PDF
Standing Contact Fatigue
Introduction
In the vicinity of a point where two parts are in contact, a surface crack has been observed in a component. There is no relative movement between the two contact interfaces; however, the contact pressure varies in time. After a long operating time, a surface crack has been observed. A further analysis of the failed component reveals that multiple cracks are present on the subsurface level. In order to gain understanding of the failure mechanism, an analysis of standing contact fatigue is performed.
The component is surface hardened. Through this procedure the near surface layer significantly changes its material properties. Both the strength, hardening and the fatigue properties are affected. Moreover a residual stress is introduced throughout the depth.
Model Definition
In a standing contact fatigue test a spherical indenter of a hard material is pressed against the tested material. The failed component is made of surface hardened chromoly steel. Through the process of surface hardening the material has undergone metallurgical changes and can be considered to consist of three distinct layers, as shown in Figure 1.
Figure 1: Standing contact fatigue material testing.
The harder surface layer is commonly called the case and the unmodified material inside the component is called the core. Between these two layers there is a thin layer called the transition layer where the material properties varies strongly through the depth.
In the test the indenter is pressed and released so that the maximum contact pressure varies between 2.7 GPa and 0 GPa.
Material properties
The elastic properties are the constant throughout the depth, with Young’s modulus and Poisson’s ratio being E = 206 GPa and ν = 0.31, respectively.
The plastic properties varies in the three layers. The hardening in the case can be considered linear and isotropic defined by
(1)
where σys is the yield stress, and εep is the equivalent plastic strain. The material constants initial yield stress and isotropic tangent modulus are set to σys0 = 570 MPa and ETiso = 69 GPa, respectively.
The core follows an isotropic exponential hardening function, also called Ludwik hardening, given by the expression
where the material constants initial yield stress, strength coefficient, and hardening exponent are given by σys0 = 515 MPa, k = 2.47 GPa and n = 0.55.
Plastic data are not directly available for the transition layer. However since the material behavior varies significantly in the transition layer it must be dependent on the distance from the surface. Moreover at the interface with the core the plastic law should follow the ore hardening function and at the interface with the case it should follow the case hardening function. In order to use a single hardening function in the transition layer, the linear isotropic hardening in the case is transformed into a Ludwik hardening with following material constants: σys0 = 570 MPa, k = 103 GPa, and n = 1.0. The variation of the parameters in the transition layer is assumed to be
•
linear in the initial yield stress,
•
linear in the logarithm of the strength coefficient,
•
linear in the hardening exponent.
The assumption leads to the following expressions for the material parameters:
 MPa
where s is a local coordinate in the transition layer which varies linearly with the depth and is 0 at case interface and 1 at core interface. The stress-strain curve at different levels in the transition layer is shown in Figure 2.
Figure 2: Hardening functions in the transition layer. s = 0 denotes the interface with the case and s = 1 denotes the interface with the core.
Residual stress
The hardening process introduces a compressive stress in the case and a tensile stress in the core. The two in-plane components of the direct stress in the case are −500 MPa and in the core 100 MPa. The profile of the residual stress in the transition layer is assumed to vary linearly.
Fatigue Data
The Dang Van model is used to evaluate fatigue. For the case material the Dang Van material parameters are a = 0.19 and b = 282 MPa. For the core material the Dang Van material parameters are a = 0.23 and b = 248 MPa.
Numerical model
The tested material volume is large in comparison with the indenter which has a radius, ri, of 7,0 mm. In the model the indenter is replaced with a Hertzian contact pressure distribution obtained from the following set of expressions
where ai is the contact radius, and P is the contact load. The relation between the contact load and the pressure distribution is given by
where p0 is the peak contact pressure in the contact zone and p is the contact pressure at the radial coordinate r.
In the testing a maximum pressure of 2.7 GPa is applied. This corresponds to a maximum load of 384 N and a maximum contact radius of 0.26 mm. In the model, the size of the geometry must be sufficiently large so that the far boundaries do not affect the stress state at the contact zone.
