FRANC3D Workshop/Training

FRANC3D Workshop/Training
Corning Glass May 7, 2012 Drs. Paul “Wash” Wawrzynek, Bruce Carter, Tony Ingraffea, and Omar Ibrahim

Objectives General introduction to FRANC3D: - capabilities and limitations Present theory and approaches to computational fracture mechanics built into the program. Hands-on sessions give participants a chance to try the code with tutors here to help. Opportunity for participants to ask questions.

Agenda Introduction to FRANC3D Demo/Hands-on: build an uncracked model
Overview of the crack insertion process Demo/Hands-on: insert initial crack and run analysis Stress Intensity Factor (SIF) computation - theory Demo/Hands-on: SIF computation - practice Crack growth - theory Demo/Hands-on: Crack growth - practice Demo/Hands-on: Student generated models

FRANC3D Product FRANC3D (FRacture ANalysis Code 3-D) uses finite element method to simulate crack growth analysis Adaptively remeshes a finite element model to simulate crack growth. Has several elements to be used for modeling the crack front 4

FRANC3D Product Designed to work in conjunction with a commercial finite element solvers: ANSYS ABAQUS NASTRAN The FRANC3D program has a programming interface that is an extension to the Python programming language. Written in the C++ programming language Support the following operating systems: Windows Linux 5

FRANC3D Development History
FRANC3D v1.0 BEM only 1994 to 2001 FRANC3D v2.0 BEM & Thin Shell FEM 2001 to 2005 FRANC3D v3.0 BEM & Thin Shell & Solid FEM (ANSYS) 2005 to 2009 FRANC3D v4.0 Solid FEM only (ANSYS, ABAQUS, NASTRAN) Completely new code written in C++ 2009 to 2010 FRANC3D v5.0 – Additional enhancements 2010 to 2011 FRANC3D v6.0 – Fretting Fatigue, Fatigue Life, Post-processing & other enhancements 2012 FRANC3D v7.0 is under development 6

FRANC3D Development History
Development of FRANC3D was funded by: USA Air Force USA Navy NASA Others 7

What Does FRANC3D Do? insert a flaw into an existing finite element mesh and remesh locally, using special crack-front elements. compute stress intensity factors (SIF’s) for all nodes along a crack front for isotropic and anisotropic materials. predict how a crack will grow (relative extension and angle) using engineering growth criteria, and will then extend the crack geometry and remesh locally.

What FRANC3D is NOT not a general finite element pre-processor or post-processor. External codes are required to build uncracked FE models and to visualize results (FRANC3D can display deformations). not a finite element analysis program. An external FE code is required (e.g., ANSYS or ABAQUS) to perform stress analysis. not a general purpose fatigue life prediction code, although some basic life prediction models are available. An external lifing code (e.g., AFGRO, NASGRO or DARWIN) can be used.

ANSYS/ABAQUS/NASTRAN ANSYS/ABAQUS/NASTRAN
FRANC3D Typical Work Flow ANSYS/ABAQUS/NASTRAN ANSYS/ABAQUS/NASTRAN Full 3D FE Model Stress Analysis portion to be cracked remainder of model Combine portions FRANC3D Insert crack(s) into portion of model and remesh Define crack(s) geometry displacements, temperatures, crack surface tractions Compute stress intensity factors Extend crack(s) geometry 10

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

FRANC3D Modifies the Sub-model
uncracked model after crack insertion FRANC3D FRANC3D modifies the sub-model, inserting a crack and remeshing the model locally. It outputs an input file that combines the global and sub-model (ABAQUS) or it outputs the sub-model and a macro command file that will combine the models (ANSYS).

FRANC3D Maintains Compatibility
mesh compatibility FRANC3D can retain surface meshes on “cut” surfaces so that there is FE compatibility between the global and sub-model. This is the preferred approach. However, FRANC3D can also instruct the FE program to insert constraint equations.

