o) = T \u2014 ( - r - cosh(Aiyi) + -f- sinh(Ajyj) + C, 1 ^p. \\ Ai Ai Pi (5.74) (5.75) 1 2A 2B cosh(Aj|\/j) - 1 - sinh(Ajyi) + C s A,; A,-(5.76) 5.2 One-dimensional Analysis of Tapered Double-doubler Joints and Reinforcements 134 The stresses for the negative sections of the double-doubler joint can then be determined utilizing the additional boundary conditions: M - i O = - r a \\ ) (5-77) V - * ) = ( 5 - 7 8 ) PA-Vi) = *<7 1<'<7 ^ = 57 mm h EPx and uPyx being the major Poisson's ratio: 1 1 - K c - ^ p J + a p x A T (5.97) e p y = jr-(-vPyxvPx + a P y) + aPyAT . (5.98) To simplify the estimation of the thermal residual stress, a rigid bond is assumed based on \u00b0 the small load transfer length in comparison to the overlap length (1\/A *

=2^-\\) s i n h ( A n \/ n ) (5 253) a\u00b0 l2 \/r>=o)cosh(A nJ n) + \/ ( ^ 2 \" - 1 ) s i n h ( A n Z n ) = - ^ A i | j r - (5-254) The corresponding half crack opening displacement vdQl is then calculated using equation (5.8) and (5.117): 0 1 2 ( i ? P l \u00a3 P l \u00a3 s \u00a3 s ) A]Ff ^ ^ 5.6 Generalization of the Rose Model for Partially Disbonded Patches 193 The additional displacements due to strains in the substrate and patch are given as: uoIl 7oIII 2 ^\u2014' E t k=2-d p\"lpk d (5.256) (5.257) which are then used to calculate the total half crack opening displacement as follows: d d d d = \u00aboi + v o i i + vom 1 2 + 2 \\EP1 \"'Pi -^s^s d , 1 2 + \\ 1 d 1 d i _ J _ _ L a\u00b0ta 1 i . , a o . 2 \\ \u00a3 , p 1 7 j p i E'gt, (5.258) (5.259) (5.260) As previously discussed, it is necessary to determine the half crack opening for a disbond extending underneath the last step of the patch separately. The half crack opening due to the shear displacement in the adhesive can be determined using equation (5.208) from the uniform thickness patch analysis while the displacements due to the strain in the substrate and patch are given in equation (5.256) and (5.257). Thus the total half crack opening displacement for a disbond extending underneath the last step of the patch is given by: crj: o\"s EPltPl + E^ts A i tanh(Ai_Zi) ( 1 _|_ 2 \\ \\ (5.261) The upper limit for the stress intensity factor under plane stress conditions can be expressed for the partially disbonded tapered repair as (5.262) 5.6 Generalization of the Rose Model for Part ia l ly Disbonded Patches 194 where A is given for disbonds not extending underneath the last step of the patch as A = 1 1 + Eat a vrF 2 V 2\u00a3P1tP1 V \u2022iFt + (_1_ + _2_) \\ ^ P l ^Pl Ests J (5.263) and for disbonds extending underneath the last step of the patch as A 1 \/ Ests TTY2 2EPltPl i kSJk U*1**+ *0 Ai tanh(Aiii) ( I _| 2_\\ \\ (5.264) A factor of 1\/(1 \u2014 f 2 ) needs to be included in A in the case of plane strain conditions. Using and as asymptotes, as suggested by the original Rose model, the stress intensity factor and the corresponding energy release rate for different crack lengths are then derived by interpolation using equation (5.220) and (5.221). It is noted that the accuracy of this analysis was improved by accounting for the shear stiffness of the adherends by using Ashear-iag (equation (5.92)) instead of A. The results of this analysis scheme are presented for the same three cases as presented in Section 5.6.1, i.e.: \u2022 Thermal residual stress loading ( A T = \u2014 64.8\u00b0C) \u2022 Remote stress loading (O-QO = 40 M P a ) \u2022 Combined thermal residual stress and remote stress loading ( A T = \u201464.8\u00b0C, (Too = 40 M P a ) The only difference between the uniform thickness patch analysis and the tapered patch analysis is the thickness change of the patch near the edge. A l l other material parameters remain unchanged. 5.6 Generalization of the Rose Model for Partially Disbonded Patches 195 The patch thickness is defined as: P l < i < 7 = 1.056 mm \u2014 i 0.132 mm (5.265) with step lengths of: lx = 57mm and . I, 2 \u00ab = \u00b0 - 3 3 = aSz = 23.29 \/ ie \/\u00b0C a 5 y = 23.45 nt\/\u00b0C F M 73M: Eax = Eay = Eaz = 2.19 GPa Gaxy = Gayz = Gaxz = 844 MPa \"axy = Vayz = \"axz - 0.3 \u00ab a x = Oiay \u2014 a a z = 50 \/ ie \/\u00b0C Note: The y-direction is aligned with the boron fiber and aluminum grain orientation. 6.2 Verification Models 204 6 .2 V e r i f i c a t i o n M o d e l s In total, five verification models were created. The initial model representing a uniform thickness reinforcement was used to determine the mesh size in regions of high shear stress. This model served as a basic reference case due to the availability of a good theoretical model for comparison. A tapered reinforcement was chosen as a second model to optimize the required number of elements in the tapered region. Both normal and reversed stacking sequence were investigated to assess the importance of detailed representation of the actual structure. Next, a model of the substrate in the cracked section was investigated. The focus of this model was placed on the stress intensity factor prediction. The mesh for the crack region had to be sufficiently fine along the crack face to predict the adhesive shear stress properly once the adhesive and patch were added to the model, i.e. the next step. The results of this model were then compared to the developed closed form approximation