USB C - 2.0 routing of hybrid SMT / through hole connector

[bobof]

Has anyone achieved an optimal USB 2.0 layout on USB C SMT/Hybrid connectors?
4 layer board I'm retrofitting to (signal/ground/power/signal), so would like to keep the USB 2.0 differential pair top side as much as possible

USB C documentation states:

"The receptacle side shall support the USB 2.0 differential pair present on Dp1/Dn1 or Dp2/Dn2. The plug orientation determines which pair is active. In one implementation, Dp1 and Dp2 may be shorted on the host/device as close to the receptacle as possible to minimize stub length; Dn1 and Dn2 may also be shorted. The maximum shorting trace length should not exceed 3.5 mm."

I like the look of this connector for mechanical robustness, as it has a staggered set of rows of through hole pins along with an SMT row; Wurth 632723100011 (or clones).

However; all the processor / hub reference boards from various vendors I've found so far for this part would appear to fail this maximum shorting trace length, meaning in one or both orientations there will be a significantly longer stub on one or both of the USB 2.0 Dp/Dn signals.  A TI AM243 reference board I found has the record so far, at around 8.5mm.

The only one I think is compliant is this crafty creation from Microchip (https://support.microchip.com/s/article/USB-Type-C-Layout-Recommendations) - but theirs results in the USB Dp/Dn on the opposite side of the board.  At first sight you think "why not just remove the via and route topside?"  but then you realise it ends up heavily asymmetric in one cable orientation due to only one wire in the through hole case being routed through a via and the through hole (so 2x PCB heights difference).   The vias and opposite side routing ensure in each case there is precisely one Z hop.


Is this overthinking?  It irks me to go against the USB C published spec, though it seems others have had little second thought in violating it...!

[Whales]

I don't like these vertical USB-C connectors with a mix of SMD and TH.  They're quite hard to solder yourself because the pads are completely concealed (ie worse than QFN, a bit more like BGA).  JLCPCB assembly sometime charge a (small) difficult handling fee or send me X-ray reports for these connectors for free, which I think is there way of saying they hate them.

Yeah I always had to tee and stub for the two USB2 RX and TX pairs.  I also recall having to shave my minimum track thickness or clearance down a tad to make it fit in places.  Screw the spec, USB 2.0 works over shitty unshielded random-impedance motherboard-to-casefront wires, so it will survive a few mm of stub.

[bobof]

I don't like these vertical USB-C connectors with a mix of SMD and TH.  They're quite hard to solder yourself because the pads are completely concealed (ie worse than QFN, a bit more like BGA).  JLCPCB assembly sometime charge a (small) difficult handling fee or send me X-ray reports for these connectors for free, which I think is there way of saying they hate them.

This one's horizontal, so at least the SMT pads are exposed.  The through hole pins are a weird hybrid though; they're not meant to be wave / hand soldered, you're supposed to squeegee the paste onto the board twice, which packs the holes with paste that melts during reflow.   Wurth have a whole application note about it, which makes me sure wherever I take it to is going to get it wrong the first time, so maybe better choose something else.

Yeah I always had to tee and stub for the two USB2 RX and TX pairs.  I also recall having to shave my minimum track thickness or clearance down a tad to make it fit in places.  Screw the spec, USB 2.0 works over shitty unshielded random-impedance motherboard-to-casefront wires, so it will survive a few mm of stub.

I hate giving away margin if I can avoid it, and you just know that if there is an issue with the USB everyone's going to be querying why I've got 5mm of stub instead of 3.5mm.  I'm sure most of us have committed all kinds of heinous cabling crimes when you just need to make something work (and gashy PC internal USB cables are a great production example!), but when committing copper to FR4 it feels like it deserves a bit more diligence to make it as good as it can reasonably be.

I had even considered a mux on the Dp/Dn, but that seems overkill when everyone appears to be getting away with it.

[tszaboo]

Würth has very good support and application engineers. They will help you for sure if you ask the questions from them directly.
And you don't need to commit to purchase large quantities to receive the support. Try it.

[bobof]

Würth has very good support and application engineers. They will help you for sure if you ask the questions from them directly.
And you don't need to commit to purchase large quantities to receive the support. Try it.

Thanks, I hadn't considered it.  I've been in touch as they themselves have a seemingly non-compliant example using this connector on the RD041 reference design.  Be interesting to see what they say. 
I make it that they've got about 4mm of trace without considering the through via height that forms part of the stub length in one orientation.
https://www.we-online.com/en/support/knowledge/application-notes?d=rd041-design-of-a-single-pair-ethernet-system-with-power-over-data-lines

[nctnico]

Has anyone achieved an optimal USB 2.0 layout on USB C SMT/Hybrid connectors?
4 layer board I'm retrofitting to (signal/ground/power/signal), so would like to keep the USB 2.0 differential pair top side as much as possible

I'd go for the Micrchip solution. Having the signals single ended for a bit isn't a problem for as long as the impedance is near the spec and you don't have large differences in stub size. You'll have the same problem with about any USB-C connector. The Microchip solution could be made a bit more symmertrical.

[bobof]

I'd go for the Micrchip solution. Having the signals single ended for a bit isn't a problem for as long as the impedance is near the spec and you don't have large differences in stub size. You'll have the same problem with about any USB-C connector. The Microchip solution could be made a bit more symmertrical.

It's certainly the cleverest and least stubby; however it has one issue that's not immediately apparent - the Dp/Dm end up routing out to the PHY over the bottom layer, which isn't great for a 4layer design.  You either have to add another via transition to each pair to route out over the top (a bit nasty, now you have a few more impedance discontinuities) - or you remove one via and route on the top.  But then one side of the pair to the through hole pins ends up with a much longer path (via down and then through hole up), and there isn't space to fix it on the other trace.

