kicad-developers team mailing list archive
Mailing list archive
Re: Github part footprint filenames
On Tue, Aug 20, 2013 at 08:03:54PM -0400, Chris Morgan wrote:
> one part footprint per-file, and use of the new s-expression format. I
> was wondering though why this format isn't the default yet? I have a
> June stable build.
AFAIK the code isn't ready, yet.
> So I was trying to figure out how we might name files that were stored
> in github. If we begin by assuming that pcbnew will use github
> directly, how should part footprints be named? Does the name inside of
If you were crazy an 'official' name is the IPC footprint name. Totally
unreadable of course! Search for 'IPC-7351B Naming Convention for
Standard SMT Land Patterns' (it's free), and be aware the revision C is
> I'm trying to figure out how we can have kicad use the blob sha. Doing
> so would let us avoid issues where the filename was the same but the
> content differed.
Probably the whole footprint-table system will handle it :P
Also, consider that pcbnew copies the footprint (unlike eeschema), so
once it get inserted it is not 'vulnerable' to library changes.
As usual, library naming is more a personal/organizational issue (since
the standard is most unfriendly I refuse to use it). Actually often the
'built in' library is often designed with different technology
parameters so at the end I always had to redraw most of the component,
with any cad... Just pick a rule and do it consistently. I do it this
way and find it useful, YMMV...
- First of all each technology uses a different lib. So 0,2mm
clearance parts have the save name as 0,1mm clearance one. but they
live in another lib (another folder, actually). The fabrication level
is part of the technology (there are exception, but these are
- Run-of-the-mill chip components are named a R, L, C followed by their
EIA size. So R0603 is a 1.6mm resistor, then. This is because at least
here in Italy the metric designation is not really used for these;
also there is an ambiguity for a couple of sizes.
- Molded tantalum are CPxxxx-y where xxxx is the metric case and y is
the Kemet package. Yes, Kemet, because we found that these are not
always compatible between brand, since the pin lenght varies... anyway
CP7343-D is a typical example.
- Aluminum capacitors are CPCASE-y where y is the Panasonic case.
Actually these *are* interchangeable, usually, so probably they could
be named with their size, too.
- Most other components are named preferably from the JEDEC name, or the
EIAJ name, or the manufacturer one, followed by the pin name pattern
(or nothing if numeric). Alternative names are stored in the tags. By
the way there are too many SOT23 variants around... example TO236 is
a numbered SOT23, TO236-AnK is a single diode in SOT23. Of course
MO220WGGD1 is not very readable as a name but at least is shorter
than the IPC one.
Example of manufacturer specific packages: NATIONAL-TJ7A is a D2PAK
regulator (IIRC), LINEAR-MSOP12 is a non-standard MSOP12 used by some
- Other stuff is named with the name of the component/series. Example:
WE-PD2-L is a Würth PD2 L-size inductor, which is *almost* the same as
SDR0805 (which is a Bourns SDR0805 inductor). Almost because the PD2
is bigger so even if the pads are the same, the courtyard is not!
- Parts with have an industry-standard size but no official size are
named from the component used as a representative. Example:
FINDER-40.52 is the typical 5-mm pitch, 2 form-C contacts relay.
- Really unique components use the component name. CB1aH-P is a huge
relay with trifurcated pins (fun to desolder).
- Solder mask is the same as the pin; the fabricator does
- I keep silk/assembly to the maximum material position and pre-trim
silk against pad (since mask enlargement is done by the fabricator we
can't use the builtin feature).
- Silk/refdes size are a big issue since they depend *a lot* on the
fabricator. I use the 'standard' 1.2/0.12mm sizes but the old
technology based on 0.2mm screen is still very common :(
Hope I have given some good ideas