The suitability of computational fluid dynamics (CFD) for marine renewable energy research and development and in particular for simulating extreme wave interaction with a wave energy converter (WEC) is considered. Fully nonlinear time domain CFD is often considered to be an expensive and computationally intensive option for marine hydrodynamics and frequency-based methods are traditionally preferred by the industry. However, CFD models capture more of the physics of wave-structure interaction, and whereas traditional frequency domain approaches are restricted to linear motions, fully nonlinear CFD can simulate wave breaking and overtopping. Furthermore, with continuing advances in computing power and speed and the development of new algorithms for CFD, it is becoming a more popular option for design applications in the marine environment. In this work, different CFD approaches of increasing novelty are assessed: two commercial CFD packages incorporating recent advances in high resolution free surface flow simulation; a finite volume based Euler equation model with a shock capturing technique for the free surface; and meshless Smoothed Particle Hydrodynamics (SPH) method. These different approaches to fully nonlinear time domain simulation of free surface flow and wave structure interaction are applied to test cases of increasing complexity and the results compared with experimental data. Results are presented for regular wave interaction with a fixed horizontal cylinder, wave generation by a cone in driven vertical motion at the free surface and extreme wave interaction with a bobbing float (The Manchester Bobber WEC). The numerical results generally show good agreement with the physical experiments and simulate the wave-structure interaction and wave loading satisfactorily. The grid-based methods are shown to be generally less able than the meshless SPH to capture jet formation at the face of the cone, the resolution of the jet being grid dependent.
In the design of floating offshore WEC structures, many of the same engineering issues arise as for floating offshore structures used in the oil and gas industry. There are some similarities between the design challenges in the two industries and some of the techniques and tools developed within the oil and gas sector can be applied to wave energy. However, there are also significant differences. WECs are usually designed to have moving parts that react to wave motion; WECs are generally much smaller than offshore structures; the water depth is usually shallower and WECs are generally expected to be deployed in arrays, so the design is not a “one off”. The structural design of offshore floating wave energy converters (WECs) generally involves three main and interacting parts of the device: the floating absorber, the mooring arrangement and the power-take-off (PTO) with its associated control system.
Unlike large offshore structures in which motions and forces are minimised, WECs are designed to perform large motions in small and intermediate seas for efficient power conversion, but to survive extreme waves in the event of a storm. These design parameters require mooring arrangements that hold the device in place but do not restrict the motion of the WEC in its energy capturing mode. The dynamics of the moorings, including the motion of the cables, risers, weights and floats, may be highly non-linear in terms of hydrodynamic and structural interaction, and this can affect the response of the device negatively (or positively). The PTO system, however, directly affects the dynamics of the WEC as it converts energy.
In the engineering design of WECs, the three areas of device hydrodynamics, mooring and PTO/control strategy can affect each other considerably and therefore should be considered together. The hydrodynamics can be described using the equations of motion to represent, for example, a single-body heaving device as a mass-spring-damper system, in which the mooring forces are included in the system stiffness and the PTO forces as external forces. Added mass and damping are shape and frequency dependent and can be evaluated using standard naval architecture techniques by physical tank tests, or by numerical methods, which solve the initial boundary value problem for radiation and diffraction for a given geometry [
Modelling in the time domain is necessary for WEC control studies and for investigation of nonlinear wave interaction. Cummins [
Here, we focus on the hydrodynamics of the WEC body and its interaction with an extreme wave and investigate a hierarchy of CFD approaches applied to this case. The design of the WEC with regards to its survivability demands a nonlinear description of the hydrodynamics. Here, steep and large waves that can generate significant water impact on the structure need to be modelled. This may involve wave breaking and green water on the deck of the device. Viscous effects may become large and also the body motions may become highly non-linear, as a floating device can become fully submerged or airborne.
