Numerical modeling of cavitation on spillway’s flip bucket

Abstract

Numerical modeling of hydraulic phenomenon by computational fluid dynamic (CFD) approaches is one of the main parts in the high cost hydraulic structure studies. In this paper, using Flow 3D as CFD commercial tool, the cavitation phenomenon was assessed along spillway's flip bucket of the Balaroud dam. Performance of numerical modeling was compared to the physical model, which was constructed to this purpose. During numerical modeling, it was found that RNG turbulence model is a suitable performance for modeling the cavitation. Physical modeling shows that minimum cavitation index is about 0.85 and minimum cavitation index based on Flow 3D results is about 0.665, which was related to the flood discharge with return period of 10000 years. The main difference between numerical and physical modeling is related to the head of velocity, which is considered in physical modeling. Results of numerical simulation show that occurrence of cavitation based on cavitation index equal to 0.25 is not possible along the spillway.

Keywords

cavitation Index / numerical simulation / spillway’s flip Bucket / CFD / Balaroud Dam / physical modeling

Introduction

Study of important hydraulic structures is usually based on physical modeling construction. Physical modeling of hydraulic structure is based on basic fluid mechanic Eq [ 1]. Spillways are one of the main parts of dam construction projects. Due to the importance of spillways in dam safety, study of hydraulic properties of this structure is conducted by numerical and physical modeling approaches [ 2]. Physical modeling is usually carried out by constructing a physical scale model in hydraulic laboratory. Physical scale model is a small size of prototype structure, the hydraulic properties of which is similar to prototype structure. Due to the high cost of physical modeling and the need for advance equipment, researchers used numerical methods along with physical modeling to reduce experimental costs [ 3– 10]. In the field of numerical modeling, governing flow equations which are usually Navier-Stokes (NS) equations are solved by various numerical methods such as finite volume and finite element [ 11, 12]. To simulate turbulent flow and to solve NS equation, many turbulence models including one equation models such as prandtl length and two equation models such as K-epsilon (k-e) turbulence model, Re-Normalization Group (RNG) methods have been proposed [ 13]. The main hazard of spillways is cavitation. To design a spillway, which is safe in terms of cavitation phenomenon, researchers have conducted several investigations on defining the condition of cavitation occurrence. Cavitation is evaporation process due to the reduction of local pressure in hydraulic structure where the temperature remains constant. Variation of roughness on the surface especially on concrete structures constructed by human causes of derivation of flow streamlines that leads to change in flow velocity ultimately redound to the cavitation [ 14, 15]. Reducing the pressure causes of evaporation and creation of bubbles, which moved along the flow and at the end bubbles are blowout when they are reached to the high-pressure zone. Blowing the bubbles sometimes creates a pressure close to 1000 mega Pascal on the surface [ 16, 17]. These values of pressure act on the fine area and create a huge force on the surface, which causes destruction of structure. This destruction occurs in high pressure zones such as chute spillway, flip bucket and stilling basin; therefore, this problem should be studied by physical and numerical modeling [ 12]. To avoid cavitation problem in hydraulic structures, especially spillways, the value and distribution of pressure and velocity should be defined in all parts of the structure [ 3]. Researcher proposed an index for defining structure potential to cavitation occurrences. This index is called cavitation index and is derived from Bernoulli equation as symptomatic of energy formula. Equation (1)–(3) shows derivation process of cavitation index. Equation (1) is Bernoulli equation which was hold between two points.

(1) {\displaystyle \frac{\rho V_o^{\mathrm{2}}}{\mathrm{2}}}+P_o+Z_o\rho g={\displaystyle \frac{\rho V^{\mathrm{2}}}{\mathrm{2}}}+P+Z\rho g,

where P_{\mathrm{o}} and V_{\mathrm{o}} are pressure and velocity of flow at the beginning of spillway and P and V are the desired location through the spillway. By a small change in Bernoulli equation, dimensionless form of energy formula can be derived as Eq. (2).

(2) {\displaystyle \frac{(P+\rho gZ)-(P_{\mathrm{o}}+\rho g{Z}_{\mathrm{o}})}{{\displaystyle \frac{\mathrm{1}}{\mathrm{2}}}\rho V^{\mathrm{2}}}}=\mathrm{1}-{\left({\displaystyle \frac{V}{V_{\mathrm{o}}}}\right)}^{\mathrm{2}}.

