In order to design future large wind turbines, knowledge is needed about the impact of aero-elasticity on the rotor loads and performance and about the physics of the atmospheric flow surrounding the turbines. The objective of the present work is to study both effects by means of high-fidelity rotor-resolved numerical simulations. In particular, unsteady computational fluid dynamics (CFD) simulations of a 2.3 MW wind turbine are conducted, this rotor being the largest design with relevant experimental data available to the authors. Turbulence is modeled with two different approaches. On one hand, a model using the well-established technique of improved delayed detached eddy simulation (IDDES) is employed. An additional set of simulations relies on a novel hybrid turbulence model, developed within the framework of the present work. It consists of a blend of a large-eddy simulation (LES) model by Deardorff for atmospheric flow and an IDDES model for the separated flow near the rotor geometry.

In the same way, the assessment of the influence of the blade flexibility is performed by comparing two different sets of computations. The first group accounts for a structural multi-body dynamics (MBD) model of the blades. The MBD solver was coupled to the CFD solver during run time with a staggered fluid–structure interaction (FSI) scheme. The second set of simulations uses the original rotor geometry, without accounting for any structural deflection. The results of the present work show no significant difference between the IDDES and the hybrid turbulence model. In a similar manner, and due to the fact that the considered rotor was relatively stiff, the loading variation introduced by the blade flexibility was found to be negligible when compared to the influence of inflow turbulence. The simulation method validated here is considered highly relevant for future turbine designs, where the impact of blade elasticity will be significant and the detailed structure of the atmospheric inflow will be important.

As future wind turbines will have unprecedentedly long and flexible blades, the necessity of understanding the effects of aero-elasticity on the rotor performance and on its structural integrity increases. Along with this, large wind turbines interact with a larger part of the atmospheric boundary layer (ABL), often exceeding the height of the atmospheric surface layer. This also needs consideration in the design phase, as the rotor blades consequently experience a large variation of flow through each revolution, and flow cases which were not relevant to consider for past designs might occur. This needed knowledge can be obtained through high-fidelity methods, such as fluid–structure interaction (FSI) simulations, which model the coupled effects of both flow and structure. These simulations can further be used to develop and improve lower-fidelity engineering models used by wind turbine designers in industry.

FSI of wind turbines in atmospheric turbulent flow is not a widely studied topic, due to the computational costs of such simulations, especially when geometrically resolved wind turbines are modeled. Instead, a more efficient approach often chosen is the use of actuator lines/discs

Looking at rotor-resolved CFD/FSI, using LES is still too computationally expensive for many practical applications. Instead, compromises are needed for the turbulence models. In the works by Santo et al., FSI for wind turbines, structurally represented through finite-element shells, were studied for steady ABL flows

An alternative more complex method for simulating geometrically resolved turbines in the ABL flow was proposed by

In general, considering presently available high-performance computing capabilities, compromises are needed when doing high-fidelity aero-elastic modeling of wind turbines in atmospheric flow using FSI – either by reducing the rotor representation by actuator lines to allow LES simulations or instead by simplifying the turbulence modeling.

The objective of the present study is to move one step up the ladder of complexity by investigating rotor aerodynamics and aero-elasticity in turbulent LES inflow, using a novel turbulence model. The model is inspired by the one of

In this section, the computational solvers are presented along with the simulation strategies such as FSI framework and precursor simulations. Further, the participating turbulence models will be introduced, to prepare for the discussion of the hybrid model. Finally, the computational grids used in the study are described along with the chosen simulation parameters.

To solve the fluid flow, the DTU in-house CFD code EllipSys3D

Several turbulence models are implemented such as two-equation Reynolds-averaged Navier–Stokes (RANS) models,

For FSI simulations, the deformation of grids is handled through a moving mesh method with a blend factor. The surface displacement is propagated along the grid lines normal to the surface, with a blend factor gradually diminishing to zero with increasing distance to the blade surface. The blending can be either linear in the distance to the blade surface or based on a tanh function. This ensures that mesh points in the vicinity of the blade surface are displaced as a solid body movement along with the blade, while points further away only move a fraction of the displacement. When using the overset grid method, the deformation is only transferred to the volume grid blocks containing the solid surface.

