PDF
Bending of a Simply Supported Composite Laminate
Introduction
A composite material is a heterogeneous material formed of two or more constituents integrated together to achieve enhanced structural performance. Owing to the improved strength and reduced weight compared to conventional materials, the range of applications of composite materials spans diverse fields. This necessitates a thorough understanding of the behavior of these materials under various loading conditions.
This verification example analyses a simply supported composite plate subjected to a transverse sinusoidal distributed load. The plate is made of three layers with a cross-ply configuration (0/90/0). The analysis is performed using both the layerwise and the Equivalent Single Layer (ESL) theories, and the results are compared with the exact 3D elasticity solutions [Ref. 1]. The estimates of the in-plane normal stress, the transverse normal stress, and the transverse shear stresses in each layer show an exact match with the reference solution.
Model Definition
The model geometry consists of a square composite plate of 200 mm side length. All the edges of the plate are simply supported. In addition to constraining the out-of-plane translation, such support conditions also constrain the in-plane translation in the edge direction.
For the bending analysis, a sinusoidally varying distributed load is applied on the top surface of the plate in the transverse direction. Because of symmetry in geometry and loading, only one quarter of the plate is modeled, with the symmetry boundary conditions at two edges as shown in Figure 1.
Figure 1: Model geometry showing one quarter of the laminated composite plate.
lamina Material Properties
The homogenized orthotropic material properties (Young’s modulus, shear modulus, and Poisson’s ratio) of the lamina are given in Table 1.
Table 1: Material properties of a lamina.
Material property
Value
{E1,E2,E3}
{25e6,1e6,1e6}(psi)
{G12,G23,G13}
{0.5e6,0.2e6,0.5e6}(psi)
{υ12,υ23,υ13}
{0.25,0.25,0.25}
Thickness and Stacking Sequence
The composite plate considered in this example is rather thick, having a thickness to side ratio of 1/4. Thus the total thickness of the laminate is 50 mm.
The laminate consists of three layers in a cross-ply layup. The stacking sequence of the laminate is shown in Figure 2, and the 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 plate showing fiber orientation in each layer from bottom to top.
Table 2: Fiber orientation in layered material
Layer number
Fiber orientation in layered material (°)
1
0
2
90
3
0
Finite element mesh
The structure (quarter plate) is discretized using a mapped mesh as shown in Figure 4. The distribution of elements along the edges is taken as 2-by-2 [Ref. 1]. Additionally, two sub-layers are used in each material layer of the plate as given in the reference.
Cubic serendipity shape functions are used in layerwise theory in order to capture the shear stress profiles accurately.
Figure 3: The laminate coordinate system used in the model.
Figure 4: Finite element mesh with 4 elements.
Nondimensional Stress Expressions
The following nondimensional stress expressions are defined in order to compare to the reference solution:
where is the laminate thickness, is the side length, and is the transverse load amplitude. The three point locations (A, A), (A, B), and (B, A) on the composite plate is shown below:
Figure 5: Points on the laminated composite plate where different stress values are compared.
Results and Discussion
Figure 6 and Figure 7 show the von Mises stress distribution in one quarter of the composite laminate computed using the layerwise theory and the ESL theory, respectively. The distribution of von Mises stress in the full composite laminate is shown in Figure 8.
Figure 6: von Mises stress distribution computed using layerwise theory.
You can also compute the through-thickness variation of different stress components using the layerwise and ESL theories. Both theories can be used to study thin to moderately thick laminates. The fact that the layerwise formulation has degrees of freedom available at each layer makes it preferable for the analysis of thick laminates. As the thickness to side ratio for the current problem is 1/4, there is good agreement between the layerwise theory and the stress values computed from 3D elastic solutions [Ref. 1] as shown in Figure 9, Figure 10, Figure 11, and Figure 12.
The transverse shear stresses, in Figure 11 and Figure 12, depict the interlaminar stress values at the junction/interface of the two respective layers. It can be seen that the in-plane normal stress, shown in Figure 9, is discontinuous across the layers and having different stress values in two layers at the junction/interface whereas the transverse shear stress is continuous across the layers. This unique value of transverse shear stress at the junction/interface is known as interlaminar stress, which is one of the deciding factors for interfacial failures like delamination.
