EEVblog Electronics Community Forum
Electronics => PCB/EDA/CAD => KiCad => Topic started by: PixieDust on July 15, 2019, 08:12:54 am
-
Hi guys, I added a filled zone, however there is a border from the edges of the board. Is there a way to remove this border and have the fill extend all the way to the edges of the board?
-
You can reduce the clearance setting on the zone, however you might want to check what the rules are from your manufacturer, usually they don't want you to have copper right to the edge.
-
Ah I see, the clearance option affects both border and the distance between traces, bummer, oh well.
-
Yes, that's one of the big shortcomings of KiCAD, to not differentiate between manufacturing constraints vs. electrical constraints.
-
At the moment (Kicad V5) the board outline of a PCB is treated as a track for calculating clearances of zones.
If you want to have the zone closer to the board outline, you can decrease the widht of the board outline graphics.
It is a very bad idea to have zones extended to the board outline.
The board outline is often made with router bits, and these generate burrs on the copper, and this can generate shorts, especially on 4 or more layer boards, so consider yourself warned.
KiCad V6 is expected to have a separate setting for the zone clearance to the Edge.cuts.
If you still want to extend a zone to the edge of a PCB then you have to set both the edge clearance of the zone to zero and the widht of the track on the Edge.Cuts layer.
If you want to preserve clearances of your zone to other tracks, then you can make use of overlapping zones in the same net. Simply use a clearance of zero for the zone near the edge, and another zone with another clearance for the inner parts.
Also note that these cleareances are not "Just a single number". Tracks, footprints, pads, zones, can all have their own clearances, and can inherit from ieach other or override them. You will need to do some reading or experimenting to figure outhow it works exactly.
-
It is a very bad idea to have zones extended to the board outline.
The board outline is often made with router bits, and these generate burrs on the copper, and this can generate shorts, especially on 4 or more layer boards, so consider yourself warned.
What's wrong with sanding the result?
Here's pre deburring and after deburring and coating with solder.
I only plan on using single sided boards for now.
-
What's wrong with sanding the result?
This is an unnecessary manual step. The routing is pretty accurate, so just leave a 50 mil border or what the manufacturer says. I think in KiCad 5 there was a trick to change the width of the edge cut tracks, but usually I just define the zones in a way that there is always a distance to the border. But it is a bit painful with curves to repeat the exact edge cuts outline.