Development and Verification of 

a Computational Fluid Dynamics 

Model of a Horizontal-Axis Tidal 

Current Turbine 

M.J. Lawson and Y. Li. 

National Renewable Energy Laboratory 

D.C. Sale 

University of Washington 

Presented at the 30th International Conference on Ocean, Offshore, 

and Arctic Engineering 

Rotterdam, The Netherlands 

June 19-24, 2011 

NREL is a national laboratory of the U.S. Department of Energy, Office of Energy 

Efficiency & Renewable Energy, operated by the Alliance for Sustainable Energy, LLC. 

Conference Paper 

NREL/CP-5000-50981 

October 2011 

Contract No. DE-AC36-08GO28308 
 

 

 

 

 

 

 

 

 

 

 

 

NOTICE 

The submitted manuscript has been offered by an employee of the Alliance for Sustainable Energy, LLC 

(Alliance), a contractor of the US Government under Contract No. DE-AC36-08GO28308. Accordingly, the US 

Government and Alliance retain a nonexclusive royalty-free license to publish or reproduce the published form of 

this contribution, or allow others to do so, for US Government purposes. 

This report was prepared as an account of work sponsored by an agency of the United States government. 

Neither the United States government nor any agency thereof, nor any of their employees, makes any warranty, 

express or implied, or assumes any legal liability or responsibility for the accuracy, completeness, or usefulness of 

any information, apparatus, product, or process disclosed, or represents that its use would not infringe privately 

owned rights. Reference herein to any specific commercial product, process, or service by trade name, 

trademark, manufacturer, or otherwise does not necessarily constitute or imply its endorsement, recommendation, 

or favoring by the United States government or any agency thereof. The views and opinions of authors 

expressed herein do not necessarily state or reflect those of the United States government or any agency thereof. 

Available electronically at http://www.osti.gov/bridge 

Available for a processing fee to U.S. Department of Energy 

and its contractors, in paper, from: 

U.S. Department of Energy 

Office of Scientific and Technical Information 

P.O. Box 62 

Oak Ridge, TN 37831-0062 

phone: 865.576.8401 

fax: 865.576.5728 

email: mailto:reports@adonis.osti.gov 

Available for sale to the public, in paper, from: 

U.S. Department of Commerce 

National Technical Information Service 

5285 Port Royal Road 

Springfield, VA 22161 

phone: 800.553.6847 

fax: 703.605.6900 

email: orders@ntis.fedworld.gov 

online ordering: http://www.ntis.gov/help/ordermethods.aspx 

Cover Photos: (left to right) PIX 16416, PIX 17423, PIX 16560, PIX 17613, PIX 17436, PIX 17721 

Printed on paper containing at least 50% wastepaper, including 10% post consumer waste. 
Proceedings of the 30th International Conference on Ocean, Offshore, and Arctic Engineering 

OMAE2011 

June 19-24, 2011, Rotterdam, The Netherlands 

OMAE2011-49863 

DEVELOPMENT AND VERIFICATION OF A COMPUTATIONAL FLUID DYNAMICS 

MODEL OF A HORIZONTAL-AXIS TIDAL CURRENT TURBINE 

Michael J. Lawson ∗ Ye Li Danny C. Sale 

National Renewable Energy Laboratory National Renewable Energy Laboratory University of Washington

National Wind Technology Center National Wind Technology Center Mechanical Engineering Deaprtment

Golden, CO 80401 Golden, CO 80401 Seattle, WA 98195

Email: michael.lawson@nrel.gov Email: ye.li@nrel.gov Email: sale.danny@gmail.com

ABSTRACT 

This paper describes the development of a computational 

fluid dynamics (CFD) methodology to simulate the hydrodynamics of horizontal-axis tidal current turbines (HATTs). First, an 

HATT blade was designed using the blade element momentum 

method in conjunction with a genetic optimization algorithm. 

Several unstructured computational grids were generated using 

this blade geometry and steady CFD simulations were used to 

perform a grid resolution study. Transient simulations were then 

performed to determine the effect of time-dependent flow phenomena and the size of the computational timestep on the numerical solution. Qualitative measures of the CFD solutions were 

independent of the grid resolution. Conversely, quantitative comparisons of the results indicated that the use of coarse computational grids results in an under prediction of the hydrodynamic 

forces on the turbine blade in comparison to the forces predicted 

using more resolved grids. For the turbine operating conditions 

considered in this study, the effect of the computational timestep 

on the CFD solution was found to be minimal, and the results 

from steady and transient simulations were in good agreement. 

