Design and analysis of cooling jacket developed for vacuum power tubes by multiphase cooling

The vacuum tubes are used extensively in electronic industries. The MW level of vacuum tube are used in RF amplifiers and microwave sources in different sectors like defence, nuclear energy, satellites and medical diagnostics. The first step in the indigenous development of MW level of vacuum tube is the design of its cooling jacket. The cooling jacket of vacuum tubes use hypervapotron (HV) fins which are known for providing efficient cooling in compact space. The key objectives of this paper are to finalize the jacket’s construction material, evaluate the cooling jacket’s heat transfer performance at the MW level of RF (radiofrequency) power, and forecast safe operating conditions for given conditions of high heat flux and water flow rates. In this design, the vacuum tubes’ external dimensions are taken into consideration when designing the cooling jacket. ETP copper (Electrolytic Tough Pitch copper) and copper-chromium-zirconium (CuCrZr) are likely materials for the jacket’s construction. For the aforementioned design of the cooling jacket, FEA (Finite Element Analysis) simulations using a steady-state thermal module and computational fluid dynamics (CFD) simulations using an ANSYS CFX module are described for flow rates of 15, 30, and 60 lpm (liters per minute) and the heat flux 1, 2, 4, and 6 MW m−2. The results of CFD and FEA simulations are found to be in close agreement. A small deviation in results is seen after the start of nucleate boiling. 30 and 60 lpm are desirable flow rates for high heat flux values greater than 2 MW m−2. CuCrZr is the ideal material for a cooling jacket’s construction as it has safe working temperature limit of 350 °C at high heat flux values. Also, 15 lpm flow rate should be avoided while using this cooling jacket at heat flux values greater than or equal to 6 MW m−2.


Introduction
The ITER's ion cyclotron resonance heating and current drive systems (ICH and CD) deliver 20 MW of radio frequency (RF) power to the tokamak plasma [1]. ITER India, a domestic organization in India, is in charge of sending nine RF sources to the ITER project [2]. Each RF source generates 2.5 MW of the RF power, which is fed to the ITER machine at a frequency of 40-55 MHz and a VSWR of 2.0 [3]. Due to a lack of power vacuum tubes with the required power-handling capacity, a 2.5 MW RF source is created by combining two 1.5 MW parallel RF amplifier chains with a wideband hybrid combiner. Each amplifier chain has three stages: pre-driver, driver, and final driver-stage amplifiers. A solid-state power amplifier was used in the pre-driver stage, and power vacuum tubes were used in the remaining stages of the amplifier chain.
D.C. pulsed voltages of kilovolts and megavolts are used in the vacuum tubes at different power and frequency levels. The several MW RF power levels are generated in continuous or pulse mode using these vacuum tubes. The development of indigenous vacuum tubes for the amplifier chain for the MW level of the RF power is challenging. The high heat dissipation in tubes requires efficient water cooling in a compact space for Any further distribution of this work must maintain attribution to the author-(s) and the title of the work, journal citation and DOI. enhanced performance. The most important aspect of its development is the understanding of its thermal management. So, the first step towards the indigenous development of vacuum tubes shall be the design and development of the cooling jacket of vacuum tubes using hypervapotron fins. Hypervapotron (HV) elements are promising heat sinks for multiphase cooling in compact spaces. A hypervapotron is a device with fins through which cooling water flows perpendicular to the fins. Multi-phase cooling using HV elements in a cooling jacket provides efficient heat removal and allows extra capacity for temporary overloads. Cooling by the multiphase consists of water and vapor phases, which cool the hypervapotron elements. The design of the cooling jacket shall comprise these HV elements.
The formation, growth, departure, and coalescence of bubbles, as well as vortex behavior within the various parts of HV devices, all have significant effects on the flow field and temperature field. The phase change and interfacial tension between the liquid and vapor phases greatly complicate heat transfer which is explained in the available literature [4][5][6]. Researchers have mostly stuck to more straightforward approaches [7,8], rather than observing the flow field and vortex formation at the microscopic scale in experiments. Studies of bubble characteristics in pool boiling under ordinary pressure and low heat flux predominate, while literature on HV heat transfer under high heat flux and high pressure [9][10][11] is scarce. The phase-change experiment is supplemented by numerical simulation in the available literature.
A recent effort has been made to use OpenFOAM to create a numerical model of subcooled nucleate boiling applicable to a variety of thermal management scenarios. Reference [12] discusses atmospheric pressure convective boiling water in a circular channel 3 mm thick, 100 mm in diameter and 400 mm deep. OpenFOAM's Euler two-fluid-based CFD model considers various factors like Reynolds numbers, inlet subcooling, and applied heat flux. The new model is suitable for boiling water at limits, as it was developed using ONB data from CFD simulations involving the properties of boiling water. A recent paper [13] simulated the flow of R-113 along a small circle at 2.69 bar pressure using 2D axisymmetric computational fluid dynamics simulations. This article explores the importance of energy interactions in flow and finally concludes that it is better to ignore energy transfer in future simulations of freeze-boiling flow.
The hypervapotron concept is well researched in above literatures for effective cooling. However, the cooling jacket design of vacuum tubes at the MW level is hardly discussed in any literature sources. So, the prime objective of this paper is to present knowledge of the design and analysis of cooling jackets using concept of hypervapotron fins at the MW level of the RF power, as it is the first step towards the development and understanding of vacuum tubes. The key objectives are the preparation of the mechanical design and model of the cooling jacket, the choice of building material, the finite element analysis (FEA) using empirical correlations, and the CFD simulation of the cooling jacket for high heat flux values to determine its wall temperature at different flow rates using ANSYS CFX module. At various combinations of flow rates and heat flux values, these simulations will also show whether the flow is single-or multi-phase. This study will assist researchers and students working in the field of RF technology to develop their own vacuum tubes at the MW level. This can be of further assistance in customizing the vacuum tube and its cooling jacket in accordance with the requirements of the individual.

