Full Text

Introduction Jet engines are some of the most complicated technologies on the planet, and they must have outstanding reliability and comply with the modern requirements for weight, noise and other things. Today, it is impossible to create a competitive jet engine without using components made of fibre-reinforced polymers (FRPs) [1-3]. Design of high-loaded parts of jet engines made of fibre-reinforced plastic is a complex problem that requires not only development of new materials and technologies, but also creating of appropriate computational tools for analysis of strength, durability and reliability of these composite parts under working loads and during an emergency. Nowadays, software packages that use finite element method (FEM), such as ANSYS, LS-DYNA, ABAQUS, Simcenter 3D are widely used for mechanical behaviour analysis of FRP parts under different loading conditions. A series of articles [4-6] on the development of methods of stress-strain state and strength analysis of CFRP outlet straightener blade for new turbofan engine PD-14 under quasi-static loading is one of the first examples of using numerical methods for designing of load-bearing composite elements in Russian aircraft engine building. A significant amount of work related to the increasing the amount of composite materials in the perspective turbofan engines PD-14 and PD-35 is performed today, and the most important task for engineers is to create a composite fan blade and a fan case for them. To solve this problem, ensuring not only static but also cyclic and impact strength of these parts is needed. The developers of aircraft engines try to minimise the number of tests of full-size structures due to their high complexity and high cost. In this regard, great attention is paid to numerical simulations. Numerical models for the analysis of deformation and fracture of composite elements during high-velocity impact are especially needed for full-scale simulations of turbofan engines with composite fan cases and blades during fan blade out and bird strike events. These computational models must satisfy the following requirements: a high numerical efficiency, a possibility to predict the deformation and fracture of FRP parts correctly and an accuracy in assessment of the amount of energy absorbed by the material in a wide range of the projectile velocities [2]. Meeting these requirements is provided by selecting an appropriate approach to composite structure modelling and sufficient computational and experimental verification of the models. It is important to note that there are lots of problems and difficulties at the stages of creation and verification of computational models. The main goal of this study was to find a suitable approach for the modelling of the high-velocity impact loading of large size FRP parts and consider the main problems arising from its application. The article structure is as follows: Section 2 contains a brief review of existing modelling approaches for analysis of mechanical behaviour of fibre-reinforced composites subjected to high-velocity impact with a discussion of their advantages and limitations. An example of a meso-scale approach application for numerical simulation of CFRP plate subjected to impact loading will be presented in Section 3. The obtained results of numerical simulations and their discussion are described in Section 4. Section 5 gives a conclusion. 1. Current and prospective approaches for simulations of the damage and failure of composite materials subjected to high-velocity impact First, it is necessary to separate the concepts of "computational model" and "material model". A computational model is a set of geometrical and mesh models of FRPs, material deformation and fracture models. The classification of the FRPs modelling approaches by depending on the detail of the geometric model is the most popular. Three approaches are used for applied calculations in practice (Fig. 1): macro-scale (lamina-level), meso-scale (ply/yarn-level) micro-scale (filament-level). Consider each of the approaches in more detail. Fig. 1. Modelling scales for analysis of the FRPs mechanical behaviour 1.1. Macro-scale (Lamina level) The macro-scale approach for simulation polymer composite materials is based on the use of classical laminated plate theory (CLPT) [7]. The composite material is simulated as a continuous homogeneous medium with orthotropic or anisotropic properties without explicit consideration of the layered structure. The heterogeneity of the mechanical properties in the thickness of the material is taken into account using special finite elements. Each layer in the real material corresponds to the integration point in the element with appropriate stiffness matrix. Standard pre-processors of various software packages, as well as specific software, for example, Fibersim [8], can be used to create computational models. The apparent advantage of this approach is the high numerical efficiency. The macro-level approach became the most widely used in the analysis of static strength of composite material structures. However, to simulate the deformation and fracture of composite parts and structures under the high-velocity impact, this approach in its pure form does not quite fit, since it does not allow taking into account material delamination. Several works may be noted [9-15], wherein the authors used a macro-scale approach in the simulation of impact loading of composite panels. The presented computational models allowed predicting the amount of absorbed energy with sufficient accuracy, but they did not provide a reasonable agreement between the computed and experimental fracture patterns. Also, there are difficulties with determining the parameters of the material model, which can be more than 30 and some of them can be selected only by calculation using the cut-and-try method. 