PDF
Flow in an Airlift Loop Reactor
Introduction
This example illustrates multiphase flow modeling in an airlift loop reactor. Air bubbles are injected through two frits at the bottom of a water-filled reactor. Due to buoyancy, the bubbles rise, inducing a circulating motion in the liquid. There is no mass transfer between the phases.
Model Definition
The model parameters are taken from the experimental work presented in Ref. 1, and are summarized in Table 1. The liquid phase in the reactor is water while the gas phase is air.
Table 1: Model data.
Property
value
description
 H
1.75 m
Reactor height
 W
0.5 m
Reactor width
 T
0.08 m
Reactor thickness
 db
3·10-3 m
Bubble diameter
 R
0.02 m
Frit radius
 L
0.16 m
Width of riser and downcomer channels
 Vin
0.015 m/s
Superficial velocity at inlet
 Cw
5·104 kg/(m3·s)
Slip-velocity proportionality constant
 ρg,in
0.9727 kg/m3
Gas density at inlet
Boundary Conditions
Inlet Boundary Condition
Two frits with radius 0.02 m are located at the bottom of the reactor (see Figure 1). Air bubbles with a diameter of 3 mm and superficial speed of 0.015 m/s are injected through the frits. For the liquid, the frits are described by a wall condition.
Outlet Boundary Condition
The top of the geometry (xz-plane, y = 1.75 m) is a free surface. The surface motion is neglected and the surface is instead approximated by a slip condition for the liquid. The gas is free to exit the reactor through this boundary.
Symmetry Condition
Mirror symmetry is invoked in the xy-plane at z = 0.04 m.
Wall Condition
Other boundaries are represented by wall functions for the liquid, and with zero gas flux for the bubbles.
Figure 1: Model geometry for the airlift loop reactor.
Bubbly Flow interface and Turbulence Modeling
The Bubbly Flow interface sets up a multiphase-flow model for gas bubbles in a liquid. The physics interface tracks the averaged gas-phase concentration rather than each bubble in detail. It solves for the liquid velocity, the pressure, and the volume fraction of the gas phase. Details of the governing equations are presented in the theory section for the Bubbly Flow interfaces in the CFD Module User’s Guide.
For laminar flow the gas velocity ug is calculated from
where ul stands for the liquid-phase velocity, and uslip stands for the relative velocity between gas and liquid, the so-called slip velocity.
The slip velocity is calculated from a slip model. The Bubbly Flow interface provides several slip models. The most appropriate slip model for this reactor is a pressure-drag balance slip model with a drag coefficient tuned for large bubbles.
The experiments in Ref. 1 suggest that the Reynolds number for the fully developed flow is 2·104, and hence that the flow is turbulent. The k-ε turbulence model for bubbly flows is similar to the single-phase k-ε turbulence model (details can be found in the theory sections for the Turbulent Flow and Bubbly Flow interfaces in the CFD Module User’s Guide). However, for bubbly flow cases, additional source terms are added to the turbulence equations. These account for the extra production and dissipation of turbulence due to the relative motion between the gas bubbles and the liquid. The additional source term in the k equation, denoted Sk, accounts for the bubble-induced turbulence and is given by (see Ref. 2)
The additional source term in the ε-equation, denoted Sε, accounting for the bubble-induced turbulence dissipation, is given by
where Ck and Cε are model constants. The values of Ck and Cε are highly problem dependent but can often be tuned to obtain good agreement between experimental data and simulations (see Ref. 3). According to Ref. 2, admissible values for Ck and Cε are in the ranges of [0.01, 1] and [1, 1.92], respectively. Ref. 3 does however use Cε values less than 1 and they obtain good agreements between the measurements and simulations. In this example Ck and Cε are set to 0.6 and 1.4, respectively.
To account for turbulent transport of the bubbles, a drift velocity is added for the gas-phase velocity field:
where
and is the turbulent Schmidt number.
Using the k-ε model, the turbulent dynamic viscosity is defined as
where Cμ is a model constant (for details, see the theory section for the Bubbly Flow interfaces in the CFD Module User’s Guide).
