Hybrid Numerical Simulation of Jet Blast Distance of a Departing Aircraft

A hybrid numerical simulation method was established by combining the Spalart-Allmaras (SA) turbulence model and detached eddy simulation (DES). Numerical simulations were carried out to model cold and hot spray conditions of a nozzle without considering the internal flow of an engine to determine jet conditions. Analysis results show that the calculated hot spray results more in line with the reality. (e jet effect of a typical aircraft engine was simulated numerically to determine the distance influenced by the jet blast from a departing aircraft engine.


Introduction
To address the strains created by an increasing number of flights and the lack of airport support capability, major airports in China have been reconstructed and expanded. At present, more than ten airports in China have adopted a multiple runway operation mode [1][2][3]. Most of China's multiple runway airports have adopted a parallel runway mode, making it difficult to avoid the problem of runway crossings during actual operation. China has the following runway-crossing protocols. First, "if one aircraft enters the runway, then other aircraft cannot cross the runway," such as at Shanghai Hongqiao International Airport and Shanghai Pudong International Airport. Second, "one can choose to cross the runway from the front side of a departing aircraft," such as at Chongqing Jiangbei International Airport.
ird, "bypass the runway in a U-shaped path to achieve the purpose of crossing," such as at Beijing Capital Airport. e above methods for crossing a runway avoid threatening aircraft safety during ground operations but seriously restrict operational efficiency of the ground. erefore, China has considered an operational mode that traverses the runway from the rear side of the departing aircraft, taxi-behind, as shown in Figure 1. e mode taxi-behind is to cross the runway behind the departing aircraft in order to reduce the operational conflict of the airport scene and improve operational efficiency, for example, O 'Hare Airport in the United States has used this model and demonstrated good safety and efficiency improvements. e jet blast of the departing aircraft is the most important factor hindering the implementation of taxi-behind. Without adequate safety interval, an aircraft crossing a runway could be blown off course or even overturned by the strong aerodynamic load of the jet blast from the departing aircraft. e magnitude of the safety interval mainly depends on the strength of the jet blast of the departing aircraft and the bearing capacity of the runway-crossing aircraft, so it is necessary to study the influence distance of the jet blast of the departing aircraft engine. At present, computational fluid dynamics (CFD) numerical simulation and the real engine test are the main methods to analyze the impact of aircraft jet blast. Due to the difficulty, high cost, and great safety risk of the real engine test on the runway and aircraft engine data are highly confidential in countries, we can only get the limited data of jet velocity distribution from the engine manufacturer or the aircraft manufacturer, and it is not enough to be used in the research of the runway operation mode. e hybrid numerical simulation method was adopted in this study for research.
Compared with domestic research, foreign research in this field was carried out earlier. In addition to the experimental method, the numerical simulation method was used to obtain the formation and evolution process of the jet as well as the parameters such as velocity, pressure, and temperature [4]. e influence of jet on landing aircraft is also analyzed in some literatures [5]. In 2006, Melber-Wilkending [6] established and verified the process chain based on the adaptive DLR TAU program, using CFD considering as example a Hangar and an AIRBUS A380 configuration, and gave the flow solver program for determining the jet wake of the rear engine. Slaboch in Volpe National Transportation Systems Center [7] presents an operational model for the prediction of jet blast, and the model was developed based upon three modules including a jet exhaust model, jet centerline decay model, and aircraft motion model. e final analysis was compared with data acquired during a jet blast study conducted by the Volpe Center in 1999. is analysis closely matched the data from the 1999 test. e analysis was then used to predict the jet blast evolution from aircraft that have been introduced since 1999, including the Boeing 777-300ER. Ishiko et al. [8] in order to examine the far-field velocity of jet blast by computational fluid dynamics (CFD) in this research, simulation