As argued above, when investigating the hydrodynamics of extreme wave-structure interaction, linear theory is of uncertain accuracy and fully non-linear numerical methods are required. Mathematically, such problems can be described by the Navier-Stokes equations incorporating a free surface. These include viscous effects and, depending on the discretisation of the equations, surface effects such as wave breaking can be simulated. When viscous effects are judged to be not important and are neglected, the Navier-Stokes equations reduce to the Euler equations. Both sets of equations can be discretised on a two- or three-dimensional mesh and numerical techniques such as the well-known Finite Volume (FV) or Finite Element (FE) formulations can be used to compute the fluid velocities and pressures at every mesh cell or node. Bodies can be modelled as cavities in the mesh and body motion can be simulated by dynamic body fitted meshes. Special attention needs to be taken when modelling the free surface motions, and Lagrangian surface tracking or Eulerian surface capturing may be used. The volume of fluid (VoF) surface capturing method is often used in CFD and involves the introduction of an additional variable, the volume fraction, which is advected with the flow and represents the fraction of water in a given cell. At the free surface, cells are partially filled and the volume fraction lies between 0 and 1. This approach has been used successfully to simulate the motions of a ship in waves, as reported by Hadzic et al. [
In this paper we use three Eulerian based methods, two that solve the Navier-Stokes equations and one the Euler equations on a three dimensional mesh, and Lagrangian SPH methods. All of the techniques are used to simulate fluid structure interaction problems of increasing complexity. First, a fixed horizontal cylinder in regular waves is modelled. The time histories of the vertical forces are compared to physical experiments and potential theory [
The last set of results compares the motions of a freely floating body interacting with extreme large waves and a counterweight, which is connected to the main float by a pulley-rope system. This case shows the capabilities of the three Eulerian CFD methods to simulate a floating body in one and two degrees of freedom in very non-linear waves, but also the interaction with a counterweight. This counterweight is represented by a force acting on the body, which can provide an option to also include non-linear PTO and mooring forces, for example to test controllers or evaluate non-linear hydrodynamic interaction between the main device and its auxiliaries.
Section 2 describes the three CFD approaches used here, namely the Navier-Stokes/Finite Volume, the Euler/ Cartesian-Cut-Cell and SPH solvers. The test cases including the results are described in Section 3 and conclusions are discussed in Section 4.
The Finite Volume solver [
Free surface calculations are performed using the VoF method [
Meshes comprising hexahedral cells are used for the simulations presented here. A typical mesh section can be seen in
shapes occur, as the boundary-fitted mesh structure is effectively cut out of the initially hexahedral mesh.
When mesh motion is included in the simulation, as for the single float in extreme waves described in Section 4, the whole domain is displaced according to the motion of the float. Thus, the connectivity of this mesh is fixed, the cut cells are not recomputed and re-meshing or dynamic meshing is not necessary at each time step. The mesh motion is taken into account by calculating the face velocities required in the discretisation of the governing equations as the difference between the fluid velocity and the face velocity resulting from the mesh motion.
The Control-Volume Finite Element (CV-FE) approach [
As above, the volume fraction field is solved using the VoF formulation [
[
In
Smoothed Particle Hydrodynamics (SPH) is a flexible Lagrangian and meshless technique for CFD simulations that can be used in complex problems. In this method the fluid system is represented by a set of particles which have individual material properties and move according to governing conservation equations [
The major advantage of using SPH is in dealing with large deformations and distorted free-surface problems. There is no mesh construction in SPH, therefore in certain problems, for instance simulation of waves, the SPH method may be easier to develop and use than Eulerian methods. Also, there is no need for special treatment of the free surface in order to simulate highly nonlinear and potentially violent flows, such as breaking waves. Furthermore, the equations used in SPH are quite simple in comparison with other methods. However, the computational cost is one of the disadvantages of SPH; the time step is much smaller than other methods due to using an explicit time integration scheme.
