COMSOL 6.4 - Material Characteristics of a Laminated Composite Shell

Material Characteristics of a Laminated Composite Shell

Introduction

This model serves the purpose of validation and verification of the model in the Shell interface.

Analyses of laminated composite shells are commonly based on one of three different theories (Ref. 1):

Equivalent Single Layer (ESL) Theory (2D)

Classical Laminated Plate Theory (CLPT-ESL)

First-Order Shear Deformation Laminated Plate Theory (FSDT-ESL)

Higher-Order Shear Deformation Laminated Plate Theory

Three-Dimensional Elasticity Theory (3D)

Traditional Three Dimensional Elasticity Theory

Layerwise Theory

Multiple Model Methods (3D and 2D)

In COMSOL Multiphysics, composites are analyzed based on either Layerwise 3D elasticity theory through the Layered Shell interface or FSDT-ESL theory through the Shell interface.

The First-Order Shear Deformation Theory (FSDT-ESL) is implemented in the model in the Shell interface available with the Composite Materials Module. This theory treats a heterogeneous laminated composite as a statically equivalent single layer. ESL theory reduces a 3D continuum problem to an equivalent 2D problem, thus reducing the size and computational time of the problem.

This example is a NAFEMS benchmark, described in Benchmarks for Membrane and Bending Analysis of Laminated Shells, Part 2: Stiffness Matrix and Thermal Characteristics (Ref. 2). Membrane and bending stiffness, flexibility matrices, midplane strains in case of unit loading, and the response to a unit change in temperature and unit temperature gradient are verified..


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

Model Definition

The geometry of the problem consists of eight square layers stacked above each other. The side length is 1 cm and each layer has a thickness of 0.1 mm, as shown in Figure 1. The laminate has [0/60/-60/0]s stacking sequence as shown in Figure 2.

Figure 1: Cross-section view of laminated composite shell showing thickness (0.1mm) of each ply.

Figure 2: Stacking sequence [0/60/-60/0]s from bottom to top, showing fiber orientation in each ply.

Material Properties

The transversely isotropic material properties (Young’s modulus, shear modulus, Poisson’s ratio, and thermal expansion coefficients) are given in Table 1.

Table 1: Material properties.
Material property	Value
{E1,E2}	{213,8.2} GPa
G12	3.2 GPa
{υ12,υ23}	{0.3,0}
{α1,α2,α3}	{1.3e-6,27e-6,27e-6} 1/K

All material properties are given in the layer coordinate system (local material directions of a layer), where the first axis is aligned with the fiber orientation.

Boundary Conditions

The constraints and loads applied on each node for unit loading and thermal loading are given in the tables below.

Table 2: Node Numbers and nodal Constraints.
Unit load and thermal cases	N1	N2	N12	M1	M2	M12	ΔΤ/ Τ'
Node
1	u, v, w,θx, θy, θz	u, v, w, θx, θy, θz	u, v, w, θx, θy, θz	u, v, w, θx, θy, θz	u, v, w, θx, θy, θz	u, v, w, θy, θz	u, v, w, θz
2	u, θz	θz	u,v, θz	u, θz	θz	w, θz	u, w, θz
3	θz	v, θz	u, θz	θz	v, θz	θz	w, θz
4	θz	θz	θz	θz	θz	v, θz	θz

Table 3: Node numbers and nodal point loads, moments.
Unit load cases	N1	N2	N12	M1	M2	M12
Node
1	0	0	0	My=-5e-3	Mx=5e-3	0
2	0	Fy=5e-3	Fx=5e-3	My=-5e-3	Mx=-5e-3	0
3	Fx=5e-3	0	Fy=5e-3	My=5e-3	Mx=5e-3	Fz=2
4	Fx=5e-3	Fy=5e-3	Fx=5e-3 Fy=5e-3	My=5e-3	Mx=-5e-3	Fz=-2

Note that the way the benchmark is specified, it is assumed that a single first-order four-node element is used. This is the only case when such a specification can give a homogeneous strain state.

The node numbers specified in the benchmark are equal to the point numbers in the COMSOL Multiphysics geometry. The signs of the point loads and moments are adjusted to give positive unit loads and moments as specified in Ref. 2. The rotation around the z-axis, θz, is automatically constrained so it does not need to be considered. The unit change in temperature and unit temperature gradient is prescribed using a subnode of the .

