ABAQUS Tutorial Version 7.3

Transcription

1 ABAQUS Tutorial Version 7.3 Fracture Analysis Consultants, Inc Revised: Dec 2018

2 Table of Contents: 1.0 Introduction Tutorial 1: Crack Insertion and Growth in a Cube Step 1: Create the ABAQUS FE Model Step 2: Reading ABAQUS FE Model into FRANC3D Step 2.1: Importing Complete ABAQUS FE Model Step 2.2: Select the Retained Items in the FE Model Step 2.3: Displaying the FE Model Step 3: Importing and Subdividing the Model Step 4: Insert a Crack Step 4.1: Define a new Crack from FRANC3D Menu Step 4.2: Insert Cracks from Files Step 5: Static Crack Analysis Step 5.1: Select Static Crack Analysis Step 5.2: Select FE Solver Step 5.3: Select ABAQUS Analysis Options Step 6: Compute Stress Intensity Factors Step 7: Manual Crack Growth Step 7.1: Select Grow Crack Rule Step 7.2: Specify Fitting and Extrapolation Step 7.3: Specify Crack Front Template Step 8: Automatic Crack Growth Step 8.1: Open FRANC3D Restart File Step 8.2: Select Crack Growth Analysis Step 8.3: Specify Growth Rules Step 8.4: Specify Fitting and Template Parameters Step 8.5: Specify Growth Plan Step 8.6: Specify Analysis Code Step 9: SIF History and Fatigue Life

3 Step 9.1: Select SIFs Along a Path Step 9.2: Select SIFs For All Fronts Step 9.3: Select Fatigue Life Predictions Step 10: Resume Growth with Larger Submodel Step 1: Extract and Save Crack Geometry Step 2: Restart from Saved Crack Geometry Step 3: Combine SIF Histories Tutorial 2: Multiple Load Cases and Crack Face Tractions Step 1: Reading ABAQUS FE Model into FRANC3D Step 1.1: Importing ABAQUS FE Model Step 1.2: Select the Retained Items in the FE Model Step 1.3: Displaying the FE Model Step 2: Insert Crack From File Step 3: Apply Crack Surface Traction Step 4: Static Analysis Step 4.1: Run ABAQUS static crack analysis Step 4.2: Compute SIFs Step 4.3: Re-Run ABAQUS static crack analysis with crack face contact Step 4.4: Compute SIFs with crack face contact Step 5: Apply Surface Treatment Residual Stress Step 6: Apply Tractions from Mesh-Based Stress Step 6.1: Create Mesh-Based Stress Field Step 6.2: Apply Mesh-Based Stress as Crack Face Traction Step 6.3: ABAQUS Mesh-Based Stress Tutorial 3: Two Cubes Glued Together Step 1: Create the ABAQUS FE Model Step 2: Import ABAQUS FE Model into FRANC3D Step 2.1: Importing ABAQUS FE Model Step 2.2: Insert a Crack Step 2.3: Static Crack Analysis Step 2.4: Compute SIFs

4 Step 2.5: Plot Deformed Shape Step 2.6: Contact surface mesh not retained Step 2.7: Specify No Crack Material Region Tutorial 4: Disk with Rotation and Temperature Step 1: Create the ABAQUS Disk Model Step 2: Run ABAQUS Thermal Analysis Step 3: Run ABAQUS Structural Analysis Step 4: Import Disk into FRANC3D Step 5: Insert Initial Crack Step 6: Static Crack Analysis Step 6: Compute SIFs Step 7: Crack Growth Step 8: Automatic Crack Growth Step 9: Analysis Results Step 10: Fatigue Life Apply Crack Face Traction (CFT) Only Tutorial 5: Multiple Cracks in a Plate Step 1: Create the ABAQUS Plate Model Step 2: Import Plate Model into FRANC3D Step 3: Insert Multiple Cracks Step 4: Static Crack Analysis Step 5: Compute SIFs for Multiple Crack Fronts Step 6: Grow Multiple Cracks SIFs History for Multiple Cracks Crack Growth Transitions Grow a Crack around a Corner Grow Crack through a Back Surface Grow Multiple Cracks in Multiple Submodel Portions Step 1: Import Plate Model into FRANC3D Step 2: Insert Multiple Cracks Step 3: Crack Analysis

5 7.0 Tutorial 6: Computing Fatigue Life Cycles Step 1: Perform Crack Growth Step 2: Compute Fatigue Crack Growth Cycles Step 3: Crack Growth and Fatigue Options Variable Amplitude Loading Spectrum Loading for Manu Model Tutorial 7: Fretting Fatigue Step 1: Saving ABAQUS Data Step 2: Fretting Model Import Step 3: Fretting Crack Nucleation Step 3: Discrete Crack Nucleation Tutorial 8: Session Log Playback Tutorial 9: Python Interface Python PyF3D Module Python Extension for User-defined Crack Growth Step 1: Read ABAQUS Cube Crack Model Step 2: Read Python Extension Step 3: Grow Crack Python Extension File Tutorial 10: Fatigue with Time Dependent Growth SubModel and Crack Insertion Define Crack Growth Parameters Load Schedule Crack Growth Rate Model Effective dk and Integration Crack Growth Analysis Life Prediction Appendix A: ABAQUS local model between *Tie constraints Appendix B: ABAQUS model with *Tied meshes Appendix C: Crack growth around and through corners

6 1.0 Introduction This set of tutorials introduces the fracture simulation capabilities of FRANC3D Version 7.3 and ABAQUS Version 6.14 (earlier or later versions should work). The FRANC3D software is introduced by first analyzing a simple surface crack in a cube. Subsequent tutorials build on this first example and describe additional capabilities and features of the software. It is intended that the user perform the operations as they are presented, but you should feel free to experiment, and you should consult the other reference documentation whenever necessary. In the tutorials, FRANC3D menu and dialog button selections are indicated by bold text, such as the File menu. Window regions along with dialog options, fields and labels are underlined. Model names and file names are indicated by italic text. The FRANC3D main window is shown in Fig 1.1. When you start a tutorial, the first thing to do is set the working directory using the File and Set Work Directory menu option, Fig 1.1. You can set a different work directory for each tutorial. After importing a model, you can set the finite element model (FEM) units, Fig 1.2. The units are applied to plots and figures that FRANC3D displays, and are used during crack growth. You can also set your preferences; specifically, it is best to set the path to the ABAQUS executable. You can view the preferences using the Edit and Preferences menu option. The Preferences dialog is described in Section 5.4 of the FRANC3D Reference Manual. 6

7 Figure 1.1: FRANC3D main window Set Work Directory menu option. Figure 1.2: FRANC3D Set Units menu option. 2.0 Tutorial 1: Crack Insertion and Growth in a Cube The first tutorial simulates a surface crack in a cube under far-field tension. It is assumed that the user is familiar with a pre-processor for ABAQUS; we use ABAQUS CAE. Once the model is created, the FRANC3D steps necessary to read the mesh, insert a crack, rebuild the mesh, perform the ABAQUS analysis, and compute stress intensity factors are all described. 7

8 2.1 Step 1: Create the ABAQUS FE Model First, create a cube model using any pre-processor for ABAQUS. Here we simply outline the necessary steps to create the model with boundary conditions to ensure that we have a complete model that can be used with FRANC3D. 1. Create a 10x10x10 cube geometry; assume units of length are mm. 2. Subdivide the edges for meshing using 10 to 20 subdivisions. 3. Define the element type as quadratic elements; use brick or tetrahedral elements. 4. Define the material properties as for the elastic modulus and 0.3 for the Poisson s ratio; assume the units for E are MPa. 5. Mesh the volume. 6. Boundary conditions consist of displacement constraints on the bottom surface and uniform traction (a negative pressure) on the top surface of 10 MPa. The bottom surface is constrained in the y-direction, the bottom left edge is also constrained in the x- direction, and the point at the origin is also constrained in the z-direction. Note that you should use unique set and surface names when defining boundary conditions. 7. Save the model as an.inp file (Abaqus_Cube.inp). The resulting model should appear as in Fig 2.1. The symbols for the boundary conditions are displayed attached to the model; the brick mesh is displayed in the lower right corner. 8

9 Figure 2.1: ABAQUS cube with boundary conditions; meshed with brick elements. Note that ABAQUS CAE uses default set and surface names such as SET-1 at both the Part and the Instance levels, Fig 2.1b. FRANC3D might not differentiate between the Part SET-1 and Instance SET-1; the Instance SET-1 can be both a node and element set. If boundary conditions are applied in CAE using the Instance SET-1 (right side image), FRANC3D might apply the boundary conditions to both Part and Instance SET-1 nodes. The solution is to name the sets and surfaces in CAE with unique names, especially when defining boundary conditions. 9

10 Figure 2.1b: ABAQUS CAE set-1 at both Part and Instance levels. 2.2 Step 2: Reading ABAQUS FE Model into FRANC3D Start by importing an existing volume element mesh into FRANC3D. We use the Abaqus_Cube.inp file from ABAQUS CAE, which was written in the previous step. You can choose to do either Step 2 or Step 3 (Section 2.3); we describe both, but we use Step 3 for subsequent steps of this tutorial. Step 2.1: Importing Complete ABAQUS FE Model Start with the FRANC3D graphical user interface and select File and Import, Fig 2.2. In the dialog shown in Fig 2.3, choose Complete Model. Switch the Mesh File Type radio button in the Select Import Mesh File window, Fig 2.4, to ABAQUS and select the file name for the model, called Abaqus_Cube.inp, Fig, 2.4. Select Next. The mesh file type can be set in the Preferences so that you do not have to change the mesh file type radio button if you always use ABAQUS. 10

11 Figure 2.2: FRANC3D graphical user interface Figure 2.3 Import type 11

12 Figure 2.4: Select Input Mesh File dialog box Step 2.2: Select the Retained Items in the FE Model The next panel, Fig 2.5, allows you to choose the mesh surface facets that are retained from the ABAQUS.inp file. Surfaces with boundary conditions appear as blue, Fig 2.6, and turn red when selected, Fig 2.7. We can retain the surfaces with boundary conditions (top and bottom of the cube) by choosing Select All. The boundary conditions will be transferred automatically to the new mesh when a crack is inserted. Select Finish to proceed. 12

13 Figure 2.5: Select Retained BC Surfaces wizard panel. Figure 2.6: ABAQUS Model retain BC Surfaces wizard panel. 13

14 Figure 2.7: ABAQUS Model retain BC Surfaces wizard panel. Surface Mesh NOT Retained The surface mesh facets do not have to be retained, and if a crack will be inserted into a surface that has boundary conditions, then the surface mesh must not be retained. In such a case, the boundary condition data is mapped to the remeshed surface. In practice, transfer of boundary condition data is simpler and more precise if the surface mesh can be retained, but sometimes this is not possible; FRANC3D will automatically map the boundary condition data to the new mesh regardless. Step 2.3: Displaying the FE Model The model is displayed in the FRANC3D modeling window, Fig 2.8. You can turn on the surface mesh, or manipulate the model view by rotating, etc. Fig 2.8 shows the retained mesh on 14

15 the top surface (the retained bottom surface is not shown) where the boundary conditions are applied. Figure 2.8: ABAQUS model imported into FRANC3D with retained facets on top of the cube. If you have not set a working directory (using the File - Set Work Directory menu option), FRANC3D might present the dialog shown in Figure 2.9 prior to displaying the model. Select Yes to set the directory to be the folder where the ABAQUS.inp file resides. Quite a large number of files are created during a crack growth simulation, and it is best to keep them all together in a single folder. Figure 2.9: Set Working Directory dialog. 15

16 2.3 Step 3: Importing and Subdividing the Model If you chose to do Step 2 above, either skip this step, or close the model using the File - Close menu option before starting this step. The ABAQUS model can be split into smaller parts before inserting the crack. Go to File and Import, and choose the Import and divide into global and local models radio button, Fig 2.10, and choose the Abaqus_Cube.inp model, Fig 2.11, as before. Remember to set the Mesh File Type radio button to ABAQUS. Fig 2.10 Import options This time, instead of the retain BC surfaces window shown in Fig 2.5, the Define a Local Submodel window, Fig 2.12 appears. Figures 2.13 and 2.14 show two of the selection tools. Selections are made using the options on the left; elements to be retained appear red, and the selection is confirmed with the Crop button. For this tutorial, the rectangular Rubberband Box is used to create a smaller portion of the cube, Fig 2.15, which has an exposed face for crack insertion. 16

17 Figure 2.11: Select Input Mesh File selection. Figure 2.12: Define a Local Submodel Window 17

18 Figure 2.13: Plane Cutting tool red elements will be retained by Crop. Figure 2.14: Element-by-Element cropping by selecting elements to remove. We are inserting a surface crack that is normal to the y-axis (loading direction) and located on the +z surface, and the selection in Fig 2.15 is designed for this. Use the Rectangular option of the Rubberband Box to select and Crop a small portion of the model. 18

19 Figure 2.15: Rectangular Rubberband Box tool used to select a submodel. Once the elements have been selected and cropped, select Next. The Save the Files dialog appears, Fig Choose the names of the local and global models and their location; use the default file names and the working directory set earlier. Select Next. Figure 2.16: Local/Global model save window 19

20 If the local cropped model has a surface with boundary conditions, then the Select Retained BC Surfaces window from Fig 2.5 appears. Otherwise, the local model appears in the FRANC3D main window, with retained mesh surfaces wherever the local and global models connect (the cut surfaces). In this case, the cropped selection in Fig 2.15 avoids all surfaces with boundary conditions. However, if there are ABAQUS node sets or surfaces in the local model, then the Select Retained BC Surfaces window will be displayed, Fig In this case, just select Finish and the local model is displayed, Fig Figure 2.17: Select Retained BC Surfaces wizard panel showing named node sets. 20

21 Figure 2.18: Local model with retained mesh facets on cut-surface 2.4 Step 4: Insert a Crack We now insert a half-penny surface crack into the model. The local submodel from Section 2.3 is used, as opposed to the full model. In Step 4.1, we describe how to define a new crack, and in Step 4.2, we describe how to insert a flaw from a file. Note that you should not try to re-insert a crack into a cracked model. Step 4.2 is described here and will be used in subsequent tutorials. Step 4.1: Define a new Crack from FRANC3D Menu From the FRANC3D menu, select Cracks and New Flaw Wizard as seen in Fig The first panel of the wizard should appear as in Fig The flaw being added is a crack with zero volume. We select the Save to file and add flaw radio button to save the file for subsequent tutorials. Select Next. The second panel of the wizard, Fig 2.21, lets you choose the crack shape; the default is the ellipse, which is what we want. Select Next. 21

22 Figure 2.19: New Flaw Wizard menu item selected. Figure 2.20: New Flaw Wizard first panel Crack (zero volume flaw) selected. 22

23 Figure 2.21: New Flaw Wizard second panel choose ellipse shape. The crack is a circle with radius=1, centered on the cube s front (+z) face, and parallel to the xzplane (normal to y). The third wizard panel lets you set the dimensions for the ellipse, Fig 2.22; set a=1 and b=1. Select Next. Figure 2.22: New Flaw Wizard third panel set ellipse dimensions. 23

24 The fourth panel lets you set the crack location and orientation, Fig We place the crack at the center of the front face at coordinates (5,5,10) and rotate the crack 90 degrees about the Global x-axis. Select Next. Figure 2.23: New Flaw Wizard fourth panel set crack location and orientation. The final panel allows you to set the crack front mesh template parameters, Fig Use the defaults; the default template radius is based on the crack dimensions and might need to be adjusted depending on the model and crack. Select Finish. At this point, you will be asked to specify the file name to save the crack information, Fig 2.25; we call it Cube_Crack.crk. Select Accept. 24

25 Figure 2.24: New Flaw Wizard final panel set template mesh parameters. Figure 2.25: New Flaw Wizard final panel save file as. The crack is inserted into the model, and then remeshing occurs. A Flaw Insertion Status window is displayed during this process, Fig There are four stages: geometric intersection of the crack with the model, surface meshing, volume meshing, and smoothing of the volume 25

26 mesh to produce better quality elements. The resulting mesh should appear as in Fig 2.27; the surface mesh is shown. Figure 2.26: Flaw Insertion Status window. Figure 2.27: Remeshed cracked local model with surface mesh turned on. 26

27 Step 4.2: Insert Cracks from Files Note that you should not do this step if you have already inserted the crack into the model in Step 4.1. If you want to try this step, you must Close the model from Step 4.1 and re-import the original uncracked (local) model. From the FRANC3D menu, select Cracks and Flaw From Files, Fig The first panel of the wizard should appear as in Fig Choose the Cube_Crack.crk file and hit Accept. The flaw being added is a circle with radius=1, centered on the cube s front face, and parallel to the xzplane. This crack was created using the New Flaw Wizard and the save to file option in Step 4.1. Figure 2.28: Flaw From Files option in Crack menu. 27

28 Figure 2.29: Flaw from file dialog to select.crk file. The next panel of the wizard, Fig 2.30, allows you to adjust the location of the flaw. The orientation cannot be changed. The final panel, Fig 2.31, allows you to set the template mesh. Select Finish to complete the insertion and remeshing. Figure 2.30: Flaw wizard panel to set location. 28

29 Figure 2.31: Flaw geometry shown in the model with crack template mesh 2.5 Step 5: Static Crack Analysis Once the crack is inserted and remeshed, we must perform the stress analysis using ABAQUS, which will provide the displacement results that are needed to compute stress intensity factors. Typically, you should run a static crack analysis of the initial crack prior to running automated crack growth; this allows you to verify that the simulation is valid. You can also do a level of template mesh refinement to verify that the computed SIFs are accurate. Step 5.1: Select Static Crack Analysis From the FRANC3D menu, select Analysis and Static Crack Analysis, Fig The first panel of the wizard, Fig 2.33, requests that you enter the file name for the FRANC3D data. We call it Abaqus_Cube_Subdivide.fdb here; select Next once you enter the File Name. Note that you cannot use the initial uncracked Abaqus_Cube.inp or Abaqus_Cube_LOCAL.inp file names, because a new.inp file will be created and saved during the analysis, and the original uncracked.inp files are reused for each step of crack growth. 29

30 Figure 2.32: Static Crack Analysis menu Figure 2.33: Static Analysis wizard first panel File Name 30

31 Step 5.2: Select FE Solver The next panel of the wizard, Fig 2.34, allows you to specify the solver; choose ABAQUS and select Next (button not shown in Fig 2.34). Figure 2.34: Static Analysis wizard second panel choose solver Step 5.3: Select ABAQUS Analysis Options The next panel of the wizard, Fig 2.35, allows you to specify the ABAQUS output and analysis options. The model is a sub-model and needs to be connected with the global model, so the Connect to global model box automatically should be checked if the FRANC3D submodeler tool was used. The next panel, Fig 2.36, allows you to set the local + global model connection. Note that if the model being analyzed is a full/complete model, the panel in Fig 2.35 is the final panel as there is no global model, and the Next button will be a Finish button. 31

