*3.7. Numerical Ventilation*

In the case of planing hulls, for very high speeds, phenomenon of ventilation can occur: A thin film of air gets caught between the hull and the water, drastically reducing the drag. This is a well-known phenomenon often exploited to improve the design of high-speed planing motor yachts to reduce the viscous drag with water. Ventilation requires a speed of an order of magnitude greater than the speeds tested; therefore, it was not tested in the real experiment, nor will the sailboat ever experiment with it.

However, the numerical model can suffer from numerical ventilation [7,8,37], even for low speed such as 3 m/s (Froude number = 0.4465), for particular hull shapes or trimming angle, especially if the bow is not piercing the sea surface but lies over it [12,13], as shown in Figure 11.

**Figure 11.** Bow is lying on the surface and not piercing it for high speeds.

When implementing a dual phase simulation, due to the numerical interpolation method in the VOF model, it is possible that a fraction of air gets caught and remains trapped under the hull, creating a mixture of phases [30], as shown in Figure 12. Air usually undergoes the hull at the bow and travels down to the stern, establishing a steady flux. As a consequence, the wall friction drag is underestimated. It is worth remarking that the contribution of the form drag to the overall drag is not affected by numerical ventilation.

**Figure 12.** Ventilated hull at 3 m/s, bottom view.

In order to solve numerical ventilation related problems, in this work, two approaches are used:

(1) The first approach is related to the refinement of the mesh near the interface between water and air in the aft part of the bow. Here, an isotropic mesh is also used for the sea surface because an anisotropic mesh is more subject to numerical ventilation. This treatment works best when paired with the high-resolution interface capturing (HRIC) scheme designed to mimic the convective transport of immiscible fluid components, and is thus suited for tracking sharp interfaces [37].

This approach requires the CFL number in the target region to remain low; therefore, the computational cost increases because a very small time step is required. Furthermore, increasing

the number of inner iterations in the implicit time-stepping scheme can reduce the likelihood of numerical ventilation; however, this numerical phenomenon remains dependent on the shape of the hull, trim angle, and speed of test, and may not be completely solved with this approach:

(2) The second method, used to completely resolve the numerical ventilation problem, is the phase-interaction substitution procedure. After the simulation is converged to a certain draft and trim angle and the wave pattern is well established around the hull, a phase interaction is applied which substitutes all fluid zones that contain mixed phases with water.

This procedure consists of the following steps:


The correct shear stress was computed, and the real wetted surface was used without changing the physics of the problem. This technique allowed for a higher time step and a coarser mesh, especially at the wall in the bow part. Numerical ventilation was solved and all the forces acting on the hull were computed correctly, as shown in Figure 13. The second approach was preferred because it worked well in a calm sea simulation and granted a faster solution than that of the first method.

**Figure 13.** Ventilation solved after the phase-interaction substitution procedure.

#### *3.8. Convergence Study*

Convergence study has key importance in every CFD simulation. This process proves that the discretization error has small influence on the result and that the solution will not change when refining the mesh. Convergence study allows the analyst to choose the best cell size, which represents an appropriate compromise between accuracy and computational speed; thus, it represents an opportunity to quantify the increment with an accuracy that a finer model would obtain, and compare it with the increase in central processing unit (CPU) hours required, as shown in Table 1.

Four different base sizes (the parametric value with which all the mesh is scaled) are investigated, associated with different cells' count: Halving the base size generates a number almost 23 times higher, since 3D volume cells are considered. When investigating grid convergence, it is important not to change other models and parameters, otherwise it would be impossible to discern what caused the different behavior in the simulation. This means scaling the time step for every different mesh size in order to maintain a constant CFL number. Similar considerations apply to the *Y*+ value, which must remain constant in all the simulations.

Therefore, a fixed value for the thickness of the first cell near the wall is used (when changing base size, not when changing the speed of the test), and the time step is scaled to maintain the same CFL for all the grids tested [38]. It is important to notice that simulation time increases significantly using the finest grid. This is not only due to the higher number of cells, but also to the smaller time step.

