All nets become GND after schematics update in PCBnew


I have an old board that I have been working with a long time and that has worked fine. Al the sudden when I did an “Update PCB with changed made in Schematics” all my nets go into GND. If I delete a symbol in my schematics and add it again, the footprint gets added as usual on the PCB when doing the next update and gets the correct net back. But if I do yet another update, nets are turned into GND again? Any ideas why this is happening? The boards are a commercial project, so I cannot share the design files unfortunately.


And your KiCad version, OS etc is?
Help - About KiCad - Copy Version Info

Backup what you have immediately

I am sorry, of course.

Application: KiCad (64-bit)

Version: (6.0.7), release build

wxWidgets 3.1.7
libcurl/7.83.1-DEV Schannel zlib/1.2.12

Platform: Windows 10 (build 19044), 64-bit edition, 64 bit, Little endian, wxMSW

Build Info:
Date: Jul 26 2022 02:49:38
wxWidgets: 3.1.7 (wchar_t,wx containers)
Boost: 1.79.0
OCC: 7.6.0
Curl: 7.83.1-DEV
ngspice: 37
Compiler: Visual C++ 1929 without C++ ABI

Build settings:

I am wondering if this is the Schematic cache bug fixed in 6.0.8

It’s worth making a backup and upgrade to 6.0.8 to see what happens.

Hello again,

I think I have found the cause of this. It is not related to the Schematics bug, but I would say that it is another bug. I suspect it is actually related to something we talked about here: Weird behavior with zone filling - #18 by ravn some time ago. @JeffYoung I am not sure if you did work on this, but I think the current/updated behavior is a bit weird.

Way to reproduce (in 6.0.7 or 6.0.8, or maybe some others)

  1. create a footprint (1) with NPTH pad that has a rectangular shape and a hole size that is the same as the pad size (so no copper around it)
  2. create another footprint (2) with an SMD pad (pad 1)
  3. connect pad 2.1 to some net != GND
  4. place footprints 1 and 2 so that pad 2.1 touches the NPTH hole from footprint 1
  5. Place a GND zone around the whole thing
  6. press “Update the PCB with changes made to Schematics”

This will change the net of any track connected to pad 2.1 to GND.

To me, this looks like a very undesirable behavior where the NPTH, that does not have a net at all, force a change of nets on the tracks:

Workaround, move the pad arbitrarily much away from the NPTH will restore the net:

I did not have this issue with earlier versions of KiCAD, so I suspect this was introduced in some recent 6.0.x update.

@ravn Please post the example board either here or (preferably) in a bug report. You can easily create a bug report from inside KiCad by using the “Help” menu and selecting “Report Bug”

As you say this is a commercial design, you can strip out the rest of the circuit away from the bug area or submit it as “confidential”, so that only the developers can see it.

Thanks guys, I reported this in All nets become GND after schematics update in PCBnew (#12622) · Issues · KiCad / KiCad Source Code / kicad · GitLab with a minimal working example causing the issue.


A bug fix has already been committed for 6.99
There is one scheduled for cherry picking into Testing, but that build is waiting for attention

Samples showing bugs make the developers life much easier

It’s good to hear that.

The latest Testing build now includes a commit to address your bug, so can you test it?

Thanks! I can test it under Linux if that is ok. I don’t have a Windows machine to run on since I have stock KiCAD on that computer. Is Testing build=nightly?.

NO!. Testing is basically the Beta of what will be 6.0.9 if it is released (high likely)

Nightly is Alpha of what will be 7.0.0 at maybe the New Year

Ok, I see. Sorry, but I cannot find where to install it from. I only find links to nightly. If you can point me in the right direction, I can install and test.

What you can do is try the Testing build on Windows and then run the 6.0.8 installer to revert to the Stable release. 6.0.x “Testing” does not permit file format changes, so going backwards works.

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