im currently trying to make a big (custom shaped) solder-pad for a small pcb.
My idea was to just use a copper-filled zone and remove the mask over the corresponding area.
So I created a copper zone on F.Cu and non-copper zone for F.Mask.
But I realized, non-copper zones have too few settings. I cannot set clearance or anything to it, so the mask would be removed further than the pad itself. It looks ugly and I dont like it.
How can I make the regular “non copper zone” with same setting as my copper zone?
I read about using named zone and some custom rules. but it seems non-copper-zone dont even have name field (anymore). (Do things have to be so restrictive/limited instead of just adding simiar options to both zone types allowing more freedom?)
What can I do to solve my issue now? Anyone has a custom rule for me?
This didnt work:
(version 1)
(rule "Clearance zone to board-edge"
(constraint edge_clearance (min 0.5mm))
(condition "A.Type =='Zone' && A.Layer == 'F.Mask'"))
Typical place of using custom shaped pads is in footprint definition (nothing stops you from making footprint having one pad). When such pad is defined in footprint the right mask opening is created automatically, I think.
My current solution is that is just edit the kicad_pcb and copy the filled_polygon from my copper to my non-copper zone. It seems that non-copper zones dont even have clearance attribute not even when you use custom rules - which I still dont understand.
Clearance is the distance from one net copper to another net copper. Clearance task is to stop electrons from jumping between conductors having different potentials. The higher potential difference the higher clearance needed.
Potential is not a property that characterizes non copper layers so also clearance does not apply.
In this example, I used the polygon tool to create the required shape and size of the pad needed.(A)
I added a pad: Place > Add Pad (B)
I moved the pad onto the polygon. (C)
I RMB click on the pad and use the function in the list now showing “Edit Pad as Graphic Shape” or “Ctrl+E”
I then (as instruction in the yellow bar show) Ctrl+E again and the entire shape becomes a pad.
See below results in the PCB Editor:
A remains a graphic shape.
B remains the original pad
C remains the original pad on the graphic shape.
D transforms the graphic shape into a pad with all the clearance attributes of a normal footprint.
Note A,B & C are only shown for demonstration purposes.