Since the geometry is axially symmetric, a 2D axial symmetry Solid Mechanics interface is used. The radius and the height of the model are selected to 5 mm. The case is 0.5 mm deep and the transition layer is 0.1 mm. A roller boundary condition is used at the bottom and at the far radial boundary.
Results and Discussion
The stress contours when the load is released after two load cycles, are shown in Figure 3. Residual stresses are present, both from the hardening and from the plastic deformation under the indenter.
Figure 3: The equivalent stress after two load cycles.
A fatigue analysis requires a stable load cycle. For this purpose the development of the plastic deformation is evaluated. Figure 4 displays where plastic deformation has occurred. Figure 5 displays the magnitude of the equivalent plastic strain. In Figure 6 it can be seen that plasticity develops only during the first load cycle. Every consecutive load cycle is elastic. The second load cycle can therefore be seen as a stable load cycle and is used in the subsequent fatigue study
Figure 4: Plastically deformed volume after two load cycles.
.
Figure 5: Equivalent plastic strain after two load cycles.
Figure 6: Development of plastic strains, integrated over the volume.
In Figure 7 and Figure 8, stress contours are shown at the peak load in the second load cycle. Both the highest equivalent stress and the maximum shear stress are found below the surface. This is commonly seen in contact problems.
Figure 7: Equivalent stress at peak load.
Figure 8: The stress contours of the shear stress at peak load.
The fatigue analysis shows that the highest risk of fatigue is in the case about 0.1 mm below the surface. At the interface between the core and the transition layer there is also an increased risk of fatigue, see Figure 9. By inspecting the material far away from the contact, one can observe that the fatigue usage factor in the case layer has a negative value while in the core it has a positive value. This is caused by the combination of the residual stress from surface hardening and almost zero stress amplitude. A compressive hydrostatic state is beneficial for fatigue prevention while positive hydrostatic stress has a negative influence on fatigue.
Figure 9: Fatigue usage factor.
Application Library path: Fatigue_Module/Stress_Based/standing_contact_fatigue
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 Axisymmetric.
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
H
5[mm]
0.005 m
Model height
dH
0.5[mm]
5E-4 m
Case depth
dT
0.1[mm]
1E-4 m
Transition depth
W
5[mm]
0.005 m
Model width
dW
0.7[mm]
7E-4 m
Fine zone width
P
384[N]
384 N
Max load
E
200[GPa]
2E11 Pa
Young's modulus
nu
0.30
0.3
Poisson's ratio
rho
7800[kg/m^3]
7800 kg/m³
Density
Es
E/(2*(1-nu^2))
1.0989E11 Pa
Hertzian contact stiffness
ri
7[mm]
0.007 m
Indenter radius
sL
0
0
Load magnifier
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 Height text field, type H-dH-dT.
4
In the Width text field, type W.
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 dW.
4
In the Height text field, type dT.
5
Locate the Position section. In the z text field, type H-dH-dT.
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 W-dW.
4
In the Height text field, type dT.
5
Locate the Position section. In the r text field, type dW.
6
In the z text field, type H-dH-dT.
Rectangle 4 (r4)
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 dW.
4
In the Height text field, type dH.
5
Locate the Position section. In the z text field, type H-dH.
Rectangle 5 (r5)
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-dW.
4
In the Height text field, type dH.
5
Locate the Position section. In the r text field, type dW.
6
In the z text field, type H-dH.
7
In the Geometry toolbar, click  Build All.
8
In the Model Builder window, click Geometry 1.
Definitions
Integration 1 (intop1)
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 Selection list, choose All domains.
4
Locate the Advanced section. From the Frame list, choose Material  (R, PHI, Z).
Solid Mechanics (solid)
Linear Elastic Material 1
1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics (solid) click Linear Elastic Material 1.
2
In the Settings window for Linear Elastic Material, locate the Linear Elastic Material section.
3
From the E list, choose User defined. In the associated text field, type E.
4
From the ν list, choose User defined. In the associated text field, type nu.
5
From the ρ list, choose User defined. In the associated text field, type rho.
