Design of an element test specimen for fatigue delamination growth of a thick laminate

Following the observation of multiple delaminations growing from a tunnelling crack in the spar cap of a wind turbine rotor blade subjected to cyclic loading, an element test specimen is proposed. Design of the element test specimen to study fatigue delamination of a thick laminate is presented. Complexities inherent to a full structure e.g., curvatures, ply drops, manufacturing defects, etc. are removed to study the fatigue delamination damage mechanism. The element test specimen is made of unidirectional layers with two embedded artificial delamination cracks connected by a tunnelling crack. In this paper, analytical and numerical (2D) models are used to design the element test specimen.


Introduction
The current design tools and certification procedure of modern wind turbine blades rely heavily on testing at different scales.Numerous versions of the so-called "testing pyramid" are available in the literature [1] [2].At the base of the pyramid there are the coupon tests needed to obtain material properties, in the middle there are typically sub-structures and/or sub-component testing specimens, while full-scale structure testing is at the top.The number of tests carried out at each of these blocks is decreasing as their complexity as well as the associated cost increase i.e., many coupon tests and a few full-scale tests.With the complexity of the specimens the statistical uncertainty also increases.This concept was developed in the aerospace industry, where tests are carried out bottom up with the final aim of ensuring structural integrity.
It has been noted that the full pyramid testing is very costly.A value of 300 million dollars has been estimated for the state-of-the-art carbon fibre epoxy composites used in aerospace [3].Such costs are preventive for materials innovation.It has been proposed [3] that in the future, numerical models of structures ("digital twins") should be so accurate in the prediction of damage evolution that the models can be trusted, and thus full-scale testing and sub-structure testing can be avoided.To reach this state, it is essential that the high accuracy of predictive models is demonstrated convincingly.This brings in element test specimens.Then, the purpose of conducting element testing will be to study (to document) the evolution of at least two interacting damage types in generic specimens relevant for critical details in structures.In parallel, the damage evolution of the element test specimens should be predicted using materials laws (cohesive laws, crack growth laws, etc.) measured independently by materials testing.1293 (2023) 012017 IOP Publishing doi:10.1088/1757-899X/1293/1/012017 2 By comparing the observed and predicted damage evolution, the accuracy of the numerical models can be assessed.
In the wind energy industry, it is a well-documented fact that wind turbine blades develop damage (e.g., delamination) during their lifecycle [4,5].As such, it makes more sense to have a pyramid testing focused on monitoring stable damage growth which more closely resembles the real service life of a wind turbine.Moreover, this would enable the development and validation of predictive damage propagation models based on a given current damage state.
With our current tools for life service prediction not fully matured, full-scale testing of composite blades is still required to certify structural integrity.This is the closest representation of the real structure subject to realistic loads.However, these tests are expensive, lengthy, and complicated, which is why very few of these tests are carried out in the conventional test pyramid.Sub-structures allow the test of smaller sections of the blade, while sub-components deal with general design details such as beams, flanges, webs, and connections [6].While these are simplifications from the full-scale tests, complexities inherent to structures, e.g., curvatures, ply-drops, and manufacturing defects remain in both (i.e., substructures and sub-components).These can lead to multiple damage mechanisms interacting with each other making it difficult to understand each damage mechanism.To address this, the idea of element tests has emerged with the intention of studying the evolution of interacting damage mechanisms in a wind turbine blade (e.g., spar cap delamination) allowing the investigation of scales larger than coupon tests (e.g., thick laminates), and to check the accuracy of predictive models.
Following the observation of delamination growth in the spar cap of a wind turbine rotor blade subjected to cyclic loading [7], an element test specimen is proposed here to investigate the delamination crack growth starting from a tunnelling crack in thick laminates under cyclic loading.The design of such an element subject to fatigue delamination is outlined in detail.The current study involves the design of the element test using numerical and analytical tools.
The present article is organized as follows; an introduction with a motivation for the study is presented in section 1 followed by the problem definition in section 2. Analytical and numerical (using FEM) approaches are presented in section 3. The results are given in section 4 followed by the discussion and conclusion in section 5 and 6 respectively.

