(keyword value)
(keyword (nested value))
(keyword
  (child1 value)
  (child2 value)
)

Common Patterns

Coordinates: (at x y angle) or (xy x y)
UUIDs: (uuid "xxxxxxxx-xxxx-xxxx-xxxx-xxxxxxxxxxxx")
Strings: "quoted string" or unquoted_identifier
Numbers: 1.234 (always decimal, no units in file)
Booleans: yes / no

2. Schematic Format (.kicad_sch)

File Structure

(kicad_sch
  (version 20231120)
  (generator "eeschema")
  (generator_version "8.0")
  (uuid "project-uuid")
  (paper "A4")
  
  ; Title block
  (title_block
    (title "Project Title")
    (date "2024-01-01")
    (rev "1.0")
    (company "Company Name")
  )
  
  ; Library symbols (embedded copies)
  (lib_symbols
    (symbol "Device:R" ...)
  )
  
  ; Placed symbols (component instances)
  (symbol ...)
  (symbol ...)
  
  ; Wires and connections
  (wire ...)
  (bus ...)
  (junction ...)
  
  ; Labels and nets
  (label ...)
  (global_label ...)
  (hierarchical_label ...)
  
  ; Hierarchical sheets
  (sheet ...)
  
  ; Text and graphics
  (text ...)
  (polyline ...)
  (rectangle ...)
)

Symbol Instance

(symbol
  (lib_id "Device:R")
  (at 100 50 0)              ; x, y, rotation (0, 90, 180, 270)
  (unit 1)                   ; Multi-unit symbols
  (exclude_from_sim no)
  (in_bom yes)
  (on_board yes)
  (dnp no)                   ; Do Not Populate
  (uuid "symbol-uuid")
  (property "Reference" "R1"
    (at 100 45 0)
    (effects (font (size 1.27 1.27)))
  )
  (property "Value" "10k"
    (at 100 55 0)
    (effects (font (size 1.27 1.27)))
  )
  (property "Footprint" "Resistor_SMD:R_0402_1005Metric"
    (at 100 50 0)
    (effects (font (size 1.27 1.27)) hide)
  )
  (property "LCSC" "C25744"
    (at 100 50 0)
    (effects (font (size 1.27 1.27)) hide)
  )
  (pin "1" (uuid "pin1-uuid"))
  (pin "2" (uuid "pin2-uuid"))
  (instances
    (project "project_name"
      (path "/root-uuid" (reference "R1") (unit 1))
    )
  )
)

Wire

(wire
  (pts
    (xy 100 50)
    (xy 120 50)
  )
  (stroke (width 0) (type default))
  (uuid "wire-uuid")
)

Label (Local Net Name)

(label "VCC"
  (at 100 50 0)
  (effects (font (size 1.27 1.27)))
  (uuid "label-uuid")
)

Global Label (Cross-Sheet Net)

(global_label "USB_D+"
  (shape input)              ; input, output, bidirectional, tri_state, passive
  (at 150 60 0)
  (effects (font (size 1.27 1.27)))
  (uuid "global-uuid")
  (property "Intersheetrefs" "${INTERSHEET_REFS}"
    (at 150 60 0)
    (effects (font (size 1.27 1.27)) hide)
  )
)

Power Symbol

(symbol
  (lib_id "power:GND")
  (at 100 80 0)
  (unit 1)
  (exclude_from_sim yes)
  (in_bom no)
  (on_board yes)
  (uuid "power-uuid")
  (property "Reference" "#PWR01" ...)
  (property "Value" "GND" ...)
  (pin "1" (uuid "..."))
)

Hierarchical Sheet

(sheet
  (at 50 50)
  (size 30 20)
  (fields_autoplaced yes)
  (stroke (width 0.1524) (type solid))
  (fill (color 255 255 255 0))
  (uuid "sheet-uuid")
  (property "Sheetname" "Power Supply"
    (at 50 49 0)
    (effects (font (size 1.27 1.27)))
  )
  (property "Sheetfile" "power_supply.kicad_sch"
    (at 50 72 0)
    (effects (font (size 1.27 1.27)) hide)
  )
  (pin "VIN" input
    (at 50 55 180)
    (effects (font (size 1.27 1.27)))
    (uuid "sheet-pin-uuid")
  )
)

3. PCB Format (.kicad_pcb)

File Structure

(kicad_pcb
  (version 20231014)
  (generator "pcbnew")
  (generator_version "8.0")
  (general
    (thickness 1.6)
    (legacy_teardrops no)
  )
  
  ; Page settings
  (paper "A4")
  (title_block ...)
  
  ; Layer definitions
  (layers
    (0 "F.Cu" signal)
    (31 "B.Cu" signal)
    (32 "B.Adhes" user "B.Adhesive")
    (33 "F.Adhes" user "F.Adhesive")
    (34 "B.Paste" user)
    (35 "F.Paste" user)
    (36 "B.SilkS" user "B.Silkscreen")
    (37 "F.SilkS" user "F.Silkscreen")
    (38 "B.Mask" user)
    (39 "F.Mask" user)
    (40 "Dwgs.User" user "User.Drawings")
    (41 "Cmts.User" user "User.Comments")
    (42 "Eco1.User" user "User.Eco1")
    (43 "Eco2.User" user "User.Eco2")
    (44 "Edge.Cuts" user)
    (45 "Margin" user)
    (46 "B.CrtYd" user "B.Courtyard")
    (47 "F.CrtYd" user "F.Courtyard")
    (48 "B.Fab" user)
    (49 "F.Fab" user)
  )
  
  ; Design rules setup
  (setup ...)
  
