Delft University of Technology
FACULTY MECHANICAL, MARITIME AND MATERIALS ENGINEERING
Department Marine and Transport Technology Mekelweg 2 2628 CD Delft the Netherlands Phone +31 (0)15-2782889 Fax +31 (0)15-2781397 www.mtt.tudelft.nl
This report consists of 67 pages and 3 appendices. It may only be reproduced literally and as a whole. For commercial purposes only with written authorization of Delft University of Technology. Requests for consult are only taken into consideration under the condition that the applicant denies all legal rights on liabilities concerning the contents of the advice.
Specialization: Transport Engineering and Logistics
Report number: 2016.TEL.8061
Title:
Crack Growth Assessment of a
Plate with Longitudinal Stiffeners
Using the Finite Element Method
Author:
M. Schiaretti
Assignment: Research Assignment Confidential: no
Initiator (university): Dr. ir. X. Jiang Supervisor: Dr. ir. X. Jiang
Delft University of Technology Department of Marine and Transport Technology Mekelweg 2 2628 CD Delft the Netherlands Phone +31 (0)15-2782889 Fax +31 (0)15-2781397 www.mtt.tudelft.nl
Student: Assignment type: Research
Supervisor: Dr. X Jiang Report number: 2016.TEL.xxxx
Specialization: TEL Confidential:
Creditpoints (EC): 15
Subject: Determination of fracture parameter based on Finite element method
Fatigue cracks exist in all kinds of engineering structures, such as aircraft assemblies,
welded ships, bridges, rail, pipelines, pressure vessels, cranes, turbines discs and blades,
and general welded components. In many cases, the crack can be proved to be harmless, as
initial cracks often turn out to be. But in other cases, they could result in disaster. Thus, it is
important to evaluate the effect of crack on structural integrity
in order to guide maintenancestrategy– making of engineering structures.
This research assignment aims to investigate the effect of crack and its propagation on the structural integrity of structural details through FE analysis. The feasibility of FEA would be verified by case studies and /or standard. In this research assignment, following aspects are required to be illustrated in the report:
• The state of art of research on fatigue and fracture of thin– walled steel structures. (Numerical methods, experimental methods and standards.)
• To identify main fracture parameters in LEFM and EPFM.
• To develop a finite element modeling to determine their values and validate its feasibility • To apply the FEM to predict the crack growth. The case studies will be provided by the
supervisor.
This report should be arranged in such a way that all data is structurally presented in graphs, tables, and lists with belonging descriptions and explanations in text.
The report should comply with the guidelines of the section. Details can be found on the website. If you would like to know more about the assignment, you may contact with Dr. X Jiang through x.jiang@tudelft.nl.
The supervisor, X Jiang
Crack Growth Assessment
of a Plate with Longitudinal
Stiffeners Using the Finite
Element Method
M. Schiaretti
Research assignment
Supervisor: Dr. ir. X. Jiang
Crack Growth Assessment of
a Plate with Longitudinal
Stiffeners Using the Finite
Element Method
by
M. Schiaretti
Student number: 4502590
Project duration: September 6, 2016 – November 14, 2016 Supervisor: Dr. ir. X. Jiang
This report have been written to describe the progress made while working on the Research Assign-ment (ME2130-15). The main topic of this report, together with the experiAssign-mental data, was proposed by Delft University of Technology professor Dr. Ir. X. Jiang. I am thankful to her for the instructive debates about the topic and the overall set up of the research.
The objective of the report has not been completely fulfilled yet, this project has extended in a grad-uation project in collaboration with Lloyd’s Register. The plan is to continue working on the topic for a period of six months, during the master thesis.
I would like to thank my friends, especially Rutger, Femke and Simone, for the advice given on the report, for the motivation during the hard work of modeling and the cheering even when all the solutions tested were not properly working. I can not deny a thank to my girlfriend, which is physically far away, but always ready to support me, and to my family, which is always a valuable resource.
TAGs: Fracture Mechanics, Fatigue Life, Finite Element Method, Stress Intensity Factor, Weld
Magnification Factor, Crack, Growth, Longitudinal Stiffener.
Abstract
Fatigue is a mechanical phenomena found in many cyclic loaded structures. This type of loading can lead to a failure of the component. Fracture mechanics is the science which studies and assess cracks and their growth in the structures. Since many different geometries can be found in reality, there is not univocal solution for the computation of a crack growth. It is therefore of utmost importance to analyze and correctly reproduce the geometry of the main structures and the resulting cracks.The main problem is to reproduce an accurate model of a crack growth in a plate with non-load-carrying longitudinal stiffeners. This type of solution is a structural component in big ships.
Since the objective is to obtain an accurate model, different methods will be tested to achieve the best results. At first an empirical model will be created by using the formulas suggested in the British Standard. The FEM method will be tested to create a model without the implemented crack and a model with the crack. At the end, the models created and validated will be tested against an experi-mental result obtained with a cyclic tension load test.
Overall the results are promising but not completely satisfactory. The empirical model has obtained results with a relative error of5%, correctly reproducing the crack growth and the Stress Intensity Factor. The FEM models have yield the same stresses found in literature for a similar geometry, but the related weight function technique has not yet been implemented. Finally, the FEM solution with an implemented crack has shown results on scale with the literature, but yet a successive refinement is needed to match completely the proposed solution. Overall, the working models match the experimental results, but further improvement are suggested to obtain a more accurate solution.
Preface ii
Abstract iii
1 Introduction 1
2 Introduction to fatigue and fracture mechanics 3
2.1 Introduction to fatigue . . . 3
2.2 Introduction to fracture mechanics. . . 5
2.2.1 Cracks characterization . . . 6
2.2.2 Definition of Stress Intensity Factor . . . 8
2.2.3 Paris Law. . . 9
2.2.4 Fatigue in welded structures. . . 10
2.3 Numerical methods. . . 10
2.3.1 Empirical equations . . . 11
2.3.2 Finite Element Method. . . 13
2.4 Standards. . . 15
2.4.1 British Standard Institution (BS) . . . 15
2.4.2 Eurocode . . . 17
2.4.3 IIW Recommendations. . . 17
2.4.4 DNV. . . 17
3 Crack growth empirical model 19 3.1 Model parameters . . . 19
3.1.1 Geometry. . . 20
3.1.2 Initial flaw dimension. . . 20
3.1.3 Load and boundaries. . . 21
3.1.4 Material . . . 21
3.2 Validation . . . 22
3.2.1 Maddox [31] - Stress Intensity Factor trend. . . 22
3.2.2 Fu et al. [19] - Weld Magnification Factor trend. . . 23
3.2.3 Smith and Smith [47] - Fatigue life comparison. . . 24
3.3 Conclusion . . . 24
4 Finite element model without crack 27 4.1 Model parameters . . . 27
4.1.1 Stiffener geometry . . . 27
4.1.2 Materials . . . 27
4.1.3 Load and boundary. . . 28
4.1.4 Mesh refinement . . . 29
4.2 Validation . . . 31
4.2.1 Glinka et al. [21] - Through-thickness stress trend . . . 32
4.2.2 Maddox [31], Xiao and Yamada [51] - Stress concentration factor. . . 32
4.2.3 Heshmati [24] - Hotspot stress and effective notch stress . . . 32
4.2.4 BS7608 - Limitations of the hotspot calculation method . . . 33
4.3 Weight function technique . . . 34
4.4 Conclusion . . . 35
5 Finite element model with crack 36 5.1 Bottom-up mesh approach. . . 36
5.1.1 Pros. . . 37
5.1.2 Cons . . . 38 iv
Contents v
5.2 Top-down mesh approach . . . 38
5.2.1 Pros. . . 38
5.2.2 Cons . . . 39
5.3 Validation . . . 40
5.3.1 Newman and Raju [33] - Geometry factor comparison. . . 40
5.4 Crack growth techniques in FEA software . . . 41
5.4.1 Scripting. . . 42
5.4.2 ANSYS Mechanical APDL. . . 42
5.4.3 ABAQUS . . . 42
5.5 Conclusion . . . 43
6 Crack growth in a finite plate with non-load-carrying longitudinal stiffeners 44 6.1 Crack growth empirical model results. . . 45
6.2 Finite element model without crack results . . . 45
6.3 FEM model with crack results . . . 46
7 Conclusion 48 Bibliography 49 A Empirical formulas from literature 53 A.1 Newman-Raju [33] . . . 53
A.2 Weight function, Glinka [20] and Shen and Glinka [44]. . . 54
A.3 Weld Magnification Factor for a longitudinal non-loadcarrying attachement [6, 10]. . . 56
B MATLAB empirical model 59
1
Introduction
Fatigue fracture is a mechanical phenomena which undermines the integrity of many cyclic loaded structures. This type of load, even if it is well below the yield stress of the material, can slowly grow cracks in the components. Structures have regions subject to high stresses, the cyclic loading would make those key points develop cracks and eventually lead to a complete failure. Complicated geome-tries and welded components are the main reason for the development of high stress spots. The prob-lem is then to correctly understand which are those key points and how to assess the existing stresses in such positions. Experimental technique can be used to test specimen, but those are usually lim-ited in shape and dimensions. Through the use of mathematical models, such as empirical equations or Finite Elements Method (FEM), more complex geometries can be quickly analyzed. Nevertheless, problems found in the use of numerical simulations are not to be underestimated. The importance of using a numerical approach is highlighted by the possibility to obtain reliable and accurate results, but accuracy and reliability can only be achieved with a scientific approach and validations of the models. Since no precise knowledge are found in literature, the main goal of this research will be to reproduce an accurate model of a crack growth in a plate with non-load-carrying longitudinal stiffeners. This geometry has never been deeply analyzed with a proper finite elements parametric study, neither an empirical solution has ever been drawn.Literature is offering solutions for similar cases, those will be used to model an empirical model of the crack growing. This model is validated through solutions found in reference studies. Finite element analysis of the geometry is the overall goal of the research, a simple model will be created and the through-thickness stress results derived. Finally, the crack will be implemented in the finite elements model and the growth will be assessed within a finite elements analysis environment.
