CHINESE JOURNAL OF MECHANICAL ENGINEERING Vol. 25, No. 5, 2012

·905·

DOI: 10.3901/CJME.2012.05.905, available online at www.springerlink.com; www.cjmenet.com; www.cjmenet.com.cn

Numerical Simulation of Turbulent Flow of Hydraulic Oil through 90° Circular-sectional Bend WANG Liwei1, 2, *, GAO Dianrong2, and ZHANG Yigong1 1 Technology Center, Taiyuan Heavy Industry Co., Ltd., Taiyuan 030024, China 2 College of Mechanical Engineering, Yanshan University, Qinhuangdao 066004, China Received November 17, 2011; revised May 21, 2012; accepted May 31, 2012

Abstract: Oil flow through pipe bends is found in many engineering applications. However, up to now, the studies of oil flow field in the pipe bend appear to be relatively sparse, although the oil flow field and the associated losses of pipe bend are very important in practice. In this paper, the relationships between the turbulent flow of hydraulic oil in a bend and the Reynolds number Re and the curvature ratio δ are studied by using computational fluid dynamics (CFD). A particular emphasis is put on hydraulic oil, which differs from air or water, flowing through 90° circular-sectional bend, with the purpose of determining the turbulent flow characteristics as well as losses. Three turbulence models, namely, RNG k-ε model, realizable k-ε model, and Reynolds stress model (RSM), are used respectively. The simulation results in the form of contour and vector plots for all the three turbulence models for pipe bends having curvature ratio of δ0.5, and the detailed pressure fields and total pressure losses for different Re and δ for RSM are presented. The RSM can predict the stronger secondary flow in the bend better than other models. As Re increases, the pressure gradient changes rapidly, and the pressure magnitude increases at inner and outer wall of the bend. When δ decreases, two transition points or transition zones of pressure gradient arise at inner wall, meanwhile, the transition point moves towards the inlet at outer wall of the bend. Owing to secondary flow, the total pressure loss factor k increases as the bend tightens, on the contrary, as Re increases, factor k decreases due to higher velocity heads, and the rapid change of pressure gradient on the surface of the bend leads to increasing of friction and separation effects, and magnified swirl intensity of secondary flow. A new mathematical model is proposed for predicting pressure loss in terms of Re and δ in order to provide support to the one-dimensional simulation software. The proposed research provides reference for the analysis of oil flow with higher Re in the large bends. Key words: hydraulic oil, 90° bend, turbulent flow, pressure loss, computational fluid dynamics (CFD)

1

Introduction ∗

Fluid flow, such as air, water, oil through pipe bends has been of considerable interest to the machine piping. One important parameter for this flow is the Dean number[1], which can be defined by the Reynolds number Re and the curvature ratio δ of the pipe bend. When the Dean number is high, the flow may become unsteady, and separation may take place. For a comprehensible depiction of the flow, it would be highly desirable to solve the Navier-Stokes equations. Furthermore, there are situations where the experiments for these bends configurations are very difficult to be carried out and with a noticeable cost, especially for large bends. Focus has been turned to the techniques of computational fluid dynamics (CFD) in order to simulate the flow. With the significant advancement of computer speed and * Corresponding author. E-mail: [email protected] This project is supported by National Natural Science Foundation of China(Grant No. 50775194), and Shanxi Provincial Natural Science Foundation of China (Grant No. 2011011026-1) © Chinese Mechanical Engineering Society and Springer-Verlag Berlin Heidelberg 2012

memory, CFD is becoming a viable tool to provide detailed information of the flow in the components composing piping. A number of examples can be found in the literature of CFD investigations, which are aimed at predicting the flow through curved pipes. SHIRAYAMA, et al[2], simulated the low and high Dean number flows in a circular curved pipe, and visualized the extensive computed results. LAI, et al[3], proceeded a detailed numerical investigation of a turbulence driven secondary flow in a curved pipe. SHAO, et al[4], studied the accuracy of using CFD for the prediction of pressure loss in heating, ventilation and air conditioning (HVAC) duct fittings, which included double pipe bends, and the factors affecting its accuracy. Recently, CRAWFORD, et al[5], presented pressure loss data for a series of pipe bends with various curvature radius using CFD calculations from four turbulence models. The applications that oil flows through pipe bends are found in many engineering applications. However, the studies of oil flow field in the pipe bend appear to be relatively sparse, although the oil flow field and the associated losses of pipe bend are very important in practice. Both air and water appear more than oil in

