I have designed the following FT232H circuitry into a board on which I require a USB to I2C interface:

enter image description here

This circuit largely comes from the schematic for the UM232H eval kit (which I have and it works) and the Adafruit FT232H Breakout board:

https://ftdichip.com/wp-content/uploads/2020/07/DS_UM232H.pdf https://learn.adafruit.com/assets/88382

I am using a bus powered configuration, so VREGIN is the USB 5V and VCCD is the 3.3V output. For some reason, however, whenever I plug the USB cable into my PC running Windows 10, I get the following error:

enter image description here enter image description here

I followed the procedures FTDI provides in their driver installation guide (https://ftdichip.com/wp-content/uploads/2022/05/AN_396-FTDI-Drivers-Installation-Guide-for-Windows-10_11.pdf), but I still see this error. I suspect a hardware issue but I have not been able to find the problem. I have confirmed that "VBUS" is approximately 5V, "3V3" is approximately 3.3V, and "VCCCORE" is approximately 1.8V. Have I missed something? I realize I have to tie ADBUS2 to ADBUS1, but that wouldn't explain why the PC isn't recognizing the device.

EDIT: I have confirmed that VCCA does not show any voltage. According to the datasheet I expected to see 1.8V:

enter image description here

EDIT 2: I have also already referred to a number of threads here, most notably this one: USB device not recognized I looked the USB device up using the Device Manager and it has not gotten to the point of recognizing the VID/PID. The error I am seeing is "Device Descriptor Request Failed":

enter image description here

  • 4
    \$\begingroup\$ FYI, device descriptor request failed typically means that the port is being pulled (pullup/down resistors) as if a device is connected, but there is no response (thus it doesn't return a descriptor). \$\endgroup\$ Commented Oct 18, 2023 at 13:34
  • \$\begingroup\$ Either the problem is not on that part of schematics, or it is but not a schematic design error but it could be a PCB design error or some manufacturing error or just faulty component. Shorted or wrong cap would do that, also incorrectly oriented chips, solder shorting stuff etc. Other options apply but if you don't get proper voltages it's pointless to try if the crystal oscillates. Show more of the surroundings in schematic, and PCB design, maybe photos of the PCB to find out what's wrong. \$\endgroup\$
    – Justme
    Commented Oct 18, 2023 at 15:18
  • \$\begingroup\$ @Justme board inspection with 10x magnification turned up no solder bridges, incorrectly oriented components, etc. VCCA cap is not shorted (and I would have expected it to drag down VCCCORE if it was). I am beginning to think the chip itself might be faulty. I see no other reason why all of the other supplies are reading fine but VCCA (which should be connected to VCCCORE internally) reads 0. All connections between the chip pin and capacitor look and measure correct \$\endgroup\$
    – DerStrom8
    Commented Oct 18, 2023 at 15:24
  • \$\begingroup\$ Have you checked if all pins are properly sodered. I had a similar problem as my TEST pin was not connected to GND properly. \$\endgroup\$
    – Janes
    Commented Nov 17, 2023 at 16:35

1 Answer 1


The FT232H chip is a USB2 high-speed (480Mbps) device. You however are using 27R/47pF filter on DP/DM wires. You cannot do this. "USB full-speed compatible" means that the FT232 device will respond to FS host traffic if the host is FS and will ignore chirping negotiations. But you cannot suppress chip-K from FT232H, and since your host is HS, it will chirp back and end the link in HS terminated state and will start 480Mbps signaling, and this signal will be severely crippled by your RC filter. Remove C2 C3 and use zero ohm in R6/R7 places, and everything will work fine. See for details this answer: https://electronics.stackexchange.com/a/311591/117785

  • \$\begingroup\$ Interesting, and very good to know! However, I'm not sure this would explain 0V on VCCA even though it is supposed to be internally connected to VCCCORE, which measures 1.8V \$\endgroup\$
    – DerStrom8
    Commented Oct 24, 2023 at 11:20
  • 1
    \$\begingroup\$ @DerStrom8, the VCCA is some other internal voltage regulator. After an attempt of enumeration has failed, the chip is likely in SUSPEND state. In many designs some powers are shut down and clocks are stopped. I am sure if you look at this pin with a scope, the pin will be up for 100-150 ms, and only then will go down. You also need to make sure that your particular XTAL is not overloaded with caps, and that the clock ever starts, during the initial start-up at least. \$\endgroup\$ Commented Oct 26, 2023 at 3:42
  • 1
    \$\begingroup\$ @DerStrom8, another one, to check the active state of the chip, you can simulate USB_RESET condition by shorting D+ to GND. The chip should wake up, clock should start running, and all voltages would go to designated levels. \$\endgroup\$ Commented Oct 26, 2023 at 3:45
  • \$\begingroup\$ This is excellent information, thank you very much! I will look into these suggestions and see if I can't get this board to work. Much appreciated! \$\endgroup\$
    – DerStrom8
    Commented Oct 26, 2023 at 12:29
  • 1
    \$\begingroup\$ Can confirm, removing the filtering seems to have fixed the issue. Thanks very much! \$\endgroup\$
    – DerStrom8
    Commented Oct 27, 2023 at 16:49

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.