Numerical Investigation of Flow and Flame Structures in an Industrial Swirling Inverse Diffusion Methane/Air Burner

Abstract

In this study, a novel gas burner combining air swirl and an inverse diffusion flame (IDF) is designed for industrial applications. Numerical simulations using the Reynolds-averaged Navier–Stokes (RANS) method and simplified reaction mechanisms are conducted to predict the turbulent flow and combustion performance of the burner. Detailed flow structures, flame structures and effects of burner configurations are examined. The simulation results indicate that the swirl action of the burner creates a central recirculation zone and two external recirculation zones at the burner head, which stabilize combustion. The tangential velocity is minimal at the center of the burner and decreases with increasing distance from the outlet. As the distance from the exit increases, the maximum tangential velocity gradually decreases, and the peak value shifts towards the wall. This decrease in tangential velocity with axial distance signifies the gradual dissipation of the swirl effect, which disappears near the chamber outlet. The comparisons reveal that altering the number of burner fuel nozzles is more effective in reducing NO emissions than changing the inclination angle of the fuel nozzles, in the given conditions. Favorable combustion conditions are achieved when there are 16 fuel nozzles and the nozzle inclination angle is 60°, resulting in a 28.5% reduction in NO emissions at the outlet, compared to the reference condition.

1. Introduction

Nitrogen oxides (NO_X) pose a significant hazard to both the environment and human health [1,2]. As a clean fuel, methane (CH₄) has garnered increasing attention; however, the emission of NO_X during its combustion, particularly thermal NO_X generated in high-temperature zones, remains an urgent issue. Numerous institutions have conducted research on low-nitrogen combustion technologies, including flue gas recirculation (FGR) [3], lean fuel premixed combustion [4], moderate or intense low-oxygen dilution (MILD) combustion [5], swirl combustion [6], and so on. Swirl combustion technology combines air swirling with the direct injection of fuel gas. The centrifugal effect of rotation creates a large radial pressure gradient, forming a central recirculation zone. Swirling flow is widely used to enhance flame stability through this recirculation zone, which carries hot combusted gas downstream and mixes it with a cold gas mixture. The combustion product is diluted with unburned gas and air, ensuring the stable combustion of low calorific value fuel and reducing NO_X emissions [7]. Reza S. et al. [8] conducted large-eddy simulations (LESs) to evaluate the performance of a swirling trapped-vortex combustor. The findings indicate that a large recirculation zone dominates the cavity for all swirl numbers, resulting in strong fuel–air mixing and high combustion efficiency. Dong et al. [9] studied the characteristics of gas production, temperature distribution, and tar pollutants, with different swirl angles. The results show that swirl flow injection exhibits stronger gasification performance than traditional straight flow injection. Compared with the other three low-nitrogen combustion technologies, swirl combustion has the advantages of fast ignition, good combustion stability, and a high burnout rate.

The main types of combustion flames are premixed flames, partially premixed flames, and diffusion flames. Premixed or partially premixed flame jets release heat quickly, have high flame temperatures, and exhibit soot-free flame structures. However, there is an inherent risk of flashback, in the absence of external stabilization facilities. Diffusion flames are divided into normal diffusion flames and inverse diffusion flames (IDFs). Normal diffusion flames offer good combustion safety and low blow-off tendencies, but suffer from issues like low heat release rates, excess soot emissions, and overly long flame lengths, due to incomplete combustion. IDFs are a type of diffusion flame, where an internal air jet is surrounded by external fuel jets, either in confined or unconfined conditions. The positions of the fuel and oxidizer are reversed compared to a conventional diffusion flame, with the oxidizer, such as oxygen or air, centrally located around the fuel. IDFs have advantages in terms of no flashback, less soot loading than normal diffusion flames, low NO_X emissions, and a wide flammability range [10]. There has been some research on the characteristics of IDFs [11,12]. Dong et al. [13] conducted an experimental study on an IDF burner designed by Sze et al. [11]. Their results indicate that fuel/air jet entrainment is a key factor in determining the flow and flame structures of concentric co-flowing IDFs. Mikofski et al. [14] studied the flame structure of laminar IDFs to gain insights into soot formation and growth in ventilated combustion. Zhen et al. [15] examined the thermal and emission characteristics of a swirl-stabilized turbulent IDF burning liquefied petroleum gas. Overall, existing studies mainly focus on the flow and combustion characteristics of lab-scale IDF gas burners. The application of IDFs to industrial gas burners is still lacking, which requires further detailed investigation into the operating performance, fluid dynamics, and geometrical parameters.