Following the work of [
The SPHysics code [
The repulsive force boundary condition [
force to the repulsive force that they exert on surrounding fluid particles. Based on the technique of Monaghan et al. [
For virtually incompressible flows such as water the divergence free condition for continuity may be directly imposed by the projection method of Chorin [
There is a further difficulty associated with highly accurate ISPH; instability can occur due to particle clustering, e.g. near stagnation points. This may be avoided without loss of accuracy or convergence by particle shifting, equivalent to remeshing. This may be slight shifting across streamlines [
The AMAZON-3D numerical wave tank (NWT) is based on the free surface capturing method for two fluid flows with moving bodies developed by Qian et al. [
The AMAZON-3D code is based on the integral form of the Euler equations for 3D incompressible flow with variable density. The free surface is treated as a contact surface in the density field that is captured automatically during a time-marched calculation without special provision in a manner analogous to shock capturing in compressible flow. A time-accurate artificial compressibility method and high resolution Godunov-type scheme replaces the pressure correction solver used in many current VoF methods. AMAZON-SC can handle break-up and recombination of the free surface as well as air entrainment into the water and, in principle, associated local compressibility effects. The total force is obtained by integration of the pressure field along the body given by
In order to assess the suitability of the four different CFD approaches to simulate WEC survivability design scenarios, they are applied to a series of benchmark test cases of increasing complexity. In each case, data from physical experiments are available and used for comparison. Grid convergence has been studied in comparisons of free surface wave simulations using FV and CV-FE, in which regular waves are simulated by using different meshes of hexahedral, polyhedral and tetrahedral shape with different resolution and is summarized in [
Dixon et al. [
The forces calculated using each of FV, CV-FE, SPH and AMAZON are compared for different wave amplitudes and cylinder axis depths. The properties including the position of the cylinder below still water level, d, the wave steepness, kA, the product of the wave number and water depth, kh and the Keulegan-Carpenter number KC for each case are summarised in
with Fz being the measured vertical force on the cylinder, g, the acceleration due to gravity, ρ, the density of water, D, the cylinder diameter and l, the length of the cylinder.
As in the physical experiments, linear regular waves are generated in the NWT to interact with the structure. For the Eulerian grid-based approaches described in Sections 2.1, 2.2 and 2.4, the wave velocity components u and w and the surface elevation η are described by
and
and are applied to the water component at the upstream end of the 3-dimensional NWT using a velocity inlet boundary condition. The velocities for the air component are set to 0.0 m/s. The top boundary is a pressure outlet, the sides are modelled as symmetry planes and the bottom, the cylinder boundary and the downstream end of the domain are defined as walls. The total number of cells for the FV meshes is approximately 114,599 and the CV-FE meshes contain approximately 695,375 cells. The number of cells on the boundary of the cylinder itself, however, is 250 for the FV solver and 236 for CV-FE. The time step to achieve a converged solution is found to be 0.001 s and 0.005 s for FV and CV-FE respectively. Details of the NWT for each of the codes used are summarised in
1 | 2 | |
---|---|---|
d' | 0 | −0.3 |
A' | 0.5 | 0.2 |
kA | 0.2 | 0.01 |
kh | 1.61 | 1.61 |
NKC | 3.1 | 1.3 |
FV | CV_FE | AMAZON SC | SPH | |
---|---|---|---|---|
Domain dimensions (m) | 12 * 1 * 0.5 | 12 * 1 * 0,5 | 12 * 1.5 * 0.21 | 6 * 1 * 1 |
No. of cells/particles | 114,599 | 79,495 | 458,850 | 7800 |
Time step (s) | 0.001 | 0.005 | 0.00025 | 0.0001 |
Convergence error/criteria | 0.0001 | 0.0001 | 0.0001 | N/A |
No. of cells across wave height | 10 | 10 | 17 | 12 |
Computer architecture used | 2 processors: Dell Optiplex 745, intel Pentium Duo Core 2.4 GHz | 2 processors: Dell Optiplex 745, intel Pentium Duo Core 2.4 GHz | 1 processor of 600 MHz NEC vector computer | 1 processor of 1.2 GHz Linux workstation |
CPU time: simulation time | 16 hours: 12 s | 11 hours: 12 s | 9 days: 12 s | 15 hours: 12 s |
In AMAZON SC, the air part of the left-hand boundary and the top and right boundary are specified as non-reflecting boundary conditions allowing air to leave or enter the domain. ditions allowing air to leave or enter the domain. The cylinder surface is defined as a reflective wall boundary. The remaining sides are slip boundaries. The NWT contains approximately 458,850 cells with a minimum edge length of 0.015 m. A time step of 0.00025s is applied. For the SPH method the calculations are carried out in a 2-dimensional NWT using 7800 particles in the domain. The boundaries at the wave maker, the bottom, the downstream end and the cylinder are treated as walls and waves are generated by moving the upstream wall similar to a piston wave maker.
