About this Journal Submit a Manuscript Table of Contents
Advances in Mechanical Engineering
Volume 2013 (2013), Article ID 537493, 10 pages
Research Article

Numerical Simulation on the Residual Stress Induction due to Welding Process and Assessment by the Application of the Crack Compliance Method

Instituto Politécnico Nacional, Sección de Estudios de Posgrado e Investigación, Escuela Superior de Ingeniería Mecánica y Eléctrica, Unidad Profesional Adolfo López Mateos Zacatenco, Edificio 5, 2do Piso, Col. Lindavista, 07738 México, DF, Mexico

Received 6 August 2013; Revised 31 October 2013; Accepted 1 November 2013

Academic Editor: Magd Abdel Wahab

Copyright © 2013 Guillermo Urriolagoitia-Sosa et al. This is an open access article distributed under the Creative Commons Attribution License, which permits unrestricted use, distribution, and reproduction in any medium, provided the original work is properly cited.


Residual stresses are mechanical effects that remain in a body after all external loads have been removed. In this sense and because a weldment is locally heated by a welding heat source, the temperature distribution is not uniform and changes as welding progresses. During the welding thermal cycle, complex transient thermal stresses are produced in the weldment and the surrounding joint. With the advancement of modern computers and computational techniques (such as the finite-element and the finite-difference methods), a renewed effort has been made in recent years to study and simulate residual stresses and the related phenomena. This paper discusses the procedure applying a finite element analysis by a 2D model to determine the residual stresses and distortions of steel AISI 316 bars under an arc welding process; additionally, the state of the stresses in the component is determined by the application of the crack compliance method (CCM); this is destructive experimental method based on fracture mechanics theory. This research also demonstrates that the residual stress distribution and the magnitude inducted into the component must be carefully assessed, or it could result in a component susceptible to failure.

1. Introduction

In general, welding is defined as a manufacture or sculptural process that joins components and produces coalescence of materials by heating them to a specific temperature. Several welding techniques have been employed during the past decades to develop numerous products or systems [1]. Nevertheless, for welding industries around the world, the induction of residual stresses and material distortion is a major concern [2, 3]. Due to autoequilibrated conditions that residual stresses provide, during the welding process residual stresses could be detrimental to the integrity and the expected service life of the component structure. It has been clearly established that welding residual stresses may promote brittle fracture, decrease buckling strength, interrupt fatigue life, and promote stress corrosion cracking [4].

Components that are manufactured by a welding process are often under high-cycle fatigue services, where the induction of residual stresses affects directly the fatigue strength of the material [5]. Several factors contribute to the development of detrimental residual stress fields in welded components like a noncontrolled heat input or constraints [6]; Influence of material properties of both (base and welding) metals [7]; be the cause, when a consumable with a low-temperature martensític phase transformation is applied, achieve a high-tensile steel structure [8]; Cases with previous loading history [9, 10]. Additionally, the application of a nonhomogeneous process causes an elastoplastic deformation into both metals, and its intensity could depend on structure, material, and manufacturing factors [4].

Heat flow theory is essential in order to understand, explain, and develop analytically, numerically, and/or experimentally a welding process. Since the pioneering work of Rosenthal, considerable interest in the thermal aspects of welding, was expressed by the engineering and research community [1113]. In this sense, the most critical input data required for welding thermal analysis are the parameters necessary to describe the heat input to the weldment. Some researchers have developed the thermal finite element simulation to investigate the temperature distribution on metal [1417]. Numerical simulation of welding processes enables engineers to predict transient residual stress fields and deformation in structures. Potential applications can be contemplated to control photothermal phenomena or heat transference induced by laser effects even in nanostructures [18]. The results obtained can be applied to evaluate structural misalignments and premature failures due to external agents. However, welding process simulation altogether is not a simple computational task, due to the involvement of multifield interactions such as thermal, mechanical, and metallurgical [1921]. Other factors that make this kind of simulation extremely complex are filler metal deposition, moving heat source, and material behavior at elevated temperature along with geometric nonlinearities. In this sense, several commercially computational programs are available, with a finite element code application such as; ANSYS, ABAQUS, FEMLAB, MSC MARC, ADINA, and SYSWELD, and can be employed to carry out such type of manufacturing process simulation.