Given the advantages of IDF and swirl combustion technology, combining these two combustion modes may yield unique potential. Despite a wider stable operation range and reduced soot luminosity, IDFs have the drawback of a long flame torch, which increases the risk of hitting the boiler walls. Swirl IDFs can mitigate this issue by reducing the flame length and size, achieving more compact combustion and compensating for this shortcoming. Thus, in this work, a new type of industrial-scale swirling IDF gas burner is designed, integrating air swirl with an inverse diffusion flame. Unlike conventional inverse diffusion burners, this design introduces air in a swirling state, enhancing the mixing degree of the fuel and the oxidizer. This approach has potential advantages, such as ensuring stable combustion and reducing NO_X emissions, simultaneously.

Researchers have employed experimental methods to investigate the combustion characteristics of gas burners, citing their strong intuitiveness and high reliability [16,17]. However, with the advancement of computer technology, numerical simulations have garnered increasing attention. In contrast to experiments, numerical simulations offer advantages, such as higher efficiency, lower costs, and offer a comprehensive understanding of detailed flame structures, flow fields, and temperature distributions. In the realm of numerical simulations for gas burners, the depiction of gas turbulence flow typically falls into three categories: direct numerical simulation (DNS), large-eddy simulation (LES) [18,19], and Reynolds-averaged Navier–Stokes (RANS) simulation [20]. While LES and DNS can yield higher simulation accuracy and efficiency given the same grid conditions [21], they entail longer computational times. On the other hand, RANS simulation can deliver satisfactory results with fewer grids. RANS equations express high-order unknown terms and turbulent transport equations through time means and low-order unknown terms, enabling closure of the equations. This approach is reasonable for predicting turbulent combustion and aligns with practical engineering requirements. Due to the substantial size of industrial-scale devices, extensive grid discretization of the computational domain is necessary, consuming significant computational resources and time. Considering computational cost and efficiency, the RANS method is widely used in engineering, demonstrating sufficient accuracy for large-scale calculations, as confirmed in previous studies [22,23,24]. Hence, in this study, the RANS method is employed to simulate turbulent gas flow in an industrial swirl IDF gas burner. Moreover, accurately depicting the interaction between turbulent flow and combustion processes necessitates the application of appropriate chemical mechanisms. Previous studies by Han X et al. and Ahn S et al. utilized global reaction mechanisms (GRMs) with several steps [25,26], while Smith, G. P. et al. adopted a detailed mechanism with 325 steps [27]. Striking a balance between accuracy and efficiency requires the utilization of simplified mechanisms. Numerous numerical investigations have delved into the reaction processes in gas burners [28,29,30].

In regard to the existing research, very few numerical studies have explored the complex flow and flame structures in industrial-scale gas burners, where combustion behaviors can differ significantly from those in laboratory-scale burners. In this work, a novel gas burner combining air swirl and an inverse diffusion flame is designed for industrial use. Prior to the actual operation of the designed swirling, inverse diffusion burner, it is crucial to study in detail the flow dynamics and thermal characteristics through numerical simulations, as these aspects are difficult to detect using experimental devices. Such simulations provide valuable guidance for industrial operation. Numerical simulations based on the Reynolds-averaged Navier–Stokes (RANS) method and simplified reaction mechanisms are conducted to predict the turbulent flow and reaction performance. First, detailed flow structures, including the recirculation zone distributions and velocity profiles, are analyzed. Next, the flame structures are comprehensively clarified, based on temperature and species distributions. Finally, the effects of burner configuration structures on the flow and flame structures, as well as pollutant emissions, are studied to evaluate the optimal operating parameters.

2. Configuration of the Industrial Swirling, Inverse Diffusion Gas Burner

Figure 1a shows the configuration of the novel inverse diffusion, swirling gas burner. The combustion chamber is a cylinder, with a diameter of 1.8 m and a length of 10 m. Air enters through the center of the burner, where eight swirl blades are distributed in the central air inlet. One side of each blade is fixed on a pivot with a diameter of 76 mm, while the other side is fixed on a tube wall with a diameter of 300 mm. These eight blades create a swirling air jet that has both axial and significant tangential inlet velocities, causing the gas to rotate towards the chamber outlet. Surrounding the central air inlet are eight tubes, each with a diameter of 32 mm and a length of 294 mm, used for fuel injection. The internal air swirl is enveloped by the external fuel jet, forming an inverse diffusion flame structure. This configuration combines the benefits of both diffusion flames and premixed flames, offering advantages in terms of operational safety, pollutant emission levels, and flame stability. The top of each tube features an elliptical incision, enhancing the mixing of fuel and air. Figure 1b shows a photo of the swirling, inverse diffusion burner designed for an industrial gas boiler. Each elliptical incision on the gas pipes has 57 small nozzles, each with a diameter of 6 mm. In numerical simulations, these nozzles are simplified to a uniform gas inlet, meaning gas is uniformly injected into the combustion chamber through the elliptical incisions. This simplification improves local grid quality and reduces grid quantity, thereby enhancing simulation efficiency to some extent.

