Mixed-Mode Debonding of a Laminated Composite

Interfacial failure by delamination or debonding is one of the main failure modes of laminate structures. Such failures can be simulated with a cohesive zone model (CZM). A key ingredient of a cohesive zone model is a traction-separation law that describes the softening in the cohesive zone near the delamination tip. This example shows how to model debonding using the decohesion model in COMSOL Multiphysics. The capabilities of the CZM to predict mixed-mode softening and delamination propagation are demonstrated in a model of the mixed-mode bending of a composite beam.

Model Definition

Cohesive Zone Model (CZM)

The CZM is in this example defined using the displacement-based damage model available in the node under . The model is used to predict crack propagation at the interface of a laminated composite beam under mixed-mode loading. The material properties needed for this constitutive model are summarized in Table 1.

Table 1: Summary of material properties of the CZM interface. The values are for AS4/PEEK.
Property	Symbol	Value
Normal tensile strength	σt	80 MPa
Shear strength	σs	100 MPa
Penalty stiffness	pn	106 N/mm3
Critical energy release rate, tension	Gct	969 J/m2
Critical energy release rate, shear	Gcs	1719 J/m2
Exponent of the Benzeggagh and Kenane (B-K) criterion	α	2.284

The CZM is defined using a bilinear traction-separation law. Traction increases linearly with a stiffness pn until the opening crack reaches a damage initiation displacement u0. When the crack opens beyond u0, the material softens irreversibly and the stiffness decreases as a function of increasing damage d. The material fails once the stiffness has decreased to zero, i.e. when d = 1. This happens at the ultimate displacement uf.

The values of u0 and uf depend on whether the separation displacement is normal (mode I) or tangential (mode II and III) to an interface. For the mixed mode, a combination is used. For the displacement based damage model, two different criteria are available to define this combination. Here the model by Benzeggagh and Kenane is used.

Mixed-mode bending of a laminated composite beam

A commonly used method to measure the delamination resistance of composite materials is the mixed-mode bending (MMB) test, see Ref. 1 and Ref. 2. This experimental procedure is here modeled to demonstrate the capabilities of the CZM.

The geometry of the test specimen is illustrated in Figure 1. It consists of a beam cracked along a ply interface halfway through its thickness. The initial crack length is cl. The beam is supported at the outermost bottom edges. A mixed-mode bending load is produced as the result of forces applied to the top edges at the cracked end and at the center of the beam.

Because of the symmetry, only half of the beam is modeled and a boundary condition is applied.

Figure 1: The geometry of the test specimen.

The material properties are those of AS4/PEEK unidirectional laminates. The orthotropic linear elastic properties assume that the longitudinal direction is aligned with the global X direction. The material properties of the laminate composite are listed in Table 2.

Table 2: Laminated composite material properties.
Property	Symbol	Value
Young’s modulus, along fibers	EX	122.7 GPa
Young’s modulus, across fibers	EY=EZ	10.1 GPa
Poisson’s ratio	νYZ	0.45
Poisson’s ratio	νXY=νXZ	0.25
Shear modulus	GYZ	3.7 GPa
Shear modulus	GXY=GXZ	5.5 GPa

The beam is supported on the bottom at its outer edges. A lever that sits on top of the beam applies a load. The lever is also attached to the cracked end and swivels around a contact area at the center of the beam. The lever is pushed down at the opposite free end, thereby simultaneously applying mode I and mode II loads on the test specimen. Arbitrary ratios of mixed-mode loading can be adjusted by varying the length of the lever ll.

In this example, the lever is omitted. Instead, the forces that the lever transmits to the beam are applied directly. A pulling force Fe is acting on the cracked side of the beam. At the center, a force Fm pushes down. The desired mixed-mode ratio mm regulates the ratio of their magnitudes lr via

Further details on the background of the equation above can be found in Ref. 1 and Ref. 2.

Results and Discussion

The model is analyzed for a mixed-mode ratio of 50%. The von Mises stress distribution of the last computed parameter step is shown in Figure 2. At this step the initial crack has propagated along the interface as shown in Figure 3. The crack now extends beyond the center of the beam.

Figure 2: The Von Mises stress distribution at the last computation step.

Figure 3: Plot showing the health of the laminate interface. The debonded part is shown in red, the intact part in green.

One of the outputs of the MMB test is a load-displacement curve. Both the load and displacement are measured at the endpoint of the lever that is used to apply the load to the test specimen. Since the lever is not explicitly modeled, the load-displacement data has to be deduced from the simulation results. Details of the analysis are contained in Ref. 1 and Ref. 2, with the following result.

The force Flp at the load point of the lever can be determined from the load applied to the cracked edge in the model Fe and the lengths of the test beam lb and load lever ll:

The length of the load lever above depends on the desired mode mixture mm:

ll measures the length from the center of the test specimen to the free end of the load lever.

