Numerical-Study of Large-Liquid Rocket Plume-Flow-Field

Aiming at the complexity of plume field structure caused by plume collision in the rising section of multi-nozzle parallel rocket, this paper establishes an analytical model of the rising section of a nine-nozzle configuration rocket. The plume field phenomenon is studied at different heights through numerical simulation. The reliability of the numerical method is verified based on the comparison of simulation and wind tunnel test data. The analytical results. Show that violent collision occurs between the jets in the ascent section of the multi-nozzles rocket, and many phenomena such as circulating vortex, gas reflux, reflux back splash and so on occur at different altitudes. When the altitude is less than 25km, gas reflux and circulation vortex appear in the rocket base. With the increasing of altitude, the jet collision impacts the base. After the altitude reaches 45km, back splash appears in some areas of the rocket base. There is an obvious flow diversion phenomenon on the side wall surface. The higher the altitude, the greater the expansion angle of the jet after the gas exits the nozzle.


Introduction
To enhance the capacity of large rockets, the United States, Russia, the European Union, and Japan have used the power scheme of multiple nozzles in parallel, such as the Saturn-IV of the United States, IV rocket [1], Russia's Proton-M rocket, the EU's Ariane-5-series of rockets [2], and Japan's H-II II A, et al.In the ascent process of multi nozzles parallel rockets, the complex interaction between the high speed, high temperature and high pressure jets at the exit of the engine and between the jets and the incoming streams leads to an extremely harsh thermal environment at the bottom of the rocket body, so the prediction of the thermal environment at the bottom of the multi nozzles parallel large rockets has a direct impact on the direction and validity of the rocket thermal protection program.However, due to the complexity of the flow field environment at the bottom of multi-nozzles rockets, there is a large gap between theoretical analysis and wind tunnel test and telemetry data, which makes it difficult to be used to predict the flow scenario at the bottom of large rockets directly [3].Therefore, it is necessary to design and establish a numerical analysis model for large rockets to predict the plume flow field and the bottom flow field environment during the launching process to provide a reference for the thermal protection program of multi nozzles large rockets.
At present, many foreign scholars have conducted relevant studies on the plume and bottom flow field of a large multi nozzles rocket launching process.Zhou Z T [4] simulated the reactive and non-reactive flow of three nozzles configurations, when the flight.altitude increases, the temperature of the rocket rises accordingly, and the bottom heat flux.shows a trend of increasing and then decreasing Whitmore S [5] analyzed the effect of radiative heating on the oxidizer to fuel ratio of additively manufactured hybrid rocket fuel and concluded that the emerging thermoplastic material combustion anomaly is due to radiative heat transfer.Cross P [6] investigated the effects of complex refractive index, particle size distribution, and exit plane radiation boundary conditions on radiative heat transfer within solid propellant rocket motors, improving the accuracy of radiative heat flux predictions for rocket nozzles.Maxim [7] analyzed the radiative heat transfer analysis for the Mars atmosphere containing carbon dioxide and nitrogen using DO radiation(Discrete ordinates, DO)) and for different spatial discretization angles.George F [8] analyzed measured data from a Delta rocket strapped with six solid boosters and concluded that solid propellant-booster exhaust plume radiation and turbine exhaust backflow and reignition are the main factors affecting the heating rate of the rocket thrust structure.
In recent years, many scholars in China have carried out a series of studies on rocket plume and bottom thermal environment problems through numerical analysis.Yang Y [9] carried out numerical simulation on the plume and thermal environment of a multi-engine parallel rocket, and analyzed the influence of the engine plume and the heat flow distribution of the rocket body at different heights.The influence of external flow field on the bottom thermal environment was analyzed by Yan Z J [10] with modeling the core stage with four boosters.Zhou.Z T [11] studied the thermal environment at the bottom of the liquid rocket, and found that the heat distribution at the bottom of the rocket shows the trend that the radiant heat decreases with the rise of the altitude, and the convective heat at the bottom of the rocket increases first and then decreases.Yang X J [12] combined theoretical and numerical analysis methods to analyze the thermal environment of solid rocket aft section, and found that there is a difference between heaven and earth, and the convective heat and radiant heat calculations under the flight environment should be fully considered.
Up to now, scholars have analyzed the plume and its thermal environment of large rockets mainly by means of numerical simulation in the domestic and abroad, and the research object mainly focuses on the heat flow distribution of single/double nozzles.However, large rockets often use the power scheme of multiple nozzles in parallel, and their bottom flow field characteristics are significantly different, and the thermal environment laws are also different.At the same time, large multi nozzle rockets need to across different altitudes in the ascent process, and their environmental conditions vary greatly.Multi stage parallel rocket plume flow field and body heat flow by the environment is seriously affected, and the bottom of the rocket flow state and the role of the mechanism is still unclear.The development of the law and the influence of the factors is still blurring, which is an urgent need to carry out research related to the configuration of the multi-nozzles for a new generation large rockets rocket body and the bottom of the anti-heat.The research on multi nozzles configuration is urgently needed to provide a reference for new generation of large rockets and bottom heat protection.
This paper takes nine-nozzle configuration liquid oxygen kerosene liquid rocket as the research object, and mainly studies the plume flow field structural characteristics at the rocket body at different heights and its influencing factors.Base on the results, the program reference is provided for the layout of the nozzle at the bottom of the multi-nozzle liquid rocket.

