COMSOL 6.4 - Micromechanics and Macromechanics of a Composite Cylinder

Micromechanics and Macromechanics of a Composite Cylinder

Fiber composites are widely used in industrial applications. Compared to more traditional metallic engineering materials, fiber composites often have superior specific stiffness and strength properties, and they are often more corrosion resistant. Also, properties like strength, stiffness, and toughness can often be tailored to specific applications. A fiber composite consists of load carrying fibers embedded in a polymer resin. The composite material is typically a laminate of individual layers, where the fibers in each layer are unidirectional. This model demonstrates how to perform a stress analysis of a laminated composite cylinder.

Modeling individual fibers in every layer in the laminate is unfeasible. A simplified micromechanics model of a single carbon fiber in epoxy is instead used to estimate the homogenized elastic properties of a single layer. These properties are then used in the macromechanical model of the laminated composite cylinder. Two approaches are used to model the laminate, namely the Layerwise (LW) theory and the Equivalent Single Layer (ESL) theory.


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

Model Definition

This model performs different types of analyses of a laminated composite cylinder. The model is divided into three parts:

•

Micromechanics analysis

•

Stress and eigenfrequency analysis using the Layerwise theory

•

Stress and eigenfrequency analysis using the Equivalent Single Layer theory

Eigenfrequencies and mode shapes are computed and compared using both theories.

Micromechanics analysis

A micromechanics analysis of a single layer is performed in order to obtain its homogenized material properties. The composite layer is assumed to be made of carbon fibers unidirectionally embedded in epoxy resin. A repeating unit cell (RUC) having a cylindrical fiber surrounded by resin is shown in Figure 1. The fiber radius is computed assuming a fiber volume fraction of 0.6.

Figure 1: Geometry of the unit cell with a carbon fiber in an epoxy resin.

Fiber and Resin Properties

The layers of the laminate are made of T300 carbon fiber and epoxy polymer. The carbon fiber is assumed to be transversely isotropic, and the epoxy resin is assumed to be isotropic. Both materials are built-in materials in the material library. The material properties of fiber and matrix are given in Table 1 and Table 2, respectively.

Table 1: carbon Fiber Material properties.
Material Property	Value
{E1, E2}	{230,15} GPa
G12	27 GPa
{υ12, υ23}	{0.2, 0.0714}
ρ	1760 kg/m3

Table 2: Epoxy resin Material properties.
Material Property	Value
E	3.25 GPa
υ	0.265
ρ	1250 kg/m3

Cell Periodicity

In order to perform a micromechanics analysis, the node in the interface is used. The node is used to apply periodic boundary conditions to the three pairs of faces of the unit cell.

In order to extract the homogenized elasticity matrix for a layer, the unit cell needs to be analyzed for six different load cases. The periodicity type needs to be selected to obtain the homogenized elasticity matrix. This is automatically done with the help of the action buttons in the node. The node has three action buttons in the tool bar of section called : , , and . The action button generates six different load groups and a stationary study with six load cases. The action button generates a with an elasticity matrix corresponding to that of the homogenized material in terms of variables. The action button generates a with an elasticity matrix corresponding to that of the homogenized material in terms of numbers after the study computed. The generated global material can be used to define the properties of individual layers in a composite laminate.

Stress and eigenfrequency Analysis Using the Layerwise Theory

Layerwise (LW) Theory

In the layerwise theory, the degrees of freedom are the displacements (u, v, w) available on the reference surface (or modeled surface) as well as in the through-thickness direction. From a constitutive equation point of view, this theory is similar to 3D solid elasticity. The layerwise theory is useful for detailed modeling of thick composite laminates because it can capture interlaminar shear stresses. It could therefore be used to also study delamination.

Geometry and Boundary Conditions

The model geometry of a composite cylinder with a length of 0.5 m and a radius of 0.1 m is shown in Figure 2. Boundary conditions and loading are:

•

One end of the cylinder is fixed.

•

The other end has a roller support.

•

A load of 1 kN is applied to a quarter of the cylinder outer surface.

Figure 2: Geometry of the cylinder showing boundary conditions and loading.

Figure 3: Through-thickness view of the laminated material with five layers.

Stacking Sequence and Material Properties

The laminate consists of five layers of 1 mm thickness, as shown in Figure 3. The orientations of the layers are different. The orientations, starting from the bottom of the laminate, are taken as 0, 45, 90, −45, and 0 degrees, as shown in Figure 4. The orientation of a layer is specified with respect to the laminate coordinate system as shown in Figure 5. The material properties for each layer are given by the homogenized material computed in the micromechanics analysis.

