PSI - Issue 39

Daniele Amato et al. / Procedia Structural Integrity 39 (2022) 582–598 Author name / Structural Integrity Procedia 00 (2019) 000–000

587

6

Figure 4 (a) Detail of the outer domain mesh. (b) Detailed view of the tube .

The creation of such a cylinder enclosing the crack front, by using quarter-point singular wedge elements, enforces the theoretical 1/ √ singularity of the stress and strain field at the crack tip, as expected by the LEFM theory. This is possible as the mid-nodes, located between two consecutive front nodes, are moved into a quarter-point position. Furthermore, as proven by Barlow [31], the chosen integration points are super-convergent, that means the stresses in these locations have the highest accuracy in comparison with all other points. After the local remeshing is performed, the global and local mesh need to be connected to create a single cracked model. The connection between the original global and the domain mesh is performed by merging the nodes of the two parts into single nodes. 3.2 Numerical problem resolution The second phase is the resolution of the numerical problem. The linear elastic finite element calculation is carried out by the commercial software ABAQUS. In this phase, for those cases in which = − 1 , the calculations also include the crack faces contact, turning the analysis into a nonlinear one. Among all the contact constraint enforcement methods available in Abaqus/Standard, the penalty method was chosen within all the analyses having a compressive axial load. This contact model is a stiff approximation of hard contact, approximating the hard pressure-overclosure behaviour. With this method the contact force is proportional to the penetration distance , cfr. Eq. (1), so some degree of penetration may occur [32]. � + � { } = { } (1) When the linear penalty method is used, Abaqus/Standard will, by default, set the penalty stiffness to 10 times a representative underlying element stiffness . The contact response is segmented in four regimes, cfr. Figure 5: • Inactive contact regime : The contact pressure remains zero for clearances greater than 0 . • Constant initial penalty stiffness regime : The contact pressure varies linearly, with a slope equal to for penetrations (overclosures) in the range − 0 to . The default initial penalty stiffness, , is equal to the representative underlying element stiffness. The default value of is 1% of a characteristic length computed by Abaqus/Standard to represent a typical facet size.