Skip to content

hashgraph-online/awesome-codex-plugins / plugins/aklofas/kicad-happy/skills/kicad

Analyze KiCad projects and PDF schematics: schematics, PCB layouts, Gerbers, footprints, symbols, netlists, and design rules. Reviews designs for bugs, traces nets, cross-references schematic to PCB, extracts BOM data, checks DRC/ERC, DFM, power trees, and regulator circuits. Every finding carries a confidence label and evidence source with trust_summary rollup. Analyzes PDF schematics from dev boards, reference designs, eval kits, and datasheets. Supports KiCad 5–10. Use whenever the user mentions .kicad_sch, .kicad_pcb, .kicad_pro, PCB design review, schematic analysis, PDF schematics, reference designs, Gerber files, DRC/ERC, netlist issues, BOM extraction, signal tracing, power budget, DFM, or wants to understand, debug, compare, or review any hardware design. Also for "check my board", "review before fab", "what's wrong with my schematic", "is this ready to order", "check my power supply", "verify this circuit", OSHWA certification readiness, or any electronics/PCB design question.

FileKindSize
SKILL.mdskill md79.1 KB
references/config-reference.mdmarkdown19.1 KB
references/datasheet-verification.mdmarkdown16.5 KB
references/deep-review.mdmarkdown9.7 KB
references/design-intent.mdmarkdown5.6 KB
references/diff-analysis.mdmarkdown17.6 KB
references/file-formats.mdmarkdown15.1 KB
references/gerber-parsing.mdmarkdown33.5 KB
references/manual-gerber-parsing.mdmarkdown24.5 KB
references/manual-pcb-parsing.mdmarkdown17.2 KB
references/manual-schematic-parsing.mdmarkdown12.8 KB
references/net-tracing.mdmarkdown12.0 KB
references/oshwa-certification.mdmarkdown4.5 KB
references/output-schema.mdmarkdown33.4 KB
references/pcb-layout-analysis.mdmarkdown27.3 KB
references/pdf-schematic-extraction.mdmarkdown15.2 KB
references/report-generation.mdmarkdown56.3 KB
references/schematic-analysis.mdmarkdown63.9 KB
references/standards-compliance.mdmarkdown33.5 KB
references/supplementary-data-sources.mdmarkdown12.5 KB
references/what-if.mdmarkdown19.5 KB
review/README.mdmarkdown4.1 KB
review/fixtures/deep_review.example.jsonconfig1.2 KB
review/fixtures/design_context.example.jsonconfig388 B
review/fixtures/review_annotations.example.jsonconfig707 B
review/prompts/design_context.mdmarkdown4.9 KB
review/schemas/deep_review.schema.jsonconfig3.3 KB
review/schemas/design_context.schema.jsonconfig2.2 KB
review/schemas/review_annotations.schema.jsonconfig1.9 KB
review/scripts/_mini_jsonschema.pyscript6.6 KB
review/scripts/build_review_plan.pyscript2.3 KB
review/scripts/deep_review_gate.pyscript27.3 KB
review/scripts/merge_annotations.pyscript7.0 KB
review/scripts/validate_review.pyscript2.6 KB
scripts/.gitignoreother13 B
scripts/README.mdmarkdown23.4 KB
scripts/analysis_cache.pyscript42.1 KB
scripts/analyze_gerbers.pyscript90.9 KB
scripts/analyze_pcb.pyscript7.4 KB
scripts/analyze_schematic.pyscript6.7 KB
scripts/analyze_thermal.pyscript48.5 KB
scripts/analyzer_envelope.pyscript15.5 KB
scripts/capability_mode.pyscript10.2 KB
scripts/check_report_sections.pyscript10.6 KB
scripts/cross_analysis.pyscript69.4 KB
scripts/cross_verify.pyscript23.1 KB
scripts/design_intent.pyscript13.5 KB
scripts/detection_schema.pyscript26.0 KB
scripts/detector_helpers.pyscript15.2 KB
scripts/diff_analysis.pyscript23.5 KB
scripts/diff_engine.pyscript47.2 KB
scripts/domain_detectors.pyscript260.5 KB
scripts/envelopes/__init__.pyscript0 B
scripts/envelopes/cross_analysis.pyscript5.9 KB
scripts/envelopes/gerber.pyscript16.1 KB
scripts/envelopes/pcb.pyscript25.9 KB
scripts/envelopes/schematic.pyscript23.1 KB
scripts/envelopes/thermal.pyscript7.4 KB
scripts/export_issues.pyscript27.6 KB
scripts/fab_release_gate.pyscript29.8 KB
scripts/finding_schema.pyscript25.7 KB
scripts/gen_output_schema_md.pyscript9.2 KB
scripts/inputs_builder.pyscript4.0 KB
scripts/kicad_core/__init__.pyscript0 B
scripts/kicad_core/classify.pyscript32.5 KB
scripts/kicad_core/cli.pyscript4.2 KB
scripts/kicad_core/coords.pyscript2.0 KB
scripts/kicad_core/diagnostics.pyscript1.9 KB
scripts/kicad_core/executables.pyscript1.0 KB
scripts/kicad_core/fields.pyscript5.9 KB
scripts/kicad_core/fileio.pyscript5.4 KB
scripts/kicad_core/hotloop.pyscript3.1 KB
scripts/kicad_core/instances.pyscript5.7 KB
scripts/kicad_core/model.pyscript4.8 KB
scripts/kicad_core/netnames.pyscript19.1 KB
scripts/kicad_core/netquery.pyscript6.7 KB
scripts/kicad_core/pairing.pyscript1.9 KB
scripts/kicad_core/parts.pyscript28.9 KB
scripts/kicad_core/passives.pyscript10.0 KB
scripts/kicad_core/pdn.pyscript1011 B
scripts/kicad_core/project.pyscript43.2 KB
scripts/kicad_core/render.pyscript2.7 KB
scripts/kicad_core/sexp.pyscript12.6 KB
scripts/kicad_core/textvars.pyscript5.4 KB
scripts/kicad_core/token_cache.pyscript2.2 KB
scripts/kicad_core/values.pyscript14.1 KB
scripts/kicad_types.pyscript15.1 KB
scripts/lifecycle_audit.pyscript6.7 KB
scripts/lifecycle_engine.pyscript52.8 KB
scripts/lookup_detectors.pyscript29.9 KB
scripts/lookup_helpers.pyscript3.0 KB
scripts/methodology_gerbers.mdmarkdown23.1 KB
scripts/methodology_pcb.mdmarkdown22.2 KB
scripts/methodology_schematic.mdmarkdown43.1 KB
scripts/netlist_queries.pyscript4.2 KB
scripts/output_filters.pyscript16.8 KB
scripts/output_io.pyscript5.3 KB
scripts/pcb/__init__.pyscript0 B
scripts/pcb/assembly.pyscript58.3 KB
scripts/pcb/connectivity.pyscript27.7 KB
scripts/pcb/copper.pyscript61.0 KB
scripts/pcb/dfm.pyscript56.9 KB
scripts/pcb/geometry.pyscript59.5 KB
scripts/pcb/pipeline.pyscript30.3 KB
scripts/pcb/presentation.pyscript24.3 KB
scripts/pcb/reader.pyscript87.1 KB
scripts/pcb/routing.pyscript53.5 KB
scripts/project_config.pyscript23.1 KB
scripts/risk_summary.pyscript3.1 KB
scripts/run_id.pyscript1.7 KB
scripts/schema_codec.pyscript5.0 KB
scripts/schematic/__init__.pyscript0 B
scripts/schematic/audits.pyscript56.0 KB
scripts/schematic/bom_stats.pyscript6.1 KB
scripts/schematic/connectivity.pyscript62.9 KB
scripts/schematic/erc_pins.pyscript8.4 KB
scripts/schematic/hierarchy.pyscript21.5 KB
scripts/schematic/ic_analysis.pyscript21.4 KB
scripts/schematic/legacy_reader.pyscript49.4 KB
scripts/schematic/net_analysis.pyscript75.5 KB
scripts/schematic/pipeline.pyscript72.2 KB
scripts/schematic/presentation.pyscript20.9 KB
scripts/schematic/reader.pyscript64.7 KB
scripts/schematic/system_analyses.pyscript126.9 KB
scripts/signal_detectors.pyscript248.0 KB
scripts/summarize_findings.pyexecutablescript17.4 KB
scripts/validation_detectors.pyscript75.3 KB
scripts/what_if.pyscript68.4 KB

