Numerical Investigations and Optimized Design of the Active Cooling Performance with Phase Change for Aircraft Rudder Shaft

Abstract

During hypersonic flight, the air rudder shaft can undergo huge aerodynamic heating load, where it is necessary to design the thermal protection system of the air rudder shaft. Aiming to prevent the rudder shaft from thermal failure due to the heat endurance limit of materials, numerical investigations are conducted systemically to predict the active cooling performance of the rudder shaft with liquid water considering phase change. The validation of the numerical simulation method considering phase-change heat transfer is further investigated by experiments. The effect of coolant injection flow velocity on the active cooling performance is further analyzed for both the steady state and transient state. Finally, to achieve better cooling performance, an optimized design of the cooling channels is performed in this work. The results of the transient numerical simulation show that, employing the initial cooling structures, it may undergo the heat transfer deterioration phenomenon under the coolant injection velocity below 0.2 m/s. For the rudder shaft with an optimized structure, the heat transfer deterioration can be significantly reduced, which significantly reduces the risk of thermal failure. Moreover, the total pressure drop of the optimized rudder shaft under the same coolant injection condition can be reduced by about 19% compared with the initial structure. This study provides a valuable contribution to the thermal protection performance for the rudder shaft, as a key component of aircraft under the aero heating process.

1. Introduction

The air rudder can provide the control torque and lift required for a high maneuverability flight for hypersonic aircraft operating at high Mach numbers, and is one of the important actuators for achieving flight attitude and trajectory control [1,2,3]. The air rudder is usually connected to the hypersonic aircraft through a rudder shaft and a certain gap is reserved to ensure the free rotation of the rudder surface [4,5]. However, high-temperature airflow can inevitably flow into the gap, which makes the air rudder flow field complicated due to shock wave/shock wave interference and shock wave/boundary layer interaction, resulting in severe local aerodynamic heating [6,7,8]. Due to extremely high aerodynamic heating, the surface of the air rudder shaft can be severely ablated, causing irreversible damage to the aerodynamic layout of the air rudder and threatening flight safety [9]. Therefore, the effective thermal protection system is crucial for the rudder shaft component of aircraft.

For the typical thermal protection system of high-temperature components for aircraft, the active thermal protection technology has attracted the widespread attention of researchers [10,11,12,13]. This can be attributed to the fact that active thermal protection can utilize the convective heat exchange and even the latent heat during the external liquid coolant injection. It becomes a reusable and promising method without consuming thermal protection materials compared with the traditional passive thermal protection technology [14,15]. Numerous wind tunnel experiments and numerical simulation research have been conducted to develop the active thermal protection technology, which mainly includes film cooling [16], regenerative cooling [17,18], and transpiration cooling [19,20], respectively. However, the experimental and numerical studies of active cooling investigations for the thermal protection system design of the air rudder shaft are still very limited in previous research.

To address this challenge, the fluid/solid coupling calculation of the air rudder shaft considering phase change under high heat flux conditions is carried out in this research. Numerical investigations are conducted systemically to predict the active cooling performance of the rudder shaft with liquid water considering phase change. The validation of the numerical simulation method considering phase-change heat transfer is further investigated by experiments. The effect of coolant injection flow velocity on the active cooling performance is further analyzed for both the steady state and transient state. Finally, to achieve better cooling performance, an optimized design of the cooling channels is performed in this work.

2. Methodology

In this section, the physical models of the original air rudder shaft and its initial coolant channel have been illustrated first. Secondly, the governing equations for the two-phase boiling simulation have been introduced.

2.1. Physical Model

As shown in Figure 1, the total length of the air rudder shaft is about 315 mm, the maximum diameter is 44.1 mm, the minimum diameter is 21 mm, and the diameter of the cooling water channel is 2 mm. The microchannel on the upper part of the rudder shaft is formed by rotational cutting, with the center of the circle on the center line of the rudder shaft, the rotation angle is 5°, and the microchannel depth is 0.5 mm, as shown in Figure 1a. The cooling water flows into the collection device at the bottom of the rudder shaft, and is transported upward along the axis from the bottom of the rudder shaft through 4 holes, collected in the liquid collecting tank on the upper part of the rudder shaft, and transported upward along the 20 axially evenly distributed microgrooves on the surface of the rudder shaft (see the red dotted area in Figure 1b), and the high-temperature area of the rudder shaft is actively cooled by convection along the way.

2.2. Governing Equations

The volume of fluid (VOF) method is employed in this work, which has been proven to be suitable for simulating the local thermodynamic and fluid dynamic characteristics of boiling flows [21,22,23]. The phase fraction, $\alpha$, of the liquid phase is tracked in the computational domain to determine the position of the phase interface to capture the motion of the two phases. This study uses the VOF model for numerical calculations, aiming to track the $\alpha$ of the liquid phase in the computational domain to determine the position of the phase interface to capture the motion of the two phases. In the VOF model, the sum of the $\alpha$ of the two phases in any control unit is 1. The physical properties of the mixed phase are calculated by weighing the physical properties of the two phases as follows:

$$y={\alpha }_l{y}_l+(1-{\alpha }_l)y_v\hspace{1em}y\in \left[\rho ,\mu ,K,C_p\right]$$

(1)

where $\alpha$ represents the phase fraction. $\rho , \mu , K, \mathrm{and} C_p$ represent density (kg/m³), viscosity (kg/(m·s)), thermal conductivity (W/(m·K)), and specific heat capacity (J/(kg·K)), respectively.

