Constraining effect of load frames during full-scale rotor blade fatigue testing

In rotor blade fatigue tests used for the certification process, load frames are used to introduce the loads to the blade. These load frames have a constraining effect on the cross-sectional deformation. This work investigates these constraining effects using a finite element contact analysis on a current-generation commercial rotor blade. Two different load frame variants are considered: a conventional load frame covering most of the cross-section and a reduced load frame covering only the main spar caps. The interaction between blade and load frame is implemented via contact formulations, which allows pretensioning in combination with a flap and a lead-lag load case. Strains on the outer surface of the blade are evaluated and compared to an artificial reference loading. The area of influence of the load application through the load frame, in which the strains deviate significantly due to clamping effects, mostly corresponds to the 0.75 times the chord length assumed for the certification [1]. The strains in the trailing edge are significantly less affected by the reduced load frame variant than by the conventional one, thus potentially making it possible to consider the trailing edge at the position of the load frame as being properly tested for certification purposes.


Introduction
A full-scale certification test of a new rotor blade type is required to validate design assumptions, i.e., to identify relevant failure modes for design details or identify manufacturing details prone to damage initiation.To this end, the design loads occurring during the lifetime of the turbine, i.e., complex loads resulting from the continuous aerodynamic, gravitational, and inertial forces, are simplified and converted into target loads.To achieve these target loads, test loads are introduced at several discrete positions along the blade span via load frames.These load frames locally constrain the deformation of the blade, which alters the stresses in the area around them.As a result, affected areas around the load frames, typically 0.5 to 0.75 times the local blade chord length in both directions, must be excluded from the certification and therefore must not contain any "critical" structural details as described in IEC 61400-23 [1].
Hence, the load frames limit the freedom of test design and introduce artificial stiffening of the blade during testing.However, the excluded areas around the load frames can be reduced if justified by simulation, for example, thereby increasing the test design freedom.This research therefore investigates the effect of the load frames on the structural behavior of the affected area.The load frames are often modeled in a simplified way using multi-point constraint (MPC) elements that can constrain the profile deformation at a radial position of the blade, as seen in [2].Chen used contact formulations for modeling load introduction to determine the cause of failure in a full-scale blade test [3].
In the present investigation, the blade section around the load frame, as well as the load frame itself, is modeled in detail using finite elements.The load transmission from the load frame to the blade is realized by means of contact formulations, which enables the analysis of the contact force distribution.The pretensioning process of the load frame is also considered in the simulation.

Methods/Approach
Two different load frame variants are investigated: (i) a state-of-the-art load frame encompassing the whole blade profile, and (ii) a reduced load frame which is only in contact with the main spar area and thus allows more deformation of the blade profile.For both variants the area of influence along the blade span in which the load frame has a significant influence on the strains in the blade structure is determined.A load distribution in which the loads are applied directly via MPC elements serves as a reference.

Load frame design
The load frames investigated are the frames used at IWES for commercial blade tests and consist of a frame made of steel beams fitted around a plywood inlay matching the outer shape of the blade.The two variants are shown in Fig. 1.A 10 mm thick layer of rubber is placed between the inlay and the blade surface to prevent the load frame from slipping and to distribute the load more homogeneously over the surface.The plywood inlay extends 300 mm along the blade.A preload for applying a clamping force is set according to the following procedure: First, the horizontal beams and the plywood inlays are attached to the blade and a pretension is applied via the threaded rods.The ratio of the pretension forces at the leading and trailing edges is set to about 1.8, so that the load is centered around the main spar cap.The pretension forces are kept the same for both load frame variants.The fasteners of the vertical beams are not yet firmly tightened, so that a relative movement between the two horizontal elements is possible and no unwanted constraint force occurs.The vertical beams are then fastened, so that the relative position of the inlays to each other is fixed.

Blade shell model
A section of a current generation commercial rotor blade, modeled in Ansys ® Academic Research Mechanical, Release 22.1, is considered for the investigation presented.The blade section consists of a main spar cap on the suction and pressure sides (SS and PS), connected via a centered web.Another set of spar caps is located in the sandwich panel toward the trailing edge, and also features a web.Shells and web are represented by 4-node SHELL181 shell elements, the trailing edge adhesive bond is modeled using 8-node SOLID185 3-D solid elements.The layup is defined using Ansys Composite PrePost (ACP) [4].The shells are meshed using predominantly rectangular elements with a side length of 50 mm.In the contact area of the load frame, the element length is reduced to 25 mm.

