Research on Constant-Flow Water-Saving Device Based on Dynamic Mesh Transient Flow Field Analysis

Abstract

For the control of the outlet flow rate of a constant-flow water-saving device under different water pressures, this study developed and implemented a custom User-Defined Function (UDF) program to simulate the dynamic motion of the water-saving valve within the Fluent environment. This simulation realistically represents the valve’s behavior under varying water pressures, thereby accurately predicting the valve opening height to comply with national regulatory standards. Firstly, a dynamic grid transient CFD simulation model of the water-saving valve was established using a Fluent UDF program written in C language. The parameters of the elastic elements in the water-saving device flow control system were designed to achieve control of the outlet flow rate. Then, the benchmarking analysis of the aforementioned simulation model was completed based on the flow rate test results of the water-saving device. Finally, the relationship between physical quantities and flow field distribution characteristics of the water-saving valve was analyzed under three different water pressures specified in the national standard. Based on the optimization calculations, the valve opening heights under three different water pressures were obtained, ensuring that the outlet flow rates meet the regulatory standards set by the national authorities. Compared with traditional methods that rely solely on steady-state simulations or empirical data, the method proposed in this paper represents a significant advancement.

1. Introduction

In practical life, the water inlet pressure of various water source devices exhibits a decreasing trend with increasing floor height due to the influence of gravity [1,2]. Excessive water pressure on low floors results in high water velocity and flow rate, leading to poor user comfort and wastage of water resources. Conversely, inadequate water pressure on higher floors results in insufficient water velocity and flow rate, failing to meet usage needs [3,4]. Therefore, it is imperative to develop a constant-flow water-saving device to ensure a consistent flow rate and velocity at the outlet of each floor. A water-saving valve that can control the flow rate at the outlet should be installed in the constant-flow water-saving device, which automatically adjusts the valve opening height according to water pressure changes to control the outlet flow rate. The performance of water-saving valves directly affects the quality of the product. Consequently, water-saving valves have become a focus of current research [5].

Tetsuhiro Tsukiji [6] simulated and analyzed the working principles of slide and conical valves, establishing the corresponding physical parameters with time and displacement changes. They concluded that the basic trend follows a sinusoidal oscillation change. Borghi et al. [7] used the integral method to calculate the pressure values on the spool surface at different opening degrees, thus inferring the proportion of hydrodynamic forces under transient and steady-state conditions. Guzzomi et al. [8] applied the relevant theories of computational fluid dynamics to analyze the motion changes in valves under different mass flow rates, inlet pressures, and internal flow field structures, and summarized simulation experiences under various working conditions. Dossena V et al. [9] combined computational fluid dynamics and theoretical analysis formulas to numerically simulate the dynamic opening process of safety valves in different fluid media. They summarized that the lift, displacement coefficients, and cross-sectional flow velocity of the valve will vary according to different fluid media during the opening process of safety valves. Vaughn et al. [10] studied the fluid motion of different poppet valves. Their results showed that the standard k-ε model performs well for relatively simple models but struggles to capture flow separation and recirculation in more complex ones. Atashafrooz et al. [11] examined the entropy generation analysis inside an enclosure with diagonal side walls via the modified blocked-off technique. The results of the numerical solution show that the maximum value of the flow irreversibility in the whole computational domain of the enclosure are related to the case with the highest values for the Grashof number, Reynolds number, and inclination angle of the side walls. Mahmoodabadi et al. [12] evaluated incompressible laminar convection in three-dimensional shells using an improved meshless local Petrov Galerkin (MLPG) scheme. They demonstrated that the scheme performs well in terms of solution accuracy, convergence, and reliability. Atashafrooz et al. [13] used CFD technology to numerically solve the governing equations, including the conservation of mass, momentum, and energy equations, in Cartesian coordinates using the truncation method. The effects of the bleeding coefficient, optical thickness, albedo coefficient, and radiation–conduction parameter on thermal behavior of the convective system are thoroughly explored by plotting the variations of the Nusselt number (total and convective), and mean bulk temperature under different conditions.

Building upon previous research, this study utilizes UDF programming and dynamic mesh techniques within the Fluent environment to simulate the dynamic motion of the water-saving valve. This research focuses on addressing the issue of controlling the outlet flow rate of the constant-flow water-saving device under varying water pressure conditions. A dynamic mesh transient CFD simulation model was established using a Fluent UDF program written in C. The model was then benchmarked against flow rate test results of the water-saving device. Lastly, the relationship between physical quantities and flow field distribution characteristics during the movement process of the water-saving valve under three different water pressures specified in the national standard was analyzed. Through optimization calculations, the valve opening heights under the three different water pressures were obtained to ensure the outlet water flow rate meets the national regulatory standards.

