The KiCad standard library has a footprint for an upright female USB-C connector called USB_C_Receptacle_G-Switch_GT-USB-7051x. I am having trouble routing the tracks to this connector because I am designing with JLCPCB’s 2-layer design rules. I am only going to use USB 2.0.
The footprint has two rule areas that disallow any copper on the front side:
The datasheet’s recommended footprint does not mention anything about needing these areas.
I am guessing that they must have been added in order to keep the signals away from the the little tabs on the side of the connector.
But why? The solder mask would electrically insulate the traces from the tabs. I guess, if I put an untented via there, there could be a short, but that doesn’t explain why tracks are not allowed. Could this be to avoid issues is the solder mask isn’t perfect?
Never, ever assume solder mask is isolation! It is only (as name says) to not solder go away from pads by wetting the tracks connected to them.
I have read that there are special solder masks (thicker, harder, I think) you can order (if factory has it in offer) that have to pass special immunity tests. For such masks you probably can assume they are functional isolation (as here needed) but I think that you still can’t assume they are safety isolation.
I have never used USB-C yet. I suppose you practically need at least 4 layers to be able to connect pads on both sides crossing all connections, having at the same time good GND.
These metal tabs would slowly punch through the soldermask as cables are inserted into the connector time and time again. Also in pick&place assembly uneven surface (as in a trace under one tab, no trace under the other) will lead to some precentage of connectors not soldering properly.
Also regarding the 2-layer PCB, are you only using USB2 or power delivery? If that’s the case you’ll probably be fine for a hobby project, but to pass any sort of EMC specification you’d want a 4-layer stackup and careful layout of the USB2 differential pair.
For USB3 lanes you need 4 layers and preferably 6 layers with very careful layout to preserve signal integrity.
OK, thank you for your replies. I am going to have to accept that a vertical USB-C connector is not feasible. I’ll go with a right angle connector which has simplified pinout.
It’s a hobby project and I am using the data lines, but it won’t have to pass any EMC testing.
For a hobby project you can put some isolating tape or extra plastic layer over those tabs, but it can’t be too thick either, or soldering will become more difficult. But for a hobby project you can also bend a few of such tabs outward a bit to compensate for the extra height of the tape, or just bend them outward completely so they just never can touch the PCB.
Just for your information, there are also USB-C PCB connectors which have only the pins needed for USB2 (plus maybe some extra pin). For example KiCad footprint libraries (version 7.99) have USB_C_Plug_ShenzhenJingTuoJin_918-118A2021Y40002_Vertical which has pins 1, 4, 5, 6, 7, 8, 9, 12. Double that and it’s a 16-pin connector which is pretty common if you do some internet search.
