Numerical and experimental analyses of a stirred vessel for a large volumetric flow rate of sparged air

Laboratory for Fluid Dynamics and Thermodynamics,Faculty of Mechanical Engineering,University of Ljubljana,A?ker?eva 6,1000 Ljubljana,Slovenia

Keywords:Mixing Stirred vessel Aeration Multiple stirrer High gassing rate Local void fraction

ABSTRACT Computational fluid dynamics(CFD)and experimental analyses of some of the basic characteristics of air sparging in a tall stirred vessel equipped with a three-stage impeller are presented.The impeller was assembled from a radial ABT impeller as the lower,a turbine 6PBT45 as the middle and an axial Scaba-type 3SHP1 impeller as the upper.All the impellers were of the same diameter,i.e.,225 mm,while the vessel diameter was 450 mm.The impeller's rotational speed was 178 r·min-1.The aeration regime was established with an air volumetric flow rate of 28.3 m3·h-1.To the best of our knowledge,this study is the first to consider the very high gassing rate by means of CFD in a tank stirred by three-stage axial/radial impellers.The numerical simulation was performed using the ANSYS Fluent(R17.2,2016)code for solving the governing equations of fluid dynamics in single-and multi-phase systems.While discussing the bubble size distribution,a discrete population balance model(PBM)was used.Adopting CFD,the stirring power and the total void fraction(the total gas holdup)were calculated.The results were in good agreement with the measured values using a laboratory experimental device.

1.Introduction

Stirred reactors with concurrent aeration are used extensively in various branches of the process industry.In this regard,the mixing vessel can be equipped with a variety of impellers that provide an axial,radial or combined discharge stream.Axial impellers are used primarily for suspending solid particles.In the case of gas-liquid dispersion,in general radial impellers are applied.Most of the available data on radial impellers were obtained by studying the Rushton turbine,which provides good mixing performance and gas dispersion based on a singleimpeller configuration.A standard tank configuration(STC)[1,2]is normally used to enable a comparison of mixing characteristics,e.g.,mixing power[3],mixing time[4-7]or gas-filled cavity structures and the appearance of flooding[8,9].Flooding phenomena studied using different methods in a STC[8,10]make it possible to determine the effective twophase flow regimes in which the characterization of the other impeller types is needed,e.g.,a double-disk impeller[5],asymmetric blade-disk impeller[11,12],different types of hollow-blade impeller[13],hydrofoil impellers[14]or various blade profiles of a disk impeller[15].All these implementations are designed to perform as efficiently as possible the homogenization,uniform gas distribution,low power consumption,high gas holdup,mass and heat transfer,etc.When a large amount of gas is to be dispersed,a tall mixing vessel equipped with a multi-stage impeller is the most often used.In such a configuration,highly nonhomogeneous conditions can appear,especially in large tanks.Due to a lack of detailed knowledge of fluid dynamics,a primary influence on the variety of mixing parameters is studied:how to handle large quantities of air,having good homogenization without flooding,significant power loss(or insufficiently mixing)or severe torque fluctuations.For these purposes in multi-stage assemblies,different impeller types were combined,such as multiple Rushton turbines[7,16-22],multiple pitched-blade turbines[23],multiple hydrofoil impellers[24-27],multiple counter-current-flow impellers[28,29]or the configuration of radial and axial impellers[18-20,30-32].Nowadays,the last of these prevails due to improved mixing characteristics,larger gas holdup,lower mixing power,more uniform void-fraction distribution with a stable two-phase flow regime and have almost entirely replaced the multiple Rushton impellers used in the past[22,33-35].

In recent years,many numerical studies of stirred reactors(e.g.,the flow induced by various impellers)in the homogenization of Newtonian fluids[26,28,29,36-38]and pseudo-plastic fluids[39,40],the performance of turbulence models in gas-liquid flow[21,37,41-44],the prediction of mixing time[5,44-49],gas-phase distribution[46,50-53],and stirring power[5,39,43,54-56]have been published,following the development of available computational resources and advances in computational fluid dynamics—CFD.CFD provides the most detailed visualization of complex three-dimensional flow structures in stirred vessels.The accuracy of CFD predictions is very much governed by the computational mesh,in combination with an appropriate choice of the turbulence model[43],the initial and boundary conditions,and the modeling approach.However,to successfully run industrial-scale devices and to validate the numerical simulations,an experimental investigation of the hydrodynamic conditions is still indispensable.

