PSI - Issue 5

Stanislav SEITL et al. / Procedia Structural Integrity 5 (2017) 737–744 Seitl, S. et al./ Structural Integrity Procedia 00 (2017) 000 – 000

740

4

where G is the shear modulus, κ is Kolosov’s constant for plane strain or the plane stress condition and r is a radius coordinate in a polar coordinate system, v is nodal displacement. An extrapolation method (direct method) was used to determinate the values of SIF from 3D numerical calculation. This method is based on stress distribution near the crack tip, and then the value of SIF is extrapolated to the crack tip. The SIF for the crack tip is ascertained from an equation of a usually linear trend line fit through K ( r ) - values calculated from numerically gained stress values in nodes ahead of the crack, see Erro! A origem da referência não foi encontrada. .

3. Numerical Modelling

3.1. 3D Numerical Model in ANSYS

A numerical model was created in the finite element (FE) software ANSYS 17.2 [ANSYS® (2016)] as one quarter of the test specimen with symmetrical boundary conditions. The dimensions of ¼ of a rectangular prism were span ( S ) × width ( W ) × thickness ( B ) 800 mm ×100 mm × 100 mm. The geometrical proportions were taken from a NASA report Calomino (1994) meaning the ratio of span/width S / W , the ratio of thickness/width B / W and the load positions, to compare the numerical solution with actual experimental results. The chevron notched cross section was defined with the following parameters: crack length a , chevron notch origin a 0 and chevron notch ending a 1 (Fig. 1). The straight through crack specimen has a relative crack length α = a / W . The variants of the chevron notched numerical model have a relative notch length and the surface ( α 1 = a 1 / W ), and a relative notch length to the chevron tip α 0 = a 0 / W see Fig. 1. The numerical model was loaded by force P /2 which has a magnitude 100 N. Boundary conditions were applied on nodes constraining nodal displacements: u x = 0 in the area which lies on the axis of symmetry, u y = 0 in the ligament area (straight through a crack or chevron notch) and u z = 0 on the line, where the rigid support lies. The geometry and boundary conditions of the numerical model are shown in Fig. 3.

Fig. 3. Boundary conditions of a 3D numerical model

The studied geometry was meshed with the element type SOLID186 taken from ANSYS ’s element library. In total 8950 elements with 14787 nodes have been used. A fine mesh was adapted around the edge, where the stress was ascertained for the direct calculation of the stress intensity factor (SIF). The material used in the presented study was Aluminium 7075-T651 with Young’s modulus E = 72.395 GPa and Poisson’s ratio  = 0.3, taken from the NASA report Calomino (1994). 3.2. Calibration of the 3D model The 3D numerical model was calibrated, by comparison of 3D and 2D results of SIF obtained from a four-point bending specimen with straight through the crack. The results obtained from the 2D model with plane strain boundary conditions were compared to the results from the direct method conducted on the 3D numerical model with various Poisson’s ratio s. Calibration was done for a relative crack length a / W = 0.4 and Poisson’s ratio varied from 0 to 0.499 (numerical calculation is not stable for  = 0.5), to see the influence of Poisson’s ratio on the direct