Three-dimensional numerical analysis of a dam-break using OpenFOAM

Abstract. This paper presents a 3D numerical analysis of flow field patterns in a dam break laboratory scale by applying the numerical code based on Finite Volume Method (FVM), OpenFOAM. In the numerical model the turbulence is treated with RANS methodology and the VOF (Volume of Fluid) method is used to capture the free surface of the water. The numerical results of the code are assessed against experimental data. Water depth and pressure measures are used to validate the numerical model. The results demonstrate that the 3D numerical code satisfactorily reproduce the temporal variation of these variables.

Three-dimensional numerical analysis of a dam-break using OpenFOAM

Introduction
A dam is an engineering structure constructed across a valley or natural depression to create a water storage reservoir. The fast-moving flood wave caused by a dam failure can result in the loss of human lives, great amount of property damage, and have a severe environmental impact. Therefore, significant efforts have been carried out over the last years to obtain satisfactory mathematical numerical solutions for this problem. Due to advances in computational power and the associated reduction in computational time, three-dimensional (3D) numerical models based on Navier Stokes equations have become a feasible tool to analyze the flow pattern in those days.
Sánchez-Cordero E., Gómez M., Bladé E. Three-dimensional numerical analysis of a dam-break using OpenFOAM. Analytical studies of the dam break for a horizontal channel were performed by Dressler [1]. Several numerical studies based on 2D approaches have been validated against experimental data sets as demonstrated in [2] and [3]. Two dimensional numerical models assume negligible vertical velocities and accelerations which results in a hydrostatic pressure distribution. However, when an abrupt failure of a dam happens, in which initially a high free surface gradients occurs, the hydrostatic pressure assumption is no longer valid. Three dimensional numerical models have been used to solve the structure of the flow in these areas. This document presents a 3D numerical analyze of a dam break (laboratory scale) using the numerical code based on the finite volume method (FVM) -OpenFOAM. Turbulence is treated using Reynolds-averaged Navier Stokes equations (RANS) k-ε (RNG) approach, and the volume of fluid (VOF) method is used to simulate the airwater interface. The numerical results of the code are assessed against experimental data obtained by Kleefsman et al [4]. Water depth and pressure measures are used to validate the model. The results demonstrate that the 3D numerical code satisfactorily reproduce the temporal variation of these variables.

Fluid Flow model
The governing equations for mass and momentum for the fluid flow can be expressed as [5]: where u is velocity vector field, is the pressure field, is the turbulent eddy viscosity, strain tensor ( = 1 2 ⁄ (∇ + ∇ ) , surface tension, surface curvature, and volume fraction function (between 0-1).

Free surface model
Volume of Fluid Method (VOF) is used for the analysis of free surface flow. A volume fraction indicator is used to determine the fluid contained at each mesh element. To calculate a new transport equation is introduced.
OpenFOAM imposes the third term of equation (3) called phase compression; where, = − . The density and viscosity in the domain are given by: where l and g denotes the different fluids (water and air).

Turbulence model
In the RANS equations the instantaneous variables of flow are decomposed into their time-averaged and fluctuating quantities. In this analysis k-ε (RNG) turbulence model is used due to provides an improved performance for types of flows that include flows with separation zones [6]. It is a two equation model which provides independent transport equations for both the turbulence length scale and the turbulent kinetic energy.

Initial and Boundary Conditions
In the numerical configuration of the model, the sides surrounding the experiment and the bottom are defined as wall. The top of the experimental box atmospheric pressure prevails. At the beginning of the simulation an initial water height is established, which is the initial water volume of the experiment.

Model validation -Grid convergence
In this subsection, three grid resolution values are evaluated for the grid convergence. The domain is discretized using a structured mesh made up of hexahedral elements.
The mesh sizes to be analyzed are 2, 1.5 and 1 cm. The water depth variable is chosen as the analysis due to the reliability of the measurement of its values. In order to quantify the numerical assessment quadratic mean value R 2 is used. Fig. 2 shows how the statistical value R 2 increases when the mesh size decreases in the four measurement points.

Numerical Simulation
In this study, after the mesh analysis a grid of 1 cm is used. The grid cells has been used with some narrowing towards the bottom and the walls of the tank. An Explicit 2nd order limited scheme for the convection term, Explicit second order scheme for the diffusion term, and first order Euler scheme for the transient term are used. The simulation is continued for 7 s with an automatically adapted time step using maximum CFL-numbers around 0.50.

Results and Discussion
In order to analyze the capabilities of the numerical model in the reproduction of the flow variables in a dam break, a comparison between RANS numerical simulation and experimental data was quantified by the quadratic mean value R 2 .

Water Depth
The evolution in time of water depth (H1, H2, H3, and H4) are shown in Fig. 3. A qualitative evaluation of the results shows that the 3D model configuration is able to reproduce satisfactorily the variability in time of the water depth in the four points of study. Additionally, a qualitative evaluation of the results shows that the 3D numerical model explains the variability in time of water depth (Fig. 4). The best numerical data occurs at the point denominated H4 (Fig. 4-d), this point is located inside the water tank formed at the beginning of the experiment. On the other hand, the worse numerical data occurs in the point denominated H3 (Fig. 4-c).

Conclusions
This study investigates the applicability of OpenFOAM code for the generation of flow field variables -water depth and pressure-in a dam-break laboratory scale using the RANS approach. The results demonstrate that the 3D numerical model configuration with RANS k-ε (RNG) approach can provide reliable results of the flow field in a dam-break case. Water depth values are reproduced better than pressure values by the 3D numerical model. Although the matching between the numerical solution and the physical experiment is quite promising, the application of the 3D numerical model for field-scale simulation would be computationally expensive.