First a wish: try to be precise with your wording. The ERC is for schematic, the DRC is for board-editor (and therefore the footprints).
Why is the error ("Does not match copy in library ") in the first place?
This DRC-check (and a similar check also on the schematic-side for symbols) is newly added from v6–>v7 development. So it’s ok that you are surprised by these new warnings.
Background for this DRC-check:
Kicad stores footprint-information inside board-files (so the board is self-conatined and independent from the library). During the board development Kicad allows the user to modify every single of these stored footprints independently from the library (through the Edit symbol/footprint command: customize pads, change 3D-model, change parameters, …).
Additionally the footprint in the original library can be developed (corrected/modified/…) during time
All the mentioned DRC test does is to check: Are the current saved footprint in the project is exactly == the current version in the library? If not equal → display warning
Kicad currently can’t check which of the two possibilities are the reason for the difference:
modified in board?
or modified in the library?
all the report says: there is a difference, you may look at that.
So it’s up to the user to decide: OK, update from library or not. If the footprint was deliberately modified in the project one should not update → as this process would overwrite the changes with the original version from the library.
If this check is tooo confusing: just disable it. Not every ERC/DRC check is for everyone (I also have some checks disabled)
How can I solve it?
In your case:
you deliberately changed the footprint on board-level (with the changed 3D-model-setting)
so the check is correctly showing the “footprint in board does not match copy in library” - warning
so you can:
ignore/approve this error (as
disable this specific DRC completely
update the footprint in the library so that the library already contains the correct 3D-model. Note: This will not work with the original kicad-libraries - these are write-protected and the next kicad-update normally overwrites your modifications
Thank you so much for your detailed answer @mf_ibfeew!
For the footprints with warnings, I moved from using standard libraries to copying them to my project folder. Then I could update them to remove all warnings and have a clean project.
I guess this could be a problem when kicad changes again, but I will see how to solve that when it comes.
As a side effect, this also allowed me to correct other warnings, like silkscreen overlapping, missing courtyards, etc.