1.2. Meso-scale (Ply/Yarn level) The meso-scale (ply/yarn-level) approach can be considered as a logical development of the macro-scale approach since the material layers/reinforcing yarns are still simulated as a continuous medium with orthotropic properties, but additional interface layers between layers/matrix material are also explicitly modelled. Fracture of these elements allows taking into account the composite delamination. There possible ways for interface layers modelling are as follows: cohesive elements with the corresponding material model (CZM); special contacts (tiebreak/breakable); common 3D elements with the corresponding material model. Hundreds of papers have been published, wherein the authors used cohesive elements in ply-level simulations of FRP impact loading [16-24]. This approach is quite effective and allows using both shell and solid elements in calculations. The use of cohesive elements involves two significant problems: 1. Sensitivity to the size of the finite elements (FE) mesh [25]. For an appropriate simulation of delamination using cohesive elements, it is necessary to have at least 3-4 elements in the crack-opening zone. Otherwise, it is necessary to adjust the properties defined experimentally for a particular mesh size in the computational model. 2. The results of static tests are used in a majority of cases to determine the parameters of the cohesive elements deformation model. The most popular tests are double-cantilever beam test and bending specimens with defects [26]. Then, it is necessary to introduce corrections for high strain rates, FE size etc. These problems are not an indicator that the use of cohesive elements is ineffective, or it gives false results. They are a signal to calibrate the computational model for specific tasks based on experimental results that are close to the simulated ones with a particular FE size. The second popular option in the meso-scale simulation of FRPs is the using of special contacts. For instance, in LS-DYNA software, the user can choose from several types of contacts formulations, including close to cohesive ones (OPTION=9). This approach is also one of the most popular in the simulation of delamination in composite structures subjected to impact loading [27-31]. The use of breakable contacts in the simulation is associated with the same difficulties as the use of cohesive elements: sensitivity to the FE size and the need to verify the parameters of the computational model based on dynamic tests data. In the case of dynamic loading, the efficiency of the use of cohesive elements and breakable contacts is almost identical [32]. Both approaches make it possible to obtain desirable results when there is enough experimental data for model verification. The third option is based on the using of standard three-dimensional elements that are used to simulate interface layers. Often this approach is used along with yarn-level models [33-35], but other options are possible [34]. The explicit matrix consideration in the simulation allows reducing the number of parameters in the model that require identification since it is possible to use simple material deformation models (linear elastic or elastic-plastic). The yarn-level approach or its combinations with ply-level one [36-41] is more often used to simulate 3D-reinforced composites under impact loading. The disadvantages of meso-scale approach include the increased (compared to the homogeneous approach) difficulties of the geometry and FE mesh creation and high computational cost. Impact tests and corresponding calculations are also required for verification of computational models. 1.3. Micro-scale (Fibre level) The use of micro-scale approach needs considerable attention to the accuracy of the composite microstructure accounting [42]. For example, Segala and Cavallaro [43] conducted studies on the impact loading of the composite based on UHMWPE applying filament-level. Micro-scale approach in its pure form is rarely used for practical calculations since the models’ computational cost and complexity in case large components will be enormous. A more common practice is the use of micro-scale simulation to obtain the integral properties of the composite layer for further macro-scale modelling [44]. 1.4. Prospective approaches for simulations of large size FRP components The given data suggest that simulations at the ply-level are the most commonly used to analyse the impact loading of structural FRPs. With a proper verification of the computational model, this approach allows obtaining an accurate assessment of the absorbed energy and the fracture pattern. At the same time, the use of this approach is associated with a computational cost increasing. This disadvantage becomes critical when modelling large parts. In this case, a combined approach can be very useful. The combined approach is a compromise between the dimensionality of the problem and the desire to obtain calculation results close to the experimental one. A layered geometric model is used in the impact zone and around it, but a homogenous approach is used in areas far from the impact site [45-47]. The connection of the model parts with different discretisation can be made in two main ways: shared nodes or specialised contact algorithms. Since there are only few works on this topic, there is not enough data about the advantages and disadvantages of both methods. Thus, meso-scale and combined approaches are the most prospective for simulation large-size FRP elements under impact loading. At the same time, to use the combined approach, it is necessary to have a working meso-scale computational model. In the next two sections, the features of simulation structural composites at the ply-level with the use of breakable contacts are considered on the example of CFRP plate. 