In the Bubbly Flow interface you can easily switch the k-ε turbulence model. You can also control whether to include or exclude the bubble-induced turbulence term Sk by adjusting the value of Ck. A Ck equal to zero means that the bubble induced turbulence is neglected.
The Physical Model settings for the Bubbly Flow interface also provides a low gas concentration option which is active per default. This option is applicable if the gas concentration is less than 2%, in which case the transport equations can be simplified compared to cases with higher gas concentrations. Ref. 1 does not specifically report the gas concentration, but photographs of the reactor indicate that the gas concentration might be high, so the low gas concentration option is not enabled in this model.
Mesh Generation
The mesh must be very fine in the vicinity of the frits in order to resolve steep gradients in bubble concentration. The mesh also needs to be relatively fine in the interior of the reactor since the presence of bubbles creates relatively complicated flow structures.
Solving the Model
The goal is to obtain a stationary solution, but when it comes to buoyant flows, the best way to reach it is often a time-dependent simulation. Buoyant flows can feature intricate flow structures that are in a delicate balance with each other. It can sometimes be difficult to find such flow structures with a stationary solver while a time-dependent simulation lets the structures evolve to their final state.
Results and Discussion
Figure 2 shows the gas volume fraction and velocity streamlines for the liquid in the symmetry plane at t = 30 s. The results are qualitatively in good agreement with Ref. 1 except that the experiments show a recirculation zone at the upper-left corner while this recirculation zone is absent in the simulation.
The maximum value of the gas concentration is about 7% close to the two frits and higher than 2% in substantial parts of the reactor. This confirms that the low-gas concentration assumption would not have been valid.
Figure 2: Results of a time-dependent simulation at t = 30 s. The surface is the gas concentration, and the streamlines are liquid velocity.
Figure 3 shows the turbulent viscosity. The effect of bubble induced turbulence can be perceived by the relatively high levels of turbulent viscosity just above the frits and also beneath the free surface. The latter can be the reason to why there is no recirculation zone by the upper-left corner. But it could also be that the missing recirculation zone is caused by sloshing which has been neglected in this example.
Figure 3: Turbulent viscosity in the symmetry plane.
Experimental data is reported for four probe position, #3, #5, #7 and #9. They correspond to lines in the symmetry plane at different, constant heights, namely y = 300 mm, y = 650 mm, y = 1250 mm and y = 1650 mm respectively. The probes are positioned in the rising part of the reactor. Comparisons between simulation and experiments are shown in Figure 4. The agreement is good in the lower part of the reactor (positions #3 and #5) where both liquid and gas velocities from the simulation are in close quantitative agreement with their experimental counterparts. However, the agreement is less good in the upper part of the reactor due to the missing recirculation zone in the upper-left corner. The simulation results are still qualitatively correct at probe position #7, but the velocities are too low close to the inner wall. The lack of the recirculation zone is apparent at probe position #9 where the experiments show negative liquid velocities along the outer wall while the simulation shows positive liquid velocities.
The overall agreement must still be deemed good considering the many modeling assumptions used in this example.
Figure 4: Comparison between simulation results and experimental results for vertical velocities at four different probe positions.
References
1. S. Becker, A. Sokolichin, and G. Eigenberger, “Gas-liquid flow in bubble columns and loop reactors: Part II. Comparison of detailed experiments and flow simulations,” Chem. Eng. Sci., vol. 49, pp. 5747–5762, 1994.
2. D. Kuzmin and S. Turek, “Numerical simulation of turbulent bubbly flows,” Third Int. Symposium on Two-Phase Flow Modeling and Experiment, Pisa, pp  22–24, Sept. 2004.
3. A. Sokolichin, G. Eigenberger, and A. Lapin, “Simulation of Buoyancy Driven Bubbly Flow: Established Simplification and Open Questions,” Fluid Mechanics and Transport Phenomena, vol. 51, no. 1, pp. 24–45, 2004.
Application Library path: CFD_Module/Verification_Examples/airlift_loop_reactor
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  3D.
2
In the Select Physics tree, select Fluid Flow > Multiphase Flow > Bubbly Flow > Bubbly Flow, Turbulent Flow > Bubbly Flow, k-ε (bf).
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies > Time Dependent.
6
Click  Done.
