ReFRESCO
ReFRESCOis a viscous-flow CFD code that solves multiphase (unsteady) incompressible flows with the RANS equations, complemented with turbulence closure models, cavitation models and volume-fraction transport equations for different phases [27]. The equations are discretised using a finite-volume approach with cell-centred collocated variables and in strong-conservation form. A pressure-correction equation based on the SIMPLE algorithm is used to ensure mass conservation [11]. Time integration is performed implicitly with first or second-order backward schemes. At each implicit time step, the non-linear system of velocity and pressure is linearised with Picard’s method and either a segregated or coupled approach is used. In the latter, the coupled linear system is solved with a matrix-free Krylov subspace method using a SIMPLE-type preconditioner [11]. A segregated approach is always adopted for the solution of all other transport equations. The implementation is face-based, permitting unstructured grids with elements consisting of an arbitrary number of faces (hexahedra, tetrahedra, prisms, pyramids, etc.). State-of-the-art CFD features such as moving, sliding and deforming grids, as well automatic grid refinement are also available in the code.
For turbulence modelling, RANS/URANS, Scale Adaptive Simulation (SAS) [16], ((I)D)DES, Partially Averaged Navier Stokes (PANS) and LES approaches are available [18]. The Spalart correction [3] to limit the production of turbulence kinetic energy based on the stream-wise vorticity can be activated. Automatic wall functions are available.
The code is parallelised using MPI and sub-domain decomposition, and runs on Linux workstations and HPC clusters. ReFRESCOis currently being developed, verified and validated at MARIN in the Netherlands in collaboration with IST (Lisbon, Portugal), USP-TPN (University of São Paulo, Brazil), Delft University of Technology, the University of Groningen, the University of Southampton, the University of Twente and Chalmers University of Technology.
Computational domain and setup
Due to the different water depths and distances of the ship to the vertical wall, separate grids had to be made for each case. Free surface deformation was not taken into account in the ReFRESCOcomputations. To account for the dynamic trim and sinkage the experimental values were applied in the grid generation. This means that also for the cases with and without propulsion, separate grids had to be generated. To ensure grid similarity between the cases and between different grid densities, the meshing process was automated using scripts. Unstructured grids with hexahedral elements were generated using HEXPRESS. At the hull and rudder surfaces, an inflation layer was added to be able to capture the high gradients in the boundary layer.
The inlet and outlet boundaries were located at 4\(L_{\text {pp}}\) forward and 4\(L_{\text {pp}}\) aft of the aft perpendicular of the ship. In Fig. 7 the domain and boundary definitions are shown. Symmetry boundary conditions were applied on the undisturbed water surface (top). On the hull and rudder surface, no-slip and impermeability boundary conditions are used (\(\overline{u} = 0\)). Due to the application of the inflation layer at these surfaces, the \(y^+_{\max }\) values are around 0.5 and therefore the boundary layer is resolved down to the wall. On the vertical wall, on the slope and on the bottom surface, the boundary condition is set to moving wall/fixed slip (\(\overline{u} = \overline{V_\infty }\) with \(V_\infty\) the inflow velocity). At these boundaries wall functions are used to avoid large grid densities. A pressure boundary condition is applied at the outflow and inflow boundary conditions at the inflow. The inflow turbulence intensity is set to \(1\%\) and the eddy viscosity at the inflow to \(\mu _t = 1\mu\). All calculations were conducted for a Reynolds number \(Re = {1.5\times 10^6}\). The ReFRESCO calculations presented in this study were all conducted without incorporating free-surface deformation and assuming steady flow, unless stated otherwise. The \(k-\omega\) SST model [17] was used as turbulence closure. For the a cases, the propeller action was achieved by coupling ReFRESCO with the potential flow code PROCAL [26] and using the obtained forces on the propeller as body forces in the viscous-flow computation [22]. In the propelled cases, the propeller rotational speed was set to 345.3 min\(^{-1}\) and the propeller thrust was obtained from the computation. For the b cases, the stopped propeller was not considered in the computations.