The momentum equation and energy equation are as follows:

$${\displaystyle \frac{\partial }{\partial \mathit{t}}}\left(\mathit{\rho }\mathbf{U}\right)+\nabla ·(\mathit{\rho }\mathbf{U}\mathbf{U})=-\nabla \mathit{P}+\nabla ·\left[{\mathit{\mu }}_{\mathit{e}\mathit{f}\mathit{f}}(\nabla \mathbf{U}+\nabla {\mathbf{U}}^{\mathit{T}})\right]+\mathit{\rho }\mathit{g}+{\mathit{F}}_{\mathit{v}\mathit{o}\mathit{l}}$$

(2)

where $U$ and $g$ are velocity (m/s) and gravitational acceleration (m/s²), respectively; $P$, $F_{vol}$, and ${\mu }_{eff}$ are pressure (Pa), surface tension per unit volume (N/m³), and effective viscosity (kg/(m·s)), respectively.

$${\displaystyle \frac{\partial }{\partial t}}\left(\rho E\right)+\nabla ·\left[U\left(\rho E+P\right)\right]=\nabla ·\left(K_{eff}\nabla T\right)+S_E$$

(3)

where $E$, $S_E$, and $K_{eff}$ are the energy density, the energy transfer rate per unit volume between the two phases, and the effective thermal conductivity, respectively.

Since evaporation and condensation cause the conversion between the gas phase and the liquid phase, considering the continuity equation of each phase, the phase fraction equations of the liquid phase and the gas phase are expressed as follows:

$${\displaystyle \frac{\partial }{\partial t}}\left({\rho }_l{\alpha }_l\right)+\nabla ·\left({\rho }_l{\alpha }_l{U}_l\right)=S$$

(4)

$${\displaystyle \frac{\partial }{\partial t}}\left({\rho }_v{\alpha }_v\right)+\nabla ·\left({\rho }_v{\alpha }_v{U}_v\right)=S$$

(5)

where $S$ represents the mass transfer source term (kg/(m³·s)) due to phase change. The above two-phase equations can be further simplified into one equation as follows:

$${\displaystyle \frac{\partial }{\partial t}}\left({\rho }_i{\alpha }_i\right)+\nabla ·\left({\rho }_i{\alpha }_i{U}_i\right)=\pm S$$

(6)

Furthermore, the continuity equation can be obtained as presented below:

$$\nabla U=S\left(1/p_l-1/p_v\right)$$

(7)

The interphase mass transfer model is the key to accurately predicting mass transfer and heat transfer in boiling heat transfer. The mass transfer model proposed by Lee assumes that both the saturated phase and the phase interface are kept at a saturated temperature, which can simulate the heat and mass transfer process between the two phases well. This study uses the Lee model [24] for simulation. It is worth noting that in the Lee model, the evaporation condensation coefficient (coeff) needs to be determined in combination with experimental results to better conform to the actual situation. The coeff can be obtained as follows:

$$coeff={\displaystyle \frac{6}{d_b}}\beta \sqrt{{\displaystyle \frac{M}{2\pi R{T}_{sat}}}}L\left({\displaystyle \frac{{\alpha }_v{\rho }_v}{{\rho }_l-{\rho }_v}}\right)$$

(8)

This work uses the finite volume method (FVM) in commercial software ANSYS Fluent 2021R1 to conduct the simulation. The meshes used are finite volume meshes, and they are unstructured tetra meshes generated by commercial software ICEM CFD 2021R1.

3. Model Validation and Simulation Details

3.1. Validation of the Numerical Simulation Method with Experimental Results

3.1.1. Experimental Setup

The test article is an actively cooled thermal protection rudder surface model. Quartz lamps manufactured by China Guangzhou Langpu Optoelectronic Technology company (Guangzhou, China) are used to heat the metal skin on the surface, while internal cooling channels provide convective active thermal protection for the rudder shaft. The test article is entirely made of 304 stainless steel components and consists of the skin, structural frame, rudder shaft, and other components. During the test, the specimen is mounted vertically on a support frame and thermally insulated from the frame using thermal insulation tiles. Quartz lamp arrays are installed parallel to both sides of the specimen to provide overall heating of the rudder surface. The distance between the quartz lamp arrays and the rudder surface is 70 mm, with a heat flux loading of 80 kW/m². The heat flux is measured at the symmetrical central area of the quartz lamp arrays on both sides. Prior to computation, the model is simplified based on the provided data. This simplification includes reducing the complexity of the bolts and some structural components, as well as performing smoothing treatment, as shown in Figure 2a. The model is discretized, and the total number of cells is about 2.7 million, as shown in Figure 2b.