Table 2 presents the different base sizes used, the associated number of cells, the relative errors, and the corresponding CPU time of the simulation. The physical quantities that were monitored in this convergence study are the total drag experienced by the hull, the translation along the z axis, and the trim angle. The obtained total drag and vertical translations are shown in Figures 14 and 15, respectively. The benchmark used to build the error metrics is the dataset from the EFD. The method used for the analysis is the Richardson extrapolation, with the correction based on the total number of cells [39]. In this regard, the base size had to have a constant increment; in order to keep the cell count low, we decided for 1.5 as the multiplier for the base size.

**Table 2.** Convergence study and comparison with experimental data for the 3 m/s test.


**Figure 14.** Drag convergence.

**Figure 15.** Translation z convergence.

As shown in Table 2, the mesh resulting from the base size equal to one was chosen, since it achieved errors similar to the finest mesh, while computing 3 times faster. Further refinement of the mesh would not significantly increase the accuracy of the simulation but would make it more expensive.

#### **4. Results: Comparison between CFD and EFD**

Results in Table 3 are obtained from the postprocessing of CFD simulations and are presented in Figures 16 and 17. The main objective of this work was to validate the numerical model through comparison with experimental data. Furthermore, it is interesting to compare results with and without correction for numerical ventilation in order to evaluate the benefit of the numerical strategy herein proposed. Values of ΔTrim angle were positive when the bow was lifted up.

**Figure 16.** Total resistance curve: EDF vs. ventilated CFD vs. CFD with ventilation correction.

**Figure 17.** Δ Trim, CFD vs. EFD.

**Table 3.** Comparison between experimental fluid dynamic (EFD), computational fluid dynamic (CFD) with numerical ventilation, and CFD after correction.


As clearly shown in Figure 16, experimental results are better approximated when the numerical ventilation correction is applied. This method increased the total advancing drag of the hull and guaranteed a reduction of the relative error with respect to the experimental data; the error of the numerical model after correction was between 0.61% and 1.94% for drag, below the 2% threshold. The difference after ventilation correction was noticeable only for 3 m/s because for the other two speeds tested the numerical ventilation under the hull was practically absent. Moreover, it is important notice that the ventilation correction did not influence the trim angle at all, leaving it unchanged.

#### **5. Conclusions**

Considering the results that emerged from this work, the advantages of the CFD model have been confirmed. Numerical RANS simulation represents an accurate mean for the test of a new hull and can be useful during the boat design and testing process. This work aimed to group all the best practices that should be implemented during a CFD study of a hull in calm sea conditions, and represents the starting point for future studies regarding motion in head sea. Two different methodologies dealing with numerical ventilation, which can also occur for low speeds such as 3 m/s, were presented in this paper. The goal of having a fast and accurate simulation, and of solving the numerical ventilation problem, was achieved using the second methodology proposed, which fits perfectly for cases in which speed is low and no real ventilation occurs. It is worth noting that the phase substitution procedure cannot be used when the ventilation is both real and numerical because this method completely removes air from the bottom of the hull; therefore, the technique proposed here should not be used for high-speed planing crafts.

**Author Contributions:** Conceptualization, P.C., O.D., and G.M.; data curation, P.C., B.F., and G.G.; formal analysis, P.C. and O.D.; funding acquisition, P.C., O.D., and G.M.; investigation, P.C., O.D., and B.F.; methodology, P.C., O.D., G.G., and S.A.S.; resources, P.C., O.D., and G.M.; software, P.C., O.D., and B.F.; supervision, G.G., S.A.S., and

G.M.; validation, P.C., O.D., S.A.S.; visualization, P.C.; writing—original draft, P.C. and O.D.; writing—review and editing, P.C., G.G. and S.A.S. All authors have read and agreed to the published version of the manuscript.

**Funding:** This research received no external funding.

**Acknowledgments:** We would like to thank the Polito Sailing Team, especially all the members of the fluid dynamic area who contributed to carrying out the tests in the naval tank, and, most importantly, to the development of the numerical model presented here. Without their fundamental contribution this work would not have been possible. A special thanks goes to University of Napoli for providing free towing tank tests for all participants in the competition, providing the students with the opportunity to validate their work.

**Conflicts of Interest:** The authors declare no conflict of interest.
