Been going through a world of pain trying to migrate ;libraries from Eagle to Kicad 8.0…
Some results - I have a large Eagle library of JLCPCB parts. I imported this and it got all the symbols and matching footprints. so far so good.
I then went and looked at the data/properties for the parts and the only thing Kicad had actually imported
was the description. the important attributes fields such as LCSC_PART field was missing. Also
the Eagle library had separate parts for each vale 1k, 2k7 etc in each SMD size. Now all I get is a single generic 0603 resistor with no value.
So if there is a way to import Eagle libraries that actually works I would love to know.
I never worked with “easy eda”, and very briefly with eagle. From my test with eagle I remember there was a list of resistor values I could set a resistor to, and this implies that eagle knows more about each of those resistors. In KiCad it is quite different. In KiCad the value of a resistor is just an editable text string, and that does not translate well between eagle / KiCad. I am guessing that setting up and using the database driven library system in KiCad may be a better choice for you. Setting up such a database does take some effort. But the idea is that the database is independent of KiCad itself. The system is built around the idea that companies already have a working database with parts (ordering numbers, price info, suitable replacement parts etc) and then want to integrate this with KiCad.
Thanks for the info. I did note there was database support in V8 - early days but may have potential as you describe. My workflow in Eagle to JLCPCB was super easy. Native scripts+ Eagle library written by JLC made every thing a few clicks away and fast and flawless.
Having done some database dev. in the dim distant past ( VisualBasic/RealBasic)
I think the issue is not making a database schema, it’s converting the existing data/library to put it in the database.
EasyEDA import - yes it can import individual component symbol/footprints, I don’t think you can just download a whole library of parts in one file though.
I did find a huge Altium library collection of JLC parts which did import - but I need to link footprints. would take a long time as even the smallest of these libraries has 6000+ parts…
Also, like many of these scripts, hacks etc. it’s a bit out of date. I’ve found a few other things but again, abandoned, out of date, broken, doesn’t work with latest Kicad etc. etc.
I think maybe some AI assisted tool might do this - not found anything yet though!
importing a eagle library which contains devices with different variants (different footprints assigned to one symbol) worked on a first try. Note you will get much more kicad symbols (one new symbol per each eagle device variant), as kicad doesn’t know this concept of “device variants”.
you may attach the eagle library which produced only “a single generic 0603 resistor with no value.”. Maybe I’m able to reproduce this behaviour.
all my statements are valid (== extra checked) for kicad v8 and eagle v7.7 ultimate (last version available for purchase == unlimited use)
The library is saved with eagle v8 format. As far as I know the import process is based on the last non-autocad eagle v7.7 documentation. (That’s also the last version I could buy).
The import function correctly detects and imports all symbols with the individual footprint variants. So I get 4 capacitors C__0402 , C__0603 , C__0805 and C__1206
The different values in the JLCPCB eagle library are achieved with adding many “technology” instances to the original “C__” device
These “technology” instances are currently not supported. If this is important for you then you will have to open a gitlab issue for this. (and hope that it get’s implemented).
added information:
There was already a open feature request for this, but it got no support from other users (no single upvote in 3 years now) and got closed some month ago:
I’m not sure if it’s better to reopen the old or to open a new feature request.