The main objective of this paper is to present a methodology for numerical analysis, carry out a coupled study considering the thermal and mechanical effects, and evaluate the residual stress field in welding components. This work is based on the application of the semilinear elastic thermal conditions, which in conjunction with the elastic-plastic mechanical properties reproduce the elastoplastic material behavior the components that induce residual stresses. To develop a proper numerical model, it was necessary to consider real welding process parameters, such as speed, heat input, efficiency, filling material supply, geometrical constrains, material nonlinearities, and different physical phenomena involved. The present work deals with the following main assumptions and features regarding the thermal model.(a)Displacements of the parts during the welding will not affect the thermal distribution of the parts themselves.(b)The material properties considered in this work are those of the material before entering into the liquid phase transformation.(c)Convection effects are considered.(d)The analysis performed is a combination of thermomechanical behavior.

Additionally, the numerical simulation of a welding process requires that the study has to be divided into two parts: transient thermal analysis and elastoplastic mechanical analysis. Nevertheless, to simplify the reproduction of the welding procedure, uncoupled numerical simulations were used. In such uncoupled research, the results of the transient thermal analysis (which include the temperature distribution) will be used for the second analysis together with the temperature dependent mechanical properties of the material.

Lastly, it is important to establish a technique to determine the residual stress field acting into the strip and caused by the welding procedure. In this sense, the crack compliance method (CCM) [2224] was selected to be numerically simulated to determine the acting residual stress field, and a comparison against numerical results is presented to assess the accuracy of both the numerical simulation and the CCM, so later it could be corroborated in an experimental manner.

2. Theoretical Background

2.1. Stress Effect due to Welding Joints

Welding is a locally heated process, and temperature distribution tends to be established in a nonuniform manner which changes as the procedure progresses. During the welding thermal cycle, complex transient thermal stresses are produced in the weldment and the surrounding joint. As the welded section undergoes shrinkage and deformation during solidification and cooling, a typical residual stresses distribution in a grooved weld is presented in Figure 1 [25].

Figure 1: Groove weld. (a) General welding composition. (b) Residual stress distribution along .

The thermal analysis performed by the finite element method is based on the consideration of the first law of thermodynamics; it states that the thermal energy is conserved, so the welding process simulation is based on heat transfer [26], which is expressed by (1) [27] where represents the heat generation, is the temperature, is the thermal conductivity, is the material density, and is the specific heat in the system. The previous equation can be written as where

Three types of boundary conditions are considered as follows.(a)Temperature acting over the surface .(b)Heat flow acting over the surface . where is the normal vector and is the heat flow.(c)Convection of the surfaces acting on the surface (Newton’s law of cooling) where is the film coefficient evaluated at , is the bulk temperature, and is the temperature at the surface of the model. Regarding the differential equation (5), by a virtual change in temperature and integrating over the volume of the element, it defined as where is the volume of the element and is the allowable virtual temperature. Initially, the thermal condition was set up to reach the plastic response of the material considering the mechanical properties conditions. The stress strain relationship is defined by (6) where where = strain vector and = thermal strain vector, The general formulation to determine the stress is given by the following expressions: where The numerical analysis, developed in this research, was a thermomechanical simulation that was divided into two sequentially coupled simulations. A transient nonlinear thermal analysis is performed to capture the thermal behavior, and this is a nodal temperature distribution followed by an iterative structural analysis. An overview of the coupled thermomechanical simulation procedure is shown in Figure 2.

Figure 2: Overview of coupled thermomechanical simulation approach adopted.
2.2. Crack Compliance Method [24]

In addition to the thermal simulation, it was necessary to implement a mechanical simulation to assess the accuracy of the finite element program by the application of the crack compliance method (CCM) and to determine the residual stress field induced into the component. The analytical solution of the CCM can be carried out only when the relaxed strain readings have been obtained by cutting a component with inherent residual stresses. In general, the analysis for the determination of the residual stress field from the strain data collected is performed in two stages, the forward solution stage, followed by the inverse solution stage. These solutions are based on linear isotropic material considerations. A brief summary of the theory relative to the CCM applied in this research follows. Let the unknown residual stress distribution in the beam be represented by the summation of an th order polynomial series [28] as follows: where are the coefficients that have to be obtained and are the power series , and so forth. Legendre polynomials are also used. However, the CCM includes a step which assumes that the stress distribution, , interacting with the crack is known. This known stress field is used to obtain the crack compliance function by using Castigliano’s approach. Therefore, it is required to evaluate the change in the strain energy due to the presence of the crack and the virtual force. One alternative is by means of the Strain Energy Density. Its main factor, , is direction sensitive. It establishes the direction of the least resistance for crack initiation. The stationary value of can be used as an intrinsic material parameter, whose value at the point of crack instability is independent of crack geometry and loading [29]. In the case of an elastic material, the expression for the intensity of the strain energy density field is as follows: This criterion is based on the local density of the energy field at the crack tip, and it does not require any assumption on the direction in which the energy is released. This is suitable for mixed mode loading. For the problem at hand, ; , as the specimen is under mode I. In this way, can be combined with Castigliano’s theorem. The displacement can be determined by taking a derivative with respect to the virtual force as [30] follows: Now differentiating, with respect to the distance , the strain in the -direction is given by [30] The strain (where = crack length and is the distance between the location of the strain gauge and the crack plane) due to the stress fields is known as the compliance function and is given by

