## 3 CFD Simulation Methodology  
For modeling in this research, given that the motion of the check valve is an interaction of structural body and fluid, we need to model this problem as an FSI simulation, shown in Figure 4. In order to do so, we chose the widely used CFD commercial software ANSYS Fluent, which is a good way of simulating fluid-body interaction, to implement mesh and the numerical simulation in this paper. To attain a totally developed flow inside the studied pump, simultaneous movement of both the inlet check valve and outlet check valve along with the piston motion is considered in this study. Because the flow through the check valve can flow in two directions: entering and exiting the chamber, the outlet and inlet boundary type are assigned as pressure outlet and pressure inlet, which are set up to be at atmospheric pressure, since the concern of this research is the pressure difference. Figure 3: The assumed relationship between the displacement of the PZT actuator and the check valves (scaled). (**a**) phase shift \(\varphi=0\), (**b**) phase shift \(\varphi=\pi/2\), (**c**) phase shift \(\varphi=\pi\). The grid simulation is defined as a trimmed mesher (predominantly hexahedral mesh), and the refinement of the boundary layer is defined as a prism layer mesher. Local grid refinement is conducted in the area near the check valve where the internal flow field is more complicated. In other words, refinement mesh is applied in areas near the movement zone of the check valve, and the piston where velocity gradients are predicted. A finer mesh tool is applied, with the size of the mesh at that zone being 0.025 mm. The grid quality is checked thoroughly. The refinement mesh of the important region is shown in Figure 5.  
For the overall mesh size, a convergence test is conducted to determine the size of elements in the modeling for computational accuracy and efficiency. In order to obtain the optimal solution, different mesh sizes comprising of 2 mm, 1.5 mm, 1 mm, 0.5 mm, and 0.25 mm are used in the convergence test. The calculated flow rate at the driving frequency of 150 Hz of the studied pump corresponding to the different mesh sizes is represented in Figure 6. It can be seen from the figure that the flow rate becomes converged when the overall mesh size is 0.5 mm. Further reducing the mesh size does not considerably affect the predicted flow rate, but does significantly increase the computational cost. The overall mesh size of 0.5 mm is, therefore, utilized in the subsequent investigations. For the transient FSI-simulations, the boundary of the check valve will change. This requires a method that treats the mesh movement. In this study, the moving direction is known, which in turn allows the dynamic layering method to be used. The dynamic mesh capability is used to model problems with check valves and piston motion. There are commonly three dynamic mesh schemes, namely layering, smoothing, and re-meshing within ANSYS Fluent. A combination of these three schemes is applied to tackle the most challenging dynamic mesh problems. In this case, however, the layering scheme is often sufficient. Check valves are often used to allow unidirectional flow. They are usually applied to act as a pressure-relieving device by allowing fluid to be pushed out of the domain when the pressure is higher than a certain level. In such a case, check valves are connected to the bending cantilever (acting as a spring) that acts to push the valve close to the pump seat and to shut off the flow. However, when the force on the valve is larger than the restoring force, the valve will move away from the pump seat and allow fluid to discharge, thus reducing the pressure upstream inside the chamber. The deformation of the valve pl  
Figure 4: The fluid domain inside the piezoelectric-hydraulic pump. Figure 5: Mesh of the fluid inside the piezoelectric hydraulic pump.