Additionally, the CFD results were compared to corresponding 

blade element momentum method calculations and reasonable 

agreement was shown. Nevertheless, we expect that for other 

turbine operating conditions, where the flow over the blade is 

separated, transient simulations will be required. 

∗Address all correspondence to this author. 

INTRODUCTION 

The kinetic energy available within tidal currents is an untapped source of renewable energy. If a cost-effective method 

of capturing this energy can be developed, tidal currents could 

be harnessed to help satisfy the world’s growing energy needs. 

Horizontal-axis tidal current turbines (HATTs) are one promising technology that is being developed for this purpose [1]. 

HATTs operate using the same mechanical principles as 

wind turbines. At their most basic, HATTs convert kinetic energy within a tidal stream into electricity. Several companies 

have developed HATTs with the intent of commercializing the 

technology. Two examples are Marine Current Turbine’s twinrotor SeaGen that is undergoing testing off the coast of Northern 

Ireland, and Verdant Power’s single rotor turbine that has been 

deployed successfully in the East River near New York City. 

The ability to design efficient HATT blades and accurately 

predict their performance is critical for the success of the tidal 

current turbine industry. Traditionally, reduced order numerical 

methods, such as the blade element momentum method and the 

vortex element method, have been used to design and predict 

the performance of wind turbine blades. Batton et al. [2, 3] and 

Baltazar et al. [4,5] recently demonstrated that these methods can 

also be employed to characterize HATT blade performance. In 

both cases, results from the numerical simulations were shown 

to be in good agreement with experimental measurements of an 

HATT made by Bahaj et al. [6, 7]. 

Nevertheless, it is important to note that the blade element 

momentum method and the boundary element method rely on experimental measurements and empirical correlations to achieve 

1 
accurate results. For example, blade element momentum calculations use compiled experimental data to estimate the hydrodynamic forces on the blade, whereas boundary element methods 

typically employ empirical correlation to account for far-field 

wake effects. Unfortunately, neither method inherently models 

the effects of viscosity, which need to be considered to achieve 

the most accurate turbine performance predictions possible. 

Conversely, computational fluid dynamics (CFD) simulations of the Navier-Stokes equations model fluid flows starting 

from first principles, and therefore inherently capture viscous effects. In the last decade, CFD models of wind turbines have been 

used to accurately reproduce experimental results (e.g. [8–12]) 

and have been used extensively to study complex flow phenomena that have not been quantifiable through the use of simplified 

numerical methods. Given the successful use of CFD in the wind 

industry, it is practical to utilize CFD tools to advance HATT 

technology. 

Objective 

The objective of this study is to develop a CFD methodology 

to simulate HATTs and to determine the effects of computational 

grid resolution and computational timestep on the accuracy of 

the simulations. First, we used the blade element momentum 

method in conjunction with a genetic optimization algorithm to 

design an HATT blade. Using this blade geometry, several CFD 

simulations were performed using computational grids with successively finer spatial resolution. Finally, transient simulations 

were performed to determine if temporal effects must be considered to make accurate predictions of HATT performance. CFD 

predictions of turbine rotor torque and blade root flap moment 

were also compared to corresponding blade element momentum 

calculations. It is noted that the CFD model only includes the turbine blade and hub geometries. Other turbine components, such 

as the tower and nacelle, were not considered in this preliminary 

study. 

TURBINE BLADE DESIGN 

Specifications and operating conditions 

In this paper we consider a hypothetical 550 KW turbine intended for deployment in the Northern Admiralty Inlet of Puget 

Sound in Washington State. An acoustic Doppler current profiler 

survey at this site [13] shows the mean water velocity is approximately 1 m/s, although velocities as high as 3 m/s occur during 

the tidal cycle. 

