Validation of a modelling methodology for wind turbine rotor blades based on a full scale blade test

Abstract. Detailed 3D finite element simulations are state of the art for structural analyses of wind turbine rotor blades. It is of utmost importance to validate the underlying modelling methodology in order to obtain reliable results. Validation of the global response can ideally be done by comparing simulations with full scale blade tests. However, there is a lack of test results for which the blade data are completely available. The aim of this paper is to validate one particular blade modelling methodology that is implemented in an in-house model 5 generator, and to provide respective test results to the public. A hybrid 3D shell/solid element model is created including the respective boundary conditions. The problem is solved via a commercially available finite element code. A full scale blade test is performed as the validation reference, for which all relevant data are available. Some data have been measured prior to or after the test in order to account for manufacturing deviations. The tests comprise classical bending tests in flap-wise and lead-lag direction as well as torsion tests. 10 For the validation of the modelling methodology, global blade characteristics from measurements and simulation are compared. These include the overall mass and centre of gravity as well as their distributions along the blade, deflections, strain levels, and natural frequencies and modes. Overall, good agreement is obtained, though some improvements might be required for the response in torsion. As a conclusion, the modelling strategy can be rated as validated.

use a detailed model at the shear web adhesive joint to analyse crack propagation in the bond line. Most of these locally detailed models are used within a global-local modelling approach like in Chen et al. (2014) to reduce the global model complexity while keeping a high level of detail at local spots. However, this paper focuses on the global elastic response of wind turbine blades, so there is no need for local sub-models.
Different FE modelling procedures can result in different deformation and stress solutions, though based on the same model parameters, see (Lekou et al., 2015). Hence, it is important to validate modelling strategies by comparing simulations with full blade tests, which is the aim of this paper. A quasi-static full scale blade test is performed, including not only bending tests in flap and lead-lag direction -as are usually executed in the context of blade certification (International Eletrotechnical Comission, 2014) -but also torsion tests. This allows for an exceptionally detailed and thorough validation. Unlike other blade tests reported in literature (?), (Chen et al., 2017), (Jensen et al., 2006), , , the aim of the tests in this work is not the validation of failure models. Hence, the blade is not loaded up to failure. The aim rather 70 is to measure the global blade behaviour expressed in terms of deflections, strains, mass distribution, and modal characteristics and to validate our own blade modelling technique. The blade under investigation is the SmartBlades DemoBlade (REFER-ENCE TO COME), a 20 m blade including pre-bend and pre-sweep towards the trailing edge. The blade is modelled with our in-house blade model creation tool MoCA (Model Creation and Analysis Tool for Wind Turbine Rotor Blades), taking into account some major manufacturing-related deviations. The test setup and the load introduction are approximated via a com-75 bination of suitable boundary conditions and multiple point constraints. The simulation results are thoroughly compared with the test measurements. Generally good agreement is observed, especially for the bending loads. However, some improvements may be required for accurately modelling the torsional behaviour of the blade.
The modelling strategy is addressed in section 2 and section 3. The test setup is described in section 4. The blade was cut into segments after the tests in order to accurately measure the mass distribution and the locations of the centres of gravity along 80 the blade. These measurements are also described in section 4. The simulation versus test comparison is reported in section 5, followed by the conclusions in section 6.

