PDF
Rotating Channel
Introduction
A lab-on-a-chip platform can be realized on a rotating disc by designing channels and other features to use the Coriolis or centrifugal forces to manipulate the flow. These forces are controlled by changing the angular velocity of the disc, so the platform is programmed by using a controlled sequence of angular velocities. In a microchannel, the centrifugal force induces a parabolic flow profile pointing in the radial direction. This is analogous to a Poiseuille or pressure-driven flow. The velocity-dependent Coriolis force produces an inhomogeneous transverse force in the tangential direction, which has its highest value in the center of the channel. This results in a change in the pressure distribution from that of a standard Poiseuille flow, which is assessed in this model. Ref. 1 computes the pressure distribution in the channel as part of a benchmarking exercise, and the results computed by COMSOL compare well with those given in this paper.
Model Definition
The geometry consists of a square cross section channel of length 10 mm with side 200 μm (see Figure 1). The channel points in the radial direction and begins at a radius of 20 mm from the center of rotation of the disc.
Figure 1: Model geometry. The radial direction corresponds to the x-direction.
Results and Discussion
Figure 2 shows the pressure along the channel axis. The results are in good agreement with those presented by Glatzel and others (Ref. 1). It should be noted that the inlet boundary condition used by Glatzel and others is unphysical, because the Coriolis force acting at the inlet implies that there should be a pressure gradient in the y direction. Just as there is a pressure perpendicular to the flow when gravity acts in the perpendicular direction, so pressure gradients in the y direction are produced by the Coriolis force. This unphysical boundary condition accounts for the “kink” in the curve observed at the inlet and the complex pressure distribution at the inlet. Alternative approaches in this instance include using a point constraint on the pressure with the open boundary condition, explicitly including the pressure gradients in the pressure constraint and locating the inlet at the center of rotation of the disc. Because these methods invalidate comparisons with the results in Ref. 1, this model uses the unphysical boundary condition.
Figure 2: Pressure along the central axis of the channel.
The total flow rate through the channel is 14.9 μl/s, in good agreement with the results in Ref. 1.
Reference
1. T. Glatzel, C. Litterst, C. Cupelli, T. Lindemann, C. Moosmann, R. Niekrawietz, W. Streule, R. Zengerle, and P. Koltay, “Computational fluid dynamics (CFD) software tools for microfluidic applications - A case study,” Computers & Fluids, vol. 37, pp. 218–235, 2008.
Notes About the COMSOL Implementation
The model is straightforward to set up using a Laminar Flow interface. The Coriolis and centrifugal forces are added explicitly as body forces.
Application Library path: Microfluidics_Module/Fluid_Flow/rotating_channel
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>Single-Phase Flow>Laminar Flow (spf).
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies>Stationary.
6
Click  Done.
Global Definitions
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
omega
100[rad/s]
100 rad/s
Angular velocity
Geometry 1
1
In the Model Builder window, under Component 1 (comp1) click Geometry 1.
2
In the Settings window for Geometry, locate the Units section.
3
From the Length unit list, choose mm.
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 Width text field, type 10.
4
In the Depth text field, type 0.1.
5
In the Height text field, type 0.1.
6
Locate the Position section. In the x text field, type 20.
Array 1 (arr1)
1
In the Geometry toolbar, click  Transforms and choose Array.
2
Select the object blk1 only.
3
In the Settings window for Array, locate the Size section.
4
In the y size text field, type 2.
5
In the z size text field, type 2.
6
Locate the Displacement section. In the y text field, type 0.1.
7
In the z text field, type 0.1.
8
Click  Build All Objects.
9
Click the  Zoom Extents button in the Graphics toolbar.
Materials
Material 1 (mat1)
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
977
kg/m³
Basic
Dynamic viscosity
mu
8.55e-4
Pa·s
Basic
The large aspect ratio of the channel is not practical for creating the model. To continue more easily, it is useful to define a different view.
Definitions
View 2
1
In the Model Builder window, under Component 1 (comp1) right-click Definitions and choose View.
2
In the Model Builder window, click View 2.
3
In the Settings window for View, locate the View section.
4
Select the Wireframe rendering check box.
Camera
1
In the Model Builder window, click Camera.
2
In the Settings window for Camera, locate the Camera section.
3
From the View scale list, choose Automatic.
4
From the Automatic list, choose Anisotropic.
5
In the x weight text field, type 6.
6
Click  Update.
7
Click the  Zoom Extents button in the Graphics toolbar.
Define a nonlocal integration coupling for the outlet boundary.
Integration 1 (intop1)
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
Select Boundaries 17–20 only.
Variables 1
1
In the Definitions toolbar, click  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
Q
intop1(u)
m³/s
Total flow rate
Laminar Flow (spf)
Volume Force 1
1
In the Model Builder window, under Component 1 (comp1) right-click Laminar Flow (spf) and choose Volume Force.
2
In the Settings window for Volume Force, locate the Domain Selection section.
3
From the Selection list, choose All domains.
4
Locate the Volume Force section. Specify the F vector as
spf.rho*x*omega^2
x
0
y
0
z
Volume Force 2
1
In the Physics toolbar, click  Domains and choose Volume Force.
2
In the Settings window for Volume Force, locate the Domain Selection section.
3
From the Selection list, choose All domains.
4
Locate the Volume Force section. Specify the F vector as
0
x
2*spf.rho*omega*u
y
0
z
Open Boundary 1
1
In the Physics toolbar, click  Boundaries and choose Open Boundary.
2
Select Boundaries 1, 4, 8, 11, and 17–20 only.
Mesh 1
Mapped 1
1
In the Mesh toolbar, click  Boundary and choose Mapped.
2
Select Boundaries 1, 4, 8, and 11 only.
Distribution 1
1
Right-click Mapped 1 and choose Distribution.
2
Select Edges 1, 2, 4, 5, 7, 9, 10, 12, 13, 15, 17, and 19 only.
Swept 1
In the Mesh toolbar, click  Swept.
Distribution 1
1
Right-click Swept 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
In the Number of elements text field, type 150.
4
Click  Build All.
Study 1
In the Home toolbar, click  Compute.
Results
Unlike pressure-driven flows, the pressure drop along the channel is not linear. Add a 3D edge dataset to enable the creation of a pressure line plot.
Edge 3D 1
1
In the Results toolbar, click  More Datasets and choose Edge 3D.
2
Select Edge 14 only.
Pressure drop
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Pressure drop in the Label text field.
3
Locate the Data section. From the Dataset list, choose Edge 3D 1.
Line Graph 1
1
Right-click Pressure drop and choose Line Graph.
2
In the Settings window for Line Graph, click Replace Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1)>Laminar Flow>Velocity and pressure>p - Pressure - Pa.
3
Click Replace Expression in the upper-right corner of the x-Axis Data section. From the menu, choose Component 1 (comp1)>Geometry>Coordinate>x - x-coordinate.
4
In the Pressure drop toolbar, click  Plot.
Compare the result with Figure 2.
Finally, evaluate the total flow rate.
Global Evaluation 1
1
In the Results toolbar, click  Global Evaluation.
2
In the Settings window for Global Evaluation, click Replace Expression in the upper-right corner of the Expressions section. From the menu, choose Component 1 (comp1)>Definitions>Variables>Q - Total flow rate - m³/s.
3
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
Q
dm^3/s
Total flow rate
4
Click  Evaluate.
Table
1
Go to the Table window.
1.56e-5 dm^3/s corresponds to 15.6 μl/s.