Strange circles in the gerber


Strange circles in the gerber.

The board house says, “Could you please tell me about the indications of two red arrows?”

The only meaning for the two big circles I can think of is, “Torby doesn’t know how to use KiCad.” I’m not sure which gerb this is, perhaps front silk?

I’ve looked at the gerbers with the gerber viewer and don’t find them there, but it does draw the board way down below and to the right of center.

I think I plotted these as format 4.6. Perhaps he needs 4.5?

I have KiCad version 4.0.2 stable in windoze 10.


What does GerbView render them like ?
Are they circles, or ARCs ? - one looks to have a break, inside the PCB area.
If they are arcs, maybe they rendered the ‘wrong way’ - do you have large radii arcs within the PCB ?


Also try with gerbv for a second opininion


A collection of gerber viewers you can use to double-check:

Also, can you make out where the center of those circles is relative to your board outline in your original layout in pcbnew (with that pic from the fab)?
Is it the absolute origin (0,0)?

I did some paintshop on the image.
The yellow stuff should help determine the center of the arcs by using the board outline in pcbnew.
The red rectangles mark out the culprits I’d say. The arcs start in a corner of them, but don’t end there. Something in those footprints arc definitions (silkscreen, etc.) has gone bad.


Did you use option Use auxilary axis as origin for plot reference point? I had similar issue long time ago when I check this option.

Gerber File Errors due to Edge Cuts not connected

Mitch Davis of Hackvana worked out what was going wrong. Use the 4.5 output format rather than the 4.6 format and see if the fab has the same problem. Let us know if that fixes things for you. As Kerusey points out, using the auxiliary axis as origin is the other condition necessary to expose this bug. The bug is in the CAM software, not KiCad.


Which CAM software, and what exactly is the bug ?
I’ve seen reports elsewhere of gerber tools struggling with circle/arc commands.
Does Pcbnew have an option to disable circle/arc ?
I see a cryptic
“include extended attributes” option, but unclear what that actually suppresses ?


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.


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 “

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.


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 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