PDF
Micromechanical Model of a Triply-Periodic-Minimal-Surface-Based Composite
Introduction
The use of composites in various industries like automotive, aerospace, infrastructure, and many others has been rising over last few decades. Ever-increasing advancement of the technology demands advancements in the materials. Triply-periodic-minimal-surface-based (TPMS-based) composites are finding increasing use in various applications due to their outstanding mechanical and thermal properties; see Ref. 1. The accuracy of structural and thermal analyses relies on an accurate estimation of the mechanical and thermal properties of the composite material. At global scale, the composite needs to be treated as a homogeneous material in the continuum mechanics, which needs homogenization techniques to get the effective properties for such materials based on the material properties of the constituents.
In this example, the homogenized elastic and thermal properties of a composite material based on a TPMS are computed and the results are compared to those presented in Ref. 1. A gyroid TPMS-based unit cell is subjected to periodic boundary conditions to get the homogenized material properties. The effects of a negative Poisson’s ratio and different volume fractions on the homogenized properties are analyzed.
Model Definition
A unit cell of a gyroid TPMS is shown in Figure 1. The size of unit cell is 100 mm. The TPMS volume fraction is computed from the wall thickness of the TPMS.
Figure 1: Geometry of the gyroid unit cell.
TPMS and Matrix Properties
The material properties are taken from Ref. 1. The elastic moduli of TPMS and matrix are not explicitly given in Ref. 1; rather a ratio of 20 is given. This example assumes the elastic moduli 200 GPa and 10 GPa of the TPMS and matrix, respectively. The Poisson’s ratio of the TPMS and matrix in Ref. 1 are taken from a set of [0.3, −0.3, −0.5, −0.75]. For this example, we vary the Poisson’s ratio of the TPMS from the above set but keep the Poisson’s ratio of the matrix fixed to 0.3. The coefficient of thermal expansion for the TMPS and matrix are given as 0.8 × 10−6 1/K and 44 × 10−6 1/K, respectively.
Results and Discussion
Figure 2, Figure 3, and Figure 4 show the variation of the effective Young’s modulus, Poisson’s ratio, and shear modulus with different Poisson’s ratio and volume fractions of the TPMS. The variation of the effective coefficient of thermal expansion is shown in Figure 5. The result matches closely with results presented in Ref. 1 (see figure 5).
The authors in Ref. 1 investigated the effect of a negative Poisson’s ratio of the TPMS on the effective properties of the composite. As reported in Ref. 1, with negative Poisson’s ratio of the TPMS, the effective Young’s modulus, shear modulus, and coefficient of thermal expansion increase, while the effective Poisson’s ratio decreases. An increasing fiber volume fraction of the TPMS increases the effective Young’s modulus and shear modulus. The coefficient of thermal expansion and effective Poisson’s ratio decrease with increases in the TPMS fiber volume fraction.
The study indicates that the properties of the gyroid-based composite can be customized by changing the Poisson’s ratio or fiber volume fraction of the TPMS.
Figure 2: Effective Young’s modulus versus TPMS volume fraction.
Figure 3: Effective Poisson’s ratio versus TPMS volume fraction.
Figure 4: Effective shear modulus versus TPMS volume fraction.
Figure 5: Effective coefficient of thermal expansion versus TPMS volume fraction.
Notes About the COMSOL Implementation
•
In order to perform a micromechanical analysis, the Cell Periodicity node in the Solid Mechanics interface is used. The Cell Periodicity node is used to apply periodic boundary conditions to the three (two) pairs of faces of the unit cell in 3D (2D).
•
The Cell Periodicity node has three action buttons in the toolbar of the Periodicity Type section: Create Load Groups and Study, Create Material by Value, and Create Material by Reference. The action button Create Load Groups and Study generates 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 Create Load Groups and Study button does not generate a parametric study by default. In many situations, a parametric study is needed and the homogenized elasticity matrix D needs to be based on the tag of the parametric solution. To do this, use the given options in the Advanced section of the feature.
•
Use the Free Expansion option with Coefficient of thermal expansion to extract the homogenized coefficient of thermal expansions.
Reference
1. K. Chawla and R. Kiran, “Numerical predictions for the effect of negative Poisson’s ratio on thermoelastic properties of triply periodic minimal surface-based composites,” Results Mater., vol. 14, p. 100273, 2022.
Application Library path: Structural_Mechanics_Module/Material_Models/micromechanical_model_of_a_tpms_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
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file micromechanical_model_of_a_tpms_composite_parameters.txt.
Geometry 1
Next, create a unit cell for a gyroid (TPMS) based composite. This unit cell like many others can be found in the built-in Part Libraries.
Part Libraries
1
In the Geometry toolbar, click  Part Libraries.
2
In the Model Builder window, under Component 1 (comp1) click Geometry 1.
3
In the Part Libraries window, select Design Module > Unit Cells and RVEs > gyroid in the tree.
Gyroid 1 (pi1)
1
Right-click Component 1 (comp1) > Geometry 1 and choose Add to Geometry.
2
In the Settings window for Part Instance, locate the Input Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
lm
L
lm
Cell length
th
th
th
Wall thickness
Use Remove Details to automatically fix small issues in the geometry. This will improve meshing and computation.
Remove Details 1 (rmd1)
1
In the Geometry toolbar, click  Virtual Operations and choose Remove Details.
2
In the Settings window for Remove Details, locate the Parameters section.
3
In the Continuous tangent tolerance text field, type 10.
4
Click  Build Selected.
Form Union (fin)
In the Geometry toolbar, click  Build All.
Definitions
Integration 1 (intop1)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Integration.
2
In the Settings window for Integration, locate the Source Selection section.
3
From the Selection list, choose Gyroid domain (Gyroid 1).
Variables 1
1
In the Model Builder window, right-click Definitions and choose Variables.
2
In the Settings window for Variables, locate the Variables section.
3
In the table, enter the following settings:
Name
Expression
Unit
Description
v_f
intop1(1)/L^3
 