The temperature of the rudder shaft under the condition of 80 kW/m² heating and waterless working conditions was calculated. Further, the fluid–solid coupled heat transfer steady-state calculation was carried out under the condition of 80 kW/m² heating and water supply at inlet flow rates of 1 and 0.2 m/s, and the results were compared and analyzed with the experimental results. Based on the existing test data and model settlement results, the evaluation of the cooling efficiency of the rudder shaft under small flow conditions was obtained.

However, due to the complexity and high computational cost of creating a comprehensive numerical model that includes the quartz lamp arrays, the surrounding flow field, and the rudder shaft itself, directly applying this heat flux condition in simulation is relatively difficult. Therefore, in this work, under no cooling water conditions, different equivalent heat fluxes (60,000, 50,000, and 45,000 W/m²) are applied to the surface of the test article in the simulation to obtain transient temperatures, which are then compared with the experimental data. As shown in Figure 3, the result with a heat flux of 45,000 W/m² aligns with the experimental data. It is worth noting that under a heat flux density of 45,000 W/m², the temperature at intermediate times is slightly higher than the experimental results but gradually converges with the experimental results after 1600s, which is favorable for subsequent steady-state simulations for cases with inlet cooling water velocities of 0.2 m/s and 1 m/s.

3.1.2. Comparison of Experimental Measurements with CFD Simulations

Cooling conditions for the rudder shaft are calculated for water flow rates of 1 and 0.2 m/s, with results presented in Figure 4 and

Table 1. Comparison of experimental values and simulation calculation results at different temperature measurement points.

	Upper Flange Measurement Point 1	Lower Flange Measurement Point 9	Measurement Point 12 at the Lower Part of the Rudder Shaft
Experimental result	566.4 °C	256.9 °C	47.4 °C
Simulation calculation results at 1.0 m/s	568.8 °C	253.2 °C	46.1 °C
Simulation calculation results at 0.2 m/s	573.8 °C	273.6 °C	49.2 °C

. The temperatures measured at the final test moment are compared with simulation results for both inlet and outlet velocities. It is observed that the 1 m/s inlet velocity condition better matches the experimental results. The temperature at the upper flange (top of the rudder shaft) does not exceed 570 °C, with simulation results slightly higher than the experimental data, showing an error of no more than 3 °C. At the lower flange measurement point, the simulation result is slightly lower than the experimental data, with a difference of about 2 °C. The temperature difference at the bottom of the rudder shaft is even smaller, approximately 1 °C. In comparison, the 0.2 m/s inlet flow rate also provides cooling but results in overall temperatures higher than both the experimental data and the 1 m/s flow condition. Specifically, the temperature at the lower flange is approximately 17 °C higher, which aligns with theoretical expectations.

Although the 0.2 m/s inlet condition meets the temperature requirements, the boiling mode also warrants examination. Figure 5 shows that under the 1 m/s conditions, the flow field exhibits mild behavior, with nucleate boiling occurring only in key areas, suggesting good safety but some inefficiency. Under the 0.2 m/s inlet flow rate, intense boiling occurs within the pipe, with some regions approaching film boiling, especially in the water supply pipe corresponding to the lower flange. This intense boiling poses significant risks. Based on the first round of results, it is recommended to slightly increase the flow rate above 0.2 m/s, ensuring that the supply flow rate remains above 0.5 m/s between 500 and 1500 s for safety, with a reduction to around 0.3 m/s in the initial and final 500 s.

3.2. Physical Properties

In this study, the coolant in the air rudder shaft is water, and the physical parameters of the liquid and vapor phases are shown in

Table 2. Physical property parameters of coolant.

Materials	Density (kg/m3)	Specific Heat Capacity (J/(kg·K))	Thermal Conductivity (W/(m·K))
Water	998.2	4182	0.6
Water vapor	0.5542	2014	0.0261

as follows:

The material of the rudder shaft is considered as GH4099 steel, for which thermophysical property variations with temperature are shown in

Table 3. Physical property parameters of GH4099 steel.

Material	Density (kg/m3)	Specific Heat Capacity (J/(kg·K))		Thermal Conductivity (W/(m·K))
		Temperature (°C)	Value	Temperature (°C)	Value
GH4099	8470	20	543	100	10.47
		100	552	200	12.56
		200	562	300	14.24
		300	572	400	15.91
		400	582	500	18
		500	595	600	19.68
		600	612	700	21.77
		700	638	800	23.45
		800	674	900	25.54
		900	726	1000	27.21
		1000	812

.

3.3. Boundary Conditions

Boundary conditions are necessary for solving the control equation. The boundary conditions for the steady-state simulations are provided in

Table 4. Boundary Conditions of the numerical model.

Boundary Name	Boundary Conditions
inlet	Speed entry 0.1 m/s, 300 K
outlet	Pressure outlet, 1 bar
Heat top	Heat flux density, 4 × 104 W/m2·K
Heat middle 1	Heat flux density, 1 × 104 W/m2·K
Heat middle 2	Heat flux density, 4 × 104 W/m2·K
Heat middle 3	Heat flux density, 1 × 104 W/m2·K
Heat middle 4	Heat flux density, 0 W/m2·K
Heat middle 5	Heat flux density, 0 W/m2·K

.