The first principal material direction showing the fiber orientation in each layer of the physical geometry are shown in Figure 6.

Figure 4: Stacking sequence [0/45/90/-45/0] for the laminate showing the fiber orientation of each layer, from bottom to top.

Figure 5: The laminate coordinate system showing the first principal direction along the cylinder axis.

Figure 6: First principal material direction showing the fiber orientation in each layer of the physical geometry. The ply angle is used as a color for each layer.

Stress and eigenfrequency Analysis using THE ESL theory

Equivalent Single Layer (ESL) Theory

In the equivalent single layer (ESL) theory, the degrees of freedom are the displacements and rotations on the midplane of the laminate. From a constitutive equation point of view, this theory is similar to 3D shell elasticity. Through-thickness homogenized material properties of the laminate are used. It is therefore computationally less expensive than the layerwise theory. It can be used for the modeling of thin to moderately thick laminates with good accuracy. An aim of this analysis is to compare the results to the results obtained from the layerwise theory.

The model setup, including geometry, boundary conditions, material properties, and so on, is the same as described in the previous section.

Results and Discussion

In the micromechanics analysis, six load cases are used to evaluate the elasticity matrix. The distribution of effective (von Mises) stress for four of the load cases is shown in Figure 7.

Figure 7: Von Mises stress distribution in the unit cell for four load cases.

The stress distribution in the fiber direction for a composite cylinder obtained from the two theories is presented in Figure 8. Both theories give similar results.

The through-thickness variation of the axial laminate stress at a particular point on the cylinder is shown in Figure 9. We see that the stress variation is discontinuous between layers, but that the two theories predict similar distributions.

Figure 8: The stress in the fiber direction in the composite cylinder obtained using the Layerwise and ESL theories.

Figure 9: Through-thickness variation of axial stress at a particular point on the cylinder.

Figure 10: The stress in the fiber direction in the five layers of the laminate.

Figure 10 shows the distribution of stress in the fiber direction in each layer of the laminate using the layerwise theory. The distributions of stress in the individual layers are remarkably different. The middle layer, with fibers perpendicular to the first principal laminate direction, shows the lowest stresses.

The first six eigenfrequencies of the constrained cylinder are shown in Table 3, and the corresponding mode shapes are shown in Figure 11. The eigenfrequencies obtained using the LW and ESL theories match within 0.3%.

Table 3: Comparison of eigenfrequencies.
Eigenfrequencies from layerwise theory (Hz)	Eigenfrequencies from ESL theory (Hz)
475.28	474.70
539.46	538.82
932.47	931.72
970.56	970.41
1182.8	1180.7
1214.4	1212.7

Figure 11: The first six mode shapes and corresponding eigenfrequencies of the cylinder.

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 and have an option to transform the given into a symmetric or antisymmetric laminate. A repeated laminate can also be constructed using a transform option.

•

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.

•

You can either use the Layerwise (LW) theory based interface or the Equivalent Single Layer (ESL) theory based node in interface.

•

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

•

To analyze the results in a composite shell, you can either create a slice plot using the plot for in-plane variation of a quantity, or you can create a plot for out-of-plane variation of a quantity at a point. To visualize the results as a 3D solid object, you can use the dataset which creates a virtual 3D solid object combining the surface geometry (2D) and the extra dimension (1D).

Composite_Materials_Module/Tutorials/composite_cylinder_micromechanics_and_stress_analysis

Modeling Instructions (Micromechanics)

From the menu, choose .

New

In the window, click

Model Wizard

In the window, click

In the tree, select > .

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 composite_cylinder_micromechanics_and_stress_analysis_parameters.txt.

Next, create a repeating unit cell (RUC) for a unidirectional fiber composite with square fiber packing. This RUC like many others can be found in the built-in .

In the window, right-click and choose > .

Part Libraries

In the window, select > > > in the tree.

Click

In the dialog, select in the list.

Click .

Geometry 1

Unidirectional Fiber Composite, Square Packing 1 (pi1)

In the toolbar, click

and choose .

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Value	Description
vf	v_f	0.6	Fiber volume fraction
wm	L	0.001 m	Cell width
dm	L	0.001 m	Cell depth
hm	L	0.001 m	Cell height

Form Union (fin)

In the window, click .

In the window for , click

Solid Mechanics (solid)

Linear Elastic Material 1

In the window, under > click .