Methodology
In the present study, the first step was to design and model the cooling jacket of a vacuum tube. The second step was to prepare the simulation setup using the model of the cooling jacket to carry out both CFD and FEA (Finite element analysis). The heat flux was considered as the reference for the study and simulation of the cooling jacket.

Design and modeling
The cooling jacket of the power vacuum tube design should be such that it can efficiently cool the tube, even at a high heat flux. The internal design of the cooling jacket of the power vacuum tube was not known in this study. There is hardly any information regarding the interior design aspects of cooling jackets. During the design process of the cooling jacket, the internal cooling fins serve as hypervapotron elements and the outer dimensions are maintained in accordance with vacuum tubes. A literature survey helped finalize the fins [14][15][16][17][18][19][20].
The typical outer dimensions of a power vacuum tube at the MW level were cylinders with a height of 400 mm and a diameter of 250 mm [15]. Therefore, the cooling jacket was designed as a cylindrical jacket with a height of 400 mm and a diameter of 250 mm, as shown in figure 1(a). The internal cooling circuit has fins throughout the cylinders such that water flows perpendicular to the fins. The water enters from the top and exits from the bottom of the cylindrical cooling jacket. This is illustrated in figure 1(b).A 3D model was prepared using CATIA V5 R28 for simulation. The cooling jacket comprises an inner cylinder, an outer cylinder, and top and bottom cover plates. The construction material for the simulation model is CuCrZr. The inner cylinder, with a thickness of 10 mm, has fins throughout the cylinder around the cylindrical axis. The height and the width of the fin are 4 mm and 3 mm, respectively, as shown in figure 2. A cut section with two fins and two grooves was modelled and used in the simulation, as shown in figure 3. The nomenclature for two fins and two grooves is shown in figure 4. The outer cylinder is 4 mm thick and cover the finned cylinder completely around the cylindrical axis. The top and bottom cover plates, each with a thickness of 4 mm, cover the cooling jacket completely on both the top and bottom faces. The top and bottom cover plates contained holes of diameter 4 mm at the water inlet and outlet, respectively. The top and bottom plates have not been used in simulation. The detailed design of this cooling jacket is not within the scope of this paper. The important design parameters are shown in table 1 below.
The construction material for the cooling jacket was copper alloy. The major alloys that can be used are ETP copper, OFHC copper, CuCrZr, and CuAl25 [14,18]. The two most probable materials are ETP (Electrolytic Tough Pitch) copper and CuCrZr (Copper Chromium Zirconium Alloy). ETP copper is 99.9% pure copper and is widely used in radio frequency coaxial transmission lines because it has excellent thermal (395 W m −1 -K −1 ) and electrical conductivity. Whereas CuCrZr has 98.6% copper, 0.8% chromium, and 0.3% zirconium and has lower thermal (320 W m −1 -K −1 ) and electrical conductivity in comparison to ETP copper. But still, the popular material to be used in high heat flux conditions is CuCrZr because it has a high softening temperature limit and is structurally stronger (has a higher yield strength than ETP copper). The safe working temperature limit of ETP copper is 160°C, whereas CuCrZr can withstand temperatures up to 350°C [16]. The selection of the copper alloy can be done based on the simulation results. The simulation was performed using the material properties of CuCrZr [16].

