COMSOL 6.4 - Mixed-Mode Delamination of a Composite Laminate

Mixed-Mode Delamination of a Composite Laminate

Interfacial failure or delamination in a composite material 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 the implementation of a CZM with a bilinear traction-separation law in a laminated composite using the Layered Shell interface. The capabilities of the CZM to predict mixed-mode softening and delamination propagation are demonstrated in this example.

This example is an extension of the Structural Mechanics Module Application Library model Mixed-Mode Debonding of a Laminated Composite in which the interface is used to model delamination. The results are compared with the model created using the Solid Mechanics interface.


	Read more about the Composite Materials Module in the COMSOL blog, Introduction to the Composite Materials Module.

Model Definition

Cohesive Zone Model (CZM)

The CZM used in this example is defined using the displacement based damage model available in the node. 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 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, that is 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 Benzeggagh and Kenane criterion 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. As the Layered Shell interface only requires a boundary selection, only the middle surface of the 3D geometry is modeled and the Midplane on boundary option is chosen in the node.

Figure 1: The geometry of the test specimen.

The material properties are those of AS4/PEEK unidirectional laminates and are listed in Table 2. The transverse isotropic linear elastic properties assume that the longitudinal direction is aligned with the global X direction. The AS4/PEEK unidirectional laminate is a built-in material in the material library.

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	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

For composite materials, von Mises stress is generally not an appropriate stress measure. In this model, however, it is applied because the stresses in directions other than the fiber direction are negligible, making von Mises stress a reasonable representation of the fiber stress in absolute terms. It is also used since the benchmark results from the interface are reported in terms of von Mises stress.

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 for the Layered Shell model. When compared with the Solid Mechanics model (see plot in model), the distribution of stresses from the Layered Shell model matches closely. At this step, the initial crack has propagated along the interface as shown in Figure 3. Here also the interface health predicted by the Layered Shell model show excellent agreement with the Solid Mechanics model.

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:

Note, that 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 for both the Layered Shell and Solid Mechanics models, the two curves closely match with each other. The load-displacement curve confirms what Figure 3 displayed. The maximal load that the beam with the initial crack can carry is exceeded and delamination occurs. After the 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

•

Modeling a composite laminate as a layered shell requires a surface geometry, in general referred to as a base surface, and a node which adds an extra dimension (1D) to the base surface geometry in the surface normal direction. You can use the functionality to model several layers stacked on top of each other having different thicknesses, material properties, and fiber orientations. You can optionally specify the interface materials between the layers, and control the number of through-thickness mesh elements for each layer.

•

The third direction for the selected coordinate system in the , , or represents the normal direction of the or physics. This is also the direction in which the layer stacking is interpreted from bottom to top, and therefore, it is crucial to know it during modeling. There are two ways to achieve this:

Using physics symbols: Go to the physics settings, find the section, and select the checkbox. Then go to the material feature, for instance, , to see the normal direction represented by green arrows in the geometry.

Using result templates: When a solution dataset is available, use the result template to plot the normal direction.

•

The built-in material library contains data for fiber and matrix constituents as well as for unidirectional and bidirectional laminae.

•

To implement a cohesive zone model in the interface, use the node, in which you can model adhesion, delamination and contact after delamination. There are two different ways to specify adhesion stiffness, with the default being taken from the interface material properties. Delamination laws based on either displacement or energy are used to model the separation of the interface. The contact after delamination is modeled by pressure penalty contact method.

•

The node can be used to model already delaminated region by setting initial state to delaminated. To model the portion of interface that is not delaminated, set the initial state to bonded. The node is only applicable to internal interface of composite laminates.

References

1. P.P. Camanho, C.G. Davila, and M.F. De Moura, “Numerical Simulation of Mixed-mode Progressive Delamination in Composite Materials,” J. Compos. Mater., vol. 37, no. 16, pp. 1415–1438, 2003.

2. J.R. Reeder and J.R. Crews Jr., “Mixed-Mode Bending Method for Delamination Testing,” AiAA J., vol. 28, no. 7, pp. 1270–1276, 2003.

