Computational fluid dynamics analysis and extended adaptive hybrid functions model-based design optimization of an explosion-proof safety valve

ABSTRACT Extremely complex flow channels and multi-parameter, highly nonlinear thermal fluid–structure interactions are the main factors restricting the exploration mechanism and optimal design of explosion-proof valves. To overcome these problems, comprehensive numerical research is performed in this paper, particularly concerning the method of valve dynamic modeling, and surrogate model-based design optimization. First, numerical models are presented; a dimensionality reduced computational fluid dynamics modeling method is proposed, using two approaches to simulate the blocking effect of flame-retardant sheets. Their accuracy is verified using both steady and transient simulations, which indicate that the equivalent volume is more accurate than the equivalent porous method. Second, to improve the flame-quenching ability of the explosion-proof valve, surrogate modeling-based design optimization is performed. In optimization, three structural parameters are selected as design variables and the extended adaptive hybrid functions (E-AHF) surrogate model is used as the predictive model. Based on the developed surrogate model, a genetic algorithm is implemented to identify the optimum structure of the flame-retardant sheets. To verify the performance of the optimized design, 3D steady-state simulations are performed. The results indicate that the cooling effect of the optimized scheme on the high-temperature gas is increased by 12.21%.


Introduction
Explosion-proof safety valves are widely used in various energy/pressure-related applications, such as the largescale diesel engines of ships, petrochemical plants and mining fields. Taking large-scale diesel engines as an example, the reciprocating motion of mechanical moving parts will cause high temperatures, leading to the lubricating oil on these moving parts evaporating into a flammable and explosive oil mist. When the concentration of the oil mist is high enough and encounters the high-temperature gas leaking from the piston cylinder, it will be ignited and trigger deflagration, causing the system pressure to rise rapidly and produce visible flames. In this case, the explosion-proof safety valves that are usually installed on the side wall of the crank cases of large-scale diesel engines will be opened in time to release the high-pressure and high-temperature gas. Meanwhile, the visible flame caused by the deflagration can also be quenched by the valve flame-retardant sheets, thereby protecting the surrounding operators and CONTACT Xueguan Song sxg@dlut.edu.cn equipment from damage. In short, the explosion-proof safety valve can be regarded as the ultimate safety barrier for large-scale diesel engine systems. To ensure that the explosion-proof safety valve can works normally and effectively, it is necessary to conduct an in-depth investigation on its dynamics and design optimization. However, as a thermal fluid-structure interaction (FSI) system, the dynamics of the explosion-proof valve are highly complex, and using traditional experimental or analytical methods for analysis and optimization of the mechanism is usually expensive and inefficient. In recent years, researchers have begun to use numerical tools to solve FSI problems, and have shown great advantages, such as higher accuracy and availability of flow details, which provide a good basis for the refined research of valves. However, for explosion-proof valves, which have extremely complex flow channels and multi-parameter characteristics, direct modeling requires a lot of computing resources and time, which brings challenges to analysis of the mechanisms and optimization design in practical engineering applications. To improve the safety and reliability of the systems, there is an urgent need to explore methods for the efficient and high-precision modeling of valves and schemes for multi-parameterbased optimal valve design.
The dynamic operation of the explosion-proof safety valve is mainly determined by the mechanical force (exerted by the valve spring) and the lift force (exerted by the fluid flow). The spring force is relatively easy to quantify because it is usually a linear function of spring constant and compression. In contrast, the fluid force is more complicated (David & Pascal, 2010;Wang et al., 2019;Yuan et al., 2019Yuan et al., , 2021 because it is affected by many factors, such as the system pressure, the flow channel geometry and the valve disc movement . Concisely, the ability to accurately predict the transient fluid force acting on the valve disc is a prerequisite for investigation of the valve dynamics, and this is also where the difficulty exists. In a broad sense, the explosion-proof safety valve is a type of safety valve. It not only contains the basic structure of spring-loaded safety valves (such as the spring, the valve disc and the nozzle), but also includes an array structure (flame-retardant sheets) which can be used for flame quenching. To understand the mechanism and/or for design optimization purposes, many safety valverelated studies have been performed since the 1960s. For example, to investigate the dynamic response of a pressure safety valve working in pneumatic service, Darby (2013), Darby and Aldeeb (2014) and Aldeeb et al. (2014) performed both numerical and experimental analyses on different sizes of spring-loaded safety valves. A mathematical model, which included a set of five coupled algebraic/differential equations, was developed to predict the dynamic response of the safety valves. To verify the accuracy, the predicted results were compared to experiments, which indicated a good consistency. In their study, the fluid disc force, which is of great importance to valve dynamic responses, was derived based on theoretical formulas. However, according to the research performed by Stone (1960), who conducted a series of experimental and analytical analyses on a hydraulic poppet valve to identify the characteristics of the fluid disc force under different operating conditions, there is a non-negligible error (about 25%) between the experimental and analytical approaches. This means that under certain conditions, using analytical methodology for fluid force prediction may be inappropriate.