Since cavitation is direct proportional of pressure, height (Z) parameters has been disregarded. Therefore, Eq. (2) can be written as Eq. (3).

(3) {{\displaystyle C}}_{\mathrm{P}}={\displaystyle \frac{P-{{\displaystyle P}}_{\mathrm{0}}}{{\displaystyle \frac{\mathrm{1}}{\mathrm{2}}}p{{\displaystyle V}}_{\mathrm{0}}^{\mathrm{2}}}}.

C_{\mathrm{P}} is the cavitation index and reminds the Euler number. For spillways, especially the flip bucket part, Eq. (3) can be used as Eq. (4).

(4) \sigma ={\displaystyle \frac{{\displaystyle \frac{P_{\mathrm{A}\mathrm{m}}}{\gamma }}-{\displaystyle \frac{P_{\mathrm{v}}}{\gamma }}+h\cos (\theta )\pm ({\displaystyle \frac{h}{g}}\times {\displaystyle \frac{V_{\mathrm{o}}^{\mathrm{2}}}{r}})}{{\displaystyle \frac{V_{\mathrm{o}}^{\mathrm{2}}}{\mathrm{2}g}}}}.

Plus symbol is related to the concave and minus is related to the convex floor. In this equation, g is gravitational acceleration, \gamma is the specific weight, \theta is the angle of floor to horizontal surface, h is the flow depth and r is the radius of the floor curvature. Studying the cavitation, researchers proposed a critical value for cavitation occurrence, which was called {\sigma }_{\mathrm{c}\mathrm{r}} [ 3, 16, 18– 23]. Values of critical cavitation for spillways are between 0.20 and 0.25. The aim of this study was assessing the potential of Balaroud spillway for cavitation occurrence through chute spillway and flip bucket using physical and numerical modeling.

Materials and method

A physical scaled model of the Balaroud Dam spillway was constructed at the hydraulic laboratory of Shahid Chamran University, Ahvaz, Iran. The model scale was 1:40. The length of the chute spillway model is near to 9 m, depth of chute channel was 0.5 m and the channel chute width was 0.5 m. Figure 1 shows the Balaroud Spillway in laboratory. As shown in Fig. (1), about 37 stations were considered for measuring the Piezomertic Head and mean velocity.

Numerical modeling

Computational fluid dynamic (CFD) technique was used for modeling flow characteristics on Balaroud dam spillway. To this purpose, Flow 3D software was used for numerical modeling of the flow characteristics along the chute and flip bucket of spillway. Figure 2 shows a 3D modeling of Balaroud dam spillway.

Flow 3D software

Flow 3D is a commercial CFD tool, which is able to solve complex fluid dynamic problems. This software has high performance for modeling free surface flow in unsteady conditions. Volume of fluid technique has been used in this software for defining free surface flow. Regular mesh is used to discrete the computational domain. Flow 3D offers five types of turbulence models: Prandtl mixing length, K-e equation, RNG models, large eddy simulation (LES) model.

Review of the governing equations in Flow 3D software

The continuity equation at three-dimensional Cartesian coordinates is given as Eq. (5).

(5) v_{\mathrm{f}}{\displaystyle \frac{\partial \rho }{\partial t}}+{\displaystyle \frac{\partial }{\partial x}}(u{A}_x)+{\displaystyle \frac{\partial }{\partial x}}(v{A}_y)+{\displaystyle \frac{\partial }{\partial x}}(w{A}_z)={\displaystyle \frac{PSOR}{\rho }},

where u,v,z are velocity components in x,y,z directions; {\mathrm{A}}_x,{\mathrm{A}}_y,{\mathrm{A}}_z are cross sectional area of the flow, \rho is fluid density, PSOR is the source term, v_{\mathrm{f}} is the volume fraction of fluid and three-dimensional momentum equations are given in Eq. (6).

