# Assessment of CFD Solvers and Turbulent Models for Water Free Jets in Spillways

^{1}

^{2}

^{*}

## Abstract

**:**

^{®}solvers, namely interFoam and twoPhaseEulerFoam, in reproducing the behavior of a free water jet was investigated. Numerical simulations were performed in order to obtain the velocity and air concentration profiles along the jet. The turbulence intensity was also analyzed. The obtained results were compared with published experimental data and, in general, similar velocity and air concentration profiles were found. InterFoam solver is able to reproduce the velocity field of the free jet but has limitations in the simulation of the air concentration. TwoPhaseEulerFoam performs better in reproducing the air concentration along the jet, the results being in agreement with the experimental data, although the computational runs are less stable and more time consuming. The sensitivity analysis of the inlet turbulent intensity showed that it has no influence in the characteristics of the jet core. With this research it is possible to conclude that: interFoam with k-Epsilon (k-ε) turbulence model is the best choice if the goal of the numerical simulations is the simulation of the velocity field of the jet. Meanwhile, twoPhaseEulerFoam with mixturek-Epsilon (mk-ε) shall be considered if the objective is the simulation of the velocity field and the air concentration.

## 1. Introduction

^{®}code, a C++ library enabling the simulation of a wide range of engineering cases, incorporating a number of solvers that cover many types of problems in continuous mechanics, such as the interFoam and twoPhaseEulerFoam solvers which were used in this study. Both solvers can model water–air flows by solving a full version of the Navier–Stokes equations. To capture the free surface position, each solver uses a specific methodology [18,19,20].

## 2. Numerical Modelling

#### 2.1. Comparison of the Used Solvers

- subscript $\mathsf{\phi}$ defines the phase;
- ${\mathsf{\alpha}}_{\mathsf{\phi}}$—phase fraction;
- ${\mathrm{u}}_{\mathsf{\phi}}$—velocity;
- $\mathrm{p}$—pressure;
- ${\mathrm{R}}_{\mathsf{\phi}}^{-\mathrm{eff}}$—combined turbulent (Reynolds) and viscous stress;
- ${\mathrm{M}}_{\mathsf{\phi}}$—inter-phase momentum transfer term.

#### 2.2. Turbulence Models

_{air}/Vol

_{tot}) The turbulent kinetic energy and the turbulent kinetic energy dissipation rate implemented in k-ε model are present in Equations (5) and (6). In the same way, in Equations (7) and (8), the turbulent kinetic energy and the turbulent kinetic energy dissipation rate used by SST k-$\mathsf{\omega}$ are represented.

- $\mathrm{k}$—turbulent kinetic energy;
- ${D}_{k}$—effective diffusivity for $\mathrm{k}$;
- ${T}_{p}$—turbulent kinetic energy production rate;
- $\mathsf{\epsilon}$—turbulent kinetic energy dissipation rate;
- ${D}_{\mathsf{\epsilon}}$—effective diffusivity for $\mathsf{\epsilon}$;
- ${c}_{1}$, ${c}_{2}$ and ${c}_{3}$—model coefficients, ${c}_{1}=1.44$, ${c}_{2}=1.92$, ${c}_{3}=0.00$;
- $\mathrm{G}$—turbulent kinetic energy production rate;
- ${\beta}^{*}$—model coefficient, ${\beta}^{*}=0.09$;
- ${S}_{k}$—internal source term for k
- $\mathsf{\Omega}$—turbulent kinetic energy dissipation rate;
- ${D}_{\mathsf{\omega}}$—effective diffusivity for $\mathsf{\omega}$;
- $\nu $—viscosity;
- $\beta $—closure coefficient;
- ${F}_{1}$—lending function;
- $C{D}_{k\mathsf{\omega}}=max\left(2{\mathsf{\rho}\mathsf{\sigma}}_{\mathsf{\omega}2}\frac{1}{\mathsf{\omega}}\frac{\delta k}{\delta {x}_{i}}\frac{\delta \mathsf{\omega}}{\delta {x}_{i}},{10}^{-10}\right)$;
- ${S}_{\mathsf{\omega}}$—internal source term for $\mathsf{\omega}$.

