parts such as impellers. The transport of the trace species is modeled using the Transport of Diluted Species interface.
Model Definition
Model Geometry
Figure 1 shows the model geometry, which is a schematic cross section of a tank with a four-blade impeller. The tank has four baffles attached to the wall to enhance mixing. The mixer blades and the impellers are approximated to be infinitely thin. The seeding of the trace species is done at the marked point.
The circle between the impeller and the tank wall is the assembly boundary where the mesh is allowed to slide when the impeller rotates.
Figure 1: Model geometry.
Domain Equation and Boundary Conditions
The mixer fluid is water, and a rotational speed of 20 rpm is prescribed for the impeller. This rotation is achieved by prescribing the inner domain to be a rotating domain. The boundary between the inner and the outer domain is prescribed to be a continuity boundary that transfers momentum to the fluid in the outer domain.
The Reynolds number based on the impeller radius and the impeller tip speed is approximately 1.9 × 106, which means that the flow is turbulent. The k–ε turbulence model is applied in this example.
There are two methods to reach operating conditions. One is to accelerate the impeller up to full speed and wait for the flow to reach a quasi steady-state. This approach is simple but can be time consuming. A computationally more efficient method is to first simulate the flow using the frozen rotor approach. Frozen rotor means that the impeller, or rotor, is frozen in position. The flow in the rotating domain is assumed to be stationary in terms of a rotating coordinate system. The effect of the rotation is then accounted for by Coriolis and centrifugal forces. This solution couples to the nonrotating parts where the flow is also assumed to be stationary, but in a nonrotating coordinate system. See the CFD Module User’s Guide for more information about frozen rotor.
The result of a frozen rotor simulation is an approximation to the flow at operating conditions. The result depends on the angular position of the impeller and cannot represent transient effects. It is still a very good starting condition to reach operating conditions. Quasi-steady state from a frozen rotor simulation is typically reached within a few revolutions, while starting from zero velocity requires tens of revolutions to reach operating conditions.
A trace species is a species introduced in very small quantities. It is often of a sharp color to be clearly visible even in small amounts. A trace species is not supposed to affect the flow, and hence, the flow can be solved for first and then the trace species transport solved for subsequently. Because it is the mixing at operating condition that is interesting, the trace species is introduced only once the flow is closed to fully developed, which it is after approximately six seconds starting from the frozen rotor simulation.
The seeding is modeled as a point source with normal distribution around the release time, t = 7.0 seconds. The absolute value of the pulse is arbitrary since the trace species does not affect the flow.
Results and Discussion
Figure 2 shows the frozen rotor velocity field. As expected, the highest velocity magnitude is found at the tip of the mixer blades. There are also clearly visible recirculation zones both before and behind the baffles.
Figure 2: The velocity field obtained from the frozen rotor simulation.
Figure 3 shows the velocity field at t = 30 s. The rotor position is the same as in Figure 2, and the results in the figures are similar. There are, however, differences. The most notably difference is the recirculation zones before the baffles that are smaller in Figure 3 than in Figure 2. The size and shape of the recirculation zones for the time-dependent simulation also vary with the position of the impeller.
Figure 3: A snapshot of the time-dependent velocity field at t=30 s.
Figure 4 shows four snapshots of the mixing process, time running from the upper-left to the lower-right picture. Since the velocity is rather slow at the seeding point (see also Figure 3), the initial transport is almost isotropic from the seeding point (t = 9 s). Some trace species is, however, entrained in the faster velocity field in the center of the mixer and becomes thereby spread in the azimuthal direction (t = 14.7 s). It only takes a few seconds more for the trace species to be almost homogeneous distributed in the mixer. The slowest spreading is to the regions in between the impeller blades. This is a well-known phenomenon and is the reason to why chemical substances are commonly added as close to the impeller axis as possible.
Figure 4: The mixing process. Surface plots of the trace species at t = 9, 14.7, 20.4 and 26.1 seconds.
