## 2 Materials and Methods
### FEM Model  
The detailed numerical calculations of the investigated samples were carried out with the use of the ANSYS Finite Element Method Software ver. 2022R2 (ANSYS Inc., Canonsburg, PA, USA) [43], which is one of the leading codes in these subjects. As it was mentioned above, all studied samples are composed of three different materials, namely, steel core and four reinforcing overlays attached to the metal part by means of the respective adhesive layers. Due to the structure composition--the relation of thicknesses to the remaining dimensions of the respective components--both 2D or 3D models can be introduced [44]. However, the application of the 3D model brings more valuable results and enables the user to thoroughly assess the strains and stress distributions in all elements (see Figure 2). Three different materials are distinguished by means of three different colors. In Figure 2, the cyan color stands for the steel core, red is equivalent to the adhesive and violet is reserved for the CFRP overlays. In this particular case, the SOLID185 finite elements were used. It is, in general, defined by eight nodes having three nodal displacements \((u,v,w)\) as the degrees of freedom. Such finite elements are suitable for the analysis of problems with plasticity, hyper-elasticity, creep, large strains and large deflections, which can be observed in hybrid structural elements under investigation. Additionally, it has also capabilities adequate for analysis of the behavior of nearly incompressible or even fully incompressible hyper-elastic materials and orthotropic materials. The main difficulty in the modeled sample is caused by the presence of sharp corners in the position when the shape of the opening hole transforms from straight to curvilinear one. This just appears in the close vicinity of the bonded overlays. This is, in fact, the notch area and a relatively high density of the finite elements mesh is demanded for the proper mapping of the stress gradient distribution. In these areas, the strong distortion of the finite elements modeling the structure is expected. Fortunately, the applied finite element allows for certain element shape degeneration without the meaningful loss of the solution accuracy. Here, in the notch area, very small prism-shape solid finite elements are generated. Also, outside the notch in the steel core, a division of the notch close sub-volumes was proposed that provides an almost regular mesh of the generated elements. The detail of the proposed mesh shape in the described area is shown in Figure 3. Due to the symmetry of geometry and loadings, even one quarter of the sample may be investigated. Here, detailed calculations were \begin{table}
\begin{tabular}{l l l l l l l} \hline \hline \multirow{2}{*}{**Adhesive**} & \multirow{2}{*}{**Structure**} & \multirow{2}{*}{**Tensile**} & \multirow{2}{*}{**Shear Strength (MPa)**} & \multirow{2}{*}{**Tensile**} & \multirow{2}{*}{**Maximal**} \\  & & & **Modulus (MPa)** & & **Steel 1** & **CFRP** \\ \hline S\&P Resin 220 & 2C Epoxy & 7000 & 26 & 26 & 14.0 & 1 \\ \hline DP 6310 NS & 2C Polyurethane & 544 & 13 & 22 & 18.0 & 54 \\ \hline HY 4080 GY & 2C Cyanoacrylate/acrylic & 355 & 25 & n.a. 2 & 11.3 & 80 \\ \hline \hline \end{tabular}  
* 1 Cold rolled steel/mild steel. 2 n.a.—not available. Data are not provided by the manufacturer.  
\end{table} 
Table 1: Mechanical properties of adhesives tested experimentally. performed for the symmetric half of the structure. Such a model enables the introduction of variable bond thickness not only on the top and bottom sides of the steel core (when % is modeled) but also on both sides of the opening in future calculations. As a result, the size of the investigated model increases but usage in calculations of the computer with four processors and a relatively large amount of RAM memory results in a reasonable calculation time for the model with approximately 1.5 million active degrees of freedom.