This study is an experimental and CFD analysis of water mixing and concurrent aeration.A three-stage impeller(radial ABT,turbine 6PBT45 and axial Scaba-type 3SHP1,from the bottom to the top,respectively)was installed concentrically in a tall,cylindrical,mixing vessel filled with tap water.All the impellers had a diameter of 225 mm.The rotational speed was 178 r·min-1(Fr=0.2).The volumetric flow rate of the sparged air was 28.3 m3·h-1(Fl=0.23).Coupling the CFD with discrete population balance modeling(PBM),the stirring power and the total void fraction(total gas holdup)were calculated.The results were in good agreement with the experimental data obtained from measurements on a laboratory experimental device.In addition,the liquid velocity fields,the local void fraction during aeration,and the distribution of the bubble size were also studied.

2.Material and Methods

2.1.Experiment

The three-stage impeller was employed for the simultaneous stirring and liquid aeration.A radial disk impeller with asymmetric blades(ABT),a pitched blade turbine impeller with six blades at a 45°pitch angle(6PBT45),and a three-blade hydrofoil impeller(Scaba-type 3SHP1),all with a 225-mm diameter(D),were installed concentrically in a tall,cylindrical,flat-bottomed vessel,from the vessel's bottom to the top,respectively.The ABT impeller allows for the dispersion of large volumetric flow rates of gas[11,12]the 6PBT45 impeller disperses and circulates the gas[2,23],and the Scaba-type 3SHP1 impeller induces liquid circulation over a wide range of viscosities[57].The distance between the adjacent impellers was 280 mm.The vessel of 450 mm in diameter(T)was filled with tap water to a height(H)of 910 mm.To prevent bulk rotation of the liquid,four baffles of width T/12 were equidistantly mounted perpendicular to the vessel's wall with a gap of T/60.The ring sparger of diameter T/3 and the bottom impeller were installed 75 mm and 150 mm above the bottom of the vessel,respectively.On the lower side of the ring sparger 68 injector holes with a diameter of 3 mm were made.Dry compressed air taken from an in-house supply line was filtered and set to a constant pressure.The volumetric gas flow rate was measured and controlled by a rotameter with an error of±0.4 m3·h-1.A pressure gauge was installed behind the flow meter to allow for a flow-rate correction.The mixing shaft was powered by a frequency-modulated,5-kW electric motor.The impeller's rotational speed was measured with an IR-pulse transmitter that has an absolute error of±1 min-1.A HBM transducer with a measurement range of 10 N?m was used to measure the torque with an accuracy of±0.02 N?m.The voltage readings of all the meters were recorded using NI DAQ and LabVIEW software and stored for future analysis.The experimental setup is shown in Fig.1.A detailed description of the instruments used,the accuracy,and the repeatability of the measured variables are detailed in[5,8,17,58].

The local void fraction(α)was measured using a single microresistivity(R)probe that was designed to detect the electrical impedance change.Its response was further discriminated into a voidfraction value based on the discrimination procedures[8,10,58,59].Every single local void-fraction measurement took 180 s at a sampling rate of 5000 Hz.The relative reproducibility error of the void fraction was smaller than 4%.The R probe was placed on a special traversal mechanism consisting of an R-probe-holder slider and a baffle.This assembly enabled local void-fraction measurements at different heights for a fixed radius of 157.5 mm with steps of 10 mm in the height of the impeller placement,otherwise 20 mm.

The total gas hold-up measurements were made with an improved three-point“level taker”,shown in Fig.1,which was based originally on the change of the height of the liquid level at only one location.With such an arrangement,the water level in the measuring cylinder was more stable than in the case of the single-point measurement.The averaged relative reproducibility error was less than 5%,based on at least 20 measurements for this hydrodynamic regime.

