Stress Concentration Factors of Dented Pipelines

Proceedings of IPC2006 6th International Pipeline Conference September 25-29, 2006, Calgary, Alberta, Canada IPC2006-10598 STRESS CONCENTRATION FACTORS OF DENTED PIPELINES Bianca de Carvalho Pinheiro COPPE/UFRJ, Ocean Engineering Dept. Ilson Paranhos Pasqualino COPPE/UFRJ, Ocean Engineering Dept. Sérgio Barros da Cunha TRANSPETRO/PETROBRAS ABSTRACT A nonlinear finite element model was developed to assess stress concentration factors induced by plain dents on steel pipelines subjected to cyclic internal pressure. The numerical model comprised small strain plasticity and large rotations. Six small-scale experimental tests were carried out to determine the strain behavior of steel pipe models during denting simulation followed by the application of cyclic internal pressure. The finite element model developed was validated through a correlation between numerical and experimental results. A parametric study was accomplished, with the aid of the numerical model, to evaluate stress concentration factors as function of the pipe and dent geometries. Finally, an analytical formulation to estimate stress concentration factors of dented pipelines under internal pressure was proposed. These stress concentration factors can be used in a high cycle fatigue evaluation through S-N curves. INTRODUCTION Mechanical damage due to external interference is one of the major causes of in service failures in oil and gas pipelines. The defects produced by mechanical damages may be of different types, like dents, excessive out of rounding, smooth localized buckles or wrinkles. Thus, the assurance of a safe pipeline operation is obtained with a consistent assessment of the mechanical damages, avoiding leaks that may cause not only financial loss to the operator but also damage to the environment and population. Additionally, the operator becomes able to decide which damaged sections must be repaired, avoiding flow interruptions for unnecessary repairs. One of the possible failure modes of oil and gas pipelines is the high cycle fatigue due to stress concentration in dented sections. This type of defect can be generated by the impact of an anchor, a rock or any other heavy object, in the case of offshore pipelines, and excavation equipment, in the case of buried pipelines. Cyclic loadings may be generated by fluid pressure and temperature changes and, in the case of marine risers, by the action of waves, wind and streams. The stress concentration factors are mainly function of the pipe and dent dimensions, the material properties and the boundary conditions [1,2]. A great effort has been done to estimate stress concentration factors in dented pipe sections through finite element models [3-5]. However, it was not proposed a practical and fast procedure to obtain stress concentration factors. Some methods to assess the fatigue life of dented pipelines have been discussed by Cosham and Hopkins [6]. Certain presented methodologies to evaluate the fatigue life reduction of damaged pipelines are based in empirical formulations. The others involved numerical simulation and are not of practical or comprehensive application. This work initiated a study to assess the reduction in the estimated fatigue life due to stress concentration in dented pipes. The aim was the determination of stress concentration factors associated with plain dents caused by mechanical damage. With these stress concentration factors it becomes possible to estimate the fatigue life through S-N curves available in literature. Until now, plain dents with a dome shape have been the focus of the study. Initially, a nonlinear three-dimensional finite element model was developed using shell elements to simulate local damage in the pipe and obtain stress concentration factors under internal pressure. The numerical model comprised small strain plasticity and large rotations. The elastic-plastic model was validated through experiments simulating the whole process. Small-scale pipe models were built and instrumented with strain gages to acquire the strain history along denting simulation and 1 Copyright © 2006 by ASME subsequent application of cyclic internal pressure. The numerical results of strain history were compared with those of the experiments to calibrate the elastic-plastic FE model. The finite element model was used to carry out a parametric study for different pipe and damage