PDF
Micromechanical Model of a Particulate Composite
Introduction
In this example, a simplified micromechanical model of a particulate composite is analyzed. A representative volume element (RVE) based on a predetermined particle spacing is assumed to represent the microstructure of the composite. The homogenized elastic and viscoelastic properties of the composite material are computed based on the individual properties of the particles and the matrix. Transient analyses of shear and normal loading of the composite microstructure yield the viscoelastic response of the composite, which is used to determine the homogenized viscoelastic parameters using curve fitting optimization.
The following considerations are important for the analysis:
•
In the particulate composite, only the matrix material is assumed to show viscoelastic behavior. This is a realistic assumption for, for example, polymer matrix composites. Polymer-like resin shows viscoelastic behavior, whereas the embedded fibers or particles are assumed to be elastic.
•
The viscoelastic properties of the matrix in the heterogeneous material and in the equivalent homogenized material are assumed to be represented by a generalized Maxwell model, having a Prony series representation.
•
The viscoelastic model of the matrix in the heterogeneous material as well as the model of the equivalent homogeneous material are isotropic.
•
The viscoelastic model of the matrix material is deviatoric. In contrast, the viscoelastic model of the homogenized material can be volumetric as well as deviatoric due to the inclusion of the particles. When determining the homogenized viscoelastic parameters through an optimization routine, it is assumed that the relaxation times of the homogenized material are the same as those of the matrix material.
•
To determine the homogenized, isotropic, viscoelastic parameters from the particulate composite, two different stress responses from a unit cell RVE are required:
-
The shear stress response, which only activates the deviatoric part of the homogeneous, isotropic, viscoelastic model.
-
The normal stress response, which activates both the deviatoric and the volumetric part of the homogeneous, isotropic, viscoelastic model.
•
During step loading in the time-dependent study, both the instantaneous and the long-term response of the heterogeneous RVE are purely elastic. They are therefore excluded when determining the homogeneous, viscoelastic parameters through the optimization routine.
•
In the current example, uniform spacing of particles is assumed in all three directions. However, it is also possible to perform micromechanical analyses for nonuniformly distributed particles.
Model Definition
The composite is assumed to be made of a periodic microstructure identified as a primitive cubic structure. A unit cube RVE having a spherical particle embedded in the center of the matrix is shown in Figure 1.
Figure 1: Geometry of the unit cell, consisting of a spherical particle embedded in epoxy resin.
Particle and Matrix Properties
The elastic material properties of particles and matrix are given in Table 1 and Table 2, respectively.
Table 1: particle material properties.
Material Property
Value
 Ep
230 GPa
 υp
0.2
Table 2: Matrix material properties.
Material Property
Value
 Em
10 GPa
 υm
0.35
The relaxation function Γ(t) in the viscoelastic model for the matrix is expressed in terms of the instantaneous shear modulus G0 and a set of N relative weights gk and relaxation times τk, so that the Prony series is given as
where gk and τk are the relative weight and the relaxation time constant of the spring-dashpot pair in branch k, respectively. In this case, the long-term shear modulus G is related to the instantaneous shear modulus G0 by the weight g∞ < 1
and the shear modulus in each branch k is defined by the weight gk
It must be assumed that the weights fulfill the constraint
The relative weights and relaxation time constants for the three branches are given in Table 3.
Table 3: Viscoelastic properties of the matrix.
Branch
Relative Weight
Relaxation Time Constant
1
0.01
0.01 s
2
0.05
0.1 s
3
0.08
1 s
Results and Discussion
The von Mises stress in the constituents when viscoelasticity is neglected is shown in Figure 2 and Figure 3 for normal and shear loading, respectively. The corresponding results when viscoelasticity in the matrix is included are reported in Figure 4 and Figure 5 for normal and shear loading, respectively. Here, the results are shown at the end of the simulation when the viscous branches are fully relaxed. Note that the stresses in the constituents are in good agreement with those computed in the elastic study, as expected.
The variation in average normal and shear stress with time for the heterogeneous RVE is shown in Figure 6. The initial response is elastic, which is followed by stress relaxation in the viscous branches.
The variations in average shear and normal stresses with time for the heterogeneous RVE and the homogenized, equivalent material are shown in Figure 7 and Figure 8, respectively. The relative weights for the deviatoric and volumetric parts obtained from the optimization routine are given in Table 4 and Table 5, respectively. It can be seen that the deviatoric relative weights for the homogenized material are close to those of the matrix due to the low particle volume fraction, which means that the viscoelastic response of the composite is dominated by the matrix viscoelasticity. Note, however, that the heterogeneity does result in nonzero volumetric relative weights.
Table 4: Homogenized viscoelastic deviatoric properties.
Branch
Relative Weight
Relaxation Time Constant
1
0.00942
0.01 s
2
0.04918
0.1 s
3
0.07934
1 s
Table 5: Homogenized viscoelastic volumetric properties.
Branch
Relative Weight
Relaxation Time Constant
1
6.516E-4
0.01 s
2
0.00436
0.1 s
3
0.00681
1 s
Figure 2: von Mises stress in matrix and particle due to axial loading (elastic conditions).
Figure 3: von Mises stress in matrix and particle due to shear loading (elastic conditions).
Figure 4: von Mises stress in particle and matrix under axial loading (viscoelasticity in matrix).
Figure 5: von Mises stress in particle and matrix under shear loading (viscoelasticity in matrix).
Figure 6: Average viscoelastic normal and shear stress in the heterogeneous RVE.
Figure 7: Average viscoelastic shear stress for the composite and the homogenized material.
.
Figure 8: Average viscoelastic normal stress for the heterogeneous RVE and the equivalent homogenized material.
