Cape Horn Engineering have recently participated in The Tidal Turbine Benchmarking Project, conducted and funded by the UK’s EPSRC1 and Supergen ORE Hub2.
The main objective of this benchmark study is to mitigate climate change by accelerating the development of tidal technolo- gies and harnessing the untapped potential of Offshore Renewable Energy. To achieve this goal, the benchmark study aims to reduce conservatism in the design of tidal turbines by addressing the modelling uncertainty and by validating engineering methods with good-quality experimental data.
The project was an excellent opportunity for Cape Horn Engineering to participate in a blind validation study to demonstrate our specialist technologies and capabilities to assist companies in exploring less carbon-intensive and more sustainable energy systems. We have proudly self-financed this research ourselves, as an internal project.
Our high-fidelity simulations are based on 20 years of experience in developing CFD technology solutions for the maritime industry, especially ship propulsion simulations with rotating propellers. The spirit of the benchmark study was a collective exploration aimed at strenghtening confidence in the accuracy of modern numerical modelling. With our engineering expertise, gained from participating in elite yacht racing for decades, and our passion to succeed, we set ourselves the goal to perform our very best, and to achieve outstanding results.
The experimental benchmarking data was produced from a large 1.6m diameter tidal rotor, the biggest that could be used in a towing tank, which was fitted with numerous sensors for data collection. The rotor was towed through the large towing tank at the QinetiQ’s Haslar facility in the UK in well-defined steady flow conditions, with and without an upstream turbulence grid to produce two sets of data for low and elevated turbulence conditions. Full details can be found in the research paper produced3.
The modelling was performed by 12 groups across academia and industry. Among those submitting their blind validation results were prestigious universities from the UK, Brazil, and France, as well as companies from the UK, Italy, Portugal and the USA. The models used by the different groups spanned different fidelity levels, from Blade Element Momentum methods to Blade Resolved Computational Fluid Dynamics (high-fidelity RANS-based CFD) of the kind used by Cape Horn Engineering. The CFD solver we used was STAR-CCM+ by Siemens Digital Industries Software, which is our preferred choice as we feel it is the best-suited software package for these types of applications4.
Our simulation philosophy aimed to replicate the experimental setup as closely as possible, and for it to be applicable to conditions without waves, as presented here, and conditions with incoming waves which will be the focus of a follow up benchmark project. In line with this philosophy, very few simplifications were made; we modelled the complete geometry including all three blades, the nacelle and tower, as well as the tank walls and floor so that blockage effects, if present, were considered. We also simulated the rotor physically rotating within the domain, and the deformation of the water surface around the surface-piercing tower and above the rotating blades, even if the waves generated by the rotor tips were very small.
The unsteady, turbulent flow was modelled with the industry common K-omega SST Turbulence model resolving the boundary layer up to the wall (with Y+ values lower than 1). The deformation of the free surface was modelled with the Volume of Fluid (VOF) and an Automatic Mesh Refinement (AMR) was used at the free surface.
To model the motion, the space around the turbine was divided into two regions: one for the full computational domain and a smaller, embedded one for the rotor. A cylindrical interface connects both regions. We used different mesh topologies in each region to gain the advantages of the respective mesh types. In the background region a trimmed mesh was used as it is well suited for free surface flows, whereas the rotor region used a polyhedral mesh. The polyhedral mesh allowed for the use of advanced features which cluster cells at the leading and trailing edges of the blades and results in a reduction in cell count and a gain in geometrical accuracy that would be prohibitively expensive otherwise, see images below.
To advance the unsteady simulations, the time step selected was based on the rotor speed such that it rotated one degree per time step. All wall surfaces were considered to be hydraulically smooth as there was no roughness specified from the experimental data. A turbulent source option was present in the domain, which was used to counteract the turbulence decay and thus allowed the propagation of the 3% turbulence from the inlet in the elevated turbulence cases. The results of the simulations showed temporal convergence and were averaged over the last 200 time steps.
It is important to note that the use of a relatively coarse mesh resolution of around 3.5 million cells (due to the effective mesh distribution) and an efficient way to ramp up the time step for faster convergence resulted in highly efficient simulation times. This were around 4 to 5 hours on a compute node with 32 cores (Intel Xeon Gold E5-6142 v5 CPU from 2017) which makes these type of analysis suitable for industrial applications. Compared to most submissions from other groups which had more of an academic character, our simulations were an order of magnitude more efficient, and were also one of the most accurate. Furthermore, other groups using blade resolved CFD methods similar to ours, made simplifications to the geometry or physics, by not including the tank wall or the tower, or by using a steady solver with moving reference frame instead of rotating blades, or by not including the free surface.
At the time of submission we presented a verification and validation (V+V) analysis to add confidence and confirm our results. Very low levels of numerical uncertainty of less than 1% were found for both key parameters, the coefficients of power and thrust. The V+V analysis was competed by performing triplet studies on the spatial (mesh) and temporal (timestep) discretisation using a refinement ratio of 2 to coarsen the simulation.
The non-dimensional values used to compare results between the experiments and the simulations are the coefficients of power and thrust. Most submissions contained at least five conditions for the low level, and some included elevated turbulence levels. The turbine was towed at a constant speed and the rotational speed was varied resulting in different cases or tip-speed-ratios (TSR). The power and thrust curves are presented below shown as coefficients, as a function of TSR. These comparisons correspond to what the organisers called the first level (L1) values, or the fully blind initial submissions. Participants had a chance to correct their submissions after the experimental data was released. The first correction (L2) allowed to correct for user-type input errors and the second correction (L3) to fine tune the models to improve the accuracy and correlation to the experimental data.
In Figure 1 below, our results are shown with red lines and the experimental data with blue lines. All other scatter points are submissions from other groups who used blade resolved CFD modelling. Below our graphs in Figure 2 (taken from the paper) the results from all participants in the project are shown, including the lower fidelity models. The lower fidelity models include a number of assumption, and this trade-off brings faster simulation speed but at the expense of accuracy, as shown the higher variability.
Figure 1: Blade Resolved Results – Low Turbulence
Figure 2: All Results – Low Turbulence
The graphs show how we achieved one of the best correlations with experiments. To quantify this, we calculated an average error from the difference between the curves. The low turbulence Cp comparison has an average difference of 0.67%, with the Ct showing an average difference 2.10%. For the elevated turbulence cases, we saw a comparison difference of 2.02% and 2.74% for Cp and Ct respectively. The maximum difference is 2.3% for Cp at low power end, and 4.6% for Ct for the highest load case. (3.9% and 5.6% for the elevated turbulence). It is noteworthy that with the graphs shown in Figure 2, the paper states ”Experimental data are shown with a 95% confidence level”3, thus our averages are within this tolerance.
According to the paper presented by the organisers of the benchmark to the European Wave and Tidal Energy Conference 20233, ”The solutions of CHE-BR-uRANS were found to be very effective with a significantly lower cell count compared to other methods, whilst returning some of the most accurate solutions”.