2. Theoretical Analysis

2.1. Mathematical Model

To facilitate simulation calculations of fluid flows within constant-flow water-saving devices, this study makes the following simplifying assumptions: [14,15,16,17]:

• The constant-flow water-saving device adjusts the water flow rate through internal valves, and the characteristic length scale of the water-saving valve is much larger than the average free path of water molecules. In order to simplify the application of mathematical models describing the dynamic changes in water flow, it is usually assumed that the fluid is a continuous medium, ignoring the discreteness between molecules;
• When the constant-flow water-saving device is in operation, its internal fluid is usually under common temperature and pressure conditions, not under specific extreme conditions; so, the changes in water density and volume are very small. In engineering design and analysis, it can be simplified as incompressible fluid;
• Inside the water-saving device, the water flow exhibits constant viscous characteristics and a linear stress–strain relationship, which makes it reasonable to assume that the water follows the Newtonian fluid model in this process;
• Assuming that the fluid is moving under constant temperature conditions, without considering the influence of temperature changes on the flow process, the surface roughness of the water-saving device components is very small, and the flow boundary is a hydraulic smooth boundary condition.

The Navier-Stokes equations are fundamental to fluid dynamics, comprehensively and accurately describing fluid motion and deformation under diverse conditions. They provide insights into the distribution of velocity and pressure fields, enabling a deeper understanding and quantitative analysis of the complex behavior of fluids. The Navier-Stokes equations are widely used to simulate complex fluid flow phenomena, including turbulence, boundary layer effects, and interactions between fluids and solid surfaces. For example, in aerospace engineering, they are used to simulate airflow around aircraft wings. Based on the characteristics and assumptions related to water-saving devices, the Navier-Stokes equations for three-dimensional incompressible fluids are employed to describe the fluid flow [18,19].

2.1.1. Continuity Equation

$${\displaystyle \frac{\partial u}{\partial x}}+{\displaystyle \frac{\partial v}{\partial y}}+{\displaystyle \frac{\partial w}{\partial z}}=0$$

(1)

In the formula, $u,v,w$ are the velocity components of the fluid in the directions of $x,y,z$, respectively.

The continuity equation is used to calculate the distribution of flow rates in conduits, ducts, and other fluid channels. By monitoring the flow velocity and density at different cross-sections, one can determine variations in fluid flow.

2.1.2. Momentum Equation

$$\rho \left({\displaystyle \frac{\partial u}{\partial t}}+u{\displaystyle \frac{\partial u}{\partial x}}+v{\displaystyle \frac{\partial u}{\partial y}}+w{\displaystyle \frac{\partial u}{\partial z}}\right)=-{\displaystyle \frac{\partial p}{\partial x}}+\mu \left({\displaystyle \frac{{\partial }^{2}u}{\partial x^2}}+{\displaystyle \frac{{\partial }^{2}u}{\partial y^2}}+{\displaystyle \frac{{\partial }^{2}u}{\partial z^2}}\right)+f_x$$

(2)

$$\rho \left({\displaystyle \frac{\partial v}{\partial t}}+u{\displaystyle \frac{\partial v}{\partial x}}+v{\displaystyle \frac{\partial v}{\partial y}}+w{\displaystyle \frac{\partial v}{\partial z}}\right)=-{\displaystyle \frac{\partial p}{\partial y}}+\mu \left({\displaystyle \frac{{\partial }^{2}v}{\partial x^2}}+{\displaystyle \frac{{\partial }^{2}v}{\partial y^2}}+{\displaystyle \frac{{\partial }^{2}v}{\partial z^2}}\right)+f_y$$

(3)

$$\rho \left({\displaystyle \frac{\partial w}{\partial t}}+u{\displaystyle \frac{\partial w}{\partial x}}+v{\displaystyle \frac{\partial w}{\partial y}}+w{\displaystyle \frac{\partial w}{\partial z}}\right)=-{\displaystyle \frac{\partial p}{\partial z}}+\mu \left({\displaystyle \frac{{\partial }^{2}w}{\partial x^2}}+{\displaystyle \frac{{\partial }^{2}w}{\partial y^2}}+{\displaystyle \frac{{\partial }^{2}w}{\partial z^2}}\right)+f_z$$

(4)

In the formula, $\rho$ is the density of the fluid; $u,v,w$ represent the pressure gradients in the three directions of $x,y,z$, respectively; $-\partial p/\partial x,-\partial p/\partial y,-\partial p/\partial z$ represent the pressure gradients in the directions of $x,y,z$, respectively; $\mu$ is the dynamic viscosity coefficient of the fluid; $\mu \left({\partial }^{2}u/\partial x^2+{\partial }^{2}u/\partial y^2+{\partial }^{2}u/\partial z^2\right)$ is the viscosity term, representing the effect of the fluid’s viscosity on the velocity field in the x direction (the same applies to the $y,z$ directions); $f_x,f_y,f_z$ are the volumetric forces in the directions of $x,y,z$.

