Conference PaperPDF Available

Blade-resolved CFD analysis and validation of blockage correction methods for tidal turbines

Authors:

Abstract and Figures

Blockage, the ratio between a turbine's swept area and the channel cross-sectional area, affects the torque and thrust characteristics of the rotor. These effects are relevant for many reasons, including the calculation of mechanical, structural and mooring systems, energy production assessment, etc. The present work describes the analysis and validation of six different blockage correction methods for tidal turbines, described in literature, with blade-resolved RANS-CFD simulations. The simulations were performed to seven different blockage rations and 5 tip speed ratios for each blockage case. The blocked results were corrected with the different methods and compared to the quasi open-flow results as a measure of the effectiveness of each one of them, showing a relatively good agreement for 4 out of 6 methods. Finally, this paper provides practical recommendations regarding the application of the different correction methods, including an assessment of the required variables and their scope of application.
Content may be subject to copyright.
137
Advances in Renewable Energies Offshore – Guedes Soares (Ed.)
© 2019 Taylor & Francis Group, London, ISBN 978-1-138-58535-5
Blade-resolved CFD analysis and validation of blockage correction
methods for tidal turbines
G. Tampier Brockhaus
Faculty of Engineering Sciences, Universidad Austral de Chile, Valdivia, Chile
F. Zilic de Arcos
Department of Engineering Science, University of Oxford, Oxford, UK
ABSTRACT: Blockage, the ratio between a turbine’s swept area and the channel cross-sectional area,
affects the torque and thrust characteristics of the rotor. These effects are relevant for many reasons,
including the calculation of mechanical, structural and mooring systems, energy production assessment,
etc. The present work describes the analysis and validation of six different blockage correction methods
for tidal turbines, described in literature, with blade-resolved RANS-CFD simulations. The simulations
were performed to seven different blockage rations and 5 tip speed ratios for each blockage case. The
blocked results were corrected with the different methods and compared to the quasi open-flow results
as a measure of the effectiveness of each one of them, showing a relatively good agreement for 4 out of 6
methods. Finally, this paper provides practical recommendations regarding the application of the different
correction methods, including an assessment of the required variables and their scope of application.
β is the blockage expressed as the ratio between tur-
bine area and channel cross-section.
A more complex approach to the problem of
modelling a turbine has been done by the appli-
cation of the Blade Element Momentum method
(BEM), widely employed for turbine and propeller
design (Hansen et al., 2006). The method has been
expanded by several authors to consider effects
such as tip-losses (Wimshurst & Willden, 2017),
turbulent wake effects (Buhl, 2005) and transient
phenomena (Hansen et al., 2004).
Turbine modelling can also be carried on by
means of viscous Computational Fluid Dynam-
ics solvers (RANS-CFD). Different approaches to
model the actual turbines have been implemented
within CFD codes such as actuator disks, actuator
lines or CFD-BEM models.
These provide different levels of detail depend-
ing on the implementation and requirements, rang-
ing from simple wake simulations to actual turbine
design for particular cases. The most complex
approach, however, consists in fully blade-resolved
simulations, where the blade geometry is modelled
as a solid, rotating boundary. This approach gives
insights about the flow in the domain, accounting
inherently for effects such as spanwise flow, flow
separation, etc. (Tampier et al., 2017).
From an engineering perspective, blockage is rel-
evant as it changes significantly the way a turbine
1 INTRODUCTION
Blockage is defined as the interaction effect
between a body under a constrained-flow con-
dition, and the boundaries surrounding it. Its
effects have long been discussed since the early
experimentation in circulation tanks for aero- or
hydrodynamics (Glauert, 1933a). The interaction
effects are typically seen, for the particular case of
turbines, as an increase in both power and thrust
forces when compared to the open-flow condi-
tion. This is caused by different effects such as an
increased flow speed around the body, a change of
pressure in the wake, differences in flow-develop-
ment for lifting surfaces such as foil sections and
longitudinal pressure gradients associated to the
tank boundary layer and fluid losses (Glauert,
1933a; Pope & Harper, 1966).