Aiming to conduct the transient phase-change cooling performance during the coolant injection, the transient boundary conditions for heat flux are also provided as shown in Figure 6.

To set appropriate thermal boundary conditions, preliminary calculations and fitting were performed on the original data. Different heat flux density boundary conditions were applied to the top and body of the rudder shaft, with monitoring points set at the top of the rudder shaft, the upper through-hole, and the lower through-hole. The heat boundary conditions that most closely matched the original data were fitted. The fitting results are shown in the figure below, in Figure 6b. The highest temperature at the top of the rudder shaft is slightly higher than the initial condition, with a maximum error of 4.9%.

3.4. Grid Independence Test

In this study, computational grids with sizes of 2.33 million, 3.59 million, 5.47 million, 11.88 million, and 17.94 million cells were generated. Steady-state simulations were performed under identical operating conditions to assess the variation rates of the relevant physical parameters, such as the rudder shaft surface temperature, the gas fraction within the water supply pipes, and the temperature within the water supply pipes. The solid material used in the calculations was GH4099 steel, and the fluid materials were liquid water and water vapor. The calculations employed a pressure-based solver with the SST k-omega turbulence model [25,26]. The phase change model used was the VOF model, and interphase mass transfer was modeled using the Lee model [24], with an initial mass transfer coefficient tentatively set to 100 and 0.1. The initial conditions were derived from the temperature distribution obtained through thermal boundary fitting at time 0 s.

Figure 7a shows the phase fraction distribution of the fluid part for five different mesh sets. The results for the 5.47 million and 11.88 million mesh grids are similar, and distinct bubbles can be observed. The axial variation in the gas phase volume fraction was examined, and Figure 7c demonstrates that, under different mesh scales, there are clear gas–liquid interfaces, which approximately appear at the same axial position. Figure 7b,d,f present the computed axial temperature distributions for both the fluid and solid parts under different mesh scales. It can be observed that the axial temperature distribution patterns are consistent, indicating that the temperature calculation results are relatively insensitive to the mesh scale. Figure 7e compares the axial pressure variations in the fluid part for five different mesh sets. There are discrepancies between the results of the two smaller mesh sets and the three larger mesh sets, while the pressure results for the 5.47 million, 11.88 million, and 17.94 million mesh grids are similar.

The comparison results of gas fraction and temperature at different monitoring points were presented in

Table 5. Comparison of temperature and gas volume fraction at monitoring points.

Mesh Number (Million)	233	359	547	1188
Maximum Axial Temperature (°C)	479.846	479.281	479.146	478.584
Gas Volume Fraction (Top)	0.0659	0.0687	0.0892	0.0774
Gas Volume Fraction (Upper Through-Hole)	0.0427126	0.0401731	0.0468843	0.0426627
Gas Volume Fraction (Lower Through-Hole)	0.0007834	0.0003438	0.0003438	0.0017856
Temperature at the Top of the Shaft (°C)	479.4	478.5	478.5	477.7
Temperature in the Upper Through-Hole (°C)	178.355	175.288	173.607	172.766
Temperature in the Lower Through-Hole (°C)	102.807	101.32	100.996	100.558

. Considering the balance between computational accuracy and time cost, the mesh grid with 11.88 million cells was finally considered for computation in the subsequent numerical simulations.

4. Results and Discussion of the Initial Cooling Channel

4.1. Steady-State Numerical Simulation Results with Phase-Change Cooling

Based on grid independence verification, steady-state parametric calculations were performed using the 11.88 million mesh and corresponding settings for the initial cooling scheme. Simulations were conducted at inlet velocities of 0.05 m/s, 0.1 m/s, 0.2 m/s, and 0.5 m/s, respectively. Observing the temperature distribution on the surface of the rudder shaft under different inlet velocities shown in Figure 8, it was found that at higher heat flux densities, the temperature near the connections with the upper and lower flanges was higher, with the maximum temperature located at the top of the rudder shaft. Overall, the temperature of the rudder shaft decreases with an increasing cooling water flow rate. At an inlet velocity of 0.05 m/s, the temperature at the top of the cooled rudder shaft remains around 500 °C. At inlet velocities of 0.1 m/s and 0.2 m/s, the temperature gradually decreases, and when the inlet velocity increases to 0.5 m/s, the highest temperature of the cooled rudder shaft is slightly above 400 °C (see Figure 8e).

Based on the steady-state calculation results, the boiling conditions in the tube under different inlet flow rate conditions are further analyzed and plotted in Figure 9. At an inlet velocity of 0.5 m/s as shown in Figure 9a, regions with higher heat flux density on the inner wall produce a nucleation center that generates bubbles. However, the central water flow has not reached saturation temperature, causing the bubbles to condense after detaching from the wall and entering the central water flow. The flow is in the surface boiling region. As shown in Figure 9b, when the inlet flow velocity is reduced to 0.2 m/s, the temperature of the central water flow inside the pipe reaches saturation temperature. The bubbles generated by the nucleation center gradually grow, with observable bubble flow and slug flow. The flow is in the saturated nucleate boiling region. When the inlet flow rate is further reduced to 0.1 m/s (see Figure 9c), the central water flow inside the pipe reaches saturation temperature, and in some areas, the fluid temperature is significantly higher than the saturation temperature. In addition to observable bubble flow and slug flow, some annular flow is present. Therefore, the flow is considered to be in the saturated nucleate boiling region. Some areas of the outlet pipe exhibit annular flow with droplet entrainment, indicating that this fluid is approaching or within the two-phase forced convective heat transfer region, which is relatively dangerous. When the inlet flow rate is set to the minimum value of 0.05 m/s as shown in Figure 9d, the regions with higher heat flux density correspond to higher gas phase content inside the pipe. The fluid largely enters the annular flow with the droplet entrainment state and is in the two-phase forced convection heat transfer region. Some sections even approach the single-phase vapor flow. With further increases in heat flux density or decreases in water flow velocity, there is a high risk of heat transfer deterioration due to boiling dry out.

