This document discusses the implementation of the Energy Domain Integral method in ANSYS to calculate the 3D J-integral of a Compact Tension fracture specimen. It begins with providing theoretical background on fracture mechanics and the J-integral. It then discusses the contour integral method and weight function approach for numerically calculating the J-integral. The document describes creating a finite element model of a standard CT specimen in ANSYS and implementing the Energy Domain Integral method to calculate the J-integral. It concludes by comparing the ANSYS simulation results to theoretical and experimental results.

1. .
Implementation of the Energy Domain Integral
method in Ansys for calculation of 3D J-integral
of CT-fracture specimen.
Siva Shankar Rudraraju
June - August 2004
1

2. INDEX
Page No.
I. Theoretical Background
4
II. J-Integral: Calculation Approaches
7
III. Contour Integral Method
8
IV. Weight Function
9
V. Finite Element Model
12
VI. ANSYS for Contour Integral Calculation
15
VII. Implementation in ANSYS
17
VIII. ANSYS Macro’s
18
IX. Theoretical Solution
21
X. Experimental Results
22
XI. ANSYS Simulation Results
23
XII. Results Comparison
25
XIII. Conclusions and Suggestions
26
XIV. References
27
3

3. Theoretical Background
Fracture is a problem that society has faced since ages. It is one of the more
catastrophic means of material failure. And just to get a grasp of the magnitude of
this catastrophe, an economic study estimated the cost of fracture in the United
States in 1978 at $119 billion. Further more this study estimated that the annual
cost could be reduced by $35 billion if current technology were applied.
Fortunately, the field of fracture mechanics has made rapid strides since then. And
now there are many methodologies and technologies in place, to help us understand
and prevent fracture. In this section a brief explanation of the theory of fracture
mechanics is presented to provide the necessary theoretical background.
How fracture failure is different from conventional tensile/brittle failure?
In case of brittle/tensile failure, the material is assumed to be a continuum, and the
material strength is calculated by taking into account the combined stress bearing
capacity of the continuum.
But in case of fracture, there are sharp discontinuities in this material continuum,
which locally magnify the stresses, and hence locally exceed the strength of the
material, thus giving rise to local failure initiation, which later spreads across the
continuum, thus leading to material failure.
So we can say that fracture is a micro level process, which destroys the macro load
bearing capacity of the material.
An attempt to understand and characterize such local stress magnifications is an
important component of fracture mechanics.
Fig 1.Stress flow in a plate near the vicinity of the elliptical crack.
4

4. Fig 2. Stress magnification in a plate near the vicinity of the sharp crack.
As seen in Fig.2, the stress in the vicinity of a sharp crack is very high. It can be
shown that the stress field in any linear elastic cracked body is given by.
⎛ k ⎞
⎟ f ij (θ ) + otherterms
⎝ r⎠
σ ij = ⎜
Where
σ ij
is the stress tensor, r and θ are the distance from the crack tip and
angle about the crack tip.
The above equation states that the stress is infinite at the crack tip (r=0). These
locally high values of stress near the crack tip may exceed the strength of the
material and lead to failure initiation. This failure once initiated, grows furthermore in
a stable(ductile) or unstable(brittle) mode.
Thus a small discontinuity (crack), in a continuum can lead to failure of the entire
structure. So a description of critical stress states is of utmost importance for
designers.
Now, the various fracture parameters, which are used to characterize these stresses,
are discussed below.
U
Fracture parameters: The most widely used fracture parameters are:
U
1. Stress intensity factor (K)
2. Elastic energy release rate (G)
3. J-integral (J)
4. Crack tip opening displacement (CTOD)
5

5. Stress Intensity Factor (K): The stress fields ahead of a crack tip in an isotropic
linear elastic material can be written as.
U
U
lim σ ij =
r →0
K
2πr
f ij (θ )
where the proportionality constant, K, is referred as the stress intensity factor. But
the above equation is only valid near the crack tip, where the
1
r
singularity
dominates the stress field. Thus, the stress intensity factor, which represents the
proportionality constant, gives an idea about the level of stress magnification around
the crack tip.
Elastic Energy Release Rate (G): According to the first law of thermodynamics, a
system goes from a non-equilibrium state to equilibrium, when there will be a net
decrease in energy.
Now when a material is loaded, its strain energy increases and hence the net energy
also increases. Thus the system is moving away from equilibrium as the net energy
is increasing. But always, the natural tendency of any system will be to jump to a
state of greater equilibrium by decreasing its net energy, thus the system is
constantly in want of a means to unload this excess strain energy.
And the continuum discontinuities (cracks) provide a means to dump the strain
energy as surface energy, by the creation of new crack surfaces during crack
formation or propagation.
Thus the energy release rate is an important parameter in understanding fracture
tendency. It is a measure of the energy available for an increment of crack
extension.
U
U
G=−
dπ
dA
It is defined as the change in potential energy per unit change in crack area.
The previous two fracture parameters, K and G, are valid within the limits of linear
elasticity, or with in the frontiers of Linear Elastic Fracture Mechanics (LEFM). But
many materials (e.g. steel) have elastic plastic behavior, though the magnitude of
plasticity may vary depending on the material and loading conditions. So, to
characterize the crack conditions to a sufficient degree of accuracy for real materials,
we need a fracture parameter, which can take into account the material plasticity.
This parameter is known as the J-integral.
6

