## 4 Fluid-Structure Interaction
The dynamic and kinematic continuity at the interface is attained through the following Equation (8) (dynamic continuity) and Equation (9) (kinematic continuity):  
\[h^{s}(t)+h^{F}(t)=0 \tag{8}\]  
\[u_{\Gamma}(t)=d_{\Gamma}^{F}(t);\;i_{\Gamma}(t)=v_{\Gamma}(t);\;\ddot{u}_{ \Gamma}(t)=\dot{v}_{\Gamma}(t) \tag{9}\]  
where \(d_{\Gamma}^{F}(t)\) represents the nodal displacement of the finite elements at the interface boundary, with \(h\) signifying the traction vector [41]. [PERSON] et al. presented eight model equations for the FSI-induced water hammer which were solved using FVM. A significant change in discharge from the chamber during the water hammer is observed, with the negligible pressure waves in the axial direction agreeing well with the experimental data [42]. The pipe is modelled with similar properties to A106 Steel. The linear elastic material properties of the computational model are given in Table 1. In addition to the general material properties, the non-linear (NL) parameters contain a yield stress of 0.220 GPa, and a 31% ultimate strain is modelled with a bilinear isotropic hardening for the pipe [43]. The material properties of the impact wall follow the NL concrete material with a compressive strength of 0.017 GPa. The use of 5 mm elements for the structural simulations is justified by the grid independence test. The element size is varied from 8 mm to 4 mm for both the 550 mm model and 150 mm model, and then their characteristics are evaluated against the von Mises stress (Figure 7). The simplified pipe models are discretized into hexahedral solid mesh of 5 mm element size in the 3D regions and 5 mm beam elements in the 1D regions, as shown in Figure 8. Both the models show similar behaviour at a 5 mm element size and, hence, all three models were solved under similar conditions using the 5 mm hexahedral solid elements, while the beam elements were kept at a 5 mm constant element size for both the simplified models. The contact of the 1D and 3D region is kept as bonded with a simplified point-to-surface contact model for the beam and solid models, as shown in Figure 9. The contact between one-dimensional and three-dimensional elements is possible with the transient structural module of Ansys from non-linear simulations, contrary to the unavailability of contact models in the Ansys LS Dyna module for beam-solid contact formulation. Hence, the general contact model formulation is used with ease for both the cases of the simulations. \begin{table}
\begin{tabular}{c c c} \hline \hline \multicolumn{3}{c}{**General Material Properties of the Computational Model**} \\ \hline  & **Pipe** & **Wall** \\  & **(A106 Steel)** & **(Concrete)** \\ \hline Density (Kg/m\({}^{3}\)) & 7844 & 2400 \\ Young’s modulus (GPa) & 207 & 27 \\ Poisson’s ratio & 0.3 & 0.2 \\ Tensile stress (GPa) & 0.399 & 0.0015 \\ \hline \hline \end{tabular}
\end{table} 
Table 1: Material properties equivalent to A106 steel and concrete. Figure 8: Finite element models of the (**a**) fully 3D, (**b**) 550 mm, and (**c**) 150 mm. Figure 7: Grid independence plot for the structural models. The output pressure from the CFD analysis is applied as the imported input pressure for the inner walls of the pipe as shown in Figure 10. The output from the different wall partitions is applied to the corresponding models to obtain the fluid behaviour at that particular surface. The elbow region is considered to be of importance since the fluid velocity varies significantly at the elbow based on the CFD simulations. Owing to be the extreme end of the free end of the cantilever pipe is also one of the reasons to have a wall-split near the elbow to provide independent pressure-imports for the FSI study. The results of displacements, impact velocity, and stresses due to fluid transients in the pipe on impact with the wall is simulated with a structural solution in Ansys, and the corresponding plots are shown in Figures 11 and 12. The displacements of all three models look similar before the impact, with negligible differences after the impact.