PDF
Disc Brake Pad Wear
Introduction
This example demonstrates how to compute wear of the friction material in a disc brake. Wear is modeled using a generalized form of the well-known Archard equation. The sliding velocity and the friction forces are computed from simple kinematic considerations. In addition, it is assumed that the disc has a much higher wear resistance than the pad, that is, only wear of the friction material has to be considered. Thermal effects on the wear rate and thermal expansion are neglected.
Model Definition
The simplified geometry of the disc and brake pad assembly is shown in Figure 1. Assuming a symmetric geometry, only half of the assembly needs to be modeled.
Figure 1: Disc brake geometry.
The entire assembly is considered to be linear elastic, and the brake disc is given material properties of steel. The material of the brake pad is assumed to have a stiffness that is one order or magnitude lower than that of the disc. All material properties are summarized in Table 1.
Table 1: Material Properties.
Property
Disc
Pad
Young’s modulus
210 GPa
10 GPa
Poisson's ratio
0.3
0.1
Density
7850 kg/m3
2000 kg/m3
The interaction between the disc and the pad is modeled using a contact condition. To ensure that the contact pressure is well resolved, the augmented Lagrangian method is used. The contact pressure is initiated by adding a boundary load to the top surface of the brake pad, and the effect of friction forces is accounted for by prescribing a relative slip velocity between the two parts. The angular velocity, ω, of the brake disc is assumed to be constant during the analysis. Since the origin of the global coordinate system is located in the center of the disc, the relative slip velocity, vslip, between the pad and the disc is given as
where r is the position vector to any point on the pad.
Wear involves a gradual removal of material at the surfaces in contact, and the process can be described with a rate equation. In this example, a generalized form of the Archard wear model is used, where the wear rate is given as
Here, hwear is the wear depth, kwear is a dimensionless wear constant, Tn is the contact pressure, Tn,ref is a reference pressure, n is a dimensionless exponent. By default, Tn,ref is set to 1 MPa and n to 1, which makes the above equation correspond to the classical form of the Archard wear equation.
Results and Discussion
Figure 2 shows the distribution of the von Mises stress at the end of the simulation. At this point, material has been removed due to wear causing any initial peak in the stress to be smoothened out,
Figure 2: Distribution of von Mises stress in the pad and disc assembly.
If the contact between the pad and the disc was frictionless, the contact pressure would have a symmetric distribution over the pad surface. However, including friction forces results in a higher contact pressure at the leading edge of the brake pad compared to its trailing edge. This is shown in Figure 3 for the worn brake pad. As a result of the locally higher pressure, the wear rate, and subsequently the wear depth, is larger at the leading edge, see Figure 4. Due to the geometric changes resulting from the removal of material, the pressure distribution changes and the pressure peak at the leading edge eventually decreases over time.
Figure 3: Pressure distribution of the worn pad surface.
Figure 4: Distribution of the accumulated wear depth.
Notes About the COMSOL Implementation
The initial contact problem is solved in a first stationary study. By adding a Slip Velocity subnode to the Contact node, you can solve for dynamic friction forces even in a stationary study. To solve for the wear depth, add a second time-dependent study, and initialize the study with the values from the first study.
Wear is in this example modeled using the deformed geometry concept. This means that geometry of the brake pad changes with time by using an adaptive meshing technique. Using this method to model wear thus also updates the contact conditions accordingly during the simulation.
Usually, wear problems require long time periods to generate any significant wear depths. One approach to avoid running long-term studies is to multiply the wear rate with an acceleration factor. The result may be interpreted as running the simulation for a time t times the wear acceleration factor, where t is the actual time period used in the simulation.
Application Library path: Structural_Mechanics_Module/Contact_and_Friction/disc_brake_wear
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 Structural Mechanics>Solid Mechanics (solid).
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies>Stationary.
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
v
60[km/h]
16.667 m/s
Vehicle speed
r_wheel
0.25[m]
0.25 m
Wheel radius
omega
v/r_wheel
66.667 1/s
Wheel angular velocity
wear_accel
100
100
Wear acceleration factor
Geometry 1
1
In the Geometry toolbar, click  Insert Sequence.
