Data Sheet

Schematic Capture
49
Any net with a bus is assigned to the BUS net class.
Any other net is assigned to the SIGNAL net class.
This gives us quite a bit of flexibility during PCB layout as we can define different trace widths,
via styles, clearances and so on for each net class. Sometimes, however, we will need a
particular set of conditions for particular connections. Proteus allows us therefore to create our
own net classes and these will then be passed through to the PCB Layout software, allowing us
to define routing and clearance properties specifically for those connections.
Let’s take an example. On the tutorial schematic consider the output of the DC/DC converter on
the Analog sheet of our design. This is the 5V switched power supply for the analog circuitry so
we really want to lay this out with a track width smaller than that on the POWER net class but
larger than on the SIGNAL net class. The procedure for specifying a new net class is very
straightforward.
To specify a new net class
Select the Wire Label Icon.
Left click the mouse on a wire we wish to assign the net class to. Any wire on the net will
do – in our case let’s place it between the output of the MAX1724 and the SW_PW
terminal. You will see a small ‘x’ under the cursor when the mouse is over the wire.
Left click the mouse over the wire to launch the wire label dialogue form. Then simply
type in ‘CLASS=ANSW’ to assign the net class.