A few conditions are assumed in order to simplify the computation. The notch radius between weld and plates is not reproduced in the FEM model. Loads conditions are limited, the models will only cover tension loading, as of now the bending conditions are not thought to be interesting. Further on, the stress ratio is always positive,𝑅 > 0, this means that there will be no discussion about the effective stress range and whether the negative load has an influence on the crack propagation. The complete research is structured as in Figure1.1, all the phases will be described in the following chapters of this report. Since the research plan is ambitious, not all the steps have a solution or a working model at the time this report is produced, but further research is already planned to complete those missing parts. Chapter2presents the basic theory of fatigue and fracture mechanics, along with the main assump-tions hold for the following models. A brief description of Finite Element Method (FEM) and standards regulations integrate the theoretical background found in Chapter2. The first solution for a stiffened plate is described in Chapter3, empirical equations are used to evaluate the crack growth. The results are validated at the end of the chapter. Moving to FEM, a simple model, without integrated crack, is analyzed in Chapter4. Different geometries and mesh refinements are tested and validated with the help of literature references. Further on, the crack is introduced in the FEM model, even if the solution found is not complete, the results obtained are presented in Chapter5. Along with the limited results,
hypothetical FEM crack growth technique are discussed toward the end of the chapter. Finally, the experimental data are compared with the results obtained from different models, the results can be found in Chapter6.
2
Introduction to fatigue and fracture
mechanics
The main focus of this report will be to address the fatigue crack growth in a plate with longitudinal stiffeners. The goal of this theoretical introduction is to give to the reader a clear view of what is the fatigue phenomena and how the fracture mechanics branch fit inside. In the latest sections, numerical and experimental techniques will be analyzed together with the given standards about the fatigue and fracture mechanics.2.1. Introduction to fatigue
Fatigue is an important phenomena found in all known materials. The essential behaviour needed to develop a fatigue failure is a cyclic load on the component or specimen. This condition is found in almost all the structures being built until now. This mechanical failure was first discovered around 1837 by Wilhelm Albert, but only in 1870 the first fatigue test was accomplished by Whöler [49]. Since then, the fatigue analysis was only considered a niche technique, highly underestimated, until late 1950s, when the first passenger jetliner, the de Havilland DH-106 Comet, failed during flight. There have been three catastrophic accident before the plane was removed from service and thoroughly inspected. Af-ter real life pressure tests in a waAf-ter tank, the root cause of the failure was found to be a fatigue crack growth starting from a high stress spot in a window [1] (see Figure2.1).
Figure 2.1 – Fracture propagating from the high stress point (corner of the window) in a de Havilland DH-106 Comet
Since this disaster, the fatigue mechanism have been deeply researched and it is now clear in every step. The fatigue life is defined as the amount of cycles that a component can withstand before reaching complete failure. This life is usually divided in two main phases: crack initiation period and crack growth period (see Figure2.2). As a common practice, different factors are mainly related to different periods, even if this relation is not exclusive. For example, the stress concentration still has importance during the crack growth phase. [41]
• 𝐾 : Stress Concentration Factor (SCF) is mainly related to the prediction of the crack initiation period, when the crack is only growing at a micro structure level
• 𝐾: Stress Intensity Factor (SIF) is related to the prediction of the macro crack growth • 𝐾 : Fracture toughness is the limit state that the crack can reach before failing
The main focus of this report will be to precisely assess the crack growth at a macroscopic level, so the crack initiation is out of scope.
Figure 2.2 – Different phases of fatigue life and relevant factors [41]
Whenever fatigue stress is involved, the components are subjected to cyclic loading. In reality, the load cycles can differ in maximum, minimum stress and frequency, creating a variable amplitude loading condition. Is common, for practical purposes, to use a wave shaped reference cycle, which shows constant amplitude and frequency. This function can be characterized by stress amplitude (𝑆 ) and mean stress (𝑆 ), or by maximum (𝑆 ) and minimum stress (𝑆 ), or even more by the stress range (Δ𝑆) and stress ratio (𝑅) (see Figure2.3) [39].
In the following report, reference will be made mainly to the stress range and stress ratio, this choice is made because many literature experiments are carried out at𝑅 ≈ 0 and stress range Δ𝑆 ≈ 𝑆 [31,43,46,52]
Figure 2.3 – Characterization of a stress cycle [39]
Fatigue life for a specific material is described by the S-N curve. This relation was found by Whöler through correlation of a number of fatigue tests at different stress levels. The test are then plotted based on the stress amplitude𝑆 and the life in cycles 𝑁. The graph uses log-log scale in order to obtain the following linear equation (see Figure2.4):
𝑆 𝑁 = costant (2.1)
The fatigue life of a specimen can be divided in low-cycle fatigue and high-cycle fatigue, despite an exact division is not defined, Schijve in [39] (see Figure2.4) refers to low-cycle up to10 and begin
2.2. Introduction to fracture mechanics 5
talking about high-cycle around10 .
The overall fatigue life of a component is divided in initiation life (𝑁 ) and fatigue-crack-propagation life (𝑁). The total fatigue life is a sum of the two phases. The main focus of this report is about the fatigue-crack-propagation period (𝑁). Selburg [43] and Schijve [40] argue that the crack-initiation threshold in a welded component cannot be clearly established. The weld itself is a discontinu-ity in the material and so the weld toe can already be considered a small crack. This assumption would lead to the equality of the total fatigue life and the crack-growth period. Further more, Chattopadhyay et al. [12] proofed that the crack-initiation life at a weld toe, without considering the residual stresses, only account for maximum 12% of the overall number of cycles to failure (𝑁 /𝑁 = 0.12). Every single analysis must be accurately evaluated, different initial thresholds are used in literature to establish the between initiation period and crack growth period. A case by case evaluation will be used to assess the crack growth life.
