Through Hole Connector stub concerns - Page 1
Forum section: electronics / general

author: PJ Bain
author_rank: Contributor
timestamp: May 06, 2020, 04:57:47 am
content: Hi all,I'm laying out out a rigid+flex PCB that has FPD (170MHz) and USB 3.0 signals. The through hole connectors from the front panel are mounted on top of the rigid PCB. All differential tracks are on the top layer so they stay on a single layer through to the end of the flex PCB which is terminated in a ZIF style to insert into a FPC connector.Given the tracks are on the top layer, I am trying to work out how the leads of the through hole connectors which continue out through the bottom of the PCB may react as stubs. Is there a Lambda (for example 1/10*Lambda) where I can say safely that the stub lead length will not be a concern? For example, if the stub length is less than 1/10*Lambda then it's not an issue?Thanks,Peter

author: T3sl4co1l
author_rank: Super Contributor
timestamp: May 06, 2020, 07:35:23 am
content: Not only that but the diameter of the pads, and what impedance that gives to surrounding ground plane.The pin length is, I guess, 1.6mm through the board, and at 0.2 mm/ps you need an edge of 8ps to be critical. Edges over 80ps won't notice, and an asymptotic impedance mismatch is all it will register as (which should be negligible on these digital signals).The transition from rigid to flex is more critical, I mean assuming the flex length is much more than 1.6mm, which seems likely? If you can do two layer flex and route over ground plane, that keeps things much more stable; flex is thin though, so the trace width may need to be very narrow indeed to stay matched.Tim

author: PJ Bain
author_rank: Contributor
timestamp: May 06, 2020, 07:43:18 am
content: Thanks Tim,Yeah the flex length is longer (about mm) and I have done it as 2 layer with a hatched ground as the reference plane on the 2nd layer. This has resulted in the track width/spacing being the same on the Rigid and Flex boards (within a couple %). Trace widths have ended up being between 5 and 6 mil (1oz copper) which is quite thin but still manufacturable I think. but I was struggling to get any wider and still maintain a stackup which I think will be flexible enough (first time doing a flex PCB).

author: PJ Bain
author_rank: Contributor
timestamp: May 06, 2020, 11:25:01 pm
content: Hi Tim, just wondering where the 0.2mm/ps comes from? Approx. speed of light (0.299mm/ps) is the closest thing I could find? I am just working through the math so that I can repeat the theory in other scenarios if I need to. Thanks!

author: T3sl4co1l
author_rank: Super Contributor
timestamp: May 07, 2020, 12:40:01 pm
content: Speed of light is slower in a medium, e.g. FR-4. That's the upper limit, yes.BTW beware of EMI issues with patterned ground: it's a leaky shield. Differential will help with that, but some will get through. Probably what you have here, wouldn't run afoul of FCC/CE commercial limits. If it's super tight (MIL spec something or other?) you'll want something quieter (micro-coax cables?), or a shield around everything. Or also slower edge rates, if you can afford it (ferrite beads at the transmitter?).Also make sure the traces follow symmetrical paths over the ground pattern. Keeps the frequency response, impedance and EMI balanced.Also, the regular pattern means there's a cutoff frequency, corresponding to the pattern pitch of course. (There's a whole science around it: electromagnetic band gaps. Basically a stop band exists in periodic geometries, for basically the same reason one exists in physical crystals, that electrons move through as waves.) Again probably not a problem, given the frequencies where that's relevant (10s GHz?), but interesting to note if you're in the same situation again with high speed signals.Tim