University of Stuttgart
The assembly of the Ampair 600 wind turbine consists of several substructures with very different material properties. Since the parameters of these materials are unknown, model updating is applied to the substructures to obtain validated finite element models. Based on experimentally determined modal parameters, the finite element models are adapted to achieve acceptable vibration behaviour. Therefore, an objective function consisting of the deviation of the eigenfrequencies and eigenvectors is used to determine Young's modulus, density and Poisson's ratio of each material.
Introduction
Dynamic Substructuring methods offer the possibility to model high order finite element models in an efficient way [1]. A separated representation of the dynamics of the participated substructures enables the application of model reduction methods like the Craig-Bampton method and a later assembly of the different parts by Component Mode Synthesis (CMS). Therefore, the degrees of freedom (DoF) can be reduced drastically. Additionally, a validation of the components can be done individually in a more efficient way. In order to get validated finite element models, model updating methods [2] can be applied to identify material parameters. For example measured modal parameters can be provided to an optimization such that the deviation of the simulation model can be minimized automatically. Within this contribution such a model updating procedure is presented.
Experimental Results
In order to have reference data for the model updating of the finite element model, three Experimental Modal Analysis (EMA) are performed to identify the modal parameters [3]. All three blades are discretized by a grid of 19 measurement points.
For the measurements the high pressure side of the blade is used and considered being a plane surface for simplicity. The extracted eigenvectors from the experimental modal analysis of these 19 points are provided to calculate the MAC values, which are part of the objective function in the model updating optimization.
- EMA of the single blades (free free condition)
The results of the EMA of the blades in free boundary condition are used to provide the eigenfrequencies and the eigenvectors, which are further used for the model updating. To provide a free boundary condition for the measurement the blade hangs on a wire, which is attached to a frame.
The identified eigenfrequencies for the three blades are listed in the table below. It can be seen that every blade features different eigenfrequencies, which are induced by diverse material properties and variations in the manufacturing process. It shall be noted that the torsional modes show the highest deviations.
| Mode | Type | Blade 1 | Blade 2 | Blade 3 | max deviation |
|---|---|---|---|---|---|
| 1 | First bending | 47,0 Hz | 47,7 Hz | 47,7 Hz | 0,7 Hz |
| 2 | Second bending | 128,2 Hz | 130,3 Hz | 130,6 Hz | 2,4 Hz |
| 3 | First torsional | 195,5 Hz | 207,0 Hz | 206,4 Hz | 11,5 Hz |
| 4 | Third bending | 250,6 Hz | 252,9 Hz | 251,3 Hz | 2,3 Hz |
| 5 | Second torsional | 329,0 Hz | 331,2 Hz | 343,6 Hz | 14,6 Hz |
- EMA of the single blades (clamped condition)
The results of the blades under a clamped boundary condition at the bolted joints verify the validity of the updated finite element model, which is adapted to the parameters from the case under free boundary conditions. For the measurement in clamped condition the blade is mounted to the table with three screws. In order to avoid contact between the blade and the table counter nuts are used.
| Mode | Type | Blade 1 | Blade 2 | Blade 3 | max deviation |
|---|---|---|---|---|---|
| 1 | First bending | 20,0 Hz | 20,7 Hz | 20,5 Hz | 0,7 Hz |
| 2 | Second bending | 71,1 Hz | 70,2 Hz | 71,9 Hz | 1,7 Hz |
| 3 | Third bending | 127,7 Hz | 137,7 Hz | 133,5 Hz | 10 Hz |
| 4 | Fourth bending | 171,5 Hz | 179,2 Hz | 176,8 Hz | 7,7 Hz |
| 5 | First torsional | 181,1 Hz | 190,6 Hz | 189,5 Hz | 9,5 Hz |
- EMA of the rotor assembly
For a later application of substructuring methods a refernce measurement of the rotor assembly consisting of the three blades and the modified hub is established. In a previous step the interior of the hub was filled with an epoxy resin to fix the rotational degree of freedom of the blades. The modal analysis is done under free boundary conditions, where the assembly is suspended by a cord with support frame.
A coarser measurement grid is used for this analysis.
Nine instead of nineteen measurement points per blade are used.
Due to the deviations of the material properties between the single blades and within the hub, distortion of the cyclic symmetry of the system can be observed. The vibrational energy is not equally spread but seems to be rather concentrated in single blades, which is indicated by strongly different amplitudes.
| Mode | Frequency | Unit |
|---|---|---|
| 1 | 16,7 | Hz |
| 2 | 23,4 | Hz |
| 3 | 31,6 | Hz |
| 4 | 56,0 | Hz |
| 5 | 75,0 | Hz |
Modeling of the Substructures
The assembly of the wind turbine consists of many different parts. Those parts have different material parameters and are connected to each other in various ways. Since the influence of each individual part on the overall dynamics is unknown, all parts are modeled such that individual material parameters can be given to reach the best matching between simulation and experiment. The first step toward a finite element model which is able to capture the dynamics of the system is to know the geometry. Therefore, the dimensions of the real parts were recorded manually and converted into CAD models.
- Blade Model
Based on the geometry a finite element model of the blade was established with the Hyperworks software by Altair. Due to the complicated shape the geometry is divided in an upper (green) and lower (red) surface of the blade and the flange (blue). The outer layer defined by these three sections is the composite part of the blade surrounding the core material (yellow). Each section can be meshed individually.
