## 4 Finite Element Analysis  
### Model Establishment  
To further analyze the deformation of photovoltaic supports, a numerical simulation was conducted using the ABAQUS finite element analysis software, which allows for a more realistic consideration of the connection conditions of components. All components of the photovoltaic supports were modeled using eight-node linear hexahedral solid elements (C3D8R). The simulation included parameters where two or three bolts were installed at the purlin hangers to investigate the effects of different connection methods on joint deformation; a schematic diagram is shown in Figure 7. Additionally, innovative connections were proposed to optimize the structural load-bearing performance of the photovoltaic support. The applied loads in the model were based on the calculation results derived from the Chinese codes. The specific modeling details are outlined below. \begin{table}
\begin{tabular}{c c c c c c c} \hline \hline  & \multicolumn{2}{c}{**Chinese Codes**} & \multicolumn{2}{c}{**American Codes**} & \multicolumn{2}{c}{**Eurocodes**} \\ \cline{2-7}
**Model** & **Stress (MPa)** & **Deformation** & **Stress (mm)** & **Deformation** & **Stress (MPa)** & **Deformation (mm)** \\ \hline Array A & 329.3 & \(-11.53\) & 401.5 & \(-12.75\) & 421.6 & \(-13.29\) \\ Array B & 275.1 & \(-7.82\) & 348.2 & \(-8.54\) & 382.5 & \(-9.28\) \\ \hline \hline \end{tabular}
\end{table} 
Table 3: Calculation results for different codes. (1) During the assembly of the FEA model, one end of the column was tied to the concrete foundation, while the other end was tied to the beam. For purlin hangers connected with two bolts, on-site observations revealed bolt rotation between the purlin hanger and the purlin, indicating that this connection allowed rotational degrees of freedom. Consequently, the connection between the purlin hanger and the purlin was modeled as a hinged connection using multipoint constraints (MPC). Conversely, for purlin hangers connected with three bolts, no significant rotation or sliding was observed between the purlin hanger and the purlin, leading to the establishment of a fixed connection between the purlin and the purlin using tie constraints. Additionally, hinged connections were modeled at both ends of the braces, where they joined the beams and columns. Fixed connections were assumed between the purlins and the photovoltaic panels. The boundary condition at the bottom of the concrete foundation was set as a fixed end. (2) The materials used in the model include concrete and steel, with the following main material properties, are given as follows:  
Precast concrete foundation: The design strength grade of the precast concrete foundation is C80. According to the provisions of GB 50010-2010 [35], the elastic modulus for concrete of this strength grade is 3.80 \(\times\) 10\({}^{4}\) N/mm\({}^{2}\), and Poisson's ratio is 0.2. Cold-formed thin-walled steel components: The columns, beams, braces, purlins, and other components of the photovoltaic support are fabricated from cold-formed thin-walled steel. The elastic modulus of steel is generally 2.06 \(\times\) 10\({}^{5}\) N/mm\({}^{2}\), and Poisson's ratio is 0.3. The yield strength of Q355B-grade steel is 355 N/mm\({}^{2}\), while the yield strength of Q420B-grade steel is 420 N/mm\({}^{2}\). The nonlinear steel behavior represented by the bi-linear stress-strain relationship was used to characterize the mechanical behavior of the steel components, which accurately captures both the elastic deformation and progressive yielding phenomena of the cold-formed thin-walled steel components under incremental loading [36]. The concrete damage plasticity model implemented in Abaqus was adopted to characterize the constitutive behavior of concrete materials, providing a robust computational framework for simulating their nonlinear mechanical responses under multiaxial stress conditions [37].