The design and operating specifications for the turbine are 

presented in Tab. 1. The turbine considered in this study had a 

20 m diameter rotor comprised of a 2 m diameter hub and two 9 

m blades. The blade design was optimized for a variable-speed 

variable-pitch (VSVP) turbine with a maximum rotation rate of 

11.5 rpm. A NACA 63(1)-424 airfoil was chosen as the priTABLE 1. TURBINE SPECIFICATIONS. 

mary shape for the turbine blade. A NACA 63-series blade was 

selected because the minimum pressure coefficient is relatively 

large, which makes this airfoil resistant to cavitation. Additionally, the NACA 63-series blades were an attractive choice for the 

current application because they are known to delay stall and are 

less sensitive to leading edge roughness than the NACA 4- and 

5-series airfoils. 

Given that the blade design was intended for a VSVP turbine, we assumed a circular cross-section at the blade root (to 

allow for a blade-pitching mechanism) that transitioned to the 

NACA 63(1)-424 airfoil shape at 20% of the blade span. It may 

be possible to improve the performance of the blade (i.e. increase power generation) by using several different airfoil shapes 

to define the blade geometry. Future studies will be performed to 

explore this possibility. 

Blade optimization 

We used our recently developed numerical tool, Harp Opt 

[14], to conduct the basic turbine blade design. Harp Opt is the 

combination of the blade element moment code WT Perf [15] 

with a genetic algorithm to optimize the blade twist angle and 

chord length distribution along the span. Harp Opt has been 

widely used by industry and academia to study HATTs. 

The optimization objective for the blade design process was 

to maximize power generation over a range of flow speeds from 

0.5 m/s to 3.0 m/s. Within this range of flow speeds, Harp Opt 

determined the rotor’s rotation speed and the blade’s pitch angle. The optimization algorithm bounded the turbine’s maximum 

power output at 550 kW and also avoided cavitation. Specifically, cavitation was avoided by comparing the minimum pressure over the blade to the fluid vapor pressure and avoiding blade 

designs and turbine operating conditions for which cavitation is 

likely. XFOIL was used to predict the NACA 63(1)-424 airfoil’s 

lift, drag, and pressure coefficients used for the blade element 

momentum analysis. 

2 
FIGURE 1. THREE-DIMENSIONAL REPRESENTATION OF THE 

TURBINE BLADE DESIGNED USING Harp Opt. 

Figure 1 presents an image of the blade and Fig. 2 summarizes turbine operating conditions determined by Harp Opt. The 

WT Perf blade element momentum calculations show that the 

angle of attack for the blade was well below the stall angle across 

the entire blade span for all operating conditions. Thus the flow 

over the blade was expected to remain fully attached under normal operating conditions. 

CFD METHODOLOGY 

CFD simulations predict the motion of a fluid within a given 

domain by discretizing the governing Navier-Stokes equations 

and solving the resulting set of algebraic equations. The remainder of this paper describes the development and verification of a 

CFD methodology to quickly and accurately simulate the performance of an HATT. 

Assumptions 

The CFD model assumed that the density of sea water was 

constant and that the flow was free of cavitation (in accordance 

with the Harp Opt design). Additionally, the effects of gravity 

were neglected in the CFD simulations, which affectively rendered the blade neutrally buoyant. Future CFD simulations could 

be easily adapted to include gravitational forces, thus allowing 

the effects of buoyancy and cavitation to be studied. 

Turbulence modeling 

The k-ω SST (shear stress transport) Reynolds-averaged 

Navier-Stokes (RANS) sub-grid scale model [16] was used to 

simulate turbulence in the flow. The k-ω SST model was selected 

because it has been successfully used to simulate turbulent flow 

over airfoils. Additionally, several CFD studies of wind turbines 

(e.g. [8–12, 17, 18]) have successfully used the k-ω SST model 

to make numerical predictions of turbine performance. A few 

of these studies (e.g. [8–12]) have shown good agreement with 

experimental measurements [19]. 

FIGURE 2. TURBINE OPERATING CONDITIONS DETERMINED USING Harp Opt. 

Computational domain and boundary conditions 

We took advantage of the 180 degree periodicity of the twobladed rotor and only simulated one blade and half of the hub. 

