## 4 The Bridge Finite Element Modelling  
For the design of the bridge and for the proof load tests definition, a conventional 3D FE model has been developed in CSI SAP2000 environment by modelling all the structural components with beam elements. Instead, for the interpretation of the proof test results, a more refined FE model has been implemented in ANSYS, adopting shell elements for all the members in order to better capture the deck torsional behavior, which is influenced by the sectorial moment of inertia and by the warping of the cross-sections. The refined model in ANSYS was created starting from a solid model (Figure 7a), developed through the SpaceClaim software, which was then converted through the \"midsurface\" command into a completely shell model with surfaces of equal thickness. Finally, the correct thicknesses were assigned to all the elements and the mesh was optimized to reduce the computational effort (Figure 7b). The two main girders and all the cross-beams were modelled with their real geometries, taking into account the presence of the relevant stiffness (e.g., steel plates on beam webs); the concrete slab was modelled with its real thickness (25 cm) and positioned just above the steel deck structure. The slab-girders connection, which consists of Nelson studs, was modeled using elastic linear links that were calibrated to represent the elastic properties of a group of studs in their area of influence. The relevant stiffness was obtained from the bilinearization of the shear connection nonlinear behavior that was obtained from the model that was proposed by [PERSON] et al. [28]. The pylons were modelled considering their real dimensions, inclinations with respect to the vertical alignment, and real cross-section thicknesses, which varies along the pylon height. The steel-concrete composite cross-sections of pylons (first 16 m from the foundation) were modelled adopting two shell elements, one representing the steel empty tube and the other one the concrete filling; the shell elements were rigidly connected to each other to simulate  
Figure 6: Arrays of sensors that were adopted for AVTs on the foundation system. the absence of slip, exploiting the software potentials. The stays were modeled as truss elements. As for the external restraints, the pylons were assumed to be fixed at the base since tests on the foundation compliance revealed a very high translational and rotational stiffness of the soil-foundation systems, as better demonstrated and explained in the sequel. The deck supports were modelled into two different ways, accounting for their different behavior during the static and dynamic tests. In detail, for the interpretation of the static test outcomes, it was assumed that the multidirectional negative-load pot bearings can move since frictions are overcome by the load intensity, and supports were modelled by only retaining the vertical displacements (i.e., horizontal displacements and rotations are allowed). Furthermore, isolators were modelled with elastic links that were characterized by a very high stiffness in vertical direction and by the horizontal stiffness of the real devices, obtained from the isolator manufacturer datasheet. On the contrary, for the interpretation of the dynamic tests, both isolators and bearings were modelled as fixed restraints, consistently with the very low amplitude of the ambient excitation that was not able to produce displacements on the multidirectional devices (because of friction), and only trigger the tangent stiffness of the isolators (stiffness at very low shear strains).