Plasticity 1
1
In the Physics toolbar, click  Attributes and choose Plasticity.
2
In the Settings window for Plasticity, locate the Domain Selection section.
3
Click  Clear Selection.
4
Select Domains 3 and 5 only.
5
Locate the Plasticity Model section. From the σys0 list, choose User defined. In the associated text field, type 570[MPa].
6
Find the Isotropic hardening model subsection. From the ETiso list, choose User defined. In the associated text field, type 69[GPa].
Linear Elastic Material 1
In the Model Builder window, click Linear Elastic Material 1.
Plasticity 2
In the Physics toolbar, click  Attributes and choose Plasticity.
Plasticity Case
1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics (solid) > Linear Elastic Material 1 click Plasticity 1.
2
In the Settings window for Plasticity, type Plasticity Case in the Label text field.
Plasticity Core
1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics (solid) > Linear Elastic Material 1 click Plasticity 2.
2
In the Settings window for Plasticity, type Plasticity Core in the Label text field.
3
Locate the Domain Selection section. Click  Clear Selection.
4
Select Domain 1 only.
5
Locate the Plasticity Model section. From the σys0 list, choose User defined. In the associated text field, type 515[MPa].
6
Find the Isotropic hardening model subsection. From the list, choose Ludwik.
7
From the k list, choose User defined. In the associated text field, type 2.47[GPa].
8
From the n list, choose User defined. In the associated text field, type 0.55.
Global Definitions
Transition function
1
In the Home toolbar, click  Functions and choose Global > Interpolation.
2
In the Settings window for Interpolation, type Transition function in the Label text field.
3
Locate the Definition section. In the table, enter the following settings:
t
f(t)
H-dH-dT
1
H-dH
0
4
Locate the Units section. In the Argument table, enter the following settings:
Argument
Unit
t
m
Definitions
Variables 1
1
In the Model Builder window, under Component 1 (comp1) 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
s
int1(z)
 
Transition layer position
nT
1-0.45*s
 
Hardening exponent transition layer
kT
10^(-1.62*s+11) [Pa]
Pa
Strength coefficient transition layer
s0T
(570e6*(1-s)+515e6*s) [Pa]
Pa
Initial yield stress transition layer
Solid Mechanics (solid)
Linear Elastic Material 1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics (solid) click Linear Elastic Material 1.
Plasticity Transition
1
In the Physics toolbar, click  Attributes and choose Plasticity.
2
In the Settings window for Plasticity, type Plasticity Transition in the Label text field.
3
Locate the Domain Selection section. Click  Clear Selection.
4
Select Domains 2 and 4 only.
5
Locate the Plasticity Model section. From the σys0 list, choose User defined. In the associated text field, type s0T.
6
Find the Isotropic hardening model subsection. From the list, choose Ludwik.
7
From the k list, choose User defined. In the associated text field, type kT.
8
From the n list, choose User defined. In the associated text field, type nT.
Global Definitions
Residual stress
1
In the Home toolbar, click  Functions and choose Global > Interpolation.
2
In the Settings window for Interpolation, type Residual stress in the Label text field.
3
Locate the Definition section. In the table, enter the following settings:
t
f(t)
0
-500
1
100
4
Locate the Units section. In the Function table, enter the following settings:
Function
Unit
int2
MPa
Solid Mechanics (solid)
Linear Elastic Material 1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics (solid) click Linear Elastic Material 1.
Initial Stress and Strain 1
1
In the Physics toolbar, click  Attributes and choose Initial Stress and Strain.
2
In the Settings window for Initial Stress and Strain, locate the Initial Stress and Strain section.
3
Specify the S0 matrix as
int2(s)
0
0
0
int2(s)
0
0
0
0
Roller 1
1
In the Physics toolbar, click  Boundaries and choose Roller.
2
Select Boundaries 2 and 13–15 only.
Prescribe load from the indenter. Both the contact pressure and the contact radius vary with load magnitude. Define the load as a function. Define the contact pressure and the contact radius as variables.
