PDF
Thermophoresis
Introduction
In a gas at nonuniform temperature, suspended particles tend to move from regions of high temperature to low, due to the thermophoretic force. This effect can be used to create thermal precipitators that filter out undesirable particles from a feed gas. It can also be used in chemical vapor deposition, to inhibit the arrival of particle contaminants on the surface of a susceptor. This tutorial predicts the size of a particle-free zone above a heated susceptor for different temperature gradients. The results agree well with Ref. 1.
Note: This application requires the Particle Tracing Module, the Heat Transfer Module, and one of the following: CFD Module, Microfluidics Module, or Plasma Module.
Model Definition
Hydrogen gas is injected into the modeling domain at a flow rate of 2000 sccm. The gas flows over a heated susceptor and out through a pump after a 90-degree bend, see Figure 1. Particles are injected into the gas stream at the beginning of the susceptor uniformly in the y direction. The initial particle velocity is set to the fluid velocity.
Figure 1: Diagram showing the model geometry (in mm) and location of the susceptor.
Drag Force
The particle positions are computed by solving second-order equations of motion for the particle position vector components, following Newton’s second law,
where
•
q is the particle position (SI unit: m),
•
v is the particle velocity (SI unit: m/s),
•
mp is the particle mass (SI unit: kg), and
•
Ft is the total force (SI unit: N).
In this example, the total force includes the drag, gravity, and thermophoretic forces,
The drag force FD is defined using the Stokes drag law,
where u and v are the fluid and particle velocity, respectively (SI unit: m/s). The particle velocity response time τp (SI unit: s) is a measure of the time scale for the particle velocity to approach that of the surrounding fluid. For the Stokes drag law,
where
•
μ is the fluid dynamic viscosity (SI unit: Pa s),
•
ρp is the particle density (SI unit: kg/m3), and
•
dp is the particle diameter (SI unit: m).
The Stokes drag law is applicable when the particles are sufficiently small and move slowly relative to the surrounding fluid. For large, heavy particles with more inertia, an alternative formulation like the Schiller-Naumann drag law might be more appropriate.
Gravity Force
The Gravity Force node also includes the buoyancy force by considering the density of the surrounding fluid ρ (SI unit: kg/m3). The gravity force, Fg, is thus
Thermophoretic Force
The Thermophoretic Force applies to particles in a nonisothermal flow. The driving mechanism behind this force is the collision of gas molecules on the particle surface. Collisions are more likely to occur on the hotter side of the particle where the average molecular velocity of the gas is greater. This results in a net force toward colder regions of the gas.
In a continuum flow, the thermophoretic force, Ftp, is defined as
where
•
k (SI unit: W/(m K)) is the thermal conductivity of the fluid,
•
kp (SI unit: W/(m K)) is the particle thermal conductivity,
•
T (SI unit: K) is the fluid temperature,
•
dp (SI unit: m) is the particle diameter,
•
ρ (SI unit: kg/m3) is the fluid density, and
•
Cs is a dimensionless constant equal to 1.17.
The Thermophoretic Force node also provides some corrections for high Knudsen number flows, when the mean free path between gas molecule collisions is comparable in size to the particle diameter. However, in the present model, such high Knudsen number corrections can safely be neglected.
Results and Discussion
The gas velocity is plotted in Figure 2 and the temperature in Figure 3. The gas velocity is higher at the outlet than at the inlet due to thermal expansion. The strong heating of the gas by the susceptor causes a decrease in density, so the gas velocity must increase in order for the total mass in the system to be conserved.
The particles begin to move from left to right due to the drag force and also vertically due to the thermophoretic force; see Figure 4. The color of the particle trajectories represents the magnitude of the thermophoretic force. This is because the susceptor temperature is higher than the temperature on the upper surface. The more the temperature of the susceptor increases, the larger the particle free zone which develops just above. The height of the particle-free zone versus the susceptor temperature is plotted in Figure 5 and agrees well with Fig 6a in Ref. 1. The height of the particle-free zone clearly increases as the susceptor temperature increases, indicating an increase in the magnitude of the thermophoretic force.
