topic Re: Changing ground plane clearance around traces in EAGLE Forum (Read-Only)

Changing ground plane clearance around traces

crchisholm — Sat, 06 Jun 2020 18:02:22 GMT

I need to increase the clearance around traces. I think it has to do with net classes, but in this case I wan to change it universally (all traces) . How would I do that?

Re: Changing ground plane clearance around traces

Anonymous — Mon, 08 Jun 2020 09:28:32 GMT

Hello @crchisholm ,

The polygon tool has an 'isolation' property. With it, you can choose the minimum distance to be left between the copper and any entity on it (vias, traces, pads...)

Re: Changing ground plane clearance around traces

Anonymous — Mon, 08 Jun 2020 19:15:35 GMT

There are actually three different values that control clearance around traces and the biggest one of them (the most restrictive) is the one that is going to be used.

DRC: Clearance ->Wire/Wire - This is the default variable that sets clearance between two different nets, including net and a copper pour that belongs to a different net.
Polygon: Properties -> Isolate - This controls net clearance for a single polygon. I use it most frequently for inner layer copper pour, because some manufacturers have a different set of rules for inner and outer layers.
Net classes: Edit -> Net Classes... -> Rules - This is a feature that lets you add a net class with special rules (clearance, width and minimum drill size). Those then apply only for nets that belong to this class. This feature is great when you are laying power traces that need bigger clearance than other traces.