*6.5. Computational Grid*

A planing hull is subject to larger variations in trim and sinkage than a conventional displacement hull. One of the greatest challenges when developing a numerical simulation modelling a planing hull is ensuring the mesh can accurately deal with these motions. For this test program, the physical model was fixed in sinkage and trim, removing the need for the mesh to be capable of modelling motion and allowing a rigid mesh to be used as opposed to morphing or overset grids.

To generate the mesh Star CCM+'s automated meshing capability was utilised [35], with the surface remesher, automatic surface repair, trimmed cell c and prism layer mesher selected. The 'trimmed cell mesher' was selected as it aligns the cells with the direction of the flow, minimising numerical diffusion. This feature relies upon the Cartesian cut-cell method. It allows for a large degree of control through the use of local surface and volumetric controls that allow the user to increase or decrease the mesh density. This method presents a robust and efficient method of producing a high-quality grid, predominantly made up of unstructured hexahedral cells with polyhedral cells next to the surface. The mesh is formed by constructing a template mesh from the target sizes input by the user, and then trimming as required, this using the input surfaces. Using a trimmer mesh enables the use of growth parameters that can be used to ensure there is smooth transitions within the mesh and help prevent the introduction of numerical errors.

Volumetric controls were used to progressively refine areas of the mesh in which flow features of interest occurred, ensuring that the mesh was capable of capturing the complex flow in these regions. The areas that were identified for progressive refinement were the free surface, the area surrounding the hull, and the wake region, with three layers of increasing refinement used for each. Additional refinements were included at the bow, the stern, and for the free surface upstream of hull. These further enhance the resolution where the largest flow gradients occurred, and to help prevent Numerical Ventilation. Figure 5 shows the computational grid and the refinements that it contains. It should be

noted that the mesh shown was for the coarsest studied in the mesh study as it shows the refinement zones clearly.

**Figure 5.** Computational Grid.

To allow the simulation to accurately resolve the high velocity gradients associated with the boundary layer flow the 'prism layer mesher' was used. This generates orthogonal prismatic cells adjacent to the hull. These are high-aspect ratio cells that are aligned with the local flow and are vital for the accuracy of the simulation. The thickness of the prism layer was calculated to be equal to the thickness of turbulent flow (δ) for a given Reynolds number (*Rn*) over a flat plate of the same wetted length (*x*), as calculated by [40]:

$$\frac{\delta}{\chi} = 0.38 R\_n^{-\frac{1}{5}} \tag{2}$$

After the simulation converged satisfactorily, a scalar plot of the Turbulent Viscosity Ratio was checked to ensure that the prism layer was thick enough. If the prism layer mesh is not thick enough then a non-trivial amount of turbulent viscosity would be present in the core mesh, indicating that part of the boundary layer has diffused into the core mesh region.

The first cell height of the prism layer was calculated to ensure that the *y*<sup>+</sup> value was below one. A stretching ratio of 1.2 as suggested by [37] was used to grow the prism layer until it reached the desired thickness. Care was taken to ensure that the outer layer of the prism layer mesh and the first layer of the core mesh were of comparable sizes to ensure that numerical errors were not introduced.

An additional volumetric refinement was included in the area in which the free surface met the hull. The prism layer thickness was reduced to 25% of the calculated thickness in this region as suggested in [30].This further reduces Numerical Ventilation as it decreases the numerical diffusion caused by the cells of the prism layer that are misaligned with the free surface.

A mesh study was undertaken to ensure that the mesh was fine enough, resulting in the final mesh consisting of around 20 million cells. The choice to follow a low *y*<sup>+</sup> approach significantly increased the cell count, however as the body was fixed this did not result in an impractical computational time to reach convergence. Simulations took between 7.5–27 h to run on the Archie-WeST High Performance Computer (HPC), equating to between 300–1080 core hours. The large variation in run time was caused by differences in the physical time the simulation had to run for to converge satisfactorily. Another factor effecting the run time was that some simulations required very large number of iterations in the early stages of the simulation to ensure that the large gradients associated with beginning a simulation did not cause divergence.