The average convective heat transfer coefficients at different flow rates were calculated and summarized in

Table 6. Average convection heat transfer coefficient at different flow rates.

Flow Rate (m/s)	0.05	0.1	0.2	0.5
Average convection heat transfer coefficient (W/m2·K)	7545	8510	12,973	6142

. At an inlet velocity of 0.5 m/s, the fluid is mainly single-phase liquid. The heat transfer relies primarily on single-phase liquid forced convection, with the convection heat transfer coefficient mainly depending on the fluid velocity. At this velocity, the water flow rate is maximized, resulting in good cooling effects with minimal internal boiling heat transfer phenomena. At inlet velocities of 0.2 m/s and 0.1 m/s, the flow is in the saturated nucleate boiling region, relying mainly on boiling heat transfer. The cooling effect on the rudder shaft is relatively good, but the overall convection heat transfer effect decreases due to reduced fluid velocity, making the cooling effect slightly worse than at 0.5 m/s. Under the 0.1 m/s condition, dual-phase forced convection heat transfer regions appear near the outlet, with risks of further deterioration. At an inlet velocity of 0.05 m/s, the gas content increases further, and the fluid undergoes two-phase forced convective heat transfer with slower fluid velocities, resulting in insufficient cooling effects. Due to direct contact with steam in some wall regions, there is a high likelihood of heat transfer deterioration and a sharp increase in wall temperature with increased heat flux density or disturbed water flow velocity. This inlet velocity condition is considered quite dangerous and unsuitable for cooling solutions.

Observing the average surface pressure at five cross sections along the fluid flow direction at different velocities as shown in Figure 10, it is noted that the surface pressure decreases along the flow direction, reducing to atmospheric pressure at the outlet (see

Table 7. Average gauge pressure of 5 sections along the fluid flow direction at different flow rates.

Inlet Flow Rate (m/s)	Outlet Cross Section (Pa)	Middle Section 1 (Pa)	Middle Section 2 (Pa)	Middle Section 3 (Pa)	Inlet Cross Section (Pa)	Average Inlet and Outlet Pressure Drop (Pa)
0.5	0	58.62	1268.14	3685.09	6412.09	6412.09
0.2	0	25.29	905.848	2431.23	4350.70	4350.70
0.1	0	20.02	270.048	1638.14	3381.95	3381.95
0.05	0	10.64	300.368	1278.63	2949.65	2949.65

). Higher inlet velocities correspond to larger average pressure drops between the inlet and outlet. Considering the above factors, for the initial cooling structure, an inlet water velocity of 0.2 m/s is deemed more reasonable. On the one hand, it provides good cooling effects for the rudder shaft and, while meeting project cooling requirements, can save 60% of the total cooling water compared to an inlet velocity of 0.5 m/s. The pressure drop between the inlet and outlet is smaller, approximately two-thirds of that at 0.5 m/s. On the other hand, the 0.2 m/s condition has a higher average convection heat transfer coefficient (referencing the inlet temperature) compared to 0.1 m/s, with only a slight increase in pressure drop. Additionally, based on boiling mode analysis, the 0.2 m/s condition is less prone to heat transfer deterioration at the channel top, offering better safety.

4.2. Transient Numerical Simulation Result Under Phase-Change Cooling

To further analyze phase change processes and evaluate boiling heat transfer mechanisms, transient calculations were conducted alongside steady-state computations. The methods largely mirrored those used in steady-state calculations, utilizing the VOF two-phase model with liquid water as the primary phase and water vapor as the secondary phase. Simulations were performed with inlet velocities of 0.1 and 0.5 m/s, with a time step of 0.0005 s.

Taking the initial structure as an example, the location, main method, morphology, and heat transfer mode of bubble generation are explored to provide a reference for subsequent analysis. As shown in Figure 11, at a 0.1 m/s inlet velocity, small bubbles first appear on the upper surface of the liquid collection ring at 440 s, with gradual growth observed in the 440–446 s period. At this stage, most of the flow remains below the saturation temperature, and boiling is just beginning, placing the flow in the surface boiling region. By 450 s, the bubbles have grown, forming a dispersed bubble film on the upper surface of the liquid collection ring, with the onset of bubble, slug, and annular flows marking the transition to the saturated nucleate boiling phase. At 490 s, bubbles coalesce, forming a continuous film on the upper surface of the liquid collection ring, indicating a fully developed annular flow and a transition to film boiling.