The code has been used extensively for a range of test cases and was validated in, e.g., the Mexico project

HAWC2

HAWC2 has a built-in aerodynamics module that calculates aerodynamic forces using BEM theory. As is common in BEM implementations, prediction of airfoil aerodynamic performance is based on pre-computed look-up tables of lift, drag, and moment, which are needed to calculate forces along the blade. Multiple correction schemes are implemented to improve the BEM aerodynamics, such as tip loss corrections, dynamic stall models, tower shadow effect, and many more; see

HAWC2 is widely used by industry, and it has been verified and validated in

The codes EllipSys3D and HAWC2 are coupled, in a partitioned manner, through the Python framework, referred to as the DTU coupling, originally created by

Using predicted displacements of nodes from HAWC2, the CFD mesh is deformed, and a new flow field is found through EllipSys3D. The loads predicted by the CFD solver are then applied to the HAWC2 structural model and a new deformation is found. All communication between EllipSys3D and HAWC2 happens through the DTU coupling framework. In

Studies involving the application of the FSI framework, for both operational and standstill configurations, include

the displacements of the present time step are predicted by HAWC2 with second-order accuracy, using kinematics from the previous time step;

displacements are sent to EllipSys3D, and the surface mesh is deformed, while displacements are propagated into the volume mesh using a volume blend method;

the Navier–Stokes equations are solved to calculate the flow field for the new time step through under-relaxed sub-iterations in EllipSys3D;

forces are computed and integrated on the CFD mesh surface and sent to HAWC2;

forces are interpolated to the aerodynamic sections of the HAWC2 model, and actual deformations are calculated;

unless the solution has reached the total simulation time, the simulation is advanced to the next time step and the procedure is repeated.

A hybrid turbulence model has been developed to consider the dominant turbulence scales from the atmospheric boundary layer (ABL) down to the blade boundary layer (BBL), within the same simulation. To do this, the Deardorff one-equation LES turbulence model for ABL flows

In the Deardorff LES turbulence model

The SGS energy,

For the

For

The length scale which appears in the

DES is known to be sensitive to sudden changes of grid refinements as grid-induced separation (GIS) can be introduced. Here, the modeled turbulent viscosity will drop instantly without the additional turbulence being resolved. It is also known to have a mismatch between the URANS and LES region, if used as a wall-modeled LES model. These issues are addressed in DDES

In order to simulate the effect of turbulence on both ABL and BBL scales, a hybrid method is suggested where the Deardorff ABL LES model is blended together with the BBL DES models to avoid the need of excessive grid resolution in the BBL otherwise needed by LES. The blending is established through a blending function

The blending function

To allow the present method to work together with the

It is noted that in the Deardorff part of the model the turbulent viscosity,

In this study, the turbulent flow of the atmospheric boundary layer is modeled through a LES precursor simulation using the Deardorff model. Here, a neutrally stratified wind profile is simulated and sampled for use as input in the successor simulation including the rotor.

In the successor simulation the hybrid LES–IDDES model is used. LES is used for turbulence modeling in the majority of the domain, except for the region close to the rotor. In this area, the IDDES model is utilized instead, which removes the LES grid requirement near the rotor surface.

The precursor conditions are approximating measurements from the DanAero field experiment

Air is described with a density of 1.22 kg m

To enable the hybrid turbulence modeling, a blending region must be defined. As mentioned in Sect.

The length scale limit of the LES region caps the frequency range of the resolved turbulent kinetic energy to the background grid resolution. Close to the rotor, however, the small-scale detached flow is still captured through the IDDES model. For studies, with long distances from refinement to object or larger resolution differences between background and overlapping sub-grids, this strategy would likely not be optimal due to the capping of resolved frequencies being based on an unnecessarily large grid size.

In the present setup the blending between LES and IDDES happens with the midpoint (

Blend factor,

Concept of precursor to successor simulations along with domain sizes of conducted precursor and successor simulations. Colored contours showing flow velocity

The structural model used for the NM80 turbine was created and validated internally at DTU Wind Energy as part of the original DanAero project

For the precursor simulation, as the first step, the turbulent flow is developed by recycling the flow using periodic boundary conditions. This resembles the flow moving over a very long distance, building up the boundary layer, and producing the turbulence through shear production. In order to ensure a mean profile close to the desired measured wind velocity profile, the SG wall model is used. This forces the surface shear stress of the first adjacent cells to the ground to fit the log law. The flow is driven trough a constant pressure gradient calibrated to obtain the desired friction velocity and resulting velocity profile with a roughness length

Initially, the grid sequencing scheme of EllipSys3D is utilized on three grid levels to speed up the simulation and reach a fully turbulent domain quickly.
When the flow is fully turbulent and the mean flow profiles match the desired flow, planes consisting of velocity components

The FSI successor simulation process is divided into phases depicted in Fig.

Process diagram of conducted simulations.

In the first phase, simulations without coupling to the structural solver are run to develop the flow and fill the domain with the sampled turbulent flow. In this phase, the grid sequencing scheme of EllipSys3D is used exploring coarser grids to minimize the simulation cost during spin-up.

Grids used for simulations.

