# Preliminary Failure Analyses of Loaded Hot Water Bottles
## 2 Methodology
### Experimental Approach
#### 2.2.3 Finite-Element (FE) Analysis  
The FE modelling was conducted by building the geometry and material models as inputs and obtaining the stresses and deformations as outputs. The model geometry was initially created as a computer-aided design (CAD) file saved in a stereolithography (STL) file of a \"Cassandra\" bottle designed with standard features as in most marketable examples. Figure 5a shows a front orthogonal view of the model within Creo Parametric 11 (Parametric Technology Corporation, Boston, MA, USA), with the coordinates of the 3D model generated within MATLAB 2024a to facilitate model meshing, as shown in Figure 5b. The hot water bottle was meshed with single-layer C3D10H hybrid 10-node tetrahedral elements, and the mild steel plates were meshed with double-layer C3D8H hybrid 8-node elements, as shown in Figure 6. The hot water bottle model was built with 17,694 nodes and 8934 elements, while each mild steel plate had 18,123 nodes and 9174 elements. The numbers of elements and layers were selected based on a mesh conversion study where different configurations were tested, and the first converged number was chosen. The values of von Mises stress at the intermediate nodes on both side edges of the bottle were used as a measure of continuity [15]. These analyses determined how small the elements should be to ensure that the mesh size did not affect the FE outcomes. The hot water bottle material model was constructed based on the material tensile test, where the particle swarm optimisation (PSO) algorithm [16; 17; 18] (MATLAB's Global Optimisation Toolbox) was used to fit experimental tensile testing data to the Ogden nonlinear material model, as shown in Figure 7. The swarm size was set to 40 with an initial span of 2000, and the maximum number of iterations was set to \(10^{3}\) with a lower bound of changing the objective function's value of \(10^{-6}\) tolerance during a single step, based on preliminary investigation [19]. The lower limits of the Ogden material model parameters \(\mu_{i}\) and \(\alpha_{i}\) were set to \(10^{-6}\) and 0, while  
Figure 4: Experimental compression test setup with a hot water bottle: (**a**) the Instron 3369 front view without the setup, (**b**) the manufactured setup as used in the laboratory, (**c**) the automatic control unit, (**d**) 3D isometric projection as designed in Creo Parametric 11 software, and (**e**) side view showing the test starting position. the upper limits were set to 10 and 50, respectively. These limits were selected based on the past practice of getting a decent mathematical fit while keeping the optimised solution within the numerical value range that does not cause FE model instability. The error was minimised between the fitted stress-strain data and the experimentally measured data via the objective function (_err_) which was set as follows:  
\[min\left(err=\frac{1}{n}\sum_{i=1}^{N}\left(\sigma_{exp}^{i}-\sigma_{pre}^{i} \right)^{2}\right) \tag{9}\]  
where \(\sigma_{exp}\) is the experimental tensile stress, which was set to the average \(\sigma_{t}\), \(\sigma_{pre}\) is the predicted Ogden stress, and \(n\) is the number of stress-strain measured data points. The constitutive Ogden strain energy equation can be articulated in terms of the three principal stretches as follows [20]:  
\[U=\sum_{i=1}^{N}\frac{2\mu_{i}}{\alpha_{i}^{2}}\left(\overline{\lambda}_{1}^{ a_{i}}+\overline{\lambda}_{2}^{a_{i}}+\overline{\lambda}_{3}^{a_{i}}-3\right) \tag{10}\]  
where \(U\) is the strain energy; \(\mu_{i}\) and \(\alpha_{i}\), are material parameters; \(\overline{\lambda}_{i}\) are the deviatoric principal stretches (ratio between the deformed length \(L_{1}\) and the initial length \(L_{0}\)) in principal directions.