Micromechanics and Stress Analysis of a Composite Cylinder

The use of fiber composites in the manufacturing industry is increasing. Compared to traditional metallic engineering materials, fiber composites are lighter and more corrosion resistant, and properties like strength, stiffness and toughness can often be tailored to a specific application. 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 uni-directional. In this model, we 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 elastic properties of a single layer. These properties are then used in the homogenized 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.

Model Definition

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

•

Micromechanics analysis

•

Stress analysis using the Layerwise theory

•

Stress 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 representative unit cell having a cylindrical fiber located at the middle of 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 914C epoxy. The carbon fiber is assumed transversely isotropic (modeled as orthotropic), and the epoxy resin is assumed isotropic. The material properties of fiber and resin are given in Table 1 and Table 2, respectively.

Table 1: carbon Fiber Material properties.
Material Property	Value
{E1,E2,E3}	{230,15,15} GPa
{G12,G23,G13}	{15,7,15} GPa
{υ12,υ23,υ13}	{0.2,0.07,0.2}
ρ	1800 kg/m3

Table 2: Epoxy resin Material properties.
Material Property	Value
E	4 GPa
υ	0.35
ρ	1100 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 two action buttons on 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. The generated global material can be used to define the properties of individual layers in a composite laminate.

Stress 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 respectively.

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. Ply angle is used as a color for each layer.

Stress 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 von Mises stress distribution in the composite cylinder obtained from the two theories is presented in Figure 8. Both theories give similar results.

The through-thickness variation of the axial second Piola-Kirchhoff 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: Von Mises stress distribution in the composite cylinder obtained using the Layerwise and ESL theories.

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

Figure 10: Von Mises stress distribution in the five layers of the laminate.

Figure 10 shows the distribution of von Mises stress in each layer of the laminate using the plot. 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 0.2%.

Table 3: Comparison of eigenfrequencies.
Eigenfrequencies from layerwise theory (Hz)	Eigenfrequencies from ESL theory (Hz)
486	485
573	572
984	984
999	999
1213	1211
1276	1274

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

Notes About the COMSOL Implementation

•

The micromechanics analysis of a single fiber in a resin can be performed using the node available in the interface. Using this functionality, the elasticity matrix of the homogenized material can be computed for the given fiber and resin properties, and the fiber volume fraction.

•

The node has two action buttons on the tool bar of section called : and . The action button generates load groups and a stationary study with loadcases. The action button generate a with homogenized material properties. The action buttons are active depending on the choices in the and lists.

•

Modeling a composite laminated shell requires a surface geometry (2D), in general called a base surface, and a node which adds an extra dimension (1D) to the base surface geometry in the surface normal direction. Using the functionality, you can model several layers of different thickness, material properties, and fiber orientations. You can optionally specify the interface materials between the layers and the control mesh elements in 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.

•

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

•

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. 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.

Geometry 1

Block 1 (blk1)

In the toolbar, click

In the window for , locate the section.

In the text field, type l.

Click

Cylinder 1 (cyl1)

In the toolbar, click

In the window for , locate the section.

In the text field, type r_f.

In the text field, type l.

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

In the text field, type l/2.

Locate the section. From the list, choose .

Click

Form Union (fin)

In the window, click .

In the window for , click

Solid Mechanics (solid)

Cell Periodicity 1

In the window, under right-click and choose the domain setting .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

From the list, choose .

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 Periodicity type section, you can find two buttons Create Load Groups and Study and Create Material. When the Average strain option is selected for computation of 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 nodes.

Click in the upper-right corner of the section. From the menu, choose to generate a global material node with computed elastic properties.

Materials

Material 1: Epoxy Resin

In the window, under right-click and choose .

Before adding the fiber material data, set the solid model to orthotropic in the node since the fiber material is assumed to have orthotropic properties. The isotropic resin material data will be automatically converted into an orthotropic format.

In the window for , type Material 1: Epoxy Resin in the text field.

Select Domain 1 only.

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


Property	Variable	Value	Unit	Property group
Young’s modulus	E	E_r	Pa	Basic
Poisson’s ratio	nu	nu_r	1	Basic
Density	rho	rho_r	kg/m³	Basic

Solid Mechanics (solid)

Linear Elastic Material 1

In the window, under click .

In the window for , locate the section.

From the list, choose .

Materials

Material 2: Carbon Fiber

In the window, under right-click and choose .

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

Locate the section. Click

In the dialog box, type 2 in the text field.

Click .

In the window for , locate the section.

In the table, enter the following settings:


Property	Variable	Value	Unit	Property group
Young’s modulus	{Evector1, Evector2, Evector3}	{E1_f, E2_f, E2_f}	Pa	Orthotropic
Poisson’s ratio	{nuvector1, nuvector2, nuvector3}	{nu12_f, nu23_f, nu12_f}	1	Orthotropic
Shear modulus	{Gvector1, Gvector2, Gvector3}	{G12_f, G23_f, G12_f}	N/m²	Orthotropic
Density	rho	rho_f	kg/m³	Basic