This work presents a system that couples the mass balance equation with the Navier-Stokes equation. By coupling the mass equation and Navier Stokes equation, the behavior of actual fluid systems can be more accurately simulated. This is crucial for accurately predicting processes such as fluid flow, heat transfer, and material transport. At the same time, the dynamic behavior of fluids over time can also be studied, which is particularly important for real-time monitoring and control systems. This comprehensive method plays a role in many practical applications, including meteorological forecasting, aerospace engineering, marine research, pollution control, etc. In the dynamic systems studied in this paper, such as water resource conservation devices, a coupled system is used as the dominant model, and grid solutions are used to obtain solutions that change over time and position. This method can effectively capture the transient behavior of water-saving valves during dynamic changes, which is crucial for optimizing their performance and ensuring constant flow under different pressure conditions.

2.2. Control of Motion Boundaries

Due to the relatively regular symmetrical structure of the fluid area inside the constant-flow water-saving device, the spring in the flow control system acts as a cylindrical elastic element, effectively preventing the radial inclination of the water-saving valve. Therefore, the radial displacement motion of the water-saving valve was not taken into account in this paper. The main focus was on the analysis of its axial forces and motion [20]. Due to the small weight of the water-saving valve, and the pressure difference on both sides of the water-saving valve and the elastic force of the spring being much greater than the gravity acting on the valve, the influence of gravity is considered negligible. The water-saving valve in the constant-flow water-saving device is subjected to three axial forces: the incoming flow pressure at the inlet, the elastic force of the elastic element, and the viscous resistance between the fluid and the components. Viscous resistance is a highly correlated function of relative velocities between objects. In this model, the movement speed and displacement of the water-saving valve exhibit characteristics significantly smaller in scale compared to the macroscopic level. Therefore, the influence of viscous resistance is considered negligible in this context [21]. Figure 1 shows a simplified force analysis diagram of the water-saving valve in a constant-flow water-saving device.

As water flows from right to left in the diagram, $F_P$ represents the incoming flow water force and $F_T$ represents the elastic force of the elastic element. The incoming flow water force $F_P$ enters the fluid region from the right inlet, pressing the valve to move to the left. At the same time, the motion of the valve generates a reaction force $F_T$ from the elastic element. As the displacement increases, the reaction force $F_T$ from the elastic element also increases continuously. The resultant force acting on the water-saving valve can be expressed as follows:

$$F=m{\displaystyle \frac{dv}{dt}}=F_{\mathrm{P}}-F_{\mathrm{T}}={\displaystyle \sum _{N_{face}}{P}_z\cdot A_z}-k_x\cdot \Delta x$$

(5)

where $P_z$ is the axial pressure component of the incoming flow water pressure on the water-saving valve; $A_z$ is the axial area component of the water-saving valve; $k_x$ is the stiffness coefficient of the elastic element; and $\Delta x$ represents the incremental axial displacement of the elastic element.

Expressing $dv/dt$ in Equation (3) using the finite difference method, we obtain the following format:

$${\displaystyle \frac{dv}{dt}}={\displaystyle \frac{v_{i+1}-v_i}{\Delta t_{i+1}}}$$

(6)

$$v_{i+1}={\displaystyle \frac{x_{i+1}-x_i}{\Delta t_{i+1}}}$$

(7)

where $v_{i+1}$ represents the velocity of the water-saving valve at time $i+1$; $x_{i+1}$ corresponds to the displacement of the water-saving valve at time $i+1$; $v_i$ denotes the velocity of the water-saving valve at time $i$; $s_i$ signifies the displacement of the water-saving valve at time $i$; and $\Delta t_{i+1}$ represents the transient time step.

By integrating the aforementioned expressions, the iterative equation for the displacement motion of the water-saving valve in the constant-flow water-saving device can be obtained as follows:

$$v_{i+1}=v_i+{\displaystyle \frac{{\displaystyle \sum _{N_{face}}{P}_z\cdot A_z}-k\cdot \Delta x}{m}}\cdot \Delta t_{i+1}$$

(8)

$$s=s_i+\left[v_i+{\displaystyle \frac{{\displaystyle \sum _{N_{face}}{P}_{\mathrm{z}}\cdot A_{\mathrm{z}}}-k\cdot \Delta x}{m}}\cdot \Delta t_{i+1}\right]\cdot \Delta t_{i+1}$$

(9)

Notably, the hydraulic load in the iterative equation is not constant but is determined through transient analysis using Fluent 2021 R1 software. The load changes numerically with the flow field distribution [22].

