## 3 Finite Element Simulation Study
### Finite Element Model  
This section focuses on the reinforced sandwich panel as the research subject, with the overall structure composed of upper and lower panels along with reinforcement ribs. The dimensions of the upper and lower panels are 690 \(\times\) 690 mm, each with a thickness of 2.55 mm. To facilitate subsequent experimental suspension, the upper panel features an extended edge, forming a U-shaped cross-section when viewed head-on. The reinforcement ribs take the form of C-shaped elements with a thickness of 1.6 mm.  
The first step involves subdividing the structural grid. Based on the experimental setup constructed as described above, the three-dimensional geometric model is established in SolidWorks software. The three-dimensional model is imported into the HyperMesh finite element meshing software to build the finite element model of the reinforced laminated plate structure shown in Figure 6a,b. In the established finite element model, QUAD quadrilateral elements are used to simulate the upper and lower panels as well as the stiffeners. The mesh size is 10 mm for all elements, totaling 17,489 elements. The connection between the stiffeners and the upper/lower panels is modeled with adhesive bonding, using RBE3 elements for meshing, resulting in a total of 20,249 elements. For the meshing of the fluid cavity, both the exterior and interior cavities of the upper and lower panels are simulated using CHEXA hexahedral elements with a mesh size of 30 mm, amounting to 25,068 elements. The complete finite element model consists of 37,738 structural elements and 25,068 acoustic elements.  
Figure 6: Finite element model of the reinforced laminated panel. (**a**) Schematic diagram of the finite element model structure for the reinforced sandwich panel. (**b**) Visualization of the finite element model for the reinforced sandwich panel.  
The constructed finite element model is imported into the acoustic finite element simulation software. Before acoustic preprocessing of the model, a quality check of all nodal and elemental aspects is conducted. Subsequently, acoustic envelope surfaces are generated, and material properties and fluid attributes for the pertinent structures are established, with detailed parameters presented in Table 1. Meanwhile, the coupling relationship between the structures and the cavity should be established. To simulate the ground effect, the plane of the lower panel's outer cavity should be defined as a reflective surface. To ensure that sound waves can completely transmit, the outer surfaces of other cavities should be defined as Automatic Matching Layers (AML).  
This paper simulates the vibration behavior in a free state without applying any constraints. In the experiment, the load is applied at a certain location on the upper panel, which is consistent with the position of the hammer impact during the experimental test. To better match the actual conditions, the load data during the experiment is imported into the acoustic simulation software, and the load direction is set as vertical, perpendicular to the upper panel. To simulate the actual measurement surface during the experiment, a 6 \(\times\) 6 plane array is created 500 mm above the upper panel, with seven measurement nodes on each side, as shown in Figure 7, which is the finite element simulation model of the reinforced laminated plate. The Vibro-Acoustic Forced Response module should be accessed, and the direct acoustic-vibration coupling method should be employed. The solution frequency range should be set to 1-1000 Hz with a step size of 1 Hz. After configuration, the acoustic solution should be performed. In the simulation, acoustic power are computed at individual nodes of the planar field points and subsequently are aggregated for overall acoustic power. Finally, a comparison is made between the simulation results and experimental data.