Shock and Vibration

Volume 2015, Article ID 794069, 12 pages

http://dx.doi.org/10.1155/2015/794069

## Numerical Simulation on Interface Evolution and Impact of Flooding Flow

College of Shipbuilding Engineering, Harbin Engineering University, Harbin 150001, China

Received 30 November 2014; Accepted 14 April 2015

Academic Editor: Hamid Hosseini

Copyright © 2015 J. Hu et al. This is an open access article distributed under the Creative Commons Attribution License, which permits unrestricted use, distribution, and reproduction in any medium, provided the original work is properly cited.

#### Abstract

A numerical model based on Navier-Stokes equation is developed to simulate the interface evolution of flooding flows. The two-dimensional fluid domain is discretised by structured rectangular elements according to finite volume method (FVM). The interface between air and liquid is captured through compressive interface capturing scheme for arbitrary meshes (CICSAM) based on the idea of volume of fluid (VOF). semiimplicit method for pressure linked equations (SIMPLE) scheme is used for the pressure-velocity coupling. A second order upwind discretization scheme is applied for the momentum equations. Both laminar flow model and turbulent flow model have been studied and the results have been compared. Previous experiments and other numerical solutions are employed to verify the present results on a single flooding liquid body. Then the simulation is extended to two colliding flooding liquid bodies. The impacting force of the flooding flow on an obstacle has been also analyzed. The present results show a favourable agreement with those by previous simulations and experiments.

#### 1. Introduction

The interaction of flooding flows with structures is a classic and important problem in many engineering applications, such as the green water loading [1, 2], dam break flowing over an obstacle [3, 4], and the wave breaking problem [5]. The unsteady loads caused by the flooding flow on fixed or floating structures have unnegligible influence on the design of marine structures [6] and marine vessels [7, 8]. In addition, some natural disasters featuring as flooding flow, such as tsunami, lava flow, and landslide [9], have attracted much of our attention because of their huge damage to the environment and economy. Thus, it is of great interest to study the behavior of flooding flow.

Among various problems related to flooding flow, the dam break problem with consequent wall impact is widely used to benchmark various numerical techniques that tend to simulate interfacial flows and impact problems [10]. Koshizuka [11] experimented on a liquid column collapsing and hitting an obstacle. Zhou et al. [12] performed a dam break flow experiment in a water tank to analyze the impact on a rigid wall. Besides the experimental studies, numerical simulation has become a more efficient and economical way in the investigation of flooding flow with the development of high performance computers. Among these numerical simulations, the potential theory [13–15] has been used for decades. A more popular way is to employ the incompressible N-S equations without neglecting the fluid viscosity. Generally, these viscous models are more suitable for handling strongly nonlinear problems. Scardovelli and Zaleski [16] provided a comprehensive review of the viscous analysis on the interface capture of multiphase flow problems. Abdolmaleki et al. [17] simulated the impact flow on a vertical wall resulting from a dam break problem.

The modelling of interface evolution is both critical and challenging in the numerical simulation of flooding flow because of the complex air-liquid interaction [18, 19]. There are mainly three numerical schemes to track the free surface of the flooding flow which are boundary element method, smoothed particle hydrodynamics (SPH) method, and volume of fluid (VOF) method [8]. Using the dynamic and kinematic conditions on free surface, the boundary element method usually employed a time stepping scheme to track the free surface based on nonviscosity assumption [20]. The SPH method offers a variety of advantages for fluid modelling, particularly for the splashing droplets problem [21, 22]. Colagrossi and Landrini [23] used SPH method to predict the dynamic behaviour of flooding flow. Proposed by Hirt and Nichols [24], the VOF method has become popular for calculating interfacial flows. Panahi et al. [25] analyzed the numerical simulation of floating or submerged body motions based on a VOF-fractional step coupling. Kleefsman et al. [26] numerically investigated a dam break problem and water entry problem. Hänsch et al. [27] simulated the two-phase flows with multiscale interfacial structures, which is a dam break model with an obstacle.

In the present study, a numerical tool based on the Navier-Stokes equations is developed to simulate the viscous flooding flow in a water tank. The paper is divided into five sections. In Section 1, the recent developments of the numerical methods for the dam breaking problem are introduced, which mainly include smoothed particle hydrodynamics method and volume of fluid method. In Section 2, the main methodology and the numerical scheme are presented in detail, especially the discretization of the fluid domain and CICSAM used to capture the air-liquid interface. In Sections 3, 4, and 5, we, respectively, studied the dam breaking problem of a single fluid body, the collision between two liquid bodies, and the impact of a flooding flow on an obstacle. A detailed analysis on the interface evolution is presented and the impact force of the flooding flow is investigated.

#### 2. Methodology

##### 2.1. Governing Equations

The Navier-Stokes equation and continuity equation on viscous flows can be described as follows [24]:where and are the velocity components in directions, respectively, is the mixture density of the fluids, is the pressure, and is the gravitational acceleration.

