1. An introduction to Computationnal Fracture Mechanics
J.Cugnoni, LMAF-EPFL, 2014

2. Stress based design vs Fracture Mechanics approach
Stress concentrator:
Critical stress is reached…
Stress based criteria (like Von Mises) usually define the onset of “damage” initiation in the material
Once critical stress is reached, what happens?
In this case, a defect is now present (ie crack)
The key question is now: will it propagate? If yes, will it stop by itself or grow in an unstable manner.
Stress analysis
A crack is formed…
Will it extend further?
If yes, will it propagate abruptly
until catastrophic failure?
Fracture mech.

3. Propagation criteria of a crack
Crack propagation : stress intensity factor
Stress intensity factors KI, KII, KIII measure the intensity of stress singularity at crack tip.
“Stress intensity factor”:
Constants of the 1/sqrt(r) term in stress field at crack tip:
“Critical Stress intensity factor”:
Maximum K that a material can sustain, considered as a material property and indentified in standard fracture tests. Units: Pa/sqrt(m), symbol: KIc KIIc KIIIc
Crack propagation occurs if
K > Kc with K=Kic +KIIc+KIIIc
In many materialy, propagation is mode I dominated:
KI>KIc
Assumed
Crack extension dA
Stress singularity
Fracture test: measure force at failure and calculate KIc
From analytical solutions or FE

4. Propagation criteria of a crack
Crack propagation : an “energetic” process
Extend crack length: energy is used to create a new surface (break chemical bonds).
Driving “force”: internal strain energy stored in the system
“Energy release rate”:
Change in potential energy P (strain energy and work of forces) for an infinitesimal crack extension dA. Units: J/m2, Symbol: G
measure the crack “driving force”
“Critical Energy release rate”:
Energy required to create an additionnal crack surface. Is a material characteristic (but depends on the type of loading). Units: J/m2, symbol: Gc
Crack propagation occurs if G > Gc
New crack surface dA:
Dissipates Ed=Gc*dA
Assumed
Crack extension dA
Potential energy: P0=U0-V0
Potential energy: P1= P0 –Er
And Er = G*dA

5. Computational Fracture Mechanics: Why?
Using numerical simulation method we can:
Apply Finite Element, Finite Volume/Difference, Boundary Element or Meshfree methods
To obtain approximations of displacement, force, stress and strain fields in arbitrary configuration.
And then? To apply fracture mechanics, we need:
to compute fracture mechanics parameters (SIF K, G) in 2D and 3D configurations;
to compute J integral in elastic-plastic analyses ;
to simulate crack growth (under general mixed- mode conditions);
FE simulation of a compact tension fracture test

6. Overview of the different techniques
Calculation of K (linear elasticity):
Stress or displacement field matching (single / mixed mode)
Indirectly from G (Interaction integrals in mixed mode)
Calculation of G:
Finite difference of potential energy (linear, evtl. non linear)
Compliance method (linear)
Virtual Crack Closure Technique VCCT (linear, mixed mode)
J-integral (non-linear)
Simulate crack growth
to VCCT criterion, node release, remeshing or XFEM
Cohesive elements / interfaces (Damage mechanics)

7. Calculation of KI: stress matching
Idea:
compare FE stress field at crack tip with theory,
fit KI from the numerical stress value
In LEFM (for r  0):
Step 1: From FE: Extract stress field Syy at =0 (along crack direction)
(eq 4.36a)

8. Calculation of KI: stress matching
Fitting method 1: Plot (as a function of r, for r  0)
Fit region
Fit a line over the quasi constant region of the plot, identify KI either as average value or as the intercept at r=0

9. Calculation of KI: stress matching
Fitting method 2: Plot as a function of
In theory the plot should be linear as:
Fit a line over the quasi linear region of the plot, identify KI either as the slope of the line
Note : the same method can be applied to get Kii from shear component at theta=0

10. Calculation of KI: displacement matching
Idea:
compare FE crack displacement opening field with theory,
fit KI from the numerical displacement value
In LEFM (for r  0):
Step 1: From FE: Extract stress field Syy at =0 (along crack direction)
(eq 4.40b) x
For plane stress:
m = shear modulus=
For plane strain:

11. Calculation of KI: displacement matching
Fitting method 1: Plot (as a function of r=-x, for r  0)
Fit region
Fit a line over the quasi constant region of the plot, identify either as the average value or as the intercept at r=0

12. Calculation of KI: displacement matching
Fitting method 1: Plot uy as a function
In theory, the plot should be linear as :
Fit a line over the quasi linear region of the plot, the slope is

13. Improving mesh convergence: singular elements
Evaluation of K from stress field requires very fine mesh. To better capture the 1/sqrt(r) stress singularity, one can use singular quadratic elements with shifted mid side nodes at ¼ of edge length (Barsoum,1976, IJNME, 10, 25; Henshell and Shaw, 1975, IJNME, 9, )
Using 8 node second order quadrangular elements, if we move the midside nodes at ¼ of edge, we make the Jacobian transformation of the element singular as 1/sqrt(r) along the element edges.
By collapsing all nodes of one edge (degenerate a quadrangle to a triangle), the 1/sqrt(r) singularity covers then the whole element.
Can be extended into 3D for 20 node hexahedrons

14. Computing K from G (and vice-versa)
For linear elastic isotropic materials, the following relations link G to K:
For plane stress:
For plane strain:
m = shear modulus=
For Mode I in plane stress and plane strain, this simplifies to:
So knowing either K or G, the other can be determined directly. This can be extended to orthotropic material.

