PDF
Piezoelectric Shear-Actuated Beam
Introduction
This example performs a static analysis on a piezoelectric actuator based on the movement of a cantilever beam, using the Piezoelectricity predefined multiphysics interface. Inspired by work done by V. Piefort (Ref. 1) and A. Benjeddou (Ref. 2), it models a sandwich beam using the shear mode of the piezoelectric material to deflect the tip.
Model Definition
Geometry
The model consists of a 100-mm long sandwiched cantilever beam (Figure 1).
Figure 1: The shear bender geometry. Note that a piezoceramic material replaces part of the foam core.
This beam is composed of a 2-mm thick flexible foam core sandwiched by two 8-mm thick aluminum layers. Furthermore, the device replaces part of the foam core with a 10-mm long piezoceramic actuator that is positioned between x = 55 mm and x = 65 mm. The cantilever beam is oriented along the global x-axis.
Boundary Conditions
•
Solid Mechanics: the cantilever beam is fixed at its surfaces at x = 0; all other surfaces are free.
•
Electrostatics: The system applies a 20 V potential difference between the top and bottom surfaces of the piezoceramic domain (Figure 2). This gives rise to an electric field perpendicular to the poling direction (x direction) and thus induces a transverse shear strain.
Figure 2: Applied voltage through the piezoelectric material.
Material Properties
The following table lists the material properties for the aluminum layers and the foam core:
Property
Aluminum
Foam
Piezoceramic
 E
70 GPa
35.3 MPa
-
 ν
0.35
0.383
-
 ρ
2700 kg/m3
32 kg/m3
7500 kg/m3
Aluminum is available as a predefined material, whereas you must define the foam material manually.
The piezoceramic material in the actuator, PZT-5H, is already defined in the material library. Thus, you do not need to enter the components of the elasticity matrix, cE, the piezoelectric coupling matrix, e, or the relative permittivity matrix, εrS.
Results
The shear deformation of the piezoceramic core layer and the flexible foam layer induce a bending action. Figure 3 shows the resulting tip deflection. The model calculates this deflection as 83 nm, a result that agrees well with those of Ref. 1 and Ref. 2.
Figure 3: Tip deflection with the piezoceramic positioned at x = 60 mm.
Notes About the COMSOL Implementation
The matrix components for the piezoelectric material properties refer to a coordinate system, where the poling direction is the z direction. Because the poling direction of the piezoceramic actuator in this model is aligned with the x-axis, you need to use a local coordinate system in the material settings to rotate the piezoceramic material.
More specifically, you define a local coordinate system that is rotated 90 degrees about the global y-axis. Then, you use this coordinate system in the piezoelectric material settings to rotate the material so that the polarization direction is aligned with the x-axis (Figure 4).
Figure 4: Definition of local coordinate system to define the piezoelectric orientation. The material is poled along the local x3 direction (blue arrow).
References
1. V. Piefort, Finite Element Modelling of Piezoelectric Active Structures, PhD thesis, Université Libre de Bruxelles, Belgium, Dept. Mechanical Engineering and Robotics, 2001.
2. A. Benjeddou, M.A. Trindade, and R. Ohayon, A Unified Beam Finite Element Model for Extension and Shear Piezoelectric Actuation Mechanisms, CNAM (Paris, France), Structural Mechanics and Coupled Systems Laboratory, 1997.
Application Library path: Structural_Mechanics_Module/Piezoelectric_Effects/shear_bender
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 > Electromagnetics–Structure Interaction > Piezoelectricity > Piezoelectricity, Solid.
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies > Stationary.
6
Click  Done.
Geometry 1
1
In the Model Builder window, under Component 1 (comp1) click Geometry 1.
2
In the Settings window for Geometry, locate the Units section.
3
From the Length unit list, choose mm.
Block 1 (blk1)
1
In the Geometry toolbar, click  Block.
2
In the Settings window for Block, locate the Size and Shape section.
3
In the Width text field, type 100.
4
In the Depth text field, type 30.
5
In the Height text field, type 18.
6
Click  Build Selected.
Block 2 (blk2)
1
In the Geometry toolbar, click  Block.
2
In the Settings window for Block, locate the Size and Shape section.
3
In the Width text field, type 100.
4
In the Depth text field, type 30.
5
In the Height text field, type 2.
6
Locate the Position section. In the z text field, type 8.
7
Click to expand the Layers section. Find the Layer position subsection. Select the Left checkbox.
8
Clear the Bottom checkbox.
9
In the table, enter the following settings:
Layer name
Thickness (mm)
Layer 1
55
Layer 2
10
10
Click  Build All Objects.
11
Click the  Zoom Extents button in the Graphics toolbar.
The model geometry is now complete.
12
Click the  Transparency button in the Graphics toolbar.
The geometry in the Graphics window should now look like that in Figure 1.
13
Click the  Transparency button in the Graphics toolbar.
Definitions
Define a coordinate system whose third axis is aligned with the global x-axis, that is, the polarization direction of the piezoceramic material. Choose the second axis to be parallel to the global y-axis.
Base Vector System 2 (sys2)
1
In the Definitions toolbar, click  Coordinate Systems and choose Base Vector System.
2
In the Settings window for Base Vector System, locate the Base Vectors section.
