PDF
Stacking Sequence Optimization
Introduction
Composite laminates are synthetic structures and there is always a possibility to optimize the design in terms of the number of layers, the material of each layer, the thickness of each layer, and the stacking sequence for the specified loading conditions. Designers need to estimate how safe the composite material is for a chosen application and under given loading conditions. With suitable failure criteria, the performance of the composite can be assessed and optimized in order to reduce the failure index or increase safety factor for specified loading conditions.
This example illustrates how to optimize the stacking sequence in a composite laminate based on the Hashin failure criterion. The composite laminate considered for the analysis has six layers with a symmetric layup. A carbon–epoxy material with transversely isotropic material properties is used for the lamina. An optimization analysis is performed to find the optimum fiber orientation in each layer under specified loading conditions with the objective of minimizing the maximum failure index in the laminate. The derivative-free BOBYQA optimization solver is applied to find the optimum stacking sequence.
Read more about the Composite Materials Module in the COMSOL blog, Introduction to the Composite Materials Module.
Model Definition
Figure 1: Model geometry of a composite laminate.
Geometry and Boundary Conditions
The geometry of a composite laminate with a side length of 0.5 m is shown in Figure 1. The following boundary conditions are applied:
•
A fixed, fully constrained, boundary condition contains the assumption that the analyzed structure is attached to an infinitely stiff support. In many cases, this is a useful approximation, but cases like optimization you may need to consider the flexibility of the supporting structure in your model. Hence, the spring foundation is used to constraint the left side of the composite laminate.
•
A total load of 12 kN, varying linearly with position, is applied to the right side of the laminate as a boundary load as shown in Figure 2.
Figure 2: A 3D representation of the composite geometry together with the applied boundary load. Note that the geometry is scaled by a factor of 10 in the thickness direction for visualization purposes.
Stacking Sequence
The laminate considered for the analysis consists of 6 layers with a symmetric layup. The original ply angles are assumed to be zero and are optimized to minimize the maximum failure index in the laminate under the loading conditions described above. The through-thickness view and the original layup of the laminate can be seen in Figure 3 and Figure 4, respectively.
Figure 3: Through-thickness view of the laminate.
Figure 4: Stacking sequence [0]6 of the original layup of the laminate.
Material Properties
Each ply is made up of AS4/APC carbon–thermoplastic composite material. The AS4/APC carbon–thermoplastic is a built-in material in the Composites material library. The transversely isotropic material properties (Young’s modulus, shear modulus, and Poisson’s ratio) are given in Table 1. The material strengths are given in Table 2.
Table 1: Material properties of a ply.
Material property
Value
{E11, E22}
{138, 8.7} GPa
G12
5 GPa
{υ12, υ23}
{0.28, 0.45}
Table 2: Material strengths of a ply.
Material property
Value
{σT1, σT2, σT3}
{2060, 78, 78} MPa
{σC1, σC2, σC3}
{1590, 200, 200} MPa
{σS12, σS23, σS13}
{157, 157, 157} MPa
Layup Optimization
In the original layup, all plies are assumed to be aligned with the laminate coordinate system axis; in other words, their ply angles are zero. The objective is to optimize the ply angles in order to minimize the maximum failure index in the entire laminate.
The laminate considered here consists of 6 plies with a 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 the lower and upper bounds are −90 degrees and 90 degrees, respectively. A parametric optimization is performed using the BOBYQA method in order to find the optimum stacking sequence.
Expressing the objective in terms of a maximum operator can cause numerical issues and therefore it is often better to use an approximate maximum. In this model a p-norm (P = 10) is used, that is
Results and Discussion
The Hashin failure criterion is a well-known failure criterion for composites that considers six failure modes: fiber failure in tension, fiber failure in compression, matrix failure in tension, matrix failure in compression, interlaminar failure in tension, and interlaminar failure in compression. The overall failure criterion of the composite is evaluated as the most critical of the underlying failure modes.
