kicad-lib-committers team mailing list archive

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

Ok, let's have both the refdes and the value on the fab layer.

On Sep 12, 2016 03:33, "jp charras" <jp.charras@xxxxxxxxxx> wrote:

> Le 12/09/2016 à 03:50, Carl Poirier a écrit :
> > The ECO layers are not paired. When you flip a footprint, the value
> stays on the same ECO layer.
> > Jean-Pierre, how is that a problem if the value is purely for user
> reference?
>
> Yes, *currently* this is a problem (due to the fact the Pcbnew behavior is
> based on the fact there
> are different layers for flipped and normal fotprints, and some are paired)
>
> - Texts not on a paired layer are not mirrored (the back side of a board
> will be not easy/not
> possible to print)
> this is the major issue.
> - You cannot have different colors or visibility for flipped and not
> flipped values
> - you cannot always print the footprints only on the top or only on the
> bottom board side (they have
> a common layer).
> - in select/edit, you cannot have a priority to the overlapping text
> values on the selected layer
> (because it it the same)
>
> But what is the problem with the current convention (values in fab layer) ?
> - values can be set as invisible (empty string is not good because in a
> library it is a dummy text
> replaced as soon as a netlist is read)
> - even with visible values you can easily enable or disable them in plot
> and in display options.
>
> In other words, what problem do you want to fix?
>
> >
> > On Sun, Sep 11, 2016 at 9:26 PM, Jean-Paul Louis <louijp@xxxxxxxxx
> <mailto:louijp@xxxxxxxxx>> wrote:
> >
> >     in 40+ years of electronic manufacturing, I almost never saw values
> in silk screen.
> >     RefDes are fine for sparse boards, but useless with very dense
> boards.
> >     Values could be on some user layer, or maybe in one of the ECO
> layers.
>
> Currently they are on the fab layer, which was added especially to put
> items which cannot be put on
> the silk screen.
>
> >
> >     Just my $0.02,
> >     Jean-Paul
> >     N1JPL
> >
> >
> >
> >
> >     > On Sep 11, 2016, at 6:00 PM, Oliver Walters <
> oliver.henry.walters@xxxxxxxxx
> >     <mailto:oliver.henry.walters@xxxxxxxxx>> wrote:
> >     >
> >     > What if we set it invisible by default, and on the F.SilkS layer?
> That way the fab houses
> >     don't have to deal with it, and if any users want to display it,
> they just have to toggle the
> >     visibility.
> >     >
> >     >
> >     > On 12 Sep 2016 07:52, "Carl Poirier" <carl.poirier.2@xxxxxxxxx
> >     <mailto:carl.poirier.2@xxxxxxxxx>> wrote:
> >     > Hi Jean-Pierre,
> >     >
> >     > I had not noticed this, thanks. The general consensus seems to be
> that values are not useful
> >     on the silkscreen layer. The comments from the assembly house
> reported by Vesa say the same.
> >     Maybe it would simply be better to leave the value field blank by
> default?
> >     >
> >     > Carl
> >     >
> >     > On Sun, Sep 11, 2016 at 7:00 AM, jp charras <jp.charras@xxxxxxxxxx
> >     <mailto:jp.charras@xxxxxxxxxx>> wrote:
> >     > Le 11/09/2016 à 04:01, Carl Poirier a écrit :
> >     > > Hi folks,
> >     > >
> >     > > Following comments
> >     > > <https://forum.kicad.info/t/why-are-the-kicad-library-
> conventions-non-ipc-compliant/3678/65
> >     <https://forum.kicad.info/t/why-are-the-kicad-library-
> conventions-non-ipc-compliant/3678/65>> on
> >     > > KiCad's forum about the KLC, I went on to make a few adjustments
> to the KLC. They can be
> >     seen here
> >     > > <https://github.com/KiCad/kicad-library/issues/687
> >     <https://github.com/KiCad/kicad-library/issues/687>>.
> >     > >
> >     > > Do any of you have comments about the changes?
> >     > >
> >     > > Regards,
> >     > >
> >     > > Carl
> >     > >
> >     > >
> >     >
> >     > Yes, for this change:
> >     > "10.4: Value is filled with footprint name, has a height of 1mm
> and is placed on the Eco1.User"
> >     >
> >     > Value can be put only on a paired layer (currently only Fab or
> Silk for a text) like any graphic
> >     > item of a footprint in a footprint library.
> >     > ECO1 layer is not paired with ECO2 layer.
> >     >
> >     > It means all flipped footprints will have a broken value text if
> on ECO1 layer.
> >     >
> >     > The "old" 10.4 rule is the only one possible option.
> >     >
> >     >
> >     > --
> >     > Jean-Pierre CHARRAS
>
>
>
> --
> Jean-Pierre CHARRAS
>
> --
> Mailing list: https://launchpad.net/~kicad-lib-committers
> Post to     : kicad-lib-committers@xxxxxxxxxxxxxxxxxxx
> Unsubscribe : https://launchpad.net/~kicad-lib-committers
> More help   : https://help.launchpad.net/ListHelp
>