15. Calculation of G: Strain energy method
compare the strain energy of several FE models with different crack length, calculate the ERR as the derivative of potential energy  = U - F
For a linear elastic material: the potential energy F = PD = 2U thus  = U – F = - U with the strain energy
Compute ERR or as the slope of U(a)
Different FE models for a0, a1, a2… a
Equations are for a unit depth, if not the case, compute use U/b instead of U

16. Calculation of G: Compliance method
Idea (similar to experimental test data reduction !)
Calculate the compliance C(a)=D(a)/P(a) for different crack lengths a0, a1 (several FE models required) and fit it with an appropriate function
For a linear elastic material: the ERR can be obtained from the C(a)
Compute ERR where dC/da is obtained from the fitted curve
(eq 3.41 & 3.43b) a
P, D
Different FE models for a0, a1, a2…

17. Calculation of G: J-integral method
Using the “J-Integral” approach (see course), it is possible to calculate the ERR G as G = J in linear elasticity.
If we know the displacement and stress field around the crack tip, we can compute J as a contour integral:
J-integral is path independent for all continuum materials. But G must be perpendicular to the interface if dissimilar materials are used.
W=strain energy density
u = displacement field
s = stress field
G = contour: ending and starting
at crack surface

18. Calculation of G: J-integral method
J-integrals are usually computed from a volume/surface integral in FE, for example in Abaqus with q = virtual crack extension vector:
With on G and on C. Using divergence and equilibrium equations we can obtain:

19. J-integral in 3D: 3D effects
J-integral can be extend in 3D by computing J on several “slices” of the model.
However, there are notable 3D effects affecting crack propagation:
in 3D, the external surface is free of normal stress, so in plane stress state
For thick specimens, the center of the specimen is closer to plane strain state
S22 on external surface
Plane stress
S22 on symmetry plane
Plane strain => higher stresses

20. J-integral in 3D: 3D effects
As a consequence, J-integral and G are not constant across the width.
This will lead to a slightly curved crack front during propagation
Need to be careful about specimen size effects when characterizing G or K
In 2D FE simulation: use plane stress for very thin specimens, and plane strain for thick ones.
G is max in the center => propagate earlier
G is min on the side => propagate last

21. Comparison of methods
Results obtained on a relatively coarse 3D mesh to highlight which methods are less mesh sensitive
External surface, plane stress
Stress fit1
Stress fit2
Displacement fit1
Displacement fit2
From J-integral
K from Abaqus K1
3870
4345
4380
5079
4337
4540
(units: Mpa*sqrt(mm))
Inside, plane strain (* please note that the FE data for u2 and s22 were extracted on free surface, a source of error)
Stress fit1
Stress fit2
Displacement fit1
Displacement fit2
J-integral
K from Abaqus K1
4345
3870
4813
5582
5144
5140
Strain energy, forward finite difference
Strain energy, backward finite difference
Strain en. centered finite difference
Strain energy fit
Compliance method
J integ. Avg G
322
282
302
302.5
301.5
296
(units: mJ/mm2)
Conclusion:
K determination is more sensitive to mesh !
G calculation using compliance, J-integral or strain energy fit are the most reliable

22. J-integral in Abaqus
Crack tip and
extension direction
Can be calculated in elasticity / plasticity in 2D plane stress, plane strain, shell and 3D continuum elements.
Requires a purely quadrangular mesh in 2D and hexahedral mesh in 3D.
J-integral is evaluated on several “rings” of elements: need to check convergence with the # of ring)
Requires the definition of a “crack”: location of crack tip and crack extension direction
Quadrangle mesh
Crack plane
Rings 1 & 2

23. J-Integral in Abaqus: application notes and demonstration
Create a linear elastic part, define an “independent” instance in Assembly module
Create a sharp crack: use partition tool to create a single edge cut, then in “interaction” module, use “Special->Crack->Assign seam” to define the crack plane (crack will be allowed to open)
In “Interaction”, use “Special->Crack->Create” to define crack tip and extension direction (can define singular elements here, see later for more info)
In “Step”: Define a “static” load step and a new history output for J-Integral. Choose domain = Contour integral, choose number of contours (~5 or more) and type of integral (J-integral).
Define loads and displacements as usual
Mesh the part using Quadrangle or Hexahedral elements, if possible quadratic. If possible use a refined mesh at crack tip (see demo). If singular elements are used, a radial mesh with sweep mesh generation is required.
Extract J-integral for each contour in Visualization, Create XY data -> History output.
!! UNITS: J = G = Energy / area. If using mm, N, MPa units => mJ / mm2 !!!
By default a 2D plane stress / plane strain model as a thickness of 1.
See demo1.cae example file

24. Singular elements & meshing tips
To create a 1/sqrt(r) singular mesh:
In Interaction, edit crack definition and set “midside node” position to (=1/4 of edge) & “collapsed element side, single node”
In Mesh: partition the domain to create a radial mesh pattern as show beside. Use any kind of mesh for the outer regions but use the “quad dominated, sweep” method for the inner most circle. Use quadratic elements to benefit from the singularity.
Refine the mesh around crack tip significantly.

25. J-integral Convergence vs # contours

26. Fracture mechanics oriented design
Stress analysis
Perform a stress analysis
Locate stress critical regions
analysis
Crack
Assume the presence of a defect in those regions (one at a time)
Consider different crack lengths and orientation
For each condition, check if the crack would propagate and if yes if it is stable or not
Design evaluation
Define operation safety conditions: maximum stress / crack length,… before failure occurs
Define damage inspection intervals / maintainance plan

27. Resources & help Abaqus tutorials: Abaqus Help:
Abaqus Help:
See Analysis users manual, section 11.4 for fracture mechanics
Presentation and demo files:
Computers with Abaqus 6.8:
40 PC in CM1.103 and ~15 in CM1.110