3. Numerical Simulation Procedures

3.1. Governing Equations

The governing equations for turbulence fluctuations are derived using Reynolds decomposition, which describes turbulent motion as random variations around a mean value. By introducing a weighting function for temporal averaging, the governing equation can be expressed as follows [31]:

Continuity equation:

$$\frac{{\overline{\partial \rho u}}_j}{\partial x_j}=0,$$

(1)

Momentum equation:

$$\begin{gathered} \frac{\partial \overline{\rho } {\overline{u}}_i{\overline{u}}_j}{\partial x_j}+\frac{\partial \overline{\rho } \overline{{u_i}^{\prime }{u_j}^{\prime }}}{\partial x_j}=-\frac{\partial \overline{p}}{\partial x_i}+\frac{\partial }{\partial x_j}\left[\mu \left(\frac{\partial \overline{u_i}}{\partial x_j}+\frac{\partial \overline{u_j}}{\partial x_i}\right)+\left({\mu }^b-\frac{2}{3}\mu \right)\frac{\partial \overline{u_i}}{\partial x_i}{\delta }_{ij}\right] \\ -[\frac{\partial \overline{{\rho }^{\prime }{u_i}^{\prime }}\overline{u_j}}{\partial x_j}+\frac{\partial \overline{{\rho }^{\prime }{u_j}^{\prime }}\overline{u_i}}{\partial x_j}+\frac{\partial \overline{{\rho }^{\prime }{u_i}^{\prime }{u_j}^{\prime }}}{\partial x_j}]+\overline{f_i}, \end{gathered}$$

(2)

where:

$$\frac{\partial \overline{{u_i}^{\prime }}}{\partial x_j}=0,$$

Energy equation:

$$\frac{\partial \overline{u_j} \overline{\rho } \overline{h}}{\partial x_j}+\frac{\partial \overline{\rho } \overline{{u_j}^{\prime }{h}^{\prime }}}{\partial x_j}=-[\frac{\partial \overline{u_j} \overline{{\rho }^{\prime }{h}^{\prime }}}{\partial x_j}+\frac{\partial }{\partial x_j}\left(\overline{{\rho }^{\prime }{u_j}^{\prime }} \overline{h}+\overline{{\rho }^{\prime }{u_j}^{\prime }{h}^{\prime }}\right)]+{\overline{S}}_h,$$

(3)

where $\rho$ is the gas density, kg/m³; $\overline{\rho }$ is the Reynolds mean density; $x_i$ are the coordinates of the fluid in direction $i$; $u_i$ is the velocity of the fluid in direction i, m/s; $x_j$ are the coordinates of the fluid in the $j$ direction; $u_j$ is the velocity of the fluid in the $j$ direction, $\mathrm{m}/\mathrm{s}$; $\overline{u_i}$, ${\overline{u}}_j$ are the Reynolds mean velocities; $\overline{{u_i}^{\prime }{u_j}^{\prime }}$ is the Reynolds mean additional stress tensor; $\overline{p}$ is the Reynolds mean pressure, $\mathrm{P}\mathrm{a}$; ${\delta }_{ij}$ is the Kronecker delta; ${\mu }^b$ is the bulk viscosity of the same order as $\mu$; $\overline{f_i}$ is the Reynolds mean volume force, $\mathrm{N}$; $\overline{h}$ is the Reynolds mean specific enthalpy, $\mathrm{J}/\mathrm{k}\mathrm{g}$; ${\overline{S}}_h$ is the Reynolds mean of the heat release per unit of the cell fuel combustion, W/m³.

In the methane combustion process, the chemical reaction time is very short compared to the convection and diffusion times of the gas species, meaning that the time–spatial scale of combustion is much smaller than that of the turbulent flow. To describe the reaction process and calculate flow scalar terms, such as the mass fraction and temperature of each component, we adopted the non-premixed diabatic steady-state, small flame model. This model is suitable for describing turbulence–chemistry interactions and predicting various gas emissions. Combustion occurs within progressively thin layers embedded in turbulence with well-defined internal structures, known as small flames [32]. The model assumes that in turbulent combustion, the micro-clusters on the flame surface are composed of a large number of very thin small flames. The turbulent flame field is obtained by averaging the characteristics of these small flames, using statistical laws.

The flow field parameters are obtained by utilizing data from the flame surface database, specifically the mixing fraction f and the scalar dissipation rate χ. The Lewis number (Le) is a dimensionless number that represents the ratio of the thermal diffusion coefficient to the mass diffusion coefficient, used to describe the relative magnitude of heat and mass transfer in convective processes. In this work, it is assumed that the heat and mass transfer in the flow process are of the same magnitude, hence the Lewis number is defined as 1. The equation describing the steady-state flame surface is expressed as:

$$\frac{1}{2}\rho \chi \frac{{\partial }^2{Y}_i}{\partial f^2}+S_i=0,$$

(4)

$$\frac{1}{2}\rho \chi \frac{{\partial }^{2}T}{\partial f^2}-\frac{1}{c_p}\Sigma H_i^{*}{S}_i+\frac{1}{2c_p}\rho \chi \frac{\partial c_p}{\partial f}\frac{\partial T}{\partial f}=0,$$

(5)

where $Y_i$ is the mass fraction of the i component; T is the temperature of the i component; $\rho$ is the density of component i; $f$ is the mixed fraction of the i component; $c_p$ is the average specific heat of the mixture; $S_i$ is the reaction rate of the i component; $H_i^{*}$ is the specific enthalpy of component i; $\chi$ is the scalar dissipation rate.

