Inkjet Nozzle — Level Set Method

Inkjet printers are attractive tools for printing text and images because they combine low cost and high resolution with acceptable speed. The working principle behind inkjet technology is to eject small droplets of liquid from a nozzle onto a sheet of paper. Important properties of a printer are its speed and the resolution of the final images. Designers can vary several parameters to modify a printer’s performance. For instance, they can vary the inkjet geometry and the type of ink to create droplets of different sizes. The size and speed of the ejected droplets are also strongly dependent on the speed at which ink is injected into the nozzle. Simulations can be useful to improve the understanding of the fluid flow and to predict the optimal design of an inkjet for a specific application.

Although initially invented to produce images on paper, the inkjet technique has since been adopted for other application areas. Instruments for the precise deposition of microdroplets often employ inkjets. These instruments are used within the life sciences for diagnosis, analysis, and drug discovery. Inkjets have also been used as 3D printers to synthesize tissue from cells and to manufacture microelectronics. For all of these applications it is important to be able to accurately control the inkjet performance.

This example demonstrates how to model the fluid flow within an inkjet using the Laminar Two-Phase Flow, Level Set interface.

Model Definition

Figure 1 shows the geometry of the inkjet studied in this example. Because of its symmetry you can use an axisymmetric 2D model. Initially, the space between the inlet and the nozzle is filled with ink. Additional ink is injected through the inlet during a period of 10 μs, and it consequently forces ink to flow out of the nozzle. When the injection stops, a droplet of ink snaps off and continues to travel until it hits the target.

Figure 1: Geometry of the inkjet.

Representation and Convection of the Fluid Interface

Level Set Method

The Laminar Two-Phase Flow, Level Set interface uses a reinitialized, conservative level set method to describe and convect the fluid interface. The 0.5 contour of the level set function

defines the interface, where

equals 0 in air and 1 in ink. In a transition layer close to the interface,

goes smoothly from 0 to 1. The interface moves with the fluid velocity, u, at the interface. The following equation describes the convection of the reinitialized level set function:

The thickness of the transition layer is proportional to ε. For this model you can use ε = hc/2, where hc is the typical mesh size in the region passed by the droplet.

The parameter γ determines the amount of reinitialization. A suitable value for γ is the maximum magnitude occurring in the velocity field.

Beside defining the fluid interface, the level set function is used to smooth the density and viscosity jumps across the interface through the definitions

Transport of Mass and Momentum

The incompressible Navier-Stokes equations, including surface tension, describe the transport of mass and momentum. Both ink and air can be considered incompressible as long as the fluid velocity is small compared to the speed of sound. The Navier-Stokes equations are

Here, ρ denotes density (kg/m3), μ equals the dynamic viscosity (N·s/m2), u represents the velocity (m/s), p denotes pressure (Pa), and Fst is the surface tension force.

The surface tension force is computed as

where n is the interface normal, σ is the surface tension coefficient (N/m),

is the curvature, and δ equals a Dirac delta function that is nonzero only at the fluid interface. The normal to the interface is

while the delta function is approximated by

The following table gives the physical parameters of ink and air used in the model:


Medium	Density	Dynamic Viscosity	Surface tension
ink	103 kg/m3	0.01 N·s/m2	0.07 N/m
air	1.225 kg/m3	1.789·10-5 N·s/m2

Initial Conditions

Figure 2 shows the initial distribution (t = 0) of ink and air. The velocity is initially 0.

Figure 2: Initial distribution of ink. Black corresponds to ink and white corresponds to air.

Boundary Conditions

Inlet

The inlet velocity in the z direction increases from 0 to the parabolic profile

during the first 2 μs. The velocity is then v(r) for 10 μs and finally decreases to 0 for another 2 μs. The time-dependent velocity profile in the z direction can then be defined as

where t is given in seconds and rect(t) is a smooth rectangular pulse function with the transition points at 1 μs and 13 μs with a 2 μs transition period. (see Figure 3).

Figure 3: Smooth step function.

Use

as the inlet boundary condition for the level set variable.

Outlet

Set a constant pressure at the outlet. The value of the pressure given here is not important because the velocity depends only on the pressure gradient. You thus obtain the same velocity field regardless of whether the pressure is set to 1 atm or to 0.

Walls

On all other boundaries except the target, set No slip conditions. Use the Wetted wall condition on the target, with a contact angle of π/2 and a slip length of 10 μm.