32 Figure 2.35: Static Analysis wizard third panel ABAQUS output options The panel in Fig 2.36 shows the options for joining the local and global models. AUTO_CUT_SURF and GLOBAL_CONNECT_SURF are the node sets created by the FRANC3D submodeling tool and should be selected automatically. Click Finish to start ABAQUS running (in batch/background mode). FRANC3D write files and then attempts to execute ABAQUS based on the ABAQUS Executable information, Fig You can monitor the FRANC3D CMD window and the ABAQUS.dat and.msg file for errors or messages. Choosing Write files but DO NOT run analysis in Fig 2.36 will create all the files without running ABQUS, if the analysis needs to be run later or on a different computer. If you need to run ABQUS on a different computer, you must bring the results file (.dtp) back to the working folder, and then you can use the File and Read Results menu option to import the results into 32

33 FRANC3D. The.dtp file is created by running the writedtpfile.py script, which extracts the.dtp data from the.odb file. In a CMD or Terminal window, the command is: > abaqus python writedtpfile.py Figure 2.36: Local/Global model connection 2.6 Step 6: Compute Stress Intensity Factors From the FRANC3D menu, select Cracks and Compute SIFs, Fig The Stress Intensity Factor wizard is displayed, Fig You should use the M-integral, but you can check that the Displacement Correlation results are similar. Select Finish and the SIFs Plot window is displayed, Fig You can view the three stress intensity factor (SIF) modes using the upper tabs: KI, KII and KIII; mode II and III values should be negligible compared to mode I. 33

34 Figure 2.37: Compute SIF s selected from the Cracks menu Figure 2.38: Compute SIF options 34

35 Figure 2.39: Stress Intensity Factor plot 2.7 Step 7: Manual Crack Growth We will manually propagate the crack at this stage. You should examine the predicted crack growth to determine suitable parameters for fitting and extrapolation before proceeding with automated crack growth, which is described in Section 2.8. Step 7.1: Select Grow Crack Rule From the FRANC3D menu, select Cracks and Grow Crack, Fig In the first panel, Fig 2.41, switch to Quasi-Static crack growth and select Next. Use the Max Tensile Stress theory to determine the kink angle, Fig 2.42; in this model, crack growth is essentially planar. Select Next. Use a Power Law relationship to determine relative growth among points along the crack front, Fig 2.43; we will use the default power n=2. There is only one load step in the model. Select Finish to proceed. You will be asked if you want to save the growth parameters to a file, Fig 2.44, you can select No. Consult the reference document for descriptions of crack extension models. 35

36 Figure 2.40: Grow Crack menu option. Figure 2.41: Crack Growth wizard first panel. 36

37 Figure 2.42: Crack Growth wizard second panel using quasi-static growth. Figure 2.43: Crack Growth wizard third panel using quasi-static growth. 37

38 Figure 2.44: Save growth parameters dialog. Step 7.2: Specify Fitting and Extrapolation The next panel, Fig 2.45 allows you to specify the crack front point fitting parameters. You can double click on the (crack) view to see the crack surface; this should be the default view. The median extension is set to 0.15; this value generally is set automatically based on the initial template radius so your value might be different. We change it to 0.1 and turn on Markers in Fig The green boxes are the computed points and the blue line is the curve-fit, Fig A Fixed Order Polynomial fit with order set to 3 and extrapolation set to 3% at both ends of the crack front is the default; the fitting parameters might need to be adjusted as the crack grows. A 4 th order polynomial provides a slightly better fit in this case; the guidelines for curve-fitting are to use the simplest fit that is reasonable. We stick with the default 3 rd order polynomial; select Next to proceed. Note that the fitted (blue) curve through the predicted new front points (green) must be extrapolated so that both ends fall outside of the model, but it should not be extrapolated too much. The median extension must be enough to provide finite space between the current and new fronts along the entire front to define new crack geometry. 38

39 Figure 2.45: Crack growth wizard panel for crack front fitting options Figure 2.46: Median crack extension of

40 Step 7.3: Specify Crack Front Template The final panel, Fig 2.47, allows you to specify the crack front mesh template parameters. The crack front mesh template extends beyond the model surface, which corresponds with the frontfit extrapolation. The template radius can be set as an absolute value or as a % of the median extension. The default 85% shown in Fig 2.47; we switch to an absolute value of 0.1, Fig 2.48, which is the same as the initial crack template radius. Select Next on this panel when ready to proceed with the actual crack insertion and remeshing. Note that the crack geometry for the extended crack is inserted into the original uncracked model, so do not overwrite or remove the original model files. Figure 2.47: Crack growth wizard panel for mesh template options 40

41 Figure 2.48: Template radius set to 0.1 The resulting model can be analyzed as was done for the initial crack (see Step 5 above). Note that you will want to give this model a different name, such as Abaqus_Cube_ step_001, so that you don t overwrite the initial crack files. Automated crack growth analysis is described next. 2.8 Step 8: Automatic Crack Growth This section describes the steps for automatic crack growth starting from the initial crack model. We start with an existing FRANC3D model, using the model created in Sections 2.4 and 2.5. Step 8.1: Open FRANC3D Restart File Start with the FRANC3D graphical user interface (see Fig 2.2) and select File and Open. Select the file name specified in Section 2.5, called Abaqus_Cube_Subdivide.fdb. Select Accept. The model will be read into FRANC3D (along with the results files that were created when running the static analysis). We will ignore the fact that we already propagated the initial crack in the previous step (but we will use the settings), and proceed with setting up the automatic crack growth analysis. 41

42 Step 8.2: Select Crack Growth Analysis From the FRANC3D menu, select Analysis and Crack Growth Analysis, Fig The first panel of the wizard, Fig 2.50, allows you to choose the method for computing SIFs. We use the default selection of M-integral. Select Next. Figure 2.49: Crack Growth Analysis menu Figure 2.50: Crack Growth Analysis wizard first panel. 42

43 Step 8.3: Specify Growth Rules The second panel, Fig 2.51, lets us set the crack growth type; we use quasi-static growth. Select Next to display the third panel, Fig 2.52; use the default MTS theory to compute the kink angle. Select Next to display the fourth panel, Fig 2.53; use the default settings for the quasi-static growth. Select Finish. You will be asked if you want to save the growth parameters to a file; you can select No. Figure 2.51: Crack Growth Analysis wizard second panel. Figure 2.52: Crack Growth Analysis wizard third panel. 43

44 Figure 2.53: Crack Growth Analysis wizard fourth panel. Step 8.4: Specify Fitting and Template Parameters The fifth panel, Fig 2.54, lets us set the crack front fitting and mesh template parameters. Use the default 3 rd order polynomial and 3% extrapolation. Set the template radius to an absolute value of 0.1. Select Next. 44

45 Figure 2.54: Crack Growth Analysis wizard fifth panel. Step 8.5: Specify Growth Plan The sixth panel, Fig 2.55, allows us to define the amount of extension for each step of crack growth. Set the number of steps to 5 and the constant median extension to 0.2. Select Next. 45

46 Figure 2.55: Crack Growth Analysis wizard sixth panel. Step 8.6: Specify Analysis Code The seventh panel of the wizard, Fig 2.56, lets us choose the analysis code; we use ABAQUS. The current crack growth step defaults to 0 representing the initial crack. If we had manually propagated the crack first, we would set this to 1. FRANC3D will extend the initial crack based on the growth rule defined in the previous panels, and then name the resulting set of files as Abaqus_Cube_Subdivide_STEP_001.*. Subsequent file names have the step number incremented as the automatic analysis proceeds. Select Next (button not shown). Figure 2.56: Crack Growth Analysis wizard seventh panel. 46

47 The eighth panel, Fig 2.57, shows the analysis settings. You should have already set the ABAQUS executable path in the FRANC3D Preferences. The Global model settings should be set automatically. The local + global connection is displayed in the next panel. Select Next. Figure 2.57: Crack Growth Analysis wizard eighth panel. The ninth panel, Fig 2.58, displays the local + global connection. The default settings use nodemerging of the cut-surfaces between the local and global portions. Select Finish to start the automated crack growth process. 47

48 Figure 2.58: Crack Growth Analysis wizard ninth panel FRANC3D saves the.fdb,.inp and other files for the first crack step model using the name Abaqus_Cube_Subdivide_STEP_001, and then ABAQUS is started in the background. If the analysis stop at any stage, it can be restarted from the last crack step. All of the required restart _STEP_# files are retained. The model for any step can be read into FRANC3D to view the stress intensity factors or to restart the analysis with a modified crack growth increment (for example). 2.9 Step 9: SIF History and Fatigue Life Once the automatic crack growth analysis from Step 8 has finished, the stress intensity factor history can be displayed. If you still have FRANC3D open and the crack growth from Step 8 is done, you can proceed with Step 9.1. Otherwise, you can restart FRANC3D and read in the.fdb file for the last step, using the File and Open menu option. 48

49 Step 9.1: Select SIFs Along a Path From the FRANC3D menu, select Cracks and SIFs Along a Path, Fig If the SIFs have not been computed yet, the Compute SIFs dialog (see Fig 2.50) will be displayed; leave the defaults and select Finish. Figure 2.59: SIFs Along a Path menu option The Stress Intensity Factors (along a path) dialog should appear, Fig The crack fronts are displayed on the left along with a path through the fronts; the SIF history along the path is shown in the graph on the right. You can use the tabs above the graph to plot the Mode II and III SIF as well as the elastic J-integral and T-stress values along the path. You can define a new path, Fig You can export the data also; for example, you might need to export the Mode I SIF history (K vs a) to compute fatigue cycles using a different program. 49

50 Figure 2.60: SIFs Along a Path dialog KI plot Figure 2.61: SIFs Along a Path dialog Define Path Step 9.2: Select SIFs For All Fronts From the FRANC3D menu, select Cracks and SIFs For All Fronts. If the SIFs have not been computed yet, the Compute SIFs dialog will be displayed; leave the defaults and select Finish. 50

51 The Stress Intensity Factors (for all fronts) dialog should appear, Fig The crack fronts are displayed on the left and the SIFs for all crack fronts are displayed on the right. You can use the tabs above the plot to display Mode II and III SIFs as well as the elastic J-integral and T-stress values. If there are multiple crack fronts or multiple load steps, these can be selected using the drop-down lists; this will be seen in subsequent tutorials. Figure 2.62: SIFs for all Fronts dialog KI plot Step 9.3: Select Fatigue Life Predictions Fatigue life or cycles can be computed next. From the FRANC3D menu, select Fatigue and Fatigue Life Predictions, Fig If the SIFs have not been computed yet, the Compute SIFs dialog will be displayed; leave the defaults and select Finish. 51

52 Figure 2.63: Fatigue Life Predictions menu option The Fatigue Life dialog should appear as in Fig The crack fronts are displayed on the left and the window on the right side should be blank (assuming that lifing parameters have not been defined previously). You must Set (or Read) Parameters. Selecting Set Parameters displays the dialog shown in Fig Set the FEM model units to MPa mm; select the Change button to display the dialog in Fig 2.66, and set the units to MPa and mm; select Accept. The FEM units can also be set in the main FRANC3D window using the Edit menu. 52

53 Figure 2.64: Fatigue Life dialog Figure 2.65: Fatigue Life parameters 53

54 Figure 2.66: FEM units dialog The crack growth load schedule is defined next. Select the New Schedule button (see Fig 2.65) to display the dialog in Fig Select the Schedule and then select the Add button; see right side image of Fig This will display the dialog shown in Fig 2.68; we use a simple cyclic load schedule where the applied load produces Kmax and Kmin is zero. Select Accept to return to the Load Schedule, Fig The stress ratio is set to 0.0. There is only one load case, which represents the Kmax condition. The Repeat count is set to FOREVER. Select Accept to finish the load schedule. 54

55 Figure 2.67: New Load Schedule dialog Figure 2.68: Event type dialog 55

56 Figure 2.69: Simple cyclic load schedule repeated forever The crack growth rate model is defined next. Select the New Model button (see Fig 2.65) to display the dialog in Fig Choose the cyclic loading growth rate model, and select Next to display the dialog in Fig Figure 2.70: Growth model type dialog 56

57 Figure 2.71: Cyclic loading growth model dialog We use a simple Paris growth model, which is the default; select Next to display the dialog in Fig The growth rate model will be temperature independent. Select Next to display the Paris growth model dialog, Fig Figure 2.72: Temperature dependent or independent growth rate model dialog 57

58 Figure 2.73: Paris growth rate model dialog First, set the units for the Paris growth model. Select the Change button to display the Units dialog, Fig Set the units the same as the FEM units that we set earlier, which were MPa and mm. Select Accept. Figure 2.74: Paris growth rate model units 58

59 In the Paris growth model dialog, click on the fields for C, n, DKth and Kc and enter the appropriate values, Fig Select Next to return the main dialog (see Fig 2.65). The other options are left at their default values; select Accept to return to the Fatigue Life dialog, Fig Figure 2.75: Paris growth rate model values Figure 2.76: Fatigue life showing Cycles vs Crack Growth Step 59

60 Note that the Paris exponent n is set to 3 whereas we used n=2 for the quasi-static growth. In practice, you can use the fatigue model and material data to compute growth so that it is consistent with the fatigue life computations done here. However, it is not strictly necessary, and it might work better to use a lower exponent to predict increments of growth. If we choose to plot cycles based on a path, we must select the Path radio button and the Define button (see Fig 2.76) to create a path, Fig The default path is through the crack front midpoints. Once a path is defined, the cycles versus crack path length is displayed, Fig Figure 2.77: Define crack path dialog Figure 2.78: Fatigue cycles versus crack length 60

61 2.10 Step 10: Resume Growth with Larger Submodel We used a local submodel for this crack growth simulation. If the crack growth exceeds the boundary of the local submodel, a larger submodel can be selected and crack growth can be continued without having to restart the simulation from the beginning. In this step, we describe the process of extracting the current crack geometry and inserting this into a larger portion of the model to resume crack growth. Step 10.1: Extract and Save Crack Geometry The crack geometry information for each step of crack growth is saved in the FRANC3D restart (.fdb) file. The data appears in this block: FLAWSURF ( VERSION: 5 NUM_SURFS: 763 SURF: ) This data can be copied from the.fdb file and saved to a.crk file, using any text editor. We open the Abaqus_Cube_subdivide_STEP_005.fdb file, copy the FLAWSURF data, and save it to a.crk file, called Abaqus_Cube _step_5.crk. At step 5, the crack is approaching the boundary of the submodel region, Fig 2.79, so we could not have grown the crack much further. 61

62 Figure 2.79: Crack step 5 in local submodel. Step 10.2: Restart from Saved Crack Geometry Start FRANC3D, and from the menu select File and Import. We could extract a larger submodel region from the cube, but for this tutorial, we will just import the full cube model and run subsequent crack growth simulations using the full model. Select Import a complete model from the dialog, Fig 2.80, set the Mesh File Type to ABAQUS, and select the Abaqus_Cube.inp file, Fig Select Accept to continue. 62

63 Figure 2.80: FRANC3D model import dialog. Figure 2.81: FRANC3D mesh import file selector. Use the Select All button in the next dialog, Fig 2.82, to retain all the mesh facets where boundary conditions are applied. Select FINISH when ready; the model will be imported and displayed in the FRANC3D main window. 63

64 Figure 2.82: Use Select All button to retain all highlighted mesh facets. From the FRANC3D menu, select Cracks and Flaw From Files. Select the Abaqus_Cube_step_5.crk file, which was extracted from the.fdb file. The.crk file is read and then displayed in the Orient User Flaw dialog, Fig Note that the crack geometry includes the original circular crack and all the subsequent steps of growth. Also note that part of the crack geometry falls outside the model so that intersections can be computed correctly. In general, a crack that is read from a file can be translated in Cartesian space, but for continuing crack growth, we do not want to do this. Select Next to set the mesh template parameters, Fig 2.84; we just use the defaults. Select Finish when ready; the crack will be inserted and the model remeshed. From the FRANC3D menu, select Static Crack Analysis and set the analysis parameters; use the same settings as in Step 5. The only thing that is changed is the file name so that we do not overwrite the original submodel step files; call it Abaqus_cube_full_STEP_

65 Figure 2.83: Step 5 crack geometry displayed in cube model. Figure 2.84: Step 5 crack mesh template. The analysis should produce SIFs that are identical (or nearly so) to the SIFs computed for the step_005 using the local submodel region. Fig 2.85 shows the Mode I SIFs for the two cases. There are small differences as the mesh around the crack front is different. At this stage, the 65

66 crack can be propagated further; do another 5 steps of crack growth. After propagating the crack an additional 5 steps, we can combine the SIF history for the two analyses. We do this using the Advanced menu option Create Growth History. Figure 2.85: Step 5 Mode I SIFs for the original submodel analysis (top) compared with the new results using the full model (bottom). Step 10.3: Combine SIF Histories Start FRANC3D, select the File and Open menu option, and select the Abaqus_Cube_sub_STEP_005.fdb file. From the Advanced menu, select Create Growth 66

67 History, Fig The dialog shown in Fig 2.87 is displayed. Note that the initial crack is labeled as CrackStep_1 and then there are 5 steps of growth after that. You can use the Plot menu command to display the crack fronts, Fig Figure 2.86: FRANC3D Advanced menu. Figure 2.87: Create Growth History dialog submodel data. 67

68 Figure 2.88: Create Growth History dialog. Using the File menu in the Create Growth History dialog, select Save History, Fig 2.89, and save the SIF history to a.fcg file, called Abaqus_Cube_sub_steps.fcg here. Close the dialog using the Cancel button, and then close the model in FRANC3D using the main File menu Close option. Now open the Abaqus_Cube_full_STEP_010.fdb file (our last step of crack growth) using the File menu Open option. As with the submodel, save the history using the Create Growth History dialog. The SIF history for the full model is shown in Fig Note that CrackStep_1 in the full model gives the same SIFs as CrackStep_6 in the submodel; however, CrackStep_1 in the full model includes extension data. Figure 2.89: Create Growth History dialog File menu. 68

69 Figure 2.90: Create Growth History dialog full model data. Save the full model SIF history to a.fcg file, called Abaqus_Cube_full_steps.fcg here. Close the Create Growth History dialog and close the model. This leaves the FRANC3D main model window empty. Select the Advanced and Create Growth History menu option to display the dialog. It does not have any CrackGrowthData. Use the File menu in the Create Growth History dialog and select Read History, Fig Select the Abaqus_Cube_sub_steps.fcg file. Then using the same menu, select Append History and select the Abaqus_Cube_full_steps.fcg file. Note that there will be 12 steps of crack data at this stage, Fig We need to delete CrackStep_6 from the Submodel data as it does not include extension data. We highlight CrackStep_6, Fig 2.93, and then right-click the mouse to display the submenu, Fig Select Delete Crack Step and it will be removed, leaving 12 crack steps. You can plot the combined fronts, Fig

