EFFICIENT NUMERICAL TECHNIQUES FOR PREDICTING PROCESS-INDUCED STRESSES A N D DEFORMATIONS IN COMPOSITE STRUCTURES by A B D U L RAHIM A H A M E D A R A F A T H B.Sc, University of Peradeniya, 1998 M.A.Sc , The University of British Columbia, 2002 A THESIS SUBMITTED IN PARTIAL FULFILMENT OF THE REQUIREMENTS FOR THE DEGREE OF DOCTOR OF PHILOSOPHY in THE F A C U L T Y OF GRADUATE STUDIES (Civil Engineering) THE UNIVERSITY OF BRITISH COLUMBIA April 2007 © Abdul Rahim Ahamed Arafath, 2007 Abstract During the last two decades of research work in numerical modelling of autoclave processing of composite structures, several models have been developed ranging from simple one-dimensional elastic to sophisticated three dimensional viscoelastic models. Some of the common problems faced by these numerical models are the non-familiarity of general users with these models, their non-versatility, their inefficiency when running large problems and the interpretation and validation of the results produced by these models. The main objective of this research work is to initiate the development of the next generation process model for autoclave processing of composite structures to address the above problems. This development is carried out by building on the already established knowledge of process modelling within the UBC Composites Group. The developed next generation process model consists of a set of numerical tools which range in complexity from a simple and robust closed-form analytical tool to a more general and adaptive shell-based finite element analysis tool that provides a modeller with a choice depending on the time and cost constraints. According to the developed closed-form solution, the axial stress variation in the thickness direction of a flat composite part varies exponentially with the through-thickness coordinate and its gradient depends on the part material and geometrical properties. It is shown that the process-induced unbalanced moment develops mainly at the initial stages of the curing process where the through-thickness stress gradient is significant. The process-induced effects in a curved part due to the thermal strain mismatch between the part and the tool in the tangential direction is similar to the process-induced effects in a flat part. Apart from the tangential thermal strain mismatch, the radial thermal strain mismatch between the part and the tool also induces stresses in a curved part. These stresses are due to the radial and tangential constraints applied by the tool on the part to conform the part to the tool shape. The unbalanced moment due to these stresses mostly develop at the cool-down portion of the cure cycle when the material is fully cured. ii Table of Contents Table of Contents Abstract ii Table of Contents iii List of Tables viii List of Figures x List of Symbols xxv Acknowledgements xxviii Chapter 1. Introduction and Background 1 1.1. Background 1 1.2. Research Objectives and Thesis Outline 2 Chapter 2. Modular Approach to Process Modelling 6 2.1. Introduction 6 2.1.1. Objectives 8 2.2. COMPRO Component Architecture (CCA) for Composite Materials 8 2.3. Sequentially-Coupled Thermal-Stress Analysis using ABAQUS 9 2.3.1. Heat Transfer Analysis 9 2.3.2. Stress Analysis 11 2.4. Verification Problems 13 2.4.1. Example 1 13 2.4.2. Example 2 14 2.4.3. Example 3 14 2.5. Warpage of a Flat Part 15 2.6. Spring-in of an L-Shaped Composite Part 16 2.7. Discussion 16 2.8. Summary and Contributions 17 Chapter 3. Surface Finish of Automotive Composite Parts Manufactured by R T M 30 3.1. Introduction 30 3.1.1. Definition of Surface Texture 31 iii Table of Contents 3.1.2. Factors that Affect Surface Quality of a Composite Panel 32 3.1.3. Numerical Modelling of Surface Waviness 34 3.1.4. Objectives 35 3.2. Numerical Prediction of Surface Waviness 36 3.2.1. Simulation of R T M Process 36 3.2.2. Identifying the Sources of Surface Waviness 36 3.2.3. Surface Deformation due to Micro-Level Stresses 37 3.2.4. Surface Deformation due to Macro-Level Stresses 46 3.3. Discussion 47 3.4. Summary and Contributions 47 Chapter 4. Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures.. 71 4.1. Introduction 71 4.1.1. Locking Phenomena and Remedies 72 4.1.2. Objective 75 4.2. 24-Noded Standard Solid Element 76 4.2.1. ABAQUS User Element Concept 76 4.2.2. Element Formulation 77 4.2.3. Numerical Integration 77 4.2.4. Geometric Description and Calculation of Jacobian Matrix 79 4.2.5. Formulation of B Matrix 79 4.2.6. Element Property Definition 80 4.2.7. Load 82 4.2.8. Pseudo Finite Element Code 83 4.3. Verification Examples 85 4.3.1. Sensitivity of Aspect Ratio of the Elements 85 4.3.2. Skew Sensitivity of the Elements 86 4.3.3. Ring under Point Load 87 4.3.4. Sandwich Cantilever Beam under Uniform Load 88 4.4. Prediction of Process-Induced Stresses and Deformations in Composite Parts during Curing Process 89 4.4.1. Warpage of a Flat Composite Part 89 4.4.2. Process-Induced Deformation of a Half Circular Composite Part on Solid Tool 90 4.4.3. Spring-in of L-Shaped Composite Part 91 4.5. Discussion 91 iv Table of Contents 4.6. Summary and Contributions 93 Chapter 5. Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part 114 5.1. Introduction 114 5.2. Theoretical Development 116 5.2.1. Homogeneous beam with shear traction specified at the bottom surface only 118 5.2.2. Two fully bonded homogeneous beams 119 5.2.3. Two homogeneous beams separated by an interface layer 121 5.3. Numerical Examples and Verification 122 5.3.1. Two fully bonded Beams: Beams 1 and 2 are isotropic 123 5.3.2. Two fully bonded Beams: Beam 1 is isotropic and beam 2 is orthotropic 123 5.3.3. Two beams separated by an interface layer: Beam 1 is isotropic and beam 2 is orthotropic 124 5.3.4. Two fully bonded Beams: Beam 1 is isotropic and beam 2 is a composite beam with multi layers 125 5.4. Warpage Prediction 129 5.4.1. Calculation of Effective Bending Rigidity 130 5.4.2. Warpage prediction compared to finite element results 132 5.5. Discussion 133 5.5.1. Influence of Initial Resin Modulus 133 5.5.2. Scaling Law 134 5.5.3. Simulation of Experimentally Observed Tool-Part Interaction with a Thin Interface Layer 134 5.5.4. Variation of Warpage with Part Lay-up 138 5.6. Summary and Contributions 139 Chapter 6. Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part 168 6.1. Introduction 168 6.2. Stresses due to Tangential Thermal Strain 169 6.2.1. Theoretical Development 169 6.2.2. Example: Stresses in a Unidirectional Composite Part on a Rigid Tool 172 6.3. Stresses due to Radial Thermal Strain 177 6.3.1. Theoretical Development 177 6.4. Curved Composite Part on a Deformable Tool 183 6.4.1. Stresses due to Tangential Thermal Strain Mismatch 183 v Table of Contents 6A.l. Stress due to Radial Thermal Strain Mismatch 185 6.5. Prediction of Process-Induced Deformations 186 6.6. Discussion 188 6.6.1. Scaling law 188 6.6.2. Variation of Warpage with the Properties of Interface Layer 190 6.6.3. Male and Female Tools 190 6.6.4. Simplification of the Solution for the Displacement due to Thermal Strain Mismatch in Radial Direction 190 6.6.5. Estimating Spring-in Angle using Nelson and Cairn's Equation 192 6.7. Summary and Contributions : 194 Chapter 7. Higher Order Finite Element Techniques for Process Modelling 228 7.1. Introduction 228 7.1.1. p- Refinements or Hierarchical Concept 230 7.1.2. h- Refinement in Thickness Direction or Layerwise Element Concept 232 7.1.3. Objective 233 7.2. Higher - Order Element Formulation :234 7.2.1. Numerical Integration 235 7.2.2. Material Orientation 235 7.2.3. Geometric Description 235 7.2.4. Displacement Interpolation 236 7.3. Verification Examples 240 7.3.1. Stress Variation in a Flat Composite Part on a Tool under Constant Thermal Load 240 7.3.2. Warpage Prediction of Flat Composite Part Cured under a Prescribed Cure Cycle 241 7.3.3. Bending of a Cantilever Sandwich Beam 243 7.3.4. Selection of number of terms or number of element layers 244 7.3.5. Reducing the Run Time in the Hierarchical Method 245 7.4. Warpage Prediction 247 7.5. Summary and Contributions 250 Chapter 8. Summary, Conclusions and Future Work 271 8.1. Summary 271 8.2. Conclusions 272 8.3. Future work 274 References 276 vi Table of Contents Appendix A. C C A Module for the ASS4/8552 Material 289 Appendix B. C C A Module for the Glass Fibre Reinforced Polyester Material 296 vii List of Tables List of Tables Table 3.1 Definition of surface waviness by different authors 49 Table 3.2 A comprehensive definition of surface waviness given by Karpala [Karpala (1993)] 49 Table 3.3 Material and geometrical parameters and their effects on surface finish 49 Table 3.4 Long-term and short-term surface waviness for different fibre preform types 50 Table 3.5 Surface roughness values for different fibre preform types 50 Table 4.1 Sensitivity of the aspect ratio of the elements. Predicted tip deflection of the cantilever beam normalized with respect to the exact (beam theory) solution for different mesh density 95 Table 4.2 Skew sensitivity of the elements. Predicted tip deflection of the cantilever beam normalized with respect to the exact solution for different element shapes and skew angles. The mesh size is 10*1 95 Table 4.3 Normalized vertical deflection at the loading point for the ring loaded with point loads (Isotropic case) 95 Table 4.4 Mechanical properties of the composite material used for the ring problem under point load .96 Table 4.5 Normalized vertical deflection at the loading point for the ring loaded with point loads (Orthotropic case) 96 Table 4.6 Sensitivity of warpage of a flat unidirectional composite part to the number of elements (24-noded) in-plane and through-thickness direction. Also shown are computational run times (clock . time) 97 Table 4.7 Warpage of flat composite part with different lay-ups 97 Table 4.8 Sensitivity of the tip deflection of quarter circular unidirectional composite part to the number of elements in-plane and through-thickness direction 97 Table 4.9 Comparison of tip deflection of a curved unidirectional composite part using cylindrical and rectangular coordinate systems to describe the element material coordinate system 98 Table 5.1 Material and geometrical properties of aluminum and steel beams for the case of two fully bonded isotropic beams subjected to thermal load 141 Table 5.2 Composite material properties at different curing stages of resin used for the analysis of stress variation in a composite part on an aluminum tool and subjected to thermal load 141 Table 5.3 Variation of the warpage of a unidirectional composite flat part fully bonded to an aluminum tool with part length and thickness. The closed-form results are compared with finite element predictions. For the finite element analysis, the run time (clock time) is also shown 142 vi i i List of Tables Table 5.4 Variation of the warpage of a composite flat part with part lay-up. The part is 600 mm long and 8 layer (1.6 mm) thick and it is separated from the tool with a thin interface layer. The closed-form results are compared with finite element predictions 142 Table 5.5 Closed-form results of the variation of warpage with part thickness and part length for different values of initial resin modulus 143 Table 5.6 Experimental warpage results for flat unidirectional composite parts with different number of layers and part lengths [Twigg et al. (2004)] 143 Table 5.7 Comparison of the warpage prediction by closed-form solution with the experimental results by Twigg [Twigg et al. (2004)]. The adjusted experimental results according to the trend given by Equation (5.50) are also shown. The matched warpage values in each set of experiments to calibrate the shear layer properties are highlighted 144 Table 5.8 Comparison of the warpage prediction by closed-form solution with the experimental results by Petrescue (2005) 145 Table 6.1 Mechanical properties of composite material at 4 different curing stages. These properties are used for the analysis of stress variation in a curved composite part under thermal load 195 Table 6.2 Thermo-mechanical properties of aluminum tool and Composite part. These properties are used for the analysis of stress variation in a curved composite part fully bonded to a curved tool and subjected to thermal load 195 Table 6.3 Variation of warpage of a unidirectional curved composite part on an aluminum tool separated by a thin interface layer with part length and thickness. The closed-form solutions are compared with finite element results 196 Table 7.1 Material properties of the CFRP composite part and the aluminum tool used for the analysis of axial stress variation in a composite part on a tool and subjected to thermal load 252 Table 7.2 Material properties of the shear layers used in the analysis of variation axial stress distribution in thickness direction with shear layer properties 252 Table 7.3 Material properties of the composite skin and the soft core of a sandwich beam under uniformly distributed load 252 Table 7.4 The selected number of element layers for the layerwise element used to simulate the experiments conducted by Twigg [Twigg et al. (2004a, 2004b)] 253 Table 7.5 Comparison of the warpage prediction by the layerwise element with contact surface with the experimental results [Twigg et al. (2004)]. The adjusted experimental results according to the trend given by Equation (5.50) and the closed-form solution with shear layer are also shown. The matched warpage value in the first set of experiment to characterize contact surface ( r m a x ) is highlighted.253 ix List of Figures List of Figures Figure 2.1 Flow chart illustrating the integrated sub-model approach used to model the processing of composite structures 19 Figure 2.2 Different numerical techniques and material constitutive models used in the current process modelling techniques available in the literature 19 Figure 2.3 Schematic showing the sub-model structure used in COMPRO [Johnston (1997)] 20 Figure 2.4 The COMPRO Component Architecture (CCA) developed to incorporate composite behaviour during cure in a commercial finite element code 20 Figure 2.5 A generalized finite element module with an evolving composite material constitutive behaviour 21 Figure 2.6 Typical 2-hold temperature cure cycle 21 Figure 2.7 A composite laminate with a stack of 8 unidirectional layers. Boundary conditions for (a) heat transfer analysis and for (b) stress analysis are shown 22 Figure 2.8 Comparison of the temperature profile along the cure cycle at top and bottom of the unidirectional composite part from COMPRO and CCA/ABAQUS 22 Figure 2.9 Comparison of the development of axial and transverse stresses along the cure cycle at the highlighted element of the unidirectional composite part from COMPRO and CCA/ABAQUS 23 Figure 2.10 Comparison of temperature profiles along the cure cycle for a 20 mm composite cube with different lay-ups (a) [0]8 (b) [45]8 (c) [90]8 from COMPRO and CCA/ABAQUS 24 Figure 2.11 Modelling the unidirectional composite cube with (a) solid and (b) shell elements for thermal analysis in CCA/ABAQUS 25 Figure 2.12 Comparison of the temperature profile along the cure cycle obtained using 8 solid elements (8-noded) and one shell element (4-noded) in thickness direction in CCA/ABAQUS 25 Figure 2.13 Schematic of a flat composite part on a solid tool 26 Figure 2.14 Schematic of the boundary conditions applied on the tool-part assembly (a) before and (b) after tool removal 26 Figure 2.15 Portion of the finite element mesh of the composite part and the tool used to study the process-induced deformation 26 Figure 2.16 Comparison of the warpage prediction of the unidirectional composite flat part after tool removal by COMPRO with CCA/ABAQUS with and without plane strain condition 27 Figure 2.17 Schematic of an L-shaped unidirectional composite part on a solid aluminum tool 27 x List of Figures Figure 2.18 Finite element mesh of the L-shaped part and the tool and the thermo-mechanical boundary conditions applied before and after tool removal 28 Figure 2.19 Schematic describing the measurement of the warpage and the corner components of the spring-in angle of an L-shaped part 28 Figure 2.20 Comparison of spring-in angle of an L-shaped unidirectional composite part predicted by COMPRO and CCA/ABAQUS with and without the plane strain condition 29 Figure 3.1 Schematic description of the RTM process 51 Figure 3.2 Schematic showing the definition of surface texture of a metallic surface 51 Figure 3.3 Schematic of the model showing a pair of fibres in parallel embedded in a resin matrix used by Kia (1986) to study surface waviness 52 Figure 3.4 Schematics of the model of woven composites used by Sanfeliz et al. (1992) to study surface waviness 52 Figure 3.5 Schematic of a composite C-shaped part in an aluminum closed mould in R T M processing .53 Figure 3.6 Typical 2-hold temperature cure cycle used for curing of polyester resin 53 Figure 3.7 Schematic of the possible deformed shape of the of a C-shaped composite part processed using R T M 54 Figure 3.8 Schematic of the dimpling between two adjacent fibres due to thermal strain mismatch between fibre and resin 54 Figure 3.9 Schematic of the C-shaped part inside the mould and the selected R V E close to the top tool surface. The applied boundary condition on the RVE before and after tool removal is also shown..55 Figure 3.10 Schematic of a unidirectional continuous fibre laminate 55 Figure 3.11 Schematic of the ideal fibre arrangement (square and hexagonal) in unidirectional fibre composite laminate 56 Figure 3.12 Schematic of the fibre spatial distribution in a unidirectional fibre laminate (a) square arrangement (b) hexagonal arrangement and (c) random arrangement 56 Figure 3.13 Finite element mesh of (a) square arrangement (b) hexagonal arrangement, and (c) part of random fibre arrangement 57 Figure 3.14 Comparison of surface deformation of square, hexagonal and random fibre arrangements....58 Figure 3.15 Schematic of random short fibre composite 58 Figure 3.16 Typical fibre length distribution (FLD) of the fibres in a random fibre mat 59 Figure 3.17 Definition of in-plane and out-of-plane fibre orientation of a fibre in a random short fibre mat 59 xi List of Figures Figure 3.18 Experimentally observed fibre orientation distribution (FOD) of a typical random fibre mat 60 Figure 3.19 Fibre length distribution (FLD) used in the analysis of the surface deformation of a part with random short fibre mat 60 Figure 3.20 Definition of centroidal position and the in-plane orientation of the fibre in the process of randomly generating the fibre in a random short fibre mat 61 Figure 3.21 Fibre orientation distribution (FOD) used in the analysis of the surface deformation of a part with random short fibre mat 61 Figure 3.22 Finite element mesh of the RVE of the generated random short fibre mat 62 Figure 3.23 Deformed top surface profile of the RVE of the random short fibre mat 62 Figure 3.24 Comparison of top surface deformation profile of the parts made of unidirectional random continuous fibre mat and the random short fibre mat 63 Figure 3.25 Schematic of the possible yarn cross section in a fabric (a) elliptical (b) lenticular 63 Figure 3.26 Schematic of a general plain weave fabric lamina geometrical unit cell 64 Figure 3.27 Geometrical description of a cross section of the plain weave fabric unit cell 64 Figure 3.28 Finite element mesh of the unit cell of plain weave fabric 65 Figure 3.29 Deformation profile of the top surface of plain weave fabric unit cell 65 Figure 3.30 Top surface deformation of plain weave fabric unit cell along the diagonal length 66 Figure 3.31 Schematic of unidirectional fabric mat 66 Figure 3.32 Geometrical description of a cross section of unidirectional fabric unit cell 67 Figure 3.33 Finite element model of the RVE of unidirectional fabric 67 Figure 3.34 Deformation profile of the top surface of unidirectional fabric 68 Figure 3.35 Finite element mesh used for the analysis of the process-induced deformation of a C-shaped part in a closed aluminum mould 68 Figure 3.36 (a) Deformed shape of the part after removed from the tool (b) the tool stretches the part as it expands 69 Figure 3.37 Deformation profile of the web of a C-shaped part after removal from the mould 69 Figure 3.38 Contribution of resin cure shrinkage and CTE mismatch to the surface deformation of a unidirectional fibre laminate 70 Figure 4.1 Schematic describing the change in shape of a L-shaped composite part due to the anisotropic thermal strain 99 xi i List of Figures Figure 4.2 Schematic describing the affect of tool-part interaction on a flat composite part during the curing process 99 Figure 4.3 Schematic to illustrate the shear locking phenomenon in a fully integrated 4-noded solid element (a) element before deformation, (b) expected deformation mode according to beam theory and (c) predicted deformation mode showing the non-zero shear strain at the Gauss points 100 Figure 4.4 Schematic of a typical aerospace composite part consisting of solid laminate and sandwich sections 100 Figure 4.5 Flow chart describing the modular approach used to implement the user element concept in a commercial finite element code 101 Figure 4.6 Schematic of the developed 24-noded isoparametric solid element and the node numbering order which describe the through-thickness direction 101 Figure 4.7 Schematic describing the in-plane and through-thickness integration points in the 24-noded composite solid element (through-thickness integration points are for the Simpson's rule) 102 Figure 4.8 Layer material property definition for a tapered sandwich element with composite skins, (x-y-z) is the reference (global) frame, (1-2-3) is the element principal material coordinate system with respect to reference frame and (1 '-2'-3') is the layer material coordinate system with respect to element material coordinate system 102 Figure 4.9 Material orientation definition in a large curved element with rectangular and cylindrical coordinate systems 103 Figure 4.10 Schematic describing the concept of the extruder which creates the solid elements for the tool and the part from a master surface of shell elements 103 Figure 4.11 Schematic describing the definition of layer thickness at 4-corner nodes of the element to model the varying layer thickness within an element 104 Figure 4.12 Schematic showing the rectangular and cylindrical coordinate systems used to describe the material coordinate of the element 104 Figure 4.13 Definition of the element rectangular material coordinate system by (a) coordinate of two points and (b) 3 nodes 105 Figure 4.14 Definition of the element material cylindrical coordinate system by coordinate of two points along the axis of the cylinder (a) typical cylindrical coordinate system where axes 1, 2 and 3 represent radial, tangential and axial coordinate axes (b) currently implemented cylindrical coordinate system where axis 3 is in the thickness (radial) direction so that additional rotation of the layer can be easily defined 105 Figure 4.15 (a) Schematic describing the pressure load acting on the top surface of the element and (b) the corresponding consistent load factors for each node at the top surface 106 Figure 4.16 Schematic of a cantilever beam under end shear and distributed loads 106 xiii List of Figures Figure 4.17 Cantilever beam is modelled with (a) regular rectangular-shaped (b) Trapezoid-shaped and (c) Parallelogram-shaped elements 107 Figure 4.18(a) Schematic of a ring under two compressive point loads at top and bottom and (b) the FE model of one quarter of the beam 107 Figure 4.19 Schematic of sandwich beams with constant (top) and varying (bottom) core thickness under uniformly distributed load 108 Figure 4.20 Comparison of the predicted results for the vertical displacement along the length of the sandwich beam with uniform thickness core using ABAQUS built-in 20-noded element and the developed 24-noded element 108 Figure 4.21 Comparison of the predicted results for the vertical displacement along the length of the sandwich beam with varying core thickness using ABAQUS built-in 20-noded element and the developed 24-noded element 109 Figure 4.22 Schematic of a flat composite part on a solid tool 109 Figure 4.23 Typical one-hold temperature cure cycle used for the curing of composite part 110 Figure 4.24 Finite Element mesh for tool-interface-part assembly. 30*8 elements used to model the part ; 110 Figure 4.25 Schematic of a half circular composite part on a confirming solid tool 111 Figure 4.26 Mechanical boundary conditions on the half-circular tool-part assembly (a) before and (b) after tool removal 111 Figure 4.27 Schematic of an L-shaped composite part on a solid tool 112 Figure 4.28 Finite element mesh of the L-shaped part on a tool (a), (b) elements with large aspect ratio (c) elements with small aspect ratio 112 Figure 4.29 Comparison of the total spring-in angle and the run time (clock time) of an L-shaped part using the three different finite element meshes shown in Figure 4.28 113 Figure 5.1 Schematic of a flat composite part on a solid tool separated by an interface layer 146 Figure 5.2 Schematic showing the displacement boundary conditions applied on the tool-part assembly before tool removal 146 Figure 5.3 Schematic of a beam under applied traction at the top and the bottom surface. The stress and displacement boundary conditions are also shown 146 Figure 5.4 Schematic of stresses acting on a differential element of a beam 147 Figure 5.5 Schematic showing the displacement and stress boundary conditions on two fully bonded homogeneous beams 147 Figure 5.6 Schematic showing the stresses acting on a small segment of tool-interface layer-part assembly 148 xiv List of Figures Figure 5.7 Variation of closed-form solution for axial stress along the length in beam-2 at y = 0 for different number of terms 148 Figure 5.8 Variation of axial stress through the thickness of beam-2 at x = 150 mm for the case of two fully bonded isotropic beams subjected to thermal load. The present closed-form solution is compared with the solutions of theories by Timoshenko and Suhir 149 Figure 5.9 Variation of axial stress along the length of beam-2 at y = 0 for the case of two fully bonded isotropic beams subjected to thermal load. The present closed-form solution is compared with the solutions of theories by Timoshenko and Suhir 149 Figure 5.10 Variation of shear stress along the length of beam-2 at y = 0 for the case of two fully bonded isotropic beams subjected to thermal load. The present closed-form solution is compared with the solution of theory by Suhir 150 Figure 5.11 Development of resin modulus along a typical 1-hold cure cycle 150 Figure 5.12 Variation of axial stress along the length of the composite part at y = 0 for the case of a unidirectional composite part fully bonded to an aluminum tool subjected to thermal load. The closed-form solution is compared with finite element result. The composite part is at cure stage-1 151 Figure 5.13 Variation of axial stress through the thickness of the composite part at x = 150 mm for the case of a unidirectional composite part fully bonded to an aluminum tool subjected to thermal load. The closed-form solution is compared with finite element result. The composite part is at 4 different cure stages as shown in Figure 5.11 151 Figure 5.14 Variation of axial stress through the thickness of the composite part at the middle span for the case of a unidirectional composite part fully bonded to an aluminum tool and subjected to thermal load. The closed-form solution is compared with finite element result. The results are shown for two different beam lengths 152 Figure 5.15 Variation of interfacial shear stress along the length for the case of a unidirectional composite part and an aluminum tool separated by a thin interface layer and subjected to thermal load. The closed-form solution is compared with finite element result 152 Figure 5.16 Variation of axial stress through the thickness of the composite part for the case of a unidirectional composite part and an aluminum tool separated by a thin interface layer and subjected to thermal load. The closed-form solution is compared with finite element result. The composite beam is at cure stage-1 153 Figure 5.17 Variation of total axial strain through the thickness of the composite part for the case of a quasi-isotropic composite part fully bonded to an aluminum tool and subjected to thermal load. The closed-form solution with equivalent layer approach is compared with finite element result. The composite beam is at cure stage-1 153 Figure 5.18 Variation of axial stress through the thickness of the composite part for the case of a quasi-isotropic composite part fully bonded to an aluminum tool and subjected to thermal load. The closed-form solution with equivalent layer approach is compared with finite element result. The composite beam is at cure stage-1 154 xv List of Figures Figure 5.19 Schematic showing the variation of the axial displacement across the layer in layerwise approach 154 Figure 5.20 Variation of total axial strain through the thickness of the composite part for the case of a quasi-isotropic composite part fully bonded to an aluminum tool and subjected to thermal load. The closed-form solution with layerwise approach is compared with finite element result. The composite beam is at cure stage-1 155 Figure 5.21 Variation of axial stress through the thickness of the composite part for the case of a quasi-isotropic composite part fully bonded to an aluminum tool and subjected to thermal load. The closed-form solution with layerwise approach is compared with finite element result. The composite beam is at cure stage-1 155 Figure 5.22 Variation of total axial strain through the thickness of the composite part for the case of a cross-ply composite part fully bonded to an aluminum tool and subjected to thermal load. The closed-form solution with layerwise approach is compared with finite element result. The composite beam is at cure stage-1 156 Figure 5.23 Variation of axial stress through the thickness of the composite part for the case of a cross-ply composite part fully bonded to an aluminum tool and subjected to thermal load. The closed-form solution with layerwise approach is compared with finite element result. The composite beam is at cure stage-1 156 Figure 5.24 Typical 1-hold temperature cure cycle 157 Figure 5.25 COMPRO Component Architecture to model the evolving composite properties with the curing of the resin 157 Figure 5.26 Variation of displacement profile of a unidirectional composite beam under constant end moment with material properties. The finite element results are compared with the solution from classical beam theory (Equation 5.49) 158 Figure 5.27 Variation of axial strain distribution at a cross section of a unidirectional composite beam with material properties. The finite element results are compared with the solution from classical beam theory (Equation 5.49) 158 Figure 5.28 Variation of displacement profile of a unidirectional composite beam under constant end moment with material properties. The finite element results are compared with the solution from modified beam theory (Equation 5.51) 159 Figure 5.29 Development of bending moment at a cross section of a unidirectional composite part along the cure cycle 159 Figure 5.30 Development of the shear modulus of the resin of a unidirectional composite part along the cure cycle 160 Figure 5.31 Variation of normalized warpage of a unidirectional composite part with number of layers (part thickness). The closed-form results are normalized according to the trend observed by Twigg [Twigg et al. (2004)]. The initial resin modulus for this case is 47.1 kPa 160 xvi List of Figures Figure 5.32 Variation of normalized warpage of a unidirectional composite part with part length. The closed-form results are normalized according to the trend observed by Twigg [Twigg et al. (2004)]. The initial resin modulus for this case is 47.1 kPa 161 Figure 5.33 Variation of normalized warpage of a unidirectional composite part with number of layers (part thickness). The closed-form results are normalized according to the trend observed by Twigg [Twigg et al. (2004)]. The initial resin modulus for this case is 4.71 kPa 161 Figure 5.34 Variation of normalized warpage of a unidirectional composite part with part length. The closed-form results are normalized according to the trend observed by Twigg [Twigg et al. (2004)]. The initial resin modulus for this case is 4.71 kPa 162 Figure 5.35 Schematic showing the shear stress distribution along the half-length of interface for the case of a composite part and a solid tool separated by a thin interface layer and subjected to thermal load (see Figure 5.15) 162 Figure 5.36 The variation of warpage number (WN) with shear layer number (SLN) for three different thicknesses of the part. A l l the points lie on a single master curve 163 Figure 5.37 The variation of warpage number (WN) with shear layer number (SLN) for three different lengths of the part. A l l the points lie on a single master curve 163 Figure 5.38 The variation of warpage number (WN) with shear layer number (SLN) for two different shear layer thicknesses. A l l the points lie on a single master curve 164 Figure 5.39 The variation of warpage number (WN) with shear layer number (SLN) for aluminum tool. This figure is the combination of Figure 5.36, Figure 5.37 and Figure 5.38. The figure also shows the approximation of the master curve by two linear segments 164 Figure 5.40 The variation of warpage number (WN) with shear layer number (SLN) for aluminum and steel tools 165 Figure 5.41 The variation of warpage number (WN) with shear layer number (SLN). The two linear curves for steel tool from Figure 5.40 are normalized according to Equation (5.59) 165 Figure 5.42 Comparison of maximum warpage prediction by closed-form solution with experimental results 166 Figure 5.43 Comparison of the closed-form prediction of variation of warpage with part lay-up with experimental results by Petrescue (2005) 167 Figure 5.44 Closed-form results of the variation of bending moment and bending rigidity with lay-up for the 1200 mm long composite part analyzed by Petrescue (2005) 167 Figure 6.1 Schematic of a curved part on a (a) a male and (b) a female cylindrical tools 197 Figure 6.2 Schematic of a curved part under applied traction at the bottom and top surfaces. The stress and displacement boundary conditions are also shown 197 Figure 6.3 Schematic of flat and curved beams on a rigid tool 198 xvii List of Figures Figure 6.4 Variation of tangential/axial stress through the thickness of the curved/flat unidirectional composite part fully bonded to a rigid tool and subjected to a thermal load. The stresses are due to thermal strain mismatch in axial/tangential direction. The closed-form solutions for the flat and curved parts are compared 198 Figure 6.5 Variation of tangential/axial stress through the thickness of the curved/ flat composite part fully bonded to a rigid tool and subjected to thermal load. The finite element results for the flat and curved parts are compared .199 Figure 6.6 Finite element solutions for the variation of transverse stress along the length of a flat composite part at y = 0 for the case of a unidirectional composite part fully bonded to a rigid tool and subjected to thermal load. The inset shows a magnified view of the stresses near the free end 199 Figure 6.7 Finite element solutions for the variation of transverse stress along the length of a curved composite part at y = 0 for the case of a unidirectional composite part fully bonded to a rigid tool and subjected to thermal load 200 Figure 6.8 Finite element solutions for the variation of the radial displacement through the thickness of the curved composite part fully bonded to a rigid tool and subjected to thermal load 200 Figure 6.9 Variation of tangential/axial stress through the thickness of the composite curved/flat parts fully bonded to a rigid tool and subjected to thermal load. The radial displacement of the curved part is constrained 201 Figure 6.10 (a) The variation of tangential stress using Equation (6.19) with the radial displacement obtained from FE (Figure 6.8) (b) the difference between the tangential stress variations based on constrained and unconstrained radial displacements (i.e. difference between Figure 6.5 and Figure 6.9) 201 Figure 6.11 Variation of tangential stress through the thickness of the curved composite part fully bonded to a rigid tool and subjected to thermal load. The stress is due to the radial displacement, (a) modified solution (Equation 6.20) compared with (b) finite element results 202 Figure 6.12 Variation of radial stress through the thickness of a curved composite part fully bonded to a rigid tool and subjected to thermal load. The closed-form solutions (Equation 6.22) are compared with finite element results 202 Figure 6.13 Variation of tangential stress through the thickness of the curved composite part fully bonded to a rigid tool and subjected to thermal load. The closed-form solutions with (Equation 6.25) and without (Equation 6.14) correction for radial displacement are compared with finite element results 203 Figure 6.14 Schematic showing the free displacement of a flat and a curved part due to transverse/radial thermal strain 203 Figure 6.15 (a) Schematic showing the displacement of a curved composite part due to radial thermal strain. The (b) radial and (c) tangential constraints applied by the tool to conform the part to the tool shape are also shown 204 Figure 6.16 Schematic showing the geometry of an un-deformed and deformed curved part due to the radial thermal strain 204 xvii i List of Figures Figure 6.17 Radial displacement profile of a curved part along the length due to radial thermal strain. The analytical solution from geometry (Equation 6.26) is compared with the radial displacement profile due to an applied moment from curved beam theory (Equation 6.27) 205 Figure 6.18 Finite element solution for the variation of tangential stress through the thickness of a curved aluminum part fully bonded to a rigid tool and subjected to thermal load. The stress is due to radial constraint applied by the rigid tool 205 Figure 6.19 Finite element solution for the variation of bending moment along the length of a curved aluminum part due to the radial constraint applied by a rigid tool 206 Figure 6.20 Variation of bending moment along the length of a curved aluminum part due to the radial constraint applied by a rigid tool. The closed-form solution is compared with finite element result 206 Figure 6.21 Variation of the rotation of the cross section of a curved composite part due to an applied displacement profile at the bottom surface. The finite element results are compared with the result from curved beam theory (Equation 6.29) 207 Figure 6.22 Schematic showing the shearing effect due to an applied displacement at the bottom surface of the part 207 Figure 6.23 Variation of the rotation of the cross section of a curved composite part due to an applied displacement profile at the bottom surface. The finite element results are compared with the result from modified curved beam theory (Equation 6.37) 208 Figure 6.24 Variation of tangential stress through the thickness of a curved composite part fully bonded to a rigid tool and subjected to thermal load. The stress is due to radial constraint applied by a rigid tool. The closed-form solutions without the correction for shearing effect (Equation 6.29) are compared with finite element solutions 208 Figure 6.25 Variation of tangential stress through the thickness of a curved composite part fully bonded to a rigid tool and subjected to thermal load. The stress is due to radial constraint applied by the tool. The closed-form solutions with the correction for shearing effect (Equation 6.37) are compared with finite element solutions 209 Figure 6.26 Variation of tangential stress through the thickness of a curved composite part fully bonded to a rigid tool and subjected to thermal load. The stress is due to tangential constraint applied by the tool (Equation 6.40) 209 Figure 6.27 Variation of tangential stress through the thickness of a curved aluminum part fully bonded to a rigid tool and subjected to thermal load. The stress is due to both radial and tangential constraints applied by the tool 210 Figure 6.28 Variation of tangential stress through the thickness of a curved composite part fully bonded to a rigid tool and subjected to thermal load. The stress is due to both radial and tangential constraints applied by the tool 210 Figure 6.29 Schematic of the tool-part assembly before and after the application of temperature load (the part is not constrained by the tool) 211 xix List of Figures Figure 6.30 Schematic of the finite element model used to separate the tangential and the radial behaviour of the tool-part assembly 211 Figure 6.31 Variation of tangential stress through the thickness of a curved composite part fully bonded to an aluminum tool and subjected to thermal load. The stress is due to the thermal strain mismatch between the part and the tool in the tangential direction 212 Figure 6.32 Variation of tangential stress through the thickness of a curved composite part separated by a thin interface layer from an aluminum tool and subjected to thermal load. The stress is due to the thermal strain mismatch between the part and the tool in the tangential direction 212 Figure 6.33 Schematic of the gap between the tool and the part in a male and a female tool due to radial thermal strain mismatch between the part and the tool 213 Figure 6.34 Schematic of the positive and negative value of the gap which depends on the value of the radial thermal strain of the tool and the part 213 Figure 6.35 Variation of tangential stress through the thickness of a curved composite part fully bonded to an aluminum tool and subjected to thermal load. The stress is due to the thermal strain mismatch between the part and the tool in the radial direction 214 Figure 6.36 Variation of tangential stress through the thickness of a curved composite part separated by a thin interface layer from an aluminum tool and subjected to thermal load. The stress is due to the thermal strain mismatch between the part and the tool in the radial direction : 214 Figure 6.37 Typical 1-hold temperature cycle used to virtually cure a composite part 215 Figure 6.38 COMPRO component architecture used for modelling the evolving properties of the composite material 215 Figure 6.39 Displacement profile of a curved composite part fully bonded to an aluminum tool. The displacements are due to thermal strain mismatch between the part and tool in tangential direction. The closed-form results are compared with FE results 216 Figure 6.40 Displacement profile of a curved composite part fully bonded to an aluminum tool. The displacements are due to thermal strain mismatch between the part and tool in radial direction. The closed-form results are compared with FE results 216 Figure 6.41 Displacement profile of a curved composite part on aluminum tool separated by an interface layer. The displacements are due to thermal strain mismatch between the part and tool in tangential direction. The closed-form results are compared with FE results 217 Figure 6.42 Displacement profile of a curved composite part on aluminum tool separated by an interface layer. The displacements are due to thermal strain mismatch between the part and tool in radial direction. The closed-form results are compared with FE results 217 Figure 6.43 Closed-form solution for the moment development in a curved composite part on aluminum tool separated by an interface layer. The moment is due to the thermal strain mismatch between the part and the tool in tangential direction 218 x x List of Figures Figure 6.44 Variation of maximum radial displacement (warpage) with part length for a curved composite part on aluminum tool and separated by an interface layer. The displacements are due to the thermal strain mismatch in the tangential direction 218 Figure 6.45 Variation of maximum radial displacement (warpage) with part thickness for a curved composite part on aluminum tool and separated by an interface layer. The displacements are due to the thermal strain mismatch in the tangential direction 219 Figure 6.46 Closed-form solution for the moment development in a curved composite part on aluminum tool separated by an interface layer. The moment is due to the thermal strain mismatch between the part and the tool in radial direction 219 Figure 6.47 Variation of maximum radial displacement (warpage) with part length for a curved composite part on aluminum tool and separated by an interface layer. The displacements are due to the thermal strain mismatch in the radial direction 220 Figure 6.48 Variation of maximum radial displacement (warpage) with part thickness for a curved composite part on aluminum tool and separated by an interface layer. The displacements are due to the thermal strain mismatch in the radial direction 220 Figure 6.49 Variation of radial displacement with shear modulus of the interface layer for a curved composite part on aluminum tool (male) and separated by an interface layer 221 Figure 6.50 Radial displacement profiles of a curved composite part on aluminum male and female tools. The displacements are due to thermal strain mismatch in radial and tangential directions 221 Figure 6.51 Variation of radial displacement with shear modulus of the interface layer for a curved composite part on aluminum tool (female) and separated by an interface layer. The figure also shows the shear modulus of the interface layer where the displacements due to radial and tangential thermal strain mismatch become equal 222 Figure 6.52 Radial displacement profile of a curved composite part on aluminum female tool with an interface layer due to thermal strain mismatch in radial and tangential directions. The figure shows that by selecting an appropriate interface layer (Figure 6.51), the resultant radial displacement can be minimized 222 Figure 6.53 Development of bending moment due to tool CTE, part CTE and part cure shrinkage along the cure cycle. The moments are due to thermal strain mismatch between the part and the tool in radial direction 223 Figure 6.54 Radial displacement profile of a curved composite part on a tool due to tool CTE, part CTE and part cure shrinkage. The displacements are due to thermal strain mismatch between the part and the tool in radial direction 223 Figure 6.55 Variation of incremental cure shrinkage strain and the ratio of bending rigidity of a curved composite part on aluminum tool along the cure cycle 224 Figure 6.56 Schematic showing the free thermal expansion of an isotropic curved part and the change in part shape (size) and included angle 224 xxi List of Figures Figure 6.57 Schematic description of (a) Spring-in (b) spring-out phenomenon which depends on the thermal strain mismatch between the tool and the part in radial direction 225 Figure 6.58 Schematic describing the calculation of change in included angle by Nelson and Cairn's equation 226 Figure 6.59 Finite element mesh of a U-shaped unidirectional composite part on a solid aluminum tool226 Figure 6.60 The radial and the tangential displacements of a U-shaped unidirectional composite part with and without a flange on a solid aluminum tool. The figure shows the influence of the flange on displacements 227 Figure 7.1 Schematic showing the uniform and selective /z-refinements 254 Figure 7.2 Schematic showing the uniform and selective ^ -refinements 254 Figure 7.3 Schematic of the standard shape functions for 2 and 3-noded bar elements 255 Figure 7.4 Schematic of the hierarchical shape functions for 2 and 3-noded bar elements 255 Figure 7.5 Schematic of the linear and the quadratic through-thickness displacement shape functions in the layerwise approach 256 Figure 7.6 Schematic of the 24-noded higher order element with the non-conventional mid surface nodes to which the additional degrees of freedom are added 256 Figure 7.7 Linear through-thickness geometrical interpolation function for both the hierarchical and the layerwise elements 257 Figure 7.8 Node arrangement in the higher order element for geometrical and displacement interpolation 257 Figure 7.9 Through-thickness displacement interpolation functions for hierarchical element. The displacement functions shown are for 3 r d order hierarchical element 258 Figure 7.10 Through-thickness displacement interpolation functions for layerwise element. The displacement functions shown are for one and two element layers 258 Figure 7.11 Schematic showing the definition of the element and material layers in a layerwise element 259 Figure 7.12 Schematic of a flat composite part fully bonded to an aluminum tool. The figure also shows the displacement boundary conditions for half of the problem modelled due to symmetry 259 Figure 7.13 The variation of axial stress at a typical cross section in a unidirectional composite beam on an aluminum tool (full bonding) predicted with various number of element layers in the layerwise element method and their comparison with the closed-form solution 260 Figure 7.14 The variation of axial stress at a typical cross section in a unidirectional composite beam on an aluminum tool (full bonding) predicted with various number of sinusoidal terms in the hierarchical element method and their comparison with the closed-form solution 260 xxn List of Figures Figure 7.15 The variation of axial stress at a typical cross section in a unidirectional composite beam on an aluminum tool (full bonding) predicted with various number of Legendre polynomial terms in the hierarchical element method and their comparison with the closed-form solution 261 Figure 7.16 Typical 1-hold temperature cure cycle 261 Figure 7.17 Comparison of the convergence rate for the maximum warpage of a flat composite part fully bonded to an aluminum tool using the layerwise and the hierarchical methods. The convergence rate is in terms of total number of degrees of freedom used in the model 262 Figure 7.18 Comparison of the convergence rate for the maximum warpage of a flat composite part fully bonded to an aluminum tool using the layerwise and the hierarchical methods. The convergence rate is in terms of number of degrees of freedom used for the interpolation of u in the thickness direction 262 Figure 7.19 Comparison of the convergence rate for the maximum warpage of a flat composite part on an aluminum tool separated by an interface layer using the layerwise and the hierarchical methods. The convergence rate is in terms of number of degrees of freedom used for the interpolation of u in the thickness direction 263 Figure 7.20 Variation of the actual and the normalized axial stress at a cross section in a flat composite part on an aluminum tool with shear layer properties. The stresses are normalized with the maximum stresses in each case. The shear layer properties are listed in Table 7.2 263 Figure 7.21 Variation of the run time with the number degrees of freedom used to model the composite flat part on an aluminum tool (full bonding) in the layerwise and the hierarchical methods 264 Figure 7.22 Schematic of a cantilever sandwich beam under uniform load 264 Figure 7.23 Comparison of the predicted vertical deflection profile of the sandwich beam under uniform load by the layerwise and the hierarchical methods. The sandwich beam is modelled with 3 element-layers (h = 3) in the layerwise method 265 Figure 7.24 The distribution of the axial displacement in the thickness direction at a cross section of a cantilever sandwich beam under uniform load 265 Figure 7.25 Variation of axial displacement in the thickness direction of a quasi isotropic composite part on an aluminum tool and subjected to thermal load. The results from the layerwise and the hierarchical methods are compared 266 Figure 7.26 Variation of axial displacement in the thickness direction of a cross ply composite part on aluminum tool and subjected to thermal load. The results from the layerwise and the hierarchical methods are compared 266 Figure 7.27 The ratio of two successive coefficients of the exponential function that describes the through-thickness stress variation in a composite part. The threshold values for