An essential component of a CFD simulation is the mesh generation and it is particularly important for the present case because of the movement of the solid body within computational domain.

It is well known that the finite volume method (FVM) involves discretization of the flow domain of interest and then integration of the flow equations over elemental cell volumes. The method enables correct flux balances across cell boundaries and conserves momentum throughout the grid. Therefore, advantage may be gained by using the FVM since the dependent variables remain at all times referenced to a Cartesian frame even when boundary-fitted using cut cells. The remainder (majority) of the cells are uncut flow cells that be treated in a straight forward manner. However, whilst the Cartesian cut cell algorithms can easily accommodate moving boundaries, there are pathological cases where the approach can sometimes provide relatively poor resolution of some particular geometric features. For example, a numerical instability may occur locally within the flow solver if cut cells become arbitrarily small. To overcome this problem, cell merging is implemented as in Clarke et al. [16], Yang et al. [17] and Qian et al. [18] who successfully applied the technique in many applications within aerospace and hydrodynamics. The basic idea is to combine the small cut cell with its neighbouring cells to form a new cell with the interface between merged cells ignored. A minimum volume criterion V_min is specified for the cut cell volumes before the flow simulation starts. If the volume of a cut cell is less than V_min that cell will be merged with neighbouring cells in the direction of the shortest side face otherwise the cut cell will remain unchanged. For computational efficiency cut cell algorithms generally assume a maximum number of cuts within a cut cell which may result in some sub-grid scale geometric features of the body being approximated and this approximation may in principle vary slightly from one time step to another if the body is in motion. However, we find that such higher-order approximations are generally consistent with the accuracy of the associated body’s surface description.

The integral form of the Euler equations for 3D incompressible flow with variable density can be written as

where Q is the vector of conserved variables which encloses the time dependent domain of interest V, F is the flux vector function and n is the outward unit vector normal to the boundary S. B is a source term for body forces. Q, F and B are given by

where

and u, v and w are the flow velocity components and u_b, v_b and w_b are the velocity components of the boundary S  which are zero when the boundary is stationary. ρ is the density, p is the pressure, β is the coefficient of artificial compressibility and g is the gravitational acceleration.

We can then discretize Equation (1) over each cell within the flow domain using a finite volume formulation, this gives

where is the average value of Q in cell stored at the cell centre and denotes the volume of the cell. F_k is the numerical flux across the face k of the cell, ΔA_k is the area of the face and m is the number of faces of the cell. The convective flux F_k is evaluated using Roe’s approximate Riemann solver, which assumes a 1D Riemann problem in the direction normal to the cell face and has the form

where and are the reconstructed values on the right and left at face k and A is the flux Jacobian evaluated by Roe’s average state. The quantities R, L and are the right and left eigenvectors of A and the eigenvalues of A respectively.

To achieve a time-accurate solution at each time step of the unsteady flow problem a first-order Euler implicit difference scheme is used to discretise Equation (5) as

Introducing a pseudo-time derivative into Equation (7), this gives

where τ is the pseudo-time and. The right-hand side of Equation (8) can be linearized using Newton’s method at the m+1 pseudo-time level and then can be written in the matrix form

where

and I_m should be defined as

.

When is iterated to zero, the density and momentum equations are satisfied, and the divergence of the velocity at time level n + 1 is zero. The system of equations can be written in matrix form as

where D is a block diagonal matrix, L is a block lower triangular matrix and U is a block upper triangular matrix. Each of the elements in D, L and U is a matrix. An approximate LU factorization (ALU) scheme as proposed by Pan and Lomax [19] can be adopted to obtain the inverse of equation (10) in the form

Within each time step of the implicit integration the sub-iteration is terminated when the L₂ norm of the iterates process

is less than a specified limit ε and in this paper.

For all test cases non-reflecting boundary conditions are applied at the top boundary allowing air to leave or enter the domain freely. The remaining boundaries are set as rigid walls.

At the interface between two immiscible fluids, the present method assumes that the system of equations for non-homogeneous, incompressible flow can treat the free surface numerically as a contact discontinuity in the density field. Special procedures to track the free surface are thus unnecessary since the free surface is captured automatically. It is asserted that the numerical solution of Equation (1) for a system containing one or more free surfaces will converge to the correct unique solution.

In the current approach, the pressure value p can be calculated from the term p/β in Equation (2) by multiplying by β. The total force is then obtained by integrating the pressure field along the body surface

, where S_b is the area of the body surface as defined by the cut cell surface fitting.

