Complex PCB edge with matching margin

[dchisholm]

@SembazuruCDE

I thought the kludge to enforce a “Clearance to PCB edge” in KiCad was to understand that the board will be milled to the centerline of the board outline on the Edge.Cuts layer, but the copper-to-copper clearance settings for the pour will treat the Edge.Cuts lines as copper traces and enforce clearance to the edge of the line. Thus if you want a larger copper-to-edge clearance than the normal copper-to-copper you make your board outline on the Edge.Cuts layer as wide as twice the difference between the two clearances.

For example, if you want 10mil clearance copper-to-copper, but also want 15mil copper-to-edge clearance. The difference is 5mil, so you would make the lines for the board outline on Edge.Cuts to be 10mil wide. This would also enforce DRC to keep traces at least 15mil from the centerline of the board outline.

I thought this technique was discussed in detail, with illustrations, 2 or 3 times in the last year or so but I can only find an old post of mine : Creating “zone outlines” for odd-shaped PCB’s

I don’t think you need to do anything more than define the fill-zone as a rectangle circumscribing the board outline, and fill it. The algorithm places copper up to the board outline, less the “clearance” parameter. You may have to be careful that the outline on the Edge.Cuts layer is a strictly closed contour.

The clever trick of adjusting the board-edge clearance isn’t too difficult in practice. Select everything on the Edge.Cuts layer, change the line width, do the fill, then re-set the line width if necessary.

@PCB_Wiz

Sounds here like Kicad really needs a Clearance to PCB edge option ?

I am NOT a programmer but my superannuated brain (which learned “Fortran II” over half a century ago) wonders if this feature could be easily implemented by defining the Edge.Cut as a special kind of Net Class, with an associated Clearance parameter just like any other Net Class.

Dale