using Reynolds-averaged Navier-Stokes (RANS) equation is carried out with very large computational domain. e velocity profiles obtained by numerical simulation agree well with those obtained by experiments. en, they performed the parametric study of wind direction. It is found that the wind direction angle that has the most effect on the deflection of jet blast is lower than ninety degrees. Supported by theoretical and wind tunnel modeling, Bennett et al. [9] have experimented with an array of aerodynamic baffles on the surface behind a set of turbofan engines of 124 kN thrust. Lidar and point sampler measurements show that, as long as the intervention takes place within the zone where the Coanda effect holds the jet to the surface (i.e., within about 70 m in this case), quite modest surface-mounted baffles can rapidly lift the jet away from the ground. is was of potential benefit in abating both surface concentrations and jet blast downstream. ere were also some modest acoustic benefits. e three-dimensional jet flow field of aircraft was simulated by Taguchi et al. [10]; they used a supersonic nozzle wall jet device, and the experimental results were compared with the calculation results of the SST turbulence model. e results show that the existing Reynolds stress database is of great significance to the establishment of the wall jet turbulence model. In recent decades, the RANS (Reynolds-averaged Navier-Stokes) method has been used to study jet flow fields in aviation. However, reliable numerical results have not been obtained [11]. Although the RANS method requires the minimal computational effort, the pulsating motion details are smoothed out by homogenizing the turbulent fluctuations [12]. erefore, it is impossible to accurately simulate the growth rate of the shear layer and turbulence details such as the inviscid velocity of the jet, which is not affected by the shear layer [13][14][15]. Scholars at home and abroad have used the LES (large eddy simulation) method to carry out numerical simulations on jet blast. e basic concept has been to directly and numerically simulate large eddies by using the spatial sieve filtration method, Fourier function, or Gaussian function to separate large and small eddies [16][17][18]. e subgrid stress model has been used to calculate small eddies [19]. In [20], the LES method was used to simulate the aerodynamic noise and coaxial twin jet flow noise before and after installing a zigzag nozzle, and the effect of the zigzag nozzle on the flow field structure and sound field was studied. In [21], free flow and jet flow numerical simulations were carried out with the LES method. e results showed that the location and shape of large turbulence structures were consistent with the experimental images. Although the LES method has achieved good results, in an actual numerical simulation process, even the LES method needs a considerable grid support to capture small eddies near the engine walls [22]. Moreover, when assessing the complex flow of engine jets, the near-wall mode of the LES method cannot accurately separate the high Reynolds number near-wall turbulence, so it can only deal with low Reynolds number turbulent flows [23,24].
At present, the DES (detached eddy simulation) method has been introduced to assist in the numerical simulation of jet engines. It is a numerical method used for the calculation of detached vortices [25,26]. e basic concept employs the RANS method to simulate small-scale turbulent fluctuations near the engine wall. In the area far away from the boundary layer, a Smagorinsky large eddy simulation is used to simulate the detached vortex to enable the subgrid Reynolds stress model [27]. is method has two advantages. First, it avoids the problem of a larger grid size in the conventional boundary layer method (LES). e method also ensures that the large-scale detached vortex energy can be accurately simulated in a range far away from the surface of the object. Liu et al. [28] used a mixed unstructured grid and an SST turbulence model to simulate a jet engine with the DES method and compared it with experimental results. e rationality of the method was proven. Dietiker and Hoffmann [29] used the DES method to study a three-dimensional unsteady jet and compared it with experimental data to obtain relatively good numerical results. Gong et al. [30] proposed an improved delay separation vortex simulation (IDDES) method based on the SST model for a high-precision simulation of the jet engine effect and conducted a numerical study of the dynamic jet effect through a RANS/ LES hybrid method. eir results showed that the velocity distribution in a jet blast can be predicted better [31,32].