·906·

YWANG Liwei, et al: Numerical Simulation of Turbulent Flow of Hydraulic Oil through 90° Circular-sectional BendY

above-mentioned and former literature, one of the reasons might be that air and water have general application in early experiment, thereafter computation research focus on comparison and validation with former experimental conclusions, so the air and water flow frame of pipe bends is understood[1–16]. Nowadays, CFD is competent for single phase fluid included air, water, and oil as well as multi-phase flow[10], moreover, in view that a 90° circular-sectional bend is widely used in hydraulic machine such as forging press, extrusion press, and so on, this investigation is to study the flow frame and losses of hydraulic oil through 90° circular-sectional bend.

2

Flow Characteristics and Bend Geometries

In this paper, the flow characteristics are found for a three-dimensional circular-sectional bend under the following conditions and limitations: the fluid is an incompressible hydraulic oil, oil density ρ875 kgm3, dynamic viscosity µ0.043 75 N • sm2; the boundaries of the pipe are rigid and stationary; the flow is turbulent and steady. The bend is preceded by a straight section of pipe where the flow can change from fully developed pipe flow and succeeded by another straight section where the flow can return to fully developed flow; the central angle of the bend is 90°, and outer and inner walls are concentric. The bend is set in the horizontal plane, and the bend geometry is shown in Fig. 1. The bend configuration is circular, and the bend has an inner diameter d of 440 mm. The pipe configurations were designed with 50d upstream and downstream of the bend in order to isolate the flow from external disturbances.

Fig. 1.

Schematic diagram of the bend geometry and coordinate system

When the fluid flows through a 90° circular-sectional bend, the flow patterns become more complex than those in a straight pipe and are characterized by the Dean number De, which represents the ratio of the product of the inertia and centrifugal forces to the viscous forces. Since the secondary flow is induced by centrifugal forces and their interaction primarily with viscous forces, De is a measure of the magnitude of the secondary flow. De can be defined as

De  Reδ 1 2 ,

(1)

where Re  dv ρ µ is the Reynolds number, δ  r R is the curvature ratio of the bend radius to curvature radius. The curvature ratio δ is a more detailed measure of the effect of geometry and the extent to which the centrifugal force varies on the cross section. Thus δ affects the balance of inertia, viscous, and centrifugal forces, and it can play a major role in pipe bends. This is discussed in the following section.

3

Computational Methodology

The commercial CFD code and mesh generation packages were used. Three-dimensional steady-state Reynolds averaged Navier-Stokes (RANS) equations were solved using the segregated implicit solver. The right choice of a turbulence model is a critical when an industrial turbulent flow problem is faced, especially when this problem involves three-dimensional flow phenomena, which need an accurate modeling. It is known that no existing turbulence model is suitable for all flow situations and one numerical set-up that yields high accuracy in simulation of one fitting may lead to a large error in that of another. Therefore, CFD validation should be performed. In this paper, the RANS equations were computed using the k-ε model and Reynolds stress model (RSM). Although the k-ε model is robust, efficient and very widely used, it is known that in highly swirling flows or in flows where significant stream curvature exists, this model becomes inadequate. In such cases, the RSM generally offers greater accuracy by modeling the Reynolds stresses directly. The relative advantages of the two models in simulating the bends will be discussed in the following section. Non-equilibrium wall functions were used for the treatment of the near wall layer. Because of the capability to partly account for the effects of pressure gradients and departure from equilibrium, the non-equilibrium wall functions are recommended for use in the complex flows involving separation, reattachment, and impingement where the mean flow and turbulence are subjected to severe pressure gradients and change rapidly. The second order scheme was used for the RANS equations calculations, with a pressure-velocity coupling achieved using SIMPLEC algorithm. The default under relaxation factors were used to aid convergence for all models. Mesh resolution was driven by the wall y+, and considerable care was taken to ensure that the aspect ratio of the cells was as uniform as possible to the general features of the flow. The expansion ratio was generally kept below 1.2 to ensure sufficient mesh refinement throughout the domain. In accordance with the requirements of the non-equilibrium wall function, the value of y+ was set to be between 30 and 300 for the majority of the calculations, and the expansion ratio was set to be 1.1. A variety of grid densities was tested to ensure that the grid is sufficiently dense for the accurate representation of the possible large

CHINESE JOURNAL OF MECHANICAL ENGINEERING gradients of flow variables and the overall grid size is as small as accuracy can allow for reasonable convergence speed. In this study, an approach introduced by SHAO, et al[4] is adopted: the doubling of grid density was not implemented simultaneously in all the three dimensions and sections of the computational domain. This arrangement enables the grid dependency tests to be carried out without dramatically increasing demands on computing resources. Fig. 2 shows a hybrid mesh topology with a prismatic core and structured cells near the walls for the bend, meshes consisted of 800 000 cells, which approach the limit that can be handled with the computing resources available.

