PDF
Micromechanics of Failure: Multiscale Analysis of a Composite Structure
Introduction
The use of fiber composites ranges from the transportation and energy sectors to the consumer industry. Compared to traditional monolithic materials, fiber composites offer various properties suitable for tailor-made applications. Along with macroscale analyses, structural composites need microscale stress and failure analyses to identify the critical constituents in laminate structures.
Composites can be analyzed at both macro or micro scales, and either analysis has its benefits and limitations. Analyses at both macro and micro scales, so-called multiscale analyses, offer an in-depth insight into the composite structure as well as its constituents’ response and help to study the micromechanics of failure based on the global scale loading.
Full multiscale analysis which involves macro analysis with micro analysis at each material point is computationally expensive. In this example, instead of carrying out a micro-level analysis at each material point, the microscale analysis is performed on a few critical material points that are near to failure or have stress concentrations according to the macro-level analysis.
The continuum-based, composite-specific failure theories are useful and give satisfactory results in many situations. However, composite structures used in critical applications may demand a more accurate prediction of failure. This is possible when the mechanics-based failure theories are applied at micro level for individual constituents. Ref. 2 provides the details of micromechanical failure.
In reality, the constituents for unidirectional composites are fiber, matrix, and the interface between them. For simplicity, the interface is often ignored for a micromechanical analysis. In this example, all three constituents are considered.
Read more about the Composite Materials Module in the COMSOL blog, Introduction to the Composite Materials Module.
Model Definition
In this model three different types of analyses are performed:
•
A micromechanical analysis to predict the homogenized material properties
•
A macromechanical analysis using layerwise theory to get the global response for given load and boundary conditions
•
A new micromechanical analysis to predict the local stress field and failure risk based on the average strains computed in the macro-level analysis
Micromechanical analysis (material properties)
A micromechanics analysis of a unidirectional repeating unit cell (RUC) is performed to obtain its homogenized material properties. The composite layer is assumed to be made of carbon fibers unidirectionally embedded in epoxy resin. Between fiber and matrix a thin interface is assumed. A RUC having a cylindrical fiber located at the middle of matrix is shown in Figure 1. The fiber radius is computed assuming a fiber volume fraction of 0.6.
Figure 1: Geometry of the unit cell with a carbon fiber, a thin interface and an epoxy matrix.
Fiber, Interface, and Matrix Properties
The layers of the laminate are made of T300 carbon fiber, epoxy resin, and a custom interface material. The carbon fiber is assumed to be transversely isotropic. The interface material and epoxy resin are assumed to be isotropic. The fiber and matrix materials are taken from built-in Composites material library and their material properties are given in Table 1 and Table 2, respectively.
We have assumed certain material properties and the thickness for the interface material based on the discussion in Ref. 1. According to Ref. 1, for fiber composite materials, the interface, or more precisely the interfacial zone, consists of near-surface layers of fiber and matrix and any layer(s) of material existing between these surfaces. Very weak or very strong interfaces are detrimental to the overall performance of the composite. Hence, an interface with optimal strength is preferred to enhance the performance. With these points in mind, this model assumes elastic properties of the interface that are not as strong as fiber nor as weak as matrix. The interface material properties are based on the discussion in Ref. 1.
Table 1: Carbon fiber material properties.
Material property
Value
{E1, E2}
{230,15} GPa
G12
27 GPa
{υ12, υ23}
{0.2, 0.0714} 
 ρ
1760 kg/m3
Table 2: Epoxy resin material properties.
Material property
Value
 E
3.25 GPa
 υ
0.265
 ρ
1250 kg/m3
Table 3: Interface material properties.
Material property
Value
 E
100 GPa
 υ
0.2
 ρ
1400 kg/m3
Thin Layer
The interface between fiber and matrix is not modeled explicitly but considered implicitly using the Thin Layer node in the Solid Mechanics interface. The feature has a Linear Elastic Material node that models the elastic behavior of the interface. The thin layer affects the homogenized material properties as well as the local stress distribution.
Cell Periodicity
To perform a micromechanics analysis, the Cell Periodicity node in the Solid Mechanics interface is used. The Cell Periodicity node is used to apply periodic boundary conditions on three pairs of faces of the unit cell.
To extract the homogenized elasticity matrix for a layer, the unit cell needs to be analyzed for six different load cases. The Average Strain periodicity type needs to be selected to obtain the homogenized elasticity matrix. This is automatically done with the help of the action buttons in the Cell Periodicity node. The Cell Periodicity node has three action buttons in the toolbar of the Periodicity Type section: Create Load Groups and Study, Create Material by Value, and Create Material by Reference. The action button Create Load Groups and Study generates six different load groups and a stationary study with six load cases. The action button Create Material by Reference generates a Global Material with an elasticity matrix corresponding to that of the homogenized material, where properties are in terms of variables. The action button Create Material by Value generates a Global Material with an elasticity matrix corresponding to that of the homogenized material, where properties are in number format. The generated global material can be used to define the properties of individual layers in a composite laminate.
Macromechanical Analysis (Global Response)
Layerwise (LW) Theory
In the Layerwise theory, the degrees of freedom are the displacements (u, v, w) available on the reference surface (or modeled surface) as well as in the through-thickness direction. From a constitutive equation point of view, this theory is similar to 3D solid elasticity. The layerwise theory is useful for detailed modeling of thick composite laminates because it can capture interlaminar shear stresses. It could therefore be used to also study delamination.
Geometry and Boundary Conditions
The model represents a composite cylinder with a length of 0.5 m and a radius of 0.1 m. It is shown in Figure 2. The boundary conditions and loading are:
•
One end of the cylinder is fixed.
•
The other end has a transverse load of 75 kN, represented as a uniform boundary load on cross section.
Figure 2: Geometry with boundary conditions and loading.
Figure 3: Through-thickness view of the laminated material with four layers.
Stacking Sequence and Material Properties
The laminate consists of four layers of 1 mm thickness, as shown in Figure 3. The orientations of the layers are different; starting from the bottom of the laminate, they are 90, 0, 90, and 0 degrees, as shown in Figure 4. The orientation of a layer is specified with respect to the laminate coordinate system. The material properties for each layer are given by the homogenized material computed in the first micromechanical analysis.
Figure 4: Stacking sequence [90/0/90/0] for the laminate showing the fiber orientation of each layer, from bottom to top.
Failure Criteria
Two composite-specific failure criteria, Hashin and Puck, are used to evaluate the critical regions in the composite cylinder for the given loading condition. These are advanced composite-specific criteria that account for multiaxial states of stress, and different failure modes for tensile and compressive loading. The failure modes considered by these two criteria are summarized in Table 4.
Table 4: Failure modes.
Failure criterion
Failure modes
 Hashin
Fiber rupture in tension and shear
Fiber buckling in compression
Matrix failure in tension and shear
Matrix failure in compression and shear
Interlaminar failure in tension
Interlaminar failure in compression
 Puck
Fiber rupture in tension
Fiber buckling in compression
Matrix failure in tension and in-plane shear (Interfiber
failure: Mode A)
Matrix failure in compression and in-plane shear (Interfiber failure: Mode B)
Matrix failure in compression and in-plane shear (Interfiber failure: Mode C
The tensile, compressive, and shear strengths of ply are taken from Ref. 2 and are given in Table 5.
Table 5: Material strengths.
Material strengths
Value
{σts1,σts2,σts3}
{1500,50,50} MPa
{σcs1,σcs2,σcs3}
{900,230,230} MPa
{σss23,σss13,σss12}
{90,90,90} MPa
The Puck criterion needs additional strength properties which are tabled in Table 6.
Table 6: Additional strength properties
Property
Variable
Value
Ultimate tensile strain, 11 direction
 εts1
0.1
Ultimate compressive strain, 11 direction
 εcs1
0.08
Linear degradation stress
 σ1D
2000 MPa
Micromechanical Analysis (Local Response)
To determine the local response of the constituents to the global loading conditions, the same unit cell geometry and material properties as in the first analysis are used, and the macro-level strains from the second analysis are prescribed. The micromechanical analysis is performed at a few material points, chosen to be where failure or maximum stress occurs in the global analysis.
Failure Criteria
At a micro level, the mechanics-based failure criteria can be used as the constituents are monolithic. These fundamental criteria predict failure more accurately than the global level phenomenological criteria; see Ref. 2.
