6.4. Cohesive zone modeling
Classic fracture mechanics is an indispensable design tool that provides the basis for structural integrity assessment in engineering standards. The need to design components that exploit material performance to its maximum has however shifted scientific research from stationary cracks to crack propagation and damage. This is particularly true in ductile metals or composites, where a stable crack propagation stage precedes catastrophic failure. Among the many damage mechanics tools available, cohesive zone models are particularly attractive to characterize the reserve strength of the system once cracking has occurred, and to design accordingly (Cornec et al., 2003). The pivotal ingredient of cohesive zone modeling is the traction-separation law that governs material degradation and separation. As depicted in Figure 1, for a given shape of the traction-separation curve, the cohesive response can be fully characterized through two parameters, the cohesive energy and the critical cohesive strength . Thus, for the bi-linear law of Figure 1, the cohesive energy can be expressed as a function of the critical separation and the critical cohesive strength ,
Figure 1: Bi-linear traction separation law characterizing the cohesive zone model.
The two parameters governing the cohesive response can be inferred from experiments. Generally, a trial and error procedure is followed, but such methodology is time consuming and error-prone. Here, a novel technique to estimate the parameters governing the traction-separation law is proposed that builds on inverse analysis and neural network optimization. Abaqus2Matlab enables such approach, not only by linking the advanced optimization tools available in Matlab with Abaqus damage modeling outcomes, but also by allowing to read and modify Abaqus input files accordingly. Thus, not only is Abaqus2Matlab useful for post-processing purposes but it can be also used to optimize and pre-process through a two-way interaction between Abaqus and Matlab.
The material under consideration in the present study is Aluminum 2024. Both uniaxial and Compact Tension tests have been performed. The former lead to a Young's modulus of = 85826 MPa (Poisson's ratio = 0.33) while the plastic behavior can be fitted through a Hollomon's law with = 733 and = 0.157. As depicted in Figure 2, the specimen has a width of = 50 mm, a thickness of = 20 and a total crack length of = 17.323 mm, being the fatigue pre-crack equal to = 7.323 mm.
Figure 2: Geometry and dimensions of the Al2024 Compact Tension specimen.
The optimization procedure proposed correlates numerical results and experimental data of load versus crack mouth opening displacement (CMOD) by following the flowchart shown in Figure 3. Thus, the first step involves assigning a set of initial values to and . These initial values should be chosen so as to span a considerably wide range, ensuring that the optimal solution falls inside. The more numerous the merrier, as the performance of the neural network increases with the number of points. Nevertheless, only 5 pairs of vs points will be employed in this example to show the model capabilities even with a few initial values (see Figure 4a).
Figure 3: Neural network optimization flowchart.
The finite element calculations are then performed, where Abaqus capabilities to model cohesive zone damage are employed and a very refined mesh of quadrilateral quadratic plane strain elements with reduced integration is adopted. The curve load versus CMOD is obtained in Abaqus2Matlab by reading the nodal reaction forces and the displacement in particular sets (record keys 104 and 101 respectively). Computations are efficiently performed for each pair of - values by taking advantage of Abaqus2Matlab capabilities to read and modify Abaqus' input file. The results obtained in each case are shown in Figure 4b; each curve is characterized by 12 equally distant points so as to correlate with the experimental data.
Figure 4: Initial neural network training steps, (a) First set of - values, and (b) corresponding load versus crack mouth opening displacement curves.
The next step involves training the neural network based on the input ( and values) and output (load versus CMOD curves) information. The network is composed of 10 hidden layers and is trained by employing the Bayesian Regulation Method available in Matlab (see Figure 5); full advantage of the Neural Net Fitting Matlab App can be gained with Abaqus2Matlab. In this example, 80% of the models have been employed to train the network, 15% of them have been used for validation purposes and the remaining 5% serve to test the final solution obtained.
Figure 5: Graphical summary of the characteristics of the Neural Network employed.
Once the neural network is fitted and tested, it is used to estimate - through least squares fitting - the optimal values of and by minimizing the differences between the load-CMOD curve obtained from the model and its experimental counterpart. To assess the quality of the neural network prediction, the optimized values of the cohesive strength and the cohesive fracture energy are provided as input to the finite element model. The outcome of this new finite element analysis is compared to the experimental data. If the norm of the differences between the curves is higher than a given tolerance, the neural network is trained again by adding new input and output information from the previous iteration. Figure 6 shows the optimal values of the strength and the cohesive energy obtained in each iteration.
Figure 6: Cohesive strength and fracture energy estimations at each iteration.
In the present example convergence is achieved after 7 iterations and the final outcome is shown in Figure 7, together with the experimental result. As it can be seen in the figure, the optimal values ( = 199.2 MPa and = 61.81 N/mm) lead to a very good quantitative agreement with the load versus CMOD curve obtained experimentally.
Figure 7: Experimental and numerically optimized predictions of load versus crack mouth opening displacement in Al2024.
Hence, quantitative insight into the initiation and subsequent propagation of damage can be obtained through neural network optimization and a hybrid experimental-numerical strategy, in what is usually referred to as a top-down approach (Martinez-Paneda et al., 2016). Thus, Abaqus2Matlab largely facilitates structural integrity assessment by taking advantage of advanced damage models available in Abaqus and modern optimization capabilities of Matlab. Moreover, its usage can be easily extended to a wide range of non-linear problems, where inverse analysis is an indispensable tool.
Abaqus2Matlab - www.abaqus2matlab.com
Copyright (c) 2017 by George Papazafeiropoulos
If using this application for research or industrial purposes, please cite:
G. Papazafeiropoulos, M. Muniz-Calvente, E. Martinez-Paneda.
Abaqus2Matlab: a suitable tool for finite element post-processing.
Advances in Engineering Software. Vol 105. March 2017. Pages 9-16. (2017)
Created with an evaluation copy of HelpSmith.
To remove this notice, you should purchase the full version of the product.