3
In the table, enter the following settings:
 
x
y
z
x1
0
0
-1
x3
1
0
0
Leave the other components at their default values. You will use this coordinate system in the piezoelectric material settings.
4
Find the Simplifications subsection. Select the Assume orthonormal checkbox.
Electrostatics (es)
1
In the Model Builder window, under Component 1 (comp1) click Electrostatics (es).
2
In the Settings window for Electrostatics, locate the Domain Selection section.
3
Click  Clear Selection.
4
Select Domain 4 only.
Solid Mechanics (solid)
Piezoelectric Material 1
1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics (solid) click Piezoelectric Material 1.
2
In the Settings window for Piezoelectric Material, locate the Domain Selection section.
3
Click  Clear Selection.
4
Select Domain 4 only.
5
Locate the Coordinate System Selection section. From the Coordinate system list, choose Base Vector System 2 (sys2).
Materials
For the aluminum layers, use a library material.
Add Material
1
In the Materials toolbar, click  Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select MEMS > Metals > Al - Aluminum.
4
Click the Add to Component button in the window toolbar.
Materials
Al - Aluminum (mat1)
1
In the Settings window for Material, locate the Geometric Entity Selection section.
2
Click  Clear Selection.
3
Select Domains 1 and 3 only.
For the foam core, specify the material properties by hand.
Foam
1
In the Model Builder window, right-click Materials and choose Blank Material.
2
In the Settings window for Material, type Foam in the Label text field.
3
Select Domains 2 and 5 only.
4
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
35.3[MPa]
Pa
Young’s modulus and Poisson’s ratio
Poisson’s ratio
nu
0.383
1
Young’s modulus and Poisson’s ratio
Density
rho
32
kg/m³
Basic
The piezoceramic PZT-5H is available as a predefined material.
Add Material
1
Go to the Add Material window.
2
In the tree, select Piezoelectric > Lead Zirconate Titanate (PZT-5H).
3
Click the Add to Component button in the window toolbar.
Add Material
1
From the Home menu, choose Add Material.
2
Select Domain 4 only.
Solid Mechanics (solid)
Fixed Constraint 1
1
In the Model Builder window, expand the Component 1 (comp1) > Materials > Foam (mat2) node.
2
Right-click Component 1 (comp1) > Solid Mechanics (solid) and choose Fixed Constraint.
3
Select Boundaries 1, 4, and 7 only.
Electrostatics (es)
In the Model Builder window, under Component 1 (comp1) click Electrostatics (es).
Electric Potential 1
1
In the Physics toolbar, click  Boundaries and choose Electric Potential.
2
Select Boundary 16 only.
3
In the Settings window for Electric Potential, locate the Electric Potential section.
4
In the V0 text field, type 20.
Ground 1
1
In the Physics toolbar, click  Boundaries and choose Ground.
2
Select Boundary 17 only.
Mesh 1
Swept 1
1
In the Mesh toolbar, click  Swept.
2
In the Settings window for Swept, click to expand the Source Faces section.
3
Select Boundaries 9, 17, and 22 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 2.
4
Click  Build All.
5
Click the  Zoom Extents button in the Graphics toolbar.
The mesh consists of 198 hexahedral elements.
6
In the Model Builder window, click Mesh 1.
Study 1
In the Study toolbar, click  Compute.
Results
Displacement (solid)
Replace the default stress plot by displacement to reproduce the plot shown in Figure 3.
1
In the Settings window for 3D Plot Group, type Displacement (solid) in the Label text field.
Volume 1
1
In the Model Builder window, expand the Displacement (solid) node, then click Volume 1.
2
In the Settings window for Volume, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Solid Mechanics > Displacement > Displacement field - m > w - Displacement field, Z-component.
3
Locate the Expression section. From the Unit list, choose nm.
4
In the Displacement (solid) toolbar, click  Plot.
5
Click the  Go to Default View button in the Graphics toolbar.
Electric Potential (es)
In the Model Builder window, expand the Electric Potential (es) node.
Multislice 1, Streamline Multislice 1
1
In the Model Builder window, under Results > Electric Potential (es), Ctrl-click to select Multislice 1 and Streamline Multislice 1.
2
Right-click and choose Delete.
Surface 1
1
Right-click Electric Potential (es) and choose Surface.
2
In the Settings window for Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Electrostatics > Electric > V - Electric potential - V.
3
In the Electric Potential (es) toolbar, click  Plot.
Zoom in to find a plot similar to Figure 2.
4
Click the  Zoom In button in the Graphics toolbar.
5
Click the  Zoom Extents button in the Graphics toolbar.
Show the base vector that defines the polarization of the piezoelectric material, shown on Figure 4.
PZT coordinate system
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type PZT coordinate system in the Label text field.
Coordinate System Volume 1
1
In the PZT coordinate system toolbar, click  More Plots and choose Coordinate System Volume.
2
In the Settings window for Coordinate System Volume, locate the Coordinate System section.
3
From the Coordinate system list, choose Base Vector System 2 (sys2).
4
Locate the Positioning section. Find the x grid points subsection. From the Entry method list, choose Coordinates.
5
In the Coordinates text field, type 60.
6
Find the y grid points subsection. In the Points text field, type 1.
7
Find the z grid points subsection. In the Points text field, type 1.
8
In the PZT coordinate system toolbar, click  Plot.