I've made a USB hub PCB using a USB2517 controller, but it's not working. When I plug it into the host computer, I get a "not recognised" message on Windows and "unable to enumerate" message on Linux.

I'm not able to identify the problem. The USB2517 seems to power on at first (current consumption goes up and 1.8 V at pin 25) and after the "unable to enumerate" message it powers off (0 V at pin 25).

You can see the schematic I've used:


You can find here the KiCad project with schematic and PCB layout: KiCad project. The idea of the PCB is to be an USB hub/power dispatch for a robot. Two batteries are plugged in - one to power the "logic" side (Arduino and STM32 boards) through the USB cable and one that is connected to power motors and actuators.

Do you have any idea what the problem can be?

Please keep in mind that I'm a computer science student, making PCBs only as a hobby.

Thanks for your help.


I have to admit, I made some dumb mistakes. I'm not a pro in electrical engineering and I'm very grateful for your answers.

Following your recommendations and Microchip's reference design, I modified my schematic.


You can find the full schematic here.

Decoupling capacitors for VDD33 were present, but not shown in the previous screenshot.

I found these ESD diodes (CG0603MLC-3.3LEA) with a capacitance of 0.5 pF. Are they good for my application?

Do you think that my new schematic is correct? I don't want to make other mistakes.

  • \$\begingroup\$ Why CFG_SEL2 is floating? Why rest of the strap pins are not strapped high or low? Why are pins 62 and 25 not connected to capacitors? \$\endgroup\$
    – Justme
    Commented Feb 26, 2020 at 12:31

1 Answer 1


I'd recommend for you to always read the datasheet of the IC you are designing a circuit for, you can NOT send your design for fab without scrubbing through every little detail. Also, take a look at Microchip's reference design for that USB hub and compare with yours: http://ww1.microchip.com/downloads/en/DeviceDoc/evb2517sch.pdf

Here are the main concerns:

  • Pin 25 and Pin 62 can NOT be floating, there are important core and PLL power output and need decoupling capacitors attached. When you see "must have" in the datasheet, it's not a fluke... The hub is most likely not booting because of those missing capacitors.

enter image description here

enter image description here

  • Where are all your decoupling capacitors for the VDD33 inputs? Are you not showing them or are they none? Please make sure you follow the datasheet and reference design recommendation for proper decoupling.

  • If you intend to use USB High-Speed (480Mbps) then use lower capacitance ESD diodes. The ones you are using (esd9b3.3st5g) have too much capacitance (15pF) and will cause poor signal quality, find some ESD diodes with under 1pF of parasitic capacitance instead.

  • Do not tie RESET_N to +3V3 without a pull-up resistor (10k or so), how would you be able to reset the hub for troubleshooting/testing?

  • 1
    \$\begingroup\$ In addition, the reference design shows an R-C combination on the RESET_N pin to provide a rising edge after power-up, which is how the chip configuration is determined. Furthermore, you have left CFG_SEL2 floating and there's no indication that this is allowed. Pull it low or high. \$\endgroup\$
    – Dave Tweed
    Commented Feb 26, 2020 at 12:36
  • 1
    \$\begingroup\$ In another addition, the VBUS_DET signal is in 3.3V domain, and it is recommended a resistor divider from VBUS to this pin, something like 50K:100K. Drect 5V to IO pin might fry the chip. Why don't you follow their reference design documents? \$\endgroup\$ Commented Feb 27, 2020 at 3:49

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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