for the stress field around a patched crack. The A M R L specimen exhibits additional in-plane bending due to the partial patching across the specimen width which are not considered in the theoretical approach making this patched crack model an assessment tool for the theoretical crack tip stress field model. The half circular geometry of the patch also complicated the finite element analysis. It was required to check if the aspect ratios found for the tapered reinforcement were acceptable for a circular patch due to the change in the material orientation with respect to the element orientation. Finally the entire A M R L specimen was modeled using the mesh specifications derived by the different verification models. The number of elements required to get an accurate representation of the A M R L specimen was so large that an attempt to verify the mesh size in the full model was too time consuming and resources were quickly exhausted. 6.2 Verification Models 205 6.2.1 Constant Thickness Double-sided Reinforcement This first model was intended to confirm the input data into MSC\/Nastran as well as compare the results with the proven one-dimensional model of L.J . Hart-Smith. In order to avoid any stress concentration effects, the model had identical areas for the substrate, adhesive and patch. In-plane quarter symmetry as well as symmetry through the constant thickness model were used. The material thickness were selected to represent the inner section of the A M R L specimen: 3.175 mm thick aluminum face sheet, 0.25 mm thick adhesive layer and the 0.924 mm thick seven layers of boron\/epoxy. This investigation was also useful for determining the required element size for the reinforced crack region in the A M R L specimen since the shear stress distribution away from the crack tip can be approximated by the shear stress distribution in a double-doubler joint. It should be noted that the shear stress distribution near the center of a double-doubler joint under thermal loading is identical to the shear stress distribution near the free edge of reinforcement considering a sufficiently long overlap length. The aluminum, adhesive and patch were modeled initially using two elements through the thickness of each material. Five elements were used across the half-width of 12.5 mm. The specimen half-length was 75 mm. The element size was reduced from 5 mm in the center of the specimen with zero shear stress to 0.25 mm, 0.0625 mm and 0.03125 mm respectively along the length to the specimen edge with the highest shear stresses. The last four elements adjacent to the free edge had the same element length when an element length of 0.25 mm and 0.0625 mm was used. Eight elements with equal length were chosen for the model with an element length of 0.03125 mm. The chosen element lengths were based on fractions of the adhesive thickness between ta and ta\/8 covering Callinan's recommendation of a maximum element length of rja\/5 near the edge [24]. A temperature change of \u2014 64.8\u00b0C was applied as a loading condition representing the cooling stage from the stress free temperature to room temperature. 6.2 Verification Models 206 Figure 6.1 shows the shear stress in the mid-plane of the adhesive along the centerline and close to the end of the specimen for the three F E M analyses and Hart-Smith's theoretical solution. The theoretical analysis shows excellent agreement up to 0.5 mm away from the free edge. This one-dimensional approach cannot account for the drop to zero shear stress at the free edge. The coarse F E M model shows the highest shear stress (21.4 MPa) 0.25 mm away from the free edge while the two finer meshes show a peak shear stress (20.0 MPa) at approximately 74.85 mm from the center of the specimen. It should be noted that the one-dimensional analysis predicts nearly the same value (19.7 MPa). Changing from an element length equivalent of 25% to 12.5% of the adhesive thickness results in only minor differences in the peak shear stress and its location. 22 20 18 16 14 12 | 8 \" 6 H 4 2 0 -2 -4 -6 -8 -1-D Theory -0.25 mm - 0.0625 mm -0.03125 mmm 74.125 74.25 74.375 74.5 y [mm] 74.625 74.75 74.875 Figure 6.1: Adhesive shear stress for a uniform thickness reinforcement using element lengths between ta and ta\/8 The mesh with an element length of 12.5% of the adhesive thickness shows a shear stress of -5.0 MPa at the free edge while the finer mesh drops to -6.1 MPa. Both meshing schemes show a significant error which is not surprising considering the large stress gradient near the free edge. The shear stress prediction for an element length equivalent to 1\/4 of the adhesive thickness shows the better result for this particular finite element verification model. 6.2 Verification Models 207 In addition, a model with a larger number of elements through the thickness was tested. The mesh with the smallest element length of (12.5%) ta was used with 6 elements through the thickness for each material. Figure 6.2 shows the variation in shear stress results for 2 and 6 elements through the thickness. 