1

Detailed Analysis of the Flow Within the Boundary Layer and

Wake of a Full-Scale Ship

Blanca Pena, Ema Muk-Pavic, Patrick Fitzsimmons

Department of Mechanical Engineering, University College London, London WC1E 7JE, UK

Abstract: This article presents a detailed numerical flow assessment of the boundary layer and wake

of a full-scale cargo ship. The assessment was conducted using a sophisticated numerical approach

that is able to resolve large turbulent scale vortices contained in the flow. The physical flow features

of the boundary layer and wake investigated include mean-velocity, near-wall shear stress and

vorticity fields. Also, the evolution of the wake from the thick boundary layer over the stern is

displayed and analysed in the highest possible detail. Additionally, the detailed information extracted

from the boundary layer and wake was the primary input to assess the overall hydrodynamic

efficiency of the full-scale general cargo ship.

The analysis method followed during this work has been a determinant factor for fast and efficient

design of energy saving devices, propellers or rudders that work within the limits of the boundary

layer of a ship. In particular, this thorough analysis avoided the necessity to use the commonly used

practice of trial and error that is typically followed in the maritime industry.

Keywords: hydrodynamics, turbulent boundary layer, CFD, full scale, ship efficiency.

1. Introduction

Experimental fluid dynamics towing tank tests have been traditionally used to evaluate the flow

around the ship. The main principle of this technique is to test a scaled model of the ship in similar

conditions to that of a full scale one. This approach is expensive, time-consuming and most

importantly carries significant limitations. Among them, due to Reynolds number differences, the full-

scale boundary layer is generally thinner than in model scale. Also, the aft boundary layer is

significantly different in model and full-scale. For applications such as ship resistance investigations,

model to full-scale scaling limitations are usually overcome by the application of empirical correlation

factors (Larsson and Raven, 2010). This is not the case for boundary layer investigations where a

model to full-scale correlation approach is not yet fully established (ITTC, 2014, ITTC, 2017).

An example of model scale assessments of the boundary layer and wake was conducted by Patel et al.

(1990). This type of investigation has been beneficial to a better understanding of the flow behaviour

2

on the ship aft end. Nevertheless, when an accurate picture of the full-scale aft end flow is required, a

model scale investigation is not the most suitable option.

An alternative method to assess the near-wall flow of the ship relies on viscous flow Computational

Fluid Dynamics (CFD). It is based on the Navier-Stokes equations and allows numerical modelling of

scenarios in full-scale, therefore avoiding scaling issues. For full-scale ship hydrodynamic

applications, Reynolds Averaged Navier–Stokes (RANS) is known to provide a quick solution as it

does not require significant computational power. Full-scale self-propulsion studies revealed that

RANS numerical model is able to provide good quality predictions of the propeller forces and

moment (Ponkratov and Zegos, 2015; Jasak et al., 2019; Bakica et al., 2020). These investigations are

in line with the results of the Lloyds Register First Full-scale Ship Hydrodynamics Workshop (Lloyds

Register, 2016). However, RANS might not be recommended for scenarios when the flow is

predominantly unsteady and/or hull flow separation is expected, this is particularly important for

calculations of the bilge vortex that typically forms at the stern of high block coefficient ships (ITTC,

2014).

If flow separation is expected, one could consider the implementation of Large Eddy Simulation

(LES) to model the turbulence contained in the flow. The principle of LES is to approach the

modelling of turbulence by considering that the large vortical structures created by the geometry

contain most of the energy within the bulk flow. LES resolves turbulent vortices everywhere in the

flow domain down to the grid size. LES could provide more accurate predictions of the fluid flow

than RANS; however, LES is still computationally unaffordable in full-scale ship hydrodynamics due

to the high Reynolds number.

A most recent approach for the simulation of turbulent ship flows is based on a combination of

RANS/LES, such as DES (Detached Eddy Simulation). This method combines the best features of

LES and RANS by only using LES away from the wall where a high level of unsteadiness of the flow

is expected (i.e. around the bilges, detached flow regions or in the wake) while RANS is applied in the

near-wall region. This method is more computationally affordable in ship hydrodynamics than LES,

allowing the study of complex unsteady flows in full-scale and being deemed as the best alternative to

calculate wake parameters, especially behind high block coefficient ships (Larsson et al., 2015). Full-

scale flow predictions using a DES97 and its improved version, a DDES, were conducted by Xing et

al. (2010). The authors established that both DES approaches improve the prediction of the total

resistance and velocity distribution for most of the propeller plane; however, the authors also revealed

that both models showed issues predicting the shear stress in the boundary layer region. Some of these

issues might be attributed to the log-layer mismatch behaviour that the DES97 and DDES models

exhibit (Spalart et al., 2006) which could be corrected using an IDDES approach and which represents

an improved version of the DDES and DES97 approaches (Shur et al., 2008a).

3

This paper presents a thorough analysis of the aft end boundary layer and wake of a full-scale ship.