With the development of computer technology, computational fluid dynamics (CFD) methods have become a powerful tool for solving FSI problems (Gao et al., 2021;Ghalandari et al., 2019;Kong et al., 2018;Liu et al., 2020;Mosavi et al., 2019). For example, to explore the cause of unstable valve responses (in certain conditions, the spring-loaded safety valve may respond in an unstable manner, such as valve flutter, chatter and low-frequency cycling, which may impair the operation of the valve and even bring safety hazards to the pressure system), Song et al. (2014) performed a thorough investigation on the dynamics of a typical American Petroleum Institute (API) standard spring-loaded safety valve. A three-dimensional (3D) CFD model was developed to simulate the details of the transient flow inside the safety valve, including extracting the transient fluid force exerted on the valve disc. With the same purpose as Song et al. (2014), Hős et al. (2014Hős et al. ( , 2017 and Bazsó and Hős (2013) developed an analytical model to predict the dynamic response of a pressure vessel-piping-safety valve system. As already mentioned, using analytical methodology to quantify the fluid disc force may result in non-negligible errors. To overcome this, they presented a numerical/experimental-based method for calculation of the fluid disc force. Specifically, CFD simulations or experimental tests were performed first, then the simulation or experimental data were used to fit the transient fluid disc force, and then the fitting force was used to solve the motion equations of the valve disc.
To further identify prior research that dealt with the dynamic response of spring-loaded safety valves, a literature survey was performed, and more than 80 studies were found. From these studies, the following three points can be summarized. (1) Most of these studies only investigated the dynamics of spring-loaded safety valves, as well as their connecting pipes and/or pressure vessels, whereas few studies in the open literature have taken the effect of flame-retardant sheets into consideration. (2) CFD is a powerful method to deal with the FSI phenomenon of safety valves; however, limitations in computing resources mean that using a 3D CFD model for valve dynamic investigations inefficient. To overcome this, a feasible way is to simplify the 3D CFD model into an equivalent two-dimensional (2D) model. To the authors' knowledge, few published studies have specifically focused on this type of CFD model simplification. (3) Finally, beside the prevention of overpressure, another important function of the explosion-proof safety valve is to quench the visible flames produced by explosion. This function is achieved through the use of flame-retardant sheets in the explosion-proof safety valve. To maximize the flame-quenching ability, highly efficient methods for flame-retardant sheet design optimization should be investigated, but few studies have been published that are specifically aimed at this area.
In the present study, both numerical model analysis and surrogate model-based design optimization were performed on an explosion-proof safety valve. For dynamics analysis, a reduced dimensionality CFD model was developed, where different simplification methods of the flame-retardant sheet were verified and compared. This could provide a reference for the model development of valves with similar structures. Thereafter, to maximize the flameout ability of the explosionproof safety valve, a surrogate model-based optimization is carried out on the flame-retardant sheets. The key points pursued in this study can be summarized as follows: (1) reduced-order CFD model development of an explosion-proof safety valve; (2) dynamic analysis of the explosion-proof valve in case of deflagration; and (3) surrogate model-based design optimization on the flameretardant sheets. These aspects are discussed in full in this paper.

Details of explosion-proof safety valves
Explosion-proof safety valves are self-actuated springloaded valves, which can provide protection for pressure systems in case of explosion/deflagration. When an explosion/deflagration occurs, high-pressure and hightemperature gas will be generated instantaneously, which is hazardous to the equipment and the surrounding operators. For safety, the explosion-proof safety valves are designed to be opened in time to reduce the system pressure and cool the high-temperature gas. Figure 1 shows a schematic diagram of an explosionproof safety valve in an opening state. The valve seat is usually connected to the side wall of the protected equipment (such as crank cases of large-scale diesel engines) by a flange. When closed, the valve disc is pressed against the valve seat by the valve spring. In case of deflagration, the valve disc will be lifted to a level to allow the generated gas to rush into the region of the flame-retardant sheets. After the airflow passes through the first sheet layer, it will be dispersed into multiple small streams, and then flow into the labyrinth channel composed of several flame-retardant sheets. In the labyrinth channel, the airflow continuously impacts and exchanges heat with the sheet wall, which will cause a lot of pressure and heat loss. When the air temperature drops below its quenching temperature, the flame will be extinguished. Finally, a safe low-pressure and low-temperature air stream is released into the atmosphere. Meanwhile, the pressure in the equipment decreases. When it is lower than the valve set pressure, the valve disc moves downwards, and the explosion-proof safety valve will be closed again.

