First of all, I want to let you know that I am a total noob, I am telecommunications engineer working for a company that manufactures embedded devices. My background is more related about embedded software / cybersecurity.
I designed everything and sent it to JLCPCB for manufactoring.
When connecting the PCBA to the USB, it was not recognised by my computer.
I started measuring 3V3 signal with a multimeter and it gave me only 0.5V and I don’t know why. I suppose that the problem is the voltage regulator (because the USB is giving me 5V).
So, I just desoldered the voltage regulator and injected and external 3V3 voltage supply. With this, my PCBA is working as expected (I flashed a simple SW to make a led flash, and it is working).
I cannot attach the files directly, so I give you screen captures of the electric schematics and PCB design.
Can you help me, please? I know that some traces have incorrect angles (more than 90 Âş). Could it be the problem? Any other good design rules or tips are appreciated.
By the way, no errors in the DRC, only warning about silkscreen, but I didn’t send the silkscreen layer to be manufactured.
Thanks in advance!!
PD: I can only upload one image, sorry. The voltage regulator is this model: RT6150BGQW (from 5V to 3V3).
Schematic or whole project would probably be more useful to check if there are any inconsistencies. If you read a few more topics/posts your membership of the forum gets upgraded and you can post more files.
This forum tries to focus on KiCad usage questions, so a design review (or troubleshooting) is not really in scope (this thread may be closed at any time). eevblog has a very active forum with a section specifically for beginners.
The inductor between pins 2 and 4 is unlikely to be suitable for a switcher. It looks like a chip inductor to me. Read the datasheet about inductor selection.
I haven’t seen the schematic, but the GND zone is also atrocious. The 5V SYS track should not cut though the GND plane, and definitely not anywhere close to the SMPS IC itself. More in general, PCB layout around SMPS circuits is quite critical.
For the rest: I also see other tracks randomly on top and bottom layer, and also sections of GND zone on both top and bottom. It’s just a big mess.
Yes, that’s pretty clear from your screenshot. I don’t want to discourage you, but on the positive side, there is lots of room for improvement. Maybe follow some course about PCB design, and look at PCB designs of people who have more experience, and then deduce why they’ve done tings in some particular ways. One of the names that springs to mind are the Youtube video’s made by Robert Feranec.
Have you any rationale for using Buck-Boost converter? Do you expect at input smaller voltage than at output?
For 1MHz DCDC PCB design is important.
I have never used DCDC converter to get 3V3 from 5V. Linear regulator gives you 66% efficiency without all DCDC converter associated problems.
At your first picture EN pin is connected to 3V3. Where from do you expect there voltage to tell IC to start operating.
I have also doubts about your inductor selection, but if it is good (we don’t know how (small) current you need) then may be the circuit only needs temporarily connecting 3V3 from exteranl source to get 1 at Enable pin and start operating.
Edit.
I supposed that schematic you linked is about the device that you are going to supply and not the schematic of your PCB so I didn’t looked at it. When I did it I see that 3V3 written at EN pin just confused me. It is not 3V3 but 5V through resistor.
Pins 1 and 10 are connected together on your PCB but they should form a feedback network via a potential divider. Pin 1 is the output and pin 10 is feedback.
Thank you for all your replies, they are really appreciated. In general, the PCB can be improved in several ways following your advices.
But the main problem was (as many of you commented) about connecting the FD pin (10) directly to VOUT (1).
I tested this manually by cutting the copper from the FD pin to the 3V3 trace and placing some through-hole resistors to build a voltage divider. Obviously, I still didn’t get the 3.3V, but 2.7, I suppose, because of the workaround is not very reliable.
The main reason of the RT6150BGQW model being placed instead of the RT6150B-33GQW (the one from the RPI PICO schematics and that gives you directly 3.3V so FD must be connected to VOUT) is beacuse the manufacturer didn’t have stock for RT6150B-33GQW, so I tried to find a replacement and didn’t check for the datasheet.
Thank you everyone.
If I can, I will try to post the fixed version of the schematics and layout.