Study setup

The six different unit load cases and two thermal loading cases requires different boundary conditions and point loads as shown in Table 2 and Table 3. To solve all these cases in a single study, different load groups and constraint groups are created, and constrains and loads corresponding to a particular case are assigned to these groups according to Table 2 and Table 3. In the node in the study, appropriate load and constraint groups are selected for each load case.

Results and Discussion

The results presented in the benchmark (Ref. 2) are for the Classical Laminated Plate Theory (CLPT-ESL). The implementation of Linear Elastic Model, Layered model is however based on First Order Shear Deformation Theory (FSDT-ESL). The difference between both theories is that FSDT theory considers transverse shear stresses, but for the benchmark example with unit in-plane loading, the results should match between both theories because of the zero or negligible shear strains. Note that the bending strains are actually curvatures, but for consistency purpose they will be called as strains throughout this document.

The relation between in-plane forces and moments with midplane strains is represented by

(1)

where A, B, and D are called extensional stiffness matrix, bending-extensional stiffness matrix, and bending stiffness matrix, respectively.

The same relation can be represented on flexibility form as

(2)

where a, b, and d are called extensional flexibility matrix, bending-extensional flexibility matrix, and bending flexibility matrix, respectively. The relationship between stiffness and flexibility matrices is

(3)

In the benchmark, the laminate flexibility matrix are computed in two ways, first directly from CLPT theory and then from midplane strains when unit loads and moments are applied. When unit in-plane forces Nij and unit moments Mij are applied, the midplane strains and curvature are the components of flexibility matrix. The midplane strains in the benchmark are computed numerically using commercial finite element software. Table 4 and Table 5 shows the flexibility matrix from the benchmark (Ref. 2).

Table 4: laminate flexibility matrix based on classical laminate Plate theory from benchmark.
Strains	N1	N2	N12	M1	M2	M12
ε1	1.131E-8	-3.697E-9	-4.42E-41	-1.59E-21	-3.8E-22	3.27E-21
ε2	-3.69E-9	2.010E-8	1.16E-40	3.977E-22	-8.0E-21	-9.6E-22
γ12	-4.42E-41	1.16E-40	5.593E-8	1.91E-21	-3.0E-21	-1.3E-20
κ1	-1.59E-21	-3.8E-22	3.27E-21	1.807E-1	-5.85E-2	-1.42E-3
κ2	3.977E-22	-8.0E-21	-9.6E-22	-5.85E-2	5.17E-1	-3.31E-1
κ12	1.91E-21	-3.0E-21	-1.3E-20	-1.42E-3	-3.31E-1	1.470E0

Table 5: laminate flexibility matrix based on midplane strains from benchmark.
Strains	N1	N2	N12	M1	M2	M12
ε1	1.131E-8	-3.697E-9	-3.30E-24	0.00E0	0.00E0	0.00E0
ε2	-3.69E-9	2.010E-8	1.44E-24	0.00E0	0.00E0	0.00E0
γ12	-2.06E-25	-1.65E-24	5.593E-8	0.00E0	0.00E0	0.00E0
κ1	0.00E0	0.00E0	0.00E0	1.807E-1	-5.85E-2	-1.42E-3
κ2	0.00E0	0.00E0	0.00E0	-5.85E-2	5.17E-1	-3.31E-1
κ12	0.00E0	0.00E0	0.00E0	-1.42E-3	-3.31E-1	1.470E0

The midplane strains for a unit change in temperature are given in the benchmark (Ref. 2).

Table 6: midplane strains for unit change in temperature from benchmark.
Strains	Theory	Numerical FEM
ε1	1.9155E-6	1.9155E-6
ε2	3.4566E-6	3.4566E-6
γ12	0.00E0	-2.117E-22
κ1	0.00E0	0.00E0
κ2	0.00E0	0.00E0
κ12	0.00E0	0.00E0

The midplane strains for a unit temperature gradient are given in the benchmark (Ref. 2).