Examining the flow state at t = 475 s, the fluid within the cooling channel undergoes phase change, as shown in Figure 12, with the gas phase reaching or exceeding the phase change temperature of water (~373 K), leading to intense boiling at the channel’s top and slug flow formation. These transient results correspond with steady-state findings but reveal a more intense boiling mode, especially at the 0.1 m/s inlet velocity, where conditions are closer to the risk of heat transfer deterioration. The results thus confirm the rationale for selecting a safer 0.2 m/s inlet velocity in steady state calculation.

At a 0.5 m/s inlet velocity, as shown in Figure 13, small vapor bubbles form around 825 s, with most of the flow remaining below saturation, marking the onset of surface boiling. Subsequently, over a prolonged period, the bubbles no longer grow and maintain a weak surface boiling state, which aligns with the steady-state calculation results. This phenomenon is attributed to the relatively high inlet velocity, where heat transfer is predominantly governed by forced convection of the single-phase liquid. As a result, the cooling water only progresses to a surface boiling state and cannot advance to more intense boiling regimes. For boiling heat transfer calculations, it is important to note that the saturation temperature for evaporation and condensation varies with the thermal environment. In this study, boundary conditions for wall heat flux also change over time, limiting steady-state calculations. Moreover, steady-state methods cannot capture dynamic changes in temperature and pressure over time, making it challenging to fully assess the cooling process. Therefore, transient simulations are essential for validating steady-state results and gaining a comprehensive understanding of real-time conditions for more accurate parameter analysis.

An inlet velocity of 0.5 m/s was applied, with a standard atmospheric pressure boundary condition at the outlet. As of the latest computation, transient calculations reached a maximum time of 1250 s, surpassing the period of most critical cooling conditions. As shown in Figure 14, the temperature distribution along the rudder shaft closely matches the steady-state results, with the highest temperature at the shaft’s top, peaking at around 475 °C at 1030 s and 460 °C at 1250 s. Temperatures decrease along the shaft, with a slight increase mid-shaft before gradually declining to the inlet temperature.

For flow resistance and pressure drop calculations, the average pressure across five cross sections was computed (see

Table 8. Average gauge pressure at different sections along the flow direction in the initial scheme.

Inlet Flow Rate (m/s)	Outlet Cross Section (Pa)	Middle Section 1 (Pa)	Middle Section 2 (Pa)	Middle Section 3 (Pa)	Inlet Cross Section (Pa)	Average Inlet and Outlet Pressure Drop (Pa)
0.5	0.4	50.8	1192.2	3490.0	6079.3	6078.9

). Transient results show slightly lower pressure drops than steady-state results, but both are within the same range, with minimal deviations in average pressure across sections. The primary difference between steady-state and transient results lies in the heat boundary conditions, leading to minor pressure differences that align with expected outcomes.

In the current work, the active cooling study is constrained to a specific rudder shaft, under a specific flight trajectory. For larger rudder assemblies and different flight regimes, the physical models and heat flux boundary will also change much, but we think the numerical methods and findings are also generally applicable to these conditions.

5. Optimized Design of the Cooling Channel and Its Cooling Performance

5.1. Structural Improvement of the Cooling Channel

In order to improve the active cooling performance and save the cooling water, another cooling channel design has been carried out, as shown in Figure 15. The improvement of the new cooling structure mainly includes three aspects. Firstly, two annular water storage channels were added internally at the junction of the rudder shaft and lower flange. These channels enhance boiling heat transfer in this region, which is characterized by the highest heat flux density. This modification helps to lower the temperature and alleviate the boiling heat transfer burden on the microchannels at the top of the rudder shaft and the liquid collection ring. Then, the volume of the liquid collection sleeve at the upper constriction of the rudder shaft was increased. This change allows cooling water to flow beyond the microchannels, thereby expanding the heat transfer area and increasing water storage capacity. Finally, the microchannels at the constriction of the rudder shaft were deepened, further increasing the heat transfer area. The results show that the improved structures can provide better active cooling effect and reduce the risks of boiling dry out. There may be a better design available. In future work, we can conduct simulations for other cooling channels and evaluate their performances.

5.2. Steady-State Simulation Result Analysis

As shown in Figure 16, a comparison of the temperature distribution along the rudder shaft at different flow rates revealed that, for both 0.1 m/s and 0.2 m/s inlet velocities, the new cooling structure exhibits a similar trend to the original design, with lower maximum temperatures as flow velocity increases. The enhanced convective heat transfer at higher fluid velocities results in better cooling performance at 0.2 m/s compared to 0.1 m/s.