Accordingly, the computational domain consisted of a single turbine blade and half of the hub placed in a large half-cylinder with 

a periodic boundary condition applied across the bottom of the 

domain as shown in Fig. 3. The domain was separated into two 

subdomains to facilitate simulating the rotation of the rotor. One 

subdomain contained the grid elements surrounding the rotor and 

those in the wake region (referred to as the rotor domain), while 

the other subdomain contained the cells in the outer region (referred to as the outer domain). 

A uniform, temporally steady velocity profile was assumed 

at the inlet of the computational domain. The authors are not 

aware of any spatiotemporal turbulent intensity measurements in 

a tidal current stream. Thus we made the simplifying assumption 

that the turbulence intensity was 5% and uniform at the inlet of 

the computational domain. A pressure outlet boundary condition 

was applied at the outlet. To reduce flow recirculations on the 

far-field boundaries and to improve the stability of the numerical 

3 
FIGURE 3. THE COMPUTATIONAL DOMAIN WITH GRID REFINEMENT REGIONS SHOWN. 

solution, a slip (or symmetry) boundary condition was applied 

across the curved cylindrical surface of the outer domain. Lastly, 

a no-slip boundary condition was specified on all rotor surfaces. 

Grid generation 

The fidelity of any CFD simulation depends on the type of 

grid utilized (e.g. structured or unstructured) and the grid resolution. Structured hexahedral grids are the most desirable because 

they inherently provide highly accurate numerical solutions. As 

such, they have generally been used in CFD simulations of turbines. The downside of using structured grids is that the grid 

generation process is a manually intensive and time consuming 

task. In contrast, the creation of unstructured grids is a more automated process that can be performed in a fraction of the time. 

However, when using unstructured grids, care must be taken to 

insure the grid quality (e.g. grid element skewness, grid element 

aspect ratio, and grid density) does not adversely impact the accuracy of the numerical solution. 

In the present study, unstructured grids consisting of polyhedral elements having an average of 14 faces per element were 

generated using the STAR CCM+ (CD-Acapco; Melville, New 

York) grid generation utility. The grid resolution was defined by 

specifying the grid size and expansion rate on all the surfaces of 

the computational domain. Additionally, we found it critical to 

use volumetric refinement zones to increase the grid resolution 

around the blade, the rotor, and in the wake region as shown in 

Fig. 3. These refinement zones allowed for the grid resolution 

to be increased in regions where high velocity gradients were 

expected, without adding additional grid elements in regions of 

the computational domain where a coarse grid was acceptable. 

Prism layer grid elements were extruded from the surfaces of the 

blade and the hub to improve the grid quality and control the grid 

TABLE 2. COMPUTATIONAL GRID STATISTICS. 

spacing in this region. The height of the first prism layer was set 

so that the grid elements against the blade surface were within 

the logarithmic region of the boundary layer between y+ = 30 

and y+ = 100, depending on the location of the grid element on 

the blade and on the turbine operating condition simulated. Wall 

functions derived from equilibrium turbulent boundary layer theory were utilized to model turbulent effects below the first grid 

cell. 

Five grids were generated for use in the grid refinement and 

timestep studies. Table 2 summarizes the statistics for each grid 

and Fig. 4 illustrates the grid resolution achieved. Henceforth, 

the grids will be referred to by the grid number given in Tab. 2. 

Numerical methods 

The commercial CFD code STAR CCM+ was used to solve 

the incompressible Navier-Stokes equations using a secondorder-accurate finite-volume discretization scheme via a segregated algebraic multi-grid iterative solver. A second-orderaccurate backward temporal discretization was used for transient 

simulations. 

Steady simulations were judged to be converged when the 

residuals of the numerical solution stabilized and were reduced 

by approximately three orders-of-magnitude. Several global parameters, including rotor torque and thrust, were also monitored 

to ensure convergence of the solution. Unsteady simulations 

were deemed converged when the average rotor torque over a 

revolution was within approximately 1% of the value from the 

previous revolution. Within each timestep, residuals were reduced by three orders-of-magnitude before the solution was advanced in time. 

A rotating reference frame model was used to simulate the 

rotation of the blade and hub. This method simulates rotation 

without the need to physically rotate the computational grid by 

forming the governing equations for the rotor domain in a reference frame that rotates with the turbine, while the outer domain 

remains in a stationary coordinate system. 