When passing to the FSI framework, phase 2, HAWC2 is run for the same amount of revolutions using BEM aerodynamics corresponding to the mean flow profile to ensure compatibility in time between the solvers when coupling and obtaining a good guess of initial blade deformations. In phase 3 the coupling of EllipSys3D and HAWC2 is initiated with a smooth linear blending of forces over two revolutions to switch from BEM to CFD loading. This is done to avoid any large force jumps in the HAWC2 solver, to suppress undesired vibrations in the system. In the final phase, phase 4, pure CFD loads are used for calculation of structural response, and a full two-way coupling is simulated for the desired amount of revolutions.

The precursor domain is

For the rotor simulations, an overset grid method is utilized

In the present setup, only the rotor is considered, omitting the tower, hub, and nacelle, with a total of three overlapping mesh groups; see Fig.

Around the rotor mesh, a cylindrical disc mesh is constructed with pre-cut holes around the blades. This mesh rotates along with the rotor mesh, speeding up the hole-cutting algorithm, as the holes move along with the rotor. Thereby, the need of searching for hole, fringe, and donor cells between rotor and disc mesh for each time step is avoided, as the relations between the two meshes remain the same.

All deformation from the rotor is propagated to the rotor mesh in such a way that only cells that lie inside the hole region of the overlapping disc mesh deform. This is done to avoid deformation of the donor cells, keeping the interpolation coefficients between fringe and donor cells unaltered. Through this simplification, there is no need for updating communication tables for donor and receiver cells between the rotor and disc mesh as these also rotate together. This choice, however, necessitates that the hole of the disc mesh be far enough from the surface to leave room for the deformation of mesh cells without impairing the cell quality. In the present setup the holes are 17m wide in the rotor axis direction, where the main deformation is present, located with the undeformed rotor in the center. Displacements are propagated to the volume mesh, such that points within the inner 15 % of the grid curve length normal to the surface are moved as solid body motion to ensure no change of quality of the inner cells resolving the high gradient flow. Further out, from 15 to 40 % the volume blend factor is linearly decaying from 1 to 0, such that points from 40 % grid curve length and out are unchanged to avoid changes to donor cells. Note that communication tables and hole cutting still need an update between disc mesh and background mesh as the latter is static. The disc and rotor grids are similar to the setup used in

Near-rotor mesh at 25 m span and surface discretization at tip. Only every second line shown.

The background domain is a box of

A total of 78 million cells are used for the combined setup.

A total of 9750 s was simulated for the precursor simulation, of which the final 1000 s (equivalent to

From the sampling plane, depicted in Fig.

Figure

Precursor results:

In the following, the results of the successor simulations are presented. First, the new turbulence model is compared to the same setup using only the IDDES turbulence model assuming a elastically stiff configuration. Further, results from simulations using the hybrid model with and without flexibility of the blades are presented to study the effect of the blade elasticity. For the initial phase 1 (see Fig.

Isobars of

Velocity

Instantaneous sections of flow velocity

To study the impact of the presented turbulence model on the flow, simulations with the hybrid LES–IDDES blending enabled along with pure IDDES simulations are conducted. In the pure IDDES simulation, a slip wall condition is used on the terrain surface, contrary to the log law used for the LES–IDDES hybrid model. Simulations with and without the rotor present were simulated. In the empty setup, the hybrid model acts as a pure Deardorff LES model, as no blending region is defined. For all simulations, inflow is interpolated from the LES precursor planes to ensure identical inlet conditions. In the simulations comparing turbulence models, only the CFD code has been used, meaning that no flexibility of the blades is considered.

Firstly, the empty setups are presented in Fig.

Instantaneous sampled profiles at time

Stiff simulations covering 35 rotor revolutions were also conducted with the two turbulence models, including the rotor in the simulations. Mean and standard deviations of azimuthal forces of the final 15 revolutions at two blade sections, near the mid-span and near the tip, are presented in Fig.

Normal and tangential forces at 48 and 92 % blade length using hybrid or IDDES turbulence model. Temporal means and standard deviations based on the final 15 revolutions.

To study the effect of the rotor flexibility, FSI simulations of flexible and stiff setups were performed. First, 35 revolutions were simulated through pure CFD, as presented before, followed by 25 revolutions with the FSI coupling enabled; see Fig.

The following results are obtained using the hybrid turbulence model only, but similar results would be expected for pure IDDES simulations, based on the aforementioned findings. The effect of including the blade flexibility is assessed through the resulting blade displacements, torsion, and rotor loading.

Figure

Integrated thrust and torque for stiff and flexible configurations.

Blade torsion is quite low as well, with less than 0.5

In Fig.

As mentioned, some differences are present in the simulation setup compared to the DanAero field experiment, being the omission of yaw, tilt, and tower along with the higher turbulence intensity of the generated flow.