Combined (Full Model) Analysis
FRANC3D does not use a global/local approach. The FE analysis is performed with the full combined model. (However, a global/local approach can be used.)

after 21 steps of crack growth
Crack growth is simulated by FRANC3D repeatedly reading and modifying the initial sub-model. At each step, the global and modified sub-model are re-combined and the full model is analyzed.

Sub-models for “free” meshes
“free mesh” cut surfaces It is possible to cut out a FRANC3D sub-model from a “free” (unstructured) mesh. (However, surface facets of tetrahedral elements with poor aspect ratios can cause local meshing problems.)

FRANC3D Tutorials Using ANSYS: Using ABAQUS:
simple global model vs sub-model with global model through-crack extract sub-model automated crack growth crack insertion & automated growth crack face traction vs far-field loading crack face traction vs far-field loading

FRANC3D Tutorials Step 1: Build the FE model
Step 2: Extract small portion from the full FE model Step 2.1: Separate element components Separate the FE model into a small portion (local model) and the remaining of the FE model (global model) Local FE model will be used for fracture analysis Local Model Global Model

FRANC3D Tutorials Step 2.2: Create node component for cut-surface
Select the nodes on the cut surfaces of each component and save a node component. For the 3x3x3 ‘local’ model, name this node component CUT_SURF. Step 2.3: Save local and global Archive each element component as a separate model for the local and other for global Global model, which consists of the exterior elements, will include the boundary conditions and material properties Local model will include the CUT_SURF node component and FRANC3D will use this information to retain those mesh facets

FRANC3D Tutorials Step 3: Read the local FE model into FRANC3D
Step 3.1: Reading Local FE Model Start with the FRANC3D graphical user interface Select File and Open Switch File Filter in the Open Model File dialog box to proper file extension name and select the file name for the local model Click Accept.

FRANC3D Tutorials Step 3.2: Selecting the Retained Items in the Local FE Model Material, mesh facet groups, contact/constraint & residual stress

FRANC3D Tutorials Step 3.3: Selecting Cut Surface Nodes
Lists the node components present in the local FE model file

FRANC3D Tutorials Step 3.4: Importing and Displaying the Local FE Model User can turn on the surface mesh and manipulate the view

FRANC3D Wizard for Defining the Crack Type and Meshing Process for the Cracked Portion of the FE Model 26

Current Crack Type Options in FRANC3D
Elliptical Crack Through-the-thickness One crack front Two crack fronts Long-shallow surface crack shape Elliptical crack shape with two fronts User-defined crack

Defining Crack Geometry
Crack geometry and location can be prescribed either by: Interactively using the Graphical User Interface (GUI) Using FRANC3D extensions to the Python programming language

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

Crack Insertion Wizard – Flaw Library

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

Surface Meshes after Crack Insertion
crack surface mesh

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

Crack Insertion: Input Sub-model Mesh
The first major input to the crack insertion procedure is a finite element mesh. Usually this is a sub-model, but a full model mesh is acceptable. In the case of a sub-model, the cut surfaces are flagged. sub-model cut surface cutting planes This model has brick elements only. However, brick, wedge, pyramid, and tetrahedral elements of both first and second order are okay. Currently, FRANC3D can handle ANSYS, ABAQUS and NASTRAN models.

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

Crack Insertion: Flaw Definition
The second major input to the crack insertion procedure is a description of a flaw shape and location. FRANC3D has tools to define and place a flaw interactively. Flaws can be zero volume (cracks) or finite volume (voids). The crack above appears to have a piecewise linear crack front, but that is a just a display artifact. Flaw surfaces are defined as Bezier patches and can have curved crack fronts. In theory, initial flaws can be non-planar, but there is currently no practical user-interface for such a capability.

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

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

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

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

Volume Meshing After completing the surface, the volume mesh starts
Options for performing volume meshing: FRANC3D ANSYS ABAQUS CAE Final mesh smoothing are used to improve the elements quality

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

Workshop Agenda Introduction to FRANC3D
Demo/Hands-on: build an uncracked model Overview of the crack insertion process Demo/Hands-on: insert initial crack and run analysis Stress Intensity Factor (SIF) computation - theory Demo/Hands-on: SIF computation - practice Crack growth - theory Demo/Hands-on: Crack growth - practice Demo/Hands-on: Student generated models

FRANC3D Tutorials – Crack Insertion Steps
Step 1: Selecting Cracks from FRANC3D Menu From the FRANC3D menu, select Cracks and New Flaw Wizard. The first panel of the wizard should appears. The default flaw type is Crack (zero volume flaw) and select Next.

