How to debug a USB 3 connection?

[Jackster]

Hi all

I have a circuit board that I freelanced out the design of.
Had it made and got a pro to solder the USB type C plug and socket on for me (0.5mm pitch I wont touch xD)

The board extends the USB Type C socket about an inch from the plug.

I can get it to work in USB 2 mode but not USB 3.
Sometimes I can get the board I soldered to work in USB 3 but this is very rare.

What are my options here to debug this and find out what is going wrong?

Thank you
Jack

[ogden]

Seems you have signal integrity problems. If you can - show schematics (at least part in question) and photos of PCB, both sides. Provide links to info/docs of chip used. If you copied (part) of some existing board like devboard of USB chip - mention it as well.

[wraper]

USB 3 will work even is there is a few cm of wiring on 2 layer board without any impedance matching. Although in such case it will become a radio transmitter killing bluetooth, wifi and wireless mouses nearby. So without giving specifics of that board, it's hard to say why it does not work.

[Jackster]

USB Socket top of board Würth Elektronik 632723300021
USB Plug bottom of board Würth Elektronik 632712000021

Board is 4 layer, the middle 2 are ground only.


Also to note, if I flip the cable from the socket to my PC, nothing works at all. No USB 2.

[wraper]

There might be other errors but on first glance I found this. Those are simply not connected.

[wraper]

Although it explains only why it does not work in one position at all. Not problem with USB 3.

[wraper]

Here is pinout for reference.

[wraper]

Also no GND connection here.

[wraper]

Also strange that CCx and SBUx are length matched as well when it's not needed at all. The best would be to just route them as short as possible.

[wraper]

These 2 holes should not be there because connector does not have such pins and they only interfere with differential pair routing. EDIT: different connector used on PCB

[jismal]

Why different part name in schematic and BOM. Those two are different connectors

[wraper]

Hmm, probably connector is not properly soldered because I don't see 2 holes for plastic guides. EDIT: different connector used on PCB

[wraper]

Why different part name in schematic and BOM. Those two are different connectors

Now I see why there are no holes for plastic guides and 2 additional holes present. Connector is different. That was misleading.

[Jackster]

I believe the schematic parts are just mislabelled.

[jismal]

Just posting though
Ti recommendation for SuperSpeed Differential Routing
Maximum single differential pair size 8 inches
Maximum mismatch within single pair 5 mils.
Group matching?
Impedance 90ohm +-15%

[wraper]

How could I miss this  . H1-H4 pads of edge connector are not grounded. Not only it's mechanically weak (I would even avoid using thermal relief on those), basically cable shield is left not connected  . Now it's obvious why it fails to work as USB 3.

Yeah, 3 different errors on such simple board  .

[Jackster]

How could I miss this  . H1-H4 pads of edge connector are not grounded. Not only it's mechanically weak (I would even avoid using thermal relief on those), basically cable shield is left not connected  . Now it's obvious why it fails to work as USB 3.

Yeah, 3 different errors on such simple board  .

I forgot to mention that we noticed that and put a mod wire in to fix the prototype.

[wraper]

I guess this has something to do with not connecting diff pairs in certain cable orientation or running diff pairs in parallel. I won't dig into type-C spec now as it's late night here but cables most likely have only one set of differential pairs (3 diff pairs in total, not 6). So running 6 diff pairs like this might cause connection working on only certain matching orientation of cables (1/4 chance of success considering missing D lines on one side) or even cause diff pairs connected in parallel through the cable.

[wraper]

Full featured type C cable seem to have 5 diff pairs. Only one diff pair for USB 2.



So as I understand schematic should be like this:

[wraper]

Oh, and Vbus trace is way too thin for supplying any serious current as it should according to USB spec. It should be much thicker and have separate traces running from all 4 pins joining into one thick trace. Not running through other 2 Vbus pins of female connector. Via stitching of GND is inferior for such high speed application as well.

[wraper]

And it would be better to not have GND fills at all at outer layers rather than having them located inconsistently around diff pairs, thus inconsistently affecting impedance.

[dmills]

That board does have a buried ground plane right? If not I think you have diff pairs crossing reference planes in a few places, never a good look at these speeds.

Regards, Dan.

[wraper]

Board is 4 layer, the middle 2 are ground only.

[dmills]

Board is 4 layer, the middle 2 are ground only.

Gaa, insufficient caffeine error!

Regards, Dan.

[Jackster]

Should I just hire someone from here to start from scratch instead of bothering with this freelancer?