the hierarchical (1.5) and the layerwise (1.0) methods are shown 267 Figure 7.28 Variation of the number of additional Legendre terms in the hierarchical method during the cure cycle to achieve the converged solution for the process-induced displacement of the composite flat part on an aluminum tool 267 xxii i List of Figures Figure 7.29 Cure cycle separated into two time regimes: one requiring higher order terms and one without 268 Figure 7.30 Variation of the run time with the number degrees of freedom used to model the composite flat part on an aluminum tool (full bonding) in the layerwise and the hierarchical methods (fixed and changing number of terms) 268 Figure 7.31 Typical 1-hold temperature and pressure cycles used for the experimental study 269 Figure 7.32 ABAQUS basic Coulomb friction model with the maximum shear stress limit 269 Figure 7.33 Comparison of maximum warpage prediction by the layerwise element used in combination with contact surface in ABAQUS with experimental results by Twigg et al. (2004) 270 xxiv List of Symbols List of Symbols A Area B Strain-displacement matrix of the element CTE Thermal expansion coefficient CTEX Longitudinal coefficient of thermal expansion CTE2 Transverse coefficient of thermal expansion CTE3 Transverse coefficient of thermal expansion CTEf Fibre coefficient of thermal expansion CTEr Resin coefficient of thermal expansion C P Specific heat capacity of the material D Material stiffness matrix E Young's modulus EI Bending rigidity En Longitudinal Young's modulus of a composite lamina E22 Transverse Young's modulus of a composite lamina Transverse Young's modulus of a composite lamina En Fully cured longitudinal Young's modulus of a composite lamina Er Young's modulus of the matrix Ef Young's modulus of the fibre GA Shear rigidity G Shear Modulus G 1 2 In-plane shear modulus of a composite lamina In-plane shear modulus of a composite lamina G 2 3 Transverse shear modulus of a composite lamina Gn Number of Maxwell elements to define relaxation modulus Gs Shear modulus of the interface layer HR Resin heat of reaction I Second moment of area XXV List of Symbols J Jacobian matrix of the element | / | Determinant of the jacobian matrix K Stiffness matrix Kele Stiffness matrix of the element kx Thermal conductivity of the material in x direction Nt Displacement shape function at i * node P Point load p Distributed pressure load on an element surface q Heat flux per unit area of the body flowing into the body Q Internal heat generation due to curing of resin R Internal load vector Rele Internal load vector of the element Ra Roughness average of a surface profile Rq Root-mean-square roughness of a surface profile SLN Shear layer number T Temperature t Time Thickness of the interface layer u Displacement vector U Material time rate of the specific internal thermal energy V Volume of solid material with surface area S Vf Volume fraction of the fibre wt Weight factors for the numerical integration WN Warpage number a Degree of cure of the resin p Density of the material pr Density of the resin CT Stress vector at an integration point ACT Incremental stress vector at an integration point for the current time step xxvi List of Symbols Ae Incremental mechanical strain vector for the current time step etot Total strain vector ether Thermal strain vector due to CTE and cure shrinkage K Shear correction factor L\<J> Change of angle in a composite part (spring-in) da ~dt dx Degree of cure of the resin Spatial gradient of temperature xxvii Acknowledgements Acknowledgements By God's will, aid, and support, the completion of this work has become a reality. I would like to take this opportunity to acknowledge the help of those without whom I could not have finished this work. Firstly, I would like to thank my supervisors Dr. Reza Vaziri, Dr. Anoush Poursartip and Dr. Goran Fernlund for their invaluable advice, expertise, and patience. Many thanks to several past and present UBC Composites Group Members for their friendship and help. Especially, I would like to thank Mr. Amir Osooly and Dr. Nima Zobeiry for our fruitful discussions and their assistance on many occasions during the course of my degree. The advice and encouragement offered by Mr. Robert Courdji was also invaluable to me during the course of my work. Financial support from the Canadian Federal Networks of Centres of Excellence (NCE) program, the University of British Columbia, and the generous support of Dr. Reza Vaziri and Dr. Anoush Poursartip is truly appreciated. Finally, my special thanks are due to my mother, brother and sister for their continuous love, encouragement and patience. Most of all, I would like to thank my lovely wife, Mirzana, for her patience and sacrifice throughout my study. She was always by my side and her words of kindness and support were my constant source of motivation This dissertation is dedicated to my father who passed away in 1994 during the first year of my undergraduate studies. His deep love for his children and sacrifices shaped my academic ambitions and all aspects of my life. xxvii i Chapter 1: Introduction and Background Chapter 1. I N T R O D U C T I O N A N D B A C K G R O U N D 1.1. B A C K G R O U N D Fibre-reinforced plastic composite materials are replacing traditional ones in many of today's structural engineering applications due to their high strength to weight ratio, high stiffness to weight ratio, and durability. When using composites, unlike their metallic counterparts, the complete (large-scale) structure is manufactured from the raw materials in one step in order to reduce the manufacturing cost. Our focus is mainly on the high-performance structural components made of advanced thermoset matrix composites typically employed in the aerospace industry. An autoclave process is commonly used to manufacture such structures. Broadly speaking, this process involves stacking of pre-impregnated sheets of unidirectional fibres (commonly called prepreg) at various orientations over a tool of desired shape and then subjecting the whole assembly to a controlled cycle of temperature and pressure inside an autoclave. The process results in the compaction and curing of the composite part. However, because of the residual stresses that build up during the process, the precise shape and dimensions of the final part after tool removal are often difficult to control. In thin-walled composite structures spring-back and warpage are commonly observed process-induced imperfections. In thick structures, residual stresses remain locked in, and may affect structural performance. There has been much work done for the last two decades to develop more sophisticated analytical and numerical models to predict the residual stress development during the processing of composite parts. These models range from very simple one-dimensional elastic analyses to very complicated three-dimensional viscoelastic analyses. In this vein, a comprehensive, multi-physics, 2D finite element code, COMPRO, has been developed at UBC to analyze industrial autoclave processing of composite structures of intermediate size and complexity [Hubert (1996), Johnston (1997)]. The model caters for a number of important processing parameters and the development of residual stresses and deformations. This model also accounts for the effects of tool/part interaction, which have been largely neglected by other investigators. The model assumptions, theoretical background, solution strategies and case studies - 1 -Chapter 1: Introduction and Background demonstrating its predictive capabilities have been documented elsewhere [Hubert et al. (1999), Johnston etal (2001)]. COMPRO has been used in industry for the last decade to resolve many practical problems encountered during autoclave processing. The main disadvantage of COMPRO is its two-dimensional limitation. Hence some approximate solution methods have been developed to tackle complicated three-dimensional problems [Fernlund et al. (2003)]. Apart from the limitation of its dimensionality, COMPRO is also hampered by some of the shortcomings that the other similar processing software codes face, such as lack of familiarity of the code to the general public, non-versatility of the code compared to general commercial finite element codes where a wide range of different options (material, element, interaction etc.) are available. Even though all sophisticated numerical codes enable us to model very complex processing problems, the interpretation and the validation of the results is a significant barrier faced by the researchers and industry. The anisotropic nature of composite materials makes the interpretation even more difficult. In addition, process models usually involve significant numerical runs, consistent with the size and complexity of the industrially relevant composite parts. This makes efficiency of the model a crucial factor in controlling modelling costs. 1.2. R E S E A R C H O B J E C T I V E S A N D T H E S I S O U T L I N E The main objective of this research work is to initiate the development of the next generation process model for autoclave processing of composite structures. This development will be carried out by building on the already established knowledge of process modelling within the UBC Composite Group rather than starting from scratch. Composite process modelling is a very complex problem. Developing a process model that can capture most of the complexities may seem to be the way forward in process modelling, but this approach may not be efficient in terms of the computational time and cost. Hence, our next generation process model consists a set of numerical tools which ranges in complexity from a simple Chapter 1: Introduction and Background analytical tool to a very complex finite element analysis tool, so that a modeller can make a choice depending on the time and cost constraints. This is accomplished by: • Modifying and transferring the current modular approach of modelling the material constitutive equation to a general platform so that it can be used in any commercial finite element code. This will provide many advantages such as the availability of other features of the finite element code used, the familiarity of the code to other users etc. • Development of closed-form solution for some simple composite part geometries. The closed-form solution serves multiple purposes: Helps us with better understanding of the physics of the problem Serve as a simple tool for quick estimation of the process-induced stresses and deformation of simple geometrical composite parts Serve as a verification tool for the finite element results • Development of more robust and efficient finite element techniques If these objectives are achieved, two different categories of process modelling tools will be available: a very simple closed-form tool to analyse simple geometrical parts for quick estimation of the process-induced deformation and a very efficient and robust finite element tool to analyse complicated geometrical parts. Based on these objectives, this thesis is organized as follows: Chapter 2 - Modular Approach to Process Modelling In this chapter, the current methodology of modelling the material constitutive equation is modified and transferred to a general platform so that it can be incorporated into any commercial finite element software. The developed methodology, called COMPRO Component Architecture (CCA), is implemented in the commercial finite element analysis software, ABAQUS, to test the methodology. Chapter 1: Introduction and Background Chapter 3 - Surface Finish of Automotive Composite Parts Manufactured by R T M In this chapter, the methodology developed in the previous chapter is used to investigate the factors that may contribute to the surface finish of automotive composite parts manufactured by resin transfer moulding (RTM). The process-induced shape distortions and surface finish imperfections resulting from property mismatches at the micro and macro levels are investigated. Chapter 4 - Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures In this chapter, a 24-noded solid element is developed with a remedy for the inherent locking effects that are encountered, so that it can be used to model shell-like structures where large aspect ratios are desirable. The developed element also can accommodate the changing layer thickness so that a composite part with features such as tapered core and ply-drop can be modelled. This element forms the basis of the higher order elements developed in Chapter 7. Chapter 5 - Closed-Form Solution for Process-Induced Stresses and Deformation in a Flat Composite Part In this chapter, a closed-form solution for the process-induced stresses and deformation of a composite flat part on a solid tool is developed. Chapter 6 - Closed-Form Solution for Process-Induced Stresses and Deformation in a Curved Composite Part In this chapter, the developed closed-form solution for the flat part is extended to a curved composite part on a conforming solid tool. Chapter 7 - Higher Order Finite Element Techniques for Process Modelling In this chapter, the knowledge gained from the closed-form solution is used to develop two robust adaptive finite elements which can be used to model complicated composite parts with just one element discretization in the thickness direction. Chapter 1: Introduction and Background Chapter 8 - Summary, Conclusions and Future Work This chapter highlights the contributions made in this thesis and the conclusions that can be drawn from this research work. Recommendations are also made for possible future extension of the work presented here. Chapter 2: Modular Approach to Process Modelling Chapter 2. M O D U L A R A P P R O A C H T O P R O C E S S M O D E L L I N G 2.1. INTRODUCTION Autoclave processing of composite structures consists of many complex physical phenomena such as heat transfer, resin flow and stress development. The real success of process modelling depends on capturing these physical phenomena as accurately as possible. Due to the complexities involved in modeling, composite processing has generally been modelled using the 'integrated sub-model' approach first introduced by Loos and Springer (1983). Based on this approach, a complex problem of process modelling is divided into three simpler sub-models, which can be studied more or less independently as shown in Figure 2.1. Many researchers have used this methodology to model autoclave processing such as Bogetti and Gillespie (1991, 1992), White and Hahn (1992a, 1992b), Johnston et al. (2001), and Zhu et al (2003). Each of these sub-models has three distinct but intersecting components: the governing equation, the material behaviour and the boundary conditions. The accuracy of the results of these three sub-models depends on the method of solving the governing equations, approximating the material constitutive behaviour and representing the physical boundary conditions. Approximation in solving the governing equations involves dimensionality and the solution technique. The dimensionality of the method of solving the governing equations ranges from ID to 3D [Loos and Springer (1983), Bogetti and Gillespie, (1991, 1992), Johnston et al. (2001), Zhu et al, (2003)]. Many numerical techniques have been used in the literature to solve the governing equations such as laminate plate theory [Hahn and Pagano (1975), Loos and Springer (1983), White and Hahn (1992) and Bogetti and Gillespie (1992)], finite difference method [Bogetti and Gillespie (1991)] and the finite element technique [Chen and Ramkumar (1988), Johnston et al. (2001), and Zhu et al (2003)]. During autoclave processing, the resin transforms from a viscous fluid to an elastic solid. The resin mechanical property development can be divided into three stages: viscous behaviour, viscoelastic Chapter 2: Modular Approach to Process Modelling behaviour and elastic behaviour. The accuracy of the stress model depends on the constitutive model used to describe the mechanical behaviour of the material along the process cycle. A number of constitutive models have been used in the literature to analyse the process-induced stresses such as purely elastic [Loos and Springer (1983), Nelson and Cairns (1989)], Cure Hardening Instantaneously Linear Elastic or CHILE [Bogetti and Gillespie (1992), Johnston et al. (2001)], pseudo viscoelastic [Zobeiry et al. (2006a)] and fully viscoelastic [Kim and White (1996), Zhu et al (2003), Zobeiry et al. (2006b)]. As seen above, the process modelling of composite structures can be carried out using various numerical techniques with the combination of different material constitutive models in a certain dimension (Figure 2.2). Most of the process models presented in the literature use a certain numerical technique in combination with a certain material constitutive model. The process model developed at UBC, COMPRO, also uses the integrated sub-model approach shown in Figure 2.3. The communication between these sub-models is done through three state variables, namely, temperature, degree of cure of the resin and the fibre volume fraction. It uses the two-dimensional finite element technique with CHILE material constitutive model. Even though the model is limited by its two-dimensional capability, the main advantage of COMPRO is its implementation of the material behaviour in a very modular fashion. The Finite element method is the most widely used numerical technique to model composite processing. The type of element used to solve the governing equations and the constitutive model to describe the material behaviour varies from problem to problem. A process model that uses only a certain type of element and a certain type of material model constrains the range of applicability of that process model. On the other hand, developing a process model that covers a vast range of application is cumbersome. There are many commercial finite element codes available in the market which have a large variety of elements and material options. Using a commercial code for process modelling has many advantages ranging from practical considerations such as familiarity and availability of codes to external users, through to engineering considerations such as the availability of ID to 3D solutions, the need for integration with other specialized material models and so forth. Chapter 2: Modular Approach to Process Modelling 2.1.1. Objectives The main objective of this study is to expand our current finite element process modelling capability to cover different dimensionality and different material constitutive behaviour. Expanding the current process modelling software, COMPRO, for this task is time consuming and cumbersome. Hence, in this study, the modular approach used in COMPRO to model the constitutive behaviour of the composite material is modified to incorporate it into any commercial finite element software. Hence, the advantages of both COMPRO and commercial finite element codes can be fully utilised. The new modular approach is called COMPRO Component Architecture (CCA). For this study, CCA is incorporated into ABAQUS (2001). 2.2. C O M P R O C O M P O N E N T A R C H I T E C T U R E ( C C A ) F O R C O M P O S I T E M A T E R I A L S In this section, the concept of COMPRO Component Architecture is presented. The basic CCA module is shown in Figure 2.4. The CCA consists of many different material subroutines implemented in COMPRO. For example, the cure kinetics module has around 6 different cure kinetics models used for different materials. Should a new material be introduced, then the new cure kinetics model for that material is simply added to the CCA module. Hence, the CCA module acts as a "Module bank" where new materials, new micro-mechanics equations and new cure kinetics and properties development models can be continuously added. The interface module is the communicator between the CCA and the commercial finite element code. Only the interface module should be modified to be compatible with any other commercial code. The rest of the modules remain the same. At each time step, the state variables, namely, the temperature (T), the degree of cure (a) and the fibre volume fraction ( Vj-) from the previous time step are passed in to CCA and updated. Based on the new state variables, the thermo-mechanical properties of the fibre and the resin are calculated. The micro-mechanics module calculates the composite properties from the updated properties of the fibre and the Chapter 2: Modular Approach to Process Modelling resin and the fibre volume fraction at that point using micro-mechanics equations. Currently the micro-mechanics equations by Hashin and Rosen (1964) are implemented. In this case, the CCA module is connected to ABAQUS through the user material option as shown in Figure 2.5. In the user material subroutine, the material constitutive behaviour is defined. The definition of the constitutive behaviour depends on the type of analysis (elastic, CHILE or viscoelastic) and the type of element (ID, 2D (plane stress, plane strain) or 3D) used in the analysis. 2.3. S E Q U E N T I A L L Y - C O U P L E D THERMAL-STRESS ANALYSIS USING A B A Q U S In the present case, only the thermochemical and the stress modules are considered for the analysis. It is assumed that there is no resin flow involved and the fibre volume fraction is uniform. A sequentially coupled thermal-stress analysis can be conducted, if the stress/displacement solution is dependent on a temperature field and there is no inverse dependency. Sequentially coupled thermal-stress analysis is performed by first solving the pure heat transfer problem, then reading the temperature solution into stress analysis as a predefined field. The temperature is predefined because it is not changed by the stress analysis solution. Such predefined fields are always read into ABAQUS at the nodes. They are then interpolated to the calculation points within elements as needed. The interface that reads the temperature history from the heat transfer analysis assumes that the node numbers are the same for corresponding nodes in the stress analysis mesh and in the heat transfer analysis mesh. When the results file is read during the stress analysis, temperatures at nodes that are not in the mesh are ignored and any additional nodes will have zero temperature values. 2.3.1. Heat Transfer Analysis Heat transfer analysis is performed to model solid body heat conduction with general, temperature-dependent conductivity, internal energy (including latent heat effects), and general convection and radiation boundary conditions. In this analysis, the temperature field is calculated without the knowledge of the stress/deformation state. Chapter 2: Modular Approach to Process Modelling 2.3.1.1. Element Type ABAQUS has mainly two types of elements for heat transfer analysis: solid and shell elements. The main disadvantage of ABAQUS solid elements is that they do not have the composite feature to model layered parts. Hence each layer of the composite part should be modelled with at least a single element or the equivalent layer properties should be used. However, ABAQUS shell elements have the composite feature. The user can specify the number of section points used for cross-section integration and thickness direction temperature interpolation for each element. 2.3.1.2. Thermochemical Module The thermochemical module is responsible for the calculation of temperature and the degree of cure in composite components. These are the two most important state variables on which the other material properties depend. The thermochemical module consists of a combination of analyses for heat transfer and resin reaction kinetics. The basic energy balance equation for the thermochemical module is: (2.1a) or (2.1b) where: V = volume of solid material with surface area S p = density of the material U = material time rate of the specific internal thermal energy q = heat flux per unit area of the body flowing into the body Cp = specific heat capacity of the material k = thermal conductivity of the material Q = internal heat generation due to curing of resin and is given by: Chapter 2: Modular Approach to Process Modelling Q = ^(\-Vf)prHR (2.2) where: a = degree of cure (DOC) of the resin Vy = Volume fraction of the fibre pr = density of the resin HR = resin heat of reaction da Numerous models are available for the calculation of the cure rate [Johnston (1997)]. dt The above energy balance equation can be implemented in ABAQUS by using the user subroutine UMATHT. The subroutine UMATHT is called at each integration point. Subroutine UMATHT must perform the following functions: it must define the internal energy per unit mass, U, and its variation with temperature and spatial gradients of temperature; it must define the heat flux vector, q, and its variation with respect to temperature and spatial gradients of temperature. The components of the heat flux and spatial gradients in user subroutine UMATHT are in local directions. To calculate the heat flux dT vector, the spatial gradient of temperature, , is passed on to the subroutine. The material properties dxj that are necessary inside the subroutine UMATHT are obtained from the CCA module. 2.3.2. Stress Analysis 2.3.2.1. Element Type ABAQUS has a vast variety of stress/displacement elements such as beam elements, shell elements, solid elements etc. Both the shell and the solid elements have the composite feature to model layered parts. However, the main disadvantage of the ABAQUS shell element is its inability to update the transverse shear stiffness of the element during the curing process. Currently ABAQUS allows only a constant value for the shear stiffness to be defined at the beginning of the analysis. Chapter 2: Modular Approach to Process Modelling 2.3.2.2. Stress Module The governing finite element equation for the stress module is given by: ele nele nele or (2.3) Ku = R where Kee is the element stiffness matrix given by: Kele = JBTDBdV (2.4) and Ree is the element nodal force vector given by: Re,e = _ ele (2.5) v • ele In general procedures ABAQUS solves the overall system of equations by Newton's method: Solve: KAu = Y Set: u = u + Au (2.6) Iterate where ! f is the residual load vector. In the stress module, the material stiffness matrix D and the stress vector <r should be defined to calculate the element stiffness matrix Kele and the element nodal force vector Rele respectively. The stress module contains two major ABAQUS subroutines: U E X P A N and UMAT. These subroutines will be called at each integration point of an element in the consecutive order. In the subroutine U E X P A N the incremental thermal strains should be defined. The incremental thermal strains are due to CTE and cure shrinkage of the composite. These values are obtained from the CCA module by passing the state variables. - 12-Chapter 2: Modular Approach to Process Modelling The subroutine U M A T is used to define the material stiffness matrix D and update the stresses vector a at each integration point. The stresses at each time step are calculated using the CHILE model as used in COMPRO: A<r = DAe 2 . 4 . V E R I F I C A T I O N P R O B L E M S In this section, some example problems are shown to demonstrate the accuracy of the above-developed subroutines. The results from ABAQUS with the combination of CCA (which will be referred to as CCA/ABAQUS in the following sections) are compared with the results from COMPRO. COMPRO has a special 2D composite solid element that can have a number of layers with different orientations. But ABAQUS has composite elements in 3D only and this 3D composite element has only displacement degrees of freedom. So it cannot be used for the heat transfer analysis. Therefore in the following examples, each layer of the composite part is modeled using one solid element and constraints are applied to the CCA/ABAQUS 3D runs to enable a plane strain state similar to COMPRO. The composite material used in this study is AS4/8852 CFRP (carbon fibre reinforced polymer). The thermo-mechanical properties of this material are given in Appendix A. 2.4.1. Example 1 The first example is to demonstrate the validity of the subroutines. A composite part 20 mm long and 20 mm thick, as shown in Figure 2.7, is cured under the prescribed cure cycle shown Figure 2.6. The part consists of 8 unidirectional layers of AS4/8852 material. The part is modelled with 8-noded isoparametric solid elements (C3D8) and has one element (2.5 mm) in the out-of-plane direction. The temperature is transferred to the part by convection at the bottom boundary. The minimum and maximum time steps used in the analysis are 1 sec and 100 sec, respectively. The analysis automatically changes the time step in between these limits by checking the increment of degree of cure with a user defined maximum - 13-Chapter 2: Modular Approach to Process Modelling allowable value. The maximum allowable value for this analysis is 0.01. The temperature at the mid-node of the bottom and top boundaries are compared with GOMPRO results in Figure 2.8. The results agree very well with each other. The temperature history is then transferred to the stress analysis. In the stress analysis, the stress development through the curing process in element 1, as shown in Figure 2.7, is investigated for the fully fixed all around boundary condition. The axial and the transverse stress development as the material cures are shown in Figure 2.9. In this case too, the results agree very well with each other. 2.4.2. Example 2 The second example is to check the layer rotation. The example is similar to the previous example, but now the temperature is applied at the left boundary. The temperature profile at the mid node of the right boundary is investigated for different lay-ups. The comparison of CCA/ABAQUS and COMPRO results for three different lay-ups (0°, 45° and 90°) are shown in Figure 2.10. The results agree very well for the 0° and 90° lay-ups. But there is some difference (~ 3° C) in the result for 45° lay-up. This difference may be due to the 2D plane strain approximation of COMPRO. 2.4.3. Example 3 The third example is to demonstrate the usage of the composite shell element to predict the through-thickness temperature distribution. Example 1 is now modelled using a single 4-node isoparametric composite shell element (DS4) as shown in Figure 2.11. The shell has in-plane dimensions of (0.4 m * 0.4 m) and the thickness of the shell is 20 mm. The temperature is applied to the part by convection at the bottom surface. The temperature profile at the top surface is compared with the temperature profile from Example 1. Figure 2.12 shows the comparison between the predictions of the solid and shell elements where it can be seen that the two results agrees very well. - 14-Chapter 2: Modular Approach to Process Modelling The above simple examples show that the developed methodology (i.e. the incorporation of CCA in ABAQUS) works very well. In the following sections, some practical examples are given to demonstrate the capability of the developed methodology. 2.5. WARPAGE O F A F L A T PART In this study, the warpage and the residual stresses in a flat composite part laid on a flat tool subjected to thermal load are investigated. The tool part assembly is shown in Figure 2.13. The tool part assembly is cured under the temperature cycle shown in Figure 2.6. At the end of the curing process, the part is removed from the tool and the warpage of the part is calculated. The boundary conditions on the assembly before and after tool removal are shown in Figure 2.14. Only half of the problem is considered due to symmetry. The sliding boundary condition at the bottom of the tool is assumed since inside an autoclave the tool-part assembly is placed on the autoclave bed and subjected to high pressure thus preventing the assembly from bending. The above problem is modelled by both CCA/ABAQUS and COMPRO. In COMPRO, it is modelled with 8-noded isoparametric composite plane strain elements and in CCA/ABAQUS it is modelled using 20-noded isoparametric composite solid elements. The finite element mesh is shown in Figure 2.15. Constraints are applied to the CCA/ABAQUS model to make it plane strain, similar to the COMPRO model. The part and the tool are 600 mm long and are assumed to be fully bonded. The tool is made of aluminum and is 5 mm thick. The part is 1.6 thick and is made of 8 unidirectional layers of AS4/8552 CFRP material. The predicted warpage profiles of the two models are shown in Figure 2.16. Also in the figure, the ABAQUS prediction without the plane strain constraints is shown. The plane strain model over-predicts the warpage results and this is one of the main shortcomings of COMPRO. - 15 -Chapter 2: Modular Approach to Process Modelling 2 . 6 . S P R I N G - I N O F A N L - S H A P E D C O M P O S I T E P A R T In this case study, the stresses and the deformations of an L-shaped composite component are numerically analysed using both COMPRO and CCA/ABAQUS. The composite part is made of 8 unidirectional layers of AS4/8552 CFRP material and the tool is made of aluminum. The modelled tool and the part geometries are shown in Figure 2.17. The part and the tool were descretized in COMPRO using 8-noded isoparametric elements and in ABAQUS using 20-noded isoparametric elements as shown in Figure 2.18. The mechanical and thermal boundary conditions are also shown in Figure 2.18. A convective heat transfer boundary condition was applied on all external boundaries. At the end of the process cycle, a simulation of the tool removal from the component was performed to predict the post-processed component shape. The part was cured under the cure cycles shown in Figure 2.6. After the simulation of tool removal, the spring-in angle was calculated. The total spring-in calculated was taken to be the included angle of the lines connecting the two end points (one at the corner and one at the end) of the flanges as shown in Figure 2.19. The corner component of this total spring-in was obtained by calculating the included angle between the tangent lines at the corner (see Figure 2.19) and the warpage component was taken to be the gradient of the warpage profile of the flange at the corner. The predicted spring-in angles for fully bonded condition are shown in Figure 2.20. The CCA/ABAQUS result with the plane strain constraint agrees very well with COMPRO results. As in the warpage case, the plane strain assumption over-predicts the spring-in angle. 2 . 7 . D I S C U S S I O N The developed methodology of using the user material option in a commercial finite element code to model composite processing may seem to be a straightforward approach. But the main advantages of the developed methodology are: - 16-Chapter 2: Modular Approach to Process Modelling 1. The CCA module is solver independent so that it can be easily incorporated into any commercial finite element code. For example, the CCA module was incorporated into MSC M A R C (2005) by Convergent Manufacturing Technologies (CMT), the spin off company of the UBC Composites Group, with minimal modification to the interface module. 2. Any new material or any new constitutive behaviour can be easily added. For example, this approach was used by Zobeiry et al. (2006) to implement the viscoelastic. behaviour of a composite material in ABAQUS. 2.8. S U M M A R Y A N D C O N T R I B U T I O N S Autoclave processing is a complicated process involving complex geometries and evolving material constitutive behaviour. In the finite element modelling of the autoclave process, various simplifications need to be made at the geometrical and material constitutive level. The main objective of this study is to develop a finite element processing tool that can handle different geometries and different material constitutive behaviour. Developing a finite element tool from scratch that can handle all the complex geometries and material constitutive behaviour is very inefficient. On the other hand, using commercial finite element software for this purpose is limited by the non-availability of the required composite material behaviour during cure. Hence, in this study, a process modelling methodology was developed to attain our objective by incorporating the well established in-house (UBC Composites Group) knowledge of process modelling into any commercial finite element software. A modular approach called COMPRO Component Architecture (CCA) to describe the constitutive behaviour of a composite material during cure was developed. The C C A module can be incorporated into any commercial finite element software with very minimal changes. The methodology was implemented in ABAQUS as an example platform and in the course of the implementation two ABAQUS material subroutines, namely U M A T and UMATHT, were developed to perform a sequentially coupled fhermomechanical analysis. - 17-Chapter 2: Modular Approach to Process Modelling The accuracy of the developed methodology was evaluated by comparing the predictions of COMPRO and CCA/ABAQUS. For the cases considered, the comparisons agreed very well. Some realistic examples were also considered to demonstrate the modelling capability. In the next chapter, the developed methodology will be used to investigate the surface finish of automotive body panels which involve complex geometries. - 1 8 -Chapter 2: Modular Approach to Process Modelling PROCESS VARABLES Temperature Pressure THERMOCHEMICAL MODEL Resin Degree of Cure Temperature Viscosity FLOW MODEL Resin Pressure Fibre Volume Fraction STRESS MODEL Stresses Strains Displacements Governing Equation Material Behaviour Boundary Condition Governing Equation Material Behaviour Boundary Condition Governing Equation Material Behaviour Boundary Condition Figure 2.1 Flow chart illustrating the integrated sub-model approach used to model the processing of composite structures Solving Governing Differential Equation Material Constitutive Behaviour Laminate Plate Theory Finite Element Method Finite Difference Method Purely Elastic Cure Hardening Instantaneously Linear Elastic (CHILE) Pseudo Viscoelastic Fully Viscoelastic ID 2D 3D Figure 2.2 Different numerical techniques and material constitutive models used in the current process modelling techniques available in the literature - 19-Chapter 2: Modular Approach to Process Modelling Figure 2.3 Schematic showing the sub-model structure used in C O M P R O [Johnston (1997)] C C A Module INTERFACE M O D U L E Pass in and update state variables T, a, V f MICRO MECHANICS M O D U L E Calculate composite properties C U R E KINETICS M O D U L E Update a RESIN PROPERTIES M O D U L E FIBRE PROPERTIES M O D U L E Figure 2.4 The C O M P R O Component Architecture (CCA) developed to incorporate composite behaviour during cure in a commercial finite element code - 2 0 -Chapter 2: Modular Approach to Process Modelling Finite Element Solver Initialize State Variables in Solver Set up Constitutive Equation in Solver Run Solver Incrementally USER MATERIAL Define the constitutive Stiffness Matrix, D Compute the Internal Stresses, rj Figure 2.5 A generalized finite element module with an evolving composite material constitutive behaviour 200 150 Time (min) 300 Figure 2.6 Typical 2-hold temperature cure cycle -21 -Chapter 2: Modular Approach to Process Modelling Stacking direction 20 mm Convection (a) 20 mm o (b) Figure 2.7 A composite laminate with a stack of 8 unidirectional layers. Boundary conditions for (a) heat transfer analysis and for (b) stress analysis are shown Figure 2.8 Comparison of the temperature profile along the cure cycle at top and bottom of the unidirectional composite part from C O M P R O and C C A / A B A Q U S - 2 2 -Chapter 2: Modular Approach to Process Modelling Figure 2.9 Comparison of the development of axial and transverse stresses along the cure cycle at the highlighted element of the unidirectional composite part from C O M P R O and C C A / A B A Q U S - 2 3 -Chapter 2: Modular Approach to Process Modelling Figure 2.10 Comparison of temperature profiles along the cure cycle for a 20 mm composite cube with different lay-ups (a) [0]8 (b) [45]8 (c) [90]8 from C O M P R O and CCA/ABAQUS - 2 4 -Chapter 2: Modular Approach to Process Modelling Stacking direction 20 mm Convection (a) 400 mm Convection (b) Figure 2.11 Modelling the unidirectional composite cube with (a) solid and (b) shell elements for thermal analysis in CCA/ABAQUS 50 100 150 200 Time (min) 250 300 Figure 2.12 Comparison of the temperature profile along the cure cycle obtained using 8 solid elements (8-noded) and one shell element (4-noded) in thickness direction in C C A / A B A Q U S -25 -Chapter 2: Modular Approach to Process Modelling 1.6 mm 5 mm 600 mm Figure 2.13 Schematic of a flat composite part on a solid tool Phi •Br (b) Figure 2.14 Schematic of the boundary conditions applied on the tool-part assembly (a) before and (b) after tool removal Part Tool Figure 2.15 Portion of the finite element mesh of the composite part and the tool used to study the process-induced deformation - 2 6 -Chapter 2: Modular Approach to Process Modelling Figure 2.16 Comparison of the warpage prediction of the unidirectional composite flat part after tool removal by C O M P R O with CCA/ABAQUS with and without plane strain condition 50 mm Fibre Direction Thickness, t-R = 5 mm t = 1.6 mm Part Tool Figure 2.17 Schematic of an L-shaped unidirectional composite part on a solid aluminum tool -27-Chapter 2: Modular Approach to Process Modelling Figure 2.19 Schematic describing the measurement of the warpage and the corner components of the spring-in angle of an L-shaped part -28-Chapter 2: Modular Approach to Process Modelling 7 Figure 2.20 Comparison of spring-in angle of an L-shaped unidirectional composite part predicted by C O M P R O and C C A / A B A Q U S with and without the plane strain condition - 2 9 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Chapter 3. S U R F A C E F I N I S H O F A U T O M O T I V E C O M P O S I T E P A R T S M A N U F A C T U R E D B Y R T M 3.1. I N T R O D U C T I O N During recent decades, polymer composite materials have grown in importance in the automotive industry. Some significant properties of these materials, such as reduction of weight, result in an advantageous use of polymer composites over conventional metallic materials. Composite structures are manufactured directly into large, complex shape structures without employing extensive machining and fastening operation to achieve cost reduction. For example, a composite pickup box is manufactured in three pieces and assembled. The main challenge in manufacturing large complex structures is to achieve the required dimensional consistency and surface finish. Resin transfer moulding (RTM) process has been widely used in automotive industries, because products of large area can be manufactured easily and the cost of manufacturing is lower than that of compression moulding or hand lay-up method [Kim and Lee (2002)]. R T M is a three-step process: preforming followed by injection and cure, as shown schematically in Figure 3.1. In the R T M process, dry (i.e., unimpregnated) reinforcement is pre-shaped and oriented into a skeleton of the actual part known as the preform, which is inserted into a matched die mould. The mould is then closed, and a low-viscosity reactive fluid is injected into the mould. The air is displaced and escapes from vent ports placed at the high points. During this time, known as the injection or infiltration stage, the resin wets out the fibres. Heat applied to the mould activates polymerization mechanisms that solidify the resin in the step known as cure. The resin cure begins during filling and continues after the filling process. Once the part is cured, it is de-moulded. Glass fibre reinforced unsaturated polyester is the common composite material used in RTM because of its ease of handling and low cost. Many factors, such as fibre volume fraction, filler content, mould - 3 0 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM temperature and injection pressure, may affect the quality of the surface finish of a composite component manufactured by R T M technique. A class-A surface finish used in the automotive industry is often referred to as an acceptable standard for exterior body panels [Rao (1988)]. The market, the type segment and the brand influence the definition for a class-A surface finish. The standards for the class-A finish are established only for the metallic parts. The general definition of a class-A surface for a composite part given by Neitzel et al [Neitzel et al. (2000)] is: "a substrate made of composite material represents a class-A surface, if its optical appearance is identical to an adjacent steel panel". 3.1.1. Definition of Surface Texture Surface texture is the repetitive or random deviation from the nominal surface that forms the three dimensional topography of the surface. Surface texture includes roughness, waviness, lay and flaws as shown in Figure 3.2 [ANSI/ASME B46.1]. 3.1.1.1. Surface Roughness Surface roughness consists of the finer irregularities of the surface texture. Surface roughness can be specified by many different parameters. Two of the popular parameters which are given in the American Standard [ANSI/ASME B46.1] are described below. Roughness Average (Ra) This parameter is also known as the arithmetic mean roughness value, arithmetic average (AA) or centerline average (CLA). The arithmetic average deviation from the centerline is defined as: o (3.1) where: / = the sampling length -31 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM y = the ordinate of the profile curve Root-Mean-Square Roughness (Rq) The root-mean-square deviation from the centerline is given by: V (3.2) 3.1.1.2. Surface Waviness Surface waviness is the more widely spaced component of surface texture. Surface waviness is intrinsically multi-dimensional and is best described by a number of surface parameters that characterize its geometric and topographical properties such as amplitude, wave length, wave shape, and spatial frequency content [Karpala (1993)]. Surface waviness is usually classified into 2 categories: short-term and long-term waviness. The dimensional scale of short-term and long-term surface waviness is a source of confusion. Different authors give different ranges of wavelengths. A summary of these wavelength ranges is given in Table 3.1. A more comprehensive definition of the wavelengths and amplitude is given by [Karpala (1993)]. In his definition, he subdivided the short-term waviness into two regimes: short-term waviness regime and orange peel regime. His definitions are summarized in Table 3.2. 3.1.2. Factors that Affect Surface Quality of a Composite Panel There are many factors that may affect the quality of a fibre reinforced composite surface. These factors can generally be divided into three categories: 1. Material parameters 2. Geometrical parameters - 3 2 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM 3. Processing parameters The material parameters include resin chemistry, fibre volume fraction and filler content. The geometrical parameters include type of fibre mat (textile, unidirectional, short fibre, random fibre, etc.), part thickness, and tool surface condition. The processing parameters may include mould temperature, pressure, cure time, etc. Kia [Kia (1987)] performed an experiment to investigate the influence of resin chemical shrinkage and resin thermal strain. In his experiment, polyurethane resin was cured at 70 °C into a thin film and was cut into rods. Then the rods were mixed with fresh resin to make a plaque and the plaque was cured at 70 °C and cooled down to room temperature. The surface of the plaque was visually examined before, during and after curing. No surface deformation was observed. Then the same experiment was repeated with glass bundles instead of the polyurethane rods. No surface deformation was observed at the moulding temperature. But surface deformation was observed when the plaque is cooled down to the room temperature. From these results, he concluded that the coefficient of thermal expansion of the resin is primarily responsible for the surface deformation and no contribution from cure shrinkage is due to the fact that the cure shrinkage takes place while the resin is fluid enough to flow. In his conclusion, he assumed that the CTE of the uncured and the cured resin are the same. But in reality, the CTE of uncured resin is almost twice as the CTE of cured resin [Svanberg and Holmberg (2001)]. He also showed that surface waviness increases with fibre content and decreases with filler content. The fillers which have a considerable aspect ratio increase the surface waviness i.e. glass bubbles gave better surface quality than milled glass fillers. Landsettle and Jensen [Landsettle and Jensen (1986)] investigated the effect of variables in the following three areas on the surface quality of SMC parts: Compounding, Moulding and Formulation. In the compounding process, they evaluated 16 oz. mat and 24 oz. mat and found out that 16 oz. mat was desirable to 24 oz. mat in surface waviness. In moulding area they evaluated parameters such as charge size, mould temperature, mould pressure and part thickness, while in the formulation area they evaluated -33 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM different resin chemistries, cure mechanisms, fillers, magnesium oxide concentration and fibreglasses. The affects of the above parameters on the surface waviness are given in Table 3.3. 3.1.3. Numerical Modelling of Surface Waviness Although much work has been done on experimentally measuring the effect of various parameters on the surface quality of composite parts, to the authors' knowledge not much work has been done on numerically modelling the surface finish. Kia [Kia (1986a) and (1986b)] developed an analytical model to simulate the surface deformation of glass-mat reinforced composites as a function of such factors as moulding temperature, thickness of glass fibres, and the thermal expansion properties of the resin and the glass fibre. Figure 3.3 shows the schematic model of two parallel glass fibre strands embedded in resin used in this analysis. The fibre strands are apart by a distance L and have an effective thickness of h. The top layer material is as same as the resin. The resin is partitioned into N infmitesimally thin sub-layers. The thermal contraction of each sub-layer is assumed to contribute to the deflection of all of the material that lies above that sub-layer. The response of the materials above each sub-layer, to the thermal contraction of that sub-layer, is assumed to be similar to that of an elastic beam. The top layer is assumed to act as a thick single layer, having no restriction from the glass walls. Based on these assumptions a mathematical expression is derived, which can be used to calculate the extent of surface deflection. Sanfeliz et al [Sanfeliz et al. (1992)] presented a numerical model of plain weave graphite/epoxy composites to simulate the effect of pressure and thermal loads on their surfaces. The woven composite model is simulated by examining two representative regions as shown in Figure 3.4. Region A represents a cross section where the warp and filling yarns cross over one another while region B isolates a matrix rich section. Regions A and B are divided into three uniform sections as shown in Figure 3.4. The material properties of each section are calculated using an in-house developed program called ICAN. Then the properties of these sections are used in a finite element model to predict the surface waviness. - 3 4 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM 3.1.4. Objectives This study was part of an Auto2l' project2. The project consisted of characterizing the material, manufacturing sample panels, measuring the surface finish of the manufactured panels and numerical modelling of the surface finish. The universities involved in the project are The University of British Columbia, McGill University, Concordia University and Ecole Polytechnique of Montreal. Our part of the project was to develop a numerical methodology to identify and quantify the effects of some of the surface finish factors that were mentioned earlier. A R T M process has two main parts: injection of the resin into the preform and curing of the resin. The numerical analysis of the resin injection is done using the finite element software, LCMFlot at McGill University [LCMFlot (2001)]. Our focus is mainly on the curing portion of the process. In order to do the numerical modelling of the curing process, some information, such as material characterization and the results from the injection simulation, from the other project partners were necessary. Since all the components of the project started at the same time, some of the necessary information had to be obtained from the literature. The objectives of this chapter are as follows: 1. To numerically simulate the curing portion of the RTM process 2. To acquire the necessary material characterization data for glass fibre reinforced polyester material from the literature 3. To identify the source of surface waviness in composite body panels 4. To numerically quantify how these sources contribute to surface waviness at different scales 1 AUT021 is a multi-disciplinary, auto-related research and development (R&D) initiative established by the Canadian Federal Networks of Centres of Excellence (NCE) program. 