PDF
Elastoplastic Low-Cycle Fatigue Analysis of Cylinder with a Hole
Introduction
A load carrying part of a structure is subjected to multi-axial cyclic loading during which localized yielding of the material occurs. In this model you perform a low cycle fatigue analysis of the part based on the Smith–Watson–Topper (SWT) model. Due to localized yielding, you can use two methods to obtain the stress and strain distributions for the fatigue evaluation. The first method is a full elastoplastic analysis with kinematic hardening, while the second is a linear elastic analysis with Neuber correction for plasticity. This example explores the first method. In the model Notch Approximation in Low-Cycle Fatigue Analysis of Cylinder with a Hole, the same problem is solved using the elastic (Neuber) approach.
Model Definition
Geometry
A cylinder contains a hole, drilled perpendicularly to its axis. The outer and inner diameters of the cylinder are 200 and 180 mm respectively. Its height is 100 mm. The diameter of the hole is 20 mm. The cylinder is loaded by an axial force which varies in time.
As the structure and loading contains several symmetries, you may model only 1/8 of the cylinder, a shown in Figure 1.
Figure 1: Model geometry with constrained and loaded faces.
Material properties
•
Elastic data: Isotropic with E = 210 GPa, ν = 0.3
•
Kinematic hardening plasticity data: Yield stress 380 MPa, Tangent modulus 75 GPa
•
Fatigue parameters for the SWT equation:
-
σf' = 1323 MPa
-
b = −0.097
-
εf' = 0.375
-
c = −0.60
Constraints
Apply symmetry conditions on the three symmetry sections shown in Figure 1.
Load
The loaded boundary of the cylinder is subjected to a pressure of 200 MPa having a sinusoidal variation with time. Since the problem is quasi static, time is not used explicitly in the problem. Instead you model the load as a function of a parameter, and use the parametric solver to trace the history.
Results and Discussion
The von Mises stress when the maximum load is reached for the first time (at a parameter value of 0.25) is shown in Figure 2. Notice that the yield limit 380 MPa is exceeded by a large factor, and you can therefore expect significant plastic strains.
After completion of the first load cycle, there are no external loads. The internal residual stresses are still high, as can be seen in Figure 3.
For a point located on the face of the hole and in the XY symmetry plane, the highest stresses appear in the Z direction. In Figure 4, you can follow the development of the normal stress and strain in this direction during the first load cycle. The accumulation of plastic strain is shown in Figure 5. This repetitive plastic deformation can be viewed as driving the generation of a fatigue crack.
After having run a second load cycle, the stress-strain loop repeats itself, and you can consider the process to have reached a steady state condition. This is shown in Figure 6. The continuation of the equivalent plastic strain history is shown in Figure 7.
Figure 2: von Mises stress level at the first maximum load.
Figure 3: Residual equivalent stress after completion of first load cycle.
Figure 4: Stress as function of strain during the first load cycle.
Figure 5: Accumulated equivalent plastic strain during the first load cycle.
Figure 6: Stress as function of strain after two load cycles.
Figure 7: Accumulated equivalent plastic strain during two load cycles.
The result of the fatigue evaluation is shown in Figure 8 below. The most critical point has a computed life of approximately 7200 load cycles.
Figure 8: Lifetime plot.
Notes About the COMSOL Implementation
Two studies are used for the elastoplastic analysis. The second study contains the strain cycle that is passed on to the fatigue evaluation. It takes the results from the first study as initial conditions. This approach is not necessary. since it in the Fatigue study step is possible to select part of a study as defining a load cycle.
Application Library path: Fatigue_Module/Strain_Based/cylinder_with_hole_plastic
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.
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.
Cylinder 1 (cyl1)
1
In the Geometry toolbar, click  Cylinder.
2
In the Settings window for Cylinder, locate the Size and Shape section.
3
In the Radius text field, type 100.
4
In the Height text field, type 100.
Cylinder 2 (cyl2)
1
Right-click Cylinder 1 (cyl1) and choose Duplicate.
2
In the Settings window for Cylinder, locate the Size and Shape section.
3
In the Radius text field, type 90.
Difference 1 (dif1)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Difference.
2
Select the object cyl1 only.
3
In the Settings window for Difference, locate the Difference section.
4
Click to select the  Activate Selection toggle button for Objects to subtract.
5
Select the object cyl2 only.
6
Click  Build All Objects.
Cylinder 3 (cyl3)
1
In the Geometry toolbar, click  Cylinder.
2
In the Settings window for Cylinder, locate the Size and Shape section.
3
In the Radius text field, type 10.
4
In the Height text field, type 220.
5
Locate the Position section. In the y text field, type -110.
6
In the z text field, type 50.
7
Locate the Axis section. From the Axis type list, choose y-axis.
8
Click  Build All Objects.
Difference 2 (dif2)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Difference.
2
Select the object dif1 only.
3
In the Settings window for Difference, locate the Difference section.
4
Click to select the  Activate Selection toggle button for Objects to subtract.
5
Select the object cyl3 only.
6
Click  Build All Objects.
