COMSOL 6.4 - Buckling of a Composite Cylinder

Buckling is a structural instability that can lead to failure of a component even without initial material failure. Computation of the critical buckling loads and mode shapes can therefore be important from a design viewpoint, even though it has previously been determined that the loading of the component only causes elastic deformations. This applies to components made from laminated composite materials, where elastic properties, ply thicknesses and stacking sequence of a composite laminate will affect buckling loads and mode shapes.

This example illustrates a linear buckling analysis of a composite cylinder under compressive loading and fixed-end conditions. The composite cylinder is made up of eight layers (plies) of a carbon fiber reinforced epoxy material having different fiber orientations. An Equivalent Single Layer (ESL) theory based approach is used for this analysis. The effect of stacking sequence on the critical load factor is analyzed for different types of balanced laminates, such as a symmetric angle-ply laminate and an antisymmetric angle-ply laminate.


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

Model Definition

The model geometry consists of a composite cylinder with height of 0.4 m and radius of 0.15 m. The bottom end of the cylinder is fixed whereas the top end is free only to translate in the z direction, as shown in Figure 1. In order to perform a linear buckling analysis, a unit compressive load is applied on the top end of the cylinder in the downward direction.

Figure 1: Model geometry of the laminated composite cylinder.

lamina Material Properties

The composite lamina is assumed to be 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 1.

Table 1: Material properties of a lamina.
Material property	Value
{E11, E22}	{134, 9.2} GPa
G12	4.8 GPa
{υ12, υ23}	{0.28, 0.28}

The density of the lamina is taken as 1700 kg/m3.

Stacking Sequence

The composite laminate consists of eight layers where each layer (ply) has a thickness of 0.125 mm. This makes the total thickness of the composite laminate 1 mm. In order to study the effect of a stacking sequence on the buckling behavior of the composite cylinder, four different laminates are compared:

•

Layered Material 1: [0/0/45/-45]s (Symmetric angle-ply laminate)

•

Layered Material 2: [90/90/45/-45]s (Symmetric angle-ply laminate)

•

Layered Material 3: [90/0/90/0]s (Symmetric cross-ply laminate)

•

Layered Material 4: [45/45/45/45]as (Antisymmetric angle-ply laminate)

The stacking sequence of each laminate is shown in Figure 2 and their corresponding fiber orientations are given in Table 2.

The fiber orientations are presented with respect to the first axis of the laminate coordinate system as shown in Figure 3.

Figure 2: Stacking sequence of laminated composite cylinder showing fiber orientation in each layer from bottom to top.

Table 2: Stacking sequences considered.
Layer Number	Fiber orientation in Layered material 1 (°)	Fiber orientation in Layered material 2 (°)	Fiber orientation in Layered material 3 (°)	Fiber orientation in Layered material 4 (°)
1	0	90	90	45
2	0	90	0	45
3	45	45	90	45
4	-45	-45	0	45
5	-45	-45	0	-45
6	45	45	90	-45
7	0	90	0	-45
8	0	90	90	-45

Figure 3: The laminate coordinate system showing the first principal direction along the cylinder axis.

Results and Discussion

Figure 4: First buckling mode shape and its corresponding critical load for Layered Material: [0/0/45/-45]_s.

The buckling analysis of a composite laminate with different stacking sequences shows that the critical buckling load and its corresponding mode shape is highly dependent on the stacking sequence of the individual laminae (plies).

For the first two stacking sequences, where the symmetric angle-ply arrangement is used, the first buckling mode is spiral-shaped as shown in Figure 4 and Figure 5. A notable difference between the two is the pitch of the spiraling.

For the third stacking sequence, where the symmetric cross-ply arrangement is used, the buckling mode is diamond-shaped, as shown in Figure 6. Last, for the fourth stacking sequence, in which an antisymmetric angle-ply arrangement is used, the buckling mode shape is axisymmetric, as shown in Figure 7.

