PDF

2D Non-Newtonian Slot Die Coating
Introduction
Achieving uniform coating quality is important in several different industries: from optical coatings, semiconductor and electronics industry, through technologies utilizing thin membranes, to surface treatment of metals. Bad coating quality will compromise the performance of the products, or lead to complete failure in some cases.
Several different coating processes exist. This tutorial investigates the performance of a slot-die coating process, a so-called pre-metered coating method. In this process, the coating fluid is suspended from a thin slot die to a moving substrate. The final coating layer thickness is evaluated from the continuity relationship for a coating liquid. Therefore, the thickness of the liquid layer is determined by the slot gap, the coating fluid inlet velocity and the substrate speed.
The final goal of coating processes is to achieve a defect-free film of a desired thickness. However, manufacturing the uniform coating is not a trivial task, various flow instabilities or defects such as bubbles, ribbing, and rivulets are frequently observed in the process. The die geometry, the size of the slot and height above the substrate, together with the non-Newtonian fluid nature of the coating fluid are important to consider.
This tutorial demonstrates how to model the fluid flow in a polymer slot die coating process using the Laminar Two-Phase Flow, Phase Field interface and an inelastic non-Newtonian power law model for the polymer fluid.
Model Definition
Model Geometry
A typical setup of the slot-die coating process is shown in Figure 1.
Figure 1: Typical geometry for a slot-die coating process with the slot die positioned over a substrate.
This model uses a 2D cross section of the die shown in Figure 1, assuming out-of-plane invariance. The inlet for the coating fluid is at the top of the die, as shown in Figure 2, and there are open boundaries at both ends. The bottom boundary is the coating substrate which is moving at the coating velocity.
Figure 2: Model geometry. 2D cross section of a slot die.
The geometrical and material parameters in this model are taken from the Ref. 1.
Domain Equations and Boundary Conditions
The flow in this model is laminar, so a Laminar Flow interface will be used together with a Phase Field interface to track the interface between the air and the polymer fluid. The coupling of these two interfaces is handled by the Two-Phase Flow, Phase Field multiphysics interface. In this interface, you can select which constitutive relationship to use for each of the fluid phases. The air is specified as a Newtonian fluid, and the coating fluid is a non-Newtonian power law fluid.
The inlet fluid velocity is increases smoothly from 0 m/s to 0.1 m/s. Both the upstream and downstream boundaries of the model are specified as open boundaries. The corresponding inlet and outlet boundary conditions must also be set in the Phase Field interface together with the initial values for both fluids to correctly define the position of the initial interface. For the moving substrate, a moving wall boundary condition with a Navier-Slip condition is used.
Results and Discussion
The Figure 3 shows the evolution of the coating fluid interface for t = 0.03 s, t = 0.1 s, and t = 0.2 s.
Figure 3: Coating fluid interface at t = 0.03 s, t = 0.1 s and t = 0.2 s (top to bottom).
The coating film attains a constant thickness downstream of the die at t = 0.2 s. The film forms upstream and downstream meniscii with the upstream and downstream walls of the die. As the substrate speed increases or the inlet velocity decreases, the upstream meniscus is pulled closer to the slot, eventually causing defects in the coating film. The evolution of the film thickness and position of the upstream meniscus as a function of time is shown in Figure 4.
Figure 4: Film thickness and upstream meniscus position as a function of time.
By changing the geometry, the inlet velocity and wall velocity, it is easy to explore the sensitivity of the design parameters towards the film thickness and coating velocity for a variety of fluid properties in a fast and efficient manner.
Notes About the COMSOL Implementation
The default method for averaging the fluid properties across the interface between the two phases is linear with respect to the volume fraction. When working with fluids that have a large difference in viscosities, switching to a different averaging method increases the performance. In this example, the Heaviside averaging method is applied. The averaged viscosity is defined as
where V2 is the volume fraction of fluid 2, μ1 and μ2 are the viscosities for phase 1 and 2, respectively, and H is a smoothed Heaviside function. The default value for lμ is 0.8. A lower value will sharpen the interface, but also increase the computation time.
In addition, this example demonstrates how to use an add-in to fit measured rheology data to a selected inelastic non-Newtonian fluid model. The add-in utilizes functionality from the Optimization Module. In case you do not have access to this module, you can skip the corresponding part of the instructions.
Reference
1. K.L. Bhamidipati, Detection and elimination of defects during manufacture of high-temperature polymer electrolyte membranes, PhD Thesis, Georgia Institute of Technology, 2011.
Application Library path: Polymer_Flow_Module/Tutorials/slot_die_coating_2d
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>Multiphase Flow>Two-Phase Flow, Phase Field>Laminar Flow.
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select Preset Studies for Selected Multiphysics>Time Dependent with Phase Initialization.
