PDF
Modular Mixer
Introduction
This model uses the Part Libraries to build a variety of mixers by combining two common types of vessels with two types of impellers. The mixers are baffled flat and dished bottom vessels with either pitched blade impellers or Rushton turbines. By changing the parameters in the model, you can modify the geometry to fit your applications. In case your mixer components cannot be built from the Geometry sequences available in the Part Libraries, you can add your own ones. The model includes three examples using the Rotating Machinery, Fluid Flow branch with the frozen-rotor study type. The first example solves a laminar mixing problem in a flat bottom mixer with a Rushton turbine. The second and third examples solve for turbulent mixing in a dished bottom mixer with a pitched blade impeller using the k-ε and k-ω turbulence models.
Model Definition
A typical mixer principally consists of two physical components — a vessel with or without baffles and an impeller structure. Baffles are used to suppress the main vortex formation in the bulk and thereby improve the mixing. The radial baffles, consisting of flat vertical solid strips set radially along the vessel wall, are evenly distributed around the perimeter of the vessel wall. Figure 1 shows the two combinations of vessels and impellers used in the simulations.
Figure 1: A baffled flat bottom mixer with a Rushton turbine (left) and a baffled dished bottom mixer with a pitched four blade impeller (right).
The Part Libraries contain geometry subsequences for building the mixer components shown in the figure. The types of components and their respective properties can be specified and varied by changing their parameters. The vessel used for mixers and reactors typically consists of a vertical cylinder with a dish-shaped or flat bottom. The vessel dimensions are defined by prescribing the vessel height H and diameter T. For the dished bottom vessel, the bottom minor radius Rd must also be specified. The mixer geometries and dimensions are shown in Figure 2.
Figure 2: Side view of a flat bottom mixer (top) and a dished bottom mixer (bottom). The specified geometric properties are the vessel height (H), diameter (T), and for the dished bottom vessel, the bottom minor radius (Rd).
The rotation of the impeller drives the mixing of the fluid in the vessel. Due to the rotation and the design of the impeller, the liquid is discharged in the axial and radial directions by the impeller. Many types of impellers, with a variety of purposes, are used in industrial applications. Impellers used for mixing are commonly classified as radial or axial impellers corresponding to the predominant discharge direction. The impellers included in this example are the pitched blade impeller and the six-blade Rushton disc turbine. The pitched blade impeller is a so-called general purpose impeller discharging the fluid both radially and axially whereas the Rushton turbine is a radial impeller used for high-shear mixing of liquid solutions. The impellers are shown in Figure 3. Other types of impellers can be found in the Part Libraries.
Figure 3: A four-blade pitched impeller (left) and a six-blade Rushton disc turbine (right).
The geometry subsequences to build the impellers and vessels are imported from the Part Libraries: Rushton Impeller, Pitched Blade Impeller, Impeller Shaft, Flat Bottom Tank and Dished Bottom Tank. An assembly for the mixer geometry is formed under the main geometry node. The subsequences also define selections, such as Rotating Wall, Rotating Interior Wall, Interior Wall, or Symmetry to facilitate setting up the physics features.
You can modify the geometry to fit your own application. In case your mixer components cannot be built from the supplied geometry subsequences, you can add your own subsequences to the geometry file using the existing ones as templates.
Laminar Mixing
The first example is a simulation of silicone oil in a flat bottom mixer with a six-blade Rushton turbine rotating at 40 rps. The simulation is set up using a Rotating Machinery, Laminar Flow interface with the Frozen Rotor study type. The geometry is built from the supplied geometry file: modular_mixer_geom.mph using the following parameters:
Table 1: :Laminar Mixer Geometry parameters
H
0.0805[m]
Vessel height
T
H
Vessel diameter
C
1/3*T
Clearance
B
4
Number of baffles
bw
T/10
Baffle width
Boz
0
Baffle offset from bottom
Rd
T/10
Minor radius of dished bottom
Da
T/3
Impeller diameter
shaft_diameter
Da/10
Shaft diameter
blade_length
Da/4
Blade length for Rushton turbine
blade_width
Da/5
Width of impeller blade
The fluid in the mixer is Silicone oil Si1000 with a density of 972 kg/m3 and a dynamic viscosity of 1.0 Pa·s.