2.1.Physical Model
The geometrical model of a nine-nozzle liquid oxygen rocket is shown in Figure 1.The length of the core stage rocket is L and the diameter of the bottom is D. The layout of the nozzle at the bottom of the rocket is shown in Figure 2, with no deflection in the center nozzle.The outlet distance from the bottom of the rocket is 1 L , and the angle of deflection of the axial nozzle of the engine outward is γ .During the ascent of a liquid rocket, the bottom flow region is mainly affected by the engine jet and the high speed incoming flow, which is a typical compressible flow [13], which is typical compressible flow.Based on the Navier-Stokes equations, the control equations based on energy, momentum and continuity equations can be expressed as follows: Where ρ is the density, U is the velocity vector, and E is the total energy, including kinetic energy, internal energy i and potential energy P , as in Eq.( 4).The p is the pressure, j j h J is the energy dissipation due to diffusion of components, r S is the radiative energy source term, and T is the viscous stress tensor.
The liquid rocket fuel and oxidizer is liquid oxygen kerosene type in this paper.The combustion products contain water vapor, carbon dioxide, carbon monoxide and other gas components, the composition of the mixture of gas.The constant specific heat of the gas is determined by the mass fraction percentage of the mixture of gases.According to the literature [14], the finite chemical reaction model can be replaced by the air-gas component mixing equivalent for the calculation of heat flow distribution of liquid fuel rocket.The calculation results of the air-gas are not much different.At the same time, the combustion process of liquid oxygen kerosene rocket motor is more complete, and the percentage of re-flammable gases in the products is very low.The effect of re flammability on the wall surface of the rocket is relatively small, especially in the conditions of thin oxygen at high altitude, and the re-flammability effect is very small.Therefore, the air-gas component mixing equivalent finite chemical reaction model can be used for engineering calculations.
The i is the gas component in the flow, the transport equation corresponding to its mass fraction Where, i R is the chemical reaction rate of the gas i , i K is the component diffusion.Meanwhile, for turbulent flow, the component diffusion can be expressed as: , , is the thermal diffusion coefficient, and 2.2.2.Spatial discrete format.In this paper, the finite volume method is used to discretize the control equations for the strong disturbances around the nozzle and the arrow in flow field.The second order windward format has faster convergence and high numerical stability, so it is used with the second order TVD format.The diffusive term is in the central difference format, and the gradient is solved based on the least squares method, and the unit surface flux discretization is in the Roe FDS format [15].The Gauss Seidel iterative method is used [16].

Turbulence model.
The SST k-w turbulence model is adopted, which is more realistic for the collision of multiple gas jets at the bottom of the rocket as well as the high Reynolds number turbulent flow simulation between the jets and the air.The density distribution of the heat fluxes obtained is in better agreement with the experimental results [17][18][19].SST(Shear Stress Transport, SST) k-w, first proposed by Menter [20], is a turbulence model for solving shear flow problems containing wall function constraints.The transport equation of the SST k w model is: Where, k is the turbulent kinetic energy, ω is the turbulent dissipation rate, Γ ω and Γ k are the equivalent diffusivities, k G and w G are the generalized generation source terms, k Y and w Y are the dissipation source terms, w D is the cross diffusion source term.

