J.Cugnoni, LMAF-EPFL, 2014

 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. A crack is formed… Will it extend further? If yes, will it propagate abruptly until catastrophic failure? Stress concentrator: Critical stress is reached… Stress analysis Fracture mech.

 Crack propagation : stress intensity factor ◦ Stress intensity factors K I, K II, K III 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: K Ic K IIc K IIIc  Crack propagation occurs if K > Kcwith K=K I +K II +K III  In many materialy, propagation is mode I dominated: K I >K Ic Assumed Crack extension dA Stress singularity Fracture test: measure force at failure and calculate K Ic From analytical solutions or FE

 Crack propagation : an “energetic” process ◦ Extend crack length: energy is used to create a new surface (break chemical bonds). ◦ Driving “force”: potential energy stored in the system  “Energy release rate”: ◦ Change in potential energy  (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: G c  Crack propagation occurs if G > Gc New crack surface dA: Dissipates E d =Gc*dA Assumed Crack extension dA Potential energy:  0=U0-V0 Potential energy:  1=  0 –E r And E r = G*dA

 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

 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 ◦ use VCCT criterion, node release, remeshing or XFEM ◦ Cohesive elements / interfaces (Damage mechanics)

 Idea: ◦ compare FE stress field at crack tip with theory, ◦ fit K I 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) r

 Fitting method 1: Plot (as a function of r, for r  0)  Fit a line over the quasi constant region of the plot, identify K I either as average value or as the intercept at r=0 Fit region

 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 K I either as the slope of the line Note : the same method can be applied to get Kii from shear component at theta=0

 Idea: ◦ compare FE crack displacement opening field with theory, ◦ fit K I from the numerical displacement value ◦ In LEFM (for r  0):  Step 1: From FE: Extract stress field Syy at  =0 (along crack direction) (eq 4.40d) x For plane stress: For plane strain:  = shear modulus=

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

 Fitting method 1: Plot u y 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

 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, )  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  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.

 For linear elastic isotropic materials, the following relations link G to K: For plane stress: For plane strain:  = 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.

◦ 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 = P  U 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

a P,   Idea (similar to experimental test data reduction !) ◦ Calculate the compliance C(a)=  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 Different FE models for a0, a1, a2… (eq 3.41 & 3.43b)

 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  = contour: ending and starting at crack surface

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

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

As a consequence, J-integral and G are not constant across the width. This will lead to a slightly curved crack front during propagation G is max in the center => propagate earlier -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 min on the side => propagate last

 Results obtained on a relatively coarse 3D mesh to highlight which methods are less mesh sensitive External surface, plane stress Stress fit1Stress fit2Displacement fit1Displacement fit2 From J- integral K from Abaqus K (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 fit1Stress fit2Displacement fit1Displacement fit2J-integral K from Abaqus K Strain energy, forward finite difference Strain energy, backward finite difference Strain en. centered finite difference Strain energy fit Compliance method J integ. Avg G (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

 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 Rings 1 & 2 Crack plane Crack tip and extension direction Quadrangle mesh

 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

 To create a 1/sqrt(r) singular mesh: ◦ In Interaction, edit crack definition and set “midside node” position to 0.25 (=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.

 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)

a P,   VCCT is based on the calculation of the work done by elastic forces to close the crack tip, ie the work done to move the 1st node of the crack to its “closed” position  By decoupling normal and tangential displacement VCCT can be used to calculate mode I and II ERR in mixed mode case.  The work done to close the crack give the ERR: Wc = G*dA  Method 1: stiffness If the system is elastic: F=k d 0 => Wc=2 x (1/2 k d 0 2 ) => 2 step: compute d0, compute k Crack surface closed dA=L b: E d =Gc*dA F, d 0 L

a P,  a  Method 1: stiffness If the system is elastic: F=k d 0 => Wc=2 x (1/2 k d 0 2 ) Step 1:  Apply loading conditions  FE solution => extract d 0 Step 2:  Apply a closure force (dipole) F  FE solution => extract d 1  Compute k=F/(d 0 -d 1 ) Compute work: Wc =2 x (1/2 k d 0 2 ) and ERR: G I = Wc/dA=Wc/(L b) d0d0 d0d0 COD Step 1: external loading measure COD = 2*d 0 F, d 1 Step 2: perturbation F measure COD = 2*d 1