2.2.Computational fluid dynamics(CFD)analysis

2.2.1.Geometrical model and computational mesh

The geometrical model of the laboratory experimental device presented in Fig.2(vessel of height 1500 mm,multi-stage impeller,sparger ring,baffles)was created in SolidWorks(Dassault Systèmes SolidWorks Corp.).Spatial discretization of the three-dimensional fluid domain was made in ANSYS ICEM CFD(R17.2,2016).Finally,the unstructured tetrahedral mesh was converted to a polyhedral mesh in ANSYS Fluent(R17.2,2016).The mesh consisted of approximately 800 k cells in a stationary computational domain.The rotating part of the domain was divided into three regions,each including a different impeller.The ABT,6PBT45,and Scaba-type 3SHP1 regions consisted of approximately 391 k,204 k,and 150 k computational cells,respectively.The overall number of computational cells was comparable to that(0.6 M to 2 M computational cells)of previous CFD studies[5,54].As in the work by Kerdouss et al.[50],the average size of the computational cells was approximately 1%of the vessel's diameter.On the other hand,the agreement between the CFD results and our laboratory measurements was good,as could be concluded from Section 3.2.Therefore,we have great confidence that our mesh resolution was sufficient to accurately simulate the complex two-phase flow in a stirred aerated vessel.

2.2.2.Governing equations

The two-phase flow(air-water dispersion)in the stirred aerated vessel was modeled using an Eulerian model,following numerous reports[5,36,41,53,54,60-62]in the literature.The continuity and momentum equations for the phase q are given by(Eqs.(1)and(2)),respectively.

uq,iis the velocity of the phase q in the i coordinate direction,xiis a position vector component,p is the pressure,and t is the time.ρqrepresents the density,and μqis the dynamic viscosity of the phase q.Fq,iis the body force and αqrepresents the volume fraction of the phase q.The subscripts i and j are the spatial position indexes.

The population balance model(PBM)was adopted to consider the size distribution of the bubbles.The PBM theory is detailed in[63].A literature review[50,52,53,64]revealed that when the bubbles are small the PBM predictions correlate well with the experimental data.

The impeller rotational speed(n)of 178 r·min-1leads to an estimated impeller Reynolds number,

Fig.1.Experimental setup.

Fig.2.Geometrical model of laboratory experimental device.(a)Stationary domain.Rotating domains;(b)Scaba 3SHP1 impeller,(c)6PBT45 impeller,(d)ABT impeller.

Hence,the flow in the stirred vessel is turbulent.In this work,the Standard k-ε mixture turbulence model with scalable wall functions was used to provide the turbulence closure.The model is robust and has been frequently used[65-67]to solve multiphase turbulent flows in stirred tanks.Furthermore,it is fast and stable(also when the gas void fraction in the two-phase mixture is large)and gives reasonable results for the most turbulent flows,especially for large Reynolds numbers[41].The standard k-ε mixture turbulence model solves two additional equations for the turbulence kinetic energy(k),

and its rate of dissipation(ε),

The density of the mixture is computed from

The mixture velocity is defined as

The turbulent viscosity μt,mis defined as

where the constant Cμ=0.09.The default values of the other model constants are as follows:σk=1.0,C1ε=1.44,C2ε=1.92.Gk,mrepresents the generation of the turbulence kinetic energy due to the mean velocity gradients.

2.2.3.Boundary and operating conditions

The rotational speed of the multi-stage impeller was 178 r·min-1(Fr=0.2).A gauge pressure of 0 Pa was prescribed at the outlet(far field)of the computational domain.The volumetric flow rate of the sparged air was 28.3 m3·h-1(Fl=0.23).At the sparger,the size of the bubbles was assumed to be in the seventh size bin(i.e.,3.17 mm)of the discrete PBM.This class was chosen because its size was the closest to the diameter of the sparger holes.A non-slip boundary condition was applied at the walls.Initially,the height of the water in the vessel was 910 mm.The acceleration due to gravity was taken as 9.81 m·s-2.

The density and dynamic viscosity of the water were 998.2 kg·m-3and 1.003×10-3Pa·s,respectively.The air density was 1.225 kg·m-3.The air's dynamic viscosity was 1.7894×10-5Pa·s.

2.2.4.Solver settings and calculation procedure

The governing equations describing the fluid motion were discretized and solved in ANSYS Fluent(R17.2,2016).To provide an initial condition for the start-up of the two-phase simulation,the mixing in the single-phase flow was solved using the multiple reference frame(MRF)approach[68].The MRF technique was previously used in multiple studies[5,54,60,62,69]relating to stirring due to its reasonable accuracy and its fast computational and turnaround times.In this first step of the simulation,the water surface level was considered to be stationary.