#### 2.3. Mesh

_{0}) wide channel, with a 0.143 m (h) free overfall at the downstream end, followed by a 0.250 m (W) wide channel. The step is located 0.620 m (x

_{0}) downstream of a sluice gate, which controls the flow in the channel (Figure 1).

^{+}in the last section of the approach channel are present.

_{0}), and at a downstream cross-section, at x = 0.10 m (S

_{1}).

- $\mathrm{z}$—vertical distance (m);
- ${\mathrm{z}}_{50}^{\mathrm{UpperNappe}}$—vertical distance of the point with C = 0.5 in the upper nappe to the floor (m);
- ${\mathrm{z}}_{50}^{\mathrm{LowerNappe}}$—vertical distance of the point with C = 0.5 in the lower nappe to the floor (m);
- ${\mathrm{d}}_{0}$—approach flow depth (m);
- $\mathrm{V}$ —flow velocity (m/s);
- ${\mathrm{V}}_{\mathrm{p}}$—potential velocity of the flow at a cross-section (m/s);
- $\mathrm{x}$—distance from the step (m).

_{0}(x = 0.000 m, Figure 4), the velocity profiles from interFoam solver with k-ε turbulent model present negligible differences between meshes, all being able to reproduce the boundary layer development of the approach flow at the step brink. In the section S

_{1}(x = 0.100 m), mesh 1 produces results differing significantly from those produced by the other two meshes, these being almost coincident. With mesh 1, the velocity profile of the jet lower nappe deviates from the experimental results, whereas meshes 2 and 3 allow a good agreement with the experimental results. The experimental data were obtained based on five different sets of experiments. Due to that, it is likely that they present some inherent scatter along the different profiles when compared with the numerical results, where the data from the three meshes are almost identical.

_{0}. In the comparison with Toombes and Chanson [9] results, a good agreement is observed. For the cross-section S

_{1}, similar to interFoam, mesh 1 produced some deviations from the experimental ones in the lower nappe zone, whereas mesh 2 and mesh 3 present analogous results and an adequate agreement with the experimental velocity profiles.

#### 2.4. Boundary Conditions

^{−7}). An open boundary was assumed on the right side of the domain. An inlet outlet velocity boundary condition was defined in this boundary. With this boundary condition, the velocity is allowed to leave the domain and to enter with a fixed value equal to a zero vector. All the other variables were left as a zero-order interpolation. The approach channel has a fixed wall with known roughness, velocity equal to zero and wall functions in the turbulent parameters which constrain the turbulence dissipation for low and high Reynolds numbers. To reduce the total simulation computational effort some simplifications were introduced. The downstream jet impact zone was left as an outlet boundary, as the flow in this area does not affect the free jet flow conditions. This type of boundary condition also easily enables the establishment of atmospheric pressure zone under the jet with the adopted 2D numerical modelling, as was the case in the experimental facility, although through a lateral expansion of the channel side walls (plan view in Figure 1). To validate this simplification, a simulation with a closed boundary under the jet and an open flow boundary at the right end of the domain was made. The imposed properties of the boundary conditions in the impact zone for this simulation have the same characteristics of the upstream channel boundary. In this simulation an additional pressure inlet boundary was created in the step wall in order to maintain atmospheric pressure around the jet. The results show no influence of the simplified boundary condition in the free jet characteristics, and thus it was adopted as it allows a significant reduction of the computational times. With these boundary conditions it was possible to obtain a flow in the domain with the same general characteristics of the experimental facility.

_{i}= 3.75 m/s, of the left side boundary condition were imposed. Regarding the simulations with mesh 2, and then, with mesh 3, initial conditions were derived from results produced by the previous coarser mesh.