geometries. The spherical indenter diameter was varied from 25% to 100% of the pipe external diameter, considering pipe diameter to thickness ratios (D/t) ranging from 20 to 60. With the aid of the Buckingham’s Π theorem, the number of involved variables was reduced to develop an analytical formulation to assess the stress concentration factors of damaged pipelines under internal pressure. the strain gages positions. From the results of Table 1, the models were assumed to be 73 mm external diameter and 3.05 mm wall thickness, resulting in an average D/t ratio of 23.93. These average dimensions and the obtained material properties were used to run the finite element analyses. Points of large strain levels around the dented region (pipe middle section) were determined for initial defects with d/D ratios of 5, 10 and 15%, where d is the radial depth of the dent (Fig. 1). The sketch of Fig. 2 shows the instrumentation of the models using four biaxial strain gages (SG1, SG2 SG3 and SG4) symmetrically positioned in relation to pipe middle section, where the axial (x) and circumferential (θ) distances, according to the d/D ratio, are presented in Table 2. EXPERIMENTAL STUDY The experimental study was developed within the workshop of the Submarine Technology Laboratory – COPPE/UFRJ. The experiments comprised the simulation of dents on small-scale pipe models followed by the application of internal pressure. The experimental results were useful to understand the strain behavior during the loading process and to validate the numerical model. Small-scale Models The models were cut off from a SAE/AISI 1020 grade steel pipe string with 5 m of length, 73 mm of external diameter (D) and 3.05 mm of wall thickness (t). Six small-scale models with total length (L) of 510 mm, approximately 7D, were machined. Prior to the experimental tests, their dimensions were measured at selected transverse sections. The obtained average values are reported in Table 1. Model 23A 23C 23D 23E 23H 23I D (mm) 72.91 73.01 73.01 73.01 73.02 73.03 t (mm) 3.06 3.04 3.02 3.05 3.05 3.06 FIGURE 1: SKETCH SHOWING THE DENT DIMENSIONS. D/t 23.86 24.01 24.20 23.95 23.98 23.88 TABLE 1: AVERAGE DIMENSIONS OF THE MODELS. Three longitudinal test coupons were cut off from the pipe string used to manufacture the models and tensile tests were carried out to determine its material properties. Strain gages were used to accurately evaluate the elastic material parameters. The average Young modulus, Poisson ratio and yield stress obtained are equal to 202213 N/mm2, 0.299 and 272 N/mm2, respectively. To investigate the strain behavior during the denting simulation and subsequent application of internal pressure, strain gages were used on the external surface of the smallscale models. The main purpose of the experiments was to acquire high levels of strain during denting simulation, without damaging the gages. Therefore, preliminary finite element analyses of denting simulation were carried out to determine FIGURE 2: SKETCH OF THE STRAIN GAGES POSITIONS. Denting Simulation An experimental set up was developed to simulate initial damages on the small-scale models, creating a localized region of stress concentration. It was comprised by a servo-hydraulic frame, with a 63.2 mm diameter cylindrical rod (indenter) with a spherical tip, and a moving rigid table monitored by an electronic displacement transducer (Fig. 3). The model was carefully laid on the rigid table, so that the resultant dent could be centered in relation to the strain gages. The vertical 2 Copyright © 2006 by ASME displacement of the table was controlled by the servo-hydraulic frame. The test signals of the strain gages, the displacement transducer and the frame LVDT (Linear Variable Differential Transformer) were transferred to a data acquisition system connected to a PC. Model 23A 23C 23D 23E 23H 23I d/D (%) 5 5 10 10 15 15 x (mm) 13.0 13.0 17.0 17.0 18.0 18.0 θ (o) 18.0 18.0 22.5 22.5 27.0 27.0 TABLE 2: PLANNED DENT DEPTHS AND STRAIN GAGES POSITIONS. FIGURE 4: SMALL-SCALE MODEL AFTER BEING DENTED. Internal Pressure Tests The strain variation under internal pressure around dented region of the small-scale models was investigated with the aid of an experimental set up (Fig. 5). It was composed of two end plugs with external grips that generate axial load under internal pressure, simulating a pressure vessel condition. An electronic pressure transducer attached to one end