Global Definitions
First, define some model parameters.
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
H
1.75[m]
1.75 m
Reactor height
W
0.5[m]
0.5 m
Reactor width
T
0.08[m]
0.08 m
Reactor thickness
d_b
3e-3[m]
0.003 m
Bubble diameter
R
0.02[m]
0.02 m
Frit radius
L
0.16[m]
0.16 m
Width of riser and downcomer channels
V_in
0.015[m/s]
0.015 m/s
Inlet velocity
Cw
5e4[kg/(m^3*s)]
50000 kg/(m³·s)
Slip-velocity proportionality constant
rhog_in
0.9727[kg/(m^3)]
0.9727 kg/m³
Gas density at inlet
Define a step function to be used when ramping up the inlet gas flux as a function of time.
Step 1 (step1)
1
In the Home toolbar, click  Functions and choose Global > Step.
2
In the Settings window for Step, locate the Parameters section.
3
In the Location text field, type 5.
4
Click to expand the Smoothing section. In the Size of transition zone text field, type 10.
5
Click  Plot.
Geometry 1
Create the geometry. To simplify this step, insert a prepared geometry sequence.
1
In the Geometry toolbar, click Insert Sequence and choose Insert Sequence.
2
Browse to the model’s Application Libraries folder and double-click the file airlift_loop_reactor_geom_sequence.mph.
Full geometry instructions can be found at the end of the document.
3
In the Geometry toolbar, click  Build All.
4
In the Model Builder window, under Component 1 (comp1) click Geometry 1.
5
Hold down the left mouse button and drag in the Graphics window to rotate the geometry. Similarly, use the right mouse button to translate the geometry and the middle button to zoom.
Now pick up the materials from the Material Library.
Add Material
1
In the Materials toolbar, click  Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Built-in > Air.
4
Click the Add to Component button in the window toolbar.
5
In the tree, select Built-in > Water, liquid.
6
Click the Add to Component button in the window toolbar.
7
In the Materials toolbar, click  Add Material to close the Add Material window.
Bubbly Flow, k-ε (bf)
Fluid Properties 1
1
In the Settings window for Fluid Properties, locate the Materials section.
2
From the Liquid list, choose Water, liquid (mat2).
3
From the Gas list, choose Air (mat1).
4
Locate the Gas Properties section. From the ρg list, choose Calculate from ideal gas law.
5
In the db text field, type d_b.
6
Locate the Slip Model section. From the Slip model list, choose Pressure-drag balance.
7
From the Drag coefficient model list, choose Large bubbles.
8
In the Model Builder window, click Bubbly Flow, k-ε (bf).
9
In the Settings window for Bubbly Flow, k-ε, locate the Physical Model section.
10
Clear the Low gas concentration checkbox.
11
Locate the Turbulence section. Find the Turbulence model parameters subsection. Select the Edit turbulence model parameters checkbox.
12
In the Cε text field, type 1.4.
13
In the Ck text field, type 0.6.
Gravity 1
1
In the Physics toolbar, click  Domains and choose Gravity.
2
Select Domain 1 only.
Wall 2
In the Physics toolbar, click  Boundaries and choose Wall.
Gravity 1
1
In the Model Builder window, click Gravity 1.
2
In the Settings window for Gravity, locate the Gravity section.
3
Specify the g vector as
0
x
-g_const
y
0
z
Wall 2
1
Click the  Zoom Extents button in the Graphics toolbar.
2
In the Model Builder window, click Wall 2.
3
Select Boundaries 6 and 7 only.
4
In the Settings window for Wall, locate the Gas Boundary Condition section.
5
From the Gas boundary condition list, choose Gas flux.
6
In the Nρgϕg text field, type V_in*rhog_in*step1(t[1/s]).
Wall 3
1
In the Physics toolbar, click  Boundaries and choose Wall.
2
Select Boundary 5 only.
3
In the Settings window for Wall, locate the Liquid Boundary Condition section.
4
From the Liquid boundary condition list, choose Slip.
5
Locate the Gas Boundary Condition section. From the Gas boundary condition list, choose Gas outlet.
Initial Values 1
When using gravity it is important to set the initial values of the pressure to hydrostatic conditions.