All simulations were performed on the 153 node Redrock 

computer cluster at the National Renewable Energy Laboratory. 

Each node is comprised of two 2.93 GHz quad-core Intel Nehalem processor with 12 GB of shared memory. All simulations 

4 
FIGURE 4. COMPARISON OF THE SPATIAL RESOLUTION 

ACHIEVED FOR (a) GRID 1 AND (b) GRID 5. THE RESOLUTION 

OF THE OTHER COMPUTATIONAL GRIDS FALLS BETWEEN 

THESE TWO EXTREMES. 

were performed using 64 cores. Steady simulations required between 64 and 960 cpu-hours, depending on the grid size. Transient simulations were performed using grid 1 and required between 256 and 1500 cpu-hours, depending on the size of the computational timestep. 

RESULTS AND DISCUSSION 

Grid resolution study 

The three turbine operating conditions presented in Tab. 3 

were simulated under a steady flow assumption using each computational grid. The results from these simulations were used to 

study the influence of the grid resolution on the numerical solution. For brevity, graphical representations of the CFD solution 

(i.e. contour plots and iso-surfaces) will only be presented for 

grids 1 and 5, the coarsest and finest resolution grids, respectively. 

Qualitatively, the features of the CFD solutions were found 

to be markedly similar for each grid. To illustrate the qualitative similarities between the solutions, examples of blade presTABLE 3. TURBINE OPERATION CONDITIONS SIMULATED 

WITH STAR CCM+. NOTE THAT THE ROTOR SPEEDS AND THE 

BLADE PITCH ANGLES FOR THE CORRESPONDING FLOW VELOCITIES WERE DETERMINED USING THE HARP OPT DESIGN 

CODE. 

FIGURE 5. BLADE PRESSURE DISTRIBUTION IN PASCALS 

FOR (a) GRID 1 AND (b) GRID 5 FOR OPERATING CONDITION 

C. 

sure distributions and velocity contours for operating condition 

C are presented in Figs. 5 and 6, respectively. Although the 

blade pressure distributions are nearly indistinguishable for the 

different grids, a close examination of the velocity contours reveals that small structures within the wake were better resolved 

using the higher resolution grid. A more diffuse wake region was 

predicted using grid 1 because the coarse grid cells in the wake 

region (see Fig. 4) were insufficient to resolve the shear layer between the turbine’s wake and the free-stream flow. Note that the 

CFD results for operating conditions A and B exhibited similar 

qualitative trends to those shown in Figs. 5 and 6. 

To quantitatively evaluate the effect of grid resolution on the 

numerical solution, the rotor torque and blade root flap moment 

were calculated for each grid. Figures 7 and 8 present these quantities plotted verses grid resolution for operating conditions A, B, 

and C. The relative differences between rotor torque and blade 

root flap moment predicted by grids 1–4 with respect to the value 

predicted using grid 5 are presented in Tab. 4. 

As Fig. 7 illustrates, the CFD rotor torque predictions exhibited monotonic convergence with increasing grid resolution. 

5 
FIGURE 6. VELOCITY CONTOURS IN A PLANE THROUGH 

THE CENTER OF THE COMPUTATIONAL DOMAIN FOR (a) GRID 

1 AND (b) GRID 5 FOR OPERATING CONDITION C. NOTE THAT 

THE FLOW IS FROM LEFT TO RIGHT. 

TABLE 4. THE RELATIVE DIFFERENCE BETWEEN ROTOR 

TORQUE AND BLADE ROOT FLAP MOMENT PREDICTIONS 

MADE USING GRIDS 1-4 AND PREDICTIONS FROM GRID 5. 

Moreover, torque predictions for grids 4 and 5 were within 1% 

of each other for all operating conditions simulated. Thus, based 

on these torque convergence data, it was concluded that further 

increasing the grid resolution would have produce a negligible 

change (almost certainly less than 1%) in the rotor torque predicted by CFD simulations. However, the results showed that 

use of a very coarse grid results in a significant under prediction 

of rotor torque. Indeed, as Tab. 4 shows, grid 1 consistently under 

predicted rotor torque by 11%–12% compared to grid 5. 

