Noé－Landry－Privace M’Bouana，F(xiàn)ei－Xiang Zhao，Qing－Hong Zhang，Hui－Lin Lu

(School of Energy Science and Engineering，Harbin Institute of Technology，Harbin 150001，China)

1 Introduction

Their geometrical simplicity， their relative economy in power and their flexibility with respect to high temperature and pressure explain their suitability in industrial deducting.The cyclone separator is a key component in the operation of the circulating fluidized bed(CFB)boiler，which has great effects on the combustion efficiency，the circulation rate and the desulfurization efficiency，by the circulation of the solid particles of the furnace.The traditional circular crosssection cyclone was commonly used as a conventional cyclone separatorforthe CFB boiler.With the development of large CFB boilers，the huge body of the conventional cyclone became a majorshortcoming because of the thick refractory wall that leads to the requirement for a long period to start the boiler.

Compared with the traditionalcircularcrosssection cyclone，a square cyclone has many advantages over the conventional cyclone，due to the convenience in construction，easier membrane wall arrangement，shorter start-stop time，and easy integration with the boiler［1］.

Several experimental investigations and numerical simulations have been made to improve the square cyclone’s performances.Among these，Darling［2］reported that the Ahlstrom Pyropower Company developed a square water-cooled cyclone separator with upward exhaust exit for high temperature separation and applied it to its compact CFB boiler design.Other authors reported the applications such as a separator in a commercial CFB boiler［3］.A water-cooled square cyclone separator and its application to CFB boiler design have been developed and patented successfully in China［4］.Su and Mao［5］investigated another type of water-cooled square cyclone separator by PDA experiment，which places the gas exhaust at the bottom of the separator instead of at the top.According to the experimental results of Zhao et al.［6］，circular crosssection cyclone separators with direct symmetrical spiral inlets have higher performance than that of cyclones with a conventional tangential single inlet.The research results demonstrated that both design and operating parameters influenced the efficiency and pressure drop of cyclone.Zhao et al.［6］and Lim et al.［7］also found by experimental study that double inlets could improve the separation efficiency while decreasing the pressure drop of the traditional circular cyclone separator.

Other authors found that the shape and structure of a cyclone determine its performance.The effect of the cylinder shape and size influenced the shape of the core-annularinterface inside the cyclone wasstudied numerically by Lee et al.［8］，which determined the overall flow and collection characteristics caused by these condition.Bernado et al.［9］calculated by CFD method the effect of inlet section angles in relation to the cyclonebodyon the separation efficiency of cyclones.They found that the efficiency of cyclones is improved when the inlet section angle is 45°compared with the normal inlet.Qian et al.［10］performed an experimental and numericalstudy ofa prolonged cyclone with an attached vertical tube at the bottom of the dust outlet and found that the length of the vertical tube influenced the efficiency and pressure drop.A type of square cyclone separator with downward-exhaust exit was developed by Qiu［11］et al.Its separation efficiency was shown to be as good as that of the traditional cyclone of circular cross-section separator and its particle cut-diameter was around 15 μm.All of the above mentioned researches results indicate that the square cyclone separator used in CFB boilers have high collection efficiency.However，the present contribution aims to add more to the existing knowledge on the function of square cyclones which represents one of the most recent applications of the technique of separation by centrifugal force.

CFD has a great potential to predict the flow field characteristicsand particle trajectories inside the cyclone as well as the pressure drop［12］.The complicated swirling turbulent flow in a cyclone places great demand on the numerical techniques and the turbulence models employed in the CFD codes.CFD has been widely used to investigate flow field inside conventional cyclones. Raoufi et al.［13］used computational fluid dynamics to simulate and optimize vortex of conventional cyclones.Although many numerical works have been conducted on conventional cyclones，there are few numerical studies of square cyclones.

As numerical investigations of square cyclones have an important role in the better understand of their flow parameters，this study is intended to obtain detailed flow information by CFD simulation within square cyclones in the case of downward gas-exit without a vortex.The square cyclones are modeled at different flow rates and flow fields are evaluated inside these square cyclones.Contours of pressure profiles and solid volume fraction within the cyclone are shown.Tangential velocity components profiles in different sections and different inlet flow are also investigated.

2 Task Formulation and Numerical Method

2.1 Geometry of Cyclone

Traditional cyclone separators have a circular cross section and a tangential or helical inlet and have been widely studied by many authors both experimentally and numerically［1，6］.

Fig.1 shows the geometry and dimension(unit m) of the square cyclone used in the studied cases，which is close to that of Shams et al.［14］.As seen in the cyclone separator model，which has a square crosssection，square body without vortex finder a rectangular inlet connected to the cyclone body and cylindrical downward gas-exit.