2 Theme C - Materials and Manufacturing C03-CPC: Polymer Composites - 3 5 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM 3 . 2 . N U M E R I C A L P R E D I C T I O N O F S U R F A C E W A V I N E S S 3.2.1. Simulation of R T M Process As stated previously, in a R T M process, the resin is injected in to the preform and cured under a prescribed cure cycle. Even though the curing process starts at the instant of injecting the resin, it is assumed that the curing process starts at the end of the injection process and after the resin wets the fibre preform uniformly (full saturation). This assumption is justified since the injection time is much smaller than the curing time. The analysis of the curing process is done using the CCA modular approach introduced in the previous chapter using the finite element software ABAQUS (CCA/ABAQUS). In order to do the simulation, the CCA modules for glass fibre reinforced polyester material are established first. The brief review of the thermo-chemical and mechanical property development models available in the literature for the glass fibre reinforced polyester material can be found in [Arafath et al. (2002)]. The CCA module developed based on this review for GFRP (Glass fibre reinforced polyester) material is given in Appendix B. 3.2.2. Identifying the Sources of Surface Waviness To identify the sources of the surface deformation, consider the deformation of a C-shaped composite part cured using the R T M process as shown in Figure 3.5. The part can be made of any type of glass preform and polyester resin. The tool is made of aluminum. The tool-part assembly is cured under the temperature cure cycle shown in Figure 3.6. The possible deformed shape of the part is shown in Figure 3.7(a). In aerospace applications, the major concern is the overall process-induced dimensional changes as shown in some of the examples in the previous chapter. These large scale dimensional changes are due to the residual stresses developed during processing at the "macro-level" i.e. at ply and higher level. The well-established sources of these stresses are tool-part interaction, anisotropic thermal strain of the part and thermal gradient in the thickness direction of the part [Johnston et al. (2001)]. In the analysis for this large scale deformation, the fibro-s e -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM resin combination is replaced by a composite material with equivalent properties which are normally calculated using micro-mechanics equations. Other than this large scale deformation, there may be other small scale deformations as shown in Figure 3.7(b) which are important in automotive applications. These deformations are similar to those observed in metallic automotive body panels. These local deformations are due to the residual stresses developed at the "micro-level" i.e. individual fibre and matrix level. These stresses are generally ignored in the analysis for the overall dimensional changes since they are very small and are self-equilibrating. The main source of the micro-level stresses is the thermal strain mismatch between the fibre preform and the resin. In the following sections, the process-induced deformation of the C-shaped part is numerically modelled using CCA/ABAQUS. The process-induced deformations due to micro-level and macro-level stresses are analysed separately and the predicted deformations are classified according to the standard surface finish classification established for metallic auto body panels. 3.2.3. Surface Deformation due to Micro-Level Stresses The micro-mechanical stresses that occur at the fibre/yarn level may lead to local wrinkling of the surface. For example, the resin top surface between two fibres deforms due to the thermal strain mismatch between the fibre and the matrix (Figure 3.8). The scale of the deformation depends on the dimensional quantities such as the fibre diameter (d) and distance between two adjacent fibres (/). This shows that the scale of deformation may be depend on the type of fibre preform used in the part. Hence, in this study the surface textures of 4 different types of fibre preform are investigated: 1. Unidirectional fibre laminate 2. Random short fibre mat 3. Unidirectional fabric 4. Two-dimensional woven fabric - 3 7 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM 3.2.3.1. Boundary Condition It is undesirable to analyze a complete structure with very small details. Due to the periodic nature of composite structures, generally a representative volume element (RVE) of the structure can be identified and analyzed instead of the whole structure. The selected RVE in this case is a small element close to the tool (Figure 3.9(a)). The dimension of the RVE depends on the fibre preform used. The RVE is constrained at the top by the tool and at the bottom and on the side by the rest of the part. When the tool is removed, the stresses in the top layer cause the top surface to deform. The boundary condition on the RVE, before and after the tool removal, is shown in Figure 3.9(b). 3.2.3.2. Unidirectional Fibre Laminates Unidirectional composite laminates are made of continuous fibres which are aligned parallel to each other (Figure 3.10). In the lamina, the fibre arrangement is random with each fibre having different cross sectional shapes and sizes. In an ideal situation, and for the purpose of theoretical analysis, the fibres can be considered to be arranged in square or hexagonal-packed arrays with each fibre having a circular cross-section and the same diameter (Figure 3.11). Finite Element Model In this analysis, the fibres are assumed to have circular cross-sections with 10 um diameter. The fibre volume fraction of the material is assumed to be 50%. The considered R V E has 90 fibres arranged in a 0. 4 mm x 0.04 mm planar domain. The fibre may be arranged randomly or in a square-packed array or in a hexagonal packed array as shown in Figure 3.12. The random arrangement is generated using the following algorithm: The centres of the reinforcements are generated using a Poisson random number generator with two constraints: 1. The minimum allowable distance between the centres of the fibres is twice the fibre radius 2. A l l the fibres are completely constrained within the domain. - 3 8 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Due to the periodic nature of the fibre arrangement for the square-packed and hexagonal-packed arrangements, only a small portion of the RVE, as shown in Figure 3.12, is considered for the analysis. For the random arrangement, the full RVE is considered for the analysis. The finite element meshes used for the analysis are shown in Figure 3.13. The square and hexagonal arrangements are modelled using 8-noded rectangular solid elements. The random fibre arrangement is modelled using a mixture of 8-noded rectangular solid elements and 6-noded triangular solid elements. Since the stresses and strains are independent of the axial coordinate, only one element is considered in the axial direction. The unit cells were virtually cured under the specified cure cycle. The temperature is assumed to be uniform in the unit cell (due to the fact that the considered layer is very thin and it is adjacent to the tool). At the end of the cure cycle the tool is removed and the deformation of the top surface is analysed. The surface deformations for all three fibre arrangements are shown in Figure 3.14. According to all of these figures, the total surface deformation is less than 1 micron and the wave length is around 10-15 microns which comes under the category of surface roughness and can be classified with a surface roughness number ( Ra ). 3.2.3.3. Random Short-Fibre Mat Random short fibre composites consist of chopped fibres laid randomly and held loosely together by an adhesive binder as shown in Figure 3.15. Advantages of this form include its high permeability and hence the easy flow of resin in the infusion step for thorough wet-out, easy handling for placement in the mould and good structural integrity. Some limitations are its relatively poor stiffness and strength, the lack of control of fibre orientation, and the ability to achieve only limited fibre volume fractions (Vj). The typical values of Vy for commercial mats are in the range of 10% - 30% [Hull (1981)]. For short random fibre composites, compared to continuous unidirectional fibre composites, there are many more micro-- 3 9 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM structural variables such as fibre length distribution (FLD) and fibre orientation distribution (FOD) which can affect the mechanical and thermal behaviour of the material. According to the data found in the literature, the FLD has a pronounced skew distribution with the tail at the long fibre end (Figure 3.16). Zak et al. [Zak et al. (2000)] reported a two parameter Weibull distribution for FLD: 6-1 EXP(- (3.3) where a and b are shape parameters and / is the fibre length. The 3D orientation of an individual fibre in a composite can be described by two angles (p and 9 as shown in Figure 3.17. In the following discussions, the angle q> and 9 will referred to the in-plane and out-of-plane orientations respectively. The probability distributions of 9 and <p for a specimen made from photopolymer and milled glass fibres are shown in Figure 3.18 [Zak et al. (2001)]. The figure shows that the FOD does not follow a distribution pattern, rather the distribution is mostly random. Numerical Modelling For the analysis, the considered representative volume element (RVE) has an in-plane dimension of 0.55 mm * 0.55 mm and a thickness of 39 urn. The RVE contains 100 fibres of diameter 10 um. The fibre length varies from 500 urn to 50 pm and has a 2 parameter Weibull distribution with a = 0.26 and b = 2.0 as shown in Figure 3.19. The number average fibre length is 227 urn and the volume fraction of the RVE is around 15%. In the example, it is assumed that the fibres are oriented two dimensionally i.e. only in-plane orientation is permitted. The orientation angle of each fibre is assigned randomly. Random Fibre Generation The fibres with the prescribed fibre length distribution were randomly placed inside the RVE using a Monte-Carlo algorithm. In this algorithm, the position of the fibre centroid and the in-plan orientation -40-Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM angle are assigned randomly to each fibre as shown in Figure 3.20. Due to symmetry, the fibre orientation angle is varied from -90° to 90°. A check for fibre overlapping has made on the currently placed fibre with the fibres placed already inside the RVE. If an overlap occurs then that fibre position and the orientation angle are rejected and a new set of random position and orientation angle is assigned to that fibre. The placement of the fibre started from the longest one to the shortest one. Even though the fibre volume fraction is relatively small, it was very difficult to place the fibres randomly inside the RVE. The seeds of the Monte-Carlo simulation were continuously changed until all the fibres were placed inside the RVE. Many simulations were made to get a homogeneous in-plarte orientation distribution. The achieved orientation distribution for this example is shown in Figure 3.21. Finite Element Analysis The RVE was meshed using the commercial finite element software, Hypermesh [Hypermesh (2004)]. Around 178,000 4-noded tetrahedron elements were used for the analysis (Figure 3.22). Meshing was time consuming and tedious. Due to the limitation of the meshing software, all the fibres were assumed to be well within the R V E (no intersection between the fibre and the R V E outer faces). The RVE was allowed to cure under the prescribed temperature cycle. At the end of the curing process, the tool was removed and the top surface profile was analysed. The deformed surface profile of the top surface is shown in Figure 3.23. A comparison between surface waviness of random short fibre composite and unidirectional continuous fibre composite is shown in Figure 3.24. For the random short fibre composite, the deformation is along x = 270 um line. Both have almost the same magnitude of roughness value which is less than 1.0 um. Hence, the surface deformation of the part made of random short fibre laminate can be classified with a roughness number as in the case for the unidirectional fibre laminate. -41 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM 3.2.3.4. 2D Woven Fabric Woven fabrics are made by interlacing two or more yarn system at an angle. The warp yarns run parallel to the weaving direction, with the fill (weft) yarns running perpendicular to the warp yarns. Various types of weaves can be identified by the repeating pattern in both directions. Based on the repeat patterns, the weaves can be classified as plain, twill, and satin. Cross Section of a Yarn Fibre yarns or strands are composed of a variable number of single filaments of diameter around 10 um. The number of filaments in each yarn depends on the type of application intended for that yarn and can vary from tens to thousands. There are several types of yarns that have distinct properties. The two most common yarns are spun yarns and multifilament yarns. Spun yarns are formed from staple fibres and twisted to provide strength to the yarn. Multifilament yarns are formed from continuous fibres that have only some nominal twist applied to add integrity. The vast majority of yarns used for composite applications are multifilament yarns [Bogdanovich and Pastore (1996)]. In this analysis, we only consider the multifilament yarn. We assume that all fibres in the yarn are run in the same direction as the yarn (no twist). The intra-yarn fibre volume fraction is assumed to be a constant. Usually, the value of the fibre volume fraction is about 75% (note that an absolute maximum of 91% is reached when the fibres are hexagonally packed). The interlacing of the yarn and the processing of the composite (application of pressure) leads to yarn flattening. Therefore, the assumption of circular yarn cross-section is unrealistic. The possible realistic yarn cross sections are elliptic or lenticular (Figure 3.25). Using the constituent properties of the resin and the fibre, the three dimensional unidirectional composite yarn properties are calculated, for specified fibre volume fraction, according to the well-established micromechanics model for continuous fibre composites [Hashin and Rosen (1964)]. - 4 2 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Plain Weave Fabric The geometrical unit cell of a plain weave fabric is shown in Figure 3.26. The unit cell consists of the interlacing region and the gap region. The interlacing region consists of warp and fill yarns one over another and the gap region consist of fill yarn or warp yarn and the pure matrix. Based on observation of the micrographs, the following requirement regarding the geometric characteristic of the plain weave is made [Kuhn and Charalambides (1999)]: 1. The cross sectional area of the yarn is assumed to be constant for different cross section along the length of the yarn 2. The width of the yarn is assumed to be constant along the longitudinal direction of the yarn. 3. The fibres and the slope of the fibres are assumed to be continuous. 4. The fill and the warp yarns are assumed to be in full contact throughout the interlace region. Many studies have attempted to define the orthogonal plain weave fabric lamina geometry mathematically. The mathematical functions used to define the geometry were linear, circular or sinusoidal functions [Ishikawa and Chou (1982), Naik and Shembekar (1992), Naik and Ganesh (1995), Ganesh and Naik (1996)]. Kuhn and Charalambides [Kuhn and Charalambides (1998a), Kuhn and Charalambides (1998b), Kuhn and Charalambides (1999), Kuhn et al. (1999)] introduced a piecewise continuous mathematical (sinusoidal) function to describe the geometry. In this study, we follow this approach to model the plain weave geometry. Finite Element Model The geometrical description of a cross section of the plain weave unit cell is shown in Figure 3.27. The sinusoidal curves that describe the geometry are given by: -43 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM V l O ) = - l c o s l y2(x) = -\ COS| V 3(JC) = -/7Cos| v 4 (x) = -h cos +1 -1 V s J KPJ n{x-{s-0)) P (0 < x < s) (0 < x < s) (0<x<a/2) (s-a/2 < x < s) (3.4) The geometrical parameters used in the finite element studies are: ctj- = aw = 2.5 cm gf =gw=0.5cm hf = hw = 0 .25 cm (3.5) These geometrical parameters are typical values for the fabrics found in the literature. The finite element mesh generated using HyperMesh software is shown in Figure 3.28. The plain weave is modelled using 8-noded isoparametric brick elements. In order to avoid collapse of the thin matrix elements at each of the 8 corners, an additional matrix thickness of 0.1 h is used. At the interlacing region, the warp and fill yarns are assumed to be in full contact throughout the curing process. In reality there may be relative movement between the two yarns. This will depend on the inter-yarn friction. In this analysis, since both yarns are impregnated with the resin, the assumption of full contact (no slip) is justifiable. The deformed top surface profile of the fabric is shown in Figure 3.29. The top surface deformation of the unit cell along the diagonal length is shown in Figure 3.30. According to this figure, the total deformation consists of about 2.5 microns of uniform deformation and relative deformation of about 15 microns and the wavelength is around 8 mm. This scale of deformation comes under the classification of short-term waviness according to the standard classification for a metallic part. -44-Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Apart from the large scale surface deformation shown above, there may be small scale deformation at the individual fibre level which makes up the yarn. This small scale surface deformation is similar to the deformation observed in the unidirectional fibre laminate. 3.2.3.5. Unidirectional Fabric Unidirectional Fabric consists of parallel filaments held loosely in place by stitches in a plane (Figure 3.31). This has high stiffness and strength in the yarn direction, but not in the direction of the stitches. The yarn cross-sections are assumed to have a lenticular shape. The yarn transverse cross-sections are assumed to be uniform through the length of the yarn. Finite Element Model The chosen RVE for the analysis is shown in Figure 3.31. The geometrical description of a cross section of the unit cell is shown in Figure 3.32. The yarn cross-sections are assumed to have a sinusoidal top and bottom profile which are given by: v, (x) -- — cosl , \ h i ^2(*) = - - C 0 S | _y3(*) = - cos ^(x-g)^ V a f r 4 W = - T C 0 S 4 n(x-g) a (0<x<d) (0 < x < a) (a + g < x < s) (a + g < x< s) (3.6) The geometrical parameters used in the finite element studies are: a = 2.5 cm g - 0.5 cm h - 0.25 cm (3.7) The finite element mesh of the R V E generated using HyperMesh software is shown in Figure 3.33. In the analysis the presence of the stitches is omitted. The RVE is modelled using 8-noded isoparametric brick - 4 5 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM elements. In order to avoid collapse of the thin matrix elements at top of the yarns, an additional matrix thickness of 0.1 h is used. The fibre-matrix arrangement is virtually cured under the prescribed cure cycle. The resulting deformed surface profile is shown in Figure 3.34. The total deformation consists of about 2.5 microns of uniform deformation and relative deformation of about 7 microns and the wavelength is 5.5 mm. Similar to the plain weave fabric, the surface deformation of the unidirectional fabric also comes under the classification of short-term waviness and there may be small scale deformation at the individual fibre level which makes up the yarn. 3.2.4. Surface Deformation due to Macro-Level Stresses To quantify the process-induced long-term waviness, the complete structure is analysed. The finite element model is shown in Figure 3.35. Full bonding condition is assumed between the tool and the part. Due to symmetry, only half of the problem needs to be analyzed. The part can be made of any of the fibre preform type discussed in the earlier section. But, in this study, it is assumed that the part is made of unidirectional continuous fibre laminates. The part is assumed to have uniform material properties and the material property of a layer is computed using micromechanical equations [Rosen and Hashin (1964)] based on the overall fibre volume fraction of the part (50%). At the end of the cure cycle, the tool is virtually removed and the deformation of the part is measured. The deformation is mainly due to the anisotropic thermal strain in the longitudinal and transverse direction and the thermal strain mismatch between the tool and the part. Due to the anisotropic thermal strain, the corner of the part springs in/out and due to the thermal strain mismatch between the tool and the part, the web and the flange of the part warps as shown in Figure 3.36(a). Since the tool is in both sides of the web and flange, it should be expected that the thermal mismatch effect will be symmetric and it will not cause the part to warp. But, as the internal tool expands, it stretches the part as shown in Figure 3.36(b) which may result in warpage of the web. The deformation of the web is shown in Figure 3.37. - 4 6 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM The maximum web deformation is around 45 microns and the wavelength is around 200 mm. This large scale deformation can be classified as long-term waviness. 3.3. D I S C U S S I O N Surface finish problem of automotive industry is essentially a dimensional control problem faced by the aerospace industry. Since the interested scale of dimensional changes in automotive applications is very small (microns), the stresses built up at different levels should be considered whereas in aerospace application only the stresses at macro and higher levels are of interest. It is shown in this study that the fibre preform type used in the manufacturing of auto body panels is the major source of different scales of surface waviness. The resultant surface deformations for different fibre preform types are summarized in Table 3.4 and Table 3.5. Apart from the fibre preform, other sources, such as resin chemistry and processing condition, may affect the surface finish. Contribution of these factors can be easily studied using the established numerical methodology. For example, Figure 3.38 shows the contributions of resin cure shrinkage and CTE mismatch to the surface deformation of a unidirectional fibre laminate which are approximately 70% and 30% respectively. This is contrary to what is found in the literature [Kia (1986a)]. Since the material data of the polyester material used in our analysis is not complete, the above fact cannot be fully verified. The above study was conducted in a deterministic manner where all the parameters involved, such as fibre diameter and fibre orientation, were assumed to have fixed values, while in reality this is not the case. Uncertainties involved in each of these parameters. Hence, the problem should be studied in probabilistic manner to determine the sensitivity of each of these parameters on surface finish. 3.4. S U M M A R Y A N D C O N T R I B U T I O N S Composite materials have the advantage of being light weight compared to their metallic counterparts in the automotive application. But the poor surface finish of composites parts is the major obstacle for their usage in the outer automotive body panels. Many factors such as the resin chemistry, fibre preform type - 4 7 -Chapter 3: Surface Finish cf Automotive Composites Parts Manufactured by RTM and processing condition can affect the surface quality of the composite parts. As part of a large project to identify and quantify the contribution of these factors to the surface quality, our main aim is to numerically predict the surface quality observed in the experiments. Since experimental data were not available at the time of this study, most of the data were obtained from the available literature. Using these data, the stresses that can develop at different scale levels were identified which can contribute to different levels of surface deformation. To the author's knowledge, this is the first study that divides the surface deformation observed in composite auto body panels into different scale levels which is consistent with the standard classification established for metallic parts. - 4 8 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Table 3.1 Definition of surface waviness by different authors Reference Wavelength (mm) Short term waviness Long term waviness Hupp (1988) <6 6-25 Reynolds (1992) <6 6-25 Neitzel et al. (2000) 0.1-0.6 0.6-10 Love etal. (2001) <0.6 >0.6 Love etal. (2001) <5 5 - 100 Table 3.2 A comprehensive definition of surface waviness given by Karpala [Karpala (1993)] Waviness Regime Wavelength (miri) Amplitude (um) Surface roughness <0.5 < 1 Orange peel 0.5-6 < 1 Short term waviness 6-25 < 10 Long term waviness >25 <25 Table 3.3 Material and geometrical parameters and their effects on surface finish Parameters Effect of the parameter on surface waviness Moulding Parameters Charge size Reduction surface waviness noted using the largest possible part coverage Mould pressure Lowest mould pressures possible to fill the tool produced the best possible quality Viscosity of materials Lower viscosities were better, however, part design dictates the required viscosity Mould temperature Lowest temperature gives the best surface quality Cure time No difference in surface quality Part thickness Thicker the part, the better the surface quality Formulation Resin chemistry Proprietary Filler particle size Smaller particle size gives better surface quality Filler content Higher filler content gives good surface quality at higher mould temperature. Lower filler content gives good surface quality at lower mould temperature3 Glass reinforcement Fibre chopped length 1" is preferred over 0.5" and 2" Fibre volume fraction Highest Vf gives better surface quality 3 It is reported that these results did not correlate with the industry's belief of "the more the filler, the better the surface". - 4 9 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Table 3.4 Long-term and short-term surface waviness for different fibre preform types Waviness type Amplitude (urn) Wave length (mm) Long-term waviness C-shaped part 45 200 Short-term waviness Unidirectional fabric 7 5.5 Plain weave fabric 15 8.0 Table 3.5 Surface roughness values for different fibre preform types Surface roughness R a (urn) Ra(um) Random short fibre laminate 0.072 0.087 Continuous unidirectional fibre laminate Square 0.031 0.034 Hexagonal 0.038 0.042 Random 0.056 0.068 -50-Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM I Resin Injection Moulding | De-moulding Curing Figure 3.1 Schematic description of the R T M process Figure 3.2 Schematic showing the definition of surface texture of a metallic surface -51 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Glass fibre / < • Figure 3.3 Schematic of the model showing a pair of fibres in parallel embedded in a resin matrix used by Kia (1986) to study surface waviness. Figure 3.4 Schematics of the model of woven composites used by Sanfeliz et al. (1992) to study surface waviness -52-Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Figure 3.5 Schematic of a composite C-shaped part in an aluminum closed mould in R T M processing Figure 3.6 Typical 2-hold temperature cure cycle used for curing of polyester resin - 5 3 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Original Shape (a) Large scale deformation (b) Small scale deformation Figure 3.7 Schematic of the possible deformed shape of the of a C-shaped composite part processed using R T M Figure 3.8 Schematic of the dimpling between two adjacent fibres due to thermal strain mismatch between fibre and resin - 5 4 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM \ \ ^ \ w ^ w \ \ ^ \ \ W M ^ \ \ ^ \ R V E Before Tool Removal \\^ \\ T^ v» TvKv\ vSv* vMv* l^ vT^^v* 4 4 If p R V E After Tool Removal vffiw n«M r^ vi ^^ v» wRvi T^vi vMv> Figure 3.9 Schematic of the C-shaped part inside the mould and the selected R V E close to the top tool surface. The applied boundary condition on the R V E before and after tool removal is also shown SECTION A - A Figure 3.10 Schematic of a unidirectional continuous fibre laminate - 5 5 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM y f y " Fibre IQOOOO^ uoM Figure 3.11 Schematic of the ideal fibre arrangement (square and hexagonal) in unidirectional fibre composite laminate 11::::::^:::::::::::::::::::: Unit Cell <f ( a ) (b) •••••••••••V • • • •••••JI ••••• ••••• ••% •% (c) Figure 3.12 Schematic of the fibre spatial distribution in a unidirectional fibre laminate (a) square arrangement (b) hexagonal arrangement and (c) random arrangement - 5 6 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Figure 3.13 Finite element mesh of (a) square arrangement (b) hexagonal arrangement, and (c) part of random fibre arrangement - 5 7 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Distance along the surface (um) -0.3 -i 1 1 1 1 1 -0.7 Figure 3.14 Comparison of surface deformation of square, hexagonal and random fibre arrangements Figure 3.15 Schematic of random short fibre composite - 5 8 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM 28 24 20 is 16 o u 1 12 s Z, fl + K1 \ \ 1 2 3 Fibre length (mm) Figure 3.16 Typical fibre length distribution (FLD) of the fibres in a random fibre mat 0 S » Sit 0S# S2K Figure 3.17 Definition of in-plane and out-of-plane fibre orientation of a fibre in a random short fibre mat - 5 9 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM -200 -100 0 100 In-plane angle, <j> (deg) (a) 200 4.5 4.0 " 3.5 " 3.0 -2.5 -2.0 " 1.5 -1.0 " 0.5 Z_ 0.0 0 20 40 60 80 Out-of-plane angle, 6 (deg) (b) 100 Figure 3.18 Experimentally observed fibre orientation distribution (FOD) of a typical random fibre mat Figure 3.19 Fibre length distribution (FLD) used in the analysis of the surface deformation of a part with random short fibre mat - 6 0 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Figure 3.20 Definition of centroidal position and the in-plane orientation of the fibre in the process of randomly generating the fibre in a random short fibre mat 12 -I : 10 1 I — I I 1 1 1 4 H 2 " 0 -1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 In-plane orientation angle (deg) Figure 3.21 Fibre orientation distribution (FOD) used in the analysis of the surface deformation of a part with random short fibre mat -61 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Figure 3.25 Schematic of the possible yarn cross section in a fabric (a) elliptical (b) lenticular - 6 3 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Figure 3.30 Top surface deformation of plain weave fabric unit cell along the diagonal length Figure 3.31 Schematic of unidirectional fabric mat - 6 6 -Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Figure 3.34 Deformation profile of the top surface of unidirectional fabric Figure 3.35 Finite element mesh used for the analysis of the process-induced deformation of a C -shaped part in a closed aluminum mould -68-Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Original Shape Deformed Shape / / / / fr / | ' S / fr / © ' a / 3 / / / L. J (a) (b) Figure 3.36 (a) Deformed shape of the part after removed from the tool (b) the tool stretches the part as it expands 0.05 10 15 20 25 30 35 40 Distance along the web from centre (mm) Figure 3.37 Deformation profile of the web of a C-shaped part after removal from the mould -69-Chapter 3: Surface Finish of Automotive Composites Parts Manufactured by RTM Distance along the top surface (pm) Figure 3.38 Contribution of resin cure shrinkage and C T E mismatch to the surface deformation of a unidirectional fibre laminate - 7 0 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures Chapter 4. USAGE OF STANDARD SOLID ELEMENTS IN THE PROCESS MODELLING OF SHELL-LIKE STRUCTURES 4.1. INTRODUCTION Shells are a special type of three-dimensional body in which one dimension, the thickness, is much smaller compared to the other dimensions. Over the past few decades numerous finite element models based on the degenerated shell concept have been proposed for the analysis of thin shell structures [Yang et al. (2000) and Kratzig and Jun (2003)]. The degenerated shell element concept was implemented and applied first by Ahmed et al. (1970) and later by many authors such as Bathe (1996) and Hughes (1987), including different alternatives and improvements. Degenerated shell elements are based on three assumptions: a straight line, normal to the mid surface, remains straight throughout deformation, the length of the normal remains unchanged throughout deformation and transverse normal stresses are negligible. The degenerated shell element uses three translational and two rotational degrees of freedom to include transverse and bending effects. The element needs only simple basic functions which satisfy C° continuity to maintain continuity across the element boundaries. When used in assumed displacement formulation, the performance of a degenerated shell element deteriorates rapidly as the thickness decreases. This phenomenon is called locking and results from the inability of an element to represent a zero in-plane strain (membrane locking) and transverse shear strain (shear locking) without disrupting the bending behaviour. Another approach to the finite element analysis of shell structures that allows for the modelling of arbitrary geometries without invoking a specific shell theory is to use three-dimensional solid elements [Kim and Lee (1988), Ausserer and Lee (1988), Park et al. (1995), Hauptmann and Schweizerhof (1998), Sze et al. (2002) and Areias et al. (2003)]. These elements are typically defined by two layers of nodes at the extreme surfaces of the shell, and are sometimes known as solid-shell elements. In fact, a solid-shell element is more convenient than a degenerated shell element since it does not need rotational degrees of freedom. However, when used in conventional assumed displacement finite element formulation, they - 7 1 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures also experience the effect of locking as degenerated shell elements do. In the solid element case, in addition to the shear and membrane locking it also experiences additional locking effects such as trapezoidal, thickness and volumetric lockings. Material anisotropy and tool-part interaction are the two main sources of process induced deformations in composite structures [Johnston et al. (2001)]. The finite element analysis should capture the residual stresses due to these sources accurately. Material anisotropy causes a curved composite part to spring-in. This is mainly due to the difference between the in-plane and through thickness thermal strains (Figure 4.1). Due to the limited ability of shell elements in capturing variations in through-thickness properties, this spring-in phenomena cannot be modelled using these elements. Tool-part interaction induces a large and non-linear stress gradient through the thickness of the part (Figure 4.2). This stress gradient causes the part to warp after removal of the tool. Due to the constant transverse shear strain assumption, classical shell elements cannot capture such highly non-linear stress gradients. These inadequacies of the shell elements may be improved by different theories such as ziz-zag theory and higher order shear deformation theories [Di Sciuva (1987), Bhaskar and Varadan (1989), Ghugal and Shimpi (2002), Carrera (2003), Sheikh and Chakrabarti (2003) and Arciniega and Reddy (2005)]. But solid elements have many advantages compared to shell elements especially in non-linear and contact problems. Hence, in our process modelling approach, the efficient use of solid elements in capturing the process-induced deformations is investigated. 4.1.1. Locking Phenomena and Remedies The locking problems mentioned earlier result from the approximations in the finite element formulations. The real displacement field is approximated by shape functions and the continuous integration is replaced by a summation at discrete points (integration points). In this section, a brief review of these locking phenomena and the different methods of alleviating them in the finite element formulation are presented. More details can be found in standard finite element text books [Zienkiewicz and Taylor (2000), MacNeal (1994), Belytschko et al. (2004) and Prathap (1993)]. - 7 2 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures Locking occurs due to the presence of "parasitic" stresses. Parasitic stresses refer to stresses that are not present in the exact solution. These are, for example, transverse shear stresses in the case of pure bending of a Kirchhoff plate element (shear locking) or membrane stresses in the case of in-extensional bending of shell elements (membrane locking). The resulting parasitic internal energy leads to an additional, artificial, stiffness. The ratio of this additional stiffness to the total stiffness of the structure can tend to one when a certain parameter approaches infinity. For example, in the case of transverse shear locking of plate elements this parameter is the slenderness of the plate, whereas in volumetric locking it is the bulk modulus. This means, that the prediction of structural behaviour is totally dominated by artificial, numerical effects and the actual mechanical or physical behaviour is not represented at all. Shear locking results from the inability of an element to bend without shearing. Shear locking predominantly occurs in linear elements with full integration (8-noded brick elements with 2*2*2 Gauss quadrature). It results in a deformation behaviour that is too stiff i.e. the displacements are too small. Consider a 4-noded linear plane stress element under pure bending at the edges as shown in Figure 4.3(a). Figure 4.3(b) shows the actual deformation shape under a uniform bending load. The plane section perpendicular to the neutral axis remains plane and perpendicular after deformation. Figure 4.3(c) shows the predicted deformation of a linear 4-noded element. The linear element is unable to accurately model the curvature caused by bending. For a 2*2 Gauss quadrature (full integration), shear strain which does not occur in a pure bending case, is introduced into the element by this deformation mode. The energy absorbed due to this shear deformation causes a reduction in energy absorbed due to bending and hence the element predicts smaller nodal displacements. Consequently, the element does not predict the bending displacements accurately and will exhibit an overly stiff behavior. Membrane locking occurs in curved shell elements when the in-plane displacement approximation is not higher order than the transverse displacement approximation and inextensional bending of the shell cannot take place [Stolarski and Belytschko (1982)]. When an element is not capable of representing -73 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures inextensional bending, parasitic membrane energy is generated. In the same manner that parasitic shear causes shear locking, this spurious membrane energy causes membrane locking. Membrane locking severely reduces the rate of convergence of shell elements. The term "trapezoidal locking" originates from the stiffening phenomenon in trapezoidal-shaped or tapered 4-noded plane elements which are unavoidable in modeling curved parts [MacNeal (1994)]. Solid-shell elements suffer from so-called thickness locking (also known as Poisson's locking), if a linear displacement assumption in thickness direction is used. In the pure bending case, the through-thickness stress should be zero. But through-thickness stress will be constant due to the constant through-thickness strain and linear due to the Poisson's coupling with the linear in-plane strains. Hence, in a pure bending situation, instead of zero through-thickness stress, a linear through-thickness stress would result, leading to an overly stiff behaviour [Buchter et al. (1994)] Volumetric locking occurs when spatial discretization of the finite element mesh is not able to describe the response of continuum in volume-preserving mode. Volumetric locking depends on the Poisson's ratio of the material. Hence, it is also called Poisson locking. In elasticity, volumetric locking occurs when the material approaches an incompressible state, i.e. the Poisson's ratio is very close to 0.5 [Doll et al. (2000)]. Most of the locking problems described above occur in linear elements. These locking effects are not adverse in higher order elements such as 20-noded solid elements. Many methods are suggested to overcome the locking problems such as the reduced integration technique, assumed natural strain method (ANS), enhanced natural strain method (ENS) and hybrid stress/strain methods [Sze (2002), Petchsasithon and Gosling (2005)]. Among all these methods, the reduced integration technique is the most attractive and computationally efficient [Zienkiewicz et al. (1971), Prathap and Bhashyam (1982), Stolarski and Belytschko (1983), Azevedo and Awruch (1999), Doll et al. (2000) and Dhondt (2002)]. - 7 4 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures 4.1.2. Objective In Chapter 2 and Chapter 3, it was shown that, with the developed CCA modular approach, any commercial finite element code can be used to model process-induced deformation of complicated composite structures. The main disadvantage of the previous analysis was that a fairly large number of solid elements were required to model the processing of a relatively small structure compared to a real industrial application. Roughly one element per layer was used to model the part in the thickness direction to capture the very large through-thickness stress gradients. This forces the use of a large number of elements in-plane in order to maintain the aspect ratio within the allowable limit (<5) for numerical accuracy. This is very inefficient since it may take days to set up and run the problem requiring enormous computing power. The ultimate goal of the present study is to lay the foundation to model a composite part as shown in Figure 4.4 with just one element in the thickness direction. The part has many features such as varying layer thickness and ply-drop. The main objective of the study in this section is to investigate the use of the solid element formulation in an efficient way to model shell-like structures. The required efficiency will be achieved by reducing the number of elements used in-plane. This will be achieved by increasing the aspect ratio limit of the solid element through alleviation of the locking problem with the reduced integration method. To investigate the effectiveness of the reduced integration technique in alleviating the locking problem, ABAQUS built-in solid elements with composite modelling features are tested with the combination of the CCA material modules. However, the ABAQUS built-in solid elements do not have all the features that are necessary to model a complicated structure such as those with arbitrarily varying layer thickness and ply-drop. To accommodate these requirements, we will develop a customized 3D solid element using the ABAQUS User Element (UEL) option. The formulation and the main features of this element are presented in the next section. -75-Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures 4 . 2 . 2 4 - N O D E D S T A N D A R D S O L I D E L E M E N T The solid-shell element developed in this section has been implemented in ABAQUS using the user element (UEL) subroutine as shown in Figure 4.5. Similar to the material constitutive module (CCA) developed in Chapter 2, the element module developed here is also general and can be implemented in any finite element code. ABAQUS is chosen as the numerical test bed in this study. 4.2.1. ABAQUS User Element Concept For a general user element, user subroutine UEL must be coded to define the contribution of the element to the model. ABAQUS calls this routine each time any information about a user-defined element is needed. At each such call ABAQUS provides the values of the nodal coordinates and all of solution-dependent nodal variables (displacements, incremental displacements, velocities, accelerations, etc.) at all degrees of freedoms associated with the element, as well as values of the solution-dependent state variables associated with the element. ABAQUS also provides the values of all user-defined properties associated with this element and a control flag array indicating what functions the user subroutine must perform. Depending on this set of control flags, the subroutine must define the contribution of the element to the residual vector, define the contribution of the element to the stiffness matrix, and update the solution-dependent state variables associated with the element. The element's principal contribution to the model during general analysis steps is that it provides nodal forces R that depend on the values of the nodal variables u. The force can be: physical force when the associated degree of freedom is physical displacement, moment when the associated degree of freedom is a rotation, heat flux when it is a temperature value, and so on. The signs of the forces in R are such that external forces provide positive nodal force values and "internal" forces caused by stresses, internal heat fluxes, etc. in the element provide negative nodal force values. -76-Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures 4.2.2. Element Formulation The solid element has 24 nodes in total as shown in Figure 4.6. A l l nodes have the 3 conventional displacement degrees of freedom (u,v,w). The element is a composite element with different number of layers. The layers may be of the same material with different orientations or different materials (hybrids). The layers are assumed to be stacked in the thickness direction. The thickness direction of the element is identified by the nodal connectivity as shown in Figure 4.6. For each element, the element contribution to the global stiffness matrix (K ) and load vector ( R ) should be defined inside the ABAQUS subroutine. These quantities are defined for an element as: where: B - Strain-displacement matrix D - Material stiffness matrix N - Displacement shape functions p - Surface tractions o~ - stress vector 4.2.3. Numerical Integration The element stiffness matrix is given by: v (4.1) v l l l (4.2) - l - l - l -77-Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures where | / | is the determinant of the Jacobian matrix. The integral is evaluated numerically by the combination of Gaussian quadrature and Simpson rule (Figure 4.7 ). 4-point reduced Gauss integration is used in-plane to avoid the locking effects described in Section 4.1.1. The reduced integration is necessary only in the in-plane direction [Robbins and Reddy, 1993]. Full integration should be used in the through-thickness direction (for an element with one layer, 3 Gauss points are necessary for full integration). The material stiffness matrix D varies from layer to layer and thus it is not a continuous function of £ . Therefore the integration is carried out layerwise in order to obtain the stiffness coefficients for the entire element. For the layerwise through-thickness integration both the Gauss and Simpson rules are used. If the integration scheme is Simpson then the number of integration points should be an odd number as shown in Figure 4.7 . In order to apply the known coefficients (weight functions) of the Gaussian and Simpson formula, the range should be between -1 and +1. This is achieved by suitably modifying the variable to £"* in layer k such that Qk varies from -1 to +1 in that layer: , - .•1 7=1 (4.3) t where t is the total thickness and tk is the k' layer thickness. Now the integration becomes: K"e = £ j J ]BTDB\J\ -*-d£dTjdGk (4.4) *=> - i - i - i f The integration procedure goes through 3 loops: First - in-plane integration, Second - layers and Third through-thickness integration. - 7 8 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures i=\ j=\ k=\ i=\ 1 (4.5) where w are the weight factors, nl is the number of layers and n^k is the number of through-thickness integration points of the k'h layer. 4.2.4. Geometric Description and Calculation of Jacobian Matrix The mapping functions for the coordinates are given by: 24 i y = flN,y, (4.6) I 24 where iV, are the typical tri-quadratic shape functions for a standard element. The Jacobian matrix is given by: dx 8y dz 3? dx dz drj dn dn dx by dz dC (4.7) 4.2.5. Formulation of B Matrix The displacement interpolation is given by: - 7 9 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures =2>,ii, i 24 i 24 = £ ; v > , . (4.8) where Nt are the same tri-quadratic shape functions used for the geometric interpolation (isoparametric element). Strains are defined according to small strain definition as: e = < £y Y xy 7* Y du dx 'dv du dv By dx (du dw^ dz dx f dv dw + dz dy (4.9) or s = Bu (4.10) 4.2.6. Element Property Definition Element property definition includes the number of layers, thickness of each layer, material id of each layer, the element orientation with global coordinate system, and the layer orientation with respect to element orientation as shown in Figure 4.8. In a complex shape composite part, these definitions are time consuming but crucial. Error in these definitions, especially orientation definition, leads to wrong results. For example, the spring-in prediction of a curved composite part with the use of rectangular and - 8 0 Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures cylindrical coordinate systems to define the element material coordinates as shown in Figure 4.9 may yield completely different results if the problem is modelled with fewer numbers of elements. The more ideal way of defining these properties is by using a pre-processor. This pre-processor can be a script file with the combination of any commercial pre-processors such as MSC Patran [MSC Software Corporation] or Fibersim [VISTAGY, Inc.] etc. The input for this pre-processor is the part master surface (tool top surface) with the lay-up information as shown in Figure 4.10. The pre-processor has two components: the extruder and property definer. The extruder meshes the master surface with general shell elements and extrudes them in the thickness direction to create the 24-noded solid element (Figure 4.10). The property definer defines the element properties at each integration point. This can be done by passing the coordinates of the in-plane integration points to the property definer. The output from the definer is the necessary layer and material orientation definitions. In the current study, the pre-processor part has not been developed. The layer thickness and the material orientation should be defined by the user. 4.2.6.1. Layer Thickness The layer thickness can vary arbitrarily. The varying layer thickness is defined at 4 points (4 coiner nodes) as shown in Figure 4.11 and the layer thickness at an integration point is obtained by linear interpolation. For example, the thickness of layer-1 at a generic point in plane is given by: ' = 1 (4.H) M , = - ( l + <f,£Xl+77,77) with corner nodes defined as = ±1 and 77, = ± 1 . 