#### **7. Verification and Validation of CFD**

In most examples of planing hull simulations available in literature validation is conducted by a straightforward comparison of the simulated result and tank testing data. This approach is rather basic and may not be used to evaluate the true accuracy of the simulation. It is possible for numerical and experimental results to be very close; however, this may be by chance with the simulation containing considerable numerical uncertainties, which combine to give the correct result. Without conducting a thorough Verification and Validation (V & V) study, there can be little confidence in any results as the accuracy and uncertainty of the simulation has not been evaluated. As such, one should be completed prior to generating any results for analysis. The ITTC has published guidelines on how best to perform aV&V study in relation to marine simulations [41]. The full V & V methodology and procedure that was followed is outlined in the aforementioned guidelines.

Before continuing, it is necessary to provide a brief definition of Validation and Verification:


The ITTC recommendations [41] are based upon the work of [43]. This approach defines errors and uncertainties in a way that is consistent with experimental uncertainty analysis, where the simulation error (δ*S*) is the difference between a simulations result (*S*) and the truth (*T*), and is made up of modelling (δ*SM*) and numerical (δ*SN*) errors.

$$
\delta\_{\mathbb{S}} = T - \mathbb{S} \tag{3}
$$

$$
\delta\_{\rm S} = \delta\_{\rm SM} + \delta\_{\rm SN} \tag{4}
$$

The procedure relies upon the Richardson Extrapolation (RE) procedure [44], which is the basis for existing quantitative numerical uncertainty and error estimates for both grid and timestep convergence [45]. Following the method, the error is expanded in a power series, with integer powers of grid spacing or timestep taken as a finite sum. When it is assumed that the solutions lie within the asymptotic range it is acceptable that only the first term is considered, leading to a so-called triplet study.

The Correction Factor approach was employed. The first step of this approach is to assess the convergence condition using the convergence ratio (*Ri*), defined as the ratio between ε*i*,21 = *Si*,2 − *Si*,1 and ε*i*,32 = *Si*,3 − *Si*,2. Here *Si*,*<sup>k</sup>* refers to the solution obtained from the *i th* input parameter using the *kth* refinement. The solutions obtained by systematically coarsening the *i th* parameter by the refinement ratio, *rk*. Four convergence conditions may exist, as defined by [43]:


For the first condition, Generalized Richardson Extrapolation is used to assess the uncertainty (*Ui*). The error and order of accuracy must be calculated:

$$
\delta\_{RE\_{i,1}}^{\*} = \frac{\varepsilon\_{i,21}}{r\_i^{P\_i} - 1} \tag{5}
$$

$$P\_i = \frac{\ln\left(\frac{\varepsilon i\_i \chi}{\varepsilon i\_i \mathbb{1}}\right)}{\ln(r\_i)}\tag{6}$$

Using a correction factor approach provides a quantitative measure of defining how far from a solution is from the asymptotic range, and then approximately accounting for the effects of higher order terms when making error and uncertainty estimates. It is based on verification studies for 1D wave and 2D Laplace equation analytical benchmarks. These showed that one-term RE error estimates are poor when not in the asymptotic range, but that multiplying them by a correction factor improved error and uncertainty estimates. The numerical error is defined as:

$$\delta\_i^\* = \mathbb{C}i\delta\_{RE\_{i,1}}^\* = \mathbb{C}i \begin{pmatrix} \frac{\mathbb{C}i,21}{r\_i^{P\_i} - 1} \\ r\_i^{P\_i} - 1 \end{pmatrix} \tag{7}$$

The correction factor (*Ci*)is based upon replacing the observed order of accuracy with an improved estimate, which roughly accounts for the effects of higher order terms. This limits the order of accuracy of the first term as spacing size goes to zero and ensures that as the asymptotic range is reached (*Ci*) tends to zero [43].

$$\mathbf{C}\_{i} = \frac{\begin{pmatrix} r\_{i}^{P\_{i}} - 1 \end{pmatrix}}{\begin{pmatrix} r\_{i}^{P\_{\text{est}}} - 1 \end{pmatrix}} \tag{8}$$