CFD model development
To efficiently and accurately simulate the dynamics of the explosion-proof valve, CFD model-related investigations are performed in this section, which includes the method of system decomposition, model development of each subsystem and model simplifications of the flameretardant sheets.

System decomposition
The most direct way to carry out valve modeling is to use a 3D CFD method, so that the dynamics of the fluid flow can be obtained in detail. However, in actual situations the pressure systems protected by explosion-proof safety valves usually have large volumes, and the flow path of the valve is complicated. Direct 3D modeling of the whole system requires a large number of mesh grids and considerable computational resources. One way to overcome this is to decompose the entire system into multiple subsystems, and then use appropriate methods to model each subsystem. Figure 2 shows the schematic diagram of the system decomposition and model development of the explosionproof safety valve. As shown in the left-hand side of the figure, the whole system can be decomposed into three subsystems, namely, the pressure vessel subsystem (which corresponds to the crank case of a diesel engine), the safety valve subsystem and the flame-retardant sheets subsystem. The pressure vessel subsystem is the main place where the explosion occurs and it usually has very complex inner geometries and large volumes, which require a large number of mesh grids for CFD modeling. However, in actual situations, explosions often occur very quickly, and the spatial gradients of the vessel pressure and the air temperature are small. Thus, for efficiency, a virtual pressure point is used to replace the pressure vessel subsystem, with the assumption that its internal physical properties (such as vessel pressure and temperature) are spatially consistent.
The safety valve subsystem is the main overpressure prevention device in the explosion-proof safety valve. It consists of two parts, namely, the fluid domain bordered by the valve seat and valve disc, and the spring-massdamping system, composed of the spring and valve moving parts. For the fluid domain, it has an axisymmetric geometric feature, which makes it feasible to perform 2D CFD model development. In this paper, both 2D and 3D CFD models of the safety valve subsystem are developed. The subsystem of the flame-retardant sheet provides a blocking effect on the high-speed and high-temperature fluid flow, and it has an extremely complicated fluid flow structure which makes it hard to model directly with 2D CFD or analytical approaches. For modeling, the most convenient way is to perform 3D CFD model development, with which both the blocking effects and the fluid details of the flow channels can be obtained. However, it will consume a large amount of computing resources. To overcome this, an alternative method is to use an accurate and efficient model equivalent to the blocking effect of the flame-retardant sheets. In this paper, two methods, namely, the equivalent volume and the equivalent porous methods, are used, and their accuracy is verified by comparison to the simulation results produced by 3D CFD models.

Model development of the pressure vessel subsystem
The pressure vessel subsystem is the power source of the explosion-proof safety valve, and it can be set as the boundary condition of CFD simulations. To correspond with CFD simulations, the pressure condition of the pressure vessel subsystem is defined as follows: where P and P 0 are the vessel pressure of the current and the previous timestep, respectively; v is the rate of pressure rise due to the explosion; t is the size of the timestep;m is the mass flow rate at the location of the valve inlet; R is the gas constant; T is the temperature; V is the volume of the pressure vessel; M is the molar mass of the air, and t Explosion is the duration of the explosion. It is worth noting that the explosion process in the pressure vessel is very complicated because it is related to many factors, such as the concentration of oil mist, the composition of the mixed gas and the temperature. Therefore, the specific values of the pressure rise rate v and the duration of explosion t Explosion need to be determined according to the specific operating conditions of the pressure vessel subsystem. Because the main purpose of this paper is model development, the specific value of v may not make much difference. To facilitate modeling, a constant value is assigned to v to simulate the pressure conditions of the pressure vessel subsystem.

