Hi Ben,
I have a copy of the RS274X specification, and this states that the G36 and G37
commands are actually used to turn on Polygon Area Fill and turn off Polygon
Area Fill (respectively). There are other commands which can be used to change
the "polarity" of a Gerber file's contents (i.e. whether any "draw" and
"stroke" commands which follow are "dark" or "clear", or "positive" or
"negative" in nature), but the G36 and G37 commands are used in conjunction
with a set of vertexes whose associated region is to be entirely "filled". The
related specification specifically states:
"... G36 and G37 provide a more efficient means of filling closed polygons than
stroke fill. When these codes are used, the filled area is defined simply by
its closed outline. Stroke fill is an inefficient method of filling a polygon.
..."
I haven't studied the relevant (source) code (for KiCad) in depth, but I am
still picking that the G36 and G37 commands have deliberately been used because
it is far easier to depict "poured" copper areas within Gerber files by using
those commands rather than by using "stroked" fills instead.
It probably would be possible to make changes to the relevant source code so
that users subsequently had the option of generating Gerber files using the G36
and G37 commands (the existing way), or otherwise by using "stroked" fills
instead. That said, while I can't speak for any of the other developers, my
personal attitude is that I would rather spend the limited amount of time that
I have available (for improving KiCad) in implementing various other
improvements.
While that attitude might seem harsh or unreasonable, I am also of the view
that PCB manufacturers *should* be able to cope with any Gerber files whose
contents are fully compliant with the RS274X specification. If you, or anybody
else, can provide proof that any Gerber files created by KiCad are *not* fully
compliant with that specification, then I would be fully prepared to look at
the relevant source code, and make any changes which would be necessary to make
those files fully compliant. But as I don't have unlimited time available for
making improvements to KiCad, I am not of an inclination to make any changes
for the benefit of any PCB manufacturers who are not capable of dealing with
any Gerber files which they *should* be capable of dealing with.
Given the circumstances, my advice would be to advise the PCB manufacturer
concerned that other PCB manufacturers are capable of dealing with Gerber files
which incorporate G36 and G37 commands, so unless they are able to prove that
there are any genuine problems with the contents of any Gerber files which you
have provided to them, then you will look at taking your business elsewhere.
While my response probably hasn't matched what you were hoping for, please note
that I still monitor all of the messages sent to this mailing list, and that I
am fully prepared, in general, to attempt to rectify any reported defects and
implement any requested improvements which are submitted by users (whenever my
available spare time, and my comprehension of the relevant source code,
permits).
Regards,
Geoff Harland.
"barkerben" wrote:
>
> I think the problem occurs when I pour copper areas:
>
> "find out how to generate your copper pour with stroke
> hatch filling instead composites and send your files again"
>
> When I do not pour, there are not G36 or G37 codes,
> when I do they appear. Any thoughts?
>
> Ben
>
>
> "barkerben" wrote:
> >
> > One more question (I have answered the above myself via
> > experimentation). I got the following from Olimex, who I use to etch
> > boards:
> >
> > Hi,
> > Your gerbers contain composite layers and negative plots (G36 G37
> > commands).
> > On such gerbers we can't do DRC check, panelization nor to ensure
> > correct
> > phototools plotting.
> > Please ask your cad vendor how to generate your copper pour with
> > stroke
> > hatch filling instead composites and send your files again.
> > Thanks
> >
> >
> > Can anyone answer his question?
> >
> > Cheers,
> >
> > Ben
____________________________________________________________________________________
Sick of deleting your inbox? Yahoo!7 Mail has free unlimited storage.
http://au.docs.yahoo.com/mail/unlimitedstorage.html