6
Load the model parameters from a text file.
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
Click  Load from File.
4
Create a step function to use for ramping up the inlet velocity. To improve convergence, define a smoothing transition zone to gently increase the inlet velocity from zero.
Step 1 (step1)
1
In the Home toolbar, click  Functions and choose Global>Step.
2
In the Settings window for Step, type step1 in the Function name text field.
3
Locate the Parameters section. In the Location text field, type 0.01.
4
Click to expand the Smoothing section. In the Size of transition zone text field, type 0.02.
Create the geometry by using a rectangle and a polygon.
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 W.
4
In the Height text field, type Hc.
5
Locate the Position section. In the x text field, type -W/2.
6
In the y text field, type H.
Add an additional layer at the bottom of the channel. You will use it later to define the initial domain for the coating fluid.
7
Click to expand the Layers section. In the table, enter the following settings:
8
Click  Build Selected.
Polygon 1 (pol1)
1
In the Geometry toolbar, click  Polygon.
2
In the Settings window for Polygon, locate the Coordinates section.
3
4
Click  Build Selected.
5
Click the  Zoom Extents button in the Graphics toolbar.
Compare the resulting geometry to Figure 2.
Definitions
Next define integration operators. First define an integration coupling that integrates along the outlet boundary, to calculate the film thickness. Then define a coupling operator that integrates along the upstream die lip. You will use it later for the integration of the volume fraction along the boundary to evaluate the location of the upstream meniscus.
Integration 1 (intop1)
1
In the Model Builder window, expand the Component 1 (comp1)>Definitions node.
2
Right-click Definitions and choose Nonlocal Couplings>Integration.
3
In the Settings window for Integration, locate the Source Selection section.
4
From the Geometric entity level list, choose Boundary.
5
Integration 2 (intop2)
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
Add Material
Define the materials for the model — air and a coating fluid.
1
In the Home toolbar, click  Add Material to open the Add Material window.
2
Go to the Add Material window.
3
4
Click Add to Component in the window toolbar.
5
In the Home toolbar, click  Add Material to close the Add Material window.
Materials
Coating Fluid
1
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose Blank Material.
2
In the Settings window for Material, type Coating Fluid in the Label text field.
The physics interface and the chosen fluid model will suggest which material properties should be defined.
Multiphysics
Two-Phase Flow, Phase Field 1 (tpf1)
1
In the Model Builder window, under Component 1 (comp1)>Multiphysics click Two-Phase Flow, Phase Field 1 (tpf1).
2
In the Settings window for Two-Phase Flow, Phase Field, locate the Fluid 1 Properties section.
3
From the Fluid 1 list, choose Air (mat1).
4
Locate the Fluid 2 Properties section. From the Fluid 2 list, choose Coating Fluid (mat2).
5
Find the Constitutive relation subsection. From the list, choose Inelastic non-Newtonian.
6
Locate the Surface Tension section. From the Surface tension coefficient list, choose User defined. In the σ text field, type 0.49.
If you have the Optimiziation module in your license, you may use an add-in to calculate the parameters for the power law fluid model based on measurement data in this example. The instructions in the following section show you how to do this. If you do not have access to that license, you may just use the parameters m=7.77 and n=0.86 for the power law coefficients.
In the Home toolbar, click  Windows and choose Add-in Libraries.
Add-in Libraries
1
In the Add-in Libraries window, click  Refresh.
2
In the tree, select Polymer Flow Module>inelastic_non_newtonian_fluid_parameter_estimation.
3
In the tree, select the check box for the node Polymer Flow Module>inelastic_non_newtonian_fluid_parameter_estimation.
4
Root
In the Developer toolbar, click  Add-ins and choose Inelastic Non-Newtonian Fluid Parameter Estimation>Inelastic Non-Newtonian Fluid Parameter Estimation.
Global Definitions
Inelastic Non-Newtonian Fluid Parameter Estimation 1
1
In the Model Builder window, under Global Definitions click Inelastic Non-Newtonian Fluid Parameter Estimation 1.
2
In the Settings window for Inelastic Non-Newtonian Fluid Parameter Estimation, click  Load from File.
3
Click Create to start the parameter estimation.
The power law parameters can now be found in the global parameters table, and thus be used in the material node for the Coating Fluid.
Materials
Coating Fluid (mat2)
1
In the Model Builder window, under Component 1 (comp1)>Materials click Coating Fluid (mat2).
2
In the Settings window for Material, locate the Material Contents section.
3
To avoid having the optimization component in the model, use the Clear button in the add-in to clean up the model tree.
Now, set up the physics of the problem by defining the domain physics conditions and the boundary conditions.
Laminar Flow (spf)
Wall 2
1
In the Model Builder window, under Component 1 (comp1) right-click Laminar Flow (spf) and choose Wall.