22 20 18 16 14 12 ^ 10 Q- 8 a - 2 Elements - 6 Elements 74.125 74.25 74.375 74.5 y [mm] 74.625 74.75 74.875 75 Figure 6.2: Adhesive shear stress for a uniform thickness reinforcement with a different number of elements through the thickness The position of the peak shear stress shifted by only 0.04 mm and the peak stress was reduced by 0.5 MPa. The shear stress at the free edge was less than 0.1 MPa, i.e. nearly the theoretical value of 0 MPa. The larger number of elements through the thickness would be preferred near the free edge, but it would increase the total number of elements since a transition should not be made in sections with high stress gradients. Based on the importance of predicting the peak shear stress and its location, it was decided to use an element length equivalent to 25% of the adhesive thickness. Generally, two elements through the thickness were used for each material except in the aluminum near the crack where four elements through the thickness were employed to improve the prediction of the crack opening. 6.2 Verification Models 208 6 . 2 . 2 T a p e r e d R e i n f o r c e m e n t w i t h a R e v e r s e d S t a c k i n g S e q u e n c e A tapered reinforcement was chosen as the second verification model. It was important to verify that a sufficient number of elements has been used for each step to determine the thermal residual strains in the adherends and the adhesive shear stress properly. The smallest number of elements was desirable to reduce the overall degrees of freedom for the A M R L sandwich type model. In the past, tapered edges have been modeled using tapered elements or a normal stacking sequence, not necessarily representing the real lay-up sequence [19, 24]. Specially tapered elements reduce the required number of elements but they do not represent the true structural details of the actual taper. As part of this verification model, a normal stacking sequence was compared to the actual reversed stacking sequence of the A M R L specimen (Figure 6.3) showing the importance of proper structural representation and design choices under given loading conditions. Reversed Stacking Normal Stacking Figure 6.3: Reverse and normal stacking sequence The reversed stacking sequence is significantly more complex to model than the normal stacking sequence if the change in material orientation in the thickness direction is included. The size of the adhesive fillet was measured using a precured patch where the peel ply was not removed. The fillet shows up as a smooth region versus the typical fabric texture of the peel ply. The size of the fillet varies with respect to the location along the outer edge in the case of a half circular patch as used for the A M R L sandwich type specimen. The fillet length is approximately 1 to 1.25 mm for boron\/epoxy if the taper is aligned with the fiber orientation, while it is only 0.25 mm where the fiber orientation is parallel 6.2 Verification Models 209 to the taper. The carrier fabric of the boron\/epoxy prepreg causes a small fillet where the fibers are perpendicular to the taper direction while the larger fillet is a result of the stiffness of the boron fibers where the fibers are parallel to the taper orientation. In order to reduce the complexity and the required number of elements to account for the fillet properly, a triangular fillet with a length of 1 mm was chosen regardless of the location in the patch. This approach can be justified by the relatively long distance from the locations of the locally thicker adhesive to the regions of high shear stress in case where the fiber orientation is not parallel to the taper orientation, thus not affecting the results in a critical area. Figure 6.4 through Figure 6.9 show results of the convergence study which was carried out for the reversed stacking sequence. The shear stress in the mid-plane of the adhesive as well as the thermal residual strains at the top and bottom surface of the patch and substrate were evaluated. The effect of smaller elements as well as more elements through the thickness are shown in these figures. Figure 6.4: Transverse shear stress at the adhesive mid-plane in the tapered region for different F E M meshes 6.2 Verification Models 210 Typical ly seven elements through the thickness of the boron\/epoxy were chosen to simplify the modeling while the adhesive and aluminum were represented by 2 elements through the thickness as shown in Figure 6.5. L i i J L . _ l l f g = a a , Figure 6.5: Detailed view of the finite element mesh in the tapered section-reversed stacking The number of elements was doubled to study the element number dependence through the thickness. These figures show the extreme cases of this convergence study for element length along the taper with the smallest element size of both 0.125 m m and 0.03125 mm at the ply drop-off. Furthermore, the number of elements was reduced along the taper for the Figure 6.6: Thermal residual strains at the top surface of the patch in the tapered region for different F E M meshes case of seven elements through the thickness of the boron\/epoxy, two elements through the adhesive and two elements through the aluminum thickness. The smallest element length 6.2 Verification Models 211 Figure 6.7: Thermal residual strains at the bottom surface of the patch in the tapered region for different F E M meshes was 0.125 mm in comparison to the curve for the model with twice as many