FRANC 3 D WorkshopTraining Corning Glass May 7

FRANC 3 D Workshop/Training Corning Glass May 7, 2012 Drs. Paul “Wash” Wawrzynek, Bruce Carter, Tony Ingraffea, and Omar Ibrahim 1

Objectives • General introduction to FRANC 3 D: - capabilities and limitations • Present theory and approaches to computational fracture mechanics built into the program. • Hands-on sessions give participants a chance to try the code with tutors here to help. • Opportunity for participants to ask questions. 2

Agenda • Introduction to FRANC 3 D • Demo/Hands-on: build an uncracked model • Overview of the crack insertion process • Demo/Hands-on: insert initial crack and run analysis • Stress Intensity Factor (SIF) computation - theory • Demo/Hands-on: SIF computation - practice • Crack growth - theory • Demo/Hands-on: Crack growth - practice • Demo/Hands-on: Student generated models 3

FRANC 3 D Product • FRANC 3 D (FRacture ANalysis Code 3 -D) uses finite element method to simulate crack growth analysis • Adaptively remeshes a finite element model to simulate crack growth. • Has several elements to be used for modeling the crack front 4

FRANC 3 D Product • Designed to work in conjunction with a commercial finite element solvers: – ANSYS – ABAQUS – NASTRAN • The FRANC 3 D program has a programming interface that is an extension to the Python programming language. • Written in the C++ programming language • Support the following operating systems: – Windows – Linux 5

FRANC 3 D Development History • 1988 to 1994 – • 1994 to 2001 – • Completely new code written in C++ FRANC 3 D v 5. 0 – Additional enhancements 2010 to 2011 – • FRANC 3 D v 4. 0 Solid FEM only (ANSYS, ABAQUS, NASTRAN) 2009 to 2010 – • FRANC 3 D v 3. 0 BEM & Thin Shell & Solid FEM (ANSYS) 2005 to 2009 – – • FRANC 3 D v 2. 0 BEM & Thin Shell FEM 2001 to 2005 – • FRANC 3 D v 1. 0 BEM only FRANC 3 D v 6. 0 – Fretting Fatigue, Fatigue Life, Post-processing & other enhancements 2012 – FRANC 3 D v 7. 0 is under development 6

FRANC 3 D Development History • Development of FRANC 3 D was funded by: – USA Air Force – USA Navy – NASA – Others 7

What Does FRANC 3 D Do? • insert a flaw into an existing finite element mesh and remesh locally, using special crack-front elements. • compute stress intensity factors (SIF’s) for all nodes along a crack front for isotropic and anisotropic materials. • predict how a crack will grow (relative extension and angle) using engineering growth criteria, and will then extend the crack geometry and remesh locally. 8

What FRANC 3 D is NOT • not a general finite element pre-processor or postprocessor. External codes are required to build uncracked FE models and to visualize results (FRANC 3 D can display deformations). • not a finite element analysis program. An external FE code is required (e. g. , ANSYS or ABAQUS) to perform stress analysis. • not a general purpose fatigue life prediction code, although some basic life prediction models are available. An external lifing code (e. g. , AFGRO, NASGRO or DARWIN) can be used. 9

FRANC 3 D Typical Work Flow ANSYS/ABAQUS/NASTRAN Full 3 D FE Model portion to be cracked Stress Analysis remainder of model FRANC 3 D Define crack(s) geometry Insert crack(s) into portion of model and remesh Compute stress intensity factors Extend crack(s) geometry Combine portions displacements, temperatures, crack surface tractions 10

Global and Sub-models “sub-model” crack growth region “global” model FE package (e. g. , ANSYS or ABAQUS) is used to define a global model and a submodel. The sub-model should encompass the crack growth region with ‘space’ 11 for remeshing.

