Validation of a 20 m Wind Turbine Blade Model

Copyright: c © 2021 by the authors. Licensee MDPI, Basel, Switzerland. This article is an open access article distributed under the terms and conditions of the Creative Commons Attribution (CC BY) license (https:// creativecommons.org/licenses/by/ 4.0/). 1 Institute of Composite Structures and Adaptive Systems, Lilienthalplatz 7, 38108 Braunschweig, Germany; rakesh.ravi@dlr.de (R.R.); falk.heinecke@dlr.de (F.H.) 2 Nordex Energy SE & Co. KG, Langenhorner Chaussee 600, 22419 Hamburg, Germany; jrieke@nordex-online.com * Correspondence: christian.willberg@dlr.de


Introduction
The trend in designing larger and larger horizontal axis wind turbines (HAWTs) seems to be still unbroken if one looks into the current developments and announcements in the offshore and onshore markets [1] and at the research [2]. This cost of energy-driven development comes with different challenges, as described in [3]-in particular, the precise prediction of the aeroelastic behaviour and the overall dynamics of a turbine equipped with large and very flexible wind turbine blades.
In contrast to current designs, three-bladed HAWTs in the early days typically had small blade deflections due to relatively high blade rigidity and small rotor diameters. Thus non-linear effects and complex structural couplings could be ignored-even the torsional deflection was usually neglected. Considering current medium large wind turbine blades of more than 60 m in length, where, e.g., geometrical (sweep) or structural bend-twist coupling is applied, this simplification is not valid. A precise prediction of the wind turbine blade behaviour is necessary for a save turbine operation. In consequence, the structural mechanical models that are used in the design process have to be validated for their capabilities to predict static and dynamic responses as well as the strength of the structure in all its details.
For complex models and large structures, such validation experiments are very expensive. The SmartBlades and SmartBlades 2 projects (both funded by the German Federal The static tests were performed for the first produced 20 m rotor blade. All the tests were conducted in the 90 m test hall of Fraunhofer IWES in Bremerhaven, Germany from 23 January to 6 February 2018, and the test description and the raw data are given in [8]. Figure 1 shows the experimental setup. The description of the test is based on the technical report of Bernd Haller from Fraunhofer IWES [8]. The rotor blade coordinate system is defined in Figure 2 and corresponds to the IEC 61400-5:2020 [9] B-system. The origin was placed in the centre of the cylindrical part of the blade root on the flange. The z-axis pointed to the rotor blade tip along the cylinder axis, the y-axis pointed to the trailing edge at 0 • pitch angle and the x-axis was obtained from e x = e y × e z in the illustrated configuration. (a) Test bench.
As shown in Figure 1a, the rotor blade was attached to a metal frame at the root (left side of the figure). This metal frame, now called the root jig, had an angle of 7.5 • of the flange plate to the vertical orientation ( Figure 3b). The blade z-axis was inclined by this angle to the ground. In numerical pre-studies, this angle was included, but no substantial effect on the numerical results (displacements and mechanical strains) was observed. For the static tests, the external loads were introduced by utilising load frames; see Figure 1b and Appendix A for size and geometry. As shown in Figure 1a, the load frames were connected by wires to hydraulic cylinders which applied the loads. Load cell sensors were used to measure the applied load at load frame, and draw wire displacement sensors (DWS) were used to measure the vertical displacements at the load frames and at the tip. Two DWS measurement positions for each load frame existed. They are defined as leading and trailing edge positions for all load cases. For the two Mx load cases, the leading edge position refers to the left-hand side position of the load frame, and the trailing edge position refers to the right-hand side. The views are given in Figure 4a,b. For all experiments two DWS were used. For the flapwise bending, one was placed on the leading edge and one at the trailing edge. For the edgewise bending, the DWS were placed on the suction side and at the pressure side. In addition to the DWS, an optical displacement sensor was used to measure the three dimensional deformation of the rotor blade. The twisting of the rotor blade root and the rotation of the load frames were measured using angle measurement sensors. The root jig is shown in Figure 3. The analysis of the stiffness has shown that it is softer in x direction. The static tests are not affected by it, but the modal analysis of the clamped rotor blade is [10].
The local structural deformation of the rotor blade was measured with strain gauges at various locations along the span, as shown in Figure 2. For the span positions L = 5000 mm and L = 8000 mm, the blade sections are strongly instrumented to be able to obtain the deformation of the cross-sections itself.  The relative measurement error of the strain gauges was ±2%. The absolute error was determined analysing the zero load time signals. It was ≈±0.5-2 µm/m. To guarantee the quality of the measurements, climate sensors were used to measure the temperature and humidity inside the test hall at regular intervals.
The rotor blade was subjected to flapwise and edgewise bending tests, and furthermore, to three torsion tests. The four bending tests were named: The three torsion test were named: • LC1: Torsional stiffness test at load frame 2. For the load case Mymin (pressure side under compression), the rotor blade was rotated to an angle of 270 • compared to the Mxmax orientation with the suction side facing upwards; cf. Figure 4d. The rotor blade was loaded on the outer three load frames for both these load cases. For this load case, the rotor blade was loaded at the load frames 2, 3 and 4.
Quasi static loading was achieved by slowly increasing the loads in four load steps (i.e., 40%, 60%, 80% and 100%). The 100% loads for all the load cases used for validation are shown in Table 1. The rotor blade was oriented with the pressure side upwards for all three load scenarios (cf. Figure 4b). Only one load frame was loaded with a pair of parallel forces pulling vertically up and down, respectively. The upper attachment was mounted in the shear centre and the lower attachment at the end of the frame near the trailing edge.

