Skip to main content
kicad-sch-tweak Edit and create KiCad schematic (.kicad_sch) files. Use when user says 'edit schematic', 'modify kicad', 'add component', 'change resistor value', 'update schematic'. Capabilities: (1) Modify schematics (change values, add/remove components, update connections), (2) Create new schematic content from specs or ASCII diagrams, (3) Analyze structure. KiCad 6+ S-expression format. Generated schematics may need GUI layout adjustment.
跳到安装 Skills Marketplace 发现并探索由社区构建的 Agent Skills
用 Codex 或 Claude 帮你安装 复制这段 Prompt，粘贴到 Codex、Claude 或其他助手里，让它检查 Skill 页面并帮你完成安装。
直接命令不会经过审查 Prompt；运行前请先检查来源。
npx skills add https://github.com/Takazudo/claude-resources --skill kicad-sch-tweak命令会保持在同一行。复制前请横向滚动并检查完整内容。
想先保存到本地？可下载 SkillsMP 当前能够提供的文件。
下载 Zip 下载中... name kicad-sch-tweak description Edit and create KiCad schematic (.kicad_sch) files. Use when user says 'edit schematic', 'modify kicad', 'add component', 'change resistor value', 'update schematic'. Capabilities: (1) Modify schematics (change values, add/remove components, update connections), (2) Create new schematic content from specs or ASCII diagrams, (3) Analyze structure. KiCad 6+ S-expression format. Generated schematics may need GUI layout adjustment.
KiCad Schematic Editor
Edit KiCad 6+ schematic files (.kicad_sch) using S-expression text format.
Quick Reference
Recommended Workflow: User + AI Collaboration
Best practice for adding components:
User adds components via KiCad GUI : Use KiCad's graphical interface to add new symbol types. This automatically:
Populates the lib_symbols section with full symbol definitions
Ensures correct UUID formats
Handles footprint assignments
Places components roughly where needed
AI performs text-based tweaks : After user adds components, AI can efficiently:
Add/modify global labels and net labels
Add wires and junctions
Change component values
Adjust coordinates
Add text annotations
Duplicate existing components (copy from file)
Why this workflow?
Adding NEW symbol types programmatically requires copying entire symbol definitions to lib_symbols - tedious and error-prone
KiCad GUI handles library caching automatically
AI excels at repetitive text operations (adding 80 labels for 8 IDC headers)
Reduces risk of file corruption from format mismatches
User: "I need 8 IDC headers and 4 fuses" → adds in KiCad, saves
AI: "Let me add power rail labels to all headers" → edits .kicad_sch
User: Opens KiCad, adjusts layout, verifies connections
Workflow
1. Safety Check & Discover Project
Verify file is version-controlled : Run git status to confirm changes can be revertedRead the target .kicad_sch file to understand current structureFind symbol libraries : Read sym-lib-table for available symbol library namesFind available symbols : Read the project's .kicad_sym file(s) referenced in sym-lib-tableGet sheet UUIDs : Read root .kicad_sch for sheet hierarchy and UUIDs
2. Understand User Request Clarify with user if needed:
Which components to add/modify/remove
Component values (resistance, capacitance, etc.)
Connection requirements (what connects to what)