FRANC 3 D Modifies the Sub-model uncracked model after crack insertion FRANC 3 D modifies the sub-model, inserting a crack and remeshing the model locally. It outputs an input file that combines the global and sub-model (ABAQUS) or it outputs the sub-model and a macro command file that will combine the models (ANSYS). 12

FRANC 3 D Maintains Compatibility mesh compatibility FRANC 3 D can retain surface meshes on “cut” surfaces so that there is FE compatibility between the global and sub-model. This is the preferred approach. However, FRANC 3 D can also instruct the FE program to insert constraint equations. 13

Combined (Full Model) Analysis FRANC 3 D does not use a global/local approach. The FE analysis is performed with the full combined model. (However, a global/local 14 approach can be used. )

Crack Growth after 21 steps of crack growth Crack growth is simulated by FRANC 3 D repeatedly reading and modifying the initial sub-model. At each step, the global and modified sub-model are re-combined and the full model is analyzed. 15

Sub-models for “free” meshes “free mesh” cut surfaces It is possible to cut out a FRANC 3 D sub-model from a “free” (unstructured) mesh. (However, surfacets of tetrahedral elements with poor aspect ratios can cause local meshing problems. ) 16

Agenda • Introduction to FRANC 3 D • Demo/Hands-on: build an uncracked model • Overview of the crack insertion process • Demo/Hands-on: insert initial crack and run analysis • Stress Intensity Factor (SIF) computation - theory • Demo/Hands-on: SIF computation - practice • Crack growth - theory • Demo/Hands-on: Crack growth - practice • Demo/Hands-on: Student generated models 17

FRANC 3 D Tutorials Using ANSYS: Using ABAQUS: simple global model vs submodel with global model through-crack extract sub-model automated crack growth crack insertion & automated growth crack face traction vs far-field loading 18

FRANC 3 D Tutorials Step 1: Build the FE model Step 2: Extract small portion from the full FE model Step 2. 1: Separate element components • Separate the FE model into a small portion (local model) and the remaining of the FE model (global model) • Local FE model will be used for fracture analysis Local Model Global Model 19

FRANC 3 D Tutorials Step 2. 2: Create node component for cut-surface • Select the nodes on the cut surfaces of each component and save a node component. For the 3 x 3 x 3 ‘local’ model, name this node component CUT_SURF. Step 2. 3: Save local and global • Archive each element component as a separate model for the local and other for global • Global model, which consists of the exterior elements, will include the boundary conditions and material properties • Local model will include the CUT_SURF node component and FRANC 3 D will use this information to retain those mesh facets 20

FRANC 3 D Tutorials Step 3: Read the local FE model into FRANC 3 D • Step 3. 1: Reading Local FE Model • Start with the FRANC 3 D graphical user interface • Select File and Open • Switch File Filter in the Open Model File dialog box to proper file extension name and select the file name for the local model • Click Accept. 21

FRANC 3 D Tutorials Step 3. 2: Selecting the Retained Items in the Local FE Model • Material, mesh facet groups, contact/constraint & residual stress 22

FRANC 3 D Tutorials Step 3. 3: Selecting Cut Surface Nodes • Lists the node components present in the local FE model file 23

FRANC 3 D Tutorials Step 3. 4: Importing and Displaying the Local FE Model • User can turn on the surface mesh and manipulate the view 24

Agenda • Introduction to FRANC 3 D • Demo/Hands-on: build an uncracked model • Overview of the crack insertion process • Demo/Hands-on: insert initial crack and run analysis • Stress Intensity Factor (SIF) computation - theory • Demo/Hands-on: SIF computation - practice • Crack growth - theory • Demo/Hands-on: Crack growth - practice • Demo/Hands-on: Student generated models 25

FRANC 3 D Wizard for Defining the Crack Type and Meshing Process for the Cracked Portion of the FE Model 26

Current Crack Type Options in FRANC 3 D • Elliptical Crack • Through-the-thickness – One crack front – Two crack fronts • Long-shallow surface crack shape • Elliptical crack shape with two fronts • User-defined crack 27

Defining Crack Geometry • Crack geometry and location can be prescribed either by: – Interactively using the Graphical User Interface (GUI) – Using FRANC 3 D extensions to the Python programming language 28

Crack Insertion Wizard (Elliptical Flaw) crack size/shape parameters Define the crack surface geometry, position and orient crack-front template parameters 29

Crack Insertion Wizard – Flaw Library 30

User Defined Crack Front Points User-defined flaw allows an analyst to define an arbitrary (planar) shape by entering (or reading from a file) a series of points that define the vertices of a polygon. Crack front vertices 31 should be flagged.