(6) \begin{array}{l}{\displaystyle \frac{\partial u}{\partial t}}+{\displaystyle \frac{\mathrm{1}}{v_f}}\left(u{A}_x{\displaystyle \frac{\partial u}{\partial x}}+v{A}_y{\displaystyle \frac{\partial u}{\partial y}}+w{A}_z{\displaystyle \frac{\partial u}{\partial z}}\right)=-{\displaystyle \frac{\mathrm{1}}{\rho }}{\displaystyle \frac{\partial P}{\partial x}}+G_x+f_x\\ {\displaystyle \frac{\partial v}{\partial t}}+{\displaystyle \frac{\mathrm{1}}{v_f}}\left(u{A}_x{\displaystyle \frac{\partial v}{\partial x}}+v{A}_y{\displaystyle \frac{\partial v}{\partial y}}+w{A}_z{\displaystyle \frac{\partial v}{\partial z}}\right)=-{\displaystyle \frac{\mathrm{1}}{\rho }}{\displaystyle \frac{\partial P}{\partial y}}+G_y+f_y,\\ {\displaystyle \frac{\partial w}{\partial t}}+{\displaystyle \frac{\mathrm{1}}{v_f}}\left(u{A}_x{\displaystyle \frac{\partial w}{\partial x}}+v{A}_y{\displaystyle \frac{\partial w}{\partial y}}+w{A}_z{\displaystyle \frac{\partial w}{\partial z}}\right)=-{\displaystyle \frac{\mathrm{1}}{\rho }}{\displaystyle \frac{\partial P}{\partial y}}+G_z+f_z\end{array}

where P is the fluid pressure, G_x,G_y,G_z are acceleration created by body fluids f_x,f_y,f_z are viscosity acceleration in three dimensions and v_{\mathrm{f}} is related to the volume of fluid, defined as Eq. (7). For modeling free surface profile, VOF technique has been used based on volume fraction of computational cells. Since the volume fraction F represents the amount of fluid in each cell, it takes a value between 0 and 1.

(7) {\displaystyle \frac{\partial F}{\partial t}}+{\displaystyle \frac{\mathrm{1}}{v_{\mathrm{f}}}}\left[{\displaystyle \frac{\partial }{\partial x}}(F{A}_{x}u)+{\displaystyle \frac{\partial }{\partial y}}(F{A}_{y}v)+{\displaystyle \frac{\partial }{\partial y}}(F{A}_{z}w)\right]=\mathrm{0}

Modeling turbulent flow requires defining suitable turbulence model, which creates close form with Navier-Stokes equation. Re-Normalization Group (RNG) model is a powerful turbulence model which has suitable performance for modeling the fine cavity, therefore, this model is very useful for modeling cavitation problems. Most equations used in RNG model are given in Eqs. (8) and (9).

(8) {\displaystyle \frac{\partial }{\partial t}}(\rho k)+{\displaystyle \frac{\partial }{\partial x}}(\rho u_{i}k)={\displaystyle \frac{\partial }{\partial x_i}}\left({\alpha }_k{\mu }_{eff}{\displaystyle \frac{\partial k}{\partial x_i}}\right)+G_k+G_b-\rho \epsilon ,

(9) {\displaystyle \frac{\partial }{\partial t}}(\rho \epsilon )+{\displaystyle \frac{\partial }{\partial x}}(\rho u_i\epsilon )={\displaystyle \frac{\partial }{\partial x_i}}\left({\alpha }_k{\mu }_{eff}{\displaystyle \frac{\partial \epsilon }{\partial x_i}}\right)+C_{\mathrm{1}\epsilon }{\displaystyle \frac{\epsilon }{k}}(G_k+C_{\mathrm{3}\epsilon }{G}_b)-C_{\mathrm{2}\epsilon }\rho {\displaystyle \frac{{\epsilon }^{\mathrm{2}}}{k}}-R.

In which G_{\mathrm{k}} is the rate kinetic energy creation, R is the density of turbulence defined as below.