The earliest attempts to explain the behavior
of a turbine were made by the means of the one-
dimensional actuator-disc theory. This concept was
employed to derive the energy extraction limit for an
open-flow condition, set by a maximum power coef-
ficient
CP max =16 27/
known as the Lanchester-Betz
limit (Betz, 1920; Lanchester, 1915). These formu-
lation was complemented by Garret and Cummins
(Garrett & Cummins, 2007) showing that the maxi-
mum power coefficient for an actuator disk in a
constrained flow is
CP max = −
( )
16 27 1 2
/ ,
β
where
138
will behave, and corrections are required. It could
be to take the results of laboratory experiments
to a real-life scenario, to calculate the expected
power and loads on a tidal turbine that is already
designed, or to economically assess the deployment
of a farm in a particular spot.
For these reasons, the availability of quick block-
age correction methods that can be employed over
existing results obtained from different sources
(Experiments, CFD or BEM) is highly valuable
from a scientific, engineering and commercial per-
spective when assessing performance and behavior
under different operational and deployment condi-
tions is necessary.
The present work exposes a series of transient,
blade-resolved, RANS CFD simulations of a
horizontal axis hydrokinetic turbine under differ-
ent blockage and tip speed ratio conditions with
the purpose of providing information regarding
the scope and validity of different blockage cor-
rection methods. RANS CFD results are used to
compare six different blockage correction methods
(Bahaj et al., 2007; Glauert, 1933b; Maskell, 1965;
Mikkelsen & Sørensen, 2002; Pope & Harper,
1966; Werle, 2010).
2 VALIDATION CASE
To analyze the different blockage methods, the
SANDIA MHKF1 hydrokinetic turbine was
selected as a benchmark case. This is a three-bladed
horizontal axis turbine designed by the SANDIA
National Laboratories and UC Davis, and for
which experimental data is published including
turbine flow field quantification, performance
characterization and cavitation, among other
results (Fontaine et al., 2013a).
For the SANDIA MHKF1 hydrokinetic tur-
bine, shown in Fig. 1, simulations for 7 different
blockage ratios were made (see Table1). For each
of these conditions, the turbine was simulated
rotating at 5 different tip speed ratios λ, from 3.5
to 5.0 in 0.5 increments, leading to a total of 35
simulations.
The simulations were validated against experi-
mental results for a blockage ratio β=0.210.
Thrust and torque are obtained by integrating
the pressures over the turbine surfaces, and results
are converted to non-dimensional power and thrust
coefficients CP and CT.
In addition to these results, the axial induction
factors a are also obtained from the simulations,
with a defined as:
a U UT
= −10/
where UT is the average flow velocity at the turbine
plane and U0 the undisturbed flow velocity.
3 BLOCKAGE CORRECTION METHODS
Most of the blockage correction methods are based
on the traditional actuator disc theory, adapted for
the special case of a blocked flow. As usual, the
turbine is considered as an actuator disc where a
pressure discontinuity occurs.
From the diagram shown in Fig.2, several vari-
ables are identified. At the inlet, the undisturbed
flow velocity UT is considered as constant through-
out the entire cross-sectional area of the tunnel C.
At the turbine plane, the velocity is defined as U1
and outside as U3. Downstream, the velocity in
the wake region is defined as U2 and, outside this
region, as U4. At this point, the cross-sectional area
of the wake is AW. From momentum theory AW can
be defined as:
Figure1. Sandia MHKF1 hydrokinetic turbine and foil
sections.
Table1. Blockage cases.
Blockage
β
Domain
diameter
[-] [m]
0.001 63.2456
0.020 14.1421
0.050 8.9443
0.100 6.3246
0.150 5.1640
0.210 4.3636
0.400 3.1623
139
A A a
a
W=
1
1 2
Most blockage correction methods attempt
to obtain an equivalent free-flow velocity UF as
function of different variables such as blockage β,
thrust coefficient CT, wake expansion or induction
factors.