Surface Meshes after Crack Insertion crack surface mesh 32

Crack-Front Template Element Types tetrahedral elements are used for the bulk of the volume quarter-point singular wedge crack-front elements pyramids enforce compatibility between brick and tetrahedral elements two or more “rings” of brick elements 33

Crack Insertion: Input Sub-model Mesh The first major input to the crack insertion procedure is a finite element mesh. Usually this is a sub-model, but a full model mesh is acceptable. In the case of a sub-model, the cut surfaces are flagged. sub-model cut surface cutting planes This model has brick elements only. However, brick, wedge, pyramid, and tetrahedral elements of both first and second order are okay. Currently, FRANC 3 D can handle ANSYS, ABAQUS and NASTRAN models. 34

Crack Insertion: Approximate Surface Geometry Curved surface geometry is approximated from the faceted surface of the input finite element mesh. Locally refined meshes near flaws will fall on the curved surface rather than on the faceted finite element input. Step 1: compute weighted average normals at all nodes. Step 2: define 1 or 2 triangular Bezier patches for each FE facet. Step 3: identify “topological” edges and group together facets that form logical faces. Bezier patches Topological edges and logical faces Note that FE facets on the cut surfaces are retained for compatibility 35

Crack Insertion: Flaw Definition The second major input to the crack insertion procedure is a description of a flaw shape and location. FRANC 3 D has tools to define and place a flaw interactively. Flaws can be zero volume (cracks) or finite volume (voids). The crack above appears to have a piecewise linear crack front, but that is a just a display artifact. Flaw surfaces are defined as Bezier patches and can have curved crack fronts. In theory, initial flaws can be non-planar, but there is currently no practical user-interface for such a capability. 36

Crack Insertion: Crack-Front Templates Crack-front templates are generated to emplace regular well-shaped elements near crack fronts. The template elements are a combination of brick and quarterpoint wedge elements. Additional processing is required where templates intersect free surfaces. Locally template element topology and geometry must be modified to conform to the surface geometry. A typical template cross -section 37

Crack Insertion: Intersections & Trimming Surface/surface intersections are computed for all body and flaw patches. The body and flaw patches are trimmed and combined into one composite object. Outside Inside Trimmed patches are divided into triangular subpatches to keep the model “water-tight”. 38

Crack Insertion: Surface Meshing Surface meshes are generated for all “logical” model surfaces. The surface meshes are constrained to conform to the meshes on cut surfaces. retained cut surface meshes 39

Crack Insertion: Pyramids & Volume Meshing Pyramid elements are generated to enforce compatibility between quadrilateral facets on both the template and “cut” surfaces and triangular faces in the volume mesh. cut surfaces template surfaces An advancing front meshing algorithm* is used to generate a tetrahedral volume mesh (not shown). This algorithm respects the special case of distinct nodes on opposite sides of crack faces, which are geometrically coincident. *Neto, J. B. , Wawrzynek, P. A. , Martha, L. F. , and Ingraffea, A. R. , “An algorithm for threedimensional mesh generation for arbitrary regions with cracks, ” Engng with Comp. , 40 vol. 17, 75 -91 (2001)

Volume Meshing • After completing the surface, the volume mesh starts • Options for performing volume meshing: – FRANC 3 D – ANSYS – ABAQUS CAE • Final mesh smoothing are used to improve the elements quality 41

A Sub-Volume Definition Issue Retained cutsurfacet It can be difficult to mesh a thin section that is constrained with a large quadrilateral patch on one side. There is not enough room for a well shaped pyramids and transition tetrahedral elements. 42

Workshop Agenda • Introduction to FRANC 3 D • Demo/Hands-on: build an uncracked model • Overview of the crack insertion process • Demo/Hands-on: insert initial crack and run analysis • Stress Intensity Factor (SIF) computation - theory • Demo/Hands-on: SIF computation - practice • Crack growth - theory • Demo/Hands-on: Crack growth - practice • Demo/Hands-on: Student generated models 43