(10) R={\displaystyle \frac{C_{\mu }\rho {\eta }^{\mathrm{3}}(\mathrm{1}-\eta /{\eta }_{\mathrm{0}})}{\mathrm{1}+\beta {\eta }^{\mathrm{3}}}}{\displaystyle \frac{{\epsilon }^{\mathrm{2}}}{k}},{\mu }_{\mathrm{t}}=\rho C_{\mu }{\displaystyle \frac{k^{\mathrm{2}}}{\epsilon }}

In these equations \beta =\mathrm{0.012},{\eta }_{\mathrm{0}}=\mathrm{1.38.}

Steps of problem solving in Flow 3D software

Computational modeling of hydraulic phenomenon by Flow 3D involved some steps given as follows: 1- Preparing 3D model by AutoCAD software and exporting 3d model with STL suffix file; 2- Summon STL file in Flow 3D software and defining the fluid properties in the software and meshing the computational domain which is usually bigger than the hydraulic structure, During CFD modeling it was attempted to refine size of meshes sufficiently; 3- Choosing the basic equations that should be solved; 4- Defining the boundary and initial conditions; 5- Adjusting the control parameters and outputs; 6- Choosing the calculation method; and 7- Running the software. Defining the mesh size and boundary conditions is an important stage of simulation with Flow 3D software. This software has a wide range of boundary conditions. Figure (3) shows the 3D modeling of Balaroud Dam spillway in Flow 3D software.

Results and discussion

Performance of Balaroud scaled model during experiments and numerical simulation was assessed and is given in Figs. 4, 5 and 6. Figures (4, 5 and 6 are the results of running Flow 3D for flow discharges of 0.0667(m³/s), 0.0859 (m³/s), and 0.1903 (m³/s). These figures show the pressure distribution along the spillway at each discharge as well. To choose the best turbulence model with the best suitable performance, a try and error process was conducted; however, recommendations proposed by Erfanain-Azmoudeh and Kamanbedast [ 24] and Chanel and Doering [ 25] were considered. During numerical simulation, RNG turbulence model has the best performance to define cavitation occurrence through spillway. For evaluating the potential of flip bucket for cavitation occurrence, four flood discharges with return periods of 2, 100, 1000 and 10000 years were considered for measuring flow characteristics such as pressure and velocity. Flood discharge related to return period in laboratory was equal to 0.0667 (m³/s), 0.0859 (m³/s), 0.160 (m³/s), and 0.1903 (m³/s), consecutively. As mentioned in the literature, the high-pressure zones are susceptible areas for occurrence of cavitation phenomenon. Therefore, as could be seen from Fig. 7, the area near flip bucket has the potential of cavitation, because these areas are placed in high-pressure zone, therefore, the focus of analysis was on these area for cavitation occurrence. The piezometer number of 22 to 37 was placed on the flip bucket part. Results of cavitation index calculation both with experimental measurement approach and Flow 3D modeling for each flood discharges are given in Table (1). Figures 8, 9 and 10 show cavitation index along the flip bucket. As shown in Figs. 8-10, by receding from the crest, cavitation index is decreased because of the increase in flow velocity and then head pressure decreased. This decrease in cavitation index for all flood discharge values continues to flip bucket structure when flow reaches the flip bucket, since the concave curve shape for the flip bucket causes the increasing in pressure and thus cavitation index increases. The main difference between measured data and Flow 3D results is related to the velocity head. In Flow 3D results, the pure pressure is directly derived whereas in physical model measurement, the Piezomertic Head is considered, which is included in velocity head in addition to the pressure head. The minimum value of cavitation index is about 0.655 that occurs in maximum flood discharge related to flood with return period of 10000 years. Overall, Figs. 8-10 show that the design of Balaroud Dam spillway is safe versus cavitation index.

Conclusions

Study on hydraulic structure characteristics is usually conducted by physical and numerical modeling. Among hydraulic structures, dam spillways are one of the most important structures, which require applying both physical and numerical approaches. The main hazard of spillways is cavitation, which in most cases leads to destruction of overall structure. Results of this study show that physical modeling and numerical simulation of flow over different parts of spillway structures including chute, flip bucket and staling basin helps to control the structure safety versus cavitation and other hazards. Result of minimum cavitation index of Balaroud is about 0.665, which occurs at flood discharge with return period of 10000 years and it means that Balaroud spillway is safe against cavitation.

References

[1] Ettema R. Hydraulic Modeling: Concepts and Practice. ASCE, 2000

[2] Chau K W. Modelling for Coastal Hydraulics and Engineering. Taylor & Francis, 2010

[3] Fattor C, Bacchiega J. Design Conditions for Morning-Glory Spillways: Application to Potrerillos Dam Spillway. In: Advances in Water Resources and Hydraulic Engineering, Springer Berlin Heidelberg. 2009, 2123–2128.