The example is taken from Ref. 1, which also includes comparisons with experiments from Ref. 2. In Ref. 1, results are presented for three different rotation rates. The mixer simulation in this example is for the highest of the three rotation rates. You can adjust the rotation rate to simulate the other two cases. This example uses the frozen-rotor study type whereas time-dependent (sliding-mesh) studies are performed in Ref. 1. Due to the topology variations resulting from the relative motion between the rotating impeller and baffled vessel, the flow field is really time dependent. The frozen-rotor solution should in this case be viewed as a quasi-steady approximation to the flow field. The solution gives a general idea of the circulation pattern set up in the mixing vessel, and may produce good approximations of certain averaged flow quantities, such as the power draw. You can use the results of the frozen-rotor simulation as initial conditions for a time-dependent study. If you want to perform a time dependent study, you will need to use an assembly on the geometry level so that the inner rotating volume as a continuity pair with sliding mesh toward the static outer volume. Then you can set the initial conditions to the frozen-rotor solution.
Results and Discussion
Figure 4 shows the velocity magnitude in the xz-plane and a projection of the velocity vectors on the yz-plane for the laminar-mixing simulation.
Figure 4: Velocity magnitude and in-plane velocity vectors (yz-plane) for laminar mixing of Silicon oil in a flat bottom mixer with a Rushton turbine.
The Rushton turbine discharges the fluid radially outward, whereby two zonal vortices are created. Mixing occurs between the top and bottom vortices but less intensely than within each vortex. This phenomenon is referred to as compartmentalization and is a characteristic feature of radial impellers.
The torque on the impeller, given by
where A is the surface area of the impeller and T is the total stress, is 0.011 Nm. The power draw is obtained from
where Ω is the angular-velocity vector. The power draw is 2.86 W in this case. In Ref. 1, a flow number is defined as
where Q is the radial flux through a cylindrical surface with a radius of 0.186T, extending axially from the bottom to the top of the impeller blades. The surface defined for the evaluation of the flow number is shown in Figure 5.
Figure 5: The surface defined for the evaluation of the flow number.
The value obtained from the simulation is 0.57, which is very close to the experimental value presented in Ref. 2. This illustrates how the frozen-rotor simulation, in addition to giving a general idea of the circulation pattern set up in the mixing vessel, can give good approximations of averaged flow quantities.
References
1. M.J. Rice, High Resolution Simulation of Laminar and Transitional Flows in a Mixing Vessel, PhD thesis, Virginia Polytechnic Institute and State University, 2011.
2. J. Hall, Study of Viscous and Visco-elastic Flows with Reference to Laminar Stirred Vessels, PhD thesis, Department of Mechanical Engineering, King’s College London, 2005.
Application Library path: Mixer_Module/Tutorials/modular_mixer
Modeling Instructions
Begin by loading the geometry file.
From the File menu, choose Open.
Browse to the model’s Application Libraries folder and double-click the file modular_mixer_geom.mph.
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 Fluid Flow>Single-Phase Flow>Rotating Machinery, Fluid Flow>Laminar Flow.
4
Click Add to Component 1 in the window toolbar.
5
In the Home toolbar, click  Add Physics to close the Add Physics window.
Materials
Add the values for Silicone oil Si1000.
Silicone oil Si1000
1
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose Blank Material.
2
In the Settings window for Material, locate the Material Contents section.
3
In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Density
rho
972
kg/m³
Basic
Dynamic viscosity
mu
1
Pa·s
Basic
4
In the Label text field, type Silicone oil Si1000.
Set up the rotating domain conditions in Definitions.
Definitions
Rotating Domain 1
1
In the Model Builder window, under Component 1 (comp1)>Definitions>Moving Mesh click Rotating Domain 1.
2
In the Settings window for Rotating Domain, locate the Domain Selection section.
3
From the Selection list, choose Rotating Fluid Domain.
4
Locate the Rotation section. In the f text field, type 40.
Use the predefined selections to set up the physics features.
Laminar Flow (spf)
Interior Wall 1
1
In the Model Builder window, under Component 1 (comp1) right-click Laminar Flow (spf) and choose Interior Wall.
2
In the Settings window for Interior Wall, locate the Boundary Selection section.
3
From the Selection list, choose Interior Wall.
Interior Wall 2
1
In the Physics toolbar, click  Boundaries and choose Interior Wall.
2
In the Settings window for Interior Wall, locate the Boundary Selection section.
3
From the Selection list, choose Rotating Interior Wall.