Problem definition
The design of the present element test specimen comes after the observation of delamination growth in the spar cap of a wind turbine rotor blade subject to cyclic loading [7].In the study, an artificial defect in the form of a tunnelling crack and two delaminations was embedded into the spar cap of the blade, consisting of a central layer surrounded by two additional layers on each side.The blade was tested under flap-wise cyclic bending induced by transverse force with a maximum strain range of 3400 με at a load ratio of approximately  = −1.Under the cyclic loading, fatigue damage in the form of two delaminations evolved from the embedded defect.The delamination crack growth was monitored via visual inspection, acoustic emission sensors, and surface thermography techniques.
In the present study we are designing an element test specimen that enables documentation of the damage growth for two interacting damage types, a central tunnelling crack and two delaminations under cyclic loading, the damage types observed in the blade [7].The element test specimen proposed here is essentially a 2D specimen that should be relative cheap to manufacture.The tunnelling crack and starter cracks for two delaminations will be made by embedding a slip foil during specimen manufacturing.A schematic of the geometry of the element test specimen is shown in Figure 1.Unlike the full-blade test [7], the present element test specimen has been designed for tension-tension loading with a loading ratio of  = 0.1 to avoid buckling since the element test specimen will be unsupported.

Modelling
In the following, we present two models; an analytical model for the prediction of the steady-state energy release rate for long cracks, disregarding friction, and a numerical finite element model (FEM), which can calculate the energy release rate for short cracks.The effect of uneven crack lengths and friction between the crack faces can be assessed with the numerical model.

Analytical model
An analytical model can be established to calculate the path-independent -integral around the fracture process zone.The problem analysed, depicted in Figure 2, is a symmetric multilayer where the central layer has a stress-free surface (the tunnelling crack) and is delaminated from the remaining layers.The central layer has a Youngs modulus in the  1 -direction,  0 , and a thickness, .Two layers, placed outside the central layer, have a Young's modulus in the  1 -direction  1 and  2 and a thickness ℎ 1 and ℎ 2 , respectively.When their crack length exceeds a few times the layer thickness, , the problem becomes a steady-state problem that can be analysed analytically by the -integral.Then, the strain component  11 in all layers will be uniform (i.e., independent of  1 and  2 ) far ahead of and far below the fracture process zone and will be denoted  + and  − , respectively.Introducing the following non-dimensional parameters: the strain far below the fracture process zone is found via force balance to be (plane stress): For plane strain, the Young's modulus, , of each layer should be replaced with  (1 −  13  31 ) ⁄ where  13 and  31 are the Poisson's ratios for each layer (here, subscripts indicates materials directions).We analyse the upper half of the problem (with only one fracture process zone) by the path-independent -integral [8], defined as where  is the strain energy density,   is the stress tensor,   is the displacement vector, and   is the outwards unit normal vector to the integration path, Γ, that runs from the lower traction-free crack surface to upper crack face in a counter-clockwise direction.Eq. ( 3) is written in index notation (i.e., indices i and j takes the values 1, 2, 3, and the Einstein summation rule applies for repeated indices).
The integration path for the half-problem, Γ  , is chosen along the external boundaries, far ahead and far below the fracture process zone and along the mid-plane.This is advantageous since far away from the fracture process zone, the stress state (plane stress) is uniaxial stress, only stress component  11 is non-zero.The integration path Γ  is split into five straight line segments, denoted Γ 1 , Γ 2 , Γ 3 , Γ 4 , and Γ 5 , as shown in Figure 2. Far below the fracture process zone the middle layer is stress free,   = 0.Then, along Γ 1 ,  = 0, and with   = 0 we get  1 = 0 (here, subscript indicates integration path).Along Γ 2 ,  =  1 so that  2 = 0 and with   = {0, −1, 0}, we get        1 ⁄ = − 2    1 ⁄ = 0, since (for  = 1)  12 = 0 and (for  = 2)  2  1 ⁄ = 0 (Γ 2 is a symmetry plane), so that  2 = 0. Along Γ 3 , we have  =  2 ⁄ ( + ) 2 (with  being the relevant Young's modulus),  =  2 ,   = {1, 0, 0} ,  11 =  + and  1  1 =  11 =  + ⁄ so we get or Along Γ 4 ,  2 = 0 and with   = {0, 1, 0}, so that        1 ⁄ =  2    1 ⁄ = 0 ( 12 =  22 = 0 since Γ 4 is a traction-free surface), we get  4 = 0. Along Γ 5 , the -integral contribution becomes: Now summing the -integral contributions, we get The analytical model presented above gives values of the J integral for the steady-state situation only.The steady-state situation is anticipated for long cracks.Since we wish to design our specimen such that the cracking will be in the steady-state situation, we will conduct finite element modelling (FEM) with different crack length to explore how long the initial crack lengths must be to ensure that the subsequent cracking occurs in steady-state.

