<!-- source-page: 421 -->

# 6.7.2 PIEZOELECTRIC ANALYSIS

Products: Abaqus/Standard Abaqus/CAE

# References

• “Piezoelectric behavior,” Section 26.5.2   
• “Defining an analysis,” Section 6.1.2   
• “Electromagnetic analysis procedures,” Section 6.7.1   
• “Defining a concentrated charge,” Section 16.9.30 of the Abaqus/CAE User’s Guide, in the HTML version of this guide   
• “Defining a surface charge,” Section 16.9.31 of the Abaqus/CAE User’s Guide, in the HTML version of this guide   
• “Defining a body charge,” Section 16.9.32 of the Abaqus/CAE User’s Guide, in the HTML version of this guide

# Overview

Coupled piezoelectric problems:

• are those in which an electric potential gradient causes straining, while stress causes an electric potential gradient in the material;   
• are solved using an eigenfrequency extraction, modal dynamic, static, dynamic, or steady-state dynamic procedure;   
• require the use of piezoelectric elements and piezoelectric material properties;   
• can be performed for continuum problems in one, two, and three dimensions; and   
• can be used in both linear and nonlinear analysis (however, in nonlinear analysis the piezoelectric part of the constitutive behavior is assumed to be linear).

# Piezoelectric response

The electrical response of a piezoelectric material is assumed to be made up of piezoelectric and dielectric effects:

$$
q _ {i} = e _ {i j k} ^ {\varphi} \varepsilon_ {j k} + D _ {i j} ^ {\varphi (\varepsilon)} E _ {j},
$$

where

$\varphi$ is the electrical potential,   
$q _ { i }$ is the component of the electric flux vector (also known as the electric displacement) in the ith material direction,   
$e _ { i j k } ^ { \varphi }$ is the piezoelectric stress coupling,

<!-- source-page: 422 -->

$\varepsilon _ { i j }$ is a small-strain component,

$D _ { i j } ^ { \varphi ( \varepsilon ) }$ is the material’s dielectric matrix for a fully constrained material, and

$E _ { i }$ is the negative of the gradient of the electrical potential along the ith material direction, $- \partial \varphi / \partial x _ { i }$ .

Defining piezoelectric and dielectric properties is discussed in “Piezoelectric behavior,” Section 26.5.2. The theoretical basis of the piezoelectric analysis capability in Abaqus is defined in “Piezoelectric analysis,” Section 2.10.1 of the Abaqus Theory Guide.

# Procedures available for piezoelectric analysis

Piezoelectric analysis can be carried out with the following procedures:

• “Static stress analysis,” Section 6.2.2   
• “Implicit dynamic analysis using direct integration,” Section 6.3.2   
• “Direct-solution steady-state dynamic analysis,” Section 6.3.4   
• “Natural frequency extraction,” Section 6.3.5   
• “Transient modal dynamic analysis,” Section 6.3.7   
• “Mode-based steady-state dynamic analysis,” Section 6.3.8   
• “Subspace-based steady-state dynamic analysis,” Section 6.3.9

# Initial conditions

Initial conditions of piezoelectric quantities cannot be specified. See “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1, for a description of the initial conditions that can be applied in static or dynamic procedures.

# Boundary conditions

The electric potential at a node (degree of freedom 9) can be prescribed using a boundary condition (see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1). Displacement and rotation degrees of freedom can also be prescribed by using boundary conditions as described in the relevant static and dynamic analysis procedure sections. See “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1.

Boundary conditions can be prescribed as functions of time by referring to amplitude curves (“Amplitude curves,” Section 34.1.2).

In an eigenfrequency extraction step (“Natural frequency extraction,” Section 6.3.5 ) involving piezoelectric elements, the electric potential degree of freedom must be constrained at least at one node to remove singularities from the dielectric part of the element operator.

# Loads

Both mechanical and electrical loads can be applied in a piezoelectric analysis.

<!-- source-page: 423 -->

# Applying mechanical loads

The following types of mechanical loads can be prescribed in a piezoelectric analysis:

• Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 34.4.2.   
• Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 34.4.3.

# Applying electrical loads

The following types of electrical loads can be prescribed, as described in “Electromagnetic loads,” Section 34.4.5:

• Concentrated electric charge.   
• Distributed surface electric charge and body electric charge.

# Loading in mode-based and subspace-based procedures

Electrical charge loads should be used only in conjunction with residual modes in the eigenvalue extraction step, due to the “massless” mode effect. Since the electrical potential degrees of freedom do not have any associated mass, these degrees of freedom are essentially eliminated (similar to Guyan reduction or mass condensation) during the eigenvalue extraction. The residual modes represent the static response corresponding to the electrical charge loads, which will adequately represent the potential degree of freedom in the eigenspace.