Results and Discussion

Figure 4 shows the ink surface and the velocity field at different times.

Figure 4: Position of air/ink interface and velocity field at various times.

Figure 5 illustrates the mass of ink that is further than 0.7 mm from the inlet. The figure shows that the mass of the ejected droplet is approximately 2·10−10 kg.

Figure 5: Amount of ink from just above the nozzle.

This example studies only one inkjet model, but it is easy to modify the model in several ways. You can, for example, change properties such as the geometry or the inlet velocity and study the influence on the size and the speed of the ejected droplets. You can also investigate how the inkjet would perform if the ink were replaced by a different fluid. It is also easy to add forces such as gravity to the model.

Notes About the COMSOL Implementation

You can readily set up the model using the Laminar Two-Phase Flow, Level Set interface. This interface adds the equations automatically, and you need only specify physical parameters of the fluids and the initial and boundary conditions.

In order to accurately resolve the interface between the air and ink, use the adaptive meshing. This means that as the interface moves during the simulation, the mesh is updated in order to keep the mesh refined in the interface region.

The simulation procedure involves two consecutive computations. First you calculate a smooth initial solution for the level set variable. Using this initial solution, you then start the time-dependent simulation of the fluid motion.

To calculate the droplet’s mass, use a nonlocal integration coupling. To visualize the droplet in 3D, revolve the 2D axially symmetric solution to a 3D geometry.

References

1. J.-T. Yeh, “A VOF-FEM Coupled Inkjet Simulation,” Proc. ASME FEDSM’01, New Orleans, Louisiana, 2001.

2. E. Olsson and G. Kreiss, “A Conservative Level Set Method for Two Phase Flow,” J. Comput. Phys., vol. 210, pp. 225–246, 2005.

3. P. Yue, J. Feng, C. Liu, and J. Shen, “A Diffuse-Interface Method for Simulating Two-Phase Flows of Complex Fluids,” J. Fluid Mech., vol. 515, pp. 293–317, 2004.

CFD_Module/Multiphase_Flow/inkjet_nozzle_ls

Modeling Instructions

From the menu, choose .

New

In the window, click

Model Wizard

In the window, click

In the tree, select .

Click .

Click

In the tree, select .

Click

It is convenient to add some parameters for the geometry.

Global Definitions

Parameters 1

In the window, under click .

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Value	Description
InletR	0.1[mm]	1E-4 m	Nozzle inlet radius
NozzleL	0.375[mm]	3.75E-4 m	Nozzle length
NozzleR	0.025[mm]	2.5E-5 m	Nozzle radius
ThroatL	0.025[mm]	2.5E-5 m	Throat length
TargetL	1 [mm]	0.001 m	Distance to target
AirW	0.1[mm]	1E-4 m	Air channel width

Geometry 1

In the window, under click .

In the window for , locate the section.

From the list, choose .

Rectangle 1 (r1)

In the toolbar, click

In the window for , locate the section.

In the text field, type InletR.

In the text field, type 2*InletR.

Polygon 1 (pol1)

In the toolbar, click

In the window for , locate the section.

In the table, enter the following settings:


r (mm)	z (mm)
0	2*InletR
InletR	2*InletR
NozzleR	2*InletR+NozzleL
0	2*InletR+NozzleL

Click

Click the

button in the toolbar.

Rectangle 2 (r2)

In the window, under right-click and choose .

In the window for , locate the section.

In the text field, type NozzleR.

In the text field, type ThroatL+TargetL.

Locate the section. In the text field, type NozzleL+2*InletR.

Rectangle 3 (r3)

Right-click and choose .

In the window for , locate the section.

In the text field, type AirW.

In the text field, type TargetL.

Locate the section. In the text field, type ThroatL+NozzleL+2*InletR.

Rectangle 4 (r4)

Right-click and choose .

In the window for , locate the section.

In the text field, type 2*AirW.

In the text field, type AirW.

Locate the section. In the text field, type ThroatL+NozzleL+2*InletR+TargetL-AirW.

Click

Click the

button in the toolbar.

Form Union (fin)

In the window, click .

In the window for , click

This completes the geometry modeling stage.

Materials

Ink

In the window, under right-click and choose .

In the window for , locate the section.

In the table, enter the following settings:


Property	Variable	Value	Unit	Property group
Density	rho	1e3[kg/m^3]	kg/m³	Basic
Dynamic viscosity	mu	1e-2[Pa*s]	Pa·s	Basic

Right-click and choose .

