The net command is used to draw individual connections (nets) onto the Net layer of a schematic drawing. The first mouse click marks the starting point for the net, the second marks the end point of a segment. Two mouse clicks on the same point end the net.
If a net wire is placed at a point where there is already another net or bus wire or a pin, the current net 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 a net wire is placed at a point where there are at least two other net wires and/or pins, a junction will automatically be placed. This function can be disabled with "SET AUTO_JUNCTION OFF;", or by unchecking "Options/Set/Misc/Auto set junction".
If the curve or @radius parameter is given, an arc can be drawn as part of the net (see the detailed description in the WIRE command).
Select Bus Signal
If a net is started on a bus, a popup menu opens from which one of the bus signals can be selected. The net then is named correspondingly and becomes part of the same signal. If the bus includes several part buses, a further popup menu opens from which the relevant part bus can be selected.
If the NET command is used with a net name then the net is named accordingly.
If no net name is included in the command line and the net is not started on a bus, then a name in the form of N$1 is automatically allocated to the net.
Nets or net segments that run over different sheets of a schematic and use the same net name are connected.
The width of the line drawn by the net command may be changed with the command:
SET NET_WIRE_WIDTH width;(Default: 6 mil).
|Index||Copyright © 2005 CadSoft Computer GmbH|