Due to the linearity of with , the second term under the integral sign in (15) is the same as in With , therefore, it can be written as follows: is the stress intensity factor due to the residual stress field when the crack depth in the beam is equal to , and is the stress intensity factor corresponding to the same depth due to a pair of virtual forces applied tangentially at a position on the beam where strain measurements will be taken during the CCM cut at the slot where is a geometry dependant function (see (13)): By following the weight function approach, and can be expressed as [31] where and is known as the weight function [32]. So, the is the stress field due to the virtual force . Once the solutions are determined, the expected strain due to the stress components in (11) can be obtained as follows: The unknown terms are determined so that the strain given by (20) matches those strains measured in the experiment at the cut, this is, . In order to minimise the average error over all data points for an th order approximation, the method of least squares is used to obtain the values of . Therefore, the number of cutting increments is chosen to be greater than the order of the polynomial, that is, . This work used with 8 constants and , this being the number of experimental slot cutting depths at which strain readings were collected. The least square solution is obtained by minimising the square of the error relative to the unknown constant [33]:

This gives where and [34] give a linear set of simultaneous solutions, from which values are determined and (11) is then used to determine the residual stress distribution. This numerical procedure was implemented in a FORTRAN program.

3. Numerical Simulation Procedure

The numerical simulation was divided into two parts: the thermal analysis and the mechanical analysis. The main reason is based on the fact that, in the thermal process, the residual stress field will be induced and, in the mechanical analysis (applying the strain data), the residual stress will be determined to corroborate the data provided by the thermal analysis.

Initially, the geometry was developed for the finite element program, and the model is illustrated in Figure 3(a). The beam model was selected because this model has been widely used by the Biomechanical group of the Instituto Politécnico Nacional, and the results obtained on the specimen of 10 mm thickness have been validated in different papers [23, 3538]. The discretization of the bar was performed in a controlled manner, taking care to obtain square elements of 1 mm by 1 mm (Figure 3(b)). The center of the bar was marked, as this is the zone where the CCM is going to be applied.

Figure 3: Simulated geometry. (a) General geometry. (b) Discretized component.

The mesh is developed by 2D second-order finite element; this element has only a temperature degree of freedom at each node. This element is also suitable to be used in a steady state or transient thermal analysis. Convection or heat flux and radiation can be the input in the element faces, and heat generation rates can then be the input as element body loads. The outputs from this analysis are the nodal temperatures, film coefficient average, temperature average, heat flow rate, and so forth. The material properties obtained from this temperature analysis are illustrated in Figure 4.

Figure 4: Thermal properties. (a) Density versus temperature. (b) Specific heat versus temperature. (c) Thermal conductivity versus temperature. (d) Enthalpy versus temperature.

In this research, the transient thermal analysis determines the temperatures and other thermal parameters that change over the time. This type of analysis follows the same principles as the steady state thermal analysis; the main difference is that the applied load changes over the time, and in this specific study the load is the temperature provided by the heat source.

The nodal temperature of the metal elements at the start is equal to the ambient temperature, and the nodal constraints are removed when the elements come under the influence of the heat source [39]. The time step in the analysis is determined by During the heating phase, the time step is kept constant and the heat source was induced moving it from bottom to top with a specified welding speed. For the cooling phase, the time steps increase as the weldments are cooling till they finally reach the ambient or initial temperature. For this case study, an initial temperature is set at 700°C which is high enough to induce the residual stresses into the material (however, the temperature could be set up to a higher level and produce a more intensive effect). The ambient temperature is considered to be 25°C and the convection heat transfer coefficient is 10 (W/m2 K). The heat source is considered to move at a constant velocity of 1 mm/sec.

