What can and can't be done by budget pcb manufacturers - Page 1
Forum section: electronics / general

author: gblades
author_rank: Contributor
timestamp: July 21, 2016, 11:04:58 am
content: I have been using Diptrace and I am ready to send the first PCB out to get manufactured. I was wondering if there is a list of common mistakes etc... that people make?I have checked the board requirements are compatible with the company I intend to use but I have a few questions.1. They want the gerber files in zipped form. Diptrace can export to 'gerber' and 'gerber X2' among others. Which should I use?2. Is there anything on the PCB that the pcb manufacturer will be unable to do?I have a 'T' shaped board which I assume will be fine. I also assume normal mounting holes are fine but what about other shapes or multiple boards with cutouts so you have small tabs to break to separate them. I know you often pay extra for multiple boards on a single pcb.Thanks

author: Rerouter
author_rank: Super Contributor
timestamp: July 21, 2016, 11:30:44 am
content: Plated slots, sub boards, and constellations (probably wrong spelling), tend to be what they will refuse or ask more for,That is what a number of them refuse to do,However you can still ask them to produce things that will piss them off, e.g. hundreds of tiny via's, running the gauntlets and reducing drill annular rings, choosing very small feature sizes on slots or board outline, having a vastly different copper density on either side (board will bend and they don't want you getting upset and asking for a free respin), or making every trace the minimum width / spacing.Then there are things that may just annoy you, e.g. making sure silkscreen is subtracted from pads, that you account for solder mask expansion so your solder paste doesn't creep through a via,In simple terms, check your Gerber's carefully before you send it, they will try and reproduce it how you told them to, not how you thought they would. and if you don't need 6/6 trace and spacing, relax it a little, as it will improve its yield.Oh and for mounting holes, run a ring of via's around where the screws will press, it will greatly reduce how much your board cold flows over time,

author: gblades
author_rank: Contributor
timestamp: July 21, 2016, 02:02:57 pm
content: Thanks.I have looked up the difference between gerber and gerber X2 and I think it will be best to stick with the original format for now especially as the pcb manufacturer asks for the files to be named in a specific way depending on what they are (should not be required in X2) and they make no reference to X2.

author: wraper
author_rank: Unknown
timestamp: July 21, 2016, 02:15:26 pm
content: Plated slots should be fine with cheap Chinese manufacturers, never had those rejected. However those located in the 1st world countries often will reject them or ask more money.

author: cowana
author_rank: Frequent Contributor
timestamp: July 21, 2016, 03:18:55 pm
content: I've always used gerber (rather than X2) files from Diptrace.On the occasions I haven't renamed Diptrace's default output into their specified naming format there haven't been any issues, however it's easy enough to do!

author: Bassman59
author_rank: Super Contributor
timestamp: July 21, 2016, 05:23:47 pm
content: Quote from: gblades on July 21, 2016, 11:04:58 amOne specific data point: Seeed Studio doesn't like Gerber X2. They bounce the files but can't tell you why. After submitting Gerbers twice and getting them bounced, I realized that I had checked the Extended Gerber box in Kicad. When I asked, "Do you support extended Gerbers?" I was told no.

author: JPortici
author_rank: Super Contributor
timestamp: July 21, 2016, 05:52:58 pm
content: Based on your supplier's seriousness, you fill find DRC rules and possibly instructions for creating the gerbers.DRC rules mean minimum clearance between traces, clearance between board edge, minimum/maximum plated hole, minimum/maximum via dimension and so onIntructions meanin the format which the gerber should use to avoid problems and which files are needed.DRC: For example with diptrace and elecrow i keep all clearances at minimum 0,25mm, 0,4mm between board and edge, 0,4mm via.Never had a board rejected or turn out to be faulty.Only faulty board i ever got was from a batch of prototypes for a remote which used 0,2 mm traces and vias.. and it was strange. there was current flowing between VDD and GND through a led but no short (but high resistance between the two points, measured after removing all the componentes of course)Gerber: For them (and for every other service i ever used) the gerber were default (no X2) with origin in design origin, imperial units.Then you wil always need to export the N/C drill file for the holes. Again, origin in the design origin, imperial units, txt file.

author: technotronix
author_rank: Regular Contributor
timestamp: August 16, 2016, 12:05:28 pm
content: I use gerber.