PDF
Micromechanical Model of a Particulate Composite
Introduction
In this example, a simplified micromechanical model of a particulate composite is analyzed. A repeating unit cell (RUC) 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 material 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 least-squares parameter estimation.
The following considerations are important for the analysis:
•
In the particulate composite, only the matrix material is assumed to exhibit viscoelastic behavior. This is a realistic assumption for, for example, polymer matrix composites. Polymer-like resin is typically viscoelastic, 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 viscoelastic parameters from the particulate composite, two different stress responses from a unit cell are required:
-
The shear stress response, which only activates the deviatoric part of the homogeneous viscoelastic model.
-
The normal stress response, which activates both the deviatoric and the volumetric part of the homogeneous viscoelastic model.
•
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 RUC 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 linear 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 is the relative weight and τk is the relaxation time constant of the spring–dashpot pair in branch k. 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 of the viscoelastic matrix 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. As expected, the stresses in the constituents computed in the viscoelastic study are in good agreement with those computed in the elastic study.
The variation in average normal and shear stress with time for the heterogeneous RUC 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 RUC and the equivalent, homogenized material are shown in Figure 7 and Figure 8, respectively. The relative weights for the deviatoric and volumetric parts obtained from the parameter estimation studies 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
0.00957
0.01 s
2
0.04970
0.1 s
3
0.07928
1 s
Table 5: Homogenized viscoelastic volumetric properties.
Branch
Relative Weight
Relaxation Time Constant
1
8.941E-4
0.01 s
2
0.00427
0.1 s
3
0.00683
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 RUC.
Figure 7: Average viscoelastic shear stress for the composite and the homogenized material.
.
Figure 8: Average viscoelastic normal stress for the heterogeneous RUC and the equivalent homogenized material.
Notes About the COMSOL Implementation
•
Micromechanical analyses RUCs 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 subnode.
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 > Unit Cells and RVEs > Particulate Composites > particulate_primitive_cubic in the tree.
2
Right-click Global Definitions and choose Add to Model.
3
In the Select Part Variant dialog, select Specify particle diameter in the Select part variant list.
4
Click OK.
Create one repeating unit cell (RUC) geometry for the heterogeneous material and one for the homogenized material.
Geometry 1
Heterogeneous RUC
1
In the Geometry toolbar, click  Part Instance and choose Particulate Composite, Primitive Cubic.
2
In the Settings window for Part Instance, type Heterogeneous RUC in the Label text field.
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
Cell width
dm
L
1 m
Cell depth
hm
L
1 m
Cell height
Homogeneous RUC
1
In the Geometry toolbar, click  Block.
2
In the Settings window for Block, type Homogeneous RUC 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 RUC).
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 RUC).
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 RUC
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 RUC in the Label text field.
3
Locate the Domain Selection section. From the Selection list, choose All (Heterogeneous RUC).
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 RUC (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 checkbox.
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 Settings section. From the Boundary conditions list, choose Average strain.
4
Locate the Effective Properties section. 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
Click  Clear Selection.
4
From the Selection list, choose Pair 1 (Heterogeneous RUC).
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 RUC).
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 RUC).
Cell Periodicity for Elastic Properties
With the Average strain option in the Cell Periodicity node, 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 Automated Model Setup in the upper-right corner of the Periodicity Settings section. From the menu, choose Create Load Groups and Study.
Mesh 1
Free Triangular 1
1
In the Mesh toolbar, click  More Generators 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 checkbox.
7
Select the Minimum element size checkbox.
8
Select the Maximum element growth rate checkbox.
9
Select the Curvature factor checkbox.
10
Select the Resolution of narrow regions checkbox.
11
Click  Build Selected.
Free Triangular 2
1
In the Mesh toolbar, click  More Generators 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 checkbox. In the associated text field, type 0.07.
8
Select the Minimum element size checkbox. In the associated text field, type 0.05.
9
Select the Maximum element growth rate checkbox.
10
Select the Curvature factor checkbox.
11
Select the Resolution of narrow regions checkbox.
12
Click  Build Selected.
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 (Heterogeneous RUC).
4
Locate the Second Entity Group section. From the Selection list, choose Pair 1, Destination (Heterogeneous RUC).
Identical Mesh 2
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 2, Source (Heterogeneous RUC).
4
Locate the Second Entity Group section. From the Selection list, choose Pair 2, Destination (Heterogeneous RUC).
Identical Mesh 3
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 3, Source (Heterogeneous RUC).
4
Locate the Second Entity Group section. From the Selection list, choose Pair 3, Destination (Heterogeneous RUC).
5
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 RUC).
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. Click the Custom button.
5
Locate the Element Size Parameters section. Select the Maximum element size checkbox.
6
Select the Minimum element size checkbox.
7
Select the Maximum element growth rate checkbox.
8
Select the Curvature factor checkbox. In the associated text field, type 0.4.
9
Select the Resolution of narrow regions checkbox.
10
Click  Build All.
Mapped 1
1
In the Mesh toolbar, click  More Generators 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 RUC)
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 RUC) 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
GPa
8
Click  Apply.
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 RUC).
5
Select the Apply to dataset edges checkbox.
6
Click to expand the Title section. From the Title type list, choose Manual.
7
In the Title text area, type von Mises stress (GPa).
8