For the fiber, the Tsai–Wu orthotropic failure criterion is the best suited. For unidirectional composites, the fibers are longitudinally continuous and have higher modulus and strength in the longitudinal direction. Hence, the fibers take the longitudinal tensile and compressive loads. In the transverse direction, the fibers are bonded by the matrix, which plays an important role for the transverse and shear loads. As stated in Ref. 2, if the transverse and shear stresses from the Tsai–Wu orthotropic failure criterion are neglected, the failure criterion for the fiber is reduced to the simple relations
where σi1 is the stress component in the fiber direction and σt1 and σc1 are the tensile and compressive strengths, respectively, of the fiber.
The matrix is isotropic and has different strengths in tension and compression. Theoretical studies and experiments show that the failure of the matrix depends on deviatoric and volumetric stresses. In Ref. 2, the following failure criterion was proposed for the matrix:
where σm is the von Mises stress and I1 is the first invariant of the stress tensor.
The interface fails primarily because the normal and tangential tractions exceed their strength limits, which results in debonding. In Ref. 2, the following quadratic failure criterion was proposed for the interface:
where tn and ts are normal (perpendicular to the interface boundary) and shear (tangential to the interface boundary) tractions, and σn and σs are the normal and shear strength, respectively. The angular brackets around the normal traction are Macaulay brackets, which return the argument if positive and zero otherwise.
The constituent’s strength properties are taken from Ref. 2 and given in Table 7.
Table 7: Constituent’s strength properties
Property
Variable
Value
Tensile strength of fiber
 σts1
2458 MPa
Compressive strength of fiber
 σcs1
1500 MPa
Tensile strength of matrix
 σts
103 MPa
Compressive strength of matrix
 σcs
265 MPa
Interfacial normal strength of interface
 σns
60 MPa
Interfacial shear strength of interface
 σss
180 MPa
Results and Discussion
In the micromechanics analysis, six load cases are used to evaluate the elasticity matrix. The distribution of the effective (von Mises) stress for four of the load cases is shown in Figure 5. From Figure 5 one can see how individual constituents respond to different load cases.
The homogenized material obtained from the first micromechanical analysis is used in the subsequent macromechanical analysis.
Figure 5: von Mises stress distribution in the unit cell for four load cases.
The stress in the fiber direction in the composite cylinder obtained from the macro-level analysis is presented in Figure 6. Both ends of the cylinder have regions with higher stresses. Figure 7 shows the stress in the fiber direction in five interfaces of the laminate, indicating that the maximum stress occurs at cylinder ends in inner and upper layers. To find the exact location of the maximum stress, a Surface Maximum node can be used (for details, see the modeling instructions). Based on this, it is clear that the maximum stress occurs in the outer layer of the laminate toward the fixed end, and in the inner layer toward the loaded end. Both positions where the maximum stress occurs are used for the subsequent micromechanical analysis.
The distributions of the Hashin and Puck failure indexes in the composite cylinder are shown in Figure 8 and Figure 9, respectively. For the Hashin failure criterion, the maximum failure index is at the outer layer toward the loaded end, while for the Puck criterion the maximum failure index is at the second layer from inside toward the loaded end. The puck criterion shows higher failure index even in inner and outer layers. Hence, the material points from inner and outer layers are used for the subsequent micromechanical analysis. Both failure criteria involve different failure modes, so it is important to check each individual mode’s failure indexes. Table 8 shows the maximum failure indexes of the individual failure mode for both failure criteria. The values indicate that for this composite structure, the matrix material would fail in the tension.
Table 8: Maximum failure indexes of different failure modes.
Failure Criterion
Failure Modes
Failure Index
 Hashin
Fiber rupture in tension and shear
Fiber buckling in compression
Matrix failure in tension and shear
Matrix failure in compression and shear
Interlaminar failure in tension
Interlaminar failure in compression
0.67063
0.93302
1.03461
0.67062
5.6948·10-5
1.5818·10-4
 Puck
Fiber rupture in tension
Fiber buckling in compression
Matrix failure in tension and in-plane shear (Mode A)
Matrix failure in compression and in-plane shear (Mode B)
Matrix failure in compression and in-plane shear (Mode C)
0.06035
0.07544
1.00741
0.81894
0.58237
Figure 6: The stress in the fiber direction in the composite laminate.
Figure 7: The stress in the fiber direction in the five interfaces of the composite laminate.
Figure 8: Hashin failure index distribution in the composite laminate.
Figure 9: Puck failure index distribution in the composite laminate.
For the second micromechanical analysis, several material locations are selected and macro strains from these locations are prescribed for the unit cell structure to get the local stress and strain fields that are eventually useful to carry out micromechanical failure analysis. Figure 10 shows the von Mises stress distribution in the constituents at a material point located in the inner layer. It shows that compared to macro stress the micro stress is very high. The stress distribution in the constituents at the various material locations is shown in Figure 11. Based on macromechanical analysis, two critical points one at inner layer and one at outer layer toward loaded end are chosen for subsequent micromechanical analysis. The micromechanical failure analysis is performed at these material points, and the results are presented in Figure 12 and Figure 13. Both figures show that the failure indexes are maximum in the matrix compared to the fiber and interface, which supports the finding based on the macromechanical failure analysis. The micromechanical failure indexes are less than one, indicating that there is no failure in the constituent materials at these critical points. Table 9 shows the maximum values of the failure indexes in the constituents at two different material locations, which are chosen as critical locations based on the macromechanical analysis.
Table 9: Maximum user defined failure indexes in the constituents at different material locations.
Material Locations
Constituents
Failure Index
Point in the inner layer at bottom of loaded edge
Matrix
Fiber
Interface
0.67705
0.56783
3.41362·10-4
Point in the outer layer at bottom of loaded edge
Matrix
Fiber
Interface
0.77868
0.24251
1.02509·10-5
Figure 10: von Mises stress in the constituents at a particular material location of the composite cylinder.
Figure 11: von Mises stress in the constituents at multiple material locations of the composite cylinder.
Figure 12: User defined failure indexes in the constituents at a particular material location of the composite cylinder.
Figure 13: User defined failure indexes in the constituents at a particular material location of the composite cylinder.
Notes About the COMSOL Implementation
•
Modeling a composite laminated shell requires a 2D surface geometry, called a base surface, and a Layered Material node that adds an extra dimension (1D) to the base surface geometry in the surface normal direction. Using the Layered Material functionality, you can model several layers of different thicknesses, material properties, and fiber orientations. You can optionally specify the interface materials between the layers and the control mesh elements in each layer.
•
The Layered Material Link and Layered Material Stack have an option to transform the given Layered Material into a symmetric or antisymmetric laminate. A repeated laminate can also be constructed using a transform option.
•
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.
•
The built-in Composites material library contains data for fiber and matrix constituents as well as for unidirectional and bidirectional laminae.
•
To analyze the results in a composite shell, you can either create a slice plot using the Layered Material Slice plot for in-plane variation of a quantity, or you can create a Through Thickness plot for out-of-plane variation of a quantity at a point. To visualize the results as a 3D solid object, you can use the Layered Material dataset, which creates a virtual 3D solid object combining the surface geometry (2D) and the extra dimension (1D).
References
1. K.K. Chawla, Composite Materials: Science and Engineering, 4th ed., Springer, 2019.
2. S.K. Ha, K.K. Jin, and Y. Huang, “Micro-Mechanics of Failure (MMF) for Continuous Fiber Reinforced Composites,” J. Comp. Mat., vol. 42, no. 18, pp. 1873–1895, 2008.
Application Library path: Composite_Materials_Module/Tutorials/composite_multiscale
Modeling Instructions (Micromechanics)
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 > Solid Mechanics (solid).
3
Click Add.
4
Click  Done.
Global Definitions
Geometric Properties
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, type Geometric Properties in the Label text field.
3
Locate the Parameters section. Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file composite_multiscale_parameters.txt.
Elastic Properties
1
In the Home toolbar, click  Parameters and choose Add > Parameters.
2
In the Settings window for Parameters, type Elastic Properties in the Label text field.
3
Locate the Parameters section. Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file composite_multiscale_material_properties.txt.
Strength Properties
1
In the Home toolbar, click  Parameters and choose Add > Parameters.
2
In the Settings window for Parameters, type Strength Properties in the Label text field.
3
Locate the Parameters section. Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file composite_multiscale_strength_properties.txt.
5
In the Model Builder window, right-click Global Definitions and choose Geometry Parts > Part Libraries.
Part Libraries
1
In the Part Libraries window, select COMSOL Multiphysics > Unit Cells and RVEs > Fiber Composites > unidirectional_fiber_square_packing in the tree.