Figure 7: von Mises stress distribution computed using the ESL theory.
Figure 8: von Mises stress distribution in the full laminate computed using the layerwise theory.
Figure 9: Through-thickness variation of normalized in-plane normal stress (SXX).
Figure 10: Through-thickness variation of normalized transverse normal stress (SZZ).
Figure 11: Through-thickness variation of normalized transverse shear stress (SYZ).
Figure 12: Through-thickness variation of normalized transverse shear stress (SXZ).
Notes About the COMSOL Implementation
•
Modeling a composite laminated shell requires a surface geometry (2D), in general called 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 mesh elements in each layer.
•
From a constitutive model point of view, you can either use the layerwise theory based Layered Shell interface, or the Equivalent Single Layer theory based Layered Linear Elastic Material node in the Shell interface.
•
In Layered Shell interface, in order to increase the accuracy in the through thickness profile at the same time keeping the total degrees of freedom less, a cubic shape order is used in out-of-plane direction keeping the in-plane shape order as quadratic.
Reference
1. J. N. Reddy, Mechanics of Laminated Composite Plates and Shells: Theory and Analysis, Second Edition, CRC Press, 2004.
Application Library path: Composite_Materials_Module/Verification_Examples/simply_supported_composite_laminate
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
In the Select Physics tree, select Structural Mechanics>Shell (shell).
5
Click Add.
6
Click  Study.
7
In the Select Study tree, select General Studies>Stationary.
8
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 simply_supported_composite_laminate_parameters.txt.
Definitions
Variables 1
1
In the Model Builder window, under Component 1 (comp1) 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 simply_supported_composite_laminate_variables.txt.
Geometry 1
Work Plane 1 (wp1)
In the Geometry toolbar, click  Work Plane.
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/2.
4
Locate the Position section. In the xw text field, type a/2.
5
In the yw text field, type a/2.
6
Click  Build Selected.
7
Click the  Zoom Extents button in the Graphics toolbar.
Definitions
Boundary System 1 (sys1)
1
In the Model Builder window, under Component 1 (comp1)>Definitions click Boundary System 1 (sys1).
2
In the Settings window for Boundary System, locate the Settings section.
3
Find the Coordinate names subsection. From the Axis list, choose x.
Global Definitions
Material 1 (mat1)
In the Model Builder window, under Global Definitions right-click Materials and choose Blank Material.
Layered Material: [0/90/0]
1
Right-click Materials and choose Layered Material.
2
In the Settings window for Layered Material, type Layered Material: [0/90/0] in the Label text field.
3
Locate the Layer Definition section. In the table, enter the following settings:
Layer
Material
Rotation (deg)
Thickness
Mesh elements
Layer 1
Material 1 (mat1)
0.0
thl
2
4
Click Add two times.
5
In the table, enter the following settings:
Layer
Material
Rotation (deg)
Thickness
Mesh elements
Layer 2
Material 1 (mat1)
90
thl
2
Layer 3
Material 1 (mat1)
0
thl
2
6
Click to expand the Preview Plot Settings section. In the Thickness-to-width ratio text field, type 0.6.
7
Locate the Layer Definition section. Click Layer Stack Preview in the upper-right corner of the section.
Materials
Layered Material Link 1 (llmat1)
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose Layers>Layered Material Link.
Global Definitions
Material 1 (mat1)
1
In the Settings window for Material, locate the Material Contents section.
2
In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
{Evector1, Evector2, Evector3}
{E1,E2,E3}
Pa
Orthotropic
Poisson’s ratio
{nuvector1, nuvector2, nuvector3}
{nu12,nu23,nu13}
1
Orthotropic
Shear modulus
{Gvector1, Gvector2, Gvector3}
{G12,G23,G13}
N/m²
Orthotropic
Density
rho
1
kg/m³
Basic
In order to have more accuracy in the through-thickness direction, use Quadratic-cubic serendipity element defining quadratic variation of displacement field on the base surface and cubic variation along the through-thickness direction.
Layered Shell (lshell)
1
In the Model Builder window, under Component 1 (comp1) click Layered Shell (lshell).
2
In the Settings window for Layered Shell, click to expand the Discretization section.
