Does an IPC Standard/Guideline exist for component proximity? - Page 1
Forum section: electronics / projects

author: Pack34
author_rank: Frequent Contributor
timestamp: October 24, 2018, 07:24:42 pm
content: Is there a guideline that dictates acceptable component proximity? This would clearly be driven by the CM's capabilities, but is there an official standard like the IPC-7351 guideline for land patterns?I'm specifically looking for two things:1. The acceptable minimum distance between an SMT part and the pins of a through-hole connector. I'm assuming there's some radius standard that takes into account the diameter of the PTH component's pad.2. The acceptable minimum SMT component distance. I'm aware of the PCB fabrication constraints for copper-to-copper spacing, solder mask slivering, etc. But this does not take into account the physical process of placing the components. If you have an Ethernet connector you can't really place a 0402 capacitor 10mils from it.In the past, I've always used general rules of thumb based on my experience and haven't had issues but feel that there should be some sort of standard or official DFM guideline for something like this.Any help?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 25, 2018, 03:06:50 am
content: Yes, '7351 includes courtyard dimensions.Component courtyards should not overlap.CMs have to deal with a lot of crap, so I doubt they care very much, at least as far as just building anything at all. If you want to talk DFM (design for manufacturing), cost reduction, rework reduction -- all of that sort of thing, you'll want to talk with them about component spacing, pad shape, pad entry (connecting traces sink heat from the pad, making problems with tombstoning of small components, or head-on-pillow or wetting failures of all sizes).A typical clearance is solder-side SMT components 100 mils from THT pads. This is a worst-case figure, driven by wave solder fixturing. Better fixtures can be made -- at greater cost, e.g. milled composite versus formed titanium sheet -- where tighter clearances must be tolerated. Or maybe it depends on component height. Or hand soldering really isn't a big cost to your product and it doesn't matter at all.Tim

author: jbb
author_rank: Super Contributor
timestamp: October 25, 2018, 06:14:11 am
content: What he said ^^You do definitely want at least a little solder mask between a through hole and an SMT pad so that they form separate solder joints.Also some investigating of the tolerances for the components is in order; the board should be laid out for max size component bodies (tolerances are frequently +-0.1mm and more) and your library might use nominal size.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 25, 2018, 02:42:21 pm
content: On a related note, keep some distance between untented vias and pasted pads. The paste spreads out on heating, and can fall onto nearby vias.If you're avoiding tenting (by convention, or because the via has to be open on one side as a test point?), you can cheat / compromise by reducing the soldermask opening to just larger than the hole. This prevents mask and solder from falling into the hole, so the via's annulus can be pretty much touching an SMT pad without thieving solder from it.Tim