2. Using of ply-level approach for numerical simulation of CFRP plate subjected to impact loading Computational studies of ballistic impact loading of the composite element were conducted to analyse the features of the meso-scale approach. The experimental results of ballistic impact testing of GFRP plates [48] were used for the validation of numerical models. In addition to computational studies, the following topics were shortly discussed: the main mechanisms of energy dissipation that must be taken into account in the developed models, the influence of the high strain rates the CFRP mechanical properties. 2.1 Main energy absorption mechanisms in composites during high-velocity impact The creation of effective numerical models for impact simulations requires an understanding of the primary energy dissipation mechanisms in composites during such loading. Consider some of the most cited papers where the authors studied the mechanisms of energy dissipation in composites under high-velocity impact loading. Morya et al. [49] conducted studies of the composites based on nylon, aramid, and UHMWPE fibres subjected to a steel ball impact. The developed and verified the analytical model of the composite-projectile interaction showed that the main part of the kinetic energy of the impactor is dissipated through the fracture of the primary yarns, elastic deformation of the composite and due to the kinetic energy transferred to the composite panel. Naik et al. (Indian Institute of Technology Bombay) published some work [50-57] with results of experimental and analytical studies of mechanical behaviour of CFRP, GFRP and hybrid composites under the high-velocity impact. The analytical model developed by the authors was quite similar with the model presented by Morya et al. The differences were in the accounting of the inhomogeneity of the deformations distribution in the composite fibres through the thickness, considering the additional mechanism of energy dissipation - shear plugging. During the researches, the authors found that the greatest amount of energy of a high-velocity projectile is dissipated by shear plugging, the acceleration of panel and fracture of the primary yarns. Similar results were obtained in [58] using numerical and analytical modelling and in [59] with the help of another analytical model. At the same time, in all these works, it was noted that the prevalence of one or another mechanism depends on the projectile velocity and geometry, composite thickness, material mechanical properties etc. It should be noted that the shear plugging fracture is typical for sufficiently thick composites and flat-end impactor. In the case of a spherical projectile, this phenomenon does not occur, that is confirmed by the results obtained in [48, 60-62]. Moreover, in [58, 59] authors showed that for thin composites, the contribution of energy dissipated by shear plugging into the overall balance is negligible. Based on the results of [58-62], it can be assumed that in the perforation of thick composites by flat-end impactors the main mechanism of energy dissipation is also the rupture of fibres due to their tension and bending, but not from the shear. A perforation scheme of the composite (Fig. 2) illustrates that. In the case of a flat-end projectile, the bending stress in the fibres near the point of contact is significantly higher than in the case of a spherical or ogival projectile, and it leads to pseudo-shear fracture. If this hypothesis is taken as a working one, it will mean that it is necessary to know and take into account the composite shear in the transversal direction for using of homogeneous approach. When using the meso-scale approach (consideration of the layered structure of the composite), the properties of the material in the plane are much more critical. Conclusions about the reliability of this hypothesis can be done only after the relevant computational studies. Fig. 2. Scheme of plug formation in the composite during high-velocity impact Regarding the remaining energy dissipation mechanisms in FRPs, the authors of papers [49-59] agree that the amount of the projectile kinetic energy absorbed by matrix cracking, and delamination is negligible. With the thickening of the material and in the case of through perforation, the role of friction between the projectile and the composite target increases. 2.2. Influence of the strain rates on the CFRP mechanical properties Nowadays, in the scientific community, there is no consensus about the changes of the CFRP mechanical properties at high strain rates. In work [63], the experimental data showed that the tensile strength of the material increased up to 55 % with increasing strain rate, while the elastic modulus and the ultimate strain increased by up to 20% and 36% respectively. In another work [64], it was found that depending on the tensile strength and the strain rate is almost linear. The increase in tensile strength was in the range from 9% to 43%. These results show significant changes in the properties of CFRP in comparison with other studies. For example, in [65-69], it was found that the tensile strength increased by 5-9%, 7%, 7.2%, 18% and 36% respectively. It should be noted that indirect methods are used to determine the properties of the composite at high strain rates in the vast majority of cases. This fact leads to an additional error in measurements. Also, the authors did not consider the