In the original ply design, the failure indices for several failure modes are near to one, indicating possibility of composite failure by different failure modes at the given load. The unidirectional composites have maximum load carrying capacity in the fiber direction. For this reason, the stress in the fiber direction in each lamina is used to the visualize the loading intensity in Figure 5; note, however, that the stacking optimization is based on the failure index.
The distribution of the maximum failure index per interface in the laminate can be seen in Figure 6. The failure index is above one in the top ply, which indicates that the structure in unsafe for the given loading conditions.
When the laminate stacking sequence is optimized with the objective of reducing the maximum failure index, both the stress in fiber direction (Figure 7) and the failure index (Figure 8) are reduced considerably. The maximum stress and maximum failure index values are reduced substantially for the optimized layup. The reduction of the failure index well below 1 indicates that the structure is safe for the given loading conditions.
Figure 5: von Mises stress distribution in the laminate with the original layup.
Figure 6: Distribution of the Hashin failure index in each interface of the laminate for the original layup.
Figure 7: von Mises stress distribution in the laminate for the optimized layup.
Figure 8: Distribution of the Hashin failure index in each interface of the laminate for the optimized layup.
The ply angles in the original and optimized layups are provided below and visualized in Figure 9.
•
Original layup: [0/0/0]s
•
Optimized layup: [12.81/2.88/2.67]s (after round-off)
Figure 9: Original and optimized ply angles.
Figure 10 compares the displacement magnitude on the deformed configuration of the laminate between the original and optimized layups. Here, the original layup result is plotted as a wireframe whereas the optimized layup result is plotted as a solid surface. The optimized layup is stiffer at the loading point and predominantly goes into a bending mode compared to the original layup which goes into a mixed bending–twisting mode.
Figure 10: Displacement magnitude plotted on the deformed configuration for the original (wireframe) and optimized (solid) layups.
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 Layered Material node which adds an extra dimension (1D) to the base surface geometry in the surface normal direction. You can use the Layered Material 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 Single Layer Material, Layered Material Link, or Layered Material Stack represents the normal direction of the Layered Shell or Shell 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 Physics Symbols section, and select the Enable physics symbols checkbox. Then go to the material feature, for instance, Linear Elastic Material, 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 Thickness and Orientation to plot the normal direction.
•
From a constitutive model point of view, you can either use the Layerwise (LW) theory based Layered Shell interface, or the Equivalent Single Layer (ESL) theory based Linear Elastic Material, Layered node in the Shell interface. The laminated composite presented in the current model is modeled using the Layered Shell interface.
•
The built-in Composites material library contains data for fiber and matrix constituents as well as for unidirectional and bidirectional laminae.
Application Library path: Composite_Materials_Module/Tutorials/stacking_sequence_optimization
Modeling Instructions
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  3D.
2
In the Select Physics tree, select Structural Mechanics > Layered Shell (lshell).
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies > Stationary.
6
Click  Done.
Global Definitions
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file stacking_sequence_optimization_parameters.txt.
COMSOL Multiphysics is equipped with built-in material properties for a number of lamina materials. Select the needed materials from the Composites material folder in the built-in material library.
Add Material
1
In the Materials toolbar, click  Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Composites > Laminae > Unidirectional fiber lamina: AS4/APC2 carbon/PEEK thermoplastic [fiber volume fraction 58%].
4
Right-click and choose Add to Global Materials.
5
In the Materials toolbar, click  Add Material to close the Add Material window.
Define a layered material with ply rotations as parameters to be optimized.
Global Definitions
Layered Material: [th1/th2/th3]
1
In the Model Builder window, under Global Definitions right-click Materials and choose Layered Material.
2
In the Settings window for Layered Material, locate the Layer Definition section.
3
In the table, enter the following settings:
Layer
Material
Rotation
Value
Thickness
Mesh elements
Layer 1
Unidirectional fiber lamina: AS4/APC2 carbon/PEEK thermoplastic [fiber volume fraction 58%] (mat1)
th1
0 rad
d_layer
1
4
Click Add two times.
