emtgen#

Elements.emtgen(ncomp='', ecomp='', pncomp='', dof='', gap='', gapmin='', fkn='', epzero='', smethod='', **kwargs)#

Generates a set of TRANS126 elements.

Mechanical APDL Command: EMTGEN

Parameters:
ncompstr

Component name of the surface nodes of a structure which attach to the TRANS126 elements. The component name must be 32 characters or less, and you must enclose the name in single quotes in the emtgen command line.

ecompstr

Component name of the TRANS126 elements generated. The component name must be 32 characters or less, and you must enclose the name in single quotes in the emtgen command line. Defaults to EMTELM.

pncompstr

Component name of the plane nodes generated by the command at an offset ( GAP ) from the surface nodes. The component name must be 32 characters or less, and you must enclose the name in single quotes in the emtgen command line. Defaults to EMTPNO.

dofstr

Active structural degree of freedom (DOF) for TRANS126 elements in the Cartesian coordinate system. You must enclose the DOF label in single quotes:

  • UX - Displacement in X direction.

  • UY - Displacement in Y direction.

  • UZ - Displacement in Z direction.

gapstr

Initial gap distance from the surface nodes to the plane. Be sure to use the correct sign with respect to Ncomp node location.

gapminstr

Minimum gap distance allowed (GAPMIN real constant) for TRANS126 elements. Defaults to the absolute value of ( GAP )*0.05.

fknstr

Contact stiffness factor used as a multiplier for a contact stiffness appropriate for bulk deformation. Defaults to 0.1. A negative value is interpreted as the modulus of elasticity on which the contact stiffness will be based.

epzerostr

Free-space permittivity. Defaults to 8.854e-6 (μMKS units).

smethodstr

Stiffness method for TRANS126 elements (KEYOPT(6) setting). You must enclose the following labels in single quotes:

  • AUGM - Augmented stiffness method (default).

  • FULL - Full stiffness method. This method must be used in a linear perturbation harmonic analysis.

Notes

The emtgen command generates a set of TRANS126 elements between the surface nodes of a moveable structure and a plane of nodes, typically representing a ground plane. The plane of nodes is created by the command at a specified offset ( GAP ). Each element attaches to a surface node and to a corresponding node representing the plane. The generated plane nodes should be constrained appropriately for the analysis.

By default, the created elements use the augmented stiffness method (KEYOPT(6) = 1), which can help convergence. You can change to the full stiffness method (KEYOPT(6) = 0) by setting Smethod = FULL. The full stiffness method is required for a linear perturbation harmonic analysis.

You can use TRANS126 elements for simulating fully coupled electrostatic structural coupling between a MEMS device and a plane, if the gap distance between the device and the plane is small compared to the overall surface area dimensions of the device. This assumption allows for a point- wise closed-form solution of capacitance between the surface nodes and the plane; i.e. CAP = EPZERO2AREA/GAP, where EPZERO if the free-space permittivity, AREA is the area associated with the node, and GAP is the gap between the node and the plane. The area for each node is computed using the ARNODE function. See the get command description for more information on the ARNODE function.

With a distributed set of TRANS126 elements attached directly to the structure and a plane (such as a ground plane), you can perform a full range of coupled electrostatic-structural simulations, including:

  • Static analysis (due to a DC voltage or a mechanical load)

  • Prestressed modal analysis (eigenfrequencies, including frequency-shift effects of a DC bias voltage)

  • Prestressed harmonic analysis (system response to a small-signal AC excitation with a DC bias voltage or mechanical load)

  • Large signal transient analysis (time-transient solution due to an arbitrary time-varying voltage or mechanical excitation)

The TRANS126 element also employs a node-to-node gap feature so you can perform contact-type simulations where the structure contacts a plane (such as a ground plane). The contact stiffness factor, FKN, is used to control contact penetration once contact is initiated. A smaller value provides for easier convergence, but with more penetration.