3. The Establishment of a Transient Simulation Model Using CFD

3.1. Geometric Model

Constant-flow water-saving devices consist of three functional parts: a pipe docking system connected to the incoming water pressure pipeline, a flow control system, and a diffuser system. Among them, the flow control system is the core component of the entire constant-flow water-saving device, which consists of four components: the inlet cover, water-saving valve, elastic element, and outlet. Figure 2 provides a visual diagram of the disassembly of the constant-flow water-saving device. The water flows through multiple small holes on the inlet cover and enters the flow control system. The load generated by fluid movement compresses the water-saving valve to move downwards, and the elastic element in contact with it is compressed to generate a reaction force. When the water-saving valve contacts the limiting step, it stops moving downward. The valve opening height stabilizes, resulting in a gradual flow rate equilibrium and achieving constant flow, thereby achieving the objective of constant flow. Figure 3 shows the dimensional drawing of constant current water-saving device, from which the relevant geometric dimensions of the constant-flow water-saving device can be obtained.

3.2. Numerical Simulation Method

In order to simplify calculations and reduce the consumption of computing resources and time, traditional water-saving device research usually adopts the steady-state analysis method [23]. This steady-state analysis method aims to evaluate the long-term performance and stability of water-saving devices and confirm their efficiency under constant flow and pressure conditions. However, due to the complexity of the internal flow field, steady-state calculations cannot capture the transient behavior of water-saving valves during startup, shutdown, or dynamic operation, limiting the evaluation of dynamic responses. To overcome these limitations, this paper conducted transient numerical simulations of the internal flow field of a constant-flow water-saving device using Fluent software. This study analyzed the changes in the internal flow field and pressure field of the water-saving device during the implementation of constant flow, as well as the behavioral changes of the valve during dynamic operation, aiming to verify the effectiveness of the constant-flow water-saving device under different effluent strategies.

In this study, finite volume method was used to numerically discretize the control equations in the CFD transient calculation of the internal flow field of a constant-flow water-saving device, and a simple algorithm was used to solve the velocity pressure coupling problem. The simulation of the internal flow field of the water-saving device is based on the k-epsilon standard turbulence model. This method requires strict control of the grid size at the wall to ensure higher computational accuracy the formula for the height of the first layer of grid is used as follows [24]:

$$y={\displaystyle \frac{y^{+}\mu }{V_t\rho }}$$

(10)

$$V_t=\sqrt{{\displaystyle \frac{{\tau }_{\omega }}{\rho }}}$$

(11)

$${\tau }_{\omega }=0.5C_f\rho v^2$$

(12)

where $y$ is the first layer grid height, $y^{+}$ is the dimensionless number, $\mu$ is the dynamic viscosity, $V_t$ is the velocity of the grid closest to the wall, $\rho$ is the water density, ${\tau }_{\omega }$ is the wall shear force, and $C_f$ is the coefficient of wall friction, which can be expressed as follows:

$$C_f=0.058R{e}^{-0.2}$$

(13)

$$Re={\displaystyle \frac{\rho vl}{\mu }}$$

(14)

$${\displaystyle \frac{A}{P}}=\left({\displaystyle \frac{\pi l^2/4}{\pi l}}\right)=l/4$$

(15)

where $Re$ is the dimensionless number that represents the flow of a fluid, $v$ is the velocity of water, $l$ is the characteristic length, $A$ is the cross-sectional area, and $P$ is the cross-sectional perimeter.

In the present study, The initial value of non-dimensional $y^{+}$ was set to 30, and the first layer height of the boundary layer was calculated as 0.19 mm.

In addition, in order to accurately simulate the changes in physical quantities such as force, velocity, and displacement during the movement of the water-saving valve, it is necessary to introduce the UDF function in Fluent and combine it with the dynamic mesh method for model setting. The dynamic movement of the flow control valve involves complex geometry and fluid flow changes. Traditional static meshes cannot effectively capture these time-varying dynamics. Moving mesh technology allows for time-dependent updates to the mesh, accurately tracking and updating the valve body and surrounding fluid changes, thus better simulating the transient behavior of the flow control valve [25]. As the valve moves downwards, the outlet area of the water flow will gradually decrease, and thus the outlet flow rate will gradually decrease. Flow Velocity and Pressure are directly affected by changes in flow area, resulting in an increase in pressure and a decrease in flow rate observed during valve adjustment. The specific flowchart is shown in Figure 4. In this study, the dynamic mesh adopts the remeshing method for mesh updating. During the dynamic process of the water-saving valve, fluid variations may lead to grid instability or numerical errors. However, the remeshing method can dynamically adjust the mesh density, thereby enhancing the stability and convergence of the simulation.

Figure 5 shows the numerical domain of the model. Fluent simulation software can set various parameters for fluid motion at specified boundaries but cannot set the motion of rigid bodies. In this case, it is necessary to combine C language to write UDF programs to compile the motion iteration equations of rigid body components and import Fluent for debugging, in order to achieve the definition of data interface, material properties, geometric mesh data, and maximum displacement of mesh nodes [26]. This paper simulates the displacement motion of a water-saving valve under inlet water pressure. Therefore, using a passive dynamic mesh simulation is more in line with the real situation. Therefore, the code implementation of the UDF program can be based on the iterative Equations (8) and (9) described in Section 2.2 and the DEFINE_CG_MOTION macro [27]. Implementing the UDF program enables control over the real-time movement of the water-saving valve during the transient CFD simulation, enhancing the dynamic realism of the calculation [28].