Fig.1 Geometry and generated mesh of square cyclone

The tetrahedral computational grids were generated by using GAMBIT grid generator.The grid independence study has been performed forthe cyclone.Three levels of grid have been tested，to be sure that the obtained results are not grid dependent.Three levels of mesh 99681，118298，129922 and 128298 cells have been used.As shown in Fig.2，the grid with 99681 cells gives a hight axial velocity near the inlet and a low axial velocity close at the bottom in the axial direction，while the grid with 118298 and 129922 show the same trends in the axial direction.Thus，for excluding any uncertaintly，the computations have been performed by using 118298 cells grid.

2.2 Description of Numerical Model

2.2.1 Selection of turbulence model

For the turbulent flow in cyclones，the key to success of Computational Fluid Dynamic(CFD)lies with the accurate description of the turbulent behavior［12］.To model the swirling turbulent flow in a cyclone separator，there are a number of turbulence models available in Fluent.They range from the standard k－ε model to more complicated Reynolds stress turbulence model(RSM).Also large eddy simulation(LES)methodology is available as an alternative to the Reynoldsaverage Navier-Stokes approach.

Fig.2 Axial velocity of gas distribution alont z-axial direction at the three different grid sizes

Many researchers have investigated the selection of a suitable turbulence model for the highly swirling flows within a cyclone.The standard k－ε，RNG k－ε and Realizable k－ε models were not optimized for strongly swirling flows found in conventional cyclone separators［15－16］.Both the standard k－ε and RNG kε turbulence model give unrealistic distribution for the axial velocity profiles(upward flow close to the wall)［17－18］.Only the Reynolds stress turbulence model (RSM)is capable of predicting the combined vortex in accordance with the experimental data.The successful application of the RSM turbulence model for different studies in cyclone separators has been reported by many researchers［6，15－16，19－21］.

However，the RNG k－ε godel and RSM are selected as turbulent model to simulation gas-solid twophase flow in square cyclone separator.

2.2.2 Model of gas－solid two phases flow

Flows in cyclone separators are multiphase.The flow in square cyclone in this study consists of gas and solid particles.Two phase flows can be solved by a number of CFD techniques.They include the Eulerian Approach，the simplified Eulerian approaches and the Lagrangian approach.In this study，the inlet solid volume fractions are 0.1 and 0.01 corresponding to a high dispersed phase concentration and therefore a dense two-phase flow regime.In the case of the dense regime，interparticles becomes of importance，both physical collisions and indirect influence through the nearby flow field，also limitations related to computer storage，calculation times and convergence arise.In those cases，the Eulerian-Eulerian approach，where a set of continuity，momentum and turbulence equations for each phase are established，therefore it becomes more adequate.

The conservation and transport equations for phase q are as follows:

with the phases’volume fraction summing up toand the effective density of phase q isαqρq.where the subscript q is gas phase(g)or solid phase(s);α is the volume fraction;ρ is the physical density of phase q;uqis the velocity vector of phase q; p is the pressure;τ is the stress tensor;g is the gavity vector and Kqpis the momentum exchange coefficient.

In Eq.(2)the Reynolds stress tensor，the interphase momentum exchange as well as the granular pressure and the granularviscosity need further modeling.A granular pressure and a granular viscosity are deduced from kinecic gas theory［22］:

and

Granularpressure and granularviscosity are depend on the radial distribution g0function and granular temperature Θs

where therrightterm ofEq.(4)describethe production ofgranular，its diffusion as wellas dissipation due to collisions and inter-phase energy exchange.The details of the modeling are once given by Gidapow［22］.

The momentum exchange between the continuous gas phase and particle phase in Eq.(2)is modeled by Syamlal et al.［23］has the form

where dsis diameter of particle，the drag function CDhas a form and the terminal velocity correlation for solid phase:

where the coefficient A and B in Eq.(5)are further detail by Syamlal and O’Brien［19，23］.

3 Results and Discussion

The simulations are performed for the square cyclone.As indicated in Fig.1，the exhaust gas through a downward exit open to the air，and the surrounding pressure is at 1 atm.The particlulate material has a density and diameter of 2400 kg/m3and 0.150 mm respectively is used.The simulations are performed at inlet velocity of 14，18，20，22，24 and 28 m/s and at a solid inlet volume fraction of 0.1，and 0.01.