Fig. 2. Model with computational grid

These were specified the velocity at the inlet and the outflow at the outlet as boundary conditions for the pipe bend. The turbulence intensity I  0.16 Re1/ 8 was determined from the hypothesis for internal flows.

4

Computational Results

Results are presented for all three turbulence models, i.e., renormalization group (RNG) k-ε, realizable k-ε and RSM, and that in terms of pressure and velocity distributions of the pipe bend. Detailed pressure, velocity and pressure loss datum are then presented from the RSM predictions for each pipe bend with different Re and parameter δ. 4.1 Different turbulence model The contours of static pressure and velocity magnitude in central symmetry plane are presented for each of the three turbulence models, as shown in Fig. 3. The pressure is seen to be transversely uniform at the far upstream and downstream in the straight pipe region. A region of high pressure occurs at the outer wall of the bend as the flow decelerates, and almost the whole round bend is covered with the high pressure with both k-ε, whereas, only halfway of the bend is in high pressure by RSM. A region of low pressure is formed at the inner wall as the flow accelerates around the bend, and the low pressure region shows a further extension and more influence on the downstream flow than the both k-ε model. The velocity contour indicates that the RSM predicts a larger low velocity zone which locates at the downstream from the separation point. The flow attached to the wall and the pressure recovers to uniform with a constant axial gradient at approximately 6.5d downstream of the bend for the RNG k-ε model, 5d

·907·

for the realizable k-ε model and 10d for the RSM, respectively. The primary flow downstream is more closed to the inner wall for RNG k-ε model than for RSM, whereas the primary flow locates in centre of the bend for realizable k-ε model. The most significant flow feature of the bend is the secondary flow in the planes perpendicular to the primary flow. The secondary flow patterns at circular-sectional angle of θ90° (Fig. 1) location and 1d downstream of the bend are presented in Figs. 4 and 5, respectively. The three turbulence models predictions show similar patterns: at θ90° location, the two helical structures, which are symmetric about the center line, present in this cross section of the bend. Although the predicted flow patterns are similar for the three turbulence models, the secondary flow magnitudes are larger for the RSM, as indicated by the larger velocity vectors. This behavior is shown more prominent in the RSM prediction, which may be attributed to the ability of this model to account for anisotropy in the Reynolds stress field. As a result of the stronger secondary flows predicted by the RSM, the more low momentum fluid is entrained from the separated region by the high momentum flow, which accounts for the larger low pressure region observed from the RSM in Fig. 3. 4.2 Effect of Re and δ The pressure variations along the inner and outer walls of the bend in central symmetry plane with different Re and δ are given in Figs. 6 and 7. The assumption was made during the computation that the oil velocity v distribution at the inlet of the pipe bend is uniform and the flow direction is normal to the inlet cross section. Because of the fixed pipe diameter, oil density and viscosity, the Reynolds number Re only depends on the oil velocity v. For the inner wall, the flow was accelerated into the bend and the wall experienced a positive pressure gradient up to θ20° location. At further downstream, an adverse pressure gradient presented, causing the local flow separation, as shown in the predicted flow fields (Fig. 3). For the outer wall, on the contrary, an adverse pressure gradient presented first, and then a positive pressure gradient, with a transition zone between θ60° and θ70°. Moreover, the increment of Re leads to the results that the pressure gradient changes rapidly, especially at inner and outer walls downstream of the bend, and the lower and higher pressure come into being. As δ decreases gradually, namely, the curvature radius increases, the transition point of pressure gradient moves towards the inlet of the bend for the outer wall but keeps almost unchanged up to enough larger curvature for the inner wall. While Re increases at the lower δ, the two transition points of pressure gradient presented at θ20° location upstream and θ80° location downstream for the inner wall. Therefore, the pressure gradient and magnitude will depend on Reynolds number Re, and that the transition point or zone of pressure gradient is determined by curvature ratio δ.