For each blockage correction method, a relation
between the tank velocity UT and a corresponding
free-stream velocity UF is given, leading to follow-
ing corrections for λ, CT and CP:
λ λ
c
T
F
U
U
=
C C U
U
Tc T
T
F
=
2
where the subscript c is meant for corrected or
equivalent free-flow values. In Table2, each of the
blockage correction is presented. Full details are
given in each of the cited articles.
4 NUMERICAL METHODS
The data-set of this study was obtained by numeri-
cally solving the Reynolds-Averaged Navier-Stokes
equations (RANS) under constant-density and
constant temperature assumptions (details e.g. in
(Ferziger & Peric, 2002)).
The simulations used a modified version of the
k-ω SST turbulence model with the correlation-
based
γ
θ
Re
transition model. This allows for the
prediction of the onset of transition in a turbulent
boundary layer (Malan et al., 2009; Menter et al.,
2005; Nichols, 2014).
The employed setup is the same used for the
bare turbine case described in (Tampier et al.,
2017). CD-Adapco’s STAR-CCM+ software was
employed to solve the models previously described.
All cases were configured as implicit unsteady sim-
ulations. Boundary conditions were defined within
the software as velocity inlet, pressure outlet, and
free slip wall for the domain limits. The turbine
itself was defined as a non-slip wall inside a rota-
tory subdomain.
The stationary and rotatory domains are sepa-
rated by an interface which is automatically defined
by the software.
The mesh was generated using the STAR-
CCM+ unstructured polyhedral mesher. The tur-
bine was configured to have a prism layer with 20
elements normal to the surface, being fine enough
to maintain a Y+<1 for the blade surfaces.
A mesh independence assessment was made
to the validation case and the results are shown
in Table 3. The intermediate mesh configura-
tion was considered sufficiently accurate for this
analysis.
For the remaining cases, the same turbine sur-
face configuration remained constant, as well as
the inflation layers and the element sizes inside
the rotatory domain and in the surrounding area.
A transverse cut of the mesh and a detailed view
of the blade mesh can be seen in Figs. 3 and 4
respectively.
Table2. Correction methods.
Method UT/UFObs.
Glauert
14 1
1
+
β
C
C
T
T
only if CT<1
Maskell
1ε
β
CT
ε empirical factor
Pope
11
+
( )
ε
t
εt empirical factor
Mikkelsen
uC
u
T
+
4
1
u=1 - a
Bahaj
U U
U
U
C
T
T
T
1
1
2
4
/
+
U1 as in orig. art.
Werle 1-βpreliminary
method
Table3. Mesh independence study.
Case No. of cells CPCT
Coarse 1.9 M 0.53433 0.94560
Medium 4.5 M 0.54027 0.91590
Fine 5.7 M 0.54171 0.90557
Figure2. Momentum diagram.
140
5 RESULTS AND DISCUSSION
The validation case was defined for a blockage ratio
of β=0.210, which is the same condition of the
experimental results obtained by Fontaine (Fon-
taine etal., 2013). In Figure5, CFD results for the
validation case are shown for thrust and power
coefficients CT and CP, along with experimental and
CFD results from ARL (Fontaine etal., 2013b).
Good agreement can be observed, especially for
the power coefficient curve.
Although acceptable for this study, larger differ-
ences are observed between numerical and experi-
mental results for thrust that were also reported by
Fontaine on their CFD simulations (Fontaine etal.,
2013b). This is likely to be caused by the differ-
ences between the simulations and the experiments
regarding the presence of structures associated to
the measuring equipment in the laboratory setup
Figure4. Detailed view of the blade mesh.
Figure 5. CFD results for validation case (β= 0.210)
compared to experimental and CFD results from
Fontaine et al. (2013b).
Figure6. Normalized axial velocities of the validation
case (β= 0.210) in longitudinal plane. From top to
bottom: λ=3, 4 and 5.
that are neglected in the computational models.
Normalized axial velocities (UX=UT) in the lon-
gitudinal plane are shown in Fig.6. As mentioned
Figure3. Mesh cut at turbine plane of the bare turbine
domain.
141
in section 2 and detailed in Table1, CFD simula-
tions were carried out for a blockage range from
β=0.001 to 0.400.