Figure 2.4 – Fatigue test results for unnotched specimen SAE4130 at – Example of S-N curve [39]
2.2. Introduction to fracture mechanics
Fracture mechanics is the science which studies the crack growth in a material. This phase of the fatigue life will deal with the macro crack growth or more clearly whenever the crack start to penetrate into the subsurface material. No clear definition of the exact length or depth of the initiation crack exist, but Chattopadhyay et al. [12], Leander et al. [29] and Smith and Smith [46] assume different values based on experience. The first one assumes a crack depth of𝑎 = 0.5 𝑚𝑚 while the second reference varies between𝑎 = 0.25 𝑚𝑚 and 𝑎 = 1 𝑚𝑚. The last reference extrapolate the initial crack depth in a speciment with a T-butt welded joint, the result is coming from an extensive microscope analysis of 278 defects. The average value observed by Smith and Smith [46] attests at𝑎 = 0.05 𝑚𝑚 (see Figure3.11), this is considered an accurate threshold between initiation period and crack growth period. According to Hobbacher [26], Equation2.2can be used to derive the crack aspect ratio. Since the crack depth threshold adopted is too small for the equation, additional literature research has defined the initial acceptable crack ratio to𝑎/𝑐 = 0.3 [12,43], which corresponds to a threshold crack length of2𝑐 = 0.33 (see Figure2.5).
Figure 2.5 – Crack parameters – Left for an elliptical shaped crack – Right for a semi-elliptical shaped crack
Fracture mechanics field of study is divided in Linear Elastic Fracture Mechanics (LEFM) and Elastic Plastic Fracture Mechanics (EPFM). The difference between those two behaviors are the assumptions made in the material characterization. LEFM assumes an isotropic and linear elastic material, which imply that the stress around the crack tip is calculated using the theory of elasticity. EPFM will take into account a large plastic deformation of the material around the crack tip, before the crack begin to grow. The material assumptions are isotropic and non-linear elastic (see Figure2.6).
The two conditions describe two different types of fracture. Little or no plastic deformations is corre-spondent to a brittle fracture, which can be considered similar to a LEFM behavior. This type of crack leaves a fairly smooth fractured surface and lead to a fast and unstable crack growth. This fracture is characterized by the Stress Intensity Factor (𝐾), the fracture toughness (𝐾 ) and the energy release rate (𝐺). Those three concepts will be introduced afterwards in this section. The EPFM is correspon-dent to a ductile fracture, where extensive plastic deformation is present at the crack tip. This conditions can be valuable to obtain a slow crack growth and longer fatigue life [23].
The type of fracture can be assessed based on the ASTM E647-05, Appendix X3.8.3 [27]. The threshold value is considered to be 60% of the material yield stress (0.6𝜎 ). If the maximum stress level reach or overhaul the threshold (𝑆 ≥ 0.6𝜎 ) then the plasticity is high and EPFM environment has to be considered. Instead, if the maximum tensile stress is kept below the threshold (𝑆 < 0.6𝜎 ), the crack tip will have a simple LEFM behavior. Because the maximum stress found in the experiment (see Section6) is below60%, from now on, in this report, the crack tip is considered to always behave as in a LEFM environment.
Figure 2.6 – Conditions around the Crack Tip
2.2.1. Cracks characterization
In order to better understand the components characterizing a fracture, in the following section the crack geometry and the conventional tip opening modes are described.
Crack tip geometry
The crack tip is considered a small region where the crack ends. This region can be a single point, if the crack is analyzed in 2D or a line, if the crack is considered in a 3D environment [23]. Those two
2.2. Introduction to fracture mechanics 7
situations are depending upon another condition, whether the crack is propagating completely through the thickness, as in figure2.7on the right, or only part through the thickness, figure2.7on the left. The first condition will lead to the use of 2D crack tip region (see Figure2.8), correspondent to a plain strain analysis, while the latter will lead to a more complicated 3D crack tip region (see Figure2.9), where plain strain conditions are used, except for the surface point, where plain stress applies [19,42].
Both the crack tips are characterized by a cartesian (𝑥, 𝑦, 𝑧) reference system, with 𝑧 always tangent to the crack and𝑥 lying on the uncracked region. Even more, a polar reference system (𝑟, 𝜃) will be used to better describe the stress region around the tip.
Figure 2.7 – Different types of cracks
Figure 2.8 – 2D crack tip region Figure 2.9 – 3D crack tip region
Opening modes
Analyzing the crack growth, three major tip opening modes are defined. They are called Mode I, Mode II and Mode III, in order they depend from the opening tension, the in-plane shear and transverse shear (see Figure2.10). Generally, Mode I is the more important in every crack growth analysis, because have been tested that even small cracks developed under pure shear loading will quickly transition to a tensile mode [41]. During experimental tests, the fracture toughness is found only for the Mode I, hence the symbol𝐾 .
2.2.2. Definition of Stress Intensity Factor
The Stress Intensity Factor is the main parameter used to describe a LEFM crack growth. The physical meaning is a factor used to correlate the stress conditions in the plate and the actual crack dimensions.
The Griffit Criterion
Griffith criterion states that, in a small crack of length𝑎 advancing of a smaller quantity 𝛿𝑎, ”if the work done by the applied loads is greater than or equal to the change of elastic energy plus the energy absorbed at the crack tip, then fast fracture will occur” [23]. This statement is condensed in eq. 2.3.
𝛿𝑊 ≥ 𝛿𝑈 + 𝐺 𝑡𝛿𝑎 (2.3)
𝛿𝑈 is the change in elastic energy and 𝛿𝑊 is the work done to form a crack extension 𝛿𝑎. 𝐺 is the critical energy release rate (or toughness) and express how easily a material can crack. For example, low toughness means it cracks easily, high toughness is hard to crack.
From the equation above, the critical energy release rate can be related to a critical stress (𝜎 ) expressing the failure in an infinite plate with central crack. The following equations apply:
𝐺 = 𝜎 𝜋𝑎
𝐸 (2.4)
or
𝜎 √𝜋𝑎 = √𝐸𝐺 = 𝐾 (2.5)
Extending the concept, the stress intensity factor𝐾 = 𝜎√𝜋𝑎. The unit of this factor is [𝑀𝑁𝑚 3 2 ] or
[𝑀𝑃𝑎𝑚 ].
The potential energy𝑃 is related to the crack growth 𝑎 through the fundamental definition 𝐺 = −𝑑𝑃
𝑑𝑎 (2.6)
The most important relations used in LEFM analysis is derived from Equation 2.6. The change in potential energy is considered to act on closing a small segment of crack length𝛿𝑎, equating this quantity to the work required to close the segment without any external work variation. The following equation is obtained for plane stress:
𝐺 = 1
𝐸 (𝐾 + 𝐾 ) +
(1 + 𝜈)
𝐸 𝐾 (2.7)
and for plane strain:
𝐺 = 1 − 𝜈
𝐸 (𝐾 + 𝐾 ) +
(1 + 𝜈)
𝐸 𝐾 (2.8)
Hellen [23] states that the plane stress equation applies for 2D cracks or surface spot of a 3D crack. While the plain strain equation is used in complicated 3D crack region, especially in the deepest spot.
The J-Integral
The J-integral is defined as ”a certain integral evaluated along a contour traversing a region around the crack tip” [23]. The J-integral concept applies for both 2D and 3D crack tip. Whenever simple conditions applies, like the 2D crack found in Figure2.11, the integral is:
𝐽 = ∫ (𝑊𝑑𝑦 − ⃗𝑇𝜕 ⃗𝑢
2.2. Introduction to fracture mechanics 9
The cartesian reference system must follow what described earlier in Figure2.8and2.9. 𝑊 = 𝑊(𝑥, 𝑦) = 𝑊(𝜖) and represent the strain energy density. ⃗𝑇 ≡ 𝑇 is the traction vector defined along the outward normal ̂𝑛 and so is the force per unit length (see Figure2.9).
Under certain conditions (LEFM and small scale yielding) [53], the result of J-integral can be con-sidered:
𝐽 = −𝑑𝑃
𝑑𝑎 = 𝐺 (2.10)
and the𝐽 value can be considered equal to 𝐺 [23]. This equalities are really important, they give the possibility to calculate the J-integral value through a FEM software and then derive the Stress Intensity Factor from it.