1
In the Model Builder window, click Initial Values 1.
2
In the Settings window for Initial Values, type g_const*bf.rhol*(1.75-y) in the p text field.
Pressure Point Constraint 1
1
In the Physics toolbar, click  Points and choose Pressure Point Constraint.
2
Select Point 23 only.
Symmetry 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry.
2
Select Boundary 4 only.
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 Coarse.
4
Right-click Component 1 (comp1) > Mesh 1 and choose Edit Physics-Induced Sequence.
Boundary Layer Properties 1
1
In the Model Builder window, expand the Component 1 (comp1) > Mesh 1 > Boundary Layers 1 node, then click Boundary Layer Properties 1.
2
In the Settings window for Boundary Layer Properties, locate the Layers section.
3
In the Number of layers text field, type 4.
4
In the Thickness adjustment factor text field, type 3.
5
Click  Build All.
6
Click the  Zoom Extents button in the Graphics toolbar.
Study 1
Step 1: Time Dependent
1
In the Model Builder window, under Study 1 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(0,0.05,1)*30.
4
From the Tolerance list, choose User controlled.
5
In the Relative tolerance text field, type 0.005.
Measurement data makes it possible to estimate manual scales for velocity and pressure.
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 1 (sol1) node.
3
In the Model Builder window, expand the Study 1 > Solver Configurations > Solution 1 (sol1) > Dependent Variables 1 node, then click Pressure (comp1.p).
4
In the Settings window for Field, locate the Scaling section.
5
From the Method list, choose Manual.
6
In the Scale text field, type 1.7e4.
7
In the Model Builder window, under Study 1 > Solver Configurations > Solution 1 (sol1) > Dependent Variables 1 click Velocity Field, Liquid Phase (comp1.u).
8
In the Settings window for Field, locate the Scaling section.
9
From the Method list, choose Manual.
10
In the Scale text field, type 0.5.
11
In the Model Builder window, collapse the Solution 1 (sol1) node.
12
In the Model Builder window, right-click Solution 1 (sol1) and choose Run.
Results
The following steps reproduce Figure 2.
Surface 1
1
In the Results toolbar, click  More Datasets and choose Surface.
2
Select Boundary 4 only.
3
In the Settings window for Surface, locate the Parameterization section.
4
From the x- and y-axes list, choose xy-plane.
2D Plot Group 5
In the Results toolbar, click  2D Plot Group.
Surface 1
Right-click 2D Plot Group 5 and choose Surface.
Streamline 1
1
In the Model Builder window, right-click 2D Plot Group 5 and choose Streamline.
2
In the Settings window for Streamline, locate the Coloring and Style section.
3
Find the Point style subsection. From the Color list, choose White.
4
Locate the Streamline Positioning section. From the Positioning list, choose Uniform density.
5
In the Density level text field, type 9.7.
6
In the 2D Plot Group 5 toolbar, click  Plot.
The following steps reproduce Figure 3.
2D Plot Group 6
In the Results toolbar, click  2D Plot Group.
Surface 1
1
Right-click 2D Plot Group 6 and choose Surface.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type bf.muT.
4
In the 2D Plot Group 6 toolbar, click  Plot.
Proceed to reproduce the 1D-plots in Figure 4. Start by importing experimental data.
vl3
1
In the Results toolbar, click  Table.
2
In the Settings window for Table, type vl3 in the Label text field.
3
Locate the Data section. Click  Import.
4
Browse to the model’s Application Libraries folder and double-click the file airlift_loop_reactor_vl_no3.txt.
vg3
1
In the Results toolbar, click  Table.
2
In the Settings window for Table, type vg3 in the Label text field.
3
Locate the Data section. Click  Import.
4
Browse to the model’s Application Libraries folder and double-click the file airlift_loop_reactor_vg_no3.txt.
vl5
1
In the Results toolbar, click  Table.
2
In the Settings window for Table, type vl5 in the Label text field.
3
Locate the Data section. Click  Import.
4
Browse to the model’s Application Libraries folder and double-click the file airlift_loop_reactor_vl_no5.txt.
vg5
1
In the Results toolbar, click  Table.
2
In the Settings window for Table, type vg5 in the Label text field.
