PDF
Surface Cracked Cylinder
Introduction
This model reproduces a NAFEMS benchmark (Ref. 1) in which a pressurized cylinder has a horizontal semi-elliptical crack on its inner surface. The energy release rate is calculated along the crack front using the J-integral method. The stress intensity factors calculated from the J-integral are then compared with reference data.
Model Definition
Since the model consists on a cylinder with a horizontal crack on its mid plane, only a quarter of the whole geometry is built. A tube around the elliptical crack front is built to generate a swept mesh along it. The swept mesh makes the J-integral curve along the crack front smoother.
A Symmetry condition is applied on the through-thickness boundaries of the cylinder. On the crack boundaries, it is overridden by a Crack node. The crack is symmetric to define explicitly the crack front. Due to the symmetry, the stress intensity factors for modes II and III will be zero.
The pressure load can be applied with a Boundary Load on the inner face of the cylinder, and with a Face Load on the crack face.
The J-integral at a point of the crack front is composed of a closed contour integral and a surface integral. The closed contour integral is composed of a circular integral around the crack front and an integral on the crack face to take into account the force applied on it:
The stress intensity factor in mode I is then computed from the J-integral
where E* is the equivalent Young’s modulus. A 2D plane strain condition is assumed, so
.
Results and Discussion
Figure 1 shows the default stress plot, where a stress concentration around the crack front is visible. Figure 2 shows a closer view of this stress concentration
Figure 1: Von Mises stress in the cylinder and at the crack front.
Figure 2: Close view of the stress concentration at the crack front.
The J-integral calculated along the crack front represents the energy release rate per surface area when the crack is locally extended in the crack plane direction. The crack extension direction, the J-integral intensity and the surface contour used for integral calculation are plotted in Figure 3
Figure 3: 3D plot of J-integral: crack growth direction, intensity, and contour used for the calculation.
Figure 4 plots the J-integral as function of the parametric angle along the elliptical crack. A jump in the curve at zero angle can be noticed. This glitch is often seen near free boundaries due to the singularities that contribute to the surface integral.
Figure 4: J-integral along the crack front.
From the J-integral the stress intensity factor in mode I can be calculated and compared to the benchmark in Ref. 1, see Figure 5.
Figure 5: Stress intensity factor along the crack front compared to the benchmark.
Reference
1. R. Judge and B. Mardsen, Three Dimensional Test Cases in Linear Elastic Fracture Mechanics, part 4: Surface Cracked Cylinder, NAFEMS, 1993.
Application Library path: Structural_Mechanics_Module/Fracture_Mechanics/surface_cracked_cylinder
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 Geometry toolbar, click Insert Sequence and choose Insert Sequence.
2
Browse to the model’s Application Libraries folder and double-click the file surface_cracked_cylinder_geom_sequence.mph.
3
In the Geometry toolbar, click  Build All.
4
In the Model Builder window, under Component 1 (comp1) click Geometry 1.
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
p
1[MPa]
1E6 Pa
Pressure load
Materials
Material 1 (mat1)
1
In the Materials toolbar, click  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
207[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
8000
kg/m³
Basic
Solid Mechanics (solid)
Symmetry 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry.
2
Select Boundaries 1, 2, 5, 6, 8, 9, 11, 12, 15, 22, and 26 only.
The Symmetry condition is applied on the whole thickness of the cylinder. It will be overridden by the Crack feature on the crack surface.
Prescribed Displacement 1
1
In the Physics toolbar, click  Points and choose Prescribed Displacement.
2
Select Point 11 only.
3
In the Settings window for Prescribed Displacement, locate the Prescribed Displacement section.
4
From the Displacement in z direction list, choose Prescribed.
Crack 1
1
In the Physics toolbar, click  Boundaries and choose Crack.
2
Select Boundaries 6 and 9 only.
3
In the Settings window for Crack, locate the Crack Definition section.
4
From the Crack surface list, choose Symmetric.