#### 2.5. Numerical Schemes

## 3. Results and Discussion

#### 3.1. Velocity

#### 3.2. Air Concentration

#### 3.3. Turbulence Intensity

## 4. Conclusions

## Author Contributions

## Funding

## Conflicts of Interest

## References

- Heller, V.; Hager, W.H.; Minor, H. Ski Jump Hydraulics. J. Hydraul. Eng.
**2005**, 131, 46–51. [Google Scholar] [CrossRef] - Bollaert, E.F.R.; Schleiss, A.J. Scour of rock due to the impact of plunging high velocity jets Part I: A state-of-the-art review. J. Hydraul. Res.
**2003**, 41, 451–464. [Google Scholar] [CrossRef] - Whittaker, J.G.; Schleiss, A.J. Scour Related to Energy Dissipaters for High. In Head Structures ETHZ VAW Report No. 73; Swiss Federal Institute of Technology Zurich: Zürich, Switzerland, 1984. [Google Scholar]
- Duarte, R.; Bollaert, E.F.R.; Schleiss, A.J.; Pinheiro, A. Dynamic pressures around a confined block impacted by plunging aerated high-velocity jets. In Proceedings of the 2nd European IAHR Congress, Munich, Germany, 27–29 June 2012. [Google Scholar]
- Beltaos, S.; Rajaratnam, N. Plane Turbulent Impinging Jets. J. Hydraul. Res.
**1973**, 11, 29–59. [Google Scholar] [CrossRef] - Ervine, D.A.; Elsawy, E.M. Effect of turbulence intensity on the rate of air entrainment by plunging water jets. Proc. Inst. Civ. Eng.
**1980**, 69, 425–445. [Google Scholar] [CrossRef] - Ervine, D.A.; Falvey, H.T. Behavior of Turbulent Water Jets in the Atmosphere and in Plunge Pools. Proc. Inst. Civ. Eng.
**1987**, 83, 295–314. [Google Scholar] - Rajaratnam, N.; Rizvi, S.A.H.; Steffler, P.M.; Smy, P.R. An experimental study of very high velocity circular water jets in air. J. Hydraul. Res.
**1994**, 32, 461–470. [Google Scholar] [CrossRef] - Toombes, L.; Chanson, H. Free-surface aeration and momentum exchange at a bottom outlet. J. Hydraul. Res.
**2007**, 45, 100–110. [Google Scholar] [CrossRef] - Lin, C.; Hwung, W.Y.; Hsieh, S.C.; Chang, K.A. Experimental study on mean velocity characteristics of flow over vertical drop. J. Hydraul. Res.
**2007**, 45, 33–42. [Google Scholar] [CrossRef] - Steiner, R.; Heller, V.; Hager, W.H.; Minor, H.-E. Deflector Ski Jump Hydraulics Remo. J. Hydraul. Eng.
**2008**, 134, 1094–1100. [Google Scholar] [CrossRef] - Pfister, M.; Hager, W.H.; Boes, R.M. Trajectories and air flow features of ski jump-generated jets. J. Hydraul. Res.
**2014**, 52, 336–346. [Google Scholar] [CrossRef] - Ho, D.K.H.; Riddette, K.M. Application of computational fluid dynamics to evaluate hydraulic performance of spillways in Australia. Aust. J. Civ. Eng.
**2010**, 6, 81–104. [Google Scholar] [CrossRef] - Deshpande, S.S.; Trujillo, M.F.; Wu, X.; Chahine, G. Computational and experimental characterization of a liquid jet plunging into a quiescent pool at shallow inclination. J. Heat Fluid Flow
**2012**, 34, 1–14. [Google Scholar] [CrossRef] - Castillo, L.G.; Carrillo, J.M.; Sordo-Ward, Á. Simulation of overflow nappe impingement jets. J. Hydroinformatics
**2014**, 16, 922–940. [Google Scholar] [CrossRef] [Green Version] - Shonibare, O.Y.; Wardle, K.E. Numerical investigation of vertical plunging jet using a hybrid multifluid-VOF multiphase CFD solver. Int. J. Chem. Eng.