The displacement at the load point ulp is computed from the mode I opening at the cracked edge uIe and the z-displacement at the center of the beam wc according to

The resulting load-displacement curve is shown in Figure 4. The curve confirms what Figure 3 displayed. The maximum load that the beam with the initial crack can carry is exceeded and delamination occurs. After exceeding a peak load, the load decreases until the displacement reaches around 7 mm. This point approximately corresponds to when the crack reaches the center of the specimen. Thereafter, the load starts to increase again, but with a much lower stiffness than before delamination.

Figure 4: Load-displacement curve of the MMB test at 50% mixed-mode loading.

Notes About the COMSOL Implementation

To implement a cohesive zone model in COMSOL Multiphysics, use the node with an subnode and a subnode. Notice that requires an active subnode.

Since no large relative deformations of the laminates are expected, the contact search can be made in the initial configuration. Setting the to in the node significantly improves the performance of the model.

To trace the solution after the peak load, the simulation must be displacement controlled. This is obtained by using a global equation, in which the distributed load is controlled by the sweep parameter, which is the displacement at the free edge.

The resolve the decohesion at the interface, a dense mesh is used in the zone where delamination is expected. If the mesh elements were too large, the crack could jump several elements in one parameter step, resulting in an unstable solution.

Reference

1. P.P. Camanho, C.G. Davila, and M.F. De Moura, “Numerical Simulation of Mixed-mode Progressive Delamination in Composite Materials,” Journal of composite materials 37.16 (2003): 1415–1438.

2. J.R. Reeder, and J.R. Crews Jr., “Mixed-mode bending method for delamination testing,” AiAA Journal 28.7 (1990): 1270–1276.

Structural_Mechanics_Module/Contact_and_Friction/cohesive_zone_debonding

Modeling Instructions

From the menu, choose .

New

In the window, click

Model Wizard

In the window, click

In the tree, select .

Click .

Click

In the tree, select .

Click

Global Definitions

Load all model parameters from a file containing parameters for the geometry, material properties and boundary conditions.

Parameters 1

In the window, under click .

In the window for , locate the section.

Click

Browse to the model’s Application Libraries folder and double-click the file cohesive_zone_debonding_parameters.txt.

Geometry 1

In the window, under click .

In the window for , locate the section.

From the list, choose .

Now draw the model geometry with three layered blocks.

Block 1 (blk1)

In the toolbar, click

In the window for , locate the section.

In the text field, type lb.

In the text field, type wb/2.

In the text field, type hb/2.

Block 2 (blk2)

In the toolbar, click

In the window for , locate the section.

In the text field, type lb/2-cl.

In the text field, type wb/2.

In the text field, type hb/2.

Locate the section. In the text field, type cl.

Union 1 (uni1)

In the toolbar, click

and choose .

Click in the window and then press Ctrl+A to select both objects.

Copy 1 (copy1)

In the toolbar, click

and choose .

Select the object only.

In the window for , locate the section.

In the text field, type hb/2.

Form Union (fin)

In the window, under click .

In the window for , locate the section.

From the list, choose .

In the toolbar, click

Definitions

Load variables for the load point from files.

Load Point Variables

In the toolbar, click

and choose .

In the window for , type Load Point Variables in the text field.

Locate the section. Click

Browse to the model’s Application Libraries folder and double-click the file cohesive_zone_debonding_load_point_variables.txt.

Integration Edge

In the toolbar, click

and choose .

The following nonlocal integration couplings make values of the selected points globally available.

In the window for , type Integration Edge in the text field.

Locate the section. From the list, choose .

Select Point 17 only.

Locate the section. From the list, choose .

Integration Center

In the toolbar, click

and choose .

In the window for , type Integration Center in the text field.

Locate the section. From the list, choose .

Select Point 26 only.

Locate the section. From the list, choose .

Contact Pair 1 (ap1)

Remove the boundaries that correspond to the initial crack from the contact pair.

In the window, click .

In the window for , locate the section.

Select the check box.

Locate the section. Select the

toggle button.

In the list, select .

Click

Select Boundaries 9 and 14 only.

Locate the section. Select the

toggle button.

In the list, select .

Click

Select Boundaries 24 and 29 only.

Since no large relative deformations of the laminates are expected, the contact search can be made in the initial configuration. This setting results in a significant speed up of the problem.

Locate the section. From the list, choose .

In the text field, type 1e-2.

Materials

Create a new material containing the orthotropic linear elastic properties of AS4/PEEK.

AS4/PEEK

In the toolbar, click

In the window for , type AS4/PEEK in the text field.

Click to expand the section. In the tree, select .

Click

Locate the section. In the table, enter the following settings:


Property	Variable	Value	Unit	Property group
Young’s modulus	{Evector1, Evector2, Evector3}	{122.7e9, 10.1e9, 10.1e9}	Pa	Orthotropic
Poisson’s ratio	{nuvector1, nuvector2, nuvector3}	{0.25, 0.45, 0.25}	1	Orthotropic
Shear modulus	{Gvector1, Gvector2, Gvector3}	{5.5e9, 3.7e9, 5.5e9}	N/m²	Orthotropic
Density	rho	1570	kg/m³	Basic