Finite Element model
A 2D finite element model of the element test specimen was created in the commercial finite element program ABAQUS.The model was created with total length  = 1800 mm, and variable total thickness  * = 6 mm -30 mm, and variable  and ℎ 1 between 2 mm and 10 mm. Figure 1 and Table 1.Mechanical properties of unidirectional layers manufactured from glass fabric and epoxy were assigned to the geometry as linear elastic orthotropic with transversely isotropy with  1 = 42 GPa,  2 = 12.6 GPa,  12 = 0.3 , and  12 = 3.89 GPa.The left edge of the model is fixed in the  1 -direction ( 1 ), while a tensile force is applied to the right edge which induces με all over the model and far away from the crack tips.Vertical displacement ( 2 ) of the middle nodes in left and right edges are constrained to prevent rigid body displacements and convergence difficulties.Figure 3 shows the applied boundary conditions schematically.A continuous seam, which is a region in the model that can open during the analysis, was considered for two crack surfaces and the connecting tunnelling crack.At seam-assigned lines, two overlapping nodes are created which allows the creation of two surfaces.Contact interaction was considered between crack surfaces to prevent surface interpenetration and simulate coulomb friction.Hard contact in normal direction and different values of friction coefficient, , was defined in the tangential direction for the contact properties.8-node quadratic plane stress elements (S8) were used for the model.The model was partitioned in two circles around crack tips and an oriented seed was used to generate a gradually finer mesh in the radial direction to the crack tips.In addition, to meet the sharp crack tip condition and create stress singularity, the elements located at the crack tip collapsed and the middle node of elements moved closer to the collapsed nodes.A mesh sensitivity analysis was done to find the maximum allowed element size in the whole model and around the crack tip.The length of the smallest element around the crack tip is 0.002 * to 0.01 * in all FE models.Figure 4 shows a zoomed view of the mesh around the crack tips.-integral for the cracks were calculated through 10 paths.Three paths close to the crack tip were inconsistent due to stress singularity, while for farther paths the -integral converges to constant values.The converged values will be compared with the analytical model for further analyses.

Analytical and FEM results
The steady-state energy release rate from the analytical model is compared with the -integral obtained from FEM results for equal crack lengths ( 1 =  2 = 120 mm) in Figure 5.It is seen the -integral decreases with increasing ℎ 1 and increases with increasing .It can be noted that the FEM simulation values are very close to the analytical values with a maximum difference of less than 2%.The -integral results from the FEM are plotted as a function of the crack length (equal crack lengths,  1 =  2 ) in Figure 6.For small crack lengths, the energy release rate is high, with increasing crack length the energy release rate decreases to an asymptotic value, the steady-state energy rate,   .It is seen that a crack length is needed to ensure a steady state has been attained for the three different  values shown in Figure 6.Moreover, the results from the FEM showed that the Mode I stress intensity factor was vanishingly small in comparison with the Mode II stress intensity factor, indicating that the delamination takes place under pure Mode II.

Design methodology of the element test specimen
In this section, we will describe the procedure followed to determine the dimensions of the element test specimen shown in Figure 1.
1.The length of the element test specimen is determined based on the maximum distance between the grips of the test machine.In this case, we chose  = 1300 mm.

