USB connector footprint on PCB - Page 1
Forum section: electronics / general

author: aurmer
author_rank: Regular Contributor
timestamp: September 09, 2016, 06:54:35 am
content: So I am new to PCB design; it has been an interesting journey learning all the nuances.But theseUSB connectorspecsheets... for real?? They aren't very descriptive. I get the impression that this stuff is common knowledge therefore unnecessary to explain in data sheets, but I just cannot figure it out.In the attached image, on the left, you see two footprint recommendations from two datasheets (linked above). On the right, you see a color coding of what I think are different NETS which I need to assign to the pads (I don't even know if they are all pads).Most important on my color coding BLUE=Pin 5=GNDDid I get it right?

author: cowana
author_rank: Frequent Contributor
timestamp: September 09, 2016, 07:46:34 am
content: The metal of the USB shield (all the outer blue pads) isn't internally connected to pin 5 - that's up to the user (or whatever is plugged into the other end of the USB cable) to do.What you connect the shield to (GND, nothing, or GND via an EMI filter) depends on the exact application.

author: andersm
author_rank: Super Contributor
timestamp: September 09, 2016, 07:49:31 am
content: The USB connectors are fully specified in the USB standards (downloadable for free), so repeating the information would be redundant. Whether the shell should be connected, and at which end, and how, is one of those things you'll find lots conflicting advice on. But it should only affect EMC, not the functionality of the bus.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 09, 2016, 08:06:54 am
content: It's [supposed to be] obvious that the housing is tinned metal, and surrounds everything. I guess. So, where you put the ground pads (under the housing) really doesn't matter. But having them broken up into pads, as shown, probably gets a more uniform solder joint. Likewise, what you connect them to doesn't really matter either, since they're all pretty damn shorted together.Best practice: pour copper around all of the grounds (no thermal relief; except for the pin pad, leave that one normal), and stitch them into the board with via-in-pad, so there's extra copper penetrating the board, holding it down. (Don't worry about via-in-pad: it's pretty reliable when done with small vias (12 mils I.D. or less), no tenting/plugging on either side.) There can be ground pour on the backside, too.Grounding: DC (galvanic) ground isn't strictly necessary for the casing, but RF bypassing is required. If you float the case, do the above with a ground island, instead of the main ground plane. Bypass the island to the plane with at least two caps, one on each side of the connector. Surround the island with ground plane.There should probably be some damping in parallel with said caps. The amount depends on the cable length, but it's probably on the order of 2.5 ohms (for a pair of 0.1uF bypass caps, and a 0.47 to 1uF in series with 2.5 ohms).In any case, the ground pin (pin 5) should always be grounded, and supply (+5V / VCC) should be bypassed to ground. Don't use common mode filtering on the data pair (because USB isn't fully differential -- two line states are unbalanced!). Just use whatever termination resistors are recommended for your device, and an ESD protection device (if possible, both combined).Also, if you're only using Full Speed, and not High Speed, you can even get resistor, ESD and RFI filtering in one tiny part, which is handy.Tim

author: aurmer
author_rank: Regular Contributor
timestamp: September 09, 2016, 06:20:35 pm
content: Thank you. It makes sense why they would not duplicate information. It seems this is what I was looking for; I can know all I need by checking out the USB protocol standards.