Can anyone here sincerely verify my schematic and let me know whether it'll work or not?

[Prajnyajit]

Hi,

I'm mounting STM32L476RGT6U on PCB. For that, I have made this schematic. I need some expert suggestions from anyone who has in-depth knowledge of this. I'll use an ST-LINK V2 to debug and upload the program to the MCU on PCB.

[KnarfB]

Read and compare to

AN4555

Application note

Getting started with STM32L4 Series and STM32L4+ Series

hardware development

hth

KnarfB

[Prajnyajit]

That I have already seen and made it referring to that only. Rather, you can give your expert opinion, if any modification is required.

[KnarfB]

You have changed NRST circuitry. This is usually a "wired or", see ref. I wouldn't use a serial capacitor in the way you did. NRST is an IO pin.

Didn't look into more details.

hth

KnarfB

[Javier1]

Why do you think it wont work?

The schematic is only half of the information needed here, could you post PCB snapshots?

[Prajnyajit]

Thanks, Javier. I have made this schematic as per best of my knowledge. I'm new to this MCU and STM too. Most of the people are placing MCU with a development board on their PCB, which is why their work is simpler as they don't have to care about MCU detail pinouts. But my work is different as I'm placing only the MCU on my PCB. If a wrong connection happens here, the entire PCB board will not work and become waste; waste of money and effort. That's why I'm seeking expert reviews and suggestions from people like you. If If you agree that everything is correct on this schematic, I'll proceed with the PCB layout.

I have mentioned all the connection-related stuff in the schematic itself. PCB file will be just the total system nothing other than that. I just wanted to verify this MCU part from you all. Anyway, if it's okay and correct I'll post the entire PCB screenshots.

[Paul1]

1. Don't like reset circuit. The cap should always be connected. Switch parallel to cap, Personally I add room for an external pullup 10K (you don't have to populate it, but I do). I don't see a good reason to do your Reset different from development PCBs.
2. VDD Caps: Better to arrange your decoupling Caps and other parts with GND downward. Caps at top with GND up is messy.
3. PCB Layout of Decoupling Caps and Oscillators is critical. Do those first with minimal length traces. Target 0mm long, yup 0mm, though <10mm will work in most cases.
4. Suggest separating VDDA/VSSA from VDD/VSS using 0ohm jumpers. That will force you to lay out those traces separately. Even if not critical in this design, it is just good proactice to keep analog and digital separate for future designs.
5. Route VDD, GND, and all unused signals to a header(s). It sounds like you are making this as a base for several projects, so bringing these signals to accessible points may be useful. If thats not correct then you can ditch the header(s).
6. Can't see where several signals go (I2C, STLINK, SPI, etc.) so can't evaluate those.
7. Does LoRa = SPI? Is NSS same as SCC chip select? Didn't check if on correct pin. Useful to show MX setup of IC has matching pin definitions.
8. Switches: You have switches on BOOT0 and NRST that can leave those pins open when in middle state - DON'T. Put a pullup/pulldown and have the switch pull the signal the other way. i.e. a Pullup with a switch to GND. You don't want your signal floating, even if the switch is only two position and spends little time between. Floating == RF Antenna == Unpredictable behaviour should the switch change slowly or become faulty or be unpopulated. A cheap pullup resistor will avoid all those cases.
9. *I use STM32L476, order chips now, stock difficult to find during Covid.

Paul

1.  

[Prajnyajit]

Have you mounted STM32L476 on PCB? Can you please provide your schematic for STM32L476 so that I can compare and modify mine as per my requirement?

If I need can I order from you?

[Paul1]

We used these ST boards before making our own board

• STM32L476G-EVAL (expensive)
• STM32L496G-DISCO
• You can load STM32L476 code onto either of these

Attached example schematic (pdf and DipTrace files)

• L476_baseV00PR_DipTrace.zip
• Proprietary circuits removed
• STLinkV2 with UART (14pin)
• Option: USB-C VCP
• Option: DAC for real time diagnostics and
• Option: Replace DCDC circuit with lower cost option if lower source voltage VH.
• Option: LEDs and switches powered from 3V3, change resistors appropriately, careful of required voltage for selected LEDs, as indicators 0.1mA is often plenty.
• RGB LED - Careful: Orientation mark is Pin4 Anode, not pin1. Ensure properly instruct solderer or factory, or delete it.

Paul