Getting started¶
Everything here needs KiCad 10 and is tested with 10.0.6. Earlier 10.0 patches cannot create a project from a template folder.
There are two ways in: start a new module from a template, or add the library to a project you already have.
Start a module from a template¶
A template is a whole project: the board outline, the bus as connector J1, the mounting holes and the board rules, with its own copy of the library. Choose the pattern first; Templates compares the two. If unsure, use Slot 0.
- Get the templates: download
cubesat-pc104-templates-<version>.zipfrom the releases page and unzip it, or clone the repository and use itstemplates/folder. - In KiCad choose File → New Project from Template, open the user
templates tab and point it at the folder holding the templates. To list
them every time, set
KICAD_USER_TEMPLATE_DIRto that folder under Preferences → Configure Paths. - Pick
CubeSat_PC104_Slot0orCubeSat_PC104_Slot1and name the project. KiCad copies the files and renames them after the project. - In the schematic, wire the bus pins the module uses and put a no-connect flag on the rest. Bus pinout lists what each pin carries.
ERC lists every bus pin as unconnected until step 4 is done; that is the template's only ERC finding. The board passes DRC as it is.
Add the library to an existing project¶
The library is one symbol file, CubeSat_PC104.kicad_sym, and one footprint
folder, CubeSat_PC104.pretty. Get them from CubeSat_PC104-<version>.zip on the
releases page,
or from library/ in a clone.
The templates load the library with the nickname CubeSat_PC104. Use the same
nickname, so the symbols' footprint links (CubeSat_PC104:CSK_PC104_Slot0)
resolve.
The project keeps its own copy, so it opens anywhere without setup.
- Copy
CubeSat_PC104.kicad_symandCubeSat_PC104.pretty/into the project folder. - Preferences → Manage Symbol Libraries, tab Project Specific
Libraries: add
CubeSat_PC104.kicad_symwith nicknameCubeSat_PC104. KiCad writes the path as${KIPRJMOD}/CubeSat_PC104.kicad_sym, relative to the project. - Preferences → Manage Footprint Libraries, same tab: add the
CubeSat_PC104.prettyfolder with nicknameCubeSat_PC104.
One copy on your machine, shared by every project.
- Unzip the library somewhere it will stay.
- Under Preferences → Configure Paths, add a variable such as
CUBESAT_PC104pointing at that folder. - In Manage Symbol Libraries and Manage Footprint Libraries, tab
Global Libraries, add
${CUBESAT_PC104}/CubeSat_PC104.kicad_symand${CUBESAT_PC104}/CubeSat_PC104.pretty, each with nicknameCubeSat_PC104.
A project made this way opens only on a machine with the same setup.
Then place CSK_Bus from CubeSat_PC104 in the schematic. Its footprint is
CSK_PC104_Slot0; change the footprint field to CSK_PC104_Slot1 for a
Slot 1 board, or to CSK_PC104_Bus for a bus connector without the board
outline. Library describes each part.
Board outline
CSK_PC104_Slot0 and CSK_PC104_Slot1 draw the board outline on
Edge.Cuts as part of the footprint, with H1 pin 1 at the origin. Delete
any outline the board already has, or use CSK_PC104_Bus and keep yours.
The specification also asks for copper to stay 1.27 mm from the edge; set
Board Setup → Constraints → Copper to edge clearance to 1.27 mm, as
the templates do.