# Predefined fields

The following predefined fields can be specified in a piezoelectric analysis, as described in “Predefined fields,” Section 34.6.1:

• Although temperature is not a degree of freedom in piezoelectric elements, nodal temperatures can be specified. The specified temperature affects only temperature-dependent material properties, if any.   
• The values of user-defined field variables can be specified. These values affect only field-variabledependent material properties, if any.

# Material options

The piezoelectric coupling matrix and the dielectric matrix are specified as part of the material definition for piezoelectric materials, as described in “Piezoelectric behavior,” Section 26.5.2. They are relevant only when the material definition is used with coupled piezoelectric elements.

The mechanical behavior of the material can include linear elasticity only (“Linear elastic behavior,” Section 22.2.1).

<!-- source-page: 424 -->

# Elements

Piezoelectric elements must be used in a piezoelectric analysis (see “Choosing the appropriate element for an analysis type,” Section 27.1.3). The electric potential, , is degree of freedom 9 at each node of these elements. In addition, regular stress/displacement elements can be used in parts of the model where piezoelectric effects do not need to be considered.

# Output

The following output variables are applicable to the electrical solution in a piezoelectric analysis:

Element integration point variables:

<table><tr><td>EENER</td><td>Electrostatic energy density.</td></tr><tr><td>EPG</td><td>Magnitude and components of the negative of the electrical potential gradient vector,  $-\partial \varphi/\partial \mathbf{x}$ .</td></tr><tr><td>EPGM</td><td>Magnitude of the electrical potential gradient vector.</td></tr><tr><td>EPGn</td><td>Component  $n$  of the negative of the electrical potential gradient vector ( $n=1, 2, 3$ ).</td></tr><tr><td>EFLX</td><td>Magnitude and components of the electrical flux (displacement) vector,  $\mathbf{q}$ .</td></tr><tr><td>EFLXM</td><td>Magnitude of the electrical flux (displacement) vector.</td></tr><tr><td>EFLXn</td><td>Component  $n$  of the electrical flux (displacement) vector ( $n=1, 2, 3$ ).</td></tr></table>

Whole element variables:

<table><tr><td>CHRGS</td><td>Values of distributed electrical charges.</td></tr><tr><td>ELCTE</td><td>Total electrostatic energy in the element,  $\int_{v} \text{EENER } dv$ .</td></tr></table>

Nodal variables:

<table><tr><td>EPOT</td><td>Electrical potential degree of freedom at a node.</td></tr><tr><td>RCHG</td><td>Reactive electrical nodal charge (conjugate to prescribed electrical potential).</td></tr><tr><td>CECHG</td><td>Concentrated electrical nodal charge.</td></tr></table>

# Limitations

Abaqus does not account for piezoelectric effects in the total energy balance equation, which can lead to an apparent imbalance of the total energy of the model in some situations. For example, if a piezoelectric truss is fixed at one end point and subjected to a potential difference between its two end points, it deforms due to the piezoelectric effect. Subsequently if the truss is held fixed in this deformed configuration and the potential difference removed, strain energy will be generated due to the constraints. This results in an equivalent increase in the total energy of the model.

<!-- source-page: 425 -->

Input file template   
```c
*HEADING
...
*MATERIAL, NAME=matl
*ELASTIC
Data lines to define linear elasticity
*PIEZOELECTRIC
Data lines to define piezoelectric behavior
*DIELECTRIC
Data lines to define dielectric behavior
...
*AMPLITUDE, NAME=name
Data lines to define amplitude curve for defining concentrated electric charge
**
*STEP, (optionally NLGEOM)
*STATIC
** or *DYNAMIC, *FREQUENCY, *MODAL DYNAMIC,
** *STEADY STATE DYNAMICS (, DIRECT or, SUBSPACE PROJECTION)
*BOUNDARY
Data lines to define boundary conditions on electrical potential and displacement (rotation) degrees of freedom
*CECHARGE, AMPLITUDE=name
Data lines to define time-dependent concentrated electric charges
*DECHARGE and/or *DSECHARGE
Data lines to define distributed electric charges
*CLOAD and/or *DLOAD and/or *DSLOAD
Data lines to define mechanical loading
*END STEP 
```

<!-- source-page: 426 -->

<!-- source-page: 427 -->

# 6.7.3 COUPLED THERMAL-ELECTRICAL ANALYSIS

Products: Abaqus/Standard Abaqus/CAE

# References

• “Defining an analysis,” Section 6.1.2   
• “Electromagnetic analysis procedures,” Section 6.7.1   
• “Electrical conductivity,” Section 26.5.1   
• \*COUPLED THERMAL-ELECTRICAL   
• \*JOULE HEAT FRACTION   
• “Specifying a joule heat fraction,” Section 12.10.4 of the Abaqus/CAE User’s Guide, in the HTML version of this guide   
• “Configuring a fully coupled, simultaneous heat transfer and electrical procedure” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Guide, in the HTML version of this guide