As alternative the union selection for Interior Wall 1 and Interior Wall 2 can be done.
Symmetry 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry.
2
In the Settings window for Symmetry, locate the Boundary Selection section.
3
From the Selection list, choose Symmetry.
Pressure Point Constraint 1
1
In the Physics toolbar, click  Points and choose Pressure Point Constraint.
2
In the Settings window for Pressure Point Constraint, locate the Point Selection section.
3
From the Selection list, choose Pressure Point Constraint.
Definitions
Define the postprocessing variables for the torque and power draw.
Variables 1
1
In the Home toolbar, click  Variables and choose Local Variables.
2
In the Settings window for Variables, locate the Variables section.
3
In the table, enter the following settings:
Name
Expression
Unit
Description
tau_riw
x*(spf.T_stress_uy+spf.T_stress_dy)-y*(spf.T_stress_ux+spf.T_stress_dx)
N/m
Torque per area (interior walls)
tau_rw
x*(spf.T_stressy)-y*(spf.T_stressx)
N/m
Torque per area (rotating walls)
P_riw
tau_riw*rot1.alphat
W/m²
Power draw per area (rotating interior walls)
P_rw
tau_rw*rot1.alphat
W/m²
Power draw per area (rotating walls)
Integration 1 (intop1)
Define a nonlocal integration coupling on Rotating Interior Wall to evaluate its contributions to the torque and power draw.
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Integration.
2
In the Settings window for Integration, locate the Source Selection section.
3
From the Geometric entity level list, choose Boundary.
4
From the Selection list, choose Rotating Interior Wall.
Integration 2 (intop2)
Define a nonlocal integration coupling on Rotating Wall to evaluate its contributions to the torque and power draw.
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Integration.
2
In the Settings window for Integration, locate the Source Selection section.
3
From the Geometric entity level list, choose Boundary.
4
From the Selection list, choose Rotating Wall.
Mesh 1
1
In the Model Builder window, under Component 1 (comp1) right-click Mesh 1 and choose Build All.
2
Click the  Zoom Extents button in the Graphics toolbar.
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 Preset Studies for Selected Physics Interfaces>Frozen Rotor.
4
Click Add Study in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Study 1
In the Home toolbar, click  Compute.
Results
Cut Plane 1
1
In the Results toolbar, click  Cut Plane.
2
In the Settings window for Cut Plane, locate the Plane Data section.
3
From the Plane list, choose xz-planes.
Cut Plane 2
In the Results toolbar, click  Cut Plane.
Define the surface used to calculate the flow number.
Parameterized Surface 1
1
In the Results toolbar, click  More Datasets and choose Parameterized Surface.
2
In the Settings window for Parameterized Surface, locate the Parameters section.
3
Find the First parameter subsection. In the Maximum text field, type 2*pi.
4
Find the Second parameter subsection. In the Minimum text field, type -Da/10.
5
In the Maximum text field, type Da/10.
6
Locate the Expressions section. In the x text field, type 0.186*T*cos(s1).
7
In the y text field, type 0.186*T*sin(s1).
8
In the z text field, type s2.
9
Click  Plot.
The surface for the calculation of the flow number is now visualized in the Graphics window.
Velocity: Magnitude and Vectors
Use the vessel and impeller surface plots set up under the Pressure (spf) results node to create a plot of the velocity magnitude and in-plane velocity vectors.
1
In the Model Builder window, expand the Results>Pressure (spf) node, then click Pressure (spf).
2
In the Settings window for 3D Plot Group, type Velocity: Magnitude and Vectors in the Label text field.
3
Locate the Data section. From the Dataset list, choose All Walls.
Pressure
1
In the Model Builder window, right-click Pressure and choose Delete.
2
Click Yes to confirm.
Upside Pressure
1
In the Model Builder window, right-click Upside Pressure and choose Delete.
2
Click Yes to confirm.
Downside Pressure
1
In the Model Builder window, right-click Downside Pressure and choose Delete.
2
Click Yes to confirm.
Surface 2
1
In the Model Builder window, right-click Velocity: Magnitude and Vectors and choose Surface.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Cut Plane 1.
4
Locate the Coloring and Style section. From the Color table list, choose RainbowLight.
Arrow Surface 1
1
Right-click Velocity: Magnitude and Vectors and choose Arrow Surface.