5
Click to expand the Crack Front section. Click  Clear Selection.
6
Select Edge 13 only.
J-Integral 1
In the Physics toolbar, click  Attributes and choose J-Integral.
Boundary Load 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
Apply a pressure load on the inner face of the cylinder. The pressure on the crack will be applied under the Crack feature.
2
Select Boundaries 4, 7, 17, 24, 27, and 31 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 p.
Crack 1
In the Model Builder window, click Crack 1.
Face Load 1
1
In the Physics toolbar, click  Attributes and choose Face Load.
2
In the Settings window for Face Load, locate the Load section.
3
In the p text field, type p.
Mesh 1
Free Triangular 1
In the Mesh toolbar, click  More Generators and choose Free Triangular.
Size
1
In the Model Builder window, 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 th/2.
5
In the Minimum element size text field, type a/200.
Free Triangular 1
1
In the Model Builder window, click Free Triangular 1.
2
Select Boundary 8 only.
Size 1
1
Right-click Free Triangular 1 and choose Size.
2
In the Settings window for Size, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Point.
4
Select Point 5 only.
5
Locate the Element Size section. Click the Custom button.
6
Locate the Element Size Parameters section.
7
Select the Maximum element size checkbox. In the associated text field, type a/100.
8
Select the Minimum element size checkbox. In the associated text field, type a/200.
9
Select the Maximum element growth rate checkbox. In the associated text field, type 1.2.
10
Click  Build Selected.
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 3 only.
5
Click to expand the Sweep Method section. From the Destination mesh generation list, choose Morph source onto destination.
Distribution 1
1
Right-click Swept 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
From the Distribution type list, choose Predefined.
4
In the Number of elements text field, type 40.
5
In the Element ratio text field, type 6.
6
Select the Reverse direction checkbox.
7
Click  Build Selected.
Free Tetrahedral 1
1
In the Mesh toolbar, click  Free Tetrahedral.
2
In the Settings window for Free Tetrahedral, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domain 2 only.
5
Click  Build Selected.
Swept 2
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 4 only.
Swept 3
In the Mesh toolbar, click  Swept.
Distribution 1
1
Right-click Swept 3 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
From the Distribution type list, choose Predefined.
4
In the Number of elements text field, type 12.
5
In the Element ratio text field, type 4.
6
Click  Build All.
Study 1
In the Study toolbar, click  Compute.
Results
Volume 1
1
In the Model Builder window, expand the Stress (solid) node, then click Volume 1.
2
In the Settings window for Volume, locate the Expression section.
3
From the Unit list, choose MPa.
4
Click to expand the Range section. Select the Manual color range checkbox.
5
In the Maximum text field, type 20.
Stress (solid)
1
In the Model Builder window, click Stress (solid).
2
In the Settings window for 3D Plot Group, locate the Plot Settings section.
3
Clear the Plot dataset edges checkbox.
4
In the Stress (solid) toolbar, click  Plot.
The default plot shows the von Mises stress. At a closer view the maximum stress is visible along the crack front, see Figure 2.
From Result Templates, you can also add a plot that shows the crack direction and the intensity of the J-integral, Figure 3. The contour used to calculate the J-integral is displayed as well.
Result Templates
1
In the Results toolbar, click  Result Templates to open the Result Templates window.
2
Go to the Result Templates window.
3
In the tree, select Study 1/Solution 1 (sol1) > Solid Mechanics > Cracks (solid).
4
Click the Add Result Template button in the window toolbar.
5
In the Results toolbar, click  Result Templates to close the Result Templates window.
Results
Cracks (solid)
Add a new plot group from Result Templates to show the J-integral along the crack front.
Result Templates
1
In the Results toolbar, click  Result Templates to open the Result Templates window.
2
Go to the Result Templates window.
3
In the tree, select Study 1/Solution 1 (sol1) > Solid Mechanics > Crack 1, J-Integral (solid).
