A systematic numerical investigation was conducted in this study, using a total of three different models in order to establish the integrity of the xFEM and CZM facilities of LS-DYNA. First, a model that was analyzed by another investigator [

1] was tried to validate the integrity of our approach. Then, since the configuration of the materials forming our 3D-FML is relatively complex, it was decided to initially simulate the response of the standard double cantilever beam to further hone our skill in using the xFEM and calibrate the properties required for conducing such analysis. Finally, the response of a less-complex equivalent model of our 3D-FML material, subjected to an axial impact, was simulated.

As briefly mentioned, the first trial involved simulation of the response of a simply-supported rectangular cross-section cast iron beam specimen subjected to an impact load at its mid-span using xFEM. The parameters required for xFEM simulation of the specimen were extracted from reference [

1]. It should be noted that the efficient approach commonly used in simulating such simple 3D geometries is by modeling them as either 2D plane-stress or plane-strain geometry, depending on the aspect ratios of the specimen. Therefore, an attempt was made to simulate the beam’s response by a plane-strain model. However, a convergent result could not be achieved when the xFEM was used in conjunction with the 2D plane strain element of LS-DYNA (even though LS-DYNA user-manual explicitly states admissibility of that element type in conjunction with xFEM). Consequently, LS-DYNA’s shell elements (type 54 in conjunction with the fully integrated base element 16) were used to continue the modeling effort. It is reckoned that shell elements are not used conventionally to simulate such geometries (i.e., geometries with an appreciable thickness-to-depth ratio); nonetheless, an accurate fracture response could be successfully predicted in comparison to the experimental results reported by Tsuda et al. [

1] (who incidentally used the same approach in modeling the specimen’s response). A detailed explanation of the modeling approach, as well as the discussion of the required parameters, are presented in the

Appendix A. In addition, the value of the parameters used in our models are given in

Table A1.

The simulated results confirmed the integrity of the selected algorithm and element type; thus, they were used in the subsequent phases of the analysis. However, before continuing with the remaining analyses, it warrants to discuss the material model and the required parameters that will be required when conducting xFEM modeling.

#### 2.1. Material Model for Cohesive and xFEM Elements

In LS-DYNA, only one material model is currently available for use in conjunction with the xFEM formulation, which is: *MAT_COHESIVE_TH. This is a cohesive material law proposed by Tvergaard and Hutchinson [

29] with tri-linear traction-separation behavior (see

Figure 1a), where the maximum traction stress and normal or tangential ultimate displacements are the governing and required parameters [

30]. The model accepts only one value of the maximum stress; therefore, it could be either the maximum normal stress or maximum shear stress, accordingly. In this study, because mode I fracture is the dominant failure mode, the maximum tensile stress is chosen as the maximum stress governing the failure of the material. Note that the lack of differentiation between the maximum normal and shear stresses is an important limitation of this model.

This cohesive model is based on the non-dimensional parameters λ

_{1}, λ

_{2,} and λ

_{fail}, defining the traction-separation law behavior, as shown in

Figure 1. These parameters correspond to various segments of the traction-separation curve (i.e., the peak traction, the beginning of softening segment, and the final failure, respectively). In other words, these parameters are used to represent a measure of the global dimensionless separation, λ, mathematically represented for the two-dimensional case as follows:

where

${\delta}_{N}$ and

${\delta}_{T}$ are the normal and tangent separation displacements,

${\delta}_{N}^{fail}$ and

${\delta}_{T}^{fail}$ are the respective separation values at failure, and the operator 〈

$\xb7$〉 refers to the Mc-Cauley brackets, used to differentiate the behavior under tension and compression.

The stress state is computed, using the trilinear traction-separation law parameters (see

Figure 1), as follows:

where

${\sigma}_{max}$ refers to the maximum tensile or shear stress, as mentioned previously.

Using a potential function, φ, defined as:

and the normal surface traction,

${\sigma}_{N}$, and the tangential surface traction,

${\sigma}_{T}$, are expressed by the following derivatives:

Finally, the development of the derivatives leads to the traction vector, expressed as:

This model is totally reversible, in other words, the loading and unloading follow the same path. In addition, the difference in behavior between tension and compression is accounted for, with the following equation describing the behavior for

${\delta}_{N}<0$:

where κ is the penetration stiffness multiplier, defined by the user.

As mentioned previously, the tri-linear behavior is controlled by the three non-dimensional parameters, which affect term A in the following equation. These parameters are related to the material’s fracture toughness, G

_{IC} or G

_{IIC} in the following manner:

where the subscript “i” relates to the normal or tangential directions and

A is the area under the normalized traction-separation curve (see

Figure 1a,b).

