EAGLE Help

BUS

Function: Draws buses in a schematic.
Syntax: BUS [bus_name] * [curve | @radius] *..
Mouse: Right button changes the wire bend (see SET Wire_Bend).
Keyboard: Shift reverses the direction of switching bend styles.
Ctrl toggles between corresponding bend styles.

See also NET, NAME, SET

The command BUS is used to draw bus connections onto the Bus layer of a schematic diagram. Bus_name has the following form:

SYNONYM:partbus,partbus,..

where SYNONYM can be any name. Partbus is either a simple net name or a bus name range of the following form:

Name[LowestIndex..HighestIndex]

where the following condition must be met:

0 <= LowestIndex <= HighestIndex <= 511

If a name is used with a range, that name must not end with digits, because it would become unclear which digits belong to the Name and which belong to the range.

If a bus wire is placed at a point where there is already another bus wire, the current bus wire will be ended at that point. This function can be disabled with "SET AUTO_END_NET OFF;", or by unchecking "Options/Set/Misc/Auto end net and bus".

If the curve or @radius parameter is given, an arc can be drawn as part of the bus (see the detailed description in the WIRE command).

Bus name examples

A[0..15]
RESET
DB[0..7],A[3..4]
ATBUS:A[0..31],B[0..31],RESET,CLOCK,IOSEL[0..1]

If no bus name is used, a name of the form B$1 is automatically allocated. This name can be changed with the NAME command at any time.

The line width used by the bus can be defined for example with

SET Bus_Wire_Width 40;

to be 40 mil. (Default: 30 mil).

Index