**2015**. [Google Scholar] [CrossRef] - Castillo, L.G.; Carrillo, J.M.; Bombardelli, F.A. Distribution of mean flow and turbulence statistics in plunge pools. J. Hydroinformatics
**2017**, 19, 173–190. [Google Scholar] [CrossRef] - OpenCFD Limited. OpenFOAM User Guide; OpenCFD Limited: Bracknell, UK, 2018. [Google Scholar]
- Manafpour, M.; Ebrahimnezhadian, H. The Multiphase Capability of Openfoam CFD Toolbox in Solving Flow Field in Hydraulic Structure. In Proceedings of the 4th International Conference on Long-Term Behavior and Eco-Friendly Dams, Tehran, Iran, 17–19 October 2017; pp. 323–330. [Google Scholar] [CrossRef]
- Schulze, L.; Thorenz, C. The Multiphase Capabilities of the CFD Toolbox OpenFOAM for Hydraulic Engineering Applications. In Proceedings of the ICHE 2014, Hamburg, Germany, 28 September–2 October 2014; pp. 1007–1014. [Google Scholar]
- Bombardelli, F. Computational multi-phase fluid dynamics to address flows past hydraulic structures. In Proceedings of the 4th IAHR International Symposium on Hydraulic Structures, Porto, Portugal, 9–11 February 2012. [Google Scholar]
- Wang, Y.; Politano, M.; Weber, L. Spillway jet regime and total dissolved gas prediction with a multiphase flow model. J. Hydraul. Res.
**2019**, 57, 26–38. [Google Scholar] [CrossRef] - Deshpande, S.S.; Anumolu, L.; Trujillo, M.F. Evaluating the performance of the two-phase flow solver interFoam. Comput. Sci. Discov.
**2012**, 5, 014016. [Google Scholar] [CrossRef] - Issa, R.I. Solution of the implicitly discretized fluid flow equations by operator-splitting. J. Comput. Phys.
**1986**, 62, 40–65. [Google Scholar] [CrossRef] - Behzadi, A.; Issa, R.I.; Rusche, H. Modelling of dispersed bubble and droplet flow at high phase fractions. Chem. Eng. Sci.
**2004**, 59, 759–770. [Google Scholar] [CrossRef] - Launder, B.E.; Spalding, D.B. The numerical computation of turbulent flows. Comput. Methods Appl. Mech. Eng.
**1974**, 3, 269–289. [Google Scholar] [CrossRef] - Menter, F.R. Two-equation eddy-viscosity turbulence models for engineering applications. AIAA J.
**1994**, 32, 1598–1605. [Google Scholar] [CrossRef] [Green Version] - Menter, F.R.; Kuntz, M.; Langtry, R. Ten Years of Industrial Experience with the SST Turbulence Model. Turbul. Heat Mass Transfer.
**2003**, 4, 625–632. [Google Scholar] - Rusche, H. Compaction of a Clay Loam Soil in Pannonian Region of Croatia under Different Tillage Systems. Ph.D. Thesis, Imperial College of Science, Technology & Medicine, London, UK, 2002. [Google Scholar]
- Falvey, H.T. Air-Water Hydraulic Flow in Structures; Engineering Monograph No. 41; United States Department of the Interior, Water and Power Resources Service: Denver, CO, USA, 1980.
- Chanson, H. Velocity measurements within high velocity air-water jets. J. Hydraul. Res.
**1993**, 31, 365–382. [Google Scholar] [CrossRef] [Green Version]

