Figure 1.4.6–1 shows the geometry of the laminate containing the blunt notch for this example. The laminate is subjected to uniaxial tension in the longitudinal direction. The laminate is made of three layers of aluminum and two layers of 0°/90° glass fiber-reinforced epoxy. Only 1/8 of the laminate needs to be modeled, with appropriate symmetric boundary conditions applied as shown in Figure 1.4.6–2. Figure 1.4.6–2 also shows the through-thickness lay-up of the 1/8 model.

The material behavior of aluminum is assumed to be isotropic elastic-plastic with isotropic hardening. The Young’s modulus is 73800 MPa, and the Poisson’s ratio is 0.33; the isotropic hardening data are listed in Table 1.4.6–1.

The material behavior of the glass fiber-reinforced epoxy layers is assumed to be orthotropic, with stiffer response along the fiber direction and softer behavior in the matrix. The elastic properties—longitudinal modulus, ; transverse modulus, ; shear moduli, and ; and Poisson’s ratios, and —are listed in Table 1.4.6–2. The subscript “L” refers to the longitudinal direction (or fiber direction), and the subscript “T” refers to the two transverse directions orthogonal to the fiber direction. The damage initiation and evolution behavior is also assumed to be orthotropic. Table 1.4.6–3 lists the ultimate values of the longitudinal failure stresses, and ; transverse failure stresses, and ; and in-plane shear failure stress, . The superscripts “t” and “c” refer to tension and compression, respectively. The fracture energies of the fiber and matrix are assumed to be =12.5 N/mm and =1.0 N/mm, respectively.

Two material models that use the parameters listed above are considered, as follows:

The adhesive used to bond neighboring layers is modeled using interface layers with a thickness of t=0.001 mm. To simulate the interlaminar delamination, these interface layers are modeled with cohesive elements. The initial elastic properties of each interface are assumed to be isotropic with Young’s modulus E=2000 MPa and Poisson’s ratio =0.33. The failure stresses of the interface layers are assumed to be ===50 MPa; the fracture energies are ===4.0 N/mm. The subscripts “n,” “s,” and “t” refer to the normal direction and the first and second shear directions (for further discussion of the constitutive modeling methods used for the adhesive layers, see “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 26.5.6 of the ABAQUS Analysis User's Manual).

The plate is loaded with displacement boundary conditions applied at the right edge. To simplify the postprocessing, the displacement loading is applied at a reference point and an equation constraint is used to constrain the displacement along the loading direction between the right edge and the reference point. Except for those files designed exclusively to study the effect of the loading direction on the strength, the loading direction (along the global X-direction) aligns with the fiber direction of the 0° fiber-reinforced epoxy layer.

For fiber-reinforced epoxy, the primary model considered is based on the built-in damage model for fiber-reinforced composites available in ABAQUS. Alternatively, the damage in the fiber-reinforced epoxy is simulated using the model proposed by Linde et al. (2004), which is implemented in user subroutine UMAT and is discussed below.

In the UMAT model, the damage initiation criteria are expressed in terms of strains. Unlike the built-in model in ABAQUS, which uses four internal (damage) variables, the UMAT model uses two damage variables to describe damage in the fiber and matrix without distinguishing between tension and compression. Although the performance of the two models is expected to be similar for monotonic loads, such as in this example problem, the results obtained might differ considerably for more complex loads in which, for example, tension is followed by compression. For the UMAT model, if the material is subjected to tensile stresses that are large enough to cause partial or full damage (the damage variable corresponding to this damage mode will be greater than zero), both tensile and compressive responses of the material will be affected. However, in the case of the built-in damage model, only the tensile response will be degraded while the material compressive response will not be affected. In many cases the latter behavior is more suitable for modeling fiber-reinforced composites. In this section the governing equations for damage initiation and evolution as proposed by Linde et al. (2004) are discussed, followed by a description of the user subroutine UMAT implementation.

Damage in the fiber is initiated when the following criterion is reached:

During progressive damage the effective elasticity matrix is reduced by the two damage variables and , as follows:

In user subroutine UMAT the stresses are updated according to the following equation:

To improve convergence, a technique based on viscous regularization (a generalization of the Duvaut-Lions regularization) of the damage variables is implemented in the user subroutine. In this technique we do not use the damage variables calculated from the aforementioned damage evolution equations directly; instead, the damage variables are “regularized” via the following equations:

To update the “regularized” damage variables at time , the above equations are discretized in time as follows:

Care must be exercised to choose an appropriate value for since a large value of viscosity might cause a noticeable delay in the degradation of the stiffness. To estimate the effect of viscous regularization, the approximate amount of energy associated with viscous regularization is integrated incrementally in user subroutine UMAT by updating the variable SCD as follows:

This user subroutine can be used with either three-dimensional solid elements or elements with plane stress formulations. In the user subroutine the fiber direction is assumed to be along the local 1 material direction. Therefore, when solid elements are used or when shell elements are used and the fiber direction does not align with the global X-direction, a local material orientation should be specified. The damage variables—, , , and —are stored as solution-dependent variables, which can be viewed in the Visualization module of ABAQUS/CAE.

The finite element model uses a separate mesh for each of the respective layers shown in Figure 1.4.6–2: two aluminium layers, two fiber-reinforced epoxy layers, and three adhesive layers. While not required, a similar finite element discretization in the plane of the laminate, such as that shown in Figure 1.4.6–3, can be used for all layers.