FRANC 3 D Tutorials – Crack Insertion Steps • Step 1: Selecting Cracks from FRANC 3 D Menu – From the FRANC 3 D menu, select Cracks and New Flaw Wizard. The first panel of the wizard should appears. The default flaw type is Crack (zero volume flaw) and select Next. 44

FRANC 3 D Tutorials – Crack Insertion Steps • Step 2: Selecting Crack Type – The next panel allows the user to choose type of crack, hint Next after the selection. 45

FRANC 3 D Tutorials – Crack Insertion Steps • Step 3: Specify the Crack Size – The next panel allows us to specify the size of the ellipse. Select Next after the size definition. 46

FRANC 3 D Tutorials – Crack Insertion Steps • Step 4: Specify Crack Location and Orientation – The next panel allows us to specify location and orientation of the flaw. After defining the location and orientation; select Next. 47

FRANC 3 D Tutorials – Crack Insertion Steps • Step 5: Specify Crack Front Template Parameters – The next panel allows us to specify the crack front template parameters. After specifying the parameters; select Finish. 48

FRANC 3 D Tutorials – Crack Insertion Steps • Step 6: Surface and Volume Meshing of Local Model after the Crack Insertion – FRANC 3 D begins the process of inserting the flaw into the original model and then meshes the resulting cracked model. – Operations is displayed on the screen – When meshing is completed, the newly meshed cracked model will be displayed. 49

FRANC 3 D Tutorials – Static analysis Steps • Step 1: Select Static Crack Analysis – From the FRANC 3 D menu, select Analysis and Static Crack Analysis. The first panel of the wizard should appear, specify the file name for the FRANC 3 D database first. 50

FRANC 3 D Tutorials – Static analysis Steps • Step 2: Select FE Solver – Next panel allows you to specify the solver 51

FRANC 3 D Tutorials – Static analysis Steps • Step 3: Select Analysis Options – Next panel allows you to specify the solver output and analysis options – Specify global models – Use all quadratic elements – Solver executable should be defined 52

FRANC 3 D Tutorials – Static analysis Steps • Step 4: Merging Local/Global FE Models – Next panel allows for the specification of whether the local and global models are combined by merging nodes or by defining constraints or contact conditions. – Specify node component names in the local and global models for nodes that will be merged or you can let the programs (FRANC 3 D and Solver) do the work. – Select Finish 53

Workshop Agenda • Introduction to FRANC 3 D • Demo/Hands-on: build an uncracked model • Overview of the crack insertion process • Demo/Hands-on: insert initial crack and run analysis • Stress Intensity Factor (SIF) computation - theory • Demo/Hands-on: SIF computation - practice • Crack growth - theory • Demo/Hands-on: Crack growth - practice • Demo/Hands-on: Student generated models 54

Stress Intensity Factors 55

Continuum Fracture Modes y, v x, u z, w Mode III Basic modes of crack loading. Positive sense shown for each: Mode I = crack opening Mode II = in-plane sliding Mode III = anti-plane tearing EACH MODE HAS ITS OWN STRESS INTENSITY FACTOR 56

Stress Intensity Factors • FRANC 3 D Computes the stress intensity factors associated with all three “modes” of fracture for the mid-side nodal points along the crack front • Under conditions of small-scale yielding, all crack front displacement fields (crack behavior) are controlled by the stress intensity factors – Stability – will the crack tip move? – Trajectory – in what direction? – Rate – how fast? 57

Computing Stress Intensity Factors FRANC 3 D has two methods to compute stress intensity factors (SIF’s): Displacement Correlation: • Relatively simple to understand implement • Relatively poor accuracy (~5% error for a reasonable mesh) • Good sanity check but not for production work M-Integral (Interaction Integral): • Somewhat involved formulation and implementation. • In the literature, the M-Integral is sometimes known an "interaction integral”. • Relatively good accuracy (<1% error for a reasonable mesh) • Requires special additional terms for crack face tractions, residual 58 stresses, FGM’s, etc.