Depending how close the numerical error (δ∗ *i* ) is to the asymptotic range determines the expression that is used to evaluate the solution uncertainty:

$$\mathcal{U}I\_{i} = \left[\Theta.6(1-\mathcal{C}\_{i})^{2} + 1.1\right] \Big| \delta\_{R\mathcal{E}\_{i,1}}^{\*}\Big|\left|1-\mathcal{C}\_{i}\right| < 0.125\tag{9}$$

$$\delta L\_i = \left[2|1 - \mathcal{C}\_i| + 1\right] \left| \delta\_{RE\_{i,1}}^\* \right| |1 - \mathcal{C}\_i| \ge 0.125 \tag{10}$$

Validation is the process of assessing the simulations modelling uncertainty (*USM*) by using benchmark experimental data, and where possible the modelling error (δ*SM*). The comparison error (*E*) is defined as the difference between the data (*D*) and the simulation solution (*S*).

$$E = D - S = \delta \mathbf{D} - (\delta\_{\rm SM} + \delta\_{\rm SN}) \tag{11}$$

Modelling error (δ*SM*) can be decomposed into modelling assumptions and use of previous data. To determine if validation has been achieved the comparison error is compared to the validation uncertainty (*UV*) as given by:

$$\mathcal{U}\_V^2 = \mathcal{U}\_D^2 + \mathcal{U}\_{\text{SN}}^2 \tag{12}$$

If the validation uncertainty is smaller than the comparison error then the combination of all of the errors in the experimental data and the numerical data is smaller than the validation uncertainty. This allows the simulation to be considered validated at the level of the validation uncertainty.

$$|E| < \mathcal{U}\_V \tag{13}$$

*V & V Case*

Having completed the setup of the simulation a V & V study was undertaken. Both grid and timestep studies were conducted, producing a triplet of results and allowing the analysis of the uncertainty attributable to both. For the grid study, a refinement ratio of <sup>√</sup> 2 was selected, as recommended by the ITTC. For the timestep study, a refinement factor of 2 was selected. These refinements were previously used by [28], and shown to provide a strong validation case. The case for which the V & V was carried out for was a trim angle of 4◦ and a speed of 4 ms<sup>−</sup>1.

The triplet of solutions for both the grid and timestep studies displayed monotonic convergence. Specific grid and timestep uncertainties were calculated following the Correction Factor approach. Prior to this, it was checked that the iterative uncertainty was negligible and would not contaminate the results. The calculated uncertainties, and whether each parameter has been validated, are shown in Tables 2 and 3, respectively.


**Table 2.** Grid Convergence Study.


As can be seen, suitably small uncertainties exist for most parameters. Larger uncertainties for *UG* were calculated for resistance and lift, showing that these parameters are reasonably sensitive to the grid resolution.

Following the calculation of the uncertainties it is possible to determine whether the simulation may be considered validated. The results for this are shown in Table 4. The validation uncertainty for both resistance and lift was found to be lower than the comparison error, deeming the simulation valid for both these parameters. The same cannot be said for trimming moment unfortunately. This however, was only included as a means of establishing the accuracy of the simulations and was not the primary focus of the study. As the simulation had been validated for both resistance and lift, it was deemed satisfactory to proceed.

**Table 4.** Validation Study.


### **8. Results**

The following section will compare and discuss the results. While only certain results are shown here, the full data set may be found in the Appendices. The results section first details the findings of the investigation into the impact of a number of parameters upon the accuracy of the CFD simulation. This attempts to highlight what may be considered vital when establishing a simulation that looks to accurately model the nearfield longitudinal wake field of a high-speed planning hull. It then goes on to discuss and compare the experimental and numerical resistance, lift and trimming moment results. This comparison is made to evaluate the accuracy of the CFD at modelling forces before investigating its ability at modelling wake profiles. Following this, the quantitative wake profile data from each method will be analysed, with qualitative wake profile data in the form of pictures. All graphs are presented with error bars as calculated in the Experimental Uncertainty andV&V sections.

The wake profile plots are presented in a format consistent with those as presented by [10], with the origin representing the point where the keel meets the transom and the horizontal axis in line with the keel, as seen in Figure 6. The distance aft of the transom, and height of the wake profile, have been nondimensionalised by beam on all figures.

**Figure 6.** Results Reference Axis.

#### *8.1. Parameters A*ff*ecting CFD Accuracy*

A number of parameters that had the potential to impact the accuracy of the CFD simulation were identified to be systematically studied. The focus of this study was to establish what effect they had on the accuracy of the calculated wake profile; however, their effects on the calculated forces and moments are also noted. The purpose of presenting these results as opposed to only these of the final set up is to provide insight to other researchers working within the same field. Over the course of this work, tens of thousands of CPU hours were used to establish what set up produced the most accurate results.