•
For test LC1, due to a mistake, the upper attachment was shifted 158 mm toward the leading edge.

•
For test LC1, the load frame 1 was dismounted; for test LC2, the load frames 1 and 2 were dismounted; and for test LC3, the load frames 1, 2 and 3 were dismounted to reduce stiffening effects. The loading and the measurement points for the three load cases LC1-LC3 at load frames 2, 3 and 4 are shown in Figure A1a-c, respectively. The test scenarios with the applied loads are shown in Table 2. To determine the twist angle, the draw wire displacement sensors and angle sensors were used. The distances between the draw wire displacement sensors are given in Table 3. By assuming that the deformations of the load frames themselves are negligible, these distances and the separate displacements can be used to find the twist angles α: (1)

Experimental Setup for Modal Tests
The setup for the modal test is given in [11]. The measurements were performed in the clamped configuration described in Section 2.1 and in a free-free configuration. The free-free configuration was realised using long rubber belts with a low eigenfrequency, which did not influence the eigenfrequencies of the rotor blade.

Model
The reference model was based on the given design of the 20 m Smartblades 2 rotor blade. The model's creation started with the aerodynamic hull. The spar, spar caps and adhesive bonds were modelled in the finite element framework Abaqus. All sections, the model segments and material definitions were created in Abaqus. The final finite element mesh was then translated to the input data format for the finite element tools Ansys and Nastran. In the following sections the model is explained in detail.

Material and Layup
The materials and their properties are given in Table 4 [12]. Three material classes are used to build the wind turbine blade. Glass fibre reinforced plastics (GFRP), foam material for sandwich stiffened regions and an adhesive material to glue the parts of the rotor blade. The foam material consider the effect of matrix infusion which leads to larger density. As an additional material, the pseudo-material was added. It can be used to select specific regions within the finite element model. The names or the material numbers of Abaqus, Ansys and Nastran are given in Table 5.  The rotor blade model (cf. Figure 5) was created within the finite element software Abaqus by meshing the aerodynamic surface and the shear web plane. The thin walled structures were modelled with quadratic serendipity finite shell elements (STRI65, S8R). For the thick adhesive joints, quadratic serendipity finite solid elements (C3D20R) were used. For Ansys and Nastran the corresponding elements were used. For all models, modal analysis simulations were performed. As expected, they had the same results, and all models can be used equally for validation purposes. In further analysis, due to the expensive license of Abaqus, this program was only used for the modal analysis. The static and the mass distribution analyses were done using Ansys. The layups are defined as stacking sequences. The material formulation within the elements utilises the classical lamination theory [13] with all its assumptions. The stacking directions for the suction side shell, pressure side shell and the spar caps are given in Figure 6. As a consequence, the middle plane of the shell had an offset to shell element nodes. Homogenised material properties for the individual layers were used, meaning fibres and matrix were not separate materials. A transversal isotropic material symmetry was assumed for the single glass fibre layers. The balsa woods, used as a sandwich core, were part of the stacking sequence and had isotropic material symmetry. The biaxial and triaxial layups were defined as one thick layer with homogenised parameters. All material properties can be found in detail in Table 4. The material numbers or names used in the different finite element models are given in Table 5. For better usability, several pseudo-layers/materials were defined to allow the selection of sets and components; i.e., multiple pseudo-materials existed for some components, e.g., root and suction side. The pseudo-material numbers and corresponding components are given in Table A3.

