kicad-developers team mailing list archive

[Chris Pavlina <pavlina.chris@xxxxxxxxx>]

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