kicad-developers team mailing list archive

[Wayne Stambaugh <stambaughw@xxxxxxxxx>]

Gerber generation is the heart and soul of a board layout program.  Get
this wrong, and all of the fancy editing features are completely
meaningless.  I applaud JP for being very conservative about making
changes to this code.  The last thing we need is for users to end up
with bad boards due to units conversion error in KiCad.  That being
said, I do believe that it is a problem that can be solved.  It is a
matter of whether or not I makes sense to allocate the manpower to solve
a complex issue when our current solution is correct.

Internally pcbnew units are nanometers stored as integers.  Generating
millimeter gerbers with six significant digits is the key.  We never
have to leave the integer domain to generate gerber coordinates.  We get
a 1 to 1 representation of the board.  Where things get murky is when we
starting decreasing the number of significant digits and/or converting
to inches and rounding.  The primary issue is with the polygons used
fill zones.  Each polygon would have to be tested for self intersection
and potential gaps and/or overlaps with adjacent polygons when making
the conversions.  This would most likely have be an iterative process
until all of the polygons where converted and verified against all of
the surrounding polygons for any potential issues.  Again, it's not
impossible but it is a significant amount of work to get it correct.

On 8/5/2015 11:00 AM, Chris Pavlina 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
>