The cohesive parameters used in this investigation, as reported in the

Appendix A, were obtained by calibrating the trial values in such a way that the numerical simulation-produced results would closely match the results obtained through the actual testing of the double cantilever beam (DCB) specimen, using the load-opening curve as the criterion, as shown in

Figure 1c. It should be noted that the experimental test data of DCB was obtained under a static loading, while the simulation of the 3D-FML specimen of our interest, as will be presented later, was carried out when the specimen was subjected to an impact loading state; therefore, there would be some discrepancies between the evaluated values and those exhibited by the actual specimen dynamically. The establishment of the CZM parameters as explained is based on matching the overall behavior, which would not include while the fluctuations that could potentially develop locally. However, in this paper, the authors’ intent is to demonstrate the feasibility of the described method, not its accuracy. The selected calibration method is meant to simply establish the values of the cohesive zone’s parameters used to facilitate the simulation. Moreover, the xFEM formulation is currently only available under the dynamic, explicit solution scheme of LS-DYNA. Therefore, to ensure a reasonable solution time, all the simulations were run in dynamic mode, with the simulated event being in the order of a millisecond.

It is also worth mentioning that, during the calibration, no significant difference was found when reducing the tri-linear law to a bi-linear one (see

Figure 1b), which facilitates a more CPU-efficient numerical solution. Consequently, λ

_{1} and λ

_{2} were both set to 0.5, thereby reducing the tri-linear model to a bi-linear model. Note that some researchers [

31,

32] have recommended the use of an initially-rigid cohesive law (i.e., λ

_{1} = λ

_{2} ≅ 0) for obtaining a more reliable estimation of the state of stress prior to the onset of a crack. However, numerical instabilities were encountered when the approach was adopted in this study. Moreover, this is not to say that adaptation of the tri-linear law and/or the initially rigid cohesive response would lead to similar issues when simulating other cases. It should be noted that the main objective of the study presented here is to demonstrate the potential of the xFEM method in simulating the response of a complex material system under a relatively complex loading state, as opposed to targeting the degree of accuracy that could be attained when using the technique. Consequently, no further calibration effort was expended towards this issue.

Finally, as mentioned earlier, this cohesive model is the only one available for use within xFEM in LS-DYNA. Therefore, for the sake of consistency, this model was also used with the cohesive elements, even though other cohesive models are available that could potentially produce more accurate predictions in the case of mixed mode fracture.

#### 2.2. xFEM’s Formulation

Here, a brief description of the xFEM formulation is presented. Consider a domain, noted Ω, that includes a crack represented by a surface discontinuity ∂Ω, as shown in

Figure 2. In xFEM, the following distance function (i.e., the function mapping the position of the closest points to the discontinuity), is used to represent the crack in Ω:

where

$\underset{\_}{x}$ is the position vector,

$\widehat{\underset{\_}{x}}$ is the position of the closest point that is projected onto the discontinuity surface ∂Ω, and

$\underset{\_}{n}$ is the unity vector normal to ∂Ω. Therefore, the discontinuity is represented by

$f\left(\underset{\_}{x}\right)=0$, and the sign of the function refers to each part of the domain, with positivity determined by

$\underset{\_}{n}$.

In order to account for the presence of the discontinuity, the element formulation is enriched for the elements concerned by the crack. Let

I be the set of all the nodes within the domain Ω and

J be the set of all the nodes belonging to the enriched elements, excluding the one containing the crack tip, which is assigned to the set

K. The nodal variable (e.g., displacement) can, therefore, be represented by [

1]:

where

${\underset{\_}{u}}_{i}$,

${\underset{\_}{u}}_{i}^{\ast}$ and

${\underset{\_}{u}}_{i}^{\ast \ast}$ are the regular and enriched nodal variables and

${N}_{i}$,

${N}_{i}^{\ast}$ and

${N}_{i}^{\ast \ast}$ are the regular and enriched shape functions. The enriched shape functions are as follow:

and

where

H is the Heaviside function and

$\beta (r,\theta )=\{\sqrt{r}\mathrm{cos}\frac{\theta}{2},\sqrt{r}\mathrm{sin}\frac{\theta}{2},\sqrt{r}\mathrm{sin}\theta \mathrm{sin}\frac{\theta}{2},\sqrt{r}\mathrm{sin}\theta \mathrm{cos}\frac{\theta}{2},\}$, with

r and

θ given in

Figure 2.

Note that the previously defined cohesive material behavior is used to obtain the crack opening displacement, and either the maximum principal stress or the maximum shear stress can be used as a criterion to establish the onset of crack propagation and its direction (noting that the former criterion is used in our models). When the criterion is reached within the element containing the current crack tip, the element is considered as failed and the crack tip is advanced by one element.

#### 2.3. Double Cantilever Beam Model

The first of the two models, whose results are presented in this study, is the double cantilever beam (DCB), which is commonly used to assess the interlaminar fracture toughness of composite materials [

33]. This model, whose geometry and boundary conditions are illustrated in

Figure 3a, was used to assess the feasibility of the contemporary use of xFEM and cohesive elements for modeling crack propagation within the adhesive layer bonding the two adherends of DCB. In addition, as briefly explained earlier, the case was used to tune the materials properties that are required as input by both xFEM and cohesive elements.

