Products: ABAQUS/Standard ABAQUS/Explicit
This example verifies and illustrates the use of ABAQUS to predict mixed-mode multidelamination in a layered composite specimen. Cohesive elements or connector elements are used to represent the bonded interfaces. The problem studied is the one that appears in Alfano (2001). The results presented are compared against the experimental results included in that reference, taken from Robinson (1999). The model with cohesive elements is analyzed in ABAQUS/Standard as well as ABAQUS/Explicit, using a damaged, linear elastic constitutive model.
The problem geometry and loading are depicted in Figure 2.7.1–1: a layered composite specimen, 200 mm long, with a total thickness of 3.18 mm and a width of 20 mm, loaded by equal and opposite displacements in the thickness direction at one end. The thickness direction is composed of 24 layers. The model has two initial cracks: the first (of length 40 mm) is positioned at the midplane of the specimen at the left end, and the second (of length 20 mm) is located to the right of the first and two layers below.
When cohesive elements are used, the problem is modeled in both two and three dimensions, using solid elements to represent the bulk behavior and cohesive elements to capture the potential delamination at the interfaces between the 10th and 11th layers and between the 12th and 13th layers, counting from the bottom. In the two-dimensional finite element model the top part of the specimen consisting of 12 layers, the middle section of 2 layers, and the bottom part of 10 layers are each modeled with a mesh of 1 × 200 CPE4I elements in ABAQUS/Standard and CPE4R elements in ABAQUS/Explicit. In both ABAQUS/Standard and ABAQUS/Explicit the initially uncracked portions of the two interfaces are modeled by one layer each of COH2D4 elements that share nodes with the adjacent solid elements. A similar, matching mesh is adopted for the equivalent three-dimensional model, where the corresponding element types used are C3D8I and COH3D8 in ABAQUS/Standard and C3D8R and COH3D8 in ABAQUS/Explicit, with one element in the width direction. The nodes where the equal and opposite displacements are prescribed are constrained in the length direction of the specimen; these are the only boundary conditions in the two-dimensional case. For the equivalent three-dimensional model all the nodes are also constrained in the width direction to simulate the plane strain effect. In addition, contact is defined between the open faces of the second, pre-existing crack to avoid penetrations if the faces are compressed against each other during the analysis.
When connector elements are used, the problem is modeled only in two dimensions in ABAQUS/Standard. Two node-based surfaces are generated: one along the top surface of the tenth layer and the other along the bottom surface of the eleventh layer. Both surfaces are tied to adjacent layers using surface-based tie constraints. CARTESIAN connector elements are used to bond the two node-based surfaces together to represent the interface. For the interface between the twelfth and thirteenth layers, matched solid element nodes along the interface are connected directly using connector elements.
The material data given in Alfano (2001) for the bulk material composite properties are 
GPa, 
GPa, 
GPa, 
, 
, 
, 
GPa, 
GPa, and 
GPa.
The response of the cohesive elements in the model is specified through the cohesive section definition as a “traction-separation” response type. The elastic properties of the cohesive layer material are specified in terms of the traction-separation response with stiffness values 
MPa, 
MPa, and 
MPa. The quadratic traction-interaction failure criterion is selected for damage initiation in the cohesive elements; and a mixed-mode, energy-based damage evolution law based on a power law criterion is selected for damage propagation. The relevant material data are as follows: 
MPa, 
MPa, 
MPa, 
× 103 N/m, 
× 103 N/m, 
=0.80 × 103 N/m, and 
.
Force-based damage initiation and a tabular form of motion-based damage evolution are used to define the connector damage mechanisms. Initiation forces are calculated based on the value of 
given above for cohesive elements. For example, the initiation force for the lower interface is calculated as 66 N, which is equal to 
× A. The interface area over one cohesive element, A, is 20 × 10–6. The stiffnesses of the connector elements are calculated as 
× 109 N/m, where L is the thickness of the cohesive element. To improve the convergence behavior of this model, viscous regularization has been applied to the model.