Notes About the COMSOL Implementation
•
The micromechanical analysis of particles in a bulk matrix can be performed using the Cell Periodicity node available in the Solid Mechanics interface. Using this functionality, the elasticity matrix of the homogenized material can be computed for given particle and matrix properties.
•
The Cell Periodicity node has three action buttons in the toolbar of the section called Periodicity Type: Create Load Groups and Study, Create Material by Value, and Create Material by Reference. The action button Create Load Groups and Study generates load groups and a stationary study with load cases. The action button Create Material by Value generates a Global Material with homogenized material properties, with material properties as numbers. The action button Create Material by Reference generates a Global Material with homogenized material properties, with material properties as variables. The action buttons are active depending on the choices in the Periodicity Type and Calculate Average Properties lists.
•
The viscoelastic model of the matrix can be modeled using the Generalized Maxwell material model available in the Viscoelasticity feature.
Application Library path: Structural_Mechanics_Module/Material_Models/micromechanical_model_of_a_particulate_composite
Modeling Instructions
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  3D.
2
In the Select Physics tree, select Structural Mechanics>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. In the table, enter the following settings:
Name
Expression
Value
Description
para
0
0
Parameter
L
1[m]
1 m
Unit cell length
dp
0.4[m]
0.4 m
Particle diameter
Material Properties
1
In the Home toolbar, click  Parameters and choose Add>Parameters.
2
In the Settings window for Parameters, type Material 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 micromechanical_model_of_a_particulate_composite_material_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>Representative Volume Elements>3D>particulate_primitive_cubic in the tree.
2
Right-click Global Definitions and choose Add to Model.
3
In the Select Part Variant dialog box, select Specify particle diameter in the Select part variant list.
4
Click OK.
Create one RVE geometry for the heterogeneous material and one for the homogenized material.
Geometry 1
Heterogeneous RVE
1
In the Geometry toolbar, click  Parts and choose Particulate Composite, Primitive Cubic.
2
In the Settings window for Part Instance, type Heterogeneous RVE in the Label text field.
To define the RVE geometry, enter the geometric properties in the input parameters of the part.
3
Locate the Input Parameters section. In the table, enter the following settings:
Name
Expression
Value
Description
dp
dp
0.4 m
Particle diameter
wm
L
1 m
Width of RVE
dm
L
1 m
Depth of RVE
hm
L
1 m
Height of RVE
Homogeneous RVE
1
In the Geometry toolbar, click  Block.
2
In the Settings window for Block, type Homogeneous RVE in the Label text field.
3
Locate the Size and Shape section. In the Width text field, type L.
4
In the Depth text field, type L.
5
In the Height text field, type L.
6
Locate the Position section. In the x text field, type 2*L.
7
Click  Build Selected.
Materials
Matrix
1
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose Blank Material.
2
In the Settings window for Material, type Matrix in the Label text field.
3
Locate the Geometric Entity Selection section. From the Selection list, choose Matrix (Heterogeneous RVE).
4
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
E_m
Pa
Young’s modulus and Poisson’s ratio
Poisson’s ratio
nu
nu_m
1
Young’s modulus and Poisson’s ratio
Particulates
1
Right-click Materials and choose Blank Material.
2
In the Settings window for Material, type Particulates in the Label text field.
3
Locate the Geometric Entity Selection section. From the Selection list, choose Particle (Heterogeneous RVE).
4
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
E_p
Pa
Young’s modulus and Poisson’s ratio
Poisson’s ratio
nu
nu_p
1
Young’s modulus and Poisson’s ratio
First, set up the Solid Mechanics interface to compute the homogenized elastic properties.
Set the structural transient behavior to quasistatic as the inertial response is of no interest.
Solid Mechanics: Heterogeneous RVE
1
In the Model Builder window, under Component 1 (comp1) click Solid Mechanics (solid).
2
In the Settings window for Solid Mechanics, type Solid Mechanics: Heterogeneous RVE in the Label text field.
3
Locate the Domain Selection section. From the Selection list, choose All (Heterogeneous RVE).
4
Locate the Structural Transient Behavior section. From the list, choose Quasistatic.
Linear Elastic Material 1
Use reduced integration to speed up the simulation.
1
In the Model Builder window, under Component 1 (comp1)>Solid Mechanics: Heterogeneous RVE (solid) click Linear Elastic Material 1.
2
In the Settings window for Linear Elastic Material, locate the Quadrature Settings section.
3
Select the Reduced integration check box.
Cell Periodicity for Elastic Properties
1
In the Physics toolbar, click  Domains and choose Cell Periodicity.
2
In the Settings window for Cell Periodicity, type Cell Periodicity for Elastic Properties in the Label text field.
3
Locate the Periodicity Type section. From the list, choose Average strain.
4
From the Calculate average properties list, choose Elasticity matrix, Standard (XX, YY, ZZ, XY, YZ, XZ).
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
Click  Clear Selection.
4
From the Selection list, choose Pair 1 (Heterogeneous RVE).
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
Click  Clear Selection.
4
From the Selection list, choose Pair 2 (Heterogeneous RVE).
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
Click  Clear Selection.
4
From the Selection list, choose Pair 3 (Heterogeneous RVE).
Cell Periodicity for Elastic Properties
With the Average strain option in the Cell Periodicity feature, appropriate load groups, a study, and a material with computed elastic properties can be generated automatically.
1
In the Model Builder window, click Cell Periodicity for Elastic Properties.
2
In the Settings window for Cell Periodicity, click Study and Material Generation in the upper-right corner of the Periodicity Type section. From the menu, choose Create Load Groups and Study.