Model Creation Framework
A framework to automatically generate fully parameterized 3D FE models of wind turbine rotor blades from a set of parameters was developed at the Institute for Wind Energy Systems at Leibniz University Hannover. The purpose of this tool called MoCA 85 (Model Creation and Analysis Tool for Wind Turbine Rotor Blades) is to enable users to investigate and analyse different blade designs or design parameter variations in an efficient way, including structural details such as e. g. adhesive joints. The following section presents a brief description of the framework.
MoCA is based on a set of input parameters categorised in Geometry, Plybook, Structure, and Material. In general all parameters that describe a distribution along the blade are stored as splines over the blade's arc length, but even material 90 parameters may be varied over the blade arc if necessary by using a spline. The parameter set Geometry contains all information on the outer geometry of the blade, i. e. the airfoils used and their positions along the blade as well as the distributions of the relative thickness, chord length, twist angle, threading point location, prebend and presweep. The Structure set is associated with the structural description of the blade. This includes the specification of shear webs, adhesive joints and additional masses as well as cross-sectional division points that are mainly used to subdivide cross-sections into different regions of interest. 95 The Plybook parameters contain the stacking information of different composite layups used in the blade. The parameter set Material comprises all material properties assigned for the different materials. These can either be isotropic or anisotropic on the macroscopic scale. The user can also specify a composite material based on microscopic characteristics of the fibre and matrix constituents, which are then transformed to a laminate via the well-known rule of mixtures.
The flowchart in figure 1 depicts the structure of the finite element creation procedure implemented in MoCA on the basis 100 of the parameter sets described above. First, the blade segmentation, i. e. the discretization in span-wise direction, is defined.
For each blade segment edge, a cross-section of the blade is calculated by evaluating the Geometry data. Then a finite element discretization of the cross-sections is executed using the information of the Structure, Material, and Plybook parameter blocks.
At this stage, an interface to the BECAS (DTU Wind Energy) software can be utilized to calculate the full 6 × 6 stiffness and mass matrices of a beam model. However, since our aim is to create a 3D blade model, we continue with the finite 105 element discretization in span-wise direction utilising a hybrid shell element/solid element strategy. Therein, we use shell elements to model the composite laminates and solid elements for the adhesives. The 3D FE mesh includes the node-toelement connectivity and elemental material assignments. The boundary conditions are added and the FE model is translated to an input file for the finite element solver of choice, which in our case is ANSYS Mechanical (ANSYS Inc.). In the following, we describe in more detail the different steps of this overall procedure.   Figure 2 visualises the process of cross-section geometry calculation. After the blade segmentation, the Geometry data splines are evaluated for the particular blade arc positions of the segment edges. Based on the spline-based interpolation of the relative thickness t rel , an airfoil AF is linearly interpolated between the basic input airfoils with the next higher and lower relative thickness. In contrast to a global blade shape interpolation, the use of a blade independent airfoil interpolation enables the user to implement an own sub-function and replacing the former.  Until here, all transformations are performed in a 2D chord coordinate system with its final origin in the threading point. The cross-sections are now shifted to the correct 3D position, locating the 2D cross-sectional threading centre on the prebended and preswept global blade axis. By doing so, the 2D chord coordinate system is still parallel to the blade root plane. Hence, the 120 cross-sections are rotated by the slope angles of the prebend and presweep spline functions so that the they are perpendicular to the threading axis. These shifted and rotated cross-sections are the final cross-sectional shapes denoted by CS Shape .
According to figure 1, the next step is the 2D cross-sectional meshing, which is executed using the cross-sectional shapes CS Shape and the parameter sets Structure, Material, and Plybook. This process is presented in figure 3. As before, all data is evaluated for the particular arc positions at the blade segment edges. The division points are generated on the cross-sectional 125 shapes. They serve to subdivide the cross-sections into regions of different material layups. They are also used to define the positions of the shear webs. Then the shapes of the shear web/spar cap and/or trailing edge adhesive joints are computed. The computation of the blade's outer geometry and its structural topology is now finished. After inclusion of the Material and Plybook information, the FE discretization on 2D cross-section level can be conducted. This yields either a two-dimensional mesh with 4-noded plane elements for the BECAS (DTU Wind Energy) interface or a cross-sectional node map representing a 130 hybrid 2D mesh with 2-noded elements for the composite laminates and 4-noded elements for the adhesives.  The last step in the creation of a 3D finite element model is to connect the 2D cross-sectional models, see figure 1. The 2D line elements on the cross-sectional level yield 4-noded shell elements on 3D level after the 3D extension, and the 4-noded plane elements on cross-sectional level become 3D solid elements, respectively.
An additional module called TestRig is included in MoCA to model the boundary conditions similar to a full scale blade 135 test. Full clamping of the blade root represents the geometrical boundary conditions, i. e. all degrees of freedom are fixed at the blade root. Figure 4 shows the process of the TestRig module for the introduction of force-like boundary conditions. In the real blade test, a number of load frames introduces loads that approximate the target bending moment distribution (or torsional moment distribution, respectively). The TestRig module approximates the load frames by means of appropriate multiple point constraints MPC and additional masses. For each load frame, the position along the blade (arc position), the load frame width, 140 the centre of gravity (CoG) and the resulting mass are specified as well as the load and sensor points.
In the range where the load frame is located, MoCA searches all elements of the blade shell and defines 2D slave elements that share their nodes. An additional cross-section is created at the desired load frame position according to the procedure depicted in figure 2. In this additional cross-section, the position of the load introduction (load point), the sensor points, and the centre of gravity of the load frame are given in the blade coordinate system. These points are defined as master nodes.  MPCs are included that connect the degrees of freedom of the master nodes and the slave nodes by means of a rigid connection, i. e. there are no relative displacements between the master and the slave nodes. The additional mass of the load frame is applied to the CoG node, while the load is applied to the position where the load is introduced in the real test (load point). In this way, we model solid and quasi-rigid load frames and their effects on the blade response without adding detailed models of the load frames themselves, which is beneficial in the context of computational costs.

