## 4 Case Study
### Numerical Implementation  
The CZM [40] and the VCCT [41; 42] were both implemented for the numerical analysis. A brief introduction of the two methods is presented here to aid the understanding of the numerical simulation.  
The CZM, introduced in [43; 44], utilizes cohesive elements at the interface. These elements are situated along the direction of the crack and are governed by a constitutive law that combines a fracture mechanics and a stress-based criterion. In general, the load in one cohesive element increases with increasing load until a maximum stress level is reached. Then, the stiffness of the element degrades following a specific softening law. A linear softening law is the simplest one and is provided by ABAQUS. These elements were used here and the necessary parameters for their implementation were evaluated using the methodology of [PERSON] et al. [45]. Finally, after loading the sample, the ERR was evaluated by integrating the stress of the first element at the tip of the crack [40].  
The VCCT, introduced in [46], directly uses the nodes of the elements to evaluate the ERR, and no cohesive elements are needed at the interface. Implementing the VCCT in ABAQUS necessitates the definition of the crack propagation region. The nodes of this region were restrained using fixed node-to-node conditions for the displacement and rotation. The fixed condition on the nodes was released when the ERR exceeded a specific value, i.e., meeting a failure criterion. The B-K criterion [39; 47] was used for this article. The reader is referred to [41; 42] for more information concerning the implementation, history, and potential of the VCCT.  
Unfortunately, the implementation of the VCCT comes with certain limitations such as inaccuracies due to the oscillatory nature of the stresses. To prevent oscillations, a thin artificial layer of epoxy was added between the two sub-beams as suggested by [3; 14]. The thickness of this layer was taken sufficiently low (0.01 mm) so that the stiffness of the composite was not affected. For reasons of consistency, this thin epoxy layer was maintained for the CZM model as well, even though it was not necessary. Finally, the critical ERR for the CZM and the VCCT was taken as 10,000 so that the crack did not propagate since this study considered a stationary crack.  
\begin{table}
\begin{tabular}{c c c c} \hline \hline  & **Aluminum** & **E-GFRP** & **Epoxy Resin** \\ \hline \(E_{11}\) (GPa) & 72.00 & 38.73 & 3.50 \\ \(E_{22}\) (GPa) & 72.00 & 6.94 & 3.50 \\ \(G_{12}\) (GPa) & 27.06 & 2.50 & 1.25 \\ \(v_{12}\) & 0.33 & 0.27 & 0.33 \\ \(a_{11}\) (\(10^{-6}/\mathrm{\SIUnitSymbolCelsius}\)) & 23.00 & 7.26 & 57.50 \\ \(a_{22}\) (\(10^{-6}/\mathrm{\SIUnitSymbolCelsius}\)) & 23.00 & 37.70 & 57.50 \\ \hline \hline \end{tabular}
\end{table}
Table 1: Properties (elastic and thermal) of aluminum 2014-T6, E-GFRP, and epoxy resin used in the simulation.  
For the modeling of the composite laminate, the eight-node reduced integration plane strain quadrilateral elements (CPE8R in ABAQUS) were used to prevent shear locking from affecting the predictions of the model. Figure 5 illustrates the model in a meshed (a) and an unmeshed (b) state. Note that for both the CZM and the VCCT, the mesh was uniform and obtained by convergence studies, and approximately 15,500 and 12,000 elements were used for the upper and the lower sub-beams, respectively. Figure 5 also contains a magnified view of the crack tip. All simulations were performed in ABAQUS using the open-source Delamination Plug-In [48], which automatizes the simulation process.