Table 3: Critical buckling load for different laminates.
Stacking sequence	Type of laminate	Critical buckling load (kN)	Mode shape
[0/0/45/-45]_s	Symmetric angle-ply	117	Spiral
[90/90/45/-45]_s	Symmetric angle-ply	101.52	Spiral
[90/0/90/0]_s	Symmetric cross-ply	92.13	Diamond
[45/45/45/45]_as	Antisymmetric angle-ply	64.50	Axisymmetric

The critical buckling loads for all the stacking sequences are listed in Table 3. The first stacking sequence, where the symmetric angle-ply arrangement is used and in which four out of eight ply angles are zero, has the highest critical load factor. Not surprisingly, the fourth stacking sequence, where an antisymmetric angle-ply arrangement is used, has the lowest critical load factor.

Interestingly, by only changing the stacking sequence from the fourth to the first, the critical buckling load can be increased by a factor of about two in the present model.

Figure 5: First buckling mode shape and its corresponding critical load for Layered Material: [90/90/45/-45]_s.

Figure 6: First buckling mode shape and its corresponding critical load for Layered Material: [90/0/90/0]_s.

Figure 7: First buckling mode shape and its corresponding critical load for Layered Material: [45/45/45/45]_as.

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.

•

From a constitutive model point of view, you can either use the Layerwise (LW) theory based interface, or the Equivalent Single Layer (ESL) theory based node in the interface. The laminated composite presented in the current model is modeled using a node in the interface.

•

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

•

In order to perform a buckling analysis, a special study is used. This consists of a study step and a study step. The stationary study step performs the stress analysis for the applied load whereas buckling study uses eigenvalue solver and computes the critical load factors for the applied load.

•

In order to run the analysis for various layered materials and compare the results, all the layered materials can be defined using a node in . This node can be selected in the node and a node is added in the study. Note that while performing material sweep over layered materials in a pres-stressed buckling analysis, prestress stationary study step results are stored only for the last layered material.

Composite_Materials_Module/Buckling/composite_cylinder_buckling

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.

In the table, enter the following settings:


Name	Expression	Value	Description
r	0.15[m]	0.15 m	Cylinder radius
l	0.4[m]	0.4 m	Cylinder length

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
Fc	shell.LFcrit*1[N]		Critical buckling load
un	unX+vnY+w*nZ	m	Normal displacement

Geometry 1

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 r.

In the text field, type l.

Click

You may want to import material data from a different file and use it while modeling. In the present example, the material properties are loaded from the file composite_cylinder_buckling_material.mph stored in the model’s Application Libraries folder.

Materials

In the window, under right-click and choose .

Material Browser

In the window, click

Browse to the model’s Application Libraries folder and double-click the file composite_cylinder_buckling_material.mph.

Click

Add Material

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.

Global Definitions

Layered Material: [0/0/45/-45]_s (lmat1)

In the window for , locate the section.

Click in the upper-right corner of the section.

Material Switch 1 (sw1)

In the window, right-click and choose .

Drag the node to node.

Layered Material: [0/0/45/-45]_s (sw1.lmat1)

Drag and drop on .

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

Right-click and choose .

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

Find the section and change the rotation angles in the column as summarized in the table below.


Layer	Rotation
Layer 1	90
Layer 2	90
Layer 3	45
Layer 4	-45
Layer 5	-45
Layer 6	45
Layer 7	90
Layer 8	90

Locate the section. Click in the upper-right corner of the section.

Layered Material: [90/0/90/0]_s

Right-click and choose .

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

Find the section and change the rotation angles in the column as summarized in the table below.


Layer	Rotation
Layer 1	90
Layer 2	0
Layer 3	90
Layer 4	0
Layer 5	0
Layer 6	90
Layer 7	0
Layer 8	90

Locate the section. Click in the upper-right corner of the section.

Layered Material: [45/45/45/45]_as

Right-click and choose .

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

Find the section and change the rotation angles in the column as summarized in the table below.


Layer	Rotation
Layer 1	45
Layer 2	45
Layer 3	45
Layer 4	45
Layer 5	-45
Layer 6	-45
Layer 7	-45
Layer 8	-45

Locate the section. Click in the upper-right corner of the section.

