Jtam.dvi JOURNAL OF THEORETICAL AND APPLIED MECHANICS 50, 2, pp. 531-548, Warsaw 2012 50th Anniversary of JTAM INVESTIGATION OF AXIAL CRUSHING BEHAVIOUR OF A COMPOSITE FUSELAGE MODEL USING THE COHESIVE ELEMENTS F. Mustapha, N.W. Sim Universiti Putra Malaysia, Department of Aerospace Engineering, Serdang, Selangor, Malaysia e-mail: faizal@eng.upm.edu.my; weisim1984@yahoo.com A. Shahrjerdi University of Malayer, Department of Mechanical Engineering, Iran e-mail: alishahrjerdi2000@yahoo.com Finite element analysis (FEA) on a new fabrication miniature com- posite fuselage structure under axial compression loading is presented. ABAQUS/Explicit simulation is employed topredict the crushingbehavio- ur andmechanical strength fromthe initial compression loading to thefinal failuremode. AwovenC-glass fiber/epoxy 200g/m2 composite laminated with orthotropic elasticmaterial properties is used for the fuselagemodel. This proposed model is established to observe the crushing load and col- lapse modes under an axial compression impact. Adhesively bonded joint progression is generated using the technique of cohesive element. Various angles of the lamina are deliberated in the analysis to acquire and imagine the effect of the angle of orientation. Composite lamina angles are exami- ned and validated using FEAmodelling as a numerical parametric study. The results show that the finite element analysis using ABAQUS/Explicit can reproduce satisfactorily the load-deflection response. It can be conclu- ded that special cases of antisymmetric lamination are found to have the strongest resistance to the applied load. Key words: adhesively bonded joint, composite fuselage, FEA, crushing behaviour, C-glass fiber/epoxy, cohesive elements 1. Introduction The significant drawbacks of the filament winding composite fabrication pro- cess can be described in terms of expensive equipment, time-consuming pro- duction process and inflexibility regarding the shape of the structure to be 532 F. Mustapha et al. wound (Koussios et al., 2004). A novel fabrication method of a miniature composite fuselage was successfully investigated by Dahdi et al. (2009). In their research, they estimated the possibility of using the combining mould technique to replace themethod of filament winding by integrating thewoven fiber composite laminated with an adhesive butt joint. This technique can su- stain an axial compression impact from debonding failure. According to the advantages of this novel fabrication technique, it can be implemented in the real aerospace world. Recently, analytical and numerical methods have been studied by many researches to present the crushing behaviour on the composite tube and cylin- drical shells. Some researchers investigated the crushing response of composite shell subjects to axial compression (Chamis andAbumeri, 2005; Vaziri, 2007). Some investigations employedABAQUS as a numerical tool to crushing simu- lation and analysis. Bisagni (2005) studied dynamic buckling of thin-walled carbon fiber reinforced plastics (CFRP) shell structures under axial compres- sion. His approach was based on the equations of motion, which were nume- rically solved using a finite element code (ABAQUS/Explicit). He also used numericalmodels thatwere validated by experimental static buckling tests. In another interesting research, modelling of delaminated composite cylindrical shellswitha linearmaterial andunderaxial compressionwas consideredbyTa- freshi (2004, 2006). Nonlinear finite element analysis usingABAQUS/Explicit was employed byMahdi et al. (2001, 2006) to study the crushing behaviour of a filament-wound laminated cone-cone intersection composite shell. The vali- dation of their research was also experimentally investigated under a uniform axial load. They considered axially crushed cotton fibre composite corrugated tubes in their researches. In another research, experimental and numerical dy- namic responses with damagemodelling of filament wound glass/epoxy tubes were explored by Tarfaoui et al. (2008). Validation of experimental crushing behaviour of a filament wound C-glass fiber/epoxy 200g/m2 miniature fuse- lage using simulation technique was executed by Yidris and Mokhtar (2007). Mamalis et al. (2006) studied the crushing response of square carbon FRP tubes using finite element modelling subjected to static and dynamic axial compression. Xiao et al. (2009) and Zarei et al. (2008) investigated the cru- shing response of braided composite tubes and thermoplastic composite crash boxes, respectively. Crushing of conical composite shells were considered also by Morthorst and Horst (2006). These research works have been verified by experimental and numerical crushing simulation using LS-DYNA. ABAQUS/Explicit as anFEA’s software is employed in this research. The reliability of ABAQUS in performing non-linear analysis on crushing has been Investigation of axial crushing behaviour... 