The mixture fraction is expressed as:

$$f=\frac{b-b_{ox}}{b_{fuel}-b_{ox}},$$

(6)

$$b=2\frac{Y_c}{M_{w,c}}+\frac{Y_H}{2M_{w,H}}-\frac{Y_o}{M_{w,o}},$$

(7)

where $Y_c$, $Y_H$, and $Y_O$ are the mass fractions of carbon, hydrogen, and oxygen; $M_{w,c}$, $M_{w,H}$, and $M_{W,O}$ are the molecular weights of carbon, hydrogen, and oxygen; $b_{fuel}$ and $b_{ox}$ are the exit parameters of the fuel side and oxidizer side. For the boundary conditions of the oxidant inlet, the mixing fraction $f$ is 0. For the boundary conditions of the fuel inlet, the mixture fraction $f$ is 1.

The scalar dissipation rate χ is defined as:

$$\chi =2D{\left|\nabla f\right|}^2,$$

(8)

where D is the corresponding diffusion coefficient.

The relationship between the mixing fraction f and the scalar dissipation rate χ is:

$$\chi =\frac{a_s\mathit{exp}(-2{\left[erf{c}^{-1}\left(2f\right)\right]}^2}{\pi },$$

(9)

where $a_s$ is the characteristic strain rate; $erf{c}^{-1}$ is the inverse of the complementary error function $erfc$.

The reaction rate $S_i$ in Equation (5) is expressed as:

$$S_{i,r}=\mathsf{\Gamma }{\sum }_{j=1}^N\left({\nu }_{i,r}^{″}-{\nu }_{i,r}^{\prime }\right)\left(k_{f,r}{\prod }_{j=1}^N{\left[C_{j,r}\right]}^{{\eta }_{j,r}^{\prime }}-k_{b,r}{\prod }_{j=1}^N{\left[C_{j,r}\right]}^{{\nu }_{i,r}^{″}}\right),$$

(10)

where ${\nu }_{i,r}^{\prime }$ is the stoichiometric number of the reactant of component i in the reaction r; ${\nu }_{i,r}^{″}$ is the stoichiometric number of the product of component i in the reaction r; ${\eta }_{j,r}^{\prime }$ is the reaction rate of the reactant of component i in r; $C_{j,r}$ is the molar concentration of component i; $\mathsf{\Gamma }$ is the effect of the third body on the reaction rate.

The reaction rate constant is translated into the Arrhenius formula:

$$k_{f,r}=A_r{T}^{{\beta }_r}{e}^{-E_r/RT},$$

(11)

where $A_r$ is the pre-exponential factor of reaction r; ${\beta }_r$ is the temperature index of reaction r; $E_r$ is the activation energy of reaction r; R is the molar gas constant, 8.314 J/(mol·K); T is the thermodynamic temperature.

The chemical reaction mechanism used in this work involves simplifying the detailed mechanism of methane combustion (GRI-Mech 3.0 mechanism) using the direct relationship diagram method, coupled error propagation, and sensitivity analysis. This process results in a simplified reaction mechanism with 23 components and 110 steps. Validation is performed using a fully stirred reactor model and a one-dimensional laminar flow, premixed reactor model. The temperature and component distributions predicted by the simplified mechanism closely match the predictions of the detailed mechanism, confirming the validity of the simplified mechanism.

3.2. Turbulence Model

To describe the turbulence flow regime of the gas, the realizable k-ε two-equation model is selected. This model has also been adopted by many researchers for simulations of the turbulent combustion of gas fuels [33,34]. The turbulent stress term is shown in Equations (12) and (13). The turbulent viscosity is determined by solving the turbulent kinetic energy k equation and the turbulent dissipation rate ε equation [31]:

$$\overline{u_j}\frac{\partial k}{\partial x_j}=\frac{\partial }{\partial x_j}(\frac{{\nu }_t}{{\sigma }_k}\cdot \frac{\partial k}{\partial x_j})+P_k-\epsilon ,$$

(12)

$$\overline{u_j}\frac{\partial \epsilon }{\partial x_j}=\frac{\partial }{\partial x_j}(\frac{{\nu }_t}{{\sigma }_{\epsilon }}\cdot \frac{\partial \epsilon }{\partial x_j})+\frac{\epsilon }{k}(C_{\epsilon 1}{P}_k-C_{\epsilon 2}\epsilon ),$$

(13)

where ${\overline{u}}_j$ is the Reynolds mean velocity; $x_j$ are the coordinates of the fluid in the $i$ direction; ${\nu }_t$ is the turbulence viscosity; $P_k$ is the rate of transfer (or production) of kinetic energy from the mean to the turbulent motion; $C_{\epsilon 1}$, $C_{\epsilon 2}$, ${\mathsf{\sigma }}_{\mathrm{k}}$, and ${\sigma }_{\epsilon }$ are empirical parameters, $C_{\epsilon 1}=1.44$, $C_{\epsilon 2}$= 1.92, ${\mathsf{\sigma }}_{\mathrm{k}}$= 1.0, and ${\sigma }_{\epsilon }=1.3$.

