PCB DRC (Design Rules Check)

PCB DRC (Design Rules Check)… For the eye it seems like most components on this board are connected with traces, though when using the “Drag” function we can see the traces are not connected to the pads. But the DRC does not say anything about this. What is the thing with this? Did I miss any settings or so, or is it a bug? Can’t be a bug at this point (late development of the software) as this is too dangerous… Example below:

Version info:
Version: (6.0.5-0), release build

  • Date: May 3 2022 12:26:25*

I saw the first 20s or so of your video, then it trailed off to unrelated issues and I had no interest to watch a further 5 minutes of it.

DRC is right in that the connections of that resistor (R14) is connected. The “Drag” with attached wires is an extra, and I guess it only works if the ends of the tracks are snapped to the attachment points of the pads (a short test I just did confirms this).

1 Like

Ok, I see, I thought it was important for all traces to be hardwired/connected to a center of the pad to make the DRC not noticing this, but it seems like KiCad allows a trace to overlap a pad just a tiny bit to see this as “connected”/OK.

Gosh, 3 repliers at the same time…

I had some difficulty believing your last screenshot would be accepted by DRC. KiCad V5 already had some tolerance for DRC and tracks did not have to align perfectly to get accepted by DRC, but your last screenshot looks just wrong.

However, during testing I verified that any overlap between the copper part of a track and a pad gets accepted by DRC, even if it has such a tiny overlap. I’m now thinking about making preparations for making a bug report for this on gitlab.

Edit: Thanks mf_ibfeew, for linking to gitlab. I added a comment on #8837.

1 Like

Be careful with these cases and try to avoid them .
The DRC-“connection”-test says connection is ok.
And the DRC-“minimal-width”-test currently doesn’t detects such narrow places - so it’s possible to build a board with such small touching tracks even with “touching-area < minimal board-copper-width” and get no warning from the DRC.

You can read for more info: DRC: min copper width rules not run against partial collisions (ie: track to round pad or round track end to whaterver). (#8837) · Issues · KiCad / KiCad Source Code / kicad · GitLab and No DRC report for bad track to via connection (#9870) · Issues · KiCad / KiCad Source Code / kicad · GitLab

For former eagle-users (for instance me) this is a regression, but to be fair some other tools (Altium CS) also don’t detect such situations.

1 Like

I find such thin slivers of overlap being considered OK by DRC quite disconcerting, and even more so because it was already reported on gitlab 7 months ago, probaby because the issue got closed because it was seen as a duplicate for an issue in the nightlies.

So just now #8837 got closed, and #/9870 got re-opened, and you can upvote it if you feel about this as I do.

1 Like

I find this curios. Weren’t people complaining not too long ago about having to ‘snap to the center’ of a pad?

1 Like

Even in KiCad V5 some distance was allowed between the endpoint of a track and the attachment point in (the center of) a pad, but the distance was quite small, and sometimes quite solid connections got flagged by DRC as “not connected” and I can also remember some complaints about this, but in itself it was harmless and easy to fix.

These very thin connections not getting flagged is new (as far as I know) in KiCad V6. These very thin connections can also lead to real faults on PCB’s, and I consider this a much more serious issue.

1 Like

Yeah. I’m just surprised these connections could even be made. To me, an extra mouse button click to make sure it came off the pad where you wanted it to was no big deal.

1 Like

Until when to long thin pad you go with enough wide track so when you end it at pad center then the track sticks out on the other side.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.