Model development of the safety valve subsystem
The safety valve subsystem is the main pressure relief device of the explosion-proof safety valve, and its behavior is essential to the dynamic analysis of the entire system. Owing to the high nonlinearity and random nature of turbulent flow, the internal fluid of the safety valve is very complicated. To perform accurate calculations, a CFD approach is used to model this subsystem. The principle of CFD simulation is to solve the algebraic/differential governing equations (including conservation equations of mass, momentum, energy and other additional source terms) applied in a designated region, namely, the fluid domain to be solved. However, owing to the high nonlinearity of the turbulent flow, solving these conservation equations directly requires very small-scale mesh grids and a large amount of computing resources. To improve the efficiency, an alternative approach is to use the Reynolds-averaged Navier-Stokes (RANS) method to divide the instantaneous quantities into time-average and fluctuating terms, and then use turbulence models to correlate them. This can not only close the governing equation set, but also avoid solving extremely complicated fluctuating terms of the flow. The fluid domain of the safety valve subsystem, the mesh grids, tests regarding the turbulence model and timestep for transient simulations are shown in this subsection. Figure 3 shows the fluid domain and mesh grids of the safety valve subsystem. Owing to the axisymmetric structure of the fluid domain, a 2D mesh is the first choice for modeling (left-hand side of Figure 3). For validation purposes, a corresponding 3D mesh model is also developed (right-hand side of Figure 3), with which the simulation results can be set as the criterion for 2D model verification.
In actual situations, the valve disc moves up and down. To follow the disc motion in simulations, the fluid domain of the safety valve subsystem is decomposed into two parts, namely, the subdomain of the valve seat and the subdomain of the valve disc. In transient simulations, the valve seat subdomain is set to be static while the valve disc subdomain is set to be a movable rigid grid, the movement of which is determined by the dynamic governing equations of the valve disc. The transient CFD simulation is performed using commercially available code, and to simulate the movement of the valve disc, the moving mesh method is implemented to change the position of the valve disc at the end of every timestep. Figure 4 shows the dynamic mesh settings and the boundary conditions for the 3D CFD models (the model settings of the 2D simulations are the same), where the velocity of the valve disc subdomain is specified using user-defined functions (UDFs).
The movement of the valve disc is determined by the interaction between the fluid force and the spring force, which can be derived according to Newton's second law: where M is the mass of the valve moving parts, x is the instantaneous valve opening,ẋ is the disc velocity, ξ is the damping coefficient, f is the friction, F Support is the impact of the valve seat when the valve is fully closed, and t is the size of the timestep. In transient simulations, Equations (3) and (4) are programmed by the UDF method, where the fluid force (F Fluid ), spring force (F Spring ) and instantaneous disc position (x) are obtained by UDF macros at the end of every timestep.

Model development of the flame-retardant sheet subsystem
For geometrically sensitive research, such as flow channel optimization, it is necessary to perform 3D CFD modeling on the flame-retardant sheets. However, for other studies, such as the dynamic analysis of explosion-proof safety valves, the 3D modeling method is inefficient and will require large amounts of mesh grid and computing resources. Therefore, it is necessary to explore a more efficient method for modeling the flame-retardant sheets. To this end, the equivalent volume and the equivalent porous methods are used here to simulate the blocking effects of the flame-retardant sheets.
The principle of the equivalent volume method is to ensure that the volume of the 2D fluid domain between different layers of flame-retardant sheets is equal to that of the 3D model, while keeping the spatial position unchanged, as shown in Figure 5. The equivalent method is as follows: where r i+1 and r i are the radii of two adjacent layers of flame-retardant sheets, b i is the thickness of the flow    of the explosion-proof safety valve. Figure 5(c) shows the equivalent 2D CFD model of Figure 5(b), where the thickness b i is calculated based on the total circumferential volume of the fluid domain framed by the red line.
The principle of the equivalent porous method is to use appropriate porous media to simulate the blocking effects of the solid structures on fluid flow. Porous media refers to a combination of multiphase substances with complex internal structures and a large number of voids, such as coal, wood, filters, soil layers and catalytic beds. For CFD model development, directly modeling porous media will require a lot of grids and huge computing resources, which is difficult to use in practical engineering situations. To overcome this, a compromise method is to replace the actual structure with an analytical model, as shown in Figure 6. The flame-retardant sheet of the explosion-proof safety valve system in this paper is made up of five circular screens, in a staggered arrangement. It can be assumed to be a porous medium, and the momentum loss of the flame-retardant sheet system to fluid flow can be calculated based on the permeability and porosity.
In CFD simulations, the porous model of the superficial velocity porous formulation was used to describe the pressure drop along the flow direction. For the heat transfer, the thermal equilibrium assumption is assumed; for the porosity, the volumes of the total domain and the fluid domain of the flame-retardant sheet are equal to 13147.60 and 9358.80 mm 3 , respectively, so the porosity of the medium is determined to be 71.18%. The inertia and viscosity coefficients of the porous media are fitted based on the results of a series of steady-state CFD simulations, and their values are calculated to be 6403.24 and 5.05 × 10 6 , respectively.