5
In the table, enter the following settings:
Layer
Material
Rotation
Value
Thickness
Mesh elements
Layer 2
Unidirectional fiber lamina: AS4/APC2 carbon/PEEK thermoplastic [fiber volume fraction 58%] (mat1)
th2
0 rad
d_layer
1
Layer 3
Unidirectional fiber lamina: AS4/APC2 carbon/PEEK thermoplastic [fiber volume fraction 58%] (mat1)
th3
0 rad
d_layer
1
6
In the Label text field, type Layered Material: [th1/th2/th3].
Geometry 1
Work Plane 1 (wp1)
1
In the Geometry toolbar, click  Work Plane.
2
In the Settings window for Work Plane, click  Go to Plane Geometry.
Work Plane 1 (wp1) > Plane Geometry
In the Model Builder window, click Plane Geometry.
Work Plane 1 (wp1) > Square 1 (sq1)
1
In the Work Plane toolbar, click  Square.
2
In the Settings window for Square, locate the Size section.
3
In the Side length text field, type a.
4
Click the  Go to Default View button in the Graphics toolbar.
5
In the Home toolbar, click  Build All.
6
Click the  Show Grid button in the Graphics toolbar.
7
In the Model Builder window, collapse the Geometry 1 node.
Materials
Layered Material Link 1 (llmat1)
1
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose Layers > Layered Material Link.
2
In the Settings window for Layered Material Link, locate the Layered Material Settings section.
3
From the Transform list, choose Symmetric.
4
Click to expand the Preview Plot Settings section. In the Thickness-to-width ratio text field, type 0.4.
5
Click Section_bar in the upper-right corner of the Layered Material Settings section. From the menu, choose Layer Cross-Section Preview.
6
Click Section_bar in the upper-right corner of the Layered Material Settings section. From the menu, choose Layer Stack Preview.
Layered Shell (lshell)
Linear Elastic Material 1
In the Model Builder window, under Component 1 (comp1) > Layered Shell (lshell) click Linear Elastic Material 1.
Safety 1
1
In the Physics toolbar, click  Attributes and choose Safety.
2
In the Settings window for Safety, locate the Failure Model section.
3
From the Failure criterion list, choose Hashin.
Spring Foundation 1
1
In the Physics toolbar, click  Edges and choose Spring Foundation.
2
Select Edge 1 only.
3
In the Settings window for Spring Foundation, locate the Spring section.
4
From the Spring type list, choose Total spring constant.
5
From the list, choose Diagonal.
6
Specify the ktot matrix as
1e12
0
0
0
1e12
0
0
0
1e9
Boundary Load 1
1
In the Physics toolbar, click  Edges and choose Boundary Load.
2
Select Edge 4 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
From the Load type list, choose Total force.
5
Specify the Ftot vector as
F*(Y/a)
z
Define a global variable, as a measure of maximum failure index in the laminate, in order to use as the objective function in the optimization analysis.
Definitions (comp1)
Integration 1 (intop1)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Integration.
2
In the Settings window for Integration, locate the Source Selection section.
3
From the Geometric entity level list, choose Boundary.
4
From the Selection list, choose All boundaries.
Variables 1
1
In the Model Builder window, right-click Definitions and choose Variables.
2
In the Settings window for Variables, locate the Variables section.
3
Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file stacking_sequence_optimization_variables.txt.
The maximum stress concentration occurs at the constrained edge. To obtain a sufficiently accurate solution, refine the mesh in this region.
Mesh 1
Mapped 1
1
In the Mesh toolbar, click  More Generators and choose Mapped.
2
Select Boundary 1 only.
Distribution 1
1
Right-click Mapped 1 and choose Distribution.
2
Select Edges 1 and 4 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
From the Distribution type list, choose Predefined.
5
In the Number of elements text field, type 40.
6
In the Element ratio text field, type 5.
7
From the Growth rate list, choose Exponential.