Table 7: midplane strains for unit temperature gradient from benchmark.
Strains	Theory	Numerical FEM
ε1	0.00E0	0.00E0
ε2	0.00E0	0.00E0
γ12	0.00E0	0.00E0
κ1	1.7218E-6	1.7218E-6
κ2	4.8753E-6	4.8753E-6
κ12	-3.1156E-6	-3.1156E-6

In COMSOL Multiphysics, the stiffness (A, B, D) and flexibility matrices (a, b, d) are available as postprocessing variables. The midplane strains are computed for each unit load cases (six load cases). The strain vector then represents a column in the full flexibility matrix for a unit load case. For example, the membrane and bending midplane strains for unit N1 forms a first column of full flexibility matrix. The full flexibility matrix based on First Order Shear Deformation Theory (FSDT-ESL) and midplane strains from COMSOL are shown in Table 8 and Table 9 below

Table 8: laminate flexibility matrix based on fsdt theory from comsol.
Strains	N1	N2	N12	M1	M2	M12
ε1	1.131E-8	-3.697E-9	2.27E-25	-4.79E-22	-2.3E-22	-1.0E-21
ε2	-3.69E-9	2.010E-8	7.80E-24	-5.75E-23	1.40E-20	4.47E-20
γ12	2.27E-25	7.80E-24	5.593E-8	-1.27E-21	3.94E-20	1.80E-20
κ1	-4.79E-22	-2.3E-22	-1.0E-21	1.807E-1	-5.85E-2	-1.42E-3
κ2	-5.75E-23	1.40E-20	4.47E-20	-5.85E-2	5.17E-1	-3.31E-1
κ12	-1.27E-21	3.94E-20	1.80E-20	-1.42E-3	-3.31E-1	1.470E0

Table 9: laminate flexibility matrix based on midplane strains from comsol.
Strains	N1	N2	N12	M1	M2	M2
ε1	1.131E-8	-3.697E-9	0.00E0	0.00E0	0.00E0	0.00E0
ε2	-3.69E-9	2.010E-8	1.55E-23	0.00E0	0.00E0	0.00E0
γ12	-6.41E-24	1.42E-23	5.593E-8	0.00E0	0.00E0	0.00E0
κ1	0.00E0	0.00E0	0.00E0	1.807E-1	-5.85E-2	-1.42E-3
κ2	0.00E0	0.00E0	0.00E0	-5.85E-2	5.17E-1	-3.31E-1
κ12	0.00E0	0.00E0	0.00E0	-1.42E-3	-3.31E-1	1.470E0

The midplane strains for unit change in temperature and unit temperature gradient from COMSOL are

Table 10: midplane strains for unit change in temperature from COMSOL.
Strains	COMSOL
ε1	1.9155E-6
ε2	3.4566E-6
γ12	-1.645E-21
κ1	-2.371E-19
κ2	-1.2757E-17
κ12	8.380E-18

Table 11: midplane strains for unit temperature gradient from COMSOL.
Strains	COMSOL
ε1	6.21611E-26
ε2	-4.60298E-25
γ12	-4.79904E-26
κ1	1.72175E-6
κ2	4.87532E-6
κ12	-3.11557E-6

When comparing Table 4 to Table 8, Table 5 to Table 9, Table 6 to Table 10, and Table 7 to Table 11, an exact match can be found between the results of benchmark model and the results computed in COMSOL Multiphysics. The full flexibility matrix is found by inverting the full stiffness matrix, so the verification of the full flexibility matrix automatically verifies also the correctness of full stiffness matrix (not presented here but shown in the model).

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 and have an option to transform given into a symmetric or antisymmetric laminate. A repeated laminate can also be constructed using a transform option.

•

The third direction for the selected coordinate system in the , , or represents the normal direction in the Layered Shell and Shell interfaces. 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 Layered Shell interface, or the Equivalent Single Layer (ESL) theory based node in the Shell interface. The laminated composite presented in the current model is modeled using a node in the Shell interface.

References

1. J.N. Reddy, Mechanics of Laminated Composite Plates and Shells: Theory and Analysis, Second Edition, CRC Press, 2004.

2. P. Hopkins, Benchmarks for Membrane and Bending Analysis of Laminated Shells, Part 1: Stiffness Matrix and Thermal Characteristics, NAFEMS, 2005.

Composite_Materials_Module/Verification_Examples/laminated_shell_material_characteristics

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

Load the material properties from a file.

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 laminated_shell_material_characteristics_parameters.txt.

In order to apply unit in-plane forces and moments, as well as unit temperature difference and unit temperature gradient, create separate load and constraint groups.

Load Group for Unit N1

In the window, right-click and choose > .

In the window for , type Load Group for Unit N1 in the text field.