3.3. Radiation Model

The gray body DO radiation model is used in the simulation. The mathematical expression is as follows:

$$\frac{d\left(I_{si}\right)}{d{x}_i}=-(\gamma +{\sigma }_s)I(\overrightarrow{r},\overrightarrow{s})+\gamma n^2\frac{\sigma T^4}{\pi }+\frac{{\sigma }_s}{4\pi }{\int }_0^{4\pi }I(\overrightarrow{r},{\overrightarrow{s}}^{\prime })\Phi (\overrightarrow{s},{\overrightarrow{s}}^{\prime })d{\Omega }^{\prime },$$

(14)

where $\gamma$ is the absorption coefficient; ${\sigma }_{\mathrm{s}}$ is the scattering coefficient; $\overrightarrow{r}$ is the position vector; $\overrightarrow{s}$ is the direction vector; $\overrightarrow{s}$ is the scattering direction vector; $\sigma$ is the Stefan–Boltzmann constant, $\sigma$ = 5.672 × 10⁻⁸ W/(m²·K⁴); n is the refraction coefficient; I is the total radiation intensity; T is the temperature; ${\Omega }^{\prime }$ is a solid angle; $\Phi$ is a phase function, representing the spatial distribution of inward scattering.

3.4. Boundary Conditions and Solution Method

The air inlet is configured as a velocity inlet, with a hydraulic diameter of 276 mm, and a temperature of 493 K. The fuel gas inlet is also set as a velocity inlet, with a hydraulic diameter of 41.52 mm, and a temperature of 300 K. The flue gas outlet is designated as a pressure outlet, with a reflux temperature of 298 K, and a turbulence intensity of 5%. For the walls, a constant temperature of 300 K is maintained. The angle of the swirl blade is set to 60°. Ansys Fluent is used for the simulation. The SIMPLE algorithm is employed for the coupling of velocity and pressure. The governing equations are discretized using a second-order upwind scheme, which is selected for its robustness and straightforward algorithmic implementation [35,36]. The convergence criteria are set to 10⁻⁶ for energy equations and 10⁻³ for other equations. Stability and convergence are indicated by observing minimal changes in the monitored quantities. Once the monitored quantity remains nearly constant, it signifies that the numerical solution is stable, and convergence has been achieved.

3.5. Grid Independence Test

Figure 2 shows the grid distribution for the gas burner. The grids in the nozzles and inlet area have been refined. The inlet area of the burner is divided using a refined unstructured mesh, while the remaining part is divided using a structured mesh. An O-type grid is used for the grid division, due to the cylindrical shape of the chamber.

To ensure grid independence, the number of grid cells is gradually increased. Five different grid schemes containing 0.57 million, 0.83 million, 1.17 million, 1.27 million, and 1.37 million cells are generated. Under certain working conditions, the axial velocity and temperature distributions along the center axis of the combustion chamber, calculated from these five different grid schemes, are compared and analyzed. Figure 3 shows that the differences between the simulation results for 0.57 million, 0.83 million, and 1.17 million cells are significant, while the differences between the results for 1.17 million, 1.27 million, and 1.37 million cells are relatively small. This indicates that further increasing the number of grid cells has little effect on the flow and reaction fields. Considering computational efficiency and accuracy, the grid scheme with 1.17 million cells is selected for further research.

3.6. Simulation Conditions

As shown in Table 1, five working conditions, with varying numbers of fuel nozzles and inclination angles of the fuel nozzles, are simulated. The excess air coefficient is 1.05. Condition 1 is set as the reference condition, with a thermal load of 40 t/h.

4. Model Validation

Due to the lack of experimental data, the pilot axisymmetric burner model studied by Christoph Schneider et al. [37] at the Technical University of Darmstadt is selected to verify the feasibility of the numerical method presented in this paper. As shown in Figure 4a, the piloted, axisymmetric burner has a main jet diameter of d = 7.2 mm and a pipe length exceeding 40 d. The diameter of the annular pilot is 18.2 mm, consisting of 72 tiny, premixed jets that create a homogeneous annular distribution of temperature and gas composition. To obtain accurate simulation results, the model’s reliability is verified by comparing the simulation results with the experimental data. Figure 4b shows the comparison of the experimental and numerical temperature distributions along the axis. The axial temperature initially increases, reaches a peak value of 1990 K at an axial distance of 0.35 m, and then decreases as the axial distance increases. The simulation results are in good agreement with the experimental data in most areas, indicating that the numerical model established can accurately simulate the inverse diffusion combustion process of natural gas.

