**3. CFD Flow Structure and Grid Independence Analysis**

#### *3.1. Two-Dimensional Flow Field Model of Weir Diaphragm Valve*

The diaphragm of Weir-Type diaphragm valve is deformed and displaced by the stem loading, and the diameter of flow passage is compressed to achieve throttling effect until it is fitted with the sealing table at the top of the ridge to realize the complete closure of the valve (Figure 5).

**Figure 5.** Working Principle of Weir Diaphragm Valve.

In this paper, the LiquidlensTMLLG4 ultra-pure water treatment system of ENTEGRIS Company is taken as the reference of working condition of diaphragm valve. The relevant size parameters of DS12-2M-12F-3 manual diaphragm valve are taken as the reference for modeling. The flow field structure size can be obtained by simplification (Figure 6). The shape of the ridge has a major influence on the flow state and loss of the medium in the weir diaphragm valve. Five different sizes of the ridge structures (Figure 6) are designed to explore their effects on the flow characteristics of the diaphragm valve.

Determine the relevant flow parameters according to the reference operating conditions (Table 1). The diaphragm valve is used at the inlet and outlet of the system, so the back pressure at the outlet of the simulated diaphragm valve is generally set to *pout* = 400 kPa. When the nominal diameter

of diaphragm valve is *DN* = 20 mm and the system flow rate *Q* is set to 8 L/min, the average velocity of flow can be calculated from Equation (3),

$$v = \frac{Q}{A} = \frac{4Q}{\pi (DN)^2} \tag{3}$$

The average velocity of flow can be calculated to be about *v* = 0.42 m/s. According to the table above, the flow rate varies in the vicinity of 8 L/min. Therefore, a set of different flow velocities is set up in simulation to explore the characteristics of diaphragm valves under different Reynolds numbers.

**Figure 6.** Flow Path Structure Dimensions and Five Ridge Profiles.


**Table 1.** LiquidlensTMLLG4 System Flow Parameter Index.

In addition, according to the deformation results of diaphragm at different openings, the two-dimensional flow field model of valve at different openings can be obtained (profile E as an example in Figure 7).

**Figure 7.** The two-dimensional flow field model of valve at different openings (profile E).

## *3.2. Boundary Conditions and Simulation Settings*

After the flow field model is established, the mesh module is used to mesh the flow field and discrete flow fields. Select the adaptation in the size function, select the course in the relevant center, and set the grid size to 1 mm, 0.5 mm, and 2 mm respectively to generate the mesh. The meshing results are as shown in Figure 8 for the profile E. The simulation parameters in detail are shown in Table A1.

**Figure 8.** Mesh of different sizes under profile E. (**a**) for 0.5 mm; (**b**) for 1 mm; (**c**) for 2 mm.

The skewness is checked in the grid quality column, and the maximum skewness of the three meshes is 0.593 (1 mm), 0.539 (0.5 mm) and 0.504 (2 mm), respectively. All of these can meet the requirements of this simulation. In order to reduce the computational complexity of the simulation iteration and ensure a certain degree of accuracy, this simulation is other. The grid size of each basin shape is set to 1 mm.

The grid file is imported into FLUENT software, and the environment is two-dimensional flow field simulation. The acceleration of gravity is added in general. Model models select standard k-ε model, and model parameters follow the default values of the system. Water-liquid is added to the liquid medium material, and the default parameters are obtained. The wall material is made of steel as the prototype. Some parameters are modified, such as the absolute roughness value is changed to Δ = 0.02. The other parameters can be maintained by default because heat exchange is not involved in this time.

Boundary conditions: The inlet is the velocity inlet. When the relationship between Reynolds number and valve flow coefficient is simulated, the velocity input range is from *v* = 0.3 m/s to *v* = 0.8 m/s, and the interval is 0.05 m/s. When investigating the influence of ridge shape, the input is *v* = 0.5 m/s; the outlet is a pressure outlet, and the back pressure is *pout* = 400 kPa; the characteristic parameters such as turbulent intensity, hydraulic diameter (*DN* = 0.02 m), turbulent energy *k*, turbulent dissipation rate ε, turbulent viscosity ratio in the setting of inlet and outlet can be calculated according to the following formulas.

$$
\dot{a} = 0.16 \text{Re}^{(-1/8)} \tag{4}
$$

$$k = 1.5(vi)^2\tag{5}$$

$$
\kappa = 0.75 \text{C}\_{\mu} k^{1.5} / l = 0.75 \text{C}\_{\mu} k^{1.5} / (0.07 d) \tag{6}
$$

$$
\mu\_t = \rho\_0 \mathbb{C}\_{\mu} \frac{k^2}{\varepsilon} \tag{7}
$$

Among them, *C*<sup>μ</sup> = 0.09, *v* is the velocity of flow, ρ<sup>0</sup> is the density of water, μ*t*/μ is the turbulent viscosity ratio, and μ is the dynamic viscosity of water.

Solver method sets pressure as standard, calculates second-order upwind, and sets reference cross-section at the center of the valve orifice, so as to output characteristic parameters at the valve orifice in the calculation results. The simulation step size is set to 5000 steps, and other parameters such as relaxation factor and convergence residual range are all defaulted by the system.

The surface integrals are selected from the simulation results to output the results. By calculating the total pressure at the inlet, outlet and the middle section of the valve, the pressure loss between the outlet and the inlet can be obtained, and the flow coefficient *Cv* (*Kv*) and local resistance coefficient ζ can be calculated according to Equations (1) and (2).