Repeat this five times to get six load groups. Rename them as shown in the table below.


Name	Label
Load Group 2	Load Group for Unit N2
Load Group 3	Load Group for Unit N12
Load Group 4	Load Group for Unit M1
Load Group 5	Load Group for Unit M2
Load Group 6	Load Group for Unit M12

In the window, under click .

Select all load groups and right click on to create a group.

Load Groups for Unit Loading

In the window, under > click .

In the window for , type Load Groups for Unit Loading in the text field.

Load Group for Unit Temperature Difference

In the window, right-click and choose .

In the window for , type Load Group for Unit Temperature Difference in the text field.

Load Group for Unit Temperature Gradient

Right-click and choose .

In the window for , type Load Group for Unit Temperature Gradient in the text field.

Select thermal load groups and right click on to create a group.

Load Groups for Thermal Loading

In the window, under > click .

In the window for , type Load Groups for Thermal Loading in the text field.

Constraint Group for Unit N1, N2, N12, M1 and M2

In the window, right-click and choose .

In the window for , type Constraint Group for Unit N1, N2, N12, M1 and M2 in the text field.

Repeat this four times to get required numbers of constraint groups. Rename them as shown in the table below.


Name	Label
Constraint Group 2	Constraint Group for Unit N1 and M1
Constraint Group 3	Constraint Group for Unit N2 and M2
Constraint Group 4	Constraint Group for Unit N12
Constraint Group 5	Constraint Group for Unit M12

Constraint Group for Unit N1 and M1

In the window, click .

Select all constraint groups and right click on to create a group.

Constraint Groups for Unit Loading

In the window, under > click .

In the window for , type Constraint Groups for Unit Loading in the text field.

Constraint Group for Thermal Loading

In the window, right-click and choose .

In the window for , type Constraint Group for Thermal Loading in the text field.

Material 1 (mat1)

In the window, under right-click and choose .

Now add a node and assign appropriate thickness and rotation angles to each layer. The laminate is symmetric. It is sufficient to define only half the laminate in the node. The transformation into a full laminate is performed through the layered material settings in the node.

Layered Material: [0/60/-60/0]_s

Right-click and choose .

In the window for , locate the section.

In the table, enter the following settings:


Layer	Material	Rotation	Value	Thickness	Mesh elements
Layer 1	Material 1 (mat1)	0	0 rad	th	1

Click three times.

In the table, enter the following settings:


Layer	Material	Rotation	Value	Thickness	Mesh elements
Layer 2	Material 1 (mat1)	60	1.0472 rad	th	1
Layer 3	Material 1 (mat1)	-60	-1.0472 rad	th	1
Layer 4	Material 1 (mat1)	0	0 rad	th	1

In the text field, type Layered Material: [0/60/-60/0]_s.

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 1e-2.

Click

Click the

button in the toolbar.

Materials

Layered Material Link 1 (llmat1)

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

The half laminate defined in the node can be transformed into a full symmetric laminate using a transform option in the layered material settings.

In the window for , locate the section.

From the list, choose .

Click to expand the section. In the text field, type 0.5.

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

Click in the upper-right corner of the section.

The geometry is in an XY-plane in which the fibers are oriented with respect to the X direction. Hence set the first axis of the laminate coordinate system in the X direction.

Definitions (comp1)

Boundary System 1 (sys1)

In the window, expand the > node, then click .

In the window for , locate the section.

Find the subsection. From the list, choose .

Shell (shell)

Click the

button in the toolbar.

In the dialog, in the tree, select the checkbox for the node > .

Click .

Set the discretization for the displacement field to in order to resemble the benchmark example.

In the window, under click .

In the window for , click to expand the section.

From the list, choose .

Linear Elastic Material, Layered 1

In the toolbar, click

and choose .

In order to study two thermal load cases separately, add two subfeatures and activate them in different load groups.

Select Boundary 1 only.

In the window for , locate the section.

From the list, choose .

Select the checkbox.

Thermal Expansion for Unit Temperature Difference

In the toolbar, click

and choose .

In the window for , type Thermal Expansion for Unit Temperature Difference in the text field.

Locate the section. From the Tin list, choose . In the associated text field, type 293.15[K] +1[K].

In the toolbar, click

and choose .

Linear Elastic Material, Layered 1

In the window, click .