Analysis by simulation of the cooling jacket
The analysis by ANSYS simulation of the cooling jacket was performed for four heat flux levels: 1, 2, 4, and 6 MW m −2 . The performance of the cooling jacket is analyzed for each heat flux value at different flow rates, which are 15 lpm (liters per minute), 30 lpm, and 60 lpm. ANSYS 18.2 is used as software.

Steady state thermal analysis
The first step in the simulation analysis is to perform a steady-state thermal analysis of the cooling jacket. The different heat-transfer regimes depend on the wall's superheat. The first regime is a forced convection with a single phase. The second regime is the start of nucleate boiling, also known as the onset of nucleate boiling. Fully developed boiling is the last regime. An intermediate regime exists that corresponds to the partial boiling regime. A forced convection regime with a single phase occurs when the incipient boiling temperature exceeds the wall superheat. Onset of the Nucleate-Boiling (ONB) occurs when the wetted surface temperature exceeds the fluid saturation temperature in a localized region. During this regime, the temperature at which the bulk water is saturated remains below the temperature of the wet surface. Different correlations are available for the aforementioned regimes. The basic assumptions behind the below equations (equations (1)- (10)) are that the flow is in a forced convection regime with a single phase in a circular tube and the fluid properties, such as dynamic viscosity and thermal conductivity, remain constant. Also, the flow is assumed to be turbulent, fully developed and incompressible.
In the single-phase forced convection regime [21], the following modified Dittus-Boelter correlation, shown in equation (1), is used: =´´T he factor ff = 1.35 is used to account for recirculating flows due to the geometry of fins or HV elements. The ff was determined by comparing the calculated results with the measured outcomes of experiments conducted at JET [21,22] obtained at a wide range of flow velocities and geometries while the heat fluxes were kept relatively low. The onset of nucleate boiling starts just after the regime of forced convection [21]. This can be calculated using equations (1) and (2).
A correlation was used in the Onset of the Nucleate-Boiling (ONB) regime given by Bergles-Rohsenow [23]. Based on the correlation in equations (3) and (4), the superheat required to calculate the incipient boiling temperature can be estimated.
The flow rate and HV element area help in calculating the heat transfer coefficient for equation (4). The value is calculated from equation (4) and then used in the RHS (right hand side) of equation (3). The value of the wall temperature is assumed and it is varied from 170°C to 200°C. T ONB is calculated by the hit-and-trial method, making LHS = RHS for equation (3) of the manuscript.
The partial boiling regime has the correlation shown in equations (5)- (7) to capture the transition region given by Bergles Rohsenow, which is a modified Kutateladze correlation [23] described below: he correlation that Thom [24] provides yields the heat transfer coefficient in fully developed boiling. The below equations, which are given in equations (8)-(10), were used to calculate the heat-transfer coefficient. The coefficient of heat transfer calculated from these correlations was then applied as a boundary condition for steady-state thermal analysis.
n this analysis, a steady-state heat diffusion equation is solved for the solid domain using the finite element analysis software ANSYS. Using empirical correlations from the literature, the heat transfer coefficient is determined and applied as boundary conditions for the forced convention and subcooled boiling regimes. This analysis employed a model consisting of a cutout portion with axis-symmetric and half-symmetric fins and grooves. This three-dimensional model has a hexahedral mesh for steady-state thermal analysis. The minimal edge length is considered to be 0.001. For this analysis, a relatively coarse mesh has been employed. Figure 5 graphically depicts this. The inner surface of the inner cylinder with fins was subjected to a constant heat flux. The heat transfer coefficient was applied to the wet surfaces. There was a temperature gradient across the fin; consequently, the coefficient was dependent on the temperature of the wet wall. This nonuniformity causes boiling at the base of the fins because the ONB temperature is lower than the base temperature. The fin tips underwent single-phase convective heat transfer. This analysis was conducted for flow rates of 15, 30, and 60 lpm at 8 bar static pressure.