Solution verification
Table 5 Grid densities for ReFRESCO grid sensitivity study, case 1b
To obtain information about the sensitivity of the solutions to the grid density, a series of grids with various densities was generated for case 1b. Each grid was made using identical levels of refinements. The grid density was controlled by adjusting the number of cells in the initial base mesh. To maximise the grid similarity between different grid densities, the refinement diffusion was increased when increasing the grid density. For the hull and rudder surface, the first cell height was adjusted as a function of the density as well. Unfortunately, the way in which HEXPRESS generates the inflation layer does not allow users to fully control the mesh similarity close to walls. This means that upon grid refinement, the inflation layer becomes thinner and eventually, extrapolation to an infinitely fine grid would result in a solution on a grid without inflation layer. Therefore, a formal uncertainty estimate based on geometrically similar grids cannot be made. The study presented should therefore be considered as a grid sensitivity study. The grid sizes that were investigated are shown in Table 5.
For the finest grid (ultimately fine), the iterative convergence for case 1b is shown by the left graph in Fig. 8. The convergence shows a clear oscillation of the forces (standard deviation of \(1.6\%\) in X and \(6.6\%\) in Y) and moments (standard deviation of \(4.0\%\) in K and 0.3 Nm in N, which is larger than the mean value) and the uncertainty in the solution due to the iterative process can therefore not be neglected. This means that the discretisation error will be contaminated by scatter due to insufficient iterative convergence [8]. All computations have been conducted assuming steady flow, but the oscillatory behaviour of the global quantities during the iterative process in each case indicates that unsteady effects may be present in the flow and an unsteady solution approach may be more appropriate. In the remainder of this article, the forces and moments shown will be based on an average of the last part of the convergence history for each case.
In graph on the right of Fig. 8, the integral results for case 1b for the various grid densities are shown. On the horizontal axis, the relative step size \(h_i/h_1 = \root 3 \of {n_{c,1} / n_{c,i}}\) is shown. A relative step size of 1 represents the result for the finest grid, while larger values correspond to coarser grid results. A formal uncertainty estimate (e.g. following [9]) could not be made due to apparent divergence of the results upon grid refinement, leading to unrealistically high uncertainty estimates. From the results, it can be concluded that even for the finest grids the solution still changes and even finer grids should be used in order to avoid too large uncertainties in the results due to discretization errors. This conclusion confirms the observations by Zou and Larsson [34] in which also large uncertainties (e.g. a numerical uncertainty in Y of more than \(24\%\) of the solution on the finest grid) were found for bank-effects computations.
In the graphs presented in this article regarding the trends of bank suction effects, ReFRESCO results for the medium grid are included. Based on the solution verification, it is found that the numerical uncertainty in the results is rather large and therefore it will be hard to draw quantitative conclusions on the accuracy of the modelling approach. Any deviations from the true value can be caused by either modelling errors, or due to uncertainties in the solutions. In future studies, finer grids and probably an unsteady solution approach should be adopted to better quantify the trends. To investigate the influence of time on the solution, an unsteady computation has been performed. The results are presented below.
Unsteady solution
A preliminary study has been done in order to quantify the effect of an unsteady solution method compared to steady computations. For the finest grid, i.e. 35 million grid points, a computation with second order time discretization was performed with a time step of 0.02 s = 1/600 \(L_{\text {pp}}/V\) and desired normalised RMS residual convergence level per time step of \(L_2 <{5\times 10^{-5}}\). The computation was restarted from a computation with coarser time step ( 0.1 s) and ran 4810 time steps, or 96.2 s. On average, about 25 outer loops per time step were required to reach the desired iterative convergence. The forces and moments as a function of time are shown in Fig. 9. This figure clearly shows the unsteady nature of the flow. Surprisingly, the loads do not converge towards an harmonic signal and even after 96 s, statistical convergence is not obtained. It should be noted that these 96 s are much longer than the time during which the model was sailing in the section with the vertical bank during the experiments, and significantly longer than the time over which the average of the experiments was taken.
A comparison of the forces and moments obtained with the steady computation and the unsteady one are given in Table 6. The result of the unsteady computation are very similar to those obtained with the coarser time step of 0.1 s and therefore the discretization error in time appears to be small. Although for Y and N a very small improvement compared to the experiment appears to be made, a significant difference still remains. Since the computing time for the unsteady calculation is 75 times larger than the steady one, the marginal improvement does not seem to justify the additional computational effort.
To investigate whether the time-averaged unsteady computation produces a wake that is similar to the wake obtained with the steady computation, Fig. 10 is made. In this figure, some differences can be seen, but the overall flow features do not appear to change much between the steady and unsteady cases.