4.2.6.2. Material Orientation The material coordinate system of the element should be defined by the user such that the 3 r d material axis is in the through-thickness direction (Figure 4.8). The element material coordinates defines the orientation -81 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures of the bottom layer with respect to the global coordinate system. The material coordinates of the other layers with respect to the element material coordinates can be calculated based on the layer thickness at the four corners of the layers. An additional rotation 6 about the 3 r d material axis of each layer can also be defined. Currently two coordinate systems are used to define the element material coordinates: Rectangular coordinate system and cylindrical coordinate system as shown in Figure 4.12. The rectangular coordinate system can be defined by giving the coordinates of two points on local axes 1 and 2 or it can be defined by specifying 3 nodes as shown in Figure 4.13. The cylindrical coordinate system can be defined by providing the coordinates of two points along the axis of the cylinder as shown in Figure 4.14. In general cylindrical coordinate system, the axes 1, 2 and 3 are in radial, tangential and axial directions respectively. In the developed element, since the 3 r d material axis is assumed to be in the through-thickness direction (radial), additional rotations are made internally to make the 3 r d material axis in the through-thickness direction as shown in Figure 4.14. 4.2.7. Load 4.2.7.1. Mechanical Load Both concentrated and distributed loads can be applied to the element. Concentrated loads are prescribed at the element nodes using the ABAQUS ' * C L O A D ' option. No calculations inside the element are necessary to account for this load. Distributed load is applied to the element using the ' *DLOAD' option. The magnitude of the load is passed onto the element at each time step. The contribution of this load to the nodal load vector should be defined inside the element. Currently only the pressure load is considered for this element. The pressure load is applied either to the top or to the bottom surface of the element as shown in Figure 4.15. The load is assumed to be uniform and acting perpendicular to the surface. To which surface the load is applied is identified by the distributed load key C/„ . If n — 1, the load is applied -82-Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures to the bottom surface of the element and if n = 2 , the load is applied to the top surface of the element. The resultant consistent load vector at a node is given by: \pN,dA X'" •RPy • =jpNr A i dAy > K dAz (4.12) where dA is the vector of incremental areas, i.e. dAx is the incremental area in the y — z plane and /V, is the shape function corresponding to that node. The integration is performed using 4-point Gauss quadrature rule. 4.2.7.2. Thermal Load The current element is only a stress-displacement element (no heat transfer analysis is done to calculate the temperatures). The thermal load is applied to the element at the nodes using the '*TEMPERATURE' option. The temperature values at the integration points are obtained using the quadratic shape functions used for the displacement interpolation. 24 T = }ZNJi (4.13) l where Nt are the shape functions used for the displacement interpolation. In the future, this element will be combined with the heat transfer element developed by Rasekh (2006). If the temperature values at integration points are available from the heat transfer analysis, then those values can be directly used in the stress analysis rather than interpolating them from the nodal values. 4.2.8. Pseudo Finite Element Code In this section, a brief description of the sequential operation of the UEL subroutine is given. Inside the UEL subroutine, the element stiffness matrix and load vectors are calculated as: - 8 3 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures ;=| y=l *=1 /=1 ' ,=1 y=l k=l 1=1 * <T = D(S"" -e'her) s'°' =Bu where STOT and STHER are the total strain and free thermal strain vectors. The free thermal strains are due to CTE and cure shrinkage and will be referred to as thermal strain. The material stiffness matrix/) and the thermal strain vector £ther are obtained from the CCA module in the local material coordinates. They are then transformed to the global coordinate system. • Loop through in-plane Gauss integration points (/ = 1. .AJ = 1 ...4) - Obtain w^.and w>n - Call Subroutine LAYER_THICKNESS to calculate the layer thicknesses at this in-plane integration point (Equation 4.11) • Loop through layers (k=1 nl) • Loop through thickness integration points (/ = 1... n£k) - Obtain <T/*and w - Call Subroutine TEMPERATURE to calculate the temperature at this point Temperature can be interpolated from nodal values (Equation 4.13) or it can be directly given to this integration point from previous thermal analysis. - Call Subroutine CCA module to calculate the D matrix and incremental thermal strain, vector Asther - Transform D and Ae'her to global coordinate system • Element rotation with respect to Global coordinates • Layer rotation with respect to element coordinates - 8 4 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures • Additional layer rotation with the 3 r d axis - Call Subroutine JACOBIAN to calculate the Det Jac | / | and J-inverse J'1 (Equation 4.7) - Call Subroutine B M A T R I X to calculate the B matrix (Equation 4.9) - Calculate the incremental total strain Ae"" = B Au (Equation 4.10) - Calculate the incremental mechanical strain Asmech = As"" — As'her - Calculate the incremental stress ACT = D Asmech - Update the stresses: <r = cr + Acr - Calculate the load vector Rp due to the external distributed pressure load (Equation 4.12) - Calculate the stiffness matrix K and the load vector R at the integration point (Equation 4.14) K = BTDB\J\^ W .W„ w, t Si ''i * - Update the element stiffness matrix KeU and the element load vector Rele: Kele = Kele + R Rete = R e l e _ R + R P 4.3. V E R I F I C A T I O N E X A M P L E S In this section, some standard example problems are modelled using the developed 24-noded element to check whether or not it addresses the locking problems. The predicted results are compared with the analytical solution and the results from ABAQUS standard elements (20-noded and 27-noded elements). 4.3.1. Sensitivity of Aspect Ratio of the Elements The first example is to test the sensitivity of the aspect ratio of the element. A cantilever beam is subjected to both end shear and uniformly distributed load as shown in Figure 4.16. The beam is 1.0 m long and 10 mm thick. The slenderness ratio of the beam is 100. The geometry of the beam is shown in -85 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures Figure 4.16. The beam is made of an isotropic material with Young's modulus of 200.0 GPa and Poisson's ratio of 0.0. The problem is modelled with only one element in the thickness direction. The number of elements along the length direction is varied to check for convergence. For ABAQUS built-in elements, both full integration and reduced integration schemes are used. In the reduced integration scheme, the reduced integration is employed only in the in-plane direction. Full integration is carried out in the thickness direction using Simpson's rule with the combination of COMPOSITE option in ABAQUS. According to Euler-Bernoulli beam theory, the maximum deflection at the end of the beam due to an end shear load, P is given by: Pl' w I M K = - — (4-15) 3 EI By assuming a unit beam width, according to Equation 4.15, the maximum vertical deflection of the beam at the tip for applied shear load of P = 100 N is 2.00 mm. The maximum deflection at the end of the beam due to a uniform pressure load, p is given by: w = - - ( 4 . 1 6 ) SEI The maximum beam displacement in this case for an applied pressure ofp = 1.0 kPa is 7.50 mm. The beam is modeled with regular rectangular shaped elements as shown in Figure 4.17(a). The results from the analysis for both types of loading cases are shown in Table 4.1. The elements with full integration show some locking at larger aspect ratios. As the aspect ratio of the elements drop, the results converge to the solution from beam theory (exact). The elements with reduced integration perform well. 4.3.2. Skew Sensitivity of the Elements In this example, the above problem of a cantilever beam with end load is modelled with irregular shape elements. The elements are skewed into parallelograms and trapezoids. The skewed angle is varied from 0 -86-Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures to 75°. The elements are skewed only in the through-thickness direction as shown in Figure 4.17. Ten elements along the length are used for the analysis. This mesh density gave converged results for all types of elements in the previous analysis with regular shaped mesh. The results from the analysis using various types of elements are shown in Table 4.2. A l l the elements gave good results for skew angles of up to 45° which is the maximum skew angle recommended in ABAQUS. For the skew angle of 75°, the 24-noded and 27-noded elements with reduced integration gave better results for parallelogram shaped element. For the trapezoid shaped element, the results from these two elements are not very good for large skew angles. If the skew angle is within the ABAQUS allowed skew angle limit of 45°, then the above developed 24-noded element gives very good results. 4.3.3. Ring under Point Load This standard example is to test the capability of the element to model curved composite parts. The ring is under two compressive point loads at the top and bottom as shown in Figure 4.18. Only one quarter of the ring is modelled using «*1 elements. The number of elements along the circumferential direction, n, was varied between 4 and 20. The elastic solution for the vertical deflection under the load for an isotropic material is given by: w =-0.1488 (4.17) EI In the first case considered, the ring is assumed to be made of an isotropic material with Young's modulus of 200.0 GPa and Poisson's ratio of 0.0. The computed normalized vertical deflection for different mesh sizes are listed in Table 4.3. The elements with full integration show severe locking at large aspect ratios. However, the elements with reduced integration perform very well for all aspect ratios. In the second case considered, the ring is assumed to be made of unidirectional layers of a composite material. The mechanical properties of this material are listed in Table 4.4. The material properties of the - 8 7 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures element are defined using the cylindrical coordinate system. There is no closed-form elastic solution available for the orthotropic case. Hence, the reference elastic solution is assumed to be: DD3 wv =-0.1488— (4.18) The normalized vertical deflections at the point of load application for different mesh sizes for this orthotropic case are shown in Table 4.5. In this case too, the elements with reduced integration technique perform well for all ranges of aspect ratios. In the above examples, it is shown that the developed 24-noded element performes well compared to the ABAQUS built-in 20-noded and 27-noded elements with reduced integration. The reduced integration technique helped to reduce the locking problem substantially. With the reduced integration technique, the element can be used to model shell-like composite structures which have large aspect ratios with fewer numbers of elements. In the next section, the capability of nonuniform layer thickness feature of the developed 24-noded element will be verified. 4.3.4. Sandwich Cantilever Beam under Uniform Load This example is to test the element capability to model varying layer thickness in a composite element. The modelled example of a cantilever sandwich beam is shown in Figure 4.19. The skins are made of unidirectional CFRP composites and the core is made of aluminum. Generally the core is made of a softer material than aluminum. In that case, more than one element in the thickness direction is necessary to model the beam due to the non-smooth variation of the in-plane displacements in the thickness direction. Here, aluminum core is selected to use just one element in the thickness direction to model the beam so that the element capability of modelling varying layer thickness can be demonstrated. In Chapter 7, the case of a'soft core will be considered. The beam is subjected to a uniformly distributed load on its top surface. Two cases, one with constant thickness core and another with varying thickness core, are considered here as shown in Figure 4.19. The problem is modelled using ABAQUS built-in 20-noded -88-Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures element and the developed 24-noded element (UEL). In the case of built-in 20-noded element, the skin and the core are each modelled with one individual element each in the thickness direction (for the case of constant thickness core, one element in the thickness direction is also considered). In the 24-noded element case, the beam is modelled with just one element in the thickness direction. The comparisons of the displacement profiles along the length in both cases considered are shown in Figure 4.20 and Figure 4.21. As shown in the figures, the predicted result using the 24-noded element agrees well with the ABAQUS results. 4.4. P R E D I C T I O N OF PROCESS- INDUCED STRESSES A N D D E F O R M A T I O N S IN C O M P O S I T E P A R T S DURING C U R I N G P R O C E S S In this section, the process induced deformation of a flat and curved part are analysed using the above developed element. These examples are similar to the ones analysed in Chapter 2. In the following examples, heat transfer analysis is not performed. The temperatures in the tool and the part are assumed to be uniform and are equal to the autoclave temperature. 4.4.1. Warpage of a Flat Composite Part This example is similar to the one analysed in Section 2.5. In this study, the warpage and the residual stresses in a flat composite part laid on a flat tool subjected to thermal load are investigated. The tool-part assembly is shown in Figure 4.22. The tool-part assembly is cured under the temperature cycle shown in Figure 4.23. At the end of the curing process, the part is virtually removed from the tool and the warpage of the part is calculated. The part and the tool are 600 mm long and are assumed to be fully bonded. The tool is made of aluminum and is 5 mm thick. The part is 1.6 mm thick and is made of 8 unidirectional layers of T-800H/3900-2 CFRP material. The above problem is modelled using the 24-noded isoparametric composite solid elements developed above. The finite element mesh is shown in Figure 4.24. The curing material model for T-800H/3900-2 material is incorporated using the CCA module approach introduced in Chapter 2. - 8 9 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures Table 4.6 shows the sensitivity of the warpage to the number of elements (in-plane and through-thickness). As shown in the table, the warpage is not very sensitive to the number of elements in the in-plane direction but the number of elements in the thickness direction is critical. In the above case, around 16 elements in the thickness direction are necessary to capture the warpage accurately. The times taken for each run are also shown in Table 4.6. The time taken for the typical way of modelling where the aspect ratio of the elements are kept at 5 (300*8 elements) is also shown in the table. This run time can be reduced by around 10 times by increasing the aspect ratio to 50 (30*8 elements) for the same accuracy in warpage prediction (in both cases, the elements are with reduced integration). In Table 4.7 the warpage of the part with different part lay-ups are shown. The prediction by the developed 24-noded element is compared with the results from ABAQUS built-in 20-noded element with reduced integration. Both results agree very well. 4.4.2. Process-Induced Deformation of a Half Circular Composite Part on Solid Tool In this example, the process-induced deformation of a half circular composite part is analysed. The part and the tool arrangements are shown in Figure 4.25. The part is 600 mm long (the mean radius is 191 mm) and 1.6 mm thick. The part is made of 8 unidirectional layers of T-800H/3900-2 material. The tool is made of aluminum and is 5 mm thick. The part and the tool are assumed to be fully bonded together. The tool-part assembly is cured under the cure cycle shown in Figure 4.23. The tool is modelled withsthe ABAQUS built-in 20-noded isoparametric elements and the part is modelled with the developed 24-noded element. Due to symmetry only half of the problem is analysed as shown in Figure 4.26. The material properties of the part elements are defined using the cylindrical coordinate system. The numbers of elements in the circumferential and through-thickness directions (radial) are varied and the tip radial deflection after the tool removal is calculated. Table 4.8 shows the tip radial deflection for different number of elements. Similar to the flat part case, the tip deflection is not very sensitive to in-plane number of elements. However, it is very sensitive to number of elements in the through-thickness direction. -90-Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures Table 4.9 shows the predicted tip deflection using both the cylindrical and the rectangular coordinate systems to define the material orientation. The rectangular coordinate system for each element is defined by 3-nodes of that element. From the results, it can be seen that the proper definition of material orientation (principal axes) is very crucial in composite parts to ensure accuracy of results in a coarse mesh. 4.4.3. Spring-in of L-Shaped Composite Part This example is similar to the one analysed in Section 2.6. In this case study, the process-induced deformations of an L-shaped composite component is numerically analysed. The composite part is made of 8 unidirectional layers of T-800H/3900-2 material and the tool is made of aluminum. The modelled tool and the part geometries are shown in Figure 4.27. The tool is modelled with ABAQUS built-in 20-noded elements and the part is modelled with the developed 24-noded elements as shown in Figure 4.28. Figure 4.28 also shows the benefits of using elements with large aspect ratios. The element size used to model the part dictates the element size in the tool. By reducing the number of elements in the part, the number of elements used in the tool is also reduced. The number of degrees of freedom used in the three meshes are 3579, 7839 and 42354 respectively. The part was cured under the cure cycles shown in Figure 4.23. After the simulation of tool removal, the spring-in angle was calculated. The predicted spring-in angles (full bonding condition) and the run time for the three meshes are shown in Figure 4.29. According to the figure, by increasing the aspect ratio of the element, the run time can be reduced by a factor of 10. In the above examples, only one element in the out-of-plane direction is considered. If the part is very long in the out-of-plane direction, the run time saving will be much higher. 4.5. D I S C U S S I O N The development of the CCA modular approach introduced in Chapter 2 enabled us to overcome the dimensional constraint faced by the current process model, COMPRO. When the CCA module was first -91 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures introduced to the industrial partners, the response was not very positive. The industry was not ready to use the CCA module with the existing solid elements to model practical large scale structures (the shell elements cannot be used due its shortcoming mentioned earlier). This is due to the fact that the practical modellers (Engineers) are bound by the "aspect ratio should be less than 5" rule for solid elements. Even though, it was investigated and suggested to use solid elements with the remedies for locking to model shell-like structures two decades ago [MacNeal (1994)], solid elements were not used for this purpose until recently [Dhondt (2002)]. This may be due to the gap in transferring the knowledge from academia to the engineers in industry. The main purpose of this study is to demonstrate that by using a simple remedy for locking (reduced integration) an existing 2 n d order solid element can be used for process modelling of shell-like composite structures efficiently. Hence a commercial finite code with the CCA module can be used in the industry to investigate process-induced stresses and deformations. Even though, the existing second order elements with reduced integration can be used for this purpose a 24-noded solid element was developed for the following reasons: 1. The existing element does not have the capability of modelling varying layer thickness. 2. Inconsistency between the solid elements used in heat transfer analysis and stress analysis. For example, the ABAQUS 3D heat transfer element does not have the composite feature. The developed element will be combined with the heat transfer element developed by Rasekh (2006) to perform the thermal-stress analysis. 3. Each commercial code has their own unpublished patches to overcome the locking problems. Hence the results do not match when the same problem is analysed using different finite element codes [Dhondt (20020]. Hence, our own element was developed to make it solver independent. 4. The developed element will be used as the base for the development of efficient higher order elements in Chapter 7. - 9 2 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures 4.6. S U M M A R Y A N D CONTRIBUTIONS Anisotropy of thermal strains and tool-part interaction are the two main sources of the process-induced deformation of autoclave cured composite parts. Anisotropy of thermal strain results in shape changes of a curved part and tool-part interaction induces a large stress gradient in the thickness direction which results in the warpage of the composite part. Degenerated shell elements are the simplified version of the 3-dimensional solid elements in order to reduce the number of degrees of freedom used and the run time. In process modelling of composite structures where the elements should capture the above affects of thermal strain anisotropy and the tool-part interaction the degenerated shell elements have limited applicability. Hence, the best choice is the use of solid elements. But, when solid elements are used for modelling shell-like structures, where large aspect ratio of elements is necessary, they also encounter the unrealistic stiffening effect called "locking". Finding the suitable solution for the locking problem has been of research interest for the last two decades. There are many remedies suggested in the literature to overcome the locking problem, out of these the "reduced integration" method is more economical and easy to implement. In this study the application of a solid element with reduced integration in the process modelling of shell-like structures was investigated. Even though the currently available solid elements in commercial finite element software are sufficient for our study, the absence of some of the features that are necessary to model composite parts with varying layer thickness and ply-drop led us to develop our own solid element. The developed element can be implemented in any of the commercial finite element codes. In this study, it was implemented in ABAQUS using the User Element concept. It was shown that the developed 24-noded isoparametric solid element with the in-plane reduced integration method was successful in overcoming the locking affects. The varying layer thickness capability of the element was also demonstrated through an example of a tapered cantilever sandwich beam under uniformly distributed load. - 9 3 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures It was shown that by increasing the aspect ratio of the solid elements by a factor of 10 (from 5 to 50), the run time can be reduced by a factor of 10 also. In the example shown, only one element in the out-of-plane direction was considered. If the part is very long in the out-of-plane direction, the run time saving will be much higher. This element will be used as the base for the higher order elements that will be developed in Chapter 7. - 9 4 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures Table 4.1 Sensitivity of the aspect ratio of the elements. Predicted tip deflection of the cantilever beam normalized with respect to the exact (beam theory) solution for different mesh density Element Type End shear load Uniformly distributed load Mesh size (Length*Depth) Mesh size (Length*Depth) 1*1 2*1 4*1 8*1 10*1 1*1 2*1 4*1 8*1 10*1 20-noded-F 0.750 0.938 0.985 0.996 0.998 0.667 0.917 0.980 0.995 0.998 27-noded-F 0.750 0.938 0.985 0.996 0.998 0.667 0.917 0.980 0.995 0.998 20-noded-R 1.000 1.000 1.000 1.000 1.000 1.000 1.000 1.000 1.000 1.000 24-noded-R 1.000 1.000 1.000 1.000 1.000 1.000 1.000 1.000 1.000 1.000 27-noded-R 0.908 0.995 1.000 1.000 1.000 0.878 0.992 1.000 1.000 1.000 F - Full integration R - Reduced integration Table 4.2 Skew sensitivity of the elements. Predicted tip deflection of the cantilever beam normalized with respect to the exact solution for different element shapes and skew angles. The mesh size is 10*1 Element Type Parallelogram Trapezoid Skew angle (Deg) Skew angle (Deg) 0° 45° 75° 0° 45° 75° 20-noded-F 0.998 0.988 0.510 0.998 0.917 0.502 27-noded-F 0.998 0.992 0.857 0.998 0.994 0.829 20-noded-R 1.000 0.997 0.726 1.000 0.984 0.356 24-noded-R 1.000 1.000 0.978 1.000 1.000 0.878 27-noded-R 1.000 1.000 0.978 1.000 1.000 0.878 F - Full integration R - Reduced integration Table 4.3 Normalized vertical deflection at the loading point for the ring loaded with point loads (Isotropic case) Element Type Mesh size (Length*Depth) 4*1 10*1 20*1 20-noded-F 0.128 0.848 0.988 27-noded-F 0.128 0.849 0.988 20-noded-R 0.992 1.000 1.000 24-noded-R 0.998 1.000 1.000 27-noded-R 0.967 0.999 1.000 F - Full integration R - Reduced integration - 9 5 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures Table 4.4 Mechanical properties of the composite material used for the ring problem under point load E„ (GPa) 126.0 E22(GPa) 10.2 E 3 3 (GPa) 10.2 V 1 2 0.265 V 1 3 0.265 V 2 3 0.467 G, 2 (GPa) 5.44 G 1 3 (GPa) 5.44 G 2 3 (GPa) 3.46 a, (u/°C) 0.037 a 2 (u/°C) 29.5 a 3 (u/°C) 29.5 Table 4.5 Normalized vertical deflection at the loading point for the ring loaded with point loads (Orthotropic case) Number of elements Element Type (Length*Depth) 4*1 10*1 20*1 20-noded-F 0.161 0.856 0.989 27-noded-F 0.161 0.856 0.989 20-noded-R 0.998 0.999 1.001 24-noded-R 0.998 0.999 1.001 27-noded-R 0.994 0.999 1.001 F - Full integration R - Reduced integration -96-Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures Table 4.6 Sensitivity of warpage of a fiat unidirectional composite part to the number of elements (24-noded) in-plane and through-thickness direction. Also shown are computational run times (clock time) Number of elements Warpage Run time (Length*Depth) (mm) (min) 10*1 73.77 1.46 20*1 73.71 2.93 30*1 73.70 4.27 30*2 47.16 5.87 30*4 37.56 9.73 30*8 35.52 18.7 30*10 35.38 23.43 30*12 35.32 25.43 30*16 35.29 35.38 300*8 35.52 170.37 Table 4.7 Warpage of flat composite part with different lay-ups Lay-up Warpage (mm) 20node-R 24node-R roi8 35.29 35.29 r0/90/0/901s 48.44 48.45 T90/0/90/0L 22.78 22.80 r0/-45/90/451s 51.67 52.00 [45/90/-45/0]s 4.17 4.20 F - Full integration R - Reduced integration Table 4.8 Sensitivity of the tip deflection of quarter circular unidirectional composite part to the number of elements in-plane and through-thickness direction Number of elements (Length*Depth) Tip deflection (mm) 5*2 -44.60 10*2 -44.27 20*2 -44.45 20*4 -34.36 20*8 -32.02 30*8 -32.10 40*8 -32.10 100*8 -32.10 -97-Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures Table 4.9 Comparison of tip deflection of a curved unidirectional composite part using cylindrical and rectangular coordinate systems to describe the element material coordinate system Number of elements (Length*Depth) Tip deflection (mm) Cylindrical Rectangular 20*8 -32.02 -7.40 30*8 -32.10 -12.10 40*8 -32.10 -15.20 100*8 -32.10 -21.10 - 9 8 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures r - ~ Figure 4.1 Schematic describing the change in shape of a L-shaped composite part due to the anisotropic thermal strain Part Tool Figure 4.2 Schematic describing the affect of tool-part interaction on a flat composite part during the curing process - 9 9 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures Figure 4.3 Schematic to illustrate the shear locking phenomenon in a fully integrated 4-noded solid element (a) element before deformation, (b) expected deformation mode according to beam theory and (c) predicted deformation mode showing the non-zero shear strain at the Gauss points Figure 4.4 Schematic of a typical aerospace composite part consisting of solid laminate and sandwich sections - 100-Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures Finite Element Solver Initialize State Variables in Solver Set up Constitutive Equation in Solver Run Solver Incrementally USER E L E M E N T S Define the Element Stiffness Matrix, K Define the Element Internal Load Vector, R Figure 4.5 Flow chart describing the modular approach used to implement the user element concept in a commercial finite element code - 101 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures 4 1 7 —©— * * 3 4 -©-•> + 6 > Layer n t2 Layer 2 -*- I'- Layer 1 Figure 4.7 Schematic describing the in-plane and through-thickness integration points in the 24-noded composite solid element (through-thickness integration points are for the Simpson's rule) Figure 4.8 Layer material property definition for a tapered sandwich element with composite skins, (x-y-z) is the reference (global) frame, (1-2-3) is the element principal material coordinate system with respect to reference frame and (l'-2'-3') is the layer material coordinate system with respect to element material coordinate system - 102-Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures + Integration points Rectangular coordinate system Cylindrical coordinate system Figure 4.9 Material orientation definition in a large curved element with rectangular and cylindrical coordinate systems Figure 4.10 Schematic describing the concept of the extruder which creates the solid elements for the tool and the part from a master surface of shell elements - 103 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures Figure 4.11 Schematic describing the definition of layer thickness at 4-corner nodes of the element to model the varying layer thickness within an element Figure 4.12 Schematic showing the rectangular and cylindrical coordinate systems used to describe the material coordinate of the element - 104-Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures Figure 4.13 Definition of the element rectangular material coordinate system by (a) coordinate of two points and (b) 3 nodes b(XM) a{xjaz: (a) (b) Figure 4.14 Definition of the element material cylindrical coordinate system by coordinate of two points along the axis of the cylinder (a) typical cylindrical coordinate system where axes 1,2 and 3 represent radial, tangential and axial coordinate axes (b) currently implemented cylindrical coordinate system where axis 3 is in the thickness (radial) direction so that additional rotation of the layer can be easily defined - 105-Chapter 4: Usage of Standard Solid Elements in the Process^ Modelling of Shell-like Structures ^ I ' l l V V 1 V (a) -1/12 1/3 1/3 -1/12 1/3 -1/12 1/3 (b) -1/12 Figure 4.15 (a) Schematic describing the pressure load acting on the top surface of the element and (b) the corresponding consistent load factors for each node at the top surface Figure 4.16 Schematic of a cantilever beam under end shear and distributed loads - 106-Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures A Rectangular shaped elements (a) Trapezoid shaped elements \ (b) Parallelogram shaped elements \ \ \ \ \ (c) Figure 4.17 Cantilever beam is modelled with (a) regular rectangular-shaped (b) Trapezoid-shaped and (c) Parallelogram-shaped elements (b) (a) Figure 4.18 (a) Schematic of a ring under two compressive point loads at top and bottom and (b) the F E model of one quarter of the beam - 107-Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures Figure 4.19 Schematic of sandwich beams with constant (top) and varying (bottom) core thickness under uniformly distributed load 0 » Distance along length (m) 0.12 Figure 4.20 Comparison of the predicted results for the vertical displacement along the length of the sandwich beam with uniform thickness core using ABAQUS built-in 20-noded element and the developed 24-noded element - 108-Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures Distance along length (m) -2.5 Figure 4.21 Comparison of the predicted results for the vertical displacement along the length of the sandwich beam with varying core thickness using ABAQUS built-in 20-noded element and the developed 24-noded element Part • l i i H H H H i HIil Figure 4.22 Schematic of a flat composite part on a solid tool - 1 0 9 -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures Figure 4.23 Typical one-hold temperature cure cycle used for the curing of composite part 8 elements 30 elements Figure 4.24 Finite Element mesh for tool-interface-part assembly. 30*8 elements used to model the part 110 Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures 5 mm Figure 4.25 Schematic of a half circular composite part on a confirming solid tool Figure 4.26 Mechanical boundary conditions on the half-circular tool-part assembly (a) before and (b) after tool removal - I l l -Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures 50 mm Fibre Direction E S C I r-R: Thickness, t-R Rj = inner radius = 5 mm R 0 = outer radius t = 1.6 mm Tool -Aluminum Part Tool Figure 4.27 Schematic of an L-shaped composite part on a solid tool Figure 4.28 Finite element mesh of the L-shaped part on a tool (a), (b) elements with large aspect ratio (c) elements with small aspect ratio - 112-Chapter 4: Usage of Standard Solid Elements in the Process Modelling of Shell-like Structures Figure 4.29 Comparison of the total spring-in angle and the run time (clock time) of an L-shaped part using the three different finite element meshes shown in Figure 4.28 - 113-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part Chapter 5. CLOSED-FORM SOLUTION FOR PROCESS-INDUCED STRESSES AND DEFORMATIONS IN A FLAT COMPOSITE PART 5.1. I N T R O D U C T I O N During processing, as the resin cures its elastic (and shear) modulus changes by as much as 6 orders of magnitude from roughly 1 kPa to 1 GPa. As the tool expands during the heat up phase, it stretches the part with it thus inducing a large gradient of stress through the thickness of the part due to its rather low shear modulus. The stress gradient so generated is locked in as the material cures. On removal of the tool, this stress causes the part to warp. It is crucial to capture the stress gradient that occurs at the initial stages of cure in order to predict the part deformation accurately. An experimental and numerical study carried out by Twigg et al. [Twigg et al. (2004a), (2004b)] shows that the through-thickness stress distribution strongly depends on the material properties of the part and at the early stages of cure it varies in an exponential manner. As shown in the previous chapters, the finite element method is the generally used technique for the process modelling of composite structures. These models are generally more complex and can capture most of the sources of process-induced deformations that are identified in the literature. But finite element analyses are costly and it is sometimes difficult to understand the physics of the problem and to verify the accuracy of the final results. Closed-form analytical solutions become very handy in this case. They are very quick methods of analysing a problem with a certain level of accuracy and they help to understand the physics of the problem better. They can be also used as the validation tool for finite element results. This study focuses on the analytical prediction of the stress development in a flat composite part laid on a solid tool as shown in Figure 5.1 subjected to a uniform thermal load. The stress transfer between the tool and the part depends on the tool-part interface condition. This interface condition is generally simulated by introducing an interface layer [Johnston et al. (2001)] or a contact surface. The displacement boundary conditions are shown in Figure 5.2. Only half of the problem is considered due to symmetry. A sliding -114-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part boundary condition is assumed to prevail at the bottom of the tool since inside an autoclave the tool-part assembly is placed on the autoclave bed and subjected to high pressure thus inhibiting any bending deformation of the assembly. The above problem is similar to the classical bi-metallic beam under thermal load. The thermal stress in a bi-metallic beam was first studied by Timoshenko [Timoshenko (1925)]. He used elementary beam theory to calculate the curvature of a bi-metallic beam subjected to a uniform temperature change. In our case, since the beams are prevented from bending, the curvature is identically zero. According to Timoshenko's analysis the axial stresses in the beams are constant in the thickness direction. The main shortcoming of his theory is that it does not account for the interfacial stresses and does not satisfy the free stress boundary condition at the edges. Suhir [Suhir (1986), (1989)] improved Timoshenko's beam theory by considering both the interfacial shear stress and the peeling stress. The axial stress obtained from Suhir's analysis is also constant in the thickness direction but it satisfies the end condition. Chen et al (1982) used an analysis based on two-dimensional elasticity theory and the variational theorem of complementary energy. They assumed a linear variation of axial strain in the thickness direction and the stress obtained from this approach also satisfies the end condition. Many other closed-form solutions for bonded beams can be found in the literature [Chen and Nelson (1979), Bigwood and Crocombe (1989), McCartney (1992), Rossettos and Shen (1995), Wang et al. (2000), Ru (2002), Hsueh and Lee (2003), Tahani and Nosier (2003), Wang and Hsu (2004), Wen and Basaran (2004), Tsai et al. (2004), Ghorbani and Spelt (2005)]. In all the approaches, the axial stress/strain variation in the thickness direction is assumed to be a polynomial function of the thickness coordinate only. However the numerical study by Twigg [Twigg et al. (2004a), (2004b)] shows a strong dependence of the axial stress on material properties too. Hence, in this work an attempt is made to find closed-form expression for the axial stress variation in an orthotropic beam under thermal load. - 115-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part 5 . 2 . T H E O R E T I C A L D E V E L O P M E N T The problem considered here is shown in Figure 5.3. Known tractions are applied at the top and the bottom surfaces of the beam and the variation of in-plane displacement/stress in the thickness direction due to these tractions are sought. Equilibrium consideration in x direction (Figure 5.4) in the absence of any body forces gives: da 9TXV x x + — 0 dx dy The stress-displacement relationship, without the Poisson's effect, is also given by: (5.1) axx=E\—-s'her xx\ ^ T =G "•xy ^xy (du dv^ dy dx (5.2) where e'heris the free axial thermal strain and wand vare the displacements in the x and y directions respectively. Using the transformation of variables u = u — s'her x , we have: du du dx dx - £ ther du _ du dy dy (5.3) Owing to the assumption that the beam is not allowed to bend during the curing process and that a sliding boundary condition at the bottom surface of the tool prevail as shown in Figure 5.2, v = const and therefore, dv dv 0 dx By Considering Equations (5.1) - (5.4) inclusive, = 0 (5.4) d ( du^ i d f Q du ^ dx XX \ dx / T dy xy V (5.5) - 116-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part Assuming that the beam is homogeneous (i.e. and Gx are independent of x and y) , we can write: „ 82u _ d2u + (5.6) ox by This is a second order partial differential equation and can be solved by the method of separation of variables. Let u = X(x) Y{y) (5.7) E„XY + GxyXY = Q X = -\Y = (5-8> X c2 Y X where c - ' The solution to the above differential equation depends on the value of x • The only kinematically admissible solution is when % < 0 (other solutions do not satisfy the boundary conditions) i.e. % = —k2 which leads to the following eigenvalue problem: X c2 Y X + k2X = 0 (5.9) Y-/32Y = 0 where (3 = ck is a diffusion-like coefficient as it is commonly referred to in shear-lag analyses. Now the general solutions for the two ODE's in Equation (5.9) are: X = Ax cos(/cx)+ Bx sin(Ax) T-J^'+B*.-" < 5 1 0 ) Therefore, the displacement and the stresses can be written as - 117-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part u = [Alcos(kx) + Bl sm{kx)lA2 epy + B2 e~Py) u = [Axcos(kx)+Bl sm(kx)lA2 epy + B2 e~Py)+ e'herx Vi* = E^Uicos(kx)+Bl sm(kx)fA2 epy + B2 e~Py) ^ ^ Txy = GxyP[Axcos(kx)+ B, sm{kx)\A2 ePy - B2 e~Py) We can now apply the relevant boundary conditions (Figure 5.3) for determination of the constants resulting in the following eigenvalues and eigenfunctions: at x = l 0 - ^ = 0 =.> cos (A : / )=0 k = l)* n = 1,2,3,.... ( 5 1 2 ) at x = 0 u - 0 => At =0 kl)=0 ^ Therefore, the solution given by Equation (5.11) reduces to infinite series solution as follows: II = ±{sm(k„x)(A2n ep"y + B2n «->-")}+ e*»x n= l ^ =Z{E-*-cos(*-*)U-eAy+521,«"/'"r)} (5-13) n=\ = I MK X)(A„ ep"y - B2n e~p*y)} «=i where A2n and B2n are unknown constants and can be found from the boundary conditions at the bottom and top surfaces (y = 0 and t). According to Equation (5.13), the axial stress variation in the thickness direction depends on the diffusion coefficient /?„ which in turn depends on the values of c and kn. The constants c and kn are responsible for the material and geometrical dependency of the stress respectively. The following section presents solutions (i.e. v42„and B2„ values) for specific examples of surface tractions applied to monolithic and bi-material beams with and without an interface layer. 5.2.1. Homogeneous beam with shear traction specified at the bottom surface only In this case, the top surface of the beam shown in Figure 5.3 is stress free. Hence: - 118-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part at y = t rxy=0 => Alne^ ^Blne-p"1 => Bln = A2n e2p"' (5.14) Therefore, we have: u = £{/)„ sm{knx)cosh\j3n{y-t)]}+£therx o-» = X fo, A,*„ c o s ( * „ *)cosh[#, (y - 0]} (5.15) n=l ^ = I {GxyD„/3n sin(A:„ x)sinh|/?„ (y - >)]} where Z)„ are unknown constants. If the applied shear traction at the bottom surface of the beam is a general function of*, i.e.: r 0 = r 0 ( x ) (5.16) Then the unknowns Dn can be found by equating the beam shear stress to the applied traction at the bottom surface (y = 0): 2Z{GxyDnP„ s in(*„x)sinh[- /?„*]}= T 0 ( X ) (5.17) Multiplying both sides by sm(knx) and integrating over the beam length gives: GxyD„Pn ^smh[-pnt]= lT0(x)sm(knx)dx £ o 2JT0(x)sm(knx)dx (5.18) D" = Gxypnlsmh[-P„t] 5.2.2. Two fully bonded homogeneous beams A schematic of the beams with the corresponding boundary conditions are shown in Figure 5.5. The stress/displacement variation in beams-1 and 2 are given by: - 119-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part For beam 1: «=i <jx = t{ExDXnkn cos{knx)cosV\f3Xn{y + tx)]} (5.19) n=\ Tx = i{GxDXn/3Xnsm(knx)smh\j3Xn{y + tx)^ For beam 2: u2 = Z{732„ sin(^x)coshK(y-?2)]}+^f x n=\ a2 = t {E2D2nk„ cos(k„ x)cosh[/52„ (y-t2 )]} (5.20) n=l r2 = Z{G2Z>2„/?2„ sin(^x)sinh[/?2„(y-r2)]} where: n;r £, nn \E2 £>inand Z)2„ are unknowns and can be found by applying the boundary conditions at the interface between the two beams (i.e. at y = 0). The conditions that must hold at the interface are: (i) continuity of the displacements ux-u2 at v = 0 t{DXn sin(*„x)cosh[/U]}- i{Dln sin(*n*)cosh[- f32nt2]} = {s'2 her-e'x her)x ( 5 ' 2 1 ) n=l n=l and (ii) equilibrium which implies continuity of the shear stresses - 120-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part r, = T2 at y - 0 l{GxDupu sin(A:„*)sinh[/Vi ]} = zZ{G2D2nP2n sm(knx)smh[-/32nt2]} ( 5 - 2 2 ) n=l n=1 Multiplying both Equations (5.21) and (5.22) by s'm(knx) and integrating over the beam length results in the following two equations for the two unknowns DXn and D2n: A . ^oshLV,]-D 2 n ^cosh[-p2nt2] = (-X)^ (^-f") DXn coshK',]"D2 n cosh[-p2nt2]=(-l/"+l) ^ ' (5.23) (5.24) G,Z>,„A» ^ i n h ^ ] = G 2 D 2 „ / ? 2 n ^ s i n h [ - / ? 2 „ f 2 ] £, G , ^ sinh[/? l n f l] ^ 2" G2 f32n smh[-p2nt2] the solution of which is D _( 0 M 2 b t o - ^ f ) G 2 / j 2 n s inh[-^ 2 „r 2 ] lk2n {G2y»2„ c o s h K ^ i l s i n h l - ^ f . l - G , ^ s inhK f l ] co sh [ - / ? 2 „r 2 ] } ( 5 . 2 5 ) D ( A n * ) ^ ~£lher) G , A n Sinh\pXntx] 2" lk2n {G2p2n coshKfJsinhh / J^r . l -G, A„ s i n h K ^ o s h [ - / ? 2 „ r 2 ] } 5.2.3. Two homogeneous beams separated by an interface layer In this case, we present the solution for two beams separated by an interface layer with shear modulus, Gs and thickness ts. It is assumed that the interface layer is very thin and the only stress that it transfers is a shear stress that is uniform across its thickness. The stresses acting on a differential element of the tool-interface-part assembly along the length are shown in Figure 5.6. The shear stress in the interface layer is given by: r 0 = G , f e ^ (5.26) - 121 -Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part where wfand w2 are the longitudinal displacements of beam 1 and 2 at y = 0, respectively and are given by: "2° = Z {D2n sm(k„x)cosh[- fi2nt2 ]}+ e'2her x (5.27) r 0 is the shear stress at y = 0 and is given by Equation (5.22): r 0 = Z{G 1A„A„sin(^x)sinh[/? 1„/ 1]}= f.{G2D2„p2H sin(*„*)sinh[-A„/ 2]} (5.28) n=l n=l From Equations (5.26) and (5.27), the unknowns DXn and D2n can be determined as: D _ , l ) ( n + l ) 2 ( g f r - g r ) G 2 /7 2 n sinh[-/?2.f2] /*„2 {C2 ft. coshK ( l]sinh[-/5 2„/ 2]-G, /?,„ sinhKf,](cosh[-/52„/2]-Z)J} ( 5. 29) G . f l . sinhLg,„?,] g 2" G 2/? 2„ s inh [ - /V 2 ] where 5.3. N U M E R I C A L E X A M P L E S A N D VERIFICATION In this section the closed-form solutions developed in the previous section are exercised by conducting numerical case studies and the results are verified with more sophisticated numerical FE analysis. In the first set of examples, the beams 1 and 2 are assumed to be monolithic (i.e. made of only one material or lay-up). The axial stress variations for an applied isothermal temperature are obtained and compared with the corresponding finite element predictions and other closed-form solutions. - 122-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part 5.3.1. Two fully bonded Beams: Beams 1 and 2 are isotropic In this case, we consider two isotropic beams made of aluminum and steel. The material and geometrical properties of the beams are listed in Table 5.1. The bi-metallic beam arrangement is subjected to a uniform temperature of 160 °C. The stress variations along the length and the through-thickness directions in the two beams are calculated using the developed closed-form solution. The predicted axial stress variation at the interface along the length in beam-2 (aluminum) is shown in Figure 5.7. As shown in the figure, the solution with increasing number of terms in the closed-form solution converges rapidly. Since a stress singularity occurs at the end, a large number of terms are necessary for convergence. The axial stress variation in the thickness direction at a specific cross section (x = 150mm) is shown in Figure 5.8. The stress is uniform across the thickness which agrees well with the assumption used in Timoshenko's beam theory. The axial and shear stress variations along the length at the interface of Beam-2 are compared in Figure 5.9 and Figure 5.10 with corresponding solution by Timoshenko and Suhir. The present results are seen to be in good agreement with the results of these previous beam theories. The above results show that for isotropic beams, the constant stress assumption through the thickness is valid. 5.3.2. Two fully bonded Beams: Beam 1 is isotropic and beam 2 is orthotropic In this example, instead of two isotropic beams, beam-2 is replaced by an orthotropic beam. The beam-1 is made of aluminum and the beam-2 is made of a unidirectional CFRP composite material. During the processing of a composite structure, the resin modulus evolves as it cures. Figure 5.11 shows an example of this modulus development during a typical cure cycle. In this analysis, the stress variations at 6 different stages of curing are considered. The material properties of the composite material at these different curing stages are listed in Table 5.2. The aluminum tool is 5 mm thick and the CFRP part is 1.6 mm thick (equivalent to 8 layers). - 123 -Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part When the material is at stage-1, the resin modulus, Er, is very low (47.1 kPa). The predicted axial stress variation of the composite part along the interface at this stage is shown in Figure 5.12. As the number of terms increases, it can be seen that the present closed-form solution approaches the finite element result. For the finite element analysis, the problem is modeled using 24-noded isoparametric solid elements developed in Chapter 4. Each layer is modelled with one element in the thickness direction and 30 elements are used along the length. The through-thickness axial stress variations for different stages of curing and for different lengths are compared in Figure 5.13 and Figure 5.14, respectively. The closed-form solution is seen to agree very well with the finite element results. The above results show the dependency of the through-thickness variation of axial stress on material properties and geometry (aspect ratio). The dominant factor that controls the stress gradient is the parameter c or the ratio of the axial (longitudinal) modulus to transverse shear modulus, i.e. EyG . As can be seen from Figure 5.13, at the early stages of curing when Ey^ is large (since = Eu is fixed and Gxy being dominated by the resin modulus is low), the stress gradient is steep. Therefore, the larger the Exyc ratio the steeper the stress gradient. Geometry also plays a role as seen from Figure 5.14. For a given thickness and material properties, the shorter the part the steeper the stress gradient. 5.3.3. Two beams separated by an interface layer: Beam 1 is isotropic and beam 2 is orthotropic This is similar to the previous case, except the beams 1 and 2 are now separated by an interface layer. The interface layer is 0.2 mm thick and its shear modulus (G s ) is 20.0 kPa. The beam-2 is assumed to be at the curing stage-1. The variation of the shear stress in the interface layer along the length is shown in Figure 5.15 and the through-thickness variation of axial stress at JC = \50mm is shown in Figure 5.16. The closed-form solution agrees very well with the results obtained from finite element analysis. - 124-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part 5.3.4. Two fully bonded Beams: Beam 1 is isotropic and beam 2 is a composite beam with multi layers In this set of examples, beam-2 is made of multi-layers of composite lamina with different fibre orientations. The stress variation in beam-2 for an applied temperature cycle is computed using two different approaches. In the first approach, equivalent orthotropic properties or lumped properties are used to model the constitutive behaviour of beam-2. 