Locate the Plot Settings section. Clear the Plot dataset edges checkbox.
9
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, Elastic Response node.
2
Right-click Volume 1 and choose Selection.
3
In the Settings window for Selection, locate the Selection section.
4
From the Selection list, choose Matrix (Heterogeneous RUC).
Deformation
In the Model Builder window, 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 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
From the Selection list, choose Particle (Heterogeneous RUC).
Solid Mechanics: Heterogeneous RUC (solid)
Before you set up the physics to analyze the viscoelastic response, create a homogenized material from the Cell Periodicity node. 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.
Cell Periodicity for Elastic Properties
1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics: Heterogeneous RUC (solid) click Cell Periodicity for Elastic Properties.
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 the computed elastic properties.
Global Definitions
Set up the physics interface to analyze the viscoelastic response of the composite.
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 RUC
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 RUC 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 RUC (solid)
Linear Elastic Material 1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics: Heterogeneous RUC (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 RUC).
4
Locate the Viscoelasticity Model section. Click  Add twice.
5
In the table, enter the following settings:
Branch
Shear modulus (Pa)
Relaxation time (s)
1
G_m0*g1
Tau1
2
G_m0*g2
Tau2
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 Effective Properties section. Clear the Compute elasticity matrix, standard notation checkbox.
4
Locate the Periodicity Settings section. Specify the εavg matrix as
(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 the Add Study button in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Transient Study for Viscoelastic Response (Heterogeneous RUC)
In the Settings window for Study, type Transient Study for Viscoelastic Response (Heterogeneous RUC) 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 checkbox.
5
In the tree, select Component 1 (comp1) > Solid Mechanics: Heterogeneous RUC (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 checkbox. In the associated text field, type 5e-7.
5
In the Study toolbar, click  Compute.
Results
Stress, Viscoelastic Response
Visualize the stress in the composite when matrix viscoelasticity is activated.
1
In the Settings window for 3D Plot Group, type Stress, Viscoelastic Response in the Label text field.
2
Locate the Selection section. From the Geometric entity level list, choose Domain.
3
From the Selection list, choose All (Heterogeneous RUC).
4
Select the Apply to dataset edges checkbox.
5
Locate the Title section. From the Title type list, choose Manual.
6
In the Title text area, type von Mises stress (GPa).
7
Locate the Plot Settings section. Clear the Plot dataset edges checkbox.
8
Locate the Plot Array section. From the Array type list, choose Linear.
Selection 1
1
In the Model Builder window, expand the Stress, Viscoelastic Response node.
2
Right-click Volume 1 and choose Selection.
3
In the Settings window for Selection, locate the Selection section.
4
From the Selection list, choose Matrix (Heterogeneous RUC).
Deformation
In the Model Builder window, 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 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
From the Selection list, choose Particle (Heterogeneous RUC).
Average Normal and Shear Stresses
1
In the Results toolbar, click  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 RUC)/Parametric Solutions 1 (sol2).
4
Locate the Plot Settings section.
5
Select the y-axis label checkbox. In the associated text field, type Average stress (GPa).
6
Click to expand the Title section. From the Title type list, choose Manual.
7
In the Title text area, type Global: Average stress (GPa).
8
Locate the Axis section. Select the x-axis log scale checkbox.
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 RUC)/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
GPa
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
GPa
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 RUC)/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
GPa
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 RUC)/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
GPa
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 RUC
In the Settings window for Group, type Heterogeneous RUC 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 the Add to Component 1 button in the window toolbar.
5
In the Home toolbar, click  Add Physics to close the Add Physics window.
Solid Mechanics: Homogeneous RUC
1
In the Settings window for Solid Mechanics, type Solid Mechanics: Homogeneous RUC 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 RUC (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
Click  Add twice.
4
In the table, enter the following settings:
Branch
Shear modulus (Pa)
Relaxation time (s)
1
G_H0*gg1
Tau1
2
G_H0*gg2
Tau2
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 Settings section. From the Boundary conditions list, choose Average strain.
4
Specify the εavg matrix as
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.
Component 1 (comp1)
Add a Parameter Estimation node with a Least-Squares Objective to set up the inverse problem for the deviatoric parameters.
Shear Stress Response
1
In the Physics toolbar, click  Optimization and choose Parameter Estimation.
2
In the Settings window for Least-Squares Objective, type Shear Stress Response in the Label text field.
3
Locate the Experimental Data section. From the Data source list, choose Result table.
4
From the Result table list, choose Evaluation Group: Shear Stress Response.
5
Locate the Data Column Settings section. In the Model expression text field, type comp1.solid2.cp1.savgXY.
6
In the Column name text field, type shear_stress.
7
In the Unit text field, type GPa.
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 the Add Study button in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Deviatoric Prony Series Parameter Estimation (Homogeneous RUC)
1
In the Settings window for Study, type Deviatoric Prony Series Parameter Estimation (Homogeneous RUC) in the Label text field.
2
Locate the Study Settings section. Clear the Generate default plots checkbox.
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 Selected Least-Squares objectives.
4
Locate the Objective Function section. In the table, select the Active checkbox for Shear Stress Response.
5
Locate the Estimated Parameters section. Click  Add three times.
6
Row by row, select the parameter name in the first column, then set the corresponding initial value, scale, and bounds as follows:
Parameter
Initial value
Scale
Lower bound
Upper bound
Unit
gg1 (Deviatoric Prony series parameter of homogenized material, branch 1)
g1
0.1
0
1
 
