Structural Design Sensitivity Analysis and Optimization of Vestas V52 Wind Turbine Blade

6 th World Congress on Structural and Multidisciplinary Optimization Rio de Janeiro, 30 May - 03 June 2005, Brazil Structural Design Sensitivity Analysis and Optimization of Vestas V52 Wind Turbine Blade Lars Chr. T. Overgaard and Erik Lund Institute of Mechanical Engineering, Aalborg University, DK-9220 Aalborg East, Denmark. E-mail: lcto@ime.aau.dk and el@ime.aau.dk. 1. Abstract The objectives are Design Sensitivity Analysis (DSA) and structural design optimization of a 12-meter section from a 25-meter laminated composite main spar in a wind turbine blade from a V52 wind turbine manufactured by Vestas Wind Systems A/S. Full scale experiments of the blade from static loading to collapse have been performed and are used as reference for verifying the finite element shell model used in this work. A geometrically nonlinear and linear prebuckling analysis have been performed for predicting the failure of the blade due to local buckling on the suction side of the airfoil, and the objective is then to apply DSA and optimization in order to improve the design. The criterion considered is the maximum strain in the main spar, when it is subjected to a static flap-wise loading moment as a cantilever beam with a shear force at the free end. The DSA of the geometrically nonlinear problem is performed using the direct differentiation approach and it is used for sensitivity studies with respect to imperfections from the manufacturing procedure and others. The structural topology of the blade is not changed, i.e., the design variables considered are material orientations of the fibre reinforced materials and layer thicknesses. An active set strategy is applied together with the bound formulation in order to solve the min max strain problem considered. 2. Keywords: Structural instability, design sensitivity analysis, composite structures, laminate optimization. 3. Introduction In a wide range within the application of composite materials structural instability phenomena are present, which under some conditions can be critical for the integrity of the construction. In the present paper a V52 wind turbine blade manufactured by Vestas Wind Systems A/S is studied. Typically the suction side of the aerofoil (spar and shell) during operation is loaded considerable in compression. Instability under such loading conditions will trigger delamination in the main spar which is the primary load-carrying structure and ultimately result in a progressive collapse of the blade. The structural instability is local buckling, which is governed by the presence of imperfections, e.g. as a consequence of the variability of the production facilities and methods. Examples of manufacturing imperfections are thickness variations of the core material in the web, angle misalignment of the large pre-consolidated plies for the flanges and finally geometric imperfections due to section variations. Thus the driving design parameter within the wind turbine blade industry has shifted from global stiffness and fatigue issues to structural instability as the blades become larger and new materials are taken into use. For this reason there is a general consensus in the industry that this issue must be addressed. Hence new design rules and methods must be addressed in order to estimate under which conditions the structural integrity of the blade is compromised and DSA can be used in order to evaluate the impact of manufacturing imperfections. This paper will take its form based on full-scale experiments of the static collapse of the wind turbine blade, see [1], which is used as reference for verifying the finite element shell model used in this work. This comparison has been based on models with all known imperfections and idealized models without any imperfection, but not all results are reported in this paper for brevity. The objectives are to apply DSA on a blade section with imperfections and laminate optimization by minimizing the maximum strain in the material direction for an idealized 12-meter section of the 25-meter blade under investigation. The DSA and structural design optimization is done in combination with a geometrically nonlinear analysis for the maximum recorded flap-wise loading moment during testing. The DSA of the geometrically nonlinear problem is performed using the direct differentiation approach, see [2], and it is used for sensitivity studies with respect to the previously mentioned imperfections. The structural topology of the blade is not changed, i.e., the design variables considered are material orientations of the fibre reinforced materials and layer thicknesses. This yields many design variables, if they are associated with each finite element. This is not the case since the design variables are linked to a real constant 1

