PSI - Issue 13

Ivica Galić et al. / Procedia Structural Integrity 13 (2018) 2109 – 2113 Galić et al. / Structural Integrity Procedia 00 (2018) 000 – 000

2110

2

Heaviside function to simulate a displacement field in the area located away from the crack tip. Moreover, Sukumur et al. (2000) introduced the Level Set Method in X-FEM to simulate problems regarding the crack extension, while Stolarska et al. (2001) contributed with the Fast Marching Method, obtaining the present-day X-FEM configuration. Many studies have been conducted to further develop X-FEM, aiming at the method accuracy improvement while retaining the basic functions. Extended finite element method uses the parameters of classical Finite Element Method (FEM) for all finite elements in the model except for the crack region. Finite elements located at the crack model and positioned away from the crack tip are improved by the Heaviside function, while elements located at the crack tip are enriched by the near tip functions. One of the main fracture mechanics parameters, which is used to predict crack growth rate is the stress intensity factor (SIF). Yi et al. (2017) conducted a numerical prediction study of SIFs by using a novel approach based on strain energy method and X-FEM. Sun et al. (2017) conducted dynamic X-FEM analysis of a pressure vessel crack propagation in the reactor body, while Feulvarch et al. (2013) studied the residual stress field effects on a crack propagation path generated as a consequence of the surface-hardening process. Kumar et al. (2015) proposed a homogenized X-FEM approach for fatigue life estimation of a plate with discontinuities and an edge crack; they expanded their research (Kumar et al., 2016) to include the influence of various flaws on load capacity of different structures. In order to analyse crack behaviour and parameters in three-dimensional space, Dirik and Yalcinkaya (2016) conducted fatigue crack growth tests under variable amplitude loading by using a special algorithm developed and integrated in the finite element software. In this paper, a stress intensity factor analysis is carried out for the cast-steel pressure valve designated as DN50 PN160. Two methods for SIF calculation are used, FEM and X FEM. The obtained results from both methods are then graphically compared. 2. Materials and methods In order to determine the SIF of the crack tip by using classical FEM and X-FEM, a crack is modelled on the valve body which is shown in Fig. 1. Mechanical properties necessary for the modelling of the valve body are presented in Table 1. When calculating SIF using the classical FEM, for computational reasons, only one half of the body is modelled and symmetric boundary conditions are applied. On the other hand, when using XFEM, full body is modelled since the extended finite element method does not account for the symmetric boundary conditions. In order to simplify the numerical model and reduce the number of finite elements required, the lateral flanges are not modelled. Since the geometry of the valve body is relatively complex, a free-meshing algorithm from Abaqus/CAE is applied. For the model discretization, a modified parabolic tetrahedral element (C3D10M) is used which is adequate for both small and large deformations. Several different meshes are analysed and the coarsest selected mesh for which the results begin to converge is chosen and shown in Fig. 2. Boundary conditions (Figure 1) are defined by restraining displacements of all nodes on the symmetry plane in the direction perpendicular to the symmetry plane. Additionally, the displacement of all nodes on the cylindrical surfaces of the lateral flanges is restrained in the radial direction. The body load is manifested as the internal pressure of p = 16 MPa, which is applied as a distributed load to the internal walls of the FE model. The pressure acting upon the upper flange is calculated into the axial screw force and given as the surface traction acting upwards and is assigned to the holes in which the screws are mounted. Nonlinear material behaviour is modelled using the incremental plasticity with von Mises yield function coupled with the associated flow rule and isotropic hardening. The large strain FE model is employed by invoking the NLGEOM option within Abaqus.

Table 1. Mechanical properties of the cast steel GP240GH Material parameter Value Modulus of elasticity, E [GPa] 205 Poisson ’s ratio , υ [-] 0.3