Step 2: Selecting Crack Type The next panel allows the user to choose type of crack, hint Next after the selection.

Step 3: Specify the Crack Size The next panel allows us to specify the size of the ellipse. Select Next after the size definition.

Step 4: Specify Crack Location and Orientation The next panel allows us to specify location and orientation of the flaw. After defining the location and orientation; select Next.

Step 5: Specify Crack Front Template Parameters The next panel allows us to specify the crack front template parameters. After specifying the parameters; select Finish.

Step 6: Surface and Volume Meshing of Local Model after the Crack Insertion FRANC3D begins the process of inserting the flaw into the original model and then meshes the resulting cracked model. Operations is displayed on the screen When meshing is completed, the newly meshed cracked model will be displayed.

FRANC3D Tutorials – Static analysis Steps
Step 1: Select Static Crack Analysis From the FRANC3D menu, select Analysis and Static Crack Analysis. The first panel of the wizard should appear, specify the file name for the FRANC3D database first.

Step 2: Select FE Solver Next panel allows you to specify the solver

Step 3: Select Analysis Options Next panel allows you to specify the solver output and analysis options Specify global models Use all quadratic elements Solver executable should be defined

Step 4: Merging Local/Global FE Models Next panel allows for the specification of whether the local and global models are combined by merging nodes or by defining constraints or contact conditions. Specify node component names in the local and global models for nodes that will be merged or you can let the programs (FRANC3D and Solver) do the work. Select Finish

Stress Intensity Factors

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

Stress Intensity Factors
FRANC3D Computes the stress intensity factors associated with all three “modes” of fracture for the mid-side nodal points along the crack front Under conditions of small-scale yielding, all crack front displacement fields (crack behavior) are controlled by the stress intensity factors Stability – will the crack tip move? Trajectory – in what direction? Rate – how fast? 57

Computing Stress Intensity Factors
FRANC3D has two methods to compute stress intensity factors (SIF’s): Displacement Correlation: Relatively simple to understand and implement Relatively poor accuracy (~5% error for a reasonable mesh) Good sanity check but not for production work M-Integral (Interaction Integral): Somewhat involved formulation and implementation. In the literature, the M-Integral is sometimes known an "interaction integral”. Relatively good accuracy (<1% error for a reasonable mesh) Requires special additional terms for crack face tractions, residual stresses, FGM’s, etc.

Computing Stress Intensity Factors
M-Integral (Interaction Integral): Numerically the M-Integral is similar to the J-Integral. M-Integral is used to compute the strain energy release energy rates (GI, GII, and GIII) and stress intensity factors (KI, KII, and KIII) associated with the three modes of fracture. Mode II (KII) is needed to predict the crack kink angle to determine the crack front direction M-integral implementation in FRANC3D allows the computation of the three modes of SIFs for isotropic and anisotropic materials. FRANC3D is the only available code that will compute stress intensity factors for generally anisotropic materials The method to use for production work 59

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

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

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

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

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

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

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

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

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

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

We use the FEM results for the (1) solution KI KII KIII a 1.0 0.0 b c We select three simple auxiliary solutions (2a), (2b), and (2c) From the analytical expressions for the crack-front fields, we obtain Substitution gives three equations for the unknown K(1)’s

Independent FRANC3D Mode I SIF Verification
CCT SEN Analyses performed by Dawn Phillips of the NASA Langley Research Center

Independent FRANC3D Mode I & II SIF Verification
Analyses performed by Dawn Phillips of the NASA Langley Research Center Slant edge crack starting from a circular hole Mode I Mode II