2
Browse to the model’s Application Libraries folder and double-click the file disc_brake_geom_sequence.mph.
Form Assembly (fin)
1
In the Model Builder window, under Component 1 (comp1)>Geometry 1 click Form Assembly (fin).
2
In the Settings window for Form Union/Assembly, locate the Form Union/Assembly section.
3
Select the Create pairs check box.
4
From the Pair type list, choose Contact pair.
5
In the Geometry toolbar, click  Build All.
Definitions
Contact Pair 1 (ap1)
1
In the Model Builder window, expand the Component 1 (comp1)>Definitions node, then click Contact Pair 1 (ap1).
2
In the Settings window for Pair, locate the Advanced section.
3
From the Mapping method list, choose Initial configuration.
Cylindrical System 2 (sys2)
A boundary system is used to define the orientation of the relative slip velocity between the pad and the disc. In this case it is convenient to define the orientation of the boundary system axes based on cylindrical coordinates.
In the Definitions toolbar, click  Coordinate Systems and choose Cylindrical System.
Boundary System 1 (sys1)
1
In the Model Builder window, click Boundary System 1 (sys1).
2
In the Settings window for Boundary System, locate the Settings section.
3
From the Frame list, choose Reference configuration.
4
Find the Coordinate names subsection. From the Create first tangent direction from list, choose Cylindrical System 2 (sys2).
5
From the Axis list, choose phi.
Materials
Disc
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 Disc in the Label text field.
3
Locate the Geometric Entity Selection section. In the list, select 3.
4
Click  Remove from Selection.
5
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
210[GPa]
Pa
Basic
Poisson’s ratio
nu
0.3
1
Basic
Density
rho
7850[kg/m^3]
kg/m³
Basic
6
Click to expand the Appearance section. From the Material type list, choose Steel.
7
Click the Show Material Color and Texture button in the Graphics toolbar.
Pad
1
Right-click Materials and choose Blank Material.
2
Select Domain 3 only.
3
In the Settings window for Material, type Pad in the Label text field.
4
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
10[GPa]
Pa
Basic
Poisson’s ratio
nu
0.1
1
Basic
Density
rho
2000
kg/m³
Basic
5
Click to expand the Appearance section. From the Color list, choose Black.
Solid Mechanics (solid)
Wear is a slow process and inertial effects can be neglected.
1
In the Model Builder window, under Component 1 (comp1) click Solid Mechanics (solid).
2
In the Settings window for Solid Mechanics, locate the Structural Transient Behavior section.
3
From the list, choose Quasistatic.
Fixed Constraint 1
1
In the Physics toolbar, click  Boundaries and choose Fixed Constraint.
2
Select Boundary 8 only.
Symmetry 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry.
2
Select Boundary 3 only.
Prescribed Displacement 1
1
In the Physics toolbar, click  Boundaries and choose Prescribed Displacement.
2
In the Settings window for Prescribed Displacement, locate the Prescribed Displacement section.
3
Select the Prescribed in x direction check box.
4
Select the Prescribed in y direction check box.
5
Select Boundary 16 only.
Boundary Load 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundary 16 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
From the Load type list, choose Total force.
5
Specify the Ftot vector as
0
x
0
y
-10[kN]
z
Contact 1
1
In the Physics toolbar, click  Pairs and choose Contact.
2
In the Settings window for Contact, locate the Pair Selection section.
3
Under Pairs, click  Add.
4
In the Add dialog box, select Contact Pair 1 (ap1) in the Pairs list.
5
Click OK.
6
In the Settings window for Contact, locate the Contact Method section.
7
From the Formulation list, choose Augmented Lagrangian.
8
Locate the Contact Pressure Penalty Factor section. From the Tuned for list, choose Speed.
9
Locate the Initial Value section. In the Tn text field, type 5e6.
Slip Velocity 1
1
In the Physics toolbar, click  Attributes and choose Slip Velocity.