Next,the unsteady simulation of the simultaneous stirring and the liquid aeration was conducted by employing the sliding-mesh technique.The dispersed two-phase flow was modeled using the Eulerian model coupled with a discrete population balance model(PBM)to consider the size distribution of the bubbles.The Phase Coupled SIMPLE algorithm was applied to solve the pressure-velocity linked equations.A second-order upwind scheme was used to discretize the convective terms in the momentum equations.The convective terms in all the other equations(i.e.,turbulence,volume fraction,PBM)were discretized using a first-order upwind scheme.The least-squares,cellbased,gradient-evaluation scheme was used to calculate the gradients.Temporal discretization was employed using the first-order implicit scheme and a time step of 0.001 s.The interphase drag force between the dispersed and continuous phases was modeled using the drag coefficient of Schiller&Naumann[70].As in similar studies[65,71],the turbulent dispersion force was neglected,as was the lift force,the virtual mass force,and the wall-lubrication force.No mass interchange between the gas and liquid phases was assumed.For the breakup of the bubbles,the breakage kernel proposed by Luo and Svendsen[72]was used.The breakage formulation for the discrete population balance modeling was based on the Hagesather method.The reason for choosing the Hagesather over the Ramkrishna formulation was the lower computational cost,as fewer integration points were used.The bubbles-aggregation rate was calculated using the Luo model(e.g.,see[63]).The size of the bubbles was assumed to be distributed across 13 classes between 1 mm and 16 mm,as listed in Table 1.The upper size limit was set based on the observed bubbles'coalescence in the experiment.On the other hand,the number of classes was still small enough for the calculation to be within acceptable computational resources.

High-performance computing(HPC)was utilized on a Prelog cluster at the Faculty of Mechanical Engineering,University of Ljubljana.The calculation for 15 s of the unsteady two-phase flow took approximately five days when the calculation was run on 72 processor(Intel Xeon X5670)cores.

3.Results and Discussion

The results presented herein are the outcome of the numerical simulation(subscript CFD)considering the mixing in single-(subscript 1P)and two-phase(subscript 2P)flows.Adopting CFD,predictions for the torque,stirring power,local void fraction,total gas holdup,and bubble size distribution during aeration were made.Qualitative information obtained from the three-dimensional,flow-field prediction was essential to visualize the potential stagnation regions in the stirred aerated vessel[60,64,73].The subscript exp denotes the results obtained with a laboratory experiment.

3.1.Single-phase stirring

In the first step the single-phase stirring was considered to initialize the CFD simulation of the stirring with concurrent aeration.The results were compared to those obtained by experiment in order to validate the mesh prior to the two-phase flow modeling and simulation.

3.1.1.Stirring power in water mixing

The power drawn by the impeller is defined as,

where ω represents the angular velocity and T is the torque.This torque is a sum of the torques due to the pressure(FP)and the viscous(FV)fluid forces on the impellers(ABT,6PBT45,Scaba-type 3SHP1)and the shaft,

Table 1 Size distribution of bubbles

rABrepresents the position vector from the centre of the rotation(A)to the location of the force application(B).Furthermore,the stirring power can be characterized using the Power number,

In water mixing the torque was 3.12 N?m,implying a stirring power(PCFD,1P)of 58.24 W for the impeller's rotational speed of 178 r·min-1.The Power number based on the CFD prediction was PoCFD,1P=3.87.The Power number of Poexp,1P=3.62 was calculated when considering the laboratory experimental device with the same configuration and under the same operating conditions.The relative percentage difference(PoCFD,1P-Poexp,1P)/Poexp,1Pof 6.9%confirms the generated mesh and our numerical experiment are appropriate.In general,if the difference between the experiment and the CFD is less than 10%,the numerical results are rated with the highest grade and considered to be acceptable[74].

3.1.2.Local flow characteristics in water mixing

The liquid flow field in the stirred vessel represented by the velocity vectors in the vertical mid-plane between the baffles(γ=45°)is shown in Fig.3a.The azimuthal location of the plane is shown in Fig.3b.The discharge stream from the bottom(ABT)impeller in the radial direction towards the vessel's wall is clearly seen.Adjacent to the wall,the stream deflects and two circulation regions are formed,above and below the plane of the impeller.The former interacts strongly with the outflow from the middle(6PBT4)impeller,oriented about 45° downwards with respect to the horizontal direction.The flow near the wall is divided into two.The stream that is deflected downwards represents the circulation region below the impeller plane.The other stream turns upwards and enters the inflow region of the upper impeller.Alongside the shaft,the downflow with the associated circulation is induced by the middle and upper(Scaba-type 3SHP1)impellers.

