Fixing the net ties properly is … taking quite some time. #2265 I linked to earlier has been open for 4 years, has 21 upvotes and apparently needs some more of those…
Note that while 2265 is not fully solved, net-ties were quite substantially improved in v7. You no longer need the “net tie” keyword, and you can explicitly specify pairs of pads that are intended to be shorted. For example, in a 4-pin kelvin resistor, you could say that pin 1 and 2 are shorted, pins 3 and 4 are shorted, but pins 1/2 are not shorted to pins 3/4.
The only thing from 2265 that hasn’t been implemented is single-pad net ties, because KiCad’s architecture is still one pad == one net. Single-pad net ties would let you say “pad 1 should be shorted to nets x, y, and z”. But you can get pretty close with what you can do in v7.
2 Likes
As I mentioned in another comment, this is accurate for v6 but not for v7. You don’t need the net tie keyword in v7. Instead you explicitly specify shorted pads in the “clearance overrides and settings” tab.
I hope @craftyjon doesn’t mind me summarizing the changes he made here…
As of today, Jon changed the 7.0 and 7.99 branches so you can short overlapping copper zones by adding a custom DRC rule that specifies a negative clearance for the zones in question (in most DRC rules, a negative clearance means to disable the clearance constraint).
This allows OP to accomplish their goal of net-tie-with-zones.
Jon’s example DRC rule is:
(rule net_tie_zones
(condition "A.Type == 'Zone' && B.Type == 'Zone' && A.NetName == 'GNDA' && B.NetName == 'GNDD'")
(constraint clearance (min -1mm)))
3 Likes
That’s great news – thanks for sharing it! Since it’s in 7.0 will it be built into an official release? Will I need to do anything specific to get this functionality?
just update to 7.0.1 when it’s released, or use tomorrow’s 7.0 testing build.
3 Likes
Sounds good.
When I have written:
I was thinking about making at inner layer GND_A island inside GND (rest of that layer) and connecting them by added filled area. Now with adding GND_B net and two negative clearance rules I suppose it will be possible with GND_A being automatically isolated anywhere else from GND.
Oops. I see a potential problem. Will GND_B fill be not removed because of lack of pad it is connected to?
The footprint with pad at inner layer will be needed. 
No, fills with zero pad connections won’t be removed as islands.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.