Table 6 Comparison between steady and unsteady computation results, ReFRESCO, case 1b
ROPES
ROPES has been developed for the prediction of ship–ship interaction forces in shallow water of arbitrary depth. The computational method used in ROPES is based on three-dimensional potential flow and the double-body assumption. This means that free-surface effects of vessels are not accounted for. Furthermore, trailing wakes are not implemented in ROPES, so the potential flow model does not include lift effects. The flow equations are solved using standard zero-order panels and Rankine sources with or without the effect of restricted water depth and channel walls [12, 19]. Based on the solution of the source strength on the panels describing the bodies, the hydrodynamic forces on the ships are computed based on equations developed by Xiang and Faltinsen [30]. These equations are used to compute the complete set of hydrodynamic forces on all bodies. ROPES is applicable to multi-body simulation scenarios involving various ships and port structures.
A close-up view of the panel distribution on the hull and on a part of the vertical wall is given in Fig. 11. The vertical wall extends from \(x/L_{\text {pp}}=-4\) to \(x/L_{\text {pp}}=4\). The hull is represented using 2438 panels, while 2184 panels are used to describe the vertical and sloped wall. Since ROPES cannot handle lifting surfaces, the rudder has been removed from the ship geometry. The computations were executed at full scale conditions and the resulting forces and moments were converted to model scale.
ISIS-CFD
The ISIS-CFD solver that is part of the FINE/Marine CFD computing suite, is an incompressible, unsteady, Reynolds-averaged Navier–Stokes (URANS) solver mainly devoted to marine hydrodynamics. The solver features several sophisticated turbulence closure models: apart from the classical two-equation \(k-\epsilon\) and \(k-\omega\) models, the anisotropic two-equation Explicit Algebraic Stress Model (EASM), as well as Reynolds Stress Transport Models, are available with or without rotation corrections [7]. All turbulence models are compatible with wall-function or low-Reynolds near wall formulations. Hybrid LES turbulence models based on Detached Eddy Simulation (DES) are also implemented and are validated on automotive flows characterised by large separations [10]. Additionally, several cavitation models are available in the code.
The solver is based on the finite volume method to build the spatial discretization of the transport equations. The unstructured discretization is face-based. While all unknown state variables are cell-centred, the systems of equations used in the implicit time stepping procedure are constructed face by face. Fluxes are computed in a loop over the faces and the contribution of each face is then added to the two cells next to the face. This technique poses no specific requirements on the topology of the cells. Therefore, grids can be completely unstructured: cells with an arbitrary number of arbitrarily-shaped faces are accepted. Pressure-velocity coupling is enforced through a Rhie and Chow SIMPLE type method: at each time step, the velocity updates come from the momentum equations and the pressure is given by the mass conservation law, transformed into a pressure equation. In the case of turbulent flows, transport equations for the variables in the turbulence model are added to the discretization. Free-surface flow is simulated with a multi-phase flow approach: the water surface is captured with a conservation equation for the volume fraction of water, discretized with specific compressive discretization schemes [21]. The technique included for the 6 degrees of freedom simulation of ship motion is described by Leroyer and Visonneau [14]. Time-integration of Newton’s law for the ship motion is combined with analytical weighted or elastic analogy grid deformation to adapt the fluid mesh to the moving ship. To enable relative motions of appendages, propellers or multiple bodies, both sliding and overlapping grid approaches have been implemented. Various options are available in ISIS-CFD to take propulsive effects into account: propellers can be modelled using actuator disc theory, by coupling with boundary element codes (RANS BEM coupling [6]), or by direct discretization through e.g. rotating frame method or sliding interface approaches. Finally, a anisotropic automatic grid refinement procedure has been developed which is controlled by various flow-related criteria [28].
Parallelization is based on domain decomposition. The grid is divided into different partitions; these partitions contain the cells. The faces on the boundaries between the partitions are shared between the partitions; information on these faces is exchanged with the MPI (Message Passing Interface) protocol. This method works with the sliding grid approach and the different sub-domains can be distributed arbitrarily over the processors without any loss of generality. Moreover, the automatic grid refinement procedure is fully parallelized with a dynamic load balancing algorithm that works transparently with or without sliding grids.
