Stacking Sequence Optimization

Composite laminates are synthetic structures and there is always a possibility to optimize its design it terms of number of layers, material of each layer, thickness of each layer, and stacking sequence for the specified loading conditions. Often, the number of layers, layer materials, and layer thicknesses are also governed by other factors. However, there is always a possibility to find the optimum stacking sequence which gives lower stresses in the structure for the specified loading conditions.

This example illustrates the optimization of stacking sequence in a composite laminate. The composite laminate considered for the analysis has six layers with symmetric layup. The Carbon-Epoxy material having orthotropic material properties is used as a lamina material. The optimization analysis is performed to find the optimum fiber orientation in each layer under specified loading conditions with an objective of minimizing maximum stress value in the laminate. The layup is assumed symmetric thus three ply angles are the control variables and BOBYQA method is applied to find the optimum stacking sequence.

Model Definition

Figure 1: Model geometry of a composite laminate.

Geometry and Boundary Conditions

The model geometry of a composite laminate with a side length of 0.5 m is shown in Figure 1. Boundary conditions and loading are:

•

Left end of the composite laminate is fixed.

•

A total load of 1 kN is applied to one of the corners of the right end of the laminate in the form of a line load as shown in Figure 2.

Figure 2: The 3D representation of model geometry together with the applied line load. Note that geometry is scaled by a factor of 10 in the thickness direction for the visualization purpose.

Stacking Sequence

The laminate considered for the analysis has 6 layers with symmetric layup. The original ply angles are assumed to be zero and are optimized for minimizing the maximum stress value in the laminate under given loading. The through-thickness view and the original layup of the laminate can be seen in Figure 3 and Figure 4.

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

Figure 4: Stacking sequence [0]6 of the original layup of the composite laminate.

Material Properties

Each ply of composite panel is assumed to be made of carbon fibers in an epoxy resin. The homogenized orthotropic material properties (Young’s modulus, shear modulus, and Poisson’s ratio) are given below:

Table 1: Material properties of a ply.
Material property	Value
{E1, E2, E3}	{134, 9.2, 9.2} GPa
{G12, G23, G13}	{4.8, 4.8, 4.8} GPa
{υ12, υ23, υ13}	{0.28, 0.28, 0.28}

Layup Optimization

In the original layup, all plies are assumed to be aligned with the laminate coordinate system axis or in other words they have zero ply angles. The objective is to optimize the ply angles in order to minimize the maximum stress values in the entire laminate.

The laminate considered here has 6 plies with symmetric layup so effectively three ply angles are the control variables for the optimization problem. The initial value of the control variables is 0 degrees and lower and upper bounds are -90 degrees and 90 degrees respectively. A parametric optimization is performed using BOBYQA method in order to find the optimum stacking sequence.

Results and Discussion

The von Mises stress distribution in the composite laminate for original layup is shown in Figure 5. The layerwise distribution of von Mises stress at the middle of each layer can be seen in Figure 6. The corresponding plots for the optimized layup are shown in Figure 7 and Figure 8.

It can be seen here that the maximum stress values are reduced by 60% in the optimized layup case. If we look at the stress distribution, it is more even within the plies as well as across the plies in optimized layup case. This helps in distributing the high stresses generated around the constrained points closer to location of applied load.

Figure 5: von Mises stress distribution in the composite laminate for original layup.

Figure 6: Layerwise von Mises stress distribution in the composite laminate for the original layup.

Figure 7: von Mises stress distribution in the composite laminate for the optimized layup.

Figure 8: Layerwise von Mises stress distribution in the composite laminate for the optimized layup.

The original and optimized ply angles are shown in Figure 9. Similarly original and optimized principal material directions can be seen in Figure 10.

The original layup and optimized layup are as follows:

•

Original layup: [0/0/0]s

•

Optimized layup: [37/13/2]s (after round-off)

Figure 9: Original and optimized ply angles.

Figure 10: Original and optimized principal material directions.