Application Library path: CFD_Module/Single-Phase_Flow/turbulent_mixing
Modeling Instructions
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  2D.
2
In the Select Physics tree, select Fluid Flow>Single-Phase Flow>Rotating Machinery, Fluid Flow>Turbulent Flow>Turbulent Flow, k-ε.
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select Preset Studies for Selected Physics Interfaces>Frozen Rotor.
6
Click  Done.
Geometry 1
Circle 1 (c1)
1
In the Geometry toolbar, click  Circle.
2
In the Settings window for Circle, locate the Size and Shape section.
3
In the Radius text field, type 0.5.
Circle 2 (c2)
1
In the Geometry toolbar, click  Circle.
2
In the Settings window for Circle, locate the Size and Shape section.
3
In the Radius text field, type 0.35.
4
Click  Build Selected.
Difference 1 (dif1)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Difference.
2
In the Settings window for Difference, locate the Difference section.
3
Select the Keep input objects check box.
4
Select the object c1 only.
5
Find the Objects to subtract subsection. Select the  Activate Selection toggle button.
6
Select the object c2 only.
Delete Entities 1 (del1)
1
In the Model Builder window, right-click Geometry 1 and choose Delete Entities.
2
In the Settings window for Delete Entities, locate the Entities or Objects to Delete section.
3
From the Geometric entity level list, choose Object.
4
Select the object c1 only.
5
Click  Build Selected.
Line Segment 1 (ls1)
1
In the Geometry toolbar, click  More Primitives and choose Line Segment.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
From the Specify list, choose Coordinates.
4
Locate the Endpoint section. From the Specify list, choose Coordinates.
5
Locate the Starting Point section. In the x text field, type -0.5.
6
Locate the Endpoint section. In the x text field, type -0.4.
Rotate 1 (rot1)
1
In the Geometry toolbar, click  Transforms and choose Rotate.
2
Select the object ls1 only.
3
In the Settings window for Rotate, locate the Rotation section.
4
Click  Range.
5
In the Range dialog box, type 90 in the Start text field.
6
In the Step text field, type 90.
7
In the Stop text field, type 270.
8
Click Replace.
9
In the Settings window for Rotate, locate the Input section.
10
Select the Keep input objects check box.
Point 1 (pt1)
1
In the Geometry toolbar, click  Point.
2
In the Settings window for Point, locate the Point section.
3
In the x text field, type 0.3.
4
In the y text field, type 0.3.
Union 1 (uni1)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Union.
The final operation will later be set to Form an assembly. Union operations are therefore necessary to merge the domains and the lines.
2
Select the objects dif1, ls1, pt1, rot1(1), rot1(2), and rot1(3) only.
Line Segment 2 (ls2)
1
In the Geometry toolbar, click  More Primitives and choose Line Segment.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
From the Specify list, choose Coordinates.
4
Locate the Endpoint section. From the Specify list, choose Coordinates.
5
Locate the Starting Point section. In the x text field, type -0.25.
6
Locate the Endpoint section. In the x text field, type 0.25.
Line Segment 3 (ls3)
1
In the Geometry toolbar, click  More Primitives and choose Line Segment.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
From the Specify list, choose Coordinates.
4
Locate the Endpoint section. From the Specify list, choose Coordinates.
5
Locate the Starting Point section. In the y text field, type -0.25.
6
Locate the Endpoint section. In the y text field, type 0.25.
Union 2 (uni2)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Union.
2
Select the objects c2, ls2, and ls3 only.
Form Union (fin)
The boundary between the rotating and nonrotating domain must be an assembly boundary so that the parts can move relative to each other.
1
In the Model Builder window, under Component 1 (comp1)>Geometry 1 click Form Union (fin).
2
In the Settings window for Form Union/Assembly, locate the Form Union/Assembly section.
3
From the Action list, choose Form an assembly.
4
In the Geometry toolbar, click  Build All.