Figure 2.11 – 2D contour definition of J-integral
𝐾 in curved cracked fronts
A special mention is needed in order to describe the behave of the stress intensity factor𝐾 in a curved cracked front. This remark is necessary since the main goal of this report will be to describe the behave of a semi-elliptical crack in a finite plate. The reference system used through the report is shown in figure2.12,𝜑 is the angle on the reference circle and 𝐶 is the corresponding point on the crack front.
Irwin [28] studied in 1962 the behave of a semi-elliptical crack, reaching an empirical expression for the variation of𝐾 along the crack front (see Figure2.13). in a simple plate with a finite thickness, the value of𝐾 is greater when the crack front intersect the minor axis, at 𝜑 = 90°. This is the deepest point of the crack and has a substantial difference compared to the surface point (𝜑 = 0°). Schijve [42] rightly affirm that the fatigue crack growth in depth will be faster than in length, leading to variation of the ratio between minor and major axis during the fatigue life.
2.2.3. Paris Law
Paris and Erdogan [35] studied the crack growth rate in many test, the result is a correlation between the crack growth rate𝑑𝑎/𝑑𝑁 and the stress intensity factor Δ𝐾. Additional experiments have shown a clear path in all the𝑑𝑎/𝑑𝑁 − Δ𝐾 graphs, with two asymptotes occurring which highlight the begin and end of a crack life (see Figure2.14). The graph has log-log axis, so the relation in the central region, called Paris region, is linear. The equation is the following:
𝑑𝑎
𝑑𝑁 = 𝐶Δ𝐾 (2.11)
where𝐶 and 𝑚 are material constants. This equation does not account for the regions below and above the Paris region. Those are called respectively threshold region and stable tearing crack growth region. Other researcher after Paris tried to include the other regions in the relation, Forman et al. [18] proposed:
𝑑𝑎 𝑑𝑁 =
𝐶Δ𝐾
Figure 2.12 – Elliptical crack reference system
Figure 2.13 – Behave of along the crack front in a
semi-elliptical surface crack – Variation of location and crack dimension
In eq. 2.12the critical stress intensity factor is considered (𝐾 ) and the therm (𝐾 − 𝐾 ) will lead to a vertical asymptot whenever the𝐾 approaches the fatigue limit. The threshold region is although not considered yet. Priddle [36] decided to integrate the stress intensity factor thresholdΔ𝐾 in the numerator, obtaining:
𝑑𝑎 𝑑𝑁 = 𝐶 [
Δ𝐾 − Δ𝐾
𝐾 − 𝐾 ] (2.13)
For a practical purpose, the Paris equation can be rearranged and integrated in order to obtain the fatigue life of a component. The initial crack size𝑎 and final crack size 𝑎 must be known, the equation is then:
𝑁 = 1 𝐶∫
1
Δ𝐾 𝑑𝑎 (2.14)
2.2.4. Fatigue in welded structures
The goal of this report is to assess the crack growth in a plate with longitudinal stiffeners. These plates are connected through welding. The welding itself needs a small consideration in term of stresses. The weld fillet and the deformed region around the connection can already be considered a micro-crack, as explained in section2.1. The welding material creates an higher notch stress, especially at the end of the longitudinal gusset plate, as described by Maddox [32], Smith and Smith [46,47]. The S-N curve for a welded specimen with a longitudinal gusset is showing fatigue life eight times lower than a normal plate (see Figure2.15). From such a drastic decrease in fatigue life, an high notch stress is expected, especially at the weld toe.
Different approaches are used in order to calculate the increased value of 𝐾. Many standards propose a unified table with different classes (S-N curves), then, they supply table with specimen or components geometries and assign to every detail a specific class. By using this technique the fatigue life can be assessed just through the knowledge of the nominal stress.
This procedure does not give insight in the crack growth process. In order to assess this, the𝑀 factor method, developed by Hobbacher [25] and [6], can be used. In the coming sections, numerical methods to obtain the stress intensity factor will be described.
2.3. Numerical methods
The assessment of the fatigue crack growth procedure is a key element in this report. Since the early age of fracture mechanics analysis, many numerical solutions were created, based mainly on equations
2.3. Numerical methods 11
Figure 2.14 – Crack growth regions highlighting the Paris law
Figure 2.15 – S-N curves of a plate, a plate with an hole and a plate with longitudinal gussets under tensile stress
defined from fitting experimental data. In the following sections, first empirical and then FEA solutions are explained.
The description of the methods will be centered only on techniques which are useful for the crack growth in a plate with longitudinal stiffeners, or similar geometries which consider a welding. The reference geometry used will be the one found in Figure2.16, corresponding to a semi-elliptical crack in a finite width plate.
2.3.1. Empirical equations
A few different techniques have been developed to assess the crack growth using empirical formulas. The oldest one have been found by Newman and Raju [33], the specific stress-intensity factor equation is explained in [33]. That function was limited in terms of𝑎/𝑡, so the weight function approach have been adopted by Wang [50] to cover the previous missing crack growth phases. Bransen [9] combined the previous formulas in a MATLAB code, obtained a smooth passage between the two and validated the new empirical technique.
Figure 2.16 – Crack shape and plate geometry for part-through surface crack in a finite plate
Newman-Raju formula
Newman-Raju formula is an ”empirical stress-intensity factor equation for a surface crack as a function of parametric angle, crack depth, crack length, plate thickness and plate width for tension and bending loads” [33]. The shape of the crack is the same as in figure2.16and the reference system as found in figure2.12. The equation considers the remote tensile stress𝑆 and bending moment 𝑀.
𝐾 = (𝑆 + 𝐻𝑆 ) √𝜋𝑎 𝑄𝐹 ( 𝑎 𝑡, 𝑎 𝑐, 𝑐 𝑏, 𝜙) (2.15)
where the validity limits are:
0 < 𝑎/𝑐 ≤ 1.0 (2.16)
0 ≤ 𝑎/𝑡 < 0.8 (2.17)
𝑐/𝑏 < 0.5 (2.18)
0 ≤ 𝜙 ≤ 𝜋 (2.19)
See AppendixA.1for the complete equations of the bending factor𝐻, tension factor 𝐹 and shape factor 𝑄. The remote bending moment is related to 𝑆 with the following equation:
𝑆 = 6𝑀
𝐵𝑇 (2.20)
Weight function
The weight function approach have been introduced by Beuckner [3] and Rice [38]. It is used to gen-eralize the stress intensity factor solution for crack subject to arbitrary loading. The standard equation to obtain the stress intensity factor is the following:
𝐾 = ∫ 𝜎(𝑥)𝑚(𝑥, 𝑎)𝑑𝑥 (2.21)
2.3. Numerical methods 13
is the weight function. The general equation which identify the weight function for a surface crack is:
𝑚(𝑥, 𝑎) = 2 √2𝜋(𝑎 − 𝑥)[1 + 𝑀 (1 − 𝑥 𝑎) 1 2 + 𝑀 (1 −𝑥 𝑎) + 𝑀 (1 − 𝑥 𝑎) ] (2.22)
At the deepest point𝑥 = 𝑎, as seen in Figure2.16. In this case, the square root in Equation2.22
would become singular, this is why the computation is limited to𝑎 . The complete formula for deep point𝑎 and surface point 𝑐 weight function is found in AppendixA.2.
Weld magnification factor
𝑀 factor is defined by Bowness and Lee [6] as 𝑀 = 𝐾in plate with attachment
𝐾in same plate but with no attachment
(2.23) The𝑀 is a factor which quantifies the change in stress intensity as a result of the presence of the weld and the attachment. This factor is usually applied to a plain plate solution to obtain the𝐾 values.
Hobbacher [25] derived the stress intensity factor for a welded joint. The𝐾 equation is:
𝐾 = √𝜋𝑎 (𝜎 𝑌 𝑀 , + 𝜎 𝑌 𝑀 , ) (2.24)
where𝑌 is the geometry correction function and can be found in literature, while the solution for 𝑀 in a longitudinal non-loadcarrying attachment is derived from FEM analysis.