150
The 3D finite element model including the mesh and the boundary conditions is translated to an input file for the finite element solver of choice via an integrated interface.

Modelling of the Test Blade
This section briefly describes the blade under consideration, which is the SmartBlades-DemoBlade, a 20m long blade with prebend and presweep. It was designed and manufactured in the coordinated research projects Smart Blades (Teßmer et al.,155 2016) and SmartBlades2 (SmartBlades2, 2016-2020). The blade is abbreviated by DemoBlade in the following.
The DemoBlade was designed to investigate bend-twist coupling effects in wind turbine rotor blades. Therefore a presweep of 1 m towards the trailing edge at the tip is intended to introduce a torsional twist into the blade. The offset between the aerodynamic centres of the swept airfoils and the pitch axis introduces a torsional moment and thus a torsional deformation, i. e. a twist in the outer part of the blade. The twist reduces the angle of attack of the respective airfoils and hence the aerodynamic coefficients. In this way the aerodynamic loads can be reduced.
The full blade design of the DemoBlade as designed and the manufacturing documentation is available to the authors. In order to allow precise modelling of the DemoBlade as built laser scanning of the blade mould was carried out in order to determine the geometry deviations. The derived chord length and absolute thickness distributions for the DemoBlade as designed and as built can be found in Noever-Castelos et al. (2021). Though the manufacturing deviations in the outer geometry are 165 negligibly small, they will be considered in the modelling process.
After the full scale blade tests, the DemoBlade was cut into segments. The masses and the centres of gravity were determined for all blade segments. The respective procedure will be addressed later in this paper, see sections 4.4 and 5.5. Besides the weighing, the geometry was measured thoroughly in each cut cross-section in order to guarantee the correct positioning of the 170 shear webs in the FE model and to determine deviations from the design due to manufacturing errors. Especially the dimensions of the shear web/spar cap adhesive joints on the pressure side of the blade showed significant deviations to the blade design and had to be adjusted in the FE model. Figure 5 shows the cut at a radial position of 5.2 m. On the suction side we see a nice, thin, and over-laminated shear web/spar cap bonding. However, on the pressure side the shear web/spar cap adhesive joint (which was the blind bond) is much thicker than specified in the design. Moerover, there is a lack of adhesive in large portions of the blade, so that the shear web flanges were not covered entirely by adhesive material. Noever-Castelos et al.

Mass and Centre of Gravity
The first structural characterization considers the blade's mass and centre of gravity (CoG). An indoor crane equipped with load cells at every hook lifted two points on each root and tip transport structure as shown in Figure 6. As the blade remained 195 still and horizontally suspended the measurements and radial position of each suspension point was recorded. After weighing the transport structures, loading chains and shackles individually, the weight was subtracted from the total recorded load at the measurement devices to obtain the total blade mass. Additionally, the weight of the blade bolts was subtracted from the total mass.
The CoG is obtained by calculating the moment equilibrium with the measured loads with respect to a pivot point, in this 200 case the blade root centre. This procedure was performed for the z-direction (along the span) and y-direction (along the chord).
The mass and CoG of the FE model is calculated during every analysis by default and can be extracted directly from the ANSYS log-file.

