Effect of some parameters on the performance of anchor impellers for stirring shear-thinning fluids in a cylindrical vessel*

Houari AMEUR

Institut des Sciences et Technologies， Centre Universitaire Salhi Ahmed， CUN-SA， BP 66， Naama 45000， Algeria，E-mail: houari_ameur@yahoo.fr



Effect of some parameters on the performance of anchor impellers for stirring shear-thinning fluids in a cylindrical vessel*

Houari AMEUR

Institut des Sciences et Technologies， Centre Universitaire Salhi Ahmed， CUN-SA， BP 66， Naama 45000， Algeria，E-mail: houari_ameur@yahoo.fr

The 3-D hydrodynamics of shear thinning fluids in a stirred tank with an anchor impeller were numerically simulated. By using a computational fluid dynamics code （CFX 13.0）， the obtained results give a good prediction of the hydrodynamics such as the velocity fields and cavern size. The multiple reference frames （MRF） technique was employed to model the rotation of the impellers. The rheology of the fluid was approximated using the Ostwald model. To validate the CFD model， some predicted results were compared with the experimental data and a satisfactory agreement was found. The effects of impeller speed， fluid rheology， and some design parameters on the flow pattern， cavern size and power consumption were explored.

CFD， computer simulation， stirred tank， anchor impeller， shear thinning fluid

Introduction

Mixing operations with non-Newtonian fluids are frequently employed in areas such as the paint， polymer， food or pharmaceutical industries. Additional difficulties for the optimization of processes often occur with such fluids. Shear thinning fluids are a common class of non-Newtonian fluids， the agitation of such fluids results in the formation of well-mixed zone （known as cavern） around the impeller with essentially stagnant and/or slow moving fluids elsewhere. The formation of the stagnant regions gives rise to poor mass and heat transfer rates， which lead to poor quality of the end products［1］. Thus， the mixing of such fluids is a difficult operation and considered as a key step in the chemical industry. It is desirable to eliminate these stagnant regions by a proper mixing design［2-5］.

Low viscosity mixing applications can usually be performed with impeller systems consisting of one or more turbines and propellers. The close-clearance impellers are highly recommended for the mixing of highly viscous fluids， especially for shear thinning fluids， in the laminar regime［6］. For instance， in polymerization reactors， it is desirable to ensure efficient mixing to prevent phenomena like hot spots， to control the molecular weight distribution of the final product，and to avoid the dead zones［7］.

Triveni et al.［7］reported that if turbine impellers are used with highly viscous liquids， flow velocities rapidly decay to low values away from the impeller affecting the blending quality. Turbine impellers are therefore not recommended for use in the laminar regime. For such conditions， close-clearance impellers such as anchors are commonly used. Chhabra and Richardson［8］reported that the flow pattern generated by an anchor agitator is tangential and the anchor is suitable for mixing of viscous Newtonian and non-Newtonian fluids. It has been shown that， at higher impeller rotational speeds， an anchor impeller creates secondary axial and radial flows as well［9］. Nagata［10］revealed by experiments that there exists an axial temperature profile within the vessel. Bertrand et al.［11］and Savreux et al.［12］simulated the 2-D laminar mixing of non-Newtonian fluids with an anchor impeller and they confirmed the finding of Nagata that the anchor is inefficient in the laminar regime. Akiti et al.［13］also studied the behavior of an anchor agitated vessel of 2 L and 4 L capacity using CFD and they observedthat the anchor impeller produces little flow and turbulence in the area beneath the impeller irrespective of the reactor configuration. Karray et al.［14］investigated the performance of the anchor for turbulent Newtonian fluid flow. They found that the use of the classical anchor in turbulent flow yields an important deformation of the anchor arm. To solve this problem，they suggested using an anchor blade. Tanguy et al.［15］measured the power consumption of an anchor agitator for the homogenization of non-Newtonian fluids and they showed that the constant Ksdefined by Metzner and Otto［16］do not vary strongly with the power law index（n）. Espinosa-Solares et al.［17］studied the combined effect of bottom clearance and wall clearance on the power consumption rate and they proposed a numerical correlation. They have observed that the power consumption decreases as the bottom and wall clearance increase， which is due to the change in the flow pattern.