plug monitored the pressure inside the pipe while a hand operated hydraulic pump imposed controlled pressurization of the model. The test signals of the strain gages and the pressure transducer were transferred to a data acquisition system. FIGURE 3: EXPERIMENTAL SET UP FOR DENTING SIMULATION. It can be verified in Fig. 4, showing the resulting dent in one model, that the indenter has punched very near the gages. Moreover, the strain levels obtained were even greater than 5%, what led in many cases to the detachment or loss of some gages. Obviously, placing gages far from the damaged region would prevent this inconvenience, but also would drive the measurements away from the area of higher strain levels. In view of this, it may be verified in Table 3 that the initial dents didn’t coincide with the planned values (Table 2), since the tests were conducted within the strain gages limits. Table 3 reports the residual strains after the spring back of the models, where the symbol (-) means a lost gage. In spite of the limitations of the adhesive used to fix the gages, strains of up to 7% were measured. Based on the position of the gages (Fig. 2), it can be seen that the strains tangent to the perimeter of the dent are always compressive, while its counter parts are positive. FIGURE 5: EXPERIMENTAL SET UP FOR INTERNAL PRESSURE. The models 23C, 23D and 23I were selected to be tested under internal pressures raging from 0 to 50% of MOP (maximum operating pressure). MOP was adopted as the pressure corresponding to the stress given by 72% of the specified minimum yield strength (typical value for recommendation codes). Based on the estimated yield stress of 3 Copyright © 2006 by ASME 272 N/mm2, it was defined an internal pressure ranging from 0 to 8.20 N/mm2 (1189 psi). As the internal pressure provides the “rerounding” effect on the dented region of the pipe, i.e., the pipe wall undergoes further plastic strain, recovering partially its initial circular shape, the experiments were carried out in two cycles. The pipe was pressurized from 0 to 8.20 N/mm2 in each cycle. It may be assumed that the final rerounded state of the dent is reached early [2]. Although Rosenfeld [7] has noted longer shakedown times in certain cases, the application of initial high pressures in finite element models will induce early large plastic deformation. It can be verified in Fig. 6, for instance, where the applied pressure is plotted versus the accumulated hoop strain (model 23I), that the analyzed region works plastically at the first cycle and elastically at the second. At the first cycle, the pipe undergoes the amount of rerounding corresponding to the applied maximum pressure. Subsequently, the strain behavior suggests the occurrence of the phenomenon of progressive plastic deformation (ratcheting). In spite of this, dented steel pipes under cyclic internal pressure may be considered to deform elastically if the maximum internal pressure is not increased. 9 8 Model 23I - 0o Hoop SG2 Pressure (N/mm2) 7 6 5 4 3 2 1 0 -0.062 -0.058 -0.054 Model Geometry The two basic components of the FE model are the pipe and the indenter. The pipe is defined by the diameter of the middle surface (Dms) and the wall thickness (t). A pipe longitudinal length of, approximately, 7D was adopted. This longitudinal length was selected based on preliminary analyses in order to minimize any interaction between the damaged region and the pipe edges. To simulate the indenter, an analytical rigid surface with a spherical shape was used. The contact between the pipe and the rigid surface was simulated with the aid of contact surfaces. To minimize computational time in the numerical analyses, a quarter-symmetry model was used, considering planes of symmetry in the longitudinal and transversal directions, planes 1-2 and 2-3, respectively. Therefore, the solid continuum discretized is half length and half diameter of the actual pipe (Fig. 7). Finite Element Mesh Since shell elements may be assumed whenever the diameter to thickness ratio is 20 or higher, solid continuum elements were not used in the analyses. Then, it was generated a three-dimensional shell model discretized by the ABAQUS S8R5 second-order quadrilateral thin shell element [8], with five degrees of freedom per node (three translations and two insurface rotations). This element type converges to thin shell theory as the thickness decreases (the Love-Kirchhoff