# Conceptual Design of Composite Bridge Sandwich Structure
## 2 Methods and Materials
### Finite Element Model of the Bridge Deck  
The research in this article aims to find an appropriate model for a bridge structure based on minimum mass and thickness, using natural wood and composite materials as a replacement for reinforced concrete and steel bridges. The total length and width of the bridge were taken at 16 m and 7.5 m, respectively. By fixing these both dimensions, work on different thicknesses was done. The selection of size is based on the previous study in which Balsa wood was used to design the bridge [27]. The model was created in ANSYS WORKBENCH using a geometric modeling tool for both ULS and SLS verifications. The layered shell element SHELL 181 was used in ANSYS WORKBENCH to develop the FEA model for global verification. Layered shell element has short computational time. It is easier to create the mesh in shell element, and also, it needs less disc space for results. Post-processing in the layered shell element type is also faster. In addition, shell elements have both translations as well as rotation degrees of freedom. The main disadvantage of the solid element is locking, in which the solid element shows the bending behavior much stiffer in comparison with an analytical solution. Layered SHELL 181 is ideal for the study of thin to medium dense shell systems. This is ideally adapted for linear, broad rotation, and wide non-linear strain applications. Throughout the domain components, both complete and reduced integration schemes are supported. Layered SHELL 181 accounts for the follower (load stiffness) effects of the distributed pressure. It is a four-node feature with six degrees of freedom at each node: transformations in x, y, and z directions, and rotations in all three axes. According to the ANSYS reference manual, layered shell 181 element can be used for layered applications for modeling composite thin to moderately thick shell or sandwich structures. The accuracy of the layered shell 181 element is based on the first-order shear deformation theory (FSDT) (usually referred to as Mindlin-Reissner shell theory). In [36; 37] [PERSON], used the shell element to design the sandwich structure. Moreover, according to [20], layered shell elements can be used in this type of bridge for global verification. Therefore, in the present case, the layered shell element shell 181 is expected to predict results with sufficient accuracy. For the discretization of the model, element size 0.1 m was used. The FEA model of the bridge structure used in this research is shown in Figure 1.  
Figure 1: (**a**) Distributed load on lane 1 (**b**) Distributed load on lane 2; (**c**) Position of vehicles on the lane; (**d**) Boundary conditions. PrePost (ACP) module for composites of the software was used to create a preliminary model of the composite lay-up using 0.001 m of thickness. While designing the lay-up in the ACP module, Rosettes and oriented selection sets were used for fiber orientation and directions. Composite flies were then created with the help of modeling groups. Orthotropic properties were used for both wood cores and FRP skins. Boundary conditions were then applied. Displacements in the X, Y, and Z directions were constrained on both ends of the bridge, as shown in Figure 1d. A total load of running traffic on the bridge was applied in two groups, one on each lane, loads of 4 \(\times\) 90 kN and 4 \(\times\) 135 kN with characteristic values were applied on lane 1 and 2, respectively. In lane 1 there was a car, and a 90 kN load was applied on each wheel. The position of the car was at the center of the bridge span. The distance between the front wheels was 2 m, and the distance between the front and rear wheel was 2.5 m. The loading area occupied by each wheel was 0.2 \(\times\) 0.4 m\({}^{2}\) shown in the four boxes on each lane, and 2.25 kN/m\({}^{2}\) of the distributed load was additionally applied.