5.3.4.1. Equivalent property approach The first obvious choice is to replace the multilayer beam with an equivalent homogenous beam. Then the analysis follows the same procedure as in the previous examples. The properties of the equivalent homogeneous beam are found from laminate plate theory. The overall behaviour of beam-2 is given by (see Equation (5.20)): u2 = l{D2n sin(*„x)cosh[/? 2 / I E(y-t2)]}+s'2herEx (5.30) n=l where /32n E - ^ - I — a n d E2 E, G2 E and £ 2 e E are the equivalent properties of beam-2 and 21 y G 2 E -D2n is given by Equation (5.25) with f52n and s2er replaced by f32n E and e2erE. The stresses in each layer of the beam-2 are given by: * 2 i = 1{E2 LD2„K cos(*„x)cosh[/? 2„ E(y-t2)]}+E2 M^E-^L) (5-31) n=l " _ _ _ where E2 L and £ 2 e r L are layer properties. The through-thickness variation of total axial strain and axial stress at x = \50mm are shown in Figure 5.17 and Figure 5.18 for a quasi- isotropic lay up (8 terms were used). Even though the equivalent property approach predicts the overall behaviour well (i.e. the axial displacements and strains at the top and bottom surfaces are very close to FE results), the prediction of the interlayer behaviour is not very good. This is mainly due to the fact that for a layered beam, the axial - 125-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part displacement variation in the thickness direction is a non-smooth function. Hence, the behaviour cannot be predicted accurately by a smooth function as in the equivalent property approach. The layerwise approach presented in the next section addresses this deficiency. 5.3.4.2. Layerwise approach This layerwise approach is similar to the approach taken by Robbins and Reddy (1993) and Zhou et al. (2004) to model the laminated composite behaviour. In the layerwise approach, the axial displacement variation in the thickness direction is assumed to be a non-smooth function as shown in Figure 5.19. For a given number of terms, n, the i'h layer axial displacement variation in the thickness direction is given by (Equation (5.10)): u2n=Aineti»y+Bine-pi"y (5.32) where f3l2n = , E'2 and G'2 are the /'''layer axial elastic modulus and transverse shear modulus 21 y G'2 respectively andA'„and B'nare unknowns associated with the /'''layer. For m layers, there are 2m unknowns which can be determined from the equilibrium and continuity conditions at the interface between the layers. At the i'h interface (y = y,), the interface boundary conditions are: and (5.33) which yield the following two equations: A'n e&"y> + B\ e-fiLy< = A1* ep^y' + B'n+] e~^y' (5.34) G^L^n^'2"*-Bt,e-&y')=G?1p£^';le&ly'-B^e'^') (5.35) - 126-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part Equations (5.34) and (5.35) constitute (2m - 2)equations for (m -1) interfaces. Two more equations can be found from the boundary condition at the top and bottom surfaces. Let the displacements at the top (y = t2) and the bottom (y = 0) surface of the beam be utn and ubn, respectively. We can then write: (5.36) The system of 2m equations can be presented in the following matrix form: 1 1 0 0 [41 Ubn efk»y\ e~P\ny\ 0 0 0 -Gift***"* • 0 0 A: >=. 0 0 0 A". \. J (5.37) Or, in a symbolic form, we can write: [c]-W=M By inversing the matrix, (5.38) *bn 0 Bl (5.39) Therefore, the layer unknowns A'n and B'n can be related to the 2 beam unknowns ubn and uu A'„=c\ubn+c'2uln K=C\Ubn+C\Utn (5.40) - 127-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part where c\ to c\ are the known layer constants from Equation (5.37). Now, the displacement of beam-2 can be written as: u2=^\sm{knx)^[Ay^+By^ • + £2 EX ;'=1 or • + £2 EX Now the shear stress at the top surface of the beam-2 is zero which implies that: (<«t* +c'2uln)e^ -(c-ubn+c'4uln)e-^ =0 or where d„ — Finally, the displacement of beam-2 can be expressed as: (5.41) (5.42) 00 m " 2 =ZlZ )2nsin(^x)Z ALeh'y + Ble-^ ' + ^2 E X (5.43) where A'n =c\ +c 2c?„and Bln = c\ + c\dnare known layer constants and D2n -ubn is the only unknown. Equation (5.43) is similar to the equation for the homogeneous case and the unknown values of Dln can be found from the boundary condition at the bottom surface of the beam as in the homogeneous case. For example, for the fully bonded case, the unknowns for beam-1 and beam-2 are given by: ( n + l ) 2 « - -e'r) G\ B\n &-Bl) G\ P\„ sinner 1*1 {Gl Pl cosh|/V,]{A]n - £ „ ' ) - G , Bxn sinh[/V,]{A* + B\)} ( 5 . 4 4 ) and the axial stress in each layer of beam-2 can be expressed as: 128 Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part 0-2 l = tU2 i D 2 „ ^ c o s ( ^ x ) f ; [ l > ^ + 5 > - ^ ] } + J E 2 M heE-4herL) (5-45) The through-thickness variation of the total axial strain and the axial stress at x = 150 mm by this layerwise approach are shown in Figure 5.20 and Figure 5.21 for a quasi isotropic lay up for the fully bonded case. The results agree really well with the finite element results. The total axial strain and axial stress variation for a cross-ply laminate are shown in Figure 5.22 and Figure 5.23 respectively. In this case too, the closed-form results agree well with the FE results. From the above two cases, it can be seen that the largest stress gradient occurs at the [0] layer where the /G x y ratio is the largest. 5.4. W A R P A G E PREDICTION In this section, the above developed closed-form solutions are used to predict the warpage of a processed composite part. The warpage of a flat part at the end of a cure cycle is calculated. The part is made of T-800H/3900-2 CFRP material and the tool is made of aluminum. The tool-part assembly is cured under the one-hold temperature cycle shown in Figure 5.24. A uniform temperature is assumed for the whole structure. For the analysis, the cure cycle is divided into small time steps (At). In each time step, the stresses in the part are calculated using the CHILE constitutive model [Johnston et al. (2001)]. Accordingly, using the layerwise approach, the increment of stress in layer-i is given by: Ao-; = j t {E'2 (Z>* >„ COS(*. xp: e*-> + B: e-*" )}+ E\ (AS^ - Aef, ) n = l (5.46) cr' =o~'J +Ao~'? whereE\ is the instantaneous elastic modulus of layer-i and AE2herE and As2e\ are the incremental thermal strains for the equivalent beam and layer-i respectively. D2N is the unknown D2N in the current time step. - 129-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part The cure dependent material properties and the incremental thermal strain for each time step are calculated using CCA module for this material by passing the temperature values at each time step as shown in Figure 5.25. At the end of the curing process, the tool is removed and the part warpage due to the residual stress developed during the cure process is calculated. The unbalanced moment due to the residual axial stress is given by: M(x)\i+Ai=M(x)[+AM(x) (5.47) Where '\ f t } AM(x) = Ao-2 y - ± dy J 2 o V The bending deformation, v , due to this resultant moment can be calculated from the differential equation governing the response of a simple beam as follows: d2v 1 =-^ = -rAr-M{x) (5.48) dx2 (El)eff where {El\ff is the effective bending rigidity of the part at the instant when the part is removed from the tool. Calculation of this quantity is presented in the next section. 5.4.1. Calculation of Effective Bending Rigidity In this section, the deformation of a flat cantilever composite part due to an applied bending moment, M, is considered. According to the strength of materials approach or Bernoulli-Euler beam assumption, the deflection of the beam is given by: - 130-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part v(*) = Mx2 2EI with (5.49) b_e_ 12 where b is the width of the beam. According to the equation above, the deformation is a function of bending rigidity El. Since the axial modulus E and hence the bending rigidity EI does not change appreciably for a unidirectional composite beam, the axial stress and the bending deformation are expected to remain the same with the changing material properties of the resin. The finite element predictions of the deformation profile of the beam at the 6 stages of cure listed in Table 5.2 are shown in Figure 5.26. The figure shows that the deflection profile is a function of the E / G ratio and depending on the state of the material (cure stage) at the time the part is removed from the tool, the profile will be different. In the strength of materials approach or simple beam theory which does not account for transverse shear deformations, the bending rigidity, EI, is calculated based on a linear distribution of axial strain in the thickness direction. However, according to the closed-form solution presented here, the axial strain varies in an exponential manner in the thickness direction as shown in Figure 5.27. i.e. the through-thickness variation of axial strain is given by: e(y). sinh ( ( ft \ V •+y sinh ( ( —y sin; (5.50) and hence the effective bending rigidity is given by: - 131 -Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part The deflection profile (Equation (5.49)) with the effective EI value given above results in the deflection profiles shown in Figure 5.28. As shown in the figure, the present results based on the modified beam theory and the finite element results agree very well. For layered parts, the computation proceeds according to the layerwise approach presented earlier. 5.4.2. Warpage prediction compared to finite element results Table 5.3 shows the warpage values obtained using the present closed-form approach for a unidirectional composite part (fully bonded to the tool) for different part lengths and thicknesses (number of layers). The table shows the maximum warpage values for different number of terms used in the closed-form solution. It can be seen that reasonable accuracies are achieved with only one term solution. In the finite element analysis, results of which are also listed in Table 5.3, the part is modelled with 20-noded isotropic 3D continuum elements in CCA/ABAQUS. Each layer is represented with one element in the thickness direction. The number of elements used in the FE and the time taken for each run are also listed in Table 5.3. These times are the run times only (time taken for setting up the problem including meshing is not included). For all these cases, the closed-form solution (with 8 terms) takes less than 10 seconds to obtain the results. Table 5.4 shows the variation of warpage with part lay-up for 600 mm long and 8 layer thick parts for two different interface layer properties (thickness ts = 0.2 mm and two different shear moduli Gs = 2.0 kPa and 20.0 kPa). The predicted closed-form solution agrees well with the FE results. (El)eff = \Es(y)ydA A (5.51) - 132-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part 5.5. D I S C U S S I O N In the above sections, it is shown that stresses and deformations predicted by the closed-form equations developed here agree well with the finite element predictions. In this section, the closed-form results will be used to explain some of the experimentally observed behaviour of composite parts. 5.5.1. Influence of Initial Resin Modulus Figure 5.29 and Figure 5.30 show the development of the bending moment and the part transverse shear modulus G for an 8-layer unidirectional composite part as it undergoes curing. For a unidirectional part, the axial modulus, E, is dominated by the fibre property and it remains almost constant throughout the cure cycle. As shown in these figures, the development of bending moment mainly occurs at the initial stages of the curing process when the value of G is very low. This shows that the characterization of material properties at the initial stages of curing is crucial in predicting the process-induced deformation accurately. However, it is difficult to determine the initial resin modulus experimentally. The usual practice is to assume that the initial resin modulus is 3 to 4 orders of magnitude less than the fully cured resin modulus. By analysing the experimentally observed warpage variation with part geometry, a reasonable assumption can be made as will be shown later in this section. Table 5.5 shows the predicted warpage for different values of the initial resin modulus. As shown in the table, the warpage results vary considerably with different values of initial resin modulus. In some cases, the warpage increases with increasing initial resin moduls and in other cases, the warpage decreases with increasing initial resin modulus. This inconsistancy is mainly due to fact that for the full-bonding interface condition, the shear stress at the tool-part interface is not constant with initial resin modulus. If the shear stress is constant at the tool-part interface (as in the case of shear layer) then the warpage will decrease with increasing initial resin modulus. - 133-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part 5.5.2. Scaling Law Twigg [Twigg et al. (2004a), (2004b)] found from a substantial number of experiments on a flat unidirectional part that the maximum warpage of the part varies with part thickness and length according to the following equation: warpage oc — (5.52) r Figure 5.31 and Figure 5.32 show the variation of the normalized maximum warpage with part thickness and part length for E r 0 =47.1kPa and compare those with the proposed trend by Twigg. The closed-form solution captures the trend very well. However, the results do not follow Twigg's equation exactly especially at larger lengths and smaller thicknesses. The variation of warpage with part thickness and length for E r 0 =4.71kPa are shown in Figure 5.33 and Figure 5.34 and the comparison is much better than the previous case. These results show that the maximum warpage of a flat part is very sensitive to the initial resin modulus and that the latter should be determined accurately to predict the experimental results correctly. Since it is very difficult to characterize the initial resin modulus experimentally, by comparing the experimental results with the numerical predictions, as shown above, a reasonable assumption can be made (for the T-800H/3900-2 material, E^, = 4.71 kPa is a reasonable choice). 5.5.3. Simulation of Experimentally Observed Tool-Part Interaction with a Thin Interface Layer Twigg [Twigg et al. (2004a), (2004b)] also investigated the variation of maximum warpage of flat unidirectional layered parts with tool-part interface condition. His 4 sets of experimental results are listed in Table 5.6. The interface conditions are the combination of applied pressure and the tool surface layer. FEP stands for the fluoro-ethylene-propylene sheets placed in-between the part and the tool and RA stands for the Release Agent (Freekote) coat applied to the tool surface before laying the part on it. - 134-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part According to the experimental results by Twigg [Twigg et al. (2003)], during the heat-up portion of the cure cycle, sliding friction is the dominant interface condition and the interfacial shear stress is constant along the length of the part. Based on the assumption of the first-ply slip to simulate the stress gradient through the thickness, Twigg proposed an analytical solution to predict the maximum warpage in a unidirectional composite part: where Tnet is the net interfacial shear stress which depends only on the tool-part interface condition and the applied pressure. rnel does not depend on the part and the tool geometry. In numerical modelling, the tool-part interface can be simulated using a contact surface or a thin interface layer. Numerical analyses that employ contact surfaces are computationally intensive. Hence the simulation of the tool-part interface using an interface layer is investigated here. Generally, the shear modulus of the interface layer is calibrated with an experimental result to represent a certain combination of the tool-part interface condition and pressure. This calibrated interface layer is then used to study warpages of different part lengths and thicknesses. According to the numerical runs and the closed-form solution (Figure 5.15), the shear stress in an interface layer varies linearly along the length of the part as shown in Figure 5.35. From the figure it can be seen that the interface layer simulates the experimentally observed sliding condition in an average sense: 7net m a x (5.54) The maximum shear stress value, r m a x , in the interface layer depends on the shear layer properties Gs and ts and the part length / as follows (Equation 5.26): - 135-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part Gl X oc max (5.55) This shows that, if an interface layer is calibrated to simulate a particular tool-part interface condition leading to interface layer properties Gs, ts and ls, then those values should be modified as follows to use in any other cases in order to keep the rmt constant (independent of part and interface layer geometry): ( i Y ? A G . = G . (5.56) Hence, from Equation (5.51), the maximum warpage of the part is given by: f / Y r V # 3 \ oc G - - II \ls A ' * J v - ' 2 . c c G l L (5.57) WN I t s s SLN where WN and SLN are defined as the warpage and shear layer numbers. The variation of the warpage number with respect to shear layer number for a unidirectional flat part of different lengths (0.25m, 0.5m and 1.0m) and different thicknesses (2mm, 4mm and 8mm) are shown in Figure 5.36 and Figure 5.37. As shown in the figures, all the points almost lie on a single master curve. After a certain value of shear layer number, the maximum warpage remains constant. This is equivalent to attaining the fully bonded condition. The variation of the warpage number with respect to shear layer number for two different shear layer thicknesses (0.2mm and 0.4mm) is shown in Figure 5.38. In this case too, all the points lie on a single master curve. This shows that an interface layer can be successfully used to model the experimentally observed warpage variation with proper calibration. On average, the variation of warpage number with the shear layer number can be given by two linear segments as shown in Figure 5.39 for an aluminum tool. The linear and the constant portions of the curve are given by: - 136-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part WN = linear C (5.58) WN = WN constant where Cand WN are constants which depend on the tool and the part properties. Figure 5.40 shows the WN\s. S L N curves for aluminum and steel tools. From the graph, the relationship between the constants of the two tool materials may be given by: cst eAI C T E S t C _ ± » E s > C T E a i (5.59) WNst = C T E S l WNAI C T E A l Even though, the above equation is obtained from the graph, it can be justified by considering the stress distribution in a composite part on aluminum and steel tools. The maximum axial stress in a composite part depends on coefficient D2n (Equations 5.20 and 5.25). Hence, the ratio of the maximum warpage of the composite part for aluminum and steel can be given by: (VmaxL (D2n) Al (Vmax )s, ) 5 , For the full-bonding condition, the above ratio can be approximated to: ( \ [ ther _ ther \ Vmax/St \ C pari c Si / (5.60) Since e'^rrt is zero for the unidirectional lay-up, the ratio of the maximum warpage becomes: (Vmax )/)/ ^ CTEAj Lx)Sl C T E S , Figure 5.41 shows the variation of warpage number with shear layer number for aluminum and steel tools with the curve for steel tool being shifted according to Equation (5.59). The figure shows that Equation - 137-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part (5.59) describes the variation of warpage with tool material very well. This shows that for a given tool-part assembly, only two points on the linear and constant segments are necessary to construct the design curve. From this curve, the warpage for different shear layer properties, part geometry and tool material can be obtained. The above analysis shows that the interface layer can be used to simulate the experimentally observed tool-part interface condition with the above mentioned adjustments. The closed-form solution with interface layer option is used to predict the experimentally obtained results by Twigg. Table 5.7 shows the predicted maximum warpage values by the closed-form solution. In the closed-form solution, the interface layer is calibrated using one experimental result from each set of experiments. Since all the experimental results do not exactly follow the average trend observed by Twigg, first the experimental results are adjusted to the trend as shown in Table 5.7. Then the shear layer is characterized to match one of the adjusted values (in this case, the adjusted warpage value of 600 mm long and 8 layer thick part). The predicted closed-form results are compared with the experimental results in Figure 5.42. The closed-form results agree very well with the experimental results in all the cases except the results for the 1200 mm part in the third set. In this case, the experimental results are not consistent with the rest of the results as shown in Table 5.6 (The RA interface is expected to give more warpage than the FEP interface. But the experimental set-3 shows much lower warpage compare to other sets). 5.5.4. Variation of Warpage with Part Lay-up Table 5.8 and Figure 5.43 show the comparison of the closed-form solution with another set of experimental results [Petrescue (2005)] for different part lay-ups. The parts are 1200 mm long and processed on an aluminum tool. The predicted closed-form solution agrees well with the experimental results. One interesting result in this experiment is that the [90/0/0/90] lay-up produces more warpage than the [0/90/90/0] lay-up. It is expected that a [90] layer at the bottom of the part minimize the thermal strain mismatch between the part and the tool and hence results in a lower unbalanced moment. The closed-form solution confirms this argument as shown in Figure 5.44. However, since the bending rigidity - 138-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part of [0/90/90/0] lay-up is much greater than the [90/0/0/90] lay-up, the latter laminate results in more warpage. 5.6. S U M M A R Y A N D CONTRIBUTIONS The finite element technique is a powerful tool for solving very complicated mechanics problems. However, setting up and running the problem takes a long time and requires finite element expertise. The interpretation and validation of finite element results is also sometimes very difficult, especially in the case of composite structures. On the other hand, closed-form analytical solutions are simple, and are fast methods for solving a simplified version of the more complicated numerical problems analyzed by the' finite element technique. In this chapter, a simple and powerful closed-form analytical solution was developed to analyse the process-induced stresses and deformations that develop during the curing process of a flat composite part laid on a solid tool. Even though many assumptions and simplifications were made in the course of the development of the closed-form solution, the comparison of the closed-form solution with the finite element results shows that the developed closed-form solution is capable enough to capture the essence of the problem accurately. The closed-form analytical technique has many advantages over the finite element technique: 1. It is very fast and no set up time is required 2. It provides physical understanding of the axial stress variation in the thickness direction. According to the closed-from solution, the axial stress variation in the thickness direction varies exponentially with the through-thickness coordinate, y, and its gradient depends on a parameter f5n. The value j3n in turn depends on two constants c and kn. The constants c = J% and kn - ""/^ give the material and geometrical dependency of the stress variation - 139-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part respectively. This result will be valuable in developing a robust finite element technique in Chapter 7. This understanding of the physics of the problem allows a more mechanistic description of some observed phenomena and refutes or reinforces certain intuition about the process-induced deformations. For example, earlier it was thought that the negligible warpage of a [90] lay-up part is due to the negligible thermal strain mismatch between the part and the tool. However, even in the presence of the thermal strain mismatch, the [90] lay-up would still result in negligible warpage because for this lay-up, the through-thickness stress gradient is almost zero. Hence, there is no unbalanced moment to cause the warpage. The methodology of using a shear-layer to simulate the tool-part interaction observed experimentally was also validated. It was shown in the analysis that with proper modification for part length and shear layer thickness this methodology can be used to simulate the experimentally observed tool-part interface condition successfully. It was also shown that a unique graph of "shear layer number" vs. "warpage number" can be constructed for a particular tool-part material combination. This graph can be used as a design tool to study the variation of warpage with part length, part thickness, tool material and the tool-part interface conditions. It was also shown that the process-induced unbalanced moment develops mainly at the initial stage of the curing process where the through-thickness stress gradient is very high. Hence, characterizing the initial resin modulus is crucial in predicting the experimentally observed trend in the variation of warpage with part length and part thickness. Since, characterizing the initial resin modulus is very difficult, it was shown that by comparing the experimentally observed trend with the numerical prediction, a reasonable assumption can be made. - 140-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part Table 5.1 Material and geometrical properties of aluminum and steel beams for the case of two fully bonded isotropic beams subjected to thermal load Properties Beam 1 (Steel) Beam 2 (Aluminum) Elastic modulus E (GPa) 200.0 69.0 Shear modulus G (GPa) 77.0 26.0 Coefficient of thermal expansion a (u/°C) 12.5 23.6 Thickness t (mm) 5.0 5.0 Length / (mm) 300.0 300.0 Temperature increment AT (°C) 160 160 Table 5.2 Composite material properties at different curing stages of resin used for the analysis of stress variation in a composite part on an aluminum tool and subjected to thermal load Cure stage Resin modulus Er (MPa) En (GPa) ^22> ^33 (MPa) V12>V\3 v 2 3 Gn>Gn (MPa) G23 (MPa) «1 (u/°C) a2,oc3 (u/°C) 1 0.0471 124.0 0.177 0.00 0.00 0.0665 0.0580 0.03 29.5 2 0.471 124.0 1.77 0.00 0.00 0.6650 0.5800 0.03 29.5 3 4.71 124.0 17.7 0.00 0.00 6.6500 5.8000 0.03 29.5 4 47.1 124.0 177.0 0.00 0.00 66.500 58.000 0.03 29.5 5 471.0 124.0 1770.0 0.00 0.00 665.00 580.00 0.03 29.5 6 4710.0 124.0 17700.0 0.00 0.00 6650.0 5800.0 0.03 29.5 - 141 -Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part Table 5.3 Variation of the warpage of a unidirectional composite flat part fully bonded to an aluminum tool with part length and thickness. The closed-form results are compared with finite element predictions. For the finite element analysis, the run time (clock time) is also shown u Finite Element Closed-form tigth (mm) "E. Warpage ( mm) tigth (mm) mber of Warpage (mm) No of elements Run time (min) 3 Terms 1 Term hJ 4 19.29 15*4 3.5 18.02 18.23 300 8 5.140 15*8 4.3 4.80 4.84 16 1.290 15*16 8.2 1.15 1.14 4 120.1 30*4 5.0 119.3 120. 9 600 8 35.52 30*8 6.7 35.38 35.80 16 9.540 30*16 12.2 9.45 9.54 4 609.9 60*4 8.1 609.5 621.1 1200 8 229.4 60*8 13.3 229.9 233.1 16 68.00 60*16 25.2 68.21 69.06 Table 5.4 Variation of the warpage of a composite flat part with part lay-up. The part is 600 mm long and 8 layer (1.6 mm) thick and it is separated from the tool with a thin interface layer. The closed-form results are compared with finite element predictions Lay-up Maximum warpage (mm) Gs = 2.00 kPa ts = 0.2 mm Gs = 20.00 kPa ts = 0.2 mm Closed-Form Finite Element Closed-Form Finite Element [Ok 1.00 1.01 7.96 7.98 T0/90/0/90L 1.40 1.41 11.08 11.13 r90/0/90/01s 1.83 1.83 10.38 10.36 r0/-45/90/45]s 1.56 1.57 12.31 12.41 f45/90/-45/0]s 0.70 0.82 2.77 3.22 - 142-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part Table 5.5 Closed-form results of the variation of warpage with part thickness and part length for different values of initial resin modulus Length (mm) Number of Plies Warpage (mm) Length (mm) Number of Plies E r 0 = 4.71E3 kPa Ert, = 4.71E4kPa E,o = 4.71E5 kPa E,o = 4.71E6kPa 300 4 6.37 18.02 36.54 24.66 8 1.56 4.80 12.36 17.20 16 0.28 1.15 3.43 7.24 600 4 48.70 119.25 139.30 37.46 8 12.69 35.38 69.10 43.01 16 3.15 9.45 23.40 29.67 1200 4 348.46 609.47 300.44 41.58 8 96.23 229.86 251.89 62.48 16 25.10 68.21 124.62 68.46 Table 5.6 Experimental warpage results for flat unidirectional composite parts with different number of layers and part lengths [Twigg et al. (2004)] Length (mm) Number of plies Maximum warpage (mm) Length (mm) Number of plies Interface = FEP Pressure = 103 kPa Interface = FEP Pressure = 586 kPa Interface = RA Pressure = 103 kPa Interface = RA Pressure = 586 kPa 300 4 0.70 0.43 0.67 0.78 8 0.13 0.15 0.26 0.25 16 0.04 0.16 0.07 0.08 600 4 3.84 3.94 2.03 4.09 8 0.81 0.86 0.97 1.23 16 0.12 0.28 0.31 0.11 1200 4 29.10 39.57 15.72 42.04 8 7.26 8.97 2.67 7.71 16 1.18 1.31 1.56 1.58 - 143 -Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part H 65 a" NJ O o O N o o o o Length (mm) Number of plies Experiment - 1 Adjusted Exp. - 1 Closed-form Experiment - 2 Adjusted Exp. - 2 Closed-form Experiment - 3 Adjusted Exp. - 3 Closed-form Experiment - 4 Adjusted Exp. - 4 Closed-form Pis a ON O O o " NJ T~ 3 o OS C p p ON O O 3 3 o o p C p ' rt n P ON o o 3 3 o N> O J P h3 —i C p ' 3 8 ON © O 3 3 © N> P >T3 C p ' rt 8 oo ON 5V •-a P 65 rt 69 rt BT c e rt rt rt 3. 3 rt E. IT 69 rt 69 "1 5" rt rt a ore BT ore rt a 69 a rt a « rt 3. 3 B 1 rt B " S B n o 3 69 55" o B 69 1 •a 69 (TQ rt T3 "1 rt a 69 rt rt O a. 3' ore B- o rt rt-1 rt B a rt B a" x i B 69 a o B 3 69 "1 rt o B rt 3 69 rt B" rt CL 69 •a 69 ore o B CT O v> rt a i "2. B o B rt rt 1 (71 -O — cr H ore H ore* ore rt NJ O O - 1 4 4 -Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part Table 5.8 Comparison of the warpage prediction by closed-form solution with the experimental results by Petrescue (2005). Lay-up Warpage (mm) Experiment Interface = RA Pressure = 586 kPa Closed-form Gs = 1.08 kPa = 0.2 mm ls = 600 mm roi4 25.20 19.43 roi 6 7.75 9.22 T9016 -1.45 0.0 T90/04/901 18.16 13.68 r0/90/02/90/01 11.96 12.10 r0/902/01 19.74 21.92 [90/02/90] 36.98 33.57 - 145-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part 1 Interface Part v 21 Figure 5.1 Schematic of a flat composite part on a solid tool separated by an interface layer Figure 5.2 Schematic showing the displacement boundary conditions applied on the tool-part assembly before tool removal 4v(v) Figure 5.3 Schematic of a beam under applied traction at the top and the bottom surface. The stress and displacement boundary conditions are also shown - 146-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part y (T, H - t W 3x Figure 5.4 Schematic of stresses acting on a differential element of a beam i / T2 = 0 / / / E2,(J-) . 2 www www A A A A A A r, =0 Figure 5.5 Schematic showing the displacement and stress boundary conditions on two fully bonded homogeneous beams - 147-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part a2 cr2 + do~2 JL. 7 4 X 7 ^ W T • CT, + J f j j Figure 5.6 Schematic showing the stresses acting on a small segment of tool-interface layer-part assembly Figure 5.7 Variation of closed-form solution for axial stress along the length in beam-2 at y = 0 for different number of terms - 148-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part -60 -50 -40 Axial stress (MPa) Figure 5.8 Variation of axial stress through the thickness of beam-2 at x = 150 mm for the case of two fully bonded isotropic beams subjected to thermal load. The present closed-form solution is compared with the solutions of theories by Timoshenko and Suhir 100 rt 09 u 75 H 50 .2 •< 25 •Presentsolution (250 terms) -Timeshenko(1925) Suhir (1986) 0.1 0.2 Distance from the centre line, x (m) 0.3 Figure 5.9 Variation of axial stress along the length of beam-2 at y = 0 for the case of two fully bonded isotropic beams subjected to thermal load. The present closed-form solution is compared with the solutions of theories by Timoshenko and Suhir - 149-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part 200 .150 C3 i loo im C3 X ! c» 50 •Present solution (250 terms) Suhir (1986) 0.1 0.2 Distance from the centre line, x (m) 0.3 Figure 5.10 Variation of shear stress along the length of beam-2 at y = 0 for the case of two fully bonded isotropic beams subjected to thermal load. The present closed-form solution is compared with the solution of theory by Suhir 200 ^ 4 . 5 n 09 3" 3 p 3 C 3" o 100 150 200 Time (min) 250 300 350 Figure 5.11 Development of resin modulus along a typical 1-hold cure cycle - 150-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part 600 Distance from the centre line, x (m) Figure 5.12 Variation of axial stress along the length of the composite part at y = 0 for the case of a unidirectional composite part fully bonded to an aluminum tool subjected to thermal load. The closed-form solution is compared with finite element result. The composite part is at cure stage! Axial stress, axx (MPa) Figure 5.13 Variation of axial stress through the thickness of the composite part at x = 150 mm for the case of a unidirectional composite part fully bonded to an aluminum tool subjected to thermal load. The closed-form solution is compared with finite element result. The composite part is at 4 different cure stages as shown in Figure 5.11 - 151 -Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part Axial stress, ( J x x (MPa) Figure 5.14 Variation of axial stress through the thickness of the composite part at the middle span for the case of a unidirectional composite part fully bonded to an aluminum tool and subjected to thermal load. The closed-form solution is compared with finite element result. The results are shown for two different beam lengths -0.12 1 Figure 5.15 Variation of interfacial shear stress along the length for the case of a unidirectional composite part and an aluminum tool separated by a thin interface layer and subjected to thermal load. The closed-form solution is compared with finite element result - 152-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part Finite element Closed-form (8 terms) 30 40 50 Axial stress (MPa) 60 70 80 90 Figure 5.16 Variation of axial stress through the thickness of the composite part for the case of a unidirectional composite part and an aluminum tool separated by a thin interface layer and subjected to thermal load. The closed-form solution is compared with finite element result. The composite beam is at cure stage-1 1 ^ \ 101 s coordinate (mm) o bo i "^ "L, _ • Closed-form (8 terms) —•— Finite element [-45] s coordinate (mm) o bo [90] [45] [45] Thicknes: V* \ [90] [-45] 1 OH 1 1 1 1 \ 1 T • • -0.05 0 0.05 0.1 0.15 0.2 0.25 0.3 0.35 0, Total axial strain (%) Figure 5.17 Variation of total axial strain through the thickness of the composite part for the case of a quasi-isotropic composite part fully bonded to an aluminum tool and subjected to thermal load. The closed-form solution with equivalent layer approach is compared with finite element result. The composite beam is at cure stage-1 - 153 -Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part h6-[0] 1 1 ss coordinate (mm) bo i —•— Closed-form (8 terms) —•— Finite element [-45] 1 1 ss coordinate (mm) bo i [90] [45[ [45] ckne: [90] Thi* : [-45] e~ ^ ^ ^ ^ ^ ',01 Axial stress (MPa) 3 0 0 Figure 5.18 Variation of axial stress through the thickness of the composite part for the case of a quasi-isotropic composite part fully bonded to an aluminum tool and subjected to thermal load. The closed-form solution with equivalent layer approach is compared with finite element result. The composite beam is at cure stage-1 Figure 5.19 Schematic showing the variation of the axial displacement across the layer in layerwise approach - 154-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part Total axial strain (%) Figure 5.20 Variation of total axial strain through the thickness of the composite part for the case of a quasi-isotropic composite part fully bonded to an aluminum tool and subjected to thermal load. The closed-form solution with layerwise approach is compared with finite element result. The composite beam is at cure stage-1 4T6-K. -50 50 100 150 200 250 300 Axial stress (MPa) 350 400 101 —— Finite element • Closed-form (8 terms) [-45] 450 500 Figure 5.21 Variation of axial stress through the thickness of the composite part for the case of a quasi-isotropic composite part fully bonded to an aluminum tool and subjected to thermal load. The closed-form solution with layerwise approach is compared with finite element result. The composite beam is at cure stage-1 - 155-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part •+6--0.05 — Finite element • Closed-form (8 terms) 0.05 0.1 0.15 0.2 0.25 Total axial strain (%) 0.3 [0] [90] [0] 0.35 0.4 Figure 5.22 Variation of total axial strain through the thickness of the composite part for the case of a cross-ply composite part fully bonded to an aluminum tool and subjected to thermal load. The closed-form solution with layerwise approach is compared with finite element result. The composite beam is at cure stage-1 -hfr -50 50 Finite element • Closed-form (8 terms) [01 [90[ [0[ [90] 100 150 200 250 Axial stress (MPa) 350 400 450 500 Figure 5.23 Variation of axial stress through the thickness of the composite part for the case of a cross-ply composite part fully bonded to an aluminum tool and subjected to thermal load. The closed-form solution with layerwise approach is compared with finite element result. The composite beam is at cure stage-1 - 156-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part CCA Module CLOSED-FORM SOLUTION INTERFACE MODULE Pass in and update state variables T, a, V f MICRO MECHANICS MODULE Calculate composite properties CURE KINETICS MODULE Update a RESIN PROPERTIES MODULE FIBRE PROPERTIES MODULE Figure 5.25 C O M P R O Component Architecture to model the evolving composite properties with the curing of the resin - 157-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part Figure 5.26 Variation of displacement profile of a unidirectional composite beam under constant end moment with material properties. The finite element results are compared with the solution from classical beam theory (Equation 5.49) Figure 5.27 Variation of axial strain distribution at a cross section of a unidirectional composite beam with material properties. The finite element results are compared with the solution from classical beam theory (Equation 5.49) - 158-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part 12 E a > a 8 w tu C cu •a j 4 Cure stage - 1 < 1 ) • j \ — • x J • / • y Finite element • Modified beam theory • >^ • >^ Cure stage - 2-^^ • i , > I T - > - i r 1 — • * Cure stage - 3 1 Distance from centre line, x (m) Figure 5.28 Variation of displacement profile of a unidirectional composite beam under constant end moment with material properties. The finite element results are compared with the solution from modified beam theory (Equation 5.51) 200 50 100 150 200 Time (min) 250 300 -10 o 3 n -20 a 3^ -30 -40 350 Figure 5.29 Development of bending moment at a cross section of a unidirectional composite part along the cure cycle - 159-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part 0 50 100 150 200 250 300 350 Time (min) Figure 5.30 Development of the shear modulus of the resin of a unidirectional composite part along the cure cycle o -I , , , 1 0 4 8 12 16 No of layers Figure 5.31 Variation of normalized warpage of a unidirectional composite part with number of layers (part thickness). The closed-form results are normalized according to the trend observed by Twigg [Twigg et al. (2004)]. The initial resin modulus for this case is 47.1 kPa - 160-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part Figure 5.32 Variation of normalized warpage of a unidirectional composite part with part length. The closed-form results are normalized according to the trend observed by Twigg [Twigg et al. (2004)]. The initial resin modulus for this case is 47.1 kPa • Closed-form -1 = 300 mm a Closed-form 600 mm Closed-form - / = 1200 mm Twigg - ytl No of layers 12 16 Figure 5.33 Variation of normalized warpage of a unidirectional composite part with number of layers (part thickness). The closed-form results are normalized according to the trend observed by Twigg [Twigg et al. (2004)]. The initial resin modulus for this case is 4.71 kPa - 161 -Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part • Closed-form - 4 layers m Closed-form - 8 layers A Closed-form - 16 layers 300 600 Part length, / (mm) 900 1200 Figure 5.34 Variation of normalized warpage of a unidirectional composite part with part length. The closed-form results are normalized according to the trend observed by Twigg [Twigg et al. (2004)]. The initial resin modulus for this case is 4.71 kPa Figure 5.35 Schematic showing the shear stress distribution along the half-length of interface for the case of a composite part and a solid tool separated by a thin interface layer and subjected to thermal load (see Figure 5.15) - 162-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part l.OE-05 SLN l.OE+00 l.OE+01 1.0E+02 1.0E+03 1.0E+04 1.0E+05 1.0E+06 1.0E+07 l.OE+08 1.0E-06 i l.OE-07 l.OE-08 Figure 5.36 The variation of warpage number (WN) with shear layer number (SLN) for three different thicknesses of the part. All the points lie on a single master curve l.OE-05 SLN l.OE+00 l.OE+01 1.0E+02 1.0E+03 1.0E+04 1.0E+05 1.0E+06 1.0E+07 l.OE+08 1.0E-06 l.OE-07 l.OE-08 4 1.0E-09 -*-l, = 0.25 m - * - / =0.50 in 1.00 m Figure 5.37 The variation of warpage number (WN) with shear layer number (SLN) for three different lengths of the part. All the points lie on a single master curve - 163-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part 1.0E-05 SLN l.OE+00 l.OE+01 1.0E+02 1.0E+03 1.0E+04 1.0E-HJ5 1.0E+06 1.0E+07 1.0E+08 1.0E+09 1.0E-06 1.0E-07 1.0E-08 1.0E-09 4.,, m * a • -a—• ts = 0.2 mm -*— ts = 0.4 mm Figure 5.38 The variation of warpage number (WN) with shear layer number (SLN) for two different shear layer thicknesses. All the points lie on a single master curve 1.0E-05 1.0E-06 1.0E-07 1.0E-08 1.0E-09 SLN Figure 5.39 The variation of warpage number (WN) with shear layer number (SLN) for aluminum tool. This figure is the combination of Figure 5.36, Figure 5.37 and Figure 5.38. The figure also shows the approximation of the master curve by two linear segments - 164-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part l.OE-05 SLN l.OE+00 l.OE+01 1.0E+02 l.OE+03 1.0E+04 1.0E+05 1.0E+06 1.0E+07 l.OE+08 1.0E-06 l.OE-07 l.OE-08 1.0E-09 _|_—.—• ----- - •]— WNs, CTE WNA, CTEAI Aluminum • • » • • » • -4—4 ~m—m—| m—m—i Steel Qv _ EAI CTESl 1 CAl i ESl CTEAI Figure 5.40 The variation of warpage number (WN) with shear layer number (SLN) for aluminum and steel tools SLN l.OE-05 l.OE+00 l.OE+01 1.0E+02 l.OE+03 1.0E+04. 1.0E+05 1.0E+06 1.0E+07 l.OE+08 1.0E-06 l.OE-07 l.OE-08 Aluminum Steel (Normalized) 1.0E-09 Figure 5.41 The variation of warpage number (WN) with shear layer number (SLN). The two linear curves for steel tool from Figure 5.40 are normalized according to Equation (5.59) - 165-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part Figure 5.42 Comparison of maximum warpage prediction by closed-form solution with experimental results - 166-Chapter 5: Closed-Form Solution for Process-Induced Stresses and Deformations in a Flat Composite Part Figure 5.43 Comparison of the closed-form prediction of variation of warpage with part lay-up with experimental results by Petrescue (2005) 5 [0/90/90/0] [90/0/0/90] Figure 5.44 Closed-form results of the variation of bending moment and bending rigidity with lay-up for the 1200 mm long composite part analyzed by Petrescue (2005) - 167-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Chapter 6. C L O S E D - F O R M S O L U T I O N F O R P R O C E S S - I N D U C E D S T R E S S E S A N D D E F O R M A T I O N S I N A C U R V E D C O M P O S I T E P A R T 6.1. I N T R O D U C T I O N This study is the extension of the analytical solution developed in the previous chapter for a flat composite part to a curved composite part. In the closed-form solution developed for a flat composite part, the stresses are only due to the in-plane thermal strain mismatch between the part and the tool. The thermal strain mismatch between the part and the tool in the thickness direction does not produce any stresses. But in a curved composite part, in addition to the stresses due to the in-plane thermal strain mismatch, the through-thickness thermal strain mismatch may also add some stresses. In the literature, the well known process-induced deformation in curved composite parts (generally referred to as spring-in) due to the anisotropy of the thermal strain of the part is estimated based on the following equation [Nelson and Cairns (1989)]: (6.1) where £^ e r and s'r e r are the tangential and radial thermal strains of the composite part, and is the change in the included angle. In the above equation, the deformation is only due to the mismatch between the tangential and radial thermal strain of the part. The effect of the thermal strain mismatch between the tool and the part is not considered. In estimating the deformation in a curing process using the above equation, generally, the effects during the heat-up portion of the cure cycle are ignored and only the effects during the cool-down are considered. To include the effect of the cure shrinkage, a percentage (normally about 10%) of the total cure shrinkage is considered by assuming most of the cure shrinkage occurs at the initial stages of the cure when the material is very soft [Albert and Fernlund (2002)]. - 168-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part In this chapter, the closed-form solution for the process-induced stresses and deformations in a curved composite part is developed. The curved parts considered here are circular in shape (i.e. they have a constant radius of curvature). The part is assumed to be thin (radius to thickness ratio is greater than 8) and on a closed circular tool as shown in Figure 6.1. To simplify the analysis and to understand the mechanisms better, the stresses due to tangential and radial thermal strain mismatch between the part and the tool are considered separately in the following sections. 6.2. STRESSES DUE TO T A N G E N T I A L T H E R M A L S T R A I N In this section, the closed-form solution for the stresses due to the tangential thermal strain mismatch between the part and the tool is developed and tested against the finite element results. In this development, the radial (through-thickness) thermal strains of the part and the tool are assumed to be zero. 6.2.1. Theoretical Development The case considered here is similar to that of a flat composite part considered in the previous chapter as shown in Figure 6.2. A known traction is applied at the top and bottom surfaces of the curved part and the variation of displacement/stress in the radial (thickness) direction due to these tractions is sought. Equilibrium consideration in the tangential (<j>) direction in the absence of any body forces gives: l ^ + ^ + 2 r ^ = 0 ( 6 2 ) r d</> dr r The stress-displacement relationship, without the Poisson's effect, is also given by: 'J_3w + v _ £lhy Krd<f> r * j ^ 1 dv du u ^ yr di/) dr r j (6.3) - 169-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part where is the free thermal strain (due to CTE and cure shrinkage) in the tangential, </>, direction and wand vare the displacements in the tangential (tj>) and radial (r) directions respectively. Using the transformation of variables u -u- s'^er r<j>, we have: 1 du _ 1 du r d(/> r d(j> ,lher du u _du u dr r dr r (6.4) Owing to the fact that the tool does not allow the part to bend during the curing process and the radial thermal strain of the part is zero, v = 0 (the validity of this assumption will be discussed later) and therefore, cr AJL = EA (\_Su) \r d(/>j (du us \dr r, (6.5) By substituting the stresses (Equation (6.5)) in the equilibrium equation (Equation (6.2)) and assuming that the part is homogeneous (i.e. EMax\& Gr^ are independent of <p and r ): EM d2u „ d2u GRIJ) du GRIJ) _ —?-—z- + Gr„—- + — -rl df r dr u=0 (6.6) This is a second order partial differential equation and can be solved by the method of separation of variables. Let u = Xfa) Y(r) X~ c2 r — + r 1 X (6.7) (6.8) where c = Tr<j> - 1 7 0 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part The solution to the above differential equation depends on the value of x • The only kinematically admissible solution is when x < 0 (other solutions do not satisfy the boundary conditions) i.e. x - ~k2 which leads to the following eigenvalue problem: X + k2X = 0 , \ (6-9) r2Y + rY-{l + p2)Y = 0 where (3 = ck is a diffusion-like coefficient as it is commonly referred to in shear-lag analyses. The general solutions to the above two ordinary differential equations are: X = A, cos(A^)+ 5, s'mikS) (6.10) where A=V(I+/?2) Therefore, the displacement can be written as: u = (4cos(^)+ 5, s in (Ar^)X^ 2 eXHr) + B2 e~mr))+ efrr<f> (6.11) We can now apply the relevant boundary conditions (Figure 6.2) for determination of the constants resulting in the following eigenvalues and eigenfunctions: at <!> = 0 w = 0 => A{=0 f (6.12) at </>-— o~,, = 0 => cos k— = 0 => k = (2n-1) n = 1,2,3 2 V 2y Therefore, the solution for the displacement reduces to an infinite series solutions as follows: M = X { s i n ( ^ ^ ) ( 4 „ ^ l n W + J B 2 „ e ^ , n W ) } + < - ^ (6.13) - 171 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part where A2n and B2n are unknown constants and can be found from the boundary conditions at the bottom and top surfaces (r = Rb and Rt). 6.2.2. Example: Stresses in a Unidirectional Composite Part on a Rigid Tool In this section, the tangential stress in a composite curved part on a rigid tool is analysed using the above equation (Figure 6.3). The stress is due to an applied temperature of 100 °C. The composite material properties are listed in Table 6.1. The given material properties are the snapshots of a CFRP composite material at 4 different curing stages for a typical cure cycle except the coefficient of thermal expansion values. For this analysis the CTE of the composite material is arbitrarily set to 29.5 y.c in the tangential direction (generally this value is zero) and zero in the radial direction. The behaviour of the part at these 4 stages for the applied temperature is analysed. The tool is assumed to have a zero CTE and the tool and part are assumed to be fully bonded. For the stress free boundary condition at the top surface (at r — Rt, - 0), we have: u = fj{D„ sm(kj)[An c o s h ( A „ l n ( / J + s i n h ( A „ l n ( / J ) ] } + ^ ^ n=l = ±\EMD„K c o s ( t » [ A - C ° S h ( A - l n f e ) ) + S i n h ( i J n f e ) ) 1 (6.14) where kn = (2M - 1 ) . This equation is similar to the following equation for a flat part (Chapter 5): - 172-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part u = fj{Dn sinfe'x)cosh[/?„(y-t)]}+ s'xher x =tKD^ Mkn ^osh\j3n{y-t)]} (6.15) = J {GxyDnPn sm{kfn *)sinh[/?