# Exploring the effects of speed and scale on a ship's form factor using CFD

Set up and background

Table of Contents

Determination of the case study I. Hullform II. Speeds III. Scale factors Introduction to the CFD approach – double body vs multiphase simulations I. Conceptual and practical differences, limitations II. Pros and cons of each approach 1. Pros 2. Cons III. Domain of applicability Numerical set-up I. Steady vs unsteady simulations II. Grid generation and the use wall functions III. Boundary conditions IV. Turbulence References

## Determination of the case study

### I. Hullform

For this study, the KRISO container ship (KCS) is chosen. The KCS is a good choice for several reasons. Firstly, the ship geometry and operational conditions are freely available to download. There is also a large volume of work carried out on the KCS by researchers. Therefore, it presents a good choice for validation purposes.

Experimental data for the KCS can be found in the following references (to name but a few):

- Shivachev, E., Khorasanchi, M. and Day, A.H., 2017, June. Trim influence on Kriso Container Ship (KCS): an experimental and numerical study. In ASME 2017 36th International Conference on Ocean, Offshore and Arctic Engineering. American Society of Mechanical Engineers Digital Collection. The paper is freely available via the Strathclyde repository.
- Simonsen, C.D., Otzen, J.F., Joncquez, S. and Stern, F., 2013. EFD and CFD for KCS heaving and pitching in regular head waves. Journal of Marine Science and Technology, 18(4), pp.435-459. The paper is freely available via the publisher.
- Kim, W.J., Van, S.H. and Kim, D.H., 2001. Measurement of flows around modern commercial ship models. Experiments in fluids, 31(5), pp.567-578. The paper is freely available via the publisher.

### II. Speeds

It is best to consider the speeds at which the analysis is to be ran via the Froude number

,

where U is the ship speed in m/s, g is the gravitational acceleration, and L is the ship length.

On the other hand, the Reynolds number (, where is the viscosity of the fluid) will be varied via the scale factor . For this study, an arbitrary number of speeds can be chosen, so long as the computational effort and the design speed of the ship are kept in mind (). It is also desirable to define the speeds according to some simple mathematical rule. This can then be used to automatically control the ship speed in the course of the simulation, thus reducing the required time and user intervention. Since a steady-state solver will be used to model the double body simulations, a ramp-up of the velocity is not needed. It is therefore proposed to begin at , and increase by 0.02 until is reached. This can be implemented easily in Star-CCM+.

NB: For model-scale simulations 3,000 iteration is likely more than enough - not necessarily so for full-scale simulations.

Star-CCM+ field functions (Java):

U=${mult}==3000*(${i}) ? 0.02*sqrt((230/75)*9.81)*(${mult}+1) : 0.02*sqrt((230/75)*9.81)*(${mult})

i=floor ($Iteration)

mult=floor(${i}/3000)+1

Note: You may find this under: Tools>Field Functions

### III. Scale factors

- The first reference cited above (Shivachev et al., 2017) examined the KCS in a scale factor of .
- The second reference cited above (Simonsen et al., 2013) examined the KCS in a scale factor of .
- The third reference cited above (Kim et al., 2001) examined the KCS in a scale factor of .

These can be used to form a geosim series.

Ship and fluid properties

## Introduction to the CFD approach – double body vs multiphase simulations

### I. Conceptual and practical differences, limitations

The adopted approach utilises the double body method to simulate the flow around the KCS. Double body simulations are used for several reasons.

For example, if the ship speed is very low, the waves generated by the hull will be proportionally small, thereby making them challenging to capture with CFD due to the increased grid refinements (at least two cells are required per wavelength, and many more if an accurate representation of the wavefield is sought). In such cases, it is reasonable to neglect the water surface and either assume the wave resistance , or estimate by a potential method.

In the early days of ship CFD (1990s, early 2000s), researchers did not have the computational power to simulate the full wave field around a ship. For this reason, the double body approach was routinely used.

The limitations of the double body approach should also be kept in mind. Most importantly, validating the double body approach is difficult from a physical point of view, because the symmetry plane representing the free surface is in the immediate vicinity of the ship and plays an important role in the flow field.

### II. Pros and cons of each approach

#### 1. Pros

- The double body approach: Allows the steady-state simulation of ship flows, improving convergence and reducing computational effort. Also models one transport equation less (volume fraction) than the multiphase approach.
- The multiphase approach: It could be argued that the wavefield is an indispensable part of ship flows. Therefore, performing double body simulations does not accurately represent the physics. A complete picture of the problem can only be obtained via multiphase simulations. Additionally, ship dynamics cannot be modelled under the double body assumption. This makes it impossible to perform studies on trim optimisation, bulbous bow optimisation, and seakeeping to name but a few.

