## 4 Validation of Proposed Empirical Model
### Nonlinear Finite Element Analysis (NLFEA)  
Numerical methods are more efficient and economical tools as compared with experiments for the structural analysis and engineering research [26]. These methods can save the cost and time by developing the numerical models that can capture the complex damage behavior accurately. The finite element modelling of cylinders confined with FRPs was done using the commercial software ABAQUS (version 6.14, Simulia corp., Providence, U.S, 2013). The results of proposed model were validated using the load-deflection curves from the literature [35]. A control cylinder was used to propose a numerical model after the calibration of different parameters such as dilation angle, viscosity parameter of concrete, mesh size and element types of the concrete. The behavior of concrete was simulated by using concrete damaged plasticity (CDP) model and FRP wraps were simulated using [PERSON]'s damage model [36; 37]. To define the contact between concrete column and FRP sheets, a perfect bond was defined by applying \"tie\" constraint between them. The accurate definition of the bonding behavior between the FRP sheets and concrete is very important for the precise predictions [38; 39]. The boundary conditions and meshing used in the numerical model of cylinder were presented in Figure 7. The bottom end of cylinders was fixed for displacements and rotations in all directions and displacement control technique was used for the application of load on the top surface. During the calibration process of finite element model, the default values for shape factor \(Kc\) = 0.667, for eccentricity = 0.1 and for compressive stresses ratios = 1.16 were taken to define the plastic behavior of concrete in ABAQUS. The compressive behavior as shown in Figure 8a, was used for concrete in the present study. The linear elastic behavior of concrete may be taken up to 0.4 \(f_{cm}\)[40]. The relations proposed by [41] were used to find the average compressive strain \(\varepsilon_{c1}\) and the ultimate strain \(\varepsilon_{c1}\) of the concrete as presented by Equations (16) and (17). \[\varepsilon_{c1} = 0.0014\big{[}2-e^{-0.024f_{cm}}-e^{-0.140f_{cm}}\big{]} \tag{16}\] \[\varepsilon_{c1} = 0.004-0.0011\big{[}1-e^{-0.0215}f_{cm}\big{]} \tag{17}\]  
Figure 7: Geometry and boundary conditions of cylinders: (**a**) rigid body surfaces, (**b**) tie constraint between FRP and concrete, (**c**) loading and boundary conditions, (**d**) meshing. To define the stress-strain relationship of concrete, the model given by Eurocode [42] was used given by Equation (18). \[\sigma_{c}\ =\ f_{cm}\frac{k\eta-\eta^{2}}{1+(k-2)\eta} \tag{18}\]  
where,  
\[k\ =\ 1.05E_{cm}\frac{\varepsilon_{c1}}{f_{cm}},\ \eta\ =\ \frac{\varepsilon_{c}}{ \varepsilon_{c1}} \tag{19}\]  
The tensile behavior of concrete was defined by modified tension stiffening model [43] (see Figure 8b). A control model was selected for the calibration purpose having a single layer of FRP material with compressive strength of 12.5 MPa. Firstly, the selected concrete cylinder was calibrated to achieve a reliable finite element model (FEM) in which the numerical results of stress-strain are in close agreement with experimental results and then, this calibrated model was utilized for the simulations of all FRP-wrapped cylinders. Various viscosity parameters of 0.00001, 0.0010, 0.0030, 0.0055, 0.0070, 0.0090 and 0.0110 were studied to predict the effect of this parameter on the stress-strain behavior of concrete. A viscosity parameter of 0.0055 gave the best approximation for the stress-strain behavior of plain concrete and hence, this value was selected for the viscosity parameter of concrete in the current work. The effect of dilation angle, viscosity parameter and mesh size of concrete are shown in Figure 9. The experimental peak value of stress was 12.5 MPa at a strain of 0.0017.