2.
The maximum load,   , of the test machine is 100 kN and the design strain is 3000 με, assuming a longitudinal modulus ( 1 ) of a unidirectional glass-epoxy laminate of 42 GPa, we obtain the maximum cross-section area,  =   /( 1  + ), as 794 mm 2 .Next, to have a larger width than thickness, we set the width as  = 50 mm, which then results in a maximum total thickness of   * , of 15.8 mm.

3.
We aim for a maximum crack growth rate (/)  of 10 −2 mm/cycle.Using data from the literature (Fig. 6(d) of [9]), the -integral of a glass-epoxy laminate loaded in Mode II for the targeted crack growth rate would be approximately   = 1000 J/m 2 .4. It was decided to omit the outer (top and bottom) layers depicted in Figure 2 since bi-axial layers are normally used, which are prone to off-axis tunnelling cracks that may obstruct the visualisation of the main delaminations. 5. Different combinations of  and ℎ 1 can produce  values of 1000 J/m 2 (See Figure 7 ).However, with a UD layer thickness of 0.9 mm [10], both  and ℎ 1 must be multiples of 0.9 mm.Here we have chosen  = 5.4 mm (6 UD layers) and ℎ 1 = 3.6 mm (4 UD layers).Now, the total thickness of the element specimen is smaller than the maximum total thickness,  * =  + 2ℎ 1 <   * .6.The initial length of the artificial defect  0 is determined such that the crack growth will be in steady state.From FE analysis (Figure 6), it can be observed that an  0 of 60 mm ensures the crack growth is in steady state.7. The position of initial crack (slip foil) is chosen to be at the centre of the test specimen,  0 = /2, since it was found that during the blade test [7], cracks grew in both directions from the slip foil.Table 1 summarizes the chosen dimensions of the element test specimen.

Issues disregarded in design process: different crack lengths and friction between crack faces
The previous figures are obtained for a frictionless, symmetric configuration (i.e., top and bottom cracks with equal initial lengths,  0−1 =  0−2 ).An asymmetric configuration with a fixed bottom crack length of 120 mm, and a varying top crack was modelled using FEM.The energy release rate obtained from such an asymmetric configuration is shown in Figure 8.The top crack, which is shorter, has a higher energy release rate, while the bottom crack (the longer crack) has a lower energy release rate.This means that for an asymmetric configuration, under cyclic loading, the shorter crack would grow faster until they reach the same length i.e., approaching the situation of equal crack lengths.
Friction between the crack surfaces is not considered in either of the two plots shown above.However, in Figure 9, it can be observed that friction influences the computed energy release rate.In Figure 9, the -integral computed from FEM is plotted using different values of friction coefficient, .The inclusion of friction in the FEM model results in lower energy release rate as it can be expected.In the case of glass/epoxy composites, where friction coefficient for dry conditions and low normal forces typically ranges between 0.2 and 0.5 [11], a reduction of 10-30% of the -integral is expected.

