Scholarly article on topic 'CFD Simulations of the Air/Water Two-phase Flow in an Annular Centrifugal Contactor'

CFD Simulations of the Air/Water Two-phase Flow in an Annular Centrifugal Contactor Academic research paper on "Chemical engineering"

CC BY-NC-ND
0
0
Share paper
Academic journal
Energy Procedia
OECD Field of science
Keywords
{"Computational fluid dynamics" / "Annular centrifugal contactor" / "Ttwo-phase flow" / "Taylor vortex"}

Abstract of research paper on Chemical engineering, author of scientific article — Chengqian Wang, Shaowei Li, Wuhua Duan, Shuo Cao

Abstract Annular centrifugal contactors (ACCs) use centrifugal force to mix and separate two immiscible liquids of different densities. The compact size, small liquid hold-up volume, short liquid residence time and high efficiency of ACCs have made them be favored for nuclear processes and destined to play a more important role for future advanced nuclear processing schemes. Computational fluid dynamics (CFD) simulations can provide a more complete understanding of the flow within the ACC for further advancements in design and operation of future ACCs. In this paper, CFD simulations of the air/water two-phase flow in the mixing zone of the ACC were carried out. The flow patterns and velocity profiles of the steady-state simulations for three different rotor speeds in the annular region and under the rotor are presented.

Academic research paper on topic "CFD Simulations of the Air/Water Two-phase Flow in an Annular Centrifugal Contactor"

Available online at www.sciencedirect.com

ScienceDirect

Energy Procedia 39 (2013) 467 - 473

Asian Nuclear Prospects 2012

CFD simulations of the air/water two-phase Flow in an Annular Centrifugal Contactor

Chengqian Wang Shaowei Li, Wuhua Duan*, Shuo Cao

Institute of Nuclear and New Energy Technology, Tsinghua University, Beijing 102201, China

Abstract

Annular centrifugal contactors (ACCs) use centrifugal force to mix and separate two immiscible liquids of different densities. The compact size, small liquid hold-up volume, short liquid residence time and high efficiency of ACCs have made them be favored for nuclear processes and destined to play a more important role for future advanced nuclear processing schemes. Computational fluid dynamics (CFD) simulations can provide a more complete understanding of the flow within the ACC for further advancements in design and operation of future ACCs. In this paper, CFD simulations of the air/water two-phase flow in the mixing zone of the ACC were carried out. The flow patterns and velocity profiles of the steady-state simulations for three different rotor speeds in the annular region and under the rotor are presented.

© 2013 The Authors. Published by Elsevier Ltd.

Selection and peer-review under responsibility of Institute of Nuclear and New Energy Technology, Tsinghua University

Keywords: Computational fluid dynamics; Annular centrifugal contactor; Ttwo-phase flow; Taylor vortex

1. Introduction

An annular centrifugal contactor (ACC) was developed based on the paddle type centrifugal contactor at Argonne National Laboratory (ANL) in the Late 1960s. Compared with mixer-settlers and extraction columns, ACCs offer some advantages including low hold-up volume, short residence time therefore less solvent degradation and reduction of solvent waste, excellent phase separation, high mass transfer efficiency, great safety with respect to nuclear criticality, compact therefore low capital and operating cost, no disturbance to the steady state when being shut down, rapid start-up and shut-down, etc.

* Corresponding author. Tel.: + 8610-80194038; fax: +8610-62771740. E-mail address: dwh203@mail.tsinghua.edu.cn.

1876-6102 © 2013 The Authors. Published by Elsevier Ltd.

Selection and peer-review under responsibility of Institute of Nuclear and New Energy Technology, Tsinghua University doi: 10.1016/j.egypro.2013.07.238

Therefore, ACCs are favored for reprocessing of spent nuclear fuel and partitioning of high level liquid waste [1,2].

The ACC is based on the principle of Taylor-vortex flow. The vortex motion in the annular region causes intense mixing of the two liquids, so the flow in a centrifugal contactor is extremely turbulent, unsteady, and consists of at least three phases (two liquid phases and air). It is difficult to understand the flow patterns in the contactor and to obtain more flow detail information to guide design and operation by traditional experimental measurements. While computational fluid dynamics (CFD) may be a key tool to visualize the flow patterns within the contactor and provide more flow detail information, flow patterns, velocity profiles, pressure distribution, and so on, which can guide design and operation of ACC. International interest in CFD of the flow in the ACC has been increasing in recent years. Much work has been done in the field of CFD simulations of the ACC [3-13]. In this work, CFD simulations of the air/water two-phase in the mixing region of the <|>70 ACC with a rotor of 70 mm in diameter were carried out.The purpose of this research is to improve the general understanding of the flow within a centrifugal contactor through the application of CFD, which can guide the ACC design, perform operational optimizations.

