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 a pad at the current position. 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).
The orientation (see description in ADD) may be any angle in the range R0...R359.9. The S and M flags can't be used here.
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.
A pad can have one of the following shapes:
|Offset||elongated with offset|
With elongated pads, the given diameter defines the smaller side of the pad. The ratio between the two sides of elongated pads is given by the parameter Shapes/Elongation in the Design Rules of the board (default is 100%, which results in a ratio of 2:1).
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 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.
The following flags can be used to control the appearance of a pad:
|NOSTOP||don't generate solder stop mask|
|NOTHERMALS||don't generate thermals|
|FIRST||this is the "first" pad (which may be drawn with a special shape)|
By default a pad automatically generates solder stop mask and thermals as necessary.
However, in special cases it may be desirable to have particular pads not do this.
The above NO... flags can be used to suppress these features.
If the Design Rules of a given board specify that the "first pad" of a package shall be drawn with a particular shape, the pad marked with the FIRST flag will be displayed that way.
A newly started PAD command resets all flags to their defaults. Once a flag is given in the command line, it applies to all following pads placed within this PAD command (except for FIRST, which applies only to the pad immediately following this option).
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.
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 © 2005 CadSoft Computer GmbH|