kicad-developers team mailing list archive

[Wayne Stambaugh <stambaughw@xxxxxxxxx>]

Out of curiosity, how does one render an invalid gerber file?  Are we to
assume that %FSD will always have the same meaning between the
applications that generated the gerbers?  If not, then we have to
determine the application that generated them and jump through hoops to
get the rendering correct not to mention the coding mess this creates.
Otherwise we are just guessing and our gerber rendering may not be
accurate which defeats the purpose of a gerber file viewer.

Given my experience with CAD tools, I suspect this was not an accident
but rather the all too common attempt at proprietary lock in although I
have no proof.  If that is the case, then I have zero interest in
supporting this.

I agree we should not attempt to fix broken gerber files.  No good can
come of that.  A warning is fine.

On 9/28/2017 2:08 PM, Seth Hillbrand wrote:
> I agree with your point that gerber viewers act as an important check. 
> Toward that end displaying a warning message should alert the user that
> they have a problematic Gerber file that shouldn't go to a manufacturer.
> 
> Fixing sounds dangerous to me as it modifies a file that explicitly
> doesn't follow a standard.  The resulting 'fixed' file will be
> standards-compliant but could very easily be not what the user intended.
> 
> Viewing non-standard Gerber files would be personally useful to me as I
> often receive gerber files from other engineers at different
> institutions working on a wide range of EDA tools.  Some of them
> generate non-standard gerbers and their users have no interest in
> switching their workflows.  At the moment, I keep 4 different viewers
> installed, two on a virtual machine to ensure that I can look at the
> files.  I would really like to expand the viewing of non-standard files
> in Kicad.  I'm happy to submit this patch if we're open to the idea.
> 
> -S
> 
> On Thu, Sep 28, 2017 at 10:53 AM, José Ignacio <jose.cyborg@xxxxxxxxx
> <mailto:jose.cyborg@xxxxxxxxx>> wrote:
> 
>     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
>     <seth.hillbrand@xxxxxxxxx <mailto:seth.hillbrand@xxxxxxxxx>> 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
>         <jp.charras@xxxxxxxxxx <mailto:jp.charras@xxxxxxxxxx>> 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 <stambaughw@xxxxxxxxx <mailto:stambaughw@xxxxxxxxx>
>             > <mailto:stambaughw@xxxxxxxxx
>             <mailto:stambaughw@xxxxxxxxx>>> 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
>             <https://launchpad.net/~kicad-developers>
>             Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
>             <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>
>             Unsubscribe : https://launchpad.net/~kicad-developers
>             <https://launchpad.net/~kicad-developers>
>             More help   : https://help.launchpad.net/ListHelp
>             <https://help.launchpad.net/ListHelp>
> 
> 
> 
>         _______________________________________________
>         Mailing list: https://launchpad.net/~kicad-developers
>         <https://launchpad.net/~kicad-developers>
>         Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
>         <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>
>         Unsubscribe : https://launchpad.net/~kicad-developers
>         <https://launchpad.net/~kicad-developers>
>         More help   : https://help.launchpad.net/ListHelp
>         <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
>