3.2.Two-phase(air-water dispersion)stirring

3.2.1.Stirring power in aeration

Using(Eq.(10)),the torque in the two-phase stirring for the impeller rotational speed of 178 r·min-1and the volumetric flow rate of sparged air equal to 28.3 m3·h-1was predicted.The torque of(2.85±0.18)N?m was calculated,averaging between the 15th and the 25th seconds of the developed flow.Hence,the stirring power in the aeration(PCFD,2P)was(53.11±3.47)W.The Power number based on the CFD prediction was PoCFD,2P=3.53±0.23.The power draw measured for the laboratory stirring device(with the same configuration and operating conditions)was Pexp,2P=(46.80±0.89)W(Poexp,2P=3.11±0.06),where the relative percentage difference(εP)between the averaged CFD and the experimental data was 13.5%.By definition,it was calculated as(PoCFD,2P-Poexp,2P)/Poexp,2P?100%.The power ratio was PCFD,2P/PCFD,1P=0.91.This suggests that the stirring power was decreased by 9%,compared to the singlephase stirring.The pumping capacity of the considered three-stage impeller was retained very well,despite the large volumetric flow rate of the sparged air.Therefore,the decrease in power draw was as small as expected.The power ratio when using the three-stage Rushton impeller under the same operating conditions would be approximately 0.65.However,in this configuration the bottom impeller(and probably the middle one as well)would be flooded[17]and therefore the effectiveness of the stirring would decrease.

Fig.3.Water velocity field(a)in the stirred vessel in the vertical mid-plane between the baffles;γ=45°.(b)Azimuthal location of the vertical mid-plane.

3.2.2.Total gas holdup and local void fraction

The total void fraction(total gas holdup)was calculated using the difference in water-level heights,αCFD/exp=(Hg-H)/Hg,where Hgis the liquid level in the dispersed regime.Considering the experimental data,the total gas holdup measured on the laboratory experimental device operating in the same regime(Fr=0.2,Fl=0.23)was αexp=10.35%.The numerically predicted total gas holdup was αCFD=9.0%,yielding a relative percentage difference of-13% between the CFD and the experiment.The lower total gas holdup(compared to the experimental data)assessed in the CFD simulations suggests that the bubbles predicted in the regions of coalescence were too large.Applying additional corrections related to the numerical parameters,we expect to be able to predict a more accurate size distribution of the bubbles in the numerical studies.Consequently,a better match between the CFD results and the experimentally determined total gas holdup will be obtained.

The local void fraction of the air-water,two-phase flow in the vessel's vertical mid-plane between the baffles(γ=45°)is shown in Fig.4a.The water velocity in the stirred vessel represented by contours and vectors in the vertical mid-plane between the baffles(γ=45°)is shown in Fig.4b.All three impellers dispersed the flow as expected.The influence of the gas phase was dominant in between the middle and the upper impellers where the flow field was greatly altered compared to the single-phase case(see Fig.3a).The velocity vectors of the liquid phase coincided with the direction of the buoyancy lift when the local void fraction was large.In contrast,the liquid inertia governed the mixing if the local void fraction was small.

After the injection the air penetrated into the region affected by the bottom impeller.Due to the asymmetrically formed blades,the mixture discharge stream was strongly affected in the radial direction towards the vessel's wall.Adjacent to the wall,the stream deflected and two circulation regions were formed above and below the impeller plane.The large differences in the flow development were found in the region bounded by the plane of the middle and upper impellers.As discussed,the gas phase governed the local flow conditions in the zone.The airwater dispersion entered the upper impeller from below and departed from it almost radially,towards the vessel's wall.

A quantitative comparison(for the same monitoring points at r=157.5 mm,γ=45°)between the CFD and the experimental results on the local void fraction is shown in Fig.5.It is clear that the numerical results were lower than the experimental measurements.One of the reasons could be that the predicted bubble sizes in the regions of coalescence were too large.The large bubbles were due to buoyancy lift,released adjacent the shaft,thus decreasing the local void fraction in the other(i.e.,inertial dominant)regions of the stirred vessel.However,the height-wise profiles of the local void fraction were similarly shaped,regardless of the chosen approach.Considering the experiment,this confirms the complex mixing flow patterns were simulated and predicted appropriately.

Fig.4.Local void fraction(a)and water velocity field(b)in the stirred vessel in the vertical mid-plane between the baffles(γ=45°)in the 24th second in the dispersed regime.