The first test involves a free falling of a cone with deadrise angle 20˚ into still water. The physical tank tests are described by Backer et al. [13]. They tested a model along tightened steel wires to make sure that the floater fell down without experiencing small rotations and big horizontal motion, They used a water tank with dimensions (l × w × h) of 1.2 m × 1.0 m × 1.25 m and our numerical domain has the same size except for height which is set to 2.6m as the body was positioned 1.0 m above the still water surface prior to release. Two nonuniform meshes were used: One is used for a mesh spacing in the refined regions close to the body geometry of 0.020 m with a total of 42 × 38 × 114 = 181,944 cells, the other is used for a mesh spacing in the refined regions close to the body geometry of 0.016 m with a total of 56 × 50 × 142 = 397,600 cells. The maximum radius of the cone is 0.15m with the height of the top cylinder section set to 0.08 m (see Figure 1) and the mass of the cone is m = 4.1 kg.

In the physical experiments, the time history of pressure on the cone surface was recorded during the impact at two locations (S1 and S2) with a horizontal distance of 0.04 m and 0.09 m respectively from the symmetrical axis as shown in Figure 2. To compare with the experimental data, the real time starting from the moment that cone is released from 1 m above the water surface has been used. In Figure 3 the calculated pressures at S1 and S2 on two meshes are compared with those from the physical experiments showing good agreement in terms of the typical shape of impact pressure, which consists of a steep rise of pressure followed by a gradually decreas-

ing part on the right side of the peak. However, there is a substantial difference in the peak pressure values between the experimental and numerical data. For example, the values of the peak pressure are 0.455 bar for the finer mesh and 0.404 bar for the coarser mesh but for the experimental this value is 0.719 bar. This indicates further mesh refinements especially for the region near the surface of the cone are still needed. To show this and to save the computation time, an axi-symmetric version of the free surface code has been applied to simulate the same flow problem. Three levels of grid (dx = dy = 0.005, 0.0025 and 0.00125 m respectively) have been used with a time step of . In Figure 4, the calculated surface pressure value at S2 is compared with the experimental ones, from which it can be seen that to get the peak pressure values very fine mesh must be used. The calculation is repeated for the intermediate mesh spacing of dx = dy = 0.0025 m using four different time steps and the results are shown in Figure 5.

From these results, it can be concluded that for the test case of a free falling cone impacting on water surface the occurrence of peak surface pressures is an extremely localised phenomenon in both space and time, so ex-

tremely small mesh size and time step at least locally must be used in order to capture those moments accurately. This highlights the need for both spatially and temporally adaptive solutions for such flow problems. On the other hand, the integrated global values such as the impact force, body acceleration and moving speed are much less affected by the localised extreme pressure values. For the same interval time as above, Figure 6 shows the vertical velocity (absolute value) from the two meshes compared with those from the physical experiments. During the impact, the velocity of the cone, according to the experimental data, has dropped from 4.4 m/s to 2.6 m/s, while for the numerical result on the fine mesh the corresponding change is from 4.4 m/s to 2.4 m/s. Similarly, for the acceleration both results are also in reasonable agreement with each other.

The small differences in velocity may be due to the laboratory model not being constrained to heave motion only. Other reasons which explain the differences may be due to the volume of cone (or associated buoyancy force) being slightly different from the laboratory model owing to small inaccuracies in the surface fitting of the geome-

try used in the cut cell model (see Figure 1).

The simulations were carried out using one processor of a 600 MHz NEC vector computer with the CPU times of 2 days for the coarse mesh and about 5 days for the finer mesh.

This test case simulates the free-decay of the Bobber as described in the physical tank tests by Thomas et al. [20]. In the physical experiments, the oscillating motion of the Bobber is controlled by the weight of the Bobber and a counterweight, which is connected through a pulley system to the Bobber as shown in Figure 7. In the numerical simulation the formula for the movement of the system is given by

where the total mass equals the Bobber mass of mf plus the counterweight mass mc, is the acceleration in the vertical direction positive upward and the integration on the right-hand side calculates the dynamic force from the pressure on the wetted area of the Bobber in the vertical direction only. According to the experimental tests by Thomas et al. [20], the Bobber mass mf = 2.1 kg and the counterweight mass mc = 1.0 kg will be used in the test. In our numerical tank, the Bobber is allowed to move in vertical motion only dictated by its body weight and the total forces.