2
In the Settings window for Slip Velocity, locate the Friction Parameters section.
3
In the μ text field, type 0.45.
4
Locate the Prescribed Velocity section. Specify the vslip vector as
omega*sys2.r
t1
0
t2
The input is given in the boundary system selected in the Coordinate System Selection section.
5
Click the  Show More Options button in the Model Builder toolbar.
6
In the Show More Options dialog box, in the tree, select the check box for the node Physics>Advanced Physics Options.
7
Click OK.
8
In the Settings window for Slip Velocity, click to expand the Advanced section.
9
Select the Store accumulated slip check box.
Contact 1
In the Model Builder window, click Contact 1.
Wear 1
1
In the Physics toolbar, click  Attributes and choose Wear.
2
In the Settings window for Wear, locate the Wear Model section.
3
In the kwear text field, type 1e-14*wear_accel.
Mesh 1
Free Triangular 1
1
In the Mesh toolbar, click  Boundary and choose Free Triangular.
2
Select Boundaries 4 and 8 only.
Size Expression 1
1
Right-click Free Triangular 1 and choose Size Expression.
2
In the Settings window for Size Expression, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Boundary.
4
Select Boundaries 4 and 8 only.
5
Locate the Element Size Expression section. In the Size expression text field, type if((x/60[mm])^2+((y-115[mm])/40[mm])^2<1, 6[mm], 40[mm]).
6
Click to expand the Smoothing section. In the Maximum size field growth rate text field, type 1.25.
Swept 1
1
In the Mesh toolbar, click  Swept.
2
In the Settings window for Swept, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domains 1 and 2 only.
Distribution 1
1
Right-click Swept 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
In the Number of elements text field, type 2.
Free Triangular 2
1
In the Mesh toolbar, click  Boundary and choose Free Triangular.
2
Select Boundary 16 only.
Size 1
1
Right-click Free Triangular 2 and choose 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. Select the Maximum element size check box.
5
In the associated text field, type 3.5[mm].
Swept 2
In the Mesh toolbar, click  Swept.
Distribution 1
1
Right-click Swept 2 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
In the Number of elements text field, type 3.
4
Click  Build All.
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
In the table, clear the Solve for check box for Deformed geometry (Component 1).
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 1 (sol1) node.
3
In the Model Builder window, expand the Study 1>Solver Configurations>Solution 1 (sol1)>Dependent Variables 1 node, then click Contact pressure (comp1.solid.Tn_ap1).
4
In the Settings window for Field, locate the Scaling section.
5
In the Scale text field, type 5e6.
6
In the Study toolbar, click  Compute.
Results
Use the default contact plot to verify that the initial friction forces on the brake pad, as computed by the Slip Velocity node, act in the expected direction.
Contact 1, Pressure
1
In the Model Builder window, expand the Contact Forces (solid) node.
2
Right-click Contact 1, Pressure and choose Disable.
Color Expression
1
In the Model Builder window, expand the Contact 1, Friction force node, then click Color Expression.
2
In the Settings window for Color Expression, locate the Coloring and Style section.
3
From the Coloring list, choose Color table.
4
From the Color table list, choose RainbowLight.
Root
In the Home toolbar, click  Windows and choose Add Study.
Add Study
1
Go to the Add Study window.
2
Find the Studies subsection. In the Select Study tree, select General Studies>Time Dependent.
3
Click Add Study in the window toolbar.
4
In the Home toolbar, click  Add Study to close the Add Study window.
Study 2
Step 1: Time Dependent
1
In the Settings window for Time Dependent, locate the Study Settings section.
2
In the Output times text field, type range(0, 0.1, 5).
3
From the Tolerance list, choose User controlled.
4
In the Relative tolerance text field, type 1e-3.
5
Click to expand the Values of Dependent Variables section. Find the Initial values of variables solved for subsection. From the Settings list, choose User controlled.
6
From the Method list, choose Solution.
7
From the Study list, choose Study 1, Stationary.