6. J-Integral (J): Path-independent integrals have long been used in physics to calculate
the intensity of singularity of a field without knowing the exact shape of this field in
the vicinity of the singularity. They are derived from conservation laws.
The singularity in the vicinity of a crack tip, thus presents a fit case for the
application of the path-independent integrals. Cherepanov3 and Rice4 were the first
to introduce path independent integrals in fracture mechanics.
Rice4 showed that the nonlinear energy release rate, J, could be written as a path
independent line integral. Hutchinson5, Rice and Rosengren also showed that the J
uniquely characterizes crack tip stresses and strains in nonlinear materials. Thus the
J-integral can be viewed as a:
• Stress intensity parameter (like K)
• Nonlinear energy release rate (like G)
U
U
P
P
P
P
P
P
P
P
Rather J is a dual equivalent of K and G, in Elastic Plastic Fracture Mechanics (EPFM)
J –integral is defined as:
Where,
γ = any path surrounding the crack tip
W = strain energy density (that is, strain energy per unit volume
tx = traction vector along x axis = σxnx + σxy ny
ty = traction vector along y axis = σyny + σxy nx
σ = component stress
n = unit outer normal vector to path γ
s = distance along the path γ
B
B
B
B
B
B
B
B
B
B
B
B
B
B
B
B
B
B
B
B
As stated earlier, J is also equal to the nonlinear energy rate.
J =−
dΠ
dΑ
Until now the necessary brief introduction of the theoretical aspects of fracture
mechanics has been presented .The reader can find the theory in a greater detail in
any of the many available books on fracture mechanics1.
Now, the actual problem, the calculation of the J integral is presented.
P
P
J-integral: Calculation Approaches
The J-integral can be calculated by invoking either of the two definitions, i.e. the line
integral or energy release rate definition. Over the years many approaches have
been developed for numerical evaluation of the J-integral. The Global energy
estimates method involves finding the rate of change in global strain energy of the
fracture model with crack growth. This technique involves minimal post-processing
but however this involves multiple solution calculations (considering different crack
lengths), which can be very cumbersome if large fracture models are to be analyzed.
An alternative method is the numerical evaluation of J-integral along a contour
surrounding the crack tip. This method is discussed in detail in the following sections
7

7. J - Integral
Global Energy Estimates
Energy release rate
Stiffness Derivative Formulation
Path Independent Integral
Virtual Crack Extension Theory
2D
Line Integral
Weight function
Area Integral
Energy Domain Integral
3D
Volume Integral
Surface Integral
J-Integral Calculation Approaches
Contour Integral Method:
The J-integral can be evaluated numerically along a contour surrounding the crack
tip. The advantages of this method are that it can be applied to linear and non-linear
problems, and path independence enables the user to evaluate J at a remote
contour, where numerical accuracy is greater.
For problems that include path-dependent plastic deformation or thermal strains, it is
still possible to compute J at a remote contour, provided an appropriate correction
term (i.e. area integral) is applied. For three-dimensional problems, however the
contour integral becomes a surface integral, which is difficult to evaluate
numerically.
Recent formulations of J apply area integration for 2D problems and volume
integration for 3D problems. Especially for 3D, the volume integral is much better
then the surface integral as it is more accurate and easier to numerically implement.
Here the Energy Domain Integral method for calculation of area and volume integrals
is implemented.
8