set by an index pointer, which gives a patch design variable approach, i.e., larger areas are forced to have the same layup. Thus the number of design variables may be reduced from 7200 to 534 design variables. An active set strategy is applied together with the bound formulation in order to solve the min max problem considered, and the optimization problem is solved using the Method of Moving Asymptotes [3]. Figure 1: (A) Overall blade terminology and (B) cross-section definitions and design topology. The overall blade terminology is shown in 1(A) and the cross-section definitions for the structural members are displayed in figure 1(B). On the structural system level the blade consists of an aerodynamic shell with suction where the structural compressive flange is located and an aerodynamic shell with pressure which corresponds to the structural tensile flange. These aerodynamic shells are adhesive bonded to the main spar, which gives the blade a leading and trailing edge. On a lower structural level the main spar consists of a winding root and a tip spar. All these structural components are pre-fabricated and joined during the assembly procedure of the blade. The design topology of the main spar is divided into a web and flange. The flange consists of a symmetric layup of winding, angle plies and pre-consolidated flange packages, where a multi-angle ply (shell) is adhesive bonded to the spar. The web is a symmetric sandwich panel layup with face sheets of winding and angle plies together with a core material. These material groups are ply-inserted and dropped along the length of the blade, where the two significant material transitions are denoted the Flange Material Transition (FMT) and Core Material Transition (CMT). The corners in the main spar give the boundary conditions to the adjacent structural members, i.e., the web and flange. These corners have a multiple ply-insert and -drop configuration, since at this junction the transition from the sandwich panel to the monolithic flange must occur. 4. Static Testing of the Blade The blade is divided into three test regions and a flap-wise load is applied corresponding to compressive and tensile strain in the aerodynamic suction and pressure side of the blade, respectively. Figure 2(A) displays the test set-up in a schematic way. Figure 2: (A) V52 static test regions and (B) structural response in critical cross-section. The wind turbine blade is instrumented with unidirectional strain gauges and Linear Variable Differential Transformer (LVDT) detectors. The compressive flange has mounted unidirectional strain gauges inside the main spar 2

and outside on the shell. Beside this there is installed LVDT detectors on the outside. The tensile flange has been equipped with unidirectional strain gauges on the outside of the shell. Furthermore unidirectional strain gauges have been mounted inside on the web toward the leading edge. Region one, two and three are each tested five, two and eight times, respectively. During each test series the load steps are increased until final collapse in the last test sequence. The data is collected continuously with a rate of 1 Hz and by a trigger file, which is a file with data dumps from the continuous logging file on the request from the test personal. The blade is loaded with a flap-wise moment at each test region and after test-to-failure the region is cut off, which enables one to perform test on the next region. The model and test data are compared in test region 3, since it is of most structural interest. Here the first failure is observed in test number seven, see fig. 2(B), which displays the strain level near the critical blade section at each test sequence. It is observed that stiffness retention has occurred in test eight compared to test seven. This stiffness indication not only states a first failure event but also at which rotor radius the critical blade section is located. 5. Predictive Model Generation The finite element models are generated through a generic blade builder program in MSC.Patran command langauge and MSC.Laminate Modeler. The material layup information is handled by ascii text file input, which is generated in a spreadsheet that averages the material properties according to the chosen element discretization of the finite element model. A complete description of the investigated 12-meter section requires more that a thousand real constants sets. Thus in the case of large system analysis some averaging of the real constant sets most take place. The generated models can be translated to MSC.Marc, MSC.Nastran and Ansys solvers. Furthermore an interface to design variables associated to the generated real constant sets is implemented to the in-house finite element system MUST (MUltidisciplinary Synthesis Tool, developed at the Institute of Mechanical Engineering at Aalborg University, Denmark). 5.1. Stiffness Representation of Adjacent Structural Members In order to assess the modelling accuracy of the interaction of the adjacent structural members a benchmark is developed. The benchmark is uniquely made for this dilemma. Hence a two-dimensional (2D) elasticity finite element solution is established as a reference model. Subsequently a linear static finite element model is employed and different finite element formulations are evaluated. This is solely done because it is not feasible to model the correct material and thickness transitions at the corner between the flange and web, since it has a multiple ply-drop and -insert configuration. In the given case a correct representation of all ply-drops and -inserts would require an element to radius ratio (R/E) of 48, i.e. 48 elements in the corner radius. Details like the main spar corner is in the scale of centimeters and the blade is meters giving a ratio between blade length and corner in the thousands. This will give a too dense discretization in order to have a feasible global finite element model of the blade and still have the correct corner stiffness representation. The stiffness benchmark is performed in such a manner that a finer discretization of the corner gives a more accurate representation of the real lay-up at the corner. Different analysis codes and elements are investigated. Common for the single-layered theory elements used is that they either are based on the Reissner-Mindlin or Kirchhoff-Love assumptions and formulated on bilinear or quadric isoparametric interpolation functions with either full or reduced integration schemes. The elements have either 4/8 nodes or are degenerated to 6/3 nodes. The Nastran element is the only element in this benchmark used with sandwich option (SMCORE). It is seen on fig. 3 that the benchmark converges toward the 2D elasticity solution when subjected to a flap-wise load i.e. the elements in the flange are exposed to an out-of-plane bending and the elements in the web are primarily exposed to in-plane loading. When MSC.Natran elements are employed with the SMCORE option then the averaging of the element constitutive properties becomes too coarse, so in this case the structure is too flexible. This is the case since the face sheets are thick compared to the core material. The Ansys Shell99 model 1 fails, since it has too large thickness-to-curvature ratio and equilibrium is not satisfied. An Ansys Shell99 model 2 has been implemented, which approximates the curved geometry with piecewise straight lines and thereby forces the element to be straight. Hence at high element densities the stiffness representation is sufficient but as the density decreases so does the geometry and stiffness representation. MSC.Patran elements based on the Kirchhoff-Love assumptions have hourglass problems when employed in the benchmark. The chosen elements for the analysis are the bilinear Marc 140 element with reduced integration and the 9-node isoparametric MUST (shell9) element. 3