By experiments， Triveni et al.［18］studied the mixing of Newtonian and non-Newtonian fluids in an anchor-agitated vessel. They observed an increase in the fraction of the well-mixed region from 0.7 to 0.95 with increase in impeller speed for both Newtonian and non-Newtonian fluids but the increase is small for viscous fluids. Anne-Archard et al.［19］studied numerically the hydrodynamics and power consumption in a stirred vessel by helical and anchor agitators. They discussed the Metzner-Otto correlation for yield stress fluids.

By CFD simulations， Prajapati and Ein-Mozaffari［6］investigated the mixing of yield stress fluids for an anchor agitator. They found that the optimum values for the impeller width-to-tank diameter and impeller clearance-to tank diameter ratios were 0.102 and 0.079， respectively. The mixing time and the specific power consumption results for different operating conditions showed that a four-blade anchor impeller is more efficient than a two-blade anchor impeller.

Our search of the literature shows that a little space has been reserved to the prediction of 3-D hydrodynamics of power-law fluids in a tank equipped with an anchor impeller， through CFD modeling. Thus，the purpose of this paper is to simulate the 3-D flow fields generated by an anchor impeller in the agitation of power-law fluids in a cylindrical tank through the CFD technique and to search another design giving better performance.

The effects of fluid rheology， agitator speed， impeller blade width， number of blades and some other design parameters on the flow pattern， cavern size and power consumption were evaluated. 0.3 m， height:H/ D=1） fitted with an anchor agitator of 0.006 m×0.012 m blade width which is mounted on a shaft of 0.018 m of diameter（ds）. The liquid level is kept equal to the vessel height. The impeller is placed at a clearance（c）from the vessel base equal to 0.02 m.

Fig.1 Simulated system

The effect of blade diameter（d ）is investigated，four geometrical configurations are realized for this purpose， which are:d/ D=0.57， 0.65， 0.73 and 0.82 respectively.

2. Mathematical modeling

The fluid simulated has a shear thinning behavior modeled by the Oswald law. Table 1 resumes the fluid properties （fluid density（ρ）， power law index（n）and consistency index（m）） according to the measure of Triveni et al.［7］.

Table 1 Properties of the non-Newtonian fluid studied

For non-Newtonian fluids， the apparent viscosity（η ） is taken as［2，20］

The average shear rate is

where Ksis the shear rate constant andNis the impeller rotational speed.

1. Simulated system

Details of the simulated system are shown in Fig.1. It consists of a stirred vessel （diameter:D=

The generalized Reynolds number （Reg）for non-Newtonian fluids is defined as

Most of the published literature on shear rate constant had considered the dependency of Kson flow behavior n. But Tanguy et al.［15］reported that Ksis independent ofn . Though the variation in term ［（3n+1）/ 4n］n（n-1）is from 0.78 to 0.87 for a range innfrom 0.9 to 0.1， the percentage deviation in Ksis 21.8% and 12.3% respectively. So we have considered the dependence ofKsonnin the calculations.

Power（P）per unit volume（V）is an important approach for scaling up of an agitated vessel as this parameter ensures a constant specific interfacial area. It can be calculated by integration of the viscous dissipation in all the vessel volume

where Qvis the viscous dissipation.

The power number（N p）is calculated as

3. CFD simulations

A commercial CFD package （CFX 13.0） was employed to solve the momentum and continuity equations using the finite volume method. A pre-processor（ANSYS ICEM CFD 13.0） was used to discretize the flow domain with an unstructured tetrahedral mesh. A mesh test is performed in order to ensure the accuracy of our predicted results. The original 3-D mesh of the stirred system had 130 451 computational cells. Then，this number was increased by a factor of about 2， until to 260 902 cells. The additional cells changed the power number by more than 3%. Thus， the number of cells was increased again until 521 804 cells. The last mesh did not change the power number by more than 2.5%， therefore， the mesh with 260 902 cells was employed in this investigation. For further details， please refer to our previous work［21］. The simulations were considered converged when the scaled residuals for each transport equations were below 10-6. Most simulations required about 2 000 iterations for convergence. The computations were performed on a 3.60 GHz Intel Pentium IV CPU having 2.00 GB of RAM. The computational time was about 5 h-6 h.

