[PROTEL EDA USERS]: Gerber file arc commands (ex Re: Drill Drawing)

["Geoff Harland" <gharland@ingenico.com.au>]

<snip>
> By the way, another device for reducing gerber file size is to turn off
> software arcs. This will permit Protel to use the gerber arc command
> instead of drawing many individual segments. The only down side, unless
one
> is using an antique plotter, is that someone who is trying to import the
> files into an older CAD program might find it difficult. I only mention
> this because I used to be in that position....

I don't know if it is still a problem in practice, but I have reason to
believe that not all PCB manufacturers could (/can?) be counted upon to be
able to properly handle Gerber files incorporating (gerber) arc commands,
and as such, the safe/conservative way of coping with this possibility was
(/is?) to avoid the use of arc commands.

Another complicating factor is that the RS274D standard went through a
revision in defining arc commands. I have an idea that in the first version,
the maximum angle of arc (for each arc) was 90 degrees (and individual arcs
couldn't pass quadrant boundaries), and there was no support for the *sign*
of the values for the I and J distances (specifying the location of the
arc's center relative to its starting point). In the revised version, those
shortcomings were rectified, but having this revision was yet another
compilcating factor for PCB manufacturers to cope with.

However, a Gerber file that doesn't use arc commands is typically
significantly larger in size; when I tested this aspect on one occasion, the
Gerber files not incorporating arc commands were typically something like
50% larger than the Gerber files that did incorporate arc commands (YMMV;
the ratio depends upon how many arc primitives within the PCB file are to be
represented within each Gerber file).

Personally, I customarily generate Gerber files with arc commands, but
because of the possibility (however small) that the PCB manufacturer might
mangle the resulting PCB, I always include the following message within the
Readme.txt file (that I provide with the Gerber files):

==
NOTES:

1. All Gerber plots are RS274X format, with embedded apertures, and targeted
for a RASTER photoplotter.

2. These Gerber plots contain Gerber arc commands (I and J codes); please
contact me if you are unable to handle such files (so that, if necessary,
you can be provided with (larger) Gerber files which do not contain such
commands).

3. These Gerber plots contain octagonal shaped apertures. All of these
apertures are to have the same orientation as road-side STOP signs. The size
specified within each associated embedded aperture definition is the vertix
to (opposite) vertix distance; the edge to (opposite) edge distance (as
specified in the Protel format aperture file provided) is smaller by a
factor of cosine 22.5 degrees. (These changes to the embedded aperture
definitions have been made to make these comply with the RS274X standard for
defining apertures of (regular) polygonal shape.)
==

(Note 3 refers to another aspect that I have also commented on in recent
times, and is also included within this file when appropriate.)

I customarily use GC-Prevue to preview Gerber files (and NC Drill files),
but I have noticed that at least one of the other Gerber file previewing
utilities available (I can't remember exactly which one(s) offhand) do not
interpret arc commands properly. (It is not out of the question that an
updated version of the application(s) concerned has overcome this
shortcoming, but keep my experience in mind.)

I don't want to frighten users into not using the option of arc commands,
but keep in mind that this might not be a totally "gotcha"-free aspect of
Gerber files. And as both Abdulrahman Lomax and I have observed, the use of
such commands nearly always results in smaller Gerber files. So be
appropriately careful if you do make use of these commands...

> Centering the plots on the film can put objects off grid, and thus the
> savings from trailing zero suppression might not exist. Centering also
> causes the gerber to have a different reference zero than the drill files,
> and for that reason and for others I never allow it.
>
> Abdulrahman Lomax

On that I also agree, and I have said as much on a number of occasions. (It
is a pain previewing Gerber files in conjunction with NC-Drill files when
the Gerber files concerned have been generated with the centered option
selected.)

Regards,
Geoff Harland.
-----------------------------
E-Mail Disclaimer
The Information in this e-mail is confidential and may be legally
privileged. It is intended solely for the addressee. Access to this
e-mail by anyone else is unauthorised. If you are not the intended
recipient, any disclosure, copying, distribution or any action taken
or omitted to be taken in reliance on it, is prohibited and may be
unlawful. Any opinions or advice contained in this e-mail are
confidential and not for public display.