Modal Analysis
The experimental modal characterization was carried out by the German Aerospace Center (DLR) for different boundary 205 conditions. The methodology is described briefly in the following. For details please refer to Gundlach and Govers (2019).
Free-free boundary conditions were applied after the blade manufacturing by means of elastic suspensions connected to lifting straps. The blade was excited using an impact hammer with soft tip at a total of 8 excitation points. Sensors distributed along the blade recorded the deformations, and the mode frequencies and shapes were extracted from the measurements.
The blade was then transported to Fraunhofer IWES and mounted on the test rig. The aim was a second modal character-210 ization with the boundary conditions of the full scale blade test. Electrodynamic long stroke shakers were employed for the excitation of the blade, and sensor outputs were evaluated for the calculation of the mode frequencies and shapes.
During the FE modal analysis, the boundary conditions are adapted to the different characterization tests. In the free-free configuration, no boundary conditions are applied at all, partially resulting in zero eigenvalues related to rigid body motions.
These are not considered in the validation process. For the test rig configuration, the blade root is fully clamped, i. e. all 6 215 degrees of freedom of the shell elements are fixed, for the sake of simplicity. Note that we neglect flexibilities of the bolts and the test rig in this way, which we have to keep in mind when evaluating the simulation results.

Static Bending and Torsion Test Configuration
The SmartBlades2 DemoBlade was loaded with extreme loads in 4 directions before and after the fatigue test. These four load cases correspond to maximum and minimum edge-wise loading (MXMAX and MXMIN) as well as maximum and minimum Each cable runs through pulleys that are mounted on the floor and redirect the forces from a horizontal to a vertical orientation.
By attaching the load cells to the load frames (load point), the actual load applied to the rotor blade is measured and friction as well as weight of the loading cables do not affect the measurements. The general test setup is shown in Figure 7. In the following, some general information is given that is valid for all test setups. The test block angle (cone angle) is 7.5°u pwards. The coordinate system referred to in this paper has its origin in the centre of the blade root. The y-axis is vertical, the z-axis points horizontally from the origin towards the blade tip (parallel to the floor, not to the pitch axis), and the x-axis follows from the right-hand rule (pointing left watching towards the tip). After turning the blade to the correct position and waiting for a static state, the signals of the load cells and the strain gauges are reset to zero. In the virtual test this is achieved 235 by activating gravity, extracting the deformed nodal coordinates and taking these as the undeformed and stress-free state for the load tests. Gravity is thus not applied in the further analysis and the nodal displacements are virtually reset to zero so that it is easier to postprocess the results. Preliminary verifications showed that the corresponding error is less than 0.5%.
In the tests, four steel load frames with wooden inlays that follow the blade shape at the respective span-wise positions are used to introduce the loads, see Haller and Noever-Castelos (2021). In the following, we refer to the load frames (LF) as LF1 The test setup is equipped with two different kinds of displacement measurements, an optical displacement measurement system and draw-wire-sensors (DWS). For the model validation in this paper, the DWS signals are considered. Using LINK11-Elements in ANSYS provides a simple and exact model of the draw-wires by defining the attachment points only. The deformation measured by the DWS is then modeled by the element-length variations of the link elements.

250
All necessary sensor positions (SP) and load introduction points (LP) on the load frames for the different test setups can be found in Haller and Noever-Castelos (2021). At each load frame position, either with or without installed load frame, two DWS are attached. One is connected to a point most to the front bottom corner, i. e. negative y-direction and one at the rear bottom corner, i. e. positive y-direction, of the load frames or blade shells in case no load frame is installed. These two DWS will be referred to as front and rear DWS in the following. At the blade tip, one DWS is attached referred to as Tip DWS. Note 255 that during several load cases, one or the other load frame is not applied due to the setup design, thus the respective DWS have to be attached directly to the blade shell.
The angle between the loading cable and the blade axis can be adjusted in the experiment by changing the pulley block location within a discrete set of fixing points on the floor. Prior to the test setup, the optimal position for each pulley was determined based on the predicted blade deformation and the desired loading cable angle. The applied loads should be aligned 2. Compensation of load cell and strain gauge measurements (reset to zero).
5. Ramp down loads, pausing at same load fractions as at ramp up. As the ceiling crane location is hard to record, but the load rope is perpendicular to the ground it was assumed that the location is 30m above (y-direction) the corresponding load point. The force facing downwards was applied onto the load frame corner 300 on the trailing edge side in order to introduce a torsional moment in that load frame location.

