CFD simulation study of a biomass pellet-fuelled boiler

Biomass energy is an important substitute for fossil energy. Direct combustion of biomass in the boiler has the problem of high emissions. In this paper, a 0.1 t/h biomass atmospheric pressure hot water boiler is used for CFD modeling, aiming at providing a low-cost and high-efficiency way for the study of biomass boilers. In this paper, the biomass pyrolysis process is divided into three processes: water evaporation, devolatilization, and coke combustion. Using the UDF function combined with a porous medium model to write code, the gas-solid combustion process in the boiler is realized, and the grate is used to split the air. The calculation results show that the model can accurately restore the temperature, velocity, and composition changes in the boiler. Compared with the actual results, the temperature difference between the furnace and the outlet is less than 20 K, and the modeling has achieved good results.


Introduction
Energy is the material basis of human survival.At present, the world energy supply is still mainly dependent on coal, oil, and natural gas.But fossil energy is limited, and exploitation and use damage the ecological environment [1] .It is becoming urgent to find alternative renewable energy sources to reform the energy system.Compared with traditional fossil energy, biomass energy is not only renewable and has zero carbon emissions but is also rich in resources and widely distributed, which is known as one of the most promising green renewable energies in the 21st century [2] .Using a straw, rice husk, wood chips, and other biomass materials by machine compression made of a directly burning biomass briquette fuel can solve this problem.In addition, there are abundant raw materials, high thermal efficiency, good combustion performance, easy-to-achieve industrialization, and other advantages [3] .However, the operation of biomass boilers releases large amounts of pollutants into the air, which is easy to cause serious air pollution and haze, and other disastrous weather.Numerous researchers have previously investigated emission reduction technologies for biomass boilers, but experimenting with boiler emission technologies takes a long time and entails huge economic costs.
Computational fluid dynamics (CFD), as an important numerical simulation method that can guide the design and improvement of practical biomass boilers, has been adopted in much research in recent years [4,5] .Zhou et al. used CFD to model the combustion of biomass in a fixed-bed burner in one dimension.They investigated the effect of parameter settings such as temperature and thermal conductivity on the simulation results [6] .However, the one-dimensional combustion model is too limited, so it is more meaningful to create a full-size three-dimensional combustion model.In this study, the porous medium model and C language were combined to simulate the combustion of biomass pellet fuel, and a full-size three-dimensional CFD combustion model was established.The purpose is to build an accurate combustion model of a small biomass fuel boiler, which can be used in the design and improvement of a small biomass fuel boiler.

Research object
The fuel used in this study is a pellet fuel made from straw as the main raw material, with a density of 1.21 kg/m 3 and a low calorific value of 13.93 kJ/kg.The industrial analysis and elemental analysis are shown in Table 1 [7] .The prototype of the boiler used in this study is a 0.1 t/h double-return domestic biomass pellet fuel heating boiler, which belongs to the automatic feed type fixed grate boiler.Figure 1 shows the physical model of the boiler, whose furnace size is 1400*1000*2000 mm.It has a fixed grate of 1400 mm*1000 mm with 66 air holes of size 300*6 mm evenly distributed for air supply and ash discharge.The boiler is not a continuous feed boiler.The combustion of biomass in the boiler presents periodicity.

Bed solid phase model
In this study, the entire combustion zone is considered continuous, with the fuel laid flat above the grate and set as a porous medium and the rest of the zone set in the gas phase.In this study, the whole combustion zone is considered to be continuous.The inertia resistance and viscous resistance of the porous media model were calculated by the Ergun formula (Eq.1), where ε is the porosity of the porous media region, its value is 0.5, and D p is the average particle diameter. α= The solid phase part of the reaction consists of drying, release, and combustion of volatile fractions and combustion of coke [8] .The energy transfer and component changes contained in the process are imported into the model in the form of a UDF as a source term for the porous media region, and the rate is determined by the Arrhenius equation (Eq.2).
κ i =Ae^(-E i /RT) (Eq.2) where i is the component type; κ is the rate constant; R is the molar gas constant; T is the thermodynamic temperature; E i is the apparent activation energy; A is the pre-exponential factor (also known as the frequency factor).

Gas phase model
The Fluent Transient Solver and Segregated Solver were used to solve the problem.The standard κ -ε turbulence model is selected as the viscosity model, the standard wall function is selected as wall flow treatment, and the DO model is selected as the radiation model.And the Species Transport / Eddy-Dissipation Concept Model was selected for component transport, which means that the chemical reaction rate is infinite compared with the turbulent mixing (diffusion) rate.The calculation method is set as follows: the second-order upwind scheme is selected as the discrete method, PRESTO is selected as the pressure interpolation format, and the SIMPLE algorithm is used to couple pressure and velocity.

Boundary conditions and initial conditions
In the boundary setting of the model, the wall is an adiabatic boundary condition.The wall of the watercooled pipe is a temperature boundary condition.The inlet is speed inlet, and the component is air, and the temperature is equal to 300.15 K.The outlet of flue gas is a pressure outlet with a gauge pressure of -50 Pa.The standard initialization is used for initialization, the patch function is used for ignition, and the ignition temperature is 1500.15K.