2
In the Settings window for Arrow Surface, locate the Data section.
3
From the Dataset list, choose Cut Plane 2.
4
Locate the Expression section. In the x component text field, type 0.
5
Locate the Coloring and Style section. From the Arrow length list, choose Logarithmic.
6
Select the Scale factor check box.
7
In the associated text field, type 0.005.
8
Locate the Arrow Positioning section. In the Number of arrows text field, type 1000.
9
Locate the Coloring and Style section. From the Color list, choose White.
Velocity: Magnitude and Vectors
1
In the Model Builder window, click Velocity: Magnitude and Vectors.
2
In the Settings window for 3D Plot Group, click to expand the Title section.
3
From the Title type list, choose Manual.
4
In the Title text area, type Velocity: magnitude and in-plane vectors.
5
In the Velocity: Magnitude and Vectors toolbar, click  Plot.
Evaluate the torque on the impeller and the power draw using the postprocessing variables you defined.
Torque
1
In the Results toolbar, click  Global Evaluation.
2
Right-click Global Evaluation 1 and choose Rename.
3
In the Rename Global Evaluation dialog box, type Torque in the New label text field.
4
Click OK.
5
In the Settings window for Global Evaluation, locate the Expressions section.
6
In the table, enter the following settings:
Expression
Unit
Description
abs(intop1(tau_riw)+intop2(tau_rw))
N*m
 
7
Click  Evaluate.
Power Draw
1
In the Results toolbar, click  Global Evaluation.
2
Right-click Global Evaluation 2 and choose Rename.
3
In the Rename Global Evaluation dialog box, type Power Draw in the New label text field.
4
Click OK.
5
In the Settings window for Global Evaluation, locate the Expressions section.
6
In the table, enter the following settings:
Expression
Unit
Description
abs(intop1(P_riw)+intop2(P_rw))
W
 
7
Click  Evaluate.
Evaluate the flow number.
Flow Number
1
In the Results toolbar, click  More Derived Values and choose Integration>Surface Integration.
2
Right-click Surface Integration 1 and choose Rename.
3
In the Rename Surface Integration dialog box, type Flow Number in the New label text field.
4
Click OK.
5
In the Settings window for Surface Integration, locate the Data section.
6
From the Dataset list, choose Parameterized Surface 1.
7
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
(u*cos(s1)+v*sin(s1))/40[1/s]/Da^3
1
 
8
Click  Evaluate.
Turbulent Mixing — k-ε Model
In the second example, turbulent mixing of water is simulated in a dished bottom mixer with a pitched four blade impeller rotating at 20 rpm. This simulation is set up using a Rotating Machinery, Turbulent Flow, k-ε interface with the frozen-rotor study type. The geometry is built from the supplied geometry file: modular_mixer_turbulent_geom.mph using the parameters in Table 2 below. Periodicity is utilized to reduce the computational time and hence a quarter of the domain is simulated in this case.
Table 2: Turbulent mixer geometry parameters
H
0.5[m]
Vessel height
T
H
Vessel diameter
C
1/4*H
Clearance
B
4
Number of baffles
bw
T/12
Baffle width
Boz
0
Baffle offset from bottom
Rd
T/10
Minor radius of dished bottom
Da
1/2*T
Impeller diameter
shaft_diameter
1/10*Da
Shaft diameter
blade_width
Da/5
Width of impeller blade
alpha
-45[deg]
Pitch angle
N_blades
4
Number of blades for pitched blade impeller
This example uses the frozen-rotor study type. Due to the topology variations resulting from the relative motion between the rotating impeller and baffled vessel, the flow field is really time dependent. The frozen-rotor solution should in this case be viewed as a quasi-steady approximation to the flow field. The solution gives a general idea of the circulation pattern set up in the mixing vessel, and may produce good approximations of certain averaged flow quantities, such as the power draw.
Results
Figure 6 shows a surface plot of the velocity magnitude and a projection of the velocity vectors on the yz-plane for the turbulent simulation with the k-ε turbulence model.
Figure 6: Velocity magnitude and in-plane velocity vectors (yz-plane) for turbulent mixing in a dished bottom mixer with a pitched blade impeller using the k-ε turbulence model.
The pitched blade impeller expels the fluid axially as well as radially, and a large zonal vortex, extending from the bottom to the top of the vessel, is formed. A smaller zonal vortex forms below the impeller and may in certain cases cause aggregation of heavy dispersed particles at the bottom center of the vessel.