Blade Segment Measurement
After finishing the full blade tests, the blade was cut into 17 segments for further characterization. Figure 5 shows a cut surface of the 7 th segment at a span-wise position of r = 5.2 m. To determine the 3D centre of gravity (CoG), the segment was suspended at one point with a flexible rope, so that the CoG settled exactly underneath this point (like a pendulum). Hence, the vector in 305 direction of the suspension rope defines an axis on which the CoG must be located (CoG axis). This procedure was repeated with different suspension points at least 2 times. The CoG was then found in the intersection point of the different CoG axes.
The measurement setup can be seen in Figure 9 as well as a digital representation of the intersection of different CoG axes.
To measure the vectors and analyse the data an optical measurement system (photogrammetry) was used. Every segment was equipped with several coded and uncoded reflecting marks to obtain the shape of the segment, the suspension points and 310 a plummet that was used to get the CoG axes. All the point clouds were analysed in Autodesk Inventor and Siemens NX. All segments were aligned in CAD and the CoG was extracted for each segment with regard to the blade coordinate system. In this way we obtained the distribution of the segment CoGs along the blade.

Comparison of Experimental and Simulation Results
In this section, we compare the experimental results with the simulations. The observation scale will continuously decrease from a global to a more local scale. We start with the global blade characteristics such as eigenfrequencies, total mass, and total centre of gravity. These give a rough estimate of the modeling correctness. Then the blade deformations by means of bending and twist distributions during the static extreme load tests will be analysed. Finally the strain levels in two cross-sections during 320 the extreme load tests and the masses and centres of gravity of the cut blade segments are compared, which give a more detailed view on a local scale. Table 1 lists the total blade mass and the location of the centre of gravity in longitudinal (z) and chord direction (y) as well as the measurement uncertainties and the deviation of the numerical model. We see that the model from MoCA is 115.5 kg lighter 325 than the real blade, which corresponds to 6.44% relative difference related to the measurement. In contrast the measurement uncertainty is 45 kg. The mass difference is likely due to manufacturing deviations and/or additional masses (e.g. sensor wires and installations) that have not been considered in the numerical model. The location of the CoG matches perfectly in the The results of the modal analysis, both experimental and numerical, are listed in Table 2. The experimental results are taken from Gundlach and Govers (2019). The flapwise frequencies are in acceptable agreement with deviations of less than 8%. The largest deviation in flapwise modes is found for the 2 nd edgewise mode in the test rig configuration (7.94%, which corresponds to an absolute deviation of 0.54 Hz). The smallest deviation can be observed for the 1 st flapwise mode in the free-free configuration, which is 5.83% or 0.28 Hz, respectively. In edgewise direction, the approximation is even better. The 335 largest relative deviation is seen for the 1 st edgewise mode in the test rig configuration, which is 4.84% (or 0.15 Hz in absolute numbers). The 2 nd edgewise mode is only 0.83% (or 0.09 Hz in absolute numbers) smaller in the simulation compared to the experiment in the test rig configuration, which is an excellent agreement. The largest absolute deviation is present in the free-free configuration, where the 1 st edgewise mode is 0.36 Hz lower than the measured value. Anyways, the deviation of the edgewise modes is less than 5% in all cases, which is a very good agreement. The 1 st torsion mode is quite well approximated 340 in the free-free configuration, where the simulation is 5.62% lower than the experiment. However, in the test rig configuration the deviation is -11.76% (more than 2 Hz less compared to the test), which is relatively high. In general, the simulations agree better with the test results in the free-free configuration than in the test rig configuration. This is likely due to the rigid representation of the test rig and the connection bolts, as already mentioned in section 4.2. Especially in torsion, the flexibility of the test rig may not be negligible.

