Numerical and experimental results are presented from a project aimed at predicting the fatigue life of a rotorcraft airframe component subjected to flight load spectrum. The airframe component is a riveted joint used on cabin frame cap splices of several civilian and military helicopters which hereafter is modeled as lap-joined nested-angle plates. This component is fatigue sensitive due to the highly cyclic and vibratory ro-torcraft mission spectrum and as such prediction of its fatigue life is an important part of the design cycle. This paper presents a systematic approach that combines 3D finite element simulation in ABAQUS and 2D damage analysis in NASGRO to estimate the life of the component. In the numerical analysis, fatigue crack growth rates for through-the-thickness crack initiating from fastener holes is computed using 2D standard and weight function models with the crack plane stress field obtained from 3D FEA analysis. Effect of load interaction due to tensile overload is included using strip-yield retardation model. Finally, results of the numerical simulations are compared with representative experimental data obtained under similar spectrum loading condition.
Fatigue crack growth prediction albeit being a relatively old subject, over 150 years, is still an empirical science rather than a theoretical one. In the early days, SN curves were used to design fail-safe structures for infinite life[1, 2]. The empirical constants of SN curves, however, are derived from constant amplitude cyclic tests and hence are not representative of the random spectrum load that many airframe structures are exposed to. Moreover, it has been determined that [3, 4] the experimental fatigue lives of specimens and components subjected to random amplitude loading can be well below the fatigue lives predicted by the SN data. Hence a better design strategy is required.
With the advent of fracture mechanics, the damage tolerance design philosophy begins to evolve mainly in the aerospace industry. Fundamental to the damage tolerant approach is an understanding of structural performance in the presence of cracks or damage[5, 6] where emphasis was on determination of critical flaw size in a give time and usage condition. Hence models for crack growth prediction have to be formulated. Paris (1961)  was the first to develop a relationship to describe the crack progression rate or da/dN and the cyclical component AK of the Irwin stress (or stress intensity factor). Paris power law is give by,
where C and n are empirical parameters determined from curve fitting of experimental data. The Paris law, although the most popular model among the material science and fracture mechanics community  doesn’t describe the experimentally observed threshold and critical growth behaviors. Moreover, Equation(1) predicts the same fatigue life regardless of the mean-stress history of the spectrum. Walker (1970)  re-formulated Paris’ law by including effects of mean-stress through the use of a load ratio, R, where R = omin/omax or Kmin/Kmax. The Walker equation is give by,
where C, n and m are again empirical parameters determined from a curve fit to a set of fatigue crack growth (FCG) experimental data. Different values of m are required in eq.(2) depending on whether R is greater than or less than zero. Forman (1972)  further modified the Paris’ power law by introducing a factor depending on (1 — R) instead of R where R = omin/omax,
here AKrms and Rrms are the RMS (Root Mean Square)stress intensity factor range and stress ratio, n and c are curve fitting constants. The above three crack growth equations (eqs.(1),(2),(3) or Paris, Walker, and Forman) doesn’t take into account crack retardation phenomenon and hence are not very accurate for estimation of crack growth in spectrum loaded components. A more ambition predictive model comes from Forman and Newman (1984)  who modified the power law by including effects of plasticity-induced crack closure using what they called crack opening function. They developed what is now known as the NASGRO equation . The NASGRO (or Nasgro) equation is a full-range crack model that mathematically represents all the three regions of the FCG curves while taking into account mean stress and crack closure effects. It is given by,
where AK is the applied stress-intensity factor range, and R is the stress ratio; AKth is the fatigue threshold, Kmax is the stress-intensity factor corresponding to the peak applied load, and Kc is the critical stress intensity factor; p and q are curve fitting constants that control the shape of the fitting in the threshold and critical crack growth regions respectively; and f is Newman’s crack opening function. The constants C and n, which are the main fitting parameters are determined by minimizing the curve fitting error equation given by,
Equation (4) estimates crack growth behavior in near threshold and critical growth regimes better than any other model and is probably the most accurate empirical model currently available . It is also good to note that the Nasgro equation may be reduced to the Paris law eq.(1) by setting parameters p and q to zero and ignoring the effect of crack closure, i.e. by setting f = R for 0 < R< 1.