For the mechanical research development and since the load for the structural analysis is the temperature distribution from the transient thermal analysis, the mesh should be the same for both studies; otherwise, the temperature mapping will be incorrect. The action is just to switch from the finite element thermal model to the structural are with the same nodes and elements. The finite element used for the structural analysis is a 2D second-order element with 8 nodes. This element has the capability to model plasticity, creep, stress stiffening, large deflection, large strain, and birth and death elements. The outputs for the elements are principal stress, equivalent stress, principal plastic strain, principal elastic strains, average plastic strains, and displacements.

The kinematic hardening option is chosen to model the mechanical properties with the elastic and plastic modulus decreasing with temperature; this is the most usual and close way to simulate the material behavior. Additionally, the viscous effect is not considered. A general material model consisting of a nonlinear kinematic and isotropic hardening component as given in (23) and (24), respectively, was used for the mechanical analysis and the application of the CCM. Consider where is the equivalent plastic strain, is the back stress, is the initial kinematic hardening modulus, determines the rate at which kinematic modulus decreases with plastic deformation, is the current yield stress, is the initial yield stress, is the maximum change in the size of the yield surface, and defines the rate at which the size of the yield surface changes as plastic straining develops. Equation (23) describes the translation of the yield surface in the stress space due to the back-stress , while (24) describes the change of the equivalent stress defining the size of the yield surface, , as a function of plastic deformation. The behavior of material properties is described in Figure 5.

Figure 5: Mechanicalthermal properties. (a) Yield strength versus temperature. (b) Ultimate strength versus temperature. (c) Modulus of young versus temperature. (d) Thermal expansion versus temperature.

The solution of the structural analysis is based on the steady loading conditions, which ignore the inertia, damping effects, and so forth. The external load applied to the model is the temperature distribution from the transient thermal analysis. The boundary conditions are critical to determine the residual stresses; therefore, the restrictions should be applied in such a way that there is not a stress concentration on the constrained nodes. The boundary conditions for this analysis were applied to the bottom edges of the model as illustrated in the Figure 6.

Figure 6: Boundary constrains.

The first step in the proposed solution is to apply the temperature and send it to be solved. The second step is to cool down the system by removing the temperature and solve it again. To apply the CCM method, it is necessary to induce a slot, which is developed by deleting elements from top to bottom of the model (Figure 7) [23, 3538]. The slot is induced by deleting a pair of elements of the first row at the center of the piece; the system is sent to be solved and the elastic strain data is recollected at the rear end of the plate (Figure 7). The introduction of the crack will produce strain relaxation data from the reaccommodation of the residual stress field. This step is continued eight more times with the respectively strain data recollection. The total elastic strain data recollected after the nine consecutive cuts was applied in the CCM program, and the residual stress acting into the element was determined and can be assessed against the results obtained by the thermal analysis.

Figure 7: Simulation of the induction of a crack for the application of the CCM.

4. Results

Figure 8 intends to show how the material cools down. The analysis starts with the heat focus applied at the bottom of the model and proceeds to move toward the top of the beam, and once the top of the beam is reached, the heat source is retired and the beam model is left to cool down until it reaches ambient temperature. Figure 8(a) shows the case of the heat source still being applied at that point and the corresponding temperature distribution five seconds after the experiment started, at this time the heat source is at the middle of the beam (velocity of 1 mm/sec). The temperature distribution in Figure 8(b) shows how the beam cools down after the heat source reaches the top and is eliminated. Figures 8(c) and 8(d) show the subsequent cool down of the element as time goes by (25 and 300 seconds, resp.).

Figure 8: Temperature distribution after. (a) 5 seconds into the process. (b) 15 seconds into the process. (c) 25 seconds into the process. (d) 300 seconds into the process.

Figure 9 shows the axial residual stress distribution in , when the piece finally cools down to room temperature. The major stresses are located at the weld area and the surrounding elements.

Figure 9: Axial residual stress distribution in direction (room temperature).

Figure 10 shows a nodal solution of the residual stress along at the welding zone; these are the most significant stresses due to the welding process.

Figure 10: Residual stress distribution at center of component.