M b
Reference loading (MPC) Load clamp (s.Two static load cases are considered, which represent cut-outs from global bending moment distributions under simplified lead-lag and flap loading.Additionally, the loads were applied in the opposite directions to determine the strains at both extreme points of a fatigue load.Figure 2 (a) illustrates an overview of the model.The inboard end of the segment is constrained in all degrees of freedom.MPC elements are used to introduce a single force in the shear center of the tip-wise end, which connect to the full circumference of the shells.The shear center position is determined using the software tool BECAS [5].To offset the applied bending moment, an additional bending moment is applied directly to the circumference of the shells on the tip-wise end.Together with the force acting on the load frame, a bilinear bending moment distribution is formed which approximates the continuous curve of the target loads.
An artificial reference load case is generated to determine the area of influence around the load frame.In this case, the same load is introduced via MPC elements, which act directly on all nodes of the spar caps within the cross-section at the load frame position.A deformable MPC formulation is used to distribute the load over the geometry without creating a rigid connection between the nodes.This method creates a local disturbance of the strains in a limited area around the cross-section which must be considered when interpreting the overloads or underloads near this cross-section.It is assumed that the area of influence in the reference case is smaller than the one in the other load cases, since the load is only applied directly in a cross-section and without clamping of the blade.
To determine the clamping-induced strain deviations, the lengthwise normal strains in the outermost layer are evaluated along the blade length at different positions, as shown in Fig. 2 (b).Paths are defined in the center of the main SC, the TE SC and in the TE panel, both on the suction and pressure side of the blade.An additional path is placed at the LE of the cross-section.The strains are normalized to the strains from the reference load case, so that values above 1.0 represent a relative overloading of the structure and values below 1.0 a relative underloading.

Load frame modeling and contact formulation
Solid elements and beam elements are used for modeling the load frames.The load frame inlays and the rubber layer are modeled using 8-node SOLID185 solid elements.The vertical beams consist of 2-node BEAM188 elements.The horizontal beams are represented by rigid connections between the beam elements and the surfaces on the top and bottom of the inlays, respectively.The bolt forces are applied in a simplified way via the bolt pretension PRETS179 elements integrated in Ansys.The vertical beams are used to apply the forces in a first load step.The position of the beams is then locked throughout the next load steps, simulating the fixing of the vertical beams to the horizontal ones.In the last load step the loads on the blade are applied as described above.
The contacts between the blade and the inlays are implemented using 3-D surface-to-surface contact element pairs consisting of CONTA174 and TARGE170 element types.A small study was performed to identify suitable parameters for the contact formulation.Asymmetric contact behavior was chosen, with the target elements on the rubber surface of the load frame inlays, and contact elements on the blade shell surface.The contacts are modeled as frictional contacts with a friction coefficient of 0.4 using a pure penalty formulation with a normal stiffness factor of 1.

Results and Discussion
Figure 4 shows the pressure distribution on the interface surface for both load frame variants, with pretension and no additional load applied.The pressure is normalized to the largest occurring pressure value.The distribution is inhomogeneous with concentrations of pressure at the position of the webs and regions of low pressure in between.In the longitudinal direction of the blade, the pressure is evenly distributed since the geometry and the layup at this point of the blade change only slightly over the width of the load frame.For load frame variant (ii), IOP Publishing doi:10.1088/1757-899X/1293/1/0120145 the pressure distribution is similar to that of the corresponding area within variant (i), but of roughly twice the magnitude.

Figure 4. Normalized contact pressure distribution due to pretension
The applied flap and lead-lag loads are superimposed with the pressure resulting from the pretension.In Fig. 5 the pressures are evaluated on a path through the center of the load frames for the two different variants (i) and (ii) and both flap and lead-lag load cases.The flap loads result in a reduction of the contact pressure on one load frame side, and an increase on the other side while the lead-lag loads lead to a shift of the pressure maxima in the main SC area in the opposite direction of the applied force on both sides of the blade.