3
From the Displacement field list, choose Quadratic-cubic serendipity.
Prescribed Displacement 1
1
In the Physics toolbar, click  Edges and choose Prescribed Displacement.
2
Select Edge 3 only.
3
In the Settings window for Prescribed Displacement, locate the Prescribed Displacement section.
4
Select the Prescribed in x direction check box.
5
Select the Prescribed in z direction check box.
Prescribed Displacement 2
1
Right-click Prescribed Displacement 1 and choose Duplicate.
2
In the Settings window for Prescribed Displacement, locate the Edge Selection section.
3
Click  Clear Selection.
4
Select Edge 4 only.
5
Locate the Prescribed Displacement section. Clear the Prescribed in x direction check box.
6
Select the Prescribed in y direction check box.
Symmetry 1
1
In the Physics toolbar, click  Edges and choose Symmetry.
2
Select Edges 1 and 2 only.
Face Load 1
1
In the Physics toolbar, click  Boundaries and choose Face Load.
2
In the Settings window for Face Load, locate the Interface Selection section.
3
From the Apply to list, choose Top interface.
4
Select Boundary 1 only.
5
Locate the Force section. Specify the FA vector as
0
x
0
y
sdl
z
Shell (shell)
In the Model Builder window, under Component 1 (comp1) click Shell (shell).
Layered Linear Elastic Material 1
1
In the Physics toolbar, click  Boundaries and choose Layered Linear Elastic Material.
2
In the Settings window for Layered Linear Elastic Material, locate the Linear Elastic Material section.
3
From the Solid model list, choose Orthotropic.
4
Select Boundary 1 only.
Simply Supported 1
1
In the Physics toolbar, click  Edges and choose Simply Supported.
2
Select Edges 3 and 4 only.
3
In the Settings window for Simply Supported, locate the In-Plane Displacement Constraints section.
4
Clear the Perpendicular to edge check box.
Symmetry 1
1
In the Physics toolbar, click  Edges and choose Symmetry.
2
Select Edges 1 and 2 only.
Face Load 1
1
In the Physics toolbar, click  Boundaries and choose Face Load.
2
Select Boundary 1 only.
3
In the Settings window for Face Load, locate the Force section.
4
Specify the FA vector as
0
x
0
y
sdl
z
Mesh 1
Mapped 1
1
In the Mesh toolbar, click  Boundary and choose Mapped.
2
Select Boundary 1 only.
Distribution 1
1
Right-click Mapped 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Edge Selection section.
3
From the Selection list, choose All edges.
4
Locate the Distribution section. In the Number of elements text field, type 2.
5
In the Model Builder window, right-click Mesh 1 and choose Build All.
Study 1
In the Home toolbar, click  Compute.
Results
Mirror 3D 1
1
In the Results toolbar, click  More Datasets and choose Mirror 3D.
2
In the Settings window for Mirror 3D, locate the Data section.
3
From the Dataset list, choose Layered Material 1.
4
Locate the Plane Data section. In the x-coordinate text field, type a/2.
Mirror 3D 2
1
Right-click Mirror 3D 1 and choose Duplicate.
2
In the Settings window for Mirror 3D, locate the Data section.
3
From the Dataset list, choose Mirror 3D 1.
4
Locate the Plane Data section. From the Plane list, choose zx-planes.
5
In the y-coordinate text field, type a/2.
Cut Point 3D: (A, A)
1
In the Results toolbar, click  Cut Point 3D.
2
In the Settings window for Cut Point 3D, type Cut Point 3D: (A, A) in the Label text field.
3
Locate the Point Data section. In the X text field, type A.
4
In the Y text field, type A.
5
In the Z text field, type 0.
Cut Point 3D: (A, B)
1
Right-click Cut Point 3D: (A, A) and choose Duplicate.
2
In the Settings window for Cut Point 3D, type Cut Point 3D: (A, B) in the Label text field.
3
Locate the Point Data section. In the Y text field, type B.
Cut Point 3D: (B, A)
1
Right-click Cut Point 3D: (A, B) and choose Duplicate.
2
In the Settings window for Cut Point 3D, type Cut Point 3D: (B, A) in the Label text field.
3
Locate the Point Data section. In the X text field, type B.
4
In the Y text field, type A.