#### 2. Cons

- The double body approach: The inability to model problems in trim optimisation, bulbous bow optimisation, and seakeeping, the neglect of waves. Strictly speaking, the double body approach has yet to be validated for flow properties on the symmetry plane.
- The multiphase approach: The computational effort is frequently too high. For instance, more advanced methods of turbulence simulation (such as Large Eddy Simulation - LES) cannot currently cope with the required cell numbers to accurately model the free surface in non-academic contexts (see Kornev et al., (2019) for an example of double body LES simulations). The turnaround time is high - convergence of results can take a long time, and may be incomplete for several minutes of numerical time in model-scale. This also scales with the dimensions of the ship, making full-scale convergence requirements difficult to satisfy.

### III. Domain of applicability

The double body approach should only be applied where there are good reasons for not using a multiphase approach. For instance, when the ship speed is very low, or when the number of cells are prohibitively high. As this is an exploratory study, we wish to control and reduce the number of phenomena observed in the simulations. For this reason, we will perform multiphase simulations at selected conditions only, instead of at all speeds and scale factors.

## Numerical set-up

### I. Steady vs unsteady simulations

As mentioned earlier, steady simulations offer advantages over unsteady simulations where possible, but they are also associated with limitations. Steady simulations cannot be used to model scale resolving approaches to modelling turbulence.

Ship resistance is treated as a pseudo-steady problem, i.e. in the frame of reference of a steadily moving ship, the flowfield is invariant. However, the modelling of the free surface in CFD, using the Volume of Fluid method, requires the definition of a temporal term to convect the volume fraction equation in the domain. Since this is missing in double body simulations, we can directly define the problem using a steady-state solver. This eliminates the discretisation error incurred by discretising the temporal term of the Navier-Stokes equations. The number of equations to be solved is also reduced (since a volume fraction is not defined), making the iterations faster. Iterative convergence is also typically achieved faster, because the fluid does not require time to develop and stabilise the ship waves. Tends to underpredict turbulent shear stresses in separated layers, lowering turbulence levels.

### II. Grid generation and the use wall functions

When investigating scale effects, the scaling up, or down, of the geometry itself is not a problem. The problem lies in constructing an adequate grid at each scale factor to ensure that all properties of the flow are captured well. This is necessary because if the grid is not adequate for a certain scale factor, the numerical simulation may produce unreliable results. The main challenge is maintaining the grid near the ship's geometry.

Prism layers allow the solver to resolve near wall flow accurately, which is critical in determining not only the forces and heat transfer on walls, but also flow features such as separation. Separation in turn affects integral results such as drag or pressure drop. Accurate prediction of these flow features depends on resolving the velocity and temperature gradients normal to the wall. These gradients are much steeper in the viscous sublayer of a turbulent boundary layer than would be implied by taking gradients from a coarse mesh. Using a prism layer mesh allows you to resolve the viscous sublayer directly if the turbulence model supports it (low y+ ~1). Alternatively, for coarser meshes it allows the code to fit a wall function more accurately (high y+ > 30).

The turbulence modelling approach that is used and the desired fidelity of the physics determine the thickness, number of layers and distribution of the prism layer mesh. Depending on the Reynolds number, a turbulent shear layer requires in excess of 10-20 cells in the cross-stream direction for accurate resolution of the turbulence flow profiles. To resolve the viscous sublayer (that is, low y+ wall treatment), more cells are required. If only the gross flow features (such as a first-order estimate of skin friction) are required, coarser, high y+ wall-function type meshes with just a few prism layers can yield acceptable results.

Prism layers do not only provide near wall mesh density, they also allow high-aspect-ratio cells to be used, thus providing better cross-stream resolution without incurring an excessive stream-wise resolution.

Prism layers also reduce numerical diffusion near the wall. Numerical diffusion is a discretization error that smears discontinuities and steep gradients in a finite volume advection scheme. Numerical diffusion is minimized when the flow is aligned with the mesh. The use of prism layers greatly enhances accuracy as a result.

(Drawn from the Star-CCM+ user manual)

Constructing a near-wall grid: problem definition

At model-scale, there is no problem to set any value of . However, if we geometrically scale the grid with the scale factor the value will change.

, where (m/s)

is the friction velocity, is the shear wall stress, is the distance from the first cell centre to the wall in metres.

, where is the (local) frictional resistance coefficient.

