Pcbnew not finding footprints

And once I add a footprint to the layout and run test footprints again (sorry about making this two posts… forum restrictions)

Clicky the Icon just to left of the LadyBug.

@Sprig, I’ve done that and everything looks good, but when I click “Update PCB” all of KiCad locks up (not just Pcbnew). I’ve let it sit overnight in this state and it never comes back to life.


Are you allowed to share your schematic? If so share it here and we can check if it is something caused by your kicad setup or if the schematic is damaged. Additionally a bugreport might be in order as a crash is never ok.

@Rene_Poschl, I can share the project but new forum users can’t post attachments… :confused:

@Joan_Sparky and/or @davidsrsb

Your footprints are inside directories which names are plural : Probably v4 footprints…

If you had v4 previously installed, read this FAQ:

@Efcis I guess I did start this project in v4. For some reason I had thought it was started in v5.

I went through and removed the online libraries and added the local copies. Then updated all footprints in eeshema and exported the netlist. Pcbnew still crashes when updating but this seems to have helped some.

If I run “load netlist” I still see exactly the same behavior as before but if I “update from schematic” I at least get 48 errors reported - but the program still crashes so I can’t figure out what the errors are.


Below the text output select only errors and make a screenshot that way. or press the save button and upload the resulting report file.

I just through of that and those errors are apparently unrelated to the crash. I had just botched the footprint assignments and assigned resistor footprints to a group of transistors.

The footprint assignments have been fixed and I’m back to where I started. Crashing with no feedback at all. I’ll upload the design once I’m given the ability to do so.

Please upload your project (File / Archive Project - in the Project manager), and specify the KiCad version you’re using (Help / About KiCad / Copy Version Info - and paste it in your next post).

As a new user I can’t upload files yet… but here’s the version info:

Application: kicad
Version: (5.1.2)-2, release build
wxWidgets 3.0.4
libcurl/7.61.1 OpenSSL/1.1.1 (WinSSL) zlib/1.2.11 brotli/1.0.6 libidn2/2.0.5 libpsl/0.20.2 (+libidn2/2.0.5) nghttp2/1.34.0
Platform: Windows 8 (build 9200), 64-bit edition, 64 bit, Little endian, wxMSW
Build Info:
wxWidgets: 3.0.4 (wchar_t,wx containers,compatible with 2.8)
Boost: 1.68.0
OpenCASCADE Community Edition: 6.9.1
Curl: 7.61.1
Compiler: GCC 8.2.0 with C++ ABI 1013

Build settings:

Put them on some cloud storage (dropbox, google drive) and add a link.

Or read a few articles on this forum which will automatically promote you. (make sure you are logged in when reading)

Here’s the project. https://drive.google.com/open?id=1CpQPdRv2XDEXfCvSgsT7PAx2sFqX83iF

You did not include your custom molex footprint library. And your custom symbol lib is missing as well (not as bad as it simply means the rescue dialog comes up on import.)

Edit: I can import to pcbnew but am currently on nightly. I will check later if 5.1.2 can do it.

You used the pspice diode symbol. This one is incompatible with all kicad footprints. (It has the pin numbers assigned to fit the pspice standard instead of the industry standard used for PCB design) Use the D or D_Small symbol from the Device lib instead.

It appears to be a problem with the custom molex footprints I have since opening them in the footprint editor crashes KiCad. Here’s a link to the library: https://drive.google.com/open?id=1D5JAY9rmH7_39_y6sL5k8E-rIvbkAxle

As a curious side note, one of the footprints (Potentiometer TC33X-2-502E.kicad_mod) somehow ended up with a null character (0x00) instead of a dot (0x2E) in the filepath before “kicad_mod”. This had to be changed before zipping the folder since 0x00 is an invalid character for a zip archive… Correcting this character does not help with the crashing.

The I’ve replaced the diodes with D_small

the polyline in the molex footprints seems to crash kicad. https://bugs.launchpad.net/kicad/+bug/1833819

Here the fixed footprints (Well they no longer crash kicad. I have not checked them in any other way.):
Molex-4.kicad_mod (941 Bytes)
Molex-8.kicad_mod (1.3 KB)

General remark: You might want to invest a bit more time into footprints. I would suggest to give them more meaningful names (include the order number) and better drawigns on silk and fab. Also include a courtyard area to ensure you leave yourself space to solder. Tutorial: How to make a footprint in KiCad 5.1.x (From scratch)?

Thanks for the help! The new footprints work and I’m now able to import the netlist.

Good point about better naming of the footprints and courtyards. At the moment I don’t have that many custom parts to keep track of but definitely a good idea going forward.

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