3.1 Validation of Numerical Model

In order to validate the obtained results，it is necessary to compare the prediction with experiemental data. The comparison performed with the experimentally measurments of Su and Mao［5］and CFD model of Shams et al.［14］The present simulations are compared with the measured and CFD simulation of z－velocity distribution at the cross-section located at 0.7 m from the bottom of cyclone as shown in Fig.3.The presentsimulation matches the experimental velocity profil with overestimation of the z－velocity in left side ofcyclone，and underestimation ofthe z－velocity in right side.Considering the complexity of the turbulent swirling flow in the square，the agreement between the present simulation and measurements is considere to be quite acceptable.

Fig.3 Comparison of the z-velocity of the model in this paper with Ref.［5］and Ref.［14］

3.2 Comparison of Turbulence Model

3.2.1 Velocity Distribution

The velocities vectors of gas and particle phase at cyclone cross-section z=0.85 m are showns in Figs.4 and 5 for RNG k－ε and RSM model respectively.For both two model the gas-solid flow enters the square cyclone at inlet velocity and directly impinges on the corner wall facing the inlet.There is an eddy at the corner facing the inlet.The flow turns its direction sharply and the particles impact the wall strongly.Some of the impacting particles rebound from the corner wall and are carried away by the gas flow.Some of them are deposited and fall down along corner surface.The energy of the flow is dissipated at the corner.

Fig.4 Velocity vector at the cross section at z=0.85 m with RNG k-ε model

Fig.5 Velocity vector at the cross section at z=0.85 m with RSM model

3.2.2 Pressure fields

The first CFD simulation of cyclone was performed about 20 years ago［24－28］by using the finite element method.It was the first to detect that the standard k－ε turbulent model was not able to accurately simulate this kind of flow.In this part the comparative studies of two turbulence models，the Reynolds Stress Model(RSM) and a variation ofthe k － ε modelbased on Renormalization Group(RNG)was evaluated.The simulations were compared with pressure field.fields

Figs.6 and 7 show the profiles of pressure drop and static pressure respectively.It shows that the pressure drop increases with the increase of inlet velocity and a slight increase in pressure of the RSM model compared to the RNG k－ε model in Fig.6.

It shows the profile of static pressure according to the height of cyclone at part of cyclone H=0.60 m in Fig.7.The results show thatthe airflow causes depression as a swirl at the center of cyclone，similar to the conventional cyclone.Also the static pressure decreases radial from wall to axis of the cyclone and the pressure is increased for the RSM model near the walls.The contours of static pressure give a clear illustration of these phenomenons in Fig.8.Although the pressure distribution shows acceptable agreement for all models，the RSM gives a higher-pressure drop compared to the RNG k－ε model.

Fig.6 Profile of pressure drop

Fig.7 Profile of static pressure in x-coordinate

Fig.8 Contour of static pressure with two different turbulence models at x-plane of cyclone

3.2.3 Solid volume fraction

The simulation results show that the particle volume fraction increases and reaches annular bed condition instantly after startup under the action of gravitational force.

Fig.9 present the profile of particlevolume fraction for RSM and RNG k－ε model at H=0.65 m height of cyclone along the x－radial direction.The results show that particle concentration along the radial direction of cyclone can be divided into two regions: the central region of the cyclone area with low particle concentration and the wall region with high particle concentration.The gas and particle flow to the wall，leading to increased particle concentration near the wall of cyclone.Fig.10 shows the particle volume fraction at the xz－plan section ofcyclone forallturbulence models，moreover these figures show that volume fraction distribution is not symmetrical.

Fig.9 Profile of solid volume fraction with x-coordinate

Fig.10 Contour plot of solid volume fraction at x-plane of cyclone

3.2.4 Separation efficiency

In addition to pressure drop，separation efficiency is also considered an important parameter in the evaluation cyclone performance.Generally，an increase in inlet velocity will increase the separation efficiency of the cyclone，and this will also increase the pressure drop.As shown in Fig.6，the pressure drop increases with the inlet velocity.Fig.11 shows the comparative measured separation efficiency of the square cyclone as a function of inlet velocities compared to the results of Yu el al.［29］and Zhao et al.［6］for a conventional cyclone.As can be seen in Fig.11，the influence of inlet velocity on separation efficiency for dense particle concentration is apparent.In a conventional cyclone it is usually expected that an increase in inlet velocity will increase separation efficiency.This has been found by both experimental and numerical studies to be the case by Zhao et al.［6］and Yu et al.［29］.The results presented here demonstrate that with an increase in inlet velocity a square cyclone willhave an increased separation efficiency in a similar manner to a conventional cyclone.The results presented here also demonstrate that the collection effcinecy ofthe square cyclone differs depending on the model used.The collection efficiency of a cyclone modeled with the RSM model is higher than that modeled with RNG k－ε.