70 Figure 2.91: Create Growth History dialog File menu. Figure 2.92: Create Growth History dialog combined SIF history data. Figure 2.93: Right-mouse button click on the CrackStep_6 to delete. 70

71 Use the File menu in this dialog to save the combined SIF history to a.fcg file, called Abaqus_Cube_combined_steps.fcg. The dialog can be closed by selecting the Cancel button at the bottom; selecting the Save button prompts you save the history data to file. Figure 2.94: Create Growth History dialog combined crack fronts. The combined SIF history data can be imported into the Fatigue Life module using the Read SIF Data button, Fig Once you have Set Parameters, you can plot cycles; see Step 9.3. Figure 2.95: Fatigue Life dialog. 71

72 3.0 Tutorial 2: Multiple Load Cases and Crack Face Tractions In the first part of Tutorial 2, we describe the process of importing a model with multiple load cases. Once a crack is inserted, an additional load case is applied as a crack face pressure. We describe how to apply a simple constant pressure in the crack in Section 3.5. We apply a surface treatment residual stress in Section 3.10, and we apply mesh-based surface crack traction in Section We use the same Abaqus_Cube.inp file from Tutorial 1, but with two additional load cases. The first of the extra load cases is a positive (far-field) surface pressure equal in magnitude to the traction in the first load case; this will compress the cube. The second extra load case is a negative (far-field) surface traction with double the magnitude of the first load case. Note that the first extra load case will cause the cube to compress, and we describe how to apply crack face contact conditions to prevent negative Mode I SIFs in Section 3.8. For ABAQUS, the load cases are defined in the.inp file and are differentiated by *STEP commands. Note that FRANC3D does not support *LOAD CASE data; you should use multiple *STEPs instead. 3.1 Step 1: Reading ABAQUS FE Model into FRANC3D Step 1.1: Importing ABAQUS FE Model Start with the FRANC3D graphical user interface, Fig 3.1, and select File and Import. In the window shown in Fig 3.2, choose Complete Model. Switch the Mesh File Type radio button in the Select Import Mesh File window, Fig 3.3, to ABAQUS. Select the file name for the model, called Abaqus_Cube.inp, Fig, 3.3. Select Next. 72

73 Figure 3.1: FRANC3D graphical user interface Figure 3.2 Import type Note that we could subdivide the cube as we did in Section 2.3, but for simplicity we just import the full model. For relatively simple models, the time to remesh the whole volume is short. However, for most models, we want to subdivide to avoid having to remesh the full model at each step of crack growth. 73

74 Figure 3.3: Select Input Mesh File dialog box Step 1.2: Select the Retained Items in the FE Model The next panel, Fig 3.4, allows you to choose the mesh surface facets that are retained from the ABAQUS files. Surfaces with boundary conditions appear in blue as shown in Fig 3.5, and turn red when selected, Fig 3.6. We retain the surfaces with boundary conditions (top and bottom of the cube) by choosing Select All. The boundary conditions are transferred automatically to the new mesh when the crack is inserted. Select Finish. Note that the boundary conditions for all load steps are applied to the same surfaces in this model. 74

75 Figure 3.4: Select Retained BC Surfaces wizard panel. Figure 3.5: ABAQUS Model retain BC Surfaces wizard panel. 75

76 Figure 3.6: ABAQUS Model retain BC Surfaces wizard panel. Step 1.3: Displaying the FE Model The model is displayed in the main window. You can turn on the surface mesh and manipulate the view. The model should appear as in Fig 3.7, which shows that the mesh is retained on the top and bottom (not shown) surfaces where the boundary conditions are applied. 76

77 Figure 3.7: ABAQUS model imported into FRANC3D, showing retained facets on the top. 3.2 Step 2: Insert Crack From File From the FRANC3D menu, select Cracks and Flaw From Files, Fig 3.8. The first panel of the wizard, Fig 3.9, lets us choose Cube_Crack.crk, which is the file we saved in the first tutorial. Select Accept. The flaw being added is a circle with radius=1, centered on the front face and parallel to the xzplane. This crack was created using the New Flaw Wizard with the save to file option in Section 2.4. The next panel of the wizard, Fig 3.10, allows you to adjust the location of the crack; a flaw from a file cannot be rotated. Just leave the crack at its location and select Next. The final panel, Fig 3.11, allows you to set the template mesh. Set the template radius to 0.05, leave all the other defaults, and select Finish. Fig 3.12 shows the resulting remeshed cracked model. The template radius is reduced here to improve the contact results. 77

78 Figure 3.8: Flaw From Files option in Crack menu. Figure 3.9: Flaw from file dialog to select.crk file. 78

79 Figure 3.10: Flaw wizard panel to set location. Figure 3.11: Flaw geometry shown in the model with crack template mesh 79

80 Figure 3.12: Remeshed cracked model 3.3 Step 3: Apply Crack Surface Traction From the FRANC3D main menu, select Loads and Crack Face Pressure/Traction, Fig Click on Add in the dialog box shown in the top left panel of Fig Choose Constant Crack Face Pressure, as show in the top right panel of Fig 3.14; it is the default, and then select Next. Set the Pressure value to 1 in the next dialog, Fig 3.14 bottom left, and select Next. There are no temperatures in this model, so the Set Temperature dialog can be ignored; select Finish. Note that a positive value of pressure will tend to open the crack. The original dialog now contains one entry, Fig 3.14 bottom right; click Accept. 80

81 Figure 3.13: Crack Face Pressure/Traction menu Figure 3.14 Crack face traction dialogs. 81

82 3.4 Step 4: Static Analysis Step 4.1: Run ABAQUS static crack analysis From the FRANC3D menu, select Analysis and Static Crack Analysis. The first panel of the wizard, Fig 3.15, requests the file name for the FRANC3D database; we call it Abaqus_Cube_LoadCases.fdb. Select Next once you enter a File Name. The next panel of the wizard, Fig 3.16, allows you to specify the solver; choose ABAQUS and select Next (button not shown). Figure 3.15: Static Analysis wizard first panel File Name. 82

83 Figure 3.16: Static Analysis wizard second panel solver. The next panel of the wizard, Fig 3.17, allows you to specify the ABAQUS analysis and output options. The Apply crack face tractions box is checked automatically. There is no global model; click Finish when ready to proceed with the ABAQUS analysis. When ABAQUS is finished running, proceed to Step 4.2. You can monitor the FRANC3D CMD window as well as the ABAQUS.dat and.msg files. Figure 3.17: Static Analysis wizard third panel ABAQUS output options. 83

84 Step 4.2: Compute SIFs We now compute the stress intensity factors for this crack. If you are able to run ABAQUS directly from FRANC3D, then the model already exists and the results (.dtp) file is read automatically. From the FRANC3D menu, select Cracks and Compute SIFs. When the Compute SIFs dialog is displayed, Fig 3.18, you can select the Advanced button and make sure that the Include Applied Crack Traction box is checked (right side image in Fig 3.18). Select Finish and the SIFs Plot dialog is displayed, Fig The initial plot shows the sum of KI for all load cases. You can view the three stress intensity factor (SIF) modes for the four separate load cases using the Analysis Load Step dropdown-menu. Fig 3.20 shows the KI values for the four load cases. Note that load case 2 has a negative KI. This is the compression load case and we did not include crack face contact in the analysis, so the crack faces penetrate each other giving a negative crack opening. In the next step, we turn on crack face contact and redo the analysis. Figure 3.18: Compute SIFs and Advanced Parameters dialogs. 84

85 Figure 3.19: Stress Intensity Factor dialog sum of Mode I SIFs. 85

86 Figure 3.20: Stress Intensity Factor dialog Mode I SIFs for each of the 4 load cases. Step 4.3: Re-Run ABAQUS static crack analysis with crack face contact Note that load step 2 gives negative KI values, meaning the crack surfaces are overlapping. From the FRANC3D menu, select Analysis and Static Crack Analysis. The first panel of the wizard should appear as seen previously in Fig We specify the file name for the FRANC3D database; we call it Abaqus_Cube_LC_CFC.fdb. Select Next once you enter the File Name. The next panel of the wizard, as seen in Fig 3.16, allows you to specify the solver; choose ABAQUS and then select Next. The next panel of the wizard, Fig 3.21, allows you to specify the ABAQUS analysis and output options. The Apply crack face tractions box should be checked automatically. We can check the Define crack face contact box, which will enable the Contact button. Click this button and the dialog shown in Fig 3.22 is displayed. In practice, you must make sure that these parameters do not conflict with any ABAQUS data already in the model. We are creating a new surface interaction, so we must enter the surface interaction name (we have used cfc-props in Fig 3.22). The coefficient of friction is set 0.5; the other parameters are left at the default values. Click Accept, and then click Finish in the previous panel (see Fig 3.21) when ready to proceed with the ABAQUS analysis. 86

87 Figure 3.21: Static Analysis wizard third panel ABAQUS output options. Figure 3.22: ABAQUS contact options. 87

88 Step 4.4: Compute SIFs with crack face contact Once ABAQUS is finished, we compute the stress intensity factors. If you are able to run ABAQUS directly from FRANC3D, then the model already exists and the results (.dtp) file will be read automatically. From the FRANC3D menu, select Cracks and Compute SIFs. When the Compute SIFs dialog is displayed, Fig 3.23, select the Advanced button and make sure that the Include Applied Crack Traction and the Include Contact Crack Pressure boxes are checked; select Finish and the SIFs Plot dialog is displayed, Fig The initial plot shows the sum of KI for all load cases. Fig 3.25 shows the KI values for the second load case. Note that value is close to 0.0, although it is not exactly equal to 0.0. Contact analyses are subject to some numerical error; to verify that the SIF results from the M-integral are reasonable, we compare to the SIF results using displacement correlation. In the Compute SIFs dialog, choose Displacement Correlation, Fig The Mode I SIFs for load case 2 are shown in Fig The results are comparable to those for M-integral, not exactly 0.0 but close. You can try different mesh refinement and/or contact options to improve the results, to obtain Mode I SIFs that are closer to zero. Figure 3.23: Compute SIFs and Advanced Parameters dialogs. 88

89 Figure 3.24: Stress Intensity Factor dialog sum of Mode I SIFs. Figure 3.25: Stress Intensity Factor dialog M-integral Mode I SIFs for the second load case. Figure 3.26: Compute SIFs dialog using Displacement Correlation. 89

90 Figure 3.27: Stress Intensity Factor dialog Displacement Correlation Mode I SIFs for second load case 3.5 Step 5: Apply Surface Treatment Residual Stress To simulate residual stress due to a surface treatment, such as shot-peening, FRANC3D allows you to define a 1-D stress profile as a function of distance from the surface. We demonstrate this using the Abaqus_cube.inp model with the one far-field tension load step. Start with the FRANC3D graphical user interface (see Fig 3.1), and select File and Import. In the window (see Fig 3.2), choose Complete Model. Switch the Mesh File Type radio button in the Select Import Mesh File window, (see Fig 3.3), to ABAQUS. Select the file name, called Abaqus_Cube.inp, and then select Next. As before, choose to retain all the boundary condition surfaces (see Figs ). The model will appear as shown in Fig 3.7. Insert the same crack from file as before (see Figs ). At this stage, we could do a static analysis to verify that the model is correct and compute the SIFs for the far-field loading only; the Mode I SIF should be the same as that shown in the top left panel of Fig We leave this as an exercise for the reader. The next step is to define the surface treatment residual stress. 90

91 From the FRANC3D main menu, select Loads and Crack Face Pressure/Traction, Fig Click on Add in the dialog box shown in the left panel of Fig Choose Surface Treatment Residual Stress, as show in the right panel of Fig 3.29, and select Next. The dialog shown in Fig 3.30 is displayed. We use Read From File to import the residual stress distribution from a.txt file. Using the Open File dialog shown in Fig 3.31, select the file surf_treat_res.txt, and then select Accept. The distribution is read and displayed in the dialog, Fig Select Next on this dialog panel to choose the surface of the model that is treated. The dialog shown in Fig 3.33 appears with all surfaces shown as blue; use the Shift key and the left mouse button to select the front surface (+z face) of the model. Once selected, the surface is colored red/pink. Ignore the Set Temperature setting. Select Finish and the original Add Traction dialog is displayed with one entry, Fig 3.34; select Accept. Figure 3.28: Loads Crack Face Pressure/Traction menu item selected. Figure 3.29: Crack Face Traction wizard panels; surface treatment selected. 91

92 Figure 3.30: Surface treatment residual stress panel. Figure 3.31: Select file for surface treatment residual stress. 92

93 Figure 3.32: Surface treatment residual stress panel - residual stress distribution displayed. Figure 3.33: Surface treatment residual stress panel to select the treated surface. 93

94 Figure 3.34: Crack Face Traction wizard panel - surface treatment added. From the FRANC3D menu, select Analysis and Static Crack Analysis. Specify the file name for the FRANC3D database; we call it Abaqus_Cube_surf_treat.fdb; select Next once you enter a File Name. The next panel of the wizard allows you to specify the solver; choose ABAQUS and the select Next. The next panel of the wizard allows you to specify the ABAQUS analysis and output options. The Apply crack face tractions box is checked automatically. Select Finish when ready to proceed with the ABAQUS analysis. Once ABAQUS is finished, from the FRANC3D menu, select Cracks and Compute SIFs. When the Compute SIFs dialog is displayed, you can check that the Include Applied Crack Traction box is checked; select Finish and the SIFs Plot dialog is displayed, Fig The initial plot shows the sum of KI for both load cases. The lower two panels of Fig 3.35 show the KI values for the first and second load cases separately. The values for the first load case are the same as previously computed. The second load case produces a negative SIF indicating that this residual stress tends to keep the crack from opening, which is generally the purpose of surface treatment. 94

95 Figure 3.35: Mode I SIF plots showing the sum (top) and the individual load case values; surface treatment load case produces a negative SIF (bottom right). 3.6 Step 6: Apply Tractions from Mesh-Based Stress Step 6.1: Create Mesh-Based Stress Field This section describes how to apply a crack surface traction using pre-computed stresses from an uncracked model. The uncracked model will typically be the same as the model that we use for 95

96 crack growth simulations. In this example, we use the Ansys_Cube model along with ANSYS stresses (from the FRANC3D/ANSYS Tutorial); we could use an ABAQUS or NASTRAN model and corresponding stresses. To create the mesh-based stresses, we start with the base cube model and define an arbitrary farfield stress on the top surface of the cube, Fig This creates a stress field that varies in the x- direction, Fig FRANC3D reads the ANSYS stress listing, Fig In ANSYS, we turn off PowerGraphics, change the format for the listing (using the /Format command), create the nodal stress component listing (using the prnsol,s command), and save the listing to a file; we call it Ansys_Cube_surf_gradient.str. The stress listing must be in the global Cartesian coordinate system. We also must save the corresponding Ansys_Cube_surf_gradient.cdb file. Note that if you use ABAQUS to generate the stresses for this tutorial, you need to write out the.fil file or write an ABAQUS CAE report (.rpt) file that contains the nodal stresses. FRANC3D will import an.inp and either the.fil or.rpt file. Additionally, if you are using ABAQUS CAE, to create the model, you should set NoPartsInputFile=ON to create a flat.inp file prior to running the analysis so that the stress listing has node ids that correspond exactly to the.inp file. See Step 6.3 for more details. If you use NASTRAN to create the stress, FRANC3D reads.bdf (or.nas) files along with.pch files with the nodal stress data. 96

97 Figure 3.36: Arbitrary far-field surface pressure. Figure 3.37: Stress in the y-direction for the arbitrary far-field surface pressure. 97

98 Figure 3.38: Nodal stress component listing. Step 6.2: Apply Mesh-Based Stress as Crack Face Traction Start with the FRANC3D graphical user interface (see Fig 3.1), and select File and Import. In the window (see Fig 3.2), choose Complete Model. Switch the Mesh File Type radio button in the Select Import Mesh File window, (see Fig 3.3), to ABAQUS. Select the file name for the model, called Abaqus_Cube.inp, and then select Next. As before, we choose to retain all the boundary condition surfaces (see Figs ). The model is shown in Fig 3.7. Insert the same crack from file as before (see Figs ). At this stage, we could do a static analysis to verify that the model is correct and compute the SIFs for the far-field loading only; the Mode I SIF should be the same as that shown in the top left panel of Fig We leave this as an exercise for the reader. The next step is to define the mesh-based crack surface traction. 98

99 From the FRANC3D main menu, select Loads and Crack Face Pressure/Traction, Fig Click on Add in the dialog box shown in the left panel of Fig Choose Residual Stress Defined on a Mesh, as show in the right panel of Fig 3.40, and select Next. The dialog shown on the left side of Fig 3.41 is displayed. We select the files for the mesh and the stress listing. There is only one load step in the stress listing. Ignore the Set Temperature setting, and select Finish; the original Add Traction dialog is displayed with one entry, Fig 3.41 right side; select Accept. Figure 3.39: Loads Crack Face Pressure/Traction menu item selected. Figure 3.40: Crack Face Traction wizard panels; residual stress defined on a mesh selected. 99

100 Figure 3.41: Crack Face Traction wizard panels for residual stress defined on a mesh. From the FRANC3D menu, select Analysis and Static Crack Analysis. We specify the file name for the FRANC3D database; we call it Abaqus_Cube_mesh_based.fdb here; select Next once you enter a File Name. The next panel of the wizard allows you to specify the solver; choose ABAQUS and the click Next. The next panel of the wizard allows you to specify the ABAQUS analysis and output options. The Apply crack face tractions box is checked automatically. Click Finish when ready to proceed with the ABAQUS analysis. Once ABAQUS is finished, from the FRANC3D menu, select Cracks and Compute SIFs. When the Compute SIFs dialog is displayed make sure that the Include Applied Crack Traction box is checked; select Finish and the SIFs Plot dialog is displayed, Fig The initial plot shows the sum of KI for both load cases. The lower two panels of Fig 3.42 show the KI values for the first and second load cases separately. The first load case is the same as previously computed. The second load case produces a negative SIF with a gradient due to the mesh-based crack face tractions. 100

101 Figure 3.42: Mode I SIF plots showing the sum (top) and the individual load case values; meshbased stress load case produces a negative SIF (bottom right). Step 6.3: ABAQUS Mesh-Based Stress This section describes how to use ABAQUS for the mesh-based stress. The Abaqus_Cube model from Tutorial #1 is modified so that the traction on the upper surface matches that used in the ANSYS model in Step 6.1. The resulting y-direction stress contours are shown in Fig 3.43; the stresses are basically the same as the ANSYS stresses shown in Fig