During the systematic testing, as many factors as possible were held constant, with only the parameter under examination being varied in an attempt to isolate its impact upon the results. In the following discussion, the percentage differences given show the difference in comparison error with the experimental results, with a negative value indicating that the result was found to be further from the experimental data.

#### 8.1.1. Use of the Symmetry Condition

It is common practice to employ a symmetry plane as a boundary condition on the centreline of the vessel when the computation is for a steady state simulation. This strategy halves the mesh count and allows for a significant reduction in computational demand. The ITTC [46] does note that this approach this may led to a loss of physics when transient flow occurs between port and starboard and recommends that if a Detached Eddy Simulation (DES) or Large Eddy Simulation (LES) approach is followed then a full domain should be modelled. When photos of the experimental study are examined elements of flow are seen to cross the centreline. It is, thus, necessary to establish whether the use of the symmetry boundary condition causes the wake field to be incorrectly calculated due to the lack of modelling of these elements.

The use of the symmetry condition was found to have no significant impact on the results of the simulation. A difference of 0.11% in resistance, −0.15% in lift, and −0.37% in trimming moment were found when it was employed, while both the centreline and quarterbeam longitudinal profiles were identical. A final check of the surface elevation plots revealed no significant differences in the wake field. The results of this suggest that a Reynolds-averaged Navier–Stokes (RANS) approach to modelling the flow does not provide enough resolution to capture the asymmetric elements of flow that are present. In order to accurately model these, it is suggested that the higher fidelity DES or LES approaches are employed.

### 8.1.2. Use of the Surface Tension Model

The inclusion of the surface tension model adds a tensile force tangential to the interface separating two fluids. This force works to keep the molecules of fluid that are at the free surface in contact with the rest of the fluid [47]. When the surface tension model is included in a simulation the Navier–Stokes equations are reformulated to contain an additional source term, which accounts for the momentum exchange across the interface due to the surface tension forces [48]. Surface tension may have a larger impact upon the hydrodynamic forces of a small-scale model due to the relative larger size of the surface tension forces. As it also effects the creation of the free surface, it is necessary to determine how its inclusion impacts both the calculated forces and wake profile.

When the surface tension model was included a difference of −1.68% in resistance, 2.87% in lift, and 11.68% in trimming moment were found. This shows that due to the small scale of the model the surface tension forces influence may be considered significant. This may in part be due to the reduction in the level of numerical ventilation as discussed in the CFD set-up section. When the centreline and quarterbeam profiles were examined, they were seen to be largely similar, with the surface tension model reducing the accuracy by a maximum of 1.51 mm. Despite the reduction in accuracy the inclusion of the surface tension model was deemed to be more physically representative.

#### 8.1.3. Approach to Turbulence Modelling

In most flow problems, walls are a source of vorticity and as such accurately predicting the flow and turbulence parameters in the wall boundary layer is essential. The presence of the wall results in the gradients of the flow variables becoming very large and as the wall distance reduces to zero. The behaviour of the flow in this region near is a complex phenomenon that is made up the viscous sublayer (where the flow is dominated by viscous effects), the buffer layer (where viscous and turbulent stresses are of the same order), and the log-law layer (where turbulence stress dominates the flow). The concept of wall y+ is used to distinguish between these components, with its value being used to determine the characteristics of the flow.

Wall treatment models are a set of configurations and assumptions that are used by a CFD solver to model the near wall turbulence quantities such as the turbulence dissipation, turbulence production and the wall shear stress. These are categorised as high or low *y*<sup>+</sup> wall treatment, with each following a different approach to resolve the flow in the boundary layer.

If a low *y*<sup>+</sup> approach is chosen, the whole near wall turbulent boundary layer is resolved, including the viscous sublayer, the buffer layer, and the log-law region. There is no modelling used to predict the flow, with the transport equations being solved all the way to the wall cell and the wall shear stress being computed as in laminar flows. In order to resolve the viscous sublayer the mesh has to be suitably fine, with a *y*<sup>+</sup> value of one or less, ensuring that the centre of the wall cell located in the viscous sublayer. This approach can be very computationally expensive as a large number of prism layer cells may be required to ensure the wall cell is placed within the viscous sublayer [47].

