I have designed two PCBs, both using a FTDI231XS USB to serial chip to program an ESP32. Both boards have the same circuit design to control the FTDI231XS chip. One board was hand soldered (board A); the other has been manufactured (board B, with smaller SMD components). Board A works without a flaw. Board B won’t however be recognised by my computer (serial port is not shown, computer has all the needed the drivers and is completely updated). The message that the attached USB device is broken is displayed as soon as the PCB is plugged in (under device manager it shows the device couldn’t be reset). In my humble opinion the circuit design to control the FTDI231XS should be correct, as it has been taken from the ESP32 thing by Sparkfun.

Here is the circuit in question (board A and B): circuit design

And here are photos of the PCB designs. Board A (I know that in this photo USB D+ and USB D- are interchanged, during soldering I rechanged it. Also, only the USB type B connector was populated during testing): board A

Board B (machine soldered): board B

To your information, I know that my board design is not perfect, I am still a beginner in this field and so very thankful for constructive critic besides an answer to this problem.

  • 1
    \$\begingroup\$ If you had a logic analyzer , where would you check? \$\endgroup\$ Commented Jun 25, 2020 at 21:24
  • 1
    \$\begingroup\$ Problem has to be between USB connector and the FTDI chip. Since boards share the schematics, that can't be the problem. They do have a wildly different PCB layout, which may explain something, because it's not routed according to good practices, so you might want to read application manuals how USB should be routed or how to place bypass caps near chips etc, maybe the FTDI appnotes even tells these. Check that 5V and 3.3V voltages are present at respective pins/capacitors, no soldering issues (loose joints or shorted joints). Also check chip is mounted the right way. \$\endgroup\$
    – Justme
    Commented Jun 25, 2020 at 23:24
  • \$\begingroup\$ Thanks for your answers. So in the meantime I have checked the joints (no problem, no shorted joints), chips are correctly mounted, 5V and 3.3V is also ok. There is a slightly lower 5V voltage present on board B (4.85V in board B instead of 4.9V of board A): I will check the FTDI USB hardware design guides as next. Can the routing design really make such a difference (maybe too many vias)? \$\endgroup\$
    – Cat Turbo
    Commented Jun 27, 2020 at 8:29
  • \$\begingroup\$ After looking into the design once again I noticed a very big issue with it: there is a serious missmatch in the length between D+ and D- for both design but it is more severe for design B. I would recommend to read up on differential signal routing and matching. There is a reason why many EDAs have dedicated tools for routing differential signals. \$\endgroup\$ Commented Jul 19, 2020 at 7:18
  • \$\begingroup\$ Thanks you very much for your answer. After I've began to read the design guidelines for the FTDI chips (see Application note AN_146) I completely agree with your observation and see that my second design is very stupid. I am in the process of redoing it. \$\endgroup\$
    – Cat Turbo
    Commented Jul 21, 2020 at 21:31

1 Answer 1


As others have pointed it already out, I didn't follow the design guidelines for USB connections. They can be found for example here or here

For USB connections the informations on page 14 of the FTDI design guidelines are especially important:

  • Equal length: Both DP and DM signals must travel the same distance. If one trace ends up longer, then the timing of the signals can be adversely affected and cause data errors.
  • Controlled impedance: The impedance of the twisted pair cabling must be matched on the PCB in order to minimize signal reflections. USB signals are 90Ω differential to each other / 45Ω each to Signal Ground. Most modern PCB layout software can be configured to route both of these signals together with these characteristics.
  • No stubs: When adding components such as transient voltage protection or additional capacitance for edge rate control, the DP and DM signals should not have any “T”s in order to minimize signal reflections.
  • Ground planes: With DP and DM being controlled impedance, they should consistently run over the USB Signal Ground plane. There should not be any splits in the plane directly under DP and DM.
  • Overall length: The DP and DM signals should be made as short as possible. For very short runs, less than 1cm, it may not be possible to observe the controlled impedance specification. In practice, this is usually acceptable provided the other practices are followed.
  • General design practices: Keep noisy sources away from the USB signals; avoid right angles; etc. USB Design Guidelines, p. 14

As it has been pointed out by Christian B. the problem lies with a high probability in the different length of the USB D+ an D- data lines. Also the arrangement of the corresponding condensators could be improved.

  • \$\begingroup\$ DId you need any special PCB fabrication to meet the controlled impedance requirements? \$\endgroup\$
    – DKNguyen
    Commented Jul 21, 2020 at 21:45

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.