Figure 2: Velocity magnitude.
Figure 3: Temperature inside the reactor.
Figure 4: Particle trajectories as they pass over the heated surface.
Figure 5: Minimum height of the particles versus temperature.
Notes About the COMSOL Implementation
The model is solved in two stages. First, the gas velocity, pressure, and temperature are computed using a Stationary study. Next, the Particle Tracing for Fluid Flow interface is added to the model and the trajectories are computed in a separate Time Dependent study. Finally, a Parametric Sweep is added with two study steps, a Stationary step for the gas flow, followed by a Time Dependent step for the particle trajectories. The parametric sweep is performed for a range of susceptor surface temperatures, meaning that both the gas flow and particle trajectories need to be recomputed for each parameter value.
Reference
1. Dimitrios I. Fotiadis, and Klavs F. Jensen, “Thermophoresis of solid particles in horizontal chemical vapor deposition reactors,” J. Crystal Growth, vol. 102 pp 743–761, 1990.
Application Library path: Particle_Tracing_Module/Fluid_Flow/thermophoresis
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  2D.
2
In the Select Physics tree, select Fluid Flow>Nonisothermal Flow>Laminar Flow.
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies>Stationary.
6
Click  Done.
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.
Rectangle 1 (r1)
1
In the Geometry toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 170.
4
In the Height text field, type 30.
Line Segment 1 (ls1)
1
In the Geometry toolbar, click  More Primitives and choose Line Segment.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
From the Specify list, choose Coordinates.
4
Locate the Endpoint section. From the Specify list, choose Coordinates.
5
Locate the Starting Point section. In the x text field, type 30.
6
Locate the Endpoint section. In the x text field, type 90.
Rectangle 2 (r2)
1
In the Geometry toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 50.
4
In the Height text field, type 40.
5
Locate the Position section. In the x text field, type -80.
6
In the y text field, type -10.
Polygon 1 (pol1)
1
In the Geometry toolbar, click  Polygon.
2
In the Settings window for Polygon, locate the Coordinates section.
3
From the Data source list, choose Vectors.
4
In the x text field, type -30 30 30 0 0 -10 -10 30.
5
In the y text field, type 30 30 30 0 0 -10 -10 30.
6
In the x text field, type -30 0 0 0 0 -30 -30 -30.
Polygon 2 (pol2)
1
In the Geometry toolbar, click  Polygon.
2
In the Settings window for Polygon, locate the Coordinates section.
3
From the Data source list, choose Vectors.
4
In the x text field, type -80 -130 -130 -130 -130 -80 -80 -80.
5
In the y text field, type 30 20 20 0 0 -10 -10 30.
Line Segment 2 (ls2)
1
In the Geometry toolbar, click  More Primitives and choose Line Segment.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
From the Specify list, choose Coordinates.
4
Locate the Endpoint section. From the Specify list, choose Coordinates.
5
Locate the Starting Point section. In the x text field, type 90.
6
Locate the Endpoint section. In the x text field, type 90.
7
In the y text field, type 30.
Rectangle 3 (r3)
1
In the Geometry toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 25.
4
In the Height text field, type 35.
5
Locate the Position section. In the x text field, type 125.
6
In the y text field, type -35.
Union 1 (uni1)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Union.
2
Select the objects pol1, pol2, r1, r2, and r3 only.
3
In the Settings window for Union, locate the Union section.
4
Clear the Keep interior boundaries check box.
Form Union (fin)
1
In the Geometry toolbar, click  Build All.
2
Click the  Zoom Extents button in the Graphics toolbar.
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
Tsusc
950[K]
950 K
Susceptor temperature
d_part
2e-6[m]
2E-6 m
Particle diameter
rho_part
2200[kg/m^3]
2200 kg/m³
Particle density
depth
74[mm]
0.074 m
Model depth
Definitions
Walls
1
In the Model Builder window, expand the Component 1 (comp1)>Definitions node.