Volume fraction of tpms
E_h
1/solid.cp1.Dinv11
 
Homogenized Young's modulus
nu_h
-E_h*solid.cp1.Dinv12
 
Homogenized Poisson's ratio
G_h
1/solid.cp1.Dinv55
 
Homogenized shear modulus
alpha_h
solid.cp2.alphaXX
 
Homogenized coefficient of thermal expansion
Solid Mechanics (solid)
Linear Elastic Material 1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics (solid) click Linear Elastic Material 1.
Thermal Expansion 1
1
In the Physics toolbar, click  Attributes and choose Thermal Expansion.
2
In the Settings window for Thermal Expansion, locate the Model Input section.
3
From the T list, choose User defined. In the associated text field, type 294.15[K].
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
From the Selection list, choose Pair 1 (Gyroid 1).
4
Right-click Boundary Pair 1 and choose Manual Destination Selection.
5
Locate the Destination Selection section. From the Selection list, choose Pair 1, Destination (Gyroid 1).
Boundary Pair 2
1
Right-click Boundary Pair 1 and choose Duplicate.
2
In the Settings window for Boundary Pair, locate the Boundary Selection section.
3
From the Selection list, choose Pair 2 (Gyroid 1).
4
Locate the Destination Selection section. From the Selection list, choose Pair 2, Destination (Gyroid 1).
Boundary Pair 3
1
Right-click Boundary Pair 2 and choose Duplicate.
2
In the Settings window for Boundary Pair, locate the Boundary Selection section.
3
From the Selection list, choose Pair 3 (Gyroid 1).
4
Locate the Destination Selection section. From the Selection list, choose Pair 3, Destination (Gyroid 1).
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. To create load groups and a study node, click the Create Load Groups and Study button in the section toolbar.
Cell Periodicity for Elastic Properties
To create a parametric study, use the options in the Advanced section of the feature. To see the section, activate the Advanced Physics option from Show button.
1
Click the  Show More Options button in the Model Builder toolbar.
2
In the Show More Options dialog, in the tree, select the checkbox for the node Physics > Advanced Physics Options.
3
Click OK.
4
In the Model Builder window, click Cell Periodicity for Elastic Properties.
5
In the Settings window for Cell Periodicity, click to expand the Advanced section.
6
From the Add parametric sweep list, choose Yes.
7
From the Sweep type list, choose All combinations.
8
Click  Add.
9
In the Parameters table, enter the following settings:
Index
Parameter name
Parameter value list
Parameter unit
1
th
range(4,2,12)
mm
2
nu_f
0.3 -0.3 -0.5 -0.75
1
10
Locate the Periodicity Settings section. Click Create Load Groups and Study in the upper-right corner of the section.
Cell Periodicity for Thermal Properties
1
Right-click Cell Periodicity for Elastic Properties and choose Duplicate.
2
In the Settings window for Cell Periodicity, type Cell Periodicity for Thermal Properties in the Label text field.
3
Locate the Periodicity Settings section. From the Boundary conditions list, choose Free expansion.
4
Locate the Effective Properties section. Select the Compute coefficient of thermal expansion checkbox.
Materials
Material 1: 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 Material 1: Matrix in the Label text field.
3
Locate the Geometric Entity Selection section. From the Selection list, choose Matrix (Gyroid 1).
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
Density
rho
rho_m
kg/m³
Basic
Coefficient of thermal expansion
alpha_iso ; alphaii = alpha_iso, alphaij = 0
alpha_m
1/K
Basic
Material 2: TPMS
1
Right-click Materials and choose Blank Material.
2
In the Settings window for Material, type Material 2: TPMS in the Label text field.
3
Locate the Geometric Entity Selection section. From the Selection list, choose Gyroid domain (Gyroid 1).
4
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
E_f
Pa
Young’s modulus and Poisson’s ratio
Poisson’s ratio
nu
nu_f
1
Young’s modulus and Poisson’s ratio
Density
rho
rho_f
kg/m³
Basic
Coefficient of thermal expansion
alpha_iso ; alphaii = alpha_iso, alphaij = 0
alpha_f
1/K
Basic
Mesh 1
1
In the Model Builder window, under Component 1 (comp1) click Mesh 1.
2
In the Settings window for Mesh, locate the Physics-Controlled Mesh section.
3
From the Element size list, choose Fine.
4
In the table, clear the Use checkbox for Geometric Analysis, Detail Size.
5
Click  Build All.