3
Locate the Data section. Click  Import.
4
Browse to the model’s Application Libraries folder and double-click the file airlift_loop_reactor_vg_no5.txt.
vl7
1
In the Results toolbar, click  Table.
2
In the Settings window for Table, type vl7 in the Label text field.
3
Locate the Data section. Click  Import.
4
Browse to the model’s Application Libraries folder and double-click the file airlift_loop_reactor_vl_no7.txt.
vg7
1
In the Results toolbar, click  Table.
2
In the Settings window for Table, type vg7 in the Label text field.
3
Locate the Data section. Click  Import.
4
Browse to the model’s Application Libraries folder and double-click the file airlift_loop_reactor_vg_no7.txt.
vl9
1
In the Results toolbar, click  Table.
2
In the Settings window for Table, type vl9 in the Label text field.
3
Locate the Data section. Click  Import.
4
Browse to the model’s Application Libraries folder and double-click the file airlift_loop_reactor_vl_no9.txt.
vg9
1
In the Results toolbar, click  Table.
2
In the Settings window for Table, type vg9 in the Label text field.
3
Locate the Data section. Click  Import.
4
Browse to the model’s Application Libraries folder and double-click the file airlift_loop_reactor_vg_no9.txt.
Define cut lines that correspond to the experimental probe positions.
No3
1
In the Results toolbar, click  Cut Line 3D.
2
In the Settings window for Cut Line 3D, type No3 in the Label text field.
3
Locate the Line Data section. In row Point 1, set y to 0.3 and z to 0.04.
4
In row Point 2, set x to 0.15, y to 0.3, and z to 0.04.
5
From the Snapping list, choose Snap to closest boundary.
No5
1
Right-click No3 and choose Duplicate.
2
In the Settings window for Cut Line 3D, type No5 in the Label text field.
3
Locate the Line Data section. In row Point 1, set y to 0.65.
4
In row Point 2, set y to 0.65.
No7
1
Right-click No5 and choose Duplicate.
2
In the Settings window for Cut Line 3D, type No7 in the Label text field.
3
Locate the Line Data section. In row Point 1, set y to 1.25.
4
In row Point 2, set y to 1.25.
No9
1
Right-click No7 and choose Duplicate.
2
In the Settings window for Cut Line 3D, type No9 in the Label text field.
3
Locate the Line Data section. In row Point 1, set y to 1.65.
4
In row Point 2, set y to 1.65.
Probe position #3
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Probe position #3 in the Label text field.
3
Locate the Data section. From the Dataset list, choose No3.
4
From the Time selection list, choose Last.
5
Click to expand the Title section. From the Title type list, choose Manual.
6
In the Title text area, type Vertical liquid and gas velocities at probe position #3.
Line Graph 1
1
Right-click Probe position #3 and choose Line Graph.
2
In the Settings window for Line Graph, locate the y-Axis Data section.
3
In the Expression text field, type v.
4
Click to expand the Coloring and Style section. From the Color list, choose Blue.
5
Click to expand the Legends section. Select the Show legends checkbox.
6
From the Legends list, choose Manual.
7
In the table, enter the following settings:
Legends
Fluid velocity, simulation
Table Graph 1
1
In the Model Builder window, right-click Probe position #3 and choose Table Graph.
2
In the Settings window for Table Graph, locate the Coloring and Style section.
3
Find the Line style subsection. From the Line list, choose None.
4
From the Color list, choose Blue.
5
Find the Line markers subsection. From the Marker list, choose Diamond.
6
Click to expand the Legends section. Select the Show legends checkbox.
7
From the Legends list, choose Manual.
8
In the table, enter the following settings:
Legends
Fluid velocity, experiments
Line Graph 2
1
Right-click Probe position #3 and choose Line Graph.
2
In the Settings window for Line Graph, locate the y-Axis Data section.
3
In the Expression text field, type bf.ugy.
4
Locate the Coloring and Style section. From the Color list, choose Red.
5
Locate the Legends section. Select the Show legends checkbox.
6
From the Legends list, choose Manual.
7
In the table, enter the following settings:
Legends
Gas velocity, simulation
Table Graph 2
1
Right-click Probe position #3 and choose Table Graph.
