I don't know. If anything it would be the most useful to be able to try to repair broken files like that (maybe a script?). Displaying broken files "correctly" is dangerous. One of the main uses for a Gerber viewer is to do a pre-manufacturing check, and if your gerbers are broken and they work in the viewer anyway it could be a problem.
On Thu, Sep 28, 2017 at 12:47 PM, Seth Hillbrand <[email protected]> wrote: > Looking at gerbv right now, it appears to silently handle decimal places > if they exist. However, in the absence of an explicit decimal place, it > treats %FSD as %FSL, which is probably why Clemens' file was correctly > displayed, as opposed to being oversized by a factor of 100. > > Personally, I would love to see Kicad following a robustness principle > that allows more files to be displayed but with a definite warning message > detailing the formatting error and cautioning that the file _may_ not be > correctly displayed because of the bad format. > > Best- > Seth > > > > On Thu, Sep 28, 2017 at 9:17 AM, jp charras <[email protected]> wrote: > >> Le 28/09/2017 à 17:58, Jon Evans a écrit : >> > Perhaps another route is to improve the messaging given to the user in >> these cases, so that it's >> > easy for them to correct the file / report an issue to their tool >> vendor? >> >> Yes. >> >> In fact, %FSD is already supported by Gerbview because (a long time ago) >> I found Gerber files in >> decimal format (not documented, because %FSD was never a official Gerber >> format statement). >> >> This is the reason no error was reported: coordinates were read as >> floating numbers (in mm) and valid. >> >> >> > >> > On Thu, Sep 28, 2017 at 11:53 AM, Wayne Stambaugh <[email protected] >> > <mailto:[email protected]>> wrote: >> > >> > On 9/28/2017 10:32 AM, jp charras wrote: >> > > Le 28/09/2017 à 16:13, Wayne Stambaugh a écrit : >> > >> On 9/28/2017 9:45 AM, jp charras wrote: >> > >>> Le 28/09/2017 à 01:27, Clemens Koller a écrit : >> > >>>> >> > >>>> On 2017-09-26 13:38, jp charras wrote: >> > >>>>> The Gerber file is broken: >> > >>>>> the line: >> > >>>>> %FSDAX33Y33*% >> > >>>>> >> > >>>>> is incorrect >> > >>>> >> > >>>> Thank you! >> > >>>> >> > >>>> Since I cannot do anything about this proprietary non >> compliant EDA tool, would it be >> > possible to support these wrong but obvious lines anyway (maybe >> after showing a warning) - so >> > would you accept a patch to support the %FSD gerber code? >> > >>>> >> > >>>> Regards, >> > >>>> >> > >>>> Clemens >> > >>>> >> > >>>> >> > >>> >> > >>> A patch is possible, but the actual issue is: >> > >>> What is the meaning of %FSD format? >> > >>> >> > >>> I saw some "Gerber" files using %FSD for a decimal format >> (coordinates in floating point >> > notation), >> > >>> that differs from your Gerber file ( that is in fact a %FSLA >> format, nothing else ). >> > >>> >> > >> >> > >> Unless %FSD is an obsolete gerber command, I'm opposed to this >> idea on >> > >> principle alone. KiCad should not be in the business of >> supporting >> > >> broken file formats created by other tools. The gerber file >> format is a >> > >> published standard and we should be following it as closely as >> possible. >> > >> You should file a bug report with the vendor of the program that >> > >> created these gerber files. >> > >> >> > >> Cheers, >> > >> >> > >> Wayne >> > > >> > > In latest Gerber doc, %FSD appears in "Errors and Bad Practices" >> list and is clearly called >> > Invalid >> > > Format Statement in the "Error" section. >> > >> > In this case we should not support %FSD. >> > >> > > >> > > only %FSLA and %FSTA exit. >> > > %FSTA is now on the deprecated list (Kicad uses the %FSLA option). >> > > >> > > >> > >> > We will have to continue to support these for legacy gerber files. >> >> >> -- >> Jean-Pierre CHARRAS >> >> _______________________________________________ >> Mailing list: https://launchpad.net/~kicad-developers >> Post to : [email protected] >> Unsubscribe : https://launchpad.net/~kicad-developers >> More help : https://help.launchpad.net/ListHelp >> > > > _______________________________________________ > Mailing list: https://launchpad.net/~kicad-developers > Post to : [email protected] > Unsubscribe : https://launchpad.net/~kicad-developers > More help : https://help.launchpad.net/ListHelp > >
_______________________________________________ Mailing list: https://launchpad.net/~kicad-developers Post to : [email protected] Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