Mesh 1
Free Triangular 1
1
In the Mesh toolbar, click  Boundary and choose Free Triangular.
2
Select Boundaries 1–3 only.
Size 1
1
Right-click Free Triangular 1 and choose Size.
2
In the Settings window for Size, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Entire geometry.
4
Locate the Element Size section. From the Predefined list, choose Finer.
5
Click the Custom button.
6
Locate the Element Size Parameters section. Select the Maximum element size check box.
7
Select the Minimum element size check box.
8
Select the Maximum element growth rate check box.
9
Select the Curvature factor check box.
10
Select the Resolution of narrow regions check box.
11
Click  Build Selected.
Free Triangular 2
1
In the Mesh toolbar, click  Boundary and choose Free Triangular.
2
Select Boundaries 6–13 only.
Size 1
1
Right-click Free Triangular 2 and choose Size.
2
In the Settings window for Size, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Entire geometry.
4
Locate the Element Size section. From the Predefined list, choose Fine.
5
Click the Custom button.
6
Locate the Element Size Parameters section.
7
Select the Maximum element size check box. In the associated text field, type 0.07.
8
Select the Minimum element size check box. In the associated text field, type 0.05.
9
Select the Maximum element growth rate check box.
10
Select the Curvature factor check box.
11
Select the Resolution of narrow regions check box.
12
Click  Build Selected.
Copy Face 1
1
In the Mesh toolbar, click  Copy and choose Copy Face.
2
In the Settings window for Copy Face, locate the Source Boundaries section.
3
From the Selection list, choose Pair 1, Source (Heterogeneous RVE).
4
Locate the Destination Boundaries section. Click to select the  Activate Selection toggle button.
5
From the Selection list, choose Pair 1, Destination (Heterogeneous RVE).
6
Click  Build Selected.
Copy Face 2
1
In the Mesh toolbar, click  Copy and choose Copy Face.
2
In the Settings window for Copy Face, locate the Source Boundaries section.
3
From the Selection list, choose Pair 2, Source (Heterogeneous RVE).
4
Locate the Destination Boundaries section. Click to select the  Activate Selection toggle button.
5
From the Selection list, choose Pair 2, Destination (Heterogeneous RVE).
6
Click  Build Selected.
Copy Face 3
1
In the Mesh toolbar, click  Copy and choose Copy Face.
2
In the Settings window for Copy Face, locate the Source Boundaries section.
3
From the Selection list, choose Pair 3, Source (Heterogeneous RVE).
4
Locate the Destination Boundaries section. Click to select the  Activate Selection toggle button.
5
From the Selection list, choose Pair 3, Destination (Heterogeneous RVE).
6
Click  Build Selected.
Free Tetrahedral 1
1
In the Mesh toolbar, click  Free Tetrahedral.
2
In the Settings window for Free Tetrahedral, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
From the Selection list, choose All (Heterogeneous RVE).
Size 1
1
Right-click Free Tetrahedral 1 and choose Size.
2
In the Settings window for Size, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Entire geometry.
4
Locate the Element Size section. From the Predefined list, choose Normal.
5
Click the Custom button.
6
Locate the Element Size Parameters section. Select the Maximum element size check box.
7
Select the Minimum element size check box.
8
Select the Maximum element growth rate check box.
9
Select the Curvature factor check box. In the associated text field, type 0.4.
10
Select the Resolution of narrow regions check box.
11
Click  Build All.
Mapped 1
1
In the Mesh toolbar, click  Boundary and choose Mapped.
2
Select Boundary 15 only.
Distribution 1
1
Right-click Mapped 1 and choose Distribution.
2
Select Edges 28 and 30 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 1.
Swept 1
1
In the Mesh toolbar, click  Swept.
2
In the Settings window for Swept, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domain 3 only.
Distribution 1
1
Right-click Swept 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
In the Number of elements text field, type 1.
4
Click  Build All.
Cell Periodicity Study for Elastic Properties (Heterogeneous RVE)
1
In the Model Builder window, click Cell Periodicity Study.
2
In the Settings window for Study, type Cell Periodicity Study for Elastic Properties (Heterogeneous RVE) in the Label text field.
3
In the Home toolbar, click  Compute.
Results
Stress, Elastic Response
1
In the Model Builder window, under Results click Stress (solid).
2
In the Settings window for 3D Plot Group, type Stress, Elastic Response in the Label text field.
3
Click to expand the Selection section. From the Geometric entity level list, choose Domain.
4
From the Selection list, choose All (Heterogeneous RVE).
5
Select the Apply to dataset edges check box.
6
Click to expand the Title section. From the Title type list, choose Manual.
7
In the Title text area, type von Mises stress (MPa) .
8
Locate the Plot Settings section. Clear the Plot dataset edges check box.
9
Click to expand the Plot Array section. Select the Enable check box.
Volume 1
1
In the Model Builder window, expand the Stress, Elastic Response node, then click Volume 1.
2
In the Settings window for Volume, locate the Expression section.
3
From the Unit list, choose MPa.
Selection 1
1
Right-click Volume 1 and choose Selection.
2
In the Settings window for Selection, locate the Selection section.
3
From the Selection list, choose Matrix (Heterogeneous RVE).
Deformation
In the Model Builder window, under Results>Stress, Elastic Response>Volume 1 right-click Deformation and choose Delete.
Volume 2
1
In the Model Builder window, under Results>Stress, Elastic Response 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 check box.
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
From the Selection list, choose Particle (Heterogeneous RVE).
Stress, Elastic Response
Click the  Go to Default View button in the Graphics toolbar.
Before you set up the physics to analyze the viscoelastic response, 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 a material with numbers.