 Method 2: self similarity If the crack length extension da is small then the fields at crack tip can be considered self-similar (invariant with da) system is elastic. Only one step is then required for VCCT : (image src Abaqus documentation) FiFi d i-1 FjFj didi But with self similarity: F j =F i and d i =d i-1

Mode mixity can be accounted for by decoupling the work into normal and tangential component:  GI is obtained from normal displacement and force dn and Fn : G I =1/2 (Fn dn) / dA  GII from tangential displacement and force dt and Ft: G II =1/2 (Ft dt) / dA dn dt Fn Ft

 Critical stress or opening displacement at a distance: Need to be calibrated on tests and are potentially mesh sensitive !! Not exactly a Fracture mechanics criterion, but can be related to ERR or K

 Mixed mode crack propagation criteria: Combine G I, II, III in an expression G eq (G I,G II,G III ). Propagation if G eq >G eqC or G eq /G eqC >1 Need to be calibrated on mixed mode tests This requires a lot of work!! BK criterion: Power law :

 Model energy dissipation in the process zone at crack tip by the work of dissipative forces.  CZM are based on damage mechanics and can model complex crack propagation in mixed mode, including fiber bridging.  Available either in the form of cohesive elements or cohesive contact formulations F, d CZM: Process zone= Cohesive forces Process zone: Plasticity, micro cracking…

Basic ideas: -Discretize the fracture process zone and replace it by “springs” to represent crack tip forces (with a high stiffness K) -Model dissipation through evolution of damage D => K=(1-D) K 0 -Evolve the damage variable D based on a “traction” – “crack opening” relationship F, d, F=  da F, d cc    max K0K0 Damage initiation (D=0)  c Damage propagation (D>0) Elastic unloading / reloading (D=cst)Dissipated Energy Final failure D=1 Total energy dissipated = G cc

Elastic unloading / reloading (D=cst, K=cst) cc    max K0K0 Damage initiation (D=0)  c Damage propagation (D>0) K=(1-D) K 0 Dissipated Energy cc K=(1-D) K 0

cc    max K0K0 Damage propagation (D>0) Elastic unloading / reloading (D=cst) Dissipated Energy Final failure D=1

cc    max K0K0 Damage propagation (D>0) Total Dissipated Energy = G = ½  c  max Final failure D=1

cc    max K0K0 Damage initiation (D=0)  c Damage propagation (D>0) Dissipated Energy G Final failure D=1 cc How to define all those constants? 1)Measure G from fracture tests and  c from a strength test 2)Calculate  max from G= ½  c  max 3)K must be set sufficiently high (penalty stiffness) Recommendation: Estimate  c ~  max / R with R ~ [10-100] Calculate K 0 as K 0 =  c /  c

cc    max K0K0 G cc Example: crack propagation in an adhesive G = 0.1 mJ/mm2 and  c = 10 MPa  max = 2 G/  c =0.02 mm  c ~  max / 10 =>  c = mm  K 0 =  c /  c = 5000 N/mm d=5mm DCB, plane strain, 25mm wide, 2x2.5 mm thick, 100mm length Adhesive layer: 0.2mm thick, 60mm long, Cohesive elements Tie constraints

 In material properties: ◦ define K in “Elastic” properties, type “Traction”; ◦ Enter critical stress in “Damage for Traction separation Law” type QuadS for example ◦ Add the option “Damage evolution”, based on Energy with Linear degradation etc... Enter G as critical ERR  Define a cohesive section and assign it to the “glue” layer: ◦ type “Traction separation”, initial thickness = 1, out of plane thickness = 25 mm here.  In mesh: ◦ Cohesive element MUST be generated as a single layer of elements using quad sweep (or hexa sweep) algorithms. The sweep direction will define the “normal” direction of the cohesive element! ◦ Assign the type of element “Cohesive” (not by default)  In Step: ◦ Set initial & max time increment to 0.05 (both) ◦ Define a field output with the variable “SDEG” (= Damage D)

Stress analysis Perform a stress analysis Locate stress critical regions Crack analysis 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

 Abaqus tutorials: ◦  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