This paper uses the NASGRO equation with stress gradients obtained from 3D finite element analysis (ABAQUS) to predict spectrum crack growth in preloaded nested-angled plates. The 3D FEA stress gradient is the result of the combined action of fastener preload, bearing contact load and friction shear forces acting on the plates. The numerical predictions so obtained are compared with experimental data from fatigue tests of two nominally identical nested-angle specimens.
The goal of the experimental study was to determine fatigue crack growth in nested angle specimens under loads that simulate the various flight regimes of a typical rotorcraft. All tests are performed in ambient laboratory conditions using a servo-hydraulic test frame which applies a predetermined spectrum load at a constant frequency. The test specimens are made of aerospace grade Al 7075-T6 alloy angle-plates with thickness of 0.063in. Schematics of the nested-angle plates is shown in Fig.(1). The two plates shown in the figure are lap joined using stainless-steel fasteners with a bolt-load of 800lbf. The fastener holes are uniformly spaced in intervals of 1.12in and are drilled and rimmed to a nominal diameter of $ = 0.1875in. Detailed description of the experimental setup is available in [12, 13, 14]
Fig. 1: Geometry of the nested angle test specimen. The two plates are made from Al 7075-T6 and the fasteners are stainless steel. The critical holes are the locations of maximum principal stresses where crack will most likely initiate. The broken lines show the displacement symmetry plane in the FEA model.
The first test specimen (specimen-A) is run at a constant load amplitude of 3350lbf and a stress ratio R=0.1 until it fails by fracture. The remaining two specimens (B & C) were tested under variable flight load spectrum that peak at Pmax=2500lbf and 3000lbf respectively. The flight spectrum used to test specimens B and C is developed from a representative mission profile of a UH-60 type class helicopter undergoing predefined maneuvers. The spectrum cycles are then constructed from recorded strain gage data where internal loads (or stresses) at control points are available for a combination of velocity, load factor and flight maneuvers. During individual specimen tests the flight spectrum is scaled by the peak test load and is input to the servo-hydraulic test frame controller. Fig.(2) shows a segment of the normalized UH-60 single flight mission spectrum used in this experiment.
The numerical analysis conducted herein involves full 3D finite element simulation of the constant spectrum test (specimen-A) at its peak load Pmax=3350lbf. Stress analysis for the variable spectrum specimens were obtained by scaling the stress values of specimen-A by the load ratios i.e. the stress distribution for specimen-B is calculated by multiplying the stress distribution of specimen-A by 2500/3350 likewise for specimen-C it is 3000/3350 times stresses on specimen-A, assuming linear behavior.
The purpose of the 3D stress analysis is two-fold. First, the analysis is used to calculate the crack plane stress gradient resulting from the combined action of the applied load, contact load, and surface shear forces resulting from friction contact pairs.
Fig. 2: A segment of the normalized flight mission spectrum (see also ). This spectrum is scaled by Pscale=2500 for specimen-B and Pscaie=3000 for specimen-C.
Second, the analysis is used to calculate the stress intensity factors at the peak load to verify if the 3D FEA obtained stress intensity factors (SIF) correlate to the one obtained from the damage tolerance analysis code (NASGRO). It is agreed upon that the stress intensity factors computed using the 3D finite element analysis would give a better estimate of the crack tip intensity as it takes full account of the stress field near the crack tip arising from friction and contact interactions. Close correlation of the FEA SIF values with NASGRO SIF is generally taken as an indication to the accuracy of the 2D life prediction methodology of NASGRO. The finite element model is also required to identify the location of the maximum tensile stress (or hot spots) near the critical fastener hole. This is where cracking will very likely initiate. Using Abaqus, a nonlinear, static, large deflection finite element model with contact and friction was developed using the displacement symmetry model shown in Fig.(1). The symmetry model enables to refine the mesh and also to simplify the geometry into a form that is readily compatible with Nasgro’s simple library models. Surface-to-surface contact with friction was included to represent the part-to-part interaction between the two plates and the stainless-steel fasteners. A frictionless contact was later simulated and compared with the frictional contact to see if introduction of friction has any effect on the predicted fatigue life of the specimen.
We applied the FEA loads into simulation steps. The first load step was used to resolve fastener clamp-up (bolt-load of 800lbf) and establish contact throughout the model. In the second step, the remote load is ramped up to its final magnitude of 3350lbf. Analyses sanity checks (such as mesh convergence and load equilibrium) were performed to ensure that the finite element model performs well.