elements through the thickness. The labels in the plots identify the number of elements for each component and the smallest element size at the ply drop-offs. 600 500 400 300 J i 200 100 0 -100 -200 - - - - 7 B\/en-2 FM73M - 2 Al-0.03125 mm 1 7 4 B\/ep - 4 FM73M - 2 Al -B\/ep - 2 FM73M - 2 Al - 0 0.125 mm 125 mm 48 51 54 57 60 63 y [mm] 66 69 72 75 78 Figure 6.8: Thermal residual strains at the top surface of the substrate in the tapered region for different F E M meshes 6.2 Verification Models 212 7 1 B\/ep - 2 FM73M - 2 Al - 0 4 B\/ep - 4 FM73M - 4 Al -B\/ep - 2 FM73M - 2 Al - 0 03125 mm D.125 mm 7 125 mm I 48 51 54 57 60 63 66 69 72 75 78 y [ m m ] Figure 6.9: Thermal residual strains at the bottom surface of the substrate in the tapered region for different F E M meshes All curves in Figure 6.4 through Figure 6.9 show good agreement, especially the ther-mal residual strains at the aluminum substrate bottom (see Figure 6.9). Location A in Figure 6.6 shows the effect of reducing the number of elements along the taper in some non-critical regions. The smaller element length at the ply drop-offs emphasizes the singu-larities in the thermal residual strains in the boron\/epoxy (see location B in Figure 6.7). The mesh with seven elements through the patch and two elements through the thickness of the adhesive as well as the substrate and an element length of 0.125 mm at the ply drop-off was chosen to model the tapered region of the A M R L specimen based on the good agreement with the finer meshes. A comparison between the normal and reverse stacking sequence was carried out next. In addition, the results of the one-dimensional analysis are plotted. Figure 6.10 shows how well the one-dimensional analysis can predict the shear stresses in the mid-plane of the adhesive especially for the normal stacking sequence. The general trend is predicted properly, even for the reversed stacking sequence but the finite element analysis shows clearly the influence of local increases in the adhesive thickness. The peak adhesive shear stress is overpredicted 6.2 Verification Models 213 14.0 13.0 12.0 11.0 10.0 9.0 8.0 a\" 7.0 2 6.0 \u00a3 5.0 4.0 3.0 2.0 1.0 0.0 -1.0 -2.0 I Reverse Stacking i Normal Stacking \/A 1 -D Theory \/\/\/ A f A A J J \/ \/ \/ . TI \\ V \\ \\i \\J \\ V \\ > 48 51 54 57 60 63 y [mm] 66 69 72 75 78 Figure 6.10: Transverse shear stress at the adhesive mid-plane for reversed and normal stacking sequence by the one-dimensional analysis, which is caused by extending the adhesive layer past the last boron\/epoxy layer. Figure 6.1 shows how well the one-dimensional theory predicts the peak adhesive shear stress if the patch and adhesive end at the same location. It should be noted that the mid-plane does not show the highest shear stress using the reversed stacking sequence. The singularities at the ply drop-offs lead to an increase in the shear stress close to the patch\/adhesive interface. Figure 6.11 and Figure 6.12 show the sensitivity of the thermal residual strains in the patch towards the choice of stacking sequence. A large discrepancy between the finite element results and the one-dimensional analysis is visible. The magnitude of the thermal residual strains predicted by the one-dimensional analysis compares only reasonably well to the strains determined in the F E M analysis at the patch\/adhesive interface with a patch utilizing the normal stacking sequence. The large spikes in the finite element results for the thermal residual strains using either stacking sequence are caused by the stress singularities at the ply drop-offs. This effect is not included in the theoretical one-dimensional analysis. A significant reduction of over 6.2 Verification Models 214 200 Figure 6.11: Thermal residual strains at the top surface of the patch for reversed and normal stacking sequence 500 fie in the peak compressive strain through the thickness of the patch is evident for the reversed stacking sequence. In addition the location of the peak compressive strain also shifts from near the ply drop-off at the bottom of the patch to the end of the adhesive fillet at the top surface of the patch. For the normal stacking sequence for the patch lay-up, Figure 6.12: Thermal residual strains at the bottom surface of the patch for reversed and normal stacking sequence 6.2 Verification Models 215 the reduction in compressive thermal residual strains through the thickness of the patch is even more significant (up to 700\/ie) for this particular loading case. Figure 6.13 and Figure 6.14 show the results for the thermal residual strains in the substrate. The effect of the stacking sequence on the aluminum substrate is not significant especially at the bottom side of the 3.175 mm thick aluminum sheet where the deviation in thermal residual strains between the normal and reversed stacking sequence is less than 15 fie. The result of the one-dimensional analysis is also quite close to the F E M analysis with generally less than 30 fie variation regardless of the stacking sequence at this location. It should also be noted that the thermal residual stresses in the substrate don't drop to zero at the patch edge due to the extended adhesive layer. The effect of the reversed stacking sequence on the thermal