Keywords

1 Introduction

Water transport is the most essential transport in many countries of the world. Its ability to undertake large quantities and long-distance carriage makes it a valuable portion of transportation. Inland vessels play an important role and the demand is increasing rapidly. Though the bulk carriers still account for a large proportion of the quantity of inland water transport, container ships are more suitable for intelligent and autonomous shipping since containers are standardized to be preferable for modular transportation. Container ships mostly sail at a relatively high speed in the open sea compared with inland container vessels. Due to the depth and width of the inland waterways, the container vessels have to lower their speeds and the flow fields are becoming fairly complex. At present, there are lots of small container vessels like 36 TEU and 64 TEU, sailing in the Zhejiang inland waterways. A typical 64 TEU inland container vessel (here and after use 64 TEU instead) is shown in Fig. 1 and a novel 64 TEU is designed based on the common 64 TEU ones. The hydrodynamic performance is of great importance at the preliminary stage of ship design. Its prediction can guide the subsequent power selection of the main engine or ship type optimization etc. Hence, how to accurately determine the hydrodynamic forces acted on the ship is meaningful.

Nowadays, Computational Fluid Dynamics (CFD) methods have been developed rapidly. Although model testing is considered to be a very important tool for determining the resistance and power requirements of ship hull forms, CFD can be used efficiently for the same purpose (Ahmed et al. 2009). Compared with Experimental Fluid Dynamics (EFD), CFD can get details of the flow field faster and cheaper. Nonetheless, as for EFD, the credibility of CFD simulations requires the assessment of the modeling and numerical uncertainties to avoid the risk of taking erroneous conclusions (Pereira et al. 2017). For the vessels sailing in inland waterways, the researchers pay more attention to the ship resistance, ship-generated waves, and squat varying with the speed and water depth using the CFD method. Senthil Prakash et al. (2013), Pacuraru et al. (2017), and Ammar et al. (2019) performed simulations to predict the shallow-water resistance of different large block coefficient ships respectively. With the application of commercial code Fluent, Jachowski (2008) validated the CFD method with the results obtained by the existing methods of squat identification and searched the influence of the water depth and ship speed on the squat and wave profile. Raven (2012) focused on the shallow water effects on viscous resistance by simulating double body viscous flow for four different ships. Raven (2019) presented the shallow-water ship model testing and the determination of water depth effect on ship resistance. Mousaviraad et al. (2015) applied Unsteady Reynolds Averaged Navier-Stokes (URANS) method to study the shallow water effect of high-speed planning crafts while Tafuni et al. (2016) put attention on the bottom pressure and wave elevation using the Smoothed Particle Hydrodynamics method. Zeng et al. (2017) used both numerical and experimental methods to investigate the resistance extrapolation of an inland ship model in shallow water. As Zeng et al. (2017) mentioned, there is an unavoidable discrepancy with the ITTC 57 line. Zeng et al. (2018) proposed a numerical friction line for correcting shallow water effects on a ship’s bottom using CFD calculations.

Based on the previous research, this paper aims to predict the ship resistance performance of a newly designed 64 TEU in restricted water. Six water depths and five Froude numbers have been considered in this study and simulations are performed using a Reynolds-Averaged Navier-Stokes (RANS) based CFD model with commercial code STAR-CCM+. The ship resistance and squat performances are analyzed combining with the details of flow fields. Section 1 presents the research background and status. Section 2 shows the details of the ships and tank tests. The applied CFD method is described and verified in Sect. 2.5. Section 3 shows the simulated conditions, results, and discussions from different aspects of resistance, ship motions, wave profiles, pressure, and velocity distributions. The conclusions are drawn in Sect. 4.

Fig. 1.
figure 1

Common 64 TEU container ships sailing in the Zhejiang inland waterways.