Computing Stress Intensity Factors M-Integral (Interaction Integral): • Numerically the M-Integral is similar to the J-Integral. • M-Integral is used to compute the strain energy release energy rates (GI, GII, and GIII) and stress intensity factors (KI, KII, and KIII) associated with the three modes of fracture. – Mode II (KII) is needed to predict the crack kink angle to determine the crack front direction • M-integral implementation in FRANC 3 D allows the computation of the three modes of SIFs for isotropic and anisotropic materials. – FRANC 3 D is the only available code that will compute stress intensity factors for generally anisotropic materials • The method to use for production work 59

Stress Intensity Factor Computations SIF’s are computed with the M-integral for isotropic and generally anisotropic materials. 60 60

Fracture mechanics gives theoretical asymptotic displacement fields. , v , u Note: for plane stress, let n = n/(1+ n) Set r = ra-b, and q = 180° 61

Displacement Correlation Methods For plane strain case: ra-b where m is the shear modulus, n is Poisson's ratio, r is the distance from the crack tip to the correlation point, and ui, vi, wi are the x, y, and z displacements at point i The same expressions can be used for plane stress assumptions if n is replaced with n = n / (1+n). 62

Energy Release Rates The crack-tip energy release rates can be determined from Irwin’s crack closure integral Substituting crack-tip stress and displacement fields yields 63

The J-Integral* measures the energy flux into the crack-tip region Under conditions of small scale yielding the J -Integral is equal to the energy release rate The contour J-Integral can be recast as an equivalent area (volume in 3 D) integral**, which is more accurate and stable in a finite element context q is a function that is one at the crack tip and zero on the boundary of the integration domain. It can be interpreted as a virtual crack extension. * Rice, J. R. (1968) A path independent integral and approximate analysis of strain concentrations by notches and cracks, Journal of Applied Mechanics, 35, 379 -386 ** Li, F. Z. , Shih, C. F. , and Needleman, A. (1985) A comparison of methods for calculating energy release rates, Engineering 64 Fracture Mechanics, 21, 405 -421

The 3 D J-Integral In 3 D, the J-Integral is evaluated within a cylindrical domain centered on a portion of the crack-front In 3 D 65

Formulating the M-Integral From the Stress and Displacement Fields For linear analysis, we can add two valid solutions and the result is a valid solution take the (1) solution to be the FEM results the (2) solution(s) are solutions we get to select Substituting these into the expression for the J-integral where 66

Formulation of the M-Integral (cont. ) Collecting terms or with A definition of M in terms of the crack tip field variables we can get from an FEM analysis (solution 1) or form theoretical expressions if we know KI, KII, and KIII (solution 2) 67

Formulating the M-Integral From the Definition of the Energy Release Rate for small scale yielding substituting into the expression for the energy release rate 68

Formulation of the M-Integral (cont. ) A definition of M in terms of K’s and material properties. equating the two definitions for the M-Integral 69

Formulation of the M-Integral (cont. ) We use the FEM results for the (1) solution We select three simple auxiliary solutions (2 a), (2 b), and (2 c) KI KIII a 1. 0 0. 0 b 0. 0 1. 0 0. 0 c 0. 0 1. 0 From the analytical expressions for the crack-front fields, we obtain Substitution gives three equations for the unknown K(1)’s 70

Independent FRANC 3 D Mode I SIF Verification CCT SEN Analyses performed by Dawn Phillips of the NASA Langley Research Center 71

Independent FRANC 3 D Mode I & II SIF Verification Slant edge crack starting from a circular hole Analyses performed by Dawn Phillips of the NASA Langley Research Center Mode II 72

Typical Isotropic M-Integral Verification Surface crack, a = c = 0. 8, remote unit traction Stress intensity factors are computed at all nodes along the crack front FRANC 3 D crack front The oscillations arise because different virtual crack extension are used for element corner and mid-side nodes. virtual crack extensions corner node mid-side node 73