2. Computational methods

2.1. Annular centrifugal contactor

The sketch of a typical ACC is shown in Fig.1. Two immiscible liquids with different densities enter through tangential ports into the annular mixing region between the rotor and the housing, where the dispersion begins to form as the fluids are mixed by turbulent Couette flow induced by the spinning rotor. Radially oriented vanes below the rotor break the rotation of the dispersion and direct it through the orifice into the hollow rotor, which the acts as a centrifuge separating the two phases and pumping the liquid upward. Vertical baffles inside the rotor accelerate the mixture to rotor speed. The separated phases then flow over their respective weirs into their collector rings in the housing, and then out the tangential exit lines flowing by gravity into an adjacent stage or collection vessels, respectively. In this way the contactor acts as mixer, a centrifuge, and a pump.

Heavy Phase Weir

Heavy Phase Exit Light Phase Collector

Rotary Vanes —

Light Phase Inlet

Rotor Housing —

Light Phase Weir

Heavy Phase Collector Light Phase Exit

Rotor Inlet

Heavy Phase Inlet iAnntoteMKng Zone

Fig.1. Sketch of an annular centrifugal contactor

2.2. Geometry and mesh

The ACC geometry for all simulations was based on the <|>70 ACC developed by Duan et al. as shown in Fig.2 [14]. Three-dimensional simulations were carried out here for the capability of capturing the actual spatial structures of the flow. The average grid size is 2 mm. The mesh was refined primarily near the rotor as this is a high shear region with the largest velocity gradients. In this way, the mesh of the base geometry consisted of 216447 total nodes and 1156757 tetrahedral cells and 78036 total Faces.The main geometric parameters are listed in Table 1. The Vane-to-rotor gap height Hgap is the vertical distance from the exterior bottom of the rotor to the upside of the radial vane.

Fig.2. Model geometry of the mixing zoon in an annular extraction contactor

Table 1. Key geometric parameters of the model

Parameter Value (mm)

Rotor radius Rr 35

Housing radius RH 52

Inlet radius Ri 15

Inlet (Rotor inlet )radius Ro 10

Radial vane height Hv 15

Vane-to-rotor gap Hgap 6

Mixing zone height Hm 104

2.3. Model setup

Computational modeling of the 3D, air/wate two-phase flow within the mixing region was done using the commercial CFD package CFX 5.6. All simulations were performed in parallel using 4 processors.

There are two important issues needing to consider. One is the treatment for modeling the turbulence. More sophisticated approaches such as Direct Numerical Simulation and Large Eddy Simulation resulting in more accurate predictions still take highly computational cost hindering their wide uses for practical

engineering problems. Most studies suggest that the Reynolds-Averaged Navier-Stokes approach such as the k-e Turbulence Model and the Reynolds Stress Model (RSM) provides acceptable predictions. In addition, the earlier work has shown that the k-e Turbulence Model has limitations for simulating the ACC [10]. Consequently, the RSM solving only for the statistical mean flow is used here. The other aspect is the strategy used to describe the air/water two-phase flow concerned. Here, we focus on the Eulerian-Eulerian models, in which the different phases are described as interpenetrating media through the concept of volume fractions.

The current simulations presented here provide a more realistic analysis of the flow in the mixing zone by including the free surface flow of water/air in the entire mixing zone. Water is treated as continuous and air discrete. The continuum surface force model with a surface tension of 73 mN/m is also used to account for surface tension effects on the water/air interface in the two-phase flow.

2.4. Boundary condition

The inlet to the separation zone was treated as a spatially and temporally constant volume flow rate boundary which did not have a noticeable effect on the predicted flow field. All simulations were done for the same inlet conditions with equal flow distribution to the two tangential inlet ports with a volume flow rate of 600 ml/min at each inlet. For the air/water two-phase flow, the volume fractions of water in both of the inlets were equal to 1.

Both the rotor and the housing walls had no-slip conditions, and the rotor wall was given a fixed rotational velocity. Different rotor speeds were presented to evaluate change in the flow due to rotor speed.

