## 2 Materials and Methods
### Finite Element Model Set-Up  
To quantify the buckling equilibrium paths of the thin-walled structures, the stress distribution and deformation extent of the structure must be calculated. [PERSON] [23] used the Differential Quadrature Method (DQM) to determine the pre-buckling in-plane stress distribution of thin rectangular FG-CNTRC plate. [PERSON] and [PERSON] [24] developed an accurate Bezier-based multi-step method and implemented it to find the nonlinear vibration \begin{table}
\begin{tabular}{c c c c c} \hline \hline  & \multirow{2}{*}{**Length/mm**} & \multicolumn{2}{c}{**Internal Radius/mm**} & \multirow{2}{*}{**Wall**} \\ \cline{3-4}  & & **Major Axis** & & **Minor Axis** & **Thickness/mm** \\ \hline FIPP & 2000 & 309.85 & 287.15 & 7.95 \\ The host pipe & 2000 & 318 & & 10 \\ \hline \hline \end{tabular}
\end{table} 
Table 1: Geometrical dimensions of FIPP liner and host pipe. Figure 1: Experimental system design and geometric dimensions of equipment. and post-buckling configurations of Euler-Bernoulli composite beams reinforced with graphene nano-platelets (GnP). Both DQM and the Bezier method divide the structure into a single element to calculate the stress and deformation during the buckling posses, but those require extensive calculations computation to improve the precision of the calculation and the calculation results must be processed to be visualized. Thus, using the finite element analysis will be a good solution to quantify the buckling equilibrium paths of the FIPP liners. ABAQUS is used for finite element simulation to study the effects of the dimension ratio (_DR_), ratio of liner major axis to host pipe radius (_a_/_R_) and ovality (_q_) on the buckling behavior. The longitudinal deformation and the boundary effect caused by the end ports of the liner are neglected and this paper only considers the buckling cross-section of the liner. Using 2D instead of 3D analysis effectively reduces simulation time while maintaining calculation accuracy. The model uses an eight-node reduced-integration plane strain element (CPE8R) and the liner elements are divided into three layers totaling 1200 elements. A total of 200 elements for steel host pipe are shown in Figure 2. Twenty-three groups of finite element model are shown in Table 2, Group A is set for the validation test, Group B to Group E are distinguished by the value of _a_/_R_ to analyze the buckling behavior under the different values of _a_/_R_. \begin{table}
\begin{tabular}{c c c c} \hline
**No. ** & _a_/_R_ & \(q\) & _DR_ \\ \hline A & 0.974 & 3.8 & 75 \\ B-1 & 0.999 & 5 & 100 \\ B-2 & 0.999 &  
The host pipe material adopts the elastic constitutive model, the mechanical parameters of FIPP liner and steel are shown in Table 3. The outer surface of the steel pipe is fully restrained from displacement and rotation in all directions. The uniform external pressure is applied to the outer surface of the liner. The property of the contact surface between the liner and host pipe is defined as \"surface to surface\" in ABAQUS and allows the liner and host pipe to separate from each other when the normal pressure is zero or negative. The friction coefficient is 0.4 for the tangential contact, considering the friction between the liner and the pipe [9]. The displacement of the steel pipe is not considered during the liner buckling process and the boundary condition of the outer surface of the steel pipe is set to limit its displacement in the x and y axes, as shown in Figure 3a. A static general analysis step is used to apply the displacement of the liner along the \(y\)-axis and control the displacement of the liner on the \(x\)-axis and the rotation along the \(z\)-axis to zero, which simulates the process of the liner floating and contacting with the inner wall of the steel pipe under the action of buoyancy. The details about the boundary and load distribution are shown in Appendix A.