Stress (shell)
You can group the default plots generated for the Layered Shell and Shell interfaces separately. Select multiple plots and right-click to create a group. Before doing so, ungroup the default plots.
Geometry and Layup (lshell)
In the Model Builder window, under Results right-click Geometry and Layup (lshell) and choose Ungroup.
Applied Loads (lshell)
In the Model Builder window, right-click Applied Loads (lshell) and choose Ungroup.
Layup (shell)
In the Model Builder window, right-click Layup (shell) and choose Ungroup.
Applied Loads (shell)
In the Model Builder window, right-click Applied Loads (shell) and choose Ungroup.
Follow the instructions below to plot the von Mises stress distribution in the full composite plate as shown in Figure 8.
Stress (LW Theory): Full Laminate
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Stress (LW Theory): Full Laminate in the Label text field.
3
Locate the Data section. From the Dataset list, choose Mirror 3D 2.
4
Locate the Plot Settings section. Clear the Plot dataset edges check box.
Slice (yz-planes)
1
Right-click Stress (LW Theory): Full Laminate and choose Slice.
2
In the Settings window for Slice, type Slice (yz-planes) in the Label text field.
3
Locate the Expression section. In the Expression text field, type lshell.mises.
4
Locate the Plane Data section. In the Planes text field, type 3.
5
Locate the Coloring and Style section. From the Color table list, choose RainbowLight.
Deformation 1
Right-click Slice (yz-planes) and choose Deformation.
Slice (zx-planes)
1
In the Model Builder window, right-click Slice (yz-planes) and choose Duplicate.
2
In the Settings window for Slice, type Slice (zx-planes) in the Label text field.
3
Click to expand the Title section. From the Title type list, choose None.
4
Locate the Coloring and Style section. Clear the Color legend check box.
5
Locate the Plane Data section. From the Plane list, choose zx-planes.
6
In the Planes text field, type 3.
7
In the Stress (LW Theory): Full Laminate toolbar, click  Plot.
Next, import the exact 3D elasticity solution and compare it with the computed solution.
Table: SXX
1
In the Results toolbar, click  Table.
2
In the Settings window for Table, type Table: SXX in the Label text field.
3
Locate the Data section. Click Import.
4
Browse to the model’s Application Libraries folder and double-click the file simply_supported_composite_laminate_stress_xx.txt.
Table: SZZ
1
In the Results toolbar, click  Table.
2
In the Settings window for Table, type Table: SZZ in the Label text field.
3
Locate the Data section. Click Import.
4
Browse to the model’s Application Libraries folder and double-click the file simply_supported_composite_laminate_stress_zz.txt.
Table: SYZ
1
In the Results toolbar, click  Table.
2
In the Settings window for Table, type Table: SYZ in the Label text field.
3
Locate the Data section. Click Import.
4
Browse to the model’s Application Libraries folder and double-click the file simply_supported_composite_laminate_stress_yz.txt.
Table: SXZ
1
In the Results toolbar, click  Table.
2
In the Settings window for Table, type Table: SXZ in the Label text field.
3
Locate the Data section. Click Import.
4
Browse to the model’s Application Libraries folder and double-click the file simply_supported_composite_laminate_stress_xz.txt.
Follow the instructions below to plot the through-thickness variation of the in-plane normal stress as shown in Figure 9.
In-plane Normal Stress (SXX)
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type In-plane Normal Stress (SXX) in the Label text field.
3
Locate the Plot Settings section. Select the x-axis label check box.
4
In the associated text field, type In-plane normal stress (SXX), normalized.
5
Select the y-axis label check box.
6
In the associated text field, type Thickness coordinate, normalized.
7
Locate the Legend section. From the Position list, choose Upper left.
Through Thickness 1
1
In the In-plane Normal Stress (SXX) toolbar, click  More Plots and choose Through Thickness.
2
In the Settings window for Through Thickness, locate the Data section.
3
From the Dataset list, choose Cut Point 3D: (A, A).
4
Click Replace Expression in the upper-right corner of the x-Axis Data section. From the menu, choose Component 1 (comp1)>Definitions>Variables>SXX_lw - In-plane normal stress (SXX), normalized.
5
Locate the y-Axis Data section. From the Parameter list, choose Expression.