In summary, DES offers great advantages in the numerical simulation of jet blast, but domestic scholars have seldom used this approach. At present, domestic and foreign scholars have performed more numerical simulations of near-field jet blasts [33][34][35][36][37]. However, for taxiing behind of the departing aircraft, more attention has been paid to the far-field flow of the jet [38][39][40]. e SA turbulence model, as a classic aviation field model, exhibits strong robustness and a rich experience value [41,42]. erefore, based on the SA turbulence model and the DES method, a DES-SA mixed numerical simulation method is built to simulate the far field of a jet blast. A nozzle model that does not consider internal engine flow is used. Two different jet states from a Boeing aircraft nozzle are calculated, and the calculated state, which is more consistent with the working conditions of the engine, is determined. On this basis, the influence distance of a typical jet blast is studied to provide the necessary theoretical and technical support for the implementation of a taxibehind mode. At the same time, it provides a reference for the study of engine jet by the DES numerical simulation method.

Methodology
N-S equations are the most complete governing equations describing fluid motion so far and can be written in the form of Cartesian tensor using summation convention. e continuity equation is e momentum equation is where u i is the Reynolds average velocity component omitting the average sign; ρ is the density; p is the pressure; u i ′ is the pulsating velocity; σ ij is the stress tensor component. Based on the SA turbulence model combining the DES method, the hybrid DES-SA numerical simulation method is used to simulate the far-field flow of a jet engine [43,44]. e integral method for the DES-SA approach is as follows: where v is the viscosity coefficient; F c,T is the convective flux term; F v,T is the viscous flux term; Q T is the source item which contains generation and destruction items. e mixed model adopts a mixed length scale l DES instead of the traditional SA turbulence model d to calculate the distance from the unit to the nearest wall; the following formula is adopted: where C DES is the adjustable coefficient, which is usually 0.65; Δ is the filter scale in the LES method. erefore, the DES-SA mixing method has d ≪ Δ(l DES � d) in the near-wall region. e traditional SA turbulence model is used for numerical simulation, which has d ≫ Δ (l DES � Δ) far away from the wall area. When there is a balance between the production term and the dissipation term, v ∝ SΔ 2 . At this point, the DES-SA mixing method is transformed into the LES method to simulate the jet flow.
At present, the main method for nozzle boundary condition construction depends on whether to consider the internal flow of the nozzle. For the case of internal nozzle flow, the boundary of the computational domain lies within the nozzle. e boundary conditions are usually set as the total pressure and total temperature inside the nozzle or the total pressure ratio of the internal combustion chamber (the combustion chamber) to the external atmosphere (P 0 /P) and total temperature ratio (T 0 /T) [45]. is method restricts the size and internal configuration of nozzle. It can fully consider the viscous effect of the inner wall in the engine nozzle [46]. e calculation accuracy is relatively high. However, considering that the nozzle is a highly proprietary product, the internal structure and size data are difficult to obtain. erefore, the internal flow of the nozzle is not considered in this study. We only require the Mach number, static pressure, and static temperature at the outlet of the nozzle and regard the nozzle outlet condition as the entry condition for the solution domain of the flow field.

Example Verification Analysis
Considering the complex working state of the engine, scholars at home and abroad typically compare the two states of cold and hot spray when calculating a jet engine field and analyze the similarities and differences between the two states of cold and hot spray. en, according to the actual situation, the conditions that are more suitable for the actual working conditions are determined for numerical simulation. In this study, the combined DES-SA method is used to study the two states of engine cold jetting and hot spraying. e setting of specific parameters is given in Table 1.
Taking a Boeing A320 aircraft (engine type is CFM56-5B) as an example, according to the actual engine size, the twin nozzle model in the calculation example is scaled down. e diameter of the CFM56-5B engine fan nozzle is 1.735 m; the specific structure is shown in Figures 2 and 3.