2
3
In the Settings window for Wall, locate the Boundary Condition section.
4
From the Wall condition list, choose Navier slip.
5
Click to expand the Wall Movement section. Select the Sliding wall check box.
6
In the Uw text field, type -U_wall.
Inlet 1
1
In the Physics toolbar, click  Boundaries and choose Inlet.
2
3
In the Settings window for Inlet, locate the Velocity section.
4
In the U0 text field, type step1(t[1/s])*U_in.
Open Boundary 1
1
In the Physics toolbar, click  Boundaries and choose Open Boundary.
2
The initial interface between the coating fluid and air is automatically assigned to the boundaries between the two initial value domains. Set up the initial coating fluid domain in the inlet channel.
Phase Field (pf)
Initial Values, Fluid 2
1
In the Model Builder window, under Component 1 (comp1)>Phase Field (pf) click Initial Values, Fluid 2.
2
Wetted Wall 1
1
In the Model Builder window, click Wetted Wall 1.
2
In the Settings window for Wetted Wall, locate the Wetted Wall section.
3
In the θw text field, type 68.5[deg].
Inlet 1
1
In the Physics toolbar, click  Boundaries and choose Inlet.
2
In the Settings window for Inlet, locate the Phase Field Condition section.
3
From the list, choose Fluid 2 (ϕ = 1).
4
Outlet 1
1
In the Physics toolbar, click  Boundaries and choose Outlet.
2
Wetted Wall 2
1
In the Physics toolbar, click  Boundaries and choose Wetted Wall.
2
3
In the Settings window for Wetted Wall, locate the Wetted Wall section.
4
In the θw text field, type 74[deg].
When working with fluids that have large viscosity and density ratios, switching from the default linear method for the properties averaging can increase the performance.
Multiphysics
Two-Phase Flow, Phase Field 1 (tpf1)
1
Click the  Show More Options button in the Model Builder toolbar.
2
In the Show More Options dialog box, in the tree, select the check box for the node Physics>Advanced Physics Options.
3
4
In the Model Builder window, under Component 1 (comp1)>Multiphysics click Two-Phase Flow, Phase Field 1 (tpf1).
5
In the Settings window for Two-Phase Flow, Phase Field, click to expand the Advanced Settings section.
6
From the Density averaging list, choose Heaviside function.
7
In the lρ text field, type 0.9.
8
From the Viscosity averaging list, choose Heaviside function.
9
In the lμ text field, type 0.9.
The mixing parameter can be decreased to sharpen the interface, but that will increase the computation time for this example.
If you want to inspect the progress of the fluids during the simulation, you can enable the plot while solving option in the Step 2: Time Dependent node. By calculating the initial values first, the solver sequence and default plots will be generated. In the following section you generate the default plot groups and use one of them for plotting the volume fraction while solving. Note that plot while solving in general will affect the computation time slightly since the plot needs to be updated in each timestep.
Study 1
In the Study toolbar, click  Get Initial Value.
Step 2: Time Dependent
1
In the Model Builder window, under Study 1 click Step 2: Time Dependent.
2
In the Settings window for Time Dependent, click to expand the Results While Solving section.
3
Select the Plot check box.
4
From the Plot group list, choose Volume Fraction of Fluid 1 (pf).
5
From the Update at list, choose Time steps taken by solver.
6
Locate the Study Settings section. In the Output times text field, type range(0,0.01,0.25).
7
In the Study toolbar, click  Compute.
Examine the default plot at t = 0.03, 0.1, 0.2 (Figure 3)
Results
Volume Fraction of Fluid 1 (pf)
1
In the Model Builder window, under Results click Volume Fraction of Fluid 1 (pf).
2
In the Settings window for 2D Plot Group, locate the Data section.
3
From the Time (s) list, choose 0.03.
4
In the Volume Fraction of Fluid 1 (pf) toolbar, click  Plot.
5
From the Time (s) list, choose 0.1.
6
In the Volume Fraction of Fluid 1 (pf) toolbar, click  Plot.
7
From the Time (s) list, choose 0.2.
8
In the Volume Fraction of Fluid 1 (pf) toolbar, click  Plot.
Proceed to reproduce the plot of the film thickness and the upstream meniscus position Figure 4.
Film Thickness and Upstream Meniscus Position
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Film Thickness and Upstream Meniscus Position in the Label text field.
3
Locate the Legend section. From the Position list, choose Upper left.
Global 1
1
Right-click Film Thickness and Upstream Meniscus Position and choose Global.
2
In the Settings window for Global, locate the y-Axis Data section.
3
A high value (0.95) for the limit of the coating fluid volume fraction is used to safeguard against air entrainment into the coating layer.
4
In the Film Thickness and Upstream Meniscus Position toolbar, click  Plot.