kicad-developers team mailing list archive

[Wayne Stambaugh <stambaughw@xxxxxxxxx>]

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.