residual strains in the substrate are more pronounced at the substrate\/adhesive interface. The thermal residual strains are reduced in the regions of increased adhesive thickness while they are in excellent agreement in the mid-section of a tapered step. 600 500 400 300 Jr 200 100 0 -100 -200 \\ Reverse S tacking acking 1 Normal St. 1 -D Theon48 51 54 57 60 63 y [mm] 66 69 72 75 78 Figure 6.13: Thermal residual strain at the top surface of the substrate for reversed and normal stacking sequence 6.2 Verification Models 216 600 Figure 6.14: Thermal residual strain at the bottom surface of the substrate for reversed and normal stacking sequence One of the most important findings are the high peel stresses in the adhesive due to the reversed stacking sequence (see Figure 6.15). The main cause is the orientation change of the upper plies passing over a ply drop-off resulting in peel forces. The peel stresses develop at different locations depending on tension or compression in the patch. The peak peel stress in the adhesive mid-plane occurs at the ply drop off in case of compressive stresses in the 10.0 8.0 6.0 4.0 2.0 0.0 -2.0 -4.0 -6.0 -8.0 -10.0 ll il Jt \/ \/ \/ \/ \/ \/ \/ J \/ \/ \/ \/ \/ \/ \/ \/ \/ \\c \/ \/ \/ \/ \/ \/ 7 \/ \/ \\ r if i I I 48 51 54 57 60 63 y [mm] 66 69 72 75 78 Figure 6.15: Peel stresses in the adhesive mid-plane for the reversed stacking sequence 6.2 Verification Models 217 patch (see location A in Figure 6.16) while for tensile stresses the peak occurs at location B. Tensile loading of the bonded repair will therefore generally change the location and reduce the magnitude of the peel stresses introduced by the thermal residual stresses, while compressive loading will reverse the peel stresses and thus may contribute to the failure of the bonded repair. A fractographic investigation by the National Research Council showed a change in failure mode at the ply drop using a reversed stacking sequence. This failure mode change was not present when using a normal stacking sequence [37]. Based on the findings in the finite element analysis, peel stresses can be associated with this failure mode change. t t A B Figure 6.16: Critical location for peel stresses in the adhesive mid-plane for the reversed stacking sequence Two conclusions can be drawn from the prediction of high peel stresses: The stresses and strains in a tapered patch with a reversed stacking sequence should not be analysed by approximating the taper using a normal stacking sequence nor a tapered element. Addi-tionally special attention should be paid to the peel stress in the tapered region when using a reversed stacking sequence under compressive loading of the bonded repair. The stresses in the substrate and in the adhesive are generally the main concern for bonded repairs. Most crack patching applications arise from cracking in sections loaded in tension. The one-dimensional analysis predicts the thermal residual strains for the aluminum sub-strate and the adhesive shear stress very well. Small discrepancies arise due to specific de-6.2 Verification Models 218 sign choices, such as extending the adhesive layer beyond the patch. Patch design choices such as the stacking sequence become far more important for reinforcements or cracked sections of components loaded in compression based on the high peel stresses found in the taper using a reversed stacking sequence. 6 . 2 . 3 C r a c k M e s h V e r i f i c a t i o n The crack mesh verification model was the first step in generating an appropriate finite element model for the cracked region of the A M R L specimen. This model deals only with the metal substrate due to the availability of a closed form solution allowing the verification of the finite element results rather than a convergence study. A large number of crack meshes were investigated. One of the main difficulties in this investigation was the small element length requirement perpendicular to the crack in order to allow for the proper determination of the adhesive shear stresses and thermal residual stresses in the adherends. This requirement was complicated by the lack of a crack tip element in MSC\/Nastran for Windows. For this reason three approaches were investigated. First, a finite element mesh was generated using only parabolic elements. In a second approach, additional bulk data cards were submitted as part of the analysis sequence creating MSC\/Nastran CRAC3D crack tip elements which are not supported in the user interface. The third approach utilized the typical quarter point method where the mid-side nodes of the elements surrounding the crack tip are moved to the quarter point location. This third approach was ruled out due to the number of warnings issued by MSC\/Nastran with respect to the determination of the stresses, i.e. crack tip stress reached 10000 GPa. The MSC\/Nastran user guide noted that this approach might also lead to an early abortion of the calculation. Another significant disadvantage of moving the mid-side is the connec-6.2 Verification Models 219 tivity to the bonded patch. If the mid-side node in the patch is moved to the quarter point location, the stress distribution will be highly distorted. The other option is to make a transition in the aluminum or