gg2 (Deviatoric Prony series parameter of homogenized material, branch 2)
g2
0.1
0
1
 
gg3 (Deviatoric Prony series parameter of homogenized material, branch 3)
g3
0.1
0
1
 
7
Locate the Parameter Estimation Method section. From the Method list, choose Levenberg–Marquardt.
8
From the Least-squares time/parameter list method list, choose Use only least-squares data points.
Step 1: Time Dependent
Disable the Solid Mechanics: Heterogeneous RUC interface.
1
In the Model Builder window, click Step 1: Time Dependent.
2
In the Settings window for Time Dependent, locate the Physics and Variables Selection section.
3
Select the Modify model configuration for study step checkbox.
4
In the tree, select Component 1 (comp1) > Solid Mechanics: Heterogeneous RUC (solid).
5
Click  Disable in Model.
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 RUC) > 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
From the Steps taken by solver list, choose Strict.
6
Select the Initial step checkbox. In the associated text field, type 5e-5.
7
In the Study toolbar, click  Compute.
Results
Average Shear Stress
1
In the Results toolbar, click  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 RUC)/Solution 5 (sol5).
4
Locate the Plot Settings section.
5
Select the y-axis label checkbox. In the associated text field, type Average shear stress (GPa).
6
Locate the Title section. From the Title type list, choose Manual.
7
In the Title text area, type Global: Average shear stress (GPa).
8
Locate the Axis section. Select the x-axis log scale checkbox.
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
GPa
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
Table Graph 1
1
In the Model Builder window, right-click Average Shear Stress and choose Table Graph.
2
In the Settings window for Table Graph, locate the Data section.
3
From the Source list, choose Evaluation group.
4
From the Evaluation group list, choose Evaluation Group: Shear Stress Response.
5
Locate the Coloring and Style section. Find the Line style subsection. From the Line list, choose None.
6
Find the Line markers subsection. From the Marker list, choose Point.
7
Click to expand the Legends section. Select the Show legends checkbox.
8
From the Legends list, choose Manual.
9
In the table, enter the following settings:
Legends
Heterogeneous RUC
10
In the Average Shear Stress toolbar, click  Plot.
Solid Mechanics: Homogeneous RUC (solid2)
Duplicate the Viscoelasticity and Cell Periodicity nodes 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 node.
Viscoelasticity 2
1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics: Homogeneous RUC (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
Click  Add twice.
5
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
2
K_H0*kg2
G_H0*withsol('sol5',gg2)
Tau2
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 Settings section. Specify the εavg matrix as
strainFunction(t)
0
0
0
0
0
0
0
0
Parameter Estimation
Add a Least-Squares Objective node for the normal stress load case.
Normal Stress Response
1
In the Parameter Estimation toolbar, click  Least-Squares Objective.
2
In the Settings window for Least-Squares Objective, type Normal Stress Response in the Label text field.
3
Locate the Experimental Data section. From the Data source list, choose Result table.
4
From the Result table list, choose Evaluation Group: Normal Stress Response.
5
Locate the Data Column Settings section. In the Model expression text field, type comp1.solid2.cp2.savgXX.
6
In the Column name text field, type normal_stress.
7
In the Unit text field, type GPa.
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 the Add Study button in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Volumetric Prony Series Parameter Estimation (Homogeneous RUC)
1
In the Settings window for Study, type Volumetric Prony Series Parameter Estimation (Homogeneous RUC) in the Label text field.
2
Locate the Study Settings section. Clear the Generate default plots checkbox.
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 Selected Least-Squares objectives.
4
Locate the Objective Function section. In the table, enter the following settings:
Objective functions from components
Active
Shear Stress Response
 