Composite_Materials_Module/Delamination/mixed_mode_delamination

Modeling Instructions

Root

In this example you will start from an existing model that is an example in the Structural Mechanics Module.

Application Libraries

From the menu, choose .

In the window, select > > in the tree.

Click

Component [Solid Mechanics]

In the window, click .

In the window for , type Component [Solid Mechanics] in the text field.

Study [Solid Mechanics]

In the window, click .

In the window for , type Study [Solid Mechanics] in the text field.

Results

Interface Health, Interface Health: Gauss Points, Stress (solid)

In the window, under , Ctrl-click to select , , and .

Right-click and choose .

Solid Mechanics Plots

In the window for , type Solid Mechanics Plots in the text field.

In the window, collapse the node.

Add a new component in order to set up a similar model with the Layered Shell interface.

Add Component

In the window, right-click the root node and choose > .

Component [Layered Shell]

In the window for , type Component [Layered Shell] in the text field.

Geometry 2

Work Plane 1 (wp1)

In the toolbar, click

In the window for , click

Work Plane 1 (wp1) > Plane Geometry

In the window, click .

Work Plane 1 (wp1) > Rectangle 1 (r1)

In the toolbar, click

In the window for , locate the section.

In the text field, type lb.

In the text field, type wb/2.

Work Plane 1 (wp1) > Rectangle 2 (r2)

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.

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

Work Plane 1 (wp1) > Union 1 (uni1)

In the toolbar, click

and choose .

Click the

button in the toolbar.

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

Form Union (fin)

In the toolbar, click

Click the

button in the toolbar.

Click the

button in the toolbar.

Definitions (comp2)

Integration Edge

In the toolbar, click

and choose .

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

Locate the section. From the list, choose .

Select Point 1 only.

Locate the section. From the list, choose .

Integration Center

Right-click and choose .

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

Locate the section. Click

Select Point 5 only.

Load Point Variables

In the window, right-click and choose .

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

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


Name	Expression	Unit	Description
u_IeL	intop3(lshell.atxd1(hb,w2))		Displacement at edge [Layered Shell]
w_cL	intop4(lshell.atxd1(hb,w2))		Displacement at center [Layered Shell]
u_lpL	(3ll-lb/2)/4/(lb/2)u_IeL+((ll+lb/2)/(lb/2))*(-w_cL+u_IeL/4)		Load point displacement [Layered Shell]
F_lpL	forceL*lb/2/ll		Load point force [Layered Shell]

Global Definitions

Layered Material 1 (lmat1)

In the window, under right-click and choose .

In the window for , locate the section.

In the table, enter the following settings:


Layer	Material	Rotation	Value	Thickness	Mesh elements
Layer 1	Unidirectional fiber lamina: AS4/APC2 carbon/PEEK thermoplastic [fiber volume fraction 50%] (mat1)	0.0	0 rad	hb/2	2

Click

Materials

Layered Material Link 1 (llmat1)

In the window, under right-click and choose > .

The geometry is in an XY-plane in which the fibers are oriented with respect to the X direction. Hence set the first axis of the laminate coordinate system in the X direction. Also set the frame of the to reference configuration.

Definitions (comp2)

Boundary System 2 (sys2)

In the window for , locate the section.

Find the subsection. From the list, choose .

From the list, choose .

Add Physics

In the toolbar, click

to open the window.

Go to the window.

In the tree, select > .

Click the button in the window toolbar.

In the toolbar, click

to close the window.

Layered Shell (lshell)

For the portion of interface that is initially delaminated, the initial state in node can be set to .

Delamination 1

In the toolbar, click

and choose .

Select Boundary 1 only.

In the window for , locate the section.

From the list, choose .

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

For the portion of interface that is not yet delaminated, the initial state in node can be set to . To model contact between delaminated interfaces, the penalty factor taken from the adhesive stiffness.

Delamination 2

In the toolbar, click