One CAM program known to have problems is an old version of CAM350. A number of gerber viewers also struggle, but that is a coincidence and not quite the same problem. The “extended attributes” can be ignored; that is for additional information to be included in the Gerber files. At this point I’m not even sure what additional information is put in there but it is to support Revision J1 and later of the Gerber RS-274X specification.
Hmm, we also had a board break a few years back, by someone using CAM350.
They edited the gerbers, (for some reason) and CAM350 decided to re-order the plotting…
That’s fine in a simple, stroke-line image, but this plot used LPC voids, and they vanished by virtue of being done too early. Serious PCB errors resulted…
Many PCB tools can disable the fancier gerber options, and this can be a good idea if you want absolute control over the final PCB.
PcbNew could/should consider that too, yes, creates a slightly more verbose file, but you really do know what you will get.
The rendering error the OP shows, does look like an ARC command inside gerbers ‘gone wrong’.
An option to remove the ARC simple avoids the issue entirely.
Re. the circles - we did establish early on that using 2x half circles avoids the problem altogether. There was some debate about what to do, but the vote against a kludge to support Old CAM Software was almost unanimous; after all if we support Buggy Software X version 0.Z how many kludges will we be spending time on in the future? If using “4.5” format fixes the problem then that’s just as good and already supported - no need for a kludge.
3 Likes
I switched to 4.5 and made sure I don’t have “Use auxiliary axis as origin” checked. I didn’t.
We’ll see what the board house thinks of them now. I use “Elecfreaks.com”
Posted from home where nobody cares what I wear
I can follow the kludge logic, but there is more of a case for optional removal of Gerber Circle commands.
ie instead, Plot uses the same segment count KiCad uses internally for rendering, so you really are WYSIWYG, and export arcs/circles as polyline segments. (possibly with user choice?)
No kludge here, and full user control.
As soon as you export too much intelligence, your PCB design becomes more and more a mere request,
You are never sure what the other tools may generate.
On some tools this is under a switch for RS274D / RS274X
You could also send the a screen shot of what GerbView shows it like, as you need to encourage them to upgrade their Gerber Software…
Hehe, na, that doesn’t work. The fab(s) in China with the outdated CAM350 system couldn’t care less.
Personally I avoid arcs/circles on silkscreen completely because of stuff like this as it’s way safer.
For outlines I never had the problem yet and they accepted pretty insane things so far.
… and they are probably cracked copies too…
Still, they start to care, when enough customers ask, and giving them a proven good render proves they are using defective tools.
Yes, safer is why I suggest above a means to remove the ARCs from the gerber files,and render as polylines.
Well, at the start I always put a 3d view screenshot of the board into the zip file with the gerbers and in problematic cases also had forth and back with the aggregator.
In the end they canceled my order, gave me my money back and I lost 2-3 weeks on this for 2 times.
I just don’t bother with it anymore.
Haven’t heard any complaints from ElecFreaks. Yet.
I used the 4.5 setting and got no complaints from the board house. Boards arrived today, well, I had to go to the PO to pick them up.
It’s 50mm by 50mm. Elecfreaks made me 10 copies for 16USD. Quality is very nice, but you have to be patient.
1 Like
That’s good. As for the strange circles, I could be confusing things a bit. In the first try did you create Gerbers with imperial units?
I created the gerbers as 4.6 format files, but that seems to be too new for elecfreaks.com to deal with. I used 4.5 format files and those worked fine. Don’t know anything about imperial units as I don’t see such an option in the plot dialog.
Well, ok, I DO know about imperial units, 12 inches to a foot, 3 feet to a yard, 220 yards to a furlong, 8 furlongs to a mile, but that doesn’t have much to do with plotting gerbers
Well, here it is and ready to light off.
Only once have I made a board that could not be made to work
I fixed the footprint footprint. The two vertical lines were in the image file I made the footprint from.
So far so good. It runs programs and twiddles bits.
RF section works.
And the motor controller works! This board’s good.
Oh man, I had this problem with a board recently but thought they drew the circles to indicate something and it kept going back and forth with me saying “I don’t see anything wrong in the picture”. They ended up fabbing the boards without silkscreen 
.
Will make sure to set the output to 4.5 next time, thanks for this post and the responses!
I often dive in and ask what may be a dumb question figuring if I stumbled over it, others have too.
I know this is very old but in case people have future issues with this weird circle, my problem was that my lines weren’t perfectly connected. I uploaded a DXF file for the edge cuts of my board (weird shape, not your typical rectangle) and I realized that in autocad, my lines weren’t perfectly. connected. After fixing that, the circle went away. Hope this helps.
I know this thread is old, but I had this exact issue now when ordering things from allpcb.com (one of those Chinese manufacturers) and I want to record my experience in case anyone else has the same problem in the future. They told me the the gerber files looked like this:
But looking through all the files with 3 different gerber viewer programs showed NO PROBLEM.
Thus I conclude that their gerber reading program is the issue.
After reading this thread I changed two things:
- Use auxiliary axis as origin = TRUE (making origo in the middle of the board instead of away in the distance towards the upper left)
- Changed gerber file format from 4.6 to 4.5 (decreasing the numeric resolution of the placements)
The PCB manufacturing house replied that the result looks OK now.
Good luck!
2 Likes
Glad my old topic was helpful. I get nice quality from my disreputable Chinese board house (elecfreaks.com), but I have to use format 4.5.