The torque on the impeller, given by
where A is the surface area of the impeller and T is the total stress, is 0.016 Nm. The power draw is obtained from
where Ω is the angular-velocity vector. The power draw is 0.033 W in this case.
The process of setting up a time-dependent study with the results of the frozen-rotor simulation as initial conditions is a bit more involved in this case because of the geometry reduction. You can either use general extrusions to define the solution on the remaining three quarters of the domain, or, you can recompute the frozen-rotor simulation on the full domain.
Modeling Instructions
Root
Begin by loading the geometry file.
1
From the File menu, choose Open.
2
Browse to the model’s Application Libraries folder and double-click the file modular_mixer_turbulent_geom.mph.
Geometry 1
Mesh Control Faces 1 (mcf1)
Click the  Zoom Extents button in the Graphics toolbar.
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 Fluid Flow>Single-Phase Flow>Rotating Machinery, Fluid Flow>Turbulent Flow>Turbulent Flow, k-ε.
4
Click Add to Component 1 in the window toolbar.
5
In the Home toolbar, click  Add Physics to close the Add Physics window.
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.
Turbulent Flow, k-ε (spf)
Use the predefined selections to set up the physics features.
Interior Wall 1
1
In the Model Builder window, under Component 1 (comp1) right-click Turbulent Flow, k-ε (spf) and choose Interior Wall.
2
In the Settings window for Interior Wall, locate the Boundary Selection section.
3
From the Selection list, choose Rotating Interior Wall.
Interior Wall 2
1
In the Physics toolbar, click  Boundaries and choose Interior Wall.
2
In the Settings window for Interior Wall, locate the Boundary Selection section.
3
From the Selection list, choose Interior Wall.
Symmetry 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry.
2
In the Settings window for Symmetry, locate the Boundary Selection section.
3
From the Selection list, choose Symmetry.
Use a Periodic Flow Condition to account for the excluded domain.
Periodic Flow Condition 1
1
In the Physics toolbar, click  Boundaries and choose Periodic Flow Condition.
2
Select Boundaries 2, 6, 22, and 23 only.
Pressure Point Constraint 1
1
In the Physics toolbar, click  Points and choose Pressure Point Constraint.
2
In the Settings window for Pressure Point Constraint, locate the Point Selection section.
3
From the Selection list, choose Pressure Point Constraint.
Definitions
Rotating Domain 1
1
In the Model Builder window, under Component 1 (comp1)>Definitions>Moving Mesh click Rotating Domain 1.
2
In the Settings window for Rotating Domain, locate the Domain Selection section.
3
From the Selection list, choose Rotating domain (Dished Bottom Tank 1).
4
Locate the Rotation section. In the f text field, type 20[rpm].
Variables 1
1
In the Home toolbar, click  Variables and choose Local Variables.
Add postprocessing variables for the torque and power draw.
2
In the Settings window for Variables, locate the Variables section.
3
In the table, enter the following settings:
Name
Expression
Unit
Description
tau_riw
x*(spf.T_stress_uy+spf.T_stress_dy)-y*(spf.T_stress_ux+spf.T_stress_dx)
N/m
Torque per area (interior walls)
tau_rw
x*(spf.T_stressy)-y*(spf.T_stressx)
N/m
Torque per area (rotating walls)
P_riw
tau_riw*rot1.alphat
W/m²
Power draw per area (rotating interior walls)
P_rw
tau_rw*rot1.alphat
W/m²
Power draw per area (rotating walls)
Integration 1 (intop1)
Define a nonlocal integration coupling on Rotating Interior Wall to evaluate its contributions to the torque and power draw.
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Integration.
2
In the Settings window for Integration, locate the Source Selection section.
3
From the Geometric entity level list, choose Boundary.
4
From the Selection list, choose Rotating Interior Wall.
Integration 2 (intop2)
Define a nonlocal integration coupling on Rotating Wall to evaluate its contributions to the torque and power draw.
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Integration.
2
In the Settings window for Integration, locate the Source Selection section.
3
From the Geometric entity level list, choose Boundary.
4
From the Selection list, choose Rotating Wall.
Mesh 1
Size
1
In the Model Builder window, under Component 1 (comp1) right-click Mesh 1 and choose Edit Physics-Induced Sequence.
2
In the Settings window for Size, locate the Element Size section.
