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.
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 ?
Unrecognized Gerber file
Re: Unrecognized Gerber file
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 ?
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
Re: Unrecognized Gerber file
Hmmm, maybe they have trouble with v scoring ?
https://jlcpcb.com/help/article/96-PCB-Panelization
https://jlcpcb.com/help/article/96-PCB-Panelization
Ardent hobbyist
Re: Unrecognized Gerber file
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"
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
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*%
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
Re: Unrecognized Gerber file
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
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
Re: Unrecognized Gerber file
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
How do we do that ?
Here's their actual reply
So it appears that the board outline file and the v-cut file need to be merged.Thank you so much for your email .
Please kindly complete your board outline layer .
How do we do that ?
Ardent hobbyist
Re: Unrecognized Gerber file
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.
- 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