Issue 75

R. Ince et alii, Fracture and Structural Integrity, 75 (20YY) 435-462; DOI: 10.3221/IGF-ESIS.75.30

between concentrated loading and distributed loading was smaller than 0.7% in the computations of the SIFs of SCB specimens. In this study, the SNCB specimen illustrated in Fig. 5a was initially analyzed using 8-noded plane elements. Because of the symmetry of the specimen, half of it, with a depth of d =100 mm and a width of b =1 mm, was considered in the modeling, as shown in Fig. 5b. The specimen was discretized into 100 finite elements to minimize computation errors along the notch line. Furthermore, a total of eight quarter-point elements with six nodes were employed to consider the stress singularity around the notch. Note that Ince [21] previously utilized the same discretization along the notch line to model split-tension cylinders containing central cracks, for which an analytical solution was available. Consequently, it was observed that this discretization provided an accuracy of 0.2%.

Figure 5: FEM discretization of simulated specimens a) characteristics of SNCB specimen b) 2D-SNCB modelling c) 3D-SNCB modelling d) SNDB modelling. In the finite element analysis (FEA) by using ANSYS Parametric Design Language (APDL), the elastic constants of the material, elasticity modulus ( E ) and Poisson’s ratio ( v ), were selected as 1.0 MPa and 0.2, respectively, and the concentrated load ( P ) at the mid-span was set to 100 N. The relative notch depths (   = a 0 / d ) were varied between 0.1 and 0.9 with a step interval of 0.1, while span-to-depth ( s/d ) ratios were chosen as 0.5, 0.6, 0.7, and 0.8. The normalized function ( Y ), based on the SIF of the SNCB specimen, was computed using both the J-integral and the CCI technique based on Eqn. (13) for each   value. In this procedure, the value of the nominal strength (  N ) in Eqn. (1) was taken as P /( 2bd ), which was previously used for the SCB specimens and SNDB specimens by Tutluoglu and Keles [14]. In above 2D FEA, the type of PLANE183 elements in ANSYS element library (8-noded isoparametric element) were utilized except around the crack, where 8 quarter point elements (6-noded singular elements) were used to account for the stress singularity at the crack tip. To simulate the SNDB specimen reliably, the SNCB specimen was also modeled in 3D. For this, a quarter of the SNCB specimen was considered due to the symmetry of the cubic geometry ( b =100 mm), as indicated in Fig. 5c. The 3D SNCB specimen containing a notch was modeled using both 8-noded (SOLID185) and 20-noded (SOLID186) solid elements without singular finite elements. In FEA, the elastic constants of the material were chosen as in the 2D analysis, while the concentrated load ( P =100 N) at the mid-span was distributed along the specimen width, as depicted in Fig. 5c. The Y values

442