2
Click  Add to Model.
3
In the Select Part Variant dialog, select Specify fiber diameter in the Select part variant list.
4
Click OK.
Component: Micromechanics (Material Properties)
1
In the Model Builder window, click Component 1 (comp1).
2
In the Settings window for Component, type Component: Micromechanics (Material Properties) in the Label text field.
Geometry 1
Unidirectional Fiber Composite, Square Packing 1 (pi1)
1
In the Geometry toolbar, click  Part Instance and choose Unidirectional Fiber Composite, Square Packing.
To customize the unit cell geometry, enter the unit cell parameters in the input parameters of the part.
2
In the Settings window for Part Instance, locate the Input Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
df
2*r_f
0.0087404 m
Fiber diameter
wm
l
0.01 m
Cell width
dm
l
0.01 m
Cell depth
hm
l
0.01 m
Cell height
4
Locate the Position and Orientation of Output section. Find the Displacement subsection. In the xwi text field, type -0.005[m].
5
In the ywi text field, type -0.005[m].
6
In the zwi text field, type -0.005[m].
Form Union (fin)
1
In the Model Builder window, click Form Union (fin).
2
In the Settings window for Form Union/Assembly, click  Build Selected.
3
Click the  Zoom Extents button in the Graphics toolbar.
In order to simplify the modeling process create explicit selections.
Interface Selection
1
In the Geometry toolbar, click  Selections and choose Explicit Selection.
2
In the Settings window for Explicit Selection, locate the Entities to Select section.
3
From the Geometric entity level list, choose Boundary.
4
On the object fin, select Boundaries 6–9 only.
5
In the Label text field, type Interface Selection.
Solid Mechanics (solid)
Linear Elastic Material 1
1
In the Model Builder window, under Component: Micromechanics (Material Properties) (comp1) > Solid Mechanics (solid) click Linear Elastic Material 1.
2
In the Settings window for Linear Elastic Material, locate the Linear Elastic Material section.
3
From the Material symmetry list, choose Orthotropic.
Add a Thin Layer feature to model the interface between the fiber and matrix.
Thin Layer 1
1
In the Physics toolbar, click  Boundaries and choose Thin Layer.
2
In the Settings window for Thin Layer, locate the Boundary Selection section.
3
From the Selection list, choose Interface Selection.
4
Locate the Boundary Properties section. In the Lth text field, type th_i.
Cell Periodicity 1
1
In the Physics toolbar, click  Domains and choose Cell Periodicity.
2
In the Settings window for Cell Periodicity, locate the Periodicity Settings section.
3
From the Boundary conditions list, choose Average strain.
4
Locate the Effective Properties section. Select the Compute density checkbox.
5
Select the Compute elasticity matrix, standard notation checkbox.
Boundary Pair 1
1
In the Physics toolbar, click  Attributes and choose Boundary Pair.
2
In the Settings window for Boundary Pair, locate the Boundary Selection section.
3
From the Selection list, choose Pair 1 (Unidirectional Fiber Composite, Square Packing 1).
Boundary Pair 2
1
Right-click Boundary Pair 1 and choose Duplicate.
2
In the Settings window for Boundary Pair, locate the Boundary Selection section.
3
From the Selection list, choose Pair 2 (Unidirectional Fiber Composite, Square Packing 1).
Boundary Pair 3
1
Right-click Boundary Pair 2 and choose Duplicate.
2
In the Settings window for Boundary Pair, locate the Boundary Selection section.
3
From the Selection list, choose Pair 3 (Unidirectional Fiber Composite, Square Packing 1).
In the upper-right corner of the Periodicity type section, you can find three buttons: Create Load Groups and Study, Create Material by Reference, and Create Material by Value. When the Average strain option is selected for the computation of the elasticity matrix, you can automatically generate load groups, a study, and a material by clicking on these buttons.
Cell Periodicity 1
1
In the Model Builder window, click Cell Periodicity 1.
2
In the Settings window for Cell Periodicity, click Automated Model Setup in the upper-right corner of the Periodicity Settings section. From the menu, choose Create Load Groups and Study to generate load groups and a study node.
COMSOL Multiphysics is equipped with built-in material properties for a number of composite constituents. Select the needed materials from the Composites material folder in the built-in material library.
Materials
Material Link 1: Matrix
1
In the Model Builder window, under Component: Micromechanics (Material Properties) (comp1) right-click Materials and choose More Materials > Material Link.
2
In the Settings window for Material Link, type Material Link 1: Matrix in the Label text field.
3
Locate the Geometric Entity Selection section. From the Selection list, choose Matrix (Unidirectional Fiber Composite, Square Packing 1).
4
Locate the Link Settings section. Click  Add Material from Library.
Add Material to Material Link 1: Matrix (matlnk1)
1
Go to the Add Material to Material Link 1: Matrix (matlnk1) window.
2
In the tree, select Composites > Matrix Constituents > Epoxy polymer.
3
Click Add Material.
Materials
Material Link 2: Fiber
1
Right-click Materials and choose More Materials > Material Link.
2
In the Settings window for Material Link, type Material Link 2: Fiber in the Label text field.
3
Locate the Geometric Entity Selection section. From the Selection list, choose Fiber (Unidirectional Fiber Composite, Square Packing 1).
4
Locate the Link Settings section. Click  Add Material from Library.
Add Material to Material Link 2: Fiber (matlnk2)
1
Go to the Add Material to Material Link 2: Fiber (matlnk2) window.
2
In the tree, select Composites > Fiber Constituents > T-300 carbon fiber.
3
Click Add Material.
Materials
Material Link 3: Interface
1
Right-click Materials and choose More Materials > Material Link.
2
In the Settings window for Material Link, type Material Link 3: Interface in the Label text field.
3
Locate the Geometric Entity Selection section. From the Geometric entity level list, choose Boundary.
4
From the Selection list, choose Interface Selection.
5
Locate the Link Settings section. Click  Blank Material.
Global Definitions
Interface material
1
In the Model Builder window, under Global Definitions > Materials click Material 3 (mat3).
2
In the Settings window for Material, type Interface material in the Label text field.
3
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
E_i
Pa
Young’s modulus and Poisson’s ratio
Poisson’s ratio
nu
nu_i
1
Young’s modulus and Poisson’s ratio
Density
rho
rho_i
kg/m³
Basic
Mesh 1
Identical Mesh 1
1
In the Mesh toolbar, click  More Attributes and choose Identical Mesh.
2
In the Settings window for Identical Mesh, locate the First Entity Group section.
3
From the Selection list, choose Pair 1, Source (Unidirectional Fiber Composite, Square Packing 1).
4
Locate the Second Entity Group section. From the Selection list, choose Pair 1, Destination (Unidirectional Fiber Composite, Square Packing 1).
Free Triangular 1
1
In the Mesh toolbar, click  More Generators and choose Free Triangular.
2
In the Settings window for Free Triangular, locate the Boundary Selection section.
3
From the Selection list, choose Pair 1, Source (Unidirectional Fiber Composite, Square Packing 1).
4
Click  Build Selected.
Swept 1
1
In the Mesh toolbar, click  Swept.
2
In the Settings window for Swept, click  Build All.
Study: Micromechanics (Material Properties)
1
In the Model Builder window, click Cell Periodicity Study.
2
In the Settings window for Study, type Study: Micromechanics (Material Properties) in the Label text field.
3
In the Study toolbar, click  Compute.
Set default units for result presentation.
Results
Preferred Units 1
1
In the Results toolbar, click  Configurations and choose Preferred Units.
2
In the Settings window for Preferred Units, locate the Units section.
3
Click  Add Physical Quantity.
4
In the Physical Quantity dialog, select Solid Mechanics > Stress tensor (N/m^2) in the tree.
5
Click OK.
6
In the Settings window for Preferred Units, locate the Units section.
7
In the table, enter the following settings:
Quantity
Unit
Preferred unit
Stress tensor
N/m^2
MPa
8
Click  Apply.
Stress, Unit Cell
1
In the Model Builder window, under Results click Stress (solid).
2
In the Settings window for 3D Plot Group, type Stress, Unit Cell in the Label text field.
3
Click to expand the Title section. From the Title type list, choose Manual.
4
Click to expand the Plot Array section. From the Array type list, choose Linear.
Selection 1
1
In the Model Builder window, expand the Stress, Unit Cell node.
2
Right-click Volume 1 and choose Selection.
3
Select Domain 1 only.
Deformation
In the Model Builder window, right-click Deformation and choose Delete.