Finite element results
Figure (3) shows the maximum principal stress contour near the critical hole of the small leg specimen (the smaller of the two nested plates shown in Fig.(1) for cases ^=0.6 and ^=0 upper and lower figures respectively. For the case where ^=0.6, the peak value of the principal tensile stress is 45.5 ksi and this stress is located at the faying surface between the two plates away from the critical hole (see Fig.(1) for critical hole). For the second case where ^=0, the hot spot is located at the usual location near the edge of the critical hole in the 3 and 9 o’clock directions with the maximum principal stress being 77.6 ksi.
As can be seen, the maximum principal stress (magnitude and location) is affected by the introduction of contact friction. Moreover, the load transfer by each of the eight fasteners also depends on the extent of the friction coefficient In the extreme case where a higher friction coefficient is assumed, most of the load transfer between the plates is through surface shear and the contribution of the load transfer through fastener shank is minimal. For ^=0.6, large amount of load is transferred by each fastener through friction contact between fastener heads and the plates. For ^=0, the load transfer is mainly between fastener shank and the hole. Figure (4) shows the principal normal stress contour in the symmetry model.
As noted earlier, the finite element analysis is the first step of the damage tolerance analysis and its purpose is to calculate the stress fields that are needed by NASGRO library models. Fig.(4) shows sections on the plate where stress distributions are required to run NASGRO code. The cross section stress at sections 1 and 2 (Sec.1 and Sec.2) are used as inputs to NASGRO’s TC03 model whereas the stress at section 3 (Sec.3) is used as an input to run model TC13.
Fig. 3: Principal tensile stress contours around the critical fastener hole. The upper figure shows the stress contours for simulation case 1 where ^ = 0.6, Pmax = 3350lbf, Boltload = 800lbf ,amax = 45.5ksi and the lower figure shows the stress contrours for simulation case 2 where ^ = 0, Pmax = 3350lbf, Boltload = 800lbf ,amax = 77.6ksi. Note that the location of the hot-spot do not coincide on the figures.
Fig. 4: Principal stress contours on the small-leg symmetry model for simulation case 1. Sec.1 and Sec.2 are planes where normal stresses are extracted for input into NASGRO’s TC03 model. Sec.3 is the section stress input into TC13.
Fatigue crack growth predictions
Fatigue crack growth prediction for the constant and mission spectrum loads are conducted using Nasgro. Since Nasgro doesn’t have a library crack geometry that models the nested-angle configuration some assumptions are needed. First, the half symmetry angle specimen is modeled as flat (or 2D) assuming that the edge radius doesn’t significantly alter the stress distribution near crack tip throughout the loading cycle. Second, contact friction is represented implicitly within bearing and bypass stresses as there is no field in Nasgro GUI that allows for friction input. We used two library crack models for the life estimation. The weighted function stress intensity model TC13 shown in Fig.(5) was used since it allows modeling of a through crack at an offset-hole in a finite plate with a nonlinear stress gradient input. The stress gradient information for fric-tional and frictionless contact cases are obtained from the 3D stress analysis as depicted by Sec.3 in Fig.(4). Figure (5) shows the principal stress distribution used as Nasgro inputs for the friction and frictionless cases.
A second simulation was conducted using the classical library model TC03 shown in Fig.(6). TC03 requires the remote stress field and bearing load be specified at the critical fastener hole locations. The remote stress field was again obtained from FE simulation by mapping the principal stresses across sections 1 and 2 as shown in Fig.(6). Since part of the load is transferred through friction, the resultant of the stresses from sections 1 and 2 and bearing load P in TC03 model won’t satisfy equilibrium. Hence contact friction has to be included indirectly as discussed below.
Fig. 5: NASGRO TC13 library model and the corresponding crack plane stress inputs for | = 0.6 and | = 0. The various curves on the graph show the stress distribution at certain depth through the plate thickness at Sec.3. Note that the principal stress near the hole are maximum for | = 0 in addition the difference in principal stress between the two cases becomes small away from the hole.
