Electronics > Projects, Designs, and Technical Stuff
stm32 implementation feedback
mariush:
Rotate the chip by 90 degrees.
Make thicker traces to the IO pins... seem unnecessarily thin.
Any particular reason the DC In connector (or whatever) has to be all the way on the opposite side of the board?
Consider using a better switching regulator (synchronous rectifier so you lose the diode, higher switching frequency so you get smaller inductors)
Plenty of cheap 500kHz or higher switching regulators.
Seems like there's enough room on the board that you could have all the components on one side... and maybe make it cheaper to do reflow soldering on the boards instead of messing around with soldering each side or using glue on the parts...
ajb:
You've left NRST unconnected, that should get a pullup resistor and should be made accessible so that you can hook up an SWD debugger. Ideally you would also have an SWD header (either the standard 10-pin 50mil header or just extra pins).
SiliconWizard:
There is an internal pull-up in most STM32 devices on the NRST pin and I personally never added an external one. Look at section 5.3.14 of the datasheet. What's recommended though is to add a capacitor to ground (like 100nF) to avoid spurious resets in case of parasitics. If your intent is to add a lower resistance external pull-up for the same reason (the typ. internal pull-up is ~40k), I think the capacitor should be enough to do the trick. Just know there *is* an internal pull-up.
As to making it accessible for SWD, I'd recommend it but it's not 100% mandatory. You can absolutely connect via SWD without it, but not in all cases. One case you can't is if the MCU is in stop mode. So yes, if you ever intend to use low-power modes, you have to make NRST accessible to your SWD probe. If it's a development board, just do that, or your users may get angry. ;D
AndyC_772:
--- Quote from: Siwastaja on April 10, 2019, 12:06:40 pm ---I wouldn't make it 4-layer on such a super simple board unless I have unlimited budget. It may be only a few dollars in mid-sized batches, but for small quantity prototypes, the two extra layers would become the biggest expense of the project.
--- End quote ---
I find the danger with trying to fit everything on 2 layers is that, even if one layer can be a reasonably solid ground plane, the other is inevitably chopped up into bits, which negates the benefit of having it. Sometimes different parts end up completely disconnected, which is OK because the PCB software should at least warn you. Often, though, different areas end up connected through a long, thin, convoluted path which won't flag an error, but it isn't obvious just how bad the plane is unless you trace it out by hand.
Unless there's a strongly compelling reason, I never use 2 layer boards these days. A 4 layer board from somewhere like AllPCB is inexpensive, and it's a good habit to get into from day one. Don't waste any part of your life debugging avoidable signal integrity problems, there's really nothing good about them, not even the learning experience.
langwadt:
--- Quote from: capt bullshot on April 10, 2019, 10:40:11 am ---Looks like you didn't fan out the SWD (serial wire debug) / JTAG pins. It's highly recommended to have them on a conveniently accessibly connector, the ST-Link style debuggers are cheap and easy to use, way more comfortable than dealing with a bootloader.
Add a GND pin to the CAN connector. CAN without GND won't work.
--- End quote ---
and might want to add the option of a termination resistor too
Navigation
[0] Message Index
[#] Next page
[*] Previous page
Go to full version