PDF
Controlled Diffusion Separator1
Introduction
This model treats an H-shaped microfluidic device for controlled separation through diffusion. The device puts two different laminar streams in contact for a controlled period of time. The contact surface is well defined, and by controlling the flow rate it is possible to maintain the laminar flow field and control the amount of species transported from one stream to the other through diffusion. The device concept is illustrated in Figure 1. The design aims to maintain a laminar flow field when the two streams, A and B, are united and thus prevent uncontrolled convective mixing. The transport of species between streams A and B should take place only by diffusion in order that species with low diffusion coefficients stay in their respective streams. In this way, light species with high diffusivity can be separated from heavy species with low diffusivity. Let us look at a mixture of light and heavy species entering through inlet A. If the separator is properly designed, the heavy species should exit almost exclusively through outlet A. The lighter species should exit through both outlet A and B in equal rates. In this way, outlet B contains only the lighter species.
Figure 1: Diagram of the device.
Model Definition
The geometry of the device is shown in Figure 2. The device geometry is split in two because of symmetry.
Figure 2: Model geometry. To avoid any type of convective mixing, the design must smoothly let both streams come in contact with each other. Due to symmetry, it is sufficient to model half the geometry, so the actual channel is twice as high in the z direction.
The flow rate at the inlet is approximately 0.1 mm/s. The Reynolds number, which is important for characterizing the flow is given by:
where ρ is the fluid density (1000 kg/m3), U is a characteristic velocity of the flow (0.1 mm/s), μ is the fluid viscosity (1 mPa⋅s) and L is a characteristic dimension of the device (10 μm). When the Reynolds number is significantly less than 1, as in this example, the Creeping Flow interface can be used. The convective term in the Navier–Stokes equations can be dropped, leaving the incompressible Stokes equations:
where u is the local velocity (m/s) and p is the pressure (Pa).
Mixing in the device involves species at relatively low concentrations compared to the solvent, in this case water. This means that the solute molecules interact only with water molecules, and Fick’s law can be used to describe the diffusive transport. The mass-balance equation for the solute is therefore
(1)
where D is the diffusion coefficient of the solute (m2/s) and c is its concentration (mol/m3). Diffusive flows can be characterized by another dimensionless number: the Peclet number, which is given by
In this model, the parametric solver is used to solve Equation 1 for three different species, each with different values of D: 1×10-11 m2/s, 5×10-11 m2/s, and 1×10-10 m2/s. These values of D correspond to Peclet numbers of 100, 20, and 10 respectively. Since these Peclet numbers are all greater than 1, implying a cell Peclet number significantly greater than 1, numerical stabilization is required when solving Fick’s equation. COMSOL automatically includes the stabilization by default, so no explicit settings are required.
Two versions of the model are solved:
•
In the first version, it is assumed that a change in solute concentration does not influence the fluid’s density and viscosity. This implies that it is possible to first solve the Navier–Stokes equations and then solve the mass balance equation.
•
In the second version, the viscosity depends quadratically on the concentration:
Here α is a constant of dimension m6/(mol)2 and μ0 is the viscosity at zero concentration. Such a relationship between concentration and viscosity is usually observed in solutions of larger molecules.
Results and Discussion
Figure 3 shows the velocity field for the case where viscosity is concentration independent. The flow is symmetric and is not influenced by the concentration field. Figure 4 shows the corresponding pressure distribution on the channel walls that results from the flow.
Figure 3: Flow velocity field.
Figure 4: Pressure distribution on the channel walls.
Figure 5: Concentration distribution for a species with diffusivity 1·10-11 m2/s.
Figure 6: Concentration distribution for a species with diffusivity 5·10-11 m2/s.
Figure 7: Concentration distribution for a species with diffusivity 1·10-10 m2/s.
Figure 8: Average concentration at the outlet of stream B as a function of the diffusion coefficient.