Anisotropic Stress Intensity Factors • FRANC 3 D includes an M-Integral implementation for general anisotropic materials. 1, 2 Wawrzynek, P. A. , Carter, B. , and Banks-Sills, L. “The M-integral for computing stress intensity factors in generally anisotropic materials, ” NASA/CR-2005 -214006 1 Banks-Sills, L. , Wawrzynek, P. A. , Carter, B. , Ingraffea, T. R. , and Hershkovitz, I. , “Methods for computing stress intensity factors in anisotropic geometries: Part II – arbitrary geometry, ” Engng. Fracture Mech. , in review 2 74

Workshop Agenda • Introduction to FRANC 3 D • Demo/Hands-on: build an uncracked model • Overview of the crack insertion process • Demo/Hands-on: insert initial crack and run analysis • Stress Intensity Factor (SIF) computation - theory • Demo/Hands-on: SIF computation - practice • Crack growth - theory • Demo/Hands-on: Crack growth - practice • Demo/Hands-on: Student generated models 75

FRANC 3 D Tutorials – SIF Computation Steps • Step 1: Re-Open FRANC 3 D restart file – From the FRANC 3 D menu, select File and Open. – Choose the *. fdb file and select OK. – FRANC 3 D will automatically read the FE solver results 76

FRANC 3 D Tutorials – SIF Computation Steps • Step 2: Select Compute SIFs – From the FRANC 3 D menu, select Cracks and Compute SIFs. The Stress Intensity Factor wizard is displayed – Use the M-Integral – User can select thermal or crack face traction terms if they are used. – Select Finish, the SIFs Plot dialog is displayed 77

FRANC 3 D Tutorials – SIF Computation Steps • Step 2 (cont’d): Select Compute SIFs – View the three stress intensity factor (SIF) modes and export the data 78

Workshop Agenda • Introduction to FRANC 3 D • Demo/Hands-on: build an uncracked model • Overview of the crack insertion process • Demo/Hands-on: insert initial crack and run analysis • Stress Intensity Factor (SIF) computation - theory • Demo/Hands-on: SIF computation - practice • Crack growth - theory • Demo/Hands-on: Crack growth - practice • Demo/Hands-on: Student generated models 79

Crack Growth 80

Crack Growth Stress Intensity Factors are used to predict the direction and relative extent of crack growth 81

Crack Growth Prediction within FRANC 3 D • Computing crack front growth is a three-step process: – Kink angle for each node (direction) • Based on the crack-front stresses in polar coordinates • Five options for computing kink angle – Relative amount of local crack extension for each node • Computed using a fatigue growth model (using one node extension with a median SIF or using a specify number of load cycles) • Simplest model is Paris growth model – Smooth the crack front • Polynomial curves are used to fit the crack front • User can specify the order of the polynomial or FRANC 3 D find the polynomial order that will give the best fit 82

Crack Growth after 21 steps of automatic crack growth Confidential 83 83

84

Crack Extension Cracks are “extended” by “reinserting” an extended crack definition. This approach to extension: 1) simplifies the code, 2) reduces the amount of information stored between steps, and 3) allows the sub-volume to be changed between crack growth steps. initial crack non-planar crack growth crack extension meshed extended crack 85

86

87

Kink Angle: Max Stress Criterion (orthotropy) The orthotropic max stress criterion says that the crack will kink in the direction where the ratio of the hoop stress to the effective toughness is maximum. Where Keff is a function of six principal toughnesses and crack orientation relative to the material predicted direction of crack propagation 88

SIF (K) time 89

load case a SIF (K) load case b time 90

time 91

92

Kink Angle: Max Stress Criterion (isotropy) The max stress criterion says that the crack will kink in the direction of a maximum value of a stress component. Some materials show a transition from Mode I to Mode II crack growth for stable tearing. LEFM Max stress Amstutz (1995) 2024 -T 3, L-T Amstutz (1995) 2024 -T 3, T-L Hallback & Nilsson (1994) 7075 -T 6 Maccagno & Knott (1989), PMMA Maccagno & Knott (1991), HY 130 @ -196 C 80 70 Mode I 60 50 40 30 Transition 2024 -T 3 Transition 7075 -T 6 20 10 Mode I only: 0 -10 Mode I or Mode II: Mode II -20 -30 0 10 20 30 40 50 60 70 80 90 93