Figure 5. Contact pressure on load frames along center path
Figure 6 shows the strain distribution in the outermost layer of the SS blade shell along different paths from Fig. 1, normalized as described in subsection 2.2.The pretension of the load frame creates compressive strain in all areas covered by the plywood inlay and a tensile strain in the longitudinal direction of the blade.In the leading edge area of the cross-section the effect is reversed, with a tensile strain maximum in the area under contact.These loads are superimposed on the bending loads applied to the blade.
Depending on the path considered, two different strain patterns can be identified: Either an overload occurs in the clamping area under contact and an underload around it, or vice versa.The width of the region in which a significant overload or underload occurs also varies.
Under flap loading, an overload in the clamping area and an underload at around three quarters of the chord length around the load frame can be identified for both spar caps.The overload in the main SC is higher for load frame (ii), resulting from the higher load concentration due to the smaller contact area.A local overload can also be observed in the TE SC, although it is not covered by the load frame.Strains in the leading and trailing edges are not evaluated for the flap load case, as they are very small and therefore do not make a significant contribution to the fatigue exposure.
For the lead-lag case, a high overload in the main SC area with a relatively high underload in the surrounding area can be seen.For load frame (ii), this overload increases, while the affected area stays the same, spanning around three quarters of a chord length in both directions.At the TE SC as well as the TE panel, an underload can be observed for load frame (i).The strains for the reduced load frame only show a small overload in a small area along the blade.The strains at the LE of the blade profile show a strong underload for both load frames together with a small overload in the surrounding area spanning an area of about 1.2 chord lengths in both directions.

Figure 6. Relative strains evaluated in lengthwise direction
The strains plotted in Fig. 6 show the blade clamping has a clear influence on the loads in the area surrounding the load frames.The influence is mainly limited to the area of three quarters of a chord length around the cross-section where the load is applied, except for the LE profiles, where the area of influence is significantly wider.
Of particular interest are the strains in the trailing edge for the lead-lag loading.In the TE panel as well as at the TE SC, the strains are only slightly affected by load frame variant (ii).The amount of over-and underload is comparable to the amount prevailing at the position of 0.75 chord lengths for the other paths.
The strains were also evaluated from the load cases, where the flap and lead-lag loads are applied in the opposite direction representing the other extremum within a fatigue test cycle.The qualitative pattern of relative strain is similar, but with the opposite sign, so that overloads become underloads and vice versa.Only in the case of the path on the TE SC with load frame variant (ii), no sign change can be observed.This behavior could result from the loading via the MPC elements in the reference load case.The area affected by the load frames and the relative strain amplitudes are similar or smaller for the opposite load cases than for the load cases shown in Fig. 6.Since the relative strain deviates in the opposite direction between the two loading directions, the deviation caused by the clamping affects mostly the mean value of the strains and not the strain ranges.

Conclusions
The aim of this study was to identify constraining effects of load frame designs in rotor blade fatigue tests by nonlinear numerical simulation including contact formulation.The results demonstrate that with conventional designs, the pressure and thus the load transfer is not evenly distributed on the surface of the load frame.
By reducing the lateral length of the load frame, the over-and underload of the trailing edge can be reduced significantly for the lead-lag load case.It might be conceivable to place a load frame at a lengthwise position where a critical detail exists on the trailing edge that needs to be included in the certification, providing additional flexibility in the design of the test setups.
Further research needs to be undertaken on the required pretension forces in order to minimize the constraining effect.However, it is necessary to ensure that the load frames do not move under alternating loads.The preload force is kept the same for both load frame variants.This results in a higher contact pressure for the reduced load frame and may also result in a higher buckling load on the shear web.The higher load in the load application area and buckling of the shear web could be compensated by local reinforcement layers.This is in accordance with the certification guidelines; however, it might be necessary to prove that these layers do not affect the loading of the trailing edge.
In this work, overload is determined by lengthwise strain only.To obtain a deeper understanding of overloads, more complex static and fatigue failure criteria should be applied which take into account the complex stress state of the laminate at all positions.Likewise, the local failure of the blade due to the increased contact pressure of the load clamp could be investigated further, especially the buckling and failure of the webs and the failure of the adhesive bonds.

Figure 1 .
Figure 1.Load frame designs for a generic cross-section; (i) full load frame design; (ii) reduced load frame design

Fig. 3 Figure 2 .
Figure 2. (a) Blade model boundary conditions; (b) Definition of paths for strain and contact pressure evaluation (generic blade cross-section; paths on suction and pressure sides; Leading edge (LE), Main spar cap (main SC), Trailing edge spar cap (TE SC), Trailing edge panel (TE panel), Contact pressure: center path of load clamp)