I Have two PCBs,pin out define as follows ,the host pcb is A connector,and the device pcb is B connector. enter image description here

I use the 1.25pitch connectors&USB3.0 cable to connect two boards,but the host board Unrecognized usb3.0 device. Cable is follow enter image description here

enter image description here

Layout is follow

Host PCB:The TX-,TX+ traces about 25mm RX-,RX+ traces about 44mm enter image description here

Device PCB:The TX-,TX+,RX-,RX+ traces both about 15mm enter image description here

  • \$\begingroup\$ Can you force the software to low speed (USB 1.0)? That should still recognize the device and confirm that the problem is the cable. \$\endgroup\$ – Edgar Brown Oct 30 '18 at 3:11
  • \$\begingroup\$ Device enumeration either needs the D+/D- lines (USB1.x/2.0) or the SS lines (USB3.0). It's unlikely both failed. Check the device. \$\endgroup\$ – Janka Oct 30 '18 at 4:47
  • \$\begingroup\$ When I use the cable ,the host board recognized USB2.0 ,unrecognized USB3.0 \$\endgroup\$ – 張簡麒耀 Oct 30 '18 at 7:26
  • 2
    \$\begingroup\$ You are extremely unlikely to be able to make this cable work for USB3, which has signals in the order of multiple GHz. \$\endgroup\$ – BeB00 Oct 30 '18 at 15:51
  • \$\begingroup\$ Given that it is standard USB3.0 cable with non-standard connectors, the cable might not be the problem. Are the PCBs commercially available or are these your own layout? Do you have the layout of the connector sections? \$\endgroup\$ – Edgar Brown Oct 30 '18 at 22:00

The specifications on that cable look pretty sketchy. In particular, I don't see anything which would specify that the differential pairs are to be twisted together, or that they need to maintain a 90Ω characteristic impedance. A cable without these features may not even support USB2, let alone USB3.

  • \$\begingroup\$ I take apart the cable,saw the differential pairs are twisted together. This cable is made of ready-made USB3.0 cable. \$\endgroup\$ – 張簡麒耀 Oct 30 '18 at 10:38

From the cable drawing, the split ends are 20 mm long. The splits generally lose the differential impedance match, so this cable, as drawn, should have difficulty to work at 5 Gbps USB 3.0 rates. 20 mm of impedance mismatch will substantially degrade the link's electrical characteristics, since 20 mm is about 1/3 of dominant wavelength of USB 3.0 signal, which is bad from transmission line standpoint.

However, as shown on photo, the shields seem to be much close to the connector, unless you pull the foil wrap accidentally during the cable disassembly. So, this cable should work, theoretically.

Practically a good deal depends on quality of PCB traces around the connectors, which you didn't reveal. Are they designed for 90 Ohm differential impedance, and how long the PCB traces are?

To get any result with this custom interconnect, you need to design and manufacture a test fixture consisting of two small PCBs with your connector, and PCB traces to high-quality SMA connectors. And then test this entire channel for compliance with USB 3.0 signal integrity requirements for USB cables. This is how the test fan-out board looks like (for a standard USB 3.0 connector, from Allion Labs):

enter image description here

In your case you need to re-engineer the test fixture by replacing the standard connector with your proprietary receptacle, and run all necessary tests using proper eye diagram and TDR equipment. To get better results, your test boards should include PCB traces as close as they appear (length and spacing and PCB stackup) on your actual host and device boards.

  • \$\begingroup\$ Host PCB:The TX-,TX+ traces about 25mm RX-,RX+ traces about 44mm . Device PCB:The TX-,TX+,RX-,RX+ traces both about 15mm. They have been designed for 90 Ohm differential impedance. \$\endgroup\$ – 張簡麒耀 Oct 31 '18 at 7:53

I am not an expert on differential microstrip PCB layout, but the problem is most likely on the host side. The problems I see with your routing:

  • A >5mm open stub on one of the differential lines. At 3GHz (~50mm/s on a microstrip), that is enough to cause a reflection that is ~20% out of phase (>70°) with the signal and present a reactive load to the line and cable.
  • Although I don't see where the termination resistors are and what is considered common practice, the delay compensation squiggle on one of the lines in a pair introduces an impedance discontinuity that will cause reflections on a microstrip that is nearly a wavelength long.
  • You should seriously consider moving your common-mode chokes as close as possible to your termination and USB 3.0 IC.

You might be able to salvage this iteration by intentionally introducing some loss by populating those 0Ω resistors with actual small resistors, but that would be a long shot at best.

  • \$\begingroup\$ Sorry,I don't understand which will cause reflections on a microstrip.Do you mean the 5mm open stub on one of the differential lines? \$\endgroup\$ – 張簡麒耀 Nov 2 '18 at 2:01
  • \$\begingroup\$ Yes. 5mm is ~10% of the wavelength. \$\endgroup\$ – Edgar Brown Nov 2 '18 at 2:02
  • \$\begingroup\$ Sorry. I misunderstood, I think you were actually talking of the serpentine section used to compensate trace length. That also causes reflections. \$\endgroup\$ – Edgar Brown Nov 2 '18 at 2:04
  • \$\begingroup\$ You said that A >5mm open stub on one of the differential lines is mean the blue lines left side of rx? \$\endgroup\$ – 張簡麒耀 Nov 2 '18 at 6:47
  • \$\begingroup\$ This might help (electronics.stackexchange.com/q/87779/202270). Any piece of transmission line that is attached to another transmission line is known as a stub. \$\endgroup\$ – Edgar Brown Nov 2 '18 at 13:23

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.