KiCad — Usage¶

The orientation guide. Read this before the Tutorial. KiCad is four editors stitched together by a project file; once you internalize the data flow, everything else is mechanical.

The four editors¶

Editor	What it edits	File extension
Project Manager	The project (the launcher)	`.kicad_pro`
Schematic Editor (Eeschema)	Schematics — symbols, wires, nets	`.kicad_sch`
Symbol Editor	Schematic symbols (libraries)	`.kicad_sym`
PCB Editor (Pcbnew)	Boards — footprints, tracks, zones	`.kicad_pcb`
Footprint Editor	PCB footprints (libraries)	`.kicad_mod` (in `.pretty` libs)

The Project Manager is just a launcher. You'll spend ~40% of your time in the Schematic Editor and ~50% in the PCB Editor; the other two are for making custom parts.

The pipeline¶

Schematic Editor          PCB Editor
   │                         │
   │   ── Update PCB ───────►│
   │      (forward annot.)   │
   │                         │
   │◄── Update Schematic ────│
   │      (back annot.)      │
   ▼                         ▼
.kicad_sch                .kicad_pcb

Forward annotation (F8 in the PCB editor): "I changed the schematic, push changes to the board."
Back annotation: "I swapped pin numbers on the board (e.g., to make routing cleaner), push that change back to the schematic." Used much more rarely.

Project anatomy¶

A KiCad project is a folder. Don't move files individually — move the folder.

blink/
├── blink.kicad_pro      # project file (settings, net classes)
├── blink.kicad_sch      # schematic
├── blink.kicad_pcb      # board
├── blink.kicad_prl      # local preferences (gitignore this)
├── sym-lib-table        # project-local symbol libs
├── fp-lib-table         # project-local footprint libs
└── fp-info-cache        # caches (gitignore)

For version control, commit .kicad_pro, .kicad_sch, .kicad_pcb, the lib tables, and any .kicad_sym / .pretty/ directories you've added. Ignore .kicad_prl and fp-info-cache.

Libraries — the most-confusing concept¶

There are two libraries: symbol libs (for the schematic) and footprint libs (for the PCB). Each can be:

Global — installed with KiCad, available in every project. Configured in Preferences → Manage Symbol/Footprint Libraries → Global.
Project — only this project. Configured in the same dialog, Project tab.

Custom symbols you draw yourself usually go in a project library until you decide they're worth promoting to global. Don't pollute your global libs with one-off parts.

A schematic symbol references a footprint by Library:Name (e.g. Resistor_THT:R_Axial_DIN0207_L6.3mm_D2.5mm_P10.16mm_Horizontal). If KiCad can't find that library at the time you open the project, the link breaks. This is the source of 90% of "missing footprint" errors.

Modes / tools¶

Both editors are mode-based like Blender, but lighter. You're either in select mode (default) or you've activated a tool (Wire, Add Symbol, Route Track). Esc always returns to select.

Essential shortcuts¶

Schematic Editor¶

Key	Action
`A`	Add symbol
`P`	Add power port
`W`	Add wire
`K`	End wire
`L`	Add label (local net name)
`H`	Add global label (cross-sheet net)
`M`	Move (no re-route)
`G`	Drag (rubber-band wires)
`R`	Rotate
`F`	Flip
`E`	Edit properties
`Del`	Delete
`Y`	Mirror Y
`Ctrl+S`	Save

PCB Editor¶

Key	Action
`X`	Route track
`V`	Add via (mid-route)
`D`	Drag track (preserves connections)
`M`	Move (breaks connections)
`B`	Refill all zones
`R`	Rotate
`F`	Flip to opposite side
`T`	Track width / layer popup (mid-route)
`+` / `-`	Cycle layers
`Alt+3`	3D Viewer
`F8`	Update PCB from Schematic

The shortcut you'll use most often is X then click, repeating for every connection. The second is B to refresh ground/power pours after you move things.

The Appearance panel (right side, PCB editor)¶

The right panel controls layer visibility and net highlighting. Things to know:

The active layer is the one you draw on. Click the layer name to make it active.
Toggle layer visibility with the eye icon. Routing on F.Cu while looking at B.Cu is a common confusion.
Use net highlighting (click on a track or pad with ~ activated, or use the Net inspector) to verify a net goes where you expect.

ERC and DRC¶

ERC (Electrical Rules Check) — schematic side. Catches dangling wires, unconnected pins, conflicting drivers (two outputs on one net).
DRC (Design Rules Check) — PCB side. Catches clearance violations, unrouted nets, holes too close to edges.

You should run ERC after every meaningful schematic change and DRC before every fabrication output. There's no "save = check"; you have to run them yourself.

Where to go next¶

Tutorial — work through Levels 1 → 5.
Best Practices — once you've finished Level 1, skim this to internalize the conventions.