4
Click the Add Result Template button in the window toolbar.
5
In the Results toolbar, click  Result Templates to close the Result Templates window.
To reproduce Figure 4 you may introduce the parametric angle along the ellipse.
Definitions
Variables 1
1
In the Definitions toolbar, click  Local Variables.
2
In the Settings window for Variables, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domains 2 and 3 only.
5
Locate the Variables section. In the table, enter the following settings:
Name
Expression
Unit
Description
angle
atan2((Z-R1)/a,X/c)
rad
Parametric angle
Study 1
In the Study toolbar, click  Update Solution.
Results
J-Integral 1
1
In the Model Builder window, expand the Crack 1, J-Integral (solid) node, then click J-Integral 1.
2
In the Settings window for Line Graph, locate the x-Axis Data section.
3
From the Parameter list, choose Expression.
4
In the Expression text field, type angle.
5
From the Unit list, choose °.
6
In the Crack 1, J-Integral (solid) toolbar, click  Plot.
Duplicate the last plot group to plot and compare the stress intensity factor to the reference value, Figure 5
Crack 1, KI
1
In the Model Builder window, right-click Crack 1, J-Integral (solid) and choose Duplicate.
2
In the Settings window for 1D Plot Group, type Crack 1, KI in the Label text field.
KI
1
In the Model Builder window, expand the Crack 1, KI node, then click J-Integral 1.
2
In the Settings window for Line Graph, type KI in the Label text field.
3
Click Replace Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1) > Solid Mechanics > Cracks > solid.crack1.jint1.KI - Stress intensity factor, mode I.
4
Locate the y-Axis Data section. In the Expression text field, type solid.crack1.jint1.KI/1e6.
Crack 1, KI
1
In the Model Builder window, click Crack 1, KI.
2
In the Settings window for 1D Plot Group, locate the Plot Settings section.
3
Select the x-axis label checkbox.
4
Select the y-axis label checkbox. In the associated text field, type Stress intensity factor.
5
Locate the Axis section. Select the Manual axis limits checkbox.
6
In the y minimum text field, type 0.
7
In the Crack 1, KI toolbar, click  Plot.
Import the stress intensity factors from the benchmark to compare with the computed results.
Table 1
1
In the Results toolbar, click  Table.
2
In the Settings window for Table, locate the Data section.
3
Click  Import.
4
Browse to the model’s Application Libraries folder and double-click the file surface_cracked_cylinder_results.txt.
Table Graph 1
1
Right-click Crack 1, KI and choose Table Graph.
2
In the Settings window for Table Graph, locate the Coloring and Style section.
3
From the Color list, choose From theme.
4
Find the Line style subsection. From the Line list, choose None.
5
Find the Line markers subsection. From the Marker list, choose Asterisk.
6
In the Crack 1, KI toolbar, click  Plot.
Crack 1, KI
1
In the Model Builder window, click Crack 1, KI.
2
In the Settings window for 1D Plot Group, locate the Legend section.
3
Select the Show legends checkbox.
4
From the Position list, choose Upper left.
KI
1
In the Model Builder window, click KI.
2
In the Settings window for Line Graph, click to expand the Legends section.
3
Select the Show legends checkbox.
4
Find the Include subsection. Clear the Solution checkbox.
5
Select the Label checkbox.
Table Graph 1
1
In the Model Builder window, click Table Graph 1.
2
In the Settings window for Table Graph, click to expand the Legends section.
3
Select the Show legends checkbox.
4
From the Legends list, choose Manual.
5
In the table, enter the following settings:
Legends
KI, reference
Result Templates
1
In the Results toolbar, click  Result Templates to open the Result Templates window.
2
Go to the Result Templates window.
3
In the tree, select Study 1/Solution 1 (sol1) > Solid Mechanics > Fracture Mechanics Results (solid).
4
Click the Add Result Template button in the window toolbar.
5
In the Results toolbar, click  Result Templates to close the Result Templates window.