Limitations of proposed element test specimen and predictive models
As mentioned, the analytical model is restricted to steady-state cracking, i.e., for long cracks.The model assumes symmetry about the horizontal midplane, and thus equal crack lengths.However, since the steady-state result is independent of crack length, it is anticipated that the analytical result would correspond to the average value of the energy release rate of the two cracks if the two-crack length differed, as indicate in Figure 8.
It is appropriate to discuss the differences between the element specimen and the situation of testing a full blade with similar, designed cracks.In comparison with a full blade, element testing offers several advantages.First, it is possible to observe the crack at both faces of the element test specimen; for a full blade, the crack can be seen from the outside, but it might be difficult to see the crack inside a full blade.Secondly, there are limitations on how high the blade can be loaded -a higher load could induce other undesired damage types.An element test specimen can be loaded higher.Thirdly, the manufacturing, instrumentation and testing of a full blade is several orders of magnitude larger than for an element test specimen.It is therefore possible to manufacture and test several nominally identical element test specimens, and get data for specimen-to-specimen variation or to explore effects of one or more geometric parameters.A drawback of the present element specimen is that it is restricted to tension loading only -a compression loading could cause buckling.A full blade includes one or more shear webs that prevents buckling, and therefore damage in a main spar can undergo tension-compression loads.It is, however, also unclear what crack growth data there can be used for a crack tip that undergoes reverse loading (i.e., the crack tip goes from positive to negative shear stresses at the crack tip).
Friction between crack faces is not considered in the analytical model.Without friction, the -integral value evaluated around the external boundaries,   , will be equal to the energy release rate of the crack tip.In case of friction, stress would be transferred across the crack faces, unloading the crack tip, as shown in Figure 9.In the analytical model, friction could approximately be modelled as a constant frictional shear stress (as opposed to the Coulomb friction modelled in FEM), see e.g., [12].Note that disregarding friction provides with conservative predictions, as friction further contributes to energy dissipation as mentioned previously.
The FEM model relies on linear elastic fracture mechanics, which assumes a small-scale fracture process zone.This means that fibre bridging is not considered.However, if there were significant fibre bridging it would have an effect decreasing the cyclic growth rate [12,13].The analytical model could model crack bridging in a simple way, e.g., as a constant shear stress acting along the bridging zone [12].Furthermore, the present models only consider the choice of literature data for the cyclic crack growth rate (using Mode II data).The present element test is designed under tension-tension cyclic load since the analytical model cannot handle compression loads.In addition, a specimen under uniaxial compression loading is vulnerable to undesired fibre micro buckling and global buckling, which needs extra constraints to be prevented.As mentioned, the proposed element test specimen is robust towards different crack lengths in that a shorter crack would be loaded higher and would thus tend to grow faster and catch up with the longer crack under cyclic loadings.

Prognosis and perspective
It is clear from the previous work that delamination is highly dependent on geometry, e.g., depth and thickness.Damages identified during inspection of wind turbine blades are assessed based on their perceived risk to the remaining operational requirement of the turbine.Information about the damage (e.g., geometry), provided by visual inspection alone often needs to be supplemented with sub-surface details provided by ultrasonic scans if a confident assessment is to be made.Highly accurate automated prognostic tools will be required within the digital twin representations of very large offshore wind turbine blades in the future [15].
The work described in this paper suggests the development of a damage predictive framework where measured crack growth rate parameters from fracture mechanics tests can be used as input to models that predict the delamination crack length as a function of the number of cycles in the element specimen.Such an approach can provide the validated test data necessary for automated prognostic assessment of damages, and thus service life, in composite structures based on known geometries and parameters.

Concluding remarks
The major outcomes from the present study are the following: • Establish a design methodology for element test specimen to study delamination crack growth initiated from a tunnelling crack.This methodology could be generalised to other element test specimens intended to study other damage types.• The designed element specimen is a steady state specimen, which means that the energy release rate is independent of the crack length.• The designed element test specimen can be used to check the accuracy for predicting delamination crack growth.• The designed element test specimen is robust in terms of handling different lengths of top and bottom delamination crack lengths.

Figure 1 .
Figure 1.Schematic of the element test specimen with dimensions denoted by variables.The artificial defects are shown with the thick red lines.

Figure 2 .
Figure 2. The problem analysed by the analytical model: Delamination of a middle layer in a symmetric five-layer structure.The applied strain in the uncracked part of the structure is  + .

Figure 3 .
Figure 3. Boundary condition applied to the finite element model of the element test specimen.

Figure 4 .
Figure 4. Crack modelling a) assigned seam on crack surfaces, b) generated mesh

Figure 5 .
Figure 5. Steady-state energy release rate plotted for different values of top layer thickness, ℎ 1 .The square markets are the FEM values, and the curves are the analytical results.

Figure 6 .
Figure 6.Energy release rate from the FEM analysis plotted as a function of the crack length (equal crack lengths,  1 =  2 ) for different ply thickness values showed with square markers.

Table 1 .
Figure 7. -integral is shown as a function of top and bottom layers thickness for different central layer thicknesses.The steps for determining  and ℎ 1 for   = 1000 J/m 2 are indicated with the dashed lines.

Figure 8 .
Figure 8. -integral plotted against the crack length with the top and bottom cracks marked with green and purple squares respectively.