Hi,
That RS-274-X spec has more holes than Swiss Cheese. For example: If you start a Poly Fill and use a ARC I guess the ARC becomes part of the the poly edge, correct? Doing so results in a polygon with circular voids. This is a huge area for "Interpretation Errors" in gerber processors. Now add to the fact that these polygons could be in clear or dark areas of a single layer and the multiple layers COULD be combined. Good luck finding 2 gerber processors that render this to the same film image. Chance are about 5% that you get a call from the PCB vendor. Chances are 95% that you get back a bad PCB. Worse yet the location for finding errors in circular voids is in an internal plane. Shorts in a plane are like an unforgivable sin, nothing can save you. After many years of doing PCB designs and the writing of a gerber reader (MUCH more difficult than writing gerbers) my suggestion is Keep It Simple (KISS Solution). The generation of gerbers and their resulting rendering to film must be ABSOLUTLY PERFECT. We live and die by this level of perfection. To achieve this level of perfection think of a gerber as a vector driven bitmap. No Aperture Macros and no Polygons need to apply. Even if 99% of the code in the industry reads and processes PERFECTLY that 1% is a reason NOT to use them. We need ROCK SOLID routines for flattening a higher level structure of shapes. The output is a set of scan lines that paints the required image. I write in Delphi, I can easily generate .dlls, and the resulting scan lines could convert directly to KISS generation of gerbers. I have a simple gerber reader that is used to read from LOTS of different apps. It took years learning what liberties every app programmer could take with gerber generation. Lets NOT to the same thing in DRIVING film plotters. Summary: We live or die with gerber generation. If we even need to talk to a fab house about gerber processing we are dead meat. I would love to see a solution got this gerber generation issue. Thanks, Bob Kondner _____ From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of Geoff Harland Sent: Friday, September 21, 2007 12:06 AM To: Kicad Users Subject: [kicad-users] Re: composite layers and negative plots 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. Get it now <http://au.rd.yahoo.com/mail/taglines/default_all/storage/*http:/au.docs.yah oo.com/mail/unlimitedstorage.html> .