3.3. Boundary Condition Setting

The boundary conditions of the flow field area of the constant-flow water-saving device include three types: inlet boundary conditions, outlet boundary conditions, and wall boundary conditions. This study simulated inlet conditions under different pressures by setting the pressure inlet boundary conditions to 0.1, 0.3, and 0.5 MPa. The pressure outlet boundary condition was set to 0 Pa. When considering the situation where the fluid inside the constant-flow water-saving device does not slide relative to the wall surface, the wall surface and outlet wall are set as non-sliding wall surfaces. The detailed boundary condition settings are shown in

Table 1. The detailed boundary condition settings.

Boundary Region	Boundary Condition Type	Parameter Setting
Water inlet	Pressure inlet	Gauge pressure 0.1/0.3/0.5 MPa
Cover	Wall	No sliding/Standard
Wall	Wall	No sliding/Standard
Water-saving valve	Wall	Motion rigid body/Dynamic mesh
Outlet wall	Wall	No sliding/Standard
Outlet for water flow	Pressure outlet	Gauge pressure 0 Pa

.

To determine the appropriate parameters of the elastic element, it is necessary to first set the hypothetical parameters in the UDF program and observe whether the analysis simulation results are reasonable. For the settings that are deemed unreasonable, timely adjustments should be made to ensure that the outflow discharge meets the national regulatory standards. To better simulate the relevant dimensions and parameters of actual constant-flow water-saving devices, assume that the initial opening height of the water-saving valve is 1mm. Through experimental measurements, it was determined that the mass of the water-saving valve is 30 g, and the stiffness coefficient of the elastic element is 327 N/m. The density of water in the fluid domain is 998.2 kg/m³, and the dynamic viscosity is 0.001003 kg/(m·s). Through iterative calculations, the initial length of the elastic component is determined to be 3.5 mm. For the transient simulation calculations, the time step size ($\Delta t_{i+1}$) is set to 0.000001 s, and the maximum number of iterations per time step is set to 80, the time discretization error is relatively small. The residual convergence thresholds for turbulence kinetic energy ($k$) and turbulence kinetic energy dissipation rate ($\epsilon$) are set at 10⁻⁶, and the continuity residual convergence threshold is set at 10⁻³, with a total of nearly 190,000 computational steps performed, The Courant number is calculated as 0.01 to handle extremely rapid dynamic changes, the model system reaches convergence. At the same time, four time steps of 5 × 10⁻⁷ s, 1 × 10⁻⁶ s, 5 × 10⁻⁶ s, and1 × 10⁻⁵ s were selected for step independence verification. The above four time steps were used as independent variables to simulate and calculate the detected outlet flow rate. The specific verification data is shown in Figure 6. From the data in the figure, it can be seen that the flow rate changes are less stable when the time step is set to 5 × 10⁻⁶ s and 1 × 10⁻⁵ s, and the iteration steps required for convergence in 5 × 10⁻⁷ are relatively large, making it unsuitable as the time step for simulation calculation. After comprehensive consideration, 1 × 10⁻⁶ s was ultimately selected as the time step for simulation calculation.

During the computation process, the reactive force of the elastic element undergoes changes under the influence of the incoming flow pressure. Therefore, Fluent needs to perform necessary post-processing on the results of each time step to fully describe the entire motion variation process of the water-saving valve [29]. Figure 7 displays radial cross-sectional views of the fluid domain model’s grid changes and grid reconstruction at different time points during the motion process of the water-saving valve in the constant-flow water-saving device.

3.4. Grid Convergence Analysis

Due to the powerful adaptive capabilities and convenient modification advantages of the Hyper Mesh 14.0 software in mesh generation, this paper primarily utilized it for mesh partitioning. Additionally, to ensure the rationality and compatibility of the mesh generation process, the same software was employed for geometric cleaning and simplification of the aforementioned geometric models. To effectively address the complex flow phenomena within the constant-flow water-saving device, this paper employs highly adaptable unstructured grids. Given the small size of the model, the expected number of elements is limited. Therefore, this study uses triangular mesh elements, with their higher accuracy and better fault tolerance, to construct the surface mesh, generating a 3D tetrahedral mesh. In order to enhance the accuracy of the results, the smaller regions of the model, such as the inlet holes, were subjected to grid refinement, with a maximum elements size set at 0.1 mm. The elements size for other regions within the model did not exceed 0.5 mm.