533 proven in the literature (Goyal and Johnson, 2008; Yang et al., 2009; Zhang et al., 2008). Furthermore, ABAQUS offers composite layups to facilitate the composite model set up. It can be added that ABAQUS allows the user to define the material properties in the modelling of the progressive damage of an adhesive bonded joint. In this paper, an FEA model on composite cylindrical structures with an adhesively bonded butt joint under axial compression is proposed to investi- gate the collapse modes and to compare various angular composite laminas. There aremanypublications available on the buckling analysis of filamentwo- und cylindrical shells and tubes subject to axial compression. To the authors’ knowledge, nopriorwork has been done in the area of crushing analysis on the adhesive bonded joint in a composite cylindrical shell structure with various angles of the lamina under axial compression. 2. FEA via ABAQUS/Explicit All physical structures are nonlinear, since a nonlinear structural problem is one inwhich the structure stiffness changes as it deforms. If the displacements in a model due to loading are relatively small during a step, the effects may be small enough and be ignored. However, in the cases where the loads acting on a model result in large displacements, nonlinear geometric effects can be- come important. A nonlinear analysis should be required to observe crushing responses from initial compression loading to final failure under geometrical- ly nonlinear deformations. Approaches of fracture mechanics are often used for simulation of damage propagation due to high-stress gradients appearing at crack fronts. The employment of solely stress-based criteria is not useful (Balzani and Wagner, 2008). The linear Elastic Fracture Mechanics (LEFM) approach is often employed in failure of the adhesive joint, and it can only be appliedwhen the starting crack exists andwhenmaterial nonlinearities can be neglected (Wimmer et al., 2006). Based on geometric andmaterial nonlineari- ty, a nonlinear solver to establish equilibrium is required. It can be explained that the geometric nonlinearity is due to large rotation kinematics and large strain, while the nonlinear material behaviour is due to degradation of the adhesivematerial properties and the stiffness during progressive failure of the damage initiation and evolutionmechanisms (Goyal andJohnson, 2008; Zhang et al., 2008). An incremental-iterative approach is taken for the nonlinear fini- te element analysis, and the Newton-Raphson method is utilized to trace the loading path of the structurewith a displacement-control analysis. During the 534 F. Mustapha et al. analysis for each load step, an additional iteration may be essential to verify whether there is another initiation of new failure events in individual elements. To obtain a converged solution maximum, the number of iterations is signifi- cant. The iteration is postponedwhen the routine cannot be reiterated with a smaller increment (Zhang et al., 2008). ABAQUS/Explicit is a special-purpose analysis product that employs an explicit dynamic finite element formulation. This product can be used for short, transient dynamic events, such as impact and blast problems, and is also very efficient for highly nonlinear problems involving changing contact conditions. ABAQUS also offers composite layups to facilitate the composite model set up, and the cohesive element technique allows theuser to definematerial properties in themodelling of the progressive damage of the adhesive bonded joint. It can be estimated that the results, on- ce the simulation has been completed, and the reaction forces, displacements, energy or other fundamental variables have been extracted. 