As shown in Fig.2, the top surface was specified as a pressure opening boundary with atmospheric pressure to enable the volume of air (incompressible) in the system to vary and allow the volume of liquid in the mixing zone to reach an equilibrium level depending on the operating conditions (i.e. inlet flow rate and rotor speed) and the mixing zone outlet pressure.

The outlet of the mixing zone is also the inlet to the separation zone. The pressure is unknown herein. Actual measurements of the pressure at the rotor inlet are difficult to perform. We calculated outlet pressure by assuming that the pressure at the center point of the outlet surface was simply equal to the pressure generated by the rotating air column within the separating zone (see Fig.1) according to the Bernoulli equation for rotating flow as Wardle et al. did [4]. Under the simulation conditions, the relative pressure at the rotor inlet was found to be slightly negative, as -16 Pa for 1000 r/min, -42Pa for 2000 r/min and -76 Pa for 3000 r/min, respectively. The impact of the outlet pressure will be investigated in the further study.

3. Results and Discussion

3.1. General Flow

Within the mixing region, under normal operating conditions there is an air space above the mixing liquid such that there is free surface flow (flow of a liquid-gas interface) and gas entrainment. The annular liquid height is an important parameter affecting the mixing and overall extraction efficiency of the contactor. The annular liquid height has been observed to be a function of the input flow rate, rotor speed, housing geometry (e.g. vane geometry, annular gap size), and rotor geometry [4].

Fig.3 shows the cross-section views of the flow of water (red) and air (blue) in the mixing zone for the three rotor speed settings. The more diffuse appearance of the air/water interface is simply an artifact of the larger computational cells used. The effect of the rotor speed was evaluated by comparing the

converged solutions for rotor speeds of 1000, 2000 and 3000 r/min, respectively. As shown in Fig.3, there are only subtle differences in each phase at all the settings. The distinctive feature of the flow in the annular mixing region is the air/water free surface. For different rotor speeds (and therefore different outlet pressures), the position and shape of the free surface is inconsistent. The average liquid height decreases apparently with increase of the rotor speed. It is observed that the free surface becomes parabolic under higher rotor speeds. It is also evident that the air/water free surface is asymmetrical, which indicates that the flow in this region is turbulent and vary. This is in accordance with the result of the experiment where the height of the free surface oscillates at near constant frequency and magnitude [4]. The yellow zone beneath the free surface at 3000 r/min can mainly attribute to the formation and collection of large air bubbles in the center of the large vortex.

(a) 1000 r/min (b) 2000 r/min (c) 3000 r/min

Fig.3. Cross-section of the density of the air-water two-phase flow at different rotor speed

3.2. Flow in the annular region

The stead-state axial mean velocity vectors on a vertical cross-sectional plane are shown in Fig.4(a). This flow pattern is characteristic of the Taylor-Couette vortex. The number of vortices depends on the rotational speed and the geometrical parameters of ACC. Fig.4(a) highlights the presence of two main vortices separating the annulus into two parts. The two vortices with high disparity in dimension swirl in opposite directions for the balance of the vortex motion. In the stable Taylor-Couette vortex just above the rotor bottom, the fluid is moving upward at the rotor and downward at the housing wall. This is consistent with the result obtained by Wardle et al [4]. Both the position and the appearance of the free surface seem to have great influence on the upper Taylor-Couette vortex in the liquid phase.

As shown in Fig4(b) for contours of axial velocity, the fluid is moving downward near the rotor and upward near the housing wall in the vortex near the inlet while that in the other is flowing in the opposite direction, upward near the rotor and down at the housing wall. This is consistent with the flow patterns observed in previous single-phase [3] and two-phase [4] simulations. From Fig4(b), it is clear that as would be expected, the flow of the highest magnitude is located near the rotor with a maximum value approximately at the center of the lower Taylor-Couette vortex.

3.3. Flow under the rotor

It is apparent from Fig.5 that the radial vanes divide the beneath of the rotor into four separate regions, and there are large vortices swirling in the counter-clockwise direction (the same as rotor rotation) in each section. The highest magnitudes are in the area of the outside wall where the directions of motion change

sharply and the forward corner of the radial vane region where the direction of motion parallel to the forward radial vanes.