3
Click the Custom button.
4
Locate the Element Size Parameters section. In the Maximum element size text field, type 0.02.
Size 1
1
Click the  Wireframe Rendering button in the Graphics toolbar to see the interior of the geometry.
2
In the Model Builder window, click Size 1.
3
Select Boundaries 1, 15, 16, and 25 only.
4
In the Settings window for Size, click  Build Selected.
Size 2
1
In the Model Builder window, right-click Mesh 1 and choose Size.
2
In the Settings window for Size, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Boundary.
4
Select Boundaries 3 and 17 only.
5
Locate the Element Size section. From the Calibrate for list, choose Fluid dynamics.
6
From the Predefined list, choose Fine.
7
Click the Custom button.
8
Click  Build Selected.
Refine the mesh in the domain defined by the control surfaces.
Size 3
1
Right-click Mesh 1 and choose Size.
2
In the Settings window for Size, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domain 3 only.
5
Locate the Element Size section. From the Calibrate for list, choose Fluid dynamics.
6
From the Predefined list, choose Finer.
7
Click the Custom button.
8
Locate the Element Size Parameters section. Select the Maximum element size check box.
9
In the associated text field, type 0.0114.
10
Select the Minimum element size check box.
11
In the associated text field, type 0.00123.
12
Select the Maximum element growth rate check box.
13
In the associated text field, type 1.08.
Refine the mesh further near the blade’s surface.
Size 4
1
Right-click Mesh 1 and choose Size.
2
In the Settings window for Size, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Boundary.
4
Select Boundary 9 only.
5
Click the  Wireframe Rendering button in the Graphics toolbar to disable wireframe rendering.
6
Locate the Element Size section. From the Calibrate for list, choose Fluid dynamics.
7
From the Predefined list, choose Extra fine.
8
Click  Build All.
9
Click the  Zoom Extents button in the Graphics toolbar.
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 Preset Studies for Selected Physics Interfaces>Frozen Rotor.
4
Click Add Study in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Study 1
In the Home toolbar, click  Compute.
Results
Cut Plane 1
1
In the Results toolbar, click  Cut Plane.
2
In the Settings window for Cut Plane, locate the Plane Data section.
3
From the Plane type list, choose General.
4
In row Point 1, set x to -0.2 and y to -0.2.
5
In row Point 2, set x to -0.2, y to -0.2, and z to 0.2.
6
In row Point 3, set y to 0.
7
Click  Plot.
Cut Plane 2
1
In the Results toolbar, click  Cut Plane.
2
In the Settings window for Cut Plane, click  Plot.
Use the vessel and impeller surface plots set up under the Pressure (spf) results node to create a plot of the velocity magnitude and in-plane velocity vectors.
Downside Pressure
1
In the Model Builder window, expand the Results>Pressure (spf) node.
2
Right-click Downside Pressure and choose Delete.
Upside Pressure
In the Model Builder window, right-click Upside Pressure and choose Delete.
Pressure
In the Model Builder window, right-click Pressure and choose Delete.
Velocity: Magnitude and Vectors
1
In the Model Builder window, under Results click Pressure (spf).
2
In the Settings window for 3D Plot Group, type Velocity: Magnitude and Vectors in the Label text field.
Surface 2
1
Right-click Velocity: Magnitude and Vectors and choose Surface.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Cut Plane 1.
4
Locate the Coloring and Style section. From the Color table list, choose RainbowLight.
Arrow Surface 1
1
Right-click Velocity: Magnitude and Vectors and choose Arrow Surface.
2
In the Settings window for Arrow Surface, locate the Data section.
3
From the Dataset list, choose Cut Plane 2.
4
Locate the Expression section. In the x component text field, type 0.
5
Locate the Coloring and Style section. From the Arrow length list, choose Logarithmic.
6
Select the Scale factor check box.
7
In the associated text field, type 0.26.
8
Locate the Arrow Positioning section. In the Number of arrows text field, type 500.
9
Locate the Coloring and Style section. From the Color list, choose White.
Velocity: Magnitude and Vectors
1
In the Model Builder window, click Velocity: Magnitude and Vectors.
2
In the Settings window for 3D Plot Group, click to expand the Title section.
3
From the Title type list, choose Manual.
4
In the Title text area, type Velocity: magnitude and in-plane vectors.