Volume 2
1
In the Model Builder window, under Results > Stress, Unit Cell right-click Volume 1 and choose Duplicate.
2
In the Settings window for Volume, click to expand the Inherit Style section.
3
From the Plot list, choose Volume 1.
4
Click to expand the Plot Array section. Clear the Apply to dataset edges checkbox.
Selection 1
1
In the Model Builder window, expand the Volume 2 node, then click Selection 1.
2
In the Settings window for Selection, locate the Selection section.
3
Click  Clear Selection.
4
Select Domain 2 only.
Surface 1
In the Model Builder window, expand the Results > Stress, Thin Layer (solid) node, then click Surface 1.
1
Drag and drop below Stress, Unit Cell > Volume 2.
2
In the Settings window for Surface, click to expand the Inherit Style section.
3
From the Plot list, choose Volume 1.
4
Click to expand the Plot Array section. Clear the Apply to dataset edges checkbox.
Deformation
1
In the Model Builder window, expand the Surface 1 node.
2
Right-click Deformation and choose Delete.
Stress, Unit Cell
In the Model Builder window, under Results click Stress, Unit Cell.
Table Annotation 1
1
In the Stress, Unit Cell 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
z-coordinate
Annotation
-l/4
-1.2*l
0
Matrix
l
-1.2*l
0
Fiber
2.2*l
-1.2*l
0
Interface
5
Locate the Coloring and Style section. Clear the Show point checkbox.
Stress, Unit Cell
1
Click the  Go to Default View button in the Graphics toolbar.
2
Click the  Show Grid button in the Graphics toolbar.
3
In the Model Builder window, click Stress, Unit Cell.
4
In the Stress, Unit Cell toolbar, click  Plot.
Stress, Thin Layer (solid)
In the Model Builder window, right-click Stress, Thin Layer (solid) and choose Delete.
Stress, Unit Cell
In the Model Builder window, under Results right-click Stress, Unit Cell and choose Group.
Micromechanics (Material Properties)
In the Settings window for Group, type Micromechanics (Material Properties) in the Label text field.
Before you add a Layered Shell interface, create a homogenized material from the Cell Periodicity feature.
The homogenized material can be created by using either of the two action buttons in the Periodicity type section: Create Material by Reference or Create Material by Value. Choose the second action button in order to generate the material with numbers.
Solid Mechanics (solid)
Cell Periodicity 1
1
In the Model Builder window, under Component: Micromechanics (Material Properties) (comp1) > Solid Mechanics (solid) click Cell Periodicity 1.
2
In the Settings window for Cell Periodicity, click Automated Model Setup in the upper-right corner of the Periodicity Settings section. From the menu, choose Create Material by Value to generate a global material node with computed elastic properties.
Modeling Instructions (Macromechanics: Global Response)
This section describes how to carry out macromechanics analysis of a laminated composite cylinder using the Layered Shell interface based on the layerwise theory.
Add Component
In the Model Builder window, right-click the root node and choose Add Component > 3D.
Component: Macromechanics (Global Response)
In the Settings window for Component, type Component: Macromechanics (Global Response) in the Label text field.
Geometry 2
Cylinder 1 (cyl1)
1
In the Geometry toolbar, click  Cylinder.
2
In the Settings window for Cylinder, locate the Object Type section.
3
From the Type list, choose Surface.
4
Locate the Size and Shape section. In the Radius text field, type rc.
5
In the Height text field, type hc.
6
Locate the Axis section. From the Axis type list, choose x-axis.
7
Click  Build Selected.
8
Click the  Show Grid button in the Graphics toolbar.
Definitions (comp2)
Boundary System 2 (sys2)
1
In the Model Builder window, expand the Component: Macromechanics (Global Response) (comp2) > Definitions node, then click Boundary System 2 (sys2).
2
In the Settings window for Boundary System, locate the Settings section.
3
Find the Coordinate names subsection. From the Axis list, choose x.
Add Physics
1
In the Home toolbar, click  Add Physics to open the Add Physics window.
2
Go to the Add Physics window.
3
In the tree, select Structural Mechanics > Layered Shell (lshell).
4
Find the Physics interfaces in study subsection. In the table, clear the Solve checkbox for Study: Micromechanics (Material Properties).
5
Click the Add to Component: Macromechanics (Global Response) button in the window toolbar.
6
In the Home toolbar, click  Add Physics to close the Add Physics window.
Global Definitions
The full laminate is a repetition of two layers. Therefore, it is sufficient to define only a part of it in the Layered Material node. The transformation into the full laminate is performed through layered material settings in the Layered Material Link node.
Layered Material: [90/0]_2
1
In the Model Builder window, under Global Definitions right-click Materials and choose Layered Material.
2
In the Settings window for Layered Material, type Layered Material: [90/0]_2 in the Label text field.
3
Locate the Layer Definition section. In the table, enter the following settings:
Layer
Material
Rotation
Value
Thickness
Mesh elements
Layer 1
Homogeneous Material (solidcp1mat)
90
1.5708 rad
th
2
4
Click Add.
5
In the table, enter the following settings:
Layer
Material
Rotation
Value
Thickness
Mesh elements
Layer 2
Homogeneous Material (solidcp1mat)
0
0 rad
th
2
Materials
Layered Material Link 1 (llmat1)
1
In the Model Builder window, under Component: Macromechanics (Global Response) (comp2) right-click Materials and choose Layers > Layered Material Link.
The laminate partially defined in the Layered Material node can be transformed into a full laminate using a transform option in the layered material settings.
2
In the Settings window for Layered Material Link, locate the Layered Material Settings section.
3
From the Transform list, choose Repeated.
4
In the Number of repeats text field, type 2.
5
Click to expand the Preview Plot Settings section. In the Thickness-to-width ratio text field, type 0.4.
6
Locate the Layered Material Settings section. Click Layer Cross-Section Preview in the upper-right corner of the section to enable the through-thickness view of the laminated material.
7
Click Layer Stack Preview in the upper-right corner of the Layered Material Settings section to show the stacking sequence including the fiber orientation.
Layered Shell (lshell)
Linear Elastic Material 1
1
In the Model Builder window, under Component: Macromechanics (Global Response) (comp2) > Layered Shell (lshell) click Linear Elastic Material 1.
2
In the Settings window for Linear Elastic Material, locate the Linear Elastic Material section.
3
From the Material symmetry list, choose Anisotropic.
Add Safety features with composite-specific Hashin and Puck failure criteria.
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.
Safety 2
1
Right-click Safety 1 and choose Duplicate.
2
In the Settings window for Safety, locate the Failure Model section.
3
From the Failure criterion list, choose Puck.
4
Find the Interfiber failure subsection. In the ptl text field, type 0.35.
5
In the pcl text field, type 0.3.
Global Definitions
Homogeneous Material (solidcp1mat)
1
In the Model Builder window, under Global Definitions > Materials click Homogeneous Material (solidcp1mat).
2
In the Settings window for Material, locate the Material Contents section.
3
In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Tensile strengths
{sigmats1, sigmats2, sigmats3}
{Sigmats1, Sigmats2, Sigmats3}
Pa
Orthotropic strength parameters, Voigt notation
Compressive strengths
{sigmacs1, sigmacs2, sigmacs3}
{Sigmacs1, Sigmacs2, Sigmacs3}
Pa
Orthotropic strength parameters, Voigt notation
Shear strengths
{sigmass1, sigmass2, sigmass3}
{Sigmass23, Sigmass13, Sigmass12}
Pa
Orthotropic strength parameters, Voigt notation
Ultimate tensile strain in longitudinal direction
epsilont1
epsilonts1
1
Orthotropic strength parameters, Voigt notation
Ultimate compressive strain in longitudinal direction
epsilonc1
epsiloncs1
1
Orthotropic strength parameters, Voigt notation
Young’s modulus of fiber in longitudinal direction
Ef1
235[GPa]
Pa
Orthotropic strength parameters, Voigt notation
In-plane Poisson’s ratio of fiber
nuf12
0.2
1
Orthotropic strength parameters, Voigt notation
Linear degradation stress
sigma1D
Sigma1D
N/m²
Orthotropic strength parameters, Voigt notation
Layered Shell (lshell)
Fixed Constraint 1
1
In the Physics toolbar, click  Edges and choose Fixed Constraint.
2
Select Edges 9–12 only.
Boundary Load 1
1
In the Physics toolbar, click  Edges and choose Boundary Load.