Despite this disclaimer, the resulting forces at four sections of the blade are depicted in Fig.

Normal and tangential forces for stiff and flexible simulations along with DanAero measurements. Sections at 33, 48, 76, and 92 % blade length.

The impact of including flexibility is quite small, and general observations are that normal and tangential forces respectively slightly increase and decrease when considering the flexibility of the rotor. This is expected for the NM80 rotor, which is quite stiff compared to modern wind turbines. The standard deviations of the forces due to turbulence are much higher than the difference between mean forces of stiff and flexible simulations. This shows that including turbulent inflow is more important than including flexibility, at least in the present rotor/flow case. In the simulations including the flexibility the standard deviations of the normal forces are up to 10 % of the mean near the tip and 15% near the root. For tangential forces this is even higher, with 24 % near the tip and 38 % near the root.

Spectral analysis of the resulting normal and tangential force signals at the 76 % blade length section are presented in Fig.

This study investigates the phenomenon of aero-elasticity of wind turbines placed in atmospheric flow conditions, by means of high-fidelity numerical methods. Fluid–structure interaction (FSI) simulations of a 2.3 MW wind turbine rotor have been conducted using a novel turbulence model, blending the Deardorff large-eddy simulation (LES) model for atmospheric flows with the improved delayed detached eddy simulation (IDDES) model for the separated flow near the rotor boundary. Precursor simulations were conducted in a large domain in order to assure sampling of realistic turbulent atmospheric boundary layer (ABL) flow, matching well with the DanAero measurements, for the successor simulations.

As the first study, the hybrid model was compared to the pure IDDES turbulence model, by computational fluid dynamics (CFD) successor simulations of the turbulent ABL inflow with and without the rotor present. In empty simulations, this corresponded to a comparison between pure Deardorff LES and pure IDDES, while for rotor simulations the hybrid model used both Deardorff LES for the domain flow and IDDES for the near-rotor flow. It was found that there was no significant difference in either the flow or the rotor loading between the two methods, likely due to the short domain considered and assumptions omitting the Coriolis force and temperature effects.

Secondly, FSI simulations were conducted by coupling the CFD simulations to a structural solver. It was found that for the specific rotor, which is relatively stiff compared to modern turbines, only a small impact was found by considering the flexibility of the blades. A general increase of

Inflow turbulence on the other hand has a large influence on the rotor loading, with standard deviations as high as 15 % of the mean for normal forces and even higher tangentially. This emphasizes the importance of correct modeling of inflow turbulence.

As has been shown in the present study, the developed hybrid turbulence model resulted in practically identical loading of the rotor to that of the IDDES model alone. Relevant future studies would be to investigate when this is not the case. This could for instance be simulations including stable/unstable stratification and/or the Coriolis force. Here, the IDDES model will probably be insufficient to capture the effects, as the model is calibrated for aerodynamics mainly and not ABL flows. The Deardorff LES model, however, is calibrated for such flows, and the mixing length scale depends on the stratification, as it is reduced for stable cases. The two models also model temperature effects differently as the flux (

A relevant future study would likewise be to compare the method to more efficient BEM-based aerodynamics solvers with the precursor turbulence as input. Here, the CFD-based results could, if needed, be used to correct airfoil polars and calibrate the many correction models needed by BEM solvers to consider e.g. tip loss effects, dynamic inflow, and dynamic stall.

In terms of FSI, it would be natural to investigate more recent/future turbine designs, which are larger and much more flexible than the considered NM80 rotor. These rotors are at a higher risk of instability phenomena and operate in a larger part of the atmospheric boundary layer.

The codes used to conduct the presented simulations are licensed and not publicly available. The structural model of the NM80 rotor is likewise not publicly available. However, result data can be shared upon request.

CG conducted all simulations, including grid generation, and implemented the presented turbulence model in the CFD code. Additionally CG did the analysis of the results and has been the main writer of the paper. NNS assisted with expertise in the code development and CFD setup, along with planning the study and analysis. SGH has supported in especially FSI setup along with planning and analysis. NT supported the development and implementation of the turbulence model. FZ assisted in the overset grid setup, and did development on the CFD code to accelerate simulations. Further, all authors contributed in writing and editing this paper.

The authors declare that they have no conflicts of interest.

The DanAero projects, from which experimental data were obtained, were funded partly by the Danish Energy Agency (EFP2007. Journal no. 33033-0074 and EUDP 2009-II. Journal no. 64009-0258) and partly by internal funding from the project partners.

This study was conducted as part of the PhD project “Fluid-structure Interaction for Wind Turbines in Atmospheric Flow”, which was internally funded by the Technical University of Denmark (DTU) – Department of Wind Energy.

This paper was edited by Johan Meyers and reviewed by two anonymous referees.