The composite part of the blade is meshed with tria elements with an element size of 10 mm. 3D tetras with the same element size are used for the core of the blade. An intersection of the blade is given in the picture below.
As already mentioned, the blade is made out of two different materials. Johansson et al. performed destructive tests in "Modeling and calibration of small-scale wind turbine blade" to obtain material properties of both the glass fiber composite and the core. Chemical tests, which were performed in their study, indicated that the core, as well as the resin of the glass fiber reinforced skin, consist of polypropylene (PP). The material properties used for the FE-model presented here and resulting from the investigation performed by Johansson et al. are collect in the tables below.
| Core | |
|---|---|
| Young's Modulus | 1745 Mpa |
| Poisson's ratio | 0.3 |
| Density | 8.18*10^-10 t/mm³ |
| Skin | |
|---|---|
| Young's Modulus perpendicular to fiber | 1745 Mpa |
| Young's Modulus in fiber direction | 14500 Mpa |
| Poisson's ratio | 0.3 |
| Density | 1.09*10^-9 t/mm³ |
| Shear Modulus in all directions | 700 Mpa |
The laminate of the composite skin consists of 4 layers, stacked by alternating the direction of the fibers in a 0°/90°/0°/90° order, where the fibers oriented in 0°, span from the blade root to the tip of the blade. Each ply has a thickness of 0.7 mm resulting in a total composite skin thickness of 2.8 mm. The following picture illustrates the laminate of the blade. The arrows point in the fiber direction of the ply. The outer ply has a 90° fiber orientation whereas the first ply on the core is oriented in a 0° angle.
A modal analysis was performed with this FE-modal in both free and clamped boundary condition. The clamped condition was realized by putting constraints on nodes of the flange. Results obtained from the free model:
| Mode | Type | FE | exp.Blade 1 | exp. Blade 2 | exp. Blade 3 | |
|---|---|---|---|---|---|---|
| 1 | First bending | 49.2 Hz | 47,0 Hz | 47,7 Hz | 47,7 Hz | |
| 2 | Second bending | 139.7 Hz | 128,2 Hz | 130,3 Hz | 130,6 Hz | |
| 3 | First torsional | 220.1 Hz | 195,5 Hz | 207,0 Hz | 206,4 Hz | |
| 4 | Third bending | 272.6 Hz | 250,6 Hz | 252,9 Hz | 251,3 Hz | |
| 5 | Second torsional | 348.5 Hz | 329,0 Hz | 331,2 Hz | 343,6 Hz |
Results of the model with constraints:
| Mode | Type | FE | exp. Blade 1 | exp. Blade 2 | exp. Blade 3 | |
|---|---|---|---|---|---|---|
| 1 | First bending | 21.5 Hz | 20,0 Hz | 20,7 Hz | 20,5 Hz | |
| 2 | Second bending | 75.8 Hz | 71,1 Hz | 70,2 Hz | 71,9 Hz | |
| 3 | Third bending | 140.2 Hz | 127,7 Hz | 137,7 Hz | 133,5 Hz | |
| 4 | Fourth bending | 189.3 Hz | 171,5 Hz | 179,2 Hz | 176,8 Hz | |
| 5 | First torsional | 208.0 Hz | 181,1 Hz | 190,6 Hz | 189,5 Hz |
.png)
.png)
.png)
.png)
.png)
- Hub Model
The hub of the wind turbine is a complex part which has numerous components. An intersection of the finite element model can be seen in the picture below. The components are modeled individually and are assembled using compatibility conditions at the contact surfaces. In addition to the parts, which can be seen in the intersection, the epoxy resin is modeled for the sake of completeness. In further investigations, measurements of the hub assembly will be established and a model updating will be performed.
- CAD Assembly Model
Geometry files of the assembly in step and iges format. STEP file of Ampair 600 Wind Turbine IGES file of Ampair 600 Wind Turbine
- Solver input files (mesh) for ABAQUS, ANSYS, and NASTRAN.
Solver input files ABAQUS,ANSYS,NASTRAN
Model Updating
Model updating is a method to adjust parameters of a simulation model automatically so that it matches the dynamic behavior of the measured part. In the present case the modal parameters from the experiments are used as reference to adjust the material parameters for the finite element model to obtain better results. For this purpose an objective function is created which includes the deviation of the measured and simulated eigenfrequencies and -vectors. Reaching a good result in optimization strongly depends on the quality of the finite element model. Since the finite element models themselves contain uncertainties with respect to the real parts a good agreement for all eigenfrequnecies and -vectors could be unachievable. To counteract this problem a weighted sum is introduced which offers more variability for a good compromise of all considered modes. The weighted sum can be written as
,
where x is the n-dimensional vector of the parameters to be updated, f represents the single objective functions, w is the vector with the weighting factors and m the number of the considered objective functions. In the present case the overall objective function J is composed of two functions. One represents the frequencies and the other the eigenvectors such that J can be written as
.
The weighted sum of the deviation of the measured and simulated eigenfrequencies is denoted by
,
and the deviation of the eigenvectors in form of weighted MAC values [3] is described by
with 
.
IMAC 2014
The group at the University of Stuttgart presented a paper at IMAC 2014 in which a finite element model is updated to correlate with measurements from a blade. The paper can be accessed here. The models used are posted on this page.
References