# Overview

Coupled thermal-electrical problems:

• are those in which coupling between the electrical potential and temperature fields make it necessary to solve both fields simultaneously;   
• require the use of coupled thermal-electrical elements, although pure heat transfer elements can also be used in the model;   
• can include a specification of the fraction of electrical energy that will be released as heat;   
• can include thermal interactions such as gap radiation, gap conductance, and heat generation between surfaces (see “Thermal contact properties,” Section 37.2.1);   
• can include cavity radiation effects (see “Cavity radiation,” Section 41.1.1);   
• can include electrical interactions such as electrical current flowing across surfaces (see “Electrical contact properties,” Section 37.3.1);   
• allow for transient or steady-state thermal solutions and for steady-state electrical solutions; and   
• can be linear or nonlinear.

# Coupled thermal-electrical analysis

Joule heating arises when the energy dissipated by an electrical current flowing through a conductor is converted into thermal energy. Abaqus/Standard provides a fully coupled thermal-electrical procedure for analyzing this type of problem: the coupled thermal-electrical equations are solved simultaneously for both temperature and electrical potential at the nodes.

<!-- source-page: 428 -->

The capability includes the analysis of the electrical problem, the thermal problem, and the coupling between the two problems. Coupling arises from two sources: temperature-dependent electrical conductivity and internal heat generation, which is a function of the electrical current density. The thermal part of the problem can include heat conduction and heat storage (“Thermal properties: overview,” Section 26.2.1) as well as cavity radiation effects (“Cavity radiation,” Section 41.1.1). Forced convection caused by fluid flowing through the mesh is not considered.

The thermal-electrical equations are unsymmetric; therefore, the unsymmetric solver is invoked automatically if you request coupled thermal-electrical analysis. For problems where coupling between the thermal and electrical solutions is weak or where a pure electrical conduction analysis is required for the entire model, the unsymmetric terms resulting from the interfield coupling may be small or zero. In these problems you can invoke the less costly symmetric storage and solution scheme by solving the thermal and electrical equations separately. The separated technique uses the symmetric solver by default. The thermal-electrical solution schemes are discussed below.

The theoretical basis of coupled thermal-electrical analysis is described in detail in “Coupled thermal-electrical analysis,” Section 2.12.1 of the Abaqus Theory Guide.

# Governing electric field equation

The electric field in a conducting material is governed by Maxwell’s equation of conservation of charge. Assuming steady-state direct current, the equation reduces to

$$
\int_ {S} \mathbf {J} \cdot \mathbf {n} d S = \int_ {V} r _ {c} d V,
$$

where V is any control volume whose surface is S, is the outward normal to ${ \cal S } , { \bf J }$ is the electrical current density (current per unit area), and $r _ { c }$ is the internal volumetric current source per unit volume.

The flow of electrical current is described by Ohm’s law:

$$
\mathbf {J} = \pmb {\sigma} ^ {E} \cdot \mathbf {E} = - \pmb {\sigma} ^ {E} \cdot \frac {\partial \varphi}{\partial \mathbf {x}},
$$

where

$\mathbf { E } ( \mathbf { x } )$ is the electrical field intensity, defined as the negative of the gradient of the electrical potential ${ \bf E } = - \partial \varphi / \partial { \bf x }$ ,

$\varphi$ is the electrical potential,

$\sigma ^ { E } ( \theta , f ^ { \alpha } )$ is the electrical conductivity matrix,

$\theta$ is the temperature, and

$f ^ { \alpha } , \alpha = 1 , 2 . .$ are predefined field variables.

Using Ohm’s law in the conservation equation, written in variational form, provides the governing equation of the finite element model:

$$
\int_ {V} \frac {\partial \delta \varphi}{\partial \mathbf {x}} \cdot \pmb {\sigma} ^ {E} \cdot \frac {\partial \varphi}{\partial \mathbf {x}} d V = \int_ {S} \delta \varphi J d S + \int_ {V} \delta \varphi r _ {c} d V,
$$

<!-- source-page: 429 -->

where ${ \boldsymbol { J } } ~ { \stackrel { \mathrm { d e f } } { = } } ~ - \mathbf { J } \cdot \mathbf { n }$ is the current density entering the control volume across $\pmb { S } .$

# Defining the electrical conductivity

The electrical conductivity, $\sigma ^ { E }$ , can be isotropic, orthotropic, or fully anisotropic (see “Electrical conductivity,” Section 26.5.1). Ohm’s law assumes that the electrical conductivity is independent of the electrical field, . The coupled thermal-electrical problem is nonlinear when the electrical conductivity depends on temperature.