In the dialog box, type Ink in the text field.

Click .

Add Material

In the toolbar, click

to open the window.

Go to the window.

In the tree, select .

Click in the window toolbar.

In the toolbar, click

to close the window.

Materials

Air (mat2)

Now, define a rectangular pulse function to use when defining the time dependence of the inlet velocity.

Global Definitions

Rectangle 1 (rect1)

In the toolbar, click

and choose .

In the window for , click to expand the section.

Locate the section. In the text field, type 1e-6.

In the text field, type 13e-6.

Locate the section. In the text field, type 2e-6.

Click

Next, define a nonlocal integration coupling that you will use when defining a variable for the droplet mass.

Definitions

Integration 1 (intop1)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

After these preliminaries, you can define variables for the inlet velocity and the droplet mass.

Variables 1

In the toolbar, click

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Unit	Description
v_in	0.56[m/s]*rect1(t[1/s])	m/s	Inlet velocity
m_d	intop1(1e3[kg/m^3]phils(z>0.7[mm]))	kg	Droplet mass

Multiphysics

Two-Phase Flow, Level Set 1 (tpf1)

In the window, under click .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

Locate the section. Select the check box.

From the list, choose . In the σ text field, type 0.07.

Laminar Flow (spf)

Inlet 1

In the window, under right-click and choose .

Select Boundary 2 only.

In the window for , locate the section.

From the list, choose .

Locate the section. In the Uav text field, type v_in.

Outlet 1

In the toolbar, click

and choose .

Select Boundary 24 only.

Level Set (ls)

Level Set Model 1

In the window, under click .

In the window for , locate the section.

In the εls text field, type 2.5e-6.

In the γ text field, type 10.

Initial Values, Fluid 2

In the window, click .

Select Domains 1–3 only.

Inlet 1

In the toolbar, click

and choose .

Select Boundary 2 only.

In the window for , locate the section.

From the list, choose ϕ .

Outlet 1

In the toolbar, click

and choose .

Select Boundary 24 only.

Multiphysics

Wetted Wall 1 (ww1)

In the window, under click .

Select Boundaries 11–13, 15, 18–20, 22, and 23 only.

In the window for , locate the section.

From the list, choose . In the β text field, type 10[um].

Mesh 1

In the window, under right-click and choose .

Study 1

Step 2: Time Dependent

In the window, under click .

In the window for , locate the section.

In the text field, type range(0,10e-6,200e-6).

Click to expand the section. Select the check box.

This choice means that the window will show a contour line of the volume fraction of Fluid 1 and velocity field while solving, and this plot will be updated at each output time step.

Click to expand the section. Select the check box.

By adjusting the scaling of the fields manually, you can reduce the computation time.

Solution 1 (sol1)

In the toolbar, click

In the window, expand the node.

In the window, expand the node, then click .

In the window for , locate the section.

From the list, choose .

In the text field, type 10.

In the window, click .

In the window for , locate the section.

From the list, choose .

In the text field, type 1e4.

In the toolbar, click

Results

Edge 2D 1

In the toolbar, click

and choose .

Select Boundaries 12, 13, 15, 19, 20, 22, and 24 only.

Revolution 2D 3

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Click to expand the section. In the text field, type 230.

Edge 2D 2

In the toolbar, click

and choose .

Select Boundaries 12, 13, and 19 only.

Revolution 2D 4

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. In the text field, type 230.

In the text field, type 130.

Isosurface 1

In the window, expand the node, then click .

In the window for , locate the section.

From the list, choose .

Slice 1

In the window, right-click and choose .

In the window for , locate the section.

From the list, choose .

In the text field, type 1.

Locate the section. From the list, choose .

Surface 1

Right-click and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

From the list, choose .

Surface 2

Right-click and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

From the list, choose .

Volume Fraction of Fluid 1 (ls) 1

In the window, click .

In the window for , locate the section.

From the list, choose .

Locate the section. Clear the check box.

In the toolbar, click

Click the

button in the toolbar.

Locate the section. From the list, choose .

In the toolbar, click

Compare the resulting plot with that in the upper panel of Figure 4.To create the remaining plots, plot the solution for the time values 2e-5, 4e-5, 8e-5, 1.2e-4, 1.6e-4, and 2e-4.

1D Plot Group 6

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. Clear the check box.

Global 1

Right-click and choose .

In the window for , click in the upper-right corner of the section. From the menu, choose .

In the toolbar, click