Block 1 (blk1)
1
In the Geometry toolbar, click  Block.
2
In the Settings window for Block, locate the Size and Shape section.
3
In the Width text field, type 100.
4
In the Depth text field, type 100.
5
In the Height text field, type 50.
6
Click  Build All Objects.
Intersection 1 (int1)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Intersection.
2
Click in the Graphics window and then press Ctrl+A to select both objects.
3
In the Settings window for Intersection, click  Build All Objects.
4
Click the  Zoom Extents button in the Graphics toolbar.
Use an extra domain for controlling the mesh. The mesh should be fine in a region close to the hole.
Cylinder 4 (cyl4)
1
In the Geometry toolbar, click  Cylinder.
2
In the Settings window for Cylinder, locate the Axis section.
3
From the Axis type list, choose y-axis.
4
Locate the Size and Shape section. In the Height text field, type 40.
5
In the Radius text field, type 15.
6
Locate the Position section. In the y text field, type 80.
7
In the z text field, type 50.
8
Click  Build All Objects.
Intersection 2 (int2)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Intersection.
2
Click in the Graphics window and then press Ctrl+A to select both objects.
3
In the Settings window for Intersection, locate the Intersection section.
4
Select the Keep input objects checkbox.
5
Click  Build All Objects.
Delete Entities 1 (del1)
1
In the Model Builder window, right-click Geometry 1 and choose Delete Entities.
2
In the Settings window for Delete Entities, locate the Entities or Objects to Delete section.
3
From the Geometric entity level list, choose Object.
4
Select the object cyl4 only.
Form Union (fin)
1
In the Geometry toolbar, click  Build All.
2
In the Model Builder window, click Form Union (fin).
Mesh Control Domains 1 (mcd1)
1
In the Geometry toolbar, click  Virtual Operations and choose Mesh Control Domains.
2
On the object fin, select Domain 2 only.
3
In the Geometry toolbar, click  Build All.
Solid Mechanics (solid)
Symmetry 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry.
2
Select Boundaries 1, 6, and 7 only.
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
para
0
0
Load cycle control
Solid Mechanics (solid)
Boundary Load 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundary 3 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
Specify the fA vector as
0
x
0
y
-200[MPa]*sin(2*pi*para)
z
Linear Elastic Material 1
In the Model Builder window, click Linear Elastic Material 1.
Plasticity 1
1
In the Physics toolbar, click  Attributes and choose Plasticity.
2
In the Settings window for Plasticity, locate the Plasticity Model section.
3
Find the Isotropic hardening model subsection. From the list, choose Perfectly plastic.
4
Find the Kinematic hardening model subsection. From the list, choose Linear.
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 Material Contents section.
3
In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
210[GPa]
Pa
Young’s modulus and Poisson’s ratio
Poisson’s ratio
nu
0.3
1
Young’s modulus and Poisson’s ratio
Density
rho
0
kg/m³
Basic
Initial yield stress
sigmags
380[MPa]
Pa
Elastoplastic material model
Kinematic tangent modulus
Ek
75[GPa]
Pa
Elastoplastic material model
Mesh 1
1
In the Model Builder window, under Component 1 (comp1) right-click Mesh 1 and choose Build All.
The default mesh cannot resolve this problem, so you need to refine it.
Once a mesh is created the mesh control domains are removed. In order to get them back, you need to clear the mesh.
2
In the Mesh toolbar, click  Clear Built Mesh.
3
In the Settings window for Mesh, locate the Sequence Type section.
4
From the list, choose User-controlled mesh.
Mapped 1
1
In the Mesh toolbar, click  More Generators and choose Mapped.
2
Select Boundary 4 only.
Distribution 1
1
Right-click Mapped 1 and choose Distribution.
2
Select Edge 4 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 6.
Distribution 2
1
In the Model Builder window, right-click Mapped 1 and choose Distribution.
2
Select Edge 5 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 15.
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 Domain 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 4.
Free Tetrahedral 1
1
In the Model Builder window, under Component 1 (comp1) > Mesh 1 right-click Free Tetrahedral 1 and choose Move Down twice.
2
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 to include para as continuation parameter.
5
In the table, enter the following settings:
Parameter name
Parameter value list
para (Load cycle control)
range(0,0.025,1)
6
In the Model Builder window, click Study 1.
7
In the Settings window for Study, type Study 1 (First Load Cycle) in the Label text field.
8
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.
Stress (solid)
1
In the Model Builder window, under Results click Stress (solid).
2
In the Stress (solid) toolbar, click  Plot.
The default plot is from the last parameter value, which has no external loads. The residual stress and corresponding displacements are shown. You may want to reduce the deformation scale in order to get a better view.
Volume 1
In the Model Builder window, expand the Stress (solid) node.
Deformation
1
In the Model Builder window, expand the Volume 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 2000.
4
In the Stress (solid) toolbar, click  Plot.
Now, set back scaling to the default and examine the stress state at maximum tension.
5
Clear the Scale factor checkbox.
Stress (solid)
1
In the Model Builder window, under Results click Stress (solid).