Typical Isotropic M-Integral Verification
Stress intensity factors are computed at all nodes along the crack front Surface crack, a = c = 0.8, remote unit traction FRANC3D crack front The oscillations arise because different virtual crack extension are used for element corner and mid-side nodes. virtual crack extensions corner node mid-side node

Anisotropic Stress Intensity Factors
FRANC3D includes an M-Integral implementation for general anisotropic materials.1,2 1 Wawrzynek, P.A., Carter, B., and Banks-Sills, L. “The M-integral for computing stress intensity factors in generally anisotropic materials,” NASA/CR 2 Banks-Sills, L., Wawrzynek, P.A., Carter, B., Ingraffea, T.R., and Hershkovitz, I., “Methods for computing stress intensity factors in anisotropic geometries: Part II – arbitrary geometry,” Engng. Fracture Mech., in review

FRANC3D Tutorials – SIF Computation Steps
Step 1: Re-Open FRANC3D restart file From the FRANC3D menu, select File and Open. Choose the *.fdb file and select OK. FRANC3D will automatically read the FE solver results

Step 2: Select Compute SIFs From the FRANC3D menu, select Cracks and Compute SIFs. The Stress Intensity Factor wizard is displayed Use the M-Integral User can select thermal or crack face traction terms if they are used. Select Finish, the SIFs Plot dialog is displayed

Step 2 (cont’d): Select Compute SIFs View the three stress intensity factor (SIF) modes and export the data

Crack Growth

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

Crack Growth Prediction within FRANC3D
Computing crack front growth is a three-step process: Kink angle for each node (direction) Based on the crack-front stresses in polar coordinates Five options for computing kink angle Relative amount of local crack extension for each node Computed using a fatigue growth model (using one node extension with a median SIF or using a specify number of load cycles) Simplest model is Paris growth model Smooth the crack front Polynomial curves are used to fit the crack front User can specify the order of the polynomial or FRANC3D find the polynomial order that will give the best fit

after 21 steps of automatic crack growth
Confidential 83 83

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

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

time SIF ( K )

time SIF ( K ) load case a load case b

Kink Angle: Max Stress Criterion (isotropy)
The max stress criterion says that the crack will kink in the direction of a maximum value of a stress component. Some materials show a transition from Mode I to Mode II crack growth for stable tearing. -30 -20 -10 10 20 30 40 50 60 70 80 90 LEFM Max stress Amstutz (1995) 2024-T3, L-T Amstutz (1995) 2024-T3, T-L Hallback & Nilsson (1994) 7075-T6 Maccagno & Knott (1989), PMMA Maccagno & Knott (1991), -196C Mode I Transition 7075-T6 2024-T3 Mode II Mode I only: Mode I or Mode II:

under development, ignore for now

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

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

NASGRO Equation Dialog

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

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

All crack increments are specified

All cycle increments are specified

FRANC3D Tutorials – Manual Crack Growth Steps
Step 1: Select Grow Crack From the FRANC3D menu, select Cracks and Grow Crack Crack Growth wizard is displayed Choose Quasi-Static or Fatigue growth type Select Next

Step 2: Specify Growth Rate Second panel of the Crack Growth allows you to specify the growth rate model data Use the Paris model and set C to 1e-10 and leave n at 2 Select Next.

Step 7.3: Specify Extension or Cycles Third panel of the Crack Growth allows you to specify whether you will grow the crack based on a median extension or a number of cycles Use a median extension Select Next.

Step 7.4: Specify Fitting and Extrapolation Fourth panel of the Crack Growth allows you to specify a value for median extension as well as the fitting and extrapolation parameters Specify a median extension of 0.1 and use a fixed 3rd order polynomial with 3% extrapolation on both ends to ensure the fitted end points fall outside the model Select Next

Step 7.5: Specify Crack Front Template Final panel allows you to specify the crack front mesh template parameters Set the template radius to 0.06 Select Next to proceed with growing the crack and remeshing Once the remeshing is completed, another Static Crack Analysis can be performed

FRANC3D Tutorials – Automatic Crack Growth Steps
Assuming the crack insertion and static analysis was completed Step 1: Re-Open FRANC3D restart file From the FRANC3D menu, select File and Open. Choose the *.fdb file and select OK. FRANC3D will automatically read the FE model and solver results

Step 2: Select Crack Growth Analysis From the FRANC3D menu, select Analysis and Crack Growth Analysis First panel of the wizard allows you to choose the method for computing SIFs Use all the default values. Select Next

Step 3: Specify Growth Parameters Second panel appears Select Quasi-Static for simplicity All other values are left as defaults Select Next.