Distribution 2
1
In the Model Builder window, right-click Mapped 1 and choose Distribution.
2
Select Edges 2 and 3 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
From the Distribution type list, choose Predefined.
5
In the Number of elements text field, type 40.
6
In the Element ratio text field, type 5.
7
From the Growth rate list, choose Exponential.
8
Select the Symmetric distribution checkbox.
9
Click  Build All.
Study 1: Original Layup
1
In the Model Builder window, click Study 1.
2
In the Settings window for Study, type Study 1: Original Layup in the Label text field.
3
In the Study toolbar, click  Compute.
Results
Failure Indices and Fiber Orientations (Original)
1
In the Results toolbar, click  Evaluation Group.
2
In the Settings window for Evaluation Group, type Failure Indices and Fiber Orientations (Original) in the Label text field.
3
Locate the Data section. From the Dataset list, choose Layered Material.
4
Locate the Transformation section. Select the Transpose checkbox.
5
Click to expand the Format section. From the Include parameters list, choose Off.
Volume Maximum 1
1
Right-click Failure Indices and Fiber Orientations (Original) and choose Maximum > Volume Maximum.
2
In the Settings window for Volume Maximum, locate the Expressions section.
3
In the table, enter the following settings:
Expression
Unit
Description
th1
deg
Fiber orientation, layer 1
th2
deg
Fiber orientation, layer 2
th3
deg
Fiber orientation, layer 3
lshell.lemm1.sf1.f_ifT
1
Hashin fiber tensile failure index
lshell.lemm1.sf1.f_ifC
1
Hashin fiber compressive failure index
lshell.lemm1.sf1.f_imT
1
Hashin matrix tensile failure index
lshell.lemm1.sf1.f_imC
1
Hashin matrix compressive failure index
lshell.lemm1.sf1.f_iiT
1
Hashin interlaminar tensile failure index
lshell.lemm1.sf1.f_iiC
1
Hashin interlaminar compressive failure index
4
In the Failure Indices and Fiber Orientations (Original) toolbar, click  Evaluate.
Increase the through thickness scale factor in various layered material datasets for better visualization.
Layered Material
1
In the Model Builder window, expand the Results > Datasets node, then click Layered Material.
2
In the Settings window for Layered Material, locate the Layers section.
3
In the Scale text field, type 10.
Stress, Layer Coordinate System (Original)
1
In the Model Builder window, under Results click Stress (lshell).
2
In the Settings window for 3D Plot Group, type Stress, Layer Coordinate System (Original) in the Label text field.
3
Locate the Color Legend section. Select the Show maximum and minimum values checkbox.
4
In the Stress, Layer Coordinate System (Original) toolbar, click  Plot.
Result Templates
1
In the Results toolbar, click  Result Templates to open the Result Templates window.
2
Go to the Result Templates window.
3
In the tree, select Study 1: Original Layup/Solution 1 (sol1) > Layered Shell > Stress, Slice (lshell).
4
Click the Add Result Template button in the window toolbar.
Results
Failure Index, Slice (Original)
1
In the Settings window for 3D Plot Group, type Failure Index, Slice (Original) in the Label text field.
2
Locate the Color Legend section. Select the Show maximum and minimum values checkbox.
Layered Material Slice 1
1
In the Model Builder window, expand the Failure Index, Slice (Original) node, then click Layered Material Slice 1.
2
In the Settings window for Layered Material Slice, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Layered Shell > Safety > Hashin > lshell.lemm1.sf1.f_i - Hashin failure index - 1.
3
Locate the Through-Thickness Location section. From the Location definition list, choose Interfaces.
4
Locate the Layout section. From the Displacement list, choose Rectangular.
5
In the Relative x-separation text field, type 0.4.
6
In the Relative y-separation text field, type 0.4.
7
Select the Show descriptions checkbox.
8
In the Relative separation text field, type 0.7.
9
Click to expand the Quality section. From the Resolution list, choose No refinement.
