Page 154 - Make Your Own PCBs with EAGLE from Schematic Designs to Finished Boards

FIGURE 5-36 Unrouted board.

As with the automated layout, we have kept the ground plane on the bottom layer.
I like to start a manual layout with the power-supply nets. In this design, many of these are
provided by the ground plane, so we can start by laying out the positive supply.

Once the Route tool has been selected, the Parameter toolbar will display the options available to
us. I described these options at the start of this chapter. In Figure 5-37, I have set these parameters
ready for routing the positive power line on the top layer.

FIGURE 5-37 Routing toolbar.

The first thing to note is that the Layer dropdown is set to “1 Top.” We then have to select the
fourth of the “Wire bend” types. It does not really matter which one you chose, but I find that this one
produces nice-looking layouts. The miter radius is set to 0 because we do not need the corners of the
tracks to be rounded. The width is set to 0.02 because this is the track width that we specified for the

power-supply net class.
We have also opted to use square vias with the size set automatically. But we will try to make a
layout that does not need any vias.

The only parts of the design that require significant current to flow are the power supply to IC2
and the supply lines to each LED. In fact, the supply to IC2 could be as much as 200 mA if all the
LEDs are lit.

When using the Routing tool, start at a pad, and an air wire will become highlighted along with
the rest of that air wire’s net. This indicates all the possible target points for your routing, so just
move the cursor along the route you want to take, left-clicking to make a waypoint in the route. When
you arrive at a valid destination, the route will stop automatically, and you can go off and find another
air wire to route.

If you go wrong, you can, of course, use the Undo command. If you find an earlier mistake that you
want to correct, the just select the Ripup command, and click on the tracks that you want to route
again and they will revert to being air wires.

You can also modify the path of the routing using the Move command if the track is just a little off
and does not need complete rerouting.

If you are concerned about just how wide your tracks need to be, then a calculator such as the one
at http://circuitcalculator.com/wordpress/2006/01/31/pcb-trace-width-calculator/can be very
2
helpful. Using this calculator, for a typical PCB with 1 oz/ft of copper and a track 1 in. long and
20 mil wide will only increase in temperature by 10°C when a current as large as 1.5 A is
flowing through it.
Thus the tracks on our circuit should barely get warm at all with the currents we are using. For
high-current circuits, though, overheating of the tracks eventually will damage the circuit board

and cause it to fail because, ultimately, the copper will melt.