3. Modelling process and FEA methodology An eight-layer composite orthotropic, woven C-glass fiber/epoxy 200g/m2 [908] with total thickness of 3mm is used to fabricate the fuselage structu- re. The fuselage dimensions are shown in Fig.1. Fig. 1. Fuselage structure section As it is shown in Fig.2 and Fig.3, in the geometric modelling process, the model consisted of two deformable parts for two fuselage sections, two adhesi- ve layers, and two rigid surfaces as tools (RS1 andRS2). It can be noted that the fuselage sections are bondedwith the zero thickness adhesive layers along the fuselage edge. The fuselage sections and adhesive elements are considered as deformable parts that can be deformed under applied loads. Tools are mo- delled as discrete rigid parts because they were much stiffer than the fuselage Investigation of axial crushing behaviour... 535 section. The discrete rigid part is assumed to be unbending, and is used in contact analyses tomodel bodies that cannot deform.RS1 is displaced 80mm downward at the Z-direction to crash toward the fuselage section bondedwith the adhesive joint; RS2 is fixed to hold in a position during axial loading. Fig. 2. Component arrangement In the finite element modelling, mesh convergence is studied for the mesh size 3, 5, and 8mm (Table 1). The agreement of the FEA with experimental results suggests that themesh used is adequate to predict the overall response accurately. In themeshingprocess, 3mmmesh size is employed in the fuselage modelling, because it is finer and more accurate as well as more realistic to capture thedeformationmodesof the structureunder compression loading. Fi- gure 4 shows themeshingmodel of the fuselage sections and the solid cohesive element. For cohesive meshing elements, a 3mmmesh size is employed in this rese- arch (Fig.4). Swept or offset meshing techniques should be used to generate the mesh in the cohesive layer because these tools produce meshes that are oriented consistently with the stack direction that is alignedwith the offset di- rection. The type of the cohesive element is COH3D8 for the adhesive bonded 536 F. Mustapha et al. Fig. 3. Assembled adhesive parts Table 1.Convergence study in themesh size Mesh size Mesh Peak load [mm] elements [kN] 3 11138 78 5 8316 76 8 3444 81 Fig. 4. Fuselage sections and solid cohesive meshing joint in ABACOUS package. It is considerable that the thickness of the co- hesive elements is defaulted to zero. The geometric region that represents the cohesive layer should be defined as a solid, even if the thickness of the layer is Investigation of axial crushing behaviour... 537 close to zero.To avoid numerical problems, it is recommended to use a value of 10−4 or greater for the thickness of the cohesive layer in themodelling process. If the actual thickness of the layer is less than this value, the actual thickness in the initial thickness field of the cohesive section editor should be specified. Themesh size of rigid surfaces was defined approximately 10mm for all edges of a part. The element shapewas considered quadrangle and an auto-meshing techniquewas used to generate themeshed structure. It can be noted that the mesh distortion can be decreased byminimizing themesh transition. 4. FEA mathematical process In the recent years, fracturemechanics has emerged as a theory which can be used successfully inbothderiving failure criteria anddeveloping computational tools. Fracture mechanics has also been used for simulation of delamination and adhesives (Trias et al., 2006). Thevirtual crack closure technique (VCCT) andcohesive elements are in themindsof all finite element softwaredevelopers. VCCT is based on the assumption that the energy released when a crack is opened from a to a+∆a is the same energy required to close the crack from the length a+∆a to the length a. A typical modelization of a single lap joint that can be employed in this research is shown in Fig.5. As it is shown there, the nodes in the adhesive region are connected through rigid links with a spring at their tip, as is performed generally. Fig. 5. Finite element modeling of the adhesive zone (Trias et al., 2006) 538 F. Mustapha et al. In the case of FEmathematicalmodelling, amesh encompassing the struc- ture is generated. The stiffness matrix of each element and the structure is determined. The loads applied to the structure are replaced by an equivalent force system such that the forces act at the nodal