102 To generate a.fil file from ABAQUS, add the following lines to the.inp file just before the *End Step : ** output displacements and stress to fil results file *File Format, ASCII *Node File, Frequency=1 U *El File, position=averaged at nodes, Frequency=1 S Then submit the ABAQUS job for analysis. Note that if you use ABAQUS CAE, you can add these lines using the ABAQUS CAE menu, under Model and Edit Keywords. An additional change should be made in ABAQUS CAE to flatten the.inp file, removing *Part, *Instance and *Assembly data: >>> mdb.models["abaqus_cube"].setvalues(nopartsinputfile=on) This eliminates any confusion with node and element numbering. This should be set prior to running the analysis. Instead of using the.fil file, you can write the stress data to a.rpt file from ABAQUS CAE. Using the Report menu in CAE, choose Field Output. The dialog in Fig 3.44 is displayed; select Stress components and click OK. This assumes that you requested stress as a field output, which you do before submitting the analysis. We request unique nodal stress values in the report. By default, ABAQUS CAE saves the data to abaqus.rpt, you can change this using the Setup tab or just remember to rename the.rpt; we use Abaqus_Cube_surf_gradient.rpt here (this file name is used for the.inp and.fil files also). 102

103 Figure 3.43: ABAQUS stress in y-direction. Figure 3.44: ABAQUS report field output dialog. 103

104 4.0 Tutorial 3: Two Cubes Glued Together In Tutorial 3, we use two cubes that are tied together to illustrate how to simulate crack growth in models where there is contact or constraint between parts of the model. Tutorial 8 also includes contact conditions. 4.1 Step 1: Create the ABAQUS FE Model We use the same initial cube geometry and boundary conditions from the first tutorial and add a second adjacent cube, Fig 4.1, with slightly different material properties. The second cube has an elastic modulus of 20,000, which is double that of the first cube; the Poisson ratio is the same. The second cube is also constrained in the y-direction and has a surface traction (negative pressure) of 10 on the upper surface, which is the same as the first cube. We define constraint conditions between the two cubes. The right-side image of Fig 4.1 shows the constraint surface. The first set of analyses use constraint conditions, Fig 4.2. The ABAQUS.inp file is exported as doublecube_abaqus_constraint.inp. Figure 4.1: ABAQUS double cube model with constraint surface between the cubes. 104

105 Figure 4.2: ABAQUS tie constraint dialog. 4.2 Step 2: Import ABAQUS FE Model into FRANC3D Import the ABAQUS model into FRANC3D, using the.inp file written in the previous step; import as a full model. Step 2.1: Importing ABAQUS FE Model Start with the FRANC3D graphical user interface, and select File and Import. In the Select Type of Import panel, choose Complete Model and select Next. Switch the Mesh File Type radio button in the Select Import Mesh File window to ABAQUS and select the file name for the model, called doublecube_abaqus_constraint.inp, Fig 4.3. Select Next. 105

106 Figure 4.3: FRANC3D FE model import. The Select Retained Surfaces dialog is displayed, Fig 4.4. The surfaces with boundary conditions and the contact surface are highlighted in blue. Choose Select All to retain all of these surfaces. Figure 4.4: FRANC3D select retained surfaces. Step 2.2: Insert a Crack Insert a surface penny crack with radius of 1.0 in the second cube, Fig 4.5. Note that this crack is the same as that defined in Tutorial #1, except that it is translated in the x-direction so it falls in the second cube. The template mesh radius is left at the default value of 0.1, which also was used for Tutorial #1. The resulting remeshed model is shown in Fig 4.6; the contact surface mesh facets between the two cubes are retained. 106

107 Note that the contact surface mesh does not have to be retained, and if the crack is located such that the contact surface must be remeshed, we must not retain it. Here we retain it for simplicity and for demonstration. We show what happens if we do not retain it in Step 2.6. Figure 4.5: FRANC3D new crack insertion panel showing location and orientation. Step 2.3: Static Crack Analysis Run a static analysis using ABAQUS. From the FRANC3D Analysis menu, select Static Crack Analysis. Set the file name, use Abaqus_constraint_cubes_crack.fdb. Select the ABAQUS solver; all the default settings are used. Note that the.inp file written by FRANC3D includes ABAQUS commands to regenerate the tie constraint between the two cubes. 107

108 Figure 4.6: Remeshed cracked model, with contact surface mesh facets retained. Step 2.4: Compute SIFs The resulting Mode I SIF is shown in Fig 4.7. The curve is not symmetric; it was for Tutorial 1. Figure 4.7: Mode I SIFs for double_cube with contact between cubes. 108

109 Step 2.5: Plot Deformed Shape We can plot the deformed shape in FRANC3D. From the Display menu select View Response, Fig 4.8. Fig 4.9 shows that the displacement is not uniform; the first cube deforms about twice as much as the second, which is expected as it has a lower elastic modulus. The tie constraint between the two cubes is maintained. Figure 4.8: FRANC3D View Response menu option. Figure 4.9: Deformed shape 200x magnification. 109

110 Step 2.6: Contact surface mesh not retained If we choose to not retain the mesh on the constraint surface when importing the FE model into FRANC3D, we have to specifically unselect the contact surfaces, Fig 4.10; note that we unselect both sides of the interface here. Unselect/select is done using the Shift key with the left mouse button. Note that you will have to use the Clipping tool to see inside the model. Insert the same crack as in Step 2.2, into the second cube. The resulting surface mesh shown in Fig 4.11 has a remeshed contact surface. The static analysis is done using ABAQUS as in Step 2.3. The resulting Mode I SIFs, Fig 4.12, are the same as computed previously (see Fig 4.7). Figure 4.10: Import FE double_cube model with constraint surface unselected. 110

111 Figure 4.11: Double_cube model with unretained constraint surface remeshed. Figure 4.12: Mode I SIFs for double_cube with unretained constraint surface mesh. Step 2.7: Specify No Crack Material Region If the crack in the second cube is allowed to propagate, it will reach the interface between the two cubes. Depending on the material interface, the crack might stop or it might cross the interface. If the crack should stop at the interface but continue growing in the second cube region, we can specify that the first cube region is not to be cracked. 111

112 From the FRANC3D Advanced menu, select No Crack Regions, Fig The dialog shown in Fig 4.14 is displayed. Set the No Crack Region by checking the appropriate region s box. Figure 4.13: Advanced menu No Crack Regions option. Figure 4.14: No Crack Regions dialog - uncracked model (left) and cracked model (right). 5.0 Tutorial 4: Disk with Rotation and Temperature In Tutorial 4, we simulate crack growth in a simple disk model that includes temperature variation and rotation. In Step 1, we describe briefly the model and the thermal analysis to produce the temperature variation. Once the temperatures are defined, we run a structural 112

113 analysis that also includes rotation. With this model, we can then proceed to do the crack growth simulation. A goal of this tutorial is to show how temperature affects computed SIFs. 5.1 Step 1: Create the ABAQUS Disk Model The first step is to build the ABAQUS FE model and to define the material properties. The model is shown in Fig 5.1. The inner disk radius is 1, the outer radius is 10 and the width is 1. We define both the thermal and structural properties, which will consist of density, specific heat, enthalpy, thermal expansion, conductivity, elastic modulus and Poisson ratio. The material can be temperature dependent; for this analysis we use constant values for all data except for the elastic modulus, Fig 5.2. Density is set to 1.0 and enthalpy is set to 0. Figure 5.1: ABAQUS disk geometry. 113

114 Figure 5.2: ABAQUS disk material properties. 114

115 5.2 Step 2: Run ABAQUS Thermal Analysis The first analysis is for heat transfer, so we set the element type (DC3D10) and create a volume mesh. The model is meshed with all tetrahedral elements, Fig 5.3. The boundary conditions consist of temperatures on two surfaces; temperature at the inner radius of the disk is set to 1000 and temperature at the outer radius is set to 100, Fig 5.3. The resulting nodal temperatures are shown in Fig 5.4. These nodal temperatures are applied to the model as initial conditions for the mechanical analysis. Figure 5.3: Volume mesh and thermal boundary conditions. 115

116 Figure 5.4: Resulting nodal temperature contours. 5.3 Step 3: Run ABAQUS Structural Analysis We switch the element type (DC3D10 to C3D10) in the model for the structural analysis. The boundary conditions for the structural analysis consist of rollers on the (symmetry) surfaces at x=0 and y=0. We also fix a point in the z-direction to prevent rigid body motion, and apply the temperatures from the thermal analysis as initial conditions. Finally, define the rotational velocity (centrif) as about the z-axis. The resulting model with boundary conditions is shown in the left panel of Fig 5.5. The resulting maximum principal stress contours from the structural analysis are show in the right panel of Fig 5.5. We save the ABAQUS.cae file in case we need to re-analyze the model. We also create an.inp file for use with FRANC3D. Note that we could create global and local model portions in ABAQUS for FRANC3D. However, for this tutorial, we rely on the FRANC3D submodeler tool, so we just archive the full model. We also save the ABAQUS stress listing as Abaqus_Disk.rpt. 116

117 Figure 5.5: Boundary conditions for structural analysis left panel, and resulting maximum principal stress contours right panel. 5.4 Step 4: Import Disk into FRANC3D Start with the FRANC3D graphical user interface, and select File and Import. In the Select Type of Import panel, choose the Import and divide into global and local models radio button and select Next. Switch the Mesh File Type radio button in the Select Import Mesh File window to ABAQUS and select the file name for the model, called Abaqus_Disk.inp, Fig 5.6. Select Next. Figure 5.6: FRANC3D FE model import. 117

118 Select a local model using the rectangular Rubberband Box tool and Crop button in the Define Local Submodel window, Fig 5.7. Select Next and save the local and global model files using the default file names. In the Select Retained BC Surfaces window, Fig 5.8, use the Select All button to retain the two surfaces with displacement constraints, and then select Finish. The model will be displayed in the FRANC3D main window, and we are ready to insert the crack into the local model. Figure 5.7: FRANC3D FE model import. Figure 5.8: FRANC3D FE model import BC surface selection. 118

119 5.5 Step 5: Insert Initial Crack Insert an elliptical crack with a radius of 0.1, Fig 5.9. The crack is located at the front of the disk, rotated 45 degrees from the x-axis, Fig The crack front template has a radius of 0.01, Fig The resulting remeshed crack model is shown in Fig Figure 5.9: Elliptical crack dimension dialog. Figure 5.10: Crack location and orientation dialog. 119

120 Figure 5.11: Crack front template dialog. Figure 5.12: Final meshed crack model. 120

121 5.6 Step 6: Static Crack Analysis We perform a static crack analysis using ABAQUS. Choose Analysis and Static Crack Analysis from the FRANC3D menu. Provide a file name (Abaqus_disk_crack.fdb) and choose ABAQUS as the solver. The ABAQUS options are shown in Fig 5.13; the default settings will cause ABAQUS to write nodal temperatures to the results (.dtp) file. The Connect to global model option is checked automatically. Select Next. Figure 5.13: Static analysis options for ABAQUS. The next dialog box has options for connecting the local and global portions, Fig We use node merging with the automatically selected local and global cut-surfaces. Click Finish to begin the ABAQUS analysis. 121

122 Figure 5.14: Static analysis ABAQUS local + global model connection dialog. 5.6 Step 6: Compute SIFs Once ABAQUS has finished, we compute the SIFs; choose Cracks and Compute SIFs from the FRANC3D menu. The dialog, Fig 5.15, allows you to specify the method for computing SIFs. If you use the M-integral, you can make sure that the Include Thermal Terms option is checked and the Reference Temperature is 0 degrees by clicking the Advanced button. The SIFs based on the M-integral are shown in Fig 5.16 and the SIFs based on Displacement Correlation (DC) are shown in Fig It should be noted that the SIFs differ very little, indicating that the SIFs are computed correctly. If your results differ significantly, you should ensure that the nodal temperatures are all correct. Note that if you do not include thermal terms when computing M-integral SIFs, the results will be very different from the DC SIFs, Fig

123 Figure 5.15: Compute SIFs dialog. Figure 5.16: M-Integral based SIFs. 123

124 Figure 5.17: Displacement correlation based SIFs. Figure 5.18: M-Integral based SIFs without thermal terms added. 5.7 Step 7: Crack Growth The next step is to propagate the crack. Choose Cracks and Grow Crack from the FRANC3D menu. We switch to quasi-static growth, Fig 5.19, and select Next. We leave all the defaults in the next two panels, Fig , and select Next and Finish. 124

125 Figure 5.19: Crack growth first wizard panel. Figure 5.20: Crack growth second wizard panel. The median extension is set to 0.015, and the extrapolation is set to 4% for both ends, Fig The template radius is set to 0.01, Fig Select Finish when ready to start the process of crack growth, insertion and remeshing. 125

126 Figure 5.21: Crack growth third wizard panel. Figure 5.22: Crack growth third wizard panel. 126

127 Note that the crack front and template should extend beyond the model surface at every step; this sometimes requires small adjustments in the fitting depending on the crack front and model surface geometry. For this model, 3% extrapolation is not quite enough to ensure that all the template end points fall outside of the model. Figure 5.23: Crack growth wizard final panel. 5.8 Step 8: Automatic Crack Growth We can continue doing static analyses and manually growing the crack at each step or we can do automatic crack growth. We proceed with automatic crack growth at this point. Select Crack 127

128 Growth Analysis from the Analysis menu. A series of dialog panels some of which you have just seen in Step 7 when manually growing the crack will be displayed; use the same settings. We specify 10 crack growth steps with a constant median increment of 0.015, Fig We set the current crack growth step to 1 as we have extended the crack but have not yet analyzed it, Fig The last two panels are the same as those for Step 6 (see Fig 5.13 and 5.14). All the default settings should be okay; select Finish to start the automatic growth. Figure 5.24: Crack growth plan dialog for automatic crack growth. Figure 5.25: Crack growth step number and base file name dialog for automatic crack growth. 5.9 Step 9: Analysis Results After 10 steps of crack growth using a constant increment of 0.015, the crack appears as in Fig You can monitor the FRANC3D CMD window for any error messages as well as 128

129 monitoring the ABAQUS logs. The SIF history is shown in Fig You can continue to grow this crack and/or you can compute fatigue cycles at this stage. We can examine the temperature contours in ABAQUS to verify that the temperatures are mapped correctly, Fig The deformed shape of the crack at step #11 is shown in Fig Figure 5.26: Crack configuration after 10 steps of automatic crack growth. Figure 5.27: Mode I SIF history after 10 steps of automatic crack growth. 129

130 Figure 5.28: Contours of structural temperatures at crack step #11. Figure 5.29: Deformed shape of crack step #

131 5.10 Step 10: Fatigue Life We will compute fatigue life or cycles based on the completed crack growth. From the FRANC3D menu, select Fatigue and Fatigue Life Predictions. If the SIFs have not been computed yet, the Compute SIFs dialog will be displayed; leave the defaults and select Finish. The Fatigue Life dialog, Fig 5.30, is displayed. In this dialog, the crack fronts are displayed on the left and the window on the right side should be blank (assuming that lifing parameters have not been defined previously). You must Set (or Read) Parameters. Selecting Set Parameters displays the dialog shown in Fig Figure 5.30: Fatigue Life parameters 131

132 Figure 5.31: Fatigue Life parameters We want to set the FEM model units to MPa mm; select the Change button to display the dialog in Fig Set the units to MPa and mm and select Accept. Figure 5.32: FEM units dialog 132

133 The crack growth load schedule is defined next. Select the New Schedule button (see Fig 5.31) to display the dialog in Fig Select the Schedule and then select the Add button; see right side image of Fig This will display the dialog shown in Fig 5.34; we will just use a simple cyclic load schedule where the applied load produces Kmax and Kmin is zero. Select Accept to return to the Load Schedule, Fig The Repeat count is set to FOREVER, Fig 5.35, and in the temperture tab, the Tempeature dependent crack growth is selected and the Use temperature from Kmax is chosen. Select Accept to finish the load schedule. Figure 5.33: New Load Schedule dialog 133

134 Figure 5.34: Event type dialog Figure 5.35: Simple cyclic load schedule repeated forever with temperature from Kmax The crack growth rate model is defined next. Select the New Model button (Fig 5.31) to display the dialog in Fig Choose the cyclic loading growth rate model and select Next to display the dialog in Fig

135 Figure 5.36: Growth model type dialog Figure 5.37: Cyclic loading growth model dialog We use a simple Paris growth model, which is the default; select Next to display the dialog in Fig The growth rate model will be temperature dependent. Select Next to display the Paris growth model dialog, Fig Figure 5.38: Temperature dependent growth rate model 135

136 Set the units for the Paris growth model. Select the Change button to display the Units dialog, and set the units the same as the FEM units that we set earlier, which were MPa and mm. Set the Number of temperatures to 2. In the the fields for temperature, C, n, DKth and Kc, enter the appropriate values, Fig Select Next to return the main dialog (see Fig 5.31). The other options are left at their default values. Select Accept to return to the Fatigue Life dialog, Fig As an exercise, you can display cycles along a path as in Tutorial 1. Figure 5.39: Paris growth rate model dialog. Figure 5.40: Fatigue Life dialog showing Cycles vs Crack Growth Step 136

137 5.11 Apply Crack Face Traction (CFT) Only We want to verify that the uncracked stress, saved to Abaqus_Disk.rpt in Section 5.3, when applied as crack face traction, provides the same SIFs as the actual applied boundary conditions. We first edit the Abaqus_Disk.inp file and remove all the rotation and temperature boundary conditions (if there were pressures or forces, we would remove those also). The displacement boundary conditions are left untouched (note that if the displacement values were non-zero, FRANC3D would zero those for the CFT load step.) Save the file as Abaqus_Disk_noload.inp. We import this model and insert the crack as was done for the original model. Once the crack is inserted, we apply the crack face traction. Select the Loads Crack Face Pressure/Traction menu option. Click the Add button, Figure 5.41, and switch to the Residual Stress Defined on a Mesh, Figure Choose the Abaqus_Disk.inp and Abaqus_Disk.rpt files, Figure 5.42, and then click Next. Set the temperature to Constant and 0.0, which is the default reference temperature, and then click Finish. Click Accept to close the Crack-Face Tractions dialog. Figure 5.41: Add CFT dialog panels. 137

138 Figure 5.42: Residual Stress CFT dialog panels. Run the static crack analysis as for the original model and then compute the SIFs using the M- integral, Figure If you click on the Advanced button, the Include Applied Crack Traction option is turned on automatically, Figure The M-integral includes terms for CFT and thermal strain. The SIFs are displayed in Figure The CFT loads are applied in separate load steps from the base model load steps. 138

139 Figure 5.43: Compute SIFs dialog. Figure 5.44: M-Integral based SIFs for CFT. To verify the M-integral terms are computed correctly, we can plot the displacement correlation SIFs. These values are usually within a couple percent of the M-integral values and are based only on ABAQUS displacements. Figure 5.45 shows the DC SIFs. 139

