PDF
Rubber Injection Molding
Introduction
Injection molding is a popular way of producing devices and equipment. A polymer fluid is injected into a mold, where it eventually will set to form the desired shape.
This tutorial demonstrates how to model the fluid flow in a rubber injection molding process of an automotive vibration damper using the Laminar Two-Phase Flow, Phase Field interface and an inelastic non-Newtonian power-law model for the rubber. The model geometry and material parameters are inspired from Ref. 1.
Model Definition
Model geometry
The geometry of the vibration damper is an imported CAD file where only the fluid domains are present. A quarter symmetry is used to reduce the computation time. The geometry can be seen in Figure 1.
Figure 1: Model geometry. A quarter piece of the fluid volume of an automotive vibration damper. The fluid inlet can be seen at the top of the small cylinder to the left. While the outlets are to the right in the figure.
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 for the tracking of the interface between the air and the rubber fluid. The coupling of these two interfaces is handled by the Two-Phase Flow, Phase Field multiphysics interface. This model uses the Multiphase Material to define the effective material properties for a material composed of two phases: the air and the rubber. The rubber is a non-Newtonian power-law fluid. The non-Newtonian material properties are specified by using the Power Law material property group.
A small portion of the inlet channel is set up to contain rubber initially. This will automatically define the initial interface between rubber and air.
At the rubber inlet, the fluid velocity is increased smoothly from 0 at t = 0, and the outlets have a uniform pressure, p = 0. The corresponding inlet and outlet boundary conditions must also be set in the Phase Field interface together with the initial values for both fluids, so that the initial interface is correctly defined.
The symmetry planes are defined as Symmetry in both the Laminar flow interface and the Phase field interface. All other boundaries are solid walls described by a no-slip boundary condition.
Results and Discussion
Figure 2-Figure 5 show the propagation of the rubber front as time progresses from t = 1s, t = 4s, t = 8s and t = 16s.
Figure 2: Rubber front after t = 1s.
Figure 3: Rubber front after t = 4s
.
Figure 4: Rubber front after t = 8s.
Figure 5: Rubber front after t = 16s.
The mold is almost completely filled after 16s. The small remaining void near the bottom corner might indicate that the mold design needs to be modified.
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. This example utilizes the Heaviside averaging method.
Reference
1. M. Erfanian, M. Anbarsooz, and M. Moghima, “A three dimensional simulation of a rubber curing process considering variable order of reaction,” Applied Mathematical Modeling, vol. 40, pp. 8592–8604, 2016.
Application Library path: Polymer_Flow_Module/Tutorials/rubber_injection_molding
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 > 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
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
U0
0.1[m/s]
0.1 m/s
Inlet velocity
Geometry 1
Import 1 (imp1)
1
In the Geometry toolbar, click  Import.
2
In the Settings window for Import, locate the Source section.
3
Click  Browse.
4
Browse to the model’s Application Libraries folder and double-click the file rubber_injection_molding.mphbin.
5
Click  Import.
Form Union (fin)
1
In the Model Builder window, click Form Union (fin).
2
In the Settings window for Form Union/Assembly, click  Build Selected.
Explicit Selection 1 (sel1)
1
In the Geometry toolbar, click  Selections and choose Explicit Selection.
2
In the Settings window for Explicit Selection, locate the Entities to Select section.
3
From the Geometric entity level list, choose Boundary.
4
On the object fin, select Boundary 14 only.
5
Locate the Resulting Selection section. From the Show in physics list, choose Off.
6
Find the Cumulative selection subsection. Click New.
7
In the New Cumulative Selection dialog, type Inlet in the Name text field.
8
Click OK.
Explicit Selection 2 (sel2)
1
In the Geometry toolbar, click  Selections and choose Explicit Selection.
2
In the Settings window for Explicit Selection, locate the Entities to Select section.
3
From the Geometric entity level list, choose Boundary.
4
On the object fin, select Boundaries 41 and 43 only.
5
Locate the Resulting Selection section. From the Show in physics list, choose Off.
6
Find the Cumulative selection subsection. Click New.