Thermal Expansion for Unit Temperature Gradient

In the toolbar, click

and choose .

In the window for , type Thermal Expansion for Unit Temperature Gradient in the text field.

Locate the section. From the list, choose .

In the T′ text field, type 1[K/m].

In the toolbar, click

and choose .

Global Definitions

Material 1 (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	{Evector1, Evector2}	{E1, E2}	Pa	Transversely isotropic
Poisson’s ratio	{nuvector1, nuvector2}	{nu12, nu23}	1	Transversely isotropic
Shear modulus	{Gvector1}	{G}	N/m²	Transversely isotropic
Density	rho	1	kg/m³	Basic
Coefficient of thermal expansion	{alpha11, alpha22, alpha33} ; alphaij = 0	{alpha1, alpha2, alpha3}	1/K	Basic

Apply different constraints and point loads for different load cases as shown in Table 2 and Table 3. Attach appropriate load and constraint groups to these constraints and load features.

Shell (shell)

Fixed Constraint for Unit N1, N2, N12, M1 and M2

In the toolbar, click

and choose .

In the window for , type Fixed Constraint for Unit N1, N2, N12, M1 and M2 in the text field.

Select Point 1 only.

In the toolbar, click

and choose .

Prescribed Displacement/Rotation for Unit N1 and M1

In the toolbar, click

and choose .

In the window for , type Prescribed Displacement/Rotation for Unit N1 and M1 in the text field.

Select Point 2 only.

Locate the section. From the list, choose .

In the toolbar, click

and choose .

Duplicate the node nine times to get required numbers of nodal constraints. Label, selection, constraints, constraint groups should be as shown in table below.


Name	Label	Selection	DOFs to be constrained	Constraint group
Prescribed Displacement/Rotation 2	Prescribed Displacement/Rotation for Unit N2 and M2	3	v	Constraint Group for N2 and M2
Prescribed Displacement/Rotation 3	Prescribed Displacement/Rotation for Unit N12 (1)	2	u, v	Constraint Group for N12
Prescribed Displacement/Rotation 4	Prescribed Displacement/Rotation for Unit N12 (2)	3	u	Constraint Group for N12
Prescribed Displacement/Rotation 5	Prescribed Displacement/Rotation for Unit M12 (1)	1	u, v, w, theta_y	Constraint Group for M12
Prescribed Displacement/Rotation 6	Prescribed Displacement/Rotation for Unit M12 (2)	4	v	Constraint Group for M12
Prescribed Displacement/Rotation 7	Prescribed Displacement/Rotation for Unit M12 (3)	2	w	Constraint Group for M12
Prescribed Displacement/Rotation 8	Prescribed Displacement/Rotation for Unit Change in Temperature (1)	1	u, v, w	Constraint Group for Thermal Loading
Prescribed Displacement/Rotation 9	Prescribed Displacement/Rotation for Unit Change in Temperature (2)	3	w	Constraint Group for Thermal Loading
Prescribed Displacement/Rotation 10	Prescribed Displacement/Rotation for Unit Change in Temperature (3)	2	u, w	Constraint Group for Thermal Loading

Select all constraint features and right click on to create a group.

Constraints

In the window, under > click .

In the window for , type Constraints in the text field.

Point Load for Unit N1

In the toolbar, click

and choose .

In the window for , type Point Load for Unit N1 in the text field.

Select Points 3 and 4 only.

Locate the section. Specify the FP vector as


Fi	x
0	y
0	z

In the toolbar, click

and choose .

Duplicate the node nine times to get required numbers of nodal loads. Label, selection, loads, load groups should be as shown in the table below.


Name	Label	Selection	Loads/Moments	Load group
Point Load 2	Point Load for Unit N2	2, 4	F_y = Fi	Load Group for N2
Point Load 3	Point Load for Unit N12 (1)	2, 4	F_x = Fi	Load Group for N12
Point Load 4	Point Load for Unit N12 (2)	3, 4	F_y = Fi	Load Group for N12
Point Load 5	Point Load for Unit M1 (1)	1, 2	M_y = -M	Load Group for M1
Point Load 6	Point Load for Unit M1 (2)	3, 4	M_y = M	Load Group for M1
Point Load 7	Point Load for Unit M2 (1)	1, 3	M_x = M	Load Group for M2
Point Load 8	Point Load for Unit M2 (2)	2, 4	M_x = -M	Load Group for unit M2
Point Load 9	Point Load for Unit M12 (1)	3	F_z = Fo	Load Group for Unit M12
Point Load 10	Point Load for Unit M12 (2)	4	F_z = -Fo	Load Group for Unit M12

Select all load features and right click on to create a group.

