Products: ABAQUS/Standard ABAQUS/CAE
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).
The electrical response of a piezoelectric material is assumed to be made up of piezoelectric and dielectric effects:
is the electrical potential,
is the component of the electric flux vector (also known as the electric displacement) in the ith material direction,
is the piezoelectric stress coupling,
is a small-strain component,
is the material's dielectric matrix for a fully constrained material, and
is the gradient of the electrical potential along the ith material direction, .
Piezoelectric analysis can be carried out with the following procedures:
Initial conditions of piezoelectric quantities cannot be specified. See Initial conditions, Section 27.2.1, for a description of the initial conditions that can be applied in static or dynamic procedures.
The electric potential at a node (degree of freedom 9) can be prescribed using a boundary condition (see Boundary conditions, Section 27.3.1). 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, Section 27.3.1.
Boundary conditions can be prescribed as functions of time by referring to amplitude curves (Amplitude curves, Section 27.1.2).
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.
Both mechanical and electrical loads can be applied in a piezoelectric analysis.
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 27.4.2.
Electrical charge is the conjugate to electrical potential at a node. Concentrated electric charge can be prescribed at nodes (or node sets). Distributed electric charge can be defined on element faces or surfaces.
Concentrated electric charge is applied to degree of freedom 9.
|Input File Usage:|
*CECHARGE node number or node set name, , electric charge magnitude
Load module: Create Load: choose Electrical for the Category and Concentrated charge for the Types for Selected Step
You can specify distributed surface charges (on element faces) or body charges (charge per unit volume). For element-based surface charges you must identify the face of the element upon which the charge in prescribed in the charge label. The distributed charge types available depend on the element type. Part VI, Elements,” lists the distributed charges that are available for particular elements.
|Input File Usage:|
*DECHARGE element number or element set name, charge label, charge magnitude
Load module: Create Load: choose Electrical for the Category and Body charge for the Types for Selected Step
Distributed surface charges in ABAQUS/CAE are always specified as surface-based loads (see below).
When you specify distributed electric charge on a surface, the element-based surface (see Defining element-based surfaces, Section 2.3.2) contains the element and face information. You must specify the surface name, the electric charge label, and the electric charge magnitude.
|Input File Usage:|
*DSECHARGE surface name, ES, charge magnitude
Load module: Create Load: choose Electrical for the Category and Surface charge for the Types for Selected Step
Electrical loads can be added, modified, or removed as described in Applying loads: overview, Section 27.4.1.
The magnitude of a concentrated or a distributed electric charge can be controlled by referring to an amplitude curve (see Amplitude curves, Section 27.1.2). If different magnitude variations are needed for different charges, the charge definitions can be repeated, with each referring to its own amplitude curve.
In the direct-solution steady-state dynamics procedure, electric charges are given in terms of their real and imaginary components.
Load module: Create Load: choose Electrical for the Category and Concentrated charge, Surface charge, or Body charge for the Types for Selected Step: Magnitude: real component + imaginary componenti
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.
The following predefined fields can be specified in a piezoelectric analysis, as described in Predefined fields, Section 27.6.1:
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-variable-dependent material properties, if any.
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 20.6.2. 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 17.2.1).
Piezoelectric elements must be used in a piezoelectric analysis (see Choosing the appropriate element for an analysis type, Section 21.1.3). 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.
The following output variables are applicable to the electrical solution in a piezoelectric analysis:
Electrostatic energy density.
Magnitude and components of the electrical potential gradient vector, .
Magnitude of the electrical potential gradient vector.
Component n of the electrical potential gradient vector (n=1, 2, 3).
Magnitude and components of the electrical flux (displacement) vector, .
Magnitude of the electrical flux (displacement) vector.
Component n of the electrical flux (displacement) vector (n=1, 2, 3).
Values of distributed electrical charges.
Total electrostatic energy in the element, .
Electrical potential degree of freedom at a node.
Reactive electrical nodal charge (conjugate to prescribed electrical potential).
Concentrated electrical nodal charge.
*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