Step 4: Specify Growth Model Data Third panel appears Set the value of n to 2 for the power-law crack growth model Select Next

Step 5: Specify Fitting and Template Parameters Fourth panel appears Set the value for the template radius to The extrapolation could be increased from 3 to 5%, but 3% should suffice for the first 5 steps Select Next.

Step 6: Specify Extension or Cycle Data Fifth panel appears Grow the crack for 5 steps using a Constant Median Crack Growth Increment of 0.1 Select Next.

Step 7: Specify Analysis Code Sixth panel appears Use ANSYS and the Current crack growth step is 1 as if you are starting from the initial crack

Step 8: Specify Analysis Options Seventh panel appears Select your FE Solver Select global model FRANC3D transfers all the boundary conditions from the global model to the combined model, so leave the Transfer all retained bc’s checked. Click Next

Step 9: Specify Local/Global Model Connection Final panel allows you to choose how the local and global models will be connected Click Finish to start the automatic crack

The Python Programming Interface
The FRANC3D program has a programming interface that is an extension to the Python programming language. Python is an open source, object oriented, scripting language, which is popular in engineering and scientific computing community (e.g., it is used to drive the ABAQUS GUI). The Python interface allows one to automate repetitive and possibly error prone tasks. It also provides a possible strategy for coupling FRANC3D with other computational applications.

A simple PyF3D Program import PyF3D # create a flaw object
# file names for the models uncracked_fname = "minidisk_submodel.cdb“ fname_base = "minidisk_crack" # lists of crack size parameters to a_sizes = [0.0160, , , 0.0640, , , ] b_sizes = [0.0160, , , ] app = PyF3D.F3DApp() # loop through the crack size matrix for a in a_sizes: for b in b_sizes: # skip cases with really #bad aspect ratios if b > 0.2 and a < 0.065: continue # create a flaw object flaw = PyF3D.Flaw("Ellipse",[a,b]) flaw.Translate([0.499,4.179,-.374]) flaw.Rotate(1,"Y",90.0) flaw.Rotate(2,"Z",-53.61) # open an uncrack model, insert the flaw app.OpenModel(uncracked_fname) app.InsertFlaw(flaw) # generate a new file name like: # minidisk_crack_160_320.fdb fname = "%s_%d_%d.fdb" % \ (fname_base,int(a*1000),int(b*1000)) # save the file app.SaveModel(fname)

Some FRANC3D Known Bugs If any of the original body patches fall completely inside the template (no intersections) the crack insertion will not be successful.

Some FRANC3D Known Bugs If the none of the crack mouth or template edges intersect any of the edges of any of the original boundary patches the crack will not be inserted successfully.

Some FRANC3D Known Bugs FRANC3D can have difficulties meshing in situations where the crack-front template (the singular crack-front element and the two surrounding rings of brick elements) intersects one of the corner of the models.

Some FRANC3D Known Bugs The code is currently able to detect that the template intersects a corner and in many cases does a reasonably good job making the external mesh compatible with both the template and the geometry of the body. However, reasonable pyramid elements cannot be added on the outside of the template. The “Simple Template Intersections Only” option may work around this issue.

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

FRANC3D Workshop/Training

Similar presentations

Presentation on theme: "FRANC3D Workshop/Training"— Presentation transcript:

Similar presentations

About project

Feedback

Log in

Auth with social network:

FRANC3D Workshop/Training

Similar presentations

Presentation on theme: "FRANC3D Workshop/Training"— Presentation transcript:

Similar presentations

About project

Feedback