In order to reduce the impact of the number of elements in the computational domain on simulation results and improve computational efficiency, it is necessary to perform grid independence checks on the model. Under the initial condition of inlet pressure of 0.1 MPa, the outlet flow rate of the constant-flow water-saving device under four different elements was measured through simulation calculation data, as shown in Figure 8. The comparison shows that, when the number of elements reaches 424,229, the change in outlet flow rate of the water-saving device during each time period is relatively small compared to the model calculation value when the number of elements is 300,239. After further increasing the number of elements, the change in outlet flow rate of the water-saving device is very small. Considering the factor of saving time and cost, this paper selected 300,239 elements as the appropriate number in the mesh division of the 3D model.

The entire mesh model was partitioned into six components using Hyper Mesh 14.0 software: the inlet region, cover, walls, outlet region, and water-saving valve. This partitioning scheme facilitated the subsequent setup of Fluent boundary conditions. The inlet region has an area of 67 mm², while the outlet region has an area of 20 mm². The final computational model consists of a mesh count of 300,000, with a mesh quality control threshold maintained at or above 0.6. The mesh model for the water-saving valve component is depicted in Figure 9.

4. Experimental and Benchmark Analysis

This paper constructs a complete CFD transient simulation analysis process based on the above. In order to verify the effectiveness of the simulation model and ensure the accuracy of the simulation results, experimental testing will be conducted to collect test data and perform benchmarking analysis with the simulation results.

To obtain the relevant material properties for the CFD model of the water-saving device, a series of experiments must be conducted. For the water flow within the device, it is essential to measure its density and dynamic viscosity. Density can be determined using a pycnometer or hydrometer, while dynamic viscosity can be measured with a viscometer, such as a rotational viscometer or a capillary viscometer. For the elastic components within the water-saving device, the stiffness coefficient must be measured, which can be ascertained through tensile or compression tests.

4.1. Experimental Testing

Prior to conducting the water flow rate tests of the water-saving device, this study determined the stiffness coefficient of the elastic components to be 327 N/m through relevant material testing. Additionally, the density of water was measured to be 998.2 kg/m³, and its dynamic viscosity was found to be 0.001003 kg/(m·s). The experimental tests in this paper were carried out using the flow rate high–low-pressure test machine from Ningbo Jiangbei Zhejiang Machinery Equipment Co., Ltd. (Ningbo, China), as shown in Figure 10. This equipment is equipped with both a cold-water tank and a hot-water tank, which can automatically adjust the water temperature to meet the needs of different test environments or operating conditions. Additionally, it is equipped with a silent high-pressure pump and a frequency converter to output different flow rates and pressures. The high-pressure testing range is 1~20 MPa, the low-pressure testing range is 0.01~1 MPa, and the flow rate testing range is 3~40 L/min. The experimental equipment’s control system uses a programmable logic controller (PLC) and a touch screen, displaying the flow rate in L/min.

The constant-flow water-saving device used in the experimental tests was constructed based on a manually polished physical model. The maximum size of this model is 21 mm, while the minimum size is 0.27 mm. The experimental tests aimed to measure the outflow rate of the constant-flow water-saving device in a steady state under three different inlet water pressure conditions: 0.1, 0.3, and 0.5 MPa. The testing time for the steady-state flow rate was set at 30 s, and each condition underwent ten data tests at different time intervals.

4.2. Benchmarking Analysis

The experimental data from the three conditions were analyzed and processed using the Six Sigma method in MATLAB [30].

Table 2. Six Sigma data analysis and processing.

Inlet Water Pressure	0.1 MPa	0.3 MPa	0.5 MPa
1st time	5.38	7.64	7.14
2nd time	5.27	7.27	7.30
3rd time	6.23	7.42	7.52
4th time	6.01	7.13	7.12
5th time	5.71	6.99	7.85
6th time	5.79	6.92	7.38
7th time	5.98	7.03	6.74
8th time	6.13	7.08	7.25
9th time	5.73	7.32	7.62
10th time	5.74	7.37	7.04
ori_average	5.80	7.22	7.30
max	6.23	7.64	7.85
min	5.27	6.92	6.74
amplitude	0.48	0.36	0.56
95%	6.01	7.38	7.55
5%	5.77	7.06	7.27
new_average	5.93	7.23	7.41

presents the data processing results. This paper provides data on the transient CFD simulation calculations and experimental tests of the constant-flow water-saving device under three different operating conditions, and the results are summarized in

Table 3. Comparison of transient analysis and experimental data.

Operating Conditions	Transient Simulation Calculation Data	Experimental Data	Relative Error
0.1 MPa	6.207 L/min	5.927 L/min	4.51%
0.3 MPa	7.213 L/min	7.234 L/min	0.29%
0.5 MPa	7.306 L/min	7.410 L/min	1.42%

. From the table, it can be seen that under the three operating conditions of 0.1, 0.3, and 0.5 MPa, the relative errors between the transient simulation results and experimental results are all within 5%, indicating that the CFD transient simulation model proposed is relatively reliable, also indirectly verifying the reliability and effectiveness of the UDF code used in this paper.