CFD settings
CFD model settings, such as the density of the mesh grid, the turbulence model and the solver configurations are critical to ensure the convergence and accuracy of CFD simulations. To obtain the most appropriate model and settings, validations regarding the CFD mesh grid, turbulence model and simulation timestep are performed in this subsection.
For the turbulence model and the mesh grid, the predictive ability of the fluid disc force is set as the evaluation criterion for verification, because it is crucial to determine the dynamics of the explosion-proof safety valve. For the turbulence model, its ability in lift force prediction has been studied by the authors, where experimental tests and CFD simulations have been performed on a commercially available pneumatic safety valve (Zong et al., 2020). The result indicates that the shear stress  transport (SST) k-omega (k-ω) model produced the minimum error and thus was identified to be the optimal choice for compressible fluid force predictions.
For the mesh grid, a reasonable density/number is essential to ensure the accuracy and efficiency of CFD simulations. To correspond with the SST k-omega turbulence model, the mesh on the wall of the valve disc was refined, and it was found that when the height of the first mesh layer is lower than 5e-6 m (the growth rate is set to 1.5), the maximum value of y+ on the valve disc is 5.76 (at the edge of the valve disc), while the average y+ value is 2.33. Considering the overall value and the requirements of the SST k-ω turbulence model, the grid scheme with the height of the first layer equal to 5e-6 m (the growth rate is set to 1.5) is adopted in this paper. To identify the optimal mesh, steady-state 1/50 3D CFD simulations are performed on three valve openings using different mesh densities, while the grid distribution on the wall of the valve disc remains unchanged. Figure 7 shows the results of mesh tests, where five mesh densities are used to predict the fluid force exerted on the valve disc for each valve opening. The results indicate that the predicted fluid force varies significantly when the mesh number increases from 14,000 to 44,000. As the mesh grid continues to increase, the fluid force changes a little. Thus, it can be concluded that the fluid force is independent of the mesh grid when the mesh number is larger than 44,000. For accuracy and efficiency, the mesh number of 44,000 is chosen for the final CFD simulations.
In addition to the mesh grid and turbulence model, the timestep size is another critical parameter to ensure the accuracy and convergence of transient CFD simulations. To obtain the optimal timestep size, transient simulations are performed on the 3D CFD model using four timesteps. Figure 8 shows the results of these simulations, where Figure 8 It can be seen from Figure 8 that the timestep size has a great influence on the dynamic predictions of the explosion-proof safety valve. When the timestep decreases from 0.10 to 0.02 ms, the predicted curves of valve opening as well as the disc velocity vary significantly. As the timestep continues to decrease, such as from 0.02 to 0.01 ms, the curves change a little, which means that the transient simulation is converged for the timestep. For accuracy and efficiency, the timestep size of 0.02 ms is identified as the optimal choice for transient simulations.
Beside the mesh grids and timestep, another important setting concerns the solver. To facilitate description, the critical solver settings of transient CFD simulations are tabulated in Table 1. Before each transient simulation, steady-state simulation will be executed, and the result will be set as the initial state of the transient simulations.