Full size image

2 Numerical Method and Verification

2.1 Model of KCS and 64 TEU

The 64 TEU is a newly designed electrically-driven vessel to operate in the waterway from Huzhou to Shanghai in China. It is proposed as green and intelligent inland vessel with multiple advanced technologies, such as a rim-driven thruster propulsion system, containerized batteries, and ship-shore coordination assisted navigation. From the appearance, the 64 TEU has a blunt bow and flat stern with a large block coefficient, which is different from the traditional 64 TEU in Fig. 1.

Fig. 2.
figure 2

Side views of the KCS and 64 TEU model.

Full size image
Table 1. Main particulars of the KCS and 64 TEU at model scale.
Full size table

To ensure the accuracy of the CFD method used in this paper, the KCS model is selected for verification. The KCS is an international standard model which has plentiful test data to be compared and verified with. It is a modern container ship with a bulbous bow and stern which has a more complex flow field than the 64 TEU. The three-dimensional ship geometric models of KCS and 64 TEU are built using Solidworks. The side views of KCS and 64 TEU are illustrated in Fig. 2. Table 1 shows the main particulars of KCS and 64 TEU at the model scale. The KCS is also chosen for its large block coefficient and midship section coefficient which are close to the 64 TEU as a container ship.

2.2 Governing Equations of the Numerical Model

The RANS equations are solved to simulate the flow field around the ship. The continuity and momentum equations in incompressible flow are shown as follows:

$$ \frac{\partial \rho }{{\partial {\text{t}}}} + \frac{{\partial \left( {\rho u_{i} } \right)}}{{\partial x_{i} }} = 0, $$
(1)
$$ \frac{\partial }{{\partial {\text{t}}}}\left( {\rho u_{i} } \right) + \frac{\partial }{{\partial x_{i} }}\left( {\rho u_{j} u_{i} } \right) = - \frac{\partial p}{{\partial x_{i} }} + \frac{{\partial \sigma_{ij} }}{{\partial x_{j} }} + \frac{\partial }{{\partial x_{j} }}\left( { - \rho u_{i}^{^{\prime}} u_{j}^{^{\prime}} } \right), $$
(2)

where the \(u_{i}\) and \(u_{j}\) are the Reynolds average velocity components in \(x_{i}\) and \(x_{j}\) directions, omitting the average sign. The \(u_{i}^{^{\prime}}\) and \(u_{j}^{^{\prime}}\) represent the fluctuating velocities. The \(\rho\), \(p\) and \(\sigma_{ij}\) are fluid density, static pressure, and stress tensor component respectively. Due to the increase of the Reynolds stress term (the last term in Eq. 2, the RANS equation is not closed. So the turbulence model needs to be established. Common turbulence models include \(k - \varepsilon\) and \(k - \varpi\). According to previous research (Querard et al. 2008), the \(k - \varepsilon\) turbulence model can save nearly 25% CPU time compared with the \(k - \varpi\) SST turbulence model for instance. It is also the most widely used turbulence model at present (Tezdogan et al. 2016; Mousaviraad et al. 2015; Castiglione et al. 2014; Jachowski 2008). To better simulate the characteristics of turbulence, the Realizable \(k - \varepsilon\) turbulence model is applied in this paper.

The High-Resolution Interface Capturing (HRIC) scheme is used for Volume Of Fluid (VOF) simulations to maintain sharp interfaces between the participating liquid phases. In the HRIC settings, the lower limit and upper limit of Courant number are set to 500, so that the result can converge quickly and the Kelvin waves can be generated clearly without a smaller time step in the STAR-CCM+ code. The Dynamic Fluid Body Interaction (DFBI) model can solve the equation of a 6-Degree of Freedom (DOF) rigid body motion. In this paper, it is activated to get a stable posture of the ship hull with two degrees of freedom (heave and pitch). Accordingly, ship resistance is calculated.