5
Click the  Zoom Extents button in the Graphics toolbar.
Add Material
1
In the Home toolbar, click  Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Built-in>Water, liquid.
4
Click Add to Component in the window toolbar.
5
In the Home toolbar, click  Add Material to close the Add Material window.
Definitions
Rotating Domain 1
1
In the Model Builder window, under Component 1 (comp1)>Definitions>Moving Mesh click Rotating Domain 1.
2
Select Domain 2 only.
3
In the Settings window for Rotating Domain, locate the Rotation section.
4
In the f text field, type -20[1/min].
Turbulent Flow, k-ε (spf)
Flow Continuity 1
1
In the Model Builder window, under Component 1 (comp1) right-click Turbulent Flow, k-ε (spf) and choose Pairs>Flow Continuity.
2
In the Settings window for Flow Continuity, locate the Pair Selection section.
3
Under Pairs, click  Add.
4
In the Add dialog box, select Identity Boundary Pair 1 (ap1) in the Pairs list.
5
Click OK.
Interior Wall 1
1
In the Physics toolbar, click  Boundaries and choose Interior Wall.
2
Select Boundaries 1–4 and 13–16 only.
Pressure Point Constraint 1
1
In the Physics toolbar, click  Points and choose Pressure Point Constraint.
2
Select Point 10 only.
The pressure level must be specified to obtain a unique solution since water is an incompressible liquid.
Mesh 1
1
In the Model Builder window, under Component 1 (comp1) click Mesh 1.
2
In the Settings window for Mesh, locate the Physics-Controlled Mesh section.
3
From the Element size list, choose Fine.
Study 1
Step 1: Frozen Rotor
In the Home toolbar, click  Compute.
Results
Velocity (spf)
Create Figure 2 using the following steps.
Streamline 1
1
Right-click Velocity (spf) and choose Streamline.
2
In the Settings window for Streamline, locate the Streamline Positioning section.
3
From the Positioning list, choose Uniform density.
4
In the Separating distance text field, type 0.02.
5
Locate the Coloring and Style section. Find the Point style subsection. From the Color list, choose White.
6
In the Velocity (spf) toolbar, click  Plot.
Add a Time Dependent study.
Add Study
1
In the Home toolbar, click  Add Study to open the Add Study window.
2
Go to the Add Study window.
3
Find the Studies subsection. In the Select Study tree, select General Studies>Time Dependent.
4
Click Add Study in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Study 2
Step 1: Time Dependent
It is important to specify frequent enough output times for the flow field. The subsequent species simulation might otherwise be affected by interpolation errors.
1
In the Settings window for Time Dependent, locate the Study Settings section.
2
In the Output times text field, type 0 range(6,0.15,30).
Start from the frozen rotor solution.
3
Click to expand the Values of Dependent Variables section. Find the Initial values of variables solved for subsection. From the Settings list, choose User controlled.
4
From the Method list, choose Solution.
5
From the Study list, choose Study 1, Frozen Rotor.
6
In the Home toolbar, click  Compute.
Results
Velocity (spf) 1
Recreate Figure 3 using the following steps.
Streamline 1
1
Right-click Velocity (spf) 1 and choose Streamline.
2
In the Settings window for Streamline, locate the Streamline Positioning section.
3
From the Positioning list, choose Uniform density.
4
In the Separating distance text field, type 0.02.
5
Locate the Coloring and Style section. Find the Point style subsection. From the Color list, choose White.
6
In the Velocity (spf) 1 toolbar, click  Plot.
Definitions
Gaussian Pulse 1 (gp1)
1
In the Home toolbar, click  Functions and choose Local>Gaussian Pulse.
2
In the Settings window for Gaussian Pulse, locate the Parameters section.
3
In the Location text field, type 7.
4
In the Standard deviation text field, type 0.25.
Add Physics
1
In the Home toolbar, click  Add Physics to open the Add Physics window.