140 Figure 5.45: DC based SIFs for CFT. Now we add the CFT load to the original model, which will be the typical modeling situation. Start with the original Abaqus_Disk.inp file and repeat Steps 4 and 5 in Sections 5.4 and 5.5. Once the model is imported and the crack is inserted, add the CFT as shown in Figures Run a static crack analysis and compute SIFs. The base load step SIFs are shown in Figure The CFT load step SIFs are shown in Figure Figure 5.46: M-integral based SIFs for base load step. 140

141 Figure 5.47: M-integral based SIFs for CFT load step. Note that the CFT SIFs are computed based on temperatures that are set to 0.0, which is the reference temperature for the analysis. The ABAQUS analysis load step has temperature set to 0.0, and the temperature dependent material properties will be determined at this temperature. If temperatures are different from the reference temperature, then the *Expansion should be set to 0.0 for the CFT load step to eliminate unwanted thermal stress or strain. 6.0 Tutorial 5: Multiple Cracks in a Plate In Tutorial 5, we simulate multiple cracks using a simple plate model. Section describes some of the issues you might encounter when growing a crack around a geometric corner of the plate. Section describes how to grow a surface crack through the plate to create middlethrough crack. 141

142 6.1 Step 1: Create the ABAQUS Plate Model The plate dimensions are defined as: 20 x 50 x 5. The bottom surface is fixed in the y-direction and the top surface has traction of 10. Additional constraints on the bottom left edge prevent motion in the x-direction, and the node at the origin is fixed in the z-direction also, Fig 6.1. Figure 6.1: ABAQUS plate model. The material properties are shown in Fig 6.2. The model is meshed with 20-noded brick elements. Once the model has been defined and analyzed in ABAQUS to verify that the boundary conditions are correct, the model can be saved to a.inp file; we call it Abaqus_plate.inp. 142

143 Figure 6.2: ABAQUS plate model material properties. 6.2 Step 2: Import Plate Model into FRANC3D From the FRANC3D menu, select File and Import. We will divide the plate into local and global portions, Fig 6.3. Extract the mid-portion of the plate using the rectangular Rubberband Box in the Submodeler dialog, Fig 6.4. Select Crop and Next in this dialog to extract the portion of the model selected. Save the local and global model files using the default names. There are no boundary conditions on this middle portion, however, there are node sets, Fig 6.5; just select Finish in the Select Retained BC Surfaces dialog. The model is then displayed in the FRANC3D main window. The cut-surface mesh facets are automatically retained, Fig

144 Figure 6.3: FRANC3D model import of plate model. Figure 6.4: FRANC3D submodel extraction for plate model. 144

145 Figure 6.5: FRANC3D Select Retained Surfaces. Figure 6.6: Local plate model with cut-surface mesh facets retained. 145

146 6.3 Step 3: Insert Multiple Cracks From the FRANC3D menu, select Cracks and Multiple Flaw Insert, Fig 6.7. The dialog shown in Fig 6.8 is displayed. Use the Add button to define each crack that will be added. Figure 6.7: Plate submodel in FRANC3D main window Multiple Flaw Insert menu selected. Note that one could also define single cracks using the New Flaw Wizard menu, save each crack to a file without adding it to the model, and then use the Flaws From Files to add the multiple.crk files. Figure 6.8: Multiple crack definition dialog. 146

147 After selecting Add, the usual Flaw Definition wizard panels are displayed. Figs provide the parameters for the first crack to be added, which is a middle (or center) through crack. This crack has two fronts. The crack geometry must be defined such that intersections between the crack and model can be computed; we set g=5.2 as the plate is 5 units thick. Figure 6.9: Flaw definition middle through crack selected. Figure 6.10: Middle through crack dimensions. 147

148 Figure 6.11: Middle through crack orientation. Figure 6.12: Middle through crack template. 148

149 Select the Meshing Parameters button in Fig 6.12 to display the dialog in Fig Turn off the Do Coarsen Crack Mouth Mesh so that we generate a more refined mesh to help improve the results. A coarse tetrahedral mesh near the crack typically leads to a rough SIF curve. We will use ABAQUS volume meshing also; set these same meshing parameters for all cracks. Figure 6.13: Meshing parameters Do Coarsen Crack Mouth Mesh turned off. Once the template is defined, select Finish, Fig 6.12, and the Multiple Crack Definition dialog shows the first crack name, Fig Select Add again to add the second crack, which will be an edge through crack, with one crack front, Fig

150 Figure 6.14: Multiple crack definition dialog with one crack defined. Figure 6.15: Flaw definition edge through crack selected. The crack width is defined such that it is bigger than the plate (5.2 compared to 5), and the crack depth is bigger (0.55) than what we intend (0.5) also, Fig You must orient the crack so that the front falls inside the model, Fig 6.17; if you are unsure of the orientation, select Next and look at the template, Fig If you set the orientation incorrectly, select Back to fix it. When you are done, select Finish. The Multiple Crack Definition dialog shows two crack names, Fig

151 Figure 6.16: Edge through crack dimensions. Figure 6.17: Edge through crack orientation. 151

152 Figure 6.18: Edge through crack template. Figure 6.19: Multiple crack definition dialog with two cracks defined. Select Add again to add the third crack, which will be a long shallow crack, Fig Note that we typically use this crack instead of high-aspect ratio ellipses as the geometry at the ends is better for the template mesh. The crack geometry is again defined such that intersection with the plate surface can easily be computed, Fig Select Finish, Fig 6.23, to return to the Multiple Crack Definition dialog, which now shows three crack names, Fig

153 Figure 6.20: Flaw definition long shallow crack selected. Figure 6.21: Long shallow crack dimensions. 153

154 Figure 6.22: Long shallow crack orientation. Figure 6.23: Long shallow crack template. Select the Display button, Fig 6.24, to show all three cracks in the model, Fig The cracks should not be overlapping or intersecting. Select Finish to close the display. 154

155 Figure 6.24: Multiple crack definition dialog with three cracks defined. Figure 6.25: Multiple cracks displayed together. Select Accept (see Fig 6.24), to start the crack insertion and remeshing process. Note that you can use the Add / save radio button to save the cracks to a.crk file first if you think you might need to restart from this initial configuration; you might want to vary the mesh refinement 155

156 (template radius) for instance. The remeshed model is shown in Fig We can now proceed with the static analysis. Figure 6.26: Remeshed model with three cracks inserted. 6.4 Step 4: Static Crack Analysis Follow the same procedure as in the previous tutorials to run the ABAQUS analysis. Select Static Crack Analysis from the FRANC3D menu, set the file name (we use Abaqus_plate_multi_crack), set the ABAQUS options, Fig 6.27, check the local + global connection, Fig 6.28, and select Finish to start the ABAQUS analysis in the background. 156

157 Figure 6.27: Static analysis wizard panel to set ABAQUS solver options. Figure 6.28: Static analysis wizard panel to set local + global connection. 157

158 6.5 Step 5: Compute SIFs for Multiple Crack Fronts Once ABAQUS has finished, select Compute SIFs from the FRANC3D menu. The SIF dialog allows you to select specific crack fronts to display SIF plots, Fig The front is identified in the image on the left by the red A and B. As you grow the crack(s), you will have SIF curves from all four crack fronts for all crack growth steps. If there were multiple load steps, you would have separate SIF curves for each of those also. Figure 6.29: Mode I SIF for crack front # Step 6: Grow Multiple Cracks Select Grow Cracks from the FRANC3D menu. We switch to quasi-static growth as in Tutorial 1 and leave all the other parameters at their default values. The resulting crack growth, using a median extension of 0.15, is shown in Fig The growth for all crack fronts is scaled based on the median increment and the relative SIFs along all the crack fronts. Setting the median extension to 0.15 ensures that we have growth for all cracks. Note that you can turn off growth for a specific crack front by unchecking the grow box (bottom left of Fig 6.30). 158

159 Each front has its own fitting parameters. In this case, this is important as the front on the left side can easily be fit to a 3 rd order polynomial (2 nd order would work too), Fig 6.31, but the front on the right must use a different type of fit, Fig For this crack front, a cubic spline or moving polynomial fit could work, but we use the multiple polynomial (you can set the order to 4 for this front if the fit is better). Once you have checked the fit for all fronts, you can proceed to the next panel to set the template mesh parameters, Fig 6.33, and then proceed with the actual process of growing and remeshing. Note that FRANC3D currently does not track crack front ids perfectly; so as the cracks grow, crack front ids might change, although this is unlikely. Figure 6.30: Crack growth wizard panel. 159

160 Figure 6.31: Crack growth wizard panel showing crack front #2. Figure 6.32: Crack growth wizard panel showing crack front #3. 160

161 Figure 6.33: Crack growth wizard panel showing crack front templates. 6.7 SIFs History for Multiple Cracks After the crack growth and remeshing process has been completed in Step 6, we set up 5 additional steps of automatic crack growth analysis using the same growth rules. Once that has completed, you can plot the SIFs for all cracks, Figs Using the dropdown tabs at the top of the dialog, you can switch between the steps of crack growth and between the crack fronts. 161

162 Figure 6.34: SIFs dialog SIFs for step 6 of front 1. Figure 6.35: SIFs dialog SIFs for step 6 of front 1. If you want to plot all SIFs for a given crack front together in a single plot, use the Cracks SIFs For All Fronts menu option, Fig You can switch between the crack fronts using the dropdown tab at the top. You can also plot the SIF history along a path through any of the crack fronts using the Cracks SIFs Along a Path menu option, and defining the path, Fig Fatigue cycles can be computed also; we leave this as an exercise for the reader. 162

163 Figure 6.36: SIFs For All Fronts dialog for crack front 2. Figure 6.37: SIFs Along a Path dialog for crack front Crack Growth Transitions Grow a Crack around a Corner In this section, we describe how to grow a crack around a 90 degree corner, creating a throughedge-crack from a corner-crack shape. We could use the model from the previous steps, as crack 163

164 4 would need to grow around the corners of the plate, but we will simplify things by using a single crack for this step. Import the local portion of the plate model that was created during Step 2. We can import as already divided or we can subdivide again choosing the retained element listing. The model should appear as in Fig 6.6. We insert a single crack, using the elliptical shape from the flaw library. The crack radius is 1.0. It is located as shown in Figure The mesh template settings are left at their default values. Figure 6.38: Single corner crack location and orientation. An initial static crack analysis is completed to obtain the initial SIFs, Fig The crack growth is done using the quasi-static growth model with n=2. The initial growth and fitting parameters are shown in Fig To keep things simple, 24 steps of automated crack growth using this same constant median extension are completed. The mesh template parameters are left at their default values. 164

165 Figure 6.39: Single corner crack SIFs. Figure 6.40: Single corner crack initial growth. 165

166 At step #24, the crack front is close to the back surface. The crack will transition from a corner crack to an edge crack, and this can happen automatically (Fig 6.41), but if a user wants to capture SIF values as the crack transitions, then some manual crack growth steps and static analyses can be performed. Fig 6.42 shows a series of manual crack growth steps where the median increment is adjusted so that the crack front transitions in a user-controlled manner around the corner. Note that when the crack front is at the corner, and when it intersects the model surface at shallow angles, we can turn on Simple Intersections for the template mesh. This forces the template to be pulled back from the model surface; FRANC3D should turn this on automatically as needed, but we can ensure that it is on by checking the box (see middle right image). If the back surface of the plate is not being refined enough when the crack front is close, you can edit the Meshing Parameters and turn on Do Local Surface Refinement (see top right panel of Fig 6.42). Figure 6.41: Single corner crack after 24 steps (left) and after 27 steps (right) of growth. 166

167 167

168 Figure 6.42: Manual steps of growth for single corner crack as it transitions around a corner Grow Crack through a Back Surface In this section, we describe how to grow a crack through a back-surface, creating a centerthrough-crack with two fronts from a surface-penny crack in a plate. The steps to grow a crack front through a back-surface are similar to those for transitioning a crack around a corner. We use manual crack growth and static analysis steps when the crack front gets close to the surface and as it breaks through. We describe the steps here using the same plate model but with a single surface-penny crack inserted on the front surface of the plate. Import the local portion of the plate model that was created during Step 2. We can import as already divided or we can subdivide again choosing the retained element listing. The model will appear as in Fig 6.6. We insert a single crack, using the elliptical shape from the flaw library. The crack radius is 1.0. It is located as shown in Figure The mesh template settings are left at their default values. 168

169 Figure 6.43: Single surface crack location and orientation. An initial static crack analysis is completed to obtain the initial SIFs, Fig The crack growth is done using the quasi-static growth model with n=2. The initial growth increment and fitting parameters are shown in Fig To keep things simple, automated crack growth is completed using a constant median extension for 10 steps, and then a slightly larger extension for another 10 steps, etc. The mesh template radius is adjusted to be 75% of the median extension. Figure 6.44: Single surface crack SIFs. 169

170 Figure 6.45: Surface crack growth parameters. As the crack grows, the crack front gets closer to the back surface. The crack will transition from a surface crack to a center-through crack, and this might happen automatically, but will often require manual steps of growth. If a user wants to capture more SIF values as the crack transitions, then some manual crack growth steps and static analyses should be performed. Fig 6.46 shows a series of manual crack growth steps where the median increment is adjusted so that the crack front transitions in a user-controlled way toward and through the back-surface. If the back surface of the plate is not being refined enough when the crack front is close, you can edit the Meshing Parameters and turn on Do Local Surface Refinement (top right image in Fig 6.46). The crack increment and template radius can be reduced to get the front close to the back surface before breaking through, but there needs to be enough room to volume-mesh (top left 170

171 image). Eventually, the crack must be propagated through the back surface (middle left image). Note that when the crack front intersects the model surface at shallow angles, we can turn on Simple Intersections for the template mesh (middle right image). This forces the template to be pulled back from the model surface; FRANC3D should turn this on automatically as needed, but we can ensure that it is on by checking the box (bottom right image). When the crack front intersects the back surface at a more reasonable angle (closer to a right angle), the Simple Intersection can be turned off. Figure 6.46: Surface crack in a plate after automatic growth to the back surface of the plate; usercontrolled growth and static analysis allows controlled break-through of the back surface. 171

172 6.9 Grow Multiple Cracks in Multiple Submodel Portions We describe how to extract multiple separate portions of a full model to create a submodel, which might be useful when inserting multiple cracks where the cracks are far apart Step 1: Import Plate Model into FRANC3D From the FRANC3D menu, select File and Import. We Import and divide the plate model, Fig We first extract the mid-portion of the plate using the Rubberband tool in the Submodeler, Fig Select Crop and then continue with the subsequent Rubberband selections and Crops as shown in Figs Note that we switch the cropping option to highlight the inverse selection in Figs Figure 6.47: FRANC3D model import of plate model. 172

173 Figure 6.48: FRANC3D first submodel extraction for plate model. Figure 6.49: FRANC3D second submodel extraction for plate model. 173

174 Figure 6.50: FRANC3D third submodel extraction for plate model. Figure 6.51: FRANC3D fourth submodel extraction for plate model. Select Next after selecting Crop. Save the local and global.inp files using the defaults. The Select Retained BC Surfaces dialog is displayed, Fig There are no boundary conditions on these two portions, so select Finish. 174

175 Figure 6.52: FRANC3D Select Retained BC Surfaces dialog. The model will be displayed in the FRANC3D main model window, Fig The cut-surface mesh facets for both portions are retained automatically. The next step is to insert edge-cracks into the two portions. Figure 6.53: FRANC3D model with two portions of the full model. 175

176 6.9.2 Step 2: Insert Multiple Cracks From the FRANC3D menu, we select Cracks and Multiple Flaw Insert. The dialog shown in Fig 6.54 is displayed. Use the Add button to define the two edge cracks. Fig 6.55 shows the dimensions for both edge cracks that will be inserted. Figs 6.56 and 6.57 show the location, orientation and mesh template for crack #1. Figs 6.58 and 6.59 show the location, orientation and mesh template for crack #2. Figure 6.54: Multiple crack definition dialog. 176

177 Figure 6.55: FRANC3D edge through crack definition. Figure 6.56: FRANC3D edge through crack location and orientation crack #1. 177

178 Figure 6.57: FRANC3D edge through crack mesh template crack #1. Figure 6.58: FRANC3D edge through crack location and orientation crack #2. 178

179 Figure 6.59: FRANC3D edge through crack mesh template crack #2. After defining both edge cracks, the Multiple Crack dialog shows the two crack names, Fig Click on Display in this dialog to show the cracks in the model, Fig Click Accept (in the dialog in Fig 6.58) to finish the insertion and remeshing. The resulting model is shown in Fig Figure 6.60: FRANC3D multiple crack insertion dialog. 179

180 Figure 6.61: FRANC3D multiple crack insertion display. Figure 6.62: FRANC3D model with edge cracks in two separate model portions. 180

181 6.9.3 Step 3: Crack Analysis Follow the same procedure as in the previous tutorials to run the ABAQUS static crack analysis. Select Static Crack Analysis from the FRANC3D menu, set the file name, make sure the local + global connection is set, and run ABAQUS. Once ABAQUS has finished, select Compute SIFs from the FRANC3D menu. The SIF dialog allows you to select specific crack fronts to display SIF plots. The front is identified on the left by the red A and B. Fig 6.63 shows the SIF for crack #1, and Fig 6.64 shows the SIF for crack #2. If your SIF curves are not as smooth as the curves in Figs , try changing the meshing parameters (see Fig 6.13); you can try the parameters shown in Fig Figure 6.63: Mode I SIF for crack #1. 181

182 Figure 6.64: Mode I SIF for crack #2. Figure 6.65: Meshing parameters dialog. The cracks can be propagated as described previously; see Section 6.6 for example. Figure 6.66 shows the tentative crack growth. Subsequent crack growth is left as an exercise for the reader. 182

183 Figure 6.66: Crack growth dialog. 7.0 Tutorial 6: Computing Fatigue Life Cycles In Tutorial 6, we describe the Fatigue module in more detail by presenting an example simulation of a surface crack in a plate under cyclic loading, comparing the computed number of cycles to experimental values from: Manu, C. (1980) Three-dimensional finite element analysis of cyclic fatigue crack growth of multiple surface flaws, PhD Thesis, Cornell University. The plate and initial crack dimensions are shown in Fig 7.1. The loading is uniaxial tension. The physical testing produced the crack growth seen in Fig 7.2. The crack grows through the plate, eventually becoming a center-through crack with two crack fronts. 183

184 Figure 7.1: Single surface crack in plate under tension: Figure 7.2: Single surface crack in plate under tension (from Manu, 1980). The crack growth is simulated using FRANC3D, and Fig 7.3 shows the crack fronts. The fatigue cycles are computed using the resulting SIF history and appropriate crack growth rate material data. For units of MPa and mm, the Paris parameters for this material are: C=1.14e-15 and m=3.85; Kth is 121 MPa mm ½ and KIc is 6949 MPa mm ½. The cycles are compared to previous simulations and experimental observations, Fig 7.4, from: Barlow, K., 2008, Propagation Simulation of Multiple Cracks in a Tensile Specimen, International Conference on Fatigue Damage of Structural Materials VII, Hyannis, MA. 184