8. Energy Domain Integral
The energy domain integral is a preferred methodology, as it has a general
framework for easy numerical analysis. This approach is extremely versatile, as it
can be applied to both quasistatic and dynamic problems with elastic, plastic, or
viscoelastic material responses.
Shih8, Moran and Nakamura gave detailed instructions for implementing the domain
integral** approach in FEM. Their method is summarized below.
P
P
P
P
In the absence of thermal strains, path-dependent plastic strains, tractions on the
crack faces and body forces within the integration volume or area, the discretized
form of the domain integral is as follows.
__
J ∆L =
⎧⎡⎛ ∂ui
⎞ ∂q ⎤ ⎛ ∂x ⎞⎫
⎪
⎜σ ij
− wδ1i ⎟ ⎥ det⎜ i ⎟⎬ wp
∑ ∑ ⎨⎢⎜ ∂x
⎟ ∂x
⎜
⎟
A*orV* p=1 ⎪⎣⎝
1
⎠ 1 ⎦ ⎝ ∂ξk ⎠⎭ p
⎩
m
(Eqn.1)
Where q is the weight function, m is the number of gaussian points per element and
wp
is the weighting factor for the gaussian integration.
Fig.3 Example of closed contour around a crack a front. S0 and S1 are inner and outer
surfaces, which enclose V*
B
B
B
B
P
Weight Function (q)
The weight function q, is merely an mathematical concept that enables the
generation an area or volume integral. But for the sake of understanding, q can be
interpreted as a normalized virtual displacement.
∆a(η ) = q(η )∆amax
where η is any point along the crack front, ∆a is the crack displacement at that
point, and ∆amax is the maximum crack displacement along the crack front.
P
**
The reader is referred to the book by T.L.Anderson1 for a detailed explanation of this method. Here it is
9
assumed, that the reader is familiar with this method, and just the FEM implementation is presented.
P
P
P

9. Fig.4 Example of a q function defined locally along the crack front.
Shih, et al. have also shown that the computed value of J-integral is insensitive to
the assumed shape of the q function. So we are free to assume any crack extension
shape, and hence any arbitrary smooth q function. But care should be taken such
that the Q-function should have the correct values on the domain boundaries.
q2=1
A
q1=1
q2=1
q2=0
q1=0
q=0
q2=1
C
q2=0
B
D
q2=0
q2=1
E
q2=0
q = q1 x q2
Y
Z
1
X
Fig.5. Representation of various possible q functions.
A: q1 plot (XY plane) B-E: q2 plot (YZ plane)
10

10. Another important benefit of the weight function is that it allows the calculation of
local values of J-integral within a model. From this we can estimate the variation of
the J-integral and hence the fracture tendency at different positions along the crack
front.
If the point-wise value of the J-integral does not vary appreciably over ∆L , an
approximation of J (η ) is given by:
__
J (η ) =
J ∆L
∫ q(η , r )dη
0
∆L
⎛ __ ⎞
⎜ J ∆L ⎟
⎠
∴ J (η ) = ⎝
⎛ ∆AC
⎞
⎜
∆amax ⎟
⎝
⎠
(Eqn.2)
Thus, from (Eqn.1) and (Eqn.2), J (η ) can be calculated at any point along the crack
front. Now the task is to numerically calculate (Eqn.1) and then J (η ) from (Eqn.2).
Hereafter, the Finite Element implementation of the J contour integral (Eqn.1) is
presented.
11

11. The Finite Element Model
The ASTM documentations refer to four standard fracture specimen configurations.
Among them the one of the most widely used model is the Compact Tension (CT)
Specimen. Here the J-integral calculations are performed on a standard CT specimen
with w=50mm.
w
a
b
h
g
s
d
n
l
A
A
=
=
=
=
=
=
=
=
=
B
Fig.6. (A) – The Standard CT Specimen, (B)-The parametric FEM model in ANSYS.
To simplify the computational complexity, the full FEM model is reduced to the
quarter symmetry model (Fig.7.) and the appropriate symmetry boundary conditions
and constraints are applied.
A
B
Fig.7. (A) Full Model
(B) Half Symmetry Model
C
(C) Quarter Symmetry Model
12
50mm
0.50*w
0.50*w
1.20*w
1.25*w
0.55*w
0.25*w
0.10*w
0.25*w

12. I.M
Fig.8. Load applied through intermediate material (I.M)
To prevent concentrated loading, loads are uniformly applied over an area through
an intermediate cylindrical wedge shaped material (shown in fig.8.) with higher
elastic modulus then the specimen material.
MESH DESIGN (Crack Tip)
As discussed earlier, the crack tip is an area of stress singularity. So while designing
the element mesh around the crack tip the following points are to be considered:
•
In Elastic problems, the crack tip is an area of stress singularity, so the
solid brick elements are to be degenerated down to wedges, and the
midside nodes (if any) are moved to ¼ points. Such a model results in a
1
singularity.
•
In plastic problems, the 1
r
singularity no longer exists at the crack tip.
r
•
So the elements are degenerated to wedges (like in elastic case), but the
midside node (if any) positions are unchanged.
The most efficient mesh design for the crack tip has proven to be the
“spider web” configuration, which consists of concentric rings of four sided
elements that are focused towards the crack tip. The innermost elements
are degenerated to wedges. Since the crack tip region contains steep
stress and strain gradients, the mesh refinement should be greatest at the
crack tip. The spider web design facilitates a smooth transition from a fine
mesh at the tip to a coarse mesh remote to the tip.
13
Fig.9. “Spider web” mesh around the crack tip, with degenerated wedge elements
near the crack tip.