2
Right-click Definitions and choose Selections>Explicit.
3
In the Settings window for Explicit, locate the Input Entities section.
4
From the Geometric entity level list, choose Boundary.
5
Select Boundaries 2–9, 12–14, and 16–18 only.
6
Right-click Explicit 1 and choose Rename.
7
In the Rename Explicit dialog box, type Walls in the New label text field.
8
Click OK.
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 Liquids and Gases>Gases>Hydrogen.
4
Click Add to Component in the window toolbar.
5
In the Home toolbar, click  Add Material to close the Add Material window.
Heat Transfer in Fluids (ht)
Temperature 1
1
In the Model Builder window, under Component 1 (comp1) right-click Heat Transfer in Fluids (ht) and choose Temperature.
2
Select Boundary 10 only.
3
In the Settings window for Temperature, locate the Temperature section.
4
In the T0 text field, type Tsusc.
Inflow 1
1
In the Physics toolbar, click  Boundaries and choose Inflow.
2
Select Boundary 1 only.
3
In the Settings window for Inflow, locate the Upstream Properties section.
4
In the Tustr text field, type 300.
Outflow 1
1
In the Physics toolbar, click  Boundaries and choose Outflow.
2
Select Boundary 15 only.
Laminar Flow (spf)
Since the density variation is not small, the flow cannot be regarded as incompressible. Therefore set the flow to be compressible.
1
In the Model Builder window, under Component 1 (comp1) click Laminar Flow (spf).
2
In the Settings window for Laminar Flow, locate the Physical Model section.
3
From the Compressibility list, choose Compressible flow (Ma<0.3).
Inlet 1
1
In the Physics toolbar, click  Boundaries and choose Inlet.
2
Select Boundary 1 only.
3
In the Settings window for Inlet, locate the Boundary Condition section.
4
From the list, choose Mass flow.
5
Locate the Mass Flow section. From the Mass flow type list, choose Standard flow rate (SCCM).
6
In the Qsccm text field, type 2000.
7
In the Mn text field, type 0.002.
8
In the dbc text field, type depth.
Outlet 1
1
In the Physics toolbar, click  Boundaries and choose Outlet.
2
Select Boundary 15 only.
Heat Transfer in Fluids (ht)
In the Model Builder window, under Component 1 (comp1) click Heat Transfer in Fluids (ht).
Heat Flux 1
1
In the Physics toolbar, click  Boundaries and choose Heat Flux.
2
In the Settings window for Heat Flux, locate the Boundary Selection section.
3
From the Selection list, choose Walls.
4
Locate the Heat Flux section. Click the Convective heat flux button.
5
In the h text field, type 10.
Thin Layer 1
1
In the Physics toolbar, click  Boundaries and choose Thin Layer.
2
In the Settings window for Thin Layer, locate the Boundary Selection section.
3
From the Selection list, choose Walls.
4
Locate the Layer Model section. From the Layer type list, choose Thermally thin approximation.
Since the Thin Layer feature has been added, material properties need to be defined on those boundaries.
Materials
Material 2 (mat2)
1
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose Layers>Single Layer Material.
2
In the Settings window for Material, locate the Geometric Entity Selection section.
3
From the Selection list, choose Walls.
4
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Heat capacity at constant pressure
Cp
800
J/(kg·K)
Basic
Density
rho
2700
kg/m³
Basic
Thermal conductivity
k_iso ; kii = k_iso, kij = 0
160
W/(m·K)
Basic
Thickness
lth
5[mm]
m
Shell
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 Fine.
4
Click  Build All.
Study 1
1
In the Home toolbar, click  Compute.
The default plots which are created automatically are a surface plot of the velocity field (Figure 2), a contour plot of the pressure, a surface temperature plot (Figure 3), and a contour plot of the temperature.