185 Figure 7.3: FRANC3D simulated crack growth for single surface crack in a plate in tension Figure 7.4: Crack growth cycles for single surface crack in plate under tension. 185

186 7.1 Step 1: Perform Crack Growth The first step is to import the ABAQUS model of the plate into FRANC3D. We import and divide the full model using the FRANC3D Submodel tool, Fig 7.5. There are no boundary conditions on the local model; it is displayed in the FRANC3D main modeling window with the cut-surface facets retained, Fig 7.6, after we Crop and finish with the Submodel tool. Figure 7.5: Local and global model portions. 186

187 Figure 7.6: Local model portion. The semi-elliptical surface crack dimensions are defined in Fig 7.1. The location and orientation are shown in Fig 7.7. We use a template radius of 0.15 and turn off the Do Crack Mouth Coarsen Mesh flag in the Meshing Parameters dialog. Figure 7.7: Surface crack location and orientation. 187

188 A static crack analysis using ABAQUS is completed after crack insertion and remeshing is completed. Once ABAQUS has finished, the mode I SIFs are computed. These can be compared with the Raju-Newman handbook solution, Fig 7.8. The solutions differ by less than 1% for most of the crack front; the ends and midpoint differ by less than 2%. Figure 7.8: Mode I SIF for initial semi-elliptical surface crack comparing FRANC3D with handbook solution. The crack growth could be simulated using a few steps with relatively large increments, but we use a larger number of steps with small increments of growth. For the initial analyses, the growth is based on constant amplitude loading with Paris crack growth rate material data given above. Variable amplitude loading options are discussed in Step 3. The series of dialog boxes in Figs show the growth model used here. Fig 7.14 shows the crack front fitting options. Figure 7.9: Growth type dialog. 188

189 Figure 7.10: Kink angle dialog. Figure 7.11: Fatigue growth parameters dialog. 189

190 Figure 7.12: Fatigue growth parameters dialog. Figure 7.13: Paris growth model dialog. Using the Crack Growth Analysis menu option in FRANC3D, the crack is propagated automatically. Fig 7.15 shows the growth plan dialog with the stopping criteria set to maximum number of cycles. 190

191 Figure 7.14: Crack front fitting dialog. Figure 7.15: Growth plan dialog. 191

192 The Mode I SIF history is shown in Fig 7.16 for a path through the first 48 crack fronts. The fatigue life computations are described in the next step. Figure 7.16: Mode I SIF history. 7.2 Step 2: Compute Fatigue Crack Growth Cycles The crack growth in Step 1 was performed using a constant amplitude loading with Paris fatigue parameters. When we select Fatigue and Fatigue Life Predictions from the FRANC3D main menu, the dialog shown in Fig 7.17 is displayed. The cycles versus crack growth step number are plotted by default. The number of cycles is computed at each step of growth and stored in the FRANC3D database; the number of cycles is an average of the values computed at each mid-side node along the crack front. 192

193 Figure 7.17: Mode I SIF history cycles vs crack step number. The Fatigue Life dialog also allows us to plot cycles versus crack length, Fig , where the length might be the crack length measured on the model surface, which is what was observed and measured during the experiments. Regardless of the path chosen, the number of cycles is consistent, if the path goes through all of the fronts. The number of cycles is 110,171 at the current configuration, where the crack front is very close to the back surface of the plate, but has not yet broken through; there is about 0.5 mm between the deepest point on the crack front and the back surface. This number of cycles is based on constant amplitude loading with R=0, which is not exactly representative of the experiment. 193

194 Figure 7.18: Mode I SIF history define a path near the model surface. Figure 7.19: Mode I SIF history cycles vs crack length. 7.3 Step 3: Crack Growth and Fatigue Options The applied (measured) loading spectrum from the Manu experiment is shown in Fig 7.4. It consists of a history of blocks of constant amplitude load cycles, where the blocks have different R values (R = minimum load /maximum load) and different numbers of cycles. There 194

195 are two different R values (0.15 and 0.575), and these values differentiate the blocks of cycles. There are 47 blocks and a total of 375,370 cycles applied during the test. Options for crack growth in FRANC3D consist of: 1) quasi-static, which implies a single constant or increasing load, 2) constant amplitude cyclic load, 3) variable amplitude sequence load, 4) variable amplitude spectrum load, and 5) variable amplitude transient load. Constant amplitude cyclic loading was used in Step 1 and 2 above, with R=0. The computed number of cycles is significantly less than the number measured in the experiment, which is expected as the K value at R=0 is higher, and thus the crack growth rate is higher. If we modify the R value in the Fatigue Life dialog (use the View/Edit button for the Crack Growth Load Schedule) and use 0.15, Fig 7.20, the computed cycles increases to 206,182. We can also try setting R to 0.575, and in that case the number of cycles is 2,973,207. (Note that your numbers should be only slightly different.) Figure 7.20: Fatigue Life Load Schedule dialog with R set to

196 7.3.1 Variable Amplitude Loading Constant amplitude loading cannot capture the number of cycles in the experiment. The variable amplitude load options in FRANC3D are briefly described here. Consult the other reference documentation for more details. The schedule option involves a number of load steps (or load cases). For example, for a jet engine component, a user defines a set of load steps where each step has a different temperature distribution and a different angular velocity; each load step represents a different time point in a typical flight (e.g., ground idle, takeoff/climb, cruse, maneuver, decent, reverse thrust). The load step order in the analysis does not need to correspond to how they would be encountered in a real flight. In FRANC3D, a user constructs a Load Sequence (or mission profile) that describes a typical mission or flight. For each stage in the sequence, an optional load and temperature multiplier can be applied, giving a sequence table such as: Load_Step Load_Mult Temp_Mult Comment Ground idle (cold) Climb Initial cruse Maneuver Second cruse Maneuver Third cruse Descent Ground idle (hot) FRANC3D computes SIFs for each of the stages in the sequence and then steps through those SIFs and find the K and R for each reversal (e.g. from off to ground idle ). For each K and R, FRANC3D finds da = da/dn( K,R,T), and sums the da's for each stage in the sequence to get da total for one pass through the sequence. Note that da is the change in crack length. Each pass through the sequence represents one flight. FRANC3D passes through the sequence as many times as necessary to predict crack length as a function of number of flights (rather than as a function of the number of cycles). 196

197 The spectrum loading option involves a load history that defines the stress level at a (typically large) number of time points. This load history is counted using a "rainflow" or other method to come up with a list of load reversals (stress_max and stress_min pairs). This is a counted load spectrum, and there are industry standard spectra (e.g. FALSTAFF, TWIST, TURBISTAN and HELIX). This is the option that we will use in the next subsection. FRANC3D steps through the spectrum one load reversal at a time. For the current crack length, FRANC3D computes the sum of the K's from one or more analysis load steps (as per the user's input) and multiplies the nominal K by the stress_max and stress_min values to get K_max and K_min for the current load reversal. FRANC3D then computes K and R, and then da = da/dn( K,R,T). The crack length is updated and the computation repeated. The transient loading option involves a series of load steps that mimic a moving load or a load that changes in time. An example of this is gear tooth contact; as two gears rotate the load on a tooth changes in magnitude and location as the tooth comes into and goes out of contact with the opposing tooth. Another example is the changing load on a railway wheel as it comes into and goes out of contact with the track as the wheel revolves. In these cases, the user defines a set of load steps in (time) sequence. FRANC3D computes the SIFs for each load step and computes an increment of crack growth, both extension and direction. The resulting vector sum of all the increments for all load steps gives the total crack growth for one instance of the transient series Spectrum Loading for Manu Model The Manu experiment load spectrum can be read into FRANC3D and used to compute cycles. The load schedule in the Fatigue Life dialog is set to Spectrum instead of Simple Cyclic, Fig After selecting Accept, the Select a load spectrum button in the Load Schedule dialog, Fig 7.21 right panel, can be selected to read the Manu load spectrum data from the file, called avg.txt. The spectrum file is ASCII text with lines of: max min count where max and min are load factors and count is the number of cycles in the block. The spectrum is shown in Fig Note the max and min can be reversed in the file. 197

198 Figure 7.21: Fatigue Life Load Schedule dialog with Spectrum selected. 198

199 Figure 7.22: Variable amplitude load spectrum for Manu avg.txt. The number of cycles computed by FRANC3D is 297,875, which is relatively close to the number of cycles in the experiment, Fig The spectrum in avg.txt is not the exact load spectrum as the data has been averaged to simplify it somewhat. The Paris crack growth model and data were not changed. If we used the NASGRO model that was used by Barlow (2008), we might improve our prediction. Figure 7.23: Fatigue Life dialog using Manu average spectrum. 199

200 8.0 Tutorial 7: Fretting Fatigue In Tutorial 7, we describe the Fretting Fatigue module by presenting an example simulation, using an ABAQUS finite element model of a fretting test rig, Fig 8.1. Figure 8.1: Fretting test rig (from: Golden, IJF, 31, 2009). 8.1 Step 1: Saving ABAQUS Data The ABAQUS model is shown in Fig 8.2. Using symmetry, only one quarter of the actual model is required. There are two load steps applied; the deformed shapes for both steps are shown in Fig 8.3. The specimen is pulled downward and then partially unloaded; the load ratio (R) is 0.1. There is contact between the specimen and the fretting pad; the coefficient of friction is

201 Figure 8.2 ABAQUS model of fretting test rig. Figure 8.3 Fretting test rig deformed shape for load step #1 (left) and #2 (right). 201

202 Results can be written to the.fil file by adding the following commands to the ABAQUS inp file or using the ABAQUS CAE Edit Model Keywords option: *File Format, ASCII *Node File, Frequency=1 U *El File, position=averaged at nodes, Frequency=1 S,E *Contact File, Frequency=1 CDISP, CSTRESS This set of commands is repeated for the second load step, minus the *File Format, ASCII line. These lines can be added just before the *End Step command. An additional change should be made in ABAQUS CAE to flatten the.inp file and.fil files, removing *Part, *Instance and *Assembly data: >>> mdb.models["fretting_rig"].setvalues(nopartsinputfile=on) This eliminates any confusion with node and element numbering. 8.2 Step 2: Fretting Model Import Start FRANC3D and from the main menu, choose Fretting and Read model and results, Fig 8.4. You are prompted to select the model file; in this case, we choose the fretting_rig.inp file, Fig 8.5; the default file type is ANSYS, so we must switch the File Filter to ABAQUS to display the.inp file(s). You are then prompted to select the results files, Fig 9.6. In this case, we have two load steps corresponding to Qmax and Qmin conditions. The.fil contains results for each load step. Select the fretting_rig.fil file for both conditions; FRANC3D requests that you specify which load step results will be used for each case, Fig 9.6. Select Finish to proceed to the next step, where we will specify the contact surface(s) where fretting is to be evaluated. 202

203 Figure 8.4 FRANC3D menu selection for fretting analysis. Figure 8.5 FRANC3D mesh model file selector for fretting module. Figure 8.6 FRANC3D results file selector for fretting module; left-side dialog is displayed if there are multiple load steps in the.fil file. The next dialog, Fig 8.7, allows you to select the contact surface. The contact-pair surfaces are listed on the left and colored blue in the model. Select the contact-pair by checking the box 203

204 beside the name, Figure 8.8. Select Finish and the model will be displayed in the FRANC3D main window; the material regions will have different colors, Fig 8.9. Figure 8.7 Fretting model data filter auto selected contact surfaces. Figure 8.8 Fretting model data filter to select master and slave contact surface nodes. 204

205 Figure 8.9 Fretting test rig model displayed in FRANC3D. 8.3 Step 3: Fretting Crack Nucleation The next step is to compute the fretting nucleation parameters. From the FRANC3D Fretting menu, select Fretting crack nucleation, Fig There are five fretting nucleation models available. The models have been described in the literature; they use some or all of the results data that was read earlier to compute a fretting nucleation parameter. The computed fretting parameter is then compared with empirical or test data to determine number of fretting cycles to discrete crack nucleation. Figure 8.10 Fretting crack nucleation menu option. 205

206 Figure 8.11 Fretting nucleation models. For this example, we choose the Critical Shear Stress nucleation model, and select Next (not shown). The next dialog, Fig 8.12, allows you to specify the model parameters used to compute the Seq value along with the number of cycles. FRANC3D computes the Seq values at nodes in the contact region and then computes number of cycles (Ni) based on the equation shown at the top of the dialog. 206

207 Figure 8.12 Equivalent stress fretting nucleation model parameters. Select Next to proceed to the final dialog, Fig 8.13, which allows you to display the contact surfaces, and color contours of fretting nucleation cycles or nucleation parameter, Fig The Equivalent Stress model requires several material dependent parameters. For this example, the material is Ti-6Al-4V, which corresponds with the default parameters in the dialog; these parameters were obtained from the literature. 207

208 Figure 8.13 Fretting nucleation display window. Figure 8.14 Seq contours on fretting specimen surface. 208

209 8.3 Step 3: Discrete Crack Nucleation Assuming that fretting fatigue causes crack nucleation, we will extract a submodel and insert a crack and run the analysis in this section. The first step is to close the fretting model; use File and Close. Next we import the model using File and Import; we choose to import and subdivide and select the fretting_rig.inp file, Fig Figure 8.15: Import the fretting rig model. The submodeler tool is displayed once the files are imported, Fig The first selection can be done using the By Element Group option; click the Select button and pick the dovetail_specimen set, Fig 9.16 left panel. Use the Crop button to remove the remainder of the model, Fig 9.16 right panel. Figure 8.16: Submodel selection based on group selection. 209

210 Next we use the rectangular Rubberband Box to select a smaller submodel, Fig Note that this submodel includes the entire contact surface region; this is important to remember when we are setting up the static analysis of the full model as we will have to redefine the contact by adding an extra connection. Figure 8.17: Submodel selection based on a Rubberband box. After extracting the appropriate submodel and saving the local and global ABAQUS.inp files, the dialog in Fig 8.18 is displayed. This allows us to retain the mesh facets where the boundary conditions are applied. In this case, we do not select these facets as the surface must be remeshed to accommodate the through crack that we are inserting. Just select Finish in this dialog, and the model will be displayed in the FRANC3D main model window. A shallow through (or edge) crack is inserted near the lower edge of contact at the location predicted by the fretting nucleation model(s). Fig 8.19 shows two views of such a crack. Note that for shallow cracks, it is a good idea to change the default meshing parameters when setting the crack front template. Fig 8.20 shows the meshing parameters dialog with Do Local Surface Refinement checked and Do Coarsen Crack Mouth Mesh unchecked. The resulting remeshed cracked submodel is shown in Fig

211 Figure 8.18: Select retained surfaces dialog do not select this surface. Figure 8.19: Through crack near the lower edge of contact. 211

212 Figure 8.20: Meshing parameters dialog. Figure 8.21: Cracked remeshed submodel. This portion of the model is combined with the global model and the analysis of this combined model is done using ABAQUS. The user controls the analysis step using the Static Analysis dialogs in FRANC3D, shown in Figs Note that the global model consists of linear brick elements and these must be tied to the quadratic elements from FRANC3D using *Tie 212

213 constraints, Fig An extra connection for the contact between the fretting pad and specimen is defined using surface to surface contact, Fig Figure 8.22: Static analysis dialog analysis code set to ABAQUS. Figure 8.23: Static analysis dialog ABAQUS options. 213

214 Figure 8.24: Static analysis dialog extra contact connection. Figure 8.25: Static analysis dialog local + global connection. The resulting contact surfaces are shown in Figure The analysis produces results as shown in Figure 8.27, which shows the deformed shape, and 8.28, which shows the Mode I SIFs for the first load step. 214

215 Figure 8.26: Newly defined contact surfaces. Figure 8.27: Deformed shape after analysis 500x magnification. 215

216 Figure 8.28: Mode SIFs for first load step. 9.0 Tutorial 8: Session Log Playback In Tutorial 8, we describe the session log and its playback. When running the FRANC3D (GUI) program, a session log file is saved for (almost) every menu command that is executed. The session log file is a text file that can be edited, played back in the FRANC3D GUI, played back from the command line, and/or converted to a Python script that can be used with the FRANC3D Python module. The session log file number in the current working directory is incremented each time FRANC3D is started using that directory. As an example, the session log file for Tutorial #1 is given here: # session log for tutorial 1 Submodeler( model_type=abaqus, orig_file_name='abaqus_cube.cdb', submodel_file_name=' Abaqus _Cube_LOCAL.cdb', global_file_name=' Abaqus _Cube_GLOBAL.cdb', elem_file_name=' Abaqus _Cube_RETAINED_ELEMS.txt') 216

217 OpenMeshModel( model_type= ABAQUS, file_name=' Abaqus _Cube_LOCAL.cdb', global_name= Abaqus Cube_GLOBAL.cdb') InsertFileFlaw( file_name='cube_crack.crk') RunAnalysis( model_type=abaqus, file_name='abaqus_cube_sub.fdb', flags=[no_write_temp,transfer_bc,no_cface_tract,no_cface_cntct], merge_tol=0.0001, connection_type=merge, executable='abaqus.bat', command='"abaqus.bat" job=abaqus_cube_sub_full -interactive -analysis ', global_model='abaqus-cube_global.inp', merge_surf_labels=[auto_cut_surf], global_surf_labels=[global_connect_surf]) ComputeSif() SetGrowthParams( load_model=qs_exponential, kink_angle_strategy=mts, const_median_step=0.15) GrowCrack( load_model=qs_exponential, kink_angle_strategy=mts, const_median_step=0.15, temp_radius_type=absolute, temp_radius=0.1) SetGrowthParams( load_model=qs_exponential, kink_angle_strategy=mts, const_median_step=0.15) AutoGrowthAbaqus( cur_step=1, file_name='abaqus_cube_sub', load_model=qs_exponential, kink_angle_strategy=mts, const_median_step=0.15, num_steps=5, step_type=sconst, const_step_size=0.15, temp_radius_type=absolute, 217

218 temp_radius=0.1, flags=[no_write_temp,transfer_bc,no_cface_tract,no_cface_cntct], merge_tol=0.0001, connection_type=merge, executable='abaqus.bat', command='"abaqus.bat" job=abaqus_cube_sub_step_001_full -interactive -analysis ', global_model='abaqus-cube_global.inp', merge_surf_labels=[auto_cut_surf], global_surf_labels=[global_connect_surf]) WriteSifPath( file_name='cube_crack_sif_hist_p5.sif', load_step=1, flags=[tab,a,ki,kii,kiii,crd]) Start the FRANC3D GUI, and choose File and Playback. Using the file selector, Fig 9.1, choose the session log file and select Accept. FRANC3D will read the log file and process the commands; so in this case the ABAQUS cube model is subdivided, the crack is inserted and analyzed, and then propagated for five steps. Finally the SIF history is extracted and written to a file. A playback.log file is written that includes all of the commands and any FRANC3D messages. If something goes wrong, you should first open the playback log file, which is a text file, and look at the last command that was attempted. The playback.log should be written to the current working directory, but if that is not set, it might be saved to the folder where FRANC3D is located. Figure 9.1: Select session log file to play back in FRANC3D. 218