In Figure 7, the obtained thrust and power
coefficient results are shown for each blockage
condition.
From these results, the lowest blockage ratio
(β=0.001) is considered as a quasi-free flow condi-
tion, and will be used as a reference for the applied
corrections. The results for β=0.210 represent the
validation case, as described previously.
The presented results for β=0.020 to 0.400 were
corrected by each of the presented methods, as
shown in Figure8.
As expected, most of the correction methods
provide results which are very close to the quasi
free-flow case (β=0.001), giving a first overview
of the effectiveness of each one of them. Due to
the superposition of results, not each CTc or CPc
curve is visible for a specific blockage ratio. Forthe
Glauert correction, results are shown only for
results with CT < 1.
From the obtained results, an error analysis was
made, considering the relative error as:
E
C C
C
C
X X
X
X
C
=0
0
where the subscript X corresponds to thrust or
power (T or P), subscript c corresponds to cor-
rected results, and subscript 0 to unblocked results
(β=0.001). The relative error is obtained for each
method along the corrected range of λc for each
blockage ratio. In order to obtain a global over-
view of error for each method, mean absolute error
values were obtained for
ECT
and
ECP:
MAE E
X CX
=
The results are shown in Table4 for each correc-
tion method.
From this table, it can be observed that the mini-
mum error is obtained by the Mikkelsen & Sørensen
method, followed by the Bahaj method. For the
Glauert method, even if only results from data with
CT<1 were considered, a higher total error can be
observed. The Werle method has an unexpectedly
high error, and is therefore not recommendable for
its application as a correction method for a large
blockage and tip speed ratio range.
Figure 7. Uncorrected thrust (in blue) and power
coefficients (in green) CT and CP, for blockage range
(β=0.001 to 0.400). Free-flow reference values (β=0.001)
are given in red for CT and magenta for CP.
Figure 8. Blockage corrected thrust (blue) and power
(green) coefficients CTc and CPc. Free-flow reference values
(β=0.001) are given in red for CT and magenta for CP
.
Table 4. Mean absolute error of thrust and power
corrections.
Method MAET (%) MAEP (%)
Glauert 5.69 9.69
Maskell 2.60 4.68
Pope & Harper 2.00 3.18
Mikkelsen & Sørensen 0.76 0.69
Bahaj 1.54 2.78
Werle 28.05 29.49
142
6 CONCLUSIONS
The use of a RANS-CFD tool to model the per-
formance of a hydrokinetic turbine over a wide
range of blockage conditions can provide useful
data to analyze existing blockage correction meth-
ods, propose improvements to these or to propose
new methods for specific applications.
The used CFD method shows good agreement
with results from literature (both numerical
and experimental for the bare turbine), giving a
validation of the presented results. Additionally, it
would be advisable to carry out experimental tests
under different blockage conditions, to have a full
validation of these cases as well.
From the presented results, the authors
recommend the use of the Mikkelsen and Sørensen
method for the correction of the blockage for hori-
zontal axis turbines subject to experimental test
or numerical simulations under conditions similar
to the presented here, especially in case of avail-
able induction factor data. In case that induction
factors are not available, the Bahaj correction is
recommended.
It is also recommended, considering the pre-
sented results, to avoid using the Werle and Glau-
ert methods, considering that other simple and
more reliable methods, such as those by Maskell or
Pope & Harper, are available.
The study of a series of different blockage ratios
for other turbines, tank sections (such as square or
rectangular sections) or other arrangements could
allow the development of new blockage correction
methods.
Further investigation could consider free surface
effects and the interaction with other devices (as in
tidal farms), to consider these effects in blockage
corrections as well.
REFERENCES
Bahaj, A.S., Molland, A.F., Chaplin, J.R., & Batten,
W.M.J. (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), 407–426.
Betz, A. (1920). Das Maximum der theoretisch mögli-
chen Ausnützung des Windes durch Windmotoren.
Zeitschrift Für Das Gesamte Turbinenwesen, 26,
307–309.
Buhl, M.L. (2005). A New Empirical Relationship
between Thrust Coefficient and Induction Factor
for the Turbulent Windmill State. Technical Report
NREL/TP-500–36834, (August).