𝑀 = 𝐶 (𝑎
𝑇) 𝑀 ≥ 1 (2.25)
Further on, Bowness and Lee [5, 6] derived a 3D solution for a semi-elliptical crack in a T-butt joint. The equation was extracted from a parametric study on 3D FEM models. The complete solution, the validity limits and the figures are found in AppendixA.3.
2.3.2. Finite Element Method
Finite element models of 2D and 3D crack growth analysis have been always used since 1970s. This technique, if applied with the requested accuracy and validating mesh and models, lead to precise solutions. The advantage of FEM is the possibility to simulate complex geometries which are not already assessed in literature. In order to obtain the stress intensity factor from the Finite Element model, there are direct or indirect methods. ANSYS®offers the Interaction Integral Method (IIM) and the Displacement Extrapolation Method (DEM) to obtain the SIF. Otherwise, the J-integral can be computed along the crack front and subsequently post-processed to calculate the𝐾. Even more, the Virtual Crack Closing Technique (VCCT) method can show the energy-release rate at the crack front, this can be further processed to obtain𝐾. Further on, ABAQUS is a Finite Element solver offered by Simulia 3DS, competitor of ANSYS, which can deliver similar crack analysis capabilities. The technique used by ABAQUS to compute the Stress Intensity Factor is discussed in the coming section.
Displacement related methods
Displacement Extrapolation Method
Displacement Extrapolation Method is an integrated method proposed by ANSYS®, it is a pure post-processing technique, which is based on the displacement of the nodes after a linear static model of an open crack have been solved. Manually a path along the crack must be defined as an input parameter. Then, the values are insert in the Westergaard equations (see Reference [23, pag. 19-20]) and the𝐾 is computed.
Energy release related methods
Interaction Integral Method
The interaction integral method is really similar to the domain integral method J-integral. It can be used for 2D through area integration and 3D through volume integration. The interaction integral is defined by ANSYS®[2] as:
𝐼 = − ∫ 𝑞, (𝜎 𝜀 𝛿 − 𝜎 𝑢 , − 𝜎 𝑢 , ) 𝑑𝑉 (2.26)
𝐼 = − ∫ 𝛿𝑞 𝑑𝑠 (2.27)
Where𝜎 , 𝜀 , 𝑢 are the stress, strain and displacement, 𝜎 , 𝜀 , 𝑢 are the stress, strain and displacement for the auxiliary field.𝑞 is the crack-extension vector.
The interaction integral method is linked to the stress intensity factor with slightly modified equations
2.7and2.8: 𝐼 = 2
𝐸∗ (𝐾 𝐾 + 𝐾 𝐾 ) + 1
𝜇𝐾 𝐾 (2.28)
where𝐾 are the stress intensity factors for different modes, the 𝐾 is the auxiliary mode stress intensity factor,𝐸∗ = 𝐸 for plain stress and 𝐸∗= 𝐸/(1 − 𝜈 ) for plain strain. 𝐸 is the Young’s modulus, 𝜈 is the Poisson’s ratio and 𝜇 is the shear modulus.
J-integral
J-integral method is explained already in Section2.2.2. Many contours in area or volume around the crack tip are computed, then the average value is used to obtain the energy release rate along the crack tip. The result can be used to evaluate𝐾, because Eq. 2.10gives the necessary relation to substitute𝐽 in Equation2.7and2.8and derive the Stress Intensity Factor. This technique uses both the software calculations for J-integral and the post-processing to find the𝐾.
Virtual Crack Closing Technique
The Virtual Crack Closing Technique is used to evaluate the energy-release rate at a crack front. The assumption at the base of this method is that the same energy is needed to separate and to close the same surface. The solution proposed in ANSYS® further assumes that the stress state does not change significantly whenever the crack grows by a small amount. the use of low-order elements is suggested around the crack-front, even more, degenerative elements shapes are not supported. This last detail is important for a 3D crack, since many times the crack front is modeled with degenerative wedge-shaped elements. The equations governing the energy-release rate are the following:
𝐺 = − 1 2Δ𝐴𝑅 Δ𝑣 (2.29) 𝐺 = − 1 2Δ𝐴𝑅 Δ𝑢 (2.30) 𝐺 = − 1 2Δ𝐴𝑅 Δ𝑤 (2.31)
where𝐺 , 𝐺 and 𝐺 are energy-release for different fracture modes, Δ𝑢, Δ𝑣 and Δ𝑤 are the dis-placements between top and bottom nodes of the crack. 𝑅 , 𝑅 and 𝑅 are the reaction forces at the crack-front nodes andΔ𝐴 is the crack-extension area, as in Figure2.17.
Contour Integral evaluation
ABAQUS [45] mainly propose just one technique to compute the energy-release rate. This method is the same proposed by ANSYS with the interaction integral method. It can be further integrated with residual stresses along the weld or in the component. An important suggestion is given by the docu-mentation, the complicated procedure of creating an enough refined mesh in a 3D crack is overcome whenever the X-FEM technique is used together with enrichment rule. This type of mesh can be used together with the usual contour integral method to extrapolate the energy results. One additional hint is given by ABAQUS, the result for J-integral computation is path independent in difference paths for the same node on the cracks front, this suggestion is useful to find the convergence of the mesh, by checking whether the contours, after the second, are yielding almost the same value.
2.4. Standards 15
Figure 2.17 – 3D crack details for VCCT technique
2.4. Standards
As of today, fatigue and crack growth are a big problem, around 90% of the mechanical failures de-rive from underestimated fractures [30]. Standards and Institutes have took the matter seriously, by developing tips and tricks about the fatigue and crack assessment.
2.4.1. British Standard Institution (BS)
The British Standard Institution have published two important papers:
• BS 7910:2013+A1:2015: Guide to Methods for Assessing the Acceptability of Flaws in Metallic Structures [10]
• BS 7608:2014+A1:2015: Guide to fatigue design and assessment of steel products [11]
Both this standards are useful to understand the fatigue assessment. BS7910 [10, Chapt. 8] has a good table describing a general procedure and a quality category procedure for known flaws.
A two stage crack growth model is proposed (see Figure2.18), this method is supposed to better consider the different growth steps of the fracture. This solution is different from the one proposed in Sec.2.2.3, since the equation is the following:
Stage A: 𝑑𝑎
𝑑𝑁 = 𝐶 (Δ𝐾) (2.32)
Stage B: 𝑑𝑎
𝑑𝑁 = 𝐶 (Δ𝐾) (2.33)
Where for𝑅 < 0.5 (the experimental case is 𝑅 ≈ 0.1) table2.1applies.
Table 2.1 – Two stage fatigue crack growth variables for steel in air
Stage A Stage B Transition pointΔ𝐾
𝐶 𝑚 𝐶 𝑚
1.21 ⋅ 10 8.16 3.98 ⋅ 10 2.88 363 𝑁 ⋅ 𝑚𝑚 /
The fatigue crack growth threshold value suggested by BS7910 isΔ𝐾 = 63 𝑁/𝑚𝑚 / .
BS7910 [10, App. M] gives a method to calculate the stress intensity factor combining the nominal stress, geometrical correction and weld factor.
BS7608 [11, App. D] gives an extensive guidance on the use of fracture mechanics. The simple Paris law applies (see Equation2.11), with constant𝐶 = 5.21⋅10 while𝑘 = 3. The following equation
Figure 2.18 – Two stage crack growth as found in BS7910 [10]
is used to computeΔ𝐾 with tension load only:
Δ𝐾 = (𝑀 𝑀 Δ𝜎 ) √𝜋𝑎
𝑄 (2.34)
Many of those variables are explained in BS7910. The stress rangeΔ𝜎 can be calculated using the nominal stress method or the hot-spot stress method. In case the hot-spot stress is used in combina-tion with the𝑀 factor, the ratio 𝐿/𝐵 in 𝑀 should be always assumed equal to 0.5.
BS7608 suggest a calibration of the FEM model in case of hot-spot stress method. This calibration is used to validate the model by:
a) Computing the fatigue strength of a joint class with detail similar to the that under consideration (empirical method)
b) Experimental data for joints which are similar to those used in the simulation (experimental method) Overall, the British Standards does not suggest any precise FEM technique which must be used to calculate the stress intensity factor. The main focus of BS7608 is the hot-spot stress. In Appendix C4.3 the through-thickness hot-spot stress is explained, this technique average many element stress results to obtain the correct stress at the required spot. Many different methods are explained in Appendix C of BS7608, suggesting the use of solid bricks or shell elements to reproduce the weld geometry (see Figure2.19.