The high *y*<sup>+</sup> approach models the viscous sub layer and the buffer layer using wall functions for the turbulence production, the turbulence dissipation and the wall shear stress. These are values are derived from equilibrium turbulent boundary layer theory. Using wall functions to model these means that the mesh is not required to resolve the viscous sublayer and the buffer layer and can therefore be far courser. For a high *y*<sup>+</sup> approach to be valid there should be *y*<sup>+</sup> that is larger than 30 to ensure that the wall cell is in the log-law region of the flow. There have been successful applications of a high *y*<sup>+</sup> approach using a *y*<sup>+</sup> value of up to 500 in marine and civil engineering applications, however best practice guides recommend an upper limit of 100 unless a thorough validation is carried out. Following a high *y*<sup>+</sup> approach results in a significant saving in computational time as far fewer prism layer cells are required [47].

The decision on whether to adopt a high or low *y*<sup>+</sup> approach is generally based upon the computational resources that are available. When the literature was reviewed in relation to planning hulls (both conventional and stepped), no examples of low *y*<sup>+</sup> approaches were found. However, for conventional marine CFD the wall function approach performs remarkably well at predicting the resistance and does not seem to compromise the quality of the solution [11].

Both a high *y*<sup>+</sup> of 40 and low *y*<sup>+</sup> of 1 were employed to assess their impact upon the results. The number of prism layers increased from 9 to 28, while the total thickness and stretching ratio remained constant. The change from high to low *y*<sup>+</sup> increased the cell count by 82% and increased the run time by 68%. It was found that changing to a low *y*<sup>+</sup> approach caused a 6.01% change in resistance, a −10.08% change in lift, and a −21.50% change in trimming moment. When the wake profiles were examined it was found that there was a maximum difference of 4.75 mm for the centreline wake profile,

and a maximum difference of 3.33 mm for the quarterbeam profile, where the low *y*<sup>+</sup> profiles were found to be more accurate.

The results show that the choice between a low and high *y*<sup>+</sup> approach is the numerical set up factor that has the single largest effect upon the accuracy of the solution. As the low *y*<sup>+</sup> approach resolves the viscous sublayer the calculation of forces should be more accurate, however it has been shown to be detrimental in terms of lift and trimming moment. Planning hulls clearly do not fall into the same category as displacement hulls where this selection has been shown to have little impact. A more comprehensive investigation into the effects of selecting a low *y*<sup>+</sup> approach over a range of speed and trim conditions is recommended in the future to gain a more detailed understanding.

#### 8.1.4. Choice of Turbulence Model

Whilst it is possible for the exact turbulence solution in a simulation to be fully described by the Navier–Stokes Equations through Direct Numerical Simulation (DNS), it is impractical due to its requirement for massive computational resources. A commonly accepted alternative that is less computationally expensive is to solve for averaged (or filtered) quantities, and approximate the impact of small fluctuating structures. This is known as a Reynolds-averaged Navier–Stokes (RANS) approach, which utilises turbulence models. These models provide closure of the RANS equation and are approximate representation of the physical phenomena of turbulence [47].

The ITTC [36] states that the two-equation turbulence models have been shown to give accurate predictions in ship hydrodynamics. Larson [16] concluded from his analysis of the entries to Gothenburg 2010 Workshop that there was no visible improvement in accuracy for resistance prediction when turbulence models that are more advanced than the two-equation models were used. It found that κ−ω was by far the most applied with 80% of the submissions for the workshop using some form of variation of them. Other authors have also concluded that for resistance calculations the turbulence modelling has little effect on the prediction accuracy [32].

A review of other studies using CFD for planing hull performance prediction found that the majority of simulations use the κ−ε [14,19–21,23] or the κ−ω *SST* [26,27,48–50] models. Despite both models being comparable in terms of resistance prediction it has been shown by [16] that the choice of turbulence model has a profound influence on the accuracy of the local flow in the stern region. It was found that the wake predicted by advanced turbulence models such as Reynolds Stress Model (RSM), Explicit Algebraic RSM (EARSM), and κ−ω *SST* clearly show better correlation with measured data. This is echoed by [36], who concluded that wake can be predicted fairly accurately using advanced models such as κ−ω *SST*.

