EAGLE Help

BUS


Function
Draws buses in a schematic.

Syntax
BUS *..
BUS bus_name *..

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".

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 Copyright © 2001 CadSoft Computer GmbH