What is the best way to copper pour into arc-defined area?

I tend to leave 0.5mm at PCB edges without any copper. However, it is not true that I want 0.5mm clearance in general.

For the example shown what is a good way to craete a copper pour that is recessed by 0.5mm around the edges?


Draw a circle (or arcs connected by lines or whatever). Select the circle (or all the arcs/segments). Right-click, choose Create from Selection > Zone.

(This of course assumes 6.0. :slight_smile: )

1 Like

Actually if I understand the scenario properly, the shape of the zone doesn’t matter in this case. It can just be a rectangle larger than the board. The key is setting a different edge clearance than copper clearance, which can be done in the design rules.

True (if you want it to spill into the “tab” area).

1 Like

if you can consider a mecanical approach, kicad StepUp can push both Edgecuts and FillZones to a kicad_pcb file.

Long time ago I have read that clearance is calculated not to center of Edge.Cuts lines but to its edges.
I have just checked it. True (5.1.12).

Actually not true – but we make it look that way for legacy boards. (If the board has a consistent-width outline on the Edge.Cuts then we set the Edge Clearance value to 1/2 that width.)

I take that back… that’s for 6.0. 5.1 does indeed use the Edge.Cuts line widths.

Lots of interesting answers :slight_smile:

For now, the simplest solution would seem to be using Design Rules. I was not aware that copper clearance to EdgeCuts could be specified there.

CrafyJon - Please can you post a screenshot of this setting? (I’m using an old Kicad version and I might have to upgrade). I can’t seem to find the right part in Design Rules.

(BTW is F9 mode still present in 6.x? I sometimes drop back to that for specific tasks).

It’s only in v6, in Board Setup -> Design Rules -> Constraints.

The old legacy mode doesn’t exist anymore. V6 has enhancements which lessen the need for the old mode. Which tasks do you use it for?

If you think of upgrading only to 5.1.12 then you can use what I have written - make border lines thicker.
If to 6.0 then you have special settings for it.

I did it in v 4.0. In v 5.1 I never had to.

Ah, I see - so I make the Edge Cuts 1mm wide --> The fill will stop 0.5mm short of the PCB edge?

I think it will stop at 0.5 + clearance so if you want 0.5 set width to 2x(0.5-clearance).
But check it - I have never used it.

Or you can draw a second line on the Margins layer. That will allow it to be independent of the shape of the board outline.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.