5
Locate the Plot Settings section. From the View list, choose View 6.
6
In the Velocity: Magnitude and Vectors toolbar, click  Plot.
Evaluate the torque on the impeller and the power draw using the imported postprocessing variables.
Torque
1
In the Results toolbar, click  Global Evaluation.
2
In the Settings window for Global Evaluation, type Torque in the Label text field.
3
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
4*abs(intop1(tau_riw)+intop2(tau_rw))
N*m
 
Due to the periodicity conditions, multiply by 4 to get the torque on the whole impeller.
4
Click  Evaluate.
Power Draw
1
In the Results toolbar, click  Global Evaluation.
2
In the Settings window for Global Evaluation, type Power Draw in the Label text field.
3
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
4*abs(intop1(P_riw)+intop2(P_rw))
W
 
Multiply by 4 to get the full power draw.
4
Click  Evaluate.
Turbulent Mixing — k-ω Model
In the third example, similarly to the second example, turbulent mixing of water is simulated in a dished bottom mixer with a pitched four blade impeller rotating at 20 rpm. Here, the simulation is set up using a Rotating Machinery, Turbulent Flow, k-ω interface with the frozen-rotor study type. The k-ω model is better suited for flows with recirculation regions but, due to the strong nonlinearity in the turbulence coefficients, takes longer to converge than the k-ε model. By using the previous k-ε model as initial condition for the flow and turbulence variables, a faster convergence can be obtained. In the interfaces for turbulent fluid flow, there is a global option for creating a new turbulent flow interface. This option will add a new turbulent flow interface with the desired turbulence model, and automatically add settings for the initial values so that the previous solution is used in a new study.
Results
Figure 7 shows a surface plot of the velocity magnitude and a projection of the velocity vectors on the yz-plane for the turbulent simulation with the k-ω turbulence model.
Figure 7: Velocity magnitude and in-plane velocity vectors (yz-plane) for turbulent mixing in a dished bottom mixer with a pitched blade impeller using the k-ω turbulence model.
Similarly to the k-ε simulation, the flow pattern is dominated by a large zonal vortex but its core appears to be more stretched in the vertical direction. The smaller zonal vortex below the impeller appears to be stretched in the radial direction.
The torque on the impeller, given by
where A is the surface area of the impeller and T is the total stress, is 0.025 Nm. The power draw is obtained from
where Ω is the angular-velocity vector. The power draw is 0.053 W in this case. These values are higher than the corresponding results from the k-ε simulation. Although the k-ω model is better suited for these types of flows, experimental results are needed to determine whether these results are indeed more accurate.
The process of setting up a time-dependent study with the results of the frozen-rotor simulation as initial conditions is a bit more involved because of the geometry reduction. You can either use general extrusions to define the solution on the remaining three quarters of the domain, or, you can recompute the frozen-rotor simulation on the full domain.
Modeling Instructions
Root
Begin by loading the model file with the k-ε-model that contains the solution.
1
From the File menu, choose Open.
2
Browse to the model’s Application Libraries folder and double-click the file modular_mixer_ke.mph.
Component 1 (comp1)
Add a new k-ω turbulent flow interface and a study that use the solution from the k-ε-model as initial values.
Turbulent Flow, k-ε (spf)
Generate New Turbulence Model Interface 1
1
In the Model Builder window, expand the Component 1 (comp1) node.
2
Right-click Component 1 (comp1)>Turbulent Flow, k-ε (spf) and choose Generate New Turbulence Model Interface.
3
In the Settings window for Generate New Turbulence Model Interface, locate the Turbulence Model Interface section.
4
From the list, choose Turbulent Flow, k-ω.
5
Locate the Model Generation section. Click Create.
Definitions
Since the new interface has different variable names for the stress components, duplicate the current variables from the previous model and replace the respective interface tag spf with spf2 to create new variables for torque and power for the k-ω-model.
Variables 2
1
In the Model Builder window, expand the Component 1 (comp1)>Definitions node.
2
Right-click Component 1 (comp1)>Definitions>Variables 1 and choose Duplicate.
3
In the Settings window for Variables, locate the Variables section.