6
In the Expression text field, type lshell.xd_rel.
7
Find the Interface positions subsection. From the Show interface positions list, choose All interfaces.
8
Click to expand the Legends section. Select the Show legends check box.
9
From the Legends list, choose Manual.
10
In the table, enter the following settings:
Legends
Layerwise Theory
11
In the In-plane Normal Stress (SXX) toolbar, click  Plot.
Through Thickness 2
1
Right-click Through Thickness 1 and choose Duplicate.
2
In the Settings window for Through Thickness, click Replace Expression in the upper-right corner of the x-Axis Data section. From the menu, choose Component 1 (comp1)>Definitions>Variables>SXX_esl - In-plane normal stress (SXX), normalized.
3
Click to expand the Title section. From the Title type list, choose None.
4
Locate the y-Axis Data section. In the Expression text field, type shell.xd_rel.
5
Find the Interface positions subsection. From the Show interface positions list, choose None.
6
Click to expand the Coloring and Style section. Find the Line style subsection. From the Line list, choose Dashed.
7
Locate the Legends section. In the table, enter the following settings:
Legends
ESL Theory
8
In the In-plane Normal Stress (SXX) toolbar, click  Plot.
Table Graph 1
1
In the Model Builder window, right-click In-plane Normal Stress (SXX) and choose Table Graph.
2
In the Settings window for Table Graph, locate the Coloring and Style section.
3
Find the Line style subsection. From the Line list, choose None.
4
From the Color list, choose Red.
5
Find the Line markers subsection. From the Marker list, choose Circle.
6
From the Positioning list, choose In data points.
7
Click to expand the Legends section. Select the Show legends check box.
8
From the Legends list, choose Manual.
9
In the table, enter the following settings:
Legends
Reference (Exact 3D Elasticity)
10
In the In-plane Normal Stress (SXX) toolbar, click  Plot.
In-plane Normal Stress (SXX)
In the Model Builder window, click In-plane Normal Stress (SXX).
Table Annotation 1
1
In the In-plane Normal Stress (SXX) toolbar, click  More Plots and choose Table Annotation.
2
In the Settings window for Table Annotation, locate the Data section.
3
From the Source list, choose Local table.
4
In the table, enter the following settings:
x-coordinate
y-coordinate
Annotation
0.6
0.17
\[0^\circ \,\,\textrm{Ply}\]
0.6
0.5
\[90^\circ \,\,\textrm{Ply}\]
0.6
0.83
\[0^\circ \,\,\textrm{Ply}\]
5
Select the LaTeX markup check box.
6
Locate the Coloring and Style section. Clear the Show point check box.
7
In the In-plane Normal Stress (SXX) toolbar, click  Plot.
In-plane Normal Stress (SXX)
1
In the Model Builder window, click In-plane Normal Stress (SXX).
2
Click  Plot.
Follow the instructions below to plot the through-thickness variation of the transverse normal stress as shown in Figure 10.
Transverse Normal Stress (SZZ)
1
Right-click In-plane Normal Stress (SXX) and choose Duplicate.
2
In the Settings window for 1D Plot Group, type Transverse Normal Stress (SZZ) in the Label text field.
3
Locate the Plot Settings section. In the x-axis label text field, type Transverse normal stress (SZZ), normalized.
Through Thickness 1
1
In the Model Builder window, expand the Transverse Normal Stress (SZZ) node, then click Through Thickness 1.
2
In the Settings window for Through Thickness, click Replace Expression in the upper-right corner of the x-Axis Data section. From the menu, choose Component 1 (comp1)>Definitions>Variables>SZZ_lw - Transverse normal stress (SZZ), normalized.
Through Thickness 2
In the Model Builder window, under Results>Transverse Normal Stress (SZZ) right-click Through Thickness 2 and choose Delete.
Table Graph 1
1
In the Model Builder window, under Results>Transverse Normal Stress (SZZ) click Table Graph 1.
2
In the Settings window for Table Graph, locate the Data section.
3
From the Table list, choose Table: SZZ.
Transverse Normal Stress (SZZ)
1
In the Model Builder window, click Transverse Normal Stress (SZZ).
2
In the Transverse Normal Stress (SZZ) toolbar, click  Plot.