points. According to the basic FE formulation, it can be written Ku=F (4.1) where K and u represent the element stiffness matrix and the displacement vector. The displacements at a point inside the element are calculated by u=Nδ (4.2) where N is the matrix of the shape vectors. The strains at a point inside the elements are calculated by ε=Bδ (4.3) where, B is the strain-displacement matrix. The elastic behaviour is written in terms of an elastic constitutive matrix that relates the nominal stresses to the nominal strains across the interface. The corresponding nominal strains can be defined as εn = δn τ0 εs = δs τ0 εt = δt τ0 (4.4) where τ and δ denote the nominal traction stress vector and displacement fields, respectively, while the parameters with the subscript n, s and t re- present the nominal, shear and the area between the top and bottom of the cohesive layer, respectively. The stresses at a point inside the element are calculated by σ=Eε (4.5) where E is the stiffness matrix characterising the composite material. The element stiffness matrix is K= ∫ V B ⊤ EB dV (4.6) where V is the volume of the element. The cohesive element formed by 4 nodes (n= 2) can be used to connect continuum plane strain elements with two degrees of freedom per node. The cohesive element formed by 8 nodes (n = 3) can be used to connect three- dimensional continuum elements with three degrees of freedom per node. The Investigation of axial crushing behaviour... 539 constitutive equations of the cohesive element relate the tractions τi at the midsurface of the element to the displacement jumps ∆m. The contribution of the element to the tangent stiffness matrix and to the residual vector, i.e., the internal force vector of the cohesive element can be shown fKi = ∫ Γdi τiBimK dΓd (4.7) where BimK =ΘimNK (4.8) The rotation tensor Θim relates the global and the local coordinates. The so- ftening nature of the cohesive element constitutive equation causes difficulties in obtaining a converged solution to the non-linear problem when using the Newton-Raphson iterative method. TheNewton-Raphsonmethod is based on Taylor’s series expansion of a set of nonlinear algebraic equations. The equ- ations must be solved using an iterative method. To formulate the equations to be solved at the (n+1)-st iteration by the Newton-Raphson method, it is assumed that the solution at the n-th iteration is known. In particular, quadratic convergence is not assured because the residual vector is not con- tinuously differentiable with respect to the nodal displacements. The tangent stiffness matrix stems from the linearization of the internal force vector and it is obtained using Taylor’s series expansion. Taking into account that the calculation of the geometric terms of the tangent stiffness matrix is computa- tionally very intensive, these terms are neglected.The tangent stiffnessmatrix, Krzik, for the cohesive element is therefore approximated as Kjkrz ≈ ∫ Γd BijkD tan in Bnrz dΓd (4.9) where Dtanin is the material tangent stiffness matrix, or a constitutive tangent tensor used to define the tangent stiffness matrix. It depends on the interfa- cial constitutive model adopted. The process of degradation begins when the stresses and/or strains satisfy certain damage initiation criteria. Damage is assumed to initiate when the maximum nominal stress ratio reaches a value of one. This criterion can be expreseed as in equation (4.10) max {Tn T0n , Ts T0s , Tt T0t } =1 (4.10) where T0n, T 0 s and T 0 t represent the peak values of the nominal stress when the deformation is either purely normal to the interface or purely in the first 540 F. Mustapha et al. or second shear direction, respectively. The symbol 〈 · 〉 used represents the Macaulay bracket with the usual interpretation. The Macaulay brackets are used to signify that a pure compressive deformation or stress state do not initiate damage. 