„ (y -t)]} {1n — X)n where kfn and the superscript/denotes parameters related to a flat part. The fully constrained boundary condition (u - 0) at the bottom surface of the part (r = Rb andy = 0) gives: X{D„sin(^>)[^cosh(AJn(%))+sinh(AJn(%))]}=-<- JR^ - Curved Zl ( 6 1 6 ) ^{Dnsm(kf x)cosh\j3n$=-e'xher x - Flat By multiplying the above equations by sm{kn</>) and sm{kfx) and integrating over the length (from^ = 0to f ): *kl [An cosh(lJn(%J)+sinh(AJn(%J)] " C u n * d Z ) „ = ( - l ) ( " + l ) , \ * I . - Flat / ( ^ ) 2 c o s h M The tangential stress variation for the applied temperature computed using the above equations (6.14) and (6.15) for the composite part is shown in Figure 6.4. As shown in the figure, both equations give identical results. The results show that, for a thin part, the closed-form solution developed for the flat part in the previous chapter can be used with x and y coordinates denoting the tangential and radial directions respectively as shown in Figure 6.3. - 173 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part 6.2.2.1. Finite Element Investigation The above problem is also analysed using the finite element technique. The part is modelled with 20-noded solid elements with reduced integration. The finite element results for the tangential stress variation in the thickness direction in the flat and curved composite parts are shown in Figure 6.5. The finite element results show that there is a difference in the stress distribution between the flat and the curved parts which is not apparent in the closed-form solution. This difference may be due to the interaction of the tangential and the radial stresses in the curved part. The equilibrium equations for the flat and curved parts in the thickness/radial direction are given by: da'yy , dT*y = Q dy dx y a (6.18) dcrrr | 1 d r r 4 | o - r r - o M ^q dr r dtj> r From this equation, it is apparent that there is an interaction between the tangential and radial stresses in a curved part other than the interaction due to the Poisson's effect (in this case Poisson's ratios are assumed to be zero). The finite element results for the radial stress variation along the length for the flat and the curved composite parts are shown in Figure 6.6 and Figure 6.7. As shown in the figures, in the curved part a significant amount of radial stress is present compared to the flat part. Figure 6.8 shows the distribution of the radial displacement (v) at a cross section in a curved part. As shown in the figure, the radial displacement is actually NOT zero as assumed in the development of the closed-form solution. When this radial displacement is constrained by the boundary condition, the tangential stress distribution in the thickness direction in both flat and curved composite parts agree well as shown in Figure 6.9. This shows that the difference in the stress distribution between the flat and the curved parts is due to the coupling between the tangential and radial stresses in the curved part. The additional tangential stress produced by non-zero radial displacements is given by: °»=Eu- (6-19) - 174-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.10(a) shows the distribution of tangential stress through the thickness using Equation (6.19) with the radial displacement, v, from the finite element predictions shown in Figure 6.8. For comparison, Figure 6.10(b) shows the difference between the finite element predictions of the tangential stress distributions based on unconstraint and constraint radial displacement shown in Figure 6.5 and Figure 6.9 respectively. The finite element result shows some shearing effect similar to Equation (6.14) at early stages of curing (stages 1 and 2). In order to capture this effect somehow analytically, Equation (6.19) is modified as follows: Figure 6.11 shows the modified results compared to the finite element results. The result from the modified Equation (6.20) follows the trend of the finite element result well. The above finite element investigation shows that the difference between the closed-form and the finite element results for a curved part is due to the non-zero radial stresses and displacements which are not accounted for in the closed-form solution. 6.2.2.2. Correction for Radial Stress in Closed-form Solution The following correction can be made to reduce the error in the closed-form solution by considering the equilibrium of the curved part in the radial direction. The equilibrium equation in the radial direction is given by: v Xn co sh (AJn^ ) )+s inh^„ ln (^J) ] (6.20) da 1 5rri dr r d<j> = 0 or (6.21) d<j> Substituting for errand Tr^ from Equation (6.14) and integrating over the radius of the part: - 175 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part o-rr = I,\D„kn cos{k„i n=\\ sinh(A„ln(^)) + ( ^ - G ^ f e - l ) ) c o s h ( / l n l n ( / f i > ) ) " • + - / ( * ) ( 6- 2 2> r where /((fi) is an unknown function and can be found by applying the stress boundary condition at the top surface (r = Rt, o~rr - 0): m=2Z\-Dnkncos(kj) n=l (6.23) The radial stress distribution through the thickness predicted by the closed-form solution (Equation 6.22) is compared with finite element solution in Figure 6.12. Compared to the finite element results, the closed-form solution predicted a similar trend, even though the magnitudes are not quite the same. The stress-displacement relation in the thickness direction is given by: cr = E, rr rr dv dr (6.24) By substituting for arr from Equation 6.22, the through-thickness displacement can be obtained: v=i\Dnk„ oos{kj) 'E„ cosh(*>(^)) ( £ # - G ^ f e - l ) ) r s i n h ( A „ l n ( / f i ( ) ) E„K Mr) (6.25) By applying the boundary condition that at r = Rb, v = 0, the unknown function g(</>) can be found. Now, this through-thickness displacement produces a tangential stress according to Equation (6.20). The tangential stress distribution at a cross section in a curved composite part before and after the above correction for the radial stress is applied is shown in Figure 6.13. After the correction, the closed-form results agree very well with the finite element results. In the above simple example, it is shown that the developed closed-form solution for the tangential stress in a curved part due to tangential thermal strain mismatch between the part and the tool yields good - 176-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part predictions compared to the finite element results. The correction for radial stress is a tedious process and the error due to ignoring this correction on the process-induced displacement will be investigated in a later section (Section 6.5). 6.3. STRESSES DUE TO R A D I A L T H E R M A L S T R A I N In this section, the closed-form solution for the stresses in a curved part due to the thermal strain mismatch in the radial direction is developed. In this case, the tangential thermal strains of the tool and the part are assumed to be zero. To simplify the development, the tool is assumed to be rigid with zero coefficient of thermal expansion (similar to the example in the previous section). Later, the developed closed-form solution will be extended to realistic tools. The part considered in the analysis is made of either aluminum or unidirectional composite. The mechanical properties of the composite material at 4 different stages of curing are given in Table 6.1. The CTE of the composite is assumed to be 29.5 y.c in the radial direction. 6.3.1. Theoretical Development The unconstrained expansion of the flat and curved parts due to the through-thickness/radial thermal strain is shown in Figure 6.14. For the flat part, when the tool constrains the part at the bottom surface, there will be no stresses developed in the part due to this constraint. The constraints applied by the tool on the curved part are shown in Figure 6.15. There are three constraints applied by the tool on the part to conform the part to the shape of the tool (since the tool is rigid, its shape does not change). Figure 6.15(a) shows the applied constraint by the tool on the rigid body displacement of the part. No stress will develop due to this constraint. Figure 6.15(b) and Figure 6.15(c) show the radial and tangential constraints applied by the tool on the part, respectively. Due to these constraints, there will be stresses developed in the part (Johnston [Johnston (1997)] also suggested in his thesis work to account for the effects of radial constraint of a tool on a curved part). - 177-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part 6.3.1.1. Stresses due to Radial Constraint The stress development due to the radial constraint applied by the tool on the part depends on the profile of the gap between the tool and the part. The profile of the gap can be obtained from the geometries before and after the expansion (Figure 6.16) and is given by [Goran Fernlund, personal communication, 2006]: where s'r is the thermal strain in the radial direction and Rb is the radius of the bottom surface of the curved part. The above gap profile is similar to the displacement profile obtained due to the application of a constant moment to a curved thin part which is given by: where R0 is the mean radius of the part. The comparison of the above two displacement profiles is shown in Figure 6.17 and the difference is only around 0.2%. The displacement is normalized with respect to the maximum tip deflection. The effect of radial constraint on the curved part is also investigated using the finite element analysis. The part is modelled with 20-noded isoparametric solid elements with in-plane reduced integration (100 elements along the tangential direction and 10 elements through the thickness are used). The finite element results for the tangential stress variation in the thickness direction and the bending moment distribution along the length of an aluminum part due to this radial constraint are shown in Figure 6.18 and Figure 6.19 respectively. The sharp drop of the bending moment to zero value at the end of the part is due to the fact that the tangential stress distribution should satisfy the stress free end condition. This is the difference between obtaining the same displacement profile by applied displacement and by applied moment. In the (6.26) v(0 = MRl (l-costf)) (6.27) EI - 178-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part first case, the stresses at the end should vanish to satisfy the stress free boundary condition. In the second case, the stress distribution should be such that it produces the applied bending moment. In our case, the radial constraint is imposed by applying a specified displacement. Let the displacement profile be given by: v W - v m a x ( l - c o s ( ^ ) ) (6.28) where v m a x is the maximum value of the gap at the tip of the part. For a quarter circular part v max = £ ' r e r R b • B Y comparing Equations (6.27) and (6.28) v m a x = M R ° EI According to Castigliano's second theorem, the rotation of the cross section of the part due to an applied moment, M , is given by: EI or (6.29) (0 = ^ * This rotation will produce equal and opposite tangential displacements at the top and bottom fibres of the part: = -^(0) = 12^.0 (6.30) According to the closed-form solution developed in the previous sections, the tangential displacement profile is given by: 11= l{s\n{kj){Ane^ +Bne-^r))} (6.31) n=l - 179-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part By applying the boundary conditions at r = Rb, u - -Dn and at r - R,, u = Dn to represent the equal and opposite displacements at the top and bottom surfaces of the part: - I n=l ( ( sinh A,sin(A:„0/) K In \ R b j ( + sinh k. ln r \R>) sinh A. In EuD„kn cos(kj) sinh ( f r \ \ \Rbjj f + sinh A. In f r w\ V \ R t JJ r sinh A. ln \ R b j (6.32) The unknown coefficients, Dn, can be found by equating the displacement to the known displacement profile at the bottom surface (i.e. at r = Rb,u-ub(^) in Equation 6.32): ub(t/>)=i{-Dnsm(kj)} 77=1 (6.33) By multiplying the above equation by s'm(kn0) and integrating over the length: "~K ) nkll Rn (6.34) The comparison of the closed-form solution with the finite element result for the variation of bending moment along the length for an aluminum part is shown in Figure 6.20. The closed-form result agrees well with the finite element solution. In the above equation, the effect of the radial stress is neglected. This is due to the fact that the radial stress should be zero at the top and bottom surface of the part to satisfy the stress free boundary condition. Hence the effect of the radial stress is not as significant as in the previous case (stress due to tangential thermal strain). - 180-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part The finite element results for the rotation of the cross section of a composite part with varying material properties (Table 6.1) is shown in Figure 6.21. According to Equation (6.29), for an applied displacement profile, the rotation angle of the cross section does not depend on the material properties. But according to Figure 6.21, the angle increases with increasing G 1 2 values {En remains constant). This may be due to the shearing effect. Figure 6.22 shows the shearing effect on a flat part. When a displacement is applied to the bottom fibre of a part, the top fibre does not bend as much as the bottom fibre due to the shearing effect. This shearing effect can be accounted for by modifying the bending rigidity, EI, of the part. The tip radial displacement of a cantilever quarter ring subjected to radial tip load P can be derived using Castigliano's energy theorem and is given as: v = °- + °— (6.35) m a x AEI AGAK where A is the cross sectional area of the part and K is the shear correction factor. For a rectangular 5 cross section K = — . 6 From the above equation, an effective bending rigidity, EI, to include the shearing effect can be defined such that: = = — + ^ r^ (6.36) EI EI RlGAK According to the above modification of the bending rigidity, the rotation of the cross section is modified as: - ~FJ *W =-=7 W (6-37) EI Figure 6.23 shows the modified analytical solution (Equation 6.37) for the rotation compared to the finite element result. The modified closed-form solution agrees well with the finite element results. - 181 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.24 and Figure 6.25 show the comparison of the closed-form solution with the finite element results for the variation of tangential stress distribution in the thickness direction in a composite part with varying material properties before (Equation (6.29)) and after (Equation (6.37)) the modification for the shearing effect. After the modification, the closed-form and the finite element results agree well. 6.3.1.2. Stresses due to Tangential Constraint When the radial constraint is applied by the tool, the part cross section rotates as shown in Figure 6.15(c). This rotation will be resisted by the tool by constraining the tangential displacements at the bottom fibre of the part. The closed-form solution for the tangential stress development due to this constraint can be obtained using: u = I {Dn sm{kj)\xn coshfc, ln(/J+ s inh(^ ln(/J]} (6.38) 71=1 The unknown coefficients, Dn, can be found by applying the displacement boundary condition at the bottom surface (at r — Rb, u = -ub) where ub is given by Equation (6.30). Hence the tangential displacement is given by: -ub(</>) = £ { / ) „ sin(M)k cosh(A„ln(%))+s inh(A„ln(%)) ]} (6.39) By multiplying the above equation by sm(kn0) and integrating over the length: Dn = H ) ( " + 1 ) - 4 T ^ L . . , , . / , < 6 - 4 ° ) 4 t v 1 ^ * max 1 nkl 2 tf0 [A„cosh(A„l4%))+sinh^„ln(% The closed-form prediction of the tangential stress variation in the composite part due to this constraint is compared with the finite element results in Figure 6.26. The closed-form results agree well with the finite element results. - 182-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part As shown above, the stresses in a curved part due to the thermal strain mismatch in the radial direction is the combination of the stresses due to radial and tangential constraints. The comparison of tangential stress induced in an isotropic aluminum part and a unidirectional composite part due to the thermal strain mismatch in the radial direction are shown in Figure 6.27 and Figure 6.28. In both cases, the predictions by the developed closed-form solution compare very well with the finite element results. 6.4. C U R V E D C O M P O S I T E P A R T ON A D E F O R M A B L E T O O L In the previous section, closed-form solutions were developed for a curved part on a rigid tool. Here the developed closed-form solutions are extended for a curved part on a flexible tool. The tool part assembly before and after the application of a temperature load is shown in Figure 6.29. To conform the part to the tool surface, radial and tangential constraints will be applied by the tool. To separate the tangential and radial behaviour of the assembly in the finite element analysis, only a quarter of the problem is modelled as shown in Figure 6.30. To simulate the isotropic expansion of the tool, bar elements are attached to the centre and the bottom of the tool surface as shown in the figure. The bar element has a unit cross sectional area and the same thermo-mechanical properties as the tool. The tool is made of aluminum and the part is made of a unidirectional composite. The part and tool thermo-mechanical material properties are given in Table 6.2. The tool and the part are 10 mm thick and the radius of the tool-part interface ( Rm ) is 636.62 mm. The tool-part assembly is subjected to an applied temperature of 100 °C. 6.4.1. Stresses due to Tangential Thermal Strain Mismatch The following equations are derived for a curved part on male tool. For the case of a curved part on a female tool, the part and the tool should be interchanged. - 183-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part For the tool: «=i v L n i . ^coshfc,,,ln(/J)+ sinhfr,,,ln(/J)]] o-i = Z j D\n K cos(A:„ <z>) 1 (6.41) ^ £ { o , D , . f e - 1 ) S i n f c ^ ) S i n h ( A " l n ^ ) ^ n=l For the part: K 2 = | { D 2 „ s i n ( M f e ^ - L n . K co gh(A 2>(^)) +sinh(A 2 l tln(x)]i] cr2 = Zj #2 A„ *» c o # » </>) ~ f ( 6 " 4 2 ) oo f / . \ . . s i n h U 2 „ l n ( ^ The unknowns Dln and £>2„ can be found by applying the continuity of displacement and equilibrium (continuity of shear stress) boundary conditions at the interface, i.e. at r = Rm, ux-u2 and rx = r 2 which leads to: n _ ( 4R»> (£S r " £'jer) C 4 G 2 (6.43) c 4 G 2 where the constants c, are defined as: c, = A,„ cosh (^„ l n ( % ) ) + s i n h ^ l n ( % ) ) c 2 = ^ „ cosh(^ 2 „ l n (%) )+ sinh(A 2„ l n ( % ) ) c 3 = f e - l ) s i n h ( ^ l n l n ( % ) ) ( 6 - 4 4 ) = fe-l)Sinh(^2„ln(^)) - 184-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part The correction for the radial stress should be added to the above equation. The comparison of the closed-form solution for the tangential stress in a composite part with the finite element solution is shown in Figure 6.31. The closed-form solution agrees well with the finite element results. For the case of a tool-part assembly separated by a thin interface layer with shear modulus Gs and thickness ts, Equation (6.43) is modified as: \(n+l) ^Rm{£2t ~ £ \ j > ) CiG2 nk2n (cxc4G2 - c2ciGl + csc4G2) c 3G, D2n=Dln^- (6.45) t where c, = c\G, — £ — m s The comparison of the closed-form solution for the tangential stress in composite part with the finite element solution is shown in Figure 6.32. The closed-form solution agrees well with the finite element results. 6.4.2. Stress due to Radial Thermal Strain Mismatch The deformation profile of the tool and the part due to the radial thermal strain is shown in Figure 6.33. The gap between the tool and the part depends on the radial thermal strain of the tool and the part. The stress in a curved part due to the radial thermal strain can be obtained by replacing the thermal strain of the part by an effective radial thermal strain: (^U ,v e =(^L-(^L (6-46) The maximum gap of the part is given by: ^=kher\ffectiveRm (6-47) - 185 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Depending on the value of the radial thermal strain of the part and the tool, the gap will be positive or negative as shown in Figure 6.34. In order to conform the part to the tool, the tool applies radial and tangential constraints. The stress due to radial constraint can be obtained from the Equations (6.32) - (6.34). The stress due to tangential constraint can be obtained from Equations (6.41) - (6.45) by replacing the tangential thermal strain values of the tool and the part by the following values: (*rL=<> t,her\ = _ ' v max for male tool (6.48) V * Ipart 2R0Rm tv _ max_ fQr f e m a l e t 0 Q l 2R0K The tangential stress distribution at a cross section of a composite part on Aluminum tool for the fully bonded condition and with shear layer interface are shown in Figure 6.35 and Figure 6.36 respectively. The closed-form solution agrees well with the finite results. 6.5. P R E D I C T I O N OF PROCESS- INDUCED D E F O R M A T I O N S In this section, the above developed closed-form solutions are used to predict the process-induced deformation of a composite part. The radial and the tangential deformation of a curved composite part at the end of a cure cycle are calculated. The part is made of unidirectional layers T-800H/3900-2 CFRP material and the tool is made of Aluminum. The tool-part assembly is cured under one-hold temperature cure cycle as shown in Figure 6.37. A uniform temperature is assumed for the whole structure. The part and the tool dimensions are same as in the previous examples. In this case, the correction for radial stress/displacement is not considered and the error due to its omission will be discussed. As In the flat part case, for the analysis, the cure cycle is divided in to small time steps (At). In each time step, the stresses in the part are calculated using the CHILE constitutive model [Johnston et al. (2002)]: - 186-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part ° " 2 , + A = 0 - 2 + A c r 2 ( 6 - 4 9 ) The cure dependent material properties and the incremental thermal strain for each time step are calculated using CCA module for this material by passing the temperature values at each time step. At the end of the curing process, the tool is removed and part warpage due to the residual stress that developed during curing is calculated. The unbalanced moment due to the residual tangential stress is given by: AM(</>) = | A C T 2 (r - R0)dr = J T A M n co$(kj) * " = l (6.50) M(t) = fj(Mn+AMn)cos(kj) The tangential and the radial deformations u and v due to this resultant moment can be calculated using the Castigliano's theorem and are given by: MRl *-= 1 7 ^ J - cosG* - 9)]d0 t. {EI )eff i = i ^ V V " ' fcos(*^)s in^ - 0)d0 «=1 Whff o ! f f " (6.51) MR' *-where {El)eff is the effective bending rigidity of the composite part at the time of tool removal. The calculation of effective bending rigidity follows the same procedure as for a flat part described in Section 5.4.1. Figure 6.39 and Figure 6.40 show the closed-form solution for the radial and tangential displacement of the composite part due to tangential and radial thermal strain mismatch respectively. The results are for the case of a part fully bonded to a tool (male). The closed-form solutions are compared with the finite element results. As shown in the figure, there is some difference between the closed-form and finite - 187-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part element results. This difference is due to the assumption of zero radial stress/displacement as discussed in the earlier section. The error is around 5%. Figure 6.41 and Figure 6.42 show the closed-form solution for the radial and tangential displacement of the composite part due to tangential and radial thermal strain mismatch respectively. The results are for the case of a part separated by a thin interface layer from the tool (male). The closed-form solutions are compared with the finite element results. The closed-form results agree very well with the finite element results and the error due to the assumption of zero radial stress/displacement is not significant. 6.6. DISCUSSION The developed closed-form solutions for a curved composite part perform well in predicting the process-induced stresses and deformations compared to finite element results. In this section, the closed-form solution will be used to explain some of the experimentally observed behaviour of curved composite parts. In the following discussion, unless otherwise stated, the following assumptions regarding the part and tool material and geometrical properties are made. The part is made of unidirectional layers of T-800H/3900-2 CFRP material and the tool is 5 mm thick and made of aluminum. The tool is in cylindrical form and the part is half cylinder. In general discussion, the part is assumed to be 600 mm long (radius of the bottom surface is 191 mm) and 8 layer (1.6 mm) thick. But other lengths (300mm and 1200 mm) and other thicknesses (4 and 16 layers) are also discussed. The part and the tool are separated by an interface layer with thickness of 0.2 mm and shear modulus of 2.60 kPa. 6.6.1. Scaling law Table 6.3 shows the variation of radial displacement with part geometry. The displacements are both due to thermal strain mismatch in tangential and radial directions. The closed-form results are compared with finite element prediction and both results agree well. - 188-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.43 shows the development of bending moment due to thermal strain mismatch in tangential direction along the cure cycle. The bending moment development occurs mostly at the heat-up portion of the cure cycle where the resin modulus is very low. This is similar to the bending moment development in a flat composite part. Twigg [Twigg et al. (2004)] proposed the following scaling law of warpage for a flat composite part: warpage (v m a x ) cc — (6.52) Figure 6.44 and Figure 6.45 show the variation of maximum radial displacement (warpage) of a curved composite part due to thermal strain mismatch in tangential direction with part length and thickness respectively. The variations are compared with Twigg's scaling law. As shown, the warpage due to thermal strain mismatch in tangential direction follows Twigg's scaling law. Figure 6.46 shows the development of bending moment due to thermal strain mismatch in radial direction along the cure cycle. The bending moment development occurs mostly at the cool-down portion of the cure cycle where the resin modulus is very high (elastic). This is opposite to the bending moment development shown above due to thermal strain mismatch in tangential direction. At the early stages of the curing process, since the resin modulus (and part shear modulus) is very low, it is easy (part shears easily) for the tool to conform the part to the tool shape. Hence no significant stress development occurs. At the cool-down portion of the cure cycle where the part shear modulus is very high, significant stress development occurs due to the constraint applied by the tool to conform the part. Figure 6.47 and Figure 6.48 show the variation of maximum radial displacement (warpage) of a curved composite part due to thermal strain mismatch in radial direction with part length and thickness respectively. As shown, the warpage varies linearly with part length and remains almost constant with part thickness. - 189-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part 6.6.2. Variation of Warpage with the Properties of Interface Layer Figure 6.49 shows the variation of warpage (maximum radial displacement) of a curved composite part due to thermal strain mismatch between the part and the tool in radial and tangential direction with shear modulus of the interface layer. The warpage due to tangential thermal strain mismatch varies linearly at the beginning and becomes constant. The constant segment represents the full bonding condition. This is similar to the variation observed for a flat part. Hence, a design curve of warpage number vs. shear layer number can also be constructed for curved parts similar to flat parts (see Section 5.5). The warpage due to radial thermal strain mismatch does not vary with the properties of the interface layer. 6.6.3. Male and Female Tools Figure 6.50 shows the radial displacement of a curved composite part on male and female tools with interface layer. The displacements are due to thermal strain mismatch in tangential and radial directions. For the male tool, the radial displacements due to these two sources are in the same direction (downward) while for the female tool they are in opposite direction. Hence by selecting a suitable interface layer as shown in Figure 6.51 the resultant radial displacement can be minimized as shown in Figure 6.52. 6.6.4. Simplification of the Solution for the Displacement due to Thermal Strain Mismatch in Radial Direction It was shown (Figure 6.46) previously that the bending moment due to thermal strain mismatch between the part and the tool in radial direction mostly develops at the cool-down portion of the cure cycle. This bending moment is due to three sources: CTE of the tool, CTE of the part, and cure shrinkage of the part. Figure 6.53 and Figure 6.54 show the contribution of each of these sources to the total bending moment and to the total radial displacement. Except the moment due to cure shrinkage, the moments due to part and tool CTE develop at the cool down portion where the material is fully cured. Hence, the radial displacement due to CTE of the part and the tool can be calculated from: - 190-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part v(</>)CTE = (CTEr1 - CTE1;0' ) (A7) Rm (l - cos(*)) (6.53) where AT is the difference between the hold and the room temperatures. According to Equation (6.53), the maximum radial displacement due to CTE mismatch between the part and the tool is 0.41 mm which is equal to the radial displacement calculated due to CTE mismatch by considering the whole cure cycle (Figure 6.54). The volumetric cure shrinkage (Vh) of this material is 10% (which is equal to linear strain (sf) of 3.2%) and it occurs between degrees of cure 0.3 and 0.9. The radial displacement due to cure shrinkage is given by: According to Equation (6.54), the maximum radial displacement due to resin cure shrinkage is 6.0 mm which is 20 times higher than the maximum radial displacement calculated considering the whole cure cycle (0.32 mm). This shows that only a certain percentage of the total cure shrinkage contributes to the displacement. As stated earlier, usual practice is to assume this percentage (around 10%). Is there a better way to estimate this percentage? According to Equation (6.36), the contribution of an applied displacement to the bending moment depend on {E'/Ei) ratio where EI is the bending rigidity of the part and EI is the modified bending rigidity to include the shearing effect and is given by Equation (6.36). {EIAi) r a u o ' s a n indication of what percentage of an applied displacement contributes to the bending moment. Figure 6.55 shows the variation of {El4:!) ratio and the incremental cure shrinkage strain along the cure cycle. According to this figure, the {E1/EI) r a n o between degrees of cure 0.3 and 0.9 remains almost constant at about 5% which is the percentage of contribution of cure shrinkage to the displacement. This shows that by looking at the development of {EI/Ei) r a n o a r*d the incremental cure shrinkage strain along the cure cycle, a reasonably good assumption can be made about the contribution of resin cure shrinkage to the part displacement. sh ^ X C l - c o s W ) (6.54) - 191 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part 6.6.5. Estimating Spring-in Angle using Nelson and Cairn's Equation As shown in the previous section, the deformation due to radial thermal strain mismatch can be estimated by only considering the cool-down portion of the cure cycle apart from the contribution from cure shrinkage. The Nelson and Cairn's equation (Equation (6.1)) also make the same assumption when estimating the change in the included angle. According to the previous analysis, the through-thickness thermal strain of the tool also contributes to the deformation. But in the Nelson and Cairn's equation, the tool thermal strain is not accounted for. Is there difference between our approach and the prediction by the Nelson and Cairn's equation? The measurement of the deformation due to the through-thickness thermal strain depends on two phenomenons: what quantity is measured (change in included angle or displacement) and with respect to what reference surface it is measured. Nelson and Cairn's equation gives the change in included angle of a curved part and our approach gives the tangential and radial deformation. Which quantity is most suitable as the measurement of dimensional discrepancy? This may depend on the application. For example, consider the free thermal expansion of an isotropic half circular part as shown in Figure 6.56. According to Nelson and Cairn's equation, the change in included angle is zero. But if the deformed shape of the part is compared to the reference (original) shape of the part, there is a discrepancy between the two shapes as shown in the figure. If the goal is to measure the change in part shape, then the change in included angle is sufficient to measure it. But, if the goal is to measure the change in shape and size, then the displacement is the suitable measure to quantify it. The measurement is also influenced by the reference surface. In the case of curved part on a tool, if the tool is assumed to be much stiffer than the part, the tool expands during the heat up and come back to its original shape during the cool down. Hence, the tool surface may be considered as the reference surface. The change of the tool-part interface during cool down is shown in Figure 6.57. In our approach of measuring the deformation, the tooling effect is the shifting of the reference (tool) surface. - 192-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part In the Nelson and Cairn's equation, the shape at the end of heat-up is considered as the reference surface (Figure 6.58). It is assumed that the included angle remain the same as the original shape. The validity of the assumption may depend on the problem. The following two examples show when the Nelson and Cairn's equation may not work or may work. The two cases considered for this example are shown in Figure 6.59. The parts are U-shaped with and without the flange. The part dimensions are shown in the figure. The tool is made of aluminum material with an isotropic thermal expansion coefficient of 30.0 y.c. The part is made of T-800H/3900-2 CFRP material with the tangential CTE equal to zero and the radial CTE equal to the part CTE. The effect of cure shrinkage is switched off to ease the analysis. The part CTE is kept constant through out the curing process. The radial and the tangential displacement of both cases are shown in Figure 6.60. According to Nelson and Cairn's equation, for this case, the change in the included angle (spring-in) should be around 0.43 degrees. But the finite element result shows almost zero change in included angle for the part without the flange. This is because, the tangential thermal strain mismatch affect is negligible due to the very short part length and the radial strain mismatch affect is zero due to the equivalent CTE of the tool and the part in the radial direction. For the case of the part with the flange, the spring-in angle around 0.38 degrees which is very close to the change in angle predicted by Nelson a Cairn's equation. This may be due to the fact the addition of the flange may help the curved portion of the part to retain its shape at the end of heat-up. This example shows that the Nelson and Cairn's equation can be used predict the spring-in angle of a very short curved part (negligible affect of the tangential tool-part thermal mismatch) with a flange. If the equation is used for a very short part without the flange, the radial thermal strain of the part should be modified according to Equation (6.39) to account for the tooling effect. - 193-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part 6.7. S U M M A R Y A N D C O N T R I B U T I O N S In this chapter, the closed-form solution developed for the flat composite part in the previous chapter was extended to a curved composite part. The behaviour of the curved part in the radial and tangential directions were analysed separately for simplicity. It was shown that the process-induced stresses and deformations of a curved part due to thermal strain mismatch between the part and the tool in the tangential direction is similar to the process-induced stresses and deformations of a flat part. Hence, all the conclusions drawn in the previous chapter are applicable to this problem too. For example, the maximum warpage of the part follows the Twigg's scaling law. Hence, the design curve of shear layer number vs. warpage number can also be constructed for the curved part. It was shown that, unlike the flat part, the assumption of zero through-thickness stress and deformation was not realistic due to the geometrical interaction between the radial and tangential stress components. Hence, a correction process was suggested to reduce the error due to this assumption. But the correction process was tedious. It was shown that the error due to the assumption of zero radial stress was only adverse for a fully bonded boundary condition. For the other interface condition, the error was negligible. The radial thermal strain mismatch between the part and the tool also induces stresses in a composite part. These stresses are due to the radial and tangential constraints applied by the tool on the part to conform the part to the tool shape. The unbalanced moment due these stresses mostly develop at the cool-down portion of the cure cycle where the material is fully cured. It is shown that the process-induced deformation due to the thermal strain mismatch in the radial direction can be estimated by considering only the cool-down portion of the cure cycle. It is also shown that the contribution by cure shrinkage can be estimated based on the ratio of the bending rigidities. It was pointed out that the change in included angle of a very short curved part predicted using Nelson and Cairn's equation introduced error when the tooling affect was not considered. Suggestions were made to eliminate this error. - 194-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Table 6.1 Mechanical properties of composite material at 4 different curing stages. These properties are used for the analysis of stress variation in a curved composite part under thermal load Cure En E22' E33 "12. 1^3 V23 G 1 2 , G 1 3 G23 stage (GPa) (MPa) (MPa) (MPa) 1 124.0 0.177 0.0 0.0 0.0665 0.058 2 124.0 1.770 0.0 0.0 0.6650 0.580 3 124.0 17.70 0.0 0.0 6.6500 5.800 4 124.0 177.0 0.0 0.0 66.500 58.00 Table 6.2 Thermo-mechanical properties of aluminum tool and Composite part. These properties are used for the analysis of stress variation in a curved composite part fully bonded to a curved tool and subjected to thermal load Composite part properties Aluminum tool properties Cure stages 1 2 3 4 E„ (GPa) 124.0 124.0 124.0 124.0 E (GPa) 69.0 E 2 2 = E 3 3 (MPa) 0.177 1.770 17.70 177.0 V 1 2 = V,2 0.000 0.000 0.000 0.000 v 2 3 0.000 0.000 0.000 0.000 V 0.327 G 1 2 = G 1 3 (MPa) 0.067 0.665 6.650 66.50 G 2 3 (MPa) 0.058 0.580 5.800 58.00 CTE, (u/°C) 0.030 0.030 0.030 0.030 CTE (u/°C) 23.6 CTE 2 = CTE 3 (u/°C) 29.50 29.50 29.50 29.50 - 195-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Table 6.3 Variation of warpage of a unidirectional curved composite part on an aluminum tool separated by a thin interface layer with part length and thickness. The closed-form solutions are compared with finite element results. Length (mm) Number of layers Warpage (Maximum radial displacement) (mm) Gs = 2.60 kPa ts = 0.2 mm Ls = 600 mm Length (mm) Number of layers Due to tangential thermal strain mismatch Due to radial thermal strain mismatch Length (mm) Number of layers FE CF FE CF 300 4 0.559 0.527 0.4 0.368 8 0.143 0.136 0.387 0.364 16 0.037 0.03 0.378 0.359 600 4 4.153 4.01 0.758 0.752 8 1.08 1.05 0.756 0.735 16 0.276 0.271 0.75 0.729 1200 4 29.73 29.06 1.6 1.62 8 8.09 8.02 1.51 1.5 16 2.105 2.11 1.51 1.47 - 1 9 6 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part (a) (b) Figure 6.1 Schematic of a curved part on a (a) a male and (b) a female cylindrical tools w = 0 Figure 6.2 Schematic of a curved part under applied traction at the bottom and top surfaces. The stress and displacement boundary conditions are also shown - 197-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.4 Variation of tangential/axial stress through the thickness of the curved/flat unidirectional composite part fully bonded to a rigid tool and subjected to a thermal load. The stresses are due to thermal strain mismatch in axial/tangential direction. The closed-form solutions for the flat and curved parts are compared - 198-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.5 Variation of tangential/axial stress through the thickness of the curved/ flat composite part fully bonded to a rigid tool and subjected to thermal load. The finite element results for the flat and curved parts are compared Figure 6.6 Finite element solutions for the variation of transverse stress along the length of a flat composite part at y = 0 for the case of a unidirectional composite part fully bonded to a rigid tool and subjected to thermal load. The inset shows a magnified view of the stresses near the free end - 199-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.7 Finite element solutions for the variation of transverse stress along the length of a curved composite part at y = 0 for the case of a unidirectional composite part fully bonded to a rigid tool and subjected to thermal load 0 0.1 0.2 0.3 0.4 0.5 0.6 0.7 Radial displacement, v (mm) Figure 6.8 Finite element solutions for the variation of the radial displacement through the thickness of the curved composite part fully bonded to a rigid tool and subjected to thermal load -200-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part ffff/*«(MPa) Figure 6.9 Variation of tangential/axial stress through the thickness of the composite curved/flat parts fully bonded to a rigid tool and subjected to thermal load. The radial displacement of the curved part is constrained Figure 6.10 (a) The variation of tangential stress using Equation (6.19) with the radial displacement obtained from F E (Figure 6.8) (b) the difference between the tangential stress variations based on constrained and unconstrained radial displacements (i.e. difference between Figure 6.5 and Figure 6.9) -201 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.11 Variation of tangential stress through the thickness of the curved composite part fully bonded to a rigid tool and subjected to thermal load. The stress is due to the radial displacement, (a) modified solution (Equation 6.20) compared with (b) finite element results Figure 6.12 Variation of radial stress through the thickness of a curved composite part fully bonded to a rigid tool and subjected to thermal load. The closed-form solutions (Equation 6.22) are compared with finite element results - 2 0 2 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Without correction With correction Tangential stress, 0^ (MPa) Tangential stress, 0„ (MPa) Figure 6.13 Variation of tangential stress through the thickness of the curved composite part fully bonded to a rigid tool and subjected to thermal load. The closed-form solutions with (Equation 6.25) and without (Equation 6.14) correction for radial displacement are compared with finite element results Figure 6.14 Schematic showing the free displacement of a flat and a curved part due to transverse/radial thermal strain -203 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.15 (a) Schematic showing the displacement of a curved composite part due to radial thermal strain. The (b) radial and (c) tangential constraints applied by the tool to conform the part to the tool shape are also shown Figure 6.16 Schematic showing the geometry of an un-deformed and deformed curved part due to the radial thermal strain - 2 0 4 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.17 Radial displacement profile of a curved part along the length due to radial thermal strain. The analytical solution from geometry (Equation 6.26) is compared with the radial displacement profile due to an applied moment from curved beam theory (Equation 6.27) 1 ™1 7:5- - & / a ~ f tu / _y less coordii) -J- —25-ThicL , -, e-- 3 - 2 - 1 0 1 2 3 Tangential stress, <T^ (MPa) Figure 6.18 Finite element solution for the variation of tangential stress through the thickness of a curved aluminum part fully bonded to a rigid tool and subjected to thermal load. The stress is due to radial constraint applied by the rigid tool -205 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part S Z 25 20 15 c « io E o 15 30 45 60 Angle <p (Degrees) 75 90 Figure 6.19 Finite element solution for the variation of bending moment along the length of a curved aluminum part due to the radial constraint applied by a rigid tool 25 20 a 1 5 g10 o Finite element • Closed-form (250 terms) 15 30 45 60 Angle <p (Degrees) 75 90 Figure 6.20 Variation of bending moment along the length of a curved aluminum part due to the radial constraint applied by a rigid tool. The closed-form solution is compared with finite element result -206-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.21 Variation of the rotation of the cross section of a curved composite part due to an applied displacement profde at the bottom surface. The finite element results are compared with the result from curved beam theory (Equation 6.29) Shearing effect Figure 6.22 Schematic showing the shearing effect due to an applied displacement at the bottom surface of the part -207-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.23 Variation of the rotation of the cross section of a curved composite part due to an applied displacement profile at the bottom surface. The finite element results are compared with the result from modified curved beam theory (Equation 6.37) Figure 6.24 Variation of tangential stress through the thickness of a curved composite part fully bonded to a rigid tool and subjected to thermal load. The stress is due to radial constraint applied by a rigid tool. The closed-form solutions without the correction for shearing effect (Equation 6.29) are compared with finite element solutions -208-Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.25 Variation of tangential stress through the thickness of a curved composite part fully bonded to a rigid tool and subjected to thermal load. The stress is due to radial constraint applied by the tool. The closed-form solutions with the correction for shearing effect (Equation 6.37) are compared with finite element solutions Figure 6.26 Variation of tangential stress through the thickness of a curved composite part fully bonded to a rigid tool and subjected to thermal load. The stress is due to tangential constraint applied by the tool (Equation 6.40) - 2 0 9 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part - 3 - 2 - 1 0 1 2 3 Tangential stress, (MPa) Figure 6.27 Variation of tangential stress through the thickness of a curved aluminum part fully bonded to a rigid tool and subjected to thermal load. The stress is due to both radial and tangential constraints applied by the tool -1 0 1 2 3 4 5 6 Tangential stress,(7^ (MPa) Figure 6.28 Variation of tangential stress through the thickness of a curved composite part fully bonded to a rigid tool and subjected to thermal load. The stress is due to both radial and tangential constraints applied by the tool - 2 1 0 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.29 Schematic of the tool-part assembly before and after the application of temperature load (the part is not constrained by the tool) Bars Figure 6.30 Schematic of the finite element model used to separate the tangential and the radial behaviour of the tool-part assembly - 2 1 1 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Tangential stress, G (MPa) Figure 6.31 Variation of tangential stress through the thickness of a curved composite part fully bonded to an aluminum tool and subjected to thermal load. The stress is due to the thermal strain mismatch between the part and the tool in the tangential direction Figure 6.32 Variation of tangential stress through the thickness of a curved composite part separated by a thin interface layer from an aluminum tool and subjected to thermal load. The stress is due to the thermal strain mismatch between the part and the tool in the tangential direction - 2 1 2 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.33 Schematic of the gap between the tool and the part in a male and a female tool due to radial thermal strain mismatch between the part and the tool Figure 6.34 Schematic of the positive and negative value of the gap which depends on the value of the radial thermal strain of the tool and the part -213 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.35 Variation of tangential stress through the thickness of a curved composite part fully bonded to an aluminum tool and subjected to thermal load. The stress is due to the thermal strain mismatch between the part and the tool in the radial direction Tangential stress, G^ (MPa) Figure 6.36 Variation of tangential stress through the thickness of a curved composite part separated by a thin interface layer from an aluminum tool and subjected to thermal load. The stress is due to the thermal strain mismatch between the part and the tool in the radial direction - 2 1 4 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part CCA Module CLOSED-FORM SOLUTION INTERFACE MODULE Pass in and update state variables T, a, V f MICRO MECHANICS MODULE Calculate composite properties CURE KINETICS MODULE Update a RESIN PROPERTIES MODULE FIBRE PROPERTIES MODULE Figure 6.38 C O M P R O component architecture used for modelling the evolving properties of the composite material -215 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part 20 10 £ E ? 0 E <u u et f - io -20 -30 — Finite element • Closed-form (8 terms) Radial, v Figure 6.39 Displacement profile of a curved composite part fully bonded to an aluminum tool. The displacements are due to thermal strain mismatch between the part and tool in tangential direction. The closed-form results are compared with F E results -3 Finite element • Closed-form (8 terms) Figure 6.40 Displacement profile of a curved composite part fully bonded to an aluminum tool. The displacements are due to thermal strain mismatch between the part and tool in radial direction. The closed-form results are compared with FE results - 2 1 6 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part 10 Figure 6.41 Displacement profile of a curved composite part on aluminum tool separated by an interface layer. The displacements are due to thermal strain mismatch between the part and tool in tangential direction. The closed-form results are compared with FE results 2 -3 Figure 6.42 Displacement profile of a curved composite part on aluminum tool separated by an interface layer. The displacements are due to thermal strain mismatch between the part and tool in radial direction. The closed-form results are compared with FE results - 2 1 7 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.43 Closed-form solution for the moment development in a curved composite part on aluminum tool separated by an interface layer. The moment is due to the thermal strain mismatch between the part and the tool in tangential direction 10 0 200 400 600 800 1000 1200 1400 Part length (mm) Figure 6.44 Variation of maximum radial displacement (warpage) with part length for a curved composite part on aluminum tool and separated by an interface layer. The displacements are due to the thermal strain mismatch in the tangential direction - 2 1 8 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part 0^ , , , , , , , , 1 0 2 4 6 8 10 12 14 16 18 Number of layers Figure 6.45 Variation of maximum radial displacement (warpage) with part thickness for a curved composite part on aluminum tool and separated by an interface layer. The displacements are due to the thermal strain mismatch in the tangential direction 200 0.3 E Z -0.3 g E o + -0.6 -0.9 50 100 150 200 Time (min) 250 300 350 Figure 6.46 Closed-form solution for the moment development in a curved composite part on aluminum tool separated by an interface layer. The moment is due to the thermal strain mismatch between the part and the tool in radial direction - 2 1 9 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.47 Variation of maximum radial displacement (warpage) with part length for a curved composite part on aluminum tool and separated by an interface layer. The displacements are due to the thermal strain mismatch in the radial direction 0.8 e 2 0.6 ^ 0.4 0.2 • - Finite element A - Closed-form 8 10 Number of layers 12 14 16 18 Figure 6.48 Variation of maximum radial displacement (warpage) with part thickness for a curved composite part on aluminum tool and separated by an interface layer. The displacements are due to the thermal strain mismatch in the radial direction - 2 2 0 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part 100 E E 5 10 E 4) U _« "a. T3 I 0.1 M s 0.01 Due to tangential thermal—, strain mismatch \ Due to radial thermal strain mismatch 1.0E+00 1.0E+01 1.0E+02 1.0E+03 1.0E+04 1.0E+05 1.0E+06 1.0E+07 Shear modulus of the interface layer (Pa) l.OE+08 Figure 6.49 Variation of radial displacement with shear modulus of the interface layer for a curved composite part on aluminum tool (male) and separated by an interface layer Figure 6.50 Radial displacement profiles of a curved composite part on aluminum male and female tools. The displacements are due to thermal strain mismatch in radial and tangential directions -221 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part 100 £ o.oi -I , , ,-1 , , , , I l.OE+00 l.OE+01 l.OE+02 l.OE+03 1.0E+04 1.0E+05 1.0E+06 1.0E+07 l.OE+08 Shear modulus of the interface layer (Pa) Figure 6.51 Variation of radial displacement with shear modulus of the interface layer for a curved composite part on aluminum tool (female) and separated by an interface layer. The figure also shows the shear modulus of the interface layer where the displacements due to radial and tangential thermal strain mismatch become equal - 0 . 