HOwever this project I have made and completed with 7.0.1. DRC highlighted only some warning about Silk Layer. I sent the project for production. There were 9 Warnings … that’s it. Yes the broken silkscreen … for which I don’t care at all (see the last screenshot to understand why. I want it so.
I updated this morning to 7.0.2.
I wanted to test DRC … here the surprise … from the night to the day: the SOP doesn’t match … why??
total 29 warnings! Come-on!!! Is it a joke??? each time one updates KiCAD should fall down in these kind of stuff?
I wanted to test DRC. from the night to the day: the SOP doesn’t match … why??
For me this DRC-message is really self-explanatory (but I must admit that there are often questions regarding this exact DRC-error - so it may not that obviously than I think).
The DRC states:
footprint “xyz” doesn’t match copy in library
so either you have changed the footprint on the board-editor (unlikely, as the warning was not at v7.0.1)
or the footprint has changed in the library
as you state that you have updated kicad:
only you know if you also have updated the libraries (there are two update-packages available - with and without libraries, at least for windows)
so with updated libraries it’s very well possible that the footprint has changed - this is the nature of an update
It’s now your responsibility to decide:
leave the “old” footprint? At least the board was already produced and worked - so no need to update
or update the footprint
The DRC is only a tool - you have to decide which checks are useful for you. You should understand the checks - otherwise you are a slave to the DRC.
Maybe for you it’s better to disable this DRC-check?
I didn’t touch anything. The project was finished 4 days ago.
I just opened it because it was one of the first in the list of “recent project” to see the 7.0.2.
Not any library was touched ever since
I updated kicad just by clicking on the .EXE for the installation.
If that is the case , than the drc-warning would be a false warning. Happens sometimes, and would hint towards a bug.
Nonetheless I still don’t believe that, I believe you also updated the libraries - and with a library-update it’s very well possible that a footprint was changed.
I updated kicad just by clicking on the .EXE for the installation.
This information is not enough. To judge if the exe includes the libraries (or not) I need the exact filename.
You could also look at the file-size:
kicad_update.exe with > 1GB: includes libraries
kicad_update.exe with ~ 250MB: lite-version, doesn’t includes the libraries
You could also look at the library-files in your installation (library “Package_SO”) and check the last-changed date of the file.
If you don’t want the newest libraries you could update with the kicad 7.0.x testing-builds (download always some days after appearance of new kicad-version) from Windows Downloads | KiCad EDA There you will find lite-versions without libraries.
I checked in GitLab and that specific footprint hasn’t change between releases:
However, if in v7.0.1 you used a footprint from your own library or another library, and now v7.0.2 is comparing it to its default library (maybe your personal libraries are not configured yet, etc.).
yes, thats the full-blown installation and includes the complete libraries. If you use that full installation there is always the possibility to get an changed/updated footprint and therefore the “footprint doesn’t match library” warning.
I checked in GitLab and that specific footprint hasn’t change between releases (der.ule)
If that’s the case than there should be no warning and it could be a bug with this special case.
At this point I can’t help anymore, because I don’t have these original libraries installed (neither from v7.0.1 nor from v7.0.2) to reproduce these issue.
To investigate further one would need to manually compare the existing footprint in the board-file with the footprint in the library and look for differences. As this is tedious there was a feature added to display the differences between board-footprint and library-footprint, but these feature is only available in the nightly development version v7.99 (and will not be backported to v7).
However, if in v7.0.1 you used a footprint from your own library or another library, and now v7.0.2 is comparing it to its default library (maybe your personal libraries are not configured yet, etc.). Just a thought.
No, this case would create a warning message similar to “library for footprint xyz not installed”. The “footprint == library-copy” - check should test if it compares the correct footprint with the correct library.
@tormyvancool : my recommendation:
for the existing board: switch off these DRC-check (as the current board-version with the currently used footprints is ok)
for new boards or the next development-round of that board: switch the check on to get the actual footprint-versions from the library, than again switch off.
In 7.0.2, it appears that if you change any of the attributes of the footprint (e.g. change the fabrication attributes or change (or add) the 3dModels), you will get that error. It seems to be saying that the footprint you are using is different from that which is in the library… not necessarily that the library model has changed. In a board that I have, there are 4 footprints that elicit that error/warning. Three of them have the “Exclude from position files” and “Exclude from Bill of Materials” boxes checked… the 4th one has different 3dmodel file declared. Knowing what they are, I then select the error/warning to be excluded and not shown any more.
Yet another reason everyone making production boards should start by building personal libraries. Sheesh, as a quick start, just copy the stuff you like from the kicad starter libraries, and stick it somewhere you wish:
or something like that. Then you have full control of your own libraries.
Of course, each footprint has a link to the 3d model, which is a bunch of text editing to change it to point to your new folder, but I did a batch edit of all my footprints to change them. Something like this:
eg: to replace ‘wrl’ with ‘step’ in all files in current folder:
$ find . -maxdepth 1 -type f -exec sed -i ‘s/wrl/step/g’ {} ;
where, for sed:
-i is in-place (save back to the original file)
s is substitute
g is global (replace all and not just the first occurrence)
which you can tweak to substitute anything in hundreds of files at a time.
(of course, copy the folder before doing this)