Including effects of friction
The crack plane stress gradient input into Nasgro’s TC13 has the friction effect included in it and hence doesn’t require further consideration. However this is not the case for TC03. As shown in the FEA analysis (see Fig.(5)), the large bolt preload used to clamp-up the two nested plates and the high friction coefficient resulted in a significant surface shear between the plates and fastener heads. This shear force has shown to alter the magnitude and location of the maximum principal stress and the likely location of crack initiation point on the plates(Fig.(3)). A logical question that needed to be addressed was whether or not this friction induced shear force will affect the fatigue life of the specimens. Also how may friction shear stress be included in Nasgro’s TC03 model? To address these questions a parametric study has been conducted. The study involves partitioning the FEA calculated friction forces and adding a certain fraction of it into the bearing load (P) and bypass stress (So) of Nasgro’s TC03 while maintaining force equilibrium of the model.
Fig. 6: NASGRO TC03 library model and the corresponding section stresses for ^ = 0.6. The stress at Sec.2 corresponds to the bypass stress So on TC03. The bearing load P is also obtained from the finite element analysis.
Four analysis cases were considered: (1). TC03-1 all the friction force is added onto the bearing hole P, (2). TC03-2 half of the friction force is added onto bearing load P and the other half is added onto the bypass stress So, (3). TC03-3 half of the friction force is added onto the bearing load and the other half is ignored (thrown away), (4). TC03-4 all the friction force is ignored. These four cases were simulated with the scaled flight spectrum loads and results are compared with experimental data.
Results and discussions
Figure (7) presents crack size vs. log-cycles for the spectrum load specimens (B&C) considered in this work. In each life prediction plots are five curves consisting of TC13 and the four cases of TC03 discussed above. Simulation results for strip-yield interaction model are also shown. In all TC03 cases, the simulations considering any portion of the friction shear stress resulted in highly conservative life estimates. The 50-50 approach (case 2), i.e., dividing the friction into two and adding it into bearing and bypass stresses has resulted in insignificant life change compared to the 100% on-bearing (case 1). A big jump, however, is observed when half of the friction is added into the bypass stress and the other half is ignored. Better TC03 correlation with the experimental data was observed when the effect of friction shear stress is ignored altogether. This observation seems to contradict the finite element simulations that have shown significant stress field around the fastener holes as seen in Fig.(5). One possible explanation for this disparity could be made by observing that; the friction shear forces do cancel each other i.e. the friction shear distribution above and below the crack plane act in the same direction so that one half of these force aids the crack opening force whereas the other half tends to close the crack with the same magnitude. These actions resulted in a net zero crack plane displacement as verified by the good correlation of TC03-4 with the experimental data. The crack retardation models (strip-yield) in general have resulted in the prediction curves to shift slightly to the right. This is always true since the crack opening stress Kopen is higher when crack advances in the wake of plastically deformed material[?]. Figure (8) compares the stress intensity factors calculated by the 3D FEA analysis and the 2D Nasgro simulation. The observed close correlation between FEA SIF and TC13 and TC03-4 SIF values justified the accuracy of the 2D assumption made at the beginning of the analysis.
Fig. 7: Comparison of numerical simulations and experimental data for specimen-B (left two plots) and specimen-C(right two plots). The four cases of friction are shown as TC03-1 through -4. The upper plots show crack length vs. cycle without considering load interaction (load history) and the lower two plots show results for strip-yield interaction model. Better correlation with experimental data is observed for TC13 and TC03-4 simulations with strip-yield interaction option engaged.
Numerical fatigue crack growth analysis on a representative rotorcraft structural component has been presented. The later is a riveted joint used on cabin frame splice of several military and civilian rotorcrafts. The stress field around the critical hole resulting from the combined action of applied load, fastener preload and friction are obtained using 3D finite element analysis. Fatigue crack growth and life prediction is performed using Nasgros TC03 and TC13 library models with and without load interactions. In general, Nasgro crack growth prediction using TC13 (with crake plane stress gradient input from 3D FEA) shows a better agreement with the experimental data. TC03 predictions without the inclusion of contact friction also provided a well correlated life estimate. However, inclusion of any portion of friction stress in the analysis has resulted in a highly conservative life prediction by the model. Effort is still underway to further refine the analysis with more experimental data.
Fig. 8: Comparison of stress intensity factors calculated by 3D finite element analysis and NAS-GRO’s 2D models TC13 and the four cases of TC03.