The κ−ε turbulence model is the baseline two-equation model, solving for the kinetic energy (k) and the turbulent dissipation (ε). This is one of the most commonly used turbulence models in industrial CFD and provides a good compromise between robustness, computational cost, and accuracy. This model is known to give good predictions for free flows with small pressure gradients [48]; however, performs poorly for complex flows with severe pressure gradients, separation, or strong streamline curvature.

The κ−ω *SST* turbulence model is a hybrid model that was developed by [51] in order to take advantage of the collective advantages of the κ−ε and the κ−ω models. It was developed to address the sensitivity issue with the free stream sensitivity faced by the standard κ−ω. The two models were combined into one using a blended function. This model uses the κ−ω model in the boundary layer, whilst the κ−ε (formulated on κ−ω) is used in the free flow [48]. The approach is accepted to have cured the biggest drawback of the κ−ω model when modelling practical flow simulations [47].

The two-layer approach allows the k-ε turbulence model to be applied to the viscous-affected layers. Following this approach, the computation is divided into two layers, where the standard turbulence model is used to turbulent kinetic energy for the whole domain and the turbulent dissipation away from the wall, while for the near wall layer the turbulent dissipation rate is calculated as a function of wall distance and local turbulent kinetic energy.

The realizable κ−ε model contains a new formulation to calculate the kinetic dissipation rate, and adds a variable damping function. This results in the model being substantially better than the standard κ−ε formulation for many applications, while the model can be relied upon to produce results that are at least as accurate as those of the standard model [47]. It is compatible with the two-layer approach, allowing it to resolve the viscous sublayer.

In the course of this study a four turbulence models were employed to gauge their effects on the calculation of forces and wake pattern. Where applicable, these were tested for both a low *y*<sup>+</sup> and high *y*<sup>+</sup> approach, resulting in seven test cases. The results showing the comparison error with the experimental data for all cases are detailed in Table 5.


**Table 5.** Turbulence Model Selection.

It is apparent that the choice of whether to employ wall functions or to resolve the viscous sub-layer remains the largest factor that effects the accuracy for all turbulence models. It is once again seen that following a low *y*<sup>+</sup> approach results in more accurate resistance prediction; however, less accurate lift and trimming moment prediction. It is seen that the choice of model has a larger effect on the results for the low *y*<sup>+</sup> cases, resulting in variations of a 4.75% in resistance, 1.91% in lift, and 10.74% in trimming moment. The variations for the high *y*<sup>+</sup> cases were significantly smaller with 2.59% in resistance, 0.20% in lift and 0.98% in trimming moment.

When the wake profile plots are examined it is found that the choice of turbulence model has no discernible impact upon the results, while the choice of turbulence modelling approach is once again seen to have some effect. For all high *y*<sup>+</sup> cases, the centreline wake profiles are almost identical, regardless of turbulence model, with a maximum difference of 0.21 mm. Low *y*<sup>+</sup> cases result in a the centreline wake profiles that is more accurate than the high *y*<sup>+</sup> results, but these are once again almost identical, regardless of turbulence model with a maximum difference of 0.15 mm. Similar trends were found for the quarterbeam profiles, where the low *y*<sup>+</sup> was seen to be more accurate. These profiles feature slightly more variation with a maximum variation of 0.58 mm for the high *y*<sup>+</sup> approach and 0.42 mm for low *y*+.

It can be concluded from this study that while the choice of turbulence model clearly effects the boundary layer and the resultant forces that are calculated for the hull, it has little impact upon the flow and the wake pattern remains largely unchanged when different turbulence models are employed.

#### 8.1.5. Spatial and Temporal Discretization

As is discussed in the V & V section the improper choice of the fineness of either the temporal or spatial discretization of the simulation space may result in inaccuracies. If the selected values for either are to large it will result in the simulation being incapable of capturing the phenomena that are occurring. The effects on the calculation of forces has been studied and discussed in the V & V section, where it was seen that the spatial discretization caused variations of 6.50% in resistance, 6.11% in lift and 13.10% in trimming moment. The temporal discretization was less influential however still caused variations of 1.33% in resistance, 1.55% in lift, and 2.17% in trimming moment.