For this study, disable the thermal expansion node and the cell periodicity feature for thermal expansion.
Cell Periodicity Study for Elastic Properties
1
In the Model Builder window, click Cell Periodicity Study.
2
In the Settings window for Study, type Cell Periodicity Study for Elastic Properties in the Label text field.
Step 1: Stationary
1
In the Model Builder window, expand the Cell Periodicity Study for Elastic Properties node, then click Step 1: Stationary.
2
In the Settings window for Stationary, 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 (solid) > Linear Elastic Material 1 > Thermal Expansion 1.
5
Right-click and choose Disable.
6
In the tree, select Component 1 (comp1) > Solid Mechanics (solid) > Cell Periodicity for Thermal Properties.
7
Right-click and choose Disable.
Solution (solidcp1sol)
1
In the Model Builder window, right-click Solver Configurations and choose Show Default Solver.
The iterative solver is lean on memory usage. Enable the default iterative solver.
2
In the Model Builder window, expand the Solution (solidcp1sol) node.
3
In the Model Builder window, expand the Cell Periodicity Study for Elastic Properties > Solver Configurations > Solution (solidcp1sol) > Stationary Solver 1 node.
4
Right-click Suggested Iterative Solver (solid) and choose Enable.
5
In the Study toolbar, click  Compute.
Add a separate study to compute the homogeneous thermal properties. For this study, disable the cell periodicity feature for elastic properties.
Add Study
1
In the Home toolbar, click  Add Study to open the Add Study window.
2
Go to the Add Study window.
3
Find the Studies subsection. In the Select Study tree, select General Studies > Stationary.
4
Right-click and choose Add Study.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Cell Periodicity Study for Thermal Properties
In the Settings window for Study, type Cell Periodicity Study for Thermal Properties in the Label text field.
Parametric Sweep
1
In the Study toolbar, click  Parametric Sweep.
This study computes the homogenized thermal properties for varying volume fraction and Poisson’s ratio. Therefore, use a parametric sweep for the parameter th along with nu_f.
2
In the Settings window for Parametric Sweep, locate the Study Settings section.
3
From the Sweep type list, choose All combinations.
4
Click  Add.
5
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
th (Wall thickness)
range(4,2,12)
mm
6
Click  Add.
7
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
nu_f (Poisson’s ratio, TPMS)
0.3 -0.3 -0.5 -0.75
1
Step 1: Stationary
1
In the Model Builder window, click Step 1: Stationary.
2
In the Settings window for Stationary, 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 (solid) > Cell Periodicity for Elastic Properties.
5
Right-click and choose Disable.
6
In the Study toolbar, click  Compute.
Results
Stress (solid)
1
In the Model Builder window, under Results click Stress (solid).
2
In the Settings window for 3D Plot Group, locate the Data section.
3
From the Parameter value (th (mm)) list, choose 4.
4
From the Load case list, choose Load case 1.
5
From the Parameter value (nu_f) list, choose 0.3.
6
In the Stress (solid) toolbar, click  Plot.
Stress (solid) 1
1
In the Model Builder window, click Stress (solid) 1.
2
In the Settings window for 3D Plot Group, locate the Data section.
3
From the Parameter value (th (mm)) list, choose 4.
4
From the Parameter value (nu_f) list, choose 0.3.
5
In the Stress (solid) 1 toolbar, click  Plot.
Homogenized Young’s Modulus vs. TPMS Volume Fraction
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Homogenized Young's Modulus vs. TPMS Volume Fraction in the Label text field.
3
Locate the Data section. From the Dataset list, choose Cell Periodicity Study for Elastic Properties/Solution 2 (solidcp1solp).
4
From the Parameter selection (Load case) list, choose First.
5
Click to expand the Title section. From the Title type list, choose Label.
6
Locate the Plot Settings section.
7
Select the x-axis label checkbox. In the associated text field, type v<sub>f</sub>.
8
Select the y-axis label checkbox. In the associated text field, type E<sub>h</sub>/E<sub>m</sub>.
9
Locate the Legend section. From the Position list, choose Upper left.
Global 1
1
Right-click Homogenized Young’s Modulus vs. TPMS Volume Fraction 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
E_h/E_m
1
 