To further investigate the cause of the discrepancy in the rotor torque predictions between the different grids, we computed 

the torque contribution from 40 evenly sized blade sections along 

the span. Figure 9 clearly shows that grid 1 significantly under 

predicted the rotor torque with respect to grid 5 on the outboard 

section of the blade, which was where the majority of the rotor 

torque was generated. This suggests that grid 1 had insufficient 

resolution to accurately capture the physical phenomena of the 

water flow over the outboard sections of the blade, where the 

6 

FIGURE 7. THE EFFECT OF GRID RESOLUTION ON ROTOR 

TORQUE PREDICTIONS FOR TURBINE OPERATION CONDITIONS (a) A, (b) B, AND (c) C. 

relative flow velocity was highest. 

One prominent difference between the predicted flow fields 

for grids 1 and 5 was visualized using iso-surfaces of vorticity 

to elucidate the blade tip-vortices. Figure 10 shows that the tipvortices predicted by grid 1 were much larger and enveloped a 

larger portion of the blade than the tip-vortices predicted by grid 

5. Effectively, grid 1 tip-vortices induced more downwash on the 

suction side of the blade, which decreased the torque generation 

near the blade tip as Fig. 9 clearly illustrates. 

Predictions of the blade root flap moment were insensitive to 

the grid resolution (see Fig. 8 and Tab. 4), although the convergence of this quantity was not monotonic. Nevertheless, given 

that the maximum difference in the predicted flap moment between grids 1 and 5 was only 1.2%, this non-monotonic convergence was not of significant concern. One possible reason this 

convergence behavior was observed is that a steady flow assumption may not be appropriate for the highly unsteady far-wake region. More specifically, the near-wake region is characterized 

by a highly organized vortex wake with a structure that is effectively time-independent with respect to the rotating reference 

frame model. In contrast, the far-wake region is inherently unsteady regardless of the reference frame used. 
FIGURE 8. THE EFFECT OF GRID RESOLUTION ON BLADE 

ROOT FLAP MOMENT PREDICTIONS FOR TURBINE OPERATION CONDITIONS (a) A, (b) B, AND (c) C. 

Although a large difference in the predicted rotor torque 

(11–12%) was seen between grids 1 and 5, a less pronounced difference (approximately 3%) was observed between grids 3 and 5. 

Thus, if the purpose of CFD simulations is to accurately predict 

global turbine performance characteristics (e.g. rotor torque, flap 

moment, and hydrodynamic forces) a grid with a resolution similar to grid 3 appears sufficient. However, if fine details in the 

flow (e.g. the structure of tip vortices and details of the blade 

boundary layer and wake) must be resolved, a finer grid is required. 

Timestep study 

Transient simulations were performed for two reasons: (1) 

to determine if time-accurate CFD simulations provide significantly different results from corresponding steady simulations; 

and (2) to evaluate the effect of the computational timestep on the 

numerical solution. Grid 1 was used for all transient simulations 

to reduce the computational resources required to perform the 

timestep study. It is generally acceptable to use separate grid and 

timestep convergence studies to determine the effect of spatial 

and temporal resolution on CFD solutions [20]. Thus we expect 

the results from the timestep study using grid 1 to be applicable 

7 

FIGURE 9. SECTIONAL TORQUE CONTRIBUTIONS FOR 

GRIDS 1, 3, AND 5. 

to transient simulations performed using the more resolved grids. 

The transient simulations were performed using timesteps of 

0.05, 0.01, and 0.005 seconds for operating condition C. These 

timesteps correspond 260, 521, and 1044 timesteps per rotor revolution, respectively. To reduce the required time for transient 

simulations to reach a quasi-steady state, the simulations were 

initialized using the steady flow solution. For all transient simulations, the torque stabilized within approximately three simulated rotor revolutions. Significant oscillations in the rotor torque 

were not observed and were not expected as the angle of attack 

of the blade over the entire span was well below the stall angle. 

Visualization of limiting streamlines on the blade confirmed the 

flow was fully attached. 