In Figures 5 and 6 the time-histories of the non-dimensionalised vertical forces, F', over one wave period are shown for all solvers. For the mesh methods, both mesh and time step convergence are achieved for the results presented. The ISPH method is converged regarding the number of particles in the NWT and the time step. Con- vergence studies for the different CFD approaches are reported in the literature [
For case 1, d' = 0.0 and A' = 0.5, the three codes give very good agreement with the experimental data. The CV-FE results follow the experimental data well and the FV also agrees well, although a third peak is evident in the numerical result but not visible in the experiment data. The AMAZON SC result also represents the force characteristic reasonably well, although the second peak is not resolved well and occurs late and reduced in size, however, the second trough is generally well reproduced. The ISPH result gives a slightly noisy signal and the first trough is shallower and offset compared with the experiment, but the general trend is in reasonable agreement with the other data. For case 2, d' = −0.3 and A'= 0.2 the results look even better and each of the mesh-based solutions follows the experimental data well and reproduces the observed characteristics. As before, the ISPH results are noisier than the other techniques and this is would be reduced by increasing particle resolution but with increasing computational cost.
The cylinder is half submerged in case 1 and three quarters submerged in case 2 and the wave amplitude in case 1 is larger than in case 2, such that the wave overtops the cylinder in case 1 but not in case 2. Thus, it is to be expected that the results predicted by the numerical codes for the less challenging case 2 will be better than those for case 1 in which wetting and drying of the cylinder occurs, as seen in Figures 7 and 8.
For the simulation of floating bodies, the eventual aim is to simulate the motion of floating WECs in extreme waves, and thus it is important to be able to calculate the forces on a moving body and the surface elevations around it correctly. For the second test case, a cone shaped body positioned with its vertex at the initially still water surface is chosen, for which physical tank tests are described by Drake et al. [
The motion of the cone is defined by the displacement d(t) from the initial position at t = 0 s following the form of a Gaussian wave packet, which is described by
where
with h = 0 or 1. A denotes the largest excursion from the still water level. N is the number of frequency components and ωn is the appropriate circular frequency. The central circular frequency ω0 [rad/s] is defined by
with m being an integer between 1 and 12. m effectively controls the linearity of the case. The larger m is and thereby the central frequency, the more non-linear the dynamics become. The results presented here are for h = 1, m = 6 and 9 and A = 0.05 m.
For the CV-FE approach the simulations are performed in a three-dimensional domain with a length and width of 2.5 m and a height of 2.0 m. The cone is placed in the centre, as can be seen in
pressure outlet with constant atmospheric pressure. The mesh consists of 820,000 hexahedral cells, where the regions around the water surface and the cone surface are highly refined to achieve cell edges of approximately 0.01 m. The outer regions are relatively coarse to save computational resources and encourage numerical damping, thus avoiding reflections from the walls. The simulations were carried out using a high performance computing, HPC, cluster on 16 CPUs. The time step is 0.0005 s. Details of the CPU run time and computer architecture used by each of the codes for this case are summarised in
For the AMAZON simulations a 2 m × 1.6 m axisymmetric domain is used. The still water level is set to 1.0 m and the initial draught of the cone is 0.148 m. The calculations are performed on a hexahedral grid using an axisymmetric (2D) version of the code with cell sizes of 0.01 × 0.01 m. The time step is 0.00005 s.
The exported vertical forces Fz from the CFD codes are non-dimensionalised using the expression
with ρ being the density of fresh water, g the acceleration due to gravity, r the cone radius at still water level and A the maximum excursion. Also the time is divided by the corresponding period of the central frequency ω0. The
CV_FE | AMAZON SC | SPH | |
---|---|---|---|
Domain dimensions (m) | 2.5 * 2.5 * 2.0 | 2.0 * 1.6 (2D) | 4.0 * 4.0 * 1.0 |
No. of cells/particles | 820,000 (3D) | 32,000 (2D) | 272,000 (3D) |
Time step (s) | 0.00005 | 0.00005 | 0.0001 |
Convergence error/criteria | 0.0001 | 0.0001 | N/A |
Computer architecture used | HPCx cluster on 16 1.5 GHz processors | 1 processor, 2.5 GHz Macbook Pro computer | 1 processor of 1.2 GHz Linux workstation |
CPU time: simulation time | 3.5 days: 6 s | 11 hours: 6 s | 1.5 days to 6 s |
measured relative motion of the water surface is divided though the maximum excursion A = 0.05 m.
