Gerber Files in GerbView is Fine but NOT in PCBway or Gerblook.org (issue with Paste Layer)

[linuxdev.io]

I have been following the same Gerber generation process this entire time, and I have successfully manufactured PCB boards from PCBway multiple times.

Now, for some reason, my Gerbers are being rejected by PCBway. I checked in Gerblook.org and they also can not be viewed when I try to upload the zip file.

I tried checking the layers one by one and I found that I can view all the layers on Gerblook.org except the Paste layers. However, I can view the Gerbers fine in GerbView in KiCad including the paste layer.

It appears that the paste layer is causing me issues. This is my first time making a SMT board. My previous boards were throughhole.

Do I need to select a different set of options to ensure my Paste layer is correct? I look in GerbView and it seems to me like both Paste layers (front and back) look fine and have data on them.

Thanks for your help. The Gerbers are attached.SS-VCO-1-REV2-Gerbers.zip (60.9 KB)

Linux Developer

[der.ule]

gerbv did opened your files and displayed correctly, however it did complain when loading the solder paste files:

Most likely found a RS-274D file…trying to open anywaysMissing apertures/drill sizes…trying to load anyways
Most likely found a RS-274D file…trying to open anywaysMissing apertures/drill sizes…trying to load anyways

[linuxdev.io]

What does that mean? Why is Gerblook.org or PCBway unable to view them? Anything I can do to re-master them? My design passes the DRC.

[davidsrsb]

Are you able to upload the Paste Layer file here?

[Peetem]

I’ve had issues with my Geber files as well. Two PCB manufacturers rejected them, but after changing output configurations several times, finally got one to approve.

However, Gerbview doesn’t display the files but Cuprum does.

So you’re not the only one having problems. It would be nice to know if others are as well…

[der.ule]

He did upload all his gerber files in the first post, or do you mean as text ?

Here you go: AS3340-VCO-B_Paste.gbp

G04 #@! TF.GenerationSoftware,KiCad,Pcbnew,5.1.7*
G04 #@! TF.CreationDate,2020-12-02T11:01:07+01:00*
G04 #@! TF.ProjectId,AS3340-VCO,41533333-3430-42d5-9643-4f2e6b696361,1*
G04 #@! TF.SameCoordinates,Original*
G04 #@! TF.FileFunction,Paste,Bot*
G04 #@! TF.FilePolarity,Positive*
%FSLAX46Y46*%
G04 Gerber Fmt 4.6, Leading zero omitted, Abs format (unit mm)*
G04 Created by KiCad (PCBNEW 5.1.7) date 2020-12-02 11:01:07*
%MOMM*%
%LPD*%
G01*
G04 APERTURE LIST*
G04 APERTURE END LIST*
G36*
G01*
X146146000Y-41912250D02*
X146146000Y-41399750D01*
G75*
G02*
X146364750Y-41181000I218750J0D01*
G01*
X146802250Y-41181000D01*
G75*
G02*
X147021000Y-41399750I0J-218750D01*
G01*
X147021000Y-41912250D01*
G75*
G02*
X146802250Y-42131000I-218750J0D01*
G01*
X146364750Y-42131000D01*
G75*
G02*
X146146000Y-41912250I0J218750D01*
G01*
G37*
G36*
G01*
X144571000Y-41912250D02*
X144571000Y-41399750D01*
G75*
G02*
X144789750Y-41181000I218750J0D01*
G01*
X145227250Y-41181000D01*
G75*
G02*
X145446000Y-41399750I0J-218750D01*
G01*
X145446000Y-41912250D01*
G75*
G02*
X145227250Y-42131000I-218750J0D01*
G01*
X144789750Y-42131000D01*
G75*
G02*
X144571000Y-41912250I0J218750D01*
G01*
G37*
M02*

[BlackCoffee]

I was able to open the files in Cuprum (did not bother with Gerbview).

They also preview in Mac’s Finder as they should… The two Paste files shown in screenshot below.

I also opened them in CopperCam (a pcb CNC machining program). I did not bother to set the Tooling/bits or anything so, it’s not something that looks pretty but, it did perform the steps as usual without problems (doing this always catches problems with file loading. Front, Back and Paste shown below, though it could be flying under the Radar… Nor did I align the layers…)

[Frederik]

I tried the zip on the Reference Gerber Viewer, which has half-decent error messages. No complaints about Gerbers, and the image looks sensible. I guess the Gerbers are right, and the problem is in the software that cannot read them.

However, the viewer complains about the drill files. And indeed, in the drill file it is not specified where the decimal point in the coordinates is, the precision of the file in other words. Furthermore, the drill files are in inch, whereas the coppers are in metric - this is asking for alignment issue due to different rounding.

[linuxdev.io]

I’ve corrected the unit mis-match and reattached the Gerbers here. They still do not open in gerblook.org. I will try resubmitting to PCBway, but I am afraid this is just a bug.

Is there a separate way to report bugs or does this thread suffice?

SS-VCO-1-REV2-Gerbers.zip (60.2 KB)

[eelik]

@linuxdev.io

Is there a separate way to report bugs or does this thread suffice?

https://gitlab.com/kicad/code/kicad/-/issues

But please make sure first that the problem isn’t in the online gerber viewer, because there are lots of broken ones out there. Sometimes I get a feeling that most of them are buggy. A KiCad developer (actually the founder of KiCad) has close connections to Ucamco, the company who governs the gerber standard, and KiCad is pretty good at obeying the standard. It wouldn’t be the first or last time when another program can’t handle standard gerber. It’s even possible that several programs make one and the same mistake with gerbers, so checking with several viewers doesn’t necessarily tell the truth. The only thing that really matters is if the manufacturer CAM software can read them. If not, it doesn’t help much if KiCad creates faultless gerbers.

[eelik]

BTW, for a bug report you should give the original KiCad project anyway, the plain gerbers aren’t enough, so if possible, you could give it here. Then we can check which KiCad feature possibly triggers the problem, if any.

KiCad (v5.1) is used probably daily around the world to create gerbers for popular manufacturers, so if there’s a bug, it’s not just any project.

[Frederik]

AFAIK these Gerbers are faultless. The issue is that PCBway cannot handle the data set, presumably a bug in their software. One may want KiCad output to work around this bug, or one may not want. This is a feature request rather than a bug report. But to develop a workaround one must know exactly what the problem is.
Maybe you should point out to PCBway that the Gerbers are faultless, and ask exactly what problem they have with it. They might even answer.
The drill file is now metric indeed. Good. However, it still misses the position of the decimal point. However, I doubt this is a PCBways problem. Many NC drill files have this problem, so no doubt PCBway can handle this, by manually defining the position for instance. A way to avoid this error is the have an explicit decimal point (XNC), or output the drill files in Gerber.

[paulvdh]

Lot’s of online gerber viewers tend to be of bad quality.
Try another one, for example:
https://gerber.ucamco.com/

[linuxdev.io]

I submitted again to PCBWay and this time it was accepted (4 rejections before). Maybe it was a glitch on their side. Although gerblook.org still doesn’t work, the other Gerber viewers suggested all seem to work.

I wonder if it was related to the unit mismatch between the gerbers and drill files?