Follow the instructions below to plot the through-thickness variation of the transverse shear stress as shown in Figure 11.
Transverse Shear Stress (SYZ)
1
In the Model Builder window, right-click In-plane Normal Stress (SXX) and choose Duplicate.
2
In the Settings window for 1D Plot Group, type Transverse Shear Stress (SYZ) in the Label text field.
3
Locate the Plot Settings section. In the x-axis label text field, type Transverse shear stress (SYZ), normalized.
Through Thickness 1
1
In the Model Builder window, expand the Transverse Shear Stress (SYZ) node, then click Through Thickness 1.
2
In the Settings window for Through Thickness, locate the Data section.
3
From the Dataset list, choose Cut Point 3D: (A, B).
4
Click Replace Expression in the upper-right corner of the x-Axis Data section. From the menu, choose Component 1 (comp1)>Definitions>Variables>SYZ_lw - Transverse shear stress (SYZ), normalized.
Through Thickness 2
1
In the Model Builder window, click Through Thickness 2.
2
In the Settings window for Through Thickness, locate the Data section.
3
From the Dataset list, choose Cut Point 3D: (A, B).
4
Click Replace Expression in the upper-right corner of the x-Axis Data section. From the menu, choose Component 1 (comp1)>Definitions>Variables>SYZ_esl - Transverse shear stress (SYZ), normalized.
Table Graph 1
1
In the Model Builder window, click Table Graph 1.
2
In the Settings window for Table Graph, locate the Data section.
3
From the Table list, choose Table: SYZ.
Table Annotation 1
1
In the Model Builder window, click Table Annotation 1.
2
In the Settings window for Table Annotation, locate the Data section.
3
From the Source list, choose Local table.
4
In the table, enter the following settings:
x-coordinate
y-coordinate
Annotation
-0.02
0.17
\[0^\circ \,\,\textrm{Ply}\]
-0.02
0.5
\[90^\circ \,\,\textrm{Ply}\]
-0.02
0.83
\[0^\circ \,\,\textrm{Ply}\]
Transverse Shear Stress (SYZ)
1
In the Model Builder window, click Transverse Shear Stress (SYZ).
2
In the Transverse Shear Stress (SYZ) toolbar, click  Plot.
Follow the instructions below to plot the through-thickness variation of the transverse shear stress as shown in Figure 12.
Transverse Shear Stress (SXZ)
1
Right-click Transverse Shear Stress (SYZ) and choose Duplicate.
2
In the Settings window for 1D Plot Group, type Transverse Shear Stress (SXZ) in the Label text field.
3
Locate the Plot Settings section. In the x-axis label text field, type Transverse shear stress (SXZ), normalized.
4
Locate the Legend section. From the Position list, choose Center.
Through Thickness 1
1
In the Model Builder window, expand the Transverse Shear Stress (SXZ) node, then click Through Thickness 1.
2
In the Settings window for Through Thickness, locate the Data section.
3
From the Dataset list, choose Cut Point 3D: (B, A).
4
Click Replace Expression in the upper-right corner of the x-Axis Data section. From the menu, choose Component 1 (comp1)>Definitions>Variables>SXZ_lw - Transverse shear stress (SXZ), normalized.
5
Locate the y-Axis Data section. Find the Interface positions subsection. From the Show interface positions list, choose None.
Through Thickness 2
1
In the Model Builder window, click Through Thickness 2.
2
In the Settings window for Through Thickness, locate the Data section.
3
From the Dataset list, choose Cut Point 3D: (B, A).
4
Click Replace Expression in the upper-right corner of the x-Axis Data section. From the menu, choose Component 1 (comp1)>Definitions>Variables>SXZ_esl - Transverse shear stress (SXZ), normalized.
5
Locate the y-Axis Data section. Find the Interface positions subsection. From the Show interface positions list, choose All interfaces.
Table Graph 1
1
In the Model Builder window, click Table Graph 1.
2
In the Settings window for Table Graph, locate the Data section.
3
From the Table list, choose Table: SXZ.
Transverse Shear Stress (SXZ)
1
In the Model Builder window, click Transverse Shear Stress (SXZ).
2
In the Transverse Shear Stress (SXZ) toolbar, click  Plot.