Figure 5, Figure 6, and Figure 7 show the species concentration for the each of the three diffusion coefficients. For the heaviest species, which has the smallest diffusivity, there is almost no significant mixing between streams A and B (Figure 5). For the lightest species, which has the largest diffusion coefficient, the mixing is almost perfect (Figure 7). Figure 8 shows how the mean concentration of the species at the outlet of stream B varies for the different species diffusion coefficients. The simulation clearly shows that the device could be used to separate lighter molecules from heavier ones. By placing a number of these devices in series, a high degree of separation could be obtained.
In some cases, especially those involving solutions of macromolecules, the macromolecule concentration has a large influence on the liquid’s viscosity. In such situations, the Navier–Stokes and the convection–diffusion equations become coupled, and so they must be solved simultaneously. Figure 9, Figure 10, and Figure 11 show the results of such a simulation, in which the Navier–Stokes equations are solved with a concentration-dependent viscosity. In this case, for the species with diffusivity 5·10−11 m2/s. The velocity field is altered slightly by the concentration dependent viscosity (see Figure 12) but this has little effect on the mean stream A outlet concentration, which changes only slightly from 0.448 to 0.45. Much more serious is the effect of the nonuniform viscosity on the pressure distribution required to maintain the two streams at the same flow rate. A larger pressure is required at the inlet of stream B to drive the higher viscosity fluid through the system. This asymmetry in the pressure distribution makes placing several devices in series much more difficult.
Figure 9: Velocity field. The viscosity varies with the concentration according to μ= μ0(1 + αc2) with α = 0.5 (m3/mol)2. It is difficult to see the differences between this figure and that in Figure 3, but careful inspection reveals a slight change in the velocity profile. This is highlighted further in Figure 12.
Figure 10: Pressure distribution. The viscosity varies with the concentration according to μ= μ0(1 + α c2) with α = 0.5 (m3/mol)2. This figure should be compared to Figure 4. There are significant differences between the two cases.
Figure 11: Concentration distribution for the species with diffusivity 5·10-11 m2/s for the case where the fluid viscosity varies with concentration. This plot is very similar to the corresponding plot for an uncoupled flow, shown in Figure 6.
Figure 12: Comparison of the velocity field for the uncoupled and coupled flow simulations showing the difference between the two cases. The coupled flow, in which the fluid viscosity is a function of concentration, is asymmetric.
Application Library path: Microfluidics_Module/Micromixers/controlled_diffusion_separator
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 > Creeping Flow (spf).
3
Click Add.
4
In the Select Physics tree, select Chemical Species Transport > Transport of Diluted Species (tds).
5
Click Add.
6
Click  Study.
7
In the Select Study tree, select General Studies > Stationary.
8
Click  Done.
Geometry 1
For many microfluidic devices it is convenient to specify the geometry dimensions using micrometers.
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 µm.
The geometry can be constructed by extruding a 2-dimensional work plane. First draw a top down view of the structure in the work plane.
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) > Rectangle 1 (r1)
1
In the Work Plane toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 140.
4
In the Height text field, type 60.
5
Click  Build Selected.
Work Plane 1 (wp1) > Rectangle 2 (r2)
1
In the Work Plane toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 120.
4
In the Height text field, type 50.
5
Locate the Position section. In the xw text field, type 10.
6
In the yw text field, type 10.
7
Click  Build Selected.
Work Plane 1 (wp1) > Difference 1 (dif1)
1
In the Work Plane toolbar, click  Booleans and Partitions and choose Difference.
2
Select the object r1 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 r2 only.
6
Click  Build Selected.
Work Plane 1 (wp1) > Fillet 1 (fil1)
1
In the Work Plane toolbar, click  Fillet.
2
On the object dif1, select Points 3 and 5 only.
It might be easier to select the correct points by using the Selection List window. To open this window, in the Home toolbar click Windows and choose Selection List. (If you are running the cross-platform desktop, you find Windows in the main menu.)
3
In the Settings window for Fillet, locate the Radius section.
4
In the Radius text field, type 10.
5
Click  Build Selected.
Work Plane 1 (wp1) > Fillet 2 (fil2)
1
In the Work Plane toolbar, click  Fillet.
2
On the object fil1, select Points 1 and 9 only.
3
In the Settings window for Fillet, locate the Radius section.