94

under development, ignore for now 95

predicted new crack front point i point with the median K value current crack front Dai computed extension Dam specified extension 96

predicted new crack front point i current crack front Dai computed extension 97

NASGRO Equation Dialog 98

Can read AFGRO formatted files and excel CSV or text files. User Equation Dialog 99

no crack front fitting user specified polynomial order Program selected polynomial order polynomial fit no smoothing 100

101

All crack increments are specified 102

All cycle increments are specified 103

Workshop Agenda • Introduction to FRANC 3 D • Demo/Hands-on: build an uncracked model • Overview of the crack insertion process • Demo/Hands-on: insert initial crack and run analysis • Stress Intensity Factor (SIF) computation - theory • Demo/Hands-on: SIF computation - practice • Crack growth - theory • Demo/Hands-on: Crack growth - practice • Demo/Hands-on: Student generated models 104

FRANC 3 D Tutorials – Manual Crack Growth Steps • Step 1: Select Grow Crack – From the FRANC 3 D menu, select Cracks and Grow Crack – Crack Growth wizard is displayed – Choose Quasi-Static or Fatigue growth type – Select Next 105

FRANC 3 D Tutorials – Manual Crack Growth Steps • Step 2: Specify Growth Rate – Second panel of the Crack Growth allows you to specify the growth rate model data – Use the Paris model and set C to 1 e-10 and leave n at 2 – Select Next. 106

FRANC 3 D Tutorials – Manual Crack Growth Steps • Step 7. 3: Specify Extension or Cycles – Third panel of the Crack Growth allows you to specify whether you will grow the crack based on a median extension or a number of cycles – Use a median extension – Select Next. 107

FRANC 3 D Tutorials – Manual Crack Growth Steps • Step 7. 4: Specify Fitting and Extrapolation – Fourth panel of the Crack Growth allows you to specify a value for median extension as well as the fitting and extrapolation parameters – Specify a median extension of 0. 1 and use a fixed 3 rd order polynomial with 3% extrapolation on both ends to ensure the fitted end points fall outside the model – Select Next 108

FRANC 3 D Tutorials – Manual Crack Growth Steps • Step 7. 5: Specify Crack Front Template – Final panel allows you to specify the crack front mesh template parameters – Set the template radius to 0. 06 – Select Next to proceed with growing the crack and remeshing – Once the remeshing is completed, another Static Crack Analysis can be performed 109

FRANC 3 D Tutorials – Automatic Crack Growth Steps • Assuming the crack insertion and static analysis was completed • Step 1: Re-Open FRANC 3 D restart file – From the FRANC 3 D menu, select File and Open. – Choose the *. fdb file and select OK. – FRANC 3 D will automatically read the FE model and solver results 110

FRANC 3 D Tutorials – Automatic Crack Growth Steps • Step 2: Select Crack Growth Analysis – From the FRANC 3 D menu, select Analysis and Crack Growth Analysis – First panel of the wizard allows you to choose the method for computing SIFs – Use all the default values. – Select Next 111

FRANC 3 D Tutorials – Automatic Crack Growth Steps • Step 3: Specify Growth Parameters – – Second panel appears Select Quasi-Static for simplicity All other values are left as defaults Select Next. 112

FRANC 3 D Tutorials – Automatic Crack Growth Steps • Step 4: Specify Growth Model Data – Third panel appears – Set the value of n to 2 for the power-law crack growth model – Select Next 113

FRANC 3 D Tutorials – Automatic Crack Growth Steps • Step 5: Specify Fitting and Template Parameters – Fourth panel appears – Set the value for the template radius to 0. 06. The extrapolation could be increased from 3 to 5%, but 3% should suffice for the first 5 steps – Select Next. 114

FRANC 3 D Tutorials – Automatic Crack Growth Steps • Step 6: Specify Extension or Cycle Data – Fifth panel appears – Grow the crack for 5 steps using a Constant Median Crack Growth Increment of 0. 1 – Select Next. 115