For the solution of the relative motion of the free surface at the cone, shown in
The grid convergence index (GCI) has been examined for the AMAZON code and results shown in
are 0.3387, 0.3400 and 0.3475 respectively, from which it can be calculated that the value of GCI32 is approximately 0.9% and GCI21 is 0.16%. For the SPH code, results for the grid convergence study are shown in
Using the CV-FE approach, simulations have been carried out in pairs in order to consider the positive direction cone displacement for a maximum excursion of A = +50 mm and the opposite negative displacement for A = ‒50 mm. To analyse the nonlinearity in the case, the time histories of the relative surface elevations for the paired tests, m = 9, have been subtracted and summed respectively and divided by 2. This enables results to be broken down into linear and higher order components and compared separately. The half-sum is given by
and the half-difference by
where C and T are the solutions for crest focussed and trough focussed cases. When the half-sum is calculated, the odd frequency components cancel out and the even frequency components remain, and the results of this manipulation on the predicted surface elevations for m = 9 are plotted in
Applying the same analysis technique for the vertical forces, results in the plots shown in
where A is the maximum excursion, Tω0 the period corresponding to the central frequency and d is the diameter of the cone at the still water level. KC describes the relationship between the drag forces over the inertia. For lower KC the inertia dominates the force contribution. This can be seen in the results. For case m = 9, with KC = 0.11, the dynamic force component, which is related to the inertia of the cone, is more developed than for case m = 6, with KC = 0.16.
Physical tank testing of the Manchester Bobber device at 70th scale was performed in the wave tank at the University of Manchester. It is 18.5 m long, 5 m wide and tests were carried out in a water depth of 0.5 m. The waves are generated using 8 piston type paddles operated using the Edinburgh Designs “OCEAN” interface. To minimise reflections from the far end wall, a curved surface piercing beach is installed [
Here, tests for a single tethered float are reproduced using two Eulerian approaches; the Euler/Cartesian- Cut-Cell and Navier-Stokes/FV Method. A schematic arrangement of the system can be seen in
For the simulation of the mechanical system in CFD it is necessary to know the relationship between the two accelerated bodies, i.e. the float and the counter weight. The reason for this is that the CFD codes do not model the pulley system and the counter weight directly, and so these are approximated using additional body forces. The free body diagram as seen in
For the left hand side of system, representing the float, the force equilibrium is achieved when
with mf being the mass of the float, the positive upward acceleration of the system, g is gravity, T1 represents the tension force in the cable and Fb is the buoyancy force. For the counterweight on the left hand side, the positive z-direction is downward, denoted z2, and the force equilibrium can be written as
where mc is the mass of the counterweight and T2 the tension force in the cable. When moving the float vertically by a distance of z1 the counterweight covers the same distance, from which follows that
The two unknowns of the system; the acceleration of the float and the tension force T, can then be written as
and
In the computational approach Fb is calculated from the integrated pressures on the float surface and thereby known at any time. The simulations are run using AMAZON and the FV solver with two alternative approaches to representing the effect of the float, pulley and counterweight arrangement. These are identified as case A and B and are defined in
For the numerical simulations NewWave focusing is used to generate the extreme wave [
where Sn(f) is the spectral density, Δf is the frequency step depending on the number of wave components and bandwidth and A is the target linear amplitude of the focussed wave. Thus, the amplitude of every spectral component in the NewWave group scales as the power density within that frequency band in the assumed sea-state. Equivalently, NewWave is simply the scaled auto-correlation function corresponding to a specified frequency spectrum such as the one obtained on the measured surface elevation time history at the location of the float without the float being in place during the physical tank tests.