10
From the Smoothing list, choose None.
11
In the Failure Index, Slice (Original) toolbar, click  Plot.
12
Click the  Zoom Extents button in the Graphics toolbar.
Failure Index, Slice (Original)
1
In the Model Builder window, click Failure Index, Slice (Original).
2
In the Settings window for 3D Plot Group, locate the Plot Settings section.
3
From the View list, choose New view.
4
In the Failure Index, Slice (Original) toolbar, click  Plot.
5
Click the  Show Grid button in the Graphics toolbar.
Result Templates
1
Go to the Result Templates window.
2
In the tree, select Study 1: Original Layup/Solution 1 (sol1) > Layered Shell > Geometry and Layup (lshell) > Ply Angle (lshell).
3
Click the Add Result Template button in the window toolbar.
Results
Ply Angle (lshell)
1
In the Settings window for 3D Plot Group, locate the Data section.
2
Click  Go to Source.
Layered Material 2 (Shell Geometry)
1
In the Model Builder window, under Results > Datasets click Layered Material 2 (Shell Geometry).
2
In the Settings window for Layered Material, locate the Layers section.
3
In the Scale text field, type 40.
Surface 1
1
In the Model Builder window, expand the Results > Ply Angle (lshell) node, then click Surface 1.
2
In the Settings window for Surface, click to expand the Range section.
3
Clear the Manual color range checkbox.
Ply Angle (Original)
1
In the Model Builder window, under Results click Ply Angle (lshell).
2
In the Settings window for 3D Plot Group, type Ply Angle (Original) in the Label text field.
3
Click the  Go to Default View button in the Graphics toolbar.
4
In the Ply Angle (Original) toolbar, click  Plot.
Result Templates
1
Go to the Result Templates window.
2
In the tree, select Study 1: Original Layup/Solution 1 (sol1) > Layered Shell > Applied Loads (lshell) > Boundary Loads (lshell).
3
Click the Add Result Template button in the window toolbar.
Results
Boundary Loads (Original)
1
In the Settings window for 3D Plot Group, type Boundary Loads (Original) in the Label text field.
2
In the Model Builder window, expand the Boundary Loads (Original) node.
Boundary Load 1
1
In the Model Builder window, expand the Results > Boundary Loads (Original) > Boundary Load 1 node, then click Boundary Load 1.
2
In the Settings window for Arrow Line, locate the Coloring and Style section.
3
Select the Scale factor checkbox. In the associated text field, type 15E-9.
4
In the Boundary Loads (Original) toolbar, click  Plot.
After solving the model for the original layup, add an optimization analysis for optimizing the layup for given loading and boundary conditions.
Add Study
1
In the Home toolbar, click  Add Study to open the Add Study window.
2
Go to the Add Study window.
3
Find the Studies subsection. In the Select Study tree, select General Studies > Stationary.
4
Click the Add Study button in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Study 2: Layup Optimization
In the Settings window for Study, type Study 2: Layup Optimization in the Label text field.
General Optimization
1
In the Study toolbar, click  Optimization and choose General Optimization.
2
In the Settings window for General Optimization, locate the Optimization Solver section.
3
From the Method list, choose BOBYQA.
4
In the Optimality tolerance text field, type 0.001.
5
Locate the Objective Function section. In the table, enter the following settings:
Expression
Description
Evaluate for
comp1.FI_max
Measure of maximum failure index
Stationary
6
Locate the Control Variables and Parameters section. Click  Add three times.
7
In the table, enter the following settings:
Parameter
Initial value
Scale
Lower bound
Upper bound
Unit
th1 (Fiber orientation, layer 1)
0[deg]
1
-90[deg]
90[deg]
rad
th2 (Fiber orientation, layer 2)
0[deg]
1
-90[deg]
90[deg]
rad
th3 (Fiber orientation, layer 3)
0[deg]
1
-90[deg]
90[deg]
rad
8
In the Study toolbar, click  Compute.