adhesive which will lead to uncertain answers due to the unknown element behaviour. Significant verification work would be required to study such element behaviour. The advantage of using the regular parabolic elements is a better spatial stress distribution. The shape of the constant stress contour lines are closer to the theoretical estimation espe-cially for elements with high through thickness aspect ratios (25:1). In order to get a good spatial distribution with the MSC\/Nastran CRAC3D elements, a through thickness aspect ratio of 6:1 was required, thus using significantly more elements through the thickness. The use of the CRAC3D elements is significantly more complex and the implementation is time consuming. In addition, the elements cannot be visually checked and results cannot be displayed although they were available in the T06 output file. It should also be noted that the computed stress intensity factor by M S C \/ N A S T R A N varied by approximately 13% de-pending on the use of the full modeling option or the symmetry option. The listed element stresses for these two modeling options varied as well based on different natural coordi-nates. The stresses, strains and displacements for the surrounding elements were compared and found identical despite the differences in the output of the crack tip element. The stress intensity predictions given by M S C \/ N A S T R A N seemed rather low in comparison to extrapolation of stress intensity factor plots based on the crack opening displacement. The theoretical stress intensity factor for this particular verification model can be calculated using [23]: (6.1) where Y = 1.12-0.23 + - \u00ab \u2022 \" ( \u00a3 ) ' (6.2) 6.2 Verification Models 220 and was determined to be Kr = 2\\.\\2MPa^\/m for a specimen containing a 20 mm long crack and a width of 50 mm under 40 MPa of remote tensile loading. This theoretical value was used to assess the quality of the finite element crack tip mesh by comparing it to the stress intensity factor calculated from the finite element results. The finite element model length was chosen to be 100 mm. It was decided to use a sheet thickness of 1.5875 mm to achieve plane stress conditions under the chosen remote loading. The choice of plate thickness also improved the aspect ratio of the elements in the crack tip region to approximately 1:6 by utilizing symmetry through the thickness and with respect to the crack. Two elements were placed to represent the half sheet thickness. The crack opening displacements determined by the finite element analysis were used to calculate the stress intensity factor as given by [25]: K IFEM 2TTE r 4 (6.3) Note that the equation for KIpEM is shown for plane stress conditions. Figure 6.17 shows the stress intensity factors calculated for the finite element crack opening displacements utilizing the different crack tip modeling approaches. The results for the stress intensity 23.5 23 22.5 22 21.5 21 QL 20.5 \\ \/ \u2014 \u2022or f * Crack tip element (CRAC3D) Crack tip element (Quarter point node) No crack tip element (Parabolic element) \u2022 \u2014A\u2014 ,i o ; ^ 5 f 3 1 0 1 2 1 4 1 6 1 8 2 20 19.5 19 18.5 18 17.5 r [mm] Figure 6.17: Stress intensity factors for different crack tip elements 6.2 Verification Models 221 factor based on the crack opening displacements are within 1% of each other for the different crack tip modeling approaches for locations which are more than 10% of the crack length away from the crack tip. Larger deviations occur closer to the crack tip. The MSC\/Nastran CRAC3D element shows a spike after the second element from the crack tip. The reason for this spike is possibly the different displacement formulation used by MSC\/Nastran for the crack tip element in comparison to the parabolic elements. The quarter point approach results also in a spike in the stress intensity factor at the interface between the crack tip element and the adjacent parabolic elements. The model with only parabolic elements shows a gentle decrease in the stress intensity factor close to the crack tip. Chan et.al.'s [25] approach of using a linear extrapolation is applied rather than calculating K I F B M just from the crack tip elements. Good linear sections of the stress intensity factor versus r are found from approximately 15% to 50% of the crack length. The extrapolated stress intensity factors are within 0.5% of the theoretical estimation for the three modeling procedures representing excellent results. This can be largely contributed to the small element size of approximately 0.3% of the crack length in the crack tip vicinity. The stress in the loading direction was investigated as a second parameter to check the performance of the crack tip modeling. Figure 6.18 shows the stress in the loading direction (ay) ahead of the crack along the through thickness center line. Negative coordinates refer in this case to the cracked section. The nodal stress for the CRAC3D element are not provided in the post-processor thereby not allowing nodal stress averaging with the adjacent elements. Generally this is not a concern with a fine finite element mesh, but the large stress gradient present at a crack tip it will distort the results. Therefore the nodal stresses in the elements next to the crack tip element were not displayed. It is apparent that the stresses for the model with the CRAC3D element are higher ahead of the crack tip than the results given by the two other modeling approaches. It should 6.2 Verification Models 222 3000 2800 2600 2400 2200 2000 1800 \u201e 1600 \u00a3 1400 ~ 1200 0 1000 800 600 400 200 0 -200 -400 X Crack tip element (CRAC3D) \u2014 \u2022 \u2014 Crack tip element (Quarter point node) \u2014A\u2014 No crack tip element (Parabolic element) v -j - & \/ s-x^ k 1 t 4_ v w w w w w ^ J\\\u2014 ML M A M. A 2 -1 75 -1 .5 -1 25 -1 -0 75 -0 .5 -0 25 0 0. 