yeah, and it says ‘experimental’ right next to it, which to me means ‘do not use, unless you want to deal with bugs and unexpected results’ 
But without @mexchip posting what settings he used we can speculate all night or day (depending on which side of the planet we’re on) 
[edit]
Well, here is the plot of @mexchip s project with the nightly from 15th Dec 2018 with my plot settings…
If both gerbv and gerbview show clean Gerber plots, the chances are that they are correct.
Are you absolutely sure that there are no artifacts off screen in these viewers?
btw… if I chose x2 for the drill file plot settings, I get 2 files and not just one.
The original gerbers from @mexchip also only contained the '.drl' file instead of the '-drl.gbr' files, so I assume he didn’t use the x2 format for the drill file either?!
And when I try to upload those zipped with the layer files I get this:
PS: if I remember my past experience with drill holes being way out the way for gerbers it usually was because I did play with the drill plot settings and used imperial or auxiliary axis coords
Thanks a lot for your comments, I’ll upload screenshots of my settings later (I’m not using X2 format).
One possible reason of why you would get much bigger gerber files (especially solder mask) in v5 vs v4 is that standard lib footprints for smd passives now use rounded rectangle pads instead of plain rectangles. In real design you usually have a fair amount of those so if you switched to using new footprint in migration to v5 your gerber will blow up because describing those round corners needs much more data.
That makes sense. Yes, when porting the design I switched to the new symbols and footprints.
And yes, as @eelik pointed out, removing the .drl file the others look fine:
(sorry for adding so many replies, but can’t attach more than one image per post)
EasyEDA probably has trouble with PostScript drill file, try changing it to gerber.
@qu1ck I tried changing drill file to gerber, same result. Howerver, I’ve just tried generating the gerberfiles in another machine, and it works!
It’s really weird, but it seems it must be something with my KiCad installation or with my computer.
For the record, both machines have the same Linux and KiCad version:
I’ll use the other machine try to generate gerber files for the original design where I found this problem and let you know what I can find with some more tests.
Thanks a lot for all of your interest.
After completely deleting KiCad 5 and reinstaling it, the gerbers I generate look correctly in the EasyEDA viewer.
I have no clue about what was causing the the drill file problem. I thought it was because of a library I had to downgrade in order to compile the KiCad code (glm), but got back to the more recent version and gerber files still look fine.
Regarding the bigger gerber file size when using KiCad 5, I got the original board created with KiCad 4, opened it with KiCad 5 and generated gerber files, they’re still bigger in almost the same proportion I mentioned in my first post, I guess I can just forget about it since the files look fine in every gerber viewer I’ve tried now.
Thanks!
There have been changes to way that arcs are translated to Gerber output, looking better but maybe a bigger file
We just tried JLCPCB and got the same problem with the drill file. It seems to interpret the scale incorrectly. (Maybe one unit is interpreted as 1/10 of the intented size? I didn’t look so closely.)
I don’t know why it happens. After all I know I must presume it’s a bug in their viewer. I generated actually two boards (and two manufacturing projects) from one KiCad project so that I had two outlines in one kicad_pcb file. After the design was ready I created a git branch for each physical board just for plotting the gerbers and deleted the non-wanted board from the layout. I generated the gerbers and the drill files with the same settings. But weirdly only one of the boards had the problem in the JLCPCB preview!
I became wiser, did some searching and found their technical support for creating gerbers: https://support.jlcpcb.com/article/44-how-to-export-kicad-pcb-to-gerber-files. The settings which could be the culprit are Zeros Format and Minimal header. @mexchip has wrong zeros format just like I did. It could also be possible that Drill Units cause this.
(Note that Drill Map File Format shouldn’t have any effect because it’s for the drill map file, not for the actual excellon drill file. Map files aren’t usually used by manufacturers AFAIK.)
I tested now with new settings and the board preview in JLCPCB is fine.
EDIT: it was probably the Zeros Format.
Yes, I just confirmed, when using “Supress leading zeros” zeros format the EasyEDA viewer fails to load the drill file, switching to “Decimal format” the gerber loads fine.
Thanks for the info!
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
