Electronics > Projects, Designs, and Technical Stuff

STM32F103 min system with USB-TTL converter?

<< < (7/10) > >>

mariush:
Layout wise i would have some suggestions

try to have traces coming out of pads from the center of the side of a pad and try to get them perpendicularly. For example:
* traces coming out of C2 in your picture are fine... in the middle of pads
* trace coming out of C1 comes out of the corner directly at 45 degrees ... not nice
* traces on R2 and C5 coming out the edge of a pad... not cool
* two traces coming out of same side on R1 ... and you have that trace betwen the pads of the resistor when it could come from a side
* see two traces coming out of the 1117 ldo .. also consider thicker traces for  higher current

consider flipping c2 to shorten and simplify traces
 consider rearranging c2,c5,r2 to simplify traces there you have pcb area so its not a must to have them all 3 in line ... you can move the silkcreen or remove the actual values or move the values in legend somewhere you don't have parts

you could move the main crystal a few mm lower (shift the regulator lower or to the sides a bit) and make room for the 32.768 kHz oscillator above the main crystal and save a couple of traces on the bottom of the chip.

not liking those long diagonal traces on the bottom layer... i'd suggest planning for having a big ground copper fill on the bottom, so aim for using vias just to sort of create jumpers, to jump over top traces by placing small segment on the bottom. break that big ground fill as little as possible.

you could move mpu 605 and c12 higher, to shorten those 2 traces going to the header
also what's with the c13 , those red traces, are those supposed to cross over or is that an error ?
same nitpicking about vias coming out of pads weirdly ..see c14 and c15

CHK resistor can be placed by the led and this way you don't need that trace that goes around the connector...after all it's supposed to go to ground, so from resistor you'd have a via to the bottom ground fill and you're done.

you have a trace from c3 looping all the way around the headers on left and going to c5 .... i guess that's ground or something for both ... use a via to make a shorter trace or get them both to bottom ground fill through vias

you could flip the serial chip horizontally ( rotate 180 degrees) ... this way the 5v and ground would go easier to pads on chip ... maybe you would have to use a via for one of the data wires to step over the other one or you may be able to get them both through the center.
The ground pad of the chip can be connected to ground fill on other side through a via.

if it makes it easier for you ... draw a thick trace on the bottom layer that goes almost from one side to the other of the board and from that thick trace, route traces out of it which then go through via to top side and connect to pads that are supposed to go to ground.
When you'll do a ground fill, that trace and small traces from vias to it will become invisible, lost inside the ground fill.

later edit: probably not needed but since you have so much room, maybe leave a small island of copper fill around the tab of the 1117 regulator to act as a heatsink?
As i said before 1117 is kinda bad choice due to that low esr on output issue, but another problem is the tab is usually output voltage so you can't use vias to connect that tab pad directly to the bottom ground fill for better cooling.
maybe consider replacing it with a regulator that uses the tab for ground or uses the bigger dpak package (to-252 to-263) etc etc.
examples :
LF33  https://www.digikey.com/product-detail/en/stmicroelectronics/LF33CDT-TR/497-1532-1-ND/592050  (requires electrolytic on output)
NCP5501 https://www.digikey.com/short/p5d1tc  (stable with ceramic caps only on output)
MC3327 https://www.digikey.com/short/p5d1c0 (stable with ceramic caps only on output)



maybe remove the actual values of components and move the values in legend somewhere you don't have parts (could be on bottom side over ground fill)

thm_w:
There is no problem with traces coming out of pads at an angle. Try not to overwhelm the guy with information.

But good suggestions either way.

bjdhjy888:
Unfortunately, my project failed again. It really broke my heart!
p
The issue is, when I plug my board to my PC, via a microUSB cable, windows 10's Device Manager would show an exclamation mark and read "Unknown USB Device(Device Descriptor Request Failed)"

I'm sure my power is ok, cuz the LED by the mircroUSB plug is working. AM1117 is fine, cuz I used my multimeter and confirmed its voltages were all correct.

CH340C must be the issue. I checked the voltage between its pin 4 and pin 18, which was only 1.8V. It is supposed to be 5V.

So what is causing the issue?  I tried to solve it but failed.

I did check my schematic many times before I sent it to my PCB factory. 

Any ideas on how to solve this issue?

many thanks!

Fire Doger:
CH340 work without crystal? :o
Make sure it's the correct model.
Also C12 must be 100n not 100p. Datasheet says 0.1uF
Also D+ D- doesn't look like differential routing.

bjdhjy888:

--- Quote from: Fire Doger on August 30, 2019, 11:33:07 am ---CH340 work without crystal? :o
Make sure it's the correct model.
Also C12 must be 100n not 100p. Datasheet says 0.1uF
Also D+ D- doesn't look like differential routing.

--- End quote ---
Thanks for your reply. But I copied someone else's schematic and I bought his board and his board is designed exactly like mine, aka, his schematic. His board works fine and it works on my PC. But mine does not, on the same PC.
So I must be wrong.
Could it be my PCB routing? The width of my wires? (I did use Altium's check funtion and found no errors! strange)
Should I delete my copper pour and get it manufactured again, using the method of elimination?

Navigation

[0] Message Index

[#] Next page

[*] Previous page

There was an error while thanking
Thanking...
Go to full version
Powered by SMFPacks Advanced Attachments Uploader Mod