Based on the forced convection boiling heat transfer range and flow pattern in the vertical tube, the boiling in the tube under different inlet flow rates is analyzed and presented in Figure 17. When the inlet flow velocity is 0.1 m/s, the fluid near the wall at the upper flange reaches the vaporization threshold, forming floating vapor bubbles, while some of the central flow remains below the saturation temperature, leading to the condensation of bubbles as they move into the central flow. This region remains in the surface boiling zone. At the lower flange, the central flow exceeds the saturation temperature, with observable bubble, slug, and annular flows. The annular vapor reaches a superheated state, with a significant liquid film remaining, indicating the saturated nucleate boiling region. When the inlet velocity increases to 0.2 m/s, the wall fluid at the upper flange reaches the vaporization threshold, but when comparing to 0.1 m/s velocity, the central flow does not reach saturation, leading to the condensation of bubbles without the significant development of bubble flow. The flow remains in the surface boiling zone. At the lower flange, the central flow reaches saturation, with gradually growing vapor bubbles and observable bubble and slug flows, indicating the saturated nucleate boiling region, albeit with relatively lower intensity.

Based on the above flow pattern analysis of the internal fluid, for both 0.1 and 0.2 m/s inlet velocities, the flow at the lower flange remains in the saturated nucleate boiling region, while the upper flange predominantly experiences surface boiling. Heat transfer at the lower flange relies on boiling in the annular water storage channel, whereas at the upper flange, boiling is less pronounced compared to the initial structure, leading to a significant role for forced convective heat transfer in the liquid phase. This suggests that the new cooling structure is safer, as it mitigates the risk of fluid boiling in the high-temperature region at the top of the rudder shaft.

The average convective heat transfer coefficient at the rudder shaft’s top is higher at 0.2 m/s inlet velocity compared to 0.1 m/s (see

Table 9. Average convective heat transfer coefficient at the rudder shaft’s top.

Flow Velocity (m/s)	0.1	0.2
Average convective heat transfer coefficient (W/m2·K)	7729	10,335

), with a pressure drop approximately 20% greater at the higher velocity. The 0.2 m/s inlet velocity offers better cooling efficiency with a moderate increase in pressure drop, making it advantageous. However, the 0.1 m/s inlet velocity also meets the cooling requirements without heat transfer deterioration, suggesting its advantage of halving the cooling water consumption and smaller pressure drop as shown in

Table 10. Average gauge pressure at five sections along the flow direction at different flow velocities.

Inlet Flow Rate (m/s)	Outlet Cross Section (Pa)	Middle Section 1 (Pa)	Middle Section 2 (Pa)	Middle Section 3 (Pa)	Inlet Cross Section (Pa)	Average Inlet and Outlet Pressure Drop (Pa)
0.1	0	55.4372	161.968	1326.6	3068.06	3068.06
0.2	0	12.163	141.859	1730.83	3649.56	3649.56

.

The axial solid temperature distribution comparison between the new and old cooling structures, as shown in Figure 18, indicates that the new structure provides superior cooling performance at the same flow rate. The addition of an annular liquid accumulation groove at the lower flange, where heat flux density is high, significantly enhances boiling heat transfer, effectively lowering the temperature compared to the old structure. Enlarging the liquid collection sleeve and deepening the channels at the constriction section further improve cooling by increasing the heat transfer area. Under the same water flow velocity, the cooling effect of forced convection of the liquid-phase fluid is improved compared to the previous structure. Consequently, the maximum temperature at the rudder shaft’s top decreases by approximately 40 °C to around 460 °C.

From the perspective of boiling regimes, although similar film boiling occurs at the top of the lower collection ring under a 0.1 m/s inlet velocity, its development is relatively constrained and does not reach the hazardous dry out region. Therefore, in the improved design, an inlet velocity of approximately 0.1 m/s can be adopted, thereby reducing the required cooling water flow. Additionally, to ensure safety in practical applications, the cooling water flow rate can be moderately increased to 0.2 m/s during the peak heat flux period between 800 and 1200 s by adjusting the valves, thus preventing heat transfer deterioration.

5.3. Transient Simulation Result Analysis

Addressing the issues of insufficient inlet flow and safety, the inlet condition with a velocity of 0.2 m/s was adopted before t = 550 s, and then the cooling water flow rate was increased to 0.3 and 0.5 m/s, respectively, with standard atmospheric boundary conditions at the outlet. As of the current analysis, the transient calculations for the improved cooling scheme have reached a maximum time of 1250 s. At this time point (t = 1250 s), the overall temperature distribution on the surface of the rudder shaft is similar to the steady-state calculations. The highest temperatures are located at the top, reaching approximately 478 and 488 °C under inlet velocities of 0.5 and 0.3 m/s, respectively, as shown in Figure 19. Additionally, higher temperatures are observed at the junctions between the rudder shaft and the upper and lower flanges, where heat flux density is significant. In other areas, particularly in the lower half of the rudder shaft, temperatures generally remain below 100 °C. Overall, the surface temperature of the rudder shaft is slightly lower under the 0.5 m/s condition, though the difference is minimal, with more noticeable variations only in the microchannel region.