physical reasons for increasing the characteristics of CFRP and carbon fibres. In [70, 71], the authors concluded that the properties of carbon fibre bundles could be considered independent of the strain rate. In [72] the authors during the yarn-level simulations and experimental research founded that the changes of the 3D-reinforced composite properties were associated with a change in the fracture mechanism and the influence of dynamic effects, but not with a change in the properties of fibres. Studies of the properties of unidirectional CFRP confirm this fact too. In work [73], it was found that the modulus of elasticity and tensile strength of unidirectional CFRP in the longitudinal direction do not depend on the strain rate. Based on the data of [70-73], it can be assumed that for CFRP based on fabrics (plain, twill, sateen etc.) changes in the integral properties at high rates will be the more significant, the higher the degree of curvature of the yarns. At the same time, the strength of the fabric-based composite will tend to the strength of the unidirectional composite with the same proportion of fibres in the direction of loading at high strain rates. This hypothesis requires additional confirmation. It is important to note that the loading conditions and the strain rates during high-velocity impact differ significantly from those in tensile tests. It means that test dynamic tensile tests data can be used only as of the first approximation for the model and additional calibration using results of high-velocity experiments as needed. The work [74] is a good example of this. 2.3. Description of the numerical models Numerical studies of CFRP plate impact loading were carried out to verify the findings of the literature review. A high-speed impact loading of a composite plate by a steel sphere is an initial boundary-value problem of the mechanics of a deformable solid. The principle of virtual work in a week form was used for the mathematical formulation of this problem: (1) Here, sij, εij are components of elastic stresses and strains tensors, and are components of displacements and accelerations vectors, pi is a vector of surface forces, r is a current density, V is a volume of deformable solids, S is an area subjected to surface forces. More details could be found in [75]. Numerical solution of equation (1) was carried out by the finite element method using LS-DYNA software with an explicit time integration scheme [76]. The ply-level approach was used in which the layered structure of the composite was considered explicitly. Calculation models were verified using experimental data published in [48]. The numerical models of the CFRP plates were created in LS-PrePost-4.5. All the computations were performed using the supercomputer «RSC Tornado SUSU» [77]. 2.3.1. Models geometry, boundary and initial conditions CFRP plates with a thickness of 4.67 mm based on a balanced fabric with lay-up [0°]24 and epoxy resin VSE-1212 [48] were considered during numerical simulations. In the geometry model, 24 layers of the real composite were replaced by 12 and 6 equivalent layers with thicknesses of 0.388 mm and 0.776 mm respectively to study the influence of the equal layers number on the simulations results. 8-nodes layered shell elements (ELEMENT_TSHELL) with ELFORM=5 formulation were used in all cases. Models with FE sizes of 2 mm, 3 mm and 4 mm (element edge length) were created to analyse mesh sensitivity of the model. One element was used through the thickness of equivalent layers. The interaction between the layers was taken into account by the contact algorithm discussed below. Figure 3 shows the mesh density and the number of equivalent plies for the all-using models. The projectile was modelled using 8-nodes solid elements (ELFORM=1). Maximum element size for projectile discretisation was equal to the size of FE in the composite model. Specimen size in the simulation had dimensions of 200 mm × 245 mm. The clamped part of the panel (55 mm) was not considered in the calculations directly. Experimental boundary conditions [48] were taken into account by a prohibition of all nodes displacements and rotations at the lower part of the specimens (Fig. 4). Preliminary simulations showed that the difference in predictions between the model being used and the full specimen model was insignificant. In accordance with [48], initial projectile velocities of 75.5 m/s, 84.5 m/s, 90.5 m/s, 110.5 m/s were considered during simulations for all mesh models. Fig. 3. The mesh density and the number of equivalent layers for all models Fig. 4. Scheme of the composite plate loading in the simulations 2.3.2 Material models and contacts Even though the authors of the work [48] did not provide any information about pre-preg, some signs (matrix type, the layer thickness of 0.19 mm, weave type) indicate that VKY-39 was most likely used [78]. This pre-preg was developed by All-Russian Institute Of Aviation Materials (VIAM). Some mechanical properties of CFRP made of this pre-preg with using different technologies could be found in [4]. Mechanical properties of the VKY-39 layer are presented in Table 1. Material density was 1525 kg/m3. Table 1 СFRP layer mechanical properties [4] E11, GPa E22, GPa G12, GPa n12 s11, MPa s22, MPa 64 64 4,1 0,3 810 810 A model of an orthotropic material *MAT_054 with fracture was used to describe the mechanical behaviour of the composite. In plane stress, the strain is given in terms of the stress as (2) Usually,

About the authors

O A Kudryavtsev

South Ural State University

M V Zhikharev

South Ural State University

N A Olivenko

South Ural State University

References

Statistics

Views

Abstract - 465

PDF (Russian) - 278