Solid Mechanics: Heterogeneous RVE (solid)
Cell Periodicity for Elastic Properties
1
In the Model Builder window, under Component 1 (comp1)>Solid Mechanics: Heterogeneous RVE (solid) click Cell Periodicity for Elastic Properties.
2
In the Settings window for Cell Periodicity, click Study and Material Generation in the upper-right corner of the Periodicity Type section. From the menu, choose Create Material by Value to generate a global material node with the computed elastic properties.
Set up the physics interface to analyze the viscoelastic response of the composite.
Global Definitions
Step 1 (step1)
1
In the Home toolbar, click  Functions and choose Global>Step.
2
In the Settings window for Step, type strainFunction in the Function name text field.
3
Locate the Parameters section. In the Location text field, type 5e-4[s].
4
Click to expand the Smoothing section. In the Size of transition zone text field, type 1e-3[s].
Definitions
Variables: Heterogeneous RVE
1
In the Model Builder window, under Component 1 (comp1) right-click Definitions and choose Variables.
2
In the Settings window for Variables, type Variables: Heterogeneous RVE in the Label text field.
3
Locate the Variables section. In the table, enter the following settings:
Name
Expression
Unit
Description
G_m
E_m/(2*(1+nu_m))
Pa
Shear modulus of matrix
sum_g
g1+g2+g3
 
Sum of weights
G_m0
G_m/(1-sum_g)
Pa
Instantaneous shear modulus of matrix
Solid Mechanics: Heterogeneous RVE (solid)
Linear Elastic Material 1
In the Model Builder window, under Component 1 (comp1)>Solid Mechanics: Heterogeneous RVE (solid) click Linear Elastic Material 1.
Viscoelasticity 1
1
In the Physics toolbar, click  Attributes and choose Viscoelasticity.
2
In the Settings window for Viscoelasticity, locate the Domain Selection section.
3
From the Selection list, choose Matrix (Heterogeneous RVE).
4
Locate the Viscoelasticity Model section. In the table, enter the following settings:
Branch
Shear modulus (Pa)
Relaxation time (s)
1
G_m0*g1
Tau1
5
Click  Add.
6
In the table, enter the following settings:
Branch
Shear modulus (Pa)
Relaxation time (s)
2
G_m0*g2
Tau2
7
Click  Add.
8
In the table, enter the following settings:
Branch
Shear modulus (Pa)
Relaxation time (s)
3
G_m0*g3
Tau3
Cell Periodicity for Viscoelastic Properties
1
In the Model Builder window, right-click Cell Periodicity for Elastic Properties and choose Duplicate.
2
In the Settings window for Cell Periodicity, type Cell Periodicity for Viscoelastic Properties in the Label text field.
3
Locate the Periodicity Type section. From the Calculate average properties list, choose None.
4
In the εavg table, enter the following settings:
(para==1)*strainFunction(t)
(para==2)*0.5*strainFunction(t)
0
(para==2)*0.5*strainFunction(t)
0
0
0
0
0
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>Time Dependent.
4
Click Add Study in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Transient Study for Viscoelastic Response (Heterogeneous RVE)
1
In the Model Builder window, click Study 1.
2
In the Settings window for Study, type Transient Study for Viscoelastic Response (Heterogeneous RVE) in the Label text field.
Parametric Sweep
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
para (Parameter)
range(1,1,2)
 
Step 1: Time Dependent
1
In the Model Builder window, click Step 1: Time Dependent.
2
In the Settings window for Time Dependent, locate the Study Settings section.
3
In the Output times text field, type range(0,0.5e-4,9.5e-4) 10^{range(-3,0.1,1.5)}.
4
Locate the Physics and Variables Selection section. Select the Modify model configuration for study step check box.
5
In the tree, select Component 1 (comp1)>Solid Mechanics: Heterogeneous RVE (solid)>Cell Periodicity for Elastic Properties.
6
Right-click and choose Disable.
Customize the solver settings by choosing a smaller initial time step for better convergence.
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 1 (sol1) node, then click Time-Dependent Solver 1.
3
In the Settings window for Time-Dependent Solver, click to expand the Time Stepping section.
4
Select the Initial step check box. In the associated text field, type 5e-7.
5
In the Study toolbar, click  Compute.
Visualize the stress in the composite when matrix viscoelasticity is activated.
Results
Stress, Viscoelastic Response
1
In the Model Builder window, under Results click Stress (solid).
2
In the Settings window for 3D Plot Group, type Stress, Viscoelastic Response in the Label text field.
3
Click to expand the Selection section. From the Geometric entity level list, choose Domain.
4
From the Selection list, choose All (Heterogeneous RVE).
5
Select the Apply to dataset edges check box.
6
Locate the Title section. From the Title type list, choose Manual.
7
In the Title text area, type von Mises stress (MPa) .
8
Locate the Plot Settings section. Clear the Plot dataset edges check box.
9
Locate the Plot Array section. Select the Enable check box.
Volume 1
1
In the Model Builder window, expand the Stress, Viscoelastic Response node, then click Volume 1.
2
In the Settings window for Volume, locate the Expression section.
3
From the Unit list, choose MPa.
Selection 1
1
Right-click Volume 1 and choose Selection.
2
In the Settings window for Selection, locate the Selection section.
3
From the Selection list, choose Matrix (Heterogeneous RVE).
Deformation
In the Model Builder window, under Results>Stress, Viscoelastic Response>Volume 1 right-click Deformation and choose Delete.
Volume 2
1
In the Model Builder window, under Results>Stress, Viscoelastic Response right-click Volume 1 and choose Duplicate.
2
In the Settings window for Volume, locate the Inherit Style section.