For new circuits: reference documentation or ASCII diagram
3. Make Edits Use the Edit tool for targeted changes. Always copy patterns from existing components in the same file.
(property "Value" "10k" ;; Change to new value
Add new component: Copy existing symbol block from same file, then update:
uuid (generate new unique UUID)(at X Y rotation) coordinates(property "Reference" "R99" - next available designator(property "Value" "..." - component valuePin UUIDs (generate new unique ones)
Instance path (copy from similar component, update reference)
(wire
(pts (xy X1 Y1) (xy X2 Y2))
(stroke (width 0) (type default))
(uuid "a1b2c3d4-e5f6-7890-abcd-ef1234567890")
)
(label "SIGNAL_NAME"
(at X Y rotation)
(effects (font (size 1.27 1.27)) (justify left bottom))
(uuid "a1b2c3d4-e5f6-7890-abcd-ef1234567890")
)
4. Validate
Ensure all UUIDs are unique (36-char format, lowercase hex: a1b2c3d4-e5f6-7890-abcd-ef1234567890)
Check S-expression syntax (balanced parentheses)
Verify library references exist (lib_id matches library in sym-lib-table)
Suggest user open in KiCad to visually verify - Claude cannot confirm connectivityFor complex edits : Recommend running KiCad ERC (Electrical Rules Check)
Project Discovery For any KiCad project, find these key files:
File Purpose Key Info *.kicad_proProject config Project name, settings sym-lib-tableSymbol libraries Library names and paths fp-lib-tableFootprint libraries Footprint library names Root .kicad_sch Main schematic Sheet UUIDs, hierarchy *.kicad_symSymbol definitions Available component symbols
Get library prefix : Read sym-lib-table to find (name "...") - use as lib_id prefix (e.g., "mylib:ComponentName").
Get sheet UUID : Read root schematic's (uuid "...") field for root UUID. For sub-sheets, find (sheet ... (uuid "...")) blocks.
Symbol Template CRITICAL: Copy from existing component in same file first! This ensures UUID format and other details match.
If creating from scratch, check the file's UUID format first (quoted vs unquoted), then use:
(symbol
(lib_id "LIBRARY:SYMBOL_NAME")
(at X Y ROTATION)
(unit 1)
(exclude_from_sim no)
(in_bom yes)
(on_board yes)
(dnp no)
(uuid UNIQUE-UUID-HERE)
(property "Reference" "R1"
(at X Y 0)
(effects
(font
(size 1.27 1.27)
)
)
)
(property "Value" "10k"
(at X Y 0)
(effects
(font
(size 1.27 1.27)
)
)
)
(property "Footprint" "LIBRARY:FOOTPRINT"
(at X Y 0)
(effects
(font
(size 1.27 1.27)
)
(hide yes)
)
)
(property "Datasheet" ""
(at X Y 0)
(effects
(font
(size 1.27 1.27)
)
(hide yes)
)
)
(property "Description" ""
(at X Y 0)
(effects
(font
(size 1.27 1.27)
)
(hide yes)
)
)
(pin "1"
(uuid PIN1-UUID-HERE)
)
(pin "2"
(uuid PIN2-UUID-HERE)
)
(instances
(project ""
(path "/ROOT-UUID"
(reference "R1")
(unit 1)
)
)
)
)
UUID format : Check existing file - use quoted "uuid" or unquoted uuid to matchPROJECT_NAME_OR_EMPTY: Check existing components - usually ""ROTATION: 0, 90, 180, or 270 degreesPin count varies by component - check symbol definition in .kicad_sym file
Power Symbols Use built-in power: library:
(symbol
(lib_id "power:GND")
(at X Y 0)
(unit 1)
(exclude_from_sim no)
(in_bom yes)
(on_board yes)
(dnp no)
(fields_autoplaced yes)
(uuid "UNIQUE-UUID")
(property "Reference" "#PWR01" (at X Y 0) (effects (font (size 1.27 1.27)) (hide yes)))
(property "Value" "GND" (at X Y 0) (effects (font (size 1.27 1.27))))
(pin "1" (uuid "PIN-UUID"))
(instances
(project "..."
(path "/..." (reference "#PWR01") (unit 1))
)
)
)
Common power symbols: power:GND, power:+5V, power:+12V, power:-12V, power:VCC, power:VDD
Coordinate System
Origin: top-left of page
Units: millimeters
Rotation: degrees (0, 90, 180, 270)
Grid: 2.54mm (0.1 inch) typical spacing
Tip : Look at nearby components for reasonable coordinates
Reference Designators Prefix Component R Resistors C Capacitors L Inductors D Diodes U ICs/Modules J Connectors TP Test points F Fuses #PWR Power symbols (hidden)
Limitations
Layout quality : Components placed programmatically may overlap. User adjusts in KiCad GUI.Wire routing : Prefer net labels over complex wire routing for drafts.Pin positions : Estimated from symbol definitions; may need adjustment.