CFD analysis of the explosion-proof safety valve
For model verification, dynamic analysis of the explosionproof safety valve is performed in this section. To facilitate comparison, 3D CFD simulation is carried out initially.
The explosion of a large diesel engine is one type of deflagration phenomenon caused by the ignition of a  high-concentration oil mist. Unlike conventional explosions such as detonation, deflagration is a subsonic combustion wave in which the pressure increases rapidly but not drastically. The pressure increase in the vessel will cause the valve disc to be lifted to release the excess fluid medium, so as to prevent catastrophic consequences; when the fuel in the container burns out, the explosionproof safety valve will be closed because there is not enough fluid force to balance the valve spring force. To simulate the valve opening process, the rate of pressure rise v (Equation 1) of the pressure vessel is defined as 3 MPa/s, and the duration of the explosion t Explosion is defined as 33 ms to ensure that the valve disc can be lifted to a certain level. For the valve reclosure process, the rate of pressure rise v is set to be 0, namely, no pressure/energy will be generated and the pressure of the vessel will be updated according to the transient flux through the valve inlet, as shown in Equation (1). Figure 9 shows the results of the transient CFD simulations, where Figure 9(a) illustrates the instantaneous valve opening obtained from 3D transient simulation.
Regions I and II correspond to the valve opening and reclosure processes, respectively. To facilitate comparison and 2D model verification, the results of these two processes are compared separately in Figure 9(b) and (c). It can be seen that for the valve opening process, both the equivalent volume and equivalent porous models produce similar results to the 3D model. In contrast, for the valve reclosure process, a different scene appears, with the 3D and 2D equivalent volume model producing similar results, and the 2D model with equivalent porous simplification leading to a longer reclosure time. The specific simulation results of the 2D and 3D simulations are tabulated in Table 2.
According to the results of Figure 9 and Table 2, it can be inferred that the 2D model with equivalent volume simplification can accurately reproduce the results of 3D simulations, and its accuracy is higher than that of the equivalent porous model. For accuracy and efficiency, the 2D equivalent volume model is considered to be the optimal choice for dynamic predictions of the explosion-proof safety valve.
Besides the overall performance of the 3D and 2D simplification models, more in-depth analysis is performed to explore the root cause of the divergence between the results of these three models. As mentioned earlier, the dynamic behavior of the explosion-proof safety valve is mainly determined by the interaction between the fluid force and the spring force, where the fluid force is more critical because it is more complex and sensitive to geometry than the spring force. Thus, to explore the cause of the divergent performance of different models, it is necessary to evaluate their ability in fluid force prediction. To achieve this, a series of steady-state CFD simulations is performed on six valve openings with the boundary condition of the pressure inlet set to be 1.0 bar. Fluid properties, such as the fluid force exerted on the valve disc, as well as the mass flow rate through the valve inlet, are compared. Figure 10 shows the results of the comparison, where Figure 10(a) and (b) show the fluid disc force and mass flow rate, respectively. It can be seen that both of the CFD models produce similar results for the mass flow rate at all six simulated valve openings, which means that the parameter setting of the porous domain is reasonable. In contrast, different performances appear in the fluid force predictions, where the 3D and 2D equivalent volume models produce close force values at almost all valve openings, but the fluid forces obtained by the 2D equivalent porous model are overpredicted or underpredicted. To explore the reason for this, more analysis is carried out. Figure 11 shows the contours of the velocity and the static pressure obtained at 5 mm valve opening. To facilitate comparison, only the critical domains, namely, the fluid domains near the valve nozzle, are illustrated and compared. It can be seen that the contours obtained from the 3D model and 2D equivalent volume are similar, but they are different from the contour obtained from the 2D equivalent porous model, which means that the 2D model with equivalent simplification cannot predict the flow pattern accurately. The flow pattern near the valve nozzle is related to the momentum conversion from the fluid flow to the valve disc (the original source of disc fluid force); thus, the inaccurate flow pattern prediction is considered to be the reason for the inaccurate predictions of the fluid disc force, and is also considered to be the root cause of the divergent behaviors of the valve dynamic operations.
In addition to the simulation results, the efficiency of different models was compared, as shown in Table 3, where the calculation times of the valve opening and reclosure process (corresponding to Figure 9, with the same solver settings: parallel, six-processes solver, 4.7 GHz) are tabulated. It can be seen that the calculation times of the 2D models are close, and are far shorter than that of the 3D model, confirming the efficiency of the 2D model developed in this paper.

Optimization of the flame-retardant sheets via a surrogate model
Besides the prevention of overpressure, the other important function of the explosion-proof safety valve is to quench the flame caused by the explosion. This is accomplished by the flame-retardant sheets, which have a very complex structure. The conventional discrete optimization typically requires many iterations to converge (Song et al., 2013). To solve this issue, a surrogate model based on limited simulations is used to replace the computationally expensive CFD simulations. The process of the surrogate model-based design optimization is shown in Figure 12.

Optimization problem definition
In this work, the optimization objective is to maximize the flame-quenching ability of the flame-retardant sheets, and the design variables are three structural parameters, namely, the thickness of each flame-retardant sheet b, the diameter of the connection channel D and the ratio of the gap thicknesses between two adjacent flameretardant sheets α, as shown in Figure 13. To quantify the performance of the flame-retardant sheets, two normalized variables regarding the mass flow rate (which is a reflection of the pressure relief ability) and temperature difference (TD) are used. The method of variable normalization, the weight assignment and the design space are shown as follows: where T Inlet and T Outlet are the temperature (in Kelvin) of the inlet and outlet of the flame-retardant sheets, respectively; ηṁ is the normalized values of mass flow rate; TD is the temperature difference,ṁ is the mass flow rate, m min andṁ max are the minimum and maximum values of the mass flow rate of all the experiments (simulations), respectively; and maximize Y (Max Y) is the objective of the present optimization.

Design of experiments
The design of experiments (DoE) usually refers to the strategy of sample point generation, and is one the key steps to ensure the accuracy of a surrogate model. Of the   (Olsson et al., 2003), and it is used to generate sample points for the surrogate model. With the three independent design variables of flameretardant sheets, 30 sample points are generated to construct the surrogate model, and 12 validation points are generated to validate its prediction accuracy. The distributions of the training and validation points are shown  in Figure 14. With the 42 generated points, different CFD models are developed. The CFD model for the original sheet design is shown in Figure 15, where the mesh grids and the boundary conditions are also illustrated. To improve efficiency, the renormalization group (RNG) k-epsilon (k-) turbulence model combined with the standard wall function was used in CFD simulations of the flame-retardant sheets, and the mesh grid on the wall boundary was controlled to a reasonable height so that the value of y+ was mainly within the range of 10-60. Because the primary purpose is to optimize the performance of the flame-retardant sheets, it was decided to isolate the effects of the safety valve to allow a clearer and more direct assessment of the abilities of the flame-retardant sheets, namely, the flow domain of the safety valve subdomain is excluded and the inlet of the CFD model is changed to the position shown in Figure 15. With the developed models, steady-state simulations were performed.

