Bank effects for KVLCC2

2.1 Towing tank facility

The tests with bank configuration have been carried out in May 2010 in the towing tank for manoeuvres in shallow water, located at FHR and administrated in cooperation with the Maritime Technology Division of Ghent University. A short summary of the particulars and possibilities of this towing tank [24] is given below.

2.2 Experimental setup

2.2.2 Ship model

FHR owns a 1/75 scale model of the KRISO Very Large Crude carrier (KVLCC2), which was built according to the lines provided by SIMMAN (2nd variant). Consequently, its main particulars including propeller data can be found on the SIMMAN website.¹ The hydrostatic dependent particulars for the bank effects test program are given in Table 2. The vertical position of the centre of gravity of the ship is located on the waterline.

Table 2

Hydrostatic particulars of KVLCC2 (model scale) for the bank effects test program

Parameter	Unit	Value
Length (\(L_{\text {pp}}\), \(L_{\text {oa}}\))	m	4.2667, 4.3400
Draft Amidships (\(T_{\text {m}}\))	m	\({0.2776 \,{\pm }\, 0.0005}\)
Beam (B)	m	0.7733
Longitudinal CoG (X\(_\text {G}\))	m	\({0.1449 \,{\pm }\, 0.002}\)
Vertical CoG (KG)	m	\({0.2776\, {\pm } \,0.0008}\)
Displacement	m\(^3\)	\({0.7410 \,{\pm }\, 0.000237}\)
Block coefficient	–	0.8098
Mass	kg	\(736.2 \,{\pm }\, 0.2\)
\(I_{XX}\)	kg m\(^2\)	\(41.0 \,{\pm }\, 1.2\)
\(I_{YY}\)	kg m\(^2\)	\(797.3\, {\pm }\, 2.6\)
\(I_{ZZ}\)	kg m\(^2\)	\(831.5 \,{\pm }\, 2.2\)

Open image in new window

Open image in new window

2.3 Analysis of experimental data

For each test case, only one experiment was executed. Hence, it is not possible to compute standard deviations for the measured values as would be the case when each experiment was repeated multiple times. To judge the steadiness of the experimental data, both the normalised cumulative moving average (nCMA) and the normalised cumulative standard deviation (nCSTD) are computed. If the derivatives of these values (dnCMA and dnCSTD, respectively) approach zero, the experimental time series converges to a steady state. In addition, the Fast Fourier Transform (FFT) of the experimental time series is computed to get an idea of the frequency content of the fluctuations.

Open image in new window

Open image in new window

Open image in new window

As an example, for case 4a the experimental data for \(X'\) is shown in Fig. 3. The top graph shows the measured force for the complete duration of the experiment in grey and in light blue (\(\approx\) 150–200 s) the actual data that corresponds to the part during which the model passes the bank section with the vertical wall. This part of the time trace is used to compute the average values. Below this graph, the plots labelled nCMA and nCSTD show the normalised cumulative moving average and the normalised standard deviation for the light blue part. Both graphs approach one. On the third row, the plots show the numerically computed first derivatives of the figures in the second row on a logarithmic scale. These plots clearly show that both the mean and the standard deviation converge as their derivatives approach zero. On row four, the frequency content of the experimental data is shown. The frequency with the highest power is located at 3 Hz. The lowest frequency has a value that is at least an order of magnitude smaller, which indicates that the time signal does not contain a (linear) trend.

For the same test case, the sinkage at the midship location (halfway between the aft and fore perpendiculars) shows a different trend (Fig. 4). Until 190 seconds the convergence of the sinkage is very good, with differences of nCMA smaller than \(1\%\). At this point, the sinkage starts to decrease with an almost linear trend until the end of the experimental data. This is reflected in the nCMA and nCSTD plots and their derivatives. The FFT plot on the lowest row shows that the lowest frequency signal has the highest power, which is an indication for a trend in the data. However, the measured difference in the sinkage between \(t={190}\) s and \(t={200}\) s is less than 0.1 mm, which is of the same order as the accuracy of the device used for the measurement of the sinkage [5].

Case 5a (\(H/T = 1.1\)) shows significant fluctuations in the lateral force \(Y'\), as shown in Fig. 5. Despite this, the derivatives of nCMA and nCSTD indicate that the time signal of the lateral force Y converges both in frequency and value. For this case, the dominant frequency is slightly larger than 0.2 Hz, which corresponds to the low-frequency fluctuations that are visible in the time plot.