2
In the Settings window for 3D Plot Group, locate the Data section.
3
From the Parameter value (para) list, choose 0.25.
4
In the Stress (solid) toolbar, click  Plot.
Plastic Strain
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Plastic Strain in the Label text field.
Point Graph 1
1
In the Plastic Strain toolbar, click  Point Graph.
2
Select Point 6 only.
3
In the Settings window for Point Graph, click Replace Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1) > Solid Mechanics > Strain > solid.epeGp - Equivalent plastic strain - 1.
4
In the Plastic Strain toolbar, click  Plot.
Stress vs. Strain
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Stress vs. Strain in the Label text field.
Point Graph 1
1
In the Stress vs. Strain toolbar, click  Point Graph.
2
Select Point 6 only.
3
In the Settings window for Point Graph, click Replace Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1) > Solid Mechanics > Stress > Stress tensor (spatial frame) - N/m² > solid.sGpzz - Stress tensor, zz-component.
4
Click Replace Expression in the upper-right corner of the x-Axis Data section. From the menu, choose Component 1 (comp1) > Solid Mechanics > Strain > Strain tensor (material and geometry frames) > solid.eZZ - Strain tensor, ZZ-component.
5
In the Stress vs. Strain toolbar, click  Plot.
Add another study for the next load cycle.
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 Studies subsection. In the Select Study tree, select General Studies > Stationary.
4
Click the Add Study button in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Study 2
Step 1: Stationary
1
In the Settings window for Stationary, locate the Study Extensions section.
2
Select the Auxiliary sweep checkbox.
3
Click  Add.
4
In the table, enter the following settings:
Parameter name
Parameter value list
para (Load cycle control)
range(1,0.025,2)
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 (First Load Cycle), Stationary.
8
In the Model Builder window, click Study 2.
9
In the Settings window for Study, type Study 2 (Steady State Load Cycle) in the Label text field.
10
Locate the Study Settings section. Clear the Generate default plots checkbox.
11
In the Study toolbar, click  Compute.
Results
Point Graph 2
1
In the Model Builder window, under Results > Plastic Strain right-click Point Graph 1 and choose Duplicate.
2
In the Settings window for Point Graph, locate the Data section.
3
From the Dataset list, choose Study 2 (Steady State Load Cycle)/Solution 2 (sol2).
4
Click to expand the Coloring and Style section. Find the Line style subsection. From the Line list, choose Dotted.
5
From the Width list, choose 4.
6
In the Plastic Strain toolbar, click  Plot.
Point Graph 2
1
In the Model Builder window, under Results > Stress vs. Strain right-click Point Graph 1 and choose Duplicate.
2
In the Settings window for Point Graph, locate the Data section.
3
From the Dataset list, choose Study 2 (Steady State Load Cycle)/Solution 2 (sol2).
4
Locate the Coloring and Style section. Find the Line style subsection. From the Line list, choose Dotted.
5
From the Width list, choose 4.
6
In the Stress vs. Strain 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 checkboxes for Study 1 (First Load Cycle) and Study 2 (Steady State Load Cycle).
5
Click the Add to Component 1 button in the window toolbar.
6
In the Home toolbar, click  Add Physics to close the Add Physics window.
Fatigue (ftg)
Strain-Based 1
1
In the Physics toolbar, click  Boundaries and choose Strain-Based.
2
In the Settings window for Strain-Based, locate the Boundary Selection section.
3
From the Selection list, choose All boundaries.
4
Locate the Solution Field section. From the Physics interface list, choose Solid Mechanics (solid).
5
Locate the Evaluation Settings section. Find the Critical plane settings subsection. In the Q text field, type 16.
Materials
Material 2 (mat2)
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
From the Geometric entity level list, choose Boundary.
4
From the Selection list, choose All boundaries.
5
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Fatigue ductility coefficient
epsilonf_CM
0.375
1
Coffin-Manson
Fatigue ductility exponent
c_CM
-0.60
1
Coffin-Manson
Fatigue strength coefficient
sigmaf_Basquin
1323[MPa]
Pa
Basquin
Fatigue strength exponent
b_Basquin
-0.097
1
Basquin
Young’s modulus
E
210[GPa]
Pa
Basic
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 3
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 2 (Steady State Load Cycle), Stationary.
5
In the Model Builder window, click Study 3.
6
In the Settings window for Study, type Study 3 (Fatigue, SWT) in the Label text field.
7
In the Study toolbar, click  Compute.
Results
Fatigue Life
1
In the Settings window for 3D Plot Group, type Fatigue Life in the Label text field.
2
Click to expand the Title section. From the Title type list, choose Manual.
3
In the Title text area, type Logarithm of lifetime in number of cycles.
4
In the Model Builder window, expand the Fatigue Life node.
Marker 1
1
In the Model Builder window, expand the Results > Fatigue Life > Surface 1 node, then click Marker 1.
2
In the Settings window for Marker, locate the Text Format section.
3
In the Precision text field, type 2.
4
In the Fatigue Life toolbar, click  Plot.