13. Element Type
For selecting the element type, a compromise has to be made between
computational accuracy and computational time. We have a choice between the
linear 8-node brick element and the quadratic 20-node brick element. Some
important comparisons between these elements are:
The 20 node brick element is formulated with quadratic polynomials so it
can yield results with greater accuracy, especially in regions of high stress
gradients like that exhibited near the crack tip. The 8-node brick element
is formulated with linear equations, so it is less suited for regions with
high stress gradients.
The computational time required to process a 20 node element model is
many times more then a similar 8 node element model
The Ansys documentation states, “In nonlinear structural analyses, you
will usually obtain better accuracy at less expense if you use a fine mesh
of these linear elements rather than a comparable coarse mesh of
quadratic elements.”
Both element types can take the degenerated wedge shapes required at
the crack tip.
T
T
Taking into consideration the above points, and noting the absence of stress
singularity at the crack tip for elastic-plastic material, the CT specimen was finally
modeled with 8-node linear brick elements, with very fine meshing around the crack
tip.
14

14. Ansys for Contour Integral Calculation
The J-integral calculation involves a lot of post processing calculations. But some of
the results required for these calculations are not readily available in ANSYS.A
description and solution of these limitations is presented below.
Limitations
1.The simulation results like displacement, stress and strain energy density are to be
obtained at the integration points of each element enclosed within the selected
contours. Unfortunately, Ansys results can only be obtained at the element nodes
rather then the integration points.
2.Ansys strain energy density results are available only as element solutions. But the
strain energy gradient varies across the element, and the available Ansys element
value is an average across the element. But for J-integral calculation, the strain
energy density values are required at each element integration points.
3.The integration point locations are available only through the PRESOL command,
and hence to obtain the integration point locations the data should be dumped into
an output file and then read into the ANSYS database.
Solutions
The above three limitations can be overcome by the following two methods:
Method-I
Step 1: Store the nodal displacement and stress results for the elements within the
contour.
Step 2: Deduce the Strain energy density values by the following method
Store the element strain energy (SENE) and element volume (VOLU)
values in the element table (ETABLE command) for all the elements
within the contour.
Calculate the element strain energy density values by dividing (SEXP)
the element strain energy by the element volume values in the
element table.
Define infinitesimally small paths (using PATH and PMAP commands)
at the nodes of the elements within the contour, such that the
corresponding node is the last point of the path.
Interpolate the strain energy density values (PDEF command) from the
element table to the defined paths at the nodes.
Store the strain energy density value at each of the nodes by reading
in the value at the last point of the defined paths. (*GET command)
Now we have the nodal values of displacement, stress and strain energy density.
Step 3: Derive the values at the integration points by interpolating the nodal values,
using the shape functions and local element coordinates of the integration
points.
Thus, we obtain all the required results at the integration points.
Method-II
Step 1: Follow the first three points of Step 2 of Method-I above.
15

15. Step 2: Printout the integration point locations (PRESOL command) into an external
file. Then read the x, y and z locations of each integration point into an array
(*VREAD command).
Step 3:
Define infinitesimally small paths (using PATH and PMAP commands) at the
integration points of the elements within the contour, such that the
corresponding integration point is the last point of the path.
Interpolate the displacements, stresses and strain energy density values to
the defined paths at the integration points. (For strain energy density, the
values must be first stored in an element table as in Method-I)
Store the results at each of the integration points by reading in the value at
the last point of the defined paths. (*GET command).
Comparison
The results obtained by the above two methods differed negligible. And the
computational time required was also comparable. So the Method-I is adopted
hereafter, as it better fits into the general architecture of the J-integral macros.
16