4
In the table, enter the following settings:
Name
Expression
Unit
Description
tau_riw2
x*(spf2.T_stress_uy+spf2.T_stress_dy)-y*(spf2.T_stress_ux+spf2.T_stress_dx)
N/m
Torque per area (interior walls)
tau_rw2
x*(spf2.T_stressy)-y*(spf2.T_stressx)
N/m
Torque per area (rotating walls)
P_riw2
tau_riw2*rot1.alphat
W/m²
Power draw per area (rotating interior walls)
P_rw2
tau_rw2*rot1.alphat
W/m²
Power draw per area (rotating walls)
Study 2
In the Home toolbar, click  Compute.
Results
Velocity (spf2)
Duplicate the cut plane datasets from the k-ε-model to make similar plots for the k-ω-model.
Cut Plane 3
1
In the Model Builder window, expand the Results>Datasets node.
2
Right-click Results>Datasets>Cut Plane 1 and choose Duplicate.
3
In the Settings window for Cut Plane, locate the Data section.
4
From the Dataset list, choose Study 2/Solution 2 (sol2).
Cut Plane 4
1
In the Model Builder window, under Results>Datasets right-click Cut Plane 2 and choose Duplicate.
2
In the Settings window for Cut Plane, locate the Data section.
3
From the Dataset list, choose Study 2/Solution 2 (sol2).
Duplicate the Velocity: Magnitude and Vectors-plot and change the data sources to be from k-ω-solution.
Velocity: Magnitude and Vectors 1
1
In the Model Builder window, right-click Velocity: Magnitude and Vectors and choose Duplicate.
2
In the Settings window for 3D Plot Group, locate the Data section.
3
From the Dataset list, choose Study 2/Solution 2 (sol2).
Surface 2
1
In the Model Builder window, expand the Velocity: Magnitude and Vectors 1 node, then click Surface 2.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Cut Plane 3.
4
Locate the Expression section. In the Expression text field, type spf2.U.
Arrow Surface 1
1
In the Model Builder window, click Arrow Surface 1.
2
In the Settings window for Arrow Surface, locate the Data section.
3
From the Dataset list, choose Cut Plane 4.
4
Locate the Expression section. In the y component text field, type v2.
5
In the z component text field, type w2.
6
In the Velocity: Magnitude and Vectors 1 toolbar, click  Plot.
Group the plots for the k-ω-model
Pressure (spf2), Velocity (spf2), Velocity: Magnitude and Vectors 1, Wall Resolution (spf2)
1
In the Model Builder window, under Results, Ctrl-click to select Velocity (spf2), Pressure (spf2), Wall Resolution (spf2), and Velocity: Magnitude and Vectors 1.
2
Right-click and choose Group.
k-omega
In the Settings window for Group, type k-omega in the Label text field.
Put the plots from the k-ε-model into a group to make it easier to know which plot that belong to the different solutions.
Velocity (spf), Velocity: Magnitude and Vectors, Wall Resolution (spf)
1
In the Model Builder window, under Results, Ctrl-click to select Velocity (spf), Velocity: Magnitude and Vectors, and Wall Resolution (spf).
2
Right-click and choose Group.
k-epsilon
In the Settings window for Group, type k-epsilon in the Label text field.
Duplicate the global evaluations for torque and power. Replace the old variable names with new variables from the k-ω-solution.
Torque 1
1
In the Model Builder window, expand the Results>Derived Values node.
2
Right-click Torque and choose Duplicate.
3
In the Settings window for Global Evaluation, locate the Data section.
4
From the Dataset list, choose Study 2/Solution 2 (sol2).
5
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
4*abs(intop1(tau_riw2)+intop2(tau_rw2))
N*m
 
6
Click  Evaluate.
Power Draw 1
1
In the Model Builder window, right-click Power Draw and choose Duplicate.
2
In the Settings window for Global Evaluation, locate the Data section.
3
From the Dataset list, choose Study 2/Solution 2 (sol2).
4
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
4*abs(intop1(P_riw2)+intop2(P_rw2))
W
 
5
Click  Evaluate.
Power Draw 1, Torque 1
1
In the Model Builder window, under Results>Derived Values, Ctrl-click to select Torque 1 and Power Draw 1.
2
Right-click and choose Group.
Power/Torque k-omega
In the Settings window for Group, type Power/Torque k-omega in the Label text field.
Power Draw, Torque
1
In the Model Builder window, under Results>Derived Values, Ctrl-click to select Torque and Power Draw.
2
Right-click and choose Group.
Power/Torque k-epsilon
In the Settings window for Group, type Power/Torque k-epsilon in the Label text field.