Combining the hotspot stress found with FEM and the formulas suggested in Appendix D from BS7608, the stress intensity factor can be computed. This solution is only suitable for weld-toe cracks. The hotspot stress already includes the stress concentration from gross structural discontinuities, the only missing information to calculate𝐾 is the 𝑀 factor, weld toe magnification factor, this can easily be obtained from BS7910.
2.4. Standards 17
Figure 2.19 – FEM model example as suggested by BS7608 - Left Solid bricks used to reproduce the beam and
the weld - Right Shell elements used to reproduce the beam and the weld
2.4.2. Eurocode
The European Union published in 2005 the latest standards about materials and fatigue. EN 1993-1-10 (2005): Eurocode 3: Design of steel structures - Part 1-10: Material toughness and through-thickness properties [17], this standard only gives vague suggestion about the technique used to assess fracture mechanics. Those mentioned are Crack Tip Opening Displacement (CTOD) values or J-integral values to be used in FEM analysis. The code advise to begin the computation from a flaw size which represent the minimum value detectable from the inspection method.
EN 1993-1-9 (2005): Eurocode 3: Design of steel structures - Part 1-9: Fatigue [16] only explains how to assess fatigue life according to weld class, depending from the geometry of the attachment, and following a specific fatigue strength curve appropriate for the detail. Overall Eurocode does not give any hint on how to assess the stress intensity factor.
2.4.3. IIW Recommendations
International Institute of Welding (IIW) has been founded in 1948 by the welding societies of 13 coun-tries. This institute, since then, is active in researching about any joining technique (mainly welding). The institute release many scientific papers about welding, one of the most famous books is the ”Rec-ommendations for Fatigue Design of Welded Joints and Components” from Hobbacher [26].
This book effectively goes through all the fracture mechanics theory. The definition of𝐾 is given, when the stress is calculated in a uncracked plate, using universal correction function𝑌(𝑎) and the weld-toe correction for non-linear peak stress𝑀 . The general formula for 𝐾 is:
𝐾 = √𝜋𝑎 (𝜎 𝑌 (𝑎)𝑀 , (𝑎) + 𝜎 𝑌 (𝑎)𝑀 , (𝑎)) (2.35)
Brief suggestion for the Finite Element programs are given. If the𝑀 factor found in Hobbacher [26, App. 6.2] is used, then the coarse meshing may be sufficient to determine a membrane stress. If the weight function approach is picked, then the mesh should be accurately refined to assess the through-thickness stress at the weld toe. Otherwise, programs like ANSYS®already have fracture mechanics components able to compute𝐾.
Fatigue resistance classes are used to find the fatigue life limit of different attachments. So, the fatigue assessment can be done using S-N curves. The stress intensity factor empirical calculation is assessed in Hobbacher [26, App. 6.2], the 𝑀 factor formula for a longitudinal non-loadcarrying attachment is given as well. The combination of the two formulas will give the overall stress intensity factor result. Both the formulas are found in AppendixA.1andA.3of this report.
2.4.4. DNV
Det Norske Veritas (DNV) and Germanischer Lloyd (GL) do not propose a specific standard regarding fatigue and fracture mechanics. DNV-RP-C203 [48] is a recommended practice to follow for fatigue design of offshore steel structures. There are a few suggestions on how to model a 3D welded joint using plates, related to the computation of the stress concentration factor or hotspot method. Section 6 of DNV-RP-C203 explain which are the basic equations (Paris law, Stress Intensity Factor) to be
used to assess the crack growth in a component, for any further detail it relates back to BS7910 and BS7608.
3
Crack growth empirical model
Fatigue crack growth assessment has been researched in the past, many papers have analyzed through FEM models or experiments the behave of cracks in different conditions. The data collected was organized and reduced to parametric equations, those solutions can be found in BS7608 [11] and IIW recommendations [26]. This is the first numerical model that is created to simulate the crack growth. In this chapter, at first, the parameters needed in the model are discussed (Section3.1). The goal of these discussion is to show how sensitive is the model to the different inputs. Subsequently the model is validated (Section3.2). Since many different empirical equations are combined inside the model, different factors have to be validated, by using different references.The equations used to create the MATLAB empirical model are discovered by Newman and Raju [33] (see Section 2.3.1) for a semi-elliptical surface crack. The goal of this research is to obtain the crack growth at the weld toe of a longitudinal stiffener, so the𝑀 equation from Bowness and Lee [7] (see Section2.3.1) is added to the computation of the Stress Intensity Factor.
Figure 3.1 – 3D reference draw used for the MATLAB emprical model
The MATLAB empirical model is formulated with a while loop which compute the crack growth at every cycle. The diagram in Figure3.2shows the schematized process used to compute the crack growth. The Bowness and Lee [6] formula is used to compute the𝑀 factor, which is also found in AppendixA.3. The formula used to compute the geometric factor for a crack on a surface in a plate is taken from Newman and Raju [33] and can be found in AppendixA.1.
3.1. Model parameters
The MATLAB empirical model requires a few initial parameters in order to begin computing the solution. It is highly important to correctly define the initial values, because the equations used in the empirical model are depending upon the geometry, the initial flaw dimensions, the load case and the material. Those are the four main information needed to assess the crack growth.
Setup initial information (Material, Geometry, Flaw size, dN) Are basic conditions met? End (N, K, Mk) Compute Mk
(Bowness and Lee, 2000) Compute K (Newman and Raju, 1981) Calculate da and dc Crack growth (Paris and Erdogan, 1963)
Has the crack reached growth limit?
(dKc, 0.8*T) Yes
No No
Yes
Figure 3.2 – Diagram of the process used in MATLAB to compute the crack growth
3.1.1. Geometry
The basic information needed for the MATLAB model are just four geometrical measures. They are shown in Figure3.1, the thickness of the main plate (𝑇), the width of the main plate (𝐵), the length of the stiffener (𝐿) and the thickness of the stiffener (𝑡).
The weld angle is another possible variable, but mainly the welding are considered to be atΘ = 45°, so the BS standard is only suggesting an𝑀 solution for this angle (see AppendixA.3).
The initial conditions are limiting the𝐿/𝑇 ratio between 0.5 and 2.75, this boundary is placed because the empirical equations for𝑀 is derived by Bowness and Lee [5,6]. The FEM analysis needed to find the fitting equation was limited to an𝐿/𝑇 ratio of 2.75. The graphs from the report [5] are showing a good convergence toward the high values, but no precise result is known. So, for values of𝐿/𝑇 higher than2.75 the limit value is used in the formula.
Figure 3.3 – Transverse stiffener used by Bowness and Lee to derive the equation [6]
Moreover, the reference paper and report by Bowness and Lee [5,6] is deriving the equation from a ”transverse stiffener” (see Figure3.3), which is geometrically different from the ”longitudinal stiffener” being analyzed in this research paper (see Figure3.1). It has been observed what seems an erroneous stress intensity factor computation determined from the transverse stiffener, this problem will be further analyzed in Section6.1.
3.1.2. Initial flaw dimension
The initial flaw dimension is the most critic value for the crack assessment. The validity limit of the Newman-Raju empirical formula and𝑀 factor require:
0.1 ≤ 𝑎/𝑐 ≤ 1.0 0.005 ≤ 𝑎/𝑡 ≤ 0.9 0.5 < 𝐿/𝑇 ≤ 2.75 𝑐/𝑏 < 0.5 (3.1) where the symbols are taken from figure3.1. Three out of four boundaries are considering the initial half-crack length𝑐 or crack depth 𝑎 . The model was checked against different initial flaw sizes. In
3.1. Model parameters 21
figure3.4the varying initial depth ratio shows how the life changes according to different values. The initial crack ratio is kept constant, with a value of𝑎/𝑐 = 0.3, as suggested in literature results [12,43]. As we can see in figure3.4, the initial crack depth has a high influence on the final fatigue life results. If the depth from a real crack is known, it can be used as initial reference. One more technique to decide the initial crack depth in a welded component is explained by Smith and Smith [46], the experimental analysis of many weld toes shows a constant depth. The weld always deform the basic plate with a small flaw of45 𝜇𝑚 along the whole weld toe. This value of 𝑎 = 0.045 𝑚𝑚 is a valid initial depth up to a plate thickness of𝑇 = 9 𝑚𝑚.