hypothesis is satisfied numerically). The change in thickness with deformation is ignored in this element. The finite element model developed assumes large rotations (geometric nonlinearity), but admits only small strains, according to the formulation of the element being employed. The mesh is more refined at the dented region of the pipe and presents a smooth transition to a coarser mesh at the end of the pipe. Figure 7 shows the finite element mesh and the analytical surface that simulates the indenter. A mesh sensitivity study determined that one element at each 5 degrees in the damaged region is enough to accurately evaluate the stress concentration factors. An aspect ratio of 1 to 1 was kept for these elements. -0.05 Strain FIGURE 6: EXPERIMENTAL HOOP STRAIN OF MODEL 23I UNDER INTERNAL PRESSURE. NUMERICAL MODEL A numerical model was developed to determine stress concentration factors in dented pipes under internal pressure. It comprises a three-dimensional shell type elastic-plastic model, based on the finite element method, developed through the mainframe ABAQUS release 6.4 [8]. The model accuracy was evaluated from a correlation between numerical and experimental results. FIGURE 7: FINITE ELEMENT MESH AND THE INDENTER. 4 Copyright © 2006 by ASME In order to accurately model the pipe response to denting, spring back and cyclic pressurization, a constitutive behavior incorporating plasticity was used within the potential flow rule. The von Mises yield function under combined isotropic and kinematic hardening was assumed. As the rerounding effect during the first cycle of pressurization confers reverse plastic deformation to the structure, the Bauschinger effect must be taken into account. Cyclic uniaxial tensile tests were not carried out, but an approximation provided by an ABAQUS routine, using only half cycle, can estimate this effect within the kinematic hardening theoretical approach. Boundary Conditions and Loading The model simulates the following load steps: indentation, removal of the indenter (spring back), and two cycles of internal pressure. Initially, the indenter punches the pipe external surface generating stress levels greater than the yield stress of the material. Figure 8, for instance, shows the FE results of von Mises stresses at dented region (outer surface) for one of the experimental models, where the stresses reached values up to 533 N/mm2 at the indentation step. When the indenter is removed the pipe wall returns elastically, but the geometry remains partially deformed according to the intensity of the indentation and the level of plasticity attained. Finally, two equal cycles of internal pressure are applied, conferring the rerounding effect (first cycle) and an elastic displacement (second cycle) at the dented region. Two boundary conditions may be applied at the pipe edge: axially constrained and closed edge (pressure vessel simulation). In the first case, the nodes of the pipe edge are left constrained to move in axial direction. In the last case (pressure vessel), a force identical to that caused by an end cap is imposed. This load is applied by coupling the edge nodes to a reference node placed in the center of the pipe edge. The load is directly applied at the reference node and transmitted to pipe edge. Model 23A 23C 23D 23E 23H 23I Exp. Num. Exp. Num. Exp. Num. Exp. Num. Exp. Num. Exp. Num. d/D (%) 4.22 3.80 6.93 6.40 10.03 9.06 7.05 6.40 9.62 9.06 12.37 11.74 SG1 SG2 Hoop -2.79 -2.68 -3.09 -5.14 -6.15 -5.29 -5.06 -3.44 -3.15 -3.05 -4.38 -5.06 -7.02 -6.09 -7.42 FIGURE 8: FE RESULTS OF VON MISES STRESSES FOR THE INDENTATION OF MODEL 23I. CORRELATION BETWEEN NUMERICAL AND EXPERIMENTAL RESULTS In order to reproduce the experimental tests, the finite element model was generated using the material properties, boundary conditions and average dimensions of the experimental models. The stress-strain data was determined through uniaxial tensile tests of the material and represented using true stress and logarithmic plastic strains. The numerical results were compared with those obtained from the experimental tests. Initially, the results of the denting simulation were correlated with the residual strains and displacements of the numerical analyses (Table 3). Some observed discrepancies can be attributed, to some extent, to the gages positions, since the prescribed values in Table 2 may have not been obtained precisely in practice. Small deviations from the planned position may have caused significant differences in strain, since large strain gradients were observed in this region with the FE simulations. Residual Strains (%) SG2 SG3 SG4 Axial Hoop 2.27 2.27 1.48 1.45 2.59 1.51 3.38 3.10 1.65 2.03 4.07 2.19 4.20 2.52 4.20 2.80 3.08 2.92 2.11 2.21 2.93 2.20 3.75 2.49 4.20 2.88 4.70 4.71 5.44 3.33 SG1 SG3 SG4 Axial -1.18 -1.61 -1.32 -2.34 -2.20 -2.42 -2.42 -2.53 -1.81 -1.90 -1.59 -2.33 -2.15 -2.39 -2.61 -2.98 TABLE 3: NUMERICAL AND EXPERIMENTAL RESULTS OF RESIDUAL STRAINS AND DISPLACEMENTS AROUND THE DENTED REGION. 