It’s a very simple project, so there is not much to comment about, but I’ll do my best to comment on anything I can find…
There are some areas in the schematic with text over text. A personal dislike for me. Especially when you want to make paper printouts of the schematic. Example:
Nordic goofed up in many ways with their chip, including (but not limited to) it’s type number. nRF24L01 and nRF24L01+ are different chips and are (If I remember well) incompatible. It’s also got a contorted way of operation. the “6-pipe model” they use is just nuts, and they make you jump through silly hoops just to get this chip going. HopeRF69 seems to be a much better board to use. (but it is slightly more expensive).
You put the power flags in the left top of the schematic and a buffer cap on the right of the schematic. I prefer to have power related stuff close together on the schematic.
You connected only one of the 3 GND pins of the Raspi connector. Normally these are all paralleled
620Ohm is not in E12, and for non critical stuff such as this I prefer to use E12 resistors, which are usually (or used to ) be cheaper then E24 (Which tend to come in lower tolerances etc. I like that you choose a relatively high resistor value for your Led’s and 3V3 power supply. (I do not like bright leds). Voltage drop over LED’s depend on color, you may want to use different resistors for different LED’s.
In your first post you wrote you wanted to keep size and therefore cost of the board down. Yet you have a lot of empty room on the PCB. The PCB could easily be shrunk to about a quarter of the size it is now.
You may consider putting the connector nearer the edge of the board. If you then have a longer connector in your junk bin you can also stick it in the PCB and just leave the extra pins.
I would not even design a PCB for this, but solder it on a piece of vero board. A method I use is to first mark the location of connectors on the vero board, then take short pieces of 0.2mm enameled wire and stick them through the right holes and then put the connectors also through the holes and solder wires, connectors and pads together.
Range of nRF24L01+ is not very good, and combined with the very mediocre layout of the breakout boards it gets worse. Apparently it helps to solder the buffer cap directly on the nRF24L01+ board instead of on your intermediate board.
Just out of habit I would also place a ceramic 100nF cap on the board near the nRF24L01+ connector.
As a general rule, always try to keep your GND plane uninterrupted, and keep interruptions small. Compare your board with this:
I’ve put C1 closer to the nRF24L01 and in such a way that you can fold it flat to the PCB.
I have also set the clearance of the zone to 10mil. That should still be plenty for having the board manufactured, and the zone sneaking in between most pins lowers impedance. For this board it is mostly useless though as it’s all relatively low frequency stuff. The big continuous GND plane may improve the RF performance of the nRF24L01+ a bit. but it’s probably negligible.
I also made a pentagon out of your zone outline. This lets KiCad clip the zone a set distance from the board edge (You can change that by changing the line width of the board outline lines. A weird shape as a pentagon gives an instant warning if anything goes wrongduring creation of Gerber files. Taking the actutal edges of the zone away from the board outline also makes it easier to select the zone for editing with e.
I’ve added a SMT ceramic cap of the same size as your resistors, and rotated the electrolytic cap so you can fold it flat between the 2 connectors. This may help a bit against mechanical damage.
I also noted that you used a very small grid for the PCB. As a habit I always put 0.1" connectors on a 0.1" grid. This prevents *&^%$#@! as with the “arduino” boards, and often helps when making modifications. A grid that is not finer then needed also helps a bit with routing the board when stuff gets denser. I usually use a grid of around 10mil (0.254mm)
I also deleted the “-resque” files. This is not something you can do blindly, but in your particular case they seemed to be unused. Some left over wich was later modified out after a revision I guess.
So here is what I made of it. I also included the directory of the project itself into the .ZIP, so you do not have to create an empty directory first to extract the files into.
msgw-pw_2020-05-18.zip (17.4 KB)
You are of course completely free to do whatever you want with your project. It’s your project.