COMSOL 6.4 - Turbulent Mixing in a Stirred Tank

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. The trace species is added when the mixer is running in steady operation. The mixing time is evaluated by comparing the concentration in a measurement point to the average concentration in the vessel.

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 seeding point. The tank also contains a measurement point, close to the wall, where the concentration can be probed.

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. Here, to make sure that the correct operating conditions are reached, a time dependent simulations is ran starting from the frozen rotor solution. The average flow quantities are inspected in order to determine when a quasi-steady state is reached.

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. The seeding is performed by injection at the seeding point during one second. Then the mixing in the vessel is simulated for 40 revolutions. The degree of mixing is evaluated by comparing the averaged concentration to the concentration measured near the wall behind one of the baffles.

For the mixing stage, the flow field and the resulting turbulent diffusion during the last revolution of the flow simulation is reused repeatedly. This reduces the computational effort substantially.

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 3 shows the velocity field at the end of the fluid flow simulation (at t = 30 s, corresponding to 10 revolutions). The rotor position is the same as in Figure 2, and the results in the figures are similar. There are, however, differences. The most notable difference is that the recirculation zones before the baffles 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 2: The velocity field obtained from the frozen rotor simulation.

Figure 3: A snapshot of the time-dependent velocity field at t=30 s.

The average velocity and the average turbulent dynamic viscosity are plotted in Figure 4 to visualize the flow field development over time. The variables are normalized using the results from the frozen rotor solution. It can be noted that there is a drift over the first couple of rotations, but the magnitude of the variations is small. The frequency with which the impeller blades are passing the baffles is clearly seen in the velocity variations. The flow is noted to have reached a cyclic steady state after around seven revolutions. This implies that the last revolution of the simulation can confidently be used repeatedly for the mixing simulation.

Figure 4: Flow development starting from the frozen rotor solution. The average velocity and average turbulent diffusion normalized by the respective initial values are shown.

Figure 5 shows four snapshots of the mixing process, with the 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 around the seeding point (t = 2 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 = 8 s). The slowest spreading is to the regions behind the left baffle, close to the measuring point, as well as behind the top baffle. Species in the space between the impeller blades is mixed poorly with species in the outer region. This is a well-known phenomenon and is the reason why chemical substances are commonly added as close to the impeller axis as possible.

Figure 5: The mixing process. Surface plots of the trace species, normalized by the average concentration, at t = 2, 8, 18 and 38 seconds.

The mixing development can be evaluated in Figure 5 where the concentration at the measurement position and the average concentration are plotted. As was noted in the previous figure it takes a number of rotations of the impeller before the species is spread to the measurement position. After about 14 rotations the concentration behind the baffle surpasses the averaged concentrations, and after around 30 rotations the average concentration has been reached.

Figure 6: Concentration development during mixing. Comparing the average concentration in the tank to the one in the measurement point.

Chemical_Reaction_Engineering_Module/Mixing_and_Separation/turbulent_mixing

Modeling Instructions

From the menu, choose .

New

In the window, click

Model Wizard

In the window, click

In the tree, select > > > > ε.

Click .

Click

In the tree, select > .

Click

Global Definitions

Import some model parameters from a text file.

Parameters 1

In the window, under click .

In the window for , locate the section.

Click

Browse to the model’s Application Libraries folder and double-click the file turbulent_mixing_parameters.txt.

Geometry 1

Circle 1 (c1)

In the toolbar, click

In the window for , locate the section.

In the text field, type tank_R.

Circle 2 (c2)

In the toolbar, click

In the window for , locate the section.

In the text field, type 0.7*tank_R.

Click

Difference 1 (dif1)

In the toolbar, click

and choose .

In the window for , locate the section.

Select the checkbox.

Select the object only.

Click to select the

toggle button for .

Select the object only.

Line Segment 1 (ls1)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

Locate the section. In the text field, type -tank_R.

Locate the section. In the text field, type -tank_R+baffle_L.

Rotate 1 (rot1)

In the toolbar, click

and choose .

Select the object only.