In the window for , locate the section.

From the list, choose .

Cell Periodicity 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. Select the checkbox.

Select the checkbox.

Boundary Pair 1

In the toolbar, click

and choose .

In the window for , locate the section.

Click

Select Boundaries 1, 5, 11, and 12 only.

Boundary Pair 2

Right-click and choose .

In the window for , locate the section.

Click

Select Boundaries 2 and 10 only.

Boundary Pair 3

Right-click and choose .

In the window for , locate the section.

Click

Select Boundaries 3 and 4 only.

In the upper-right corner of the section, you can find three buttons , and . When the option is selected for the computation of the elasticity matrix, you can automatically generate load groups, a study, and a material by clicking on these buttons.

Cell Periodicity 1

In the window, click .

In the window for , click in the upper-right corner of the section. From the menu, choose to generate load groups and a study node.

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

Materials

Material Link 1: Matrix

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

In the window for , type Material Link 1: Matrix in the text field.

Locate the section. From the list, choose .

Locate the section. Click

Add Material to Material Link 1: Matrix (matlnk1)

Go to the window.

In the tree, select > > .

Click .

Materials

Material Link 2: Fiber

Right-click and choose > .

In the window for , type Material Link 2: Fiber in the text field.

Locate the section. From the list, choose .

Locate the section. Click

Add Material to Material Link 2: Fiber (matlnk2)

Go to the window.

In the tree, select > > .

Click .

Mesh 1

Identical Mesh 1

In the toolbar, click

and choose .

Size

In the window, click .

In the window for , locate the section.

Click the button.

Identical Mesh 1

In the window, click .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

Free Triangular 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Click

Swept 1

In the toolbar, click

In the window for , click

Cell Periodicity Study

In the toolbar, click

Set default units for result presentation.

Results

Preferred Units 1

In the toolbar, click

and choose .

In the window for , locate the section.

Click

In the dialog, select > in the tree.

Click .

In the window for , locate the section.

In the table, enter the following settings:


Quantity	Unit	Preferred unit
Stress tensor	N/m^2	MPa

Click

Stress, Unit Cell

In the window, under click .

In the window for , type Stress, Unit Cell in the text field.

In the toolbar, click

Before you add another physics, create a homogenized material from the feature.

The homogenized material can be created by using either of the two action buttons in the section, or . Choose the second action button in order to generate the material with numbers.

Solid Mechanics (solid)

Cell Periodicity 1

In the window, under > click .

In the window for , click in the upper-right corner of the section. From the menu, choose to generate a global material node with computed density and elastic properties.

Modeling Instructions (Stress and Eigenfrequency Analysis Using the Layerwise (LW) Theory)

This section describes how to model a laminated composite cylinder using the interface based on the layerwise theory.

Add Component

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

Geometry 2

Cylinder 1 (cyl1)

In the toolbar, click

In the window for , locate the section.

From the list, choose .

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

In the text field, type hc.

Locate the section. From the list, choose .

Click

Definitions (comp2)

Boundary System 2 (sys2)

In the window, expand the > node, then click .

In the window for , locate the section.

Find the subsection. From the list, choose .

Add Physics

In the toolbar, click

to open the window.

Go to the window.

In the tree, select > .

Find the subsection. In the table, clear the checkbox for .

Click the button in the window toolbar.

In the toolbar, click

to close the window.

Global Definitions

The laminate is antisymmetric when the middle layer is excluded. Therefore, it is sufficient to define only a part of it in the node. The transformation into the full laminate is performed through layered material settings in the node.

Layered Material: [0/45/90/-45/0]

In the window, under right-click and choose .

In the window for , type Layered Material: [0/45/90/-45/0] in the text field.

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


Layer	Material	Rotation	Value	Thickness	Mesh elements
Layer 1	Homogeneous Material (solidcp1mat)	0	0 rad	th	1

Click two times.

In the table, enter the following settings:


Layer	Material	Rotation	Value	Thickness	Mesh elements
Layer 2	Homogeneous Material (solidcp1mat)	45	0.7854 rad	th	1
Layer 3	Homogeneous Material (solidcp1mat)	90	1.5708 rad	th	1

Materials

Layered Material Link 1 (llmat1)

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

The laminate, partially defined in the node, can be transformed into a full laminate using a transform option in the layered material settings. The middle layer is merged in order to create a five layer laminate.

In the window for , locate the section.

From the list, choose .

Select the checkbox.

Click to expand the section. In the text field, type 0.4.