CRITICAL: lib_symbols Section (KiCad 9.0+) When adding a NEW symbol type to a schematic, you MUST also add its definition to the lib_symbols section.
KiCad caches symbol definitions inside the schematic file. If you add a symbol instance without adding its definition to lib_symbols, the file will crash on open.
How to add a new symbol:
Copy symbol definition from the .kicad_sym library fileAdd to lib_symbols with library prefix (e.g., "zudo-bus:CL10B104KB8NNNC")Add symbol instance referencing the same lib_id Example lib_symbols entry:
(lib_symbols
(symbol "library-name:SymbolName"
(exclude_from_sim no)
(in_bom yes)
(on_board yes)
(property "Reference" "C"
...
)
;; Copy entire symbol definition from .kicad_sym file
;; Including all properties, graphics, and pins
(embedded_fonts no)
)
)
Symbol name in lib_symbols must include library prefix: "library:Symbol" not just "Symbol"
Copy the ENTIRE symbol definition including all (symbol "Name_0_1" ...) graphics blocks
Add (embedded_fonts no) at the end of each symbol in lib_symbols
If adding multiple symbols, each needs its own definition in lib_symbols
CRITICAL: Format Matching ALWAYS match the existing file's format exactly. Different KiCad projects may use slightly different S-expression styles. Key variations:
UUID Format (CRITICAL - causes crashes if wrong!) Check how UUIDs appear in the existing file:
;; Some projects use UNQUOTED UUIDs:
(uuid 26efc87e-0264-438c-bf9f-152a5d6f0f11)
;; Some projects use QUOTED UUIDs:
(uuid "26efc87e-0264-438c-bf9f-152a5d6f0f11")
You MUST use the same format as existing UUIDs in the file! Mixing formats causes KiCad to crash on open.
Pin Format Pins should have uuid on its own line:
(pin "1"
(uuid 00000001-0001-0001-0001-000000000002)
)
Instances Format The path should have reference and unit on separate lines:
(instances
(project ""
(path "/26efc87e-0264-438c-bf9f-152a5d6f0f11"
(reference "C1")
(unit 1)
)
)
)
Text Elements Text elements should NOT have (exclude_from_sim no):
;; CORRECT:
(text "POWER INPUT"
(at 25.4 25.4 0)
(effects (font (size 3.81 3.81) (bold yes)))
(uuid a0000001-0001-0001-0001-000000000001)
)
;; WRONG - causes crashes:
(text "POWER INPUT"
(exclude_from_sim no) ;; <-- DO NOT ADD THIS TO TEXT
(at 25.4 25.4 0)
...
)
Labels Format Net labels follow this format:
(label "SIGNAL_NAME"
(at X Y rotation)
(effects
(font
(size 1.27 1.27)
)
(justify left bottom)
)
(uuid c0000001-0001-0001-0001-000000000001)
)
sym-lib-table Required If the project doesn't have a sym-lib-table file, create one:
(sym_lib_table
(version 7)
(lib (name "library-name")(type "KiCad")(uri "${KIPRJMOD}/symbols/library-name.kicad_sym")(options "")(descr ""))
)
All libraries referenced by lib_id in the schematic MUST be listed in sym-lib-table.
Error Recovery If schematic won't open in KiCad:
Check UUID format - must match existing file (quoted vs unquoted)
Check text elements don't have (exclude_from_sim no)
Verify sym-lib-table exists and references all used libraries
Parenthesis mismatch : Check line-by-line for missing ). Common: deleted symbol block with dangling reference.
Invalid UUID : Must be exactly 36 chars, lowercase hex (0-9, a-f). Quick fix: copy existing UUID and change last 4 digits.
Missing lib_id : Symbol not in library. Check:
sym-lib-table file existsLibrary is listed in sym-lib-table
Symbol name exists in the .kicad_sym file
git checkout -- path/to/file.kicad_sch
Required properties : Reference, Value, Footprint (Datasheet and Description recommended).