Loads

In the window, under > click .

In the window for , type Loads in the text field.

Mesh 1

Use a single quadrilateral element.

Mapped 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Distribution 1

Right-click and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. In the text field, type 1.

Click

Study 1

Disable the default plots for this study.

In the window, click .

In the window for , locate the section.

Clear the checkbox.

Create eight different load cases each for six unit loads/moments and two for thermal loading. Assign appropriate load groups and constraint groups for each load cases as per Table 2 and Table 3.

Step 1: Stationary

In the window, under click .

In the window for , click to expand the section.

Select the checkbox.

Click

seven times.

In the table, select the load cases and select appropriate load and constraint groups.


Load case	Active load groups and constraint groups
Load case for unit N1	lg1 cg1 cg2
Load case for unit N2	lg2 cg1 cg3
Load case for unit N12	lg3 cg1 cg4
Load case for unit M1	lg4 cg1 cg2
Load case for unit M2	lg5 cg1 cg3
Load case for unit M12	lg6 cg5
Load case for unit change in temperature	lg7 cg6
Load case for unit temperature gradient	lg8 cg6

In the toolbar, click

In order to find the laminate flexibility and stiffness matrices, use node under .

Results

Extensional Flexibility Matrix

In the toolbar, click

In the window for , locate the section.

From the list, choose .

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

In the text field, type Extensional Flexibility Matrix.

Point Matrix Evaluation 1

In the toolbar, click

and choose .

Select Point 3 only.

In the window for , click in the upper-right corner of the section. From the menu, choose > > > > .

Extensional Flexibility Matrix

In the window, click .

In the toolbar, click

Extensional Flexibility Matrix

Go to the window.

To compute the remaining flexibility and stiffness matrices, duplicate the above node seven times and change the expression to compute shell.Db, shell.Dd, shell.Das, shell.DA, shell.DB, shell.DD and shell.DAs.

Select evaluation groups corresponding to the flexibility and stiffness matrices, and right click on to create a group.

Results

Flexibility and Stiffness Matrices

In the window, under click .

In the window for , type Flexibility and Stiffness Matrices in the text field.

Use a node under to compute the midplane strains for each load case. The choice of point does not matter as the model gives a uniform strain field.

While evaluating the midplane strains corresponding to each load case, evaluate the corresponding in-plane force or moment postprocessing variable in order to verify the correctness of the applied forces and constraints.

Layered Material 1

In the toolbar, click

and choose .

Cut Point 3D 1

In the toolbar, click

In the window for , locate the section.

From the list, choose .

Locate the section. In the text field, type 1e-2.

In the text field, type 0.

Midplane Strains for Unit N1

In the toolbar, click

In the window for , type Midplane Strains for Unit N1 in the text field.

Locate the section. From the list, choose .

From the list, choose .

In the list box, select .

Locate the section. Select the checkbox.

Locate the section. From the list, choose .

Point Evaluation 1

Right-click and choose .

In the window for , locate the section.

In the table, enter the following settings:


Expression	Unit	Description
shell.eml11	1	Membrane part of strain tensor (local), 11 component
shell.eml22	1	Membrane part of strain tensor (local), 22 component
2*shell.eml12	1	Membrane part of strain tensor (local), 12 component
shell.ebl11	1/m	Bending part of strain tensor (local), 11 component
shell.ebl22	1/m	Bending part of strain tensor (local), 22 component
2*shell.ebl12	1/m	Bending part of strain tensor (local), 12 component
shell.Nl11	N/m	Local in-plane force, 11 component

Midplane Strains for Unit N1

In the window, click .

In the toolbar, click

Midplane Strains for Unit N1

Go to the window.

To compute the midplane strains for remaining load cases, duplicate the above node seven times and change the load case in the section of corresponding node. Replace the in-plane force/moment variable in the last row of table in node with appropriate variable corresponding to the load cases.

Select evaluation groups corresponding to the midplane strains, and right click on to create a group.

Results

Midplane Strains

In the window, under click .

In the window for , type Midplane Strains in the text field.