4
In the Radius text field, type 20.
5
Click  Build Selected.
Work Plane 1 (wp1) > Mirror 1 (mir1)
1
In the Work Plane toolbar, click  Transforms and choose Mirror.
2
Select the object fil2 only.
3
In the Settings window for Mirror, locate the Input section.
4
Select the Keep input objects checkbox.
5
Locate the Normal Vector to Line of Reflection section. In the xw text field, type 0.
6
In the yw text field, type 1.
7
Click  Build Selected.
Work Plane 1 (wp1) > Union 1 (uni1)
1
In the Work Plane toolbar, click  Booleans and Partitions and choose 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 Selected.
Extrude the 2D geometry to create a 3 dimensional geometry.
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 (µm)
10
4
Click  Build Selected.
5
Click the  Zoom Extents button in the Graphics toolbar.
Create parameters to define the model.
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
D
5e-11[m^2/s]
5E-11 m²/s
Diffusion constant
fr
15[pl/s]
1.5E-14 m³/s
Inlet flow rate
c0
1[mol/m^3]
1 mol/m³
Inlet concentration
alpha
0.5[(m^3/mol)^2]
0.5 m6/mol²
Viscosity c^2-term prefactor
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
1000
kg/m³
Basic
Dynamic viscosity
mu
1e-3
Pa·s
Basic
Use the Reacting Flow, Diluted Species multiphysics couplings to couple the velocity.
Multiphysics
Reacting Flow, Diluted Species 1 (rfd1)
In the Physics toolbar, click  Multiphysics Couplings and choose Domain > Reacting Flow, Diluted Species.
Creeping Flow (spf)
Add a Fully developed flow inlet boundary condition.
Inlet 1
1
In the Physics toolbar, click  Boundaries and choose Inlet.
2
Select Boundaries 2 and 10 only.
3
In the Settings window for Inlet, locate the Boundary Condition section.
4
From the list, choose Fully developed flow.
5
Locate the Fully Developed Flow section. Click the Flow rate button.
6
In the V0 text field, type fr/2.
Set the flow rate to one half of the parameter value, since only half of the geometry is modeled.
Add an outlet with a Pressure boundary condition.
Outlet 1
1
In the Physics toolbar, click  Boundaries and choose Outlet.
2
Select Boundaries 23 and 25 only.
The default pressure of 0 Pa is appropriate in this case.
Add a Symmetry boundary condition in the symmetry plane.
Symmetry 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry.
2
Select Boundaries 4 and 9 only.
Now set up the mass transport physics. Start by raising the element order to quadratic, in order to match the discretization for the velocity.
Transport of Diluted Species (tds)
1
In the Model Builder window, under Component 1 (comp1) click Transport of Diluted Species (tds).
2
In the Settings window for Transport of Diluted Species, click to expand the Discretization section.
3
From the Concentration list, choose Quadratic.
Fluid 1
The diffusion coefficient is set to use the parameter previously defined.
1
In the Model Builder window, under Component 1 (comp1) > Transport of Diluted Species (tds) click Fluid 1.
2
In the Settings window for Fluid, locate the Diffusion section.
3
In the Dc text field, type D.
Note that the velocity field for the species convection is controlled by the Reacting Flow, Diluted Species multiphysics coupling.
Specify the concentration at the two inlets.
Concentration 1
1
In the Physics toolbar, click  Boundaries and choose Concentration.
2
Select Boundary 2 only.
3
In the Settings window for Concentration, locate the Concentration section.
4
Select the Species c checkbox.
5
In the c0,c text field, type c0.
Concentration 2
1
In the Physics toolbar, click  Boundaries and choose Concentration.
2
Select Boundary 10 only.
3
In the Settings window for Concentration, locate the Concentration section.
4
Select the Species c checkbox.
In this case the concentration should take the default value of 0.
Use the Outflow condition to allow species to leave the domain by convection. Since we will ultimately be interested in the weighted average concentration, add two Outflow features, each of which will provide its own value.
Outflow 1
1
In the Physics toolbar, click  Boundaries and choose Outflow.