Figure 3: (A) Stiffness benchmark and (B) results for flap-wise load. The corner should be modelled with a minimum of elements corresponding to the best averaging of the stiffness represented by the number of UD (Unidirectional) ply-drops, i.e. in the given case an R/E ratio of 5 is required. A finer mesh and thereby better stiffness representation is possible but not advisable since the gain is below 5% from the coarse to the finest mesh. This ensures a minimum of 90% representation of the stiffness compared to the 2D solid model. 5.2. Implemented Models A finite element model with 7200 shell elements is employed in the examples. Two models are considered namely a idealized model without any manufacturing imperfections and a second model with a imposed imperfection pattern. The latter is used in the DSA and the idealized model is employed in the laminate design optimization problem. The imperfection sensitivity of the blade is evaluated by imposing the strain gauge measurement for the full-scale experiment as a imperfection pattern. This is done by looping over a number of simulations and then employing an unconstrainted optimization with a conjugated gradient method to minimize the error function of the simulated blade response and the actual measured strain gauge response. Figure 4: Imperfection sensitivity of blade. 4

Fig. 4 to the left displays the response of the obtained imperfection amplitude where the 23% amplitude model fits the best of the evaluated models. It is seen that the imposed imperfection pattern is directly proportional with the longitudinal strain measured in the strain gauges, see fig. 5 to the right. This means that the model with a 23% imposed imperfection pattern is used for DSA and the idealized model for the optimization problem. Most important is the discovery that the buckling shape is unaffected by the presence of imperfections, but the local strain at the maximum Geometric Imperfection Amplitude (GIA) is linearly depending on the imperfection amplitude. The epic center of the buckling shape mode is at the CMT and FMT as seen in fig. 5 but the structural collapse of the structure is at the GIA. Figure 5: Buckling mode and strain state for 12-meter section of the V52 blade. This implies that design sensitivity analysis w.r.t. the thickness of the core material in the web and the angle alignment of the five flanges is of main interest. 6. Design Sensitivity Analysis The DSA of the geometric nonlinear problem for the V52 blade section is considered for two design variables describing the core material thickness along the length of the blade and the core material thickness at the CMT. Furthermore five design variables for each of the angle alignments of the flange packages are considered separately. It is chosen not to consider the flange thickness, since it is required that the global stiffness is maintained. The analysis and DSA method used in MUST are shortly outlined here. element discretized problem are written in residual form as The state equations for the finite R(U(x), x) =0 (1) where R is the residual, U represents displacements and x contains design variables x i,i=1,...,i. Due to the geometrically non-linear response of the system, Newton s method is applied for solving the equilibrium equation given by Eq. (1), i.e., a step k + 1 in the solution procedure can be described as R(U k ) U ΔUk = R(U k ) where U k+1 = U k +ΔU k (2) The Jacobian of the problem, R/ U, is also known as the tangent stiffness matrix K T. Based on the nonlinear displacement field, the element strain vector ɛ can be determined. In case of minimization of the maximum strain in the material direction in the structure, the number of criteria functions will in most cases be larger than the number of laminate design variables, and thus the direct differentiation approach to design sensitivity analysis is applied. Differentiating the residual R(U(x), x) w.r.t. a design variable x i,i = 1,...,I, yields the linearized global sensitivity equation [2] to be solved for each design variable x i: dr dx i = R du + R du = 0 i.e., K T = R (3) U dx i x i dx i x i 5