Fig.11 Separation efficiency of the cyclone at different inlet velocity

3.3 Effect of Solid Concentration on Square Cyclones

The following section examines simulations perform in two cases:case 1 with solid volume fraction 0.01 and case 2 with volume fraction 0.1.Only the RSM turbulence model is used in this part.

3.3.1 Flow fields

Experimental measurements of the velocities in square cyclone separator without a vortex finder do not exist to validate the velocity prediction at present，but the predicted velocity field is seen to be similar to the conventional cyclone separators.Only the tangential velocity components are presented here sincethe contour of the velocity magnitude within the cyclone are almost identicalwith those oftangentialvelocity.Additionally within the cyclone the tangential velocity is the dominant velocity component.It should be noted that the tangential velocity distribution inside a square cyclone basically agrees with the rotational flow that consists of inner forced and outer free vortexes.In this part the tangential velocity is investigated in the differentheights of cyclone and different inlet velocities.

Fig.12 presents the tangential velocities for different inletvelocitiesforcase 1 and case 2 respectively.The results show that the tangential velocity magnitude increases by increasing the inlet velocity and the value of tangential velocity equals zero on the walland atthe centerofthe cyclone.Additionally，for all cases the tangentialvelocity distributions are not symmetrical.

Fig.12 Gas tangential velocities with different inlet velocities

Fig.13 shows the profiles of the tangential velocity along the radial orientation at different heights of cyclone for all cases.For different volume fractions the tangential profiles show that inside the square cyclone the swirling flow consist of an outer free vortex and inner forced vortex close to center，these results are seen to be similar to those in conventional cyclones.Moreover，in the inner region the tangential velocity is relatively similar at different heights of square cyclone for both two cases.The tangential velocity distribution in the outer region is rather similar at different height of square cyclone for case 1 and is completely different for the case 2.Note that increases of solid inlet volume also effect the tangential velocity distribution.

Fig.13 Gas tangential velocity with different section of cyclone

3.3.2 Pressure fields

One of the most important parameters in the investigation of cyclone performance is the pressure drop in the cyclone.Figs.14(a)and 14(b)present the radial profiles of static pressure at H=600 mm from the bottom of cyclone for cases 1 and 2，respectively.The static pressure shows the low pressure zone in the center of the cyclone for each inlet velocity.

The result shows that the static pressure decreases radially from wall to axis of the square cyclone. Moreover，the results show that case 2 gives higher static pressure compared to case 1.

The comparison between pressures drops of the square cyclone in two cases are presented in Fig.15 respectively(a)with solid volume fraction 0.01 and (b)with solid volume fraction 0.1.The pressure drop increases with the increased inlet velocity and case 2 gives a higher-pressure drop compared to case 1.The pressure drop increases proportionally with inlet solid volume fraction.

Fig.14 Profile of static pressure

Fig.15 Profile of pressure drop with different inlet velocity

4 Conclusions

A numerical simulation by CFD，based on the Reynolds Stress Model(RSM)and RNG k－ε model was use to study the flow in square cyclone separators with a downward gas-exit.The comparison of the results given by tangential velocity component，pressure fields and volume fraction can describe the turbulent flow within a square cyclone.The tangential velocity profiles show that inside the square cyclone the swirling flow consist of an outer free vortex and inner forced vortex close to center.These results are similar to those seen in a conventional cyclone.Additionally，this study indicates thatthe pressure drop and separation efficiency increase with increasing inlet velocities for both the Reynolds stress model and the RNG k－ε model.Moreover，the Reynolds stress model gives a higher-pressure drop distribution and high separation efficiency compared to the RNG k－ε model.The Reynolds stress model provides well for the forced vortex and free vortex，and the lower pressure in center of square cyclone is seen to be similar to that of a conventional cyclone.Moreover，comparison of the pressure drop for two cases in a square cyclone show that the pressure increases considerably by increasing the solid volume fraction.However these numerical simulations results have to be validating in future work by the experimental.

［1］Sommerfeld M，Ho C H.Numerical calculation of particle transportin turbulent wall bounded flows.Powder Technology，2003，131(1):1－6.

［2］Darling S L.Pyroflow compact:the next generation CFB boiler.Proceedings of the 1995 International Joint Power Generation Conference.Minneapolis.1995，1:403－412.

［3］Makkonen P.Foster wheeler，CFB with the new INTREXTMsuperheated.VGB Power Technology，2000，80:30－34.