2
In the Settings window for Outflow, locate the Boundary Selection section.
3
Click  Paste Selection.
4
In the Paste Selection dialog, type 23 in the Selection text field.
5
Click OK.
Outflow 2
1
In the Physics toolbar, click  Boundaries and choose Outflow.
2
In the Settings window for Outflow, locate the Boundary Selection section.
3
Click  Paste Selection.
4
In the Paste Selection dialog, type 25 in the Selection text field.
5
Click OK.
Set up the mesh. By default, COMSOL will create a mesh for the physics currently in the model. Often this is good enough, but in this case, we want to make some small edits to the default mesh sequence.
Mesh 1
By default, the fine mesh is not applied to interior boundaries. Typically this is wanted, since interior boundaries are transparent to the fluid flow. However, in this case, the mixing of the two streams occurs close to this interior boundary, so we can add boundary 16 to the Size 1 and also the Boundary Layer Properties 1 mesh feature.
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.
Size 2
1
In the Model Builder window, under Component 1 (comp1) > Mesh 1 click Size 2.
2
In the Settings window for Size, locate the Geometric Entity Selection section.
3
Click  Paste Selection.
4
In the Paste Selection dialog, type 16 in the Selection text field.
5
Click OK.
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 Boundary Selection section.
3
Click  Paste Selection.
4
In the Paste Selection dialog, type 16 in the Selection text field.
5
Click OK.
6
In the Settings window for Boundary Layer Properties, click  Build All.
Study 1
Now set up a study to solve the problem. Initially it is assumed that the fluid flow and diffusion problems are uncoupled. In this case it makes sense to solve the fluid flow problem first and then to use the velocity field as an input for the diffusion problem. This will save time and memory, particularly since the diffusion problem is solved for three parameters.
Since the study will automatically generate a large number of default plots, default plots are disabled.
1
In the Model Builder window, click Study 1.
2
In the Settings window for Study, locate the Study Settings section.
3
Clear the Generate default plots checkbox.
For Step 1, solve only the creeping flow problem.
Step 1: Stationary
1
In the Model Builder window, under Study 1 click Step 1: Stationary.
2
In the Settings window for Stationary, locate the Physics and Variables Selection section.
3
In the Solve for column of the table, under Component 1 (comp1), clear the checkbox for Transport of Diluted Species (tds).
Add a second study step.
Step 2: Stationary 2
1
In the Study toolbar, click  Stationary.
Disable the solution of the creeping flow problem for this step.
2
In the Settings window for Stationary, locate the Physics and Variables Selection section.
3
In the Solve for column of the table, under Component 1 (comp1), clear the checkbox for Creeping Flow (spf).
Solve the diffusion problem for three values of the diffusion coefficient.
4
Click to expand the Study Extensions section. Select the Auxiliary sweep checkbox.
5
Click  Add.
6
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
D (Diffusion constant)
1e-10 5e-11 1e-11
m^2/s
7
In the Study toolbar, click  Compute.
Create a Surface dataset to view the pressure on the channel walls.
Results
Surface 1
1
In the Model Builder window, expand the Results node.
2
Right-click Results > Datasets and choose Surface.
3
In the Settings window for Surface, locate the Selection section.
4
Click  Paste Selection.
5
In the Paste Selection dialog, type 1 3 5 6 7 8 11 12 13 14 15 17 18 19 20 21 22 24 26 27 in the Selection text field.
6
Click OK.
Velocity (Uncoupled Flow)
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Velocity (Uncoupled Flow) in the Label text field.
Use a Slice plot to view the data on one or more slices through the geometry.
Slice 1
1
Right-click Velocity (Uncoupled Flow) and choose Slice.
2
In the Settings window for Slice, locate the Expression section.
3
From the Unit list, choose mm/s.
Velocity (Uncoupled Flow)
Add additional slices in different directions.
Slice 2
1
In the Model Builder window, right-click Velocity (Uncoupled Flow) and choose Slice.
2
In the Settings window for Slice, locate the Expression section.
3
From the Unit list, choose mm/s.
4
Locate the Plane Data section. From the Plane list, choose xy-planes.
