How to create guard traces?

Layout
1

Hi forum!

I’m wondering if anyone has any hints on how to create guard traces using Kicad?

Guard traces are traces without solder mask (with exposed copper), which are meant to stop creepage current across the surface of the PCB. This can be useful in things like high sensitivity analog frontends.

I can’t seem to figure out how to do this, if it’s possible. Ideally I’d like to have a way to select a net in pcbnew and have it not be covered with solder mask.

2

I’d say it’s possible, you can either add those traces just in PCBNew (OpenGL mode, press ‘x’ and start drawing) or you could create a special schematic symbol with a tiny footprint and connect two together with regular traces.

The first method is easier and more on the fly, but risks losing the traces on netlist import if “Delete Unconnected Traces” is selected. Second method has the benefit of setting up trace clearances other than what’s already containing in the “Default” net class.

Either way, you’ll need to draw lines (F.Mask or B.Mask) the same thickness as your traces over top of the traces you want exposed. Seems like it sucks, but it’s not too bad.

1 Like
3

The ideal is not quite supported, but it is possible.
You can manually draw, or looking at the data base with a quick test reveals

(segment (start 110.132 120.5) (end 114.087 116.545) (width 0.299) (layer F.Cu) (net 4))
(segment (start 114.087 116.545) (end 117.05 116.545) (width 0.299) (layer F.Cu) (net 4))

(gr_line (start 114.1476 116.5352) (end 110.0836 120.5484) (layer F.Mask) (width 0.311))
(gr_line (start 117.094 116.5352) (end 114.1476 116.5352)  (width 0.311) (layer F.Mask))

The last line I swapped W/L and it tolerates that on load (but saves as line above)
If you edit the trace widths on the ones you want unmasked, you can then easily find them, and clone them in an editor, Adjust mask width too, if you want.
If you have a lot to do, probably a script could clone for you.

1 Like