2.3 Computational Domain and Boundary Condition

Because the studied ships in this paper are geometrically symmetric, only half a ship is researched. The coordinate system of the computational domain is right-handed: the x-axis is oriented against the direction of ship navigation; the y-axis points to the starboard side of the ship; the z-axis is vertical to the sea level upward; the origin is at the point of intersection of aft perpendicular plane, symmetry plane and still water plane. To make the flow field fully developed but save computing resources, the mid-ship section is 1.5 LPP to the inlet plane and 2.5 LPP on the contrary. The side plane is 2 LPP away to ensure the wake is fully developed. The ship is 1 LPP to the upper plane and 2 LPP to the bottom plane for verification. In the following cases for different water depths, except for the distance to the bottom, the rest remains the same.

The initial conditions must be defined depending on the physics of the problem to be solved (Tezdogan et al. 2015). Boundary conditions are settled as Fig. 3. The computational domain is divided into the background mesh region and the overset mesh region. For the background mesh region, the upper plane and the negative x-direction plane are set as velocity inlet. The positive x-direction plane is settled as pressure outlet to prevent backflow. Since only half of the ship is taken for study, the xoz plane is set as symmetry. The ship wall is set as a non-slip stationary wall. So is the bottom plane considering the shallow water effect. The boundary conditions of the overset mesh region are set as overset except the xoz plane which is set as same as the background mesh region.

Fig. 3.
figure 3

Boundary conditions of the computational domain.

Full size image

2.4 Discrete Grid

Commercial code STAR-CCM+ is used to perform the mesh generation, which can automatically generate unstructured hexahedral trimmed meshes with high quality. The KCS model is divided into multiple parts defined with different mesh sizes according to their surface curvature. Three boxes are set surrounding the ship to refine the mesh. The size of the outer box mesh is doubled to the previous box. The mesh near the waterplane needs to be finer to catch the Kelvin waves, which also uses three control boxes of different sizes. The control boxes refine the mesh in different degrees at x, y, z directions. The match between overset and background mesh is also considered.

The boundary layer, which was firstly proposed by Prandtl (1904), has a great influence on the accuracy of the resistance and flow field prediction. In the STAR-CCM+ code, the prism layer mesh is applied to individually define the mesh near the ship. The most important parameter is the thickness near the ship wall, which is described by a non-dimensional number y+. When applying the wall function method, the y+ is generally required to be between 30 to 300. In this paper, the full y+ wall treatment is used, and the y+ is chosen to 80 with 8 prism layers after trials. Also, the bottom plane is set with 4 prism layers for catching the complex flow near the bottom wall at shallow water conditions and a good transition to the upper mesh. Mesh distributions from different views are shown in Fig. 4.

Fig. 4.
figure 4

Mesh distributions from different views.

Full size image

2.5 ITTC Verifications of KCS and 64 TEU

It is desirable in CFD computations to perform an Uncertainty Analysis (UA) to evaluate the accuracy of the results (Castro et al. 2011). The recommended UA procedures (The Specialist Committee on UA 2008) include verification and validation, only the former is researched in this paper. In the uncertainty analysis, the mesh size is the most influential parameter compared to others like time step, iteration number, etc. Series of mesh with three different densities are used to simulate the KCS model at the Fr = 0.1516 condition and 64 TEU at Fr = 0.2032 condition. The base size of the three sets of mesh is diminishing by the scale \(\sqrt 2\).

Firstly, mesh convergence is studied. Then the procedures described in The Specialist Committee on UA (2008) are used for verification. The mesh parameters and results of the KCS and 64 TEU model are listed in Table 2, where the \(R_{G}\), \(P_{G}\), \(C_{G}\), \(U_{G}\), \(\delta_{G}^{*}\) and \(S_{C}\) are convergence factor, order-of-accuracy, correction factor, the uncertainty of mesh, error of mesh, and corrected solution.

