| |
By N. Mandas, C.E. Carcangiu, and F. Cambuli, Department of Mechanical
Engineering, Università degli Studi di Cagliari, Cagliari, Italy
View the pdf of this article
Computational domain and boundary conditions
The environmental impact of burning fossil fuels and their inevitable
depletion have led to a growing interest in renewable energy sources.
These sources of energy can no longer be overlooked, because of the need
to achieve sustainable development and compliance with the provisions
of the recently enforced Kyoto protocol. Wind energy, for example, is
a low density source of power, available almost everywhere but not necessarily
all the time, and its efficient exploitation requires continued in-depth
studies. To make wind power economically feasible, it is important to
maximize the efficiency of converting wind energy into mechanical energy.
Of all the different aspects involved in this process, rotor aerodynamics
is a key determinant for achieving this goal. In addition, the ability
to predict the downstream wake from a wind turbine is significant factor
for determining the interactions between turbines. A model for describing
this perturbed flow can provide a useful tool for optimizing the placement
of wind turbines and the aerodynamic and structural design of the rotors.
Rotor surface mesh
Mechanical power and power coefficient determined using the BEM
method and CFD, for different wind velocities, V0, and tip speed ratios,
ë
Research work conducted in this area has resulted in a substantial improvement
in the overall efficiency of the conversion process, to the extent that
the capital costs of installing wind power can now compete effectively
with other renewable energy sources. Three approaches can be pursued to
analyze the flow around and downstream of a wind turbine: field testing,
which provides accurate results but is highly complex and expensive; analytical
and semi-empirical models, which adopt simplifying assumptions and are
thus not universally reliable; and CFD, which offers the best alternative
to direct measurements.
At the University of Cagliari, FLUENT has been used to analyze an aerodynamic
problem that would be difficult to tackle experimentally [1]. The study
concerned a 41 m diameter wind rotor; the disturbed flow field, including
the wake, extends over hundreds of meters in the axial direction with
a very large cross section. Understandably, field measurements over such
a vast swept area (moderate in size, compared to other wind turbines in
existence) would be extremely time-consuming and costly. The stall controlled
rotor with fixed blades, rotating at a constant speed of 27rpm, was simulated
using CFD and a simplified analytical model. Design operating conditions
with a range of wind speeds were investigated.
The computational domain used is in the shape of a diffuser, extending
in the axial direction roughly 5 diameters upstream and 10 diameters downstream
of the rotor. In the plane of the rotor, the domain diameter is five times
that of the rotor. The multiple reference frames (MRF) model was used
to simulate the incompressible, steady-state flow field. A uniform wind
speed profile was assumed at the entrance of the domain. The one-equation
Spalart- Allmaras model with standard wall functions was chosen for turbulence
closure. Due to rotational periodicity, only one of the rotor blades was
simulated, and periodic boundary conditions were used at the rotational
boundaries. The wind turbine tower and ground were not included in the
model. GAMBIT was used to build a multi-block hexahedral mesh of approximately
1.5 million cells. The preprocessing phase accounted for about 80% of
thetotal project time as a result of the range of geometric scales represented:
the length of the domain (600 m), size of the rotor (41 m), typical chord
lengths (0.5-3 m), and boundary layer (10 mm).
Contours of total pressure illustrate the wake
Iso-surface of vorticity generated by the turbine
The classical blade element momentum (BEM) method was adopted for the
design of the turbine rotor [2], using the specifications for the three-bladed
horizontal axis Nordtank 41/500 turbine [3] and NACA 63-4xx profiles [4].
The active part of the blade was extended to the hub, in keeping with
the style used in modern wind turbine designs. The BEM results were compared
with those obtained using FLUENT.
To compare the models, the overall performance of the turbine was computed.
This included an assessment of the mechanical power generated on the shaft
axis as a function of inlet velocity, and the corresponding power coefficient
as a function of tip speed ratio. The CFD results were found to be in
good agreement with those obtained using the BEM method. Contours of total
pressure predicted by FLUENT were used to show the wake development downstream
of the turbine. Axial velocity contours were used to identify the transition
from the near wake to the far wake region. In the far wake, diffusion
phenomena cause the overall wake cross section to expand while the de-energized
core in the central region reduces. Near the blade tip, the pressure difference
between the pressure and suction sides of the blade were shown to lead
to the formation of tip vortices.
Axial velocity, showing the reduction of the
de-energized core in the far wake region
Pathlines showing the tip vortex
While the CFD results confirmed the validity of the BEM method, the latter
yields unsatisfactory results when used to analyze wind turbines operating
at off-design conditions. CFD, on the other hand, enables engineers to
study the flow in deep stall or even standstill conditions. Furthermore,
the detailed description of the physical phenomena provided by CFD can
be captured neither by a simplified analysis method nor through experimental
measurements. With the continued advances in computing technology and
the availability of increasingly powerful computers, CFD will become more
popular for solving the aerodynamic problems associated with wind turbines
in the years to come. References: 1 Carcangiu, C.E. Simulazione Numerica
del Flusso Attorno al Rotore di una Turbina Eolica. Tesi di Laurea Specialistica,
DIMeCa – Università di Cagliari, Dic. 2004. 2 Mandas, G. Progetto
Fluidodinamico di un Rotore di Turbina ad Asse Orizzontale. Tesi di Laurea,
DIMeCa – Università di Cagliari, Ott. 2002. 3 Hansen, M.O.L.
Aerodynamics of Wind Turbines: Rotors, Loads and Structure. James &
James: London, 2000. 4 Abbott, J.H.; Von Dohenhoff, A.E. Theory of Wing
Sections, Dover Publications Inc.: New York, 1959.
References:
- Carcangiu, C.E. Simulazione Numerica del Flusso Attorno al Rotore
di una Turbina Eolica. Tesi di Laurea Specialistica, DIMeCa – Università
di Cagliari, Dic. 2004.
- Mandas, G. Progetto Fluidodinamico di un Rotore di Turbina ad Asse
Orizzontale. Tesi di Laurea, DIMeCa – Università di Cagliari,
Ott. 2002.
- Hansen, M.O.L. Aerodynamics of Wind Turbines: Rotors, Loads and Structure.
James & James: London, 2000.
- Abbott, J.H.; Von Dohenhoff, A.E. Theory of Wing Sections, Dover
Publications Inc.: New York, 1959.
|
|
|