The overall model’s specimen dimensions are 150 mm × 25 mm × 9 mm, with the initial crack length of 50 mm embedded within the mid-plane of the adhesive, in one end of the specimen, (see

Figure 3a). This model is a simplification of the hybrid composite used for the experimental tests, consisting of a hybrid magnesium sheet and FRP forming the upper adherend, and biaxial FRP forming the lower adherend. It should be noted that, to further simplify the analysis (without compromising the overall accuracy), each of the two 4-mm thick adherends was homoginzed into an equivalent elstic material. In this way, the equivalent materials had the same flexural stiffness as the combined hybrid materials, but the analysis would concume significantly less CPU. The adopted scheme also facilitates more effective debugging. The 1-mm thick adhesive layer was modeled in three ways, by using (i) a combination of elastic and cohesive elements, as shown in

Figure 3b, (ii) xFEM elements only, as shown in

Figure 3c, and (iii) a combination of xFEM and cohesive elements, as shown in

Figure 3d. These models are referred to as COHESIVE, XFEM, and MIXED, respectively, hereafter. The same cohesive material model was used in conjunction with both cohesive and xFEM elements; moreover, the xFEM elements were also assigned elastic model properties. In other words, the elements defined as xFEM would initially behave elastically until the stresses reach to a level at which xFEM’s enrichment is activated, thereby using the assigned cohesive properties. It should be noted that one could also assign other material models (e.g., elasto-plastic) to the xFEM elements instead of the elastic model [

32].

The generation of the precrack, for the XFEM and MIXED models, was done using the *BOUNDARY_PRECRACK keyword, which enriches the elements to account for the presence of an initial crack. Note that the conventional practice in fracture mechanics, that is, having a series of disconnected adjacent layers of elements to model the crack, cannot be used in conjunction with xFEM elements. This is because xFEM element formulation allows for the crack to propagate only within the element. For the COHESIVE case, however, the crack was generated as done conventionally, that is by simply deleting the appropriate number of elements corresponding to the location of the actual crack/delamination. Therefore, to maintain consistency of the results when comparing the results generated by the three models, only the elements forming a portion of the adhesive that would be cracking (i.e., at the midplane of adhesive) were modeled by the cohesive material model, while the remaining portions were modeled with the elastic model, hereafter referred to as “elastic element”. This approach also saves the CPU time.

Finally, the adhesive layer was discretized with seven layers of elements as shown in

Figure 3 and its density was kept constant along the bond length. The mesh density was stablished upon conducting a convergence study by which a reasonable accuracy could be attained by consuming an optimal CPU time.

#### 2.4. Delamination-Buckling Analysis

The delamination-buckling of an initially partially delaminated clamped-clamped fiber-metal laminate subjected to an axial impact was simulated, with the geometry and dimensions of the original sample reported in

Figure 4a. An equivalent simplified model, as shown in

Figure 4b, consisting of three components was constructed. The model consisted of a 0.5-mm thick magnesium skin, a 0.5-mm thick adhesive layer, and a 2-mm thick fiberglass substrate. The symmetry in geometry and boundary conditions warranted modeling only one-half of the specimen, thus, reducing CPU computation. As shown in

Figure 4b, the transverse displacement (

u_{y}) of the nodes located at the far-end of the specimen was restrained, and the same nodes were displaced at a rate of 1 m/s in the negative x-direction (-

u_{x}), to simulate the applied impact. In addition, the rotation (in xy-plane) of the nodes were also restrained. This combination of restrains mimics the actual clamped boundary condition. As also shown in the figure, the symmetric boundary condition at the left end of the half-symmetry model was ensured by restraining the longitudinal displacement (

u_{x}) and rotation about the y-axis at that location, while displacement in the transverse direction was permitted. Lastly, the out-of-plane displacement of all nodes (i.e., (

u_{z})) was restrained to guarantee a purely planar deformation.

Similar to the DCB specimen’s model, the adherends of the FML were modeled using elastic elements, while the adhesive layer was modeled using (i) the cohesive element only and (ii) a combination of both xFEM and cohesive elements. Moreover, similar to the previous case-study, the models will be referred to as COHESIVE and MIXED. The XFEM model was not considered here because of the inconsistent results obtained when the xFEM element was used in modeling the DCB, as will be discussed in

Section 3.1. Moreover, the adhesive thickness was assumed to be 0.5 mm, so to facilitate more discrete simulation of the influence of the through-thickness location of a crack within the adhesive layer. Therefore, the mesh, established based on a convergence study, has nine layers of elements through the thickness of the adhesive.

In addition, the upper and lower delaminated portions of the specimen were assumed to have a sinusoidal geometric imperfection with small amplitudes of 0.1 mm and −0.02 mm in the y-direction, respectively, to promote the instability and to ensure that the upper and lower adherends would deflect in two opposite directions.