Fig.4. The air-water two-phase flow in the annulus at 3000 r/min

waîer.Superficial Velocity (Projection)

Vector 2

Fig.5. Velocity vectors of the air-water two-phase flow on horizontal plane under the rotor at 3000 r/min

It is also apparent that there's a kind of symmetry in the flow pattern of every two opposite regions. Conversely, the flow in the regions directly adjacent to the inlets is dissimilar with those away from the inlets which have slightly higher value of the highest magnitudes. It is a manifestation of the influence of the inlets positions. There are two vortices in the two opposing sections adjacent to the inlets and the center of each vortex appears slightly shifted outwards the forward rotational direction and the vortex is somewhat less compact than those in the two regions not adjacent to the inlets. The result is similar to

that in the previous simulations [3,5] and experiment [15] in different geometric model under different conditions respect to the movement characteristics of the Taylor vortex.

4. Conclusions

This work presented the results of CFD simulations of the air/water two-phase flow in the mixing region of the <|>70 ACC. The steady state air/water two-phase simulations were performed to compare qualitatively with other experiments and simulations for the model validation. It found that the flow patterns observed in the CFD model accord with those in other study. It was demonstrated that the model used in the study was acceptable. The Effects of changes in operational parameters were also evaluated. It finds out the Taylor vortices in the mixing zone have a significant impact on the flow pattern and the distribution of the turbulent energy dissipation rate, consequently on the mixing.

References

[1] Leonard RA. Recent advances in centrifugal contactor design. Sep Sci Technol 1988; 23: 1473-1487.

[2] Duan WH, Cheng Q, Zhou XZ, Zhou JZ. Development of a <|>20 mm annular centrifugal contactor for the hot test of the total TRPO process. Prog Nucl Energ 2009; 51: 313-318.

[3] Wardle KE, Allen TR, Swaney R. Computational fluid dynamics (CFD) study of the flow in an annular centrifugal contactor. Sep Sci Technol 2006; 41(10):2225-2244.

[4] Wardle KE, Allen TR, Anderson MH, Swaney RE. Free surface flow in the mixing zone of an annular centrifugal contactor. AIChE J 2008; 54(1):74-84.

[5] Wardle KE, Allen TR, Anderson MH, Swaney RE. Analysis of the effect of mixing vane geometry on the flow in an annular centrifugal contactor. AIChE J 2009; 55(9):2244-2259.

[6] Wardle KE, Allen TR, Swaney RE. CFD simulation of the separation zone of an annular centrifugal contactor. Sep Sci Technol 2009; 44(3):517-542.

[7] Wardle KE. Open-source CFD simulations of liquid-liquid flow in the annular centrifugal contactor. Sep Sci Technol 2011; 46:2409-2417.

[8] Gandhir A, Wardle KE. CFD analysis of fluid flow above the upper weir of an annular centrifugal contactor. Sep Sci Technol 2012; 47:1-10.

[9] Sreepriya V, Jyeshtharaj BJ, Sudhir BK. CFD simulation of RTD and mixing in the annular region of a Taylor-Couette contactor. Ind Eng Chem Res 2006; 45:6360-6367.

[10] Deshmukh SS, Sreepriya V, Jyeshtharaj BJ , Sudhir BK. Computational flow modeling and visualization in the annular region of annular centrifugal extractor. Ind Eng Chem Res 2007; 46:8343-8354.

[11] Padial-Collins NT, Zhang DZ, Zou QS, Ma X, Brian VanderHeyden W. Centrifugal contactor: separation of an aqueous and an organic stream in the rotor zone (LA-UR-05-7800). Sep Sci Technol 2006; 41:1001-1023.

[12] Deshmukh SS, Joshi JB, Koganti SB. Flow visualization and three-dimensional CFD simulation of the annular region of an annular centrifugal extractor. Ind Eng Chem Res 2008; 47:3677-3686.

[13] Deshmukh SS, Sathe MJ, Joshi JB, Koganti SB. Residence time distribution and flow patterns in the single-phase annular region of annular centrifugal extractor. Ind Eng Chem Res 2009; 48:37-46.

[14] Duan WH, Song CL, Wu QL, Zhou XZ, Zhou JZ. Development and performance of a new annular centrifugal contactor for semi-industrial scale. Sep Sci Technol 2005; 40: 1871-1883.

[15] Wardle KE, Allen TR, Anderson MH, Swaney RE. Experimental study of the hydraulic operation of an annular centrifugal contactor with various mixing vane geometries. AIChE J 2010; 56( 8): 1960-1974.