5
In the Planes text field, type 1.
The extra slices should use the same scale and colors for the velocity plot as the existing slice.
6
Click to expand the Inherit Style section. From the Plot list, choose Slice 1.
To avoid duplicate titles, turn off the title for additional slices.
7
Click to expand the Title section. From the Title type list, choose None.
Add slices in a third plane.
Slice 3
1
Right-click Slice 2 and choose Duplicate.
2
In the Settings window for Slice, locate the Plane Data section.
3
From the Plane list, choose zx-planes.
4
In the Planes text field, type 2.
Use the Arrow Volume plot to visualize the flow direction.
Arrow Volume 1
1
In the Model Builder window, right-click Velocity (Uncoupled Flow) and choose Arrow Volume.
2
In the Settings window for Arrow Volume, locate the Arrow Positioning section.
3
Find the x grid points subsection. In the Points text field, type 14.
4
Find the y grid points subsection. In the Points text field, type 21.
5
Find the z grid points subsection. In the Points text field, type 3.
6
Locate the Coloring and Style section. From the Color list, choose Black.
7
In the Velocity (Uncoupled Flow) toolbar, click  Plot.
Next add a pressure plot, using the dataset created previously.
Pressure (Uncoupled Flow)
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Pressure (Uncoupled Flow) in the Label text field.
3
Locate the Data section. From the Dataset list, choose Surface 1.
First add a uniformly colored surface, to highlight the channel walls.
Surface 1
1
Right-click Pressure (Uncoupled Flow) and choose Surface.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type 1.
4
Locate the Coloring and Style section. From the Coloring list, choose Uniform.
5
From the Color list, choose Gray.
Next use contours to visualize the pressure.
Contour 1
1
In the Model Builder window, right-click Pressure (Uncoupled Flow) and choose Contour.
2
In the Settings window for Contour, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Creeping Flow > Velocity and pressure > p - Pressure - Pa.
3
In the Pressure (Uncoupled Flow) toolbar, click  Plot.
Next create a Slice plot to visualize the concentration in the device. Use the existing velocity slice plot as a basis for this plot.
Concentration (Uncoupled Flow)
1
In the Model Builder window, right-click Velocity (Uncoupled Flow) and choose Duplicate.
2
In the Settings window for 3D Plot Group, type Concentration (Uncoupled Flow) in the Label text field.
For each of the slice subnodes, change the plotted quantity to concentration.
Slice 1
1
In the Model Builder window, expand the Concentration (Uncoupled Flow) node, then click Slice 1.
2
In the Settings window for Slice, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Transport of Diluted Species > Species c > c - Molar concentration, c - mol/m³.
Slice 2
1
In the Model Builder window, click Slice 2.
2
In the Settings window for Slice, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose c - Molar concentration, c - mol/m³.
Slice 3
1
In the Model Builder window, click Slice 3.
2
In the Settings window for Slice, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose c - Molar concentration, c - mol/m³.
Disable the Arrow Volume plot.
Arrow Volume 1
In the Model Builder window, right-click Arrow Volume 1 and choose Disable.
Concentration (Uncoupled Flow)
Look at the plot for each of the three diffusion coefficient levels.
The plots on the next page show the results for each of the diffusion coefficients solved for. For the heaviest species, which has the smallest diffusivity, there is limited mixing between streams A and B. For the lightest species, which has the largest diffusion coefficient, the mixing is almost perfect.
1
In the Model Builder window, click Concentration (Uncoupled Flow).
2
In the Concentration (Uncoupled Flow) toolbar, click  Plot.
3
In the Settings window for 3D Plot Group, click  Plot Previous.
4
Click  Plot Previous.
Add a Global plot to show how the concentration at the output differs with diffusion coefficient.
Output Concentration (Uncoupled Flow)
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Output Concentration (Uncoupled Flow) in the Label text field.
Global 1
1
Right-click Output Concentration (Uncoupled Flow) and choose Global.
Use the built in variable to compute the average concentration at the device output.
