Zone clearance to NPTH in one layer

Layout
1

I want to increase zone clearance to a few NPTH in just the top layer. After searching I found that this is best achieved with a custom rule and found this one:

(rule "Mounting_holes_zone_clearance"
	(layer F.Cu)
	(condition "A.Type == 'Pad' && B.Type == 'Zone'")
	(constraint clearance (min 1.0mm))
)

It took a while, but I finally found out that this works fine with SMD pads and PTH, but doesn’t work with NPTH.

According to the documentation the Type can be set to: One of “Bitmap”, “Dimension”, “Footprint”, “Graphic”, “Group”, “Leader”, “Pad”, “Target”, “Text”, “Text Box”, “Track”, “Via”, or “Zone”.

There doesn’t seem to be a better “Type” for NPTH pads.

Is this a bug that I should report, or is this by design?

I tried fixing it by setting A.Pad_Type == ‘NPTH, mechanical’, but that doesn’t work either.

(rule "Mounting_holes_zone_clearance"
	(layer F.Cu)
	(condition "A.Pad_Type == 'NPTH, mechanical' && B.Type == 'Zone'")
	(constraint clearance (min 1.0mm))
)

If I change the NPTH to a SMD pad it works great with both A.Pad_Type == ‘SMD’ and A.Type == ‘Pad’

Edit: I’m using KiCad 8.0.6 on Windows. Cannot figure out a way to make this work with NPTH…

2

I think ‘clearance’ is for copper/copper, and npth doesn’t have copper. Try hole_clearance or whatever it is.

1 Like
3

I thought that I had already tried that, but apparently not. It works great! Thank you!

(rule "Mounting_holes_zone_clearance"
	(layer F.Cu)
	(condition "A.Pad_Type == 'NPTH, mechanical' && B.Type == 'Zone'")
	(constraint hole_clearance (min 1.2mm))
)
1 Like