16. Implementation in ANSYS
The following Block Diagram represents the general structure of the problem and functions of the
macros involved.
Title
Assign Element attributes and Material Properties
Macro “Plasticity. Mac”
Define Plasticity
Curve
Input all problem parameters
Plastic Material
Macro “Parameters. Mac”
Build Parametric Geometric Model
Build 2D FEM model
Extrude 2D model to 3D model
Modify Crack Tip wedge elements
Macro “Modify. Mac”
Set Solution Controls
Apply Loads and Constraints
Solve
Macro “Module1.Mac”
Select elements within the Contour
Sort selected elements
Macro “Module2.Mac”
Deduce required results at nodes
Deduce Q-Function values at nodes
Macro “Qfunc.Mac”
Interpolate Nodal values to get Integration point Values
Deduce the gradients of displacement and Q-Function
Calculate J-Integral
Macro “Shape. Mac”
Store all required values
End of File
17
Macro “Module3.Mac”

17. Macros:
The problem description is:
“Building numerical parametric models of the CT fracture Specimen and calculation of
the 3D J-Integral of standard fracture specimens by implementing the energy
domain integral method in Ansys”
This has been implemented through a sequence of 8 Macros (3 main Module macros
and 5 auxiliary macros) as shown in the block diagram previously. These macros are
described below.
Macro “Parameter.Mac”:
This is the first macro in the sequence, where the problem “TITLE”, Element
attributes, material properties and other required parameters are defined. This
macro acts as the user interface to the entire problem. Varying the parameters in
this macro can control almost all problem characteristics. The only other parameters,
which should be defined by the user, are the contour position parameters at the start
of “Module2.Mac” and the plasticity parameters in “Plasticity.Mac”
Macro “Module1.Mac”:
This is the main macro of the problem, where the parametric solid model is build,
then converted to FEM model and solved. This Macro encompasses the PreProcessing and Solution Routines.
Macro “Plasticity.Mac”:
This is an auxiliary macro for defining the Multi-linear isotropic hardening (plasticity)
curve as a data table.
Macro “Modify.Mac”:
Ansys documentation states that, “Generating a 3-D fracture model is considerably
more involved than a 2-D model. The KSCON command is not available, and you
need to make sure that the crack front is along edge KO of the elements”
And when the 3D mesh is generated directly by extruding 2D mesh, the crack front
is along the edge JN rather than KO (face KL-OP). So we need to reorder the node
numbering to place the edge KO (face KL-OP) along the crack front
This Macro performs two functions:
Reordering element node numbers.
Creating new nodes to change the point crack tip to a circular crack tip,
with very small radius “CKTIP”
T
T
Macro “Module2.Mac”:
This is a Post-Processing macro. The macro involves selection of elements within the
specified contours, and sorting them depending on the element centroid coordinates.
Macro “Module3.Mac”:
This is the J-Integral calculation macro. In this macro Equation 4 and Equation 5 are
implemented. This Macro calls:
“Qfunc.Mac” to get the value of Q-function at any point (x, y, z).
“Shape.Mac” to get the required displacement gradients, Qfunc
gradients, stresses and strain energy density values.
Macro “Qfunc.Mac”:
This Macro passes on the Q-Function values at any point (x, y, z) to “Module3.Mac”
18

