No, I'm working in Altium (and mostly generating my own footprints and/or using old ones that are proven in practice with previous generations of product).
Are you using EasyEDA, or at least running your design through EasyEDA and creating the Gerbers from it ? We found early on that sending the ones direct from Altium did have a few issues which importing into EasyEDA before sending them off solved.
I'm in a slightly different position from you in that I'm generally using JLCPCB to build prototypes for products that are ultimately going to be built elsewhere. It's a bit of chicken-and-egg: my clients mostly have fixed relationships with their assembly contractors and I've been reluctant to push them towards JLC despite the price advantage as they certainly won't get the personal contact they are used to, and I would probably get it in the neck if they ended up with yield problems or whatever.
But it's true that I've already learned the lesson about following "the JLC way" for an easy life - with JLC part numbers in my Altium library parts and Altium OutJob files to generate BoMs etc in either JLC format or "usual contractor" format. And you are telling me that I ought to take that one step further, which does make sense.
This is very useful info, thank you.Also quite a few footprints in EasyEDA are not the same as the manufacturers - they've been optimised for their process, so now we import those the other way into Altium. For example capacitors and resistors of nominally the same size have very different footprints because of the way they absorb heat during reflow.
Unfortunately the two parts that have given me significant grief didn't at the time have EasyEDA footprints, though I see that they both now do.
The QFN one (C783599) can't be totally captured in the footprint as it has a belly pad which is inevitably going to have vias in it, and so it's going to vary with what size vias you choose, whether they are plugged etc. However, I do notice that they have larger-than-manufacturer pads around the edges, albeit with a negative paste expansion, which is a meaningful difference from the footprint I use and well worth trying.
It was on 4 layers, but this (C2649370) is an oddball part that's only 4 rows of balls that's intended to be routed out on the top layer without vias. The footprint is very simple, but I notice that the EasyEDA footprint they've now added has slightly smaller pads than I do (and mine were fractionally smaller than manufacturer recommended in order to meet the pad/track spacing). Seems counterintuitive that smaller pads would be better here, with opens rather than shorts being the problem, but always possible.Was the BGA on a 6 layer or greater board ? Their 2 and 4 layer aren't really suitable for that spec as they don't have plugged vias so surprised they didn't reject the submission in the first case. But should have been fine if 6 or more.
No, I didn't - not expecting that (with the trivial amounts of money I am spending with them) they would be willing to do much, or indeed able to do much as the boards were now in my hands. But it sounds like it would be worth investing more in this relationship - it wouldn't cost much to run a couple of extra batches of boards I don't really need to bottom out the production problems rather than just accepting them.I've never seen paste variations though. Did you take this up with your assigned engineering contact ? They are very helpful when you have problems so that future iterations or new designs don't have the same problem.
Aside from the two "problem" parts which clearly needed refinement, the other one I've had regularly enough to remember (but not often enough to rate as a "problem") is occasional pins on RP2040 not soldered - easily touched up with an iron when found so no big deal for prototypes but maybe unacceptable yield for production.
I've now checked the EasyEDA footprint and it has significantly longer pads than the ones in the Rpi datasheet recommendation: 1.1x0.2 rather than 0.875x0.2. It claims to have a negative paste expansion but I don't think it really means it - the belly pad has the same 0.1 negative expansion and renders on screen as significantly less paste than the pad (which makes sense for that pad), but the 0.1 negative on a 0.2 width pad would give no paste at all, while the on-screen render looks like paste same size as pad.
Many thanks for sharing your experience with us - this has been a really useful conversation.
Statistics: Posted by arg001 — Tue Jul 01, 2025 9:42 am