Results
Velocity (spf)
Next, set up the Particle Tracing Interface.
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>Particle Tracing>Particle Tracing for Fluid Flow (fpt).
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 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>Time Dependent.
4
Click Add Study in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Particle Tracing for Fluid Flow (fpt)
In the Model Builder window, under Component 1 (comp1) click Particle Tracing for Fluid Flow (fpt).
Drag Force 1
1
In the Physics toolbar, click  Domains and choose Drag Force.
2
Click in the Graphics window and then press Ctrl+A to select both domains.
3
In the Settings window for Drag Force, locate the Drag Force section.
4
From the u list, choose Velocity field (spf).
5
From the μ list, choose Dynamic viscosity (spf).
6
Locate the Model Input section. From the T list, choose Temperature (ht).
7
From the pA list, choose Absolute pressure (spf).
Thermophoretic Force 1
1
In the Physics toolbar, click  Domains and choose Thermophoretic Force.
2
Click in the Graphics window and then press Ctrl+A to select both domains.
3
In the Settings window for Thermophoretic Force, locate the Fluid Properties section.
4
From the μ list, choose Dynamic viscosity (spf).
5
From the ρ list, choose Density (spf).
6
Locate the Advanced Settings section. Select the Use piecewise polynomial recovery on field check box.
7
Locate the Model Input section. From the T list, choose Temperature (ht).
8
From the pA list, choose Absolute pressure (spf).
Wall 2
1
In the Physics toolbar, click  Boundaries and choose Wall.
2
Select Boundary 11 only.
Gravity Force 1
1
In the Physics toolbar, click  Domains and choose Gravity Force.
2
Click in the Graphics window and then press Ctrl+A to select both domains.
3
In the Settings window for Gravity Force, locate the Gravity Force section.
4
From the ρ list, choose Density (spf).
Release from Grid 1
1
In the Physics toolbar, click  Global and choose Release from Grid.
2
In the Settings window for Release from Grid, locate the Initial Coordinates section.
3
Click  Y Range.
4
In the Range dialog box, choose Number of values from the Entry method list.
5
In the Start text field, type 0.01.
6
In the Stop text field, type 29.99.
7
In the Number of values text field, type 50.
8
Click Replace.
9
In the Settings window for Release from Grid, locate the Initial Velocity section.
10
Specify the v0 vector as
u
x
v
y
Particle Properties 1
1
In the Model Builder window, click Particle Properties 1.
2
In the Settings window for Particle Properties, locate the Particle Properties section.
3
From the ρp list, choose User defined. In the associated text field, type rho_part.
4
In the dp text field, type d_part.
5
Locate the Additional Material Properties section. From the kp list, choose User defined. In the associated text field, type 1.38.
Study 2
Step 1: Time Dependent
1
In the Model Builder window, under Study 2 click Step 1: Time Dependent.
2
In the Settings window for Time Dependent, locate the Study Settings section.
3
Click  Range.
4
In the Range dialog box, choose Number of values from the Entry method list.
5
In the Stop text field, type 5.
6
In the Number of values text field, type 50.
7
Click Replace.
8
In the Settings window for Time Dependent, locate the Physics and Variables Selection section.
9
Select the Modify model configuration for study step check box.
10
In the Physics and variables selection tree, select Component 1 (comp1)>Laminar Flow (spf).
11
Click  Disable in Solvers.
12
In the Physics and variables selection tree, select Component 1 (comp1)>Heat Transfer in Fluids (ht).
13
Click  Disable in Solvers.
14
In the Physics and variables selection tree, select Component 1 (comp1)>Multiphysics Couplings>Nonisothermal Flow 1 (nitf1).
15
Click  Disable in Solvers.
16
Click to expand the Values of Dependent Variables section. Find the Values of variables not solved for subsection. From the Settings list, choose User controlled.
17
From the Method list, choose Solution.
18
From the Study list, choose Study 1, Stationary.
19
In the Home toolbar, click  Compute.