Differences from the Design
To reduce the complexity of the model, several assumptions and adaptations were used within the finite element model. In this section, these differences from the design are illustrated.
In contrast to Figure 6, the core material was not chamfered in the trailing edge area (Figure 7), where the direct bond of suction and pressure sides was present. In consequence, this led to a higher local bending stiffness at the trailing edge. E.g., the analysis of trailing edged buckling load as described by [14] will be overestimated. Additionally, local strain measurements at the trailing edge will be affected and may result in larger deviations. On a global scale or sufficiently far from the trailing edge, the effects can be expected to be small, because the additional tensile stiffness due to the core material is very small. In the finite element model, all adhesive joints were thicker compared to the designed rotor blade. The adhesive was modelled with three-dimensional volume elements between the reference planes of the shell elements. The reference planes were the aerodynamic shape of the rotor blade; cf. Figure 6.
As a result, the thickness of all adhesive joints was increased by the thickness of the local design layup. This is illustrated in Figure 8a. The thin blue line is the reference plane. If the thickness shell elements are included (cf. Figure 8b) an overlap occurs. The thicker adhesives will change the mass distribution of the rotor blade and have an impact on its stiffness. Both effects are assumed to be small. Further, the adhesive joint at the leading edge has not been modelled. It is very thin and was assumed to be negligible.
Due to the finite shell element formulation, there was overlap between the shell elements and volume elements, and between shell elements at the trailing edge illustrated in a cross-section in Figure 8b.
For manufacturing reasons the root was built separately. In a later process the root was joined to the rest of the rotor blade. This skew adhesive joint has not been modelled. Further, neither bolts for the rotor blade connection nor the T-bolt connection were included in the FE model in detail.
Another simplification was made at the tip of the rotor blade. The lighting protection aluminium tip was not modelled. The tip does not effect static measurements and due to the small weight (Section 4.2) could only have a minor impact on the modal results. Due to its shape, the meshing of the region is challenging, and it adds more elements without adding additional information.

Boundary Conditions
The root jig consisted of very thick steel frames. It was shown that the stiffness of the frame was very high in z direction perpendicular to the ground. Parallel to the ground it was softer. This is relevant for the eigenfrequency tests but not for the static tests. A clamped boundary condition has been assumed. For all root nodes all translations and rotations were set to zero (fixed in all six DOF).

Load Introduction
The loads in the experiment were introduced with load frames for the different load cases, which are listed in Table 1. The load frames were simplified for the finite element model. They were realised as pilot nodes connected with infinite stiff connections to the outer shell of the rotor blade model. The mass distribution of the frame was not considered and did not influence the experimental results. The deformation sensors and strain gauges were set to zero in the state, where all weights were already applied.
The rotor blade was connected to the root jig in an angle of 7.5 • in relation to the ground. This angle influences the load introduction, because the load vector is perpendicular to the ground. This means for the torsion load cases that torsional moment is not parallel to the rotor blade z-axis (i.e., the pitch axis). However, the angle between the load vector and the rotor blade z-axis was smaller than 7.5 • due to the weight of the rotor blade and the load frames. The simulation of one bending and one torsion case show that the error in displacements is lower than 0.1% if the angle is not taken into account. Therefore, the load vector has not been adapted for all other load cases.

Scenarios and Variations
All experimental scenarios are given in Table 1 for the bending load cases and in Table 2 for torsion load cases. All these experiments were modelled in Ansys Mechanical.

Solver
All static finite element analyses were performed with a linear static solver which does not take large deformations, large rotations or the effect of profile deformation due to the rotor blade bending into account.

Bending-Displacements
For all four bending load scenarios the displacements at four specific positions at the leading and trailing edge were measured. The positions were L = 6700, 9700, 14,000 and 17,700 mm. The measurements were done at the load frame. To compare the results, the measured displacements were mapped to the surface using a linear function. For the two Mx load cases the leading edge position refers to the left-hand side position of the load frame and the trailing edge position refers to the right-hand side. The views are given in Figure 4a,b. A comparison between the simulation and the experiment at each position for the four bending load cases is shown in Figure 9a-d. All numerical results are in good agreement with the corresponding experimental data. The biggest difference was found in load case Mymax. A significantly more pronounced bending-torsion coupling was measured for this load case compared to simulation. This behaviour cannot really be explained, because the Mymin load case did not show such behaviour. The blade was rotated by 180 • in both load cases (Mymin and Mymax) and the amplitudes were in the same order of magnitude, but the magnitude of the bending-torsion coupling was different. The simulation did not show this behaviour. For three positions (1600, 8000 and 15,000 mm) the spar caps were instrumented with additional strain gauge rosettes. The components of a strain gauge rosette ε a , ε b and ε c illustrated in Figure 10 had to be transformed to the strain components in local laminate coordinates (L-longitudinal in 0 • direction; T-transversal in 90 • direction) ε LL , ε TT and ε LT [15]. For α = 45 • , β = 45 • and the engineering shear strain defined as γ LT The sensors used for ε a , ε b and ε c are given in Table A2. These measurements are not considered for validation because of poor instrumentation.