CFD analysis of cooling jacket
The CFD analysis used a multiphase (two-fluid) model. A vapor is a dispersed fluid, whereas a liquid or water is a continuous fluid. This model uses interfacial momentum transfer, mass transfer, and heat transfer [17,25,26], as shown below: Interface momentum transfer The constitutive terms are modelled using equations (11)- (13), which also include the phase interaction terms ( , kj G M , kj Q kj ) to achieve closure. Momentum transfer, energy transfer, and mass transfer for each phase occur across the interfaces, which leads to the derivation of a closure model. The vapor phase (dispersed) and liquid phase (continuous) have closure relationships that are included in the model and also included in the ANSYS CFX module.
The generation of bubbles, which occurs on the hot surface of the wall, uses a boiling model at the wall; ANSYS CFX uses the same model [25]. There are three types of heat-transfer mechanisms: evaporative, quenching, and convective. These three types of heat transfer together constitute wall heat. Kurul proposed a model for the partitioning of wall heat [26], Q w where the total heat flux at the wall is given by equation (14) ( ) Equation (15), which takes the local Stanton number [25] into account, provides the heat transfer by convection.
ere, the temperature of the wall was T w and the temperature of the liquid was T l and the velocity of the cell next to the wall was U .
l The fractional area of the total area subjected to cooling by convection was A .
f When the heated surface comes into contact with the liquid, a bubble forms and departs, and this is the point at which heat transfer from quenching occurs. The Q q is given by equation (16) from Mikic and Rohsenow [27].
he heat transfers due to vapor formation, Q e shown by equation (17), on a heated surface is given by: he term 'n' is the density of the nucleation site for the bubble, ' f ' is the detachment frequency for the bubble, 'd ' bw is the departure diameter of the bubble and 't ' w is the waiting time. The ' A q ' is the portion of the wall's total area cooled by quenching. The above equations include these parameters, and the correlations below are used to calculate them.
There are fundamental presumptions that lie beneath equations (11)-(22) that have been made. It is presumed that there is a state of local thermodynamic equilibrium within both the liquid and the vapor phases individually. This means that the fluid properties, such as temperature, pressure, and composition, are assumed to be uniform within each phase at any given point. This can occur at any point in the system. Additionally, it is presumed that the temperature of the liquid and vapor phases at the interface is in a state of local equilibrium. The second premise is that the interface between vapor and liquid has a negligible amount of interfacial and thermal resistance. This assumption makes it possible for the numerical model to successfully transfer heat, mass, and momentum across the vapor-liquid interface with barely any sort of resistance. It is also presumed that the deformation or movement of the surface of the boiling liquid caused by the formation and collapse of bubbles is not a significant factor. Because of this assumption, a more straightforward analysis of heat transfer can be carried out without considering the influence of surface motion.
Using the symmetry of the model and flow, a cut-out portion comprising two fins and two grooves was modelled and meshed. The cover plate is not considered in the simulations. The simulation was performed for all the heat fluxes, i.e., 1, 2, 4, and 6 MW m −2 . The coolant flow is analyzed using CFD under both single-phase flow (SPF) and sub-cooled boiling (SCB) conditions, with the same boundary conditions and steady-state conditions. This study employs the shear stress transport (SST) k-omega Reynolds averaged Navier-Stokes (RANS) turbulence model. Assuming a constant heat transfer coefficient in the forced convection regime. As the vapor phase is assumed to be dispersed in a continuous liquid phase by the interphase transfer models, a Eulerian dispersed two-phase flow model is selected for a nucleate boiling model. Ansys CFX employs the RPI (Rensselaer Polytechnic Institute) model for multiphase simulations, which includes wall-generated vapor generation (bubble nucleation).

Mesh independence study and boundary condition for CFD simulation
The mesh independence study is important to get reliable results. Because the HV (hypervapotron) elements shown in figure 4 resemble the HV profile used by Milnes [17], a separate mesh independent study has not been conducted. As a result, Milnes' [17] study on grid independence served as the basis for the mesh size. The cell near the wall is taken as 5 μm, and the non-dimensional y + is taken as less than 2.5 in all the CFD simulations. The fluid wall interface of the mesh model has small grids with a first layer thickness of 10 μm. Figure 6 depicts the mesh model used in the 3D CFD simulation.
The details about inlet and boundary conditions are shown in the table below. A few set-up details used in CFD simulation are also shown in table 2.
An 8-bar static pressure was the outlet boundary condition. The data were taken from the NIST ('National Institute of Standards and Technology') [28], and they show that the characteristics of vapor and fluid are temperature-dependent. For the advection scheme, high resolution was used. The Milnes method [17] is the  foundation upon which the CFD setup is developed. On the basis of this reference, the RPI model is used. As a convergence criterion, a value less than 1e-04 was employed. At roughly 178°C, the saturation temperature remained constant. The heated wall received a constant heat flux under the no-slip scenario. A value of 250 was chosen for logarithmic y-plus [29]. Figure 7 illustrates the fluid portion, which is the highlighted area with the water inlet and outlet. Figure 8 depicts the solid portion (wall).