4
Locate the x-Axis Data section. From the Axis source data list, choose th.
5
From the Parameter list, choose Expression.
6
In the Expression text field, type v_f.
7
Click to expand the Coloring and Style section. Find the Line markers subsection. From the Marker list, choose Cycle.
8
From the Positioning list, choose Interpolated.
9
Click to expand the Legends section. From the Legends list, choose Manual.
10
In the table, enter the following settings:
Legends
\nu<sub>f</sub>= 0.3
\nu<sub>f</sub>= -0.3
\nu<sub>f</sub>= -0.5
\nu<sub>f</sub>= -0.75
11
In the Homogenized Young’s Modulus vs. TPMS Volume Fraction toolbar, click  Plot.
Homogenized Poisson’s Ratio vs. TPMS Volume Fraction
1
In the Model Builder window, right-click Homogenized Young’s Modulus vs. TPMS Volume Fraction and choose Duplicate.
2
In the Settings window for 1D Plot Group, type Homogenized Poisson's Ratio vs. TPMS Volume Fraction in the Label text field.
3
Locate the Plot Settings section. In the y-axis label text field, type \nu<sub>h</sub>.
4
Locate the Legend section. From the Position list, choose Lower left.
Global 1
1
In the Model Builder window, expand the Homogenized Poisson’s Ratio vs. TPMS Volume Fraction node, then click Global 1.
2
In the Settings window for Global, locate the y-Axis Data section.
3
In the table, enter the following settings:
Expression
Unit
Description
nu_h
1
 
4
In the Homogenized Poisson’s Ratio vs. TPMS Volume Fraction toolbar, click  Plot.
Homogenized Shear Modulus vs. TPMS Volume Fraction
1
In the Model Builder window, right-click Homogenized Young’s Modulus vs. TPMS Volume Fraction and choose Duplicate.
2
In the Settings window for 1D Plot Group, type Homogenized Shear Modulus vs. TPMS Volume Fraction in the Label text field.
3
Locate the Plot Settings section. In the y-axis label text field, type G<sub>h</sub>/G<sub>m</sub>.
Global 1
1
In the Model Builder window, expand the Homogenized Shear Modulus vs. TPMS Volume Fraction node, then click Global 1.
2
In the Settings window for Global, locate the y-Axis Data section.
3
In the table, enter the following settings:
Expression
Unit
Description
G_h/G_m
1
 
4
In the Homogenized Shear Modulus vs. TPMS Volume Fraction toolbar, click  Plot.
Homogenized Coefficient of Thermal Expansion vs. TPMS Volume Fraction
1
In the Model Builder window, right-click Homogenized Young’s Modulus vs. TPMS Volume Fraction and choose Duplicate.
2
In the Settings window for 1D Plot Group, type Homogenized Coefficient of Thermal Expansion vs. TPMS Volume Fraction in the Label text field.
3
Locate the Data section. From the Dataset list, choose None.
4
Locate the Plot Settings section. In the y-axis label text field, type \alpha<sub>h</sub>/\alpha<sub>m</sub>.
5
Locate the Legend section. From the Position list, choose Upper right.
Global 1
1
In the Model Builder window, expand the Homogenized Coefficient of Thermal Expansion vs. TPMS Volume Fraction node, then click Global 1.
2
In the Settings window for Global, locate the y-Axis Data section.
3
In the table, enter the following settings:
Expression
Unit
Description
alpha_h/alpha_m
 
 
Homogenized Coefficient of Thermal Expansion vs. TPMS Volume Fraction
1
In the Model Builder window, click Homogenized Coefficient of Thermal Expansion vs. TPMS Volume Fraction.
2
In the Settings window for 1D Plot Group, locate the Data section.
3
From the Dataset list, choose Cell Periodicity Study for Thermal Properties/Parametric Solutions 1 (sol22).
Global 1
1
In the Model Builder window, click Global 1.
2
In the Settings window for Global, locate the x-Axis Data section.
3
From the Axis source data list, choose th.
4
In the Homogenized Coefficient of Thermal Expansion vs. TPMS Volume Fraction toolbar, click  Plot.