In the window for , locate the section.

Click

In the dialog, type 90 in the text field.

In the text field, type 90.

In the text field, type 270.

Click .

In the window for , locate the section.

Select the checkbox.

Point 1 (pt1)

In the toolbar, click

In the window for , locate the section.

In the text field, type inject_x.

In the text field, type inject_y.

Click

Point 2 (pt2)

In the toolbar, click

In the window for , locate the section.

In the text field, type -tank_R*0.97.

Click

Rotate 2 (rot2)

In the toolbar, click

and choose .

Select the object only.

In the window for , locate the section.

In the text field, type -10.

Click

Union 1 (uni1)

In the toolbar, click

and choose .

The final operation will later be set to . Union operations are therefore necessary to merge the domains and the lines.

Select the objects , , , , , , and only.

Line Segment 2 (ls2)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

Locate the section. In the text field, type -0.25.

Locate the section. In the text field, type 0.25.

Line Segment 3 (ls3)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

Locate the section. In the text field, type -0.25.

Locate the section. In the text field, type 0.25.

Union 2 (uni2)

In the toolbar, click

and choose .

Select the objects , , and only.

Form Union (fin)

The boundary between the rotating and nonrotating domains must be an assembly boundary so that the parts can move relative to each other.

In the window, under > click .

In the window for , locate the section.

From the list, choose .

In the toolbar, click

Click the

button in the toolbar.

Create a selection for the interior boundaries representing the impeller and baffles.

Definitions

Impeller and Baffles

In the toolbar, click

In the window for , locate the section.

From the list, choose .

Select Boundaries 1–4 and 13–16 only.

In the text field, type Impeller and Baffles.

Create an average operator to be used for computing average quantities in the tank.

Average 1 (aveop1)

In the toolbar, click

and choose .

In the window for , type tankAv in the text field.

Locate the section. From the list, choose .

Add Material

In the toolbar, click

to open the window.

Go to the window.

In the tree, select > .

Click the button in the window toolbar.

In the toolbar, click

to close the window.

Moving Mesh

Rotating Domain 1

Select Domain 2 only.

In the window for , locate the section.

In the f text field, type -rpm.

Turbulent Flow, k-ε (spf)

Interior Wall 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Pressure Point Constraint 1

In the toolbar, click

and choose .

Select Point 10 only.

The pressure level must be specified to obtain a unique solution since water is an incompressible liquid.

Hide the internal boundaries between the moving and the stationary part of the geometry. First copy the boundary selection from the continuity feature.

Flow Continuity 1

In the window, click .

In the window for , click to expand the section.

Click

Definitions

Hide for Physics 1

In the window, right-click and choose .

In the window for , locate the section.

From the list, choose .

Click

In the dialog, Press CTRL+V to paste the copied boundary selection.

click .

Mesh 1

In the window, under click .

In the window for , locate the section.

From the list, choose .

Right-click > and choose .

Size 1

In the window, right-click and choose .

In the window for , locate the section.

From the list, choose .

Select Point 11 only.

Locate the section. Click the button.

Locate the section.

Select the checkbox. In the associated text field, type 3e-3.

Click

Study 1

Step 1: Frozen Rotor

In the toolbar, click

Results

Velocity (spf)

Create Figure 2 using the following steps.

Streamline 1

Right-click and choose .

In the window for , locate the section.

From the list, choose .

In the text field, type 9.

Locate the section. Find the subsection. From the list, choose .

In the toolbar, click

Add a study.

Pressure (spf), Velocity (spf), Wall Resolution (spf)

In the window, under , Ctrl-click to select , , and .

Right-click and choose .

Fluid Flow, Frozen Rotor

In the window for , type Fluid Flow, Frozen Rotor in the text field.

Definitions

Variables 1

In the window, under right-click and choose .

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Unit	Description
U0	withsol('sol1',tankAv(spf.U))	m/s	Average velocity, frozen rotor
muT0	withsol('sol1',tankAv(spf.muT))	Pa·s	Average turbulent dynamic viscosity, frozen rotor