18. Macro “Shape.Mac”:
This is the main calculation Macro, where the displacement gradients, Qfunc
gradients, stresses and strain energy density values are computed for the
integration points. Here the nodal values are transformed to integration point values
using element shape functions and a series of matrix operations.
The basic two matrices involved in this macro are JS, JP. From these two matrices
the Jacobian matrix and then the inverse Jacobian matrix are formed. Then through
a series of matrix operations involving the inverse Jacobian matrix, we obtain all the
required values at the integration points. The sequence of matrix operations is
described below.
Input Matrices:
Here, N-shape functions, u-displacements, q- Q Function, σ - Stress, w-strain
energy density, (x, y, z): Global coordinates, (s, t, r): Local element coordinates
JS = [N 1
y1
y2
y3
y4
y5
y6
y7
y8
N3
N4
N5
N6
N7
N8]
⎡ ∂N1
⎢
⎢ ∂s
∂N
JP = ⎢ 1
⎢ ∂t
⎢ ∂N1
⎢
⎣ ∂r
⎡ x1
⎢x
⎢ 2
⎢ x3
⎢
x
JX = ⎢ 4
⎢ x5
⎢
⎢ x6
⎢x
⎢ 7
⎢ x8
⎣
N2
∂N 2
∂s
∂N 2
∂t
∂N 2
∂r
∂N3
∂s
∂N3
∂t
∂N3
∂r
∂N 4
∂s
∂N 4
∂t
∂N 4
∂r
∂N5
∂s
∂N5
∂t
∂N5
∂r
∂N 6
∂s
∂N 6
∂t
∂N 6
∂r
∂N 7
∂s
∂N 7
∂t
∂N 7
∂r
∂N8 ⎤
⎥
∂s ⎥
∂N8 ⎥
∂t ⎥
∂N8 ⎥
⎥
∂r ⎦
1
⎡u1
⎢ 1
⎢u 2
1
⎢u 3
⎢ 1
u
MU = ⎢ 4
⎢u 1
⎢ 5
1
⎢u 6
⎢u 1
⎢ 7
1
⎢u 8
⎣
z1 ⎤
z2 ⎥
⎥
z3 ⎥
⎥
z4 ⎥
z5 ⎥
⎥
z6 ⎥
z7 ⎥
⎥
z8 ⎥
⎦
1
⎡σ 11
⎢ 2
⎢σ 11
3
⎢σ 11
⎢ 4
σ
MS = ⎢ 11
⎢σ 5
⎢ 11
6
⎢σ 11
⎢σ 7
⎢ 11
8
⎢σ 11
⎣
1
σ 22
2
σ 11
3
σ 11
4
σ 11
5
σ 11
6
σ 11
7
σ 11
8
σ 11
1
σ 33
2
σ 11
3
σ 11
4
σ 11
5
σ 11
6
σ 11
7
σ 11
8
σ 11
u12
2
u2
2
u3
2
u4
2
u5
2
u6
2
u7
2
u8
1
σ 12
2
σ 11
3
σ 11
4
σ 11
5
σ 11
6
σ 11
7
σ 11
8
σ 11
1
⎡ q1
⎢ 1
⎢q 2
1
⎢ q3
⎢ 1
q
MQ = ⎢ 4
⎢q1
⎢ 5
1
⎢q 6
⎢q 1
⎢ 7
1
⎢ q8
⎣
u13 ⎤
3⎥
u2 ⎥
3
u3 ⎥
3⎥
u4 ⎥
3
u5 ⎥
⎥
3
u6 ⎥
3
u7 ⎥
⎥
3
u8 ⎥
⎦
1
σ 23
2
σ 11
3
σ 11
4
σ 11
5
σ 11
6
σ 11
7
σ 11
8
σ 11
1
σ 13
2
σ 11
3
σ 11
4
σ 11
5
σ 11
6
σ 11
7
σ 11
8
σ 11
w1 ⎤
2 ⎥
w11 ⎥
3
w11 ⎥
4 ⎥
w11 ⎥
5
w11 ⎥
⎥
6
w11 ⎥
7
w11 ⎥
⎥
8
w11 ⎥
⎦
q12
2
q2
2
q3
2
q4
2
q5
2
q6
2
q7
2
q8
q13 ⎤
3⎥
q2 ⎥
3
q3 ⎥
3⎥
q4 ⎥
3
q5 ⎥
⎥
3
q6 ⎥
3
q7 ⎥
⎥
3
q8 ⎥
⎦
19

19. Matrix Operations:
U
JACO
=
(JP)*(JX)
INV_JACO =
(JACO)-1
MC
=
(INV_JACO)*(JP)
DU
=
(MC)*(MU)
DQ
=
(MC)*(MQ)
MRES
=
(JS)*(MS)
P
Resultant Matrices:
JACO
⎡ ∂x
⎢ ∂s
⎢ ∂x
= ⎢
⎢ ∂t
⎢ ∂x
⎢ ∂r
⎣
∂y
∂s
∂y
∂t
∂x
∂r
⎡ ∂N 1
⎢
⎢ ∂x
∂N
MC = ⎢ 1
⎢ ∂y
⎢
⎢ ∂N 1
⎢ ∂z
⎣
⎡ ∂u 1
⎢ ∂x
⎢
∂u 1
DU = ⎢
⎢ ∂y
⎢ ∂u 1
⎢
⎣ ∂z
MRES
∂z ⎤
∂s ⎥
∂z ⎥
⎥
∂t ⎥
∂x ⎥
∂r ⎥
⎦
∂N 3
∂x
∂N 3
∂y
∂N 3
∂z
∂N 2
∂x
∂N 2
∂y
∂N 2
∂z
∂u 2
∂x
∂u 2
∂y
∂u 2
∂z
= [σ 11
INV _ JACO
∂u 3
∂x
∂u 3
∂y
∂u 3
∂z
σ
22
∂N 4
∂x
∂N 4
∂y
∂N 4
∂z
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎦
∂N 5
∂x
∂N 5
∂y
∂N 5
∂z
∂N 6
∂x
∂N 6
∂y
∂N 6
∂z
⎡ ∂s
⎢ ∂x
⎢ ∂s
= ⎢
⎢ ∂y
⎢ ∂s
⎢
⎣ ∂z
∂N 7
∂x
∂N 7
∂y
∂N 7
∂z
⎡ ∂q 1
⎢ ∂x
⎢
∂q 1
DQ = ⎢
⎢ ∂y
⎢ ∂q 1
⎢
⎣ ∂z
σ
33
σ 12
σ
23
σ 13
∂t
∂x
∂t
∂y
∂t
∂z
∂N 8
∂x
∂N 8
∂y
∂N 8
∂z
∂q 2
∂x
∂q 2
∂y
∂q 2
∂z
w
∂r
∂x
∂r
∂y
∂r
∂z
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎦
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎦
∂q 3
∂x
∂q 3
∂y
∂q 3
∂z
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎦
]
Thus, as seen above the entire calculations are condensed to only 6 matrix
multiplications per integration point. This matrix method is simple to implement and
leads to faster and very efficient analysis.
20