Results
Layered Material 2
1
In the Model Builder window, under Results > Datasets click Layered Material 2.
2
In the Settings window for Layered Material, locate the Layers section.
3
In the Scale text field, type 10.
Stress, Layer Coordinate System (Optimized)
1
In the Model Builder window, under Results click Stress (lshell).
2
In the Settings window for 3D Plot Group, type Stress, Layer Coordinate System (Optimized) in the Label text field.
3
Locate the Color Legend section. Select the Show maximum and minimum values checkbox.
4
In the Stress, Layer Coordinate System (Optimized) toolbar, click  Plot.
Result Templates
1
Go to the Result Templates window.
2
In the tree, select Study 2: Layup Optimization/Parametric Solutions 1 (sol3) > Layered Shell > Stress, Slice (lshell).
3
Click the Add Result Template button in the window toolbar.
Results
Failure Index, Slice (Optimized)
1
In the Settings window for 3D Plot Group, type Failure Index, Slice (Optimized) in the Label text field.
2
Locate the Color Legend section. Select the Show maximum and minimum values checkbox.
Layered Material Slice 1
1
In the Model Builder window, expand the Failure Index, Slice (Optimized) node, then click Layered Material Slice 1.
2
In the Settings window for Layered Material Slice, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Layered Shell > Safety > Hashin > lshell.lemm1.sf1.f_i - Hashin failure index - 1.
3
Locate the Through-Thickness Location section. From the Location definition list, choose Interfaces.
4
Locate the Layout section. From the Displacement list, choose Rectangular.
5
In the Relative x-separation text field, type 0.4.
6
In the Relative y-separation text field, type 0.4.
7
Select the Show descriptions checkbox.
8
In the Relative separation text field, type 0.7.
9
Locate the Quality section. From the Resolution list, choose No refinement.
10
From the Smoothing list, choose None.
Failure Index, Slice (Optimized)
1
In the Model Builder window, click Failure Index, Slice (Optimized).
2
In the Settings window for 3D Plot Group, locate the Plot Settings section.
3
From the View list, choose View 3D 4.
4
In the Failure Index, Slice (Optimized) toolbar, click  Plot.
Result Templates
1
Go to the Result Templates window.
2
In the tree, select Study 2: Layup Optimization/Parametric Solutions 1 (sol3) > Layered Shell > Geometry and Layup (lshell) > Ply Angle (lshell).
3
Click the Add Result Template button in the window toolbar.
4
In the Results toolbar, click  Result Templates to close the Result Templates window.
Results
Ply Angle (lshell)
1
In the Settings window for 3D Plot Group, locate the Data section.
2
Click  Go to Source.
Layered Material 3 (Shell Geometry)
1
In the Model Builder window, under Results > Datasets click Layered Material 3 (Shell Geometry).
2
In the Settings window for Layered Material, locate the Layers section.
3
In the Scale text field, type 40.
Surface 1
1
In the Model Builder window, expand the Results > Ply Angle (lshell) node, then click Surface 1.
2
In the Settings window for Surface, locate the Range section.
3
Clear the Manual color range checkbox.
Ply Angle (Optimized)
1
In the Model Builder window, under Results click Ply Angle (lshell).
2
In the Settings window for 3D Plot Group, type Ply Angle (Optimized) in the Label text field.
3
Click the  Go to Default View button in the Graphics toolbar.
4
In the Ply Angle (Optimized) toolbar, click  Plot.
Create a plot to compare the deformation profile of the laminate for original and optimized layup.
Failure Index, Slice (Original) 1
1
In the Model Builder window, right-click Failure Index, Slice (Original) and choose Duplicate.
2
In the Settings window for 3D Plot Group, locate the Plot Settings section.
3
Clear the Plot dataset edges checkbox.
Layered Material Slice 1
1
In the Model Builder window, expand the Failure Index, Slice (Original) 1 node, then click Layered Material Slice 1.
2
In the Settings window for Layered Material Slice, locate the Data section.