3
From the Plot list, choose Volume 1.
4
Locate the Plot Array section. Clear the Apply to dataset edges check box.
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
From the Selection list, choose Particle (Heterogeneous RVE).
Stress, Viscoelastic Response
Click the  Go to Default View button in the Graphics toolbar.
Average Normal and Shear Stresses
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Average Normal and Shear Stresses in the Label text field.
3
Locate the Data section. From the Dataset list, choose Transient Study for Viscoelastic Response (Heterogeneous RVE)/Parametric Solutions 1 (sol2).
4
Locate the Plot Settings section.
5
Select the y-axis label check box. In the associated text field, type Average stress (N/m<sup>2</sup>).
6
Click to expand the Title section. From the Title type list, choose Manual.
7
In the Title text area, type Global: Average stress (N/m<sup>2</sup>) .
8
Locate the Axis section. Select the x-axis log scale check box.
9
Locate the Legend section. From the Position list, choose Lower right.
Global 1
1
Right-click Average Normal and Shear Stresses and choose Global.
2
In the Settings window for Global, locate the Data section.
3
From the Dataset list, choose Transient Study for Viscoelastic Response (Heterogeneous RVE)/Parametric Solutions 1 (sol2).
4
From the Parameter selection (para) list, choose First.
5
Locate the y-Axis Data section. In the table, enter the following settings:
Expression
Unit
Description
solid.cp2.savgXX
N/m^2
Average stress, XX direction
6
Click to expand the Legends section. From the Legends list, choose Manual.
7
In the table, enter the following settings:
Legends
Average normal stress
Global 2
1
Right-click Global 1 and choose Duplicate.
2
In the Settings window for Global, locate the Data section.
3
From the Parameter selection (para) list, choose Last.
4
Locate the y-Axis Data section. In the table, enter the following settings:
Expression
Unit
Description
solid.cp2.savgXY
N/m^2
Average stress, XY direction
5
Locate the Legends section. In the table, enter the following settings:
Legends
Average shear stress
6
In the Average Normal and Shear Stresses toolbar, click  Plot.
Evaluation Group: Normal Stress Response
1
In the Results toolbar, click  Evaluation Group.
2
In the Settings window for Evaluation Group, type Evaluation Group: Normal Stress Response in the Label text field.
3
Locate the Data section. From the Dataset list, choose Transient Study for Viscoelastic Response (Heterogeneous RVE)/Parametric Solutions 1 (sol2).
4
From the Parameter selection (para) list, choose First.
5
From the Time selection list, choose Manual.
6
In the Time indices (1-66) text field, type range(21,1,61).
Global Evaluation 1
1
Right-click Evaluation Group: Normal Stress Response and choose Global Evaluation.
2
In the Settings window for Global Evaluation, locate the Expressions section.
3
In the table, enter the following settings:
Expression
Unit
Description
t
s
Time
solid.cp2.savgXX
N/m^2
Average stress, XX component
Evaluation Group: Normal Stress Response
1
In the Model Builder window, click Evaluation Group: Normal Stress Response.
2
In the Settings window for Evaluation Group, click to expand the Format section.
3
From the Include parameters list, choose Off.
4
In the Evaluation Group: Normal Stress Response toolbar, click  Evaluate.
Evaluation Group: Shear Stress Response
1
In the Results toolbar, click  Evaluation Group.
2
In the Settings window for Evaluation Group, type Evaluation Group: Shear Stress Response in the Label text field.
3
Locate the Data section. From the Dataset list, choose Transient Study for Viscoelastic Response (Heterogeneous RVE)/Parametric Solutions 1 (sol2).
4
From the Parameter selection (para) list, choose Last.
5
From the Time selection list, choose Manual.
6
In the Time indices (1-66) text field, type range(21,1,61).
Global Evaluation 1
1
Right-click Evaluation Group: Shear Stress Response and choose Global Evaluation.
2
In the Settings window for Global Evaluation, locate the Expressions section.
3
In the table, enter the following settings:
Expression
Unit
Description
t
s
Time
solid.cp2.savgXY
N/m^2
Average stress, XY component
Evaluation Group: Shear Stress Response
1
In the Model Builder window, click Evaluation Group: Shear Stress Response.
2
In the Settings window for Evaluation Group, locate the Format section.
3
From the Include parameters list, choose Off.
4
In the Evaluation Group: Shear Stress Response toolbar, click  Evaluate.
Average Normal and Shear Stresses, Evaluation Group: Normal Stress Response, Evaluation Group: Shear Stress Response, Stress, Elastic Response, Stress, Viscoelastic Response
1
In the Model Builder window, under Results, Ctrl-click to select Stress, Elastic Response, Stress, Viscoelastic Response, Average Normal and Shear Stresses, Evaluation Group: Normal Stress Response, and Evaluation Group: Shear Stress Response.
2
Right-click and choose Group.
Heterogeneous RVE
In the Settings window for Group, type Heterogeneous RVE in the Label text field.
Global Definitions
Optimization parameters
1
In the Home toolbar, click  Parameters and choose Add>Parameters.
2
In the Settings window for Parameters, type Optimization parameters in the Label text field.
3
Locate the Parameters section. In the table, enter the following settings:
Name
Expression
Value
Description
gg1
0
0
Deviatoric Prony series parameter of homogenized material, branch 1
gg2
0
0
Deviatoric Prony series parameter of homogenized material, branch 2
gg3
0
0
Deviatoric Prony series parameter of homogenized material, branch 3
kg1
0
0
Volumetric Prony series parameter of homogenized material, branch 1
kg2
0
0
Volumetric Prony series parameter of homogenized material, branch 2
kg3
0
0
Volumetric Prony series parameter of homogenized material, branch 3
Definitions
Variables: Homogenized material
1
In the Model Builder window, under Component 1 (comp1) right-click Definitions and choose Variables.