8 Figure 6.52 Radial displacement profile of a curved composite part on aluminum female tool with an interface layer due to thermal strain mismatch in radial and tangential directions. The figure shows that by selecting an appropriate interface layer (Figure 6.51), the resultant radial displacement can be minimized - 2 2 2 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part 0 -I 1 1 1 , , , V -1.5 0 50 100 150 200 250 300 350 Time (min) Figure 6.53 Development of bending moment due to tool C T E , part C T E and part cure shrinkage along the cure cycle. The moments are due to thermal strain mismatch between the part and the tool in radial direction -1.2 Figure 6.54 Radial displacement profile of a curved composite part on a tool due to tool C T E , part C T E and part cure shrinkage. The displacements are due to thermal strain mismatch between the part and the tool in radial direction -223 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.56 Schematic showing the free thermal expansion of an isotropic curved part and the change in part shape (size) and included angle -224 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.57 Schematic description of (a) Spring-in (b) spring-out phenomenon which depends on the thermal strain mismatch between the tool and the part in radial direction -225 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Tool-part interface » ^ before cool down Part after _\ cool down ' \ Figure 6.58 Schematic describing the calculation of change in included angle by Nelson and Cairn's equation 5 mm' Figure 6.59 Finite element mesh of a U-shaped unidirectional composite part on a solid aluminum tool - 2 2 6 -Chapter 6: Closed-Form Solution for Process-Induced Stresses and Deformations in a Curved Composite Part Figure 6.60 The radial and the tangential displacements of a U-shaped unidirectional composite part with and without a flange on a solid aluminum tool. The figure shows the influence of the flange on displacements -227-Chapter 7: Higher Order Finite Element Techniques for Process Modelling Chapter 7. H I G H E R O R D E R FINITE E L E M E N T TECHNIQUES FOR PROCESS M O D E L L I N G 7.1. INTRODUCTION As shown in the previous chapter, the unbalanced moment due to the through-thickness stress gradient in a composite part causes the part to deform after the tool removal. This stress gradient mainly occurs at the beginning of the curing process when the ratio of the longitudinal modulus to transverse shear modulus is very high. As the material cures, the stress gradient diminishes. In Chapter 4, it was shown that by eliminating the locking effects, 3D solid elements with high aspect ratios can be used to model shell-like structures. This enabled us to reduce the number of elements in-plane. But the number of elements necessary in the thickness direction to capture the stress gradient is unknown and depends on the material and geometrical properties of the part. Finding the number of elements necessary by trial and error is costly and time consuming as it involves successive refinement of the finite element mesh. Adaptive mesh refinement has been the subject of extensive investigation with the objective of obtaining solutions with pre-specified accuracy with minimum cost of model preparation and computation [Zienkiewicz et al. (1983), Robinson (1986), Zhu and Zienkiewicz (1988), Wiberg and Moller (1988), Babuska et al. (1989), Szabo (1990), Babuska et al. (1992), Babuska and Suri (1994), Duster et al. (2001), Kuhlmann and Rolfes (2004), Rank et al. (2005)]. Finite element mesh is sequentially upgraded in such a way that the discretization error in the final solution is reduced and reaches the desired level. The computational effectiveness of a refinement method depends on several factors such as type of refinement, error estimator used and equation solver. The main two categories of refinements are the /z-refinement and the /^-refinement. In adaptive h-refinement, a mesh with -a fixed type of low order elements is repeatedly refined by reducing the size of the elements. There are two types of A-refinement. The first type is the selective element subdivision. - 2 2 8 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling Here some of the existing elements are divided into smaller ones keeping the original element boundary intact. This procedure is cumbersome since many hanging points are created as shown in Figure 7.1. The second type is done by complete mesh regeneration. Here all the elements are subdivided by the same number or a new mesh is generated with the new element size (uniform refinement). This method is computationally expensive. In contrast, adaptive p-refinement assumes that elements of the mesh remain fixed in both size and position. However, the polynomial order, p, of the shape functions is enriched by adding higher order terms without changing the existing lower order shape functions (Figure 7.2). The polynomial order can be increased uniformly throughout the whole domain or increased locally. There are many advantages and disadvantages in these two methods. The //-refinement procedure can be directly incorporated into existing finite element codes. For this reason, the //-refinement method has been more widespread in commercial finite element programmes than /^-refinement method. However, mathematical approaches and numerical examinations appearing in the literature have shown that the p-refinement method offers some significant advantages as compared to the //-refinement method. The rate of convergence of the //-refinement is more than twice as fast as the rate of convergence of the h-refinement with respect to number of degrees of freedom [Babuska and Suri (1994)]. Mesh generation for adaptive ^-refinement is simpler than for adaptive //-refinement [Szabo (1986)]. The hierarchical shape functions in the ^ -refinement procedure allow the reusability of all existing element stiffness matrix terms in the next solution. It was theoretically and numerically shown that the /^-version is free of locking problem, if the polynomial degree is chosen to be moderately high [Suri (1996)]. In the following section, a brief discussion of these two methods will be presented. For the //-refinement procedure, a specialized //-version, called the layerwise approach will be introduced. - 2 2 9 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling 7 . 1 . 1 . p - Refinements or Hierarchical Concept The essence of the displacement finite element formulation is in approximating the unknown displacement field, u, by an expansion such as: « = (7.1) ;=1 where TV,- are the shape functions, n is the total number of functions used and a, are the unknowns. If the a, are the displacement values at the element nodes, the method is called the "standard" finite element method. The usual choice for the shape functions is polynomial expansion and these shape functions have the value of unity at the corresponding node and zero value at other nodes. The standard shape functions for one-dimensional linear and quadratic elements are shown in Figure 7.3. The drawback of these standard shape functions is when element refinement is made, totally new shape functions have to be generated. This drawback can be avoided with "hierarchical shape functions". In this concept, the form of the shape functions does not depend on the number of nodes of the element. If a node is added, an additional shape function corresponding to this node will be introduced. But the other shape functions will remain the same. The hierarchical shape functions for 2-noded and 3-noded bar elements are shown in Figure 7.4. The hierarchical shape functions for the 2-noded element are the same as the standard shape functions and the unknowns ai are the displacements at the corresponding nodes. But in the 3-noded element case, the shape function corresponding to the 3 r d node is simply added with the unknown a 3 without modifying the shape functions TV, and 7V 2 . The unknowns ax and a2 represent the displacements, w, and u2, at nodes 1 and 2. But the unknown a3 does not have a physical meaning. 7.1.1.1. Choices of Hierarchical Shape Functions There are many possibilities of shape functions. Some of the choices are: - 2 3 0 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling a) Polynomials [Zienkiewicz and Taylor (2000)] An infinite number of choices of polynomial functions are available. Two examples are given below: (i) J V , = ± ( l - # ) N, 0+1) • # " -2 ) ( W 2 ) i = 2,3...p (7.2) (ii) tf,=i(l-£) W-t) iodd i = 2,3 /? (7.3) b) Legendre polynomials [Babuska et al. (1989)] # 2 = ± ( l + #) N(i+\)=<l>i i = 2,3,...p (7.4) where: J (PJ-PJ-T) 7=2,3,. . . (7.5) and Pj are the well known Legendre polynomials: 1 dk 2Kk\d? \t2-\f k = 0,1,2. (7.6) -231 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling c) Trigonometric functions [Wiberg (1985)] (7.7) = sin \i-\)n < 2 0 + <?) J i = 2,3...p The Legendre polynomials have orthogonal properties. The use of orthogonal polynomials brings some numerical advantages, like avoidance of round-off errors usually associated with polynomials of high degree. In addition, coupling between hierarchical degrees of freedom is minimized and a more dominant diagonal form of the stiffness matrix is obtained [Babuska et al. (1989)]. 7.1.2. h - Refinement in Thickness Direction or Layerwise Element Concept The layerwise element method is a specialized ^-refinement technique where the refinement is done only in the thickness direction of a shell-like element. The layerwise element method which is first introduced by Reddy [Reddy (2004), Robbins and Reddy (1993), Moorthy and Reddy (1998)] is used in the literature mainly to capture the continuity of transverse normal and shear stresses across the layer interfaces in a composite shell-like element [Zhou et al. (2004)]. A brief description of the method is given in this section. In the layerwise theory, the displacements are continuous through the laminate thickness but the derivatives of the displacement with respect to the thickness coordinate may be discontinuous. The displacement interpolation of the k'h layer is given by: m u(x,y,z)= 2Zuj(x,y)tj>j(z) m v(x,y,z)= I,Vj(x,y)jj(z) (7.8) m w(x,y,z)= zZuj(x,y) y/y(z) - 2 3 2 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling where <f>j (z) and y/j (z) are layerwise continuous functions and m is the number of nodes per layer. One-dimensional Lagrange polynomials are used for <f>j(z) and y/j{z) . The number of nodes through the layer thickness defines the polynomial degree as shown in Figure 7.5. Any desired degree of displacement variation through thickness can be obtained by increasing the element layers or increasing the order of the Lagrange polynomials (increasing the number of nodes per layer). The element layers can be less than, equal to or higher than the number of material layers. If the element layers are less than the material layers, then the material layers within an element layer should be represented as an equivalent single homogeneous layer. 7.1.2.1. Layerwise model versus 3D finite element The layerwise finite element approach is the same as a conventional 3D finite element model. The only difference is that a variable thickness plate should be approximated as an element-wise constant thickness plate in order to use Reddy's layerwise element. This restriction is mainly due to the integration technique used in the layerwise element. The layerwise model assumes that the displacements, material properties and element geometry can be approximated by a sum of separable interpolation functions. This allows the thickness integration to be performed independent of the in-plane integration. The result of the single through-thickness integration then can be used at each Gauss points in the subsequent in-plane integration. This method is mainly used to reduce the computational time. 7.1.3. Objective The objective of this study is to use the above two adaptive methods to make the process modelling more efficient. Here efficiency means not only the efficiency of the computational run time of a problem but the efficiency of the whole process of analysis. The process modelling procedure has three main components: setting up, solving and post processing. The setting up component takes a significant portion of the total time taken to solve a problem. Here both h- and /^-refinement techniques are used to automate the setting up procedure so that a single mesh can be used to study different lay-ups, different initial resin -233 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling modulus etc. In both cases the refinement is uniform for the whole domain of the composite part so that there is no inconsistency such as hanging points. The advantages of each method are also investigated to select the most suitable method for the composite processing. 7.2. H I G H E R - O R D E R E L E M E N T F O R M U L A T I O N Two types of higher order elements are described in this section based on the h- and /^-refinement procedure. The refinement is through the thickness direction only. The basic element has 24-nodes in total (8 on bottom, 8 on top and 8 on mid-plane) as shown in Figure 7.6. This element is similar to the element developed in Chapter 4. The bottom and top plane nodes have the 3 conventional displacement degrees of freedom (w,v ,w). The number of degrees of freedom at the mid-plane nodes varies depending on the number of terms used in /^-refinement and number of element-layers used in //-refinement. In the p-refinement case, the degrees of freedom at the mid-plane nodes are some unknowns and do not have any physical meaning. In the //-refinement case, the degrees of freedom at the mid plane nodes correspond to the displacements but the location of these displacement components depends on the number of elements in the through-thickness direction. The element is a composite element with different number of layers. The layers may be of the same material with different orientations or different materials. The layers are assumed to be stacked in the thickness direction. The layer thickness can vary arbitrarily. The varying layer thickness is defined at 4 corner nodes as the case for the 24-noded standard element described in Chapter 4. For each of these elements, the element contribution to global stiffness matrix (K ) and load vector (R) should be defined. These quantities are defined for an element as: v (7.9) s v - 2 3 4 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling 7.2.1. Numerical Integration Reduced Gauss quadrature (2*2 points) is used for in-plane integration to avoid locking effects and combination of Gauss and Simpson's rules are used for through-thickness integration similar to the 24-noded element. Generally, in a composite element, at least one integration point per layer is needed to capture the effect of different layer properties, if the integration scheme is Gaussian. If the integration scheme is Simpson, at least three integration points per layer are needed in the thickness direction. In a typical composite part, there are around 8 - 6 4 layers and the number of integration points in the thickness direction should be enough to integrate the higher order terms accurately. The efficiency of the run time is very sensitive to the number of integration points used to calculate the load and the stiffness matrices. The necessary number of integration points or the efficient technique of integration in the thickness direction should be well investigated. Even though our goal is the efficiency in the whole procedure of process modelling, the main focus here is on automating the process of selecting the number of elements in the thickness direction, so that the pre-processing time can be reduced or the costly successive mesh refinement for achieving solution convergence can be avoided. 7.2.2. Material Orientation The material orientation of the element should be defined by the user such that the 3 r d material axis is in the through-thickness direction. An additional rotation 6 about the 3 r d material axis can also be defined. Currently two material coordinate systems are implemented: Rectangular coordinate system and cylindrical coordinate system. Full details of the material orientation definition are given in Section 4.2.6. 7.2.3. Geometric Description The geometry of the element is only described by 16 nodes on the top and the bottom surface of the element. The through-thickness interpolation function for the geometry is linear (Figure 7.7). The mapping functions for the coordinates are given by: -235 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling 16 /=i V = f > , V , (7.10) i=i 16 Z = £ A T Z , <=i Since the order of the geometric interpolation is less than the order of the displacement interpolation, the element is subparametric. For a thin shell-like structure, linear interpolation should be accurate enough to describe the variation of geometry through thickness. 7.2.4. Displacement Interpolation The in-plane interpolation (shape) functions are similar to the shape functions of a 2-dimensional conventional serendipity 8-noded solid element (Figure 7.8). The eight in-plane shape functions (Qn) are given by: a =^ (1+^ x1+^ X +^^ ,-1) ' = i - 4 g 6 = i ( i + <f)(i-,72) (7.ii) The shape functions corresponding to each surface node are obtained by multiplying the in-plane shape functions with the corresponding through-thickness shape functions. If the through-thickness shape functions corresponding to the bottom, top and mid surface are denoted as R(,,R,and Rm respectively, then the displacement nodal shape functions are given by: - 2 3 6 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling Nj =QjRD Bottom surface nodes ~QiRt Top surface nodes JV ! + 1 6 - QtRm M i d surface nodes The displacement interpolation is given by: / = 1---8 (7.12) v = £ i V , v , . 1=1 (7.13) The number of shape functions, n and the form of the shape functions Nt depend on the type of elements used (h- or /^-refinement). Strains are defined according to the small strain definition (Section 4.2.5). 7.2.4.1. Hierarchical Elements In the hierarchical element formulation, the order of the through-thickness displacement interpolation is increased by adding additional degrees of freedom to the mid-surface nodes. The basic element has a quadratic interpolation function with 3 degrees of freedom at the mid-plane nodes. The degrees of freedom are arranged in the following manner: (u) = Uul v, w, —ut v 8 w g ) ( w 9 v 9 w9 • • • K 1 6 v 1 6 w 1 6 ) (a„ b„c„— a 2 4 b24 c 2 4 ) \ 1 » ' > v ' * « ' / (7.14) i=l 1=17 16 24 . 1=1 1=17 16 24 (7.15) 1=1 1=17 - 2 3 7 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling Only the order of interpolation for u and v are increased and the through-thickness interpolation function for w remains quadratic. The interpolation can be increased by one order by adding 2 more degrees of freedom to the mid-surface nodes (total of 16 dofs). (u) = ( (M, v, w , • yi/ , v 8 wg){u9 v9 w9 • •-M, 6 v,6 w16)jfl17 bi7c„ • •-<324 6 2 4c 2 4)(a 2 5 b25 • • -o^6 3 2 ) • • • I (7. 16) mtdsurface (=1 /=17 1=25 16 24 nv V = £ J V ( V < + 2 ^ ^ + S ^ A ( 7- 1 7) ;=1 1=17 1=25 16 24 (=1 As an example, the shape functions for a 3 r d order element are shown in Figure 7.9. As mentioned in Section 7.1.1.1, many different types of shape functions can be used for the hierarchical elements. The only requirement is that their values should be zero at the top and bottom nodes. The most generally used shape functions are the Legendre polynomials due to their orthogonal properties. The advantage of the orthogonality of the shape functions cannot be fully utilized in the composite element formulation, since the material properties are not constant in the thickness direction. Hence, both the sinusoidal functions and the Legendre polynomial functions are used. The sinusoidal functions are used due to their easy formulation. The through-thickness interpolation functions are given by: -238 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling *3=(i-<r2) (7.18) sin (i-\)n 0 + <f) 2 J i = 2,3,...p or The number p is the polynomial order and the hierarchical element is identified by this number. For example, the basic quadratic element is represented by p = 2. The advantages and disadvantages of the sinusoidal functions compared to the Legendre polynomials will be investigated in terms of the rate of solution convergence (Section 7.3.2). 7.2.4.2. Layerwise Element In the layerwise element method, each layer is a quadratic 24-noded element (the through-thickness interpolation is quadratic). The through-thickness shape function for a one element-layer is given by: An additional element-layer can be added to the element by adding two. more nodes in the thickness direction as shown in Figure 7.10. To add physical nodes, the meshes should be regenerated. To avoid the regeneration of the finite element mesh the addition of an element-layer is done by adding degrees of freedom to the mid nodes. The layerwise element is a composite element with multiple material-layers (Figure 7.11). The number of element-layers (h) and the number of material-layers within each element-layer are user input for the (7.19) - 2 3 9 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling current implementation and the selection process can be automated. The main differences between the current approach and Reddy's approach [Reddy (2004)] are: 1. Each element layer can have any number of material-layers and the user does not need to provide the equivalent properties of the layers. 2. The material-layers do not need to have a constant thickness. The main restriction of the current layerwise approach is that the number of element layers cannot be dynamically added or dropped. This is due to the difficulty in changing the nodal locations and adjusting the material layers within each element layer when an element layer is added or dropped. The number of element layers necessary for a particular problem is selected at the beginning of the analysis and kept constant throughout the analysis. But the selection process of the necessary number of element layers can be automated. The number h indicates the number of element layers in the layerwise element and the element is identified by this number. For example, the basic quadratic element is represented by h = 1. 7.3. VERIFICATION E X A M P L E S 7.3.1. Stress Variation in a Flat Composite Part on a Tool under Constant Thermal Load In this example the stress variation in a composite flat part on a tool under uniform thermal load (isothermal condition) is investigated. The tool part arrangement is as shown in Figure 7.12. The part is made of 8 layers of CFRP composite materials and the tool is made of aluminum. The part and the tool properties are given in Table 7.1. A uniform temperature of 160 °C is applied to the tool-part assembly and the axial stress variation in the thickness direction is investigated. The problem is modelled using both the hierarchical and the layerwise elements and the results are compared with the closed-form solution (Section 5.3.2). The axial stress variation through the thickness obtained using different number of element layers in the layerwise element technique is shown in Figure 7.13. As shown in the figure, as the number of element layers increases through the thickness, the stress - 240 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling distribution converges to the closed-form solution. The axial stress variations obtained using different number of sinusoidal and Legendre polynomial terms in the hierarchical element technique are shown in Figure 7.14 and Figure 7.15, respectively. As shown in the figures, as the number of terms increases, the stress distribution converges to the closed-form solution. The convergence rates of these elements will be compared in the next example. 7.3.2. Warpage Prediction of Flat Composite Part Cured under a Prescribed Cure Cycle This example is to study the convergence rates of the layerwise and the hierarchical elements. The warpage of a flat unidirectional composite part on aluminum tool is studied using both elements. The part is made of 8 unidirectional layers of T-800H/3900-2 CFRP material. The tool and the part geometry are the same as in the previous example. The part is cured under the temperature cure cycle shown in Figure 7.16. This is similar to the example problem studied in Chapter 4 using the standard 24-noded element where the maximum warpage of 35.29 mm was obtained using around 16 elements in the thickness direction. The convergence rate is generally measured in terms of total number of degrees of freedom used in the model. The variation of the warpage with the total number of degrees of freedom in both methods for the full bonding case is shown in Figure 7.17. As shown in the figure, the hierarchical method converges faster than the layerwise element method. Among the hierarchical methods, the element with Legendre polynomial terms shows a faster rate of convergence than the element with sinusoidal terms. The convergence rate depends on the approximation of axial displacement, u, (which varies in an exponential manner according to the closed-form solution) in the thickness direction by the assumed displacement functions in both the layerwise and hierarchical methods. Hence, it is appropriate to compare the number of degrees of freedom used for the interpolation of axial displacement, w, in the thickness direction. The variation of the warpage with the number of degrees of freedom used for the axial displacement interpolation in the thickness direction in both methods for the full bonding case is -241 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling shown in Figure 7.18. As shown in the figure, the hierarchical method has only slightly faster convergence rate than the layerwise method. The rate of convergence for the tool-part arrangement separated by an interface layer (Gs = 26.0 kPa, ts = 0.4 mm) is shown in Figure 7.19. Similar to the fully bonded case, the hierarchical method has a slightly faster convergence rate than the layerwise element method. One would expect that since the interface layer reduces the stress transformation between the tool and the part, the steepness of the stress gradient should be less in this case than the full bonding case. Hence, the solution should converge faster than the full bonding case. Contrary to our expectation, in this case too, the same number of terms and the same number of element layers are necessary to achieve the fully converged solution as in the full bonding case. To find out the reason, the variation of axial stress distribution at a cross section of the composite part with the interface layer properties is investigated. The properties of the interface layers used are given in Table 7.2. The actual and the normalized, ( ^ . ^ ) , axial stress distributions in the thickness direction at a cross section of the part are shown in Figure 7.20. As shown in the figure, even though the maximum axial stress value may vary with the interface layer properties, the through-thickness stress distribution does not depend on the interface layer properties. Hence, regardless of the interface layer properties, for a specific case of a tool and a part, it will take the same number of terms and number of element layers to obtain convergence in hierarchical and layerwise methods, respectively. The variation of run time with number of degrees of freedom in both methods is shown in Figure 7.21. As shown in the figure, in the hierarchical method, the run time increases in an exponential manner. Even though the convergence rate of the hierarchical method is slightly faster than the layerwise method, it is not as efficient as the layerwise method in terms of the run time. The ways of selecting the number of terms and the number of element layers in both methods and the way of reducing the run time of the hierarchical element method will be discussed in the following sections (Section 7.3.5). - 2 4 2 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling The convergence rate strongly depends on the variation of in-plane displacements in the thickness direction. In the above analysis of a unidirectional composite part, the axial displacement variation in thickness direction is a smooth function. If the variation of displacement is a non-smooth function as in the case of a sandwich beam or a part with layers of different orientation, the layerwise approach may converge faster. An example of a sandwich cantilever beam will be given to demonstrate this in the next section. 7.3.3. Bending of a Cantilever Sandwich Beam This is similar to the sandwich beam example studied in Section 4.3.4. The cantilever sandwich beam under uniformly distributed load is shown in Figure 7.22. The top and the bottom skins are made of unidirectional composite materials and the core is made of a soft isotropic material. The material properties of the skin and the core are given in Table 7.3. The problem is modelled with both the hierarchical and the layerwise elements. In the layerwise element case, the skin and the core are each modelled with one individual element layer in the thickness direction. In the hierarchical element case, only one element is used in the thickness direction and the number of terms is increased to obtain converged solution. The vertical displacement profiles predicted by the two methods are shown in Figure 7.23. As shown in the figure, the hierarchical method needs large number of terms to converge. This is due to the very non-smooth in-plane displacement distribution in the thickness direction as shown in Figure 7.24. To approximate this non-smooth function with high order smooth functions, a large number of terms is necessary. This example demonstrates that the rate of convergence highly depends on the actual distribution of the in-plane displacements in the thickness direction. Since most practical composite parts are made of layers with different orientation, the displacement variation in the thickness direction is a non-smooth function. Hence, the layerwise elements may be more suitable in those cases compared to the hierarchical elements. The variations of axial displacement in the thickness direction for 2 different lay-ups from the layerwise and hierarchical methods are shown in -243 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling Figure 7.25 and Figure 7.26, respectively. As shown, a large number of terms is necessary to approximate the non-smooth displacement function in the hierarchical method. 7.3.4. Selection of number of terms or number of element layers In the closed-form presented in Chapter 5, it is shown that the through-thickness variation of the axial displacement, u, is an exponential function which depends on the material and geometrical properties of the composite part: Py P = ^. 21 V G 13 7 (7.24) where y is a non-dimensional thickness coordinate varying from 0 to 1.0. By expanding the above equation using Taylor series: 1! 2! 3! (7.25) * \ + py + C0y2 +C]y3 +••• The additional number of terms and the number of element layers necessary will be decided based on the following procedure. The basic element (24-noded element) has a 2 n d order shape function or one element in the thickness direction. The additional order of the shape function or the additional number of element layers is decided based on (c"*y^ ) ratio. If this ratio is less than a certain threshold value, then the order of the shape function is n and the number of element layers is y . The threshold values for the hierarchical and the layerwise approaches are currently unknown and are decided based on some trial runs. (C"*x/C ) for the composite part studied in the above example during the initial stages of curing is shown in Figure 7.27. Based on the number of terms and the number of element layers needed in the - 2 4 4 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling previous example used to study the convergence rates, the threshold value of 1.5 and 1.0 are selected for the hierarchical and layerwise methods, respectively. 7.3.5. Reducing the Run Time in the Hierarchical Method The run time of the hierarchical method can be reduced by the following two ways: 1. Efficient integration technique 2. Dynamically changing the number of terms In the recent literature there have been a number of efficient numerical techniques recommended for the hierarchical method to reduce the run time such as the vector integration technique [Hinnant (1994), Nubel et al. (2001), and Wagner (2003)]. This methodology will not be investigated here. The second method of reducing the run time is to dynamically change the number of terms used in the hierarchical elements. As noted in the previous section, higher order terms may be necessary only at the initial stages of the curing process when the stress gradient is steep. The additional number of terms necessary during the cure cycle to achieve the converged solution based on the threshold value of 1.5 for the above example of a flat part is shown in Figure 7.28. As shown in the figure, the large number of terms is only necessary at the initial stages of the cure cycle. 7.3.5.1. Implementation in A B A Q U S To change the number of terms dynamically, the degrees of freedom at the mid surface nodes of the element should be able to change dynamically. At this time, the finite element code ABAQUS does not allow such capability. Currently for the user element, the number of nodes and the degrees of freedom at each node should be predefined and remain fixed throughout the analysis. To implement the above concept, the developed element should be implemented in a finite element code that will allow the degrees of freedom to be changed dynamically. -245 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling To verify the benefit of the concept of dynamically changing the terms in the hierarchical method, the dynamic variation of active degrees of freedom is implemented through the application of dynamically changing the boundary conditions. In this case, the mid surface nodes of the element have the predefined number of degrees of freedom which is sufficient for the highest number of terms necessary for that particular problem. The number of terms necessary along the cure cycle is a user input and is read inside the element. The element calculates only the required components of the load vector and stiffness matrix for the active degrees of freedom at that time step. The rest of the components of the load vector and the stiffness matrix are set to zero. In the input file, the unnecessary degrees of freedom are set to zero using prescribed displacement boundary condition. The implementation of dynamically varying the number of terms through dynamically changing the boundary condition is done by dividing the cure cycle into two segments as shown in Figure 7.29 Cure cycle separated into two time regimes: one requiring higher order terms and one without . In the first segment, higher order terms were used and the second segment only the basic element without any additional hierarchical terms is used. The run time as a function of degrees of freedom using the above method is shown in Figure 7.30. As shown in the figure, the run time is substantially cut down (around 50%) by changing the number of terms in two steps. If the number of steps are increased then the run time will be further decreased. But the run time of the hierarchical method will be still greater than the layerwise method. To increase the efficiency of the hierarchical method, the efficient integration technique mentioned earlier should be employed. From the above example problems, it is apparent that the layerwise element method has many advantages over the hierarchical element method such as efficiency in run time and the ability to model non-smooth displacement variation through thickness. Hence, in the following section, the layerwise element method will be adopted with the combination of contact surface in ABAQUS to predict the results of the warpage experiments conducted by Twigg [Twigg et al. (2004b, 2004c)]. - 2 4 6 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling 7.4. W A R P A G E P R E D I C T I O N In Chapter 5, the experimentally observed results of the warpage of flat unidirectional composite parts of three different lengths (1200 mm, 600 mm and 300 mm) and three different thicknesses (16 ply, 8ply and 4 ply) were predicted by the closed-form solution. The tool-part interface condition was simulated by a thin interface layer. The predicted results agreed well with the experimental trend observed by Twigg [Twigg et al. (2004b, 2004c)]. The main disadvantage of the interface layer was that the interface layer properties depended on the part length. Hence, the shear layer properties had to be modified, if the part length was not the same as the length of the part for which the shear layer was characterized. In this section, the tool-part interface condition is simulated with the ABAQUS contact surface. The part is made of T-800H/3900-2 material and the tool is made of aluminum. The tool part assembly is cured under the one-hold temperature-pressure cycle as shown in Figure 7.31. A uniform temperature is assumed for the whole structure (i.e. a heat transfer analysis is not carried out). The part is modelled with the layerwise element and the tool is modelled with the 20-noded ABAQUS built-in element. The number of elements along the length and the number of element layers necessary to achieve the converged solution are shown in Table 7.4. The number of element layers in the thickness direction is selected based on the threshold value of 2 (c-*yc = 2). It was shown in Chapter 5 that most of the unbalanced moment, which is responsible for the final part warpage, develops at the early stages of the cure cycle. Hence, it is very important to capture the tool-part interaction at the early part of the cure cycle accurately. It was shown experimentally [Twigg et al. 2003), Ersoy et al. (2005)] that a sliding interface condition exists at the early stages of the cure when the resin has very low modulus. During the hold of the cure cycle the part sticks to the tool and during the cool down, the part debonds from the tool and slides on it again. Our focus is the sliding interface condition during the heat-up portion of the cure cycle since stresses that develop at the later stages of the cure cycle do not contribute to the unbalanced moment. A more detailed study of the contact surface method to - 2 4 7 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling capture the experimentally observed interface behaviour throughout the cure cycle can be found in the recent doctoral thesis by Osooly [Osooly (2007)]. The basic Coulomb friction model available in ABAQUS with the maximum shear stress limit is used to model the sliding interface condition (Figure 7.32). The basic concept of the Coulomb friction model is to relate the maximum allowable frictional (shear) stress across an interface to the contact pressure between the contacting bodies. In the basic form of the Coulomb friction model, two contacting surfaces can carry shear stresses up to a certain limit across their interface before they start sliding relative to one another; this state is known as sticking. The Coulomb friction model defines this critical shear stress, xcrit, at which sliding of the surfaces starts as a fraction of the contact pressure, p, between the surfaces (Tcru = MP)- The stick/slip calculations determine when a point transitions from sticking to slipping or from slipping to sticking. The fraction, p , is known as the coefficient of friction. An optional equivalent shear stress limit, r m a x , can be also specified so that, regardless of the magnitude of the contact pressure, sliding will occur if the magnitude of the shear stress reaches this value: Tcril =minC"/7,rmax) (7.26) In this analysis, a p value will be selected depending on the autoclave pressure so that r m a x w i l l always be the minimum ( r m a x < pp). When using the contact surface in ABAQUS, the following difficulties were encountered: 1. According to the micromechanical equation used to calculate the equivalent composite properties [Rosen and Hashin (1964)], the transverse properties of the composite are dominated by the resin properties. Hence at the initial stages of cure, the composite part has a very low (17.7 kPa) modulus in the thickness direction. When high pressure is applied to the part, the through-thickness strain becomes very large and in the absence of large strain capability of the element the part element flips and causes numerical problem. - 2 4 8 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling 2. ABAQUS allows only a nodal based surface to be defined for the user element where the nodal area should be provided in order to calculate the contact pressure. Calculation of the associated area of each node in a non-regular mesh is very difficult. 3. A constant pressure applied to the face of a second-order element, which does not have a mid-face node (20-noded or 24-noded), produces consistent nodal forces at the corner nodes acting in the opposite sense of the pressure which leads the code to make a wrong decision on the contact. Hence, a 27-noded element should be used in such circumstances. To overcome the above difficulties, a single 27-noded element in the thickness direction is superposed on the layerwise element. This dummy element has higher through-thickness modulus in order to prevent the element flipping and the rest of the properties are made negligible so that it does not interfere with the in-plane behaviour of the layerwise element. The contact surface is also defined on this element in order to avoid the nodal based surface definition on the layerwise element. Twigg reported the following dependency of the warpage on the pressure: V P 2 0.2 (7.27) where v and are warpages corresponding to autoclave pressures of pt and p2 • However, according to our curve fitting to Twigg's results, we found a slightly lower sensitivity to pressure. Hence, r m a x is modified for pressure dependency as: T 'max T, max \f 1 y (7.28) The predicted results with contact surface are compared with the experimental results as shown in Table 7.5 and Figure 7.33. Only two sets of experiments are considered here since the other two sets also follow the same procedure. Since all the experimental values do not exactly follow the average trend observed by - 2 4 9 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling Twigg (Equation 5.50), first the experimental results are adjusted to the trend as shown in the table. Then the contact surface property, r m a x , is calibrated to match one experimental value as highlighted in the table. The contact surface property of the second experimental set is calculated according to Equation (7.28). The predicted results agree well with the experimental results. The results from the shear layer approach presented in Chapter 5 are also shown for comparison. The results from the two approaches are almost the same and the critical shear stress value from the contact surface approach and the average shear stress value from the shear layer approach are of the same order (the average shear stress value of the shear layer approach is calculated at the initial stage of the cure). This shows that the shear layer approach is a simple approximate alternative to simulate the tool-part interaction. Even though the shear layer properties should be modified for different part lengths, it is a very fast method to simulate the tool-part interaction compared to the contact surface. Finite element analysis for warpage of a 600 mm long, 8-ply thick composite part with the shear layer approach is about 40% faster than the finite element analysis with the contact surface approach. 7.5. S U M M A R Y A N D CONTRIBUTIONS The closed-form solutions presented in the previous chapters showed that the in-plane stress gradient in the thickness direction depends both on the material and geometrical properties. If the curing process of a composite part is modelled with the standard solid elements, the number of elements necessary in the thickness direction to achieve the converged solution may vary from problem to problem. Finding the number of elements by trial-and-error method is costly and cumbersome since it involves successive refinement of the mesh in the thickness direction. In this study, based on the knowledge gained from the closed-form solutions, two adaptive finite element techniques were developed so that just one element in the thickness direction can be used to study different problems. The two developed finite elements were based on the hierarchical and layerwise concept available in the literature. The developed methods use the same 24-noded subparametric element as the base. The element has three 8-noded surfaces (bottom, mid and top). The number of terms in the - 2 5 0 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling hierarchical method and the number of elements in the layerwise method can be increased without changing the original mesh by adding the required additional degrees of freedom to the mid surface nodes. A methodology was developed to select the number of elements or the number of terms automatically based on the material and geometrical properties. The elements were implemented in ABAQUS using the user defined element feature. It was shown that the layerwise element has many advantages over the hierarchical element in terms of the run time efficiency and representing the non-smooth displacement variation in the thickness direction. Even though the developed layerwise element is similar to the element introduced by Reddy [Reddy (2004)], the current element formulation is more general such that it can have varying layer thicknesses and any number of material layers within an element-layer. Even though the hierarchical elements have the drawbacks mentioned above, their faster convergence rate and their easy implementation make them attractive. Two methods were suggested to reduce the computational run time: efficient spatial integration technique and the ability to change the number of terms continuously. It was shown that by continuously changing the number of terms, the run time can be reduced by 50%. The developed layerwise element was used with the combination of the contact surface in ABAQUS to predict the experimentally observed warpage of flat composite parts. The predicted results agreed very well with the experimental results. The predicted results were almost the same as the results from the analytical shear layer approach presented in Chapter 5. It was shown that for a particular example of 600 mm long and 8-ply thick unidirectional composite part, finite element analysis with the shear layer approach is around 40% faster than the contact surface approach. -251 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling Table 7.1 Material properties of the CFRP composite part and the aluminum tool used for the analysis of axial stress variation in a composite part on a tool and subjected to thermal load Part Properties Tool Properties E„(GPa) 124.0 E (GPa) 69.0 E 2 2 = E 3 3 (kPa) 177.0 Vl2 = V i 2 0.261 v 2 3 0.523 V 0.327 G, 2 = G 1 3 (kPa) 66.5 G 2 3 (kPa) 58.0 CTE, (u/°C) 0.03 CTE (u/°C) 23.6 CTE 2 = CTE 3 (u/°C) 29.5 Table 7.2 Material properties of the shear layers used in the analysis of variation axial stress distribution in thickness direction with shear layer properties Shear Layer E{,, E22 (MPa) £33 (GPa) v\2> V13 ' V 2 3 G]2,GU,G23 (MPa) OC ^ y CC 2 5 CC^ (u/°C) 1 0.069 69.0 0.0 0.026 0.0 2 0.690 69.0 0.0 0.260 0.0 3 6.900 69.0 0.0 2.600 0.0 4 69.00 69.0 0.0 26.00 0.0 3 is the through-thickness direction. E 3 3 is kept higher to prevent element flipping under higher autoclave pressure Table 7.3 Material properties of the composite skin and the soft core of a sandwich beam under uniformly distributed load Part Properties Skin Core E,,(GPa) 126.0 0.10 E 2 2 = E 3 3 (GPa) 10.20 0.10 V , 2 = V , 2 0.265 0.00 V 2 3 0.467 0.00 G, 2 = G 1 3 (GPa) 5.440 0.05 G 2 3 (GPa) 3.460 0.05 CTE, (u/°C) 0.030 23.5 CTE 2 = CTE 3 (u/°C) 29.50 23.5 - 2 5 2 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling Table 7.4 The selected number of element layers for the layerwise element used to simulate the experiments conducted by Twigg [Twigg et al. (2004a, 2004b)] Length (mm) Number of Plies Number of Elements Length*Thickness 4 15*4 300 8 15*8 16 15*16 4 30*2 600 8 30*4 16 30*8 4 60*2 1200 8 60*2 16 60*4 Table 7.5 Comparison of the warpage prediction by the layerwise element with contact surface with the experimental results [Twigg et al. (2004)]. The adjusted experimental results according to the trend given by Equation (5.50) and the closed-form solution with shear layer are also shown. The matched warpage value in the first set of experiment to characterize contact surface ( r m a x ) is highlighted Warpage ( mm) Interface = = FEP Interface = = FEP Pressure 103 kPa Pressure = 586 kPa Shear layer - tave = 5.0 kPa Shear layer - tave = 5.6 kPa Contact surface - r m a x = 5.8 kPa Contact surface - r m a x = 6.4 kPa Number of layers _ Contact surface • ts Length (mm) Number of layers Contact surface 8 Length (mm) Number of layers Exp. results Adjusted Exj Closed-form Contact surface Exp. results Adjusted Exj Closed-form Contact surfi 4 0.70 0.48 0.48 0.48 0.43 0.53 0.52 0.53 300 8 0.13 0.12 0.12 0.14 0.15 0.13 0.13 0.16 16 0.04 0.03 0.03 0.06 0.16 0.03 0.03 0.08 4 3.84 3.80 3.63 3.57 3.94 4.20 4.0 3.93 600 8 0.81 0.95 0.95 0.95 0.86 1.05 1.05 1.06 16 0.12 0.24 0.24 0.27 0.28 0.26 0.27 0.31 4 29.1 30.4 26.5 25.0 39.6 33.6 29.0 27.5 1200 8 7.26 7.60 7.28 7.05 8.97 8.40 8.0 7.77 16 1.18 1.90 1.9 1.89 1.31 2.10 2.09 2.09 -253 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling -Hanging points Uniform refinement Selective refinement Original mesh Figure 7.1 Schematic showing the uniform and selective //-refinements Original mesh Uniform refinement -Hanging points Selective refinement Figure 7.2 Schematic showing the uniform and selective //-refinements - 2 5 4 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling A^(l-#) iV,=I(l-£) Figure 7.4 Schematic of the hierarchical shape functions for 2 and 3-noded bar elements -255 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling Figure 7.5 Schematic of the linear and the quadratic through-thickness displacement shape functions in the layerwise approach x Bottom surface Figure 7.6 Schematic of the 24-noded higher order element with the non-conventional mid surface nodes to which the additional degrees of freedom are added - 2 5 6 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling Bottom Figure 7.7 Linear through-thickness geometrical interpolation function for both the hierarchical and the layerwise elements Top M i d Bottom Figure 7.8 Node arrangement in the higher order element for geometrical and displacement interpolation - 2 5 7 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling Figure 7.9 Through-thickness displacement interpolation functions for hierarchical element. The displacement functions shown are for 3 r d order hierarchical element Figure 7.10 Through-thickness displacement interpolation functions for layerwise element. The displacement functions shown are for one and two element layers - 2 5 8 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling I— Material layer m • (> 1 • II - - - J l II . . . J iI— Material layer 1 • < Element layer n y Element layer 2 Element layer 1 Figure 7.11 Schematic showing the definition of the element and material layers in a layerwise element 300 mm Figure 7.12 Schematic of a flat composite part fully bonded to an aluminum tool. The figure also shows the displacement boundary conditions for half of the problem modelled due to symmetry -259-Chapter 7: Higher Order Finite Element Techniques for Process Modelling Element layers -m— h = l h = 2 h = 3 h = 4 Closed-form 200 x (MPa) Figure 7.13 The variation of axial stress at a typical cross section in a unidirectional composite beam on an aluminum tool (full bonding) predicted with various number of element layers in the layerwise element method and their comparison with the closed-form solution Figure 7.14 The variation of axial stress at a typical cross section in a unidirectional composite beam on an aluminum tool (full bonding) predicted with various number of sinusoidal terms in the hierarchical element method and their comparison with the closed-form solution - 2 6 0 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling -100 0 100 200 300 400 500 Oxx(MPa) Figure 7.15 The variation of axial stress at a typical cross section in a unidirectional composite beam on an aluminum tool (full bonding) predicted with various number of Legendre polynomial terms in the hierarchical element method and their comparison with the closed-form solution - 2 6 1 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling 80 1000 2000 3000 4000 5000 6000 Number of degrees of freedom Figure 7.17 Comparison of the convergence rate for the maximum warpage of a fiat composite part fully bonded to an aluminum tool using the layerwise and the hierarchical methods. The convergence rate is in terms of total number of degrees of freedom used in the model 80 30-^ , , , , , 1 0 2 4 6 8 10 12 Number of degrees of freedom used for u interpolation in thickness direction Figure 7.18 Comparison of the convergence rate for the maximum warpage of a flat composite part fully bonded to an aluminum tool using the layerwise and the hierarchical methods. The convergence rate is in terms of number of degrees of freedom used for the interpolation of u in the thickness direction - 2 6 2 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling 0 2 4 6 8 10 12 Number of degrees of freedom used for u interpolation in thickness direction Figure 7.19 Comparison of the convergence rate for the maximum warpage of a flat composite part on an aluminum tool separated by an interface layer using the layerwise and the hierarchical methods. The convergence rate is in terms of number of degrees of freedom used for the interpolation of u in the thickness direction 1.6 1.2 * 0.8 -Shear layer - 1 -Shear layer - 2 -Shear layer-3 - Full bonding 1.6 » 200 300 C„(MPa) 500 Shear layer- 1 Shear layer-2 Shear layer - 3 Full bonding 0.4 0.6 Figure 7.20 Variation of the actual and the normalized axial stress at a cross section in a flat composite part on an aluminum tool with shear layer properties. The stresses are normalized with the maximum stresses in each case. The shear layer properties are listed in Table 7.2 -263 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling 120 0 " I 1 1 . r — 1000 2000 3000 4000 5000 Number of degrees of freedom Figure 7.21 Variation of the run time with the number degrees of freedom used to model the composite flat part on an aluminum tool (full bonding) in the layerwise and the hierarchical methods A A A I I I I I I I I I I I I I 1 skin Core skin 2 mm 10 mm 2 mm 100 mm Figure 7.22 Schematic of a cantilever sandwich beam under uniform load - 2 6 4 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling -40 Distance along length (m) Z 0J32 0*4 * A A 01)6 . 