2.4 Average values

2.5 Water surface elevation

Data from multiple wave gauges were recorded during the experiments. One of these gauges is located halfway between the beginning and the end of the bank configuration, between the vertical wall and the ship, at a longitudinal position of \(x_{\text {wg}} = {19}\) m. Its lateral position in the tank is \(y_{\text {wg}} = {-2.68}\) m. Hence, there is a gap of two centimetres between the vertical wall and the wave measurement device, as the vertical wall is located at \(y = {-2.7}\) m (as shown in Fig. 2). For computations where the free surface is taken into account, these water surface elevation measurements can be used to validate the prediction of the free surface position. The waiting interval between tests was 2000 s long. Conversion of the position of the wave gauge to a ship-fixed coordinate system is done as follows:

$$\begin{aligned} x_{{\text {wg,rel}}} = \frac{x_{{\text {ship}}} - x_{{\text {wg}}}}{L_{\text {pp}}} \end{aligned}$$

(1)

where \(x_{{\text {ship}}}\) is the longitudinal position of the midship location in the towing tank coordinate system. The converted wave measurements are shown in Fig. 6 for the cases with and without propulsion, positive x-coordinates correspond to positions ahead of the midship location, and positive y-coordinates correspond to an increase in water surface height.

Open image in new window

For all cases, an upward peak is observed when the ship bow passes the wave gauge. The peak value is inversely proportional to the lateral distance to the quay; for cases 3, 4 and 5 the peak value is the same. Between the ship and the quay, the depression is more pronounced as the ship sails closer to the quay, but here, also the depth value has an influence on the maximum depression. For cases 1 and 2 (both a and b), the depression is not symmetric with respect to the ship length, but shows a peak near \(L_{\text {pp}}/4\) ahead of the midship location. Case 5a is the only one for which the peak in water surface elevation near the aft perpendicular is higher than the peak at the bow.

3.1 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.

3.2 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.

Open image in new window

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.

3.3 Solution verification

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.

Open image in new window

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.

3.4 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.

Open image in new window

Open image in new window

3.5 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.

Open image in new window

3.6 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.

3.6.1 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 (\(y^+_{\max } \approx 0.5\)).

Open image in new window

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

Case id	Number of cells \(n_c\)
case 1a,b	15,638,287
case 2a,b	15,569,011
case 3a,b	16,843,438
case 4a,b	17,086,694
case 5a,b	15,855,507

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.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.

3.6.2 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

Grid id	Number of cells \(n_c\)	Faces on hull surface	\(y^+_{\max }\) on hull surface
Very coarse	3,595,215	86,302	1.08
Coarse	7,180,624	158,641	0.87
Medium	9,888,790	207,245	0.75
Fine	15,638,287	319,748	0.52

Open image in new window

3.7 Overview of computational settings

4.1 Forces and moment comparison

Qualitatively speaking, the CFD results are able to capture the trends that are present in the EFD results. Both CFD codes predict the trends in the forces and moments as a function of the distance to the bank and the under keel clearance. For example, ReFRESCO and ISIS-CFD predict that as the ship approaches the bank, the drag on the hull and the bank attraction force increase. The differences between the roll moments (K) and yawing moments (N) are small between the two CFD codes.

Quantitatively, large differences can be seen, especially for the more extreme conditions, i.e. close to the vertical wall (Fig. 14), or with small under-keel clearance (Fig. 15). For example, ReFRESCO and ISIS-CFD predict for the \(H/T = 1.1\) case that the lateral force Y acts repulsive, whereas the EFD results show that for all water depths the lateral forces attracts the ship to the wall. Unfortunately, uncertainty estimates are not available for the experiments, and therefore it is not possible to conclude whether the deviations are due to modelling errors in the CFD, or due to inaccuracies in the EFD (or both). Future work on experimental uncertainties and more in-depth CFD studies for the extreme cases is highly recommended.

The ISIS-CFD results with AGR (Figs. 14, 15) show little improvement over the results obtained using the fixed grid. The improvement is significant if a comparison is made with the results obtained on the coarse base grid that was used as a starting point for the AGR computation (compare the results of ISIS-CFD-c2 with those of ISIS-CFD (AGR) in Fig. 20e. From a user point

The differences between the steady and unsteady computation with ISIS-CFD for case 1b (Fig. 16) show that generally speaking, a small improvement is achieved with a second-order time discretization compared to a first-order time discretization. However, the computing time to reach a sufficiently converged solution is significantly higher for the second-order method.

Open image in new window

Open image in new window

Open image in new window

ROPES predicts the wrong sign for the yawing moment (Figs. 14, 15), i.e. a moment turning the bow towards the vertical wall, instead of away from the wall as predicted by the viscous-flow codes and found during the experiments. Furthermore, the force towards the bank is considerably over-predicted. More details of the differences between the potential flow results and the viscous-flow results will be discussed in Sect. 5.8. The ROPES results have been left out of the relative comparisons (Fig. 16) due to the large errors in the absolute plots. With some exceptions (such as case 5a), the ReFRESCO results are closer to the experimental values than those of ISIS-CFD or SHIPFLOW, especially for X and Y. Differences between the results for the roll and yawing moment are rather small. For case 4b, the SHIPFLOW results show errors that are significantly larger than the errors for the other contributions.

