PSI - Issue 23

Stanislav Žák et al. / Procedia Structural Integrity 23 (2019) 239 – 244 Stanislav Žák et al. / Structural Integrity Procedia 00 (2019) 000 – 000

241

3

To evaluate the J -integral as a function of the crack length, a 2D parametric model was created using the Abaqus finite element (FE) code. The model was constructed to simulate a thin Cu layer on top of the Si substrate, where the Cu layer thickness t and the crack length a were the main parameters (see Fig. 1) dividing the geometry model into several sections. In the modelling procedure, the symmetry conditions were used and only one crack flank has been modelled. The whole model was created with general dimension (width and height) by two orders of magnitude larger than the Cu film thickness t and on the far sides of the model (for x max and y max coordinates) the infinite boundary conditions were applied to avoid influencing the results. The model was loaded by the force F applied perpendicular to the crack advance direction (to model mode I loading) and it was used to control the nominal stress σ yy in the Cu film. Used FE mesh consisted of quadratic 2D elements (CPE8) (Dassault-Systemes, 2015) under the plane strain conditions. The mesh was well-refined in the vicinity of the crack tip (see Fig. 1 b) by a circular alignment of the mesh elements. This elements distribution is suitable for the evaluation of the J -integral by the contour ( I -integral) integration method and also for a good description of the crack tip plastic zone. The integration method and used I -integral approach were well-described in (Walters et al., 2005) or for use with Abaqus code in (Dassault-Systemes, 2015). The Si material model was defined by the Young’s modulus E Si = 165 000 MPa and Poisson’s ratio μ Si = 0.22 (Dolbow and Gosz, 1996) to model elastic behavior of Si. The Cu thin film material model was defined by its elastic properties E Cu = 130 000 MPa and μ Cu = 0.34 (Freund and Suresh, 2003), its yield stress σ yield = 100 MPa (Zhang et al., 2011) and hardening modulus E Cu, pl = 600 MPa which is low (bringing used model close to the elastic-ideally plastic material) but still in conjunction with experiments in (Zhang et al., 2011). The simulation was executed only with the use of elastic material properties for the first time to get a reference results and then with the elastic-plastic behavior of Cu 7-times in succession with increasing loading force F . For each loading level the crack length was changed from a / t = 0.06 to a / t = 0.94 (0.994 for the fully elastic model). In all simulations the J -integral and the crack tip plastic zone radius r p (length in the crack extension direction, see Fig. 2) were evaluated.

3. Results

The main observed results throughout the simulations were the shape and the characteristic dimension r p of the crack tip plastic zone as well as the J -integral as functions of the relative crack length and loading level represented by the ratio of nominal stress σ yy in the Cu thin film and its yield stress σ yield .

Fig. 2. Comparison of the crack tip plastic zone for crack with a / t = 0.56 (on the left) and a / t = 0.8 (on the right) for loading ratio σ yy / σ yield = 0.75, red line represents the interface between Cu and Si; on the left figure an indication of the major model dimensions ( a and t ), material composition and where the crack tip plastic zone radius r p was evaluated is denoted From Fig. 2 it is clearly visible that the presence of the interface close to the crack tip has some influence on the crack tip plastic zone which changes the shape and seems to be attracted by the interface. Moreover, this change in crack tip plasticity and the proximity of the interface changes the actual value of the mode I J -integral ( J I ).