The size of the computational timestep was found to have 

very little effect on the magnitude of torque generated by the turbine as Tab. 5 shows. Further, the difference between the torque 

predicted by the steady and unsteady simulations was within 

2.5%. This suggests that for attached flow conditions, steady 

CFD simulations sufficiently captured the physical phenomena 

that determine the magnitude of hydrodynamic loading on the 

blade. This conclusion must, however, be considered carefully 

given the set of assumptions used for the present simulations. It 

was assumed the inflow conditions were spatiotemporally uniform. If a time-varying nonuniform velocity profile containing 

realistic turbulent structures is used, time-accurate simulations 

are required. 
FIGURE 10. VISUALIZATION OF BLADE TIP-VORTICES FOR 

(a) GRID 1 AND (b) GRID 5. NOTE THAT THE SAME VORTEX 

THRESHOLD IS USED IN BOTH IMAGES. 

TABLE 5. RESULTS FROM THE TIMESTEP STUDY. FOR COMPARISON, THE CORRESPONDING RESULT FROM THE STEADY 

SIMULATIONS IS ALSO SHOWN. NOTE THAT ALL RESULTS 

ARE FOR GRID 1. 

Comparison of the CFD results with blade element momentum method predictions 

The rotor torque and blade root flap moment predictions 

from steady CFD simulations performed using grid 5 were compared with the corresponding blade element momentum predictions from WT Perf. Figure 11 presents this comparison. It is 

clear that the blade element momentum method significantly underestimated the hydrodynamic forces on the blade compared to 

the CFD solution. Indeed, plotting the sectional torque contributions to the total rotor torque (Fig. 12) revealed that the hydrodyFIGURE 11. COMPARISON OF ROTOR TORQUE AND BLADE 

ROOT FLAP MOMENT PREDICTIONS FROM STAR CCM+ (USING GRID 5) AND WT Perf FOR OPERATING CONDITION C. 

namic forces were under predicted across the entire blade span 

by WT Perf in comparison to the CFD solution. Unfortunately, 

there is no experimental data available for the current blade design, making it impossible to assess the accuracy of either numerical method. Nevertheless, the reasonable agreement between 

the CFD results and the blade element momentum method calculations provides confidence in the results obtained with both 

numerical methods. 

CONCLUSIONS AND FUTURE WORK 

A RANS CFD methodology to simulate HATTs was developed and the numerical results were verified via a grid refinement 

study and a timestep study. Steady simulations were performed 

using successively more resolved computational grids to determine the effect of grid resolution on CFD predictions. Qualitatively, the CFD solutions calculated using the different grids 

were markedly similar. However, the use of a coarse computational grid resulted in a significant under prediction of rotor 

torque compared to results obtained with higher resolution grids. 

Transient simulations were performed using successively 

smaller computational timesteps to determine if temporal effects 

8 
FIGURE 12. CONTRIBUTIONS TO ROTOR TORQUE PREDICTED USING CFD AND WT Perf FOR OPERATING CONDITION C. 

must be considered to make accurate predictions of turbine performance. For the turbine operating conditions considered, the 

computational timestep was shown to have little effect on the numerical solution. Additionally, the results from steady and transient simulation were shown to be in general agreement. 

It is important to note that the flow over the turbine blade was 

fully attached for all the operating conditions simulated herein. 

The consideration of more extreme operating conditions, where 

the flow over the blades is separated and inherently unsteady, will 

likely require the use of transient CFD simulations to achieve 

accurate numerical results. Moreover, when the flow over the 

blades is separated, predictions of transition, separation, and flow 

reattachment have a significant influence on the accuracy of CFD 

solutions [8]. Thus, in these cases, advanced RANS models capable of predicting these complex physical phenomena may be 

required. 

This work represents the first step in the development of a 

CFD methodology to characterize HATT performance. We plan 

to further develop this model by considering realistic inlet velocity profiles and turbulence levels. Additionally, we hope to 

include structural elements of the turbine, such as the tower and 

the nacelle, in future simulations. 

REFERENCES 

[1] Fraenkel, P., 2002.	 “Power from marine currents”. Proceedings of the Institution of Mechanical Engineers, Part 

A: Journal of Power and Energy, 216(1), pp. 1–14. 

[2] Batten, W. M. J., Bahaj, A. S., Molland, A. F., and Chaplin, J. R., 2008. “The prediction of the hydrodynamic performance of marine current turbines”. Renewable Energy, 

33(5), pp. 1085–1096. 