2
In the Settings window for Table Graph, locate the Data section.
3
From the Table list, choose vg3.
4
Locate the Coloring and Style section. Find the Line style subsection. From the Line list, choose None.
5
From the Color list, choose Red.
6
Find the Line markers subsection. From the Marker list, choose Square.
7
Locate the Legends section. Select the Show legends checkbox.
8
From the Legends list, choose Manual.
9
In the table, enter the following settings:
Legends
Gas velocity, experiments
Probe position #3
1
In the Model Builder window, click Probe position #3.
2
In the Settings window for 1D Plot Group, locate the Axis section.
3
Select the Manual axis limits checkbox.
4
In the x minimum text field, type 0.
5
In the x maximum text field, type 0.15.
6
In the y minimum text field, type -0.15.
7
In the y maximum text field, type 0.85.
8
In the Probe position #3 toolbar, click  Plot.
Probe position #3.1
Right-click Probe position #3 and choose Duplicate.
Probe position #3
In the Model Builder window, collapse the Results > Probe position #3 node.
Probe position #5
1
In the Model Builder window, under Results click Probe position #3.1.
2
In the Settings window for 1D Plot Group, type Probe position #5 in the Label text field.
3
Locate the Data section. From the Dataset list, choose No5.
4
Locate the Title section. In the Title text area, type Vertical liquid and gas velocities at probe position #5.
Table Graph 1
1
In the Model Builder window, expand the Probe position #5 node, then click Table Graph 1.
2
In the Settings window for Table Graph, locate the Data section.
3
From the Table list, choose vl5.
Table Graph 2
1
In the Model Builder window, click Table Graph 2.
2
In the Settings window for Table Graph, locate the Data section.
3
From the Table list, choose vg5.
4
In the Probe position #5 toolbar, click  Plot.
Probe position #5
1
In the Model Builder window, click Probe position #5.
2
Click  Plot.
Probe position #5.1
Right-click Probe position #5 and choose Duplicate.
Probe position #5
In the Model Builder window, collapse the Results > Probe position #5 node.
Probe position #7
1
In the Model Builder window, under Results click Probe position #5.1.
2
In the Settings window for 1D Plot Group, type Probe position #7 in the Label text field.
3
Locate the Data section. From the Dataset list, choose No7.
4
Locate the Title section. In the Title text area, type Vertical liquid and gas velocities at probe position #7.
Table Graph 1
1
In the Model Builder window, expand the Probe position #7 node, then click Table Graph 1.
2
In the Settings window for Table Graph, locate the Data section.
3
From the Table list, choose vl7.
Table Graph 2
1
In the Model Builder window, click Table Graph 2.
2
In the Settings window for Table Graph, locate the Data section.
3
From the Table list, choose vg7.
Probe position #7
1
In the Model Builder window, click Probe position #7.
2
In the Probe position #7 toolbar, click  Plot.
Probe position #7.1
Right-click Probe position #7 and choose Duplicate.
Probe position #7
In the Model Builder window, collapse the Results > Probe position #7 node.
Probe position #9
1
In the Model Builder window, under Results click Probe position #7.1.
2
In the Settings window for 1D Plot Group, type Probe position #9 in the Label text field.
3
Locate the Data section. From the Dataset list, choose No9.
4
Locate the Title section. In the Title text area, type Vertical liquid and gas velocities at probe position #9.
Table Graph 1
1
In the Model Builder window, expand the Probe position #9 node, then click Table Graph 1.
2
In the Settings window for Table Graph, locate the Data section.
3
From the Table list, choose vl9.
Table Graph 2
1
In the Model Builder window, click Table Graph 2.
2
In the Settings window for Table Graph, locate the Data section.
3
From the Table list, choose vg9.
Probe position #9
1
In the Model Builder window, click Probe position #9.
2
In the Probe position #9 toolbar, click  Plot.
3
In the Model Builder window, collapse the Probe position #9 node.
Appendix. Geometry 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  3D.
2
Click  Done.
Global Definitions
First, define some model parameters.