Using the ITTC line in model and full-scale for the highest Reynolds number in each case, we can obtain an estimate of

.

If we want to ensure that our value at the final speed, corresponding to is within a specified range, we can create the grid for the highest speed. Then, all other cases will fall below the targeted value.

If we seek to set the same values for a model and full-scale ship

The boundary layer thickness (δ) grows with the Reynolds number according to:

,

where x is the distance from the leading edge of a plate.

For the given Reynolds numbers (highest values at each scale), we can estimate δ:

The manner in which we can set the dimensions oxf the prism layer can be summarised as follows:

- Determine the height of the first layer over the wall, as shown above.
- Compute the thickness of the boundary layer δ, as shown above.
- Multiply by 150 to determine the surface element length, and set this number as the value defining the tessellation of the ship surface.
- Define a stretching ratio S (recommended values 1.5), with any valid.
- Determine the distribution of n prism layers over a boundary layer thickness δ for a known first layer, . This can be obtained by expressing the distribution of layers as a geometric progression .
- Use to determine the value of n, by using (it may not always be possible to obtain an integer number of prism layers - round up to the nearest integer instead).

### III. Boundary conditions

The boundary conditions are of critical importance. If selected inappropriately, the solution will not resemble the case study sought. To perform double body simulations, a symmetry plane is used in place of the undisturbed water surface. A second symmetry plane is used to model half of the ship, thereby saving computational resource. The side, inlet and bottom boundaries are set as velocity inlets at a sufficient distance from the ship (at least 1 ship length away). The outlet boundary is set as a pressure outlet.

### IV. Turbulence

There are many approaches to modelling turbulence. The most popular of these are two-equation eddy-viscosity models. These introduce two additional equations to close the Navier-Stokes equations. Typically, one equation is used to solve for the turbulent kinetic energy (k), and one for a dissipation rate (ε) or frequency (ω) of turbulent eddies.

The most frequently used eddy-viscosity models in ship hydrodynamics are

- The Shear Stress Transport (SST) model
- The Wilcox model
- The model

One of the most significant contributions to turbulence modelling was presented in 1877 by Boussinesq. His idea is based on the observation that the momentum transfer in a turbulent flow is dominated by the mixing caused by large energetic turbulent eddies. The Boussinesq hypothesis assumes that the turbulent shear stress depends linearly on the mean rate of strain, as in a laminar flow. The proportionality factor is the eddy viscosity. The concept of a turbulent eddy viscosity makes it possible to model the stress tensor as a function of mean flow quantities.

More advanced models account for each component of the Reynolds stress tensor. Reynolds Stress Transport (RST) models, also known as second-moment closure models, directly calculate the components of the Reynolds stress tensor by solving their governing transport equations. The most recent variant of the RST model, implemented in Star-CCM+ is the Quadratic Pressure-Strain model, and its low variant, the Elliptic Blending model. The Quadratic Pressure-Strain model was developed by Speziale et al. (1991).

## References

Kornev, N., Shevchuk, I., Abbas, N., Anschau, P. and Samarbakhsh, S., 2019. Potential and limitations of scale resolved simulations for ship hydrodynamics applications. Ship Technology Research, 66(2), pp.83-96. https://doi.org/10.1080/09377255.2019.1574965

Terziev, M., Tezdogan, T. and Incecik, A., 2020. Application of eddy-viscosity turbulence models to problems in ship hydrodynamics. Ships and Offshore Structures, 15(5), pp.511-534. https://doi.org/10.1080/17445302.2019.1661625; freely available via the Strathclyde repository.

Simonsen, C.D., Otzen, J.F., Joncquez, S. and Stern, F., 2013. EFD and CFD for KCS heaving and pitching in regular head waves. Journal of Marine Science and Technology, 18(4), pp.435-459. The paper is freely available via the publisher.

Kim, W.J., Van, S.H. and Kim, D.H., 2001. Measurement of flows around modern commercial ship models. Experiments in fluids, 31(5), pp.567-578. The paper is freely available via the publisher.

Shivachev, E., Khorasanchi, M. and Day, A.H., 2017, June. Trim influence on Kriso Container Ship (KCS): an experimental and numerical study. In ASME 2017 36th International Conference on Ocean, Offshore and Arctic Engineering. American Society of Mechanical Engineers Digital Collection. The paper is freely available via the Strathclyde repository.

Speziale, C.G., Sarkar, S. and Gatski, T.B., 1991. Modelling the pressure–strain correlation of turbulence: an invariant dynamical systems approach. Journal of fluid mechanics, 227, pp.245-272. Freely available as a NASA report.