7
In the New Cumulative Selection dialog, type Outlet in the Name text field.
8
Click OK.
Explicit Selection 3 (sel3)
1
In the Geometry toolbar, click  Selections and choose Explicit Selection.
2
In the Settings window for Explicit Selection, locate the Entities to Select section.
3
From the Geometric entity level list, choose Boundary.
4
On the object fin, select Boundaries 1, 11, 35, and 44 only.
5
Locate the Resulting Selection section. From the Show in physics list, choose Off.
6
Find the Cumulative selection subsection. Click New.
7
In the New Cumulative Selection dialog, type Symmetry in the Name text field.
8
Click OK.
Disable the analysis of the geometry as the remaining small geometric details can be kept.
9
In the Model Builder window, click Geometry 1.
10
In the Settings window for Geometry, locate the Cleanup section.
11
Clear the Automatic detection of small details checkbox.
12
In the Geometry toolbar, click  Build All.
Now, add the material properties for the two phases, air and rubber.
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 Material Properties section.
3
Click  Add Multiphase Material.
Materials
Phase 1 (mpmat1.phase1)
1
In the Model Builder window, under Component 1 (comp1) > Materials > Multiphase Material 1 (mpmat1) click Phase 1 (mpmat1.phase1).
2
In the Settings window for Phase, locate the Link Settings section.
3
Click  Add Material from Library . This button is found when expanding the options next to the Material list.
Add Material to Phase 1 (mpmat1.phase1)
1
Go to the Add Material to Phase 1 (mpmat1.phase1) window.
2
In the tree, select Built-in > Air.
3
Click Add Material.
Materials
Phase 2 (mpmat1.phase2)
1
In the Model Builder window, under Component 1 (comp1) > Materials > Multiphase Material 1 (mpmat1) click Phase 2 (mpmat1.phase2).
2
In the Settings window for Phase, click to expand the Material Properties section.
3
In the Material properties tree, select Fluid Flow > Inelastic Non-Newtonian > Power Law.
4
Click  Add to Material.
5
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Fluid consistency coefficient
m_pow
5503
Pa·s
Power law
Flow behavior index
n_pow
0.2929
1
Power law
Density
rho
1200
kg/m³
Basic
The default method for averaging the viscosity 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 model we use the Heaviside averaging method. The mixing parameter can be made smaller to sharpen the interface, but that will increase the computation time.
Multiphase Material 1 (mpmat1)
1
In the Model Builder window, click Multiphase Material 1 (mpmat1).
2
In the Settings window for Multiphase Material, locate the Material Contents section.
3
Click to select row number 1 in the table.
4
Right-click and choose Edit Mixing Rule.
5
In the Edit Mixing Rule dialog, choose Heaviside function from the Mixing rule list.
6
In the lmix text field, type 0.8.
7
Click  Next Row (Store Changes).
8
From the Mixing rule list, choose Heaviside function.
9
Click OK.
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, in the tree, select the checkbox for the node Physics > Advanced Physics Options.
3
Click OK.
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, locate the Surface Tension section.
6
Clear the Include surface tension force in momentum equation checkbox.
At the startup of a transient simulation of a filling process you can assume that the initial velocity in the domain is zero. To get consistent initial values, the initial velocity at the inlet should also be zero. Use a step function as described in the section below to ramp up the inlet velocity.
Definitions
Step 1 (step1)
1
In the Model Builder window, expand the Component 1 (comp1) > Definitions node.
2
Right-click Definitions and choose Functions > Step.
3
In the Settings window for Step, locate the Parameters section.
4
In the Location text field, type 0.05.
5
Click to expand the Smoothing section. In the Size of transition zone text field, type 0.095.
Variables 1
1
Right-click Definitions and choose Variables.
2
In the Settings window for Variables, locate the Variables section.
3
In the table, enter the following settings:
Name
Expression
Unit
Description
U_in
U0*(step1(t[1/s])-step1(t[1/s]-15))
m/s
Inlet velocity
Laminar Flow (spf)
Inlet 1
1
In the Physics toolbar, click  Boundaries and choose Inlet.
