COMSOL 6.4 - Progressive Delamination in a Laminated Shell

Progressive Delamination in a Laminated Shell

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 composites using the Layered Shell interface. The capabilities of the CZM to predict mixed-mode softening and delamination propagation are demonstrated in the model.

The example illustrates the delamination initiation and propagation in a composite plate having two layers with an initial delaminated region at the interface. A bending load is gradually applied and removed in a parametric study in order to predict the total interfacial damage in one load cycle.


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

Model Definition

The geometry of a composite plate is shown in Figure 1. The composite plate consists of two layers where each layer has a thickness of 1.5 mm with [0/45] stacking sequence.

Figure 1: The geometry of a composite plate having two layers with an initial delaminated region at the interface.

The geometry consists of circular regions where the interface between the two layers is in delaminated or debonded state.

Material Properties

The material properties are those of AS4/PEEK unidirectional laminates and are listed in Table 1. 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 1: 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	νXY=νXZ	0.25
Poisson’s ratio	νYZ	0.45
Shear modulus	GXY=GXZ	5.5 GPa

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 under different loading. The material properties needed for this constitutive model are summarized in Table 2.

Table 2: 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	GIc	969 J/m2
Critical energy release rate, shear	GIIc	1719 J/m2
Exponent of Benzeggagh and Kenane (B-K) criterion	η	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 model by Benzeggagh and Kenane is used.

Boundary conditions

•

Face load with a total maximum value of 28 kN is applied at the top surface of the composite plate in negative z-direction. The load is parametrically increased and then decreased to zero using a sinusoidal function.

•

Fixed constraints are used on the exterior edges of the plate which are parallel to y-axis.

Finite element mesh

A rather fine mapped mesh is used in the geometry in order to accurately predict the initiation and propagation of delamination in the structure.

Figure 2: A mapped finite element mesh used to accurately model the delamination propagation in the composite plate.

In the thickness direction, each layer has only one mesh element in order to reduce the overall computation time.

Results and Discussion

The stress distribution in the fiber direction for both layers of the composite plate when the applied load is having maximum value is shown in Figure 3. The corresponding stress distribution at the midplane of two layers is shown in Figure 4. In this figure, the bottom layer undergoes higher stresses than the top layer due to the bending effects and fiber orientation.

Figure 3: The stress distribution in the composite plate for maximum applied force value.

The state of delaminated region when the applied load is having maximum value is shown in Figure 5, where debonded part is shown in red and bonded part is shown in green color. It can be seen the delamination starts near the comparatively weaker regions or high stress regions. The two such locations in the plate are the boundaries of initially delaminated region and the region near fixed edges.

The adhesive stress in the first tangent direction when the applied load is having maximum value is shown in Figure 6. Figure 7 illustrates the variation of applied load and total damage area as a function of parameter. It can be seen that the interfacial damage is irreversible and it stays permanently in the structure even if the load is removed.

Figure 4: The stress distribution at layer midplanes for maximum applied force value.

Figure 5: Plot showing the health of the laminate interface for maximum applied force value. The debonded part is shown in red, the intact part in green.

Figure 6: Adhesive stress in first tangent direction for maximum applied force value.

Figure 7: Load vs. damage curve. The overall damage area as well as area where 90% or more damage has occurred are shown.

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 interface, use the node which allows you to model adhesion, delamination and contact after delamination. There are two different ways to specify adhesive stiffness with default being taken from the interface material properties. Cohesive zone models are based on either displacement or energy in order to predict the interfacial separation. The contact after delamination is modeled by 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 which is not delaminated set the initial state to bonded. The node is only applicable to the internal interfaces of composite laminates.

Composite_Materials_Module/Delamination/progressive_delamination_in_a_laminated_shell

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

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 progressive_delamination_in_a_laminated_shell_parameters.txt.

Add Material

COMSOL Multiphysics is equipped with built-in material properties for a number of lamina materials. Select the needed materials from the material folder in the built-in material library.

In the toolbar, click

to open the window.

Go to the window.

In the tree, select > > .

Right-click and choose .

In the toolbar, click

to close the window.

Global Definitions

Add a node and assign appropriate thickness and rotation angles to each ply.

Layered Material: [0/45]

In the window, under right-click and choose .

In the window for , type Layered Material: [0/45] in the text field.

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 rad	hb	1

Click

In the table, enter the following settings:


Layer	Material	Rotation	Value	Thickness	Mesh elements
Layer 2	Unidirectional fiber lamina: AS4/APC2 carbon/PEEK thermoplastic [fiber volume fraction 50%] (mat1)	45	0.7854 rad	hb	1

Definitions

Variables 1

In the window, under right-click and choose .

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Unit	Description
F	Fmaxsin(pipara)	N	Applied force

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 to reference configuration.

Boundary System 1 (sys1)

In the window, click .

In the window for , locate the section.

From the list, choose .

Find the subsection. From the list, choose .

Geometry 1

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/2.

In the text field, type wb.

Click

Click the

button in the toolbar.

Work Plane 1 (wp1) > Circle 1 (c1)

In the toolbar, click

In the window for , locate the section.

In the text field, type lb/10.

Locate the section. In the text field, type lb/5.

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/5.

In the text field, type wb.

Click

Work Plane 1 (wp1) > Mirror 1 (mir1)

In the toolbar, click

and choose .

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

In the window for , locate the section.

Select the checkbox.

Locate the section. In the text field, type lb/2.

Click

Form Union (fin)

In the toolbar, click

Ignore Edges 1 (ige1)

In the window, right-click and choose > .

On the object , select Edges 8 and 20 only.

In the toolbar, click

Click the

button in the toolbar.

Click the

button in the toolbar.

Materials

Layered Material Link 1 (llmat1)

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

Layered Shell (lshell)

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

Delamination 1

In the toolbar, click

and choose .

Select Boundaries 2 and 5 only.

In the window for , locate the section.

From the list, choose .

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

Delamination 2

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

In the toolbar, click