Ferziger, J.H., & Peric, M. (2002). Computational Meth-
ods for Fluid Dynamics. Springer.
Fontaine, A.A., Straka, W.A., Meyer, R.S., & Jonson,
M.L. (2013a). A 1:8.7 scale water tunnel verification &
validation test of an axial flow water turbine (Vol. 53).
Fontaine, A.A., Straka, W.A., Meyer, R.S., & Jonson,
M.L. (2013b). A 1:8.7 scale water tunnel verification
& validation test of an axial flow water turbine, 53(9),
1689–1699.
Garrett, C., & Cummins, P. (2007). The efficiency of a
turbine in a tidal channel. Journal of Fluid Mechanics,
588, 243–251.
Glauert, H. (1933a). Wind Tunnel Interference on Wings,
Bodies and Airscrews. Aeronautical Research Commit-
tee, (1566), 1–52.
Glauert, H. (1933b). Wind Tunnel Interference on Wings,
Bodies and Airscrews. Aeronautical Research Commit-
tee, (1566), 1–52.
Hansen, M.H., Gaunaa, M., & Aagaard Madsen, H.
(2004). A Beddoes-Leishman type dynamic stall model
in state-space and indicial formulations. Risoe-R.
Hansen, M.O.L., Sørensen, J.N., Voutsinas, S., Sørensen,
N., & Madsen, H.A. (2006). State of the art in wind
turbine aerodynamics and aeroelasticity. Progress in
Aerospace Sciences, 42(4), 285–330.
Lanchester, F.W. (1915). A contribution to the theory
of propulsion and the screw propeller. Journal of
the American Society for Naval Engineers, 27(2),
509–510.
Malan, P., Suluksna, K., & Juntasaro, E. (2009). Calibrat-
ing the γ-Reθ transition model for commercial CFD.
In 47th AIAA Aerospace Science Meeting Including
The New Horizons Forum and Aerospace Exposition
(pp. 1–14). Orlando, Florida.
Maskell, E.C. (1965). A Theory of Blockage Effects on
Bulff Bodies and Stalled Wings in a Closed Wind Tun-
nel. Her Majesty’s Stationery Office, 1–27. https://doi.
org/AD-A955 243.
Menter, F.R., Langtry, R., Völker, S., & Huang, P.G.
(2005). Transition Modelling for General Purpose
CFD Codes. Engineering Turbulence Modelling and
Experiments 6, (August), 31–48.
Mikkelsen, R., & Sørensen, J.N. (2002). Modelling of
Wind Turbine Blockage. In EWEC. Paris.
Nichols, R.H. (2014). Turbulence models and their appli-
cation to complex flows (Vol. Rev.4.01).
Pope, A., & Harper, J. (1966). Low-speed wind tunnel
testing.
Tampier, G., Troncoso, C., & Zilic, F. (2017). Numerical
analysis of a diffuser-augmented hydrokinetic turbine.
Ocean Engineering, 145(September), 138–147.
Werle, M.J. (2010). Wind Turbine Wall-Blockage Per-
formance Corrections. Journal of Propulsion and
Power, 26(6), 1317–1321.
Wimshurst, A., & Willden, R.H.J. (2017). Extracting
lift and drag polars from blade-resolved computa-
tional fluid dynamics for use in actuator line model-
ling of horizontal axis turbines. Wind Energy, 20(5),
815–833.
Article
A way to quantified diffuser-rotor interaction is presented for a micro-diffuser-augmented hydrokinetic turbine (MDAHT) base on the actuator disc theory (Jamieson, 2011). The large eddy simulation/Reynolds-averaged Navier–Stokes model (DES) for computational fluid dynamics were employed to simulate for bare turbine, bare diffuser and diffuser-augmented turbine, respectively. The axial induction factor of bare diffuser was obtained via the average speed of the turbine center plane, and that of both bare turbine and diffuser-augmented turbine were obtained based on the computational CP and CT. The result shows that the interaction between the diffuser and rotor are corresponding to equivalent axial induction factor ai and ai+ ad, which is tightly relative to diffuser shape parameters and the operational parameters. Bigger angle of attack and camber of diffusers contributes to higher positive ai and higher negative ai+ ad, and more energy harvesting performance on MDAHT is acquired. Besides, angle of attack and camber of diffuser also affected the variation of the CP and CT curve. The maximum TSR point was shifted to higher TSR position with the increase of angle of attack and camber of diffuser, and the angle of attack has a larger influence on the energy harvesting performance for MDAHT comparing with the camber of diffuser. Moreover, the influences of the tip clearances and diffuser contraction ratios on energy harvesting performance versus TSRs were also investigated.