5. Material properties Thematerial properties of each layer of fiberglass 200g/m2 are obtained from the material characterisation test data that was cited by Dahdi et al. (2009). The summary ofmechanical properties of C-glass/epoxy 200g/m2 is shown in Table 2. Table2.Mechanical propertiesofC-glass/epoxy200g/m2 (Dahdi et al., 2009) Properties C-glass/Epoxy 200g/m2 E11 3.5GPa E22 3.5Gpa ν12 0.158 G12 2.340Gpa G13 2.340Gpa G23 2.340Gpa Formanymaterial systems, the fracture toughness can bemeasured expe- rimentally; however, the value of separation at the final failure as well as the shape of the softening portion of the traction-separation relationmay be diffi- cult, if not impossible, to determine. Thus, it is easier to use an energy-based damage evolutionwith linear softening behaviour. The adhesive bondbetween the layers is modelled using the cohesive element functionality via ABAQUS (Lapczyk and Hurtado, 2007). A triangular traction-separation cohesive law with linear softening is used to represent themechanical response of the cohe- sive element. Adhesive epoxy material properties in Table 3 are also used in the proposed model (Lapczyk and Hurtado, 2007). Herein, Kn, Ks, and Kt are the initial interface stiffnesses, and T o n, T o s and Tot are the interface strengths. GIC, GIIC and GIIIC also define the interface fracture toughness and the modal dependence of damage evolution. The parameters coming with the subscript n, s and t represent the material properties at the normal mode, first and second shear direction, respectively. Investigation of axial crushing behaviour... 541 Table 3. Summary of mechanical properties of adhesive epoxy (Lapczyk and Hurtado, 2007) Properties Adhesive epoxy Kn 2000MPa Ks 2000MPa Kt 2000Mpa Ton 50MPa Tos 50MPa Tot 50MPa GIC 4N/mm GIIC 4N/mm GIIIC 4N/mm ν 0.33 6. Results and disscussion FEA results of the fuselage model with the cohesive elements obtained using ABAQUS/Explicit for the deformation modes, and load-displacement are shown in Figs.6 and 7. Fig. 6. Load-displacement vs. axial force It can be seen that in Fig.6, at the beginning of the loading operation, the applied load rises linearly up to point 2, where the loadmaximum is obtained. The maximum recorded load at point 2 was 78kN at 2.4mm displacement. In the next step, the load-displacement curve drops off suddenly to point 4. 542 F. Mustapha et al. During compression of 5.2mm at point 4, debonding was observed between the fuselage sections. Figure 7 clearly shows the collapse modes at each stage. Fig. 7. Collapsemodes from FEAmodel 7. Verification of FEA modelling It can be concluded that there is a good agreement between the experimental and FEA results throughout the loading process (Fig.8). The tendency thro- ugh the crushing loading for both experiment and simulation is very close. Clearly, the applied load at the start of the loading process increases linear- ly up to the point where the load maximum is reached. It can be seen that after the maximum loading step, the experimental and the numerical load- displacement curves drop off sharply at nearly the same displacement. Investigation of axial crushing behaviour... 543 From the visual comparison of the peak load value achieved by the experi- ment and the numerical analysis in Table 4, the peak load for the experiment specimen is 77kN and 78kN for the numerical results. One-percent error is estimated for the peak load between the experiment and the failure theories used to simulate the progressive damage (see Table 4). According to Figs.8 and 9, the collapse modes and crushing behaviour for both the experiment and simulation are found correlated. Table 4.Peak load deviation [%] between FEA and experimental results Test Peak load Displacement [kN] [mm] FEA simulation 78 2.4 Experiment test 77 3.79 Discrepancy [%] 1 39 Fig. 8. Load-displacement vs. axial force for comparing experimental and FEA results Fig. 9. Collapse modes for experimental test vs. FEA results 544 F. Mustapha et al. 8. Parametric study The finite element results show a good agreement with the experimental ones, and give confidence in replacing very time consuming actual quasi-static tests with computer simulations. After confirmation of numerical analysis by an experimental study, the effect of the angle of orientation and special cases of laminates on the crushing behaviour of a C-glass/epoxy fuselage section by FEA can be discussed and presented. To obtain and visualize the effects of each angle orientation of the lami- na, various angles of the lamina are deliberated. As can be seen from Ta- ble 5, fuselage sections that are modelled in this study consisted of 8 plies of C-Glass/Epoxy 200g/m2 in the special cases of laminates (Bisagni, 2005). Symmetric, cross-ply, angle-ply, antisymmetric, balanced and quasi-isotropic laminates are