2
Select Edges 1, 2, 4, and 6 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
0
x
0
y
-7.5E4
z
Mesh 2
Mapped 1
1
In the Mesh toolbar, click  More Generators and choose Mapped.
2
In the Settings window for Mapped, locate the Boundary Selection section.
3
From the Selection list, choose All boundaries.
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 20.
5
Click  Build All.
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
Find the Physics interfaces in study subsection. In the table, clear the Solve checkbox for Solid Mechanics (solid).
5
Click the Add Study button in the window toolbar.
6
In the Home toolbar, click  Add Study to close the Add Study window.
Study: Macromechanics (Global Response)
1
In the Settings window for Study, type Study: Macromechanics (Global Response) in the Label text field.
2
In the Study toolbar, click  Compute.
Results
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 5.
Stress (lshell)
1
In the Model Builder window, under Results click Stress (lshell).
2
In the Settings window for 3D Plot Group, locate the Title section.
3
From the Title type list, choose Manual.
4
Locate the Color Legend section. Select the Show maximum and minimum values checkbox.
Surface 1
1
In the Model Builder window, expand the Stress (lshell) node, then click Surface 1.
2
In the Stress (lshell) 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: Macromechanics (Global Response)/Solution 1 (3) (sol1) > Layered Shell > Stress, Slice (lshell).
4
Click the Add Result Template button in the window toolbar.
5
In the Results toolbar, click  Result Templates to close the Result Templates window.
Results
Stress, Slice (lshell)
1
In the Model Builder window, expand the Results > Stress, Slice (lshell) node, then click Stress, Slice (lshell).
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, click Layered Material Slice 1.
2
In the Settings window for Layered Material Slice, click to expand the Title section.
3
From the Title type list, choose Manual.
4
Locate the Through-Thickness Location section. From the Location definition list, choose Interfaces.
5
Locate the Layout section. From the Displacement list, choose Rectangular.
6
From the Orientation list, choose zx.
7
In the Relative x-separation text field, type 0.3.
8
In the Relative z-separation text field, type 0.7.
9
Select the Show descriptions checkbox.
10
In the Relative separation text field, type 0.6.
11
Click to expand the Quality section. From the Resolution list, choose No refinement.
Deformation
1
In the Model Builder window, expand the Layered Material Slice 1 node.
2
Right-click Deformation and choose Disable.
Stress, Slice (lshell)
1
In the Model Builder window, under Results click Stress, Slice (lshell).
2
In the Stress, Slice (lshell) toolbar, click  Plot.
From the Stress, Slice it is clear that the maximum stress in fiber direction occurs either at the inner or outer layer of the composite cylinder. To get the position where the maximum stress in fiber direction occurs in the laminate, add a Surface Maximum derived-values node. These coordinates are useful for the next micromechanical analysis.
Surface Maximum 1
1
In the Model Builder window, under Results right-click Derived Values and choose Maximum > Surface Maximum.
2
In the Settings window for Surface Maximum, locate the Data section.
3
From the Dataset list, choose Study: Macromechanics (Global Response)/Solution 1 (3) (sol1).
4
Locate the Selection section. From the Selection list, choose All boundaries.
5
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
lshell.atxd1(0,lshell.sllGp11)
N/m^2
Stress in the inner layer
lshell.atxd1(lshell.d,lshell.sllGp11)
N/m^2
Stress in the outer layer
6
Click to expand the Configuration section. Select the Include position checkbox.
7
Click  Evaluate.
Use the following instructions to plot the through-thickness variation of the stress in fiber direction at a point where the stress is maximal.
Cut Point 3D 1
1
In the Results toolbar, click  Cut Point 3D.
2
In the Settings window for Cut Point 3D, locate the Data section.
3
From the Dataset list, choose Study: Macromechanics (Global Response)/Solution 1 (3) (sol1).
4
Locate the Point Data section. In the X text field, type 0.
5
In the Y text field, type 0.
6
In the Z text field, type -rc.
7
From the Snapping list, choose Snap to closest boundary.
Cut Point 3D 2
1
Right-click Cut Point 3D 1 and choose Duplicate.
2
In the Settings window for Cut Point 3D, locate the Point Data section.
3
In the X text field, type hc.
4
In the Y text field, type 0.
5
In the Z text field, type rc.
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: Macromechanics (Global Response)/Solution 1 (3) (sol1) > Layered Shell > Stress, Through Thickness (lshell).
4
Click the Add Result Template button in the window toolbar.
5
In the Results toolbar, click  Result Templates to close the Result Templates window.
Results
Stress, Through Thickness (lshell)
1
In the Settings window for 1D Plot Group, locate the Plot Settings section.
2
In the x-axis label text field, type Stress tensor, layer coordinate system (MPa).
Through Thickness 1
1
In the Model Builder window, expand the Stress, Through Thickness (lshell) 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 1.
4
Locate the x-Axis Data section. In the Expression text field, type lshell.sllGp11.
5
Click to expand the Legends section. From the Legends list, choose Manual.
6
In the table, enter the following settings:
Legends
Cut Point 1
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 2.
4
Locate the x-Axis Data section. In the Expression text field, type lshell.sllGp11.
5
Click to expand the Legends section. From the Legends list, choose Manual.
6
In the table, enter the following settings:
Legends
Cut Point 2
7
In the Stress, Through Thickness (lshell) 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: Macromechanics (Global Response)/Solution 1 (3) (sol1) > Layered Shell > Failure Indices (lshell) > Failure Index (Safety 1).
4
Click the Add Result Template button in the window toolbar.
Results
Hashin Failure Index
1
In the Settings window for 3D Plot Group, type Hashin Failure Index in the Label text field.
2
Locate the Title section. From the Title type list, choose Manual.
3
In the Title text area, type Hashin Failure Index.
4
Locate the Color Legend section. Select the Show maximum and minimum values checkbox.
5
Locate the Data section. Click  Go to Source.
Layered Material 2 (Safety)
1
In the Model Builder window, under Results > Datasets click Layered Material 2 (Safety).
2
In the Settings window for Layered Material, locate the Layers section.
3
In the Scale text field, type 12.
Marker 1
1
In the Model Builder window, expand the Results > Hashin Failure Index node.
2
Right-click Surface 1 and choose Marker.
3
In the Settings window for Marker, locate the Display section.
4
From the Display list, choose Max.
5
Locate the Text Format section. In the Precision text field, type 3.
6
Locate the Coloring and Style section. In the Point radius text field, type 4.
7
From the Background color list, choose Gray.
8
From the Anchor point list, choose Lower right.
9
In the Hashin Failure Index toolbar, click  Plot.
Result Templates
1
Go to the Result Templates window.
2
In the tree, select Study: Macromechanics (Global Response)/Solution 1 (3) (sol1) > Layered Shell > Failure Indices (lshell) > Failure Index (Safety 2).
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
Puck Failure Index
1
In the Settings window for 3D Plot Group, type Puck Failure Index in the Label text field.
2
Locate the Title section. From the Title type list, choose Manual.
3
In the Title text area, type Puck Failure Index.
4
Locate the Color Legend section. Select the Show maximum and minimum values checkbox.
Marker 1
1
In the Model Builder window, expand the Puck Failure Index node.
2
Right-click Surface 1 and choose Marker.
3
In the Settings window for Marker, locate the Display section.
4
From the Display list, choose Max.
5
Locate the Text Format section. In the Precision text field, type 3.
6
Locate the Coloring and Style section. In the Point radius text field, type 4.
7
From the Background color list, choose Gray.
8
From the Anchor point list, choose Lower right.
9
In the Puck Failure Index toolbar, click  Plot.
Hashin Failure Indexes (Study: Macromechanics (Global Response))
1
In the Results toolbar, click  Evaluation Group.
2
In the Settings window for Evaluation Group, type Hashin Failure Indexes (Study: Macromechanics (Global Response)) in the Label text field.
3
Locate the Data section. From the Dataset list, choose Layered Material 2 (Safety).
Volume Maximum 1
1
Right-click Hashin Failure Indexes (Study: Macromechanics (Global Response)) and choose Maximum > Volume Maximum.
2
In the Settings window for Volume Maximum, click Add Expression in the upper-right corner of the Expressions section. From the menu, choose Component: Macromechanics (Global Response) (comp2) > Layered Shell > Safety > Hashin > lshell.lemm1.sf1.f_ifT - Hashin fiber tensile failure index - 1.
3
Click Add Expression in the upper-right corner of the Expressions section. From the menu, choose Component: Macromechanics (Global Response) (comp2) > Layered Shell > Safety > Hashin > lshell.lemm1.sf1.f_ifC - Hashin fiber compressive failure index - 1.
