kicad-developers team mailing list archive

[Cirilo Bernardo <cirilo.bernardo@xxxxxxxxx>]

I think a big problem which is not in our control was already
mentioned by Jean-Pierre: some Gerber readers do not accept
the longer decimal strings. So even if you could detect and fix
intersecting polygons in inch units you also have to ensure that
defective readers don't choke. UCAMCO have declared that no
one is obliged to support such defective products and in fact
discourages such support in order to promote more uniform
behavior of software, but the reality is that there will be
defective software out there for a very long time. Since there
seems to be no problem with mm output I'd say it's a non-issue.
If anyone has Gerber software which will not display a mm file on
an imperial grid I would question the suitability of that software.

- Cirilo

On Thu, Aug 6, 2015 at 1:00 AM, Chris Pavlina <pavlina.chris@xxxxxxxxx>
wrote:

> Agreed 90%. I don't have so much of a problem with "fixing" the
> dimensions as long as they're only fixed in the Gerber export, not in
> the master - it's just part of exporting, you're rendering things with
> the features available to you in the destination format. But that's a
> minor point, obviously I don't want to turn the alternative units back
> on if they don't work. I wasn't aware of this problem.
>
> On Wed, Aug 05, 2015 at 10:56:02AM -0400, Wayne Stambaugh wrote:
> >
> >
> > On 8/4/2015 3:03 PM, jp charras wrote:
> > > Le 04/08/2015 08:29, Lorenzo Marcantonio a écrit :
> > >> On Tue, 04 Aug 2015 05:38:26 +0200,
> > >> Chris Pavlina wrote:
> > >>>
> > >>> pcbnew used to be able to plot Gerbers in imperial units. What
> happened
> > >>> to that? Some (particularly older and non-Asian) board houses still
> > >>> expect those... Is there any reason they were removed, or did they
> just
> > >>> "fall out"? And can they be put back in?
> > >>
> > >> Since the new plotting infrastructure the gerber plotter already
> > >> supported both units; the IN was simply the compatibility default and
> it
> > >> only needed an UI option to be bound.
> > >>
> > >> If someone changed the default without adding a radio button or
> > >> something then blame to him:P
> > >>
> > >> AFAIK there would be no technical reason to not do inch plotting...
> > >>
> > >
> > > There is a technical reason to not do inch plotting.
> > > I recently explained it.
> > >
> > > Pcbnew internally uses nanometers, corresponding to 6 digits mantissa
> in
> > > Gerber.
> > >
> > > If we use a 6 digits mantissa and mm in Gerber, there is no rounding
> issue.
> > > If we convert these values to inches, I am pretty sure rounding issues
> > > will appear.
> > >
> > > For most of coordinates, a rounding issue has no matter.
> > > However, for complex polygons (copper zones) rounding coordinates can
> > > create self intersecting polygons from non intersecting polygons.
> > > Self intersecting polygons are not allowed in Gerber files (see gerber
> > > file format spec).
> > >
> > > The advice from Ucamco is (especially for this issue) is:
> > > use the max resolution for coordinates (see also the gerber file format
> > > spec).
> > >
> > >
> > > The only one reason the 5 digits mantissa option exists in Pcbnew is
> the
> > > fact Ucamco told me a few Gerbers tools do not accept the 6 digits.
> > >
> > > I verified some Gerber files which are OK with 6 digits mantissa create
> > > self intersecting polygons when using 5 digits from the same board.
> > > (Tests with GC-Preview)
> > >
> > > (to tell the True, the Gerber image on screen was the same)
> > >
> > > We already have a bug report about self intersecting polygons in Gerber
> > > files from Kicad.
> > >
> > > It also explains why a Gerber reader can gives warnings about that
> > > issue, and an other Gerber reader does not find any issue: it depends
> > > also on internal units of the reader.
> > >
> > >
> > > Therefore, until someone give me a *very good reason* why inches are
> > > better than mm in Gerber files, I *do not want* a inch option in Gerber
> > > plot menu ( or, if this option exists, commit an algo to avoid self
> > > intersecting polygons).
> > >
> >
> > I'm going to side with JP on this one.  Simply enabling the conversion
> > from the internal nanometer units to inches for gerber plotting is not
> > an acceptable solution no matter how harmless it may seem on the
> > surface.  The combination of loss of precision and the floating point
> > rounding errors can potentially lead to self intersecting polygons as JP
> > has mentioned.  Whether or not these errors are significant is design
> > dependent.  It's most likely that they would not result in an issue for
> > most designs but I would rather error on the side of caution on this
> issue.
> >
> > Any solution to this problem must include an algorithm to detect and
> > potentially correct the problem.  The issue I see with this is the
> > correction algorithm.  Programmatically fixing the self intersecting
> > polygons when they occur may or may not be what the user intended.  The
> > question then becomes what to do about.  One option is to warn the user
> > and tell them to fix the offending object dimensions.  Another option is
> > to fix the offending object and warn the user of the change.  I would
> > oppose silently fixing the offending objects without the user's
> knowledge.
> >
> > _______________________________________________
> > Mailing list: https://launchpad.net/~kicad-developers
> > Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
> > Unsubscribe : https://launchpad.net/~kicad-developers
> > More help   : https://help.launchpad.net/ListHelp
>
> _______________________________________________
> Mailing list: https://launchpad.net/~kicad-developers
> Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
> Unsubscribe : https://launchpad.net/~kicad-developers
> More help   : https://help.launchpad.net/ListHelp
>