25 0 5 0. 75 1. 25 1 5 1. 75 2 r [mm] Figure 6.18: Stress perpendicular to the crack (ay) for different crack tip elements be noted that this difference only becomes evident for stresses exceeding the yield stress of the material (310 MPa) very close to the crack tip ( \u00ab 0.35 mm). The modeling approach using the quarter point method and no crack tip element have excellent agreement ahead of the crack tip except that the stresses for the quarter node element approach generate extremely large values (> lOOOOGPa) in the crack tip element while the parabolic element adjacent to the crack tip reaches nine times the yield stress of the material. A point of verification is that the stress along the crack face should be zero. All modeling approaches reach this value within 1-1.5% of the total crack length from the crack tip. The parabolic element shows the highest over shoot in the element adjacent to the crack tip, which is not surprising considering the steep gradient and the element formulation. It should be noted that the crack tip displacements the in x-direction (ahead of the crack tip) using the CRAC3D element were not satisfactory. The crack front through the thickness appeared jagged and possibly unreliable. 6.2 Verification Models 223 Having investigated these different modeling approaches, it was decided to use parabolic elements at the crack tip. All three methods can be used to determine the stress intensity factor quite accurately utilizing Chan's [25] extrapolation technique. The quarter node method was rejected due to the difficulties in connectivity to the patch. The CRAC3D element approach showed generally good results but required a tedious input as well as a larger number of elements through the thickness to avoid distortion of the in-plane stress field. Additionally the jagged displacements found along the crack front were unrealistic. The behaviour of the parabolic elements was quite good due to the small element size in the crack tip vicinity. The parabolic element also handled higher aspect ratios through the thickness better. The only short fall was the approximately 10% overshoot in comparison to the peak stress along the crack front. Having established a good mesh scheme using parabolic elements for the crack region of the substrate, the adhesive layer and the patch were added to the model as shown in Figure 6.19. 6 . 2 . 4 P a t c h e d C r a c k M o d e l The patched crack verification model was chosen to evaluate the theoretical crack tip stress field model for bonded repairs. The previous crack mesh verification model provided con-fidence in a proper mesh for the substrate. A constant thickness patch of 0.924 mm as well as the 0.25 mm thick adhesive layer were added to the crack tip verification model after increasing the thickness of the substrate to 3.175 mm thereby representing the center section of A M R L sandwich type specimen. The honeycomb used in the A M R L specimen is neglected since the theoretical model doesn't account for it. A uniform thickness patch over the entire substrate was chosen to avoid any additional bending due to partial coverage of the patch across the width of the model. The model length of 100 mm was chosen long enough to avoid an interaction between the load transfer zone at the free edge of the model and the high stress region around the crack tip. No mesh refinement was carried out near 6.2 Verification Models 224 the free edge due to the focus on the stress distribution in the vicinity of the crack tip. Two elements were used through the thickness of the adhesive, while four elements through the thickness of the seven ply patch were applied. The first layer of elements was used to represent the boron\/epoxy layer next to the adhesive. The three remaining element layers for the patch always represented two boron\/epoxy plies each. The mesh for the aluminum substrate was left identical to the previous verification model. Figure 6.19 shows the finite element mesh used in this investigation: One of the most difficult decisions to be made in this finite element approach was the modeling of the adhesive along and across the crack. Modeling the adhesive continuously across the crack implies that no crack opening occurs at the adhesive\/substrate interface based on no crack opening in the initial unstressed state. In order to model the adhesive continuously across the crack using a discrete modeling approach such as finite elements, a small crack opening displacement must be present and the adhesive must be extended past the crack face towards the symmetry line of the repair. A plasticity analysis can then be carried out