kicad-developers team mailing list archive

[Jean-Paul Louis <louijp@xxxxxxxxx>]

I do not understand why 6 significant digit will cause rounding error if Gerber generation uses inches as unit.
you have a nanometer resolution which provides 6 decimals for millimeter units.
When you divide this number by 25.4 to convert to inches, you might loose a bit of resolution, but you will not generate a rounding error.
123.456789mm = 4.86050350” wich is now 4.860503 when using only 6 decimals.

Where is the rounding error coming from? From the software processing gerber data? I really doubt that CAM software will care about 1 micro-inch error.

Just curious,

Jean-Paul
AC9GH


 
> On Aug 4, 2015, at 3:03 PM, jp charras <jp.charras@xxxxxxxxxx> 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).
> 
> -- 
> Jean-Pierre CHARRAS
> 
> _______________________________________________
> 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