To investigate the ground effect, the calculation domain is chosen as follows: according to the assembly height of the A320 aircraft engine (the vertical height of the axis from the ground is approximately 1.68 m), the height distance from the ground is 1.7348 m and perpendicular to the direction of the incoming flow. e width of the flow field is 45.533 m, and the height is 24.5013 m along the streamline direction. e length of the flow field is 341.498 m. To obtain more accurate calculation results, the boundary conditions are set as follows: the ground is set as the boundary condition of the material surface, the outlet is set as the pressure outlet condition, and the three planes and the flow inlet surface parallel to the flow are set as the far-field pressure condition. e calculation domain size is shown in Figure 4. During mesh processing, the mesh at the nozzle outlet is encrypted to better simulate the velocity change at the nozzle outlet, as shown in Figures 5(a) and 5(b). During the volume Mathematical Problems in Engineering mesh generation, in order to take the ground effect into account, the mesh at the ground and the nozzle is encrypted, as shown in Figures 5(c) Table 2 e boundary conditions of the external flow field are as follows: static pressure P � 101325 Pa, static temperature T � 298 K, and working gas is the ideal gas. According to formula (5) and the total temperature ratio, the static temperature and static pressure at the outlet of the inner nozzle and outer nozzle can be determined. Figures 6 and 7 show the results of the numerical simulation of the nozzle axis velocity varied with the nozzle distance obtained from the numerical simulation. In the graph, we can see that the axial velocity of the nozzle decreases rapidly within the distance from the front 100 m; regardless of whether the nozzle is heated or not, the velocity slows down from 100 m, and the axis velocity at 300 m is still approximately 60 m/s. Compared with the incoming velocity (16.6 m/s), the speed is still greater. ere is a risk in crossing the runway at this distance. erefore, it can be concluded that the static temperature at the outlet of the nozzle has a little effect on the speed drop in the range from 100 m to 300 m downstream.   Figure 2: ree-dimensional structure of the nozzle (x, axial direction; y, radial direction; z, height direction). Figures 8 and 9 show the velocity clouds of the nozzle outlet under cold spray and hot spray conditions, respectively. Figure 8 shows that the velocity at the outlet of the nozzle is the greatest. As the distance increases, the velocity decreases gradually due to the dissipation of energy, and the incoming gas flow also creates a shearing action with the tail  Mathematical Problems in Engineering jet stream at high speed, resulting in an increase in the gas flow velocity near the tail jet stream. It can be seen in Figure 9 that although the Mach number at the outlet is less than the Mach number at the culvert, the speed at the outlet is faster than that at the culvert. e reason is that the total temperature at the outlet is higher and the static temperature is higher than the static temperature at the culvert, so the corresponding sound speed is also faster. Although the Mach number is relatively low, the absolute velocity of the calculated airflow is still faster. Figures 10 and 11 show the temperature cloud map at the outlet of the nozzle calculated under cold spray and hot spray conditions, respectively. In the figures, we can see that the influence range of the tail jet increases with increasing distance. e absolute value of the difference between the center and the ambient temperature decreases with increasing distance. However, the total temperature ratio is 1 under the cold spray condition, and the gas energy inside and outside the nozzle is the same. According to formula (5), when the total temperature is constant, the larger the Mach number is, the lower the static temperature is. erefore, the static temperature at the outlet of the nozzle is lower than that of the outside atmosphere. It is obvious that this example is different from an actual engine situation.

and 5(d). e specific number of grid nodes and cells is shown in
During the heating state, the static temperature of the outlet is higher than the ambient temperature, while the static temperature of the outlet is lower than the ambient temperature. is is due to the heating at the outlets and the higher total gas temperature at the outlets. At a certain Mach number, the static temperature at the outlet of the inner nozzle is far higher than that of the environment. However, the Mach number is larger than the external atmosphere, so the static temperature at the outlet is lower. It is worth noting that the static temperature at the center of the tail gas jet is higher than that of the external atmosphere compared with the cold spray state, which is also due to the higher static temperature of the gas in the cones. From the above analysis, the hot injection state is more consistent with the real working situation of the engine.

Numerical Simulation Analysis of Typical Jet
Engine Flow e influence distance of a departing aircraft's jet blast is very important for determining the safe clearance of the rear crossing mode. erefore, this section performs a numerical simulation analysis on the jet effect of a typical engine. According to CAAC data, as of February 2019, the proportion of Airbus and Boeing aircrafts in domestic airlines is 94.66%. Among them, the A320, B777, and B737-800 account for up to 78.18% of the total. e CRJ900, as a typical representative of the regional aircraft, is favored for its excellent flight performance and low fuel consumption. erefore, the above four models are selected and categorized according to their wake ratings: light-duty (CRJ900), medium-duty (A320 and B737-800), and heavy-duty (B777). e thermal jet method is used to analyze and calculate the influence distance of the jet blast.
