I can’t modify footprint in PCB editor
doubleclick the footprint and click on “edit footprint” / “edit footprint in library”. This is the normal way of modifying the footprint.
I can’t place things exactly the way I want in a smooth way
not really clear what you mean / what you want to achieve.
silkscreen clipped by solder mask:
all silkscreen-drawings (and texts) should not exist on places where soldermask is removed. This includes all Pads were you later want to solder some parts. So if you want round circles around your holes these circles must have a bigger diameter than the solder-mask-circle on the same Pad. These change should be made in the footprint-library.
I personally would not do that, the rectangle around the multi-pin-connector is sufficient. The silkscreen-circles vanish anyway after soldering the pins onto the pcb.
fixation holes:
I would place them inside of the footprint → if placed correctly once (in the footprintlibrary) they are correct in every following design.
To connect these fixation-holes to GND you have to give these holes also a pad number. Than you have to add additional GND-Pins in the symbol so that you can connect the additional holes/pads to GND-Pins in the symbol.
As a first step try with simple holes (which you have already placed in the footprint). The get the extra reinforcement-vias around the big hole (like the shoen GND-Hole in your video) look into the footprint-definition of these hole-footprint and look how that was created.
1.) good done with the GND-fixation holes. looks nice.
2.) Judging the design/layout in a video is very very difficult. If you would receive good advice you have to upload your kicad-project so one can look directly onto the board. (And it needs someone who takes the time to look onto the board). In the main kicad-manager there is an option to zip-archive the whole project.
3.) regarding the routing: There is always room for improvement and it also depends on ersonal preferences. But I think don’t worry to much, it will work. For instance to make the 3,3V-track wider was a good move.
4.) regarding the GND-plane:
make the GND-zone for TOP+BOTTOM and place vias between top+bottom on every border (where a track crosses the gnd-plane). The goal is to “play like you are a gnd-current” and try to run from one point (edge) of the board to any other point (opposite edge) of the board. The way for this “GND-current” should be very straight (with as little deviation from straight line as possible). Tracks on bottom could be crossed with a via to top, than travel the next way on the top-gnd-zone, before the next top-trace should be a via to go back to bottom gnd-zone and continue there.
(take this description only as assistance, not as mandatory instructions)
3.) regarding the routing: There is always room for improvement and it also depends on ersonal preferences. But I think don’t worry to much, it will work. For instance to make the 3,3V-track wider was a good move.
The question is also should I make 3.3V as a bigger “BUS” with lines straight in to the pin?
Explanation 4 I have hard time understanding, I have seen on som PCBs that ther are hundereds of smal vias between top and botto. But on for example arduino ther is much les vias, but larger. You don’t happen to know a god youtube video I can see abot this to better understand?
Also I wonder how to select center of PAD from footprint?
No ide if it is possible to open it? I dont know if I have saved the footprint and symbol the right way.
uploaded project works, was the right way to archive and upload. I place all output-files (gerbers) into a subdirectory, this gives a better overview in the filemanager.
+3,3V: never mind, both variants will work. I would take the “bus bar”-version (picture above in your last answer) with constant 0,75mm width. The short thickened track in your last picture doesn’t help much in reducing resistance.
remarks to the dimensioning on board: your dimension-lines are drawed on the Bottom-copper-layer. They end up as part of the gerber-output-files. Is this really what you want?
oky, forget my explanation. But for a good video you have to look for yourself (or someone other chimes in).
select center of pad for measuring tool: the snapping of tools is currently not 100% consistent througout the program. It seems the measuring tool (have not used it before - so also few experience with it) has no snapping facility at all for start-point of the measurement.
In the video it seems you want to measure the pad-diameter. better option for this: select pad, “E” for edit pad-parameters (don’t change anything), read value in cell “hole”