5. Results and Discussion

5.1. Flow Structure

Condition 1 in Table 1 is set as the reference condition to study the detailed flow and flame structure in the swirling, inverse diffusion gas burner.

Figure 5 illustrates the flow structure in the swirling, inverse diffusion gas burner. Velocity is symmetrically distributed about the central axis. The swirling jet exhibits both axial and significant tangential velocities. Consequently, the initial disturbance of the flow is pronounced. Streamlines reveal the presence of recirculation zones near the air inlet and in the near-wall region, referred to as the central recirculation zone and external recirculation zone, respectively, in Figure 5. The central recirculation zone is primarily formed due to the swirling flow of air. The inlet air velocity, being approximately half of the inlet fuel velocity, restricts the formation of the recirculation zone near the root wall of the swirling blade at the entrance. The development of the central recirculation zone is further constrained by the distribution of the fuel flow, preventing its extension to the near-wall area. This zone continuously entrains high-temperature flue gas to heat the inlet gas and enhance the mixing of air and CH₄. On the other hand, the external recirculation zone is formed by two opposite gas flows: one moving axially towards the burner outlet and the other moving back. This zone entrains the surrounding high-temperature flue gas from the outer boundary of the high-speed gas flow, effectively utilizing the high-temperature flue gas near the wall to heat the mixed gas near the gas inlet and promote combustion. In traditional swirl diffusion combustion, the gas velocity is generally lower than that of the central air, leading to the formation of a central recirculation zone, while a large external recirculation zone, as depicted in Figure 5, is not typically observed. Consequently, compared to traditional swirl diffusion combustion, the higher fuel inlet velocity in the swirling, inverse diffusion burner generates a larger external recirculation zone, which is more conducive to heating the mixed gas and improving combustion efficiency.

The distribution of tangential velocity reflects the swirl intensity of the gas. Figure 6a illustrates the tangential velocity distributions in six different cross-sections. It is observed that the tangential velocity reaches a minimum value at the center of the burner, with this minimum value decreasing as the distance to the outlet increases. Additionally, as the distance to the exit increases, the maximum tangential velocity gradually decreases, and the peak value shifts towards the wall. At cross-sections of Z = 0.5 m, Z = 1 m, Z = 1.5 m, and Z = 2 m, the tangential velocity exhibits two peaks within the radial distance between 0.1 m and 0.2 m, with a maximum tangential velocity of −27 m/s. This phenomenon arises due to the high-speed expulsion of fuel gas from the nozzle, resulting in the formation of a central recirculation zone, as depicted in Figure 6b. By comparing the tangential velocity distributions at cross-sections of Z = 0.5 m, Z = 1 m, Z = 1.5 m, and Z = 2 m, it is evident that the tangential velocity gradually decreases with increasing axial distance, indicating the gradual dissipation of the swirl. In cross-sections Z = 4 m and Z = 6 m, the tangential velocity is relatively small, with values close to zero at the center, indicating the disappearance of the swirl effect near the chamber outlet. Furthermore, with increasing radial distance, the tangential velocity reaches its peak value near R = 0.8 m, with values of −4 m/s and −2.7 m/s, respectively, and gradually decreases to zero due to the wall constraints. This signifies the disappearance of the influence of external recirculation zones.

5.2. Flame Structure and Thermal Characteristics

The temperature contour of the flame in Figure 7 reveals a symmetrical temperature distribution about the Z axis, with a maximum temperature of approximately 1914 K. The swirling IDF exhibits a three-part structure: a base flame, a flame neck, and a flame torch. The high-temperature region is concentrated in the burner head and tail areas, near the central axis. The presence of two high-temperature zones, symmetrically, about the central axis at the burner head, with temperatures around 1900 K, is attributed to the rolling action of the external recirculation zone. Additionally, a high-temperature zone at the head of the combustion chamber arises due to the heating of the air by the recirculating gas, elevating the temperature to about 1800 K. The high-speed fuel gas entering the combustion chamber induces a pressure gradient on the central recirculation zone, resulting in incomplete mixing of fuel and air. Consequently, the reaction primarily occurs in the middle and bottom sections of the combustion chamber, where the temperature reaches approximately 1900 K. Examining the temperature profile along the central axis in Figure 7, it is evident that the flame temperature gradually increases as the axial distance at Z = 3 m increases. At the tail of the combustion chamber, the influence of swirling flow diminishes, accompanied by a gradual reduction in the jet velocity. Consequently, under the influence of wall cooling, the flame temperature decreases.

5.3. Species Concentration Distributions

To gain a more comprehensive understanding of the flame structure, the distributions of the species concentrations are investigated, and the results are depicted in Figure 8.