5. The Analysis of Transient Calculation Results

5.1. The Analysis of the Motion Parameters of the Water-Saving Valve

Analyzing the dynamic behavior of water-saving valves under fluid action can help determine the structural parameters of the limit step of constant-flow water-saving devices. National regulatory standards specify a stable flow rate of approximately 6 L/min at 0.1 MPa and approximately 7 L/min at 0.2–0.5 MPa. Transient simulations were conducted at three different inlet pressures: 0.1, 0.3, and 0.5 MPa. The termination condition for transient calculations was taken as the condition where the water-saving valve entered a stable working state after the end of its movement. The simulations monitored various motion parameters of the water-saving valve in real time, continuously tracking the water flow rate as the valve moved downward. A UDF was used for data collection, with results recorded in a text file. After confirming that the water flow rate meets the specified standards, record the displacement and duration of valve movement according to the output file. By subtracting the initial opening height of the water-saving valve (1 mm) from the displacement value at specific instances, the valve’s current opening height could be determined. Subsequently, the critical step height under these operating conditions was assessed to ensure compliance with flow rate requirements. The subsequent analysis was conducted using the collected data file.

Figure 11, Figure 12 and Figure 13 show the dynamic process of the water-saving valve from a static state to a flow rate that meets national regulatory standards under three different water pressure conditions (0.1, 0.3, and 0.5 MPa). From the curve graph, it can be seen that the movement time of the water-saving valve under three different water pressure conditions (0.1, 0.3, and 0.5 MPa) is 0.0074, 0.0067, and 0.0058 s, respectively. In these cases, the corresponding displacement of the water-saving valve is 0.2617, 0.6482, and 0.7884 mm, respectively. Therefore, the valve opening heights under three different water pressures can be calculated as 0.7383, 0.3518, and 0.2116 mm, respectively. The speed of the water-saving valve reaches its maximum value at the moment of opening and then continuously fluctuates and decreases. Throughout the process, the direction of the water-saving valve speed remains unchanged, and the valve core opening is constantly increasing. At the end of the movement, the valve opening reaches its maximum value. The speed of the water-saving valve fluctuates greatly under a water pressure of 0.3 MPa, but the overall trend is still within a reasonable range. The maximum speeds during the movement of the water-saving valve under three different water pressure conditions are 0.0849, 0.2012, and 0.4512 m/s, respectively. Compared to the 0.5 MPa condition, lower water pressures of 0.1 MPa and 0.3 MPa exhibit more unstable speed variations as the valve transitions from a stationary state to a stable state. Furthermore, the positions and timings of the speed peaks differ under these lower pressure conditions. This phenomenon may be attributed to the lower control accuracy of the water-saving valve’s control system at reduced water pressures, which makes it challenging to precisely adjust the valve opening, thereby increasing the instability of the valve’s dynamic response. Additionally, lower water pressures may induce bubble formation or cavitation, which can disrupt fluid flow and further exacerbate the unpredictability and control difficulty of the valve’s stabilization process.

The variation of flow rate over time under dynamic valve movement is primarily governed by the following mechanisms. At the beginning of valve movement, the water-saving valve has the highest outlet opening, the highest water output, and the highest flow rate. As inlet pressure acts on the valve, forcing it downward, the opening and outlet flow rate gradually decrease. At the same time, the elastic component compresses and generates a reactive force, increasing the resistance to valve movement and slowing down the rate of flow reduction. Eventually, the elastic force of the elastic element balances with the inlet pressure, and the opening no longer changes. The flow rate reaches its minimum value, and the water outlet of the water-saving device also reaches a stable state. The observed transient flow rate changes result from the dynamic interaction between inlet pressure, valve movement, and elastic force.

At the same time, the minimum flow rate reflects the minimum water flow rate of the water-saving device during steady-state operation. When the fluid passes through the water-saving valve, the valve opening interacts with the fluid dynamics state, which affects the change in flow rate. Bernoulli’s principle states a close relationship between fluid pressure, velocity, and height, implying that the flow rate will be limited under specific valve opening and pressure conditions. The minimum flow rate indicates a dynamic equilibrium state, at which the inlet pressure and the reaction force of the internal elastic components of the valve reach equilibrium, and the valve no longer moves. This equilibrium state reflects the stable characteristics of the physical system. At the same time, this also involves the conversion of energy. When the flow rate reaches its minimum value, the kinetic energy of the fluid decreases, and some of the energy is converted into elastic potential energy, which conforms to the law of conservation of energy, that is, in a closed system, the total energy remains unchanged and only formal conversion occurs.

Table 4. Summary of transient simulation results.