5 Copyright © 2006 by ASME 6 8 Model 23D - 0o Hoop SG2 Hoop (Numerical) Axial SG2 Axial (Numerical) 7 5 Displacement (mm) Displacement (mm) 6 Model 23E - 0o Hoop SG1 Hoop SG2 Hoop (Numerical) Axial SG1 Axial SG2 Axial (Numerical) 5 4 3 4 3 2 2 1 1 0 -0.06 -0.02 0.02 0 -0.04 0.06 -0.02 Strain FIGURE 9: DISPLACEMENT OF THE INDENTER VERSUS STRAIN FOR THE MODEL 23D (SG2). 0.02 0.04 FIGURE 11: DISPLACEMENT OF THE INDENTER VERSUS STRAIN FOR THE MODEL 23E (SG1 AND SG2). 8 6 Model 23D - 22.5o Hoop SG3 Hoop SG4 Hoop (Numerical) Axial SG3 Axial SG4 Axial (Numerical) 6 Model 23E - 22.5o Hoop SG3 Hoop SG4 Hoop (Numerical) Axial SG3 Axial SG4 Axial (Numerical) 5 Displacement (mm) 7 Displacement (mm) 0 Strain 5 4 3 4 3 2 2 1 1 0 -0.04 -0.02 0 Strain 0.02 0 -0.03 0.04 FIGURE 10: DISPLACEMENT OF THE INDENTER VERSUS STRAIN FOR THE MODEL 23D (SG3 AND SG4). -0.02 -0.01 0 0.01 0.02 0.03 Strain FIGURE 12: DISPLACEMENT OF THE INDENTER VERSUS STRAIN FOR THE MODEL 23E (SG3 AND SG4). 6 Copyright © 2006 by ASME experimental strains. It proves that the thin shell FE model developed can reproduce accurately the wall pipe straining, even for a D/t ratio of approximately 24. Finally, there were compared the experimental and numerical strain behavior under internal pressure. These results are presented in Figs. 13 and 14 for model 23D. Unfortunately, several gages were not preserved for the pressurization test, but the few results available proved that the numerical model can reproduce the experiments within engineering accuracy. In fact, since the reversed behavior was not evaluated through the uniaxial tensile tests of the material, the amount of strain due to dent rerounding is not precisely determined by the numerical model. On the other hand, it will only affect the residual strain simulated. The stress concentration factors to be determined are mainly dependent on the elastic strain change under cyclic internal pressure and this variation can be precisely determined. 9 o 8 Model 23D - 0 Hoop SG2 Hoop (Numerical) Pressure (N/mm2) 7 6 5 4 3 2 1 0 -0.054 -0.05 -0.046 Strain -0.042 FIGURE 13: INTERNAL PRESSURE VERSUS HOOP STRAIN FOR THE MODEL 23D (SG2). 9 o 8 Model 23D - 22.5 Axial SG3 Axial (Numerical) Pressure (N/mm2) 7 6 5 4 3 2 1 0 -0.026 -0.024 -0.022 -0.02 Strain FIGURE 14: INTERNAL PRESSURE VERSUS AXIAL STRAIN FOR THE MODEL 23D (SG3). The strains observed during indentation of models 23D and 23E are shown in Figs. 9 to 12, where a comparison of the numerical and experimental results is made. In general, the graphs showed good agreement between numerical and PARAMETRIC STUDY After the validation of the numerical model it was possible to carry out a parametric study to determine stress concentration factors, referred to the von Mises equivalent stress, for different dent and pipe geometries. The experiments and the numerical simulation showed that dented steel pipes under cyclic internal pressure may be considered to deform elastically after the first cycle, if the maximum internal pressure is not increased. It shows that stress concentration factors may be obtained from simple linear elastic analyses. In this case, the dented pipe geometry is assumed as an initial configuration of the FE mesh and, consequently, the effect of residual stresses due to the indentation step is neglected. To generate the dented pipe geometry for the elastic analysis, the elastic-plastic FE model was run with the following steps: indentation and removal of the indenter. The obtained deformed geometry (after spring back) was then used as the initial geometry for the elastic analysis. The elastic model has only one load step that comprises the application of a small internal pressure, sufficient to generate the elastic response of the model. This procedure was used to carry out a parametric study for different dimensions of initial dents and pipe