FRANC 3 D Tutorials – Automatic Crack Growth Steps • Step 7: Specify Analysis Code – Sixth panel appears – Use ANSYS and the Current crack growth step is 1 as if you are starting from the initial crack 116

FRANC 3 D Tutorials – Automatic Crack Growth Steps • Step 8: Specify Analysis Options – – Seventh panel appears Select your FE Solver Select global model FRANC 3 D transfers all the boundary conditions from the global model to the combined model, so leave the Transfer all retained bc’s checked. – Click Next 117

FRANC 3 D Tutorials – Automatic Crack Growth Steps • Step 9: Specify Local/Global Model Connection – Final panel allows you to choose how the local and global models will be connected – Click Finish to start the automatic crack 118

The Python Programming Interface • The FRANC 3 D program has a programming interface that is an extension to the Python programming language. • Python is an open source, object oriented, scripting language, which is popular in engineering and scientific computing community (e. g. , it is used to drive the ABAQUS GUI). • The Python interface allows one to automate repetitive and possibly error prone tasks. • It also provides a possible strategy for coupling FRANC 3 D with other computational applications. 119

A simple Py. F 3 D Program import Py. F 3 D # create a flaw object # file names for the models flaw = Py. F 3 D. Flaw("Ellipse", [a, b]) flaw. Translate([0. 499, 4. 179, -. 374]) flaw. Rotate(1, "Y", 90. 0) flaw. Rotate(2, "Z", -53. 61) # open an uncrack model, insert the flaw app. Open. Model(uncracked_fname ) app. Insert. Flaw(flaw) # generate a new file name like: # minidisk_crack_160_320. fdb fname = "%s_%d_%d. fdb" % (fname_base, int(a*1000), int(b*1000)) # save the file app. Save. Model(fname) uncracked_fname = "minidisk_submodel. cdb“ fname_base = "minidisk_crack" # lists of crack size parameters to a_sizes = [0. 0160, 0. 0320, 0. 0480, 0. 0640, 0. 0787, 0. 2362, 0. 3937] b_sizes = [0. 0160, 0. 0787, 0. 2362, 0. 3937] app = Py. F 3 DApp() # loop through the crack size matrix for a in a_sizes: for b in b_sizes: # skip cases with really #bad aspect ratios if b > 0. 2 and a < 0. 065: continue 120

Some FRANC 3 D Known Bugs If any of the original body patches fall completely inside the template (no intersections) the crack insertion will not be successful. 121

Some FRANC 3 D Known Bugs If the none of the crack mouth or template edges intersect any of the edges of any of the original boundary patches the crack will not be inserted successfully. 122

Some FRANC 3 D Known Bugs FRANC 3 D can have difficulties meshing in situations where the crack-front template (the singular crack-front element and the two surrounding rings of brick elements) intersects one of the corner of the models. 123

Some FRANC 3 D Known Bugs The code is currently able to detect that the template intersects a corner and in many cases does a reasonably good job making the external mesh compatible with both the template and the geometry of the body. However, reasonable pyramid elements cannot be added on the outside of the template. The “Simple Template Intersections Only” option may work around this issue. 124

What to do when something goes wrong If the program crashes before you see the “Flaw Insertion Status” window: • Use the “Advanced -> Flaw to File Wizard” option to create a. crk file that describes the flaw you are trying to insert. • Send the. crk file along with the mesh file (. inp or. cdb) to us. If the program crashes during flaw insertion or the program reports that it cannot insert the flaw: • Check to make sure that no part of the flaw or crack-front template is in the retained (cut surface) portion of the sub-model. • Look for a file called “debug. tst” in your working directory and send it to us. 125

Workshop Agenda • Introduction to FRANC 3 D • Demo/Hands-on: build an uncracked model • Overview of the crack insertion process • Demo/Hands-on: insert initial crack and run analysis • Stress Intensity Factor (SIF) computation - theory • Demo/Hands-on: SIF computation - practice • Crack growth - theory • Demo/Hands-on: Crack growth - practice • Demo/Hands-on: Student generated models 126