Once the residual stress field has been induced into the component, by simulating the introduction of a crack, it was possible to determine the existing residual stress field acting into the component. A crack has been induced in a sequence of 9 steps; each crack step is 1 mm long. Each time material is removed, and the crack will redistribute the residual stress in the material, causing a deformation which can be recorded as a strain at the rear location with respect to the direction where the crack should propagate. The relaxation for the mechanical component developed as strain data, during the 9 cuts, as shown in Figure 11.

Figure 11: Elastic strain relaxation due to the introduction of the slot.

In Figure 12, the residual stress field as determined by the CCM as well as data for the residual stress field determined by the thermal finite element simulation is presented. It can clearly be seen that the data obtained by the CCM is very similar to the thermal analysis, so it can be concluded that the CCM is a potential technique to predict residual stress.

Figure 12: CCM results assess against the numerical distribution.

5. Conclusions

This paper analyzes the residual stress caused by the temperature raise of the welding heat source in a coupled thermal-structural analysis. The finite element analysis as well is a potential methodology to determine the residual stress during the design stage, which saves time and cost in the product development. To develop a coupled thermal-structural finite element analysis, it is important to consider the appropriate thermal properties of the material to obtain a high accuracy temperature distribution during the transient thermal analysis; otherwise, the structural analysis will not predict the residual stress properly.

For a structural analysis, when the external load comes from the temperature distribution, the boundary conditions generate a stress concentration on the displacement constrains; therefore, constrains have to be applied in such way that the stress concentration does not lie on the constrained nodes.

From Figure 9 it can be observed that the bending introduction will tend to be detrimental to the component because a high tensile residual stress field will be left lying on the surfaces of the material.

This research has several applications as the welding process has been widely used in several fields, and generally the thermal residual stress is neglected; however, this research shows that the magnitude of the stresses could produce an early failure in the component function if they are ignored.

Additionally, in this research, the CCM was numerically evaluated; Figure 10 shows a very good correlation with those from the FEM results. The CCM method has proved to be a very good tool to obtain residual stresses when the component is under bending behavior and could be extremely useful to avoid certain problems when it is applied in the laboratory.

Lastly, an additional objective of this work was the convergence evaluation of the numerical solution proposed. Previous papers have evaluated the advantages of the application of the crack compliance method (CCM) when the residual stresses are uniformly distributed over the surface layer. In particular, in this paper, an experimental-numerical approach has been followed and encouraging results have been obtained. Nevertheless, for the case of a welded joint, the residual stress distribution is complex, as the heat that affected zone (HAZ) has a great influence. Therefore, it has been intended to find, by using codes at hand (ANSYS, ABAQUS, FEMLAB, MSC MARC, ADINA, and SYSWELD), which one gives the best results. Such codes are in a continuous process for quality improvement. Everyone knows that the algorithms involved are carefully validated. Therefore, it is considered that the procedures involved in the finite element analysis have already been accepted. So, the research was focused only on the comparison of diverse solutions.

Conflict of Interests

The authors declare that their academic interest is not influenced by any financial gain and that they do not have any conflict on interests.


The authors gratefully acknowledge the financial support from the Mexican government by the Consejo Nacional de Ciencia y Tecnología, Instituto de Ciencia y Tecnología del Distrito Federal and the Instituto Politécnico Nacional. Additionally are very grateful to Mr. Michael Hartman, Dr. Neal Fellows, and Professor John Durodola from Oxford Brookes University, for the advice and time spent in this research.