219 To run this in the background without the GUI, use a cmd or xterm window and execute franc3d from the command line as: franc3d batch session01.log 10.0 Tutorial 9: Python Interface In Tutorial 9, we briefly describe how to use the Python module. The Python module is designed to work with Python version 2.7.8; it should work with versions between and Python PyF3D Module The FRANC3D session log (see Tutorial 8) can be converted to Python using the Fcl2Py executable that is shipped with FRANC3D. This program takes one argument, which is the session (command) file name. It reads the commands from the file, converts them to equivalent Python script, and writes the information to stdout, which can be piped to a file. For example: C:/examples/Fcl2Py.exe session01.log > ses01.py The ses01.py file will be similar to: #!/usr/bin/python import sys sys.path.append("/home/bruce/franc3d_v7") import PyF3D f3d = PyF3D.F3DApp() # session log for tutorial 1 f3d.submodeler( model_type="abaqus", orig_file_name='cube.inp', submodel_file_name='cube_local.inp', global_file_name='cube_global.inp', 219

220 elem_file_name='cube_retained_elems.txt') f3d.openmeshmodel( model_type="abaqus", file_name='cube_local.inp', global_name='cube_global.inp') f3d.insertfileflaw( file_name='cube_02.crk') f3d.runanalysis( model_type="abaqus", file_name='cube_surf_v7.fdb', flags=["no_write_temp","transfer_bc","no_cface_tract","no_cface_cntct"], merge_tol=0.0001, connection_type="merge", executable='abaqus', command='abaqus job=cube_surf_v7_full -interactive -analysis ', global_model='cube_global.inp', merge_surf_labels=["auto_cut_surf"], global_surf_labels=["global_connect_surf ]) f3d.computesif() You can run this script from the command line: python ses01.py This assumes that Python (2.7.8) is in your PATH and that you are running from within the folder where the ses01.py and corresponding FE files exist Python Extension for User-defined Crack Growth FRANC3D allows you to define your own crack growth rules using the Python extensions. The full set of Python extensions is documented in the FRANC3D Commands & Python manual. Using the cube model from Tutorial #1, we briefly describe how to define Python extensions for crack growth. For this tutorial, we start from analyzed initial crack model (see Tutorial 1: Sec ). 220

221 Step 1: Read ABAQUS Cube Crack Model Start with the FRANC3D graphical user interface (see Fig 2.2) and select File and Open. Select the file name specified in Section 2.2, called Abaqus_Cube_crack.fdb. Select Accept. The model will be read into FRANC3D (along with the results files that were created when running the static analysis). Step 2: Read Python Extension Use the FRANC3D Advanced menu to select the Read User Extensions option, Fig The file selector dialog is displayed with a list of.py files. Select the user_python.py file, Fig This file will be described below. Figure 10.1: ABAQUS Cube Crack model Read User Extensions menu option. 221

222 Figure 10.2: ABAQUS Cube Crack model Read User Extensions menu option. The user_python.py file should be in the working directory. FRANC3D will read the file and display the list of functions that are included, Fig The functions can be turned on or off as needed. Select Accept when ready to continue. Figure 10.3: User Python functions available in the.py file. 222

223 Step 3: Grow Crack From the FRANC3D Cracks menu, select the Grow Crack option, Fig Use the default method to compute SIFs, Fig 10.5, and select Next. The User defined crack growth option will be selected in the Growth Type dialog, Fig You can save the growth parameters to a file if desired. The subsequent dialog, Fig 10.7, shows the computed new crack front points. The options in this dialog are similar to those in Section 2.7; the difference is the extension scale factor in the Crack Extension subpanel, which allows the relative extension to be adjusted without having to edit the Python functions and recomputing growth. Subsequent crack growth, remeshing and analysis is the same as for the built-in crack growth routines. Figure 10.4: Cracks Grow Crack menu option. Figure 10.5: Compute SIFs dialog. 223

224 Figure 10.6: Growth Type dialog with User-defined crack growth selected. Figure 10.7: Crack Growth dialog for user-defined growth. 224

225 10.3 Python Extension File The Python functions in the user_python.py file are listed here. See the Commands & Python manual for a description of these functions and a list of all the functions. import math # ===================================================================== # User defined crack extension function: # # This version computes an extension based on a temperature dependent # Paris model for a specified number of cycles. # ===================================================================== # # initialization function # def on_initialize(): global C_b, C_m, n, cycles C_b = C_m = 10.0 n = 3 cycles = return # # crack extension function # def on_extension(): global C_b, C_m, n, cycles C = C_m * GetTemp() + C_b dadn = C * GetK()[0]**n return dadn * cycles # ===================================================================== # User defined kink angle function: # # This version computes the Max Tensile Stress criterion 225

226 # for the sum of the K's from all load cases # ===================================================================== # # function to compute the hoop stress # def hoop_stress(theta,ksum): KIf = Ksum[0] * (math.cos(theta/2) * (1.0-math.sin(theta/2)**2)) KIIf = 0.75 * Ksum[1] * (math.sin(theta/2) + math.sin(3*theta/2)) return KIf - KIIf # # kink angle function # def on_kink_angle(): # compute the sum of the K's for all load steps (note # load steps are numbered from 1 to n Ksum = Vec3D(0,0,0) for i in xrange(numloadsteps()) : Ksum += GetK(i+1) # call the F3D builtin Maximize function to find the # angle where the hoop stress is maximum max_ang = Maximize(-math.pi/2,math.pi/2,hoop_stress,Ksum) return max_ang # ===================================================================== # User defined new point function: # # This version computes a new crack front point location # base on a max hoop stress angle criterion and an assumed # Paris like growth model # ===================================================================== # # new point function #

227 def on_new_point(): # compute the sum of the K's for all load steps (note # load steps are numbered from 1 to n Ksum = Vec3D(0,0,0) for i in xrange(numloadsteps()) : Ksum += GetK(i+1) # call the F3D builtin Maximize function to find the # angle where the hoop stress is maximum angle = Maximize(-math.pi/2,math.pi/2,hoop_stress,Ksum) # compute an exention based on a Paris like model extend = * Ksum[0]**3.2 return extend, angle 11.0 Tutorial 10: Fatigue with Time Dependent Growth This tutorial illustrates subcritical growth of a crack under combined cyclic load and time dependent crack growth. The model is shown in Figure Figure 11.1: DENT specimen. Two load steps are defined: 1. Tension: 17.4 MPa 2. Compression: MPa 227

228 Crack growth is assumed to take place under the loading sequence shown in Figure Kmax and Kdwell will be the stress intensity factors associated with load step 1, and Kmin will be the stress intensity factor associated with load step 2. Hold time, tdwell, is 20 min/cycle. Figure 11.2: A constant amplitude load sequence including hold times. The local crack extension for each load cycle will be determined from the expression: da dn tdwell m n C K A Kdwell dt 0 Kmax Kmin K Kmax if if Kmin Kmin 0 0 Parameters and constants for the crack growth analysis are: Paris C 4.e-11 Paris m 3 Hold time A 5e-18 Hold time n 5 tdwell 20 Kthreshold 1 Kc 10,000 with stress intensity factors in MPa*sqrt(mm), time in minutes, and da/dn in mm/cycle. Temperatures units are set to degrees C, but the temperature is constant and not used SubModel and Crack Insertion First, read the uncracked ABAQUS.inp file into FRANC3D and define a submodel. 228

229 Start FRANC3D and select Import from the File menu. We want the default type of import, which allows us divide the ABAQUS model into local and global models. Select Next. Select the.inp file (dent_uncracked.inp), and then select Next. The Define a Local Submodel dialog will appear, Fig Use the rectangular Rubberband Box to select the submodel, Crop the selection, and select Next. We save the local and global files using the default names; select Next. Figure 11.3: The Define a Local Submodel dialog local submodel selected. The Select Retained BC Surfaces dialog is shown next, Fig There are no boundary conditions applied to the submodel, so just select Finish. 229

230 Figure 11.4: The Select Retained BC Surfaces dialog. Use the Cracks and New Flaw Wizard menu option. Select the Crack (zero volume flaw) in the first panel, and then select the user mesh crack type in the second panel. An ABAQUS surface mesh was created to define the initial crack, Fig The crack front node set is defined by the red-nodes in Fig Figure 11.5: ABAQUS surface mesh with crack front node set. 230

231 Click the Read Mesh File button, Fig 11.6, and select the dent_cae_crack_wfront.inp file. The Select a Crack Front Group dialog displays the available node sets; pick the front set and Accept. Figure 11.6: User-mesh crack with front node set indicated. The crack needs to be positioned. The left panel of Fig 11.7 shows the location and rotation. The template mesh radius is set to Select Finish to insert the crack and remesh. The remeshed model is shown in Fig 11.8; the Mesh is turned on. Figure 11.7: Crack location and front template mesh. 231

232 Figure 11.8: The mesh after crack insertion Define Crack Growth Parameters The next step is to perform a crack growth analysis. Typically, we would run the initial crack using the Static Analysis option and then grow the crack manually to ensure that we have the growth model and parameters correct and consistent. For this tutorial, however, we skip immediately to automatic crack growth. Select Crack Growth Analysis from the Analysis menu. The first dialog shown is the Compute SIFs dialog. We use the default values, so select Next. The Growth Type dialog is shown next, Fig The default option, Subcritical crack growth, is used; select Next. 232

233 Figure 11.9: The Growth Type dialog. The next dialog allows you to select the algorithm used to predict a kink angle during crack growth (Figure 11.10). We use the defaults; select Next. Note that for most analyses, the default option, Max Tensile Stress, works well. This criterion predicts that the crack will grow perpendicular to the maximum local tensile stresses. When subjected to high levels of shear loading at the crack front (KII and KIII), some materials show a transition from tension dominated crack growth to shear dominated crack growth. The Max Shear Stress criterion predicts that the crack will grow in the direction where the shear stress is maximum. The Generalized Stress criterion computes both the tensile and shear stresses and predicts the direction of the greater. The Strain Energy Release Rate option predicts that the crack will grow in a direction that is a combination of tensile and shear stresses. The Planar option forces the crack growth to be planar. 233

234 Figure 11.10: The Kink Angle Model dialog. The Subcritical Growth Parameters dialog is displayed next, Fig The yellow warning triangles indicate that parameters need to be set before you can continue. Select the Change button on the right side of the FEM units to display the Units dialog box, Fig The SI units are MPa, mm, and C; time units are min. Note that FRANC3D needs to match the finite element (FE) model units with crack growth rate model units, which can be different. By explicitly specifying the units used for the FE model and for the growth model, FRANC3D can perform unit conversions automatically. 234

235 Figure 11.11: The Subcritical Growth Parameters Dialog. Figure 11.12: The Units dialog. 235

236 Load Schedule Next we define a load schedule. A load schedule does two main things. First, it defines a mapping from the load steps defined in the ABAQUS model to stress intensity factors used to predict crack growth rates. Second, it defines the sequence with which these loads will be applied to the model. Select the New Schedule button on the Subcritical Growth Parameters dialog to display the Load Schedule dialog, Fig Figure 11.13: The initial Load Schedule dialog. A load schedule is comprised of a collection of load events. Load events are organized in a treelike structure. The root of the tree is a Schedule event. Initially, the upper part of the dialog (Fig 11.13) shows one Schedule event, which is the tree root. Left-clicking on the root event does two things: 1) it makes the Add button active, and 2) it brings the Repeat tab to the front in the lower part of the dialog. 236

237 Select the Add button to display the Event Type dialog, Fig There are six different available event types: Simple Cyclic a simple K = Kmax Kmin cycle, where the Kmax and Kmin loadings are proportional, so Kmin = R*Kmax, and R is given by the analyst. Non-Proportional Cyclic a K = Kmax Kmin cycle, where the Kmax and Kmin loadings are not proportional (they come from different load steps), and R = Kmin/ Kmax is computed. Transient For a transient event, a list of analysis load steps, sub-steps (frames), or a combination are specified. FRANC3D will examine all of the associated K s, and select Kmax and Kmin from among these to define K = Kmax Kmin. Spectrum For a spectrum event, one or more load spectra are specified. A load spectrum is a list of load multipliers used to define a sequence of Kmax and Kmin values, which are used to define a sequence of K s. If multiple spectra are specified, they are superimposed. Hold Event The four load events defined above can include a hold (dwell) time. A hold event allows one to define a hold time without any companion load cycling. Schedule A schedule event can contain children events and allow a tree-like structure to be constructed. For this analysis, Kmax comes from load step 1 and Kmin comes from load step 2. Since these are two different load steps, a Non-Proportional Cyclic event should be selected. Select Accept after selecting this option. Figure 11.14: The select an event type dialog. 237

238 Once the event type is selected, the Load Schedule dialog is updated, Fig 11.15; the Load Steps tab is automatically selected. The yellow triangles indicate that the load steps associated with Kmax and Kmin must be specified. The Select a load step buttons bring up the dialog shown to the right in Fig Load step 1 is selected from the pull-down list of load steps for the Kmax load step. Set load step 2 for Kmin. There is only one sub-step (frame) for this step, so the Load Sub-Step option is unavailable. A load and temperature scaling factor can be defined. Note that the temperature multiplier does not account for coupling between the temperature and the stress intensity factors, so it should be used with care. The temperature offset can be used if the analysis was done using relative temperatures while the crack growth rate models assume thermometer temperatures. Figure 11.15: The Load Schedule dialog with a non-proportional cyclic load event added. The Select a load step button displays the dialog on the right. 238

239 Note that in Fig 11.15, the Sum Multiple Steps button allows Kmax and Kmin to be defined as the sum of the K s associated with two or more load steps (each with its own load multiplier). The updated Load Schedule dialog after selecting the load steps is shown in Figure Figure The Load Schedule dialog after load steps have been selected. In this model, temperature is not assigned. The specified crack growth rate equation is not temperature dependent either. However, we describe the settings for a temperature dependent model here for illustration. The Load Schedule dialog with the Temperature tab selected is shown in Fig 11.17, with Temperature dependent crack growth checked. 239

240 Figure The temperature tab of the load schedule dialog. Because predicting crack growth might involve a number of different finite element load steps, each of which can have associated temperatures, it is not obvious what temperature to use when evaluating a temperature dependent growth model. FRANC3D provides the following options: Constant a constant temperature, provided by the user, is assumed for all crack front nodes and is used for evaluating temperature dependent growth models. Kmin the crack-front temperatures associated with the load step used for determining Kmin is used when evaluating growth models. Kmax the crack-front temperatures associated with the load step used for determining Kmax is used when evaluating growth models. Khold the crack-front temperatures associated with the load step used for determining Khold is used when evaluating growth models. 240

241 External the crack-front temperatures are read from an independent set of analysis results. This will be a mesh file (e.g..inp file) and the associated results file (e.g..odb or.dtp file). Interpolate the crack front temperatures will be linearly interpolated between the Kmin and Kmax temperatures using a user provided parameter that can vary between zero and one, where zero is the Kmin temperature and one is the Kmax temperature. Note that if Kmin, Kmax, or Khold are specified to be computed from the sum of multiple load steps, only temperatures from the first load step specified in the list of steps will be used to determine crack-front temperatures. You can uncheck the Temperature dependent crack growth option, Fig The analysis includes a hold (dwell) time for each load cycle. Simple Cyclic, Non-Proportional Cyclic, Transient, and Spectrum Load event types all allow a hold time. A hold time can also be specified as an independent Hold event. In this analysis, it does not matter which option is used to define the hold time. Note that one might consider separate cyclic and hold events if, for example, the cyclic growth rate and hold growth rates were to be computed for different temperatures. FRANC3D will compute the crack extension for all the cyclic loading in an event before computing the extension due to a hold time. If it is desired to have the time dependent growth computed first, that should be done with a hold event that appears before the cyclic event in the load schedule. For this example, the hold time is added as part of the Non-Proportional Cyclic event. Fig shows the Load Schedule dialog after the Time tab has been selected, the hold time of 20 min has been entered, and the load step associated with the hold (step 1 in this case) has been selected. 241

242 Figure The load schedule dialog with the Time tab selected. The Hold FOREVER option makes the hold time infinitely long. This could be used, for example, if one wanted to simulate time dependent crack growth (e.g., stress corrosion cracking) and keep the crack growth simulation going until a critical stress intensity factor was reached. The Static tab is not used in this analysis. It allows the analyst to specify that the K from a load step (or sum of load steps) is to be added to both Kmax and Kmin. This will not change the K, but it will change the stress ratio, R, for crack growth models sensitive to R. This could be, for example, in situations where there is a steady fixed load, and an alternating cyclic load. The static load can be defined as a crack face traction, with stresses read from external analyses results (e.g.,.inp and.odb files). 242

243 By default, a load event (load cycle, hold time, or combination) will be applied once. The Repeat tab allows the analyst to specify that the load event should be applied some finite number of times. It also allows one to specify that the event will be repeated FOREVER. All load events must be the child of a Schedule event. When the repeat count is set for a Schedule event, all the child events are repeated for the specified number of times. By organizing the events into a tree like structure and setting repeat counts for the Schedule and loading events, arbitrarily complex load sequences can be defined. These options, along with options set for the crack growth rate model, will determine when FRANC3D will stop a crack growth simulation. Crack growth will always stop if the Kmax at any point on a crack front reaches a critical value. It will also stop if the K for all points on the crack front fall below a threshold K. In addition, if none of the load event events in the load schedule is set to repeat FOREVER, FRANC3D will make one complete pass through the load schedule and then stop the crack growth. If a FOREVER repeat is specified, FRANC3D will continue to apply the corresponding load event (sequence of children events in the case of a Schedule event) until one of the stopping criteria from the crack growth rate model is reached. For this example, the load sequence is to be applied FOREVER, this could be specified either in the Non-Proportional Cyclic event or in the root Schedule event. In such a case, it would be preferential to specify repeat FOREVER for the root Schedule event. This will allow FRANC3D to more easily determine if an accelerated cycle counting algorithm can be used when computing a fatigue life. As shown in Figure 11.19, left-click on the root Schedule event in the upper part of the dialog, and select Repeat FOREVER in the lower part. 243

244 Figure 11.19: Load schedule dialog with Repeat FOREVER selected for the whole schedule. The load schedule is complete, so select Accept Crack Growth Rate Model The Subcritical Growth Parameters dialog (see Fig 11.10) requires that you set a Crack Growth Rate Model. Select the New Model button to display the dialog shown in Fig For this analysis, we want to define both a cyclic loading and a time dependent rate model, so check both options. Figure 11.20: The growth model types dialog. 244

