I had JLCPCB raise a minimum clearance violation on 2oz copper (min 0.2mm clearance) of the last two spins of a design that I’ve run a number of times previously without issue.
The only thing I can think of that has changed on my end between then and now is I’ve updated from KiCad 7.0.0 to 7.0.2. I’ve always generated gerbers with X2 disabled, and aperture macros enabled.
Looking at the gerbers from JLCPCB’s production files, I see discrepancy between the original gerber exports and their production gerbers.
As an example looking at both gerbers in gerbview - a meander section:
On the left is the JLCPCB production file, and on the right is the original gerber:
It seems JLCPCB has expanded the copper to compensate for etching deviations. They need to do this.
Then the question is whether the clearance is specified before or after compensation.
If it is after compensation it could be that the compensation factor changed since your last order.
I guess your best bet is to ask them, as your pre-compensation jobs seems to meet the clearance.
That makes sense. I assume the compensation would be higher for the 2oz copper too, which would explain the obvious deviation. Still wonder why they’re flagging it now.
In the email from them they provided a screenshot of the violations and measurements from their software, and it looks like it would have been post-compensation as the distance was 0.111mm, and they wanted to shrink the traces by 0.008mm
I have my min clearance in pcbnew set to 0.2mm and DRC is passing. I guess as a workaround I could bump the min spacing and reroute everything
I think the explanation from @Frederik makes sense.
JLC always creates production gerbers, based on the originals. In my case they panelized them for me as well, so you can check the panels in detail before approving.
When you click on the “Confirm Production File” for an order, there’s a link to download the production files which is a .rar containing the original and final grbs. I usually peek at them if I know they’ve made modifications, but never actually measured things on them before.
When did JLCPCB changed their spec? Was it recently? I have a template I use for their fabrication which is a few months old at least and wondering if I should check it against their current spec.
No fabricator ever produces directly from the incoming gerber files. They always read them in their CAM system, and output files for fabrication from CAM.
The incoming gerbers too often have flaws.
More importantly. Fabricators must panelize the data. Actually, there are two separate, nested, panelizations. First is the assembly panel, used by the assembler to fit his pick and place machines. This is the one you see. But the fabricator also needs a panel, even if there is only a single unit on it. This is the fabrication panel. This panel you never see.
Fabricators must compensate for deviations in the process, etch compensation, modify the hole size to drill sizes to make room for plating, scale to compensate for distortions in lamination and so forth.
Provide the additional info needed by the machines, e.g. feeds and speeds for drilling, fiducial marks to be used in imaging. When areas must be routed the exact routing pattern must be defined. And so on.
Consequently, fabricators never ever produce directly from the incoming gerber files.
Hi,
The working/production Gerber file is correct. The production Gerber is the file after compensation.
After etching, the finished trace width will be same to that in your Gerber. We also offer our customers working Gerber file similar to this.