  1. L. F. Jeffus, Welding: Principles and Applications, Thomson Delmar Learning, 5th edition, 2002.
  2. R. H. Leggatt, “Residual stresses in welded structures,” International Journal of Pressure Vessels and Piping, vol. 85, no. 3, pp. 144–151, 2008. View at Publisher · View at Google Scholar · View at Scopus
  3. D. Deng, “FEM prediction of welding residual stress and distortion in carbon steel considering phase transformation effects,” Materials and Design, vol. 30, no. 2, pp. 359–366, 2009. View at Publisher · View at Google Scholar · View at Scopus
  4. B. Taljat, B. Radhakrishnan, and T. Zacharia, “Numerical analysis of GTA welding process with emphasis on post-solidification phase transformation effects on residual stresses,” Materials Science and Engineering A, vol. 246, no. 1-2, pp. 45–54, 1998. View at Scopus
  5. M. Mochizuki, “Control of welding residual stress for ensuring integrity against fatigue and stress-corrosion cracking,” Nuclear Engineering and Design, vol. 237, no. 2, pp. 107–123, 2007. View at Publisher · View at Google Scholar · View at Scopus
  6. N. S. Boulton and H. E. Lance-Martin, “Residual stresses in arc welded plates,” Proceedings of the Institution of Mechanical Engineers, vol. 133, no. 1, pp. 295–347, 1936. View at Publisher · View at Google Scholar
  7. C. B. Buchalet and W. H. Bamford, “Stress intensity factor solutions for continuous surface flaws in reactor pressure vessels,” Mechanics of Crack Growth, ASTM STP 590, pp. 385–402, 1976.
  8. A. Ota, C. Shiga, Y. Maeda et al., “Fatigue strength improvement of box welded joints by using low transformation temperature welding material,” Welding International, vol. 14, no. 10, pp. 801–805, 2000. View at Publisher · View at Google Scholar
  9. T. L. Teng, C. P. Fung, P. H. Chang, and W. C. Yang, “Analysis of residual stresses and distortions in T-joint fillet welds,” International Journal of Pressure Vessels and Piping, vol. 78, no. 8, pp. 523–538, 2001. View at Publisher · View at Google Scholar · View at Scopus
  10. G. Urriolagoitia-Sosa, J. F. Durodola, and N. A. Fellows, “Determination of residual stress in beams under Bauschinger effect using surface strain measurements,” Strain, vol. 39, no. 4, pp. 177–185, 2003. View at Publisher · View at Google Scholar · View at Scopus
  11. V. Kamala and J. A. Goldak, “Error due to two dimensional approximation in heat transfer analysis of welds,” Welding Journal, vol. 72, no. 9, pp. 440–446, 1993.
  12. N. T. Nguyen, A. Ohta, K. Matsuoka, N. Suzuki, and Y. Maeda, “Analytical solutions for transient temperature of semi-infinite body subjected to 3-D moving heat sources,” Welding Journal, vol. 78, no. 8, pp. 265s–274s, 1999. View at Scopus
  13. R. Komanduri and Z. B. Hou, “Thermal analysis of the arc welding process—part I: general solutions,” Metallurgical and Materials Transactions B, vol. 31, no. 6, pp. 1353–1370, 2000. View at Scopus
  14. H. G. Kraus, “Thermal finite element formulation and solution versus experimental results for thin-plate GTA welding,” Journal of Heat Transfer, vol. 108, no. 3, pp. 591–596, 1986. View at Publisher · View at Google Scholar
  15. P. Tekriwal and J. Mazumder, “Finite element analysis of three-dimensional transient heat transfer in GMA welding,” Welding Journal, vol. 67, no. 7, pp. 150s–157s, 1988. View at Scopus
  16. K. S. Yeung and P. H. Thornton, “Transient thermal analysis of spot welding electrodes,” Welding Journal, vol. 78, no. 1, pp. 1s–6s, 1999. View at Scopus
  17. E. A. Bonifaz, “Finite element analysis of heat flow in single-pass arc welds,” Welding Journal, vol. 79, no. 5, pp. 121s–125s, 2000. View at Scopus
  18. C. Torres-Torres, N. Peréa-López, J. A. Reyes-Esqueda et al., “Ablation an optical third order nonlinearities in Ag nanoparticles,” International Journal of Nanomed, vol. 5, pp. 925–932, 2010. View at Publisher · View at Google Scholar
  19. T. Muraki, J. J. Bryan, and K. Masubuchi, “Analysis of thermal stresses and metal movement during welding—part I: analytical study,” Journal of Engineering Materials and Technology, vol. 97, no. 1, pp. 81–84, 1975. View at Scopus
  20. T. Muraki, J. J. Bryan, and K. Masubuchi, “Analysis of thermal stresses and metal movement during welding—part II: comparison of experimental data and analytical results,” Journal of Engineering Materials and Technology, vol. 97, no. 1, pp. 85–91, 1975. View at Scopus
