I’m a newbie Kicad user. I’m looking for libraries and footprints for Adafruit Power Booster 1000C. If someone already has the library, please share with me?
I just used the ‘eaglecad’ import on the project. Kinda/sorta works. At least it is a starting point. Really depends on what you need to do with it I guess.
Yes, I try that too but It looks very faulty and how could we add the entire PCB as a one device library?
You probably don’t want the full board (traces, component silkscreens, non-connector components, etc) as a footprint. I’ve used the Eagle import in the past to get the board outline (which can’t be part of footprints with the footprint editor yet) and the important pin locations. I honestly forget if I just used the Eagle import to check my footprint against, or if I deleted all unnecessary elements and then converted what was left into a footprint. If the latter, I probably had to do some hand editing of the files in a text editor. This was back in the pre-v5 nightlies, and I don’t remember the details.
It might also not be a bad thing to directly ask AdaFruit if they have KiCad libraries and footprints for their breakout boards and modules, specifically stating you plan on using the Power Booster 1000C. They probably don’t, and probably don’t currently plan on providing these libraries. But if all of us who plan on using their parts ask (politely ask, that is) then hopefully eventually they will see a community demand.
It depends on what you do.
If you want to modify the board, then getting the project from github and importing it in KiCad is a pretty good start, compared to starting from scratch.
Importing the schematic works to a very usable degree. All the components, pins and connections look OK at first sight. ERC checker in Eeschema finds 4 unconnected pins, which is logical because Eagle simply ignores unconnected pins (Yuck).
ERC also finds errors because of missing power flags / inputs, which is also expected because (as far as I know) this functionality is not implemented in eagle.
After import in Pcbnew, If I disable the errors about the missing courtyards with:
Pcbnew / File / Board Setup / Design Rules / [ ] Require courtyard definitions in footprints
Then re-calculate the zone boundaries with ‘b’ and a DRC check only finds 4 errors which seems easily fixable, and 7 unconnected items, which may be due to some clearance differences and zones rendered differently in KiCad.
For example: GND pins 5 and 7 of the connector are connected with a thin sliver on the ADAfruit PCB, which gets lost when KiCad re-generates the GND plane:
I have not looked into further details.
The board does not look “very faulty” to me. It’s just a normal PCB.
The components on the board are pretty dense and this looks like a mess on first sight but it really is quite normal.
If you want to make another board which fits onto this board, with the same outline and connector layout, then the most logical way would be to simply remove most of the components and tracks from the board ( Only leave the connectors and mounting holes you want to keep on the board) and then save it as a separate “template” project.
Then you can start a new project and start a schematic.
In your schematic you must also use the the same RefDes designators and Footprint values of the connectors as used in the Eagle PCB.
After that you can close your own project, and open Pcbnew in “stand alone mode”. which enables the a bunch of menu items such as :
Pcbnew / File / Append Board
With this and a bit of fiddling you can combine the 2 projects into 1 and re-use the board outline, holes and connector layout.
I’ve skipped over a lot of details and this is not a good project for “beginners”, because you get confronted with too many small details while also learning KiCad.
I’m Impressed, you guys have a great community here. Actually, I need to power my rpizerow phat board with some more modules and components. But first of all, I need to watch more Kicad youtube videos and I think I need to hang out here more to go advance. Thank you for the clarifications.
Please be aware that V5 is pretty new and probably most of the videos you find will be V4. Lots of carryover but don’t expect one to one correspondence.
Edit: Or the newer features mentioned.
Not directly. But there are ways to do it.
Place the outline on some layer of your choice. (Use one that is not used for anything else)
Save the footprint, close kicad and use a text editor to replace that layer with “Edge.Cuts” (make a bacup first should you screw this up)
Then open the footprint again. You can now even edit the outline later on and i think even duplicate segments of it.