Unrecognized Gerber file

Making PCB Layouts, Manual routing, Auto-routing, Copper pouring, Updating from Schematic, Manufacturing Output
Post Reply
Message
Author
fastbike
Posts: 61
Joined: 06 Mar 2021, 06:42

Unrecognized Gerber file

#1 Post by fastbike » 28 May 2023, 07:39

I've got a 4 layer design which I've previously had JLCPCB manufacture 5 boards for a hand built prototype run.
Now that I've debugged and proven the design I'm going for a small pre production run and have panelised the board into a 3 row x 2 column layout, with 3mm gaps between boards and added fiducials and board/stencil alignment holes in the edge rails .
The problem is that when I upload the design to JLCPCB the preview feature does not display the board, the dimensions are not populated and the Gerber Preview pages shows many errors, see the attached screen shot.
Screenshot 2023-05-29 at 06-35-31 PCB Prototype - JLCPCB.png
Screenshot 2023-05-29 at 06-35-31 PCB Prototype - JLCPCB.png (64.31 KiB) Viewed 1118 times
Comparing the contents of the zip files, the only different I can see is that the panelised board has an additional file "V-Scoring.gbr"

Does anybody know how to fix this ?
Ardent hobbyist

fastbike
Posts: 61
Joined: 06 Mar 2021, 06:42

Re: Unrecognized Gerber file

#2 Post by fastbike » 28 May 2023, 07:51

Ok, I just removed the panelising, and the fiducials and alignment holes. I exported all layers and uploaded to JLCPCB. That works fine without the panelising.

I then just reset the panels, without the fiducials and alignment holes and exported all layers.
Uploading to JLCPCB has broken the file recognition again, so something to do with the panelising ?
Ardent hobbyist

fastbike
Posts: 61
Joined: 06 Mar 2021, 06:42

Re: Unrecognized Gerber file

#3 Post by fastbike » 28 May 2023, 08:05

Hmmm, maybe they have trouble with v scoring ?
https://jlcpcb.com/help/article/96-PCB-Panelization
Ardent hobbyist

fastbike
Posts: 61
Joined: 06 Mar 2021, 06:42

Re: Unrecognized Gerber file

#4 Post by fastbike » 28 May 2023, 19:36

I've done some more digging and it looks like the Gerber exporter in DipTrace is non standard.
According to the Gerber specification from Ucamco (who hold the copyright on the format) v scoring is covered by section 5.6.3

This section covers the FileFunction attribute and shows "Vcut" for lines that must be v cut. Diptrace outputs this as "V-Scoring"

Code: Select all

%TF.GenerationSoftware,Novarm,DipTrace,4.3.0.1*%
%TF.CreationDate,2023-05-29T18:26:55+11:00*%
%FSLAX26Y26*%
%MOIN*%
%TF.FileFunction,V-Scoring*%
%TF.Part,Single*%
%ADD10C,0.004724*%
Editing the output zip file however does not result in any improvement.

So my next attempt was to alter the file names (via the export sub-dialog) and change the "V-Scoring.gbr" file to "V-Cut.gbr".

This removes the error but the JLCPCB importer ignores the size of the Edge rails around the board. However the gerber preview adds it back in.

I will check the JLCPCB option to Confirm Production file to make sure it has been processed correctly
Ardent hobbyist

fastbike
Posts: 61
Joined: 06 Mar 2021, 06:42

Re: Unrecognized Gerber file

#5 Post by fastbike » 28 May 2023, 19:49

For a panelised board with no internal cut outs which is separated by v cuts, I also switch off the "board" file in the Gerber x2 output. This reduces the noise in the JLCPCB importer.

Hopefully this thread is useful for others, or at least for me in the future when I'm battling with exported file settings again :)
Ardent hobbyist

fastbike
Posts: 61
Joined: 06 Mar 2021, 06:42

Re: Unrecognized Gerber file

#6 Post by fastbike » 30 May 2023, 23:33

So I sent the zip file to JLCPCB, who have said the board outline needs to contain the v-cut (or something like that).
Here's their actual reply
Thank you so much for your email .

Please kindly complete your board outline layer .
Screenshot from 2023-05-31 22-34-44.png
Screenshot from 2023-05-31 22-34-44.png (15.76 KiB) Viewed 1103 times
So it appears that the board outline file and the v-cut file need to be merged.
How do we do that ?
Ardent hobbyist

fastbike
Posts: 61
Joined: 06 Mar 2021, 06:42

Re: Unrecognized Gerber file

#7 Post by fastbike » 05 Aug 2023, 16:49

If anyone has this issue I have created a simple utility that makes the corrections to the Gerber zip file that are required:
- copying the v score data from its own file to the board outline file
- deleting the v score file

I've written the utility in Delphi (Pascal) - the same tooling that DIPTrace use. You can compile with a free version, or try your luck with FreePascal/Lazarus. I've also included a ready to run EXE .

https://github.com/fastbike/GerberFix

The end result has been tested using the Ucamco Gerber viewer.
Ardent hobbyist

Post Reply