4.2 Thrust comparison

In Fig. 17, the thrust values obtained in the ReFRESCO computations are presented together with the experimental values on an absolute scale, first as a function of the lateral position for case 1, 2 and 3 (Fig. 17a), and afterwards, as a function of the under keel clearance for case 3, 4 and 5 (Fig. 17b). The relative errors computed using Fig. 2 are displayed for all cases in Fig. 17c. On an absolute scale, the computed thrust values deviate no more than 0.5 Newton from the experimental values. For case 1a and 2a, the trust is under-predicted by approximately \(15\%\), whereas for case 3a and 4a, it is predicted too high by about 11 and \(9\%\), respectively. For case 5a, the error is less than \(0.5\%\). In general, it is seen that the trend as a function of the water depth is reasonably captured, but not the trend due to the distance to the bank. In the present computations, no special treatment of the water depth or distance to the bank was done, and PROCAL has not been specifically developed for propellers operating in severely separating flow such as found in this study (see the discussion of the flow below). For example, it is assumed that the flow is fully attached to the propeller blade. Also the flow is assumed to leave the blade exactly at the trailing edge. These assumptions are certainly violated in a massively separated wake field and may therefore explain part of the deviations from the measurements.

Open image in new window

5.1 Discussion of the flow

As can be expected, the influence of the bank or bottom becomes more severe when the ship is located closer to the side wall or when the water depth reduces. In Fig. 18, the limiting streamlines on the hull and the shear stress distribution on the hull and bottom are given to illustrate the flow. For all considered cases, a stagnation point is found on the bow. Depending on the proximity of the bank, the stagnation point tends to move to the starboard (bank) side, due to the displacement effect of the hull, deflecting the flow around the hull towards port side, away from the bank, in the fore ship area. This can be seen in the direction of the limiting streamlines aft of the bow. The flow accelerates between the vertical side of the ship and the side wall, resulting in a low pressure area and subsequently a suction force towards the bank. Just forward of midship, the limiting streamlines gradually change direction and show that the flow is directed towards the bank again in the aft area of the hull. Around the aft ship, the restriction of the flow due to the bottom and/or bank causes the flow to separate and reversal occurs. This is clearly seen in the diverging stream lines and low shear stress values at the starboard side of the aft ship. The separation also pushes the flow in the aft ship away from the bank again. In Fig. 19, the axial velocity distributions at the propeller plane (looking aft) are given for cases 1b, 3b and 5b. In each case large areas of flow reversal are found and it is seen that these areas increase when moving closer to the wall (case 1b) or when the water depth reduces (case 5b).

Open image in new window

Open image in new window

5.2 Water surface elevation

For the ISIS-CFD computations, the water surface elevation was extracted along a line parallel to the quay, 0.02 m from the quay. The longitudinal coordinate is made non-dimensional using the characteristic ship length \(L_{\text {pp}}\) and an offset is applied to set the origin at the midship location. After conversion to millimetre, the results as shown in Fig. 20 are obtained for the cases with and without propulsion. For case 3b, results for a computation with adaptive grid refinement (AGR) are presented as well, these are labelled ISIS-CFD (AGR). The result obtained on the base mesh that is used as a starting point for the AGR computation is given as well (ISIS-CFD-c2). For cases 1b, the result of a computation using a second-order time integration scheme is shown as well, this is labelled ISIS-CFD (unsteady).

All computational results predict the maximum value of the trough with an error less than 1 mm. The largest errors occur for the cases with \(H/T = 1.1\) (cases 5a (Fig. 20i) and 5b (Fig. 20j): the depth of the trough at the midship location is overpredicted by about 0.6 mm. The asymmetry in the depression observed for cases 2a and 2b in the experimental data is predicted with the CFD results, see Fig. 20c, d. This asymmetry is also observed for cases 1a and 1b.

Open image in new window

For case 3b (Fig. 20f), the ISIS-CFD (AGR) result does show an improvement both in the shape of the trough and the maximum depression when compared to the coarse result from which it was started (ISIS-CFD c2): at the midship location, the error is now approximately 0.3 millimetre (this was 1.2 for the ISIS-CFD c2 result, shown in a light green colour in Fig. 20f) and the shape shows better agreement with the experimental measurement. From a user point of view, adaptive grid refinement is useful when engineering time (mesh generation) should be minimized.