Computational domain and setup
The computational domain with boundary conditions is shown in Fig. 12. The top of the domain is located 0.5\(L_{\text {pp}}\) above the water surface. At this surface, the pressure is prescribed using the Updated hydrostatic pressure boundary condition of ISIS-CFD. The inlet is located 1.5\(L_{\text {oa}}\) ahead of the bow of the ship, and the outlet is located 2.5\(L_{\text {oa}}\) aft of the stern, hence the total domain length is approximately 5\(L_{\text {oa}}\). For both of these surfaces, a far-field boundary condition is applied (\(V = V_{\infty }\)). The bottom and the surface-piercing tank walls are modelled as solid walls having a relative velocity with respect to the ship. Wall function boundary conditions are applied at these surfaces. A no-slip condition is applied to the rudder surfaces and the hull except for the deck, where a slip condition is applied. The lateral wall on port side has a slip condition as well. No wall functions are used on the the hull and rudder surfaces, i.e. the flow is resolved down to the wall (\(y^+_{\max } \approx 0.5\)).
Propulsion is modelled using an actuator disk, for which the measured thrust and torque values are used as input (see Table 4). This method requires extra grid refinements near the propeller location. The same grids are used for the propulsive cases and the non-propulsive cases, hence five meshes are generated. For each combination of lateral position and water depth, first a computation without propulsion is executed after which the propulsive cases are computed using the solution of the non-propulsive case as initial condition. For the non-propulsive cases, the stopped propeller is not taken into account.
Trim and sinkage are solved for in the ISIS-CFD computations. To ensure that due to sinkage, the cells below the hull are not compressed too much (which may result in negative cell volumes), the hull is meshed 3 mm below the hydrostatic position. Vertically, the centre of gravity is located on the waterline. Longitudinally, it is located 0.1482 m ahead of the midship location. This value is approximately 2 mm aft of the longitudinal location of the centre of gravity as recorded in the experiments (see Table 2). For each case the grid contains approximately \({16\times 10^{6}}\) cells, the actual numbers are documented in Table 7.
Table 7 Grid sizes for the computations of FHR Initially, all computations were run using a first-order time discretization scheme that uses a quasi-static approach to update the attitude and vertical position of the ship such that the resulting accelerations approach zero. For case 1b, a second-order time discretization scheme—where Newton’s laws are tightly coupled to the flow motion at each time step—has been used as well.Footnote 2 For this case, the inertia moments of the ship hull are required as input. In the analyses that follow, the ISIS-CFD computations using a first-order time discretization are labelled ISIS-CFD, whereas the computation that uses a second-order time discretization is labelled ISIS-CFD unsteady.
Solution verification
For case 1b, additional grids were generated for solution verification. The cell sizes were modified by adjusting the cells sizes in the initial Cartesian grid. For example, the medium mesh was generated by increasing the linear dimensions of the initial cells by a factor 1.25. Furthermore, for refinement surfaces and refinement boxes with absolute target cell sizes (such as the surfaces used for water surface refinement), the target cell size values were multiplied by this refinement factor as well. For the hull and rudder, the first cell size was adjusted (increased) as well, resulting in lower \(y^+\) values for the finer meshes (as shown in Table 8).
The iterative convergence on the fine grid (left) and the values of the integral quantities obtained on the four grids (right) are shown in Fig. 13. Similar to the solution verification of ReFRESCO (Sect. 3.3), the horizontal axis of the right-hand graph in this figure shows the relative step size \(h_i/h_1 = \root 3 \of {n_{c,1}/n_{c,i}}\): the finest grid has a relative step size of one. These results show that the iterative convergence for ISIS-CFD is good, especially when compared to the iterative convergence of ReFRESCO (shown earlier in Fig. 8). For the longitudinal force X grid convergence is oscillatory. On the finest grid, the lateral force Y shows a very slight divergent trend. Although integral values do not change very much between the fine and medium mesh, a finer grid should be used to verify that the finest mesh used here is sufficient.
Table 8 Grid densities for ISIS-CFD grid sensitivity study, case 1b
Adaptive grid refinement
For case 3b, ECN/CNRS performed a computation using ISIS-CFD with adaptive grid refinement (AGR) starting from a steady solution obtained on a coarse mesh (with approximately \({5\times 10^{6}}\) cells) that was provided by FHR. A new combined refinement criterium for both the free-surface and the vortical structures has been used [29]. The minimum size limit for refined cells has been retained to 0.002 m and is activated each 50 steps of the time marching procedure in order to find a steady solution. This leads to a refined grid of about \({20\times 10^{6}}\) cells.
Overview of computational settings
For the five test cases without propulsion, results from [35] will be included in the comparison between CFD predictions and the experiments. A summary of the settings for the computations used in the force and flow field comparisons as discussed later in this report is given in Table 9.
Table 9 CFD computation settings