The waves are generated using a velocity inlet at the left hand boundary of the numerical wave tank (NWT) at x = 0. Here, the surface elevation of the wave group is prescribed using the same techniques as described for the regular waves in Section 3.1 by specifying the vertical location of the water volume fraction of 0.5. The horizontal and vertical velocity components derived from NewWave theory are applied at the inlet boundary, such that t0 and x0 are the chosen focus time and location in the tank, here set to 4.6 s and 3.5 m respectively. N is the number of wave components, here 15. The numerically reproduced wave without the float in place using AMAZON and the FV solver can be seen in
computer architecture used by each of the codes for this case are summarized in
Figures 21 (Case A) and 22 (Case B) show the comparison of predicted and measured vertical translation of the float as it interacts with the extreme wave. The set-up, including details of the mesh and the applied forces as well as an example of the NWT showing the free surface at a point in time as the focused wave approaches the float are shown in
Case A, in which a constant tension force of T = mcg and the mass of float, mf ‒ mc are applied, predicts significant damping of the vertical motion response after the focused wave has passed although the initial motion of the float is predicted well. In case B, the tension force varies with the acceleration of the float calculated within the solution as, with the mass of float, mf. This leads to a much better prediction of the vertical motion in general, and whereas the response is slightly over-predicted as the extreme wave interacts with the float, its response is much better predicted following the extreme event. Thus the solution is much improved when the tension force includes the instantaneous acceleration of the float rather that assuming it is constant as in case A.
In case C, another Bobber shape is tested in the wave tank at Manchester University. In this test, the geometry of the Bobber is a flat-bottomed cylinder of radius 0.074 m with a corner radius of 0.033 m. The vertical sides extend to 0.085 m above the flat base and a conical upper surface with a 30 degree base angle decreases the radius of the geometry to 0.025 m at the upper cylindrical section (see
According to the experimental tests by Stallard et al. [
A | B | C | |
---|---|---|---|
Mass of float | mf − mc | mf | mf − mc |
Vertical Motion | yes | yes | yes |
Horizontal Motion | - | - | yes |
Tension force T | mcg | mc(g − | mc(g − |
Solvers | FV/AMAZON | FV | SPH |
FV | AMAZON SC | SPH | |
---|---|---|---|
No. of cells/particles | 530,000 | 287,550 | 118,000 |
Time step (s) | 0.0005 | 0.00005 | 0.0001 |
Convergence error/criteria | 0.0001 | 0.0001 | N/A |
Computer architecture used | HPCx cluster on 8 processors, 2.5 GHz, 2 GB per node with Infiniband | 1 processor of 600 MHz NEC vector computer | 16 processors of 1.2 GHz Linux workstation |
CPU time: simulation time | 3 days: 8 s | 20 days: 8 s | 1 day: 8 s |
wave amplitude produces the second peak in the device-response profile at t = 4.6 s or t/Tp = 3.2. The results are in agreement in terms of phase and magnitude. However, the SPH result for the coarse simulations seems to be oscillatory because the number of fluid particles interacting with the device is small, whereas for the finer resolution the response is considerably smoother and all the peaks are reproduced by the SPH results. In order to achieve a smoothed profile of device response, the number of fluid particles around the device needs to be considerably greater. Clearly, the SPH results for the system with six degrees of freedom are smoother and in better agreement (
Three non-linear wave-structure interaction cases have been modelled using state-of-the-art CFD techniques that include three mesh-based techniques solving the Euler and Navier-Stokes equations, and one particle method. The cases increase in complexity, starting with a fixed horizontal cylinder in regular waves. The second case involves rigid vertical motion of a cone, which is forced to oscillate and radiate waves at the surface in still water. The last experiment shows the ability of the CFD methods to cope with highly non-linear wave and floating body interaction. Furthermore, in the last test the body not only interacted with waves, which was modelled sufficiently for smaller waves by Hadzic et al. [
The use of CFD for wave-structure interaction is usually only considered for situations in which assumptions such as inviscid and irrotational flow, linear wave theory and small body motion do not apply. In these situations, the detailed information provided through CFD modelling is of interest and must be considered alongside the accuracy of the results given by CFD, the computational costs and the flexibility in setup and problem definition. Generally the accuracy of the results increases with the number of cells/particles in the domain, and it is possible to capture highly non-linear effects like spray at the cost of larger run-times. Here, fluid forces, surface elevations and motions are predicted and compared with experimental data. For a fixed structure, the forces are well resolved by all methods applied and non-linear surface interaction was also captured successfully.
