13th International Conference on Fracture June 16–21, 2013, Beijing, China -3- 3. Computational analysis 3.1. FE model Commercial code ABAQUS [19] was used. One half of the specimen was modelled using the second-order 8-node quadrilateral shell element. All elements are offset to the back surface (flat surface) to model the thickness variation in the pad-up and clamping areas. Due to the thickness change in the pad-up and four load-end clamping areas, there is considerable out-of-plane bending deformation even the panel is subjected to in-plane tensile load. This secondary bending can cause variation in the stress intensity factors (SIF). Therefore, prior to performing the fracture mechanics analysis, crack-free specimen was modelled first to verify the FE model against the strain gauge measurement at locations indicated in Fig. 1a. To model the secondary bending more accurately, 3D solid elements were used to provide a benchmark solution to the subsequent shell element models. In order to capture the bending deformation more accurately four elements are used through the 1.6 mm thickness. Out-of-plane deformation and strains were also calculated by the shell element model. Calculated strains and deformation agree with the 3D model output. Model geometry detail is given in Table 2. Table 2 Configurations in FE models (unit: mm) Configuration ao h t1 t2 1 10 30 2.80 1.60 2 20 56 3.11 1.55 Note: Configuration 1 is for numerical model only; Configuration 2 has the same dimension as the test specimen; ao is half initial crack length, h is the pad-up width; t1, t2 are the pad-up and skin pocket thickness, respectively. 3.2. Fracture mechanics analysis SIF is calculated using the interaction integral method available in the ABAQUS, which is similar to the J-integral method. FE model with an initial crack is shown in Fig. 1b. The middle nodes of the rosette elements around the crack tip are moved to the quarter-point position in order to model the crack tip stress singularity more accurately. User can instruct the ABAQUS code to extract the KI, KII and T-stress for each given crack length using the integration integral technique and then predict the crack propagation trajectory using the maximum tangential stress criterion. Subsequent crack configuration will be implemented by the user to manually extend the crack tip in the predicted direction by a specified crack extension increment. Subsequently, the area around the crack path will be re-meshed and the calculation of the SIF and crack growth angle repeated until a user-defined or critical crack length is reached. Calculated SIF (KI) is normalised by the crack length and applied stress perpendicular to the crack plane, y, to find the factor: a K y I (1) The vs. a relation is then used in conjunction with the measured weld metal da/dN vs. ΔK data for life prediction. For variable amplitude loading with the same biaxial load ratio (k), K for a specific load cycle can be found by multiply by the applied stress range perpendicular to the crack growth path ( y). Weld metal crack growth rate (da/dN vs. ΔK) was measured under uniaxial-load [20] using “middle crack tension” geometry specimen, M(T), made of the same alloy and same welding
RkJQdWJsaXNoZXIy MjM0NDE=