0.08 0.1 * • A A A A \ * •» A A 2 - 20noded - 3 elements • Layerwise - h = 3 A Hierarchical - p= 2 • Hierarchical - p = 4 Hierarchical - p= 8 Figure 7.23 Comparison of the predicted vertical deflection profile of the sandwich beam under uniform load by the layerwise and the hierarchical methods. The sandwich beam is modelled with 3 element-layers (ft = 3) in the layerwise method Figure 7.24 The distribution of the axial displacement in the thickness direction at a cross section of a cantilever sandwich beam under uniform load -265 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling -0.1 0 0.1 0.2 0.3 0.4 0.5 0.6 Axial displacement (mm) Figure 7.25 Variation of axial displacement in the thickness direction of a quasi isotropic composite part on an aluminum tool and subjected to thermal load. The results from the layerwise and the hierarchical methods are compared 1 h6 - i H • [01 - f 1 2 ( —*- Layerwise (h = 8) —•— Hierarchical (p = 10) [90] [0] G 12 0.8 -o o : o.6-vs cu - J - e . 4 -[90[ [90] [0] [90] H 0.2 -e ^ - 1 i I —. Id i i =•—m -0.1 0 0.1 0.2 0.3 0.4 0.5 0.6 Axial displacement (mm) Figure 7.26 Variation of axial displacement in the thickness direction of a cross ply composite part on aluminum tool and subjected to thermal load. The results from the layerwise and the hierarchical methods are compared -266-Chapter 7: Higher Order Finite Element Techniques for Process Modelling 8 7H Jill Threshold 1.5- Threshold 1.0 c, c, c 3 c 4 c 6 c 7 CQ Cir C M Cis Ci-; Figure 7.27 The ratio of two successive coefficients of the exponential function that describes the through-thickness stress variation in a composite part. The threshold values for the hierarchical (1.5) and the layerwise (1.0) methods are shown Figure 7.2S Variation of the number of additional Legendre terms in the hierarchical method during the cure cycle to achieve the converged solution for the process-induced displacement of the composite flat part on an aluminum tool - 2 6 7 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling 200 0 -I 1 1 — ' 1 1 1 1 1 0 50 100 150 200 250 300 350 Time (min) Figure 7.29 Cure cycle separated into two time regimes: one requiring higher order terms and one without Figure 7.30 Variation of the run time with the number degrees of freedom used to model the composite flat part on an aluminum tool (full bonding) in the layerwise and the hierarchical methods (fixed and changing number of terms) - 2 6 8 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling Time (min) Figure 7.31 Typical 1-hold temperature and pressure cycles used for the experimental study A / Stick region • p Figure 7.32 ABAQUS basic Coulomb friction model with the maximum shear stress limit - 2 6 9 -Chapter 7: Higher Order Finite Element Techniques for Process Modelling Figure 7.33 Comparison of maximum warpage prediction by the layerwise element used in combination with contact surface in ABAQUS with experimental results by Twigg et al. (2004) -270-Chapter 8: Summary, Conclusions and Future Work Chapter 8. SUMMARY, CONCLUSIONS AND FUTURE W O R K 8.1. S U M M A R Y During the last two decades of research work in numerical modelling of autoclave processing of composite structures, several models have been developed ranging from simple one-dimensional elastic to sophisticated three dimensional viscoelastic models. Some of the common problems faced by these numerical models are the non-familiarity of general users with these models, their non-versatility, their inefficiency when running large problems and the interpretation and validation of the results produced by these models. In this work, 4 different numerical methodologies are developed to address the above problems: 1. Simple and robust closed-form solutions are developed to analyse the process-induced stresses and deformation of flat and curved composite parts. The closed-form solution serves many purposes: i . it provides a quick numerical tool to estimate the process-induced stresses and deformation of simple geometries i i . it is a robust mechanistic tool to better understand the physics of the processing problems and ii i . it can be used to validate the results from other complicated numerical models. 2. A simple methodology called "COMPRO Component Architecture (CCA)" was developed so that the evolving constitutive behaviour of the composite material of interest can be simply incorporated into any existing commercial finite element code. This will enable a general user to use any of the commercial finite element codes to perform process modelling while at the same time providing the user the other general features of the commercial code. -271 -Chapter 8: Summary, Conclusions and Future Work 3. Since the existing elements in commercial finite element codes do not have all the features necessary to model complicated composite part such as ply drop and varying layer thickness, a 24-noded isoparametric solid element is developed to addresses those issues. The element can be easily incorporated into any commercial finite element code. The element uses the simple reduced integration technique to overcome locking problems so that a shell-like structure can be modelled with fewer numbers of elements. This methodology enables us to model large complicated problems efficiently. 4. Even though the efficiency of modelling can be increased by the previous methodology, the modelling is hampered by the incapability of the developed element to capture the very sharp stress gradients through the thickness of the composite part. To address this problem, an adaptive finite element methodology is developed where the number of element layers or the order of the shape function in the thickness direction can be changed automatically (implicitly) depending on the geometrical and material properties of the composite part. This enables the modelling to be more efficient by reducing the set up time. 8.2. C O N C L U S I O N S The conclusions based on the work presented in this thesis are as follows: • A modular approach presented here, which is independent of the finite element solver, is well suited for process modelling rather than developing an entire process model from scratch. In this approach, the advanced features of well established commercial finite element codes can be fully utilized. • The well established surface finish classification of metallic auto body panels can also be applied to their composite counterparts. Different surface textures can be predicted by analysing the residual stresses that develop at different scale levels. The surface finish of a composite auto body part strongly depends on the fibre preform type used. Hence, when choosing a fibre preform - 2 7 2 -Chapter 8: Summary, Conclusions and Future Work type, in addition to the strength requirement, the surface finish requirement should also be considered. • The reduced integration technique is a very efficient method of overcoming the inherent locking problems so that solid elements can be used to model shell-like structures. Even though this methodology was well established two decades ago, it has been successfully applied only in the very recent past. • According to the closed-from solution, the axial stress variation in the thickness direction is an exponential function of both material and geometrical properties. • With appropriate modifications for part length and layer thickness, the interface layer approach can be used to simulate the experimentally observed tool-part interface condition successfully. The interface layer approach is about 2 times faster than the contact surface approach and is easy to characterize and implement. v t2 • A unique graph of "warpage number (WN = ~~^—)" v s - "shear layer number — / T (SLN = Gs =•—)" can be constructed for a particular tool-part material combination. This graph can be used as a design tool to study the variation of warpage with part length, part thickness, too material and tool-part interface conditions. • The process-induced unbalanced moment mainly develops at the initial stages of the curing process where the through-thickness stress gradient is very high. Hence, characterizing the initial resin modulus is crucial in predicting the experimentally observed trend in the variation of warpage with part length and part thickness. • The process-induced effects in a curved part due to the thermal strain mismatch between the part and the tool in the tangential direction is similar to the process-induced effects in a flat part. -273 -Chapter 8: Summary, Conclusions and Future Work • Apart from the tangential thermal strain mismatch, the radial thermal strain mismatch between the part and the tool also induce stresses in a curved part. The process-induced deformation due to the thermal strain mismatch in the radial direction can be estimated by considering only the cool-down portion of the cure cycle. • The layerwise element is more advantageous than the hierarchical element in terms of the run-time efficiency and representing the non-smooth displacement variation in the thickness direction. 8.3. F U T U R E W O R K The approach introduced in this thesis is only a stepping stone towards a fully robust process model. Despite the success of the proposed models in fulfilling the initial goals, improvements need to be made in order to expand the applicability of the approach. The recommendations for future work are: • The CCA modular approach should be implemented in other commercial finite element codes to further demonstrate its applicability. • Other techniques recommended in the literature for alleviating the locking problems should be tested and compared with the reduced integration technique. • A pre-processor for extruding the base surface mesh and assigning element and material properties should be developed. • More general closed-form solutions for geometries that involve a combination of flat and curved parts as well as spherical and double curvature geometries should be developed. • The adaptive hierarchical element developed here should be implemented in codes that allow the degrees of freedom to be changed dynamically. • Other types of error estimators such as energy norm should be studied to select the appropriate number of elements in the case of layerwise element and appropriate the number of terms in the case of hierarchical elements. -274 -Chapter 8: Summary, Conclusions and Future Work • More efficient numerical spatial integration techniques should be investigated to reduce the run-time when using the hierarchical element method. -275 -References R E F E R E N C E S ABAQUS, Version 6.4, ABAQUS Inc., 2003. Ahmed, S., Irons, B . M . and Zienkiewicz, O.C., "Analysis of Thick and Thin Shell Structures by Curved Finite Elements", International Journal for Numerical Methods in Engineering, Vol. 2, 1970, pp. 419-451. Albert, C , and Fernlund, G., "Spring-in and Warpage of Angled Composite Laminates", Composites Science and Technology, Vol. 62, No. 14, pp. 1895-1912, 2002. ANSI/ASME B46.1-1995, "Surface Texture (Surface Roughness, Waviness and Lay), American Society of Mechanical Engineers, 1995. Arafath, A.R.A, Vaziri, R. and Poursartip, A., "Thermo, Chemical and Mechanical Property Development of Glass Reinforced Polyester Material: Literature Review", First Interim Report, NCE Auto 21, 2002. Arciniega R.A. and Reddy, J.N., "Consistent Third-Order Shell Theory with Application to Composite Circular Cylinders", A I A A Journal, Vol. 43, No. 9, 2005, pp. 2024-2038. Areias, P.M.A., Cesar de Sa, J.M.A., Conceicao Antonio, C A . and Fernandes, A.A. , "Analysis of 3D Problems using a New Enhanced Strain Hexahedral Element", International Journal for Numerical Methods in Engineering, Vol. 58, No . , 2003, pp. 1637-1682. Ausserer, M.F., and Lee, S.W., "An Eighteen-Node Solid Element for Thin Shell Analysis", International Journal for Numerical Methods in Engineering, Vol. 26, No. , 1988, pp. 1345-1364. Azevedo, R.L., and Awruch, A . M . , "Geometric Nonlinear Dynamic Analysis of Plates and Shells Using Eight-Node Hexahedral Finite Elements with Reduced Integration", Journal of the Brazilian Society of Mechanical Sciences, Vol. 21, No. 3, 1999, pp. 446-462. Babuska, I., Griebel, M . and Pitkaranta, J., "The Problem of Selecting the Shape Functions for a p-Type Finite Element", International Journal for Numerical Methods in Engineering, Vol. 28, No. , pp. 1891-1908, 1989. - 2 7 6 -References Babuska, I., Szabo, B.A. and Actis, R.L., "Hierarchic Models for Laminated Composites", International Journal for Numerical Methods in Engineering, Vol. 33, No. 3, pp. 503-535, 1992. Babuska, I., and Suri, M . , "The p and hp Version of the Finite Element Method, Basic Principles and Properties", SIAM Review, Vol. 36, No. 4, pp. 578-632, 1994. Bathe, K. J., "Finite Element Procedures", Prentice Hall, Englewood Cliffs (USA), 1996. Belytschko, T., Liu, W. K., and Moran, B., "Nonlinear finite elements for continua and structures ", Wiley, New York, 2004. Bhaskar, K. and Varadan, T.K., "Refinement of higher-order laminated plate theories", AIAA Journal, Vol. 27, No. 12, 1989, pp. 1830-1831. Bigwood, D.A. and Crocombe, A.D., "Elastic Analysis and Engineering Design Formulae for Bonded Joints", International Journal of Adhesion and Adhesives, Vol. 9, No. 4, pp. 229-242, 1989. Bogdanovich,A.E. and Pastore,C.M., "Mechanics of Textile and Laminated Composites", 1996. Bogetti,T.A. and Gillespie Jr,J.W., "Two-Dimensional Cure Simulation of Thick Thermosetting Composites", Journal of Composite Materials, Vol. 25, No. 3, pp. 239-273, 1991. Bogetti,T.A. and Gillespie Jr,J.W., "Process-Induced Sterss and Deformation in Thick-Section Thermoset Composite Laminates", Journal of Composite Materials, Vol. 26, No. 5, pp. 626-660, 1992. Buchter, N . , Ramm, E. and Roehl, D., "Three-Dimensional Extension of Non-Linear Shell Formulation based on the Enhanced Assume Strain Concept", International Journal for Numerical Methods in Engineering, Vol. 37, No. 15, pp. 2551-2568, 1994. Carrera, E., "Historical Review of Zig-Zag Theories for Multilayered Plates and Shells", Applied Mechanics Reviews, Vol. 56, No. 3, pp. 287-308, 2003. Chen, D., Cheng, S., Geerhardt, T.D., "Thermal stresses in laminated beams", Journal of Thermal Stresses, Vol. 5, No. 1, pp. 67-84, 1982. -277-References Chen, P.C. and Ramkumar, R.L., "RAMPC - An Integrated Three-dimensional Design Tool for Processing Composites", 33rd International SAMPE Symposium, Anaheim, CA, 7-10 March, 1988, pp. 1697-1708. Chen, W.T. and Nelson, C.W., "Thermal stresses in Bonded Joints", IBM Journal of Research and Development, Vol. 23, No. 2, pp. 179-188, 1979. Di Sciuva, M . , "An Improved Shear-Deformation Theory for Moderately Thick Multilayered Anisotropic Shells and Plates", Journal of Applied Mechanics, Vol. 23, pp. 589-596, 1987 Dhondt, G.D., "The Right Solid Element: a Challenge to Industry", Proceeding of the Fifth World Congress on Computational Mechanics (WCCM V), Vienna, Austria, 2002. Doll, S., Schweizerhof, K., Hauptmann, R. and Freischlager, C , "On Volumetric Locking of Low-Order Solid and Solid-Shell Elements for Finite Elastoviscoplastic Deformations and Selective Reduced Integration", Engineering Computations, Vol. 17, No. 7, 2000, pp. 874-902. Duster, A., Broker, H. and Rank, E., "The p-Version of the Finite Element Method for Three-Dimensional Curved Thin Walled Structures", International Journal for Numerical Methods in Engineering, Vol. 52, No., pp. 673-703,2001. Ersoy, N . , Potter, K., Wisnom, M.R. et al., "An Experimental Method to Study the Frictional Processes during Composite Manufacturing", Composites Part A , Vol. 36, No. 11, pp. 1536-1544, 2005. Fernlund, G., Osooly, A., Poursartip, A. et al., "Finite element based prediction of process-induced deformation of autoclaved composite structures using 2D process analysis and 3D structural analysis", Composite Structures Vol. 62, No. 2, pp. 223-234, 2003. Fibersim, VISTAGY, Inc., Waltham, M A , USA, 2001 - 2 7 8 -References Ganesh,V.K. and Naik,N.K., "Failure Behavior of Plain Weave Fabric Laminates Under On-Axis Uniaxial Tensile Loading: I - Laminate Geometry", Journal of Composite Materials, Vol. 30, No. 16, 1996, pp. 1748-1778. Ghorbani, H.R., and Spelt, J.K., "Interfacial Thermal Stresses in Trilayer Assembly", Journal of Electronic Packaging, Vol. 127, No. 3, pp. 314-323, 2005. Ghugal, Y . M . , and Shimpi, R.P., "A Review of Refined Shear Deformation Theories of Isotropic and Anisotropic Laminated Plates", Journal of Reinforced Plastics and Composites, Vol. 21, No. 9, 2002, pp. 775-813. Hahn,H.T. and Pagano,N.J., "Curing Stresses in Composite Laminates", Journal of Composite Materials, Vol. 9, No. 1, pp. 91-106, 1975. Hashin,Z. and Rosen,B.W., "The Elastic Moduli of Fiber-Reinforced Materials", Journal of Applied Mechanics, Vol. 31, pp. 223-232, 1964. Hauptmann, R., and Schweizerhof, K., "A Systematic Development of Solid-Shell Element Formulations for Linear and Non-linear Analysis Employing only Displacement Degrees of Freedom", International Journal for Numerical Methods in Engineering, Vol. 42, No. 1, 1998, pp. 49-69. Hinnant, H.E., "A Fast Method of Numerical Quadrature for p-Version Finite Element Matrices", International Journal for Numerical Methods in Engineering, Vol. 37, No . , pp. 3723-3750, 1994. Hsueh, C.H. and Lee, S., "Modelling Elastic Thermal Stresses in Two materials Joined by a Graded Layer", Composites: Part B - Engineering, Vol. 34, No. 8, pp. 747-752, 2003. Hubert, P., "Aspects of Flow and Compaction of Laminated Composite Shapes during Cure", PhD Thesis, The University of British Columbia, Vancouver, Canada, 1996. - 2 7 9 -References Hubert, P., Vaziri, R. and Poursartip, A . , " A Two-Dimensional Flow Model for the Process Simulation of Complex Shape Composite Laminates", International Journal for Numerical Methods in Engineering, Vol. 44, No. 1, 1999, pp. 1-26. Hughes, T. J. R., "The Finite Element Method", Prentice Hall, Englewood Cliffs (USA), 1987. Hull,D., "An Introduction to Composite Materials", Cambridge University Press, 1981. Hypermesh, Version 6.0, Altair Engineering, Troy MI, USA, 2004. Ishikawa,T. and Chou,T.W., "Elastic Behavior of Woven Hybrid Composites", Journal of Composite Materials, Vol. 16, No. 1, 1982a, pp. 2-19. Ishikawa,T. and Chou,T.W., "Stiffness and Strength Behaviour of Woven Fabric Composites", Journal of Materials Science, Vol. 17, 1982b, pp. 3211-3220. Johnston,A.A., "An Integrated Model of the Development of Process-Induced Deformation in Autoclave", PhD Thesis, The University of British Columbia, Vancouver, Canada, 1997. Johnston,A.A., Vaziri,R. and Poursartip,A., "A Plane Strain Model for Process-Induced Deformation of Laminated Composite Structures", Journal of Composite Materials, Vol. 35, No. 16, pp. 1435-1469, 2001. Karpala,F., "TPS-LORIA Correlation of Surafce Waviness", 48th Annual Conference and Exposition of SPI, Composite Institute., 1993, pp. 20A: 1-6. Kia,H.G., "Modeling Surface Deformation of Glass Fiber Reinforced Composites", 41st Annual Conference , Reinforced Plastics/Composites Institute, January 27-31, 1986b. Kia,H.G., "Modeling Surface Deformation of Glass Fiber Reinforced Composites", Journal of Composite Materials, Vol. 20, No. 4, 1986a, pp. 335-346. Kia,H.G., "The Effect of Resin Formulation on the Surface Appearence of Glass Fiber Reinforced Polymers", Journal of Composite Materials, Vol. 21, No. 12, 1987, pp. 1145-1163. - 2 8 0 -References Kim, Y.H. , and Lee, S.W., "A Solid Element Formulation for Large Deflection Analysis of Composite Shell Structures", Computers and Structures, Vol. 30, No. 1/2, 1988, pp. 269-274. Kim,Y.K. and White,S.R., "Stress Relaxation Behaviour of 3501-6 Epoxy Resin During Cure", Polymer Engineering and Science, Vol. 36, No. 23, pp. 2852-2862, 1996. Kim,P.J. and Lee,D.G., "Surface Quality and Shrinkage of the Composite Bus Housing Panel Manufactured by RTM", Composite Structures, Vol. 57, No. 1-4, pp. 211-220, 2002. Kratzig, W.B. and Jun, D., "On Best Shell Models - From Classical Shells, Degenerated and Multi-Layered Concepts in 3D", Archive of Applied Mechanics, Vol. 73, 2003, pp. 1-25. Kuhlmann, G., and Rolfes, R., "A Hierarchic 3D Finite Element for Laminated Composites", International Journal for Numerical Methods in Engineering, Vol. 61, No. 1, pp. 96-116, 2004. Kuhn,J.L. and Charalambides,P.G., "Elastic Response of Porous Matrix Plain Weave Fabric Composites: Part I - Modeling", Journal of Composite Materials, Vol. 32, No. 16, 1998a, pp. 1426-1471. Kuhn,J.L. and Charalambides,P.G., "Elastic Response of Porous Matrix Plain Weave Fabric Composites: Part II - Results", Journal of Composite Materials, Vol. 32, No. 16, 1998b, pp. 1472-1507. Kuhn,J.L. and Charalambides,P.G., "Modeling of Plain Weave Fabric Composite Geometry", Journal of Composite Materials, Vol. 33, No. 3, 1999, pp. 188-220. Kuhn,J.L., Haan,S.I. and Charalambides,P.G., "A Semi-Analytical Method for the Calculation of the Elastic Micro-Fields in Plain Weave Composites Subjected to In-Plane Loading", Journal of Composite Materials, Vol. 33, No. 3, 1999, pp. 221-266. Landsettle,G.A. and Jensen,J.C., "Factors That Affects Class A Surface Quality", 41st Annual Conference of SPI, Composites Institute, 1986, pp. 18B: 1-6. LCMFlot, ESI Group, Paris, France, 2001. -281 -References Loos, A.C. and Springer, G.S., "Curing of Epoxy Matrix Composites", Journal of Composite Materials, Vol. 17, No. 2, pp. 135-169, 1983. MacNeal, R.H., "Finite Elements: Their Design and Performance", Marcel Dekker, New York, 1994. McCarteney, L .N. , "Analytical Models of Stress Transfer in Unidirectional Composites and Cross-ply Laminates and their Application to the Prediction of Matrix/Transverse Cracking", IUTAM Symposium on Local Mechanics Concepts for Composite Material Systems, Blacksburg, V A , pp. 251-282, 1991. Moorthy, C.M.D. and Reddy, J.N., "Modelling of Laminates using a Layerwise Element with Enhanced Strains", International Journal for Numerical Methods in Engineering, Vol. 43, No . , pp. 755-779, 1998. MSC M A R C 2005, MSC Software Corporation, Santa Ana, CA, USA, 2005. MSC Patran 2005, MSC Software Corporation, Santa Ana, CA, USA, 2005. Naik,N.K. and Ganesh,V.K., "An Analytical Method for Plain Weave Fabric Composites", Composites, Vol. 26, No. 4, 1995, pp. 281-289. Naik,N.K. and Shembekar,P.S., "Elastic Behavior of Woven Fabric Composites: I - Lamina Analysis", Journal of Composite Materials, Vol. 26, No. 15, 1992, pp. 2196-2225. Neitzel,M., Blinzler,M., Edelmann,K. and Hoecker,F., "Surface Quality Characterization of Textile-Reinforced Thermoplastics", Polymer Composites, Vol. 21, No. 4, 2000, pp. 630-635. Nelson,R.H. and Cairns,D.S., "Prediction of Dimensional Changes in Composite Laminates During Cure", Proceedings of Tomorrow's Materials: Today. Society for the Advancement of Material and Process Engineering, 1989, pp. 2379-2410. Nubel, V., Duster, A . and Rank, E., "Adaptive Vector Integration as an Efficient Quadrature Scheme for p-Version Finite Element Matrices", ECCM-2001: European Conference on Computational Mechanics, Cracow, Poland, 2001. - 2 8 2 -References Osooly, A. , " Contact Formulation at Tool-Part Interface and Large Strain/Deformation Corotational Stress Based Constitutive Equation in Thermoset Ccomposites during Autoclave Processing ", PhD Thesis, The University of British Columbia, Vancouver, Canada, In progress. Park, H.C., Cho, C. and Lee, S.W., "An efficient assumed strain element model with six DOF per node for geometrically nonlinear shells", International Journal for Numerical Methods in Engineering, Vol. 38, No. 24, pp. 4101-4122, 1995. Petchsasithon, A., and Gosling, P.D., "A Locking-Free Hexahedral Element for the geometrically Non-Linear Analysis of Arbitary shells", Computational Mechanics, Vol. 35, No. 2, pp. 94-114, 2005. Petrescue, L., "Detemination of Warpage in Autoclaved-Cured Composite Laminates", Internal Report, Composites Group, The University of British Columbia, June 2005. Prathap, G., and Bhashyam, G.R., "Reduced Integration and the Shear-Flexible Beam Element", International Journal for Numerical Methods in Engineering, Vol. 18, No. 1, pp. 195-210, 1982. Prathap, G., "The Finite Element Method in Structural Engineering", Kluwer Academic, Dordrecht , Boston, 1993. Rank, E., Duster, A., Nubel, V., Perusch, K. and Bruhns, O.T., "High Order Finite Elements for Shells", Computer Method in Applied Mechanics and Engineering, Vol. 194, No . , pp. 2494-2512, 2005. Rao, N . , "Surface Requirement Factors in Process Selection", In: Engineered Materials Handbook: Engineering Plastics, eds. C.A.Dostal, M.S.Woods and H.J.Frissell, A S M International, USA, pp. 302-307,1988. Rasekh, A., "Efficient Methods for Non-Linear Thermochemical Analysis of Composite Structures Undergoing Autoclave Processing", PhD Thesis, The University of British Columbia, Vancouver, Canada, In progress. -283 -References Reddy, J.N., "Mechanics of Laminated Composite Plates and Shells: Theory and Analysis", CRC Press, Boca Raton, 2004. Robbins, D.H., and Reddy, J.N., "Modelling of Thick Composites using a Layerwise Laminate Theory", International Journal for Numerical Methods in Engineering, Vol. 36, No. 2, 1993, pp. 655-677. Robinson, J., "An Introduction to Hierarchical Displacement Elements and the Adaptive Technique", Finite Element Analysis and Design, Vol. 2, No. , pp. 377-388, 1986. Rosettos, J.N. and Shen, X. , "On the Axial and Interfacial Shear Stresses due to Thermal Mismatch in Hybrid Composite Sheets", Composites Science and Technology, Vol. 54, No. 4, pp. 417-422, 1995. Ru, C.Q., "Interfacial Thermal Stresses in Bimaterial Elastic Beams: Modified Beam Models Revisited", Journal of Electronic Packaging, Vol. 124, No. 3, pp. 141-146, 2002. Sanfeliz,J.G., Murthy,P.L.N. and Chamis,C.C, "Computational Simulation of Surface Waviness in Graphite/Epoxy Woven Composites Due to Initial Curing", 37th International SAMPE Symposium and Exhibition, Anaheim, CA, March 9-12, 1992, pp. 1325-1333. Sheikh, A.H. , and Chakrabarti, A., "A New Plate Bending Element Based on Higher-Order Shear Deformation Theory for the Analysis of Composite Plates", Finite Element Analysis and Design, Vol. 39, No. , 2003, pp. 883-903. Stolarski, H., and Belytschko, T., "Membrane Locking and Reduced Integration for Curved Elements", Journal of Applied Mechanics, Vol. 49, No. l , 1982, pp. 172-179. Stolarski, H., and Belytschko, T., "Shear and Membrane Locking in Curved CO Elements", Computer Methods in Applied Mechanics and Engineering, Vol. 41, No. , 1983, pp. 279-296. Suhir, E., "Stresses in bi-metal thermostats", Journal of Applied Mechanics, Vol. 53, No. 3, pp. 657-660, 1986. - 2 8 4 -References Suhir, E., "Interfacial stresses in bimetal thermostats", Journal of Applied Mechanics, Vol. 56, No. 3, pp. 595-600, 1989. Suri, M . , "Analytical and Computational Assessment of Locking in the hp Finite Elements Method", Computer Method in Applied Mechanics and Engineering, Vol. 133, No. 1, pp. 347-371, 1996. Svanberg,J.M. and Holmberg,J.A., "An Experimental Investigation on Mechanisms for Manufacturing Induced Shape Distortions in Homogeneous and Balanced Laminates", Composites: Part A , Vol. 32, No. 6, 2001, pp. 827-838. Szabo, B.A., "Implementation of a Finite Element Software System with h and p Extension Capabilities", Finite Elements in Analysis and Design, Vol. 2, No. 1-2, pp. 177-194, 1986. Szabo, B.A., "The p- and hp Version of the Finite Element Method in Solid Mechanics", Computer Method in Applied Mechanics and Engineering, Vol. 80, No. 1, pp. 185-195, 1990. Sze, K .Y . , "Three-Dimensional Continuum Finite Element Models for Plate/Shell Analysis", Progress in Structural Engineering and Materials, Vol. 4, No. 4, 2002, pp. 400-407. Sze, K.Y. , Lo, S.H. and Yao, L.Q., "Hybrid-Stress Solid Elements for Shell Structures based upon Modified Variational Functional", International Journal for Numerical Methods in Engineering, Vol. 53, No. 12, 2002, pp. 2617-2642. Tahani, M . and Nosier, A. , "Free Edge Stress of General Cross-Ply Composite Laminates under Extension and Thermal Loading", Composite Structures, Vol. 60, No. 1, pp. 91-103, 2003. Timoshenko, S.P., "Analysis of bi-metal thermostats", Journal Optical Society of America, Vol. 11, pp. 233-255, 1925. Tsai, M.Y. , Hsu, C.H., and Han, C.N., "A Note on Suhir's Solution of Thermal Stresses for a Die-Substrate Assembly", Journal of Electronic Packaging, Vol. 126, No. 1, pp. 115-119, 2004. -285 -References Twigg, G., Poursartip, A. , Fernlund, G., "An experimental method for quantifying tool-part shear interaction during composites processing", Composites Science and Technology, Vol. 63, No. 13, pp. 1985-2002 2003. Twigg, G., Poursartip, A., Fernlund, G., "Tool-Part Interaction in Composites Processing. Part I: Experimental Investigation and Analytical Model", Composites: Part A , Vol. 35, No. 1, 2004, pp. 121-133 2004a. Twigg, G., Poursartip, A. , Fernlund, G., "Tool-Part Interaction in Composites Processing. Part II: Numerical Modelling", Composites: Part A, Vol. 35, No. 1, 2004, pp. 135-141 2004b. Wagner, M . M . , "On Efficient Integration of p-Version Finite Element Stiffness Matrices", Internal Report No: 4, Universitt der Bundeswehr Munchen, Germany, 2003. Wang, K.P., Huang, Y . Y . , Chandra, A . and Hu, K.X. , "Interfacial Shear Stress, Peeling Stress, and Die Cracking Stress in Trilayer Electronic Assemblies", IEEE Transactions on Components and Packaging Technologies, Vol. 23, No. 2, pp. 309-316, 2000. Wang, W.C. and Hsu, J.S., "Re-Examination on Thermal Stresses of Bonded Structures", The Journal of Strain Analysis for Engineering Design, Vol. 39, No. 3, pp. 261-270, 2004. Wen, Y . and Basaran, C , "An Analytical Model for Thermal Stress Analysis of Multi-Layered Microelectronic Packaging", Mechanics of Materials, Vol. 36, No. 4, pp. 369-385, 2004. White,S.R. and Hahn,H.T., "Process Modeling of Composite Materials: Residual Stress Development During Cure. Part I. Model Formulation", Journal of Composite Materials, Vol. 26, No. 16, pp. 2402-2422, 1992. White,S.R. and Hahn,H.T., "Process Modeling of Composite Materials: Residual Stress Development During Cure. Part II. Experimental Validation", Journal of Composite Materials, Vol. 26, No. 16, pp. 2423-2453, 1992. - 2 8 6 -References Wiberg, N.E., Moller, P., and Samuelsson, A., "Use of Trignometric Functions for Hierarchical Improvement of Finite Element Solutions of 2D Static Elastic Problems", NUMETA 85: Proceeding of the International Conference on Numerical Methods in Engineering, Theory and Applications, Swansea, pp. 77-86, 1985. Wiberg, N . and Moller, P., "Formulation and Solution of Hierarchical Finite Element Equations", Internationa] Journal for Numerical Methods in Engineering, Vol. 26, No . , pp. 1213-1233, 1988. Yang, H.T.Y., Saigal, S., Masud, A. and Kapania R.K., "A Survey of Recent Shell Finite Elements", International Journal for Numerical Methods in Engineering, Vol. 47, No. 1, 2000, pp. 101-127. Zak,G., Haberer,M., Park,C.B. and Benhabib,B., "Estimation of Average Fibre Length in Short-Fibre Composites by Two-Section Method", Composites Science and Technology, Vol. 60, 2000, pp. 1763-1772. Zak,G., Park,C.B. and Benhabib,B., "Estimation of Three-Dimensional Fibre-Orientation Distribution in Short-Fibre Composites by a Two-Section Method", Journal of Composite Materials, Vol. 35, No. 4, 2001, pp. 316-339. Zhou, X . , Chattopadhyay, A. and Kim, H.S., "An Efficient Layerwise Shear-Deformation Theory and Finite Element Implementation", Journal of Reinforced Plastics and Composites, Vol. 23, No. 2, pp. 131-152,2004. Zhu, J.Z. and Zienkiewicz, O.C., "Adaptive Techniques in the Finite Element Method", Communication in Applied Numerical Methods, Vol. 4, No. 1, pp. 197-204, 1988. Zhu,Q., Geubelle,P.H., L i , M . , et al, "Dimensional Accuracy of Thermoset Composites: Simulation of Process-Induced Residual Stresses", Journal of Composite Materials, Vol. 35, No.24, pp. 2171-2205, 2001. - 2 8 7 -References Zienkiewicz, O.C., Taylor, R.L., and Too, J.M., "Reduced Integration Technique in General Analysis of Plates and Shells", International Journal for Numerical Methods in Engineering, Vol. 3, No. 1, 1971, pp. 275-290. Zienkiewicz, O.C., Gago, J.P. De S.R. and Kelly, D.W., "The Hierarchical Concept in Finite Element Analysis", Computers and Structures, Vol. 16, No. 1-4, pp. 53-65, 1983. Zienkiewicz, O.C. and Taylor, R.L., "The Finite Element Method", Butterworth-Heinemann, London, 2000. Zobeiry,N., Vaziri,R., and Poursartip,A., "An Efficient Pseudo-Viscoelastic Model for Evaluation of Residual Stresses in Thermoset Composites during Cure", Composites: Part A, submitted. Zobeiry,N., Vaziri,R., and Poursartip,A., "Differential Implementation of the Viscoelastic Response of a Curing Thermoset Matrix for Composites Processing", A S M E Journal of Engineering Materials and Technology, Vol. 128, No. 1, pp. 90-95, 2006. - 2 8 8 -Appendix A: CCA Module for the ASS4/8552 Material Appendix A. CCA M O D U L E FOR T H E ASS4/8552 M A T E R I A L Thermo-Chemical Module In this section, the following material properties are determined: • Fibre Volume Fraction and Density • Thermal Conductivity • Specific Heat • Resin Cure Kinetics Density Resin: Pr = PrO+arp(T-To)+brp(<X-a0) ( A Fibre: Pf=P/o +afp(T-T0) Parameters Description Value Units Vf Fibre volume fraction 0.573 Resin PrO Initial density of resin 1790.0 kg/m3 arp Temperature constant of resin 0 kg/(m3*°C) To Initial temperature 20.0 °C brp Degree of cure constant of resin 0 kg/m3 Initial degree of cure 0 Fibre P/o Initial density of fibre 1300.0 kg/m3 afP Temperature constant of fibre 0 kg/(m 3*°C) To Initial temperature 20.0 °C - 2 8 9 -Appendix A: CCA Module for theASS4/8552 Material Specific Heat Capacity Resin: Cpr = CprO + aCr (T ~ T0)+bCr (« - «0 ) Fibre: Cpf =Cpfo+ac/(T-To) Parameters Description Value Units Resin CprO Initial specific capacity of resin 904.0 J/kgK <*Cr Temperature constant of resin 2.05 J/kgK2 bCr Degree of cure constant of resin 0 J/kgK To Initial temperature 75.0 °C a0 Initial degree of cure 0 -Fibre CprO Initial specific capacity of resin 1005.0 J/kgK aCf Temperature constant of fibre 3.74 J/kgK2 T0 Initial temperature 20.0 °C Thermal Conductivity Resin: kr=kr0+akr(T-T0)+bkr(a-a0) Fibre: (A.3) ^11/ = ^11/0 + ak\\f (T ~ T0 ) ^22/ ~ ^33/ = ^33/0 + ak2if(T ~T0) - 2 9 0 -Appendix A: CCA Module for the ASS4/8552 Material Parameters Description Value Units Resin krO Initial thermal conductivity of resin 0.148 W/m°C akr Temperature constant of resin 3.43E-4 W/m°C2 bkr Degree of cure constant of resin 6.07E-2 W/m°C To Initial temperature of resin 0 °C a0 Initial degree of cure 0 Fibre ^ l l / O Initial longitudinal thermal conductivity of fibre 7.690 W/m°C ak\\f Temperature constant of fibre 1.56E-2 W/m°C2 ^33/0 Initial transverse thermal conductivity of fibre 2.40 W/m°C ° * 3 3 / Temperature constant of fibre 5.07E-3 W/m°C2 To Initial temperature of fibre 0 °C Resin Cure Kinetics COMPRO resin cure kinetics model 6 is used for resin: da _ Kam(\-a)n dt ~ \ + ecia-(aco+"crT)} (A.4) Variable Description Values Units a Resin degree of cure. -T Resin Temperature °C Total resin heat of reaction (a - 0 to 1) 5.40E5 J/kg 4 Pre-exponential factor. 1.528E5 Is AE, Activation energy. 6.65E4 J/mol m Equation superscript. 0.8129 -n Equation superscript. 2.736 -R Gas Constant 8.3143 J/(mol K ) C Diffusion constant 43.09 -aco Diffusion constant -1.684 -aCT Diffusion constant 5.475E-3 /°C -291 -Appendix A: CCA Module for the ASS4/8552 Material STRESS MODULE In this section, the following material properties are determined: • Thermal Expansion • Resin Cure Shrinkage • Resin Modulus • Resin Poisson's Ratio • Elastic Properties Thermal Expansion Resin CTE: CTE, = CTEr0 +ar(T-T0) + br(a-a0) (A.5) Fibre CTE: CTE/L=CTEJL0+aJL(T-T0) CTEp- — CTE+ a /j (T — T0) Parameters Description Value Units Resin CTER0 Initial resin coefficient of thermal expansion 144.0 ft/°C ar Constant 0 p./°C2 K Constant -72.0 p.l°C Initial resin degree of cure 0 To Initial temperature 0 °c Fibre CTEJLO Initial fibre longitudinal C T E 0.03 p./°C Constant 0 p./°C2 CTEJTQ Initial fibre transverse C T E 7.20 pl°C afT Constant 0 p.l°C2 - 2 9 2 -Appendix A: CCA Module for the ASS4/8552 Material Resin Cure Shrinkage V? =0.0 a < a c i Vrs =Aas+(vrs"-A}z2s aC]<a<aC2 Vrs=Vrs™ a>aC2 (A.7) a-a c\ aC2 -a c i Variable Description Values Units Vs Resin volumetric cure shrinkage -r Total volumetric resin shrinkage from a>= 0 to 1. 0.099 -The 'cure shrinkage' degree of cure. -ac\ Degree of cure after which the resin shrinkage begins. 0.055 -aC2 Degree of cure after which the resin shrinkage stops. 0.670 -A Linear cure shrinkage coefficient 0.173 -Resin Modulus Er=E°r T*<T*CX E'r = E? T > TC2 (A.8) Er=E'r[\ + aEr(T-T0)] where -J* = (Tga + Tgb * a) - T;T*CX = T*CXa + Tc\b * T -293 -Appendix A: CCA Module for the ASS4/8552 Material Variable Description Values Units a The resin degree of cure -E« The resin elastic modulus at very low degrees of cure 4.67E6 Pa E™ The resin elastic modulus at To and a = 1.0 4.67E9 Pa T Resin temperature °C r Difference between resin temperature and resin instantaneous T g °C Glass transition temperature at a = 0 2.68E2 K Factor expressing the degree of cure dependence of resin glass transition temperature 2.20E2 K Tela T* above which resin modulus begins to increase at T = O K -45.7 K Tcib Factor expressing the temperature dependence of the T above which resin modulus begins to increase 0.00 -T* above which resin modulus has reached its full value -12 K T0 Resin modulus development reference temperature 20 °C aEr Factor expressing the temperature dependence of resin modulus 0.00 Pa/°C Resin Poisson's Ratio (A.9) Variable Description Values Units Resin Poisson's ratio -Er Resin elastic modulus Pa E? Resin elastic modulus at a = 1.0 4.67 GPa r Resin Poisson's ratio at a = 1.0 0.37 - 2 9 4 -Appendix A: CCA Module for theASS4/8552 Material Fibre Elastic Properties En = ^11(0) +aE\\V^- -T0) ~ ^33(0) + ° £ 3 3 ft -T0) " l3 = V\3(0) +avn(T- To) 2^3 = V23(0) +^vlAT-T0) G 1 3 = ^13(0) + aG\3V^ -To) Parameters Description Value Units E\ i(o) Initial fibre longitudinal modulus 210 GPa •£33(0) Initial fibre transverse modulus 17.24 GPa ^23(0) Initial fibre in-plane shear modulus 27.6 GPa v23(0) Initial fibre major Poisson's ratio 0.2 ^12(0) Initial fibre minor Poisson's ratio 0.25 Temperature constant 0 Pa/K °£33 Temperature constant 0 Pa/K avl3 Temperature constant 0 / K av23 Temperature constant 0 / K aG\3 Temperature constant 0 Pa/K To Reference temperature 0 °C -295 -Appendix B: CCA Module for the Glass Fibre Reinforced Polyester Material Appendix B. CCA M O D U L E FOR T H E GLASS FIBRE REINFORCED POLYESTER MATERIAL Thermo-Chemical Module In this section, the following material properties are determined: • Fibre Volume Fraction and Density • Thermal Conductivity • Specific Heat • Resin Cure Kinetics Density The 'lumped' density model for the composite is given by: p = p{0)+ap{T-T0) + bp(a-a0) (B.l) Parameters Description Value Units Vf Fibre volume fraction 0.54 Initial density of composite 1.89E3 kg/m 3 Constant 0 kg/(m 3*°C) To Initial temperature 0 °C K Constant 0 kg/m3 a0 Initial degree of cure 0 Specific Heat Capacity The 'lumped' specific heat capacity model for the composite is given by: C = C(0)+ac(T-T0) + bc(a-a0) (B.l) - 2 9 6 -Appendix B: CCA Module for the Glass Fibre Reinforced Polyester Material Parameters Description Value Units Co Initial specific capacity of composite 1260 J/kgK ac Constant 0 J/kgK2 be Constant 0 J/kgK To Initial temperature 0 °C a0 Initial degree of cure 0 -Thermal Conductivity The 'lumped' thermal conductivity model for the composite is given by: ku = K m + a k n { T - T o ) + bkn{a-aQ) k22 = k33 — &33(0) + a A33 (T — T0) + bk33 (ct — a0) Parameters Description Value Units 1^1(0) Initial longitudinal thermal conductivity 0.4272 W/m°C Constant 0 W/m°C 2 h\\ Constant 0 W/m°C ^33(0) Initial transverse thermal conductivity 0.2163 W/m°C a A 3 3 Constant 0 W/m°C2 ^ 3 3 Constant 0 W/m°C To Initial temperature 0 °C a0 Initial degree of cure 0 Resin Cure Kinetics COMPRO resin cure kinetics model 2 is used for Polyester: da kam(\-a)n dt ( B . 4 ) - 2 9 7 -Appendix B: CCA Module for the Glass Fibre Reinforced Polyester Material Parameters Description Value Units A Pre-exponential factor 6.17E20 Is AE Activation energy 1.674E5 J/mol m Constant 0.524 n Constant 1.476 HR Total resin heat of reaction 77500 J/kg STRESS MODULE In this section, the following material properties are determined: • Thermal Expansion • Resin Cure Shrinkage • Resin Modulus • Resin Poisson's Ratio • Elastic Properties Thermal Expansion Resin CTE: CTEr = CTEr0 +ar(T-T0) + b,(a-a0) (B.5) Fibre CTE: CTE^^CTE^+a^T-T,) ^ CTEfj. =CTEfro+afr{T-T0) - 2 9 8 -Appendix B: CCA Module for the Glass Fibre Reinforced Polyester Material Parameters Description Value Units Resin CTER0 Initial resin coefficient of thermal expansion 72.0 pl°C ar Constant 0 ft/ °C2 K Constant 0.0 fi/°C a0 Initial resin degree of cure 0 To Initial temperature 0 °C Fibre CTEJLO Initial fibre longitudinal C T E 5.04 ft/°C Constant 0 fi/°C2 CTEJJQ Initial fibre transverse C T E 5.04 fi/°C Constant 0 /u/°C2 Resin Cure Shrinkage KH = A x ash +(VshT -A)x a s h 2 acX < a < ac2 Vsh=VshJ cc>ac2 (B.7) Parameters Description Value Units Total volumetric resin cure shrinkage 0.06 A Linear cure shrinkage coefficient 0.06 <*c\ Degree of cure after which the resin shrinkage begins 0 aC2 Degree of cure after which the resin shrinkage stops 1.0 - 2 9 9 -Appendix B: CCA Module for the Glass Fibre Reinforced Polyester Material Resin Modulus E = (l - « m o d )E° + «mod EX+ r « m o d 0 - «mod )(E E = EX Emod=E{l + aErT) where amod =(a- acx )/(aC2 - acx) Parameters Description Value Units Initial resin elastic modulus 27.57 M P a E" Elastic modulus of fully cured resin 27.57 GPa r Resin hardening rate factor 0 «C1 Degree of cure above which the resin modulus begins to increase 0 aC2 Degree of cure at which the resin modulus reaches full value 1.0 T Reference temperature 0 °C Temperature constant 0 /°C Resin Poisson's Ratio v r = v r 0 + a „ r ( r - r 0 ) + M a - a 0 ) ( B l 9 ) Parameters Description Value Units T Reference temperature 0 °C °vr Temperature constant 0 / °C Kr Degree of cure constant 0 /°c Vr0 Initial resin Poisson's ratio 0.40 a <a, c i -E ) acx <a < a, lC2 a> a C2 (B .8) -300 -Appendix B: CCA Module for the Glass Fibre Reinforced Polyester Material Fibre Elastic Properties — ^11(0 ) +aE\\^J' ' F £,33 = ^33 (0 ) + aE33 "13 ^o) ^23 = ^23(0) + av23(T ~ •To) G 1 3 = ^ 1 3 ( 0 ) + a G 1 3 -To) Parameters Description Value Units -^ 11(0) Initial fibre longitudinal modulus 73.08 GPa £33(0) Initial fibre transverse modulus 73.08 GPa ^23(0) Initial fibre in-plane shear modulus 29.92 GPa V23(0) Initial fibre major Poisson's ratio 0.22 V\2(0) Initial fibre minor Poisson's ratio 0.22 aE\l Temperature constant 0 Pa/°C aE33 Temperature constant 0 Pa/°C av\3 Temperature constant 0 /°C av23 Temperature constant 0 /°C aG\3 Temperature constant 0 Pa/°C To Reference temperature 0 °C -301 -
- Library Home /
- Search Collections /
- Open Collections /
- Browse Collections /
- UBC Theses and Dissertations /
- Efficient numerical techniques for predicting process-induced...
Open Collections
UBC Theses and Dissertations
Featured Collection
UBC Theses and Dissertations
Efficient numerical techniques for predicting process-induced stresses and deformations in composite… Arafath, Abdul Rahim Ahamed 2007
pdf
Notice for Google Chrome users:
If you are having trouble viewing or searching the PDF with Google Chrome, please download it here instead.
If you are having trouble viewing or searching the PDF with Google Chrome, please download it here instead.
Page Metadata
Item Metadata
Title | Efficient numerical techniques for predicting process-induced stresses and deformations in composite structures |
Creator |
Arafath, Abdul Rahim Ahamed |
Publisher | University of British Columbia |
Date Issued | 2007 |
Description | During the last two decades of research work in numerical modelling of autoclave processing of composite structures, several models have been developed ranging from simple one-dimensional elastic to sophisticated three dimensional viscoelastic models. Some of the common problems faced by these numerical models are the non-familiarity of general users with these models, their non-versatility, their inefficiency when running large problems and the interpretation and validation of the results produced by these models. The main objective of this research work is to initiate the development of the next generation process model for autoclave processing of composite structures to address the above problems. This development is carried out by building on the already established knowledge of process modelling within the UBC Composites Group. The developed next generation process model consists of a set of numerical tools which range in complexity from a simple and robust closed-form analytical tool to a more general and adaptive shell-based finite element analysis tool that provides a modeller with a choice depending on the time and cost constraints. According to the developed closed-form solution, the axial stress variation in the thickness direction of a flat composite part varies exponentially with the through-thickness coordinate and its gradient depends on the part material and geometrical properties. It is shown that the process-induced unbalanced moment develops mainly at the initial stages of the curing process where the through-thickness stress gradient is significant. The process-induced effects in a curved part due to the thermal strain mismatch between the part and the tool in the tangential direction is similar to the process-induced effects in a flat part. Apart from the tangential thermal strain mismatch, the radial thermal strain mismatch between the part and the tool also induces stresses in a curved part. These stresses are due to the radial and tangential constraints applied by the tool on the part to conform the part to the tool shape. The unbalanced moment due to these stresses mostly develop at the cool-down portion of the cure cycle when the material is fully cured. |
Genre |
Thesis/Dissertation |
Type |
Text |
Language | eng |
Date Available | 2011-01-20 |
Provider | Vancouver : University of British Columbia Library |
Rights | For non-commercial purposes only, such as research, private study and education. Additional conditions apply, see Terms of Use https://open.library.ubc.ca/terms_of_use. |
DOI | 10.14288/1.0063214 |
URI | http://hdl.handle.net/2429/30707 |
Degree |
Doctor of Philosophy - PhD |
Program |
Civil Engineering |
Affiliation |
Applied Science, Faculty of Civil Engineering, Department of |
Degree Grantor | University of British Columbia |
Campus |
UBCV |
Scholarly Level | Graduate |
AggregatedSourceRepository | DSpace |
Download
- Media
- 831-ubc_2007-266717.pdf [ 24.53MB ]
- Metadata
- JSON: 831-1.0063214.json
- JSON-LD: 831-1.0063214-ld.json
- RDF/XML (Pretty): 831-1.0063214-rdf.xml
- RDF/JSON: 831-1.0063214-rdf.json
- Turtle: 831-1.0063214-turtle.txt
- N-Triples: 831-1.0063214-rdf-ntriples.txt
- Original Record: 831-1.0063214-source.json
- Full Text
- 831-1.0063214-fulltext.txt
- Citation
- 831-1.0063214.ris
Full Text
Cite
Citation Scheme:
Usage Statistics
Share
Embed
Customize your widget with the following options, then copy and paste the code below into the HTML
of your page to embed this item in your website.
<div id="ubcOpenCollectionsWidgetDisplay">
<script id="ubcOpenCollectionsWidget"
src="{[{embed.src}]}"
data-item="{[{embed.item}]}"
data-collection="{[{embed.collection}]}"
data-metadata="{[{embed.showMetadata}]}"
data-width="{[{embed.width}]}"
data-media="{[{embed.selectedMedia}]}"
async >
</script>
</div>
Our image viewer uses the IIIF 2.0 standard.
To load this item in other compatible viewers, use this url:
https://iiif.library.ubc.ca/presentation/dsp.831.1-0063214/manifest