0.25mm track-track distance for 250V on PCB - how big of a problem? - Page 1
Forum section: electronics / projects

author: daqq
author_rank: Super Contributor
timestamp: May 29, 2017, 06:04:50 am
content: Hi guys,I put a PCB prototype into production and then noticed that I've screwed up on the two internal layers and the bottom layer. A track that will have around 250V max on it with respect to GND copper pour has a track-copper pour distance of 0.254mm. This is present around one through hole pad only.Since this a prototype I can "fix" it by drilling out the offending pad and replacing the connection with a wire. I'd rather avoid that though, since it is a rather nasty hack.Is such a distance safe(-ish) for this kind of voltage? The material is standard FR4.Best regards,David

author: RobertHolcombe
author_rank: Frequent Contributor
timestamp: May 29, 2017, 06:11:16 am
content: If my interpretation of the uRuler table is correct, then @300V - 16mils (~0.4mm) if there is solder mask, or 50mils (~1.25mm) for bare traces.

author: ebclr
author_rank: Super Contributor
timestamp: May 29, 2017, 06:18:31 am
content: Unfortunately Not, You can still make a CNC cut to try to enlarge a little bit. This is critical don't sell this board, will return

author: daqq
author_rank: Super Contributor
timestamp: May 29, 2017, 09:02:52 am
content: Thanks guys for the answers.I did not intend it for production purposes, just as a quick hack to get the prototype working... I guess I'll go get the drill

author: Zero999
author_rank: Super Contributor
timestamp: May 29, 2017, 09:06:58 am
content: Quote from: daqq on May 29, 2017, 06:04:50 amWhether it's safe or not depends on if the user will be shocked or a fire could start, due to failure of the insulation. If neither conductor goes to protective earth, is completely electrically isolated from the user and adequate over current protection is provided (there's a suitable fuse upstream) then the insulation is said to be functional only.For functional insulation, the internal layers should be fine, since the resin will have a much higher dielectric strength than air. The bottom layer is more of a concern, since the breakdown voltage for air is around 1kV/mm (that's a simplification, it depends on thework functionof the electrodes also has an effect on arcing and is normally not taken into account but may be a factor at low voltages) so it's marginal design and certainly won't meet regulatory requirements.Rather than drilling anything, another possible solution is to conformally coat the offending area with a thick enough layer of an insulating substance.

author: MagicSmoker
author_rank: Super Contributor
timestamp: May 29, 2017, 10:24:13 am
content: Quote from: Hero999 on May 29, 2017, 09:06:58 amThis is what I was going to suggest as well - dab some proper urethane conformal coating on top of the errant pad and the immediate surrounding ground fill. Note that this will not fly with ISO900x, and it might not even fly with UL60950-1, so if you intend to go through safety testing I'd definitely ask whether this hack is ok ahead of time. Needless to say, you'll want to correct this in the next board revision.

author: Zero999
author_rank: Super Contributor
timestamp: May 29, 2017, 06:18:13 pm
content: Quote from: MagicSmoker on May 29, 2017, 10:24:13 amIt seems like this is a viable option. I just googled for the dielectric strength of polyurethane. It looks like a fairly thin layer, 1mil or 25.4µm thick, will be more than enough to hold off 250V.https://plastics.ulprospector.com/generics/45/c/t/polyurethane-pur-properties-processing

author: nctnico
author_rank: Super Contributor
timestamp: May 29, 2017, 10:06:27 pm
content: But you have the risk of moisture creeping underneath the polyurethane.

author: MagicSmoker
author_rank: Super Contributor
timestamp: May 30, 2017, 11:06:34 am
content: Quote from: nctnico on May 29, 2017, 10:06:27 pmAnd even if some moisture did make it through the polyurethane the situation still wouldn't be any worse than leaving the pad exposed.