Radiation model.
The products of mixed combustion include CO2 and strong radiative gases such as water vapor in the engine combustion chamber during the flight of a liquid rocket [21].Meanwhile, solid particles results from the rapid cooling of the under combusted portion of the fuel.Under the high temperature environment, the strong radiative gases and solid particles work together to transfer part of the radiative energy to the solid bottom of the rocket and be absorbed, heating the bottom wall.DO(Discrete Ordinates, DO) [7,22,23], discretizing the space into a finite number of three dimensional angles to calculate the radiation problem, can generally be improved by denser discretization with the high calculation accuracy.DO radiation model can calculate the radiation problem in all optical depth intervals, especially the radiation heat transfer problem with medium, and the calculation theory is mature, the numerical results are stable.DO can be used to solve the bottom of the large scale liquid rockets radiant heat problem.The space transport radiation of DO model is as follows transfer equation is: Where, λ is the wave length, λ a is the spectral absorption coefficient, λ I is the spectral radiant intensity, bλ I is the black body intensity given by Planck's equation, s r is the path length, r r and s  r are the positional coordinates and scattering vectors respectively, s σ is the scattering coefficient, Ω is the steric angle.
When the liquid rocket rises to a high altitude, the water vapor and carbon dioxide content in the space is high.The Planck average absorption coefficient is used to fit the absorption coefficient of the medium, which can more efficiently and accurately simulate the condition of weakening of the radiation intensity caused by the absorption of the radiant energy in the transmission process.Grey body model [24], the absorption coefficient is calculated by using the Planck average absorption coefficient [13,25], which is expressed as Eq (10).The absorption coefficient is expressed as: Where, η κ is the absorption coefficient of absorption corresponding to the wave number η , ηb I is the black body intensity corresponding to the wave number η .Table 1 gives the molar percentage distribution of different gas components in the environment.

Grid division and boundary conditions
The geometric model is symmetric, so one-half model is used for calculation in this paper.During high altitude flight, the flow at the bottom of the rocket is the most intense and complex.Thus, the mesh is encrypted in the region of the bottom plate of the arrow body to ensure the accuracy of numerical calculations.The whole fluid domain is a cylinder with a radius of d and a length of e L .Meanwhile, to capture the flow condition near the wall more accurately, the boundary layer theory is used to analyse the flow separation at the wall, with a total of 18 boundary layers and an initial thickness of in h .The incoming flow direction is the pressure far field boundary condition, and the back end is the pressure outlet boundary condition.The rocket wall is the constant temperature wall, and the nozzle interior is the adiabatic wall.The engine inlet temperature in T is 3539.6K,and the pressure in P is 17.2MPa.The grid division and boundary conditions are shown in Figure 3.

Model validation
To verify the accuracy and validity of the numerical methods, the four nozzle rocket [14] and L [26], with downsizing test condition [27], numerical simulation is carried out.The four-nozzle downsizing model is used to simulate the effect of gas jet on the heat shield at the bottom of the rocket under the real incoming flow conditions in the wind tunnel.The distribution of the heat flow density at the bottom is measured by the sensors pre-set in the radial fixed position at the bottom of the rocket.In the wind tunnel test, the Mach number of the incoming stream at infinity M  is 2, and the nozzle expansion ratio is 6.9, and the expansion angle is 17.5°, and the throat diameter is 0.021m.In the numerical validation, the pressure ratio of the nozzle / c p p  is 1190.the nozzle arrangement of the simulation model is as follows Figure 4, with 4 nozzles in total.The sampling line is the intersection line between the symmetry plane of the nozzle and the bottom plate.The comparison between the ICMSOA-2023 Journal of Physics: Conference Series 2755 (2024) 012038 IOP Publishing doi:10.1088/1742-6596/2755/1/0120386 measured values of the sensor under wind tunnel test conditions and the numerical calculations in this paper after smoothing and dimensionless processing, the dimensionless processing method is shown in Eq (12).The dimensionless results shows that the temperature distribution on the wall surface of the four nozzle rocket in the numerical simulation agrees well with that measured in the wind tunnel test, which indicates that the numerical calculation method of this paper has good accuracy in calculating the distribution law of the plume field of the multiple nozzle plume.

Analysis and discussion
During the ascent phase of a large multi nozzle rocket, there will be a large altitude span, during which the external incoming flow environment will change significantly, and the main parameters include the ambient pressure, temperature, and the incoming flow Mach number.the incoming flow Mach number and environmental conditions at different altitudes are listed in Table 2.According to the nine working conditions corresponding to different altitudes in Table 2, the development of the external plume of the liquid rocket and the distribution of the heat flow in the heat shield at the bottom of the rocket at different altitudes are mainly analyzed.In the radial distribution plots, the larger / b r r is, the closer to the edge of the bottom plate.Due to the large changes in environmental parameters, the development of the multi nozzle plume is affected by the external pressure and the Mach number of the incoming flow.The plume expansion and collision between the plumes will produce differences in the liquid rocket ascent phase.Two different cuts of A/B in the flow field, the grey line is the base plate of the rocket, the outer orange indicates the side wall of the rocket are shown in Figure 5, and the green circle indicates the nozzle, and the sampling lines of the base plate in the following text are the intersection lines of the B cut and the base plate.

