# Flexural Behavior of Reinforced Concrete Beams Retrofitted with Modularized Steel Plates
## 3 Parametric Studies  
### Analytical Model  
Finite element analysis was performed to determine the details of the proposed retrofitting systems. The commercial FE analysis software ANSYS 16.0 was employed to analyze stress for beams. A three-dimensional and eight-node solid element was applied to the model. The steel plates are fixed to the concrete surface using bolts. Automatic surface to surface contact option was used to model the contact interfaces between concrete and steel plates. A surface element was placed and attached to the beam inside the steel plates and around the steel plates. The thickness, stiffness, and strength were not considered for the surface element. The surface of concrete and steel plates are designated as master and slave surface, respectively. Contact interaction was defined between the concrete and steel plates. The friction contact between the parts was defined using Coulomb friction with friction coefficient of 0.3 [14].  
The steel plates and concrete were modelled as isotropic materials. Material and geometric nonlinearity are considered. The elastic-perfectly plastic uniaxial material model with bilinear isotropic hardening is used for the concrete model. The yielding stress is equal to the concrete compressive strength and tangent modulus equals zero. The steel plates and bolts are considered to be elastic-perfectly plastic. Steel are assumed to be linear elastic until the yield stress, and after that, the stress remains constant. The yield strength and ultimate strength of the steel plates were 250 MPa, and 460 MPa, respectively. The compressive strength of the concrete was 24 MPa. The material properties are listed in Table 1.  
The thickness of the bottom plate (A), the thickness of the L-shaped lower plate (B), the thickness of the Z-shaped side plate (C), and the spacing of bolts (D) were considered as variables as shown in Figure 2. T-shaped beam is designed with a 1000 mm \(\times\) 150 mm slab, 300 mm \(\times\) 650 mm beam, and 4 m length. The concrete beam model had simply supported  
\begin{table}
\begin{tabular}{c c c c} \hline \hline  & **Compressive Strength (MPa)** & **Modulus of Elasticity (MPa)** & **Poisson’s Ratio** \\ \hline Concrete & 24 & 24,500 & 0.18 \\ \hline  & **Yield strength (MPa)** & **Tensile strength (MPa)** & **Modulus of elasticity (MPa)** & **Poisson’s Ratio** \\ \hline Steel plate & 250 & 460 & 200,000 & 0.3 \\ \hline \hline \end{tabular}
\end{table}
Table 1: Material properties used in the analytical models.  
Figure 1: Proposed retrofitting system: (**a**) The components of proposed retrofitting system; (**b**) The retrofitted beam with the proposed system.  
condition. The displacement was applied at the node of top surface center of beam in the downward direction. The purpose of the analysis is to compare the stress distribution according to each component details, the displacement of 10 mm was applied for efficiency of analysis. The element mesh size was determined to be 1.5 mm \(\times\) 1.5 mm considering that the smallest dimension among the components, L-shaped lower plate and Z-shaped side plate, was 2.5 mm. The finite element model is shown in Figure 3.  
Four models with different mesh sizes, 20 mm, 10 mm, 5 mm, 1.5 mm, were performed to determine a reasonable mesh size that could be reasonably evaluated for the stress of each component. As a results, the stress converged from the mesh size of 5 mm as shown in Figure 4. A sufficient number of elements are needed to observe the stress distribution of each component. Therefore, the mesh size of 1.5 mm would be applicable to this study.