Static Bending Tests
The results of the static bending tests will be illustrated by means of deflection lines. For each test setup, two lines exist, one   For load case MXMIN, Figure 10 (b) illustrates the front DWS results. Except for LF1 the results are in very good agreement with a maximum deflection error of -1.6 % at LF2 at full load. However, the results in LF1 return maximum errors of 3.8 % at 40 % load, which decreases to 1.8 % at full load. Similar behaviour is found for the rear DWS ( Figure A1 (b)); excluding LF1 360 the maximum error is 1.7 % in LF3 and the tip during 40 % load.
The results of the front DWS during the maximum flap-wise setup (MYMAX, Figure 10 (c)) are in very good agreement, when excluding the LF1 data. The LF1 results tend to show the highest errors. This might probably be due to the smallest absolute deflection values, as a systematic sensor/measurement inaccuracy will have a higher impact on relative errors. Concerning the other load frames the maximum error is found to be -2.6 % for the LF4 DWS at full load, which corresponds to     Here again, by analysing the twist behaviour of the blade all load frames show significant twist differences and after estimating a correction, e.g. the accuracy of the LF1 front sensor would decrease to a deviation of -11 %, while that of the rear sensor increases to -10.4 %. This is the worst approximation of the simulation for the static extreme load bending setups. Anyways, the other load frames are in very good agreement.

395
Full scale blade tests in pure torsion are usually not included in certification processes according to (International Eletrotechnical Comission, 2014) and are thus rarely available. As described in section 4.3 the blade is twisted during three different setups successively at the load frames LF2, LF3 and LF4. The results of the tests and the simulations are plotted in Figure 11. The structural behaviour behind the actual loaded frame position to the tip will not be addressed in this paper and is highlighted as grey-coloured areas, as the areas loaded in torsion are located between the root and the respective load frame. Though the raw  Figure 11 (a) shows the first torsional test loaded at LF2. The absolute angle deviation from experiment to simulation are in between -0.06°and -0.15°but yields high relative deviation up to 30 % due to the small twist angles of -0.55°at LF1 and -1.72°at LF2 during 100 % load.   Moving the load application to LF3 (Figure 11 (b)) does not change the situation. At the load application position the 405 absolute error is high with up to -0.6°at a maximum twisting of -4.3°. All errors exceed -10 % dramatically. However, the experiment with torsional loading on LF4, see Figure 11 (c), shows reasonably good results for the twist angle at LF2 and LF3 with angle deviations of 3.7 % and 1.8 %, respectively. The results at LF4, where the load is applied and which shows the highest twist angle keeps high deviations of about 20 % for full load. Such high errors during torsional loading may base on the shell element with a node offset to the exterior surface used for this model. Pardo and Branner (2005) and especially Laird et al.

410
(2005) already stressed the high inaccuracy of shell elements with node offsets to predict the structural behaviour of hollow structures subjected to torsional loading. However, the twisting is generally overestimated throughout the three torsional tests, which is inline with the aforementioned references.

Local Strain Comparison
As stated in section 4.3 the highly instrumented cross-sections at r = 5 m and r = 8 m offer a more detailed view on the local 415 strain levels in the rotor blade. The strain results are used to compare the simulations with the tests and to verify that local effects are correctly reproduced. We have selected a few representative load cases in this section. The remaining load cases can be found in appendix B.
In Figure 12    The cross-wise strain shows partially good agreement with the experiments, except for the aforementioned characteristics 450 which are more dominant than in the bending tests. E. g. the peaks at the trailing edge is more pronounced. As for the longitudinal strain, the cross-wise strain shows a disagreement between simulation and experimental results, which is even stronger due to a shifted curvature in the plot. These can also be seen during the remaining two torsion tests. The MZLF4 load case in Figure C1 (d) is very similar to the MZLF3 load case, whereas the MZLF2 load case ( Figure C1 (c)) shows all of the stated characteristics in a more pronounced manner as the load introduction is shifted closer to the evaluated section at r = 5 m.