Figure 11 shows the comparison of displacement and deformation profile of the laminate under given loading for original and optimized layup. Here original layup result is plotted in wireframe mode whereas optimized layup result is plotted as solid surface plot. It can be seen that the optimized layup has higher local stiffness at the loading point and predominantly goes in a bending mode compared to the original layup which goes in bending-twisting mode.

Figure 11: Displacement and deformation profile in a composite laminate for original layup (wireframe) and optimized layup (solid).

Notes About the COMSOL Implementation

The objective function for the optimization requires the computation of maximum stress values in the composite laminate. Under the given loading conditions, the bending would occur in the composite which would give maximum stresses in the outer layers. Hence, the maximum stress value in the outer interfaces of each layer is found out, and then the maximum value among all the layers is found out.

Composite_Materials_Module/Tutorials/stacking_sequence_optimization

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 stacking_sequence_optimization_parameters.txt.

Layered Shell (lshell)

Linear Elastic Material 1

In the window, under click .

In the window for , locate the section.

Select the check box.

Global Definitions

Material: Carbon-Epoxy

In the window, under right-click and choose .

In the window for , type Material: Carbon-Epoxy in the text field.

Define a layered material with ply rotations or stacking sequence as parameters to be optimized.

Layered Material: [th1/th2/th3]

Right-click and choose .

In the window for , locate the section.

In the table, enter the following settings:


Layer	Material	Rotation (deg)	Thickness	Mesh elements
Layer 1	Material: Carbon-Epoxy (mat1)	th1	d_layer	1

Click

In the table, enter the following settings:


Layer	Material	Rotation (deg)	Thickness	Mesh elements
Layer 2	Material: Carbon-Epoxy (mat1)	th2	d_layer	1

Click

In the table, enter the following settings:


Layer	Material	Rotation (deg)	Thickness	Mesh elements
Layer 3	Material: Carbon-Epoxy (mat1)	th3	d_layer	1

In the text field, type Layered Material: [th1/th2/th3].

Geometry 1

Work Plane 1 (wp1)

In the toolbar, click

Work Plane 1 (wp1)>Plane Geometry

In the window, click .

Work Plane 1 (wp1)>Square 1 (sq1)

In the toolbar, click

In the window for , locate the section.

In the text field, type a.

Click the

button in the toolbar.

In the toolbar, click

In the window, collapse the node.

Materials

Layered Material Link 1 (llmat1)

In the window, under right-click and choose .

In the window for , locate the section.

From the list, choose .

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

Click in the upper-right corner of the section. From the menu, choose .

Global Definitions

Material: Carbon-Epoxy (mat1)

In the window, under click .

In the window for , locate the section.

In the table, enter the following settings:


Property	Variable	Value	Unit	Property group
Young’s modulus	{Evect1, Evect2}	{E1, E2}	Pa	Transversely isotropic
Poisson’s ratio	{nuvect1, nuvect2}	{nu12, nu12}	1	Transversely isotropic
Shear modulus	Gvect1	G12	N/m²	Transversely isotropic
Density	rho	1	kg/m³	Basic

Layered Shell (lshell)

Fixed Constraint 1

In the toolbar, click

and choose .

Select Edge 1 only.

Line Load 1

In the toolbar, click

and choose .

Select Point 4 only.

In the window for , locate the section.

From the list, choose .

Specify the Ftot vector as


0	x
0	y
F	z

Define a global variable, corresponding to the maximum von Mises stress in the laminate, in order to use as the objective function in the optimization analysis.

Definitions (comp1)

Maximum 1 (maxop1)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Select Boundary 1 only.

Variables 1

In the window, right-click and choose .

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Unit	Description
mises_max_l1	maxop1(lshell.atxd1(0,lshell.mises))		Maximum von Mises stress, layer 1
mises_max_l2	maxop1(lshell.atxd1(d_layer,lshell.mises))		Maximum von Mises stress, layer 2
mises_max_l3	maxop1(lshell.atxd1(2*d_layer,lshell.mises))		Maximum von Mises stress, layer 3
mises_max	max(max(mises_max_l1,mises_max_l2),mises_max_l3)		Maximum von Mises stress