For the cohesive element models the plots of the prescribed displacement versus the corresponding reaction force for the delamination problem are presented in Figure 2.7.1–2 and compared with the experimental results included in Alfano (2001). Both the ABAQUS/Standard and ABAQUS/Explicit results displayed in the graph are from the two-dimensional analyses. The results from the equivalent three-dimensional models are almost identical to their two-dimensional counterparts and are not included in Figure 2.7.1–2. Good agreement is observed between the cohesive element predictions and the experimental results up to an applied displacement of approximately 20 mm. As seen from Figure 2.7.1–2, a sharp drop in the reaction force is predicted at this point by the ABAQUS analysis, after which the reaction force values appear to be underpredicted by approximately 30% when compared to the experimental data. The reason for this deviation, which appears to coincide with the simultaneous propagation of both the cracks, is related to the sudden failure of a relatively large number of cohesive elements in a very short period of time. While the ABAQUS/Explicit results follow the same pattern as the ABAQUS/Standard results, they are not as smooth due to inertia effects. A second-order Butterworth-type filter was applied to the nodal reaction force history output from the ABAQUS/Explicit analysis to eliminate high-frequency oscillations from the response curve.
Figure 2.7.1–3 shows the results from a series of ABAQUS/Standard analyses incorporating a viscous regularization scheme to improve convergence and demonstrates the effect on the predicted results of the choice of the viscosity parameter, μ. Larger values of μ, while providing better convergence, affect the results more than smaller viscosity values. The appropriate value of the viscosity parameter that results in the right balance between improved convergence behavior of the nonlinear system and accuracy of the results is problem dependent and requires judgement on the part of the user. In the cohesive zone approach to modeling delamination, the complex fracture process at micro-scale is modeled using only a few macroscopic parameters (such as peak strength and fracture energy). While viscous regularization is not intended to be used to model rate effects, it does provide an additional parameter that can be “fitted” to the material model at hand. For the particular delamination problem analyzed, as can be seen from Figure 2.7.1–3, a larger value of μ causes the first peak of the reaction force curve to be higher than the experimental value and predicts a milder and smoother drop in the reaction force following the peak compared to the experimental data. However, the results with viscous regularization (for example, the curve for μ = 1.0 × 10–4 in Figure 2.7.1–3) appear to match the experiments better for prescribed displacement values greater than 20 mm.
Figure 2.7.1–2 also shows the results from the analysis using connector elements to model the bonded interfaces. The same trend of delamination is observed as seen in the experimental data. Figure 2.7.1–4 illustrates the effect of viscous regularization. In one case a viscous regularization factor of 0.0008 and maximum degradation factor of 0.99 are used. In the other case the values are 0.0005 and 0.9, respectively. As can be seen in Figure 2.7.1–4, a larger value of viscous regularization causes the peak of the reaction force to be higher.
ABAQUS/Standard two-dimensional model.
ABAQUS/Standard two-dimensional model using viscous regularization.
ABAQUS/Standard three-dimensional model.
ABAQUS/Explicit two-dimensional model.
ABAQUS/Explicit three-dimensional model.
ABAQUS/Standard two-dimensional model using connector elements and a viscous regularization factor of 0.0005.
ABAQUS/Standard two-dimensional model using connector elements and a viscous regularization factor of 0.0008.
Script for creating the two-dimensional version of this model using ABAQUS/CAE.
Alfano, G., and M. A. Crisfield, “Finite Element Interface Models for the Delamination Analysis of Laminated Composites: Mechanical and Computational Issues,” International Journal for Numerical Methods in Engineering, vol. 50, pp. 1701–1736, 2001.
Robinson, P., T. Besant, and D. Hitchings, “Delamination Growth Prediction Using a Finite Element Approach,” 2nd ESIS TC4 Conference on Polymers and Composites, Les Diablerets, Switzerland, 1999.