all types of lamina models that are examined in this research. Table 5. Special cases of laminates Laminate Orientation Abbreviation Antisymmetric [454/-454] Antisym Angle-ply symmetric [-45/45/-45/45]s APLSym Angle-ply [-45/45/-45/45/-45/45/-45/45] APL Cross-ply symmetric [0/90/0/90]s CPLSym Cross-ply [0/90/0/90/0/90/0/90] CPL Balanced [45/-45/-45/45/-45/-45/45/45] BalL Quasi-isotropic [45/-45/90/0]s QuaIso The results obtained from the load-displacement response for the special cases of laminates are shown in Figs.10 and 11 and Table 6, when they are applied to the fuselage sections. It is apparent from these figures that there are twopatterns of load-displacement curves, namely the pattern X (i.e.CPLSym with CPL) and Y (i.e. Antisym, APLSym, APL, BalL with QuaIso). The pattern X seems to have more resistance to the applied load than Y . The most striking result emerging from FEA is more or less the same amount of peak load for laminates Antisym, APLSym, APL and BalL namely 90kN (Table 6). As can be seen fromTable 6, CPLSymandCPL laminates seem to have approximately the same amount of peak load, 78-80kN. Further analysis showed that QuaIso laminated peak load goes down between the two groups that are 85kN.This study confirmed that both patternsmore or lessmaintain constant loads after reaching the lowest load and fail at an approximately 2.4mmdisplacement. It can be said thatCPLSymandCPLwere foundgiving similar trends to the baseline model of [908]. Investigation of axial crushing behaviour... 545 Table 6.Baseline and special cases comparison for the peak load and displa- cement of laminates Test Peak load Displacement [kN] [mm] Baseline 78 2.4 Antisymmetric 91 2.4 Angle-ply symmetric 90 2.4 Angle-ply 90 2.4 Cross-ply symmetric 80 2.4 Cross-ply 78 2.4 Balanced 90 2.4 Quasi-isotropic 85 2.4 Fig. 10. FEA load-displacement curve of special laminates 9. Conclusion In this research, FEA simulation of a fuselage structure under axial com- pression loading is investigated to predict the crushing behaviour andmecha- nical strength. A woven C-glass fiber/epoxy 200g/m2 composite laminated with orthotropic elastic material properties is modelled by employing ABA- QUS/Explicit. Various angles of the lamina are considered in the analysis to obtain the effect of the angle of orientation. The following summary may be drawn: • Finite element analysis usingABAQUS/Explicit can reproduce accepta- ble load-deflection responses compared with the experimental works. 546 F. Mustapha et al. Fig. 11. FEA load-displacement curve of special laminates (Enlarged) • Finite element simulation results concerning themain crushing characte- ristics such as the peak load and crush energy absorption are very close to the experimental results. • Using ABAQUS/Explicit, a reliable FEAmodel to predict the adhesive joint of composite fuselage structure was successfully developed. • The adhesive joint was successfully modelled utilizing the cohesive ele- ments to predict the adhesive behaviour and strength. • The validated FEA model was also applied for parametric study, and was used to provide a good insight on how the ply orientation affects the structure strength. • It can be suggested that antisymmetric lamination is found to have the most resistance to the applied load. Acknowledgment This research was supported by Fundamental Research Grant Scheme (FRGS5524003). References 1. BalzaniC.,WagnerW., 2008,An interface element for the simulation of de- lamination in unidirectional fiber-reinforced composite laminates, Engineering Fracture Mechanics, 75, 9, 2597-2615 2. Bisagni C., 2005, Dynamic buckling of fiber composite shells under impulsive axial compression,Thin-Walled Structures, 43, 3, 499-514 Investigation of axial crushing behaviour... 