The methane contours in Figure 8a reveal a swift mixing of CH₄ with air, followed by combustion over a short distance. Any remaining CH₄ is predominantly concentrated near the fuel nozzle at R = 0.3 m. Towards the end of the chamber, the methane content diminishes significantly, indicating near-complete fuel combustion. Meanwhile, as depicted in Figure 8b, water vapor (H₂O), a byproduct of CH₄ combustion, is predominantly concentrated in the intense combustion region, with a peak molar fraction of 0.18. With increasing distance from the burner inlet, diffusion intensifies, and the reactions become more pronounced, resulting in a notable increase in water vapor concentration towards the end of the chamber. Notably, H₂O is absent in the chamber’s center, suggesting that no CH₄–air reactions occur in this region. This absence could be attributed to two factors: (1) insufficient momentum of the fuel gas to reach the chamber’s center due to swirling; (2) rapid reaction rates leading to complete fuel combustion before reaching the chamber’s center.

Figure 9 illustrates the contour of the NO volume concentration and the NO volume concentration profile along the central axis. The concentration of NO exhibits a characteristic trend of initially increasing and then decreasing along the axis, peaking near Z = 7 m at approximately 386 ppm. Notably, the concentration of NO is lower in the cooler region near the head of the combustion chamber, attributed to the incomplete mixing of gas and air in this area. Conversely, in the high-temperature region at the chamber head, recirculated flue gas mixes with fuel and oxygen, leading to reduced oxygen content, which mitigates the formation of certain thermal NO. At a distance of approximately 0.4 m from the wall, the NO concentration is notably higher compared to other locations, indicative of a flame front where substantial thermal NO generation occurs. Subsequently, as a result of the cooling effect exerted by the combustion chamber wall, the temperature is reduced, and NO production diminishes.

5.4. Influence of the Inclination Angle of the Fuel Nozzles

The outlet of the fuel nozzle is designed as an elliptical incision, facilitating the uniform injection of gas into the combustion chamber. The primary purpose of the elliptical incision is to alter the direction of the inlet fuel gas. As the gas traverses the inclined portion, its inertia prompts a shift towards the center, consequently causing the flame to converge towards the central axis. Therefore, to investigate the effects of the structural parameter, specifically the inclination angle of the elliptical incision, conditions 3, 4, and 5 in Table 1 delineate specific parameter settings for this purpose.

Figure 10 illustrates the impact of the inclination angle of the fuel nozzle on the distribution of air and CH₄ streamlines. With an inclination angle of 60°, the air and CH₄ streamlines are more uniformly distributed. Initially, the swirling air causes a portion of CH₄ to flow at high velocity, while the remainder diffuses outward at a slower swirl. In contrast, at 20° and 40° inclination angles, the uniformity of the air and CH₄ distribution is compromised. Smaller inclination angles prevent CH₄ from gathering internally and mixing effectively with the air. Additionally, the fast CH₄ flow causes the air to diffuse outward prematurely, hindering efficient mixing with CH₄ internally.

As shown by the axial velocity contours in Figure 11, when the inclination angles of the fuel nozzles are 20° and 40°, the regions of higher axial velocity shift closer to the wall, compared to an angle of 60°. This displacement prevents the mixed gas from gathering internally, hindering internal reactions and potentially causing wall-sticking combustion and instability. Preliminary analysis suggests that reducing the nozzle inclination angle is detrimental to combustion stability, indicating that the optimal inclination angle of the fuel nozzles is 60°, in the given conditions.

Figure 12 shows the temperature contours and the temperature profile of the central axis. When the fuel nozzle inclination angle is 40° or 20°, the temperature distribution is less uniform compared to an inclination angle of 60°. The flame structure also differs significantly. Additionally, a high-temperature region forms near the wall due to high-speed airflow. From the temperature distribution along the central axis, it is evident that an inclination angle of 60° produces a smooth curve with an overall upward trend and a slight decrease at the burner outlet. In contrast, when the nozzle inclination is 40° or 20°, the temperature variations are more erratic, with larger fluctuations. This increased fluctuation is due to the non-uniform temperature distribution at these smaller inclination angles.

As shown in Figure 13, the CO₂ concentration in the combustion chamber gradually decreases as the fuel nozzle inclination angle decreases. When the nozzle inclination angle is set to 40° or 20°, the CO₂ distribution becomes less uniform. This indicates that reducing the fuel nozzle inclination is detrimental to the stability of methane combustion.

As shown in Figure 14 and Table 2, when the fuel nozzle inclination angles are 40° and 20°, the NO concentration at the combustion chamber outlet reaches 303.45 mg/m³ and 222.68 mg/m³, which is due to the high combustion outlet temperature.

As shown in Table 3, when the fuel nozzle inclination is 40° and 20°, the methane concentration at the combustion chamber outlet is 0.029 and 0.039, respectively, which is higher than that with the inclination angle of 60°. This indicates incomplete methane combustion under these settings, further proving that a smaller nozzle inclination angle is not conducive to efficient combustion.