455
The next highly equipped cross-section is at r = 8 m. While the previous cross-section was located at maximum chord, this one is already in a region where geometric curvatures are smoother. For direct comparison the same three load cases were selected for this cross-section. As depicted in Figure 13  Comparing the results of the MYMAX test depicted in Figure 13 (b), the good agreement between the simulation and the test are evident. Even the stepped raise at the two spar caps (S = 0.3 and S = 0.67) exist in the experimental results. The strain 465 error range is approximately between ± 100 µm/m, which is less than for the other cross-section, while having slightly higher strain levels. This excellent agreement is also found in figure D1 (b) for the MYMIN load case.
However, the results from the torsional tests do not agree. As seen in figure D1 (c) the simulation results of the longitudinal strain during the MZLF3 test may follow some correct trend of the experiments, but has significant variations. The same applies to the cross-wise strains. Though the strain errors are in the same range as the bending test results, compared to the absolute 470 strain levels these have the same magnitude as the error. The remaining torsional test results ( Figure D1 (c) and (d)) show similar problems.

Segment mass and CoG comparison
In this subsection, we compare the experimental mass and CoG measurement of each segment with the respective simulation results. Table 3 contains the segment numbers, the segment locations along the blade defined by the span-wise positions of the 475 left and the right cutting sections r 1 and r 2 , respectively, and the differences of the segment masses and the CoG locations (in absolute and relative numbers). The relative difference of the mass is related to the measured segment mass and the CoG positions are with respect to the corresponding geometrical mid cross-sectional dimensions, i. e. absolute thickness (X), chord length (Y) and radial segment length(Z). It was not possible to measure segment 15. The mass differs from -4.8 % to -9.9 % except for segment 1,14, and 17, 480 where the mass was overestimated. Unfortunately it was not possible to calculate an overall blade mass as one segment result was missing. Concerning the CoG differences, the coordinate in cross-section thickness direction (X) varied up to -15 % but was most of the time predicted closer to the suction side. The CoG location in chord direction (Y) agreed very well with the measurement, except for segment 16, the variation were below ±4 %. The radial locations match well for most of the segments (≤ 6 %). However, the sections 10, 11, 12, 14, and 16 resulted in higher variations, predicting the CoG position closer to the 485 tip by more than 10 % of the segment length.

Conclusions
The aim of this paper was the validation of a parametrization and modelling methodology for wind turbine rotor blades. This methodology was implemented in the in-house 3D finite element model generator MoCA (Model creation and analysis tool), which creates hybrid shell/solid finite element models.

490
Full-scale blade tests were performed on the SmartBlades DemoBlade as an experimental reference. The blade has a length of 20 m and is designed with pre-bend and pre-sweep. The following magnitudes were determined experimentally: The total mass and the centre of gravity of the full blade, the mass and centre of gravity distributions along the blade by weighing of blade segments, the natural frequencies in a free-free and a clamped cantilever configuration, the deflection curves along the blade for both flap-wise and edge-wise bending as well as torsion, and the strains in the cross-sectional and longitudinal direction 495 close to the maximum chord position. The governing parameters such as geometry, material layup, manufacturing deviations, additional sensor and load frame masses were extracted from the blade and test documentations. These were fed into MoCA.
Finite element models for all test setups were created and the simulations were executed in the commercially available finite element code ANSYS. Then, the simulations were compared with the experimental results.
The mass and centre of gravity of the full blade compared very well (error of -6%). The masses and centres of gravity of the 500 blade segments, i. e. the mass and centre of gravity distributions along the blade, were also in good agreement (error of 5-10%).
Modal analysis concluded for th natural frequencies with free-free boundary conditions also well (error <6%) matching results, those for the clamped cantilever configuration matched reasonably well (error <8% for bending, 11.7% for torsion).
The deflections for bending in edge-wise direction was in excellent agreement (error <4%). While the deflection curve for bending in flap-wise direction showed a comparably large deviation of 13% at the root, which decreased substantially towards 505 the tip (error at the tip <4%). A reason for that was an elastic twist during the test that was not replicated in the simulations.
During torsion, the authors identified quite large deviations in the elastic twist distributions along the blade, because shell models cannot properly replicate torsional behaviour, as is also reported in literature.