［4］Lu J，Zhang J，Zhang H，et al.Performance evaluation of a 220t/h CFB boiler with water-cooled square cyclones.Fuel Process.Technol.，2007，88(2):129－135.

［5］ Su Y，Mao Y.Experimental study on the gas-solid suspension flow in a square cyclone separator.Chemical Engineering Journal，2006，121(1):51－58.

［6］Zhao B，Shen H，Kang Y.Development of a symmetrical spiral inlet to improve cyclone separator performance.Powder Technol.，2004，145(1):47－50.

［7］Lim K S，Kwon S B，Lee K W.Characteristics of the collection efficiency for a double inlet cyclone with clean air.Journal of Aerosol Science，2003，34(8):1085－1095.

［8］Lee J W，Yang H J，Lee D Y.Effect of the cylinder shape of a long-coned cyclone on the stable flow-field establishment.Powder Technol.，2006，165(1):30－38.

［9］Bernado S，Mori M，Peres A P，et al.3－D computational fluid dynamics for gas and particle flows in a cyclone with different inlet section angles.Powder Technology，2006，162(3):190－200.

［10］Qian F P，Zhang J G，Zhang M Y.Effects of the prolonged vertical tube on the separation performance of a cyclone.Journal of Hazardous Materials，2006，136(3):822－829.

［11］Qiu K Z，Yan J H，Li X D，et al.Experimental study and structure optimization of a uniflow square shaped cyclone separator.Journal of Engineering for Thermal Energy and Power，1999，14(3):193－194.

［12］Griffiths W D，Boysan F.Computational fluid dynamics (CFD)and empirical modeling of the performance of a number of cyclone samplers.Journal of Aerosol Science，1996，27(2):281－304.

［13］Raoufi A，Shams M，F(xiàn)arzaneh M，et al.Numerical simulation and optimization of fluid flow in cyclone vortex finder.Chemical Engineering and Processing，2008，47(1):128－137.

［14］Raoufi A，Shams M，Kanani H.CFD analysis of flow field in square cyclones.Powder Technology，2009，191(3):349－357.

［15］Chuah T G，Gimbun J，Choong T S.A CFD study of the effect of cone dimension on sampling aerocylones performance and hydrodynamics.PowderTechnology，2006，162(2):126－132.

［16］Wan G J，Sun G G，Xue X H，et al.Solids concentration simulation of different size particles in cyclones separators.Powder Technology，2008，183(1):94－104.

［17］Hoekstra A J.Gas Flow Field and Collection Efficiency of Cyclone Separators.Delft:Delft University of Technology，2000.

［18］Kaya F，Karagoz I.Performance analysis of numerical schemes in highly swirling turbulent flows in cyclones.Current Science，2008，94(10):1273－1278.

［19］Xiang R B，Lee K W.Numerical study of flow field in cyclones of different height. Chemical Engineering Processing:Process Intensification，2005，44(8):877－883.

［20］Zhao B，Su Y，Zhang J.Simulation of gas flow pattern and separation efficiency in cyclone with conventional single and spiral double inlet configuration.Chemical Engineering Research and Design，2006，84(12):1158－1165.

［21］Gimbun J，Chuah T G，Choong T S Y，et al.A CFD study on the prediction of cyclone collection efficiency.International Journal for Computational Methods in Engineering Science and Mechanics，2005，6(3):161－168.

［22］Gidsapow D.Multiphase Flow and Fluidization.San Diego: Academic Press，1994.

［23］Syamlal M，O’Brien T J.Computer simulation of bubbles in a fluidized bed.AIChE Symp Ser，1989，85(27):22－31.

［24］Choudhury D.Introduction to the Renormalization Group Methodand TurbulentModeling.New York:Fluent Incorporated，1993.

［25］Hu L Y，Zhou L X，Zhang J，et al.Studies on strongly swirling flows in a full space of a volute cyclone separator.AIChE Journal，2005，51(3):740－749.

［26］Wilcox D C.Turbulence modeling for CFD.La Canada: DCW Industries inc.，1998，2:103－217.

［27］Hinds W C.Properties Behavior and Measurement of Airborne Particles，Aerosol Technology.Manhattan:John Wiley and Sons，2012.

［28］Boysan F，Swithenbank J，Ayers W H.Mathematical modeling ofgas-particle flows in cyclone separators.Encyclopedia of Fluid Mechanics，1986，4:1307－1329.

［29］Wang B，Xu D L，Chu K W，et al.Numerical study of gas—solid flow in a cyclone separator. Applied Mathematical Modelling，2006，30(11):1326－1342.