5.5. Influence of the Number of Fuel Nozzles

Given that the number of nozzles affects the distribution of the inlet fuel, this section studies the influence of the number of fuel nozzles on combustion efficiency. The specific parameter settings are shown in regard to running conditions 1, 2, and 5, in Table 1.

Figure 15 illustrates the effects of the number of fuel nozzles on the distribution of air and CH₄ streamlines. The air streamlines show that increasing the number of fuel nozzles influences the accumulation of air in the front section of the burner. With more fuel nozzles, air becomes more centralized along the axis. This centralization helps trap CH₄ and enhances the mixing of air and CH₄. Regarding the CH₄ streamlines, with eight fuel nozzles, CH₄ tends to distribute in the center. For 12 and 16 nozzles, the middle section also sees denser mixing, with 16 nozzles showing the highest density, indicating better conditions for methane accumulation.

Comparing the axial velocity contours in Figure 16, it can be observed that as the number of fuel nozzles increases, the high-speed area gradually elongates. This elongation helps reduce the high-temperature zone in the front section of the combustion chamber. Thus, it can be preliminarily concluded that with 16 nozzles, the mixture of CH₄ and air before the middle section of the burner is more optimal, promoting stable combustion in the middle and rear sections.

Figure 17 shows the effects of the number of fuel nozzles on the temperature contours and the temperature profile along the central axis. From the temperature contours, it is evident that increasing the number of burner nozzles does not significantly alter the overall flame structure. With 8 and 12 fuel nozzles, the flame is longer, and combustion is primarily concentrated at the tail of the combustion chamber, resulting in a higher outlet temperature compared to the 16-nozzle configuration. This higher temperature may lead to excessive NO emissions at the outlet. Additionally, with 12 nozzles, the longer flame and increased number of nozzles compared to eight nozzles result in more intense combustion, extending the high-temperature area to the tail and causing the highest burner outlet temperature under these conditions. In contrast, with 16 fuel nozzles, the combustion chamber’s outlet temperature is lower than in other configurations. This is because the full combustion area is farther from the outlet, indicating better mixing of fuel and air in this configuration.

Figure 18 and Table 4 show the concentration of NO in the combustion chamber and at the outlet, respectively. It can be observed that as the number of fuel nozzles increases, the NO concentration at the outlet of the combustion chamber gradually decreases. This decrease is due to a reduction in the high-temperature area at the end of the combustion chamber, which is consistent with the temperature distribution within the chamber. With 8 and 12 fuel nozzles, the NO concentration at the outlet is higher. This is attributed to the poor mixing of methane and air, resulting in combustion primarily occurring in the tail area of the combustion chamber and creating an excessively large high-temperature zone. Conversely, with 16 fuel nozzles, the NO concentration at the combustion chamber outlet is the lowest, measured at 81.56 mg/m³. Compared with the reference condition of 114 mg/m³, the NO emissions decreased by 28.5%.

6. Conclusions

In this work, we designed a novel gas burner that combines air swirl and an inverse diffusion flame (IDF) for industrial applications. Numerical simulations based on the RANS method and simplified reaction mechanisms are conducted to predict the turbulent flow and reaction performance of the burner. This study examines the influence of the number and inclination angle of the fuel nozzles on the flow field and combustion characteristics. The main conclusions are as follows:

(1)

The swirl action of the burner creates a central recirculation zone and two external recirculation zones at the burner head. These zones stabilize combustion by heating the mixed gas through the entrainment of high-temperature flue gas. The tangential velocity is minimal at the center of the burner, with this minimal value decreasing as the distance from the outlet increases. As the distance to the exit increases, the maximum tangential velocity gradually decreases, and the peak value shifts towards the wall. The effect of the swirl disappears near the chamber outlet. The tangential velocity reaches its peak near R = 0.8 m with increasing radial distance and, then, gradually decreases to zero due to the wall constraints, indicating that the influence of the external recirculation zones has dissipated;

(2)

The swirling IDF exhibits a three-part structure consisting of a base flame, flame neck, and flame torch. The methane content reaches zero at the end of the chamber, indicating almost complete fuel combustion. H₂O, a product of CH₄ combustion, is predominantly distributed in the intense combustion area, with a maximum molar fraction of about 0.18, under the reference condition. The concentration of NO initially increases along the axis, peaking at around Z = 7 m, with a maximum value of approximately 386 ppm, and then decreases;

(3)

Improvements to the burner structure reveal that altering the number of fuel nozzles more effectively reduces NO_X emissions than changing the fuel nozzle inclination. With 16 fuel nozzles and a nozzle inclination angle of 60°, the NO emissions at the outlet are reduced from 114 mg/m³ under reference conditions to 81.56 mg/m³, a decrease of 28.5%.