2
In the Settings window for Inlet, locate the Boundary Selection section.
3
From the Selection list, choose Inlet.
4
Locate the Velocity section. In the U0 text field, type U_in.
Outlet 1
1
In the Physics toolbar, click  Boundaries and choose Outlet.
2
In the Settings window for Outlet, locate the Boundary Selection section.
3
From the Selection list, choose Outlet.
Symmetry 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry.
2
In the Settings window for Symmetry, locate the Boundary Selection section.
3
From the Selection list, choose Symmetry.
The initial interface between the rubber fluid and air is automatically assigned to the boundaries between the two initial value domains. Assign the initial values of fluid two to be in the small domain close to the inlet.
Phase Field in Fluids (pf)
Initial Values, Fluid 2
1
In the Model Builder window, under Component 1 (comp1) > Phase Field in Fluids (pf) click Initial Values, Fluid 2.
2
Select Domain 2 only.
Inlet 1
1
In the Physics toolbar, click  Boundaries and choose Inlet.
2
In the Settings window for Inlet, locate the Boundary Selection section.
3
From the Selection list, choose Inlet.
4
Locate the Phase Field Condition section. From the list, choose Fluid 2 (φ = 1).
Outlet 1
1
In the Physics toolbar, click  Boundaries and choose Outlet.
2
In the Settings window for Outlet, locate the Boundary Selection section.
3
From the Selection list, choose Outlet.
Symmetry 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry.
2
In the Settings window for Symmetry, locate the Boundary Selection section.
3
From the Selection list, choose Symmetry.
When working with two-phase flows, the mesh should be fine enough to resolve the initial fluid interface. It is also advantageous to have a relatively uniform mesh element size in the domain. Modify the default mesh sequence to achieve a better mesh for this model.
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
In the table, clear the Use checkbox for Geometric Analysis, Detail Size.
4
Locate the Sequence Type section. From the list, choose User-controlled mesh.
Size
1
In the Model Builder window, under Component 1 (comp1) > Mesh 1 click Size.
2
In the Settings window for Size, locate the Element Size section.
3
Click the Custom button.
4
Locate the Element Size Parameters section. In the Maximum element size text field, type 0.00125/2.
Size 1
1
In the Model Builder window, click Size 1.
2
In the Settings window for Size, locate the Element Size section.
3
Click the Custom button.
4
Locate the Element Size Parameters section.
5
Select the Maximum element size checkbox. In the associated text field, type 0.00125/2.
6
Click  Build All.
Study 1
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, locate the Study Settings section.
3
In the Output times text field, type range(0,1,16).
4
In the Study toolbar, click  Compute.
Results
Injected fluid
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, locate the Data section.
3
From the Time (s) list, choose 8.
4
In the Label text field, type Injected fluid.
5
Locate the Plot Settings section. From the View list, choose New view.
6
In the Injected fluid toolbar, click  Plot to generate a dedicated view for this plot that you can rotate independently of the default view.
7
Click the  Show Axis Orientation button in the Graphics toolbar.
Volume 1
1
Right-click Injected fluid and choose Volume.
2
In the Settings window for Volume, 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 Cyan.
6
Click to expand the Title section. From the Title type list, choose Manual.
7
In the Title text area, type Rubber fluid in mold.
Filter 1
1
Right-click Volume 1 and choose Filter.
2
In the Settings window for Filter, locate the Element Selection section.
3
In the Logical expression for inclusion text field, type pf.Vf2>0.5.
Injected fluid
1
In the Model Builder window, under Results click Injected fluid.
2
In the Settings window for 3D Plot Group, click to expand the Title section.
Surface 1
1
Right-click Injected fluid 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.
6
Click to expand the Title section. From the Title type list, choose None.
Transparency 1
1
Right-click Surface 1 and choose Transparency.
2
In the Settings window for Transparency, locate the Transparency section.
3
Find the Transparency subsection. Set the Transparency value to 0.75.
Injected fluid
1
In the Model Builder window, under Results click Injected fluid.
2
In the Injected fluid toolbar, click  Plot.