Mxmax Results
The results for the load case Mxmax (cf. Figure 4a) are shown in Appendix D.1. Due to the orientation of the rotor blade and the loading in edgewise direction, it can be expected that the mechanical strains at leading and trailing edge are higher compared to the spar cap strains. Both the simulation and the experiment fulfilled that expectation; cf. Figure A2 for the mechanical strains at the spar caps and Figures A3-A12 for the mechanical strains of the leading and trailing edges.
The absolute deviations were small for most positions. As expected, the relative deviations were higher in areas with small mechanical strains than in areas with larger mechanical strains. This behaviour can be seen very well when comparing the mechanical strains of the suction side spar cap with the pressure side spar cap. The deviations of the strains were less than 20 µm m. These are in the range of absolute error values for strain gauges. Therefore, the deviations are relatively high. The mechanical strains of the suction side match well between simulations and experiments. In the case of the pressure side, there are bigger differences close to the root.
The comparison of the mechanical strains between the experimental and numerical results of the heavily instrumented cross-sections at L = 5000 and L = 8000 mm are shown in Figures A5-A8. Both the simulated ε LL (cf. Figure A5a) and ε TT (cf. Figure A6a) strain distributions at the suction side are in very good agreement with the experimental results at L = 5000 mm. For the results of ε LL at the pressure side (cf. Figure A5b), the mechanical strain distribution between 0 and 800 mm from the leading edge differs between the experiments and the simulations. It is not clear where this non-linearity came from, because the suction side did not show such behaviour. For ε TT at the pressure side, this distribution error did not occur. However, the strain between 1800 and 2200 mm was underestimated by the simulation (cf. Figure A6b).
For L = 8000 mm the simulated ε TT suction side (cf. Figure A7a) and pressure side (cf. Figure A7b) strain distribution values are in very good agreement with the experiment. The simulated ε TT strains for the suction side match also with experiments (cf. Figure A8). For the pressure side the experiment shows a weak non-linear strain distribution, and the strain distribution of the numerical results is nearly linear (cf. Figure A8b).
All measured values ε TT for the cross-sections at L = 1600, 2700, 11,000, 13,000, 15,000 and 17,000 mm are in good agreement with the simulations. In these cross-sections only the leading and trailing edges were instrumented with strain gauges. Therefore, the cross-sectional circumferential strain distribution is unknown.

Discussion of Mxmin, Mymax and Mymin Results in Relation to Mxmax
The results for the other three load cases are only discussed briefly. The overall behaviour is equal to the Mxmax load case. The results for Mxmin (cf. Figure 4b) are shown in Appendix D.2. As in the Mxmax load case, the Mxmin simulation and the experiment showed the highest strains at leading and trailing edges, as expected; cf. Figure  For the three load cases, Mxmin, Mymax and Mymin, the absolute deviations were small for most sensor positions. As expected, the relative deviations were higher in areas with small strains than in areas with larger strains. This behaviour can be seen very clearly when comparing the suction side spar cap strains with the pressure side spar cap strain. These are the absolute values for the pressure side. Therefore, the deviations are relatively high. The suction side course matches well in the simulations and experiments. In the case of the pressure side, there are bigger differences close to the root. Besides some exceptions, all measured values ε LL and ε TT are in good agreement with the simulations.

Torsion-Displacements
The comparisons of the torsion stiffness measurement (see Section 2.1.2) results and the numerical results are illustrated in Figure 11a-d. Three scenarios (LC1, LC2 and LC3) were measured and simulated. The load vectors for the load cases are given in Table 2. The scenario LC1 is in good agreement for all measurement positions. In this scenario, the error is dominated by the load introduction point L = 9700 mm. As this error is small, the outer radial cross-section errors are small as well.
For scenario LC2 the error is bigger compared to LC1 for the cross-sections L = 14,000 and L = 17,700 mm. The numerical model is softer compared to the tested rotor blade, because the angle of rotation (inclination of the curve) is larger.
For scenario LC3 the largest error occurred at L = 17,700 mm, where the load was introduced. The conclusion is that the rotor blade model was modelled too flexibly at the outer third of the rotor blade. The torsion angles at various positions are given in Table 6. It must be noted that for the LC1 load case all angles determined at positions L > 9700 mm have the same value. The reason is that no additional load was applied further away and no additional torsion deformation was induced.