Surrogate modeling
Based on the CFD results of 30 sample points, four surrogate models, namely, polynomial regression surface (PRS) (Myers & Montgomery, 1995), radial basis function (RBF) (Gutmann, 2001), kriging (KRG) (Jerome et al., 1989) and support vector regression (SVR) (Smola & Scholkopf, 2004), are constructed. A brief list of the parameters and functions of the four surrogate models used in this paper is shown in Table 4.
Before performing further optimizations, the accuracies of the four developed surrogate models were assessed. The results of the surrogate modeling are shown in Figure 16. (To facilitate visualization, D was set to a constant value of 3.25 mm.) It can be seen from Figure 16 that the PRS and KRG models produce similar predictions, but they are somewhat different from those of the RBF and SVR models. For validation purposes, 12 additional confirmatory simulations were performed (as mentioned, the 12 validation points were also generated using the LHS approach, but not generated at the same time as the 30 base sample points). To quantify the error of each model, several evaluation indices, namely, the coefficient of determination (R 2 , Equation 9), the root mean square error (RMSE,Equation 10) and the maximum absolute percentage error (MAPE, Equation 11) were used: where m = 12 is the number of the validation points, y i is the value of the validation point,ŷ i is the value predicted by the surrogate model, andȳ i is the average value of the 12 validations. The index R 2 reflects the overall performance of a surrogate model, with a value of R 2 closer to 1 meaning better accuracy.
Note: PRS = polynomial regression surface; KRG = kriging; RBF = radial basis function; SVR = support vector regression. Table 5 shows the results of the model validations. It can be inferred that the abilities of the different surrogate models are diverse; among them, the KRG model produces the highest values of R 2 and the lowest RMSE and MAPE, which means that it is the optimal choice among the four models. However, as shown by Table 4, although each individual surrogate model has a good R 2 value in temperature and flux predictions, they have high MAPE values (both are greater than 12.5%), which means that each model will produce a certain local error, and this may lead to inaccurate final optimization results.

Extended adaptive hybrid functions (E-AHF) model
For the purpose of improving the accuracy, an advanced and robust ensemble surrogate model, namely, the E-AHF model, was used in this paper to construct the relationship between the design variables and the response of the flame-retardant sheets (Song et al., 2018). The E-AHF is a model that is constructed with adaptive weights based on the Gaussian process-estimated error and a redundant model-eliminating strategy, aiming to take advantage of the diversity of well-performing individual surrogate models to improve the prediction accuracy and robustness for various problems (Song et al., 2018). There are two steps in E-AHF model development, namely, step 1, selection of individual surrogate models, and step 2, weight calculations and model ensemble.
Step 1, the selection of individual surrogate models, is accomplished by comparing the global accuracy of each model, where the global accuracy is obtained by using the leave-one-out (LOO) cross-validation (CV) method (Song et al., 2018): where CV error is the cross-validation error of one individual surrogate model, n is the number of sample points, y j andŷ j , respectively, represent the real response and prediction value of the jth sample points, and in the calculation, all sample points except for the jth point are used. Using Equation (12), the accuracy of each individual surrogate model can be quantified. A smaller CV error value represents higher model accuracy, and thereby the surrogate model with highest precision can be selected, and it will be set as the baseline model of the hybrid surrogate model.
Step 2, weight calculations and model ensemble, can be divided into three substeps, namely, (1) local measure estimation, (2) probability estimation and (3) local weight determination. The details of these three substeps are shown in Equations (13)-(15) (Song et al., 2018). (1) Local measure estimation: where σ is the constant process variance of the Gaussian field, and ψ is the correlation matrix with the elements.
(2) Probability estimation: where P i (x) is the function of the probability coefficient of the ith model, and y i (x) and y base (x) are predictions produced by the ith model and baseline model, respectively.
(3) Local weight determination: where m is the number of surrogate models, and ω i (x) is the coefficient of each individual surrogate model. After performing the above three substeps, the final form of the E-AHF model can be expressed as Equation (16):ŷ whereŷ(x) andŷ i (x) are predictions produced by the E-AHF model and the ith individual surrogate model, respectively.
Similarly to the individual surrogate model, the performance of the E-AHF model in flux and temperature predictions is tested. To verify its applicability, the R 2 , RMSE and MAPE of the individual models and the E-AHF model are compared, as shown in Figure 17. In addition, to conduct a direct test, the comparison between the 12 validation points and the E-AHF model predictions is also performed, as shown in Figure 18. The x-axis and y-axis represent the results of E-AHF and the validation points, respectively (for ease of comparison, all data are normalized to 0-1).
It can be seen from Figure 17 that among the five test models, the E-AHF produced the highest value of R 2 , and the lowest values of RMSE and MAPE. From Figure 18, it can be seen that the E-AHF model can accurately predict almost every validation point, confirming its accuracy and applicability in flux and temperature predictions.