4
Click Add Expression in the upper-right corner of the Expressions section. From the menu, choose Component: Macromechanics (Global Response) (comp2) > Layered Shell > Safety > Hashin > lshell.lemm1.sf1.f_imT - Hashin matrix tensile failure index - 1.
5
Click Add Expression in the upper-right corner of the Expressions section. From the menu, choose Component: Macromechanics (Global Response) (comp2) > Layered Shell > Safety > Hashin > lshell.lemm1.sf1.f_imC - Hashin matrix compressive failure index - 1.
6
Click Add Expression in the upper-right corner of the Expressions section. From the menu, choose Component: Macromechanics (Global Response) (comp2) > Layered Shell > Safety > Hashin > lshell.lemm1.sf1.f_iiT - Hashin interlaminar tensile failure index - 1.
7
Click Add Expression in the upper-right corner of the Expressions section. From the menu, choose Component: Macromechanics (Global Response) (comp2) > Layered Shell > Safety > Hashin > lshell.lemm1.sf1.f_iiC - Hashin interlaminar compressive failure index - 1.
Hashin Failure Indexes (Study: Macromechanics (Global Response))
1
In the Model Builder window, click Hashin Failure Indexes (Study: Macromechanics (Global Response)).
2
In the Settings window for Evaluation Group, locate the Transformation section.
3
Select the Transpose checkbox.
4
In the Hashin Failure Indexes (Study: Macromechanics (Global Response)) toolbar, click  Evaluate.
Puck Failure Indexes (Study: Macromechanics (Global Response))
1
In the Results toolbar, click  Evaluation Group.
2
In the Settings window for Evaluation Group, type Puck Failure Indexes (Study: Macromechanics (Global Response)) in the Label text field.
3
Locate the Data section. From the Dataset list, choose Layered Material 2 (Safety).
Volume Maximum 1
1
Right-click Puck Failure Indexes (Study: Macromechanics (Global Response)) and choose Maximum > Volume Maximum.
2
In the Settings window for Volume Maximum, click Add Expression in the upper-right corner of the Expressions section. From the menu, choose Component: Macromechanics (Global Response) (comp2) > Layered Shell > Safety > Puck > lshell.lemm1.sf2.f_ifT - Puck fiber tensile failure index - 1.
3
Click Add Expression in the upper-right corner of the Expressions section. From the menu, choose Component: Macromechanics (Global Response) (comp2) > Layered Shell > Safety > Puck > lshell.lemm1.sf2.f_ifC - Puck fiber compressive failure index - 1.
4
Click Add Expression in the upper-right corner of the Expressions section. From the menu, choose Component: Macromechanics (Global Response) (comp2) > Layered Shell > Safety > Puck > lshell.lemm1.sf2.f_imA - Puck interfiber mode A failure index - 1.
5
Click Add Expression in the upper-right corner of the Expressions section. From the menu, choose Component: Macromechanics (Global Response) (comp2) > Layered Shell > Safety > Puck > lshell.lemm1.sf2.f_imB - Puck interfiber mode B failure index - 1.
6
Click Add Expression in the upper-right corner of the Expressions section. From the menu, choose Component: Macromechanics (Global Response) (comp2) > Layered Shell > Safety > Puck > lshell.lemm1.sf2.f_imC - Puck interfiber mode C failure index - 1.
Puck Failure Indexes (Study: Macromechanics (Global Response))
1
In the Model Builder window, click Puck Failure Indexes (Study: Macromechanics (Global Response)).
2
In the Settings window for Evaluation Group, locate the Transformation section.
3
Select the Transpose checkbox.
4
In the Puck Failure Indexes (Study: Macromechanics (Global Response)) toolbar, click  Evaluate.
Hashin Failure Index, Puck Failure Index, Stress (lshell), Stress, Slice (lshell), Stress, Through Thickness (lshell)
1
In the Model Builder window, under Results, Ctrl-click to select Stress (lshell), Stress, Slice (lshell), Stress, Through Thickness (lshell), Hashin Failure Index, and Puck Failure Index.
2
Right-click and choose Group.
Macromechanics (Global Response)
In the Settings window for Group, type Macromechanics (Global Response) in the Label text field.
Modeling Instructions (Micromechanics: Local Response)
This section describes how to carry out micromechanical failure analysis of a unit cell using the macro level strain field from the global analysis of the Layered Shell interface.
In order to do a micromechanical analysis at multiple material points, create a list of such point coordinates using a Parameter node. The points where the maximum stress occurs in inner and outer layers are included in this list.
Global Definitions
Material Point Location
1
In the Home toolbar, click  Parameters and choose Add > Parameters.
2
In the Settings window for Parameters, type Material Point Location in the Label text field.
3
Locate the Parameters section. In the table, enter the following settings:
Name
Expression
Value
Description
X0
0[m]
0 m
Material point, X coordinate
Y0
0[m]
0 m
Material point, Y coordinate
Z0
-rc
-0.1 m
Material point, Z coordinate
4
In the Home toolbar, click  Parameter Case.
5
Right-click Global Definitions > Material Point Location > Case 1 and choose Duplicate.
6
In the Settings window for Case, locate the Parameters section.
7
In the table, enter the following settings:
Name
Expression
Description
X0
hc/2
Material point, X coordinate
Y0
0[m]
Material point, Y coordinate
Z0
-rc
Material point, Z coordinate
8
Right-click Global Definitions > Material Point Location > Case 2 and choose Duplicate.
9
In the Settings window for Case, locate the Parameters section.
10
In the table, enter the following settings:
Name
Expression
Description
X0
hc
Material point, X coordinate
Y0
0[m]
Material point, Y coordinate
Z0
-rc
Material point, Z coordinate
11
Right-click Global Definitions > Material Point Location > Case 3 and choose Duplicate.
12
In the Settings window for Case, locate the Parameters section.
13
In the table, enter the following settings:
Name
Expression
Description
X0
0[m]
Material point, X coordinate
Y0
0[m]
Material point, Y coordinate
Z0
rc
Material point, Z coordinate
14
Right-click Global Definitions > Material Point Location > Case 4 and choose Duplicate.
15
In the Settings window for Case, locate the Parameters section.
16
In the table, enter the following settings:
Name
Expression
Description
X0
hc/2
Material point, X coordinate
Y0
0[m]
Material point, Y coordinate
Z0
rc
Material point, Z coordinate
17
Right-click Global Definitions > Material Point Location > Case 5 and choose Duplicate.
18
In the Settings window for Case, locate the Parameters section.
19
In the table, enter the following settings:
Name
Expression
Description
X0
hc
Material point, X coordinate
Y0
0[m]
Material point, Y coordinate
Z0
rc
Material point, Z coordinate
Component: Micromechanics (Material Properties) (comp1)
The model setup can be simplified by copying the Component: Micromechanics (Material Properties) component.
In the Model Builder window, right-click Component: Micromechanics (Material Properties) (comp1) and choose Copy.
Component: Micromechanics (Material Properties) 1 (comp3)
In the Model Builder window, right-click the root node and choose Paste Multiple Items.
Component: Micromechanics (Local Response)
1
In the Messages from Paste dialog, click OK.
2
In the Model Builder window, click Component: Micromechanics (Material Properties) 1 (comp3).
3
In the Settings window for Component, type Component: Micromechanics (Local Response) in the Label text field.
The unit cell is analyzed at different through-thickness locations of the composite cylinder where the layers have different rotation angles with respect to the laminate coordinate system. Hence, rotate the unit cell geometry with a conditional rotation angle expression.
Geometry 1
Rotate 1 (rot1)
1
In the Geometry toolbar, click  Transforms and choose Rotate.
2
Select the object pi1 only.
3
In the Settings window for Rotate, locate the Rotation section.
4
In the Angle text field, type if(xd==0,90[deg],0).
5
Click  Build Selected.
In order to input the fiber material properties in the correct coordinate system, use a Rotated System.
Definitions (comp3)
Rotated System 4 (sys4)
1
In the Definitions toolbar, click  Coordinate Systems and choose Rotated System.
2
In the Settings window for Rotated System, locate the Rotation section.
3
Find the Euler angles subsection. In the α text field, type if(xd==0,90[deg],0).
Boundary System 1 (sys3)
1
In the Model Builder window, click Boundary System 1 (sys3).
2
In the Settings window for Boundary System, locate the Settings section.
3
Find the Coordinate names subsection. From the Create first tangent direction from list, choose Rotated System 4 (sys4).