4. Validation of the cfd model

The performance of the anchor impeller has been evaluated based on cavern size and power consumption. First， we have seen necessary to validate the CFD model. For this purpose， we have referred to the work of Prajapati and Ein-Mozaffari［6］. We note that the same geometrical conditions undertaken by these authors have been considered. The variation of power number versus Reynolds number is presented in Fig.2. The comparison of our predicted results with the experimental data given by Prajapati and his co-worker shows a satisfactory agreement.

Fig.2 Impeller power number versus Reynolds number

On the other hand， we remark that the power number data fall along the line with the slope of -1 at Reg＜30， indicating that the flow is laminar. At Reg＞30， the data start deviating from the line with the slope of -1. This means that the flow within the mixing tank is in the transitional regime.

5. Results and discussion

Results of the 3-D hydrodynamics in the whole vessel volume are presented in this section. Figure 3（a）shows the variations of tangential and radial velocities along the dimensionless vessel radiusR∗， where R∗=2R/ D，Ris the radial coordinate. We note that the dimensionless tangential velocityand thedimensionless radial velocityare defined as:andrespectively.

Fig.3 For 1 % CMC，，Z∗=0.5，D/ d=0.57

From Fig.3（a）， it is observed that both components reach up their maximum at the impeller blade tip，and begin to decay continuously until becoming negligible at the immediate contact with the side vessel wall. In comparison between the two velocity components， the tangential one is the dominant （Fig.3（b））. These results agree well with the finding of Chhabra and Richardson［8］.

Fig.4 Streamlines for 1 % CMC，Z∗=0.5，d/ D　=0.57

5.1 Effect of Reynolds number

The mixing performance is a function of the flow pattern generated by the impeller. Parameters such as impeller geometry， rotational speed and fluid rheology affect the flow pattern generated by the impeller in the mixing tank. In our study， different parameters have been investigated， we begin the test by searching the effects of impeller rotational speed.

It would be very useful to improve the knowledge of hydrodynamics， particularly the sheared/unsheared region distribution， in order to provide a predictive tool for designers. Figure 4 presents the streamlines for different Reynolds numbers at the middle height of vessel （Z∗=Z/ D=0.5，Zis the vertical coordinate）. The important remark from these slices is the formation of dead zones at the outside corner of the vertical arm. These dead zones can be eliminated by increasing the impeller rotational speed.

5.2 Effect of fluid rheology

The influence of fluid rheology is discussed in this section. We recall that the CMC （sodium carboxymethyl cellulose） solution is simulated in this study which has a shear thinning behavior. Two concentrations of CMC have been used and all the fluid properties are reported in Table 1.

Streamlines are presented in Fig.5 for the two CMC concentrations at a location upper the horizontal arm of the anchor impeller. For a laminar regime（Reg=20）and due to the insufficient impeller rotational speed， two vortices are formed at the blade tip. These vortices are detached from the blade tip going away to the vessel wall with the increase of CMC percentage.

Fig.5 Streamlines for the classical anchor，Z∗=0.2，d/ D　=0.57

Fig.6 Power number for the classical anchor （Case 1），d/ D= 0.57

The power number is calculated also for the two cases， as show in Fig.6， this parameter is greater with increase of viscosity. On the other hand， the continuous increase of the impeller rotation speed permits a reduction in the power required. However， for Reg＞30（transitional regime）， the decrease ofNp is slight when compared with the laminar regime.

5.3 Effect of blade diameter

A mixing operation can be defined as an artificial creation of the fluid flow to decrease its heterogeneity，to accelerate its transfer and to achieve a certain degree of homogeneity. These factors are related to the impeller design and the flow behavior. For this purpose， we have taken into account the impeller shape and some design parameters.

In this section， we investigate the influence of impeller blade diameter（d）. For the same number of blades（α=2）， four geometrical configurations are realized and which are:d/ D=0.57， 0.65， 0.73 and 0.82， respectively. Figure 7 gives an insight about the flow pattern generated by changing the ratiod/ D. For low Reynolds numbers（Reg=20）， the formation of recirculation loops is observed at each corner of the blade. Reducing the little space between the impeller blade and vessel wall can participate to eliminate these dead zones. On the other hand， the power required（Table 2） is increased， and this is due to the wall effects and inertial forces.

Fig.7 Streamlines for， 1% CMC，Z∗=0.5，α=2

Table 2 Power number for Reg=20， 1% CMC，α=2

5.4 Effect of blade number

Another parameter which can touch the performance of agitated system is the impeller blade number（α）. For this end， three geometrical configurations have been tested， which are:α=2， 4 and 6， respectively.

