Kicad 8 DRC errors on unconnected SMD and TH combination pads

[Kstandifo]

I am using Pi Pico footprints with overlapping through hole and SMT pads, a fairly standard technique. Pins marked “no connection” in the schematic cause ERC errors in layout:

The message says:
Pad net (unconnected-(U1-GPIO2-Pad4)_0) doesn’t match…schematic(unconnected-(U1-GPIO2-Pad4))
Pad 4[unconnected-(U1-GPIO2-Pad4)_0] of U1 on F.Cu

The netlist from schematic says
(net (code “53”) (name “unconnected-(U1-GPIO2-Pad4)”)
(node (ref “U1”) (pin “4”) (pinfunction “GPIO2”) (pintype “bidirectional+no_connect”)))

Connected pins are fine, and this used to work in Kicad 7.

[ML9104]

Do you mean DRC? plus20characters.

[baldengineer]

Which Schematic Symbol and PCB Footprint are you using?

[davidsrsb]

And you must post KiCad and OS details from help -about kicad - copy version…
There have been a lot of bug fixes since 8.0.0 release

[Kstandifo]

The error is from DRC in the PCB Editor. System is Windows 10. Kicad rev is 8.0.1 released version.

Footprint and symbols are the one from Raspberry Pi for the picoW: https://datasheets.raspberrypi.com/rp2040/VGA-PicoW-KiCAD.zip

And again, this used to work fine in Kicad 7.x

[mf_ibfeew]

And again, this used to work fine in Kicad 7.x

That might be, but does not really help to find a solution for your current situation in v8.

The easiest way would be to attach the archived project, so others can investigate your problem.

As you are a new user please read (and follow) this FAQ-article: New Member Information
This allows you to promote yourself to basic forum user level, which is needed to attach a project archive in your thread.

edit: I overlooked that the link already included a project, not only symbol+footprint.

[baldengineer]

For me, the project included in that download does not produce any ERC DRC errors about the pads. (It has other issues, but nothing related to the one you are seeing.)This computer is running KiCad 8.0.0.

Your project might be different, of course.

If you open that project as-is, do you still get the same ERC DRC issue?

Edit: I had schematics on the brain.

[ML9104]

Could we be clear about the difference between ERC and DRC here, please?
It seems some posters don’t understand the difference.

[mf_ibfeew]

I have now played some time with the linked project and I think there is a small bug hidden in the DRC. Used kicad version: v8.0.1 and v8.99

This affects the following situation:

• correctly synchronized project (schematic+board)
• symbol on schematic side has some pins with “no connect” cross attached
• the corresponding footprint in the board has multiple pads with this pad number.
  • it’s not important if these doubled pads (with same padnumber) overlap
  • laso the type of these pads is not relevant
• running the DRC then gives a schematic parity warning for these doubled (multiple) pads

Simplified example project (if someone likes to confirm this):
erc_drc_reduced_fp_selfdefined.zip (40.9 KB)

additional remark: the “ERC” was a false sign already in the opening post, this is about the DRC

As I got no opposition I opened this error report: false positive drc error (#17635) · Issues · KiCad / KiCad Source Code / kicad · GitLab

[Kstandifo]

Yes, this matches the behavior I got on my larger project. I was short of time to figure out how to post the whole thing as a newby. It never occurred to me to just try the RP example where I got the symbol and footprint. Brilliant!!! Thanks for running with this. I’ve never had to post a bug before (It’s always me…). Maybe I’ll have to flatter myself and learn how. (I saw it in the help menu!) Thanks again.

[edmondhma]

Same error and same situation.

[paulvdh]

Maybe same solution too?

Without more input from your side, there are also no more suggestions we can give. At the very least, show us that you are willing to put some effort into formulating your question. I will lock this thread now, because the original issue has apparently been solved. I suggest you open a new thread, explain your problem more elaborately, and possibly create a link to this older thread too.