245 Select Next to display the Cyclic Loading Growth Model dialog, Fig FRANC3D supports two general types of cyclic growth models, pared models and inclusive models. The difference between them is how stress ratio effects are incorporated. For a paired model, the shape of the crack growth rate curve (Paris, Sigmoidal, etc.) is selected independently from the stress ratio algorithm (Walker, Newman Closure, etc.). The inclusive models (two different versions of the NASGRO equation) have stress ratio effects built-in. Figure The cyclic loading growth model. For this analysis, the Paris crack growth rate model is selected, with no stress ratio effects. Select Next. The next dialog allows you specify either a temperature dependent or independent model, Fig For this analysis, the growth rate model is temperature independent. This means that only one set of growth rate parameters (C and m for the Paris model) are required. For temperature dependent models, different sets of growth model parameters are specified for different temperatures, and FRANC3D interpolates among these values to find the appropriate growth rate for the crack-front temperature. Select Next. 245

246 Figure The temperature independent model selected. The dialog shown in Fig is displayed. The Model Label, and Description fields are optional. These might be useful if the model parameters are stored in a file for later reuse. The units must be specified. The units need not be the same units use in the finite element analysis. If the units are different, FRANC3D will automatically perform the necessary unit conversions. However, FRANC3D assumes that the units used within the growth model description (or within the finite element analysis) are self-consistent. For this model, we use the same units for the growth rate model as for the FE model. The Paris parameters are entered by selecting the fields and typing in the data. Figure The dialog for entering the cycling loading growth model parameters. 246

247 Note that FRANC3D labels the exponent for the Paris model as n. In addition to C and n, FRANC3D requires that values be entered for Kthreshold and Kc. Specifying a very small value for Kthreshold or a very large value for Kc will effectively turn off the possibility that the crack growth simulation will be stopped due to a below-threshold or above-critical condition. After selecting Next, the dialog to select a time dependent growth model, Figure is displayed. For this analysis, a Power Law model is used. Figure Dialog to select a time dependent growth model type. After selecting Next, the dialog to select a temperature dependent or a temperature independent growth model, Fig 11.25, is displayed. In this case a temperature independent model will be used. Figure 11.25: Dialog to specify a temperature dependent or independent growth model. The dialog to specify the power law time dependent growth model parameters is shown in Fig Again, as for cyclic loading, Units must be specified. For time dependent rates, the 247

248 threshold (Kth) is an actual K value rather than a K value. If Khold is below this value for any crack front point, there will be no time dependent crack extension for that point. Select Finish to return to the Subcritical Growth Parameters dialog, Fig Figure 11.26: Dialog box for entering time dependent power law growth model parameters Effective dk and Integration The lower half of the Subcritical Growth Parameters dialog, Fig 11.27, is described next. 248

249 Figure 11.27: Subcritical Growth dialog completed. There are two options for how K is computed. The default behavior is to simply compute K = Kmax Kmin. In cases where minimum loading at the crack front is actually compressive (and contact elements are not explicitly inserted into the crack faces to prevent crack overlap) the computed Kmin, and corresponding stress ratio (R) will be negative. Such crack face overlap is physically unrealistic, but it is common practice to accept the negative values, and meaningful engineering predictions can be performed with these values provided the appropriate parameters are used with the growth rate and/or stress ratio models. Optionally, FRANC3D can be instructed to compute a more physically realistic K that only considers portions of a load cycle where the K s are positive. That is: 249

250 Kmax Kmin K Kmax if if Kmin Kmin 0 0 This option is selected for this analysis. The dialog box, Fig 11.27, also includes two options that affect how the crack growth integrations are performed when computing total life. If the Accelerated counting option is selected (the default), FRANC3D will try to use an accelerated cycle counting algorithm based on Runga-Kutta integration. If this option is turned off, FRANC3D will perform cycle-by-cycle counting. The accelerated counting might be slightly less accurate than cycle-by-cycle counting, but usually the difference in the computed fatigue lives for the two methods is less than 1-2% of the total cycle count. On the other hand, for analyses where the per cycle crack extension is small, for some models the accelerated counting has been shown to give greater than 1000x reductions in the time required to compute total fatigue lives. The Constant K for time integration option can be set to speed-up the integration of time dependent growth. In general, the stress intensity factor will be function of time, so FRANC3D evaluates the integral: t m a A K hold ( ) d 0 where t is the hold time. The integral is evaluated using Runge-Kutta integration. If, however, the crack growth over a hold interval is small, K can be assumed to be constant during the interval leading to the (much faster to evaluate) expression: a A K m hold t If this option is selected, FRANC3D will assume that K is constant over all time intervals. Select Next (Fig 11.27) to display the dialog shown in Fig You can save the parameters to a file. If a file is saved, it can be read with the Read growth parameters from file option in the dialog shown in Fig

251 Figure 11.28: Save growth parameters to file option Crack Growth Analysis The next dialog box (Fig 11.29) has three parts. The upper section allows the analyst to select the method used to fit an analytical curve through a collection of predicted new crack front points. The fitting serves two purposes. First, it tends to smooth out numerical noise in the predicted new crack front point positions. More importantly, the curve is extrapolated to find the exact locations where new crack fronts intersect free surfaces. The middle part of the dialog allows the analyst to modify parameters regarding crack front templates and other meshing related options. FRANC3D determines the default crack-front template radius from the initial crack size. We will set the template radius to use an absolute value of The lower part of the dialog selects how the amount of crack extension for each crack growth step will be specified. The default option is to specify the amount of crack extension for the point on the crack front that has the median predicted crack growth rate. This is the recommended option. The other two options are to specify either a fixed number of cyclic loads or a fixed amount of elapsed time. While these options are intuitive from an engineering perspective, the relationship between crack extension amount and either a cycle count or elapsed time can be highly nonlinear with respect to the crack size. Unless these values are highly tuned, one often has a situation within one analysis where the predicted crack growth steps are extremely small for small cracks and extremely large for big cracks. 251

252 Figure 11.29: Fitting and template parameters dialog. The upper part of the next dialog (Fig 11.30) allows the analyst to set the criteria that will be checked for stopping a crack growth simulation. The analysis will stop when the first of these conditions is reached. The first three criteria will always be checked and cannot be turned off. The first says that if the load schedule does not contain any load events with the repeat count set to FOREVER, FRANC3D will take one pass through the load schedule and stop (note that multiple crack growth steps might be required for a full pass through the schedule). The second says that crack growth will stop when Kmax for any point on a crack front reaches a critical value. The third says that crack growth will stop if the K (cyclic) and/or Kmin (time dependent) for all crack front points fall below their respective threshold values. 252

253 Other criteria for stopping are shown in the dialog. With respect to the maximum crack depth, defining a crack depth for an arbitrarily shaped crack can be very ambiguous. The current algorithm that FRANC3D uses to determine a crack depth is not very robust, and might give surprising results, so it should be used with caution. Figure 11.30: Growth termination and step size dialog. The lower part of this dialog allows you to specify the nominal crack step increment. For this analysis we will use a constant crack increment for each crack growth step. FRANC3D determines this value from the initial crack size, so the suggested size might be poor. We set it to 0.05 for this model. The following three dialogs (Figures ) allow you to select an analysis program, set the base file name for the crack growth models, and set analysis code specific options. Much of this information can be set in the Preferences and will not need to be changed. 253

254 Figure 11.31: Select an analysis code and base file name. Figure 11.32: Analysis Code options. 254

255 Figure 11.33: Options for joining the global and sub-models Life Prediction After sufficient crack growth has been completed, you can examine the SIF history and compute fatigue life. Use the Cracks and SIFs Along a Path menu to display the SIF history, Fig Figure 11.34: SIF history. 255

256 Use the Fatigue and Fatigue Life Predictions menu option to display the Fatigue Life dialog, Fig The number of load cycles and total time are displayed at the bottom right. Crack growth will continue beyond what is shown here. Figure 11.35: Fatigue life. 256

257 Appendix A: ABAQUS local model between *Tie constraints This tutorial describes how one can use an already-divided ABAQUS model, where the local portion is tied to the global portion using *TIE constraints. Figure A1 shows the complete model of a simple hinge. The local portion that will be extracted and imported into FRANC3D is contained between the two *TIE surfaces. This complete model can be copied to a local and global model and the appropriate portions of the model saved as separate.inp files. In this example, the files are named: hinge-global.inp and hinge-local.inp. Once these two files are saved, we can proceed to FRANC3D. Figure A1. ABAQUS hinge model; local portion is contained between two *TIE surfaces. 257

258 From the FRANC3D File menu, select Import. The first dialog is shown in Figure A2; select the Import an already divided model option and click Next. The second dialog, Figure A3, allows one to choose the global and local inp files. Make sure the ABAQUS Mesh File Type is selected and then use the Browse button to specify the two files. Once the hinge-global and hinge-local.inp files are selected, click Next. Figure A2. Select type of import dialog. Figure A3. Specify inp files dialog for an already-divided model. The next dialog, Figure A4, allows one to retain mesh facets. There are no boundary conditions, but we will retain the *TIE surfaces. Click on the Show Surfaces button and check the tie-local surface. Note that the tie-local surface was defined in ABAQUS CAE and is part of the local portion. There is a corresponding tie-global surface for the global portion. Click Finish to proceed to the FRANC3D main window, Figure A5. 258

259 Figure A4. Select retained surfaces dialog; the *TIE constraint surfaces are selected. Figure A5. FRANC3D local model imported with the *TIE surface mesh retained. The next step is to define and insert a crack. We have defined and saved a crack to a file previously, so we use the Cracks menu and choose Flaws from Files. Figure A6 shows the dialog box that allows us to choose the hinge.crk file. Once the file is selected, click Accept. Figure A7 shows the crack location in the local portion; we can move it if needed. The crack is a 259

260 center-through type crack with two crack fronts. Click Next to advance to the crack front template mesh settings, Figure A8. The template radius is saved with the.crk file as 0.1; we leave all the settings at their default values and click Finish to insert the crack and remesh. The remeshed configuration is shown in Figure A9. Figure A6. Dialog to choose the.crk file. 260

261 Figure A7. Crack location dialog. Figure A8. Crack front template mesh settings dialog. 261

262 Figure A9. Remeshed cracked local portion. Once the crack is inserted and the model is remeshed, we can perform a static analysis. From the Analysis menu, select Static Crack Analysis; the first dialog, Figure A10, allows us to specify the file name. We call it hinge_crack. Click Next and check that the solver is ABAQUS, Figure A11. Click Next to set the ABAQUS solver options and to specify the global file name. Figure A12. Figure A10. Static analysis file name dialog. 262

263 Figure A11. Specify the solver as ABAQUS. Figure A12. Specify the ABQUS analysis options. 263

264 The Global model file name is already filled in by default based on the imported file selection. Click Next to advance to the next dialog, Figure A13, where we specify how the local and global model portions will be re-connected. The tie-local and tie-global surfaces must be selected along with the Tie constraint option. Click Finish to start the process of saving all of the analysis files and running ABAQUS in the background. Once ABAQUS finishes running, we can compute the SIFs and analyze the results to verify that FRANC3D correctly processed all the ABAQUS information. Once ABAQUS finishes running, a.dtp file is created, and this file is automatically imported into FRANC3D. (This assumes that you are running ABAQUS on the same PC as FRANC3D.) Use the Cracks menu and select Compute SIFs; the dialog shown in Figure A14 is displayed. Click Finish to display the SIFs for the two crack fronts, Figure A15. Figure A13. Specify the ABQUS local + global model connection. 264

265 Figure A14. Compute SIFs dialog. Figure A15. Display SIFs dialog. The SIFs indicate that the hinge is bending, which is what we expect. The deformed shape for the uncracked hinge is shown in Figure A16. The contours show the displacement magnitude. Figure A17 shows the same displacement magnitude contours for the cracked hinge model. Even with the crack, the contours are essentially identical. Figure A18 shows a close up of the crack mouth; the displacement scaling is 10x and the contours show the maximum principal stress. 265

266 Figure A16. Displacement magnitude contours for the uncracked hinge. Figure A17. Displacement magnitude contours for the cracked hinge. 266

267 Figure A18. Maximum principal stress contours for the cracked hinge. Appendix B: ABAQUS model with *Tied meshes This tutorial describes how one can simulate crack growth in models with mixed meshes with *Tie constraints. Figure B1 shows a simple cube model with a shell surface attached to the cube. The cube has two components with a coarse mesh and a small section with a more refined mesh. The two components are connected by *Tie constraints, as the meshes on the two adjacent surfaces do not match. 267

268 Figure B1. ABAQUS model with mixed meshes and *Tie constraints. From the FRANC3D File menu, select Import. In the first dialog, the import and divide option is the default, so just click Next. Select the.inp file and click Accept to display the dialog shown in Figure B2. The shell elements will be displayed but cannot be selected; these elements will be part of the global inp file. The local model should be selected so that the *Tie surface between the mismatched mesh surfaces stays with the global portion also. Figure B2 show the local portion highlighted; a layer of elements from the refined mesh is not selected. 268

269 Figure B2. ABAQUS model with local FRANC3D portion highlighted. The local portion will be displayed in the subsequent dialog, Figure B3. AUTO_CUT_SURF is created by FRANC3D to define the cut-surface. The mesh facets for this will be retained by default. Click Finish to proceed to the main FRANC3D window; the resulting local model should appear as in Figure B4. A surface elliptical crack is defined and inserted into the local model, Figure B5. Once this crack is inserted and remeshing is completed, the model can be analyzed. The local is reconnected with the global portion. We left the existing *Tie surface between the mismatched meshes in the global portion so we do not have to worry about that. The original mesh was composed of linear brick elements and the remeshed crack portion consists of second order bricks, wedges, pyramids (or collapsed bricks if pyramids are not supported and tetrahedral. Consequently, the local cracked portion is connected to the global using additional *Tie constraints, Figure B6. The AUTO_CUT_SURF and GLOBAL_CONNECT_SURF are defined by FRANC3D and these are selected automatically along with the *Tie radio button. 269

270 Figure B3. Local model portion. Figure B4. Local model with retained mesh facets on the cut-surface. 270

271 Figure B5. Elliptical surface crack inserted into the local model. Figure B6. Local + global model connection. 271

272 The resulting Mode I SIFs for the crack are shown in Figure B7. The displacement magnitude contours for the original uncracked and the cracked model are shown in Figures B8 and B9. The results match reasonably well. Figure B7. Initial crack Mode I SIFs. Figure B8. Uncracked model displacement contours. 272

273 Figure B9. Cracked model displacement contours. Appendix C: Crack growth around and through corners This tutorial briefly describes simulation of crack growth around and through a corner. A simple T-shaped ABAQUS model is shown in Figure C1. The model is constrained on the back (-z) side and a fixed displacement is applied to the front (+z) side. The dimensions, properties and displacement values are not important as this example is designed to just give guidelines on the crack growth procedures. 273

274 Figure C1. T-shape model. The ABAQUS model is imported into FRANC3D and divided into local and global portions the local portion is highlighted in Figure C2. An initial penny-shape crack (Figure C3) is inserted into the model to create an initial corner quarter-circular crack. The cracked and remeshed local portion is recombined with the global portion and analyzed in ABAQUS. The resulting Mode I SIF is shown in Figure C4 (the values and units are not important). To simplify the crack growth process, planar crack growth is used with a quasi-static growth rule with a median crack growth step of 0.1. Automatic crack growth is then started, specifying 40 additional steps of growth. The default crack front fitting options fixed 3 rd order polynomial are used throughout. The automatic growth stops at step #21 with a fitting error. 274

275 Figure C2. T-shape model with local FRANC3D portion highlighted. Figure C3. Initial corner crack. 275

276 Figure C4. Mode I SIFs for the initial corner crack. The crack front at step #21 is shown in Figure C5. Note that the default fitting options require excessive extrapolation at this stage to ensure that the curve intersects the model surface. If the fitting option fails to produce a good fit during automatic crack growth growth will stop and a message will be displayed indicating that the fitting failed. To improve the fit, we switch to a moving-polynomial with order=1 and cut down the extrapolation (Figure C6). The moving polynomial is a useful option but it should be used with care as it will tend to capture numerical noise in the SIFs (predicted points) and can lead to ever increasing oscillations in the predicted fronts. The crack is manually propagated to step #22 and analyzed. One more step of manual crack growth is performed at this stage to revise the fitting options again; Figure C7 shows the front fitted with a 2 nd order polynomial with just enough extrapolation to ensure that the ends of the curve are outside of the model. Note that the shallow intersection angle requires that we use simple intersections for the crack front template (Figure C8). To ensure that there are enough predicted new front points near the 276

277 ends of the crack front, the template radius must be reasonably small (Figure C9). Note that SIFs are computed at the mid-side nodes of the regular wedge (and brick) elements. The combination of numerical noise in the SIFs and simple intersections can cause problems with predicting good points for the next crack front. To prevent additional numerical noise, the fitting options can be simplified to produce reasonable crack front shapes as the crack grows. Automatic crack growth using a fixed polynomial of 2 nd order is set for an additional 20 steps with a median increment of Figure C5. Crack growth at step #

278 Figure C6. Crack growth at step #21 with revised fitting options. Figure C7. Crack growth at step #22 with a 2 nd order poly. 278

279 Figure C8. Crack growth at step #22 showing crack front template with simple intersections turned on. Figure C9. Crack front mesh at step #23 simple intersections turned on. 279

280 The automatic crack growth continues from step #23 to #29. It fails to grow further because step #29 is not good; the crack front reaches the corner of the T-shape (Figure C10), but it does not adequately break through the corner. FRANC3D needs to ensure that the crack surface geometry, the crack front template geometry, and the model geometry intersect and create water-tight regions that can be meshed. Step #29 leads to subsequent errors on the next step of growth due to some current limitations in breaking the crack surface geometry to get two crack fronts instead of one front. To continue crack growth, step #28 is read into FRANC3D and the crack is regrown with a larger median increment (0.25 instead of 0.125). This produces the crack shown in Figure C11. The crack front has clearly broken through the corner. There is enough geometry outside of the model corner to allow FRANC3D to clearly separate the crack fronts. From step #29, automatic crack growth can be continued using the prior increment of and a 2 nd order polynomial fit. The automatic growth will continue until the crack front reaches the top of the T shape. Depending on the increment the growth might stop or it might cut through completely so that there is only a single front again (Figure C12). Crack growth might stop prior to cutting through the top of the T if the model cannot be meshed because the template is too close to the top surface. If it stops, restart from the previous step and take a bigger step of growth. 280

281 Figure C10. Crack front at step #29. Figure C11. Revised crack front at step #

282 Figure C12. Crack shape at step #36. The crack should always cut through cleanly. The View Response dialog (Figure C13) can be used to quickly verify that the deformed mesh is correct. Figure C13. Crack shape at step #