geometries. The pipe geometric parameters adopted were D/t ratios equal to 20, 30, 40, 50 and 60. The model was set with a longitudinal length of 10D (5D, considering the symmetry condition). This length is considered sufficient to prevent any interaction between the dent area and the pipe edge. The boundary condition at the pipe edge was adopted as axial constraint. The indenter was considered with a spherical shape with diameters of 0.25, 0.50, 0.75 and 1D. The elastic properties adopted were a Young modulus of 205,000 N/mm2 and a Poison ratio of 0.3. A small internal pressure was applied (0.1 N/mm2) to obtain the peak (maximum) von Mises equivalent stress and calculate the stress concentration factor. 7 Copyright © 2006 by ASME 10 9 8 7 Kt 6 5 Φ = 0.25D D/t = 20 D/t = 30 D/t = 40 D/t = 50 D/t = 60 4 3 2 1 0 20 40 FIGURE 15: DENT DIMENSIONS AT HALF DEPTH. as: The theoretical stress concentration factor (Kt) is defined K t = σ max σ nom 60 80 100 (ldw)/(D2t) FIGURE 16: Kt FOR Φ = 0.25D. 12 (1) 11 10 9 8 7 Kt where σmax is the peak (maximum) stress and σnom is the nominal stress [9]. Here, the nominal stress is assumed to be equal to that of a thin walled circular cylinder under internal pressure. The stress concentration factors (Kt) were plotted against the term (ldw)/(D2t), where the parameters l and w correspond, respectively, to the length and width of the dent evaluated at d/2 (Fig. 15). The term (ldw)/(D2t) was proposed by Rinehart and Keating [2] and appointed to be inversely proportional to pipe fatigue life. This term is the product of the terms d/D, w/t and l/D. Figures 16 to 19 show the curves of stress concentration factors (Kt) against the term (ldw)/(D2t) for indenter diameters (Φ) ranging from 0.25D to 1D. The obtained results are consistent with the behavior observed in [2], since the term (ldw)/(D2t) is directly related to the stress concentration factors, which are inversely related to the fatigue life. Besides the quality of the obtained curves (smooth and continuous) the used parameter represents the complete geometry of the dent and the pipe. 6 Φ = 0.50D 5 D/t = 20 D/t = 30 D/t = 40 D/t = 50 D/t = 60 4 3 2 1 0 20 40 60 80 100 120 140 2 (ldw)/(D t) FIGURE 17: Kt FOR Φ = 0.50D. 8 Copyright © 2006 by ASME σ max = f (σ nom ,d,l,w,D,t ) 12 11 (2) From Buckingham’s Π theorem this can be reduced to a relationship between non-dimensional variables, such as: 10 9 σ max ⎛D d l ⎞ = F⎜ , , ⎟ σ nom ⎝ t D w⎠ 8 7 (3) Kt It was assumed that this relationship can be expressed as the following series: 6 Φ = 0.75D 5 σ max = σ nom D/t = 20 D/t = 30 D/t = 40 D/t = 50 D/t = 60 4 3 2 1 0 20 40 60 80 100 120 140 ⎡⎛ D ⎞ α1 ⎛ d ⎞ α2 ⎛ l ⎞ α3 ⎤ A ∑ n ⎢⎜ ⎟ ⎜ ⎟ ⎜ ⎟ ⎥ n=0 ⎣⎢⎝ t ⎠ ⎝ D ⎠ ⎝ w ⎠ ⎦⎥ ∞ n (4) Since σmax/σnom ≥ 1, it can be deduced that A0 = 1. Neglecting terms with powers n > 1 and considering that σmax/σnom = Kt the approximate relationship was considered: (ldw)/(D2t) α α 1 2 ⎛D⎞ ⎛ d ⎞ ⎛ l ⎞ K t = 1 + A1 ⎜ ⎟ ⎜ ⎟ ⎜ ⎟ ⎝ t ⎠ ⎝ D⎠ ⎝ w⎠ FIGURE 18: Kt FOR Φ = 0.75D. α3 (5) Then, representing the product of the non-dimensional variables by a new variable β, Eq. (5) can be written as: 12 11 K t − 1 = A1 β 10 9 where A1 is the angular coefficient of the linear equation. The parameters α1, α2, and α3 were determined through the least square method in order to produce the best correlation between all available data. This was obtained for α1 = 0.67, α2 = 0.62, α3 = 1 and A1 = 1.423, yielding to the compact relationship: 8 Kt 7 6 Φ=D D/t = 20 D/t = 30 D/t = 40 D/t = 50 D/t = 60 5 4 (6) ⎛D⎞ K t = 1 + 1.423 ⎜ ⎟ ⎝ t ⎠ 0.67 ⎛d⎞ ⎜ ⎟ ⎝D⎠ 0.62 ⎛l ⎞ ⎜ ⎟ ⎝ w⎠ (7) FIGURE 19: Kt FOR Φ = 1D. In Fig. 20 the proposed straight line fitting for the stress concentration factor (Kt) is compared against the numerical results. It can be verified that for Kt < 5 the proposed equation (Eq. (7)) gives an excellent approximation. The formulation accuracy is reduced for Kt ≥ 5, as terms with powers n > 1 were neglected. The proposed line fitting is within a coefficient of determination equal to 0.998 with a mean deviation of 2.93%. Analytical Formula Using the results of the parametric study, an equation for the stress concentration factor was developed. The peak stress in a given case can be assumed to depend on the major variables, that is Fatigue Notch Factor The theoretical stress concentration factor (Kt) considered until now is defined for static loadings. Therefore, for fatigue loadings it is adopted the concept of fatigue notch factor (Kf) [9], defined as 3 2 1 0 20 40 60 80 100 120 140 160 2 (ldw)/(D t) 9 Copyright © 2006 by ASME K f = σ f σ nf (8) where σf and σnf are the fatigue limit of unnotched and notched specimens, respectively. The magnitude of Kf must be obtained experimentally. To express the relationship between Kf and Kt the concept of notch sensitivity (q) is introduced [9]: K f = q(K t − 1) + 1 (9) Also, it is observed that 1 ≤ Kf ≤ Kt. For the correct determination of the q value fatigue tests must be carried out. At present, fatigue tests of small-scale dented pipes under cyclic internal pressure are being accomplished. 