8
In the Study toolbar, click  Get Initial Value.
Results
Wear Depth
1
In the Home toolbar, click  Add Plot Group and choose 3D Plot Group.
2
In the Settings window for 3D Plot Group, type Wear Depth in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study 2/Solution 2 (sol2).
4
Locate the Plot Settings section. Clear the Plot dataset edges check box.
Surface 1
1
Right-click Wear Depth and choose Surface.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type 1.
Selection 1
1
Right-click Surface 1 and choose Selection.
2
In the Settings window for Selection, locate the Selection section.
3
Click  Paste Selection.
4
In the Paste Selection dialog box, type 1-12 in the Selection text field.
5
Click OK.
Material Appearance 1
In the Model Builder window, right-click Surface 1 and choose Material Appearance.
Arrow Surface 1
1
In the Model Builder window, right-click Wear Depth and choose Arrow Surface.
2
In the Settings window for Arrow Surface, locate the Expression section.
3
In the X component text field, type omega*(sin(-omega*t/200)*x + cos(-omega*t/200)*y).
4
In the Y component text field, type -omega*(cos(-omega*t/200)*x - sin(-omega*t/200)*y).
5
In the Z component text field, type 0.
6
Locate the Arrow Positioning section. In the Number of arrows text field, type 100.
7
Locate the Coloring and Style section. From the Color list, choose Black.
Selection 1
1
Right-click Arrow Surface 1 and choose Selection.
2
Select Boundary 4 only.
Deformation 1
1
In the Model Builder window, right-click Arrow Surface 1 and choose Deformation.
2
In the Settings window for Deformation, locate the Expression section.
3
In the X component text field, type cos(-omega*t/200)*x - sin(-omega*t/200)*y - x.
4
In the Y component text field, type sin(-omega*t/200)*x + cos(-omega*t/200)*y - y.
5
In the Z component text field, type 0.
6
Click to expand the Title section. Locate the Scale section. Select the Scale factor check box.
7
In the associated text field, type 1.
Surface 2
1
In the Model Builder window, right-click Wear Depth and choose Surface.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type solid.htot.
4
In the Unit field, type um.
5
Click to expand the Quality section. Locate the Coloring and Style section. From the Color table list, choose WaveLight.
Selection 1
1
Right-click Surface 2 and choose Selection.
2
In the Settings window for Selection, locate the Selection section.
3
Click  Paste Selection.
4
In the Paste Selection dialog box, type 15 in the Selection text field.
5
Click OK.
Deformation 1
1
In the Model Builder window, right-click Surface 2 and choose Deformation.
2
In the Settings window for Deformation, locate the Expression section.
3
In the X component text field, type 0.
4
In the Y component text field, type 0.
5
In the Z component text field, type 2[mm].
6
Locate the Scale section. Select the Scale factor check box.
7
In the associated text field, type 1.
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, click to expand the Results While Solving section.
3
Select the Plot check box.
4
From the Plot group list, choose Wear Depth.
Solver Configurations
In the Model Builder window, expand the Study 2>Solver Configurations node.
Solution 2 (sol2)
1
In the Model Builder window, expand the Study 2>Solver Configurations>Solution 2 (sol2)>Dependent Variables 1 node, then click Contact pressure (comp1.solid.Tn_ap1).
2
In the Settings window for Field, locate the Scaling section.
3
In the Scale text field, type 5e6.
4
In the Model Builder window, click Time-Dependent Solver 1.
5
In the Settings window for Time-Dependent Solver, click to expand the Time Stepping section.
6
From the Steps taken by solver list, choose Strict.
7
Find the Algebraic variable settings subsection. From the Consistent initialization list, choose Off.
8
In the Model Builder window, expand the Study 2>Solver Configurations>Solution 2 (sol2)>Time-Dependent Solver 1>Segregated 1 node, then click Solid Mechanics.
9
In the Settings window for Segregated Step, locate the General section.
10
Under Variables, click  Add.
11
In the Add dialog box, select Material mesh displacement (comp1.material.disp) in the Variables list.