20. Theoretical Solution:
The Electric Power Research Institute (EPRI) J estimation scheme provides a means
for computing the J-Integral in a variety of configurations and materials. A fully
plastic solution is combined with the stress intensity solution to obtain an estimate of
the elastic-plastic J.
The EPRI scheme is presented here:
J total = J el + J pl
K 12
J el = '
E
Where
E' = E
1 −ν 2
P0 = 1.455η Bb σ 0
, Plain Strain
, Plain Stress
B
B
B
⎛σ ⎞
ε
σ
=
+α⎜
⎟
⎜σ ⎟
ε0 σ 0
⎝ 0⎠
2
4a
⎛ 2a ⎞
⎛ 2a
⎞
+2 −⎜
+ 1⎟
η= ⎜ ⎟ +
b ⎠
b
b
⎝
⎝
⎠
n +1
b - characteristic length
h1 - geometric factor
P - characteristic load
P0 - reference load
Other parameters are flow properties
defined by Ramberg-Osgood fit:
B
P0 = 1.072η Bb σ 0
E' = E
J pl
⎛P⎞
= αε 0σ 0bh1 ⎜ ⎟
⎜P ⎟
⎝ 0⎠
n
And the stress intensity factor, K1 is given by:
B
B
K1 =
Pf ( a / w)
B w
And for a CT specimen
a
2
3
4
w ⎡0.866 + 4.64⎛ a ⎞ − 13 .32 ⎛ a ⎞ + 14 .72⎛ a ⎞ − 5.60 ⎛ a ⎞ ⎤
f ( a / w) =
⎜ ⎟
⎜ ⎟
⎜ ⎟
⎜ ⎟ ⎥
⎢
3/ 2
⎝ w⎠
⎝ w⎠
⎝ w⎠
⎝ w⎠ ⎥
a⎞ ⎢
⎛
⎦
⎜1 − ⎟ ⎣
w⎠
⎝
2+
These above theoretical solutions are used to verify the simulation results. However,
these theoretical solutions assume plane stress or plain strain conditions, whereas in
case of a real specimen neither pure plane stress or plane strain conditions exist.
21

21. Experimental Results:
The main objective of this FEM simulation was to verify the previously conducted
experiments for calculation of J-Integral using the unloading compliance technique,
as described in “ASTM Standard E1820-01: Standard Test Method for Measurement
of Fracture Toughness, ASTM 2001”
3D J-integral
180
J-integral (kN/m)
160
140
120
100
Experimental Data
80
60
40
20
0
0
20
40
60
80
Load (kN)
Fig.10.Experimental Results
The experiments were conducted at 1000 C. And hence a tensile test using a video
extensometer was conducted to obtain the stress-strain curve at this temperature.
P
P
Stress - Strain Curve
800
700
stress [MPa]
600
500
400
300
200
100
0
0
0.5
1
1.5
2
2.5
3
3.5
4
total strain [ - ]
Fig.11.True stress strain curve
Fig.12.Side grooved Specimen
It should be noted that, there exist small difference in the specimen and FEM model
structure. The test specimen is side grooved to avoid tunneling and maintain a
straight crack front. However in the FEM model, the model width was reduced to
account for the side groove.
Beff = B −
(B − BN )2
B
22

22. FEM Simulation Results
The simulation results are presented below.
1. J-Integral: The following (Load – J Integral) plot was obtained for the CT
specimen, with width=24.44mm.The experimental values are also shown for
comparison.
3D J-integral
180
160
J-integral (kN/m)
140
120
Experimental Data
100
Ansys Results
80
60
C T Specimen
w=50.81 mm
B=24.44 mm
a=25.5 mm
40
20
0
0
20
40
60
80
Load (kN)
2. Path independent J-Integral: This plot shows contours at various sections
along the width of the specimen. (Width of the specimen, w=B/2).These
results are in line with the expected path independent nature of J-Integral.
3D J-integral
200
180
J-integral (kN/m)
160
140
120
100
80
Section ,0< Z<B/10
60
Section ,(2B/10)< Z<(3B/10)
40
Section ,(4B/10)< Z<(5B/10)
20
0
0
20
40
60
80
Load (kN)
23

