I am creating a project for the first time and want to know the opinion on my layout of electronic components. Isn’t such a layout considered bad form? Or are there any comments on the placement of electronic components and sockets on the PCB?
The reason for the tight layout of courtyards of the footprints. - limitations of the stack placement of the Teensy board on one side and the finished main board, for which I am making an expansion board.
MP MIDI ext. 2.0 board.kicad_pcb (555.8 KB)
I don’t think your layout is “tight” at all. There is quite a lot of room in between your footprints.
The biggest problem I see is a lack of a proper GND plane (this is also the very most common mistake beginners make). The GND plane must be continuous, without being cut into pieces by tracks. It’s unfortunate that with KiCad’s default settings, the GND plane does not go in between THT IC’s and headers. Reducing the clearance is a “quick fix”, but I never use the default DIP symbols, but always modify them to have oval pads, and make them narrow enough so the GND plane connects in between the pads.
Next thing, I do see a few decoupling capacitors (C11, C12, C13) but their placement is not so good. Make the tracks that connect them to your IC’s as short as you can.
I also see very little power conditioning. Apart from the decoupling capacitor, it’s also very common to add a bigger buffer capacitor (something like 100uF) (but this also has it’s problems with inrush current). On my breadboards and matrix boards (which don’t have a decent GND plane) I’ve also had a lot of trouble with induced noise, especially from switching incandescent and halogen lights. The only real fix for this is to add filtering such as ferrite cores, chokes or an inductor.
Another consideration is to think a bit about input protection. From over voltage to reverse voltage protection. I normally add local voltage regulators, which allows for higher input voltage, and also allows for some voltage drop over the power cable. A reverse voltage protection can be as simple as a (reverse connected) diode that shorts out the power, combined with a fuse.
The placement of your caps is bad:
Put them close to the input pin. Route 3V3 to the cap and only then to the input pin. That way, a spike/noise first has to pass the cap. In your example, a spike first sees the input pin and then the cap. Too late!
Also, some vias are placed too close to a track, thus interruping flooding (near upper left corner of U12)
OK, this is a 4 layer board, but still a better routing. Also note, that I use less isolation, so the flooding passes between pins (an SMD SOIC with 1.27 pin spacing).
I bet, your board could be laid out with all components on the top.