2
In the Settings window for Global, click Replace Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1) > Transport of Diluted Species > Outflow 2 > tds.out2.c0_avg_c - Average concentration - mol/m³.
No legend is necessary for this plot, as only one quantity is plotted.
3
Click to expand the Legends section. Clear the Show legends checkbox.
Add a marker in the computed data points.
4
Click to expand the Coloring and Style section. Find the Line markers subsection. From the Marker list, choose Point.
5
Locate the x-Axis Data section. From the Parameter list, choose Expression.
6
In the Expression text field, type D.
Change the axis titles. Note that html tags and a range of mathematical symbols and Greek letters can be entered in the axis and plot titles.
Output Concentration (Uncoupled Flow)
1
In the Model Builder window, click Output Concentration (Uncoupled Flow).
2
In the Settings window for 1D Plot Group, click to expand the Title section.
3
From the Title type list, choose None.
4
Locate the Plot Settings section.
5
Select the x-axis label checkbox. In the associated text field, type Diffusion Coefficient (m<sup>2</sup>/s).
6
Select the y-axis label checkbox. In the associated text field, type Concentration at Stream B Outlet (mol/m<sup>3</sup>).
Change the axis limits for the plot.
7
Locate the Axis section. Select the Manual axis limits checkbox.
8
In the y minimum text field, type 0.
9
In the y maximum text field, type 0.5.
10
In the Output Concentration (Uncoupled Flow) toolbar, click  Plot.
This plot shows that the concentration of the species at the output is strongly dependent on the diffusion coefficient of the molecule. Thus the device could be used to separate species with different diffusion coefficients, particularly if multiple stages of the device were arranged in series.
In some cases, particularly if the solution consists of large macromolecules, the dissolved species has a large influence on the liquid’s viscosity. In such situations, the Navier–Stokes and the convection–diffusion equations become coupled, and so they must be solved simultaneously.
Add a new Fluid Properties node that will be used to set up the fully coupled problem. To make the viscosity a function of the species concentration simply type an expression into the Dynamic viscosity field of the Fluid Properties node.
Creeping Flow (spf)
Fluid Properties: Uncoupled
1
In the Model Builder window, under Component 1 (comp1) > Creeping Flow (spf) click Fluid Properties 1.
2
In the Settings window for Fluid Properties, type Fluid Properties: Uncoupled in the Label text field.
Fluid Properties: Coupled
1
Right-click Fluid Properties: Uncoupled and choose Duplicate.
2
In the Settings window for Fluid Properties, type Fluid Properties: Coupled in the Label text field.
3
Locate the Fluid Properties section. From the μ list, choose User defined. In the associated text field, type 1e-3[Pa*s]*(1+alpha*c^2).
Deactivate the Fluid Properties: Coupled node in Study 1 to be able to reproduce the uncoupled results in the future. Then, add a new study to solve the fully coupled problem. In this instance only a single diffusion coefficient will be solved for, so no parametric sweep will be required. The model will default to the parameter entered on the Parameters node for the diffusion constant: 5e-11 m^2/s.
Study 1
Step 1: Stationary
1
In the Model Builder window, under Study 1 click Step 1: Stationary.
2
In the Settings window for Stationary, locate the Physics and Variables Selection section.
3
Select the Modify model configuration for study step checkbox.
4
In the tree, select Component 1 (comp1) > Creeping Flow (spf) > Fluid Properties: Coupled.
5
Right-click and choose Disable.
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 > Stationary.
4
Click the Add Study button in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Study 2
Turn off the default plot groups again.
1
In the Settings window for Study, locate the Study Settings section.
2
Clear the Generate default plots checkbox.
3
In the Study toolbar, click  Compute.
Add another surface dataset that points to the new solution.
Results
Surface 2
1
In the Model Builder window, under Results > Datasets right-click Surface 1 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Study 2/Solution 3 (sol3).
Recreate the velocity, pressure and concentration plots for the fully coupled problem.
Velocity (Coupled Flow)
1
In the Model Builder window, right-click Velocity (Uncoupled Flow) and choose Duplicate.
2
In the Settings window for 3D Plot Group, type Velocity (Coupled Flow) in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study 2/Solution 3 (sol3).