[Whales]

> The maximum shorting trace length should not exceed 3.5 mm

They're giving a deceptive number of decimal points here.

The stubs electrically continue into the pins of the USB-C connector itself.  Different USB C connectors are different heights.

[thm_w]

https://www.reddit.com/r/AskElectronics/comments/1vkkl8e/how_am_i_supposed_to_route_this_usbc_connector/

> The maximum shorting trace length should not exceed 3.5 mm

They're giving a deceptive number of decimal points here.

The stubs electrically continue into the pins of the USB-C connector itself.  Different USB C connectors are different heights.

Yes but they want to give a number that is low enough that everything will work at full speed even given various connectors.
It is overly conservative, but you can understand their logic. Ass covering.
TI even states <2.5mm

[bobof]

> The maximum shorting trace length should not exceed 3.5 mm

They're giving a deceptive number of decimal points here.

The stubs electrically continue into the pins of the USB-C connector itself.  Different USB C connectors are different heights.

I think it's not even just wrong in so far as the decimal point; some of the connectors in the market must have significantly longer contact tails in the order of mm than this one (eg stacked connectors that are offset vertically by several mm, 90 degree connectors where the tails would appear to get progressively longer from top to bottom).  Ideally each contact would have a length and you'd be given the actual max stub length to be able to calculate how much PCB stub you could tolerate.

There is an assumption there that those tall / rotated connectors are actually compliant though when used with the recommended stub lengths, none of those connectors actually feature in the spec doc so it is possible they are all stealing from the same pot...

Yes but they want to give a number that is low enough that everything will work at full speed even given various connectors.
It is overly conservative, but you can understand their logic. Ass covering.
TI even states <2.5mm

I'd also seen the TI note, I wasn't sure if it was typo, an engineer being even tighter with his margin (maybe their silicon steals some also...), or just trying to make it even more likely you'd choose to stick a mux on it once the dissatisfaction set in that a single thru via on a 1.6 mm PCB stole nearly/over half the 3.5/2.5mm margin.

It's also interesting to see how many designs give little care to the matching of the pairs, with one leg frequently being observed doing two via hops while the other does none. 

I guess folk unwittingly end up accepting that the price for that reversible convenience is that long cables stop working a bit sooner.

This 12 pin USB C USB 2.0 connector layout is probably about the only one I've seen that I look at and think... yeah, I can get behind that.  But it looks mechanically not brilliant by comparison.

[tszaboo]

> The maximum shorting trace length should not exceed 3.5 mm

They're giving a deceptive number of decimal points here.

The stubs electrically continue into the pins of the USB-C connector itself.  Different USB C connectors are different heights.

I think it's not even just wrong in so far as the decimal point; some of the connectors in the market must have significantly longer contact tails in the order of mm than this one (eg stacked connectors that are offset vertically by several mm, 90 degree connectors where the tails would appear to get progressively longer from top to bottom).  Ideally each contact would have a length and you'd be given the actual max stub length to be able to calculate how much PCB stub you could tolerate.

There is an assumption there that those tall / rotated connectors are actually compliant though when used with the recommended stub lengths, none of those connectors actually feature in the spec doc so it is possible they are all stealing from the same pot...

Yes but they want to give a number that is low enough that everything will work at full speed even given various connectors.
It is overly conservative, but you can understand their logic. Ass covering.
TI even states <2.5mm

I'd also seen the TI note, I wasn't sure if it was typo, an engineer being even tighter with his margin (maybe their silicon steals some also...), or just trying to make it even more likely you'd choose to stick a mux on it once the dissatisfaction set in that a single thru via on a 1.6 mm PCB stole nearly/over half the 3.5/2.5mm margin.

It's also interesting to see how many designs give little care to the matching of the pairs, with one leg frequently being observed doing two via hops while the other does none. 

I guess folk unwittingly end up accepting that the price for that reversible convenience is that long cables stop working a bit sooner.

This 12 pin USB C USB 2.0 connector layout is probably about the only one I've seen that I look at and think... yeah, I can get behind that.  But it looks mechanically not brilliant by comparison.
[ Attachment Invalid Or Does Not Exist ]

I think in practice, the protocol and the physical layer can handle more clumsy design, than what the standard allows.
If you see all these Arduino boards where people put random resistors in series USB, just because they saw that on another board with another IC... Type C, 3.0 also is faster than 2.0. So the cables are typically shorter, and the 2.0 signals have easier time.
IMHO obsessing about signal integrity is often times doesn't result a better product.

[bobof]

I think in practice, the protocol and the physical layer can handle more clumsy design, than what the standard allows.
If you see all these Arduino boards where people put random resistors in series USB, just because they saw that on another board with another IC... Type C, 3.0 also is faster than 2.0. So the cables are typically shorter, and the 2.0 signals have easier time.
IMHO obsessing about signal integrity is often times doesn't result a better product.

Sure, in this case on balance this product would probably be "worse" (for some definition of) in using a mechanically weaker connector purely to have a slightly shorter stub lengths.  But at the same time, one doesn't necessarily lead to the other, the original point was about trying to get the best possible layout with the connector which seems likely to have the most mechanical advantage. 

As you say, you can buy all manner of cruft in the market, but those of us making professional products seek to deploy work to the highest possible standards; what they're doing and "getting away with" has little relevance. 

The collected evidence would seem to indicate that USB C perhaps just is a bit worse from an SI perspective in respect of USB A-B connection at the PCB level, given most USB B implementations can be done all top side from PHY to connector, and matched to within fractions of a mm.