## 3 Numerical Methodology: Finite Element Analysis.  
The main issues regarding the Finite Element modelling methodology will be briefly described in this section. The present work is based on numerical calculations made by means of the finite element method (FEM). For the numerical analysis, ANSYS software v19 research license has been used. The methodology is applied to the previous described problem of circular membranes. The availability of some analytical formulations for the problem under study provide us the necessary validation of our model.  
Once the model is validated, the parametric formulation of our programming allows to analyse features between ideal plate and membrane behaviours, filling the gap between them. In addition, it must be taken into account that the goal of this work is to extend the conclusions to other generic geometries more complex. As described in introduction section, one of the research lines that support this work is the hearing mechanics simulation. In particular, the tympanic membrane does not respond to a perfect circular membrane. It has a slight conic shape and a lack of symmetry due to the presence of other elements of the hearing system. It can also present an unknown internal tension.  
In this work, circular shapes have been modelled into the program to simulate the circular membranes with boundary conditions clamped in the edges. Several radii and thickness dimensions and two material properties have been simulated. The materials simulated are steel and eardrum equivalent material. For the case of the steel, it has been used 1 m diameter with different thicknesses: 10, 1, 0.1, 0.01 and 0.001 mm. The properties used for the steel are: density 7850 kg/m\({}^{3}\), [PERSON]'s  
Figure 2: Modal shapes of the first nine vibration modes.  
ratio 0.30 and [PERSON]'s modulus 2.1 GPa. In the case of the eardrum equivalent material, the diameter is 1 cm, thickness 0.05 mm, density 1200 kg/m\({}_{3}\), [PERSON]'s ratio 0.30 and [PERSON]'s modulus 32 MPa. All simulations are under small deformations hypothesis and no plastic behaviour is necessary to be introduced in the model.  
The simulations of the models in ANSYS were made in two different situations: without load, and with radial load in the plane of the membrane (i.e. with pre-strain) [28]. The pre-strain of the membrane was introduced by means of an imposed radial displacement, which produces a radial deformation and the desired axial stress in the membrane.  
Figure 3 shows a scheme of the finite element simulation. It presents the circle area geometry (Figure 3b) which is meshed (Figure 3d) with a shell element (Figure 3c). The element selected is a four nodes one with six degrees of freedom at each node (translations in the \(x\), \(y\), and \(z\) directions, and rotations about the \(x\), \(y\), and \(z\)-axes) suitable for analysing thin to moderately thick shell structures (reference SHELL181 in ANSYS software). Figure 3c shows the geometry, node locations, and the element coordinate system for this element.  
The mesh density is stablished to minimize numerical error. The minimum element size parameter (P\({}_{\text{mes}}\)) used is referred to the radius of the membrane. In this way, we can ensure a constant mesh density for all simulations, regardless of the size of the plate. A P\({}_{\text{mes}}\) of 160 radius divisions was selected.  
Once the model is defined, natural frequencies and mode shapes are obtained through a modal analysis routine. Figure 3e presents some displacement results obtained in modes 2, 3 and 4. The coloured areas represented the total translation displacement of each node of the model.  
In cases with pre-strain, a previous static analysis was performed. To simulate pre-strain levels, 56 different values of radial strain were imposed on the perimeter of the circular membrane. These strain values are in the range of \(\varepsilon=10^{-8}\) to \(2\times 10^{-2}\).