Validation
Validation is a crucial step prior to discussing results. As part of the model validation process, a few references [17,19,20,30] were reviewed and their simulation setup and results were compared to those listed below. This simulation makes use of the RPI wall boiling model and various sub-models (bubble diameter, bubble detachment). The setup for CFD analysis using the RPI model is based on Milnes's [17] reference to computational modelling. Kim used a similar simulation setup and the same reference (Milnes et al [17]) for his 2D CFD analysis of HV ion dumps, as described in section 3 of his paper [19]. In addition, the results obtained for the 2D CFD analysis of the cooling jacket of the vacuum tube have been validated against the simulation results of Ying [20]. In addition, the use of ANSYS CFX software for boiling heat transfer is supported by Vyskocil et al [30], where it is stated that ANSYS CFX can be used to simulate boiling heat transfer with bubble formations and validated with experimental data.
The only difference between the HV elements is the height of the cavity. The HV cooling fins of the tube jacket have a fin width of 3 mm, a cavity width of 3 mm, and a height of 4 mm. Ying's [20] HV fins have dimensions of 3 mm fin width, 3 mm cavity width, and 2 mm height. To validate the below results, a 2 mm tall HV fin model was created. This new model employs the CFD analysis setup detailed in table 2 of this paper. To According to the data presented in table 2 of the research paper written by Ying [20], the wall temperature registers at a value of 268.5°C. In contrast, the wall temperature that was calculated using a simulation of this HV fin modelled with a height of 2 mm was found to be 260°C (533 K), as can be seen in figure 9 below. The results that were obtained after simulation are only slightly different from the results that were found in table 2 of Ying [20], which indicates that the difference is only about 4%. This demonstrates that the configuration of the simulation, as well as the result obtained through CFD analysis, is consistent with the results that have already been validated. The validation of the theoretical model against the experimental data will be a future task.

Results
These analyses have led to the results presented here. Table 3 displays the results of a single set of 2D and 3D CFD simulations. A 2D CFD simulation was performed for the remaining heat flux and flow values due to the small discrepancy between the results derived from the 2D and 3D CFD simulations.
First, a FEA study was run. The TONB and heat transfer coefficient values for the water flows were estimated using equations (1)- (10). Using the trial-and-error method with equations (3) and (4), we found that the TONB for 15 lpm, 30 lpm, and 60 lpm was 180°C, 186°C, and 190°C. For 15 lpm, the calculated value is 2.2 MW m −2 , for 30 lpm, 4.01 MW m −2 , and for 60 lpm, 6.8 MW m −2 . The effectiveness of the heat transfer was evaluated based on the temperature of the wall facing the heat flux. The temperature of the wet wall was also simulated using steady-state thermal calculations. Second, 2D CFD simulations were run for all of the heat flux values. Tables 4-7 show the FEA and CFD findings for various heat fluxes and flow rates. In accordance with table 7, figures 10(a) and (b) display the 2D CFX analysis and FEA results for a heat flux of 6 MW m −2 and a flow rate of 30 lpm, respectively. Figures 11 and 12 depict the vapor volume fraction and fluid velocity determined by 2D CFX analysis for a heat flux of 6 MW m −2 and a flow rate of 30 lpm, respectively. Figure 10 shows that the vapor volume fraction was 0.5 for the sole purpose of demonstrating the existence of a twophase simulation for the specified heat flux and flow rate. Figure 11 shows a fluid moving at a velocity of 2.2 m s −1 .
Tables 4 and 5 display the outcomes for 1 MW m −2 and 2 MW m −2 heat flux values, respectively. The outcomes listed in tables 6 and 7 correspond to heat fluxes of 4 and 6 MW m −2 . Both FEA and CFD analyses recorded the inner cylinder wall temperature and wet-wall temperature. The results of the CFD analysis indicate that the inner cylinder wall temperature decreases as the flow rate increases. This is consistent with the expected heat transfer behavior in the system. At a flow rate of 15 lpm, for instance, the 2D CFX analysis revealed that the inner cylinder wall temperature was 180°C. In 2D CFX analysis, the inner cylinder wall temperature decreased to 154°C as the flow rate increased to 30 lpm. In addition, the difference between FEA and CFD results is minimal in tables 4 and 5, but it increases in tables 6 and 7. Figure 13 depicts the relationship between flow rate (lpm) and wall temperature (°C). It shows the temperatures of the walls at various heat-flux levels. The saturation temperature, represented by the dotted line at 178°C, is shown. The curves above the dashed line represent the transition to a two-phase flow.