0
2
4
6
8
10
N [cycles]
10
40
0.1
0.2
0.3
0.4
0.5
2c/B [mm]
a/t = 0.005
a/t = 0.01
a/t = 0.02
a/t = 0.04
a/t = 0.07
a/t = 0.1
a/t = 0.2
Figure 3.4 – Fatigue life comparison for different initial depth - / .
In figure3.5the difference in initial crack ratio is shown. The initial crack depth was kept constant at a value of𝑎 /𝑇 = 0.005 𝑚𝑚, the minimum possible value for our model. The results of the varying ratio show that the initial𝑎 /𝑐 is of minor importance, since all the results converge after 4 ⋅ 10 cycles. The final number of cycles to failure is not exactly the same but quite similar. The initial ratio𝑎/𝑐 = 0.3 is the average result and the closest to the initial convergence value. Even in experimental results it has found to be a correct initial ratio [12,43].
3.1.3. Load and boundaries
The MATLAB model requires the loading conditions to be specified. The boundaries conditions are implicitly set to a standard tension-only fatigue life test. One of the two edges of the main plate is completely fixed, either clamped or bolted. The other edge of the main plate is attached to an hydraulic cylinder reproducing a cyclic load. The load can be set in MATLAB model as an initial value. The load ratio𝑅 is required together with the maximum 𝜎 or minimum stress 𝜎 . This information combined results in the stress rangeΔ𝜎, needed to calculate the stress intensity factor.
3.1.4. Material
The material is considered in the MATLAB empirical model through the Paris law. This equation uses different parameters (𝐶 and 𝑚) depending on the type and conditions of the main plate material. The weld material is not anyhow considered in this empirical approximation, since the crack develops in the main plate and the concentration factor is dependent only upon the weld angle. As pointed out in section2.2.3and2.4.1, following the original Paris law equation, many other variations have been
0
2
4
6
8
10
N [cycles]
10
40
0.2
0.4
0.6
0.8
1
a/c
a
i/c
i= 0.1
a
i/c
i= 0.2
a
i/c
i= 0.3
a
i/c
i= 0.4
a
i/c
i= 0.7
a
i/c
i= 1
Figure 3.5 – Fatigue life comparison for initial flaw size - / .
provided. The British Standard 7910 suggests to use a 2-steps Paris law for steel in air (Section
2.4.1), this solution have been tested against a 1-step Paris law suggested in BS 7608 [11] for steel in air (Equation3.2), with a lower threshold value of Δ𝐾 63 𝑁𝑚𝑚 / . The upper stress intensity factor limit is given by theΔ𝐾 , above this value the crack is considered unstable and no precise life prediction is possible. In our model, the critic stress intensity factor is considered a boundary, if any Δ𝐾 overcome the threshold, immediately the simulation stop and the specimen is considered broken. The reference value used for steel is an average for high strength steels found on eFunda website [15]. British Standard suggests not to use any upper limit in the crack growth computation, this solution seems a bit unrealistic, that is why theΔ𝐾 = 3.162 ⋅ 10 𝑁𝑚𝑚 / have been chosen.
𝑑𝑎
𝑑𝑁 = 5.21 ⋅ 10 ⋅ Δ𝐾 (3.2)
The fatigue life results using the 2-steps or the 1-step is different, it is of utmost importance to under-stand which is the most correct law for our model. In Section3.2.2and further on in6.1the results for the two laws is shown, it is clear than that the 1-step law is more conservative and precise in the validation and in the experimental results.
3.2. Validation
The empirical model was assembled from different equations coming from different papers. The vali-dation is needed in order to be able to correctly reproduce the final experiment and to make sure the equations combined are correctly representing experimental cases. Three references are chosen to validate in the following order the stress intensity factor, the𝑀 factor and the fatigue life are validated. Each solution found in literature highlight a different trend or value that is correctly reproduced by our model.
3.2.1. Maddox [
31
] - Stress Intensity Factor trend
Maddox [31] analyze a 2D plate with transverse stiffener with different weld angles. The graph in Figure
3.2. Validation 23
found by our empirical MATLAB model, shown in Figure3.7. In the reference graph (Figure3.6), since a 2D model is used, only the𝐾 at the deepest point of the crack is shown. 𝐾 is correctly higher than𝐾 in Figure3.7, this is given by the notch concentration factor found at the weld toe and so corresponding with the𝑐 surface point.
Figure 3.6 – Relative Stress Intensity Factor calculated
by Maddox [31] —• - ° fillet — × - ° fillet — solutions for edge cracked plate
0 0.2 0.4 0.6 0.8 1 a/T 0 1 2 3 KI(a) KI(c)
Figure 3.7 – Relative Stress Intensity Factor computed
with MATLAB empirical model for °
3.2.2. Fu et al. [
19
] - Weld Magnification Factor trend
Fu et al. [19] have analyzed a transverse stiffener (Figure3.3) on top of a plate. A 3D finite element model was used, and the Virtual Crack Extension (VCE) method in ABAQUS FEA software gave the energy rate needed to compute the Stress Intensity Factors. The goal of Fu et al. [19] was to develop an analytic weld magnification factor. By experimenting with the FEM model, they have shown an interesting trend for the Stress Intensity Factor along the crack front in a semi-elliptical crack. Figure
3.8shows the𝐾 and𝐾 for a surface crack in a plane plate (- - dotted line) and for a transverse butt joint (— solid line). The𝐾 is higher than 𝐾 because the surface point, where the stress is computed, is on the weld toe line, where the notch stress has the higher influence. This raise in stress is correctly shown in our MATLAB model,𝐾 is higher than𝐾 in Figure3.7as well as in Figure3.10.
Figure 3.8 – Normalized distributions for surface crack in a plane plate (- -) and in a transverse butt joint (—) –
/ . , / . and .
The Weld Magnification Factor has been described in Section2.3.1 and extensive formulas are found in AppendixA.3.
Fu et al. [19] calculated the𝑀 values for a crack growing, subject to tension load and a fixed elliptic ratio of𝑎/𝑐 = 0.2. The values along the crack front are normalized as they were placed at the deepest
point with the following formula: 𝑦
𝑇 = 𝑎
𝑇𝑠𝑖𝑛Θ (0 ≤ Θ ≤ 90°) (3.3)
where𝑎 and 𝑇 are the flaw depth and plate thickness, while Θ is the angle between the surface and the point along the crack front (see Figure2.12). This result is comparable to the𝑀 factor found with the MATLAB model (Figure3.10).
Figure 3.9 – Weld magnification factor calculated by Fu
et al. [19] — Tension load - / .
0 0.2 0.4 0.6 0.8 a/t 0 2 4 6 M k M ka Mkc
Figure 3.10 – Weld Magnification Factor computed
us-ing the empirical model
3.2.3. Smith and Smith [
47
] - Fatigue life comparison
Smith and Smith [46,47] have researched about the same geometry considered in our case, a plate with two symmetrical non-loadcarrying longitudinal stiffeners welded on top. The findings of those two papers are quite useful for validation and for general knowledge about the topic. Smith and Smith [46] analyzed nine different weld toes for a total of 278 defects, every section was measured with a microscope and the flaw depth at the end of the weld toe measured (see Figure3.11). The average result is0.045 𝑚𝑚, where 𝑎/𝑇 = 0.0045 for the thickness found in Smith (𝑇 = 10 𝑚𝑚). The crack depth over thickness ratio is close to𝑎/𝑡 = 0.005, the lower validity limit of our MATLAB model. This means that the initial flaw depth is known for this experiment, is then possible to reproduce the crack growth experiment and validate our empirical model.