The pseudo load vector R/ x i is evaluated using central difference approximations at the element level. A direct solver is used such that the factored tangent stiffness matrix K T can be reused when solving the sensitivity equations. Having obtained the displacement sensitivities du/dx i the strain sensitivities are computed using a finite difference approximation as the analytical strain sensitivities are quite cumbersome to implement for the shell elements used and no inaccuracy problems have been observed on the strain sensitivities. The DSA of geometrically nonlinear problems are implemented in MUST and used to evaluate the discussed imperfections. 6.1. Core Material Thickness The design sensitivity w.r.t. core material thickness at the CMT and the overall core material thickness along the blade length is given by DElmenStrain D1 and DElmenStrain D2 in fig. 6, respectively. It is seen that the local strain field in the neighborhood of the collapsed section, hence at GIA, is moderately affected by the core material thickness at the CMT which also moderately influences the strain state at the start of the buckling critical region, see fig. 6 to the left. Figure 6: DSA of maximum strain for the variables DElmenStrain D1 and DElmenStrain D2 which are the design variables for the core material thickness along the blade and the thickness at the CMT, respectively. However the strain state in the buckling critical region is highly sensitive to the overall thickness of the core material, see fig. 6 to the right. The strain state at GIA is only mildly affected by the overall thickness of the web, whereas the buckling critical region is highly sensitive to the core material thickness along the whole buckling critical region. 6.2. Flange Angle Alignment The sensitivities to the angle misalignment of the pre-consolidated flanges are shown in sequential order in fig. 7, where the inner flange is the design sensitivity DElemStrain D1 w.r.t. to the ply angle at flange one and design sensitivity DElemStrain D2 is for flange two and so on up to flange 5. The strain state in the region of interest is not affected by the orientation. There is a small impact precisely at the GIA since the fibers are rotated in- and out-of-plane compared to the surrounding surface and therefore it will have a small effect however the strain state is only mildly affected by the misalignment of the flange. Nevertheless the alignment of the outer flange number five (DElemStrain D5) at the FMT has some effect over a larger region, but only mildly sensitive to the alignment. 6

Figure 7: DElmenStrain D1 to DElmenStrain D5 is the design variables for the angle misalignment of the flange packages number one to five, respectively. 7. Structural Design Optimization of V52 blade The design optimization problem of the V52 blade is written in a general form as a mathematical programming problem: Minimize maximum ɛ z x Subject to (4) mass M x i x i x i, i =1,...,I where the objective function is the maximum strain in the material direction ɛ z at any layer in the laminated composite structure and M is the mass constraint. The min-max problem is solved using the so-called bound formulation, [4, 5], where an additional scalar design variable β is introduced: Minimize x,β Subject to β ɛ k z β k =1,...,n 0 mass M x i x i x i, i =1,...,I (5) The number of strain values included in the optimization problem is denoted n 0, and this number is determined using an active set strategy. In the example shown only values exceeding 85% of the maximum strain value are included in the optimization problem. The mathematical programming problem is solved using the Method of Moving Asymptotes by Svanberg [3]. The closed loop of analysis, design sensitivity analysis and optimization is repeated until convergence in terms of no change of the design variables is reached or until the maximum number of design iterations have been performed. 7.1. Constraints and Restrictions It is required that the global stiffness is maintained during the closed loop of analysis. Thus the flange packages are not a part of the design space. The root is also not a part of the design space, basically because it is a well produced and inexpensive prefabricate of the blade. Moreover it consists of so many plies that is can not be managed, still with simplification the number of design variables used in order to describe the root is approximately the same as for the rest of the whole model. Furthermore the corner stiffness is not included in this the design optimization, since it triples the number of design variables. Winding plies are constrained to have an antisymmetric layup of two unidirectional plies and be in between 7