# Specifying the amount of thermal energy generated due to electrical current

Joule’s law describes the rate of electrical energy, $P _ { e c } ,$ dissipated by current flowing through a conductor as

$$
P _ {e c} = \mathbf {J} \cdot \mathbf {E} = \frac {\partial \varphi}{\partial \mathbf {x}} \cdot \pmb {\sigma} ^ {E} \cdot \frac {\partial \varphi}{\partial \mathbf {x}}.
$$

The amount of this energy released as internal heat within the body is $\eta _ { v } { \cal P } _ { e c } ,$ , where $\eta _ { v }$ is an energy conversion factor. You specify $\eta _ { v }$ in the material definition. It is assumed that all the electrical energy is converted into heat $( \eta _ { v } = 1 . 0 )$ if you do not include the joule heat fraction in the material description. The fraction given can include a unit conversion factor, if required.

Input File Usage: \*JOULE HEAT FRACTION

Abaqus/CAE Usage: Property module: material editor: Thermal→Joule Heat Fraction

# Steady-state analysis

Steady-state analysis provides the steady-state solution directly. Steady-state thermal analysis means that the internal energy term (the specific heat term) in the governing heat transfer equation is omitted. Only direct current is considered in the electrical problem, and it is assumed that the system has negligible capacitance. (Electrical transient effects are so rapid that they can be neglected.)

Input File Usage: \*COUPLED THERMAL-ELECTRICAL, STEADY STATE

Abaqus/CAE Usage: Step module: Create Step: General: Coupled thermal-electric: Basic: Response: Steady state

# Assigning a “time” scale to the analysis

A steady-state analysis has no intrinsic physically meaningful time scale. Nevertheless, you can assign a “time” scale to the analysis step, which is often convenient for output identification and for specifying prescribed temperatures, electrical potential, and fluxes (heat flux and current density) with varying magnitudes. Thus, when steady-state analysis is chosen, you specify a “time” period and “time” incrementation parameters for the step; Abaqus/Standard then increments through the step accordingly.

Any fluxes or boundary condition changes to be applied during a steady-state step should be given using appropriate amplitude references to specify their “time” variations (“Amplitude curves,” Section 34.1.2). If fluxes and boundary conditions are specified for the step without amplitude

<!-- source-page: 430 -->

references, they are assumed to change linearly with “time” during the step—from their magnitudes at the end of the previous step (or zero, if this is the beginning of the analysis) to their newly specified magnitudes at the end of this step (see “Defining an analysis,” Section 6.1.2).

# Transient analysis

Alternatively, the thermal portion of the coupled thermal-electrical problem can be considered transient. As in steady-state analysis, electrical transient effects are neglected. See “Uncoupled heat transfer analysis,” Section 6.5.2, for a more detailed description of the heat transfer capability in Abaqus/Standard.

Input File Usage: \*COUPLED THERMAL-ELECTRICAL

Abaqus/CAE Usage: Step module: Create Step: General: Coupled thermal-electric: Basic: Response: Transient

# Time incrementation

Time integration in the transient heat transfer problem is done with the same backward Euler method used in uncoupled heat transfer analysis. This method is unconditionally stable for linear problems. You can specify the time increments directly, or Abaqus can select them automatically based on a userprescribed maximum nodal temperature change in an increment. Automatic time incrementation is generally preferred.

# Automatic incrementation

The time increment size can be selected automatically based on a user-prescribed maximum allowable nodal temperature change in an increment, $\Delta \theta _ { m a x }$ . Abaqus/Standard will restrict the time increments to ensure that these values are not exceeded at any node (except nodes with boundary conditions) during any increment of the analysis (see “Time integration accuracy in transient problems,” Section 7.2.4).

Input File Usage: \*COUPLED THERMAL-ELECTRICAL, DELTMX=

Abaqus/CAE Usage: Step module: Create Step: General: Coupled thermal-electric: Basic: Response: Transient; Incrementation: Type: Automatic: Max. allowable temperature change per increment: $\Delta \theta _ { m a x }$

# Fixed incrementation

If you select fixed time incrementation and do not specify $\Delta \theta _ { m a x }$ , fixed time increments equal to the user-specified initial time increment, $\Delta t _ { 0 }$ , will then be used throughout the analysis.

Input File Usage: \*COUPLED THERMAL-ELECTRICAL $\Delta t _ { 0 }$

Abaqus/CAE Usage: Step module: Create Step: General: Coupled thermal-electric: Basic: Response: Transient; Incrementation: Type: Fixed: Increment size: $\Delta t _ { 0 }$