Schematic review and suggestion needed

Schematic
1

hey, this is my first 4 layer design and yesterday only I got the PCB assembled by pcbway, also this is the first time I am using renesas mcu so don’t know much about it. can anyone point out if few things are wrong in this???
the issues I am facing right now after testing PCB with multimeter.

  1. board is not powering up with micro USB port also I found out that the vbus pad on the micro USB port is giving me 0.4v where it should give 5v~. when tested further q1 and q2 mosfet seems to be damaged but how could this have happened as soon as I plugged the micro USB cable for the first time? please give suggestions on this.
  2. from ldo side it should give 3.3v but it’s giving 3.195v but then to the renesas mcu it’s giving 3.045v~ is this ok for mcu to operate?
  3. I wanted to see if I can flash the firmware for that I have to pull down MD and connect USB but since USB didn’t worked so this also didn’t work.
  4. then I thought of connecting the board with st-link(in swd interface) to see if it’s at least detecting the mcu. i am not sure if st-link would work with renesas mcu or not but I found on other forums that it worked for some. what are the others ways to just see that if mcu is getting detected by PC or not? overall can anyone see if the connection for the renesas mcu swdio,swclk and USB connection looks correct or not…
    another thing is while testing the vbus voltage I though because of the damaged mosfet it might be showing 0.45v so I desoldered q2 and then checked it was still 0.45v.
    thank you
    image
    image1461×986 114 KB
1 Like
2

What is you KiCad specific question ? this Forum is, after all, specifically about KiCad … . .

1 Like
3

Your schematic looks like a mess, and I don’t want to go too far into it. Most of your questions are also outside the scope of this forum.

I see some open wire ends on U2 pins 4 and 8. Does ERC complain about anything?
Why not keep all the power delivery stuff together. Connect Q2 directly to U1 and also put the decoupling capacitors there. Also connect the LED directly to the power supply. Keep related parts together to reduce clutter and get a better overview of the whole thing.

Your microcontroller symbol is also a big mess, Pins in footprint order on the schematic do not work well. You’d have to go hunting for any sort of logical connection with both the power and GND pins hidden somewhere along those rows.

And another dislike for various overlapping texts. It just makes it more difficult to verify connectivity.

It also looks like you have used R_Small. I never use it, because you can place the value of resistors inside the normally sized version. As a result the total schematic area needed is smaller. Use RKM_code for resistor and capacitor values. Quicker to type, and it avoids doubts about dots on too far compressed JPG’s or low resolution png’s.

What is the use of Q1? For reverse power protection, you may as well replace it with a piece of wire.
I never like FET’s connected directly to connectors. There are too many non-obvious paths for EMC / ESD.

You can also never exclude a simply faulty part or a short circuit. You will never find those by analyzing the schematic. Another common thing you should verify is the pin mapping between symbols and footprints.

Does ST-Link work with Renesas processors. Gosh.

How can anything work that way? It looks like that is the only power entry into your circuit, so is there another power input hidden in between all those little sections, or is the pin mapping between your USB connector and the footprint wrong?

Operating voltage for your uC is in the datasheet. That is easier for you to verify then for me (I’d have to download the datasheet first).

Little circuits such as Q2 / Q3 can easily be simulated or verified on a breadboard. For fault finding, you can disable and bypass them on the PCB.

1 Like
4

Yes, I was wondering exactly what Q1 / Q2 were doing, then I realised it had nothing to do with the big chip at all! (and still don’t see what they are doing!).

In terms of debugging: if the input 5v is getting dragged down, then remove stuff (Q1 / Q2) until the volts are right again. I’m guessing that the USB is plugged into a PC port… how much power can that port provide? Maybe not enough? What happens if you plug into a suitable 5v power supply?

And there ends lesson one of ‘debugging a non working circuit’!

As others have said, debugging non-working PCBs is beyond the remit of this forum, you need a more general ‘electronics’ forum.

5

They probably protect against using specially prepared USB cable with crossed GND and +5V wires.

1 Like
6

image
image749×704 4.85 KB

found the problem i stupidly used the default kicad footprint for the mosfet(1=d,2=g,3=s) which is different from what I am using right now.(1=g,2=s,3=d) Now how do I change pinout for this mosfet in kicad I can see an option to edit the pinout

7

You can change the pin numbering of any footprint in the Footprint Editor but that is a very bad Idea in this case, because pinouts are (mostly) standardized. SOT-23 is always a bit problematic, because different locations of pin 1 have existed from the beginning of that footprints existence, but the “alternative” pinouts have (finally) mostly become obsolete (or at least I think / hope so).

The normal way to do this is to change the schematic symbol. KiCad has Q_NMOS_ fets with GSD in all 6 possible pin combinations.

image
image1041×736 111 KB

8

Can you tell us the voltages around Q1 and Q2?

rom ldo side it should give 3.3v but it’s giving 3.195v

What voltage is the LDO input?

3.045v~ is this ok for mcu to operate

What does the Renesas datasheet say?

When you draw a circuit like this with all references and few / no wires it becomes difficult for someone to get a sense of what is going on. The result is most folks will not bother to try.

I’m going to guess you copied most of the circuit from somewhere else and are not familiar with all the functions. IMHO you should have made this board with two layers by making it larger. Being a whole new design that you aren’t familiar with (I think I’m being kind here) on a 4 layer board takes balls.

9

I am (since always) afraid of doing such mistakes. Because of it I have in my libraries only symbols with assigned (and carefully checked) footprints and after placing a symbol at schematic I never edit any its parameters. I have never went through footprint assignment at schematic.

1 Like
10

Before ordering I print out a 1:1 of the layout. I them put the actual part on the printout.