Table 2. Mesh convergence study and verification of KCS (Fr = 0.1516) and 64 TEU model (Fr = 0.2032).
Full size table

For the KCS model, as the mesh becomes finer, the calculated resistance is decreasing and gradually going to converge with a small deviation to the EFD data. The \(U_{G}\) and \(\delta_{G}^{*}\) are small and the corrected solution has a deviation within 5% to the EFD data. For the 64 TEU model, the result shows a convergent trend and the \(U_{G}\) and \(\delta_{G}^{*}\) are also small. Hence, it can be considered that the CFD method is verified. The verified method is applied to the other Froude number conditions of the KCS model. Compared with the EFD data, the calculated total resistance coefficient is shown in Fig. 5.

Fig. 5.
figure 5

Comparison of numerical and experimental Ct results of KCS model at different Froude numbers.

Full size image

It is shown that the numerical results are in good agreement with the experimental results in the figure. The maximum deviation is around 4%. And the mesh convergence index shows uncertainties around 4%. Thus, all the results fall within the uncertainty area and all results can be considered validated.

3 Numerical Results

For inland vessels, which commonly navigate in shallow waters, the shallow water effect is a significant part of the research. Based on the previous research (Vantorre 2003), shallow water is usually defined as the water depth draft ratio (h/T) is smaller than 1.5. The waterway from Shanghai to Huzhou is a three-class channel and the minimum depth is 3.2 m. Hence, h/T=1.2 is the shallowest condition for the 64 TEU. However, for the simulation at h/T = 1.5 condition, the ship squats severely, and the overset mesh region exceeds the background mesh region which causes the unexpected stop in the first few seconds of the iteration.

After trials, the simulations are performed at h/T = 2, 2.5, 3, 4, 5, 16 and five Froude numbers within 0.1129 to 0.2032. Two degrees of freedom (heave and pitch) are considered. Details of the studied cases are listed in Table 3. The computed results are analyzed from the aspects of

Table 3. Details of simulated cases.
Full size table

3.1 Ship Resistance

The ship resistance components against the speed and water depth are shown in Fig. 6. For the cases from V = 0.7m/s to V = 0.9m/s, that the Froude numbers vary from 0.1580 to 0.2032, the total and residual resistance increase with the speed at different water depths while the frictional resistance decreases. In some water depths, like h/T = 2, 2.5,4, the total and residual resistance slightly decreases then increases with the speed. Overall, the highest speed condition has the highest total and residual resistance at different water depths.

Fig. 6.
figure 6

Ship resistance coefficients (Ct, Cr, and Cf) change with the speed and water depth.

Full size image

With the water getting shallower, the total, residual, and frictional resistance are gradually rising. These three resistance components are close between h/T = 4 and h/T = 16, which means the water depth has little effect on the resistance in this range. However, while h/T=4 shows higher residual resistance, h/T = 16 shows higher frictional resistance. There are significant resistance increases at h/T = 2.5 and h/T = 3. Then the rise becomes small from h/T = 2.5 to h/T = 2. The resistance components at V=0.5m/s and V=0.6m/s have different or even opposite laws of change in restricted water conditions like h/T = 2, 2.5, 3. It seems that at these two speeds, the total, residual, and frictional resistance firstly increase with a decrease of the water depth. There is a sudden change at the h/T = 3 condition. Then, the resistance components decrease when the water gets shallower.

The trends of the residual and total resistance are nearly parallel, which can be observed in Fig. 7. This figure compares the ship resistance components at h/T = 2 condition. From this figure, the frictional resistance keeps at the same level at different speeds. It is shown that the change of velocity has little effect on the frictional resistance at the shallowest water depth. The lines of residual and total resistance are almost parallel which means that the residual resistance dominates the change of total resistance.

Fig. 7.
figure 7

Comparison of ship resistance components at h/T = 2 condition.

