2
\$\begingroup\$

A stm32f407vet6 module route DP (PB15/Pin54 of LQFP100) and DM (PB14/Pin53 of LQFP100) of one USB full speed port to two separate header connectors which are 7cm from each other. The module designer doesn't consider this USB port to be used (there is another USB port on PA11/PA12).

Since the MCU is placed in the center of the module, the trace length should be 3~6 cm each. It is possible the traces have via too. The board should be 2 layer to be low cost.

Will the USB full speed port work fine? Does the trace length need to be matched to some precision (like < 1cm) on the carrier board?

I'v read this How critical is the layout of USB data lines / how does my layout look?, but I'm still not sure about this specific case with separated trace that is routed without considering USB at all.

Update: This two wires are routed as non USB wire separately on the module, and are separated by 7cm, then also need to be routed by ~3cm each on the carrier board to go together again. The question is about how long can USB full speed traces be routed separated? If based on frequency and wave length, differential cable won't be needed for USB full speed - any to wire will work.

\$\endgroup\$
3
  • \$\begingroup\$ I think the answer you linked pretty much answers your question doesn't it? (I don't think you can have traces of different lengths without them being separated) Or do you mean with regards to capacitance to other traces near/under/over them being different for the + and -? \$\endgroup\$ Apr 22, 2020 at 4:41
  • \$\begingroup\$ The two pin are adjacent to each other on the IC, but after that , they goes apart to be 7cm far from each other. They are not routed as USB traces at all on the module, intended to be used as GPIO by the carrier board. This is like if you just use two separated wire instead of differencial pair/calbe, will full speed still work? \$\endgroup\$
    – jw_
    Apr 23, 2020 at 8:58
  • \$\begingroup\$ @user3052786 see my comment above, forgot to @ you \$\endgroup\$
    – jw_
    Apr 23, 2020 at 9:15

2 Answers 2

4
\$\begingroup\$

In accord with many USB layout guides, it is still recommended to route FS traces as 90-Ohm differential transmission line. However, it is nearly impossible to make 90-Ohm trace on a cheap 2-layer 1.6 mm thick PCB. It will take a lot of PCB space if done correctly.

FS signaling is not something of very high frequency. The carrier is 6 MHz, edges, let say, 24 MHz, so the wavelength is ~600 cm. So 1/10 of the wavelength is a lot, 60 cm, and 3-6 cm should not make big impact on signal waveform or essential impedance mismatch. So route your traces as a pair of ~0.5 mm traces 0.2 mm apart, and forget it.

\$\endgroup\$
3
  • \$\begingroup\$ Typo: "wavelength is a lot, 60 cm" - 600cm? But the traces are already routed as non-USB traces, 7cm apart on the module, in the carrier board, each trace need to be first routed to travel ~ 3cm to each other then after that they can be routed together. What about this 7-10 cm of separation? \$\endgroup\$
    – jw_
    Apr 23, 2020 at 8:56
  • 1
    \$\begingroup\$ If 7 cm is a SEPARATION between D+ and D-, then it is very bad. The traces should be routed together, as a pair. \$\endgroup\$ Apr 23, 2020 at 22:19
  • \$\begingroup\$ But the signal rate is very low, is there an estimate of how can the pair be separated? What about low speed? \$\endgroup\$
    – jw_
    Apr 25, 2020 at 4:12
0
\$\begingroup\$

Since the signal lines are not routed as a differential pair, I would avoid using this as USB. While the bus may work (e.g. if each trace is close to 45 Ohms), the large loop formed by 7cm separation could make for a decent amount of radiated emissions (and noise pick-up). Plus if they designed these signals only for general I/O they probably didn't put any ESD protection on them either.

Sounds like your module is something like this Banggood one: https://www.banggood.com/STM32F407VET6-Development-Board-Cortex-M4-STM32-Small-System-ARM-Learning-Core-Module-p-1460490.html Note that their "chip introduction" lists the possible features of the MCU, not what they have implemented on the board.

\$\endgroup\$

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.