2
In the Settings window for Variables, type Variables: Homogenized material in the Label text field.
3
Locate the Variables section. In the table, enter the following settings:
Name
Expression
Unit
Description
G_H
solid2.D66
 
Shear modulus of homogenized material
K_H
solid2.D11-4*G_H/3
 
Bulk modulus of homogenized material
sum_gH
gg1+gg2+gg3
 
Sum of weights
sum_kH
kg1+kg2+kg3
 
Sum of weights
G_H0
G_H/(1-sum_gH)
 
Instantaneous shear modulus of homogenized material
K_H0
K_H/(1-sum_kH)
 
Instantaneous bulk modulus of homogenized material
Materials
Homogeneous Material
1
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose More Materials>Material Link.
2
In the Settings window for Material Link, type Homogeneous Material in the Label text field.
3
Select Domain 3 only.
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>Solid Mechanics (solid).
4
Click Add to Component 1 in the window toolbar.
5
In the Home toolbar, click  Add Physics to close the Add Physics window.
Solid Mechanics: Homogeneous RVE
1
In the Settings window for Solid Mechanics, type Solid Mechanics: Homogeneous RVE in the Label text field.
2
Select Domain 3 only.
3
Locate the Structural Transient Behavior section. From the list, choose Quasistatic.
4
Click to expand the Discretization section. From the Displacement field list, choose Linear.
Two separate studies are required to compute the homogenized viscoelastic parameters. First, apply a unit (engineering) shear strain in order to find the homogenized deviatoric Prony series parameters.
Linear Elastic Material 1
1
In the Model Builder window, under Component 1 (comp1)>Solid Mechanics: Homogeneous RVE (solid2) 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.
Viscoelasticity 1
1
In the Physics toolbar, click  Attributes and choose Viscoelasticity.
2
In the Settings window for Viscoelasticity, locate the Viscoelasticity Model section.
3
In the table, enter the following settings:
Branch
Shear modulus (Pa)
Relaxation time (s)
1
G_H0*gg1
Tau1
4
Click  Add.
5
In the table, enter the following settings:
Branch
Shear modulus (Pa)
Relaxation time (s)
2
G_H0*gg2
Tau2
6
Click  Add.
7
In the table, enter the following settings:
Branch
Shear modulus (Pa)
Relaxation time (s)
3
G_H0*gg3
Tau3
Cell Periodicity: Shear Strain Loading
1
In the Physics toolbar, click  Domains and choose Cell Periodicity.
2
In the Settings window for Cell Periodicity, type Cell Periodicity: Shear Strain Loading in the Label text field.
3
Locate the Periodicity Type section. From the list, choose Average strain.
4
In the εavg table, enter the following settings:
0
0.5*strainFunction(t)
0
0.5*strainFunction(t)
0
0
0
0
0
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
Click  Clear Selection.
4
Select Boundaries 15 and 20 only.
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
Click  Clear Selection.
4
Select Boundaries 16 and 19 only.
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
Click  Clear Selection.
4
Select Boundaries 17 and 18 only.
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>Time Dependent.
4
Find the Physics interfaces in study subsection. In the table, clear the Solve check box for Solid Mechanics: Heterogeneous RVE (solid).
5
Click Add Study in the window toolbar.
6
In the Home toolbar, click  Add Study to close the Add Study window.
Deviatoric Prony Series Parameter Estimation (Homogeneous RVE)
1
In the Model Builder window, click Study 2.
2
In the Settings window for Study, type Deviatoric Prony Series Parameter Estimation (Homogeneous RVE) in the Label text field.
3
Locate the Study Settings section. Clear the Generate default plots check box.
To get the homogenized viscoelastic parameters, the initial and final elastic responses of the heterogeneous RVE can be neglected. This means that the interesting time range is from 0.001 s to 10 s.
Step 1: Time Dependent
1
In the Model Builder window, under Deviatoric Prony Series Parameter Estimation (Homogeneous RVE) click Step 1: Time Dependent.
2
In the Settings window for Time Dependent, locate the Study Settings section.
3
In the Output times text field, type 10^{range(-3,0.1,1)}.
Parameter Estimation
1
In the Study toolbar, click  Optimization and choose Parameter Estimation.
2
In the Settings window for Parameter Estimation, locate the Experimental Data section.
3
From the Data source list, choose Result table.
4
From the Result table list, choose Evaluation Group: Shear Stress Response.
5
Locate the Column Settings section. In the table, click to select the cell at row number 2 and column number 1.
6
In the Model expression text field, type comp1.solid2.cp1.savgXY.
7
In the Unit text field, type N/m^2.
8
Locate the Parameters section. Click  Add three times.
9
Row by row, select the parameter name in the first column, then set the corresponding initial value, scale, and bounds as follows:
Parameter name
Initial value
Scale
Lower bound
Upper bound
gg1 (Deviatoric Prony series parameter of homogenized material, branch 1)
g1
1
0
1
gg2 (Deviatoric Prony series parameter of homogenized material, branch 2)
g2
1
0
1
gg3 (Deviatoric Prony series parameter of homogenized material, branch 3)
g3
1
0
1
10
Locate the Parameter Estimation Method section. From the Method list, choose Levenberg-Marquardt.
Solution 5 (sol5)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 5 (sol5) node.
3
In the Model Builder window, expand the Deviatoric Prony Series Parameter Estimation (Homogeneous RVE)>Solver Configurations>Solution 5 (sol5)>Optimization Solver 1 node, then click Time-Dependent Solver 1.