Table3.1shows the values used as input load in the MATLAB model. The geometry of the specimen is shown in Figure3.12. Figure3.13shows the results of the experiments run by Smith and Smith [47] (• black dots) and the output of the empirical model (blue diamonds). The output from the model is slightly conservative, since always yield a lower fatigue life. This is not a negative trend, since we are looking at a model, being conservative always help to do not take risks in the assessment. Even more, the results obtained from Smith and Smith [46] are purely experimental, some fluctuation in the results is expected. For example, test number 3, 6 and 8 have an experimental fatigue life which is 2.5 times higher then the one computed with the model. This can be given by the slightly different material composition, or test set up, or weld dimensions. All those possible disturbances are derived from the human action.
3.3. Conclusion
In this chapter, at first, the parameters of the empirical model have been analyzed. Section3.1.2shows how crack growth life is sensible to the initial flaw dimensions. The number of cycles obtained starting with a flaw of𝑎/𝑡 = 0.005 is almost 5 times more than the one obtained starting with 𝑎/𝑡 = 0.2. Fur-thermore, the initial crack ratio has shown not to be of huge importance if the fatigue life is higher than 4 ⋅ 10 , all the results are converging to a ratio of 𝑎/𝑐 = 0.3 The material constants used in the Paris Law are found in the British Standard, they seem to be correct for the steel we are considering, but further precision could be achieved by having experimental crack growth results for the same material. The validation process has overall seen a correct trend in the Stress Intensity Factor curve at the begin of the crack growth. The Weld Magnification Factor has the same trend found in Fu et al. [19],
3.3. Conclusion 25
Figure 3.11 – Longitudinal section of the weld toe
(B-B in Figure3.12) – Depth of the flaw at the weld toe highlighted
Figure 3.12 – Specimen used for validation purpose (see
Smith and Smith [47])
Table 3.1 – Experimental setup and results for Smith and Smith [46] compared to the results obtained with empir-ical model
Stress range Stress ratio Smith and Smith [46] MATLAB
Test Δ𝜎 𝑅 = 𝑆 /𝑆 𝑁 𝑁
No. 𝑀𝑃𝑎 10 cycles 10 cycles
1 62 0.67 41 41 2 79 0.60 23 19.7 3 80 0.56 50 19.0 4 90 0.50 26 13.3 5 121 0.25 9.3 5.48 6 129 0.17 15 4.52 7 144 0.14 7.3 3.25 8 183 0.07 4.0 1.58
furthermore, the value of𝑀 at the crack surface is correctly higher then the one found at the deepest point, because of the high influence of the notch stress at the weld toe. Finally the crack growth life is compared to the results obtained by Smith and Smith [46], showing a slightly conservative result, against the experimental values given by the reference. This solution is believed to possibly achieve a better fitting if using a most accurate𝑀 equation in the model [22]. The plasticity factor at the crack tip can be considered in further researches, as well as additional type of crack growth laws [8].
10
510
610
7N [cycles]
40
60
80
100
120
140
160
180
200
[MPa]
Validation MATLAB Empirical Model [S-N graph]
Smith & Smith, 1982
Emprical model
4
Finite element model without crack
The first attempt to obtain a Finite Element Model is taken using ANSYS Mechanical APDL software. The goal of this modeling is to obtain good results in terms of through thickness and surface stresses. The reference for validation will be the stress concentration factor at the weld toe, the hotspot stress at weld toe and the effective notch stress. The FEM model is created through ANSYS APDL scripting technique, leaving the possibility to change all the main parameters in case of different dimensions or material properties. Once the through thickness stress is obtained, the weight function technique can be used to calculate the crack growth. This latest technique is using empirical formulas, together with the stresses from the FEM model, to quickly compute the stress intensity factor.4.1. Model parameters
The parametric script uses ANSYS Mechanical APDL commands to create the model, the mesh, set the boundaries and solve. The main parameters open to the user decision are described in the following section. The overall geometry is fixed, as shown in Figure4.1, but it is possible to change dimensions, material properties, load conditions and mesh refinement.
4.1.1. Stiffener geometry
The geometry reproduced by the scripts is just an eight of the complete model. This quicker solution is possible thanks to the symmetry of the specimen. Many different parameters can be changed in order to create different geometries, Figure4.1shows them.
Regarding the geometry of the model, two possible ways to simulate the weld and the stiffener were found in literature. The weld corners can be shaped as a cone or as a pyramid, while the stiffener itself can be completely attached to the main plate or partially attached only through the welding surface. In literature many solutions are found, in Table4.1there is a comparison between the four main different type. The attached stiffener solution seems to be the most used, the reason is probably a less cumber-some procedure needed to model the geometry in the FEM software. The most used corners shape is the pyramid, probably for the same reason as the previous choice, this solution require less time in modeling. In our model two combinations have been tested:
1. Cone corners – Attached Stiffener (Figure4.2- Detail4.3) 2. Pyramid corners – Detached Stiffener (Figure4.4- Detail4.5)
No precise decision can be deducted from the previous works, for convenience, both shapes will be analyzed and the one giving the best fitting results will be used.
4.1.2. Materials
Materials in FEM models have to be set for different meshes. Since the specimen and the experiment we are trying to reproduce does not give precise hints on the materials, parameters have been intro-duced in order to be able to simulate different situations. It is possible to set two materials, the first one for the plate and stiffeners, which are known to be of the same material, and second one for the weld. Since the weld material is unknown as of now, a safe assumption is to use the same material given for
28 Finite element model without crack
Lp/2
Bp/2
Tp/2
La/2
Ha/2
ta/2
Ww
Hw
A
A
B
B
C
C
D
D
E
E
F
F
4
3
2
1
DISEG. VERIF. APPR. FABB. Qual. SE NON SPECIFICATO: QUOTE IN MILLIMETRI FINITURA SUPERFICIE: TOLLERANZE: LINEARE: ANGOLARE: FINITURA: INTERRUZIONE BORDI NETTINOME FIRMA DATA
MATERIALE:
NON SCALARE DISEGNO REVISIONE
TITOLO: N. DISEGNO SCALA:1:5 FOGLIO 1 DI 1
A4
PESO:3D_Crack
Figure 4.1 – Geometry and parameters of an eight of the model, as used in ANSYS Mechanical APDLTable 4.1 – Comparison between different FEM geometries found in literature
Cone Pyramid
Corners Corners
Detached Stiffener [21] [11], [31], [24]
Attached Stiffener [12], [14], [24], [52] [5,6], [11], [19], [34]
Figure 4.2 – Geometry with cone corners and attached
stiffener
Figure 4.3 – Detail of cone corners and attached
stiff-ener
the plates. Since data are known for a tensile test on the plate, it is safe to assume that we are dealing with high strength steel, with a yield stress of375 𝑀𝑃𝑎 and ultimate strength of 522 𝑀𝑃𝑎. The Young’s elastic modulus is205 𝐺𝑃𝑎 and the Poisson ratio 0.3. The same characteristics are used for the weld, for the plate and for the stiffener.
4.1.3. Load and boundary
The specimen under investigation is subject to a pure tension loading. This load condition is reproduced in the FE model by applying a uniform outward pressure on one side, as shown in red in Figure4.6.
4.1. Model parameters 29
Figure 4.4 – Geometry with pyramid corners and
de-tached stiffener
Figure 4.5 – Detail of pyramid corners and detached
stiffener
The arbitrary pressure is1 𝑀𝑃𝑎, so the hotspot stress and concentration factor can be easily derived. The boundary conditions are dictated by the symmetry of the model. The symmetry planes have the displacement constrained in the out-of-plane direction, as can be seen in Figure4.6.
Figure 4.6 – Boundary conditions found in the FEM model without crack
4.1.4. Mesh refinement
The FEM model is composed by a finite number of elements which produce the full geometry. The goal is to obtain results which are close to reality, in order to achieve so, the mesh has to be refined and validated. By acting on two parameters in the script, es (element size) and div (number of divisions), the trend of Stress Concentration, Hotspot Stress and Effective Notch Stress have been studied. All