For an angular position θ=90o， the variation of mean velocity along the vessel height for different impeller blade numbers is presented in Fig.8. The observation of this figure indicates that there is a great difference between the first case and second one， and just a slight difference between the second and third cases. For the two blades impeller， the fluid motion is less intense which is marked by the formation of a recirculation zone at the blade corner （Fig.9）. At the same Reynolds number， these dead zones are eliminated in the second and third cases.

Fig.8 Mean velocity for Reg=20， 1% CMC，d/ D　 =0.57，R∗=0.3，θ=90o

Fig.9 Flow fields for Reg=20， 1% CMC，d/ D　=0.57，Case 1

The agitation of shear thinning fluids results in the formation of zone of intense motion near the impeller （called cavern） with essentially stagnant zone elsewhere. Fig.9 （Line 2） presents the cavern size for the three cases studied， as illustrated: the increase in blade number enlarges the cavern size and enhances the mixing performances. Nevertheless， it is penalizing in terms of power consumption （Table 3）. From all of these remarks， and since the dead zones can be elimi-nated by the impeller with four blades， thus α=4can be chosen as a sufficient number.

Table 3 Power number for Reg=20， 1% CMC，d/ D=

5.5 Effect of impeller design

In laminar mixing of highly viscous fluids， the mixing is obtained by a sequence of stretching， folding and breaking mechanisms and not by highly energetic eddies， which makes the design of an optimal mixing device very challenging［22-24］.

Here， we tried to add arm blades at different heights and positions （horizontal and/or vertical）， four cases have been investigated and summarized in Fig.10. Values of the power number obtained for all cases studied are summarized in Table 4.

Fig.10 Cavern size for Reg=20， 1% CMC

Table 4 Power number for Reg=20， 1% CMC

The classical anchor is inefficient at low Reynolds numbers （Case 1） and the well stirred region is limited at the tank bottom. Mixing may be enhanced at the upper part of the vessel by adding an horizontal arm in this region （Case 2）， and a better enhancement of the axial circulation may be obtained if this arm is placed vertically （Case 3） but with additional power cost.

6. Conclusion

In this study， the CFD technique was used to investigate the agitation of CMC solution， which is a shear thinning fluid， with an anchor impeller. The cavern size and the specific power consumption results for different operating conditions showed that the insufficient impeller rotational speed and little blade diameter permit the formation of dead zones at the upper corner of blade. For Reg＞20， the decrease of power consumption continues but very slightly. The classical anchor is found inefficient in the laminar regime， thus to eliminate the dead zone， to increase the cavern size and to avoid the deformation of blade we suggest the use of arms （horizontal and vertical）. The increase of blade number is also important， based on the comparison made previously we can choose the four bladed as sufficient for obtaining the best performance.

References

［1］ AMANULLAH A.， HJORTH S. A. and NIENOW A. W. Cavern sizes generated in highly shear thinning viscous fluids by Scaba 3SHP1 impeller［J］. Food and Bioproducts Processing， 1997， 75（4）: 232-238.

［2］ WOZIWODZKI S.， BRONIARZ-PRESS L. and OCHOWIAK M. Transitional mixing of shear-thinning fluids in vessels with multiple impellers［J］. Chemical Engineering and Technology， 2010， 33（7）: 1099-1106.

［3］ MAAß S.， EPPINGER T. and ALTWASSER S. et al. Flow field analysis of stirred liquid-liquid systems in slim reactors［J］. Chemical Engineering and Technology，2011， 34（8）: 1215-1227.

［4］ IRANZO A.， BARBERO R. and DOMINGO J. et al. Numerical investigation of the effect of impeller design parameters on the performance of a multiphase bafflestirred reactor［J］. Chemical Engineering and Technology， 2011， 34（8）: 1271-1280.

［5］ WOZIWODZKI S. Unsteady mixing characteristics in a vessel with forward-reverse rotating impeller［J］. Chemical Engineering and Technology， 2011， 34（5）: 767-774.

［6］ PRAJAPATI P.， EIN-MOZAFFARI F. CFD Investigation of the mixing of yield- pseudoplastic fluids with anchor impellers［J］. Chemical Engineering and Technology，2009， 32（8）: 1211-1218.