12
Click OK.
13
In the Settings window for Segregated Step, click to expand the Method and Termination section.
14
From the Nonlinear method list, choose Constant (Newton).
15
From the Termination technique list, choose Tolerance.
16
In the Model Builder window, under Study 2>Solver Configurations>Solution 2 (sol2)>Time-Dependent Solver 1>Segregated 1 right-click Material frame coordinates and choose Delete.
17
In the Home toolbar, click  Compute.
Results
Surface 1
1
In the Results toolbar, click  More Datasets and choose Surface.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Study 2/Solution 2 (sol2).
4
Locate the Parameterization section. From the x- and y-axes list, choose XY-plane.
5
Locate the Selection section. Click  Paste Selection.
6
In the Paste Selection dialog box, type 15 in the Selection text field.
7
Click OK.
Plot the contact pressure. In order to correctly interpolate from discrete Gauss point data to a continuous field, the pressure variable is wrapped in a gpeval() operator.
Pressure Distribution
1
In the Results toolbar, click  2D Plot Group.
2
In the Settings window for 2D Plot Group, type Pressure Distribution in the Label text field.
3
Locate the Data section. From the Dataset list, choose Surface 1.
Surface 1
1
Right-click Pressure Distribution and choose Surface.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type gpeval(4, solid.cnt1.wear1.Tn).
4
From the Unit list, choose MPa.
5
In the Pressure Distribution toolbar, click  Plot.
Slip Distance
1
In the Model Builder window, right-click Pressure Distribution and choose Duplicate.
2
In the Settings window for 2D Plot Group, type Slip Distance in the Label text field.
Surface 1
1
In the Model Builder window, expand the Slip Distance node, then click Surface 1.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type gpeval(4, solid.sliptot)*wear_accel.
4
From the Unit list, choose km.
5
In the Slip Distance toolbar, click  Plot.
Wear Rate
1
In the Model Builder window, right-click Slip Distance and choose Duplicate.
2
In the Settings window for 2D Plot Group, type Wear Rate in the Label text field.
Surface 1
1
In the Model Builder window, expand the Wear Rate node, then click Surface 1.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type gpeval(4, solid.h_tEff).
4
In the Unit field, type um/s.
5
In the Wear Rate toolbar, click  Plot.
Evaluation Group 1
1
In the Results toolbar, click  Evaluation Group.
2
In the Settings window for Evaluation Group, locate the Data section.
3
From the Dataset list, choose Study 2/Solution 2 (sol2).
4
From the Time selection list, choose Last.
Surface Average 1
1
Right-click Evaluation Group 1 and choose Average>Surface Average.
2
In the Settings window for Surface Average, locate the Selection section.
3
Click  Paste Selection.
4
In the Paste Selection dialog box, type 15 in the Selection text field.
5
Click OK.
6
In the Settings window for Surface Average, locate the Expressions section.
7
In the table, enter the following settings:
Expression
Unit
Description
solid.htot
um
Average wear depth
Surface Minimum 1
1
In the Model Builder window, right-click Evaluation Group 1 and choose Minimum>Surface Minimum.
2
In the Settings window for Surface Minimum, locate the Selection section.
3
Click  Paste Selection.
4
In the Paste Selection dialog box, type 15 in the Selection text field.
5
Click OK.
6
In the Settings window for Surface Minimum, locate the Expressions section.
7
In the table, enter the following settings:
Expression
Unit
Description
solid.htot
um
Minimum wear depth
Surface Maximum 1
1
Right-click Evaluation Group 1 and choose Maximum>Surface Maximum.
2
In the Settings window for Surface Maximum, locate the Selection section.
3
Click  Paste Selection.
4
In the Paste Selection dialog box, type 15 in the Selection text field.
5
Click OK.
6
In the Settings window for Surface Maximum, locate the Expressions section.
7
In the table, enter the following settings:
Expression
Unit
Description
solid.htot
um
Maximum wear depth
8
In the Evaluation Group 1 toolbar, click  Evaluate.