## 3 Numerical Model Solution  
The beam specimens used in the experiment were fabricated using the ANSYS-V22 (APDL) software package. Considering the inherent brittleness of concrete, the element type \"SOLID65\" was selected, as it effectively accounts for both cracking and crushing modes [49]. The \"SOLID65\" element is an eight-node structural component that encompasses compressive crushing, tensile cracking, creep, and plastic deformation phenomena. It is specifically designed for static analysis scenarios. The finite element model includes four distinct materials: concrete, reinforcement, the reinforcing substance, and the wrapping element [50]. The \"LINK180\" element type represented the transverse and longitudinal reinforcement. This element type possesses three degrees of freedom in three spatial directions and can undergo plastic deformation. The finite element modeling in the ANSYS package program utilized the Hognestad model due to the absence of any winding in the reference specimen. The \(\sigma\)-\(\epsilon\) correlation in the Hognestad model is depicted in Figure 20[51]. The program utilized a multilinear isotropic hardening behavior to represent the concrete, and the stress-strain values produced by the Hognestad concrete model were subsequently applied to our model. Figure 20 illustrates \(\epsilon_{\rm c0}\), which denotes the unit shortening associated with the highest stress. In this context, \(\rm E_{c}\) refers to the modulus of elasticity of the model, while \(\rm f_{c}\) represents the compressive strength of the concrete. The strength of concrete in a model is typically calculated as 85% of the strength exhibited by a cylinder specimen. The formula is provided in Equation (1) [52]. The variable \(\rm f_{c}\) represents the compressive strength of concrete, while \(\rm f_{ck}\) denotes its typical compressive strength. \[f_{c}=0.85f_{ck} \tag{1}\]  
The \"SHELL181\" element was employed to model the building materials utilized in the wrapping of the reinforcing components in the experimental setup. The \"SHELL181\" finite element analysis software is well suited for examining and evaluating shell structures that possess thin to medium thicknesses. The element in question is a quadrilateral consisting of four nodes. Each node possesses six degrees of freedom. This particular system is very suitable for nonlinear applications characterized by linear behavior, significant rotational  
Figure 20: \(\sigma\)–\(\epsilon\) relationship in the Hognestad model [51]. forces, and/or substantial stress levels. Shell thickness variation is also considered in nonlinear analysis. The actual failure criterion of the model was implemented based on the William-Warnke model [53]. The model exhibits a conical shape with a convex cross-sectional profile, as depicted in Figure 21. The cross-sectional shape exhibits both symmetry and uniformity. In this context, the variables \(\sigma_{\text{xp}}\), \(\sigma_{\text{yp}}\), and \(\sigma_{\text{zp}}\) represent major stresses that are mutually perpendicular, while fc denotes the uniaxial compressive strength. The contact elements in ANSYS were utilized to simulate the adhesive properties of the materials employed in the experiment, specifically to bond the concrete surface with the wrapping materials. These elements are assigned stiffness values to represent the experimental contact function accurately. The element with a high degree of stiffness was designated Targe170, while the other element was designated Conta 174. It is essential to establish contact surfaces at the interface between concrete and geogrids in certain studies, as elaborated upon in the forthcoming modeling section. A contact surface may exist between two surfaces, two nodes, or a surface and a node. In ANSYS, surface-surface contact necessitates aligning the surface normals between the two parts, thus establishing the contact surface.