While the discretization of the simulation space was seen have a large impact upon the calculation of forces, it was found to have negligible impact upon the wake profiles. As the data was extracted from the V & V study, all data variations for one factor were made with the finest selection of the other. The spatial discretization was found to produce a maximum difference of 0.85 mm while the temporal discretization was found to produce a maximum difference of 0.38 mm.

#### 8.1.6. Conclusions

From the study of factors effecting the accuracy of the CFD, it can be seen that the calculation of forces is far more sensitive than the calculation of the wake profiles. The approach to modelling turbulence was found to be the most influential on the calculation of the wake profile, with simulations where the laminar sub-layer is resolved found to be more accurate. The selection of the turbulence model itself was shown to have limited impact on the wake profile. The second most influential factor was found to be the inclusion of the surface tension model; however, further investigation is required to establish if this is the case for all simulations or it is accountable to the small scale testing approach that was employed and the scale of surface tension effects relative to the calculated values. The spatial and temporal discretization showed that the choice of grid refinement was more important than that of timestep to accurately predict the wake pattern; however, this study also showed relatively course set ups to be capable of modelling the wake with a surprising degree of accuracy. Finally, it was shown that for RANS simulations the use of a symmetry boundary condition on the centreline has no effect on the calculation of the wake profiles.

#### *8.2. Resistance*

The choice of hull positions was selected in order to provide a broad range of conditions for which the ability of CFD at predicting the wake profiles would be assessed. As such, there were no systematic changes between each of the conditions tested, and no real conclusions can be drawn from a comparison between the measured forces of each.

The comparison error in resistance varies between 4.63% and 19.74%, with an average value of 12.43%. The comparison error is made significantly worse by the results for trim condition 3◦, which have an average error of 16.76% and is notably larger than for 4◦ & 1.9◦, which have average comparison errors of 11.49% & 9.04%, respectively. The relatively large errors that are found by this study are likely attributable to issues arising from small scale testing, as outlined by [10]. The key points of this discussion were in relation to the fact that the effects of positioning errors were amplified for a small-scale model when compared to a larger, more conventional model, and also that a standard absolute error value becomes a larger percentage value for the smaller forces associated with a small model.

It is commonplace for CFD simulations of High Speed Vessels to achieve an error of 10% [11]. While the 1.9◦ and 4◦ were found to have an average error in this region it is expected that the accuracy of these simulations should have been higher due to the high cell number used, and the higher fidelity low y+ scheme that was employed. It is seen that for the 3◦, which has a considerable higher average error. The errors in the resistance are caused predominantly by errors arising from the accuracy of the hull positioning. Accurately determining the position of the hull and measuring this relative to a known location was one of the main challenges outlined for small scale testing. It is likely the case the position of the models in the experiments does not exactly match the hull position in the CFD simulations due to this. A sensitivity study was undertaken determine the effect of a small positioning error, finding that a small change in position did have a large effect upon the results and confirming that the large errors were accountable to positioning errors.

The sensitivity study found that a 1 mm positioning alteration to sinkage caused a 3.27% change to resistance, a 0.55% change to lift, and a 8.45% change in trimming moment. A 0.1◦ alteration in trim produced respective changes of 7.96%, 5.10%, and 7.78%. Finally, a combined alteration of 1 mm in sinkage and 0.1◦ in trim caused respective changes of 11.21%, 6.50%, and 13.97%. This study goes some way to highlight the problems associated with small scale testing, showing how sensitive to plausible positioning errors the results are. When the wake profiles for all cases studied in the sensitivity study were examined; however, they were found to contain no significant changes. This allows a higher

degree of confidence in both the experimental and numerical results of the wake profiles that for the forces and moment.

Despite the errors, it can be seen in Figure 7 that for all cases the CFD results show relatively good agreement with the experimental results. It has been reported by [52] that once a hull is in the fully planning regime a linear trend between resistance crests may be expected. When a linear data is applied to the experimental results, an *R*<sup>2</sup> value of 0.99 is returned, indicating that the speed range studied is showing this linear trend between resistance crests. A linear data fit applied to the CFD results also returns an *R*<sup>2</sup> value of 0.99, showing CFD is modelling the same trend as is apparent in the experimental data.