4
From the Axis list, choose x1.
The failure criteria used for fiber, matrix, and interface materials are user defined, so use a Variable node to define them.
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 composite_multiscale_variables.txt.
Solid Mechanics (solid2)
Linear Elastic Material 1
1
In the Model Builder window, expand the Component: Micromechanics (Local Response) (comp3) > Solid Mechanics (solid2) node, then click Linear Elastic Material 1.
2
In the Settings window for Linear Elastic Material, locate the Coordinate System Selection section.
3
From the Coordinate system list, choose Rotated System 4 (sys4).
Add Safety features to the matrix, fiber, and interface domains. Use user-defined criteria.
Fiber Failure Criterion
1
In the Physics toolbar, click  Attributes and choose Safety.
2
In the Settings window for Safety, type Fiber Failure Criterion in the Label text field.
3
Select Domain 2 only.
4
Locate the Failure Model section. From the Failure criterion list, choose User defined.
5
In the g  (σ) text field, type g_f.
6
In the sf  (σ) text field, type sf_f.
Linear Elastic Material 1
In the Model Builder window, click Linear Elastic Material 1.
Matrix Failure Criterion
1
In the Physics toolbar, click  Attributes and choose Safety.
2
In the Settings window for Safety, type Matrix Failure Criterion in the Label text field.
3
Select Domain 1 only.
4
Locate the Failure Model section. From the Failure criterion list, choose User defined.
5
In the g  (σ) text field, type g_m.
6
In the sf  (σ) text field, type sf_m.
Thin Layer 1
In the Model Builder window, expand the Component: Micromechanics (Local Response) (comp3) > Solid Mechanics (solid2) > Thin Layer 1 node.
Linear Elastic Material 1
In the Model Builder window, expand the Component: Micromechanics (Local Response) (comp3) > Solid Mechanics (solid2) > Thin Layer 1 > Linear Elastic Material 1 node, then click Linear Elastic Material 1.
Interface Failure Criterion
1
In the Physics toolbar, click  Attributes and choose Safety.
2
In the Settings window for Safety, type Interface Failure Criterion in the Label text field.
3
Locate the Failure Model section. From the Failure criterion list, choose User defined.
4
In the g  (σ) text field, type g_i.
5
In the sf  (σ) text field, type sf_i.
Cell Periodicity 1
1
In the Model Builder window, under Component: Micromechanics (Local Response) (comp3) > Solid Mechanics (solid2) click Cell Periodicity 1.
2
In the Settings window for Cell Periodicity, locate the Periodicity Settings section.
3
From the Boundary conditions list, choose Mixed.
4
Find the XX component subsection. In the εavgXX text field, type eXX.
5
Find the YY component subsection. In the εavgYY text field, type eYY.
6
Find the ZZ component subsection. In the εavgZZ text field, type eZZ.
7
Find the XY component subsection. In the εavgXY text field, type eXY.
8
Find the YZ component subsection. In the εavgYZ text field, type eYZ.
9
Find the XZ component subsection. In the εavgXZ text field, type eXZ.
Mesh 1
Swept 1
1
In the Model Builder window, expand the Component: Micromechanics (Local Response) (comp3) > Mesh 1 node.
2
Right-click Component: Micromechanics (Local Response) (comp3) > Mesh 1 > Swept 1 and choose Build Selected.
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
Find the Physics interfaces in study subsection. In the table, clear the Solve checkboxes for Solid Mechanics (solid) and Layered Shell (lshell).
5
Click the Add Study button in the window toolbar.
6
In the Home toolbar, click  Add Study to close the Add Study window.
Study: Micromechanics (Local Response)
1
In the Settings window for Study, type Study: Micromechanics (Local Response) in the Label text field.
2
Locate the Study Settings section. Clear the Generate default plots checkbox.
Parametric Sweep
1
In the Study toolbar, click  Parametric Sweep.
Add two Parametric Sweep nodes, one for different in-plane locations and another for different through-thickness locations.
2
In the Settings window for Parametric Sweep, locate the Study Settings section.
3
From the Sweep type list, choose Parameter switch.
4
Click  Add.
5
In the table, enter the following settings:
Switch
Cases
Case numbers
Material Point Location
All
range(1,1,6)
Parametric Sweep 2
1
In the Study toolbar, click  Parametric Sweep.
2
In the Settings window for Parametric Sweep, locate the Study Settings section.
3
Click  Add.
4
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
xd (Extra dimension location)
0 4*th
mm
Step 1: Stationary
1
In the Model Builder window, click Step 1: Stationary.
2
In the Settings window for Stationary, click to expand the Values of Dependent Variables section.
3
Find the Values of variables not solved for subsection. From the Settings list, choose User controlled.
4
From the Method list, choose Solution.
5
From the Study list, choose Study: Macromechanics (Global Response), Stationary.
6
In the Study toolbar, click  Compute.
Results
Micromechanics (Local Response)
1
In the Model Builder window, right-click Micromechanics (Material Properties) and choose Duplicate.
2
In the Settings window for Group, type Micromechanics (Local Response) in the Label text field.
Stress, Unit Cell (At First Material Point in Inner Layer)
1
In the Model Builder window, expand the Micromechanics (Local Response) node, then click Stress, Unit Cell 1.
2
In the Settings window for 3D Plot Group, type Stress, Unit Cell (At First Material Point in Inner Layer) in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study: Micromechanics (Local Response)/Parametric Solutions 1 (9) (sol3).
4
From the Parameter value (xd (mm)) list, choose 0.
5
From the Material Point Location list, choose Case 1.
6
Locate the Title section. Clear the Parameter indicator text field.
Volume 1
1
In the Model Builder window, expand the Stress, Unit Cell (At First Material Point in Inner Layer) node, then click Volume 1.
2
In the Settings window for Volume, locate the Expression section.
3
In the Expression text field, type solid2.mises.
Selection 1
1
In the Model Builder window, expand the Volume 1 node, then click Selection 1.
2
In the Settings window for Selection, locate the Selection section.
3
Click to select the  Activate Selection toggle button.
4
Select Domain 1 only.
Volume 2
1
In the Model Builder window, under Results > Micromechanics (Local Response) > Stress, Unit Cell (At First Material Point in Inner Layer) click Volume 2.
2
In the Settings window for Volume, locate the Expression section.
3
In the Expression text field, type solid2.mises.
Selection 1
1
In the Model Builder window, expand the Volume 2 node, then click Selection 1.
2
In the Settings window for Selection, locate the Selection section.
3
Click to select the  Activate Selection toggle button.
4
Select Domain 2 only.
Surface 1
1
In the Model Builder window, under Results > Micromechanics (Local Response) > Stress, Unit Cell (At First Material Point in Inner Layer) click Surface 1.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type solid2.mises.
Selection 1
1
In the Model Builder window, click Selection 1.
2
In the Settings window for Selection, locate the Selection section.
3
Click to select the  Activate Selection toggle button.
4
Select Boundaries 6–9 only.
5
Click the  Zoom Extents button in the Graphics toolbar.
6
In the Stress, Unit Cell (At First Material Point in Inner Layer) toolbar, click  Plot.
Stress, Unit Cell (At Multiple Material Points)
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Stress, Unit Cell (At Multiple Material Points) in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study: Micromechanics (Local Response)/Parametric Solutions 1 (9) (sol3).
4
Locate the Title section. From the Title type list, choose Manual.
5
In the Title text area, type von Mises stress (MPa).
6
Clear the Parameter indicator text field.
7
Locate the Plot Settings section. Clear the Plot dataset edges checkbox.
Surface 1
1
Right-click Stress, Unit Cell (At Multiple Material Points) and choose Surface.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Study: Micromechanics (Local Response)/Parametric Solutions 1 (9) (sol3).
4
From the Parameter value (xd (mm)) list, choose 0.
5
From the Material Point Location list, choose Case 1.
6
Locate the Expression section. In the Expression text field, type solid2.mises.
7
Click to expand the Range section. Select the Manual color range checkbox.
8
In the Maximum text field, type 100.
9
Locate the Coloring and Style section. From the Color table list, choose Prism.
10
Click to expand the Quality section. From the Evaluation settings list, choose Manual.
11
From the Resolution list, choose Custom.
12
In the Element refinement text field, type 2.
13
From the Smoothing threshold list, choose Manual.
14
In the Threshold text field, type 0.2.
Transformation 1
1
Right-click Surface 1 and choose Transformation.
2
In the Settings window for Transformation, locate the Transformation section.
