I hereby certify that I am not simply asking someone else to design a footprint for me.
I ran into an error with all the footprints used in the existing “Arduino Nano” Shield example that I cannot correct since I cannot re-assign any footprints.
I am willing to redesign any footprints used, however I would expect the existing examples to contain all needed footprints and libraries. All footprints in the PCB view and 3d view seem to be okay as well. Is this a bug? Or am I missing something?
I tried to give an image of the PCB but I am unable to post 2 media files. If it is requested I will try again.
Note that this is my first PCB design that is for an Arduino Nano connecting to an RF24L01 radio module. I have failed to research an answer to this for multiple days. so All your experienced eyes will be of great help
You could have posted a text version of those warnings by using the Save button. That would enable us to see the text cut off in the screenshot.
Nontheless, those are only warnings. As the footprints are already in the file, there is no problem continuing with the PCB file you have. You’d have to compare the footprints to see what the differences are. It could be as minor as a change in the UUID, or some small tweaks to the footprint. If you deem that the library version is better, you can Tools > Update Footprints from Library, one at a time if need be. For the one that was not found, you’d have to work out where the library version went, if anywhere.
Usually the Warning: Footprint XXXX does not match copy in libary YYYY does not mean much. It is commonly triggered by very minor changes to a footprint. Another reason why it does not matter much is that KiCad projects (Starting from V6.0.0) are completely independent of external libraries. Even if you completely delete all existing libraries, or post your project on an USB stick to someone in farawayland then it’s still as easy to view and modify the project as if nothing happened.
If you really want to know what these error messages mean (they do indeed have a meaning) then you would have to dive a bit deeper into library management. But overall, I think the KiCad developers are getting a bit overzealous and are throwing a bit too many errors and warnings lately.
For example, the message Warning: Footprint XXXX does not match copy in libary YYYY may be better served not by regular ERC, but maybe only when an update from library action is attempted.
Here is the saved version txt for future reference:
** Found 7 DRC violations **
[lib_footprint_issues]: Footprint 'MountingHole_65mil' not found in library 'Arduino_MountingHole'.
Local override; warning
@(101.2700 mm, 83.4900 mm): Footprint MH2
[lib_footprint_issues]: Footprint 'MountingHole_65mil' not found in library 'Arduino_MountingHole'.
Local override; warning
@(141.9100 mm, 98.7300 mm): Footprint MH4
[lib_footprint_issues]: Footprint 'MountingHole_65mil' not found in library 'Arduino_MountingHole'.
Local override; warning
@(101.2700 mm, 98.7300 mm): Footprint MH1
[lib_footprint_mismatch]: Footprint 'SW_Slide_SPDT_Culewet_CYT1107_L12.7mm_W5.7mm_P17.4mm' does not match copy in library 'Button_Switch_THT'.
Local override; warning
@(135.6500 mm, 108.2500 mm): Footprint SW1
[lib_footprint_issues]: Footprint 'MountingHole_65mil' not found in library 'Arduino_MountingHole'.
Local override; warning
@(141.9100 mm, 83.4900 mm): Footprint MH3
[lib_footprint_mismatch]: Footprint 'PinHeader_1x15_P2.54mm_Vertical' does not match copy in library 'Connector_PinHeader_2.54mm'.
Local override; warning
@(103.8100 mm, 98.7300 mm): Footprint J1
[lib_footprint_mismatch]: Footprint 'PinHeader_1x15_P2.54mm_Vertical' does not match copy in library 'Connector_PinHeader_2.54mm'.
Local override; warning
@(103.8100 mm, 83.4900 mm): Footprint J2
** Found 0 unconnected pads **
** Found 0 Footprint errors **
** End of Report **
4 out of the 7 violations are for **Footprint XXX not found in library YYY". The compare straubm mentioned is of no help here, because there is nothing to compare it to. The footprint that is saved inside the project itself is the only available reference KiCad has for that project.
One quick way to get rid of all the violations is with:
PCB Editor / File / Export / Footprints to new Library.
Accept it when KiCad suggests to link the used footprints to this new library.
PCB Editor / Tools / Update Schematic from PCB This is the other way around from the normal workflow. It pushes the changes you made back to the schematic, so the the schematic (which is always KiCad’s first reference) also uses the footprint links to your newly exported library.
I do of course not know if you want to go in that direction.
I recommend turning off the warning entirely. I had it alot for reasons I couldn’t explain. I suspected it had maybe to do with an old project being opened in a new KiCad version.
And sometimes I just deliberately change a footprint for you know… reasons and than I have me a warning…
Whatever the cause was, the warning was always annoying me and it is also completely usesless IMHO. I think I even had it or something similars with power symbols. PITA
Turnings things off because your don’t understand them is… not very good advise.
I do agree though that simply turning off these warnings is a sensible solution in this case. But they are not:
For hobbyists, sure. But if you are working with database libraries or big / complex / expensive PCB’s then you want all the help you can get to verify correctness of a project, and comparing footprints on the PCB with vetted and verified libraries is a part of that.
So if you think these checks are a PITA for you, then turn them off, it’s a single radio button, and also available directly from the DRC window by right clicking on the text. No big deal.
I value the DRC above all else. I value it’s errors because they prevent failed PCB’s. The warnings otoh I value less.
I understand the warning and I know what it is saying. I am just saying that it keeps complaining about all kinds of default library footprints. Things I never touched suddenly became warnings. This rendered this ‘warning’ meaningless to me. I have not yet met the situation where this specific warning was actually a PCB saving warning.
I disabled more warnings, Overlapping silk texts, overlapping footprints (because of scew terminals)
