## 4 Finite Element Analyses
### Numerical Modeling  
The finite element analyses were carried out using MSC.Marc/Mentat [56], a general-purpose FEA software optimized for non-linear analyses. Note that 2D plain strain finite element models (FEMs) were created for the analyses. The elastomer was modeled using a compressible Neo-Hookean hyperelastic material model. The strain energy density function for a compressible generalized Rivlin model is described by the equation [57]:  
\[W=\sum_{p,q}^{n}C_{p,q}\big{(}\overline{I}_{1}-3\big{)}^{p}\big{(}\overline{I} _{2}-3\big{)}^{q}+\sum_{r=1}^{m}\frac{1}{D_{r}}(J-1)^{2r} \tag{18}\]  
being:  
\[ \begin{array}{ll}\overline{I}_{1}=J^{-2/3}I_{1}&I_{1}=\lambda_{1}^{2}+ \lambda_{2}^{2}+\lambda_{2}^{2}\\ \overline{I}_{2}=J^{-4/3}I_{2}&I_{1}=\lambda_{1}^{2}\lambda_{2}^{2}+\lambda_{ 2}^{2}\lambda_{3}^{2}+\lambda_{3}^{2}\lambda_{1}^{2}\end{array}  \tag{19}\]  
with \(\lambda_{i}\) as the principal stretches. \(\overline{I}_{1}\) and \(\overline{I}_{2}\) are the first and the second invariant of the unimodular component of the left Cauchy-Green deformation tensor \(\mathbf{B}=\mathbf{FF}^{T}\); \(I_{1}\) and \(I_{2}\) are the first and the second invariant of the right Cauchy-Green deformation tensor \(\mathbf{C}=\mathbf{F}^{T}\mathbf{F}\); \(J=\text{det}(\mathbf{F})\) is the determinant of the deformation gradient \(\mathbf{F}\). \(C_{pq}\) and \(D_{r}\) are material constants related to the distortional response and the volumetric response, respectively. For a compressible Neo-Hookean material, \(n=1,\ m=1,\ C_{10}=C_{1},\ C_{01}=0,\ C_{11}=0\), and Equation (18) reduces to:  
\[W_{NH}=C_{1}\big{(}\overline{I}_{1}-3-2\ln J\big{)}+D_{1}(J-1)^{2} \tag{20}\]  
For consistency with linear elasticity, it must be \(C_{1}=G_{e}/2\) and \(D_{1}=K/2\). In all FEMs, the bulk modulus of the rubber has been set equal to 2000 MPa. This simplified material model allows for a direct design of the material properties of the rubber layers, as a single parameter is needed when considering these layers as incompressible. Multi-parameters hyperelastic material models may be used to account for the complex response of the rubber, such as viscous behavior. The fiber reinforcement is modeled with a linear elastic isotropic material, fully defined by two parameters: the Young's modulus \(E_{f}\) and the thickness \(t_{f}\). The elastomer is modeled with arbitrary quadrilateral plane strain with the Hermann formulation element (element 80 in Marc [58]). It is a four-node, isoparametric element written for plane strain incompressible applications. This element uses bilinear interpolation functions, and the strains tend to be constant throughout the element; therefore, a fine mesh is needed. The stiffness is formed using four-point Gaussian integration. This element is preferred over higher-order elements when used in a contact analysis. The reinforcement is modeled with a four-node plane strain rebar element (element 143 in Marc [58]). It is an isoparametric, four-node hollow quadrilateral element, in which a single strain member (such as a reinforcing rod or s cord) could be placed. The element is then \begin{table}
\begin{tabular}{c c c c c c c} \hline \hline
**2a** & \(\mathbf{H}\) & \(\boldsymbol{t_{e}}\) & \(\boldsymbol{t_{f}}\) & \(\boldsymbol{S_{1}}\) & \(\boldsymbol{S_{2}}\) & \(\boldsymbol{G_{e}}\) \\ \hline
**[mm]** & **[mm]** & **[mm]** & **[mm]** & **[-]** & **[-]** & **[MPa]** \\ \hline
110 & 120 & 10.0 & 1.00 & 5.500 & 1.00 & 0.500 \\
220 & & & & & 11.00 & 2.00 & 0.700 \\
275 & & & & & 13.75 & 2.50 & 0.900 \\
330 & & & & & 16.50 & 3.00 & 1.10 \\
385 & & & & & 19.25 & 3.50 & 1.30 \\
440 & & & & & 22.00 & 4.00 & 1.50 \\ \hline \end{tabular}
\end{table} 
Table 4: Overview of the geometric and mechanical parameters used for the parametric FEAs. used in conjunction with the four-node plane strain continuum element of the rubber to represent cord-reinforced composite materials.