·908·

YWANG Liwei, et al: Numerical Simulation of Turbulent Flow of Hydraulic Oil through 90° Circular-sectional BendY Velocity v(m • s–1) 1.53 1.37 1.22 1.07 0.92 0.76 0.61 0.46 0.30 0.15 0.00

Pressure pkPa 1.20 1.07 0.94 0.81 0.68 0.55 0.42 0.29 0.16 0.03 –0.10 (a) RNG k-ε

Velocity v(m • s–1) 1.47 1.33 1.18 1.03 0.88 0.74 0.59 0.44 0.30 0.15 0.00

Pressure pkPa 1.20 1.07 0.94 0.81 0.68 0.55 0.42 0.29 0.16 0.03 –0.10 (b) Realizable k-ε Pressure pkPa 1.20 1.07 0.94 0.81 0.68 0.55 0.42 0.29 0.16 0.03 –0.10

Velocity v(m • s–1) 1.64 1.48 1.31 1.15 0.98 0.82 0.66 0.49 0.33 0.16 0.00 (c) RSM

Fig. 3.

Contours of pressure and velocity in central symmetry plane of the bend for different turbulence model, δ0.5, v1 ms

(a) RNG k-ε

Fig. 4.

(c) RSM

Normalized velocity magnitude showing the secondary flow patterns of bend, θ90°, δ0.5, v1 ms

(a) RNG k-ε

Fig. 5.

(b) Realizable k-ε

(b) Realizable k-ε

(c) RSM

Normalized velocity magnitude showing the secondary flow patterns 1d downstream of bend, δ0.5, v1 ms

CHINESE JOURNAL OF MECHANICAL ENGINEERING

·909·

Fig. 6. Static pressure distribution along inner and outer walls of the bend with δ0.5

Fig. 7. Static pressure distribution along inner and outer walls of the bend with δ0.2

Generally, most bends used in hydraulic machine have been designed with reciprocal of curvature ratio δ, and Rr≤5. The total pressure loss predictions for the bends with Rr2, 2.5, 3, 3.5, 4, 4.5 and 5 at different Re are given in Fig. 8, expressed in which incorporate pressure loss factor k. This factor k is given by

k

∆p , 0.5 ρ v 2

the bend also lead to increasing of friction and separation effects, and magnified swirl intensity of secondary flow, despite of lower pressure loss factor k due to higher velocity heads.

(2)

where ∆p is the total pressure loss across a bend. In this case, the reference pressure was taken 5d upstream of the bend. It is known that the pressure loss for turbulent flow through 90° pipe bends arises from frictional and separate effects. The latter can be viewed as the sum of two separate effects. The first is due to the adverse pressure gradient at the outer wall, which results in excess friction at the outer wall of the bend. The second effect arises from the flow separating from the inner wall of the bend. Owing to the secondary flow, which adds significantly to the pressure loss, causing a rapid rise in pressure loss factor as the bend tightens, as shown in Fig. 8. Moreover, as Re increases, the rapid changes of pressure on the surface of

Fig. 8. Variation in total pressure loss with the R/r at different Re

In order to construct the mathematical models of the pressure loss in terms of Re and δ, the fitted formula involving factor k to be predicted, and can be expressed as

·910·

YWANG Liwei, et al: Numerical Simulation of Turbulent Flow of Hydraulic Oil through 90° Circular-sectional BendY k  Bδ A ,

(3)

where

[6]

A  1.67e13 Re3  7.53e9 Re 2  1.15e4 Re  0.094 3, B  41.954 Re0.383 6 .

5

[7]

[8]

Conclusions [9]

