COMSOL 6.3 - Modeling of a Variable-Angle Tow Laminate

Modeling of a Variable-Angle Tow Laminate

In traditional composite laminates, fibers within each ply are straight, and the global stiffness response is tailored through the selection of an appropriate stacking sequence. In contrast, variable-angle tow (VAT) laminates employ curvilinear fibers within each layer. By allowing the fiber orientation to vary spatially, VAT laminates significantly expand the design space and deliver improved structural performance. This enhanced capability can potentially reduce the required number of plies and the overall weight of the structure.

This example demonstrates the modeling of variable-angle tow laminates in which the fiber orientation varies linearly along the global x direction, with each ply assigned a different fiber angle. The results are compared against a full 3D solution obtained using the Solid Mechanics interface.


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

Model Definition

A two-layer square plate is considered. The plate lies in the global xy-plane, with its center located at the origin. Both layers are composed of the same fiber and matrix materials, however, the fiber orientations across the xy-plane differ between the plies.

The following law describes the angle with respect the global x-axis,

(1)

where a is the side length, and ϕe and ϕc correspond to the angles on the edge and at the center of the plate, respectively. The values are given in the following table:

Table 1: Angles at edge and center of the plate for both layers.
Angle	Top layer	Bottom Layer
Angle at the edge	60 deg	45 deg
Angle at the center	0 deg	90 deg

The fiber paths are shown in

Figure 1.

Figure 1: Fiber paths on the bottom and top layers.

Material properties

The composite lamina is made of carbon fibers in an epoxy resin. The homogenized transversely isotropic material properties, Young’s modulus, shear modulus, and Poisson’s ratio, are given in Table 2.

Table 2: Material Properties of a lamina.
Material property	Value
{E11, E22}	{40, 10} GPa
G12	4.5 GPa
{υ12, υ23}	{0.28, 0.28}

Results and Discussion

The first principal material direction in the layers is shown in Figure 2.

Figure 2: The first principal material direction in the layers. It coincides with the fiber direction.

The displacement and stress components across the thickness at a particular point are shown in Figure 3 and Figure 4. It can be seen that both in-plane and out-of-plane displacements are continuous across the interfaces. The same holds for the transverse shear and normal stress components, as shown in Figure 5 and Figure 6. This is due to the stress continuity in the normal direction

(2)

The in-plane normal and shear stresses are discontinuous across layers with discontinuous material properties (Figure 7 and Figure 8). In the absence of delamination, the compatibility equation ensures continuity for the in-plane strains, which implies that the in-plane stresses are discontinuous when the laminae have different material properties.

The results obtained with the Layered Shell interface closely match the results obtained with the Solid Mechanics interface.

Figure 3: x-component of the displacement across the laminate thickness.

Figure 4: z-component of the displacement across the laminate thickness.

Figure 5: zz-component of the stress tensor across the laminate thickness.

Figure 6: xz-component of the stress tensor across the laminate thickness.

Figure 7: xx-component of the stress tensor across the laminate thickness.

Figure 8: xy-component of the stress tensor across the laminate thickness.

Notes About the COMSOL Implementation

•

Modeling a composite laminate requires a surface geometry, referred to as the base surface, and a node, which adds an extra dimension in the normal direction. You can use the functionality to model several layers stacked on top of each other, each with a different thickness, material properties, and fiber orientation. You can optionally specify the interface materials between the layers and control the number of through-thickness mesh elements for each layer. To model a curvilinear fiber, add an expression as a function of the local coordinates in the field.

•

The third direction for the selected coordinate system in the , , or represents the normal direction. This is also the direction in which the layer stacking is interpreted from bottom to top, and therefore, it is crucial to visualize 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.

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

•

From a constitutive model viewpoint, you can either use the Layerwise (LW) theory available in the Layered Shell interface, or the Equivalent Single Layer (ESL) theory available in the node in the Shell interface. The laminated composite presented in this example uses the Layered Shell interface.

•

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

Composite_Materials_Module/Tutorials/variable_angle_tow_laminate

Modeling Instructions

From the menu, choose .

New

In the window, click

Model Wizard

In the window, click

In the tree, select > .

Click .

In the tree, select > .

Click .

Click

In the tree, select > .

Click

Global Definitions

Parameters 1

Load the parameters from a file.

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 variable_angle_tow_laminate_parameters.txt.

Geometry 1

Block 1 (blk1)

In the toolbar, click

In the window for , locate the section.

In the text field, type a.

In the text field, type 2*th.

Locate the section. From the list, choose .

In the text field, type th.

Click to expand the section. In the table, enter the following settings:


Layer name	Thickness (m)
Layer 1	th

Click

Global Definitions

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

Add Material from Library

In the toolbar, click

and choose .

Add Material

Go to the window.

In the tree, select > > .

Click the button in the window toolbar.

In the toolbar, click

to close the window.

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: E-glass/epoxy [fiber volume fraction 60%] (mat1)	0.0	0 rad	th	nelz

Click

Create the functions to describe the fiber angle variation in each layer. These functions are inserted in the field in the node.

Fiber Angle (Bottom Layer)

In the toolbar, click

and choose > .

In the window for , locate the section.

In the text field, type 2/a*(thetae1-thetac1)*abs(x) + thetac1.

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

In the table, enter the following settings:


Argument	Unit
x	m

In the text field, type Fiber Angle (Bottom Layer).

In the text field, type fiberAngleBot.

Fiber Angle (Top Layer)

Right-click and choose .

In the window for , type Fiber Angle (Top Layer) in the text field.

In the text field, type fiberAngleTop.

Locate the section. In the text field, type 2/a*(thetae2-thetac2)*abs(x) + thetac2.

Layered Material 1 (lmat1)

In the window, under > click .

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: E-glass/epoxy [fiber volume fraction 60%] (mat1)	fiberAngleBot(X)	-	th	nelz
Layer 2	Unidirectional fiber lamina: E-glass/epoxy [fiber volume fraction 60%] (mat1)	fiberAngleTop(X)	-	th	nelz

The interface is used to verify the results. The spatially varying orthotropic material properties due to the presence of curvilinear fibers are obtained with the use of rotated coordinate systems.

Definitions

Rotated System (Solid, Bottom Layer)

In the toolbar, click