The numerical approach used during this analysis is based on an IDDES approach that was previously

validated against sea trials torque data (Pena et al., 2020). Also, the computational mesh was tailored

to allow for the resolution of the largest turbulent vortex that is expected to be shed from the hull: the

bilge vortex. Nominal wake, resistance distribution and velocity fields have been post-processed to

assess the hydrodynamic performance of the 'MV Regal' (Lloyds Register, 2016), a full-scale general

cargo ship.

2. Benchmark Case Study

The 'Regal' is a 138m single screw vessel (Figure 1) with the following main particulars (Table 1):

Table 1 Regal main particulars (Lloyds Register, 2016)

Parameter

Length between perpendiculars, Lpp

138 m

Breadth moulded, B

23 m

Depth moulded, D

12.1 m

Draught, T

Ballast

Propeller diameter, D

5.2 m (four-bladed)

Before the sea trials, the vessel was dry-docked, the hull was cleaned, and the propeller surface was

polished. In this clean condition, the hull, rudder and propeller were 3D laser scanned to obtain an

accurate geometric representation. The scanned geometry was directly imported into the CFD

computations, thus ensuring high accuracy of the geometry CAD models.

Figure 1 Regal general cargo ship (Lloyds Register, 2016)

4

The sea trials were conducted in a reasonably calm condition, in compliance with the ISO 15016:2015

standard (ISO, 2015) and recommended sea trails procedure ITTC 7.5-04-01-01.1 (ITTC, 2014b). The

speed trials were conducted at ballast draught at three different shaft speeds.

Therefore, the scope of the analysis corresponds to the programme conducted during the Lloyds

Register full-scale Hydrodynamics workshop. These numerical study simulations of the flow around

the ship were conducted using the commercial CFD code Siemens Star CCM+. The numerical

experiments were undertaken for the full-scale ship Regal at the ballast draft and in a clean hull

condition for the bare hull simulations (with rudder only) at the range of speeds given in Table 2. This

set of simulations significantly reduces the complexity of the aft end flow (compared with self-

propulsion tests), allowing to study the nominal wake fields.

Table 2 Bare-hull simulation conditions

Speed (knots)

Re

Fr

8

6.43E+08

0.11

10

8.03E+08

0.14

12

9.64E+08

0.17

14

1.12E+09

0.20

3. Numerical Approach

3.1 Turbulence Modelling Strategy

This work uses the Improved Delayed Detached Eddy Simulation (IDDES) turbulence modelling

strategy and following the approach described in previous work (Pena et al., 2019; Pena et al., 2020).

The IDDES belongs to the DES family, and it is based on the model developed by Shur et al. (2008).

In general, this model switches between the RANS SST k-ω model, which has demonstrated maturity

and reliability calculating skin friction coefficients and steady flow features (Wilcox, 1993; Menter,

1994); and LES in away from the wall, where it can capture the larger unsteady eddies such as the

bilge vortex. This approach ensures that attached regions are modelled by RANS whereas the

immediate region in front of the propeller (which contains the unsteady bilge vortex) is solved by

LES; ensuring that the aftermost region turbulence is better predicted than by using pure RANS.

The IDDES approach is obtained by modifying the dissipation term of the transport equation for the

turbulent kinetic energy (k). After introducing a length scale, L

hybrid

, the turbulence model equations in

tensor form are given as (Shur et al, 2008).:

5

(1)

(2)

where

represents the strain tensor,

the stress tensor,

is the blending function. The length

scale, L

hybrid

is defined as:

(3)

where

,

is given in k-Omega Model Coefficients taken as 0.09.

,

being

, and is the grid length scale. The elevating-function

prevents an excessive

reduction of the RANS Reynolds Stresses (Shur et al., 2008b). The key of this model is the empirical

blending-function,

, which presents a switching function from RANS (

) to LES model (

).

3.2 Numerical Model of the Ship

The ship model was placed in a prismatic fluid domain with the inlet boundary placed one length

upstream of the ship's bow, the outlet boundary two ship lengths downstream of the transom of the

ship and the sides of the fluid domain one ship length towards the port and the starboard sides as

shown in Figure 6 (left). This approach follows the ITTC recommended practices (ITTC, 2014c,

Lloyds Register, 2016). A Dirichlet condition was imposed on the inlet. The DFBI (Dynamic Fluid

Body Interaction) module was used to simulate the motion of the ship in response to pressure and

shear forces exerted by the fluid on the solid body, as well as gravity. The ship model is allowed to

sink and trim freely. The resultant force and moment acting on the ship are calculated, and the

governing equations of rigid body motion are solved every time step to find the new position of the

ship. This approach was selected as it allows for direct comparison of the CFD computation integral

forces with benchmark data from the 2016 Workshop in Ship Hydrodynamics (Lloyds Register,

2016).

The properties of the ship that are defined in the simulation (Table 3) correspond to the values

determined during the sea trials (Lloyds Register, 2016).