547 3. Chamis C.C., Abumeri G.H., 2005, Probabilistic dynamic buckling of com- posite shell structures,Composites PartA:Applied Science andManufacturing, 36, 10, 1368-1380 4. Dahdi I., Edi Y., Mustapha F., Zahari R., 2009, Novel fabrication for tubular and frusto conical composite product for aerospace application,Confe- rences Proceeding of Aerotech III 5. Goyal V.K., Johnson E.R., 2008, Predictive strength-fracture model for composite bonded joints,Composite Structures, 82, 3, 434-446 6. Koussios S.,BergsmaO.,BeukersA., 2004,Filamentwinding.Part 1:De- terminationof thewoundbody relatedparameters,Composites Part A:Applied Science and Manufacturing, 35, 2, 181-195 7. Lapczyk I., Hurtado J.A., 2007, Progressive damage modeling in fiber- reinforced materials,Composites Part A: Applied Science and Manufacturing, 38, 11, 2333-2341 8. Mahdi E.,MokhtarA., Asari N., Elfaki F., AbdullahE., 2006,Nonli- nearfinite element analysis of axially crushed cottonfibre composite corrugated tubes,Composite Structures, 75, 1/4, 39-48 9. Mahdi E., Sahari B., Hamouda A., Khalid Y., 2001, An experimental investigation into crushing behaviour of filament-wound laminated cone-cone intersection composite shell,Composite Structures, 51, 3, 211-219 10. MamalisA.,ManolakosD., IoannidisM., PapapostolouD., 2006,The static and dynamic axial collapse of CFRP square tubes: finite elementmodel- ling,Composite Structures, 74, 2, 213-225 11. Morthorst M., Horst P., 2006, Crushing of conical composites shells: a numerical analysis of the governing factors,Aerospace Science and Technology, 10, 2, 127-135 12. Tafreshi A., 2004, Efficient modelling of delamination buckling in composi- te cylindrical shells under axial compression, Composite Structures, 64, 3/4, 511-520 13. Tafreshi A., 2006, Delamination buckling and postbuckling in composite cy- lindrical shells under combined axial compression and external pressure,Com- posite Structures, 72, 4, 401-418 14. Tarfaoui M., Gning P., Hamitouche L., 2008, Dynamic response and damage modeling of glass/epoxy tubular structures: Numerical investigation, Composites Part A: Applied Science and Manufacturing, 39, 1, 1-12 15. Trias D., Rojo R., Nuin I., Lasa M., 2006, Fracture mechanics and new techniques and criteria for the design of structural components for wind turbi- nes, Technical paper presented at EWEC06. 16. Vaziri A., 2007,On the buckling of cracked composite cylindrical shells under axial compression,Composite Structures, 80, 1, 152-158 548 F. Mustapha et al. 17. Wimmer G., Schuecker C., Pettermann H., 2006, Numerical simulation of delamination onset and growth in laminated composites, The e-Journal of Nondestructive Testing, 11, 1-10 18. Xiao X., McGregor C., Vaziri R., Poursartip A., 2009, Progress in braided composite tube crush simulation, International Journal of Impact En- gineering, 36, 5, 711-719 19. Yang Z., Su X., Chen J., Liu G., 2009,Monte Carlo simulation of complex cohesive fracture in randomheterogeneousquasi-brittlematerials, International Journal of Solids and Structures, 46, 17, 3222-3234 20. Yidris H.N.,MokhtarA.M., 2007,Crush Simulation and Experimental Va- lidation of a Composite Unmmaned Aerial Vehicle Fuselage Section, Universiti PutraMalaysia, pp.161 21. Zarei H., Kroeger M., Albertsen H., 2008, An experimental and nu- merical crashworthiness investigation of thermoplastic composite crash boxes, Composite Structures, 85, 3, 245-257 22. Zhang Z., Chen H., Ye L., 2008, Progressive failure analysis for advanced grid stiffened composite plates/shells,Composite Structures, 86, 1/3, 45-54 Badania przebiegu osiowego zgniatania modelu kompozytowego kadłuba z wykorzystaniem elementów kohezyjnych Streszczenie Pracę poświęcono analizie elementów skończonychw zastosowaniu do badańmo- delu miniaturowego kadłuba wykonanego z laminatu i poddanego osiowemu ściska- niu. Przeprowadzono symulacje numeryczne z użyciem komercyjnego oprogramowa- nia ABAQUS/Explicit w celu określenia wytrzymałości kompozytu oraz zbadania przebiegu procesu zgniatania, aż do uzyskania ostatecznej postaci zniszczenia prób- ki. Na materiał kadłuba wybrano kompozyt w włóknem szklanym typu C o gęstości 200g/m2 i właściwościach ortotropowych. Podczas badań obserwowano pojawianie się kolejnych postaci wgnieceń, aż do zupełnej utraty stateczności układu przy udaro- wymobciążeniu ściskającym.Zastosowanometodę elementówkohezyjnychdo analizy zmianw adhezyjnympołączeniuwarstw laminatu. Zbadanowpływ kąta laminowania na właściwości próbki. Przeprowadzono także badania parametryczne wpływu kąta laminowania modelu metodą elementów skończonych. Uzyskane wyniki wykazały, że symulacje wykonane w systemie ABAQUS/Explicit wiarygodnie odtwarzają rzeczy- wisty przebieg zgniatania w funkcji przykładanego obciążenia. Zaobserwowano rów- nież, że niektóre przypadki laminowania antysymetrycznego są szczególnie odporne na zniszczenie wywołane siłą osiową. Manuscript received July 18, 2011; accepted for print October 7, 2011