4
In the Settings window for Time-Dependent Solver, click to expand the Time Stepping section.
5
Select the Initial step check box. In the associated text field, type 5e-5.
6
In the Study toolbar, click  Compute.
Results
Average Shear Stress
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Average Shear Stress in the Label text field.
3
Locate the Data section. From the Dataset list, choose Deviatoric Prony Series Parameter Estimation (Homogeneous RVE)/Solution 5 (sol5).
4
Locate the Plot Settings section.
5
Select the y-axis label check box. In the associated text field, type Average shear stress (N/m<sup>2</sup>).
6
Locate the Title section. From the Title type list, choose Manual.
7
In the Title text area, type Global: Average shear stress (N/m<sup>2</sup>) .
8
Locate the Axis section. Select the x-axis log scale check box.
Global 1
1
Right-click Average Shear Stress and choose Global.
2
In the Settings window for Global, locate the y-Axis Data section.
3
In the table, enter the following settings:
Expression
Unit
Description
solid2.cp1.savgXY
N/m^2
Average stress, XY direction
4
Locate the Legends section. From the Legends list, choose Manual.
5
In the table, enter the following settings:
Legends
Homogenized material model
Global 2
1
Right-click Global 1 and choose Duplicate.
2
In the Settings window for Global, locate the Data section.
3
From the Dataset list, choose Transient Study for Viscoelastic Response (Heterogeneous RVE)/Parametric Solutions 1 (sol2).
4
From the Parameter selection (para) list, choose Last.
5
From the Time selection list, choose Interpolated.
6
In the Times (s) text field, type 10^{range(-3,0.1,1)}.
7
Locate the y-Axis Data section. In the table, enter the following settings:
Expression
Unit
Description
solid.cp2.savgXY
N/m^2
Average stress, XY direction
8
Click to expand the Coloring and Style section. Find the Line markers subsection. From the Marker list, choose Point.
9
Find the Line style subsection. From the Line list, choose None.
10
Locate the Legends section. In the table, enter the following settings:
Legends
Heterogeneous RVE
11
In the Average Shear Stress toolbar, click  Plot.
Duplicate the Viscoelasticity and Cell Periodicity features to set up a normal strain load case in order to compute the homogenized volumetric Prony series parameters. Use the homogenized deviatoric Prony series parameters obtained in the previous optimization study in the new Viscoelasticity feature.
Solid Mechanics: Homogeneous RVE (solid2)
Viscoelasticity 2
1
In the Model Builder window, under Component 1 (comp1)>Solid Mechanics: Homogeneous RVE (solid2)>Linear Elastic Material 1 right-click Viscoelasticity 1 and choose Duplicate.
2
In the Settings window for Viscoelasticity, locate the Viscoelasticity Model section.
3
From the Viscoelastic strains list, choose Volumetric and deviatoric.
4
In the table, enter the following settings:
Branch
Bulk modulus (Pa)
Shear modulus (Pa)
Relaxation time (s)
1
K_H0*kg1
G_H0*withsol('sol5',gg1)
Tau1
5
Click  Add.
6
In the table, enter the following settings:
Branch
Bulk modulus (Pa)
Shear modulus (Pa)
Relaxation time (s)
2
K_H0*kg2
G_H0*withsol('sol5',gg2)
Tau2
7
Click  Add.
8
In the table, enter the following settings:
Branch
Bulk modulus (Pa)
Shear modulus (Pa)
Relaxation time (s)
3
K_H0*kg3
G_H0*withsol('sol5',gg3)
Tau3
Cell Periodicity: Normal Strain Loading
1
In the Model Builder window, right-click Cell Periodicity: Shear Strain Loading and choose Duplicate.
Apply a unit step in the normal strain.
2
In the Settings window for Cell Periodicity, type Cell Periodicity: Normal Strain Loading in the Label text field.
3
Locate the Periodicity Type section. In the εavg table, enter the following settings:
strainFunction(t)
0
0
0
0
0
0
0
0
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>Time Dependent.
4
Find the Physics interfaces in study subsection. In the table, clear the Solve check box for Solid Mechanics: Heterogeneous RVE (solid).
5
Click Add Study in the window toolbar.
6
In the Home toolbar, click  Add Study to close the Add Study window.
Volumetric Prony Series Parameter Estimation (Homogeneous RVE)
1
In the Model Builder window, click Study 3.
2
In the Settings window for Study, type Volumetric Prony Series Parameter Estimation (Homogeneous RVE) in the Label text field.
3
Locate the Study Settings section. Clear the Generate default plots check box.
To get the homogenized viscoelastic parameters, the initial and final elastic responses of the heterogeneous RVE can be neglected. This means that the interesting time range is from 0.001 s to 10 s.
Step 1: Time Dependent
1
In the Model Builder window, under Volumetric Prony Series Parameter Estimation (Homogeneous RVE) click Step 1: Time Dependent.
2
In the Settings window for Time Dependent, locate the Study Settings section.
3
In the Output times text field, type 10^{range(-3,0.1,1)}.
4
Locate the Physics and Variables Selection section. Select the Modify model configuration for study step check box.
5
In the tree, select Component 1 (comp1)>Solid Mechanics: Homogeneous RVE (solid2)>Linear Elastic Material 1>Viscoelasticity 1 and Component 1 (comp1)>Solid Mechanics: Homogeneous RVE (solid2)>Cell Periodicity: Shear Strain Loading.
6
Right-click and choose Disable.
Parameter Estimation
1
In the Study toolbar, click  Optimization and choose Parameter Estimation.