Boiler temperature distribution
Figure 2 shows the temperature distribution of the boiler center section with different time steps.At t=3 s, as the cold air continues to pass through the porous medium zone into the furnace, the water in the fuel begins to absorb heat and precipitate out.The temperature in the fuel zone drops from 1500 K ignition temperature to about 1000 K, and the local temperature in the chamber exceeds 1500 K, which is because the excessively high ignition temperature speeds up the devolatilization process of the fuel.The gas flow through the fuel zone will bring many volatiles into the furnace and burn quickly.The effect of high ignition temperature lasted until 20 s, and the temperature in the furnace remained in a stable range after t=21 s, indicating that the heat conduction process and combustion process in the fuel zone tended to be stable.After t=27 s, the fuel temperature is kept at 700-800 K, and the temperature in the chamber is also kept at 800-1100 K, and the combustion enters the stable stage.It is of practical significance to select the calculation result data at t=33 s for the subsequent calculation.To verify the accuracy of the model, the study compared the simulation results with actual boiler test data from a combustion performance test done by Jilin University on a biomass pellet fuel combustion plant [9] .Firstly, the temperature of the boiler chamber was compared.As shown in Figure 3, the temperature of the flue gas at the exit of the boiler as a result of the simulation is not much different from the actual one.In the middle of the chamber, the actual result is also higher than the simulation result by more than 30 K.This is because, in reality, the test results of the boiler are influenced by various factors such as air temperature, air humidity, local atmospheric pressure and the dryness of the fuel layer.In contrast, the simulation results are calculated under absolutely ideal conditions.However, in the bed fuel zone, the simulated temperature is higher than the actual one by about 50 K.This is due to the fact that the simulation uses a finite rate combustion model where volatilization will complete the reaction with air in a very short period of time after detachment from the solid fuel.

Boiler flow field distribution
Figure 4 shows the flow field distribution in the central section of the boiler.It can be seen that the airflow enters the boiler high speed from the air inlet and then decreases in speed under the blocking diversion effect of the grate, and then enters the bed uniformly through the grated aperture.Due to the increase in temperature and the addition of gases from combustion, the velocity of the gas stream leaving the fuel zone will be greater than the velocity on entry.The gas flow forms a large reflux zone in the center due to the different velocities of the different gas apertures entering the chamber and the blockage of the inner walls of the boiler.In the reflux area, the high-temperature flue gas above the combustion chamber is sucked into the lower part of the combustion chamber for the reignition reaction, thus forming a high-temperature area in the center of the combustion chamber, corresponding to the temperature distribution in Figure 2. The formation of a high-temperature zone, although beneficial for increasing the fuel burn-up rate and reducing the unburned component at the boiler exit location, leads to an uneven temperature distribution throughout the combustion chamber, affecting the boiler's thermal efficiency.The results for each time step show that at t=3 s, the airflow distribution within the combustion chamber is very non-uniform, which is related to the instability of the model at the beginning of the calculation.After t=27 s, the airflow distribution stabilizes.

Gas component distribution
Figure 5 shows the composition distribution in the vertical section of the boiler.It can be seen that CH 4  and H 2 are mainly distributed near the bed due to their fast combustion rate.However, the volume fraction of CH 4 is greater than the volume fraction of H 2 , which is related to the characteristics of the biomass fuel during pyrolysis [10] .And the distribution of CO is not uniform, with the CO concentration on the left side of the chamber being significantly lower than on the right side.This is due to the creation of a reflux zone in the chamber resulting in a greater air inflow on the left side than on the right side, resulting in more CO from incomplete combustion of the coke on the right side.In addition, the calculations show that the volume fraction of CO at the outlet is less than 0.001, which proves that the combustion in the furnace chamber is adequate.

Conclusion
In this study, the pyrolysis process of biomass pellet fuel was written in C++.The CFD model of a smallscale biomass-forming fuel boiler was established by using the UDF function to implement gas-solid combustion in FLUENT software.In terms of the model, a large air inlet was used to make use of the splitting effect of the grate to make the air enter the furnace chamber uniformly, which is closer to the actual situation.
The simulation results show that the small biomass boiler model can accurately simulate the flow and combustion process in the furnace.The simulation results were compared with the experimental results, and it was found that the difference in temperature in the furnace chamber and at the outlet was not significant.At the bed location, the simulation results were slightly higher than the actual test results due to the finite rate model taken, but overall, the model was successful.The reliability of the model can be used not only to analyze the combustion performance of the boiler but also to study the pollutant emission characteristics of the boiler by using the low-cost feature of CFD simulation.

Figure 1 .
Figure 1.Geometric model of a biomass boiler.

Figure 2 .
Figure 2. Temperature distribution on the center cross section.

Figure 3 .
Figure 3. Furnace temperature comparison between simulation and test data.

Figure 4 .
Figure 4. Flow field distribution on the center section.

Figure 5 .
Figure 5. Gas fraction in the longitudinal section of the boiler.

Table 1 .
Ultimate analysis and proximate analysis of tested biomass