Materials

Layered Material Link 1 (llmat1)

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

Shell (shell)

Linear Elastic Material, Layered 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

Select the checkbox.

Fixed Constraint 1

In the toolbar, click

and choose .

Select Edges 2, 3, 7, and 10 only.

Prescribed Displacement/Rotation 1

In the toolbar, click

and choose .

Select Edges 4, 5, 8, and 11 only.

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

Edge Load 1

In the toolbar, click

and choose .

Select Edges 4, 5, 8, and 11 only.

In the window for , locate the section.

From the list, choose .

Specify the Ftot vector as


0	x
0	y
-1[N]	z

Mesh 1

In the window, under click .

In the window for , locate the section.

From the list, choose .

In the table, clear the checkbox for .

Click

Study 1

In the window, collapse the node.

Material Sweep

In the toolbar, click

and choose .

In the window for , locate the section.

Click

In the toolbar, click

Results

Mode Shape: [0/0/45/-45]_s

Click the

button in the toolbar.

Click the

button in the toolbar.

Use the following instructions to plot the first critical buckling mode shape of the first laminate as shown in Figure 4.

In the window for , type Mode Shape: [0/0/45/-45]_s in the text field.

Locate the section. From the list, choose .

Click to expand the section. From the list, choose .

In the text area, type Mode shape : layered material-[0/0/45/-45]_s, critical load =eval(lambda) N.

Clear the text field.

Locate the section. Clear the checkbox.

Surface 1

In the window, expand the node, then click .

In the window for , locate the section.

In the text field, type un.

In the toolbar, click

Follow the instructions below to plot the first critical buckling mode shape of the second laminate as shown in Figure 5.

Mode Shape: [90/90/45/-45]_s

In the window, right-click and choose .

In the window for , type Mode Shape: [90/90/45/-45]_s in the text field.

Locate the section. From the list, choose .

Locate the section. In the text area, type Mode shape : layered material-[90/90/45/-45]_s, critical load =eval(lambda) N.

Follow the instructions below to plot the first critical buckling mode shape of the third laminate as shown in Figure 6.

Mode Shape: [90/0/90/0]_s

Right-click and choose .

In the window for , type Mode Shape: [90/0/90/0]_s in the text field.

Locate the section. From the list, choose .

Locate the section. In the text area, type Mode shape : layered material-[90/0/90/0]_s, critical load =eval(lambda) N.

In the toolbar, click

Follow the instructions below to plot the first critical buckling mode shape of the fourth laminate as shown in Figure 7.

Mode Shape: [45/45/45/45]_as

Right-click and choose .

In the window for , type Mode Shape: [45/45/45/45]_as in the text field.

Locate the section. From the list, choose .

Locate the section. In the text area, type Mode shape : layered material-[45/45/45/45]_as, critical load =eval(lambda) N.

In the toolbar, click

Follow the instructions below to compare the buckling mode shape for all four laminates.

Mode Shape: Comparison

Right-click and choose .

In the window for , type Mode Shape: Comparison in the text field.

Locate the section. From the list, choose .

Find the subsection. Clear the checkbox.

Click to expand the section. From the list, choose .

From the list, choose .

In the text field, type 0.5.

Surface 1

In the window, expand the node, then click .

In the window for , locate the section.

From the list, choose .

Deformation

In the window, expand the node, then click .

In the window for , locate the section.

Select the checkbox. In the associated text field, type 1.

Solution Array 1

In the window, right-click and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

Table Annotation 1

In the window, right-click and choose .

In the window for , locate the section.

From the list, choose .

In the table, enter the following settings:


x-coordinate	y-coordinate	z-coordinate	Annotation
0	0	-0.15*l	[0/0/45/-45]_s
0	1.3*l	-0.15*l	[90/90/45/-45]_s
0	0	-0.15l+1.3l	[90/0/90/0]_s
0	1.3*l	-0.15l+1.3l	[45/45/45/45]_as