Global Definitions
Periodic load
1
In the Home toolbar, click  Functions and choose Global > Analytic.
2
In the Settings window for Analytic, type Periodic load in the Label text field.
3
Locate the Definition section. In the Expression text field, type 0.5*(1-cos(x*2*pi)).
Definitions
Variables 1
1
In the Model Builder window, under Component 1 (comp1) > Definitions click Variables 1.
2
In the Settings window for Variables, locate the Variables section.
3
In the table, enter the following settings:
Name
Expression
Unit
Description
ai
(3/4*P*an1(sL)*ri/Es)^(1/3)
m
Indentation radius
p0
3*P*an1(sL)/(2*pi*ai*ai)
N/m²
Max pressure
Solid Mechanics (solid)
Boundary Load 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundary 7 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
From the Load type list, choose Pressure.
5
In the p text field, type if(r<ai,p0*sqrt(1-(r/ai)^2),0).
Create a fine mesh in the vicinity of the contact area.
Mesh 1
Mapped 1
1
In the Mesh toolbar, click  Mapped.
2
In the Settings window for Mapped, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domains 2 and 3 only.
Distribution 1
1
Right-click Mapped 1 and choose Distribution.
2
Select Boundaries 4, 6, and 7 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 70.
Distribution 2
1
In the Model Builder window, right-click Mapped 1 and choose Distribution.
2
Select Boundaries 5 and 10 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 50.
Distribution 3
1
Right-click Mapped 1 and choose Distribution.
2
Select Boundaries 3 and 8 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 10.
Free Triangular 1
1
In the Mesh toolbar, click  Free Triangular.
2
In the Model Builder window, right-click Mesh 1 and choose 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, click to expand the Study Extensions section.
3
Select the Auxiliary sweep checkbox.
4
Click  Add.
5
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
sL (Load magnifier)
range(0.0,0.025,0.5) range(0.55,0.05,2)
 
6
In the Study toolbar, click  Compute.
Set default units for result presentation.
Results
Preferred Units 1
1
In the Results toolbar, click  Configurations and choose Preferred Units.
2
In the Settings window for Preferred Units, locate the Units section.
3
Click  Add Physical Quantity.
4
In the Physical Quantity dialog, select Solid Mechanics > Stress tensor (N/m^2) in the tree.
5
Click OK.
6
In the Settings window for Preferred Units, locate the Units section.
7
In the table, enter the following settings:
Quantity
Unit
Preferred unit
Stress tensor
N/m^2
MPa
8
Click  Apply.
Surface 1
In the Model Builder window, expand the Stress (solid) node.
Deformation
1
In the Model Builder window, expand the Surface 1 node, then click Deformation.
2
In the Settings window for Deformation, locate the Scale section.
3
Select the Scale factor checkbox. In the associated text field, type 1.
Surface 1
In the Model Builder window, expand the Stress, 3D (solid) node.
Deformation
1
In the Model Builder window, expand the Surface 1 node, then click Deformation.
2
In the Settings window for Deformation, locate the Scale section.
3
Select the Scale factor checkbox. In the associated text field, type 10.
Stress (solid)
Evaluate development of plasticity.
Plastically deformed volume
1
In the Model Builder window, right-click Stress (solid) and choose Duplicate.
2
In the Settings window for 2D Plot Group, type Plastically deformed volume in the Label text field.
Surface 1
1
In the Model Builder window, expand the Plastically deformed volume node, then click Surface 1.
2
In the Settings window for Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Solid Mechanics > Strain > solid.epeGp - Equivalent plastic strain - 1.
3
Locate the Expression section. In the Expression text field, type solid.epeGp>0.
Deformation
1
In the Model Builder window, expand the Surface 1 node.
2
Right-click Deformation and choose Delete.
Plastic strain
1
In the Model Builder window, right-click Plastically deformed volume and choose Duplicate.
2
In the Settings window for 2D Plot Group, type Plastic strain in the Label text field.
