Electronics > Projects, Designs, and Technical Stuff
STM32F103 min system with USB-TTL converter?
thm_w:
--- Quote from: bjdhjy888 on August 14, 2019, 01:43:36 pm ---I re-drew my schematic from scratch, correcting all my previous mistakes.
Would you please help me review my latest schematic? Thank you so much!
The STM32 min. systems is supposed to blink an LED, with the function of USB-TTL.
--- End quote ---
Looks good and neat.
NRST should be 100nF not 100pF, but its optional like you said.
What is the purpose of the diode on RxD line?
bjdhjy888:
--- Quote from: thm_w on August 15, 2019, 10:36:26 pm ---
--- Quote from: bjdhjy888 on August 14, 2019, 01:43:36 pm ---I re-drew my schematic from scratch, correcting all my previous mistakes.
Would you please help me review my latest schematic? Thank you so much!
The STM32 min. systems is supposed to blink an LED, with the function of USB-TTL.
--- End quote ---
Looks good and neat.
NRST should be 100nF not 100pF, but its optional like you said.
What is the purpose of the diode on RxD line?
--- End quote ---
Thanks for your help.
As far as the diode is concerned, I previously copied it from another schematic from the Internet, and now it's been removed from my latest schematic.
I've also fixed some minor mistakes today.
Here's my current schematic and layout. Any suggestions would be highly appreciated.
I will get the PCB manucfactured once it's free of mistakes. (The GPIO is left out doing nothing on purpose. I will wire it to STM32 in my next design. And I will pour some copper once the schematic is free of mistakes.)
Bless you.
profdc9:
If it would help, I have a kicad project with my own version of the bluepill STM32F103C8T6 you could start with if you want to make your own development board.
https://github.com/profdc9/STM32alt
I also made one for the STM32F4 as well
https://github.com/profdc9/STM32F4ThruPill
I made these so that generic through-hole parts can be used, but you can change the footprints if you choose.
thm_w:
--- Quote from: bjdhjy888 on August 15, 2019, 11:58:05 pm ---Thanks for your help.
As far as the diode is concerned, I previously copied it from another schematic from the Internet, and now it's been removed from my latest schematic.
I've also fixed some minor mistakes today.
Here's my current schematic and layout. Any suggestions would be highly appreciated.
I will get the PCB manucfactured once it's free of mistakes. (The GPIO is left out doing nothing on purpose. I will wire it to STM32 in my next design. And I will pour some copper once the schematic is free of mistakes.)
Bless you.
http://chuantu.xyz/t6/702/1565913407x2073530527.png
http://chuantu.xyz/t6/702/1565913446x2073530527.png
http://chuantu.xyz/t6/702/1565913459x2073530529.png
--- End quote ---
- I normally like to see some outlines around the capacitors/resistors in the silkscreen to make it clear where to place it (like C9 has). But that is more for convenience when building, you dont have to have it. I wonder why yours do not show up.
- The placement of C6 is not bad, but C7 and C8 can be improved. They can be closer to pins 24, 36, 48, and two do not share the same pin. So you have one at 24 one at 36, etc.
- TX1 and TX2 should be closer to the microcontroller. For example, TX1 you have long traces traveling to the left, what you can do is move TX1 into the space to the left of the chip, so the traces will be a lot shorter.
- I would put your name and date on the PCB as well on the silkscreen, if you ever want to show someone.
mariush:
The board's a bit of a mess...
Get your oscillators closer to the ICs ... get your capacitors closer to the oscillators/crystals.
I'd leave space to lay the 32kHz crystal flat on the board... maybe solder it to a third pad with a bit of solder, or have a loop of wire keep it from vibrating or hitting the board.
careful with 1117 regulators.... some are unstable if the output capacitance has too low ESR ... some 1117 linear regulators require ESR on output between 0.1 and 1 ohm ... a ceramic capacitor on output will have too low esr... so either add a tiny resistor in series with the output capacitor , something like 0.22... 0.47 ohm or whatever, or just use a regular electrolytic capacitor (ex a 10..100uF 10v electrolytic )
or just use a better linear regulator.
add some decoupling capacitors between vin and ground on your micro ... a 100nf ceramic (0.01uF)
200 ohm is kinda non standard value... no need for such value for a status led... i'd say just use 330 ohm or even 470 ohm... more common value.
I wouldn't use surface mounted electrolytics (c9)... i'd suggest plain boring through hole, or polymer surface mount
Navigation
[0] Message Index
[#] Next page
[*] Previous page
Go to full version