3
In the X text field, type X0.
4
In the Y text field, type Y0.
5
In the Z text field, type Z0+18*th.
Surface 2
1
In the Model Builder window, under Results > Micromechanics (Local Response) > Stress, Unit Cell (At Multiple Material Points) right-click Surface 1 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Material Point Location list, choose Case 2.
4
Locate the Inherit Style section. From the Plot list, choose Surface 1.
Surface 3
1
Right-click Surface 2 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Material Point Location list, choose Case 3.
Surface 4
1
Right-click Surface 3 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Material Point Location list, choose Case 4.
Transformation 1
1
In the Model Builder window, expand the Surface 4 node, then click Transformation 1.
2
In the Settings window for Transformation, locate the Transformation section.
3
In the Z text field, type Z0-18*th.
Surface 5
1
In the Model Builder window, under Results > Micromechanics (Local Response) > Stress, Unit Cell (At Multiple Material Points) right-click Surface 4 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Material Point Location list, choose Case 5.
Surface 6
1
Right-click Surface 5 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Material Point Location list, choose Case 6.
Surface 7
1
Right-click Surface 6 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Parameter value (xd (mm)) list, choose 4.
4
From the Material Point Location list, choose Case 1.
Surface 8
1
Right-click Surface 7 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Material Point Location list, choose Case 2.
Surface 9
1
Right-click Surface 8 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Material Point Location list, choose Case 3.
Surface 10
1
Right-click Surface 9 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Material Point Location list, choose Case 4.
Transformation 1
1
In the Model Builder window, expand the Surface 10 node, then click Transformation 1.
2
In the Settings window for Transformation, locate the Transformation section.
3
In the Z text field, type Z0+18*th.
Surface 11
1
In the Model Builder window, under Results > Micromechanics (Local Response) > Stress, Unit Cell (At Multiple Material Points) right-click Surface 10 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Material Point Location list, choose Case 5.
Surface 12
1
Right-click Surface 11 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Material Point Location list, choose Case 6.
Line 1
1
In the Model Builder window, right-click Stress, Unit Cell (At Multiple Material Points) and choose Line.
2
In the Settings window for Line, locate the Expression section.
3
In the Expression text field, type 0.
4
Locate the Data section. From the Dataset list, choose Layered Material 2 (Safety).
5
Locate the Coloring and Style section. From the Coloring list, choose Uniform.
6
From the Color list, choose Black.
Stress, Unit Cell (At Multiple Material Points)
1
Click the  Zoom Extents button in the Graphics toolbar.
2
In the Model Builder window, click Stress, Unit Cell (At Multiple Material Points).
3
In the Settings window for 3D Plot Group, locate the Plot Settings section.
4
From the View list, choose New view.
5
In the Stress, Unit Cell (At Multiple Material Points) toolbar, click  Plot.
User Defined Failure Indexes (At First Material Point in Inner Layer)
1
In the Model Builder window, right-click Stress, Unit Cell (At First Material Point in Inner Layer) and choose Duplicate.
2
In the Settings window for 3D Plot Group, type User Defined Failure Indexes (At First Material Point in Inner Layer) in the Label text field.
3
Locate the Title section. In the Title text area, type User Defined failure index (1).
4
Locate the Color Legend section. Select the Show maximum and minimum values checkbox.
Volume 1
1
In the Model Builder window, expand the User Defined Failure Indexes (At First Material Point in Inner Layer) node, then click Volume 1.
2
In the Settings window for Volume, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component: Micromechanics (Local Response) (comp3) > Solid Mechanics > Safety > User defined > solid2.lemm1.sf2.f_i - User-defined failure index - 1.
Volume 2
1
In the Model Builder window, click Volume 2.
2
In the Settings window for Volume, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component: Micromechanics (Local Response) (comp3) > Solid Mechanics > Safety > User defined > solid2.lemm1.sf1.f_i - User-defined failure index - 1.
Surface 1
1
In the Model Builder window, click Surface 1.
2
In the Settings window for Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component: Micromechanics (Local Response) (comp3) > Solid Mechanics > Safety > User defined > solid2.tl1.lemm1.sf1.f_i - User-defined failure index - 1.
User Defined Failure Indexes (At First Material Point in Inner Layer)
1
Click the  Zoom Extents button in the Graphics toolbar.
2
In the Model Builder window, click User Defined Failure Indexes (At First Material Point in Inner Layer).
3
In the User Defined Failure Indexes (At First Material Point in Inner Layer) toolbar, click  Plot.
User Defined Failure Indexes (At First Material Point in Outer Layer)
1
Right-click User Defined Failure Indexes (At First Material Point in Inner Layer) and choose Duplicate.
2
In the Settings window for 3D Plot Group, type User Defined Failure Indexes (At First Material Point in Outer Layer) in the Label text field.
3
Locate the Data section. From the Parameter value (xd (mm)) list, choose 4.
4
Click the  Zoom Extents button in the Graphics toolbar.
5
In the User Defined Failure Indexes (At First Material Point in Outer Layer) toolbar, click  Plot.
User Defined Failure Indexes at First Material Point in Inner Layer (Study: Micromechanics (Local Response))
1
In the Results toolbar, click  Evaluation Group.
2
In the Settings window for Evaluation Group, type User Defined Failure Indexes at First Material Point in Inner Layer (Study: Micromechanics (Local Response)) in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study: Micromechanics (Local Response)/Parametric Solutions 1 (9) (sol3).
4
From the Parameter selection (xd) list, choose First.
5
From the Material Point Location list, choose First.
Volume Maximum 1
1
Right-click User Defined Failure Indexes at First Material Point in Inner Layer (Study: Micromechanics (Local Response)) and choose Maximum > Volume Maximum.
2
Select Domain 1 only.
3
In the Settings window for Volume Maximum, click Replace Expression in the upper-right corner of the Expressions section. From the menu, choose Component: Micromechanics (Local Response) (comp3) > Solid Mechanics > Safety > User defined > solid2.lemm1.sf2.f_i - User-defined failure index - 1.
4
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
solid2.lemm1.sf2.f_i
1
User-defined matrix failure index
Volume Maximum 2
1
In the Model Builder window, right-click User Defined Failure Indexes at First Material Point in Inner Layer (Study: Micromechanics (Local Response)) and choose Maximum > Volume Maximum.
2
Select Domain 2 only.
3
In the Settings window for Volume Maximum, click Replace Expression in the upper-right corner of the Expressions section. From the menu, choose Component: Micromechanics (Local Response) (comp3) > Solid Mechanics > Safety > User defined > solid2.lemm1.sf1.f_i - User-defined failure index - 1.
4
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
solid2.lemm1.sf1.f_i
1
User-defined fiber failure index
Surface Maximum 3
1
Right-click User Defined Failure Indexes at First Material Point in Inner Layer (Study: Micromechanics (Local Response)) and choose Maximum > Surface Maximum.
2
In the Settings window for Surface Maximum, locate the Selection section.
3
From the Selection list, choose Interface Selection.
4
Click Replace Expression in the upper-right corner of the Expressions section. From the menu, choose Component: Micromechanics (Local Response) (comp3) > Solid Mechanics > Safety > User defined > solid2.tl1.lemm1.sf1.f_i - User-defined failure index - 1.
5
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
solid2.tl1.lemm1.sf1.f_i
1
User-defined interface failure index
User Defined Failure Indexes at First Material Point in Inner Layer (Study: Micromechanics (Local Response))
1
In the Model Builder window, click User Defined Failure Indexes at First Material Point in Inner Layer (Study: Micromechanics (Local Response)).
2
In the Settings window for Evaluation Group, locate the Transformation section.
3
Select the Transpose checkbox.
4
Click to expand the Format section. From the Include parameters list, choose Off.
5
In the User Defined Failure Indexes at First Material Point in Inner Layer (Study: Micromechanics (Local Response)) toolbar, click  Evaluate.
User Defined Failure Indexes at First Material Point in Outer Layer (Study: Micromechanics (Local Response))
1
Right-click User Defined Failure Indexes at First Material Point in Inner Layer (Study: Micromechanics (Local Response)) and choose Duplicate.
2
In the Settings window for Evaluation Group, type User Defined Failure Indexes at First Material Point in Outer Layer (Study: Micromechanics (Local Response)) in the Label text field.
3
Locate the Data section. From the Parameter selection (xd) list, choose Last.
4
In the User Defined Failure Indexes at First Material Point in Outer Layer (Study: Micromechanics (Local Response)) toolbar, click  Evaluate.