[3] Batten, W. M. J., Bahaj, A. S., Molland, A. F., Chaplin, 

J. R., and Sustainable Energy Res, G., 2007. “Experimentally validated numerical method for the hydrodynamic design of horizontal axis tidal turbines”. Ocean Engineering, 

34(7), pp. 1013–1020. 

[4] Baltazar, J., and de Campos, J., 2008.	 “Hydrodynamic 

Analysis of Horizontal Axis Marine Current Turbine with 

a Boundary Element Method”. Proceedings of the 27th International Conference on Offshore Mechanics and Arctic 

Engineering. 

[5] Baltazar,	 J., and de Campos, J. A. C. F., 2009. “Unsteady analysis of a horizontal axis marine current turbine 

in yawed inflow conditions with a panel method”. First International Symposium on Marine Propulsors. 

[6] Bahaj, A., Batten, W., and McCann, G., 2007.	 “Experimental verifications of numerical predictions for the hydrodynamic performance of horizontal axis marine current 

turbines”. Renewable Energy, 32(15), pp. 2479–2490. 

[7] Bahaj, A., Molland, A., Chaplin, J., and Batten, W., 2007. 

“Power and thrust measurements of marine current turbines 

under various hydrodynamic flow conditions in a cavitation tunnel and a towing tank”. Renewable Energy, 32(3), 

pp. 407–426. 

[8] Pape, A., and Lecanu, J., 2004. “3D Navier–Stokes computations of a stall-regulated wind turbine”. Wind Energy, 

7(4), pp. 309–324. 

[9] Sorensen,	 N., Michelsen, J., and Schreck, S., 2002. 

“Navier-stokes predictions of the NREL phase vi rotor in 

the NASA Ames 80 ft by 120 ft wind tunnel”. Wind Energy, 5(2-3), pp. 151–169. 

[10] Johansen, J., Sorensen, N., Michelsen, J., and Schreck, S., 

2002. “Detached-eddy simulation of flow around the NREL 

Phase VI blade”. Wind Energy, 5(2-3), pp. 185–197. 

[11] Duque, E., Burklund, M., and Johnson, W., 2003. “NavierStokes and comprehensive analysis performance predictions of the NREL phase VI experiment”. Journal of Solar 

Energy Engineering, 125, p. 457. 

[12] Tongchitpakdee, C., Benjanirat, S., and Sankar, L., 2005. 

“Numerical simulation of the aerodynamics of horizontal 

axis wind turbines under yawed flow conditions”. Journal 

of solar energy engineering, 127, p. 464. 

[13] Polagye, B., and Thomson, J., 2010. Tidal Energy Reference Model Inflow Conditions. Tech. Rep. Unpublished, 

University of Washington. 

[14] Sale, D. C., and Li, Y., 2010.	 “Preliminary results from 

a design methodology and optimization code for horizontal axis wind and hydrokinetic turbines.”. The 29th Inter9 
national Conference on Ocean, Offshore And Arctic Engineering. 

[15] http://wind.nrel.gov/designcodes/simulators/wtperf/. 

NWTC Design Codes - WT Perf, Accessed January 15, 

2011. 

[16] Menter, F., 1994. “Two-equation eddy-viscosity turbulence 

models for engineering applications”. AIAA journal, 32(8), 

pp. 1598–1605. 

[17] Laursen, J., Enevoldsen, P., and Hjort, S., 2007. “3D CFD 

quantification of the performance of a multi-megawatt wind 

turbine”. In Journal of Physics: Conference Series, Vol. 75, 

IOP Publishing, p. 012007. 

[18] Johansen, J., Madsen, H., Gaunaa, M., Bak, C.,	 and 

Sørensen, N., 2009. “Design of a wind turbine rotor for 

maximum aerodynamic efficiency”. Wind Energy, 12(3), 

pp. 261–273. 

[19] Simms, D., 2001.	 NREL unsteady aerodynamics experiment in the NASA-Ames wind tunnel: a comparison of 

predictions to measurements. Tech. Rep. NREL/TP-500­

29494, NREL. 

[20] Roache, P. J., 1998. Verification and Validation in Computational Science and Engineering. Hermosa, Albuquerque, 

NM. 

10