Gerber drawings altered by fabricator, is this normal? - Page 1
Forum section: electronics / projects

author: alexg
author_rank: Regular Contributor
timestamp: January 16, 2019, 04:43:25 pm
content: Hello, I do not have enough experience working with fabricators for production projects, I had a gerber files of single board and sent it to fabricator to order a of boards placed into panel 2x5 array with rails, fiducials, etc.I have received a gerber files of the panel to approve before production and I noticed that all copper sizes were increased, for example traces that were 7mil are now 10mil, via pads that were 19mil are now 22mil, many circular via pads were swelled to the point that there is only little clearance between them, I am just not sure if this is normal practice, for example, see attached illustraton of row of pads on one of ICs, one picture is the original gerber as it comes out from PCB design software and then another picture is how it came back to approve. I am just trying to undersand if this is normal thing to do by fabricators.

author: Benta
author_rank: Super Contributor
timestamp: January 16, 2019, 05:19:18 pm
content: Normal no, but not unusual. Every PCB manufacturer has a Design Rule Check software, where the Gerber is sent through before manufacturing. This reflects the capabilities of the processes available.The fact that the company sends back the Gerbers with modifications is a signal to you that there are potential problems with your design.I've had many PCBs done, but as I mostly work with leaded parts, trace width and spacing have not been an issue, I've never had a Gerber come back, they took it as it is.Regard it as a good service and be thankful they caught it. You can always insist on them using the original Gerbers, but this might bring a yield/price issue.Edit: the PCB manufacturers I know list the minimum spacing/trace width up front, which you should adhere to. There are price differences depending on how fine etching you need.

author: Conrad Hoffman
author_rank: Super Contributor
timestamp: January 16, 2019, 06:09:38 pm
content: That doesn't look right. Are you sure it isn't for a mask?

author: alexg
author_rank: Regular Contributor
timestamp: January 16, 2019, 06:15:53 pm
content: Quote from: Benta on January 16, 2019, 05:19:18 pmThank you for a reply, this board has been manufactured before few times before with different fabricator and is designed above manufacturer minimum specifications for sure, they sent me files for approval because I requested that to make sure I can double check it before it goes into production since it is a new fabricator. Waiting to hear from them directly of course, but also just curious whether I should let it go or request to stick to original layout.

author: alexg
author_rank: Regular Contributor
timestamp: January 16, 2019, 06:17:00 pm
content: Quote from: Conrad Hoffman on January 16, 2019, 06:09:38 pmYes, I double checked. That was not the mask.

author: Benta
author_rank: Super Contributor
timestamp: January 16, 2019, 07:53:25 pm
content: Quote from: alexg on January 16, 2019, 06:15:53 pmIn that case, please call the manufacturer directly to clarify the issue. And please post the results here, I'm certain a number of members are interested. Thanks.

author: mvs
author_rank: Frequent Contributor
timestamp: January 16, 2019, 09:35:02 pm
content: Quote from: alexg on January 16, 2019, 04:43:25 pmIf the fab has 4/4 mil space/trace process with good yield, 4-5 mil clearance on some few places may not be a major problem for them. They probably optimize for drilling alignment errors or drill bit costs (22 mil via can be done with regular 0.3mm (12 mil) hole).Quote from: alexg on January 16, 2019, 06:15:53 pmYour design might be in spec, but it does not mean that it is production friendly or cost efficient. Typically recommended min. via size for conventional PCBs is 24 mil (12 mil hole + 2x6 mil annular ring) or 0.6 mm (0.3 mm hole + 2x0.15 mm ring).

author: KL27x
author_rank: Super Contributor
timestamp: January 16, 2019, 11:34:17 pm
content: IME, a professional manfucturer will inform you about any problems they discover and throw your project in limbo until you give them the ok or submit a new file, usually requiring at least half a dozen emails/texts and taking the better part of a week.This would be "nice" that they took the initiative. If this helps you or them or both, and they did this on their own, that's great. But they should inform you of what they did to get your ok. Now you have a production board you don't even have the board files for, and in some cases they can screw up your board.I have worked with a pcb designer and assembler/fabricator that made unsolicited cosmetic changes to the board on every batch. Gotta get your money's worth out of that Altium license, I suppose. One day he made an unsolicited "improvement" that quintupled the error rate. He's no longer around.

author: bson
author_rank: Unknown
timestamp: January 18, 2019, 03:49:58 am
content: I'm very interested also in their reasoning; I can think of a number of reasons: etching for less space is more reliable than etching for less copper; saves on etchant; since due to the staggered pattern, and that this is likely a connector, thin copper is more likely to lift during soldering and/or mechanical stress; and more, that in general leads to "more copper is better, up to minimum clearance". But it would be really interesting to see their reply!

author: SiliconWizard
author_rank: Super Contributor
timestamp: January 18, 2019, 06:39:54 pm
content: If those are the final production gerbers, this could just be to account for the etching process, although here, it looks like they inflated the shapes a bit much.Also beware of what you see, what the gerber viewer shows may be a bit misleading. Can you be certain of the measurements you get? 7mil to 10mil seems a LOT (+42%).Now even if that were to account for the etching process (but I don't believe this would require +42% inflating), given the clearance, that yields round pads that become distorted and even if the etching gets you dimensions closer to the original ones, that would make some pads very thin at the spots where they are "truncated".So in any case, obviously ask the manufacturer before approving.

author: kony
author_rank: Regular Contributor
timestamp: January 25, 2019, 10:12:42 pm
content: TBH, your pad entry is quite atrocious on the example. Your package should be sceaming about acid traps in DFM check. Vias not aligned in rows don't help that either.Setting generic via to pad rule to nonzero clearance even for same net will prevent you in creating this next time during layout.Otherwise still, the added via teardrops and trace width adjustments are quite large even to what is normal for when fabhouse tries to fix your gerbers. Isn't there some extra criterion not mentioned such as using 35+um layer base copper lamination and this being just a compensation for bad underetching?