kicad-lib-committers team mailing list archive

[Carl Poirier <carl.poirier.2@xxxxxxxxx>]

These have been added to the KLC as a new section. Thanks all for
participating to the discussion and thanks to Michal for the initial
suggestions.

On Sat, Jan 31, 2015 at 7:05 PM, Carl Poirier <carl.poirier.2@xxxxxxxxx>
wrote:

> OK, so with the discussed changes, we get this:
>
> 3.7 wil become 1.7 and apply convention-wide: Reference fields are
> prefilled with the reference designator of the part (IEEE 315-1975).
>
> 6.10. Text is placed on silkscreen and uses a height of 1mm.
> 6.11. Doc property contains a full description of footprint.
> 6.12. Keywords are separated by spaces.
> 6.13. Value is filled with footprint name.
> 6.14. Attributes is set to the appropriate value, see tooltip for more
> information.
> 6.15. All other properties are left to default values. (Move and Place:
> Free; Auto Place: 0 and 0,  Local Clearance Values: 0)
> 6.16. 3D Shape ".wrl" files are named the same as their footprint and are
> placed in a folder named the same as the footprint library replacing the
> ".pretty" with ".3dshapes".
>
> I will amend the convention shortly.
>
> On Mon, Jan 26, 2015 at 3:34 PM, Carl Poirier <carl.poirier.2@xxxxxxxxx>
> wrote:
>
>>
>> On Mon, Jan 26, 2015 at 10:23 AM, Wayne Stambaugh <stambaughw@xxxxxxxxx>
>> wrote:
>> >
>> > On 1/26/2015 6:49 AM, jp charras wrote:
>> > > Le 26/01/2015 02:46, Carl Poirier a écrit :
>> > >> Hi MIchal,
>> > >>
>> > >> This is the wording I have for now.
>> > >>
>> > >> 6.11. Doc property contains a full description of footprint.
>> > >> 6.12. Keywords are separated by spaces.
>> > >> 6.13. Reference is filled with footprint name.
>> > >
>> > > Perhaps better fill value with footprint name.
>> >
>> > Using the footprint name as the default value field makes sense to me.
>> > I would also like to see visibility of the default value field set to
>> > hidden.  I don't think I've ever seen a board with component values on
>> > the silkscreen layers.  I know I've never the luxury of that much extra
>> > room on any boards that I've designed.
>> >
>>
>> That makes sense to me, but indeed we need to change the default values.
>>
>> > >
>> > > Reason: reference is usually a short word (like Uxxx).
>> > > Value and footprint name are usually a more long name (like 330K-1% or
>> > > BGA_0.5_128x128).
>> > > So, the default values (which will be replaced by they actual values)
>> > > are more representative of these actual texts.
>> > >
>> > > Also, avoid too long names for fp names and 3d shape names. They
>> always
>> > > create issues.
>> >
>> > Please consider this advice.  There are some footprint names that are
>> > really long which makes displaying them less than ideal.  I'm not saying
>> > there will never be long footprint file names, I suggesting that we make
>> > them no long than necessary.  I don't see revision and date information
>> > in the file name as necessary.  Add this to the description field if
>> needed.
>> >
>>
>> Eradicating revision and date from footprint names has been mostly done
>> by Dick already.
>>
>> > >
>> > > Just my 2 cents, or, if you prefer, my 2€ (looks like the same, now).
>> > >
>> > >> 6.14. Attributes is set to the appropriate value, see tooltip for
>> more
>> > >> information.
>> > >> 6.15. All other properties are left to default values. (Value:
>> VAL**, Move
>> > >> and Place: Free; Auto Place: 0 and 0,  Local Clearance Values: 0)
>> > >> 6.16. 3D Shape ".wrl" files are named the same as their footprint
>> and are
>> > >> placed in a folder named the same as the footprint library without
>> the
>> > >> ".pretty".
>> > >
>> > > Perhaps the folder could be named the same as the footprint library
>> > > without the ".pretty" but with something like *.3dshapes or _3dshapes*
>> > >
>> > > This is more easy to filter and list with fp lib wizard.
>> > >
>> > > Wayne, what is your opinion?
>> >
>> > I'm OK with either .3dshapes or _3dshapes for the model paths that we
>> > provide.
>> >
>>
>> .3dshapes sounds good to me.
>>
>> >
>> > >
>> > >>
>> > >> For the text size, I'll have to check for the default value. If it's
>> not
>> > >> 1mm, I'll ask to make it the default.
>> >
>> > Whatever size you make the default text, please do this for all symbols
>> > including the power symbols.  As of right now the default text sizes are
>> > all over the place.  This is really bad for power symbols because you
>> > cannot edit power symbol fields in Eeschema.  Yes, you can edit the
>> > schematic file by hand or modify the power symbol library but neither
>> > solution is friendly.
>> >
>>
>> For symbols, it's been decided a good while ago that text size was
>> 50mils. The question here was for value and reference in footprints. Right
>> now the default is 1.5mm.
>>
>> > >>
>> > >
>> > > Carl and all contributors to the Kicad Libraries: Thanks!
>> > > I know this is a hard work, with very few reward from users.
>> > >
>> >
>> > Thank you Carl for taking the lead on this.
>> >
>> >
>>
>> You are welcome. I have got a hand from some other members for
>> elaborating the convention, mainly Lorenzo, Jean-Paul and John. Kerusey has
>> helped a lot approving pull requests and contributing as well as Michał
>> Stec more recently.
>>
>
>