Fig.5.Local void fraction determined vessel height-wise using CFD and experiment(micro-resistivity probe).

Fig.6 shows the local void fraction(αl＜20%)in the two-phase mixture in multiple vertical mid-planes.It is clear that the gas phase occupied almost the entire domain.If the local void fraction is considered for different vertical vessel's mid-planes,i.e.,γ=0°(Fig.6a),γ=45°(Fig.6b),γ=90°(Fig.6c),γ=135°(Fig.6d),at the same time instance,its asymmetrical distribution is recognized.Therefore,the aeration regime in stirring should always be considered by means of a 3D CFD simulation.In our configuration,in contrast to the multi-stage Rushton impeller,no regions of gas-phase stagnation between the circulation zones were found.

3.2.3.Flow characteristics and size distribution of the bubbles

The size distribution of the bubbles is shown in Fig.7b.The largest bubbles were found adjacent to the shaft.In this region,the local void fraction was large(see Fig.7a)and lift dominated the flow development.Large bubbles were also found near to the free surface.Middle-size bubbles were present at the larger vessel diameters and in the regions of large shear stresses near the ABT impeller.Smaller bubbles were present in the injection region.The smallest bubbles were found near the vessel's bottom,wherethey were being held by therecirculation region(the inertia of liquid flow prevailed over the bubbles'buoyancy).Similar qualitative bubble distributions(sizes up to 5 mm)can be assessed by the bubble break-up and coalescence predictions in the works by Kerdouss et al.[50]and Petitti et al.[53].Due to the great specifics of the stirred vessel configuration(multistage impeller assembled from ABT,6PBT45,and Scaba-type 3SHP1 impellers of diameter 0.5T)and the operating conditions,quantitative data to compare with our CFD simulation could not be found in the literature.

4.Conclusions

Fig.6.Local void fraction(αl＜20%)in multiple vertical mid-planes;(a)γ=0°,(b)γ=45°,(c)γ=90°,(d)γ=135°in the 24th second in the air-water dispersion.

Fig.7.Size distribution of bubbles in the vertical mid-plane between the baffles(γ=45°)in the 24th second in the air-water dispersion.

Stirring in the single-and two-phase regimes was studied by means of a CFD simulation.A three-stage impeller was used.It was assembled from ABT,6PBT45,and Scaba-type 3SHP1 impellers,from the bottom to the top,respectively.The rotation of the impellers was considered using a sliding-mesh approach.The standard k-ε mixture turbulence model with scalable wall functions was used to model the turbulent fluid flow.The air-water dispersion was modeled using the Eulerian model.To account for the size distribution of the bubbles,a discrete population balance model was employed.The impeller's rotational speed was 178 r·min-1.The volumetric flow rate of the sparged air was 28.3 m3·h-1.This is the first study to consider such a large aeration rate,to the best of our knowledge.Furthermore,the experimental measurements were taken on the same laboratory experimental device.The hydrodynamic regimes considered in the CFD matched the experimental operating conditions.In the water mixing,the CFD prediction of the Power number was in good agreement with the experimental data.The relative difference between the two was 6.9%.Considering the size distribution of the bubbles between 1 mm and 16 mm the results were as follows.The CFD stirring power in the two-phase regime decreased by approximately 9%,with respect to the water mixing.Relative to the experimental data,the CFD predicted the stirring power in the dispersed regime was larger by 13.5%.The largest bubbles were found adjacent to the shaft,where a strong buoyancy lift dominated(due to the large local void fraction),and near the free surface.As shown by the CFD,the influence of the gas phase was dominant in between the middle and the upper impellers,where the flow field was strongly altered compared to the water mixing.Middle-sized bubbles were presented at the larger vessel diameters and in the regions of the large shear stresses near the ABT impeller.Small bubbles were found near the injection region,and the smallest bubbles were located near the vessel's bottom.The total gas holdup predicted by means of the numerical experiment was 13%smaller than the measured one,considering the laboratory experimental device.Therefore,we speculate that the predicted bubble sizes in the regions of coalescence were too large.A significant difference was found when comparing(in a quantitative manner)the local void fraction of the air between the CFD and the experiment.On the other hand,the qualitative agreement between the two was acceptable.However,the numerical input parameters for the CFD analysis and for the population balance model should be analyzed in more detail in future studies.

Acknowledgements

This research was supported by the Slovenian Ministry of Education,Science and Sport under contract no.P2-0162.