17.6.5.6. EM (Electro-Mechanical) Transducer

Using the EM Transducer boundary condition, you can model simple Micro-Electro-Mechanical Systems (MEMS) devices.

This page includes the following sections:

Analysis Types

EM Transducer is available for the following analysis types:

Dimensional Types

The supported dimensional types for the EM Transducer boundary condition include:

  • 3D Simulation. Node-based Named Selections only support face node selection.

  • 2D Simulation. Node-based Named Selections only support edge node selection.

Geometry Types

The supported geometry types for the EM Transducer boundary condition include:

  • Solid

  • Surface/Shell

Topology Selection Options

The EM Transducer boundary condition is scoped via node-based Named Selections only. For more information, see the Specifying Named Selections by Direct Node Selection Help section.

Define By Options

The loading for this boundary condition is always defined as a Voltage Difference.

Magnitude Options

The supported Magnitude options for EM Transducer include the following:

  • Constant. This value can be Parameterized.

  • Tabular (Time Varying). This value cannot be Parameterized.

  • Tabular (Step Varying): Supported for Static Structural only. This value cannot be Parameterized.

  • Function (Time Varying). This value cannot be Parameterized.

Applying an EM Transducer Boundary Condition

To apply an EM Transducer:

  1. On the Environment Context tab, click Direct FE > EM Transducer. Alternatively, right-click the Environment tree object or in the Geometry window and select Insert > EM Transducer.

  2. Enter a Voltage Difference value.

  3. Specify a GAP Direction, either X, Y, or Z based on the default Nodal Coordinate System or a user-defined nodal coordinate system.

  4. Enter Initial Gap and Minimal Gap values.

Details Pane Properties

The selections available in the Details pane are described below.

CategoryProperty/Options/Description
Scope

Scoping Method: Read-only field that displays scoping method - Named Selection.

Named Selection: Drop-down list of available node-based Named Selections.

Definition

Type: Read-only field that describes the node-based object - EM Transducer.

Voltage Difference: Input field for Voltage value.

Stiffness Method: Property options include Program Controlled (default), Augmented, and Full. The application determines which setting, Full or Augmented, the Program Controlled option uses based upon the configuration of your system or systems. The Program Controlled option selects the Full setting when your Static Structural analysis includes a downstream pre-stressed Harmonic Response or Modal analysis and the Augmented setting for all other cases. The Full setting is required in order to obtain accurate results when your Static Structural analysis includes a downstream pre-stressed Harmonic Response system.

These settings are based on a system’s stiffness in an electro-mechanical scenario. The stiffness of such systems consists of structural stiffness and electrostatic stiffness. Because forces increase when a spring is stretched, structural stiffness has a positive value. However, given a parallel plate capacitor, the attraction force between the plates decreases with an increasing gap, resulting in a negative electrostatic stiffness. As a result, you can be presented with a negative system stiffness and the analysis can experience convergence problems near unstable solutions.
When the Augmented option is specified for the Stiffness Method, the application sets the electrostatic stiffness to zero, ensuring that the analysis has a positive system stiffness, in order to address convergence issues. In addition, once convergence is reached, the application automatically re-establishes electrostatic stiffness for subsequent analyses.

Note:  For additional technical information about the operation of the Stiffness Method, see the TRANS126 Element section in the Mechanical APDL Element Reference and the EMTGEN command in the Mechanical APDL Command Reference.

Suppressed: Include (No - default) or exclude (Yes) the boundary condition.

Voltage Surface Location

Coordinate System: Read-only field that displays the coordinate system - Nodal Coordinate System.

GAP Direction: Specify the structural DOF used, X, Y, or Z based on the Nodal Coordinate System. This is used with the Volt DOF.

Initial Gap: Input field for initial range of motion (in GAP Direction). Can be Parameterized.

Minimal Gap: Input field for minimal range of motion (in GAP Direction). Can be Parameterized.

Function [1]

Unit System: Read-only field displaying the unit of measure associated with the Voltage.

Angular Measure: Read-only field displaying the unit of measure for the voltage’s angle.

Graph Controls [1]

Number of Segments: The function is graphed with a default value of 200 line segments. You can change this value to better visualize the function.

  1. This category displays only when Voltage Difference is specified as a Function.

Mechanical APDL References and Notes

This boundary condition uses the EMTGEN command to generate a set of TRANS126 elements between the surface nodes of a moveable structure and a plane of nodes, typically representing a ground plane.

Note:  The newly created (by EMTGEN command) ground plane nodes (of TRANS126 elements) are assumed to be fixed.

API Reference

For specific scripting information, see the EM (Electro-Mechanical) Transducer section of the ACT API Reference Guide.