Skip to content

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.

  1. Get the templates: download cubesat-pc104-templates-<version>.zip from the releases page and unzip it, or clone the repository and use its templates/ folder.
  2. 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_DIR to that folder under Preferences → Configure Paths.
  3. Pick CubeSat_PC104_Slot0 or CubeSat_PC104_Slot1 and name the project. KiCad copies the files and renames them after the project.
  4. 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.

  1. Copy CubeSat_PC104.kicad_sym and CubeSat_PC104.pretty/ into the project folder.
  2. Preferences → Manage Symbol Libraries, tab Project Specific Libraries: add CubeSat_PC104.kicad_sym with nickname CubeSat_PC104. KiCad writes the path as ${KIPRJMOD}/CubeSat_PC104.kicad_sym, relative to the project.
  3. Preferences → Manage Footprint Libraries, same tab: add the CubeSat_PC104.pretty folder with nickname CubeSat_PC104.

One copy on your machine, shared by every project.

  1. Unzip the library somewhere it will stay.
  2. Under Preferences → Configure Paths, add a variable such as CUBESAT_PC104 pointing at that folder.
  3. In Manage Symbol Libraries and Manage Footprint Libraries, tab Global Libraries, add ${CUBESAT_PC104}/CubeSat_PC104.kicad_sym and ${CUBESAT_PC104}/CubeSat_PC104.pretty, each with nickname CubeSat_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.