Surface 1
1
In the Model Builder window, expand the Plastic strain node, then click Surface 1.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type solid.epeGp.
Plastic Strain History
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Plastic Strain History in the Label text field.
Global 1
1
In the Plastic Strain History toolbar, click  Global.
2
In the Settings window for Global, locate the y-Axis Data section.
3
In the table, enter the following settings:
Expression
Unit
Description
intop1(solid.epeGp)
mm^3
Integrated plastic strain
4
In the Plastic Strain History toolbar, click  Plot.
Evaluate stresses at peak load.
Equivalent stress at peak load
1
In the Model Builder window, right-click Stress (solid) and choose Duplicate.
2
In the Settings window for 2D Plot Group, type Equivalent stress at peak load in the Label text field.
3
Locate the Data section. From the Parameter value (sL) list, choose 1.5.
Shear stress at peak load
1
In the Model Builder window, expand the Equivalent stress at peak load node.
2
Right-click Equivalent stress at peak load and choose Duplicate.
3
In the Settings window for 2D Plot Group, type Shear stress at peak load in the Label text field.
Surface 1
1
In the Model Builder window, expand the Shear stress at peak load node, then click Surface 1.
2
In the Settings window for Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Solid Mechanics > Stress > Stress tensor (spatial frame) - N/m² > solid.sGprz - Stress tensor, rz-component.
3
In the Shear stress at peak load toolbar, click  Plot.
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 Structural Mechanics > Fatigue (ftg).
4
Find the Physics interfaces in study subsection. In the table, clear the Solve checkbox for Study 1.
5
Click the Add to Component 1 button in the window toolbar.
Fatigue (ftg)
Stress-Based 1
1
In the Physics toolbar, click  Domains and choose Stress-Based.
2
In the Settings window for Stress-Based, locate the Domain Selection section.
3
From the Selection list, choose All domains.
4
Locate the Fatigue Model Selection section. From the Criterion list, choose Dang Van.
5
Locate the Solution Field section. From the Physics interface list, choose Solid Mechanics (solid).
6
In the Physics toolbar, click  Add Physics to close the Add Physics window.
Materials
Material 1 (mat1)
1
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose Blank Material.
2
In the Settings window for Material, locate the Geometric Entity Selection section.
3
Click  Clear Selection.
4
Select Domains 3 and 5 only.
5
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Hydrostatic stress sensitivity coefficient
a_DangVan
0.19
1
Dang Van
Limit factor
b_DangVan
282[MPa]
Pa
Dang Van
Material 2 (mat2)
1
Right-click Materials and choose Blank Material.
2
Select Domains 1, 2, and 4 only.
3
In the Settings window for Material, locate the Material Contents section.
4
In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Hydrostatic stress sensitivity coefficient
a_DangVan
0.23
1
Dang Van
Limit factor
b_DangVan
248[MPa]
Pa
Dang Van
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 Physics interfaces in study subsection. In the table, clear the Solve checkbox for Solid Mechanics (solid).
4
Find the Studies subsection. In the Select Study tree, select Preset Studies for Selected Physics Interfaces > Fatigue.
5
Click the Add Study button in the window toolbar.
6
In the Home toolbar, click  Add Study to close the Add Study window.
Study 2
Step 1: Fatigue
1
In the Settings window for Fatigue, locate the Values of Dependent Variables section.
2
Find the Values of variables not solved for subsection. From the Settings list, choose User controlled.
3
From the Method list, choose Solution.
4
From the Study list, choose Study 1, Stationary.
5
From the Parameter value (sL) list, choose From list.
6
In the Parameter value (sL) list, choose 0.6, 0.65, 0.7, 0.75, 0.8, 0.85, 0.9, 0.95, 1, 1.05, 1.1, 1.15, 1.2, 1.25, 1.3, 1.35, 1.4, 1.45, 1.5, 1.55, and 1.6.
7
In the Study toolbar, click  Compute.
Results
Fatigue Usage Factor (ftg)
Two new plot groups are added to plot the fatigue usage factor both in 2D (Figure 9) and in 3D revolution.