The boost converter has an inductor that is too big for its switching frequency. It has to be replaced by one of 3.3uH

at moment I've set a creative common license,
but we need to evaluate other options.

Can I replace by the WROOM ?

The IO0 pin should be connected to the GPIO0 and to the transistor circuit to allow the MCU programming

license and open source hw logo on board

The input of the battery charger is connected to its output (5V), provoking a loop. It needs to be connected to VBUS

The datasheet recommends a capacitor in parallel to the resistor that is between the diode and the feedback node

The SDA and SCL signals are swapped. Since they are coherently swapped in the whole design, it is enough to swap them at the silkscreen of the 40-pin connector

The UART0 is the one that programs the microcontroller, while the UART1 is a generic one. In the current design, the UART1 is connected to the USB/UART transceiver, so it is not possible to program the microcontroller through the USB interface

Hello @dorvan , @Doenec ,

I am @clearemc we discussed about doing a first revision oriented to Electromagnetic Compatibility (EMC).
First of all, congratulations for your work and for your efforts to make it an open hardware project!
Thank you for letting me participate in it.
I have done a general review of the schematic and indicated some modifications that can reduce problems during the certification phases.
I have also indicated some points that an affect to the functionality of the board.
Here it goes!

On Schematic:

• Connector J3: SPI
• The 3 critical signals for SPI (MOSI, MISO, SCK) arrive all together to the connector. If possible, add a grounding pin in the middle of them, so you reduce crosstalk as much as possible. The ideal solution would be MOSI – GND – MISO – SCK – GND, but that would be too much space, so, try to isolate at least the SCK signal, because it will be always active during the communication.
• U7: ADDR pin à Datasheet states that it can be left floating, but since it is an input, it is better to connect it to ground to avoid susceptibility issues.
• This is applicable to all input pins that are floating, is it recommendable to tie them to ground or to a fixed voltage.
• U8:
• I7 input: if not used, better connect it to ground.
• J1: it is better to connect the shield to ground.
• I recommend you to leave the footprint for 1 or 2 components in parallel to ground, so you can add one or two capacitors, or even a RC circuit.
• U5:
• Pin 6 goes to a decoupling capacitor, but it is not connected to any power net.
• Connector J4: 12 V line. Add some protecting components, such as a diode for polarity reversion protection and a TVS to limit transients and overvoltages.
• RTC:
• Add reverse polarity and overvoltage protection to the coin cell battery.
• The oscillator Y2 has not capacitors, it needs 12.5 pF capacitors to oscillate.
• Power connector J5: if this is the general power input of the board, it will need protections for reverse polarity and also a common-mode and differential-mode filter.

General:

• Communication and digital lines: it is nice to add a series resistor of about 100 ohms to control the slew rate of the communication lines, as well as to limit the current for the digital ones. It can be quite useful in tests such as susceptibility, ESD, or even to avoid crosstalk.
• Net I34 is not connected to resistor R52

Please, let me know if you have any question or remark.
When possible,
I will perform a review of the layout!

Kind regards
@clearemc

The connection of the pins RX/TX between the CP2102N and the SP3485EN are swapped. The connection should be as follows:

There is a floating ground plane under the inductor L2. It has to be removed to reduce noise and guarantee a correct functioning of the converter