Mach number distribution of the plume field
Figure 6 shows the distribution of the plume of the multi nozzle rocket at different altitudes, with the cut surface is A. As the flight altitude rising, the expansion angle of the gas jet increases, and the collision between the jets forms a collision zone.The upper boundary of the collision zone is constantly close to the base plate of the rocket, and the jet collision gradually forms the gas flow to the base plate, the gas reflux.With the height increasing, the incoming pressure decreases sharply, the degree of compression of the jet is weakened, and the degree of expansion of the jet is further aggravated.bottom of the arrow is lower, the air supply flow is closer to the bottom of the arrow, as shown in Figure 7(d～e).As the height increasing further, the pressure gradient from the collision zone of the jet to the bottom plate increases, resulting in part of the jet in the collision zone impacting the bottom plate in the reverse direction, as shown in Fig. 7(d to e) shows.The ambient pressure is reduced, the effect of gas reflux is strengthened, resulting in the pressure between the bottom plate is greater than the ambient pressure, the circulating vortex near the bottom plate disappears, and the collision zone away from the bottom plate is formed by the sidewall incoming and outgoing jets as shown in Fig. 7(d to e). Figure •7(f i).Meanwhile, at high altitude(H>35 km), obvious flow separation phenomenon can be observed in the sidewall and part of the reflux splash zone in the bottom plate.

Dynamic pressure distribution at the base of the rocket
Figure 7 shows the dynamic pressure distribution at the bottom of the rocket with the flight altitude, where different colors represent different magnitudes of the dynamic pressure, and the section mode is B. At low altitude, due to the gas jet ejection effect [28], the surrounding air flows into the bottom region of the rocket, forming a gas feed flow.As the altitude increasing, the velocity of the incoming flow increases, and the pressure at the bottom of the arrow is lower, the air supply flow is closer to the bottom of the arrow, as shown in Figure 7(a ～ c).As the height increasing further, the pressure gradient from the collision zone of the jet to the bottom plate increases, resulting in part of the jet in the collision zone impacting the bottom plate in the reverse direction, as shown in Figure 7 (d～e).with the ambient pressure is reducing, the effect of gas reflux is strengthened, resulting in the pressure between the bottom plate is greater than the ambient pressure, the circulating vortex near the bottom plate disappears, and the collision zone away from the bottom plate is formed by the sidewall incoming and outgoing jets as shown in Figure 7(f ～ i).Meanwhile, at high altitude(H>35 km), obvious flow separation phenomenon can be observed in the sidewall and part of the reflux splash zone in the bottom plate.

Conclusion
This paper establishes an analytical model of nine-nozzle rocket for the plume flow field and thermal environment at the bottom of the ascent section of multi nozzle rocket.The plume flow field and thermal environment is discussed at the bottom of the plume under a total of nine altitudes.After discussing, the following conclusions: The collision between different jets occurs in the flow field of the nine-nozzle rocket, and the flow structure of the bottom plate differs greatly.When the altitude is less than 25km, jet reflux and circulating vortex appear in the bottom area of the rocket.With the increase of altitude, the jet collision impacts on the bottom plate.After the altitude reaches 45km, part of the back splash occurs in the bottom area of the rocket.There is an obvious flow diversion phenomenon in the side wall.The higher the altitude is, the larger the jet expansion angle is.
The results of this paper can provide a certain reference for the thermal protection of new generation of large multi nozzle liquid rockets.

Figure 1 .
Figure 1.Geometric model of the launch rocket.Figure 2. Disposition of nozzle installation.
(a) Symmetric mesh (b) Refinement of local mesh

Figure 4 .
Figure 4.The Nozzle layout at the bottom of rocket.

Figure 7
shows the dynamic pressure distribution at the bottom of the rocket with the flight altitude, where different colors represent different magnitudes of the dynamic pressure, and the section mode is B. At low altitude, the surrounding air flows into the bottom region of the rocket, forming a gas feed flow.As the altitude increasing, the velocity of the incoming flow increases, and the pressure at the (

Figure 7 .
Figure 7. Contours of dynamic pressure distribution in the bottom of rocket.

Table 1 .
Molar percentage of gases.