**Figure 7.** Numerical Resistance Results.

*8.3. Lift*

The experimental set up only measured dynamic lift, whereas the CFD measured both the buoyant and dynamic components. As such, the CFD results were corrected to dynamic lift by determining the buoyant contribution and subtracting it from the total lift. The results for the dynamic lift are shown in Figure 8.

For trim angles of 3◦ and 4◦, the CFD results show good correlation with the experimental data, however at the higher speeds of 3◦ accuracy is lost a little. This can be seen to a lesser extend for 4◦ as well. For 1.9◦, the CFD trend is very different from the experimental trend. The CFD trend remains linear, with an *R*<sup>2</sup> of 0.99, and does not plateau as the experimental data does. This fits more with what was expected for the lift, given that the experimental results of 3◦ & 4◦ are shown to vary linearly with speed.

#### *8.4. Trimming Moment*

Trimming moment is more closely linked to lift than resistance due to the larger moment arm, so as would be expected given that the CFD lift data shows good correlation with the experimental data, so too does the trimming moment. The results for the trimming moment can be seen in Figure 9. There is good correlation between the two methods for 3◦ & 4◦, with linear fits returning *R*<sup>2</sup> values of 0.99 for all cases. Similar to the lift results, for 1.9◦, the CFD trimming moment maintains a linear trend and does not feature the plateau of the experimental data as it is heavily influenced by the lift.

**Figure 9.** Numerical Trimming Moment Results.

#### *8.5. Centreline Wake Profiles*

This section presents the experimental and numerical results upon the same graphs, allowing an easy comparison to be made. The results of Savitsky's Wake Equations and the Linear Wake Assumption as calculated by [10] are not presented in this section, however they are included in the appendixes to allow for an easy comparison between methods. The results for all cases will not be presented here as to do so would require 20 individual graphs, which instead will be detailed in Appendix A. The data presented in this section has been selected to highlight key findings and trends in the results.

It should be noted that the experimental uncertainty in the measurements of the wake profile amplitudes was 0.56 mm. This uncertainty is not displayed as error bars on the graphs, as they are not visible due to the scale of the graphs. Unfortunately, it was not possible to determine the uncertainty in the CFD results. Following the mesh and timestep studies, the wake profiles were shown to be have insignificant differences between them so it can be assumed that the numerical uncertainty is negligible.

In all cases, the centreline wake profile as calculated by the numerical solution is shown to have good correlation with the experimental results. It shows CFD to be an accurate and robust method of calculating wake profiles across a range of speed and trim conditions. At the lower speeds of 2 and 3 ms−1, the CFD results are seen to marginally under predict the amplitude of the wake profile; however, at the larger velocities of 4 and 4.5 ms−<sup>1</sup> the opposite is true, with CFD being shown to slightly over predict the wake profiles.

Figure 10 shows what is considered the best-fit result when all cases are compared. As can be seen the CFD profile may be considered an extremely good fit with the experimental data, passing almost exactly through the data points from zero to −0.4 m. Following this there is a slight deviation, with a maximum difference of 2.56 mm, which has a corresponding comparison error of 3.83%. The best fitting point in this case has a deviation of 0.03 mm, or a corresponding comparison error of 0.04%.

**Figure 10.** Best-Fit Computational Fluid Dynamics (CFD) Results.

Figure 11 shows what is considered the worst fit of CFD results to experimental data. Despite this there is still seen to be a very good correlation between the data. The maximum deviation is 4.72 mm, or a comparison error of 10.87%. When the other centreline cases are examined, it is found that the second worst deviation is 4.18 mm with a comparison error or 7.37%.

**Figure 11.** Best-Fit Computational Fluid Dynamics (CFD) Results.

The comparison of experimental centreline profiles to those calculated numerically validates the use of CFD in this application. The results are shown to have good correlation for all conditions, with the best and worst fit being discussed here. Whilst all the data points were not analysed, the best and worst have been, showing the CFD results to have a deviation of between 0.03 mm and 4.72 mm. When the results of Savitsky's Wake Equations and The Linear Wake Assumption are considered, the results generated through CFD are considerably more accurate. This method may be considered accurate and capable of modelling the nearfield longitudinal wake profiles of a high-speed planing hull.