4
In the Velocity (Coupled Flow) toolbar, click  Plot.
There are significant differences in the flow pattern, although these are hard to see when comparing this plot with the similar one generated previously. The flow through a slice of the channel will be investigated in more detail later to better highlight these differences.
Pressure (Coupled Flow)
1
In the Model Builder window, right-click Pressure (Uncoupled Flow) and choose Duplicate.
2
In the Settings window for 3D Plot Group, type Pressure (Coupled Flow) in the Label text field.
3
Locate the Data section. From the Dataset list, choose Surface 2.
4
In the Pressure (Coupled Flow) toolbar, click  Plot.
The pressure distribution in the channel has changed significantly as a result of the increased viscosity of the fluid that contains the added species. Thus the two inlets must be maintained at different pressures. This may be possible for a single stage, but it would significantly complicate the design of a multiple stage device.
Concentration (Coupled Flow)
1
In the Model Builder window, right-click Concentration (Uncoupled Flow) and choose Duplicate.
2
In the Settings window for 3D Plot Group, type Concentration (Coupled Flow) in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study 2/Solution 3 (sol3).
4
In the Concentration (Coupled Flow) toolbar, click  Plot.
The concentration distribution is affected only slightly by the coupling between the flow and the concentration.
Next add a Cut Plane dataset in the center of the channel, for both the uncoupled and fully coupled solutions. These will be used to visualize the change in the flow profile induced by the coupling.
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
In the x-coordinate text field, type 70.
Cut Plane 2
1
Right-click Cut Plane 1 and choose Duplicate.
2
In the Settings window for Cut Plane, locate the Data section.
3
From the Dataset list, choose Study 2/Solution 3 (sol3).
Cut Plane 1
Then add a Contour plot of the velocity magnitude.
Velocity Comparison
1
In the Results toolbar, click  2D Plot Group.
2
In the Settings window for 2D Plot Group, type Velocity Comparison in the Label text field.
3
Locate the Data section. From the Dataset list, choose Cut Plane 1.
4
From the Parameter value (D (m^2/s)) list, choose 5E-11.
Contour 1
1
Right-click Velocity Comparison and choose Contour.
2
In the Settings window for Contour, locate the Levels section.
3
In the Total levels text field, type 5.
Create a duplicate Contour plot, using the same colors and scales, but showing the coupled data.
Contour 2
1
Right-click Contour 1 and choose Duplicate.
2
In the Settings window for Contour, locate the Data section.
3
From the Dataset list, choose Cut Plane 2.
4
Click to expand the Title section. From the Title type list, choose None.
5
Locate the Coloring and Style section. Clear the Color legend checkbox.
6
Click to expand the Inherit Style section. From the Plot list, choose Contour 1.
7
In the Velocity Comparison toolbar, click  Plot.
8
Click the  Zoom Extents button in the Graphics toolbar.
Now it is possible to compare the velocity distributions more carefully. It is clear that the coupling has introduced an asymmetry into the flow pattern, as a result of the higher viscosity in the fluid containing the dissolved species.
Finally compare the output concentration between the two solutions.
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) > Transport of Diluted Species > Outflow 2 > tds.out2.c0_avg_c - Average concentration - mol/m³.
3
Click  Evaluate.
Table 1
Go to the Table 1 window.
Global Evaluation 2
1
Right-click Global Evaluation 1 and choose Duplicate.
2
In the Settings window for Global Evaluation, locate the Data section.
3
From the Dataset list, choose Study 2/Solution 3 (sol3).
4
Clicknext to  Evaluate, then choose New Table.
Only a small difference occurs in the output concentration as a result of the coupling between the problems. However the coupling would make adding multiple stages of the device together much more difficult, as different pressures are required at the two inlets to obtain the same flow velocity in the two streams.
1
This example was originally formulated by Albert Witarsa under Professor Bruce Finlayson’s supervision at the University of Washington in Seattle. It was part of a graduate course in which the assignment consisted of using mathematical modeling to evaluate the potential of patents in the field of microfluidics.