Design optimization
The objective of the optimization is to maximize the overall performance of the flame-retardant sheets to ensure that high-pressure and high-temperature gas produced by the deflagration can be discharged and cooled efficiently. To achieve this, a genetic algorithm (GA)-based optimization is carried out in this subsection. The maximum Y (in Equation 8) is set as the optimization objective and the E-AHF model is used as the fitness function. The optimization parameter settings are as follows. When the optimization is converged, an optimal value of TD equal to 386.14 K is obtained, which is 12.21% higher than that produced by the original structure of the flame-retardant sheets (TD = 344.11 K, with D, b and α, respectively, equal to 2.40 mm, 3.20 mm and 0.80). The corresponding parameters of the optimized scheme of the flame-retardant sheets are: D, b and α equal to 2.00 mm, 4.00 mm and 1.00, respectively.
To validate the results of the optimization, additional 3D CFD simulation is performed with the optimized structure of the flame-retardant sheets. Figure 19 shows the results of the simulations regarding the initial and optimized structure, where streamlines and temperature contours at the middle-plane of the flame-retardant sheets are compared. It can be seen that in the original design scheme, the internal flow of the flame-retardant sheets is relatively uniform, and the air temperature is continuously reduced; however, in the optimized scheme, the flow upstream of the flame-retardant sheets (where the temperature difference between the air and the wall is the largest) is more complicated, making the air fully collide on the surface of wall and conduct heat transfer. This is considered to be the main reason for the large temperature drop caused by the optimization scheme. To explore the flow process of different design schemes in more depth, the pressure and temperature distributions (along the red line in Figure 19) are plotted and  compared, as shown in Figure 20. It can be seen that the trend and distribution of the flow pressures are similar (Figure 20a), which means that the optimized design will not reduce the pressure relief function of the flame-retardant sheet (explosion-proof valve). In terms of temperature distribution, there are obvious differences along the flow direction. The differences begin to appear upstream of the flow, and continue to accumulate. This corresponds to the temperature difference-related analysis mentioned; that is, the full collision and heat exchange between the fluid and the wall caused by the upstream complex flow is the reason why the optimized solution has a better cooling function than the original solution.

Conclusions
This paper performed comprehensive research on an explosion-proof valve, particularly concerning the dynamic model construction and structural optimization of the valve, with regard to the most two important functions of the explosion-proof valve, namely, pressure relief and flame-retardation. The conclusions of this study can be summarized as follows. (1) Both 2D and 3D CFD explosion-proof safety valve models are developed, which can be used to predict the dynamics of the explosion-proof safety valve. To simplify the model, two methods, namely, the equivalent porous and the equivalent volume method, are proposed to simulate the blocking effect of the flameretardant sheets. The accuracy of these two simplified methods is verified by 3D transient simulations, which indicate that the model with equivalent volume simplification is more accurate than that with equivalent porous simplification.
(2) To discover the reason for the different abilities of different models, steady-state simulations are performed and analyzed. The results indicate that the different abilities of the models in flow pattern prediction are the root cause. (3) To optimize the performance of the flame-retardant sheets, a surrogate model-based design optimization is proposed, where the LHS-based 3D CFD simulation, the E-AHF approach and the GA are used for design of experiments, surrogate modeling and optimization, respectively. To validate the optimized scheme, comparisons between the original and optimized designs are performed, and the results show that the flame-quenching ability of the optimized flame-retardant sheets is 12.21% higher than that of the original structure.
This research is an extension of previous research on safety devices. Although it cannot include all actual situations present in industry, the authors believe that it could provide a reference for the design and optimization of similar related devices. However, there are several limitations in this study: (1) limited by the test conditions, experimental tests are absent, which may weaken the convincibility of the dynamic analysis of the explosionproof safety valve, although the method of CFD modeling has been verified in our previous research, which was a study on safety valve model development (Zong et al., 2020); (2) only three parameters of the flame-retardant sheets have been used for optimization, which may compromise the ability of the optimization method; and (3) although the E-AHF model used in this paper showed good performance in mass flow rate and temperature predictions, its predictive ability in other more complex physical processes needs further verification. These limitations should be addressed carefully in future studies.