Figure 20b shows the variation in the maximum surface temperature of the rudder shaft over time after the inlet flow rate increases, specifically for t > 600 s. It can be observed that, under both inlet velocity conditions, the maximum temperature of the rudder shaft rises rapidly between approximately 600 and 1050 s, with an increase exceeding 120 °C in both cases. Under the 0.5 m/s inlet condition, the maximum temperature reaches approximately 505 °C around t = 1050 s, while under the 0.3 m/s condition, it reaches about 515 °C, which is 10 °C higher. Following this, the maximum temperature of the rudder shaft begins to decrease rapidly, dropping to 478 °C at t = 1250 s under the 0.5 m/s condition, and to 488 °C, at t = 1250 s under the 0.3 m/s condition, with minimal difference between the two. Overall, during the heating phase before t = 1050 s, the rate of temperature increase under the 0.5 m/s inlet condition is lower than that under the 0.3 m/s condition. However, during the cooling phase after t = 1050 s, the temperature change rates under both conditions become similar. When considering the heat flux density changes depicted in Figure 6a, the heat flux density at the top of the rudder shaft peaks at t = 1000 s and then decreases rapidly, while other regions maintain their peak values. In contrast, in the transient calculation results of this round, the maximum temperature of the rudder shaft under both inlet velocity conditions peaks at approximately t = 1250 s, showing a lag of about 50 s relative to the heat flux boundary condition, which is consistent with theoretical expectations. It is noteworthy that the maximum temperature achieved with the improved scheme is higher than that of the original scheme. This is because the improved scheme employed an inlet velocity of 0.2 m/s during the initial 550 s, which is only 67% and 40% of the original scheme’s velocity, respectively. This led to a faster temperature rise in the early stages, accumulating more thermal energy. As the inlet velocity increased to match the same conditions, this difference gradually diminished, particularly after 1050 s when the temperature at the top of the rudder shaft decreased rapidly, indicating that the improved scheme offers better cooling performance.

The phase change in the cooling water within the channel is illustrated in Figure 21. Observing the simulation results under the 0.5 m/s inlet velocity condition, in regions with higher heat flux, particularly on the upper surface of the micro-channel at the top, there is evidence of bubbly bubble and slug flow, as well as some annular flow. This suggests that the overall flow is in the saturated nucleate boiling regime. Additionally, in a small portion of the area, the fluid enters a droplet-annular flow state, indicating the presence of two-phase forced convection heat transfer. Overall, the degree of boiling in high-risk areas is relatively low, remaining within a safe range. In comparison, under the 0.3 m/s inlet velocity condition, a higher degree of phase change can be observed. On the upper surface of the collection chamber, there is a greater presence of fluid entering the droplet-annular flow state, with a larger area experiencing two-phase forced convection heat transfer. This presents a certain risk of heat transfer deterioration. However, within the drainage channel, the gas–liquid two-phase flow can still pass relatively smoothly in the form of saturated nucleate boiling. Therefore, it is determined that the risk under this condition is relatively controllable.

The average surface pressure at the five cross sections shown in Figure 10 was calculated, and the results are presented in

Table 11. Average gauge pressure at different sections along the flow direction in the improved scheme.

Inlet Flow Rate (m/s)	Outlet Cross Section (Pa)	Middle Section 1 (Pa)	Middle Section 2 (Pa)	Middle Section 3 (Pa)	Inlet Cross Section (Pa)	Average Inlet and Outlet Pressure Drop (Pa)
0.5	0.4	37.0	395.3	2188.9	4941.3	4940.9
0.3	0.6	21.9	217.0	1651.2	3861.8	3861.2

. Overall, the pressure drop corresponding to the 0.3 m/s inlet velocity condition is lower, approximately 78% of the total pressure drop under the 0.5 m/s inlet velocity condition. Additionally, the total pressure drop under the 0.5 m/s inlet velocity condition in the improved design is about 81% of that in the initial design at the corresponding inlet velocity. This indicates that the improved cooling scheme also has an advantage in reducing flow resistance.

6. Conclusions

In this study, the problem of the risk of heat transfer deterioration occurred in the transient calculation results of the inlet flow velocity conditions of 0.1 and 0.2 m/s calculated in the steady state. It is necessary to increase the flow rate appropriately and timely to enhance the cooling capacity. Therefore, the transient simulation in the optimization scheme starts at t = 550 s, and the inlet flow velocities corresponding to the improved scheme are increased to 0.3 and 0.5 m/s, respectively. The results indicate that the 0.5 m/s inlet velocity condition in the improved scheme offers better cooling performance compared to the 0.3 m/s condition. Firstly, at any given moment, the surface temperature of the rudder shaft is consistently lower under the 0.5 m/s inlet velocity condition, with the maximum temperature difference at the top being approximately 10 °C. Additionally, during the initial rapid heating phase, the rudder shaft’s temperature rise rate is slower under the 0.5 m/s inlet velocity condition. Secondly, the boiling mode under the 0.5 m/s condition is safer, with the critical regions mostly in a saturated nucleate boiling state, posing minimal risk. In terms of pressure drop, the 0.3 m/s inlet velocity condition results in lower flow resistance. Furthermore, under the same 0.5 m/s inlet velocity condition, the total pressure drop in the improved scheme is reduced by approximately 19% compared to the initial design. In future work, new design structures, influences of inlet temperature, influences of alternative coolants, and effect of different flight regimes can be further investigated. Under a high temperature and cyclic thermal loading, the rudder shaft may encounter long-term fatigue problems, which will bring high risks in the applications. In future work, the thermal load distributions of the rudder shaft can be simulated and analyzed further.