Torsion-Strains
The strain distributions for the intensively instrumented cross-sections L = 5000 and L = 8000 mm are given in Appendix D.6 for all three load cases LC1LC3. Most of the numerical results are not in good agreement with the experimental data. Generally speaking, most of the strains were lower than 100 µm/m. As in the bending cases, these small strains were more sensitive against minor orientation and placement errors. For larger strains above 100 µm/m, the curves are in better agreement and fit best for Figures A54b and A56a

Validation of the Mass Distribution
The mass of the first produced rotor blade (blade 1) was measured before testing at the test bench. The masses of the other three rotor blades (blade 2, 3 and 4) were measured after the finish. The reference finite element model did not include specific parts, such as i Varnishing (14 kg The mass of rotor blade 1 has to be reduced by 119.5 kg, because the rotor blade was not finished (excluding points i, iv and v). The masses of rotor blades 2-4 were measured after the finish, and their mass has to be reduced by 135.7 kg to be comparable with the finite element model. The mass and the centre of mass of the reference rotor blade in comparison to the measured four wind turbine blades are given in Table 7. Blade 1 was measured before mounting to the test bench at test facility (no finish). Blades 2-4 were measured at the finisher company. The extra masses were subtracted from the measured values, because they were not included in the reference model. The masses of the model and the built rotor blades had differences of 4.1% for blade 1 and 2.8% for the blades 2-4's average mass.
The centre of mass measurement of the finite element model and the measurements are in the same order. The effects of the bolts on the centre of mass were tested by including them. It can be seen that the centre of mass was in good agreement with rotor blade 1 with an error of 2.7% without the bolts and 1.4% with bolts. For the finished rotor blades 2-3, the error was 11.4% without the bolts and 6.8% with bolts, respectively.

Section-Wise Centre of Mass
Blade 1 was cut into sections, as shown in Figure 12. For each section the mass and the centre of mass was measured.  The comparison between the model and the measured results is given in Table 8. The coordinates are given in global rotor blade coordinates. The results of the numerical model and the measurements are in agreement. The main discrepancy was present due to manu-facturing problems at rotor blade 1. As shown in Figure 12a the adhesive joint between the spar cap and the shear web flange was not filled. Therefore, the mass distributions between the numerical model and the real rotor blade were different. It must be noted that the section 16.5-17.5 m was not measured because the part was missing.   As linear eigenvalue solver the Lanczos method [16] was used to perform all modal analyses.

Eigendynamics
Two configurations were analysed and measured. A clamped configuration and a freefree configuration. In this paper the eigenmodes were not compared with a Modal Assurance Criterion (MAC) criterion [17]. The data of the eigenfrequencies and eigenmodes are taken from [11], where more detailed analysis of the modes and the experimental setup can be found.
The first 8 eigenfrequencies of the clamped rotor blade are given in Table 9. The results of the reference model are compared to the design model [18] (R/D) and the experimental data (R/E). The comparison between the simpler design model lead to errors lower 10% except the torsion mode. As the frequency error was too large for the analysis some of the masses excluded for the mass comparison were added to the model; see Section 4.2. This includes the torsion sensor (iii), wind turbine blade tip (iv), trimming mass in balancing chamber (v) and the reflector system (vii). The bolts does not influence the clamped rotor blade and were not in place for the free-free experiment. The varnishing was not done for the actual rotor blade tested in the test bench. The mass of the lightning protection system was excluded. The errors between the reference model and experiment without any model updating for all bending eigenmodes is lower than 6%. However with an error greater 5 % it would not be conform to certification requirements. For the first flapwise bending mode the difference can be found due to lower tip masses in the finite element model compared to the real rotor blade; cf. Table 8. This leads to a reduction in the eigenfrequencies. The first torsion mode has a difference of −7.6% and it is assumed that the stiffness of the root section is underestimated by the finite element model. The eigenmodes are shown in Figure 13. For the free-free configuration the first 6 non-rigid body eigenfrequencies are shown in Table 10. Analysis results of the design model do not exist and are therefore not compared. The eigenmodes are shown in Figure 14. Except for the second torsion mode all errors are lower than 10%. It must be noted that the first torsion mode has an error of 0.3%. This is an indication that the root area has been modelled with insufficient stiffness or the mass distribution is incorrect as stated for the clamped configuration [10]. Comparing both analysis it can be seen, that the torsion frequencies differ stronger for the clamped configuration. The reason might be in a stiffer root section of the real rotor blade. This leads for the clamped configuration to higher frequencies compared to the free-free configuration. The mass distribution for the torsion modes seems to be okay. Differences of the center of gravity between the finite element model and the real rotor blade would not have a massive impact, because the pre bend over compensate this effect.