  21. E. F. Rybicki, D. W. Schmueser, R. W. Stonesifer, J. J. Groom, and H. W. Mishler, “A finiteelement model for residual stresses and deflection in girth butt welded pipes,” Journal of Pressure Vessel Technology, vol. 100, no. 3, pp. 256–262, 1978. View at Scopus
  22. G. Urriolagoitia-Sosa, G. Urriolagoitia-Calderón, J. M. Sandoval-Pineda et al., “Residual stresses in beams (with and without prior history) numerically assessed by the crack compliance method,” Strain, vol. 47, no. 1, pp. e595–e604, 2011. View at Publisher · View at Google Scholar
  23. G. Urriolagoitia-Sosa, A. Molina-Ballinas, G. Urriolagoitia-Calderón, L. H. Hernández-Gómez, B. Romero-Ángeles, and A. Michtchenko, “Numerical and experimental analysis in the manipulation of the mechanical properties for enhancing the mechanical resistance of a material,” Journal of Applied Research and Technology, vol. 9, no. 2, pp. 156–172, 2011. View at Publisher · View at Google Scholar
  24. G. Urriolagoitia-Sosa, B. Romero-ángeles, L. H. Hernández-Gómez, C. Torres-Torres, and G. Urriolagoitia-Calderón, “Crack-compliance method for assessing residual stress due to loading/unloading history: numerical and experimental analysis,” Theoretical and Applied Fracture Mechanics, vol. 56, no. 3, pp. 188–199, 2011. View at Publisher · View at Google Scholar · View at Scopus
  25. G. Labeas and I. Diamantakos, “Numerical investigation of through crack behaviour under welding residual stresses,” Engineering Fracture Mechanics, vol. 76, no. 11, pp. 1691–1702, 2009. View at Publisher · View at Google Scholar · View at Scopus
  26. X. K. Zhu and Y. J. Chao, “Effects of temperature-dependent material properties on welding simulation,” Computers and Structures, vol. 80, no. 11, pp. 967–976, 2002. View at Publisher · View at Google Scholar · View at Scopus
  27. R. W. Lewis, P. Nithiarasu, and K. N. Seetharamu, Fundamentals of the Finite Element Method for Heat and Fluid Flow, John Wiley & Sons, New York, NY, USA, 2004.
  28. W. Cheng and I. Finnie, “An overview of the crack compliance method for residual stress measurement,” in Proceedings of the 4th International Conference on Residual Stress, pp. 449–458, Society for Experimental Mechanics, Baltimore, Md, USA, 1994.
  29. G. C. Sih, Mechanics of Fracture Initiation and Propagation, Kluwer Academic, New York, NY, USA, 1991.
  30. W. Cheng, M. B. Prime, and I. Finnie, “Measurement of residual stresses through the thickness of a strip using the crack compliance method,” in Proceedings of the 3rd International Conference of Residual Stress: Residual Stress III-Science and Technology, vol. 2, pp. 1127–1132, 1997.
  31. H. J. Schindler, W. Cheng, and I. Finnie, “Experimental determination of stress intensity factors due to residual stresses,” Experimental Mechanics, vol. 37, no. 3, pp. 272–277, 1997. View at Scopus
  32. X. R. Wu and A. J. Carlsson, Weight Function and Stress Intensity Factor Solutions, Pergamon Press, Oxford, UK, 1991.
  33. W. Cheng and I. Finnie, “The crack compliance method for residual stresses measurements,” Welding in the World, vol. 28, pp. 103–110, 1990.
  34. W. H. Press, B. P. Flannery, S. A. Teukolsky, and W. T. Vetterling, Numerical Recipes, Cambridge University Press, New York, NY, USA, 1987.
  35. G. Urriolagoitia-Sosa, Analysis of prior strain history effect on mechanical properties and residual stress in beams [Ph.D. thesis], Oxford Brookes University, 2005.
  36. G. Urriolagoitla-Sosa, J. F. Durodola, and N. A. Fellows, “Effect of strain hardening on residual stress distribution in beams determined using the crack compliance method,” Journal of Strain Analysis for Engineering Design, vol. 42, no. 2, pp. 115–121, 2007. View at Publisher · View at Google Scholar · View at Scopus
  37. G. Urriolagoitia-Sosa, G. Urriolagoitia-Calderón, J. M. Sandoval-Pineda et al., “Numerical evaluation of the crack compliance method (CCM) in beams with and without prior history,” Applied Mechanics and Materials, vol. 13-14, pp. 173–182, 2008.
  38. J. M. Sandoval-Pineda, G. Urriolagoitia-Sosa, G. Urriolagoitia-Calderón et al., “Numerical and experimental evaluation of the residual stress relaxation and the influence zone due to application of the crack compliance method,” Journal of Physics, vol. 1811, pp. 52–59, 2009.
  39. L. E. Lindgren, Computational Weld Mechanics: Thermo-Mechanical and Microstructural Simulations, Woodhead, Cambridge, UK, 2007.