By applying the gauss theorems, the integration of (1) over each cell with respect time can be presented aswhere the subscript represents the centre of the control volume, is the centre of the cell boundaries, is the volume of the control volume, is the volumetric flux at the face of control volume, and is the area vector of the control volume face.

Three schemes, explicit scheme, the Crank-Nicolson scheme, and Euler implicit scheme can be used for the temporal discretisation of the N-S equations. In this paper, Euler implicit scheme is chosen and (2) of the velocity in direction is discretised asSimilarly, we can discretise (2) of the velocity in direction.

In order to keep the numerical stability, the normalized variable diagram (NVD) method is applied when handling the convection item. In this paper, a second-order upwind discretization scheme is used to calculate the values on the control volume faces. The algebraic equation obtained ultimately for each variable in each control volume is described as follows:where denotes the scalar quantity of general variable, denotes the coefficient of the linear equations, and the subscripts , , , and denote the upper, bottom, left, and right boundaries of the cell.

For the interfacial flow, the water and air are assumed to be one type of fluid with different densities. Thus, we can use a single set of (1) to describe the entire flow field and interface terms. The mixture density can be described asin which and are the density of water and air, respectively, is the fluid volume fraction which is set to 1 in the water region, and 0 is in the air region. In the vicinity of the interface, is between 0 and 1.

Similarly, the mixture viscosity of the fluids can be described asin which and are the viscosity of water and air, respectively.

The conservative form of the scalar convection equation for the volume fraction is as follows:

The volume fraction of each phase is solved in all computational cells. In each time step, should satisfy the governing equations (1). In each cell, only knowing the value of is not enough to determine the local interface position and direction. As a step function, the volume fraction also often causes numerical diffusion when using finite difference method to obtain variable derivatives. In addition, the amount of flow convected over a cell during a time step should be less than the amount available in a doner cell. The computational grid should be fine enough with respect to the maximum flow velocity, also for a distinct gas-liquid interface. Thus, the inclusion of water and air with different densities will greatly complicate the numerical method.

As the real liquid has viscosity, the RANS (Reynolds-averaged Navier-Stokes) equations are used to solve the mean flow velocity and turbulent model is used for the closure of RANS equations [28]. In standard model, is the turbulent kinetic energy and is turbulent dissipation rate. Then the turbulent kinetic viscosity can be presented aswhere is empirical constant. Taking and as basic unknown variables, the corresponding transport equations arewhere and are the turbulent kinetic energy caused by mean velocity gradient and buoyancy, respectively. , , and are the empirical constant, and are the Prandtl Numbers of and . where is the component of the flow velocity parallel to the gravitational vector and is the component of the flow velocity perpendicular to the gravitational vector. .

##### 2.2. Free Surface Capture

For the cells in the vicinity of the air-liquid interface, the volume fraction undergoes a step change, which is a challenge to simulate the surface. In present paper, we adopt the CICSAM (compressive interface capturing scheme for arbitrary meshes) method developed by Ubbink and Issa [29], which is capable of predicting a well-defined interface. In this method, the convection of fluid is simulated by weighting the available fluid in the donor cell with a weighting factor based on the face Courant number and the cell Courant number . The face fraction values are predicted with linear interpolation:where subscripts and represent the value at the centre and border of cell, respectively. Subscripts and indicate the donor cell and the acceptor cell, respectively, is the amount of element grids, is the volume of the cell, is the flux out of the donor cell, is the CICSAM weighting factors, and upwind form and downwind form are both used and switched flexibly to get smooth or sharp interface [30].

For transient calculations, the initial velocity and density fields can be specified according to the specific test cases. Also the implicit body force formulation can be used in conjunction with the VOF method to improve the convergence of the solution by accounting for the partial equilibrium of the pressure gradient and body forces in the momentum equations. In solving the Navier-Stokes and continuity equations, one needs physical properties density and viscosity distribution in the computational domain. The N-S equations are solved in every cell with fluid containing.

To increase the stability and the accuracy of the present simulation, Euler implicit scheme is applied for the temporal discretisation, which can guarantee the stability of iteration process even with a relatively large time step. Meanwhile, the courant numbers and are adjusted to be small enough to ensure the accuracy of the simulation. The second order procedure for solving N-S equations can also increase the accuracy, as the central difference finite volume method is used for viscous terms. Also a second-order upwind discretization scheme is used to calculate the values on the control volume faces. In handling convection item, the normalized variable diagram (NVD) method also stabilizes the computation effectively.

#### 3. The Interface Evolution of a Single Flooding Body in a Square Tank

In this section, a dam break experiment [12] involving complex free surface evolution is used to verify present simulations, which is performed in a tank measuring 3.22 × 1 × 1.8 m. Two probes A and B located at m and m on the tank bottom are used to measure the water heights. According to the experimental configuration, a 2D numerical model is established, as shown in Figure 1. A water column located on the left side of the tank is contained by the tank boundaries and a vertical board. Once the board is lifted, the water with an initial height and width flows freely.