Inlet Water Pressure	0.1 MPa	0.3 MPa	0.5 MPa
The time required for the motion to reach a steady state.	0.0074 s	0.0067 s	0.0058 s
The distance travelled by the water-saving valve during motion.	0.2617 mm	0.6482 mm	0.7884 mm
The height of the limit step of the valve.	0.7383 mm	0.3518 mm	0.2116 mm
The maximum velocity achieved during the motion process.	0.0849 m/s	0.2012 m/s	0.4512 m/s
The maximum resultant force exerted on the water-saving valve.	−6.9760 N	−20.9787 N	33.8751 N
The steady-state flow rate at the outlet of the water outlet.	6.207 L/min	7.213 L/min	7.306 L/min

presents a summary of the transient simulation results for three different water pressure conditions. Taking the case of 0.1 MPa as an example, when the water-saving valve reaches a displacement that corresponds to the effluent flow rate meeting the requirements of the national regulatory standards, the displacement is approximately 0.2617 mm. At this point, the height of the limit step of the water-saving valve is 0.7383 mm, and the corresponding flow rate is approximately 6.207 L/min, which is in line with the requirements of the national regulatory standards. Similar results are observed for the 0.3 MPa and 0.5 MPa conditions.

5.2. The Analysis of Pressure and Velocity in the Flow Field

Figure 14 and Figure 15 show the pressure and velocity cloud maps of the radial mid-section of the flow field corresponding to different times during the dynamic process of the water-saving valve from its static state to the outlet flow rate meeting national regulatory standards under the working condition of 0.1 MPa. From Figure 13 and Figure 14a–f, it can be observed that the distance between the top of the water-saving device inlet and the top of the water-saving valve gradually increases over time. This indicates that the water-saving valve is dynamically moving downwards, causing the valve opening height to continuously decrease. Meanwhile, over time, the pressure in most areas of the internal flow field of the water-saving device gradually increases, while the flow velocity gradually decreases. At the time of 0.0074 s, the water-saving valve reaches a steady state, at which point the flow field pressure reaches its maximum, and the flow velocity reaches its minimum.

From a positional perspective, the fluid region between the upper portion of the water-saving valve and the water inlet cover experiences the highest pressure, whereas the fluid regions on both sides and the lower portion of the valve experience relatively lower pressure. Furthermore, it is observed that the velocity distribution pattern in the aforementioned positions is inversely related to the pressure pattern, which aligns with the Bernoulli principle [31]. Specifically, locations with higher flow velocity have lower pressure, while locations with lower flow velocity have higher pressure.

6. Conclusions

This paper takes a constant-flow water-saving device as an example and conducts an analysis and study of its internal flow field and water-saving valve through transient CFD simulation. By utilizing dynamic mesh technology and UDF programs, a comprehensive design method for a constant-flow water-saving device including integrating theoretical analysis, numerical simulation, and experiments has been established. The main conclusions are as follows:

• A transient CFD model of a water-saving device was successfully developed and validated using UDF program, facilitating the design of elastic component parameters in water-saving device flow control systems. Through iterative computation, the initial length of the elastic component in the flow control system was determined to be 3.5 mm, and the initial opening height of the water-saving valve was set at 1 mm;
• In response to the aforementioned simulation calculations, relevant flow testing experiments were conducted, and the results of the experimental tests were subjected to necessary processing using the Six Sigma data analysis method. Based on the comparative analysis, it was demonstrated that the relative error between the simulated and experimental results is within 5%, which provides the evidence to support the accuracy of the transient CFD simulation model employed in this paper and the feasibility of the research methodology;
• The opening height of the valve under three different pressures was determined through simulation calculations. The analysis determined the water-saving valve opening heights under three operational pressures (0.1, 0.3, and 0.5 MPa) to be 0.7383 mm, 0.3518 mm, and 0.2116 mm, respectively, with corresponding outlet flow rates of 6.207 L/min, 7.213 L/min, and 7.410 L/min. These results satisfactorily meet national regulatory standards, validating the applied methodology.
• During dynamic valve motion, internal pressure within the flow field increased while flow velocity decreased. At the valve’s limit, the pressure peaked, and the velocity was minimized, consistent with Bernoulli’s theorem and indicating rational flow field distribution dynamics. The simulation analysis of the dynamic pressure and velocity changes in the internal flow field of the constant-flow water-saving device further confirms the accuracy of the mode and provides valuable data for further design improvements.

In summary, this paper successfully developed and validated a transient CFD model for optimizing constant flow water-saving devices, which significantly shortened the product development cycle. The model identified the optimal valve opening height under various pressure conditions and demonstrated compliance with national standards. Additionally, an in-depth understanding of the dynamic pressure and velocity changes within the device confirmed the model’s accuracy and provided valuable data for further design improvements, offering both theoretical guidance and practical application value. Future research should focus on exploring the underlying physical mechanisms of the VOF multiphase flow model to achieve a more accurate description of complex fluid flow characteristics. In addition, it is necessary to consider the influence of radial force on water-saving valves and combine it with multi-degree-of-freedom motion analysis to achieve more comprehensive simulation research.