an angle set of either 15 0 to 75 0 or 15 0 to 75 0. This is done in order to be able to wind the material. Angle plies between the pre-consolidated flange packages consist of two unidirectional plies and both can be between 90 0 to 90 0. The two outer plies in the multi-angle ply are also constrained to be either 15 0 to 75 0 or 15 0 to 75 0,since the most outer plies must be angles plies in order to obtain a good surface finish. The first ply in the multi ply can vary from 90 0 to 90 0. The core material thickness is also considered in the design space and this can vary between 3 4 the nominal core material thickness. Since only core material thickness is considered no mass constraint has been employed. to 2 times 7.2. Optimization Results The iterative history of the optimization procedure is displayed in fig. 8. It is seen that the objective function converges toward a local optimum with an improvement of lowering the maximum strain with 14.7 % compared to the original design. The size of the active element set is also stable with a value of 6% compared to the 0.6% in the original design. Figure 8: Iterative history of optimization routine. The design variables are not fully converged as they seem to oscillate even though the objective function has converged. 7.2..1 Optimization of Flange The results are presented in such a manner that the upper part of the fig. 9 shows the initial flange design space in schematic way and the graphs below displays the angle as a function of the blade length of the winding, angle and multi-angle plies determined in the optimization routine, respectively. The outer winding ply is restricted to take the value of 0 0 and therefore it reaches the constraint of 15 0.Atthe buckling critical region the angle is approximately 30 0. The outer ply is symmetric however the inner winding ply is antisymmetric after the buckling critical region. The angle plies reach 90 0 at the load introduction and inward to the buckling critical region where they shift to 30 0 and decrease downward to 0 0. At the root end the angle ply shifts periodically from cross-plies to pure 90 0 at every stiffness transition in the root section. The multi-angle ply does the same as the winding plies, since it is constrained in the same manner. final ply goes towards ±90 0. The 7.2. Optimization of Web The results for the web are displayed in the same manner as for the flange and can be seen in fig. 10. 8

Figure 9: Original flange topology and the optimal angle as a function of the normalized blade length. There are many thickness transition in the web due to the winding of the root and the core material therefore the result is a multi-valued image compared to the flange. The inner winding plies are anti-symmetric and the outer winding plies are symmetric. All winding plies go to the lower limit value of 15 0, except the single antisymmetric ply. At the buckling critical region the inner winding plies go toward 30 0 whereas they decrease further to 15 0 in the middle of the critical buckling region due to the thickness transition in the web. The angle plies take the value of 90 0 toward the load introduction. Toward the more complex strain state of the web at the many thickness transitions a multi-valued image is given. The original thickness transition of the core material at the GIA is moved so that thicker core material is located at the buckling critical region at FMT and CMT. 8. Conclusion on Results The strain value is directly proportional with the imposed imperfection pattern from the strain gauge measurements. The imperfect model reveals that the epic center of the buckling mode is not located at the collapsed zone at the maximum GIA, but primarily controlled by the thickness transitions in the web. The strain state at the maximum GIA is moderately sensitive to the core material at the CMT and less than mildly sensitive to the misalignment of the flange packages. The strain state at the critical buckling region is moderately sensitive to the overall core material thickness and not sensitive to the misalignment of flange packages one to four however it is less than mildly sensitive to the misalignment of flange package 5. The strain level in the material direction can be reduced by 14.7% by changing the angle of the winding, angle and multi-angle plies along with the alteration of the core material distribution along the blade length. 9

Figure 10: Original web topology and the optimal angle as a function of the normalized blade length. The overall trend of the optimization is that the winding, angle and multi-angle plies should be ±30 0 at the buckling critical region. Furthermore, at the load introduction the angle of the inner plies should be ±90 0 and the outer plies should be 0 0. This corresponds to optimization results for a 2D composite structure studied in [6]. Additionally at the thickness transition at the root end the plies tend to be either 0 0 or 90 0. 9. Further Work Further work within the nonlinear optimization is considered especially in order to design for local buckling. This will require the implementation and investigation of different critical-point test functions. 10. References [1] Christian Leegaard Thomsen et al. V52 statisk styrke (in danish). Risø-I-1980(DA), Forskningscenter Risø, Roskilde:133 139, April 2003. [2] J. Sobieszczanski-Sobieski. Sensitivity of complex, internally coupled systems. AIAA Journal, 28(1):153 160, 1990. [3] K. Svanberg. The method of moving asymptotes - a new method for structural optimization. Numerical Methods in Engineering, 24:359 373, 1987. [4] M.P. Bendsøe, N. Olhoff, and J.E. Taylor. A variational formulation for multicriteria structural optimization. 11:523 544, 1983. [5] N. Olhoff. Multicriterion structural optimization via bound formulation and mathematical programming. Structural Optimization, 1:11 17, 1989. [6] J. Stegmann. Analysis and optimization of laminated composite shell structures. Ph.D. Thesis, Institute of Mechanical Engineering, Aalborg University, Denmark, 2004. Special report no. 54. 10