Body motion has been modelled in two ways. First, a cone-shaped body was forced at the free surface to radiate waves. The difficulties of this case for the mesh methods lay in the presentation of the body and its small maximum displacement. For free surface flow, the mesh should normally use hexahedral cells, as stated in Westphalen et al. [
The second case involving rigid body motion is the heave response of a floating body to interaction with an extreme focussed wave. Here, the results for the CFD packages differ. While the Navier-Stokes/FV solver computed the translation of the body with good agreement when the tension force was modelled by the gravitational component only, it overestimates the motion of the float when the tension force also includes the time-varying body acceleration. The problem of overestimation of the motion due to using the unsteady part of the tension force, needs to be resolved, and may well be due to the numerical solutions being limited to heave motion, whereas the experiments clearly show large surge motions as seen in
The extreme wave loading presented in this paper makes use of a NewWave design wave to reduce the run times. In reality, irregular waves excite the body continuously and these long-term irregular waves are needed to model the final device with mooring and PTO. The computational cost for such runs would increase significantly, not only for running the simulations but also for storing the results. The parallel capability of all the CFD packages used for this work makes it possible to reduce the wall clock time significantly, and in some cases symmetry can be employed to achieve further reductions. As the simulations presented here were performed on different platforms, direct comparisons are difficult. To give an example for the Navier-Stokes FV solver: The final simulation of 8 s of the floating body needed 5 days on 8 partitions using a desktop workstation (16 GB RAM, 2.5 GHz). The same simulation on a cluster took 3 days (2.5 GHz, 2 GB per node, Infiniband).
In this paper the use of CFD for wave loading on WECs is considered using four different CFD techniques. From the results presented it can be concluded that CFD is a versatile tool, capable of solving highly complex and non-linear wave-structure interaction problems. Each of the CFD methods considered predicted the wave structure interaction well and in generally good agreement with experimental results. The jet flow developed in the oscillating cone case is challenging for the Eulerian mesh based approaches as the resolution of the jet is limited by the grid size, and SPH is not limited in the same way and is better able to capture the jet.
The authors would like to acknowledge the support of the Engineering and Physical Sciences Research Councilfunded under the project title “Extreme Wave Loading on Offshore Wave Energy Devices using CFD: a Hierarchical Team Approach” (Grant No. EP/D077508).
Furthermore, many thanks go to Dr. Kevin Drake of University College London (UCL) for providing the high quality physical test data used for the cone simulations.
A = Wave amplitude or maximum excursion
A' = Relative amplitude
An = Amplitude of each wave component
B = Body force
c = Volume fraction (the water surface of the c = 0.5) or crest focussed
d = Displacement
d' = Relative axis depth
d(t) = Displacement of motion of the cone
D = Diameter of cylinder
F = Force
F = Flux vector function
F' = Non-dimensionalised force
Fb = Buoyancy force
Fz = Vertical force
G = Acceleration duo to gravity
H = Water level
K = Wave number
kA = Wave steepness
l = Length of cylinder
m = Integer
mc = Mass of the counterweight
mf = Mass of the float
n = Normal vector
N = Number of frequency components
KC = Keulegan-Carpenter number
P = Pressure
R = Radius of cone at still water level
S = Source term
Sb = Body surface
Sn(f) = Spectral density
T = Time
t0 = Focussed time
T = Wave period, Trough focussed or tension force
T1, T2 = Tension force in the cable
U = Velocity vector
u,v,w = Components of u
V = Domain of interest
X = Position vector
x,y,z = Coordinate directions
z1 = Positive upward z distance
z2 = Positive downward z direction
Δωn = Central circular frequency step
Δf = Frequency step
Δx = Particle resolution
ɳ = Surface elevation
ω = Frequency
ω0 = Central circular frequency
ρ = Density
f = General flow property