Schematic needs rescuing, J1 isn’t found in my library setup. You might want to copy it to a project specific library and add it to the project.
See Option 2 in this FAQ article for more information about the rescue feature:
I had to pick something 
Since this is all very low current I didn’t see any direct benefit from larger traces, but your point about manufacturability is a good one. Thanks.
That symbol is already in a project library and is included in the ZIP file (I used the KiCAD archive tool and double-checked that it included the symbol files).
I agree.
And more, if BUS1 is conected to J1-pin4 and BUS3 is connected to J1-pin8, the board can be routed with:
-Bottom side only a GND zone covering all the board
-Top side +5V zone covering all the board and all the other signals with a 15mil track width.
1 Like
OK, I see now. But it’s not in the project specific sym-lib-table. KiCad doesn’t find it automatically.
/.$/in 5.0.2./
Should work find in 5.1rc2
What should work? I’m using 5.1.0-rc2-38-g4612175da. In the project the .lib file is in the project directory but KiCad doesn’t find it because there’s no sym-lib-table in the project. I had to add the .lib file to Project Specific Libraries in the Symbol Library manager.
Archiving a project should include sym-lib-table in 5.1
Ah! So the original poster used older version to archive and it wasn’t included. @kpfleming, either add sym-lib-table manually or archive with a nightly build or soon-to-be 5.1.
Thanks, I am indeed using 5.0.2.
Thanks for all the guidance; here’s a new version of the board using filled zones. I had to relocate some of the components to make routing easier, and I had to use a via jumper to connect the 5V zone, but I think I like this version better.
One-Wire Bus Board with Planes.zip (150.2 KB)
Yep, I’m just about to upload a new version which is even cleaner
1 Like
One-Wire Bus Board.kicad_pcb (347.3 KB)
I think this one is really done, I even took the time to clean up the fab and silkscreen layers.
Good!
There is only one thing I don’t like, maybe it is a fixation or historical background: electrons don’t like 90 degree angles unless on a T junction of traces, if possible make 45 degree angles. Some people use teradrops on T junctions, only available in kicad as an external plugin.
I’ll consider it, but my OCD prefers right angles!
I see you have +5V copper fill on top. Be careful about screw heads digging into the copper fill and shorting +5V to casing or maybe bottom layer.
You can use the leftover inverters in parallell to the used ones for more drive capability.
Good point; I’m fairy certain that the mounting holes are large enough for ‘normal’ screw heads but when I give boards to other people I’ll suggest fiber washers under the screw heads to protect the board.
I’ve chosen super-low-current (1ma) LEDs because the total power budget on this board is very low, so the additional drive current capacity wouldn’t be beneficial.
To me it looks like the copper is right on the edge of the hole. I recommend using Schematic symbol Mechanical -> MountingHole_Pad, connect it to ground and then use mounting hole symbol with exposed copper “shielding” for the correct screw size, for instance Mounting_Holes -> MountingHole_5.3mm_M5_Pad_Via for M5 screws. You can see the isolation from +5V on top and the quite large pad to counter for the M5 screw head. On bottom there is thermal relief connections to GND. I also rounded the corner.
Raytracing rendering was not nice to me on bottom side of the board?
1 Like
Will definitely do that on the next revision!