Discussion
The general findings of the study will be discussed below. For the static loads, it can be seen that the global deformations are in good agreement between the simulation and the experiment. This applies to all bending and torsion load cases. For the torsional loads, the largest deviation is in the outer area of the rotor blade. There are two main reasons. First, the introduction of a pure torsional load is difficult. Second, minor deviations due to manufacturing have a culmunative effect on the errors in the direction of the blade tip.
The error between the simulation and experiment of the mechanical strains for all load cases are usually larger compared to the errors in the displacements. The reason for this can be found in the positioning of the strain gauges and in manufacturing deviations. The position of the strain gauges refers to a local coordinate system measured on the blade. The origin is the nose of the rotor blade for the instrumented profile. The finite element model refers to the aerodynamic shape. The real manufactured blade without finish does not correspond to this everywhere. This means that the distance from the nose to a specific sensor can differ in the range of centimeters. Thus, there are certain differences between real positioning and model-side positioning, because a pre finished blade was tested.
As stated manufacturing errors influence the strain measurements as well. The fibre placement usually does not correspond exactly to the orientation assumed in the finite element model. This can lead to errors in the strain measurement due to the locally different stiffness.
The argumentation on the effects of production-related deviations is supported by the mass distribution. There, it can be seen from the measurement that there are deviations in the centers of gravity. It is to be expected that these are in the same order of magnitude for the stiffnesses. This, of course, affects the inherent dynamics of the rotor blade. There, especially the lower natural frequencies are strongly subjected to errors and would fail the certification. To improve the results, the manufacturing deviations would have to be taken into account in the FEM model. Depending on the available database, this can be achieved by using measurement data from the real rotor blade or by automatic model updating.
Two very important issues were identified during the validation process • Experimental and computational engineers do not speak exactly the same language. Therefore, a close communication is key, because a lot of information which is not important for the experimental engineer is very important for the computational engineer, vice versa. • A good documentation of the experiment with many fotos are very important. This holds especially for seemingly trivial information.

Conclusions
The paper presents a finite element model of a 20 m wind turbine blade and its validation. The finite element model was created using manufacturing specifications. The validation was based on mass distribution data and static and modal test data. The static test data were composed of displacement and strain measurements. The validation indi-cated that the difference between simulated and measured displacements for all bending tests was less than 10 %. For the torsion tests, the resulting rotor blade rotations were in good agreement for most of the tests. The largest differences were seen in the third torsion test, where the load was applied in the outer area.
However, except for the spar caps, simulated strains were in good agreement with the measured strains. The reason for that was a faulty instrumentation of the experimental setup. The natural frequencies matched in some cases with an error below 5 % and would conform to certification requirements. In other cases (first flapwise mode; first torsion mode) the error was above that, which does not work with the certification requirements. Further investigation of, e.g., clamping and mass distribution impacts, has to be done. The mass distribution also matches the experimental data. The finite element model was translated into Abaqus, Ansys and Nastran, and is provided as a reference model. The dataset includes also the measurement data used, and python scripts as easy-access solutions for other researchers [7].

Data Availability Statement:
The reference finite element models, the simulation data and adapted measurement data and Python scripts for evaluation can be found here [7].

Acknowledgments:
The authors like to acknowledge the members of the Research Alliance Wind Energy (https://www.forschungsverbund-windenergie.de/de/ (accessed on 22 April 2021)) for the project organisation and discussion. The work in this paper was funded by the German Federal Ministry for Economic Affairs and Energy (Funding number: 0324032)).

Conflicts of Interest:
The authors declare no conflict of interest.

Appendix D. Strain Plots
The relative measurement error of the strain gauges was ±2% and the absolute error was ≈±0.5-2 µm/m. The strain gauge sensor names are given in Table A1 and for the shear strain sensors in Table A2.                               Figure A65. Strain comparison ε TT at radial position R = 8000 mm for torsion load case LC_3.