# Wind Vulnerability of Flexible Outdoor Single-Post Billboards
## 2 Methodology
### Description of Structural Model  
The ANSYS commercial finite element package [18] was used to perform the structural and fluid computational models of one flexible single-post billboard under different wind speeds. In the structural model (Figure 5), isoparametric solid elements identified as SOLID18 were used to simulate the panel, header, vertical steel pole support, base plate, angles, brackets, pedestal, nuts and anchor rods. This type of element is a higher order 3-D solid element with quadratic displacement behavior. The element is defined by 20 nodes having three degrees of freedom per node: translations in the nodal x, y and z directions. The element supports plasticity, hyperelasticity, creep, stress stiffening, large deflection  
Figure 4: Probability of failure and reliability index for normal probability distribution variables. Adopted from [PERSON] et al. [17]. and large strain capabilities. It also has mixed formulation capability for simulating deformations of nearly incompressible elastoplastic materials, and fully incompressible hyperelastic materials. SOLID187 element was also used for modeling zones of the single-post billboard where irregular meshes were required: some zones of vertical steel pole support, base plate and brackets. This solid is a higher order 3-D, 10-node element, which includes a quadratic displacement behavior, and this has three translational degrees of freedom at each node. To reduce the computational effort, the damage in the pedestal was ignored. Figure 5: Three-dimensional nonlinear numerical model of a flexible single-post billboard, based on FEM using ANSYS [18]: (**a**) isometric view (panel, vertical steel pole support and angles); (**b**) back view including the header; (**c**) mesh independence study; (**d**) isometric view (vertical steel pole, brackets, pedestal, nuts and anchor rods); (**e**) lateral view (vertical steel pole, brackets, pedestal, nuts and anchor rods). For static structural analysis, the joints between anchor rods and base plate and the joints between anchor rods and the pedestal were modeled by using contact elements (Figure 5), whilst modal analysis was not included in these types of the elements due to the nature of this analysis; any nonlinearities such as plasticity and contact elements are ignored. Contact elements used are identified in ANSYS as CONTA174 and TARGE170; with these types of elements it is possible to create discontinuous finite element models. Thus, these elements can be used to model the following characteristics:  
* The sliding, closure or opening of joints is allowed. * When the joint is closed, there are transmissions of compressive and shear stresses but not of tensile stresses. * When the joint is opened, there is no transmission of stresses. * The transmission of shear stresses is according to Coulomb's law. * Changes in the geometry can be detected because of the relative movement of the elements that form the joint. For the joints, sliding between surfaces was considered according to Coulomb's law by using one coefficient of friction (isotropic friction) of 0.44 [19]. A mesh independence study was performed by considering the maximum total displacement obtained from the billboard as a function of the number of nodes generated in each simulation, obtaining a variation of this maximum displacement of less than 2% (Figure 5c), concluding that with 572,316 nodes generating 325,205 elements an average mesh quality of 0.74 is achieved; consuming a computational effort of 30 min by a workstation using 10 cores and 40 GB of RAM. The mechanical and geometrical properties used in the structural model are depicted in Tables 1 and 2, respectively.