[4] Gourbesville P, Cunge J, Caignaert G. Advances in Hydroinformatics: SIMHYDRO 2012 – New Frontiers of Simulation. Springer Singapore Pte. Limited, 2013

[5] Parsaie A, Haghiabi A. The effect of predicting discharge coefficient by neural network on increasing the numerical modeling accuracy of flow over side weir. Water Resources Management, 2015, 29(4): 973–985

[6] Parsaie A, Yonesi H, Najafian S. Predictive modeling of discharge in compound open channel by support vector machine technique. Modeling Earth Systems and Environment, 2015, 1(2): 1–6

[7] Parsaie A, Haghiabi A, Moradinejad A. CFD modeling of flow pattern in spillway’s approach channel. Sustainable Water Resources Management, 2015, 1(3): 245–251

[8] Parsaie A, Haghiabi A. Computational Modeling of Pollution Transmission in Rivers. Applied Water Science, 2015, 1–10

[9] Parsaie A, Haghiabi A. Predicting the longitudinal dispersion coefficient by radial basis function neural network. Modeling Earth Systems and Environment, 2015, 1(4): 1–8

[10] Parsaie A, Yonesi H, Najafian S. Predictive modeling of discharge in compound open channel by support vector machine technique. Modeling Earth Systems and Environment, 2015, 1(1–2): 1–6

[11] Kim D, Park J. Analysis of flow structure over ogee-spillway in consideration of scale and roughness effects by using CFD model. KSCE Journal of Civil Engineering, 2005, 9(2): 161–169

[12] Gessler D. CFD modeling of spillway performance. In: Proc. World Water and Environmental Resources Congress. May, 2005

[13] Aydin M C. CFD simulation of free-surface flow over triangular labyrinth side weir. Advances in Engineering Software, 2012, 45(1): 159–166

[14] Johnson M C, Savage B M. Physical and numerical comparison of flow over ogee spillway in the presence of tailwater. Journal of Hydraulic Engineering, 2006, 132(12): 1353–1357

[15] Chanson H. 19- Design of weirs and spillways, in Hydraulics of Open Channel Flow. 2nd ed. Chanson H, 2004, Oxford: Butterworth-Heinemann, 2004, 391–430

[16] Wu J, Ma F. Cavity flow regime for spillway aerators. Science China Technological Sciences, 2013, 56(4): 818–823

[17] Dong Z Y, Chen L, Ju W J. Cavitation characteristics of high velocity flow with and without aeration on the order of 50 m/s. Journal of Hydrodynamics. Ser. B, 2007, 19(4): 429–433

[18] Chatila J, Tabbara M. Computational modeling of flow over an ogee spillway. Computers & Structures, 2004, 82(22): 1805–1812

[19] Toloshinov A V, . Development of the design for the No. 2 spillway at the Boguchany hydroproject. Power Technology and Engineering, 2009, 43(3): 135–142

[20] Szymkiewicz R. Numerical Modeling in Open Channel Hydraulics. Springer, 2010

[21] Kirkgoz M S, Akoz M S, Oner A A. Numerical modeling of flow over a chute spillway. Journal of Hydraulic Research, 2009, 47(6): 790–797

[22] Lv J, Liu M. Research to the Stilling Basin Types of the Spillway Outlet. In: Advances in Water Resources and Hydraulic Engineering. Springer Berlin Heidelberg, 2009, 1536–1540

[23] Aydin M C, Ozturk M. Verification and validation of a computational fluid dynamics (CFD) model for air entrainment at spillway aerators. Canadian Journal of Civil Engineering, 2009, 36(5): 826–836

[24] Erfanain-Azmoudeh M H, Kamanbedast A A. Determine the appropriate location of aerator system on Gotvandoliadam’s spillway using Flow 3D. American-Eurasian Journal of Agricultural & Environmental Sciences, 2013, 13(3): 378–383

[25] Chanel P G, Doering J C. Assessment of spillway modeling using computational fluid dynamics. Canadian Journal of Civil Engineering, 2008, 35(12): 1481–1485

RIGHTS & PERMISSIONS

Higher Education Press and Springer-Verlag Berlin Heidelberg