**Figure 1.**Scheme of the experimental facility (adapted from [9]).

**Figure 6.**(

**a**) CFD domain boundary definition and initial condition of water volume fraction for simulations with mesh 1; (

**b**) side left velocity profile.

**Figure 7.**Velocity field along the free jet for V

_{i}= 3.75 m/s and d

_{0}= 0.0296 m: (

**a**) interFoam solver with, k-ε; (

**b**) twoPhaseEulerFoam with mk-ε.

**Figure 8.**Dimensionless velocity profiles along the free jet for V

_{i}= 3.75 m/s and d

_{0}= 0.0296 m.

**Figure 9.**Dimensionless velocity profiles along the free jet for V

_{i}= 3.75 m/s and d

_{0}= 0.0296 m with interFoam solver, k-ε and SST k-$\mathsf{\omega}$ turbulence models.

**Figure 10.**Dimensionless velocity profiles along the free jet for V

_{i}= 3.75 m/s and d

_{0}= 0.0296 m with twoPhaseEulerFoam solver, mk-ε and SST k-$\mathsf{\omega}$ turbulence models.

**Figure 11.**Air concentration along the free jet for V

_{i}= 3.75 m/s and d

_{0}= 0.0296 m: (

**a**) interFoam solver with k-ε; (

**b**) twoPhaseEulerFoam with mk-ε..

**Figure 12.**Dimensionless air concentration distribution in the free jet with interFoam solver for V

_{i}= 3.75 m/s and d

_{0}= 0.0296 m.

**Figure 13.**Dimensionless air concentration distribution in the free jet with twoPhaseEulerFoam solver for V

_{i}= 3.75 m/s and d

_{0}= 0.0296 m.

Features | interFoam | twoPhaseEulerFoam |
---|---|---|

Formulation | Euler-Euler (VOF) | Euler-Euler (Dispersed) |

Phases | Two continuous | One continuous One dispersed |

Mass and momentum equations | One set of equations | Two sets of equations |

Interphase mass and momentum transfer | No | Yes |

Mesh | Sub-Domains | Cell Dimensions (mm) | Number of Cells in a Cross-Section of the Jet | Total Number of Cells of the Mesh | y^{+} |
---|---|---|---|---|---|

1 | All domain | 2.00 | ≈15 | 86.430 | 150 |

2 | Far from the jet Jet and vicinity | 2.00 1.00 | ≈30 | 227.545 | 75 |

3 | Far from the jet Jet and vicinity | 2.00 0.25 | ≈120 | 2.074.297 | 75 |

Term | interFoam | twoPhaseEulerFoam |
---|---|---|

convection | Gauss Van Leer | Gauss Van Leer |

artificial compression | Gauss linear | Gauss Van Leer |

momentum transport | Gauss linear Upwind grad(U) | Gauss upwind |

turbulence | Gauss upwind | Gauss upwind |

Inlet Turbulence Intensity (%) | interFoam (%) | twoPhaseEulerFoam (%) |
---|---|---|

10.00 | 1.86 | 2.67 |

1.00 | 1.83 | 2.65 |

0.10 | 1.93 | 2.66 |

0.01 | 1.87 | 2.75 |

© 2020 by the authors. Licensee MDPI, Basel, Switzerland. This article is an open access article distributed under the terms and conditions of the Creative Commons Attribution (CC BY) license (http://creativecommons.org/licenses/by/4.0/).

## Share and Cite

**MDPI and ACS Style**

Muralha, A.; Melo, J.F.; Ramos, H.M.
Assessment of CFD Solvers and Turbulent Models for Water Free Jets in Spillways. *Fluids* **2020**, *5*, 104.
https://doi.org/10.3390/fluids5030104

**AMA Style**

Muralha A, Melo JF, Ramos HM.
Assessment of CFD Solvers and Turbulent Models for Water Free Jets in Spillways. *Fluids*. 2020; 5(3):104.
https://doi.org/10.3390/fluids5030104

**Chicago/Turabian Style**

Muralha, António, José F. Melo, and Helena M. Ramos.
2020. "Assessment of CFD Solvers and Turbulent Models for Water Free Jets in Spillways" *Fluids* 5, no. 3: 104.
https://doi.org/10.3390/fluids5030104