Greetings all, I ran into something interesting today while working on a zone using 5.1.0 and 5.1.2. I changed the clearance from 0.5mm to 2mm on a ground plane zone and the ratsnest between most GND pads re-appear (the unrouted number also increases). Taking the clearance back down removes the GND ratsnests (as it should). It seems 1.75-1.87mm is the tripping point between a nest and no nest and is dependent on the size of the component pad. Re-filling the zone or performing a DRC has no effect. In some cases the copper is connected to the pad but others the copper skips the pad.
Note in the picture (2mm clearance) a mounting hole pad (1 GND) is connected. However, P3, C18 have copper connections but ratsnests are still present and D3 the copper misses the pad completely. The second picture (which I can’t upload due to being a new user) uses a .508mm clearance in which all ratsnest are properly connected.
This is more of a curiosity as to why. Does the clearance of the non-net pads take presidence over the zone net pads?. I have several work arounds such as manually running traces or using keepout areas so it’s not a show stopper.
This.
Anything else would be illogical.
From the POV of the zone those pads are violating the clearance rule, by being too close to the pad/track of the other net. Really simple.
My comments are in regards to the 2mm zone clearance.
It looks like P3-2 should be connected, but the way KiCad calculates connectivity it isn’t. The insertion point of a pad (for THT pads, this is the center of the hole) is how KiCad determines electrical connection to net copper. Because the center of the P3-2 pad is over the zone clearance put in by the existence of non-GND-net P3-1, KiCad doesn’t consider it connected to the zone copper. So even though the annular ring of P3-2 is on the zone copper, KiCad doesn’t realize that the pad is connected.
Also, C18 is connected to the zone. The reason for the rats nest lines to it is because it is the closest connected pad in the GND net for both P3-2 and D3-1.
To @Joan_Sparky point, if you imagine the zone fill as the bucket tool in your favorite paint program, this tool avoids other nets by respecting their clearance spacing.
If you need to ensure connectivity, an explicit ground trace or solid region on copper is recommended. Ground pours (zones) are most convenient for solid internal planes, and surface coverage. As design density increases the likelihood of an isolated island increases.
If you set the clearance very high you increase the chance of getting disconnected islands of pads on a pour as well.
To not display lack of connectivity as a ratsnest would lead to very severe errors like isolated ground sections and usually leading to total circuit failure which is very hard to diagnose.
Thanks all for the comments. Makes sense as to how and why now.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.