(1) Determine the shrinkage of the calculation model When calculating the far-field tail jet flow due to the lack of actual size data, the model is scaled according to the actual engine's fan diameter (2) Calculate the true flow of internal and external channels e air flow in the ducts is calculated according to the bypass ratio and the total air flow rate. e formula is as follows: (3) Calculate the speed of internal and external channels For a turbofan engine, the ratio of internal and external ducts is 2 : 8. erefore, the velocity of the internal and external ducts can be calculated according to the momentum theorem under the   FΔt � _ mΔV.
(4) Determine the Mach numbers inside and outside the culvert To determine the speed and temperature inside and outside the culvert, the Mach number of the inner and outer ducts can be calculated according to the following formulas.
Ma � V a .
Taking A320 as an example, the real jet blast tail effect is calculated. e A320 mainly uses the CFM56-5B engine, and the relevant parameters are given in Table 3.
According to formulas (6)-(10), the boundary conditions at the nozzle outlet can be obtained, as given in Table 4. rough numerical simulations of the above cases, the jet velocity distribution curve and the velocity profile of the jet XZ section are obtained (Figures 12 and 13). According to the limitations in the Flight Crew Operation Manual (FCOM), this study mainly analyzes jet engines at speeds of 44 m/s, 22 m/s, and 16 m/s. Figure 13 shows that the influence distances of A320 jet blast at speeds of 44 m/s, 22 m/s, and 16 m/s are 90 m, 296 m, and 451 m, respectively.
Similarly, numerical simulations for the B777, B737-800, and CRJ900 are carried out to obtain the velocity distributions of their jet blasts, as shown in Figures 14-16.        In summary, the influence distances of the B777, A320, B737-800, and CRJ900 jet blast at speeds of 44 m/s, 22 m/s, and 16 m/s are given in Table 5.

Conclusion
Based on the safe operation of the taxi-behind mode, the influence distance of jet flow in aircraft engine under the taxi-behind mode is numerically simulated. Based on the SA turbulence model, the DES-SA hybrid method is constructed. Cold spray and hot spray conditions are calculated using a nozzle model without considering the internal flow of the engine, and the state of the engine's actual working condition is determined. According to the selection of four presently used typical aircraft models, the jet effect of the engine is numerically simulated, and the influence distance of the jet blast is determined.
(1) e numerical simulation results for two jet types under cold and hot spray conditions indicate the following: whether the coning channel is heated or not, the speed at the axis of the engine nozzle decreases with the increase of the nozzle distance, and the velocity decreases rapidly within 100 m of the engine nozzle and decreases slowly beyond 100 m. Compared with the unheated condition, the inner channel heating condition is more consistent with the actual working state of the engine. (2) e numerical simulation results for a typical jet engine effect show the following: medium-duty and heavy-duty aircrafts typically use a more powerful engine with more horsepower than a light-duty aircraft. When the jet speed is 16 m/s, the influence distance is far greater than 300 m. When the jet velocity speed is 16 m/s, the impact distance of the light-duty aircraft is much less than 300 m. In the follow-up work of this study, a typical aircraft type will be selected to carry out the real engine jet effect experiment at the airport, and the corresponding parameters of the jet blast will be collected. e experimental data obtained will further verify the numerical simulation results in this study.
Data Availability e data on engine parameters of typical aircrafts are derived from https://www.prattwhitney.com ∼∼∼∼∼∼∼∼ ∼^∼^∼^∼^∼∼∼∼∼∼∼∼∼∼∼amp and https://http://www. cfmaeroengines.com. Disclosure e funders had no role in the design of the study; in the collection, analyzes, or interpretation of data; in the writing of the manuscript; or in the decision to publish the results.

Conflicts of Interest
e authors declare that they have no conflicts of interest.