Normal Stress Response
√
5
Locate the Estimated Parameters section. Click  Add three times.
6
Row by row, select the parameter name in the first column, then set the corresponding initial value, scale, and bounds as follows:
Parameter
Initial value
Scale
Lower bound
Upper bound
Unit
kg1 (Volumetric Prony series parameter of homogenized material, branch 1)
0.001
0.001
0
1
 
kg2 (Volumetric Prony series parameter of homogenized material, branch 2)
0.001
0.001
0
1
 
kg3 (Volumetric Prony series parameter of homogenized material, branch 3)
0.001
0.001
0
1
 
7
Locate the Parameter Estimation Method section. From the Method list, choose Levenberg–Marquardt.
8
From the Least-squares time/parameter list method list, choose Use only least-squares data points.
Step 1: Time Dependent
Make sure to disable the Solid Mechanics: Heterogeneous RUC interface as well as the Viscoelasticity and Cell Periodicity nodes that you set up for the shear strain load case, since they only apply for the homogenized deviatoric response.
1
In the Model Builder window, click Step 1: Time Dependent.
2
In the Settings window for Time Dependent, locate the Physics and Variables Selection section.
3
Select the Modify model configuration for study step checkbox.
4
In the tree, select Component 1 (comp1) > Solid Mechanics: Heterogeneous RUC (solid).
5
Right-click and choose Disable in Model.
6
In the tree, select Component 1 (comp1) > Solid Mechanics: Homogeneous RUC (solid2) > Linear Elastic Material 1 > Viscoelasticity 1 and Component 1 (comp1) > Solid Mechanics: Homogeneous RUC (solid2) > Cell Periodicity: Shear Strain Loading.
7
Right-click and choose Disable.
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 RUC) > 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
From the Steps taken by solver list, choose Strict.
6
Select the Initial step checkbox. In the associated text field, type 5e-5.
7
In the Study toolbar, click  Compute.
Results
Average Normal Stress
1
In the Results toolbar, click  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 RUC)/Solution 6 (sol6).
4
Locate the Plot Settings section.
5
Select the y-axis label checkbox. In the associated text field, type Average shear stress (GPa).
6
Locate the Title section. From the Title type list, choose Manual.
7
In the Title text area, type Global: Average normal stress (GPa).
8
Locate the Axis section. Select the x-axis log scale checkbox.
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
GPa
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
Table Graph 1
1
In the Model Builder window, right-click Average Normal Stress and choose Table Graph.
2
In the Settings window for Table Graph, locate the Data section.
3
From the Source list, choose Evaluation group.
4
From the Evaluation group list, choose Evaluation Group: Normal Stress Response.
5
Locate the Coloring and Style section. Find the Line style subsection. From the Line list, choose None.
6
Find the Line markers subsection. From the Marker list, choose Point.
7
Locate the Legends section. Select the Show legends checkbox.
8
From the Legends list, choose Manual.
9
In the table, enter the following settings:
Legends
Heterogeneous RUC
10
In the Average Normal Stress toolbar, click  Plot.
Result Templates
Collect the calibrated Prony series parameters of the homogenized material in an Evaluation Group.
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 Deviatoric Prony Series Parameter Estimation (Homogeneous RUC)/Solution 5 (sol5) > Solid Mechanics: Homogeneous RUC > Estimated Parameters (std2).
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
Homogenized Prony Series Parameters
In the Settings window for Evaluation Group, type Homogenized Prony Series Parameters in the Label text field.
Global Evaluation 2
1
Right-click Homogenized Prony Series Parameters and choose Global Evaluation.
2
In the Settings window for Global Evaluation, locate the Data section.
3
From the Dataset list, choose Volumetric Prony Series Parameter Estimation (Homogeneous RUC)/Solution 6 (sol6).
4
From the Time selection list, choose Last.
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
6
In the Homogenized Prony Series Parameters toolbar, click  Evaluate.
Average Normal Stress, Average Shear Stress, Homogenized Prony Series Parameters
1
In the Model Builder window, under Results, Ctrl-click to select Average Shear Stress, Average Normal Stress, and Homogenized Prony Series Parameters.
2
Right-click and choose Group.
Homogeneous RUC
In the Settings window for Group, type Homogeneous RUC in the Label text field.