［7］ TRIVENI B.， VISHWANADHAM B. and MADHAVI T. et al. Mixing studies of non-Newtonian fluids in an anchor agitated vessel［J］. Chemical Engineering Research and Design， 2010， 88（7）: 809-818.

［8］ CHHABRA R. P.， RICHARDSON J. F. Liquid mixing: In non Newtonian flow in process industries［M］. Oxford， UK: Butterworth-Heinemann， 1999， 324-391.

［9］ OHTA M.， KURIYAMA M. and ARAI K. et al. A twodimensional model for the secondary flow in an agitated vessel with anchor impeller［J］. Journal of Chemical Engineering of Japan，1985，18（1）: 81-84.

［10］ NAGATA S. Heat transfer in agitated vessel. In mixing: Principles and applications［M］. New York， USA: Wiley，1975， 385-387.

［11］ BERTRAND F.， TANGAY P. A. and BRITO-DE LA FUENTE E. A new perspective for the mixing of yield stress fluids with anchor impellers［J］. Journal of Chemical Engineering of Japan， 1996， 29（1）: 51-58.

［12］ SAVREUX F.， JAY P. and ALBERT M. Viscoplastic fluid mixing in a rotating tank［J］. Chemical Engineering Science， 2007， 62（8）: 2290-2301.

［13］ AKITI O.， YEBOAH A. and BAI G. et al. Hydrodynamic effects on mixing and competitive reactions in laboratoryreactors［J］. Chemical Engineering Science， 2005， 60（8-9）: 2341-2354.

［14］ KARRAY S.， DRISS Z. and KCHAOU H. et al. Hydromechanics characterization of the turbulent flow generated by anchor impellers［J］. Engineering Applications of Computational Fluid Mechanics， 2011， 5（3）: 315-328.

［15］ TANGUY P. A.， THIBAULT F. and BRITO DE LA FUENTE E. A new investigation of the Metzner-Otto concept for anchor mixing impellers［J］. Canadian Journal of Chemical Engineering， 1996， 74（2）: 222-228.

［16］ METZNER A. B.， OTTO R. E. Agitation of non-Newtonian fluids［J］. AIChE Journal， 1957， 3（1）: 3-10

［17］ ESPINOSA-SOLARES T.， BRITO-DE LA FUENTE E. and THIBAULT F. et al. Power consumption with anchor mixers-effect of bottom clearance［J］. Chemical Engineering Communications， 1997， 157（1）: 65-71.

［18］ TRIVENI B.， VISHWANADHAM B. and VENKATESHWAR S. Studies on heat transfer to Newtonian and non-Newtonian fluids in agitated vessel［J］. Heat Mass Transfer， 2008， 44: 1281-1288.

［19］ ANNE-ARCHARD D.， MAROUCHE M. and BOISSON H. C. Hydrodynamics and Metzner-Otto correlation in stirred vessels for yield stress fluids［J］. Chemical Engineering Journal， 2006， 125（1）: 15-24.

［20］ MURTHY S. S.， JAYANTI S. Mixing of power-law fluids using anchors: Metzner-Otto concept revisited［J］. AIChE Journal， 2003， 49（1）: 30-40.

［21］AMEUR H.， BOUZIT M. and HELMAOUI M. Numerical study of fluid flow and power consumption in a stirred vessel with a Scaba 6SRGT impeller［J］. Chemical and Process Engineering， 2011， 32（4）: 351-366.

［22］ IRANSHAHI A.， DEVALS C. and HENICHE M. et al. Hydrodynamics characterizations of the Maxblend impeller［J］. Chemical Engineering Science， 2007， 62（14）: 3641-3653.

［23］ AMEUR H.， BOUZIT M. Mixing in shear thinning fluids［J］.Brazilian Journal of Chemical Engineering， 2012，29（2）: 349-358.

［24］ AMEUR H.， BOUZIT M. and HELMAOUI M. Hydrodynamic study involving a Maxblend impeller with yield stress fluids［J］. Journal of Mechanical Science and Technology 2012， 26（5）: 1523-1530.

10.1016/S1001-6058（16）60671-6

February 10， 2015， Revised June 13， 2015）

* Biography: Houari AMEUR （1982-）， Male， Ph. D.，Assistant Professor

2016，28（4）:669-675