## 4 Numerical Model of the Retrofitted Joints  
In this study a designed RC frame has been considered which has been used in the literature to investigate the effects of retrofitting joints via the CFRP web-bonded scheme [24; 25; 42]. The ANSYS 2019 R1 finite element software was used for modeling, as shown in Figure 6. In the finite element modeling process, the contact between the CFRP  
Figure 5: Crack pattern after conducting an experimental test. sheets and concrete is defined as the tie bonding since it is assumed that both concrete and CFRP sheets are properly bonded to each other using an adhesive. At each node of the elements, three degrees of freedom were considered, comprising eight-noded solid elements (possible translations in the nodal X-, Y-, and Z-directions). This element renders possible cracks in three orthogonal directions, plastic deformations, and crushing. Link180 element is used to model the steel reinforcements. A bi-linear curve with 2% post-yield strain hardening was used to represent the steel stress-strain relation. The steel plates were modeled at the hinge support by Solid185, which is a solid element with eight nodes. These elements were applied to undo the possibilities of cracks resulting from stress concentration. Eight nodes were assumed for these elements, each having the three DOFs. CFRP sheets were modeled using Solsh190, a solid-shell-type element with eight nodes. Figure 6: Finite element model of considered RC joints. This type of element possesses the geometry of a continuum solid element at each node. Finally, the columns' end was modeled considering suitable boundary conditions to apply an axial compression force at the joint throughout the analysis. To perform the non-linear pushover analyses, stepwise equal and opposite loads were applied to the beams' ends. The modified Newton-Raphson method was implemented to solve the pushover problem. However, the convergence criteria that were considered were based on displacement, whose tolerance limit was taken equal to the FE software. In order to conduct non-linear analysis, automatic time stepping in FE, which predicted and controls load steps, was used. The FE mesh of the joint retrofitted with the flange-bonded scheme is shown in Figure 6b. Nearby, 3144 Solid65 elements were used to model concrete elements, while for the steel bars, 1363 Link180 elements were used, and CFRP sheets were modeled with 264 Solsh190 elements. Nonetheless, using the beam element instead of the link element for modeling steel bars may lead to more accurate outcomes by considering the bending behavior of the steel bars. The mesh sensitivity analysis has been conducted to assess the effect of mesh size and the number of elements on the finite element analysis results. Therefore, the final analysis results were obtained from the most stable model, where changing mesh size did not affect the results by more than \(+/-1\%\). The William-Warnke model was employed to account for the failure criterion of concrete and cracking, as well as possible models of crushing failure [43]. Therefore, for failure surface failure, compressive strength and ultimate uniaxial tensile strength are required. Figure 7 shows a three-dimensional concrete failure surface [32]. It is seen that the stiffness of the cracked concrete vanishes in the FE model; hence, tension cannot be resisted. Since principal stresses are all compressive and lie outside of the failure surface, the concrete starts to crush; thus, the elastic modulus in all directions decreases rapidly. Additionally, \(\beta\)_(t) and \(\beta\)_c are coefficients of shear transfer with values between 0 and 1 introduced for the definition of concrete for open and closed cracks. The value of \"0\" represents a smooth crack (i.e., complete loss of shear transfer), and \"1\" stands for a rough  
Figure 7: Three-dimensional failure surfaces based on William–Warnke criterion [3]. crack (i.e., no loss of shear transfers).