to get a proper result for the crack opening displacement in the substrate. The approach taken in this research work is based on a discontinuous adhesive layer across the crack. Its advantage is that the analysis can be carried out using a linear-elastic Figure 6.19: Finite element mesh for the patched crack verification model 6.2 Verification Models 225 approach thus reducing the computational requirements. Additionally it presents an upper bound approach for the crack opening displacement. Failure of the adhesive in tension on top of the crack is a realistic possibility. Planned fractographic investigations of the region around the crack after fatigue failure will hopefully give a better indication about the true failure sequence. Unfortunately, papers dealing with the finite element modeling of this critical region have not discussed this problem in detail. The approach taken in this research work is similar to finite element models of bonded repairs developed by other researchers using spring elements to represent the adhesive [19]. A spring model implies that the adhesive is discontinuous across the crack. These models have been successfully used to predict the crack growth rate in bonded repairs. The finite element stress distributions for ax, ay and rxy along 9 = 0\u00b0 and 90\u00b0 are presented and compared to the closed form theoretical analysis in Figure 6.20 through Figure 6.25. All graphs show the theoretical results for plane stress and plane strain conditions. The stress intensity factor caused by the thermal residual stresses alone will generally lead to plane strain conditions for the crack analysis while combined with other external loading plane stress conditions at the crack tip are common. The finite element results for the substrate are displayed at the bottom and top surface of the aluminum face-sheet. The substrate bottom surface is the critical case due to the larger crack opening displacement. The adhesive restricts the crack opening displacement at the top surface of the substrate to a significant degree. The difference in the crack opening displacement between the top and bottom surface of one face-sheet at the edge of the A M R L specimen is approximately 22% which compares well with the 19% given by Baker for the F E M analysis of a simple double-doubler joint [18]. Figure 6.20 shows excellent agreement with the theoretical stresses in the loading direction along 9 = 0\u00b0 for plane strain conditions and the finite element results for the substrate bottom. Note that the substrate bottom coincides with the through thickness symmetry 6.2 Verification Models 226 plane due to neglecting the honeycomb. The difference between the fracture mechanics analysis for plane stress and plane strain conditions is approx. 5% for stresses below 150 MPa. Significant difference is visible between the finite element results for the top and bottom surface of the substrate. Good agreement between the closed form theoretical analysis and the F E M analysis for the symmetry plane can be attributed to accounting for the shear-lag in the adherends. The discrepancy in the stresses at locations more than 17 mm from the crack tip is due to modeling an edge crack in the F E M analysis and using the center crack assumption in the theoretical approach. The estimation of the stress intensity factor for the substrate using the finite element results imposes some difficulties. Typically the crack opening displacement is used to estimate the stress intensity factor for a cracked sheet. The questions that arises is, can this approach be applied to bonded repairs? Inspecting the stress field behind the crack tip (6 > 90\u00b0) for a bonded repair reveals differences in comparison to the typical stress field of a crack in an unreinforced sheet due to the load transfer into the patch rather than through the remaining 150 100 CO I 50 o II \u2014 0 -50 -100 Fracture Mechanics Theory (Plane Strain) Fracture Mechanics Theory (Plane Stress) FEM Substrate Symmetry Plane FEM Substrate Top -20 -15 -10 10 15 20 25 30 Figure 6.20: Stress in loading direction (ay) for the patched substrate along 9 = 0\u00b0 6.2 Verification Models 227 uncracked section. This finding makes the application of the crack opening displacement method based on an unreinforced sheet questionable. On the other hand, the stress field observed ahead of the crack tip for a bonded repair shows the typical stress distribution. It seems therefore more appropriate to use a stress extrapolation method to determine the stress intensity factor for different through thickness locations in the substrate. This approach is also supported due to the stresses ahead of the crack tip being the driving force for the crack rather than the crack opening displacement. The stress extrapolation method can be based on the usual one term approximation if data points are selected close to the crack tip. The corresponding stress intensity factor for a given stress in loading direction at a distance r from the crack tip along 9 = 0\u00b0 can be determined using: Kr = V27rray (6.4) Alternatively the correct elastic solution for a center crack in an infinite plate can be used to determine the stress intensity factor. In addition to the local stress