2
In the Settings window for Parameter Estimation, locate the Experimental Data section.
3
From the Data source list, choose Result table.
4
From the Result table list, choose Evaluation Group: Normal Stress Response.
5
Locate the Column Settings section. In the table, click to select the cell at row number 2 and column number 1.
6
In the Model expression text field, type comp1.solid2.cp2.savgXX.
7
In the Unit text field, type N/m^2.
8
Locate the Parameters section. Click  Add three times.
9
Row by row, select the parameter name in the first column, then set the corresponding initial value, scale, and bounds as follows:
Parameter name
Initial value
Scale
Lower bound
Upper bound
kg1 (Volumetric Prony series parameter of homogenized material, branch 1)
0.001
1
0
1
kg2 (Volumetric Prony series parameter of homogenized material, branch 2)
0.001
1
0
1
kg3 (Volumetric Prony series parameter of homogenized material, branch 3)
0.001
1
0
1
10
Locate the Parameter Estimation Method section. From the Method list, choose Levenberg-Marquardt.
Solution 6 (sol6)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 6 (sol6) node.
3
In the Model Builder window, expand the Volumetric Prony Series Parameter Estimation (Homogeneous RVE)>Solver Configurations>Solution 6 (sol6)>Optimization Solver 1 node, then click Time-Dependent Solver 1.
4
In the Settings window for Time-Dependent Solver, locate the Time Stepping section.
5
Select the Initial step check box. In the associated text field, type 5e-5.
6
In the Study toolbar, click  Compute.
Results
Average Normal Stress
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Average Normal Stress in the Label text field.
3
Locate the Data section. From the Dataset list, choose Volumetric Prony Series Parameter Estimation (Homogeneous RVE)/Solution 6 (sol6).
4
Locate the Plot Settings section.
5
Select the y-axis label check box. In the associated text field, type Average shear stress (N/m<sup>2</sup>).
6
Locate the Title section. From the Title type list, choose Manual.
7
In the Title text area, type Global: Average normal stress (N/m<sup>2</sup>) .
8
Locate the Axis section. Select the x-axis log scale check box.
Global 1
1
Right-click Average Normal Stress and choose Global.
2
In the Settings window for Global, locate the y-Axis Data section.
3
In the table, enter the following settings:
Expression
Unit
Description
solid2.cp2.savgXX
N/m^2
Average stress, XX direction
4
Locate the Legends section. From the Legends list, choose Manual.
5
In the table, enter the following settings:
Legends
Homogenized material model
Global 2
1
Right-click Global 1 and choose Duplicate.
2
In the Settings window for Global, locate the Data section.
3
From the Dataset list, choose Transient Study for Viscoelastic Response (Heterogeneous RVE)/Parametric Solutions 1 (sol2).
4
From the Parameter selection (para) list, choose First.
5
From the Time selection list, choose Interpolated.
6
In the Times (s) text field, type 10^{range(-3,0.1,1)}.
7
Locate the y-Axis Data section. In the table, enter the following settings:
Expression
Unit
Description
solid.cp2.savgXX
N/m^2
Average stress, XX direction
8
Locate the Coloring and Style section. Find the Line markers subsection. From the Marker list, choose Point.
9
Find the Line style subsection. From the Line list, choose None.
10
Locate the Legends section. In the table, enter the following settings:
Legends
Heterogeneous RVE
11
In the Average Normal Stress toolbar, click  Plot.
Evaluation Group: Homogenized Prony Series Parameters
1
In the Results toolbar, click  Evaluation Group.
2
In the Settings window for Evaluation Group, type Evaluation Group: Homogenized Prony Series Parameters in the Label text field.
3
Locate the Data section. From the Dataset list, choose Deviatoric Prony Series Parameter Estimation (Homogeneous RVE)/Solution 5 (sol5).
4
From the Time selection list, choose First.
Global Evaluation 1
1
Right-click Evaluation Group: Homogenized Prony Series Parameters and choose Global Evaluation.
2
In the Settings window for Global Evaluation, locate the Expressions section.
3
In the table, enter the following settings:
Expression
Unit
Description
gg1
 
Deviatoric Prony series parameter of homogenized material, branch 1
gg2
 
Deviatoric Prony series parameter of homogenized material, branch 2
gg3
 
Deviatoric Prony series parameter of homogenized material, branch 3
Global Evaluation 2
1
Right-click Global Evaluation 1 and choose Duplicate.
2
In the Settings window for Global Evaluation, locate the Data section.
3
From the Dataset list, choose Volumetric Prony Series Parameter Estimation (Homogeneous RVE)/Solution 6 (sol6).
4
From the Time selection list, choose First.
5
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
kg1
 
Volumetric Prony series parameter of homogenized material, branch 1
kg2
 
Volumetric Prony series parameter of homogenized material, branch 2
kg3
 
Volumetric Prony series parameter of homogenized material, branch 3
Evaluation Group: Homogenized Prony Series Parameters
1
In the Model Builder window, click Evaluation Group: Homogenized Prony Series Parameters.
2
In the Settings window for Evaluation Group, locate the Transformation section.
3
Select the Transpose check box.
4
Locate the Format section. From the Include parameters list, choose Off.
5
In the Evaluation Group: Homogenized Prony Series Parameters toolbar, click  Evaluate.
Average Normal Stress, Average Shear Stress, Evaluation Group: Homogenized Prony Series Parameters
1
In the Model Builder window, under Results, Ctrl-click to select Average Shear Stress, Average Normal Stress, and Evaluation Group: Homogenized Prony Series Parameters.
2
Right-click and choose Group.
Homogeneous RVE
In the Settings window for Group, type Homogeneous RVE in the Label text field.