PSI - Issue 13

Moritz Lessmann et al. / Procedia Structural Integrity 13 (2018) 1232–1237 Author name / Structural Integrity Procedia 00 (2018) 000–000

1233

2

In the past, defect tolerance assessments would generally follow analytical procedures, simplifying the assessed geometry to available hand-book solutions, or be conducted through elastic two-dimensional (2D) cracked-body finite element analysis (CBFEA). These approaches often require a range of simplifications, including, but not limited to, the component’s geometry, the precise defect location within the component, or the details of the loading conditions. Elastic assessments were then adjusted to allow for varying levels of plasticity which may occur due to the presence of primary and secondary stresses, which influence the local crack tip driving force. Necessarily, this led to conservatisms being introduced to allow for limitations in the generic methods applied. For industrial components this may result in significant over-estimates of crack tip driving forces. With improvements in computational capabilities, it is now possible to conduct more detailed elasto-plastic three dimensional (3D) CBFEA without recourse to separate consideration of elastic plastic interaction. This paper presents and discusses modelling techniques recently adopted to the assessment of industrial components, which have released conservatisms and permitted detailed assessment of complex geometries and load cases. The method for defect tolerance assessment through finite element cracked body modelling may be broken down into the following steps: 1. Construction of a geometrical model of the component which is to be assessed; 2. Specification of the shape, orientation and location of the defect in the geometrical model; 3. Mesh generation, paying particular attention to the region surrounding the defect front and any interaction with model discontinuities; 4. Appropriate selection of the loading conditions and material properties. The resulting models are then analysed to: 1. Extract Stress Intensity Factors (SIFs) and/or strain energy release rates (J-Integral) along the defect front; 2. Perform a limit load analysis for assessment against plastic collapse. The results (SIFs/J-Integrals/limit load) may be used in failure assessment diagram (FAD) or the assessment against a material allowable toughness. Combination of these results for a range of defect lengths/ orientations/locations and load cases permits the derivation of a tolerable defect size or informs subcritical crack growth calculations. 2. Three-Dimensional Meshing Techniques Meshes of 2D cracked body are generally constructed with a radial ring of elements refined at crack tip, Figure 1. The crack front may be modelled with a range of degenerate elements, with one such example consisting of the crack tip nodes constrained to each other and with the mid side nodes on the crack front side moved to the quarter points. Approaching the crack tip, this gives a crack tip singularity of σ→r -1/2 as r→0. This type of singularity is generally adopted for elastic analyses, but may also be adopted for inelastic analyses when combined with a refined mesh.

Figure 1 – Illustration of a 2D cracked-body mesh

For 3D models this radial ring of elements is required along the complete defect front, with planes of nodes forming the contour integrals which must remain normal to the defect front. Generation of such 3D cracked body meshes in geometrically complex regions can pose significant challenges. Refined mesh densities in the near-defect region may lead to difficulties in obtaining a sufficiently coarse mesh in the surrounding structure. When considering curved or non planar defects (i.e. semi-elliptical), commercial meshing algorithms may struggle to construct planar elements aligned normal to the defect front within refined near-defect region, especially in proximity to model discontinuities.