12 11 pressure is not increased. Consequently, the stress concentration factors were obtained from simpler linear elastic FE analyses. In this case, it was assumed an initial deformed geometry without residual stresses. A parametric study was carried out to evaluate elastic stress concentration factors as a function of pipe and dent geometries. Finally, it was proposed an analytical formulation to estimate stress concentration factors of dented pipelines under internal pressure as a function of geometric parameters. It was obtained a good fitting between the proposed equation and the available numerical results. The mean deviation was equal to 2.93%. The ongoing research project will accomplish fatigue tests of small-scale dented pipe specimens with cyclic internal pressure to determine the notch sensitivity factor (q). After that, the stress concentration factors can be used in a high cycle fatigue evaluation through S-N curves. ACKNOWLEDGMENTS The authors would like to acknowledge the technician Marcos Tadeu A. Dias and the financial support from PETROBRAS, FINEP and National Petroleum Agency (ANP) at different stages of this research work. 10 9 8 Kt 7 6 5 4 3 2 1 0 1 2 3 4 5 6 7 8 (D/t)0.67(d/D)0.62(l/w) FIGURE 20: STRAIGHT LINE FITTING OF THE FE RESULTS. CONCLUSIONS This work is part of a numerical and experimental study to assess the reduction in fatigue life of damaged pipelines under cyclic internal pressure. The analytical procedure to be developed aims to estimate the fatigue life of damaged pipes through formulations of practical application. Initially, an elastic-plastic three-dimensional finite element model was developed to determine stress concentration factors of dented pipes under internal pressure. This model was validated through experimental tests simulating indentation followed by internal pressure in small-scale pipe models. The experimental and numerical results of strains correlated within engineering precision. From the obtained results, it was verified that dented steel pipes under cyclic internal pressure may be considered to deform elastically after the first cycle, if the maximum internal REFERENCES [1] Seng, O. L., Wing, C. Y., Seet, G., 1989, “The Elastic Analysis of a Dent on Pressurized Pipe”, International Journal of Pressure Vessels and Piping, 38, pp. 369–383. [2] Rinehart, A. J., Keating, P. B., 2002, “Length Effects on Fatigue Behavior of Longitudinal Pipeline Dents”, IPC200227244, Proceedings of the 4th International Pipeline Conference, Calgary, Canada. [3] Beller, M., Mattheck, C., Zimmermann, J., 1991, “Stress concentrations in pipelines due to presence of dents”, Proceedings of the 1st International Offshore and Polar Engineering Conference, Edinburgh, UK, II, pp. 421-424. [4] Fowler, J. R., 1993, “Criteria for Dent Acceptability in Offshore Pipeline”, OTC 7311, Proceedings of the 25th Offshore Technology Conference, Houston, USA, pp. 481-493. [5] Alexander, C. R., Kiefner, J. F., 1997, “Effects of Smooth and Rock Dents on Liquid Petroleum Pipelines”, Final Report to The American Petroleum Institute, API Publication 1156, Stress Engineering Services, Inc. and Kiefner and Associates, Inc. [6] Cosham, A., Hopkins, P., 2004, “The Effect of Dents in Pipelines—Guidance in the Pipeline Defect Assessment Manual”, International Journal of Pressure Vessels and Piping, 81(2), pp. 127-139. [7] Rosenfeld, M. J., 1998, “Investigations of Dent Rerounding Behavior”, Proceedings of the 2nd International Pipeline Conference, Calgary, Canada, 1, pp. 299-307. [8] ABAQUS, 2004, “User’s and Theory Manuals”, Release 6.4, Hibbitt, Karlsson, Sorensen, Inc. [9] Pilkey, W. D., 1997, Peterson’s Stress Concentration Factors, 2nd ed, John Wiley & Sons, New York. 10 View publication stats Copyright © 2006 by ASME