5.3 Influence of distance to the bank

When the distance between the ship hull and the bank decreases, lower pressures are generated on the starboard side of the ship and therefore the suction force towards the bank increases. This can be easily seen in Fig. 21 (left), which shows the pressure distribution on the hull and channel boundaries for three different distances to the vertical wall. The lower pressure area also results in an increase of the heeling moment. The change in yaw moment as a function of the distance to the bank is less pronounced. For the smallest bank distance, it can be seen that a significant low pressure area develops at the starboard side of the bow, which results in a change of the trend of the yaw moment.

Open image in new window

5.4 Influence of water depth

As expected, a smaller water depth amplifies the low pressure area on the bottom of the hull, see Fig. 21 (right). Additionally, the blockage of the flow in the channel increases and more flow separation is found around the aft ship (see also the regions with low axial velocity shown in Fig. 25 for case 3b with 35% under-keel clearance and Fig. 23 (bottom) for case 5b with 10% under-keel clearance). Due to the blockage, the flow is deflected around the model towards port side and the pressure at the port side of the model reduces. Additionally, a shift of the stagnation point on the bow to starboard is found. In the \(H/T = 1.50\) case, the side force is directed to the bank, but in reduced depth conditions the low pressure area on port side and the high stagnation pressure on the starboard bow area result in a decrease of the side force. This was also found and discussed by [34]. Both ISIS-CFD and ReFRESCO predict that in the \(H/T = 1.1\) case the side force will even be directed away from the bank. This is however not confirmed by the measurements.

5.5 Influence of propeller

In Fig. 22 (left), the pressure distribution on the hull, vertical wall and channel bottom is compared for the case with the smallest distance to the bank with (case 1a) and without (case 1b) propeller action. It is seen that the suction of the propeller accelerates the flow in the aft ship, leading to slightly lower pressures. This results in a slightly higher side force and more negative (pulling the stern to the wall) yaw moment, see Fig. 14. Due to the propeller action, the flow does not separate as much as in the case without propeller and higher axial velocities are found in the area of the aft ship, see Fig. 22 (right). These findings agree with the conclusions from [34].

Open image in new window

5.6 Double body vs. free surface

Open image in new window

The computations with ReFRESCO have been done under the assumption that the free surface deformation does not strongly influence the results for this specific case. In the ISIS-CFD computations performed by FHR and ECN/CNRS, the flow was resolved including the free surface effects. In Fig. 23, the results from ReFRESCO are compared with the ISIS-CFD results obtained by FHR for case 5b. Case 5 has the smallest under-keel clearance and therefore the lowest water level in the channel and for this case the free surface effects are probably the largest, due to the largest blockage. From these figures, differences can be seen, showing especially a larger low-pressure area around midship in the double-body computation. It is therefore concluded that for this condition the free surface deformation may play a significant role. However, this case also exhibits a large area of flow separation [see the low velocity area behind the ship in Fig. 23 (right)] and this introduces instationary flow. The difference therefore may also be caused by uncertainties in the results from the different solvers.

For a less severe case, case3b, the differences between the double body approach and the approach with free surface is less pronounced, see case 3b from ReFRESCO in Fig. 21 (left) and from ISIS-CFD in Fig. 21 (right). Here, only small differences can be seen, which can be caused by differences due to the solver and grid, or by the use of the free surface. It is expected that for this case, with a relatively large distance to the bank and an intermediate water depth, the influence of the free surface modelling is not significant.

5.7 Effect of automatic grid refinement

In Fig. 24 the differences in the pressure distribution obtained with the original grid and with automatic grid refinement is illustrated. Only around midship, small shifts in the contour lines are found. Also in the axial velocity distribution, see Fig. 25, only small differences can be observed. Generally, it is concluded that the automatic grid refinement does not change the flow field drastically.

Open image in new window

Open image in new window

Open image in new window

5.8 Potential flow vs. viscous flow

To investigate the discrepancy of the ROPES predictions with respect to the measurements and the results for the viscous-flow predictions, the pressure distribution on the hull predicted by ROPES and by ReFRESCO are compared, see Fig. 26. It is seen that on the starboard (bank-side) of the hull, lower pressures are predicted by ROPES than by ReFRESCO. This results in a larger positive Y force, which is directed towards the bank. At the forward shoulder on port side, the low pressure trough is less in ROPES than in ReFRESCO. Additionally, the pressure recovery in the aft ship is much more pronounced according to ROPES. Subsequently, a higher pressure area appears to exist at the starboard side of the stern. The differences in the pressure distribution computed by ROPES will induce a larger positive yawing moment (turning the bow towards the vertical bank). These observations confirm the discrepancies found in Fig. 14. Apparently, when sailing close to a vertical bank, potential flow models will not be able to accurately predict the bank effects, and viscous-flow methods have to be adopted to obtain the right trends of bank suction or repulsion.