Results
Particle Trajectories (fpt)
1
Click the  Zoom Extents button in the Graphics toolbar.
2
In the Model Builder window, expand the Particle Trajectories (fpt) node.
Particle Trajectories 1
1
In the Model Builder window, expand the Results>Particle Trajectories (fpt)>Particle Trajectories 1 node, then click Particle Trajectories 1.
2
In the Settings window for Particle Trajectories, locate the Coloring and Style section.
3
Find the Line style subsection. From the Type list, choose Line.
4
Find the Point style subsection. From the Type list, choose None.
5
In the Particle Trajectories (fpt) toolbar, click  Plot.
Color Expression 1
1
In the Model Builder window, click Color Expression 1.
2
In the Settings window for Color Expression, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1)>Particle Tracing for Fluid Flow>Forces>Thermophoretic force - N>fpt.thpf1.Ftfy - Thermophoretic force, y component.
3
In the Particle Trajectories (fpt) toolbar, click  Plot.
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 Some Physics Interfaces>Stationary.
4
Click Add Study in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Study 3
Step 1: Stationary
1
In the Settings window for Stationary, locate the Physics and Variables Selection section.
2
In the table, clear the Solve for check box for Particle Tracing for Fluid Flow (fpt).
Time Dependent
1
In the Study toolbar, click  Study Steps and choose Time Dependent>Time Dependent.
2
In the Settings window for Time Dependent, locate the Physics and Variables Selection section.
3
Select the Modify model configuration for study step check box.
4
In the Physics and variables selection tree, select Component 1 (comp1)>Laminar Flow (spf).
5
Click  Disable in Solvers.
6
In the Physics and variables selection tree, select Component 1 (comp1)>Heat Transfer in Fluids (ht).
7
Click  Disable in Solvers.
8
In the Physics and variables selection tree, select Component 1 (comp1)>Multiphysics Couplings>Nonisothermal Flow 1 (nitf1).
9
Click  Disable in Solvers.
10
Locate the Values of Dependent Variables section. Find the Values of variables not solved for subsection. From the Settings list, choose User controlled.
11
From the Method list, choose Solution.
12
From the Study list, choose Study 3, Stationary.
13
Locate the Study Settings section. Click  Range.
14
In the Range dialog box, choose Number of values from the Entry method list.
15
In the Stop text field, type 5.
16
In the Number of values text field, type 10.
17
Click Replace.
Parametric Sweep
1
In the Study toolbar, click  Parametric Sweep.
2
In the Settings window for Parametric Sweep, locate the Study Settings section.
3
Click  Add.
4
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
Tsusc (Susceptor temperature)
500 600 700 800 900 950
K
5
In the Study toolbar, click  Compute.
Results
Particle 3
1
In the Model Builder window, expand the Results>Datasets node.
2
Right-click Results>Datasets>Particle 2 and choose Duplicate.
Selection
1
In the Results toolbar, click  Attributes and choose Selection.
2
In the Settings window for Selection, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Boundary.
4
Select Boundary 11 only.
Minimum 1
1
In the Results toolbar, click  More Datasets and choose Evaluation>Minimum.
2
In the Settings window for Minimum, locate the Data section.
3
From the Dataset list, choose Particle 3.
4
Locate the Settings section. From the Geometry level list, choose Point.
Particle position
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, locate the Data section.
3
From the Dataset list, choose Minimum 1.
4
From the Time selection list, choose Last.
5
Right-click 1D Plot Group 11 and choose Rename.
6
In the Rename 1D Plot Group dialog box, type Particle position in the New label text field.
7
Click OK.
Global 1
1
Right-click Particle position and choose Global.
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)>Particle Tracing for Fluid Flow>Particle position>qy - Particle position, y component - m.
3
Locate the x-Axis Data section. From the Axis source data list, choose Outer solutions.
4
In the Particle position toolbar, click  Plot.
5
Click to expand the Legends section. Clear the Show legends check box.