Update PCB from Schematic - some components are missing

[dhaillant]

Hello,
I’m experiencing a weird behaviour:
I added some components on the schematics, assigned footprints, switched to PCBnew, and clicked “Update PCB from Schematic”.
The dialog complained about missing annotations, offered to annotate them, and then, in PCBnew, only 3 components on 10 are now visible.
They are present and annotated in eeschema, but can’t be found in pcbnew.
When I try to re-update PCB from schematic, no new component get listed, as if everything was fine.
It looks like there are corrupted links between schematic and PCB…
Any idea on how to clean things?
Thank you very much!

Application: KiCad

Version: 6.0.6-3a73a75311~116~ubuntu20.04.1, release build

Libraries:
wxWidgets 3.0.4
libcurl/7.68.0 OpenSSL/1.1.1f zlib/1.2.11 brotli/1.0.7 libidn2/2.2.0 libpsl/0.21.0 (+libidn2/2.2.0) libssh/0.9.3/openssl/zlib nghttp2/1.40.0 librtmp/2.3

Platform: Linux 5.4.0-122-generic x86_64, 64 bit, Little endian, wxGTK, xubuntu, x11

Build Info:
Date: Jun 20 2022 15:49:56
wxWidgets: 3.0.4 (wchar_t,wx containers,compatible with 2.8) GTK+ 3.24
Boost: 1.71.0
OCC: 7.5.2
Curl: 7.83.1
ngspice: 36
Compiler: GCC 9.4.0 with C++ ABI 1013

Build settings:
KICAD_USE_OCC=ON
KICAD_SPICE=ON

[dhaillant]

After closing and re opening Kicad, when retrying to update pcb from schematic, I have:
“Updated h1 symbol association from /00000000-0000-0000-0000-00005baa5140 to /e633f5e4-4f6c-4e3a-b8de-c790e364dad2.”
But nothing gets corrected…

[mf_ibfeew]

In the “Update pcb from schematic” dialog: Uncheck the “relink according to reference designator”.

[dhaillant]

Thank you for your suggestion.
Unfortunately, I tried it already and it makes no difference at all…

Oh I think I found something!
I have components with identical References, but the first group have lower case (h1, h2, h3, etc) and the others have UPPER case References (H1, H2, H3, etc…)!!

Surprisingly I have no warning about this situation.

And of course, when updating pcb from schematic, there’s some kind of mismatch.

Plus, some of the components were tagged “exclude from board” in eeschema, which prevented the other components to be imported to pcbnew.

[dhaillant]

And indeed, once renamed with upper case and re annotated, the components that are supposed to be present in pcbnew are correctly synchronized!

[paulvdh]

I have experimented a bit with this case sensitivity in the Reference designators and I can confirm this issue and have created a bug report for it on gitlab:

Received an error while reading netlist. Please report this issue to the...

Also, did you get a message like this:

[dhaillant]

I didn’t get such message.

However, I use the command “update pcb from schematic” within pcbnew, not from eeschema.

Thank you for having created the bug report.

[eelik]

update board from schematic: netlist error due to same RefDes with lowercase...

EDIT: oh, @gkeeth noticed this already.

[dhaillant]

I get this message with a new project.
But I can’t get it with my older project (started in V4 IIRC)

[paulvdh]

I’ve just closed the issue myself now.

#11862 is apparently scheduled to be included in KiCad V6.0.7 and bug fix releases (bumps in the third digit) are made approximately once a month, so I expect V6.0.7 to be released in a few weeks. See the KiCad Blog for when updates have arrived. (Or if you have Linux, just do your normal system updates, which also handles KiCad updates.)