23. 3. Variation of local J-integral: The advantage of contour integral method is that
it allows the evaluation of J-integral locally at any location within the
specimen width. The following plot shows the comparison of the local Jintegral values and experimental values for different contours along specimen
width.
Variation of local J-integral along specimen thickness
140
J-Integral (kN/m)
120
Load=58 kN
100
80
Load= 58kN (Exp
Value)
Load=34 kN
60
40
Load=34 kN (Exp
Value)
Load=42 kN
20
0
0
5
10
Contours along Specimen Thickness
15
Load=42 kN (Exp
Value)
24

24. Results Comparison
Now the simulation results obtained are compared with the experimental results and
theoretical solutions described earlier.
Results Comparison
250
J-integral (kN/m)
200
Experimental Results
150
Ansys Results
Theoritical (pl. stress)
100
Theoritical (pl. strain)
50
0
0
20
40
60
80
Load (kN)
We can infer the following from the above plot:
1.The experimental and Ansys results are almost identical.
2.The results lie in between the theoretical solutions for plain stress and plain strain
conditions.
3.Within the elastic range of deformation (load less than 40 kN), the results and
theoretical solutions are identical.
The slight deviation in experimental and simulation results may be due to the
following differences:
• The experimental specimen was side grooved to maintain a straight crack
front,
But there is some deformation at the crack front boundaries in the FEM
model.
The material properties of the specimen material and the FEM model vary
slightly. The values inputted to the FEM model where through the RambergOsgood relation.
800
700
600
500
Stress [MPa]
•
400
300
200
100
experimental data
ramberg-osgood fit
0
0
0.05
0.1
0.15
0.2
0.25
0.3
Strain [-]
Fig 13.Plot of experimentally determined stress strain curve and Ramberg-Osgood fit
25

25. Conclusions
Experimental and FEM simulation results identical, hence this implementation in
ANSYS very effective in calculation of 3D J-Integral
Local J-Integral evaluation by domain integral method leads to a better
understanding of the crack front behavior.
The specimen geometry independent nature of the macros allows their usage
for J-Integral evaluation of other standard fracture specimens.
Suggestions
During the course of this work, many observations have encouraged in thinking
beyond the domains of this project and resulted in ideas for further extension of the
present work. So the following suggestions regarding possible future work in this field
are summarized below.
Finite Element calculation of K, G, J and CTOD and their mutual comparison
through available theoretical relations.
Comparison of different methods for calculation of J-Integral.
• Element Crack Advance Method
• Domain Integral Method
• 3D Line Integral
Extending J-integral calculations to dynamic crack length models.
26

26. References
1. T.L. Anderson., Fracture Mechanics: Fundamentals and Applications, CRC Press,
Boca Raton, FL, 1991.
2. Hertzberg, Richard W., Deformation and Fracture Mechanics of Engineering
Materials, John Wiley & Sons, 1996.
3. Prashant Kumar., Elements of Fracture Mechanics, Wheeler Publication, New
Delhi.
3. Cherepanov,C.P., Crack propagation in continuous media, Appl.Math.Mech.31
(1967),476-488
4. Rice,J.R., A path independent integral and the approximate analysis of strain
concentrations by notches and cracks,J.Appl.Mech.35(1968),379-386.
5. Hutchinson,J.W., ”Singular Behavior at the End of a Tensile Crack tip in a
hardening material.” Journal of the Mechanics and Physics of Solids, Vol. 16,
1968, pp.13-31
6.
Atluri, S.N., Energetic Approaches and Path-Independent Integrals in Fracture
Mechanics., Computational Methods in the Mechanics of Fracture, Chapter 5,
S.N. Atluri, Ed., pps. 121-165, 1986
7. Brocks.W, Scheider.I, Numerical Aspects of the Path-Independence of the J
-Integral in Incremental Plasticity.,GKSS-Forschungszentrum Geesthacht, October
2001.
8. Shih, C.F., Moran. B, Nakamura. T., Energy Release Rate along three dimensional
crack front in a thermally stressed body, International Journal of Fracture, Vol.30,
1986, pp.79-102.
9. Chandrupatla, T. R. and Belegundu, A. D., Introduction to Finite Elements in
Engineering, Prentice-Hall India, New Delhi, 2003.
27