(1) For all the three turbulence models in terms of the predicted flow structures of hydraulic oil through 90° circular-sectional bend, the RSM is the best suited for the cases involving stronger secondary flows, although it requires additional computational effort. (2) The pressure gradient and magnitude will change with different Reynolds number Re, the increment of Re will leads to the results that the pressure gradient changes rapidly, especially at inner and outer walls downstream of the bend, and the lower and higher pressure come into being. The transition point or zone of pressure gradient is related with curvature ratio δ. As the curvature ratio δ decreases gradually, the transition point of pressure gradient moves towards the inlet of the bend for the outer wall but keeps almost unchanged up to an enough larger curvature for the inner wall. (3) Owing to the secondary flow, which adds significantly to the pressure loss, causing a rapid rise in pressure loss factor k as the bend tightens. A new mathematical model of the pressure loss in terms of Reynolds number Re and curvature ratio δ is proposed which offers accurate data to one-dimensional simulation software. (4) The above conclusions and data refer specifically to the oil flow in the large bends with higher Re and may not necessarily apply to other bends. References [1] DEAN W R. Fluid motion in a curved channel[J]. Proceedings of the Royal Society of London. Series A, 1928, 121(787): 402–420. [2] SHIRAYAMA S, KUWAHARA K. Computational study of flow in a curved pipe with circular cross section[J]. Journal of Mechanical Science and Technology, 1987, 1(1): 52–59. [3] LAI Y G, SO R M C, ZHANG H S. Turbulence-driven secondary flows in a curved pipe[J]. Theoretical and Computational Fluid Dynamics, 1991, 3(3): 163–180. [4] SHAO L, RIFFAT S B. Accuracy of CFD for predicting pressure losses in HVAC duct fittings[J]. Applied Energy, 1995, 51(3): 233–248. [5] CRAWFORD N, SPENCE S, SIMPSON A, et al. A numerical

[10]

[11]

[12]

[13]

[14]

[15]

[16]

investigation of the flow structures and losses for turbulent flow in 90° elbow bends[J]. Proc. IMechE, Part E: J. Process Mechanical Engineering, 2009, 223(1): 27–44. BERGER S A, TALBOT L, YAO L S. Flow in curved pipes[J]. Annual Review of Fluid Mech., 1983, 15: 461–512. CHEN Xuejun, ZHU Caiguang. An investigation on flow characteristics of air-water mixtures through angle pipes[J]. Chinese Journal of Mechanical Engineering, 1983, 19(3): 71–83. SUDO K, SUMIDA M, HIBARA H. Experimental investigation on turbulent flow in a circular-sectioned 90-degree bend[J]. Experiment in Fluids, 1998, 25(1): 42–49. JAKIRLIC S, HANJALIC K, TROPEA C. Modeling rotating and swirling turbulent flows: a perpetual challenge[J]. AIAA Journal, 2002, 40(10): 1 984–1 996. SPEDDING P L, BENARD E, MCNALLY G M. Fluid flow through 90 degree bends[J]. Dev. Chem. Eng. Mineral Process, 2004, 12(1–2): 107–128. ZHANG Shiqiao, YIN Zegao, MAO Genhai. Numerical simulation of turbulence in curved circular duct[J]. Journal of Hydroelectric Engineering, 2005, 24(3): 61–65. (in Chinese) ZHANG Dunfu, WANG Xiping, ZHANG Hongwei. Direct method for limit velocity of a semi-circle curved pipe conveying fluid[J]. Chinese Journal of Mechanical Engineering, 2005, 41(5): 221–224. (in Chinese) SPEDDING P L, BENARD E. Gas-liquid two phase flow through a vertical 90° elbow bend[J]. Experimental Thermal and Fluid Science, 2007, 31(7): 761–769. JIANG Shan, ZHANG Jingwei, WU Chongjian, et al. Numerical simulation of inner flow in 90° bending duct of circular-section based on FLUENT[J]. Chinese Journal of Ship Research, 2008, 3(1): 37–41. (in Chinese) LI Shengyuan, LIU Ningning, LI Yong. Numerical simulation on flow field of 90° elbow pipe[J]. Journal of Northeast Dianli University (Natural Science Edition), 2009, 29(1): 67–70. (in Chinese) YANG Xianglong, HUANG Shehua, XIONG Yuan. A comparative study of numerical simulation of turbulent flow in bending duct of circular-section and turbulence models[J]. Journal of Xi’an University of Technology, 2010, 26(1): 116–120. (in Chinese)

Biographical notes

WANG Liwei, born in 1980, is currently a PhD at Taiyuan Heavy Industry Co. Ltd., China. She received her PhD degree from Yanshan University, China, in 2009. Her research interests include hydraulic power transmission and control system. Tel: +86-13994280421; E-mail: [email protected] GAO Dianrong, born in 1962, is currently a professor at Yanshan University, China. He received his PhD degree from Yanshan Universtiy, China, in 2001. His research interests include numerical simulation and visualization of flow field. Tel: +86-13930349706; E-mail: [email protected] ZHANG Yigong, born in 1960, is currently a senior engineer at Taiyuan Heavy Industry Co. Ltd., China. Tel: +86-13903514663; E-mail: [email protected]