EAGLE Help

PAD


Function
Adds pads to a package.

Syntax
PAD *..
PAD pad_diameter pad_shape 'name' *..

Mouse
Right button rotates elongated pads.

See also SMD, CHANGE, DISPLAY, SET, NAME, VIA, Design Rules

The PAD command is used to add pads to a package. When the PAD command is active, a pad symbol is attached to the cursor and can be moved around the screen. Pressing the left mouse button places the pad at the current position and attaches a new pad symbol to the cursor. Entering a number changes the diameter of the pad (in the actual unit). Pad diameters can be up to 0.51602 inch (13.1 mm).

Example


PAD 0.06 *
The pad will have a diameter of 0.06 inch, provided the actual unit is "inch". This diameter remains as a presetting for succeeding operations.

Pad Shapes

A pad can have one of the following shapes (pad_shape):

Square
Round
Octagon octagonal
XLongOct elongated in x direction
YLongOct elongated in y direction

The two sides of elongated pads have a fixed ratio of 2:1. The smaller one has to be entered as the parameter when such a pad is defined.

The pad shape or diameter can be selected while the PAD command is active, or it can be changed with the CHANGE command, e.g.:


CHANGE SHAPE OCTAGON *
The drill size may also be changed using the CHANGE command. The existing values then remain in use for successive pads.

Because displaying different pad shapes and drill holes in their real size slows down the screen refresh, EAGLE lets you change between real and fast display mode by the use of the SET commands:


SET DISPLAY_MODE REAL | NODRILL;
Note that the actual shape and diameter of a pad will be determined by the Design Rules of the board the part is used in.

Pad Names

Pad names are generated by the program automatically and can be changed with the NAME command. The name can also be defined in the PAD command. Pad name display can be turned on or off by means of the commands:


SET PAD_NAMES ON | OFF;
This change will be visible after the next screen refresh.

Single Pads

Single pads in boards can be used only by defining a package with one pad. Via-holes can be placed in board but they don't have an element name and therefore don't show up in the netlist.

Alter Package

It is not possible to add or delete pads in packages which are already used by a device, because this would change the pin/pad allocation defined with the CONNECT command.


Index Copyright © 2002 CadSoft Computer GmbH