Discussions
The 2D and 3D CFD simulations were in close agreement with one set of results, as shown in , the CFD result for the T wall indicated a low bubble formation and is shifting towards the twophase simulation. The T wall was very close to the ONB temperature for the flow rate and heat flux mentioned above. The CFD results listed in tables 6 and 7 are due to two-phase simulations in the subcooled boiling regime for the given heat flux and flow rate. The T wall was significantly above the ONB temperature for the above-mentioned flow rate and heat flux. Figure 11 shows the result value for the vapor fraction. The vapor fraction is shown just to prove the existence of a two-phase condition in HV fins. It is clear from figure 13 that the T wall values for 1 MW/m 2 are below the saturation temperature line. The bubble formation starts at 15 lpm and 2 MW m −2 , as the line of saturation temperature just intersects it. The T wall values for 6 MW m −2 and 4 MW m −2 are above the saturation temperature line and lie in the boiling regime. The wet wall temperature is  15  444  380  470  359  30  296  227  290  224  60  269  200  262  195 the localized temperature at the fluid-wall interface. The wet wall temperature is lower than the wall temperature, as shown in tables 4-7. This is because the localized heat transfer coefficient at the fluid-wall interface is higher due to the bubble's formation at the interface.  The results in tables 4-7 and figures 10(a)-(b) demonstrate a close agreement between the FEA and CFD simulations. The inherent nature of FEA and CFD analysis is the cause of the slight deviation. The FEA approach, which is macroscopic in nature and built to consider various uncertainties in fluid dynamics and boiling behavior, is based on the correlations of coefficients of heat transfer that earlier researchers had generated for various experiments. Standard boiling models created for CFX, however, depended solely on studies done on circular tubes. This correlation, which considers the microscopic nature of fluids, needs to be modified or established specifically for HV principles to be able to increase CFD accuracy. The analytical calculations and the CFD results diverge as a result of this. Further, the deviations are quite low (8%) when the flow is in a single phase, but the difference rises up to 15% when the flow enters a two-phase condition. For example, the deviation is small for 4 MW m −2 and 60 lpm from table 6 because the T wall value is just above ONB temperature, and so the boiling phenomenon just begins in this case. But, for flows of 15 lpm and 30 lpm at 4 MW m −2, the results differ more because the flow enters the two-phase condition completely.

Conclusion and future work
The results of CFD and FEA simulations are in close agreement. After the onset of nucleate boiling, a slight deviation is observed in the results. This deviation increases with an increase in the incident heat flux. The results  discussed above provide a clear idea of the operating scenarios that should be used for the cooling jackets of highpower RF vacuum tubes. These results provide a few important lessons. The desirable flow rates for high heat flux values greater than 2 MW m −2 are 30 lpm and 60 lpm. These flow rates help in keeping the jacket temperature well within the safe working temperature limit of CuCrZr (350°C). The desirable material of construction for a cooling jacket is CuCrZr. It can withstand the high heat flux values at the mentioned flow rates. The cooling jacket can also be manufactured using ETP copper as an alternative material, but then it should be used for lower heat flux values like 1 MW/m 2 and 2 MW m −2 , so that the jacket temperature lies well within the safe temperature range of 160°C. Also, the flow rate of 15 lpm cannot be used with 6 MW m −2 because the wall temperature value crosses the safe working temperature limit of 350°C for CuCrZr. So, 15 lpm should be avoided while using this cooling jacket at heat flux values greater than or equal to 6 MW m −2 .
The future work will consist of further simulation and experimentation. The detailed CFD simulations for different flow rates and heat flux values will be done with a complete 3D model. The different boiling models and the different profiles of HV elements will be explored as part of the future research work. Finally, a prototype similar to the simulated model will be manufactured for mock-up tests. Although the data produced by the CFD method are comparable to the theoretical correlations (these relationships are based on experimental data), it is necessary to validate the CFD results with experimental data in the future. Therefore, although the design of the cooling jacket for a vacuum tube appears valid, further research using mock-up tests is required. It is expected that this study will provide a solid basis for the design and analysis of cooling jackets for high-power RF vacuum tubes.