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
H
1.75[m]
1.75 m
Reactor height
W
0.5[m]
0.5 m
Reactor width
T
0.08[m]
0.08 m
Reactor thickness
d_b
3e-3[m]
0.003 m
Bubble diameter
R
0.02[m]
0.02 m
Frit radius
L
0.16[m]
0.16 m
Width of riser and downcomer channels
V_in
0.015[m/s]
0.015 m/s
Inlet velocity
Cw
5e4[kg/(m^3*s)]
50000 kg/(m³·s)
Slip-velocity proportionality constant
rhog_in
0.9727[kg/(m^3)]
0.9727 kg/m³
Gas density at inlet
Geometry 1
Work Plane 1 (wp1)
1
In the Geometry toolbar, click  Work Plane.
2
In the Settings window for Work Plane, click  Go to Plane Geometry.
Work Plane 1 (wp1) > Plane Geometry
In the Model Builder window, click Plane Geometry.
Work Plane 1 (wp1) > Polygon 1 (pol1)
1
In the Work Plane toolbar, click  Polygon.
2
In the Settings window for Polygon, locate the Coordinates section.
3
In the table, enter the following settings:
xw (m)
yw (m)
0
0
L
0
W
L
W
H
0
H
4
In the Work Plane toolbar, click  Build All.
Work Plane 1 (wp1) > Polygon 2 (pol2)
1
In the Work Plane toolbar, click  Polygon.
2
In the Settings window for Polygon, locate the Coordinates section.
3
In the table, enter the following settings:
xw (m)
yw (m)
L
0.11
0.34
0.2
0.34
1.47
L
1.56
4
In the Work Plane toolbar, click  Build All.
Work Plane 1 (wp1) > Difference 1 (dif1)
1
In the Work Plane toolbar, click  Booleans and Partitions and choose Difference.
2
Select the object pol1 only.
3
In the Settings window for Difference, locate the Difference section.
4
Click to select the  Activate Selection toggle button for Objects to subtract.
5
Select the object pol2 only.
6
In the Work Plane toolbar, click  Build All.
Extrude 1 (ext1)
1
In the Model Builder window, under Component 1 (comp1) > Geometry 1 right-click Work Plane 1 (wp1) and choose Extrude.
2
In the Settings window for Extrude, locate the Distances section.
3
In the table, enter the following settings:
Distances (m)
T
4
Click  Build All Objects.
Work Plane 2 (wp2)
1
In the Geometry toolbar, click  Work Plane.
2
In the Settings window for Work Plane, locate the Plane Definition section.
3
From the Plane list, choose zx-plane.
4
Click  Go to Plane Geometry.
Work Plane 2 (wp2) > Circle 1 (c1)
1
In the Work Plane toolbar, click  Circle.
2
In the Settings window for Circle, locate the Size and Shape section.
3
In the Radius text field, type R.
4
Locate the Position section. In the xw text field, type T/2.
5
In the yw text field, type 0.11.
Work Plane 2 (wp2) > Circle 2 (c2)
1
In the Work Plane toolbar, click  Circle.
2
In the Settings window for Circle, locate the Size and Shape section.
3
In the Radius text field, type R.
4
Locate the Position section. In the xw text field, type T/2.
5
In the yw text field, type T/2.
6
In the Work Plane toolbar, click  Build All.
Union 1 (uni1)
1
In the Model Builder window, right-click Geometry 1 and choose Booleans and Partitions > Union.
2
Click in the Graphics window and then press Ctrl+A to select both objects.
3
In the Settings window for Union, click  Build All Objects.
Block 1 (blk1)
1
In the Geometry toolbar, click  Block.
2
In the Settings window for Block, locate the Size and Shape section.
3
In the Depth text field, type 2.
4
Locate the Position section. In the z text field, type T/2.
5
Click  Build All Objects.
6
Click the  Zoom Extents button in the Graphics toolbar.
Difference 1 (dif1)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Difference.
2
Select the object uni1 only, to add it to the Objects to add list.
3
In the Settings window for Difference, locate the Difference section.
4
Click to select the  Activate Selection toggle button for Objects to subtract.
5
Select the object blk1 only.
6
In the Geometry toolbar, click  Build All.
7
Click the  Zoom Extents button in the Graphics toolbar.