Article
The current work presents a novel way to evaluate the interaction effects in a diffuser-augmented hydrokinetic turbine (DAHT) under the terms presented on the generalized actuator disc theory described by Jamieson (2011). Transient RANS CFD methods are employed to obtain the performance, thrust, and average flow speeds at the turbine plane in simulations performed in three comparable cases: bare turbine, bare diffuser and diffuser-augmented turbine. After validating the bare turbine case comparing numerical results against the experiments presented by Fontaine et al. (2013), the axial induction factors are obtained for the three cases based on the average speeds of the turbine plane. The analysis of the results shows the importance of considering rotor-diffuser interaction for the design of diffuser-augmented devices, and that these interaction effects are just as relevant as the bare diffuser and the bare turbine characteristics.
Article
Low order rotor models such as the actuator line method are desirable as an efficient method of computing the large range of operating and environmental conditions, required to design wind and tidal rotors and arrays. However, the integrated thrust and torque predictions for each rotor are dominated by the blade loading on the outboard sections, where three-dimensional (3D) effects become increasingly significant, and the accuracy of the reduced order methods remains uncertain. To investigate the accuracy of the spanwise blade loading on an individual rotor, actuator line and blade boundary layer resolved computations of the Model Rotor Experiments in Controlled Conditions (MEXICO) rotor are presented. The high fidelity blade-resolved simulations give good agreement with measured pressure coefficient and particle image velocimetry data. Alternative lift and drag polars are extracted from the 3D simulated flow fields as a function of radial position. These are then used as replacement inputs for the actuator line method. Significant improvement in the accuracy of the actuator line predictions is found when using these 3D extracted polars, compared with using simulated two-dimensional lift and drag polars with empirical correction applied to the spanwise loading distribution. Additionally, the 3D flow field data is used to derive different axial and tangential spanwise loading corrections for use with the two-dimensional blade polars. Copyright
Article
The large influences that can be encountered for relatively small propeller-to-wind-tunnel area ratios due to the amplifying effect of the wake's downstream growth were investigated. The assumptions applied includes that inviscid incompressible flow is through a conduit of constant cross-sectional area Ac, flow with specified uniform pressure and velocity enters at upstream infinity. The flow exits at downstream infinity at uniform pressure po and a slipstream occurs between the mainstream fluid exiting at velocity Vc and the fluid exiting at velocity Vo, which passed through the actuator-disc model of the rotor and the cuts around the propeller shrink to its surface. The computational fluid dynamic (CFD) methods that necessarily employ a finite domain size should avoid imposing a pressure boundary condition at the downstream outlet station.
Article
There is an upper bound to the amount of power that can be generated by turbines in tidal channels as too many turbines merely block the flow. One condition for achievement of the upper bound is that the turbines are deployed uniformly across the channel, with all the flow through them, but this may interfere with other uses of the channel. An isolated turbine is more effective in a channel than in an unbounded flow, but the current downstream is non-uniform between the wake of the turbines and the free stream. Hence some energy is lost when these streams merge, as may occur in a long channel. We show here, for ideal turbine models, that the fractional power loss increases from 1/3 to 2/3 as the fraction of the channel cross-section spanned by the turbines increases from 0 to close to 1. In another scenario, possibly appropriate for a short channel, the speed of the free stream outside the turbine wake is controlled by separation at the channel exit. In this case, the maximum power obtainable is slightly less than proportional to the fraction of the channel cross-section occupied by turbines.