3
From the Dataset list, choose Study 1: Original Layup/Solution 1 (sol1).
4
Locate the Expression section. In the Expression text field, type lshell.disp.
5
Locate the Through-Thickness Location section. From the Location definition list, choose Reference surface.
6
Locate the Layout section. From the Displacement list, choose None.
7
Clear the Show descriptions checkbox.
8
Locate the Coloring and Style section. From the Color table list, choose Twilight.
9
Select the Wireframe checkbox.
Layered Material Slice 2
Right-click Results > Failure Index, Slice (Original) 1 > Layered Material Slice 1 and choose Duplicate.
Deformation
1
In the Model Builder window, expand the Results > Failure Index, Slice (Original) 1 > Layered Material Slice 1 node, then click Deformation.
2
In the Settings window for Deformation, locate the Scale section.
3
Select the Scale factor checkbox. In the associated text field, type 1.
Transparency 1
1
In the Model Builder window, right-click Layered Material Slice 1 and choose Transparency.
2
In the Settings window for Transparency, locate the Transparency section.
3
Find the Transparency subsection. In the Transparency text field, type 0.2.
Layered Material Slice 2
1
In the Model Builder window, under Results > Failure Index, Slice (Original) 1 click Layered Material Slice 2.
2
In the Settings window for Layered Material Slice, locate the Data section.
3
From the Dataset list, choose Study 2: Layup Optimization/Parametric Solutions 1 (sol3).
4
Click to expand the Title section. From the Title type list, choose None.
5
Locate the Coloring and Style section. Clear the Wireframe checkbox.
6
Click to expand the Inherit Style section. From the Plot list, choose Layered Material Slice 1.
Line 1
1
In the Model Builder window, right-click Failure Index, Slice (Original) 1 and choose Line.
2
In the Settings window for Line, locate the Data section.
3
From the Dataset list, choose Layered Material.
4
Locate the Expression section. In the Expression text field, type lshell.atxd1(lshell.d/2,mean(lshell.disp)).
5
Click to expand the Title section. From the Title type list, choose None.
6
Locate the Coloring and Style section. From the Line type list, choose Tube.
7
Select the Radius scale factor checkbox. In the associated text field, type 0.001.
8
From the Color table list, choose Twilight.
9
Click to expand the Inherit Style section. From the Plot list, choose Layered Material Slice 1.
Deformation 1
1
Right-click Line 1 and choose Deformation.
2
In the Settings window for Deformation, locate the Expression section.
3
In the x-component text field, type lshell.umX.
4
In the y-component text field, type lshell.umY.
5
In the z-component text field, type lshell.umZ.
Line 1
1
In the Model Builder window, click Line 1.
2
In the Settings window for Line, locate the Data section.
3
From the Dataset list, choose From parent.
Line 2
1
Right-click Results > Failure Index, Slice (Original) 1 > Line 1 and choose Duplicate.
2
In the Settings window for Line, locate the Data section.
3
From the Dataset list, choose Study 2: Layup Optimization/Solution 2 (sol2).
Displacement: Original and Optimized
1
In the Model Builder window, under Results click Failure Index, Slice (Original) 1.
2
In the Settings window for 3D Plot Group, type Displacement: Original and Optimized in the Label text field.
3
Locate the Plot Settings section. From the View list, choose Automatic.
4
In the Displacement: Original and Optimized toolbar, click  Plot.
5
Click the  Zoom Extents button in the Graphics toolbar.
Failure Indices and Fiber Orientations (Optimized)
1
In the Model Builder window, right-click Failure Indices and Fiber Orientations (Original) and choose Duplicate.
2
In the Settings window for Evaluation Group, type Failure Indices and Fiber Orientations (Optimized) in the Label text field.
3
Locate the Data section. From the Dataset list, choose Layered Material 2.
4
From the Parameter selection (th1, th2, th3) list, choose Last.
5
In the Failure Indices and Fiber Orientations (Optimized) toolbar, click  Evaluate.