  ; Net definitions
  (net 0 "")
  (net 1 "GND")
  (net 2 "VCC")
  
  ; Footprints (component instances)
  (footprint ...)
  
  ; Traces
  (segment ...)
  
  ; Vias
  (via ...)
  
  ; Zones (copper pours)
  (zone ...)
  
  ; Graphics
  (gr_line ...)
  (gr_rect ...)
  (gr_circle ...)
  (gr_text ...)
)

Footprint

(footprint "Package_SO:SOIC-8_3.9x4.9mm_P1.27mm"
  (layer "F.Cu")
  (uuid "footprint-uuid")
  (at 100 50 0)              ; x, y, rotation
  (descr "SOIC-8 package")
  (property "Reference" "U1"
    (at 0 -3.5 0)
    (layer "F.SilkS")
    (uuid "ref-uuid")
    (effects (font (size 1 1) (thickness 0.15)))
  )
  (property "Value" "ESP32-S3"
    (at 0 3.5 0)
    (layer "F.Fab")
    (uuid "val-uuid")
    (effects (font (size 1 1) (thickness 0.15)))
  )
  (property "Footprint" "Package_SO:SOIC-8..."
    (at 0 0 0)
    (layer "F.Fab")
    (hide yes)
    (uuid "fp-uuid")
  )
  
  ; Pads
  (pad "1" smd rect
    (at -1.905 -2.475)
    (size 0.6 1.5)
    (layers "F.Cu" "F.Paste" "F.Mask")
    (net 1 "GND")
    (uuid "pad-uuid")
  )
  (pad "2" thru_hole circle
    (at 0 0)
    (size 1.7 1.7)
    (drill 1.0)
    (layers "*.Cu" "*.Mask")
    (net 2 "VCC")
    (uuid "pad-uuid")
  )
  
  ; Silkscreen graphics
  (fp_line
    (start -2.5 -2.5)
    (end 2.5 -2.5)
    (stroke (width 0.12) (type solid))
    (layer "F.SilkS")
    (uuid "line-uuid")
  )
)

Trace (Segment)

(segment
  (start 100 50)
  (end 120 50)
  (width 0.25)
  (layer "F.Cu")
  (net 1)
  (uuid "segment-uuid")
)

Arc Trace

(arc
  (start 100 50)
  (mid 105 45)
  (end 110 50)
  (width 0.25)
  (layer "F.Cu")
  (net 1)
  (uuid "arc-uuid")
)

Via

(via
  (at 110 60)
  (size 0.8)
  (drill 0.4)
  (layers "F.Cu" "B.Cu")
  (net 1)
  (uuid "via-uuid")
)

Zone (Copper Pour)

(zone
  (net 1)
  (net_name "GND")
  (layer "F.Cu")
  (uuid "zone-uuid")
  (hatch edge 0.5)
  (connect_pads
    (clearance 0.25)
  )
  (min_thickness 0.25)
  (filled_areas_thickness no)
  (fill yes
    (thermal_gap 0.5)
    (thermal_bridge_width 0.5)
  )
  (polygon
    (pts
      (xy 0 0)
      (xy 100 0)
      (xy 100 100)
      (xy 0 100)
    )
  )
  (filled_polygon
    (layer "F.Cu")
    (pts ...)
  )
)

Board Outline

(gr_rect
  (start 0 0)
  (end 100 100)
  (stroke (width 0.1) (type default))
  (fill none)
  (layer "Edge.Cuts")
  (uuid "outline-uuid")
)

4. Common Operations

Adding a Component to Schematic

Add symbol to (lib_symbols ...) if not already present
Add (symbol ...) block with:
- Unique UUID
- Position (at x y rotation)
- Reference property
- Value property
- Footprint property
- Pin mappings

Adding a Trace to PCB

Find the net number for the connection
Add (segment ...) block with:
- Start and end coordinates
- Width
- Layer
- Net number
- Unique UUID

Creating a Net

In PCB file, add: (net N "NetName")
Reference the net number in pads and segments

5. Units and Coordinates

Context	Unit
Schematic	mils (1/1000 inch), stored as mm in file
PCB	millimeters
Angles	degrees (0, 90, 180, 270 typical)

Coordinates are absolute from origin (0,0).

6. UUID Generation

All elements require unique UUIDs. Format: xxxxxxxx-xxxx-xxxx-xxxx-xxxxxxxxxxxx

Generate with: uuidgen command or programming language UUID library.

7. Parsing Tips

Reading S-Expressions

# Simple recursive descent parser concept
def parse_sexpr(text):
    tokens = tokenize(text)
    return parse_list(tokens)

def parse_list(tokens):
    result = []
    while tokens and tokens[0] != ')':
        if tokens[0] == '(':
            tokens.pop(0)
            result.append(parse_list(tokens))
        else:
            result.append(tokens.pop(0))
    if tokens:
        tokens.pop(0)  # Remove closing ')'
    return result

Writing S-Expressions

Maintain consistent indentation (2 spaces)
Preserve existing UUIDs when editing
Keep order of elements as expected by KiCad
Use proper quoting for strings with spaces

8. File Validation

After editing:

Open in KiCad to verify parsing
Run ERC/DRC via kicad-cli
Check for warnings about unknown tokens

Important: Always backup files before programmatic editing. KiCad may add/remove fields on save.

kicad-file-format

KiCad File Format Reference

1. S-Expression Basics

Syntax

More from o2scale/electronics-agent-kit

platformio

kicad-cli