I am designing a USB full speed board around the STM103XX MCU and was wondering how to physically position the 1.5K pullup resistor on D+. Should it be next to the MCU or close to the receptacle or what? Does it even make a difference? I have attached a snapshot of the layout below. Thank you.
Best Answer
The placement may not be that critical, but it never hurts to apply what application notes usually suggest for USB designs.
Since the R3&R4 are the termination resistors to match impedance, the 1k5 pull-up resistor should be on the connector side of R4, not on the MCU side.
USB terminating resistors R3&R4 should be close to the chip, within 200 mils, not close to the connector.
1k5 pull-up should be controllable by the MCU, as it could take more time to boot the STM32 firmware than the host tolerates for enumeration
Stubs should be avoided. The trace from the differential pair to R5 basically forms a stub, even if it is very small. The resistor pad could be just in-line with the trace without stub. Smaller size resistors would have smaller pads. The stub length is well within recommendations.
It is not suggested to connect USB shield directly to ground plane and shorting to USB GND, but via capacitor.
VBUS and/or GND are sometimes filtered with ferrite beads.
Don't put more than the allowed 10uF capacitance on VBUS
Don't draw more than the allowed 100mA until MCU has completed enumeration to request more current from host, and the host has allowed it
USB DP/DN is a differential pair whose impedance should be 90 ohms
Avoid traces that run in parallel near USB traces. There should be 20 mil gap to non-periodic low speed signals, or 50 mil gap to clock signals.
If you don't pass EMI testing, you might need to add a common-mode choke near the connector. The ESD protection should be located between connector and common-mode choke.
Match trace lengths to within 150 mils. Looks fine.