2
Go to the Add Physics window.
3
In the tree, select Chemical Species Transport>Transport of Diluted Species (tds).
4
Find the Physics interfaces in study subsection. In the table, clear the Solve check boxes for Study 1 and Study 2.
5
Click Add to Component 1 in the window toolbar.
6
In the Home toolbar, click  Add Physics to close the Add Physics window.
Add Study
1
In the Home toolbar, click  Add Study to open the Add Study window.
2
Go to the Add Study window.
3
Find the Studies subsection. In the Select Study tree, select General Studies>Time Dependent.
4
Find the Physics interfaces in study subsection. In the table, clear the Solve check box for Turbulent Flow, k-ε (spf).
5
Click Add Study in the window toolbar.
6
In the Home toolbar, click  Add Study to close the Add Study window.
Transport of Diluted Species (tds)
Transport Properties 1
In the Model Builder window, under Component 1 (comp1)>Transport of Diluted Species (tds) click Transport Properties 1.
Turbulent Mixing 1
1
In the Physics toolbar, click  Attributes and choose Turbulent Mixing.
2
In the Settings window for Turbulent Mixing, locate the Turbulent Mixing Parameters section.
3
From the νT list, choose Turbulent kinematic viscosity (spf/fp1).
4
In the ScT text field, type 1.
Transport Properties 1
1
In the Model Builder window, click Transport Properties 1.
2
In the Settings window for Transport Properties, locate the Convection section.
3
From the u list, choose Velocity field (spf).
Continuity 1
1
In the Physics toolbar, click  Pairs and choose Continuity.
2
In the Settings window for Continuity, locate the Pair Selection section.
3
Under Pairs, click  Add.
4
In the Add dialog box, select Identity Boundary Pair 1 (ap1) in the Pairs list.
5
Click OK.
Thin Impermeable Barrier 1
1
In the Physics toolbar, click  Boundaries and choose Thin Impermeable Barrier.
2
Select Boundaries 1–4 and 13–16 only.
Line Mass Source 1
1
In the Physics toolbar, click  Points and choose Line Mass Source.
2
Select Point 10 only.
3
In the Species Source text field, type gp1(t[1/s])/10.
Study 3
Step 1: Time Dependent
1
In the Model Builder window, under Study 3 click Step 1: Time Dependent.
2
In the Settings window for Time Dependent, locate the Study Settings section.
3
In the Output times text field, type range(6,0.15,30).
4
Locate the Values of Dependent Variables section. Find the Values of variables not solved for subsection. From the Settings list, choose User controlled.
5
From the Method list, choose Solution.
6
From the Study list, choose Study 2, Time Dependent.
The Automatic Time setting would only use the last solution from Study 2. Change to All.
7
From the Time (s) list, choose All.
8
In the Home toolbar, click  Compute.
Results
Concentration (tds)
The following steps create an animation that contains the plots in Figure 4.
Plot the dataset edges on the spatial frame to make them follow the rotation.
1
In the Settings window for 2D Plot Group, locate the Plot Settings section.
2
From the Frame list, choose Spatial  (x, y, z).
Surface 1
1
In the Model Builder window, expand the Concentration (tds) node, then click Surface 1.
2
In the Settings window for Surface, click to expand the Range section.
3
Select the Manual color range check box.
4
In the Minimum text field, type 0.
5
In the Maximum text field, type 1.
Streamline 1
In the Model Builder window, right-click Streamline 1 and choose Disable.
Animation 1
1
In the Results toolbar, click  Animation and choose File.
2
In the Settings window for Animation, locate the Target section.
3
From the Target list, choose Player.
4
Locate the Scene section. From the Subject list, choose Concentration (tds).
Set the frames to be displayed for as long as the time between the saved solutions.
5
Locate the Playing section. In the Display each frame for text field, type 0.15.
6
Locate the Frames section. From the Frame selection list, choose All.
7
Right-click Animation 1 and choose Play.