Full size image

This special phenomenon may be caused by the design of the ship hull. Different from the common 64 TEU in Fig. 1, this ship has a blunt bow and the transition between bow and bottom is not smooth enough. The particularity of the ship hull may lead to this phenomenon of resistance performance at low speeds. According to the bottom view of Reynolds number distributions in Fig. 8, most regions of the ship bottom at V = 0.5m/s and V = 0.6m/s have Reynolds numbers that are smaller than 106. The turbulent flow near the bottom of the ship is not yet fully developed. Hence, the turbulence model may not be suitable to perform the simulations under these conditions.

Fig. 8.
figure 8

The bottom view of Reynolds number distributions near the ship hull at h/T = 2 condition.

Full size image

3.2 Ship Squat

When a ship proceeds the water, it generally drops vertically and trims forward or aft. The overall decrease in the static under keel clearance, forward or aft, is called ship squat Derrett 2006). The ship squat is a common phenomenon that can be severe when navigating in restricted waters and cause safety issues. So the study of squat has great significance. Figure 9 shows the ship pitching and heaving against the speed and water depth. The positive angle represents the ship trimming by stern and the negative value of sinkage represents the ship moving downwards. The sinkage is non-dimensionalized by dividing the water depth

Fig. 9.
figure 9

Ship trim and sinkage change with the speed and water depth.

Full size image

In the relatively deep water conditions, the ship trims by the stern and gradually becomes trimmed by the ship bow. At the medium-deep condition like h/T = 3, the ship trims by the stern at all considered speeds but the angle is getting smaller. When the water gets shallower, the ship keeps trimming by the stern, and the angle changes in a small range. The mechanism is that, at the most restricted condition, the water is accelerated at the ship’s bottom. The flat bottom under the ship’s bow makes it have a larger high-speed region than that at the stern. The uneven velocity distribution leads to a bigger sinkage at the bow than at the stern. Hence, the ship keeps trimming by the ship bow at the shallowest condition. The non-dimension sinkage refers to the movement of the center of gravity relative to water depth. According to the previous study (Linde et al. 2016), the sinkage is more significant when the water depth is restricted. As expected, its absolute value increases with an increase in speed and a decrease in water depth.

3.3 Wave Profiles

The free-surface cuts at y/LPP = 0.1 are shown in Fig. 10. The x-coordinate is 0 which represents the middle of the ship, with the positive x-axis pointing towards the ship bow. At relatively low speeds, the section wave profiles are close to each other at different water depths in Fig. 10(a) and Fig. 10(b). The effect of limited water depth becomes more obvious and the wave amplitude becomes larger with the speed. It can be observed that the h/T = 2 condition has the highest bow and stern wave crest among all the water depth conditions in Fig. 10(c). Also, the wave near the ship side is higher than other water depth conditions. But with the speed increasing, the bow wave crests of the h/T = 2.5 and h/T = 3 are also increasing and gradually become close to the h/T = 2 condition in Fig. 10(e).

Fig. 10.
figure 10

Free-surface cuts computed at y/LPP = 0.1.

Full size image

4 Conclusions

This paper focuses on the resistance and flow field of a newly designed 64 TEU sailing in restricted waters at the model scale. The CFD method is verified according to ITTC recommended procedures with the KCS and 64 TEU model. After that, it is applied to different speeds and water depths of the 64 TEU model. Conclusions are drawn as follows.

  1. 1.

    The ship’s total resistance at higher speeds increases with an increase in speed and a decrease in water depth as expected.

  2. 2.

    At lower speeds, the resistance performance is unusual at restricted water conditions. There is a sudden change at h/T = 3 condition. With the water getting shallower, the total resistance decreases, which is different from that at high speeds. This phenomenon may be caused by the blunt ship bow and the low Reynolds number near the hull at the model scale. The mechanism of this phenomenon needs further study.

  3. 3.

    The ship squat is not severe at h/T = 2 condition at all considered speeds, which guarantees safety at shallow water conditions.

  4. 4.

    As the water depth decreases, the wave amplitude becomes larger and the wave crests near the ship bow and stern also increase, while the troughs change slightly at different water depths.