references/file-formats.md

View on GitHub
# KiCad File Format Reference

Detailed field-by-field documentation for all KiCad file types. Consult this when manually parsing or inspecting raw KiCad files.

## Table of Contents

1. [S-Expression Format Basics](#s-expression-format-basics)
2. [Schematic (.kicad_sch)](#schematic-kicad_sch)
3. [PCB Layout (.kicad_pcb)](#pcb-layout-kicad_pcb)
4. [Symbol Library (.kicad_sym)](#symbol-library-kicad_sym)
5. [Footprint (.kicad_mod)](#footprint-kicad_mod)
6. [Custom Design Rules (.kicad_dru)](#custom-design-rules-kicad_dru)
7. [Netlist (.net)](#netlist-net)
8. [Legacy KiCad 5 Schematic (.sch)](#legacy-kicad-5-schematic-sch)
9. [Project File (.kicad_pro)](#project-file-kicad_pro)

---

## S-Expression Format Basics

Modern KiCad schematic, board, symbol and footprint files use Lisp-like S-expressions (the project file `.kicad_pro` is JSON; see below): `(keyword value1 (child_keyword value2) ...)`.

- **Coordinates**: millimeters, origin top-left, X right, Y **down** in schematic and board files; library symbol definitions (`lib_symbols`, `.kicad_sym`) use a symbol-local origin with Y **up**, which KiCad negates when it places them
- **Angles**: degrees, counterclockwise positive
- **UUIDs**: stable object identifiers (KiCad 6+)
- **Strings**: quoted if containing spaces/special chars

The parser is `kicad_core/sexp.py` (`parse`, `parse_file`, `find_all`, `find_first`, `get_value`). The 2.x modules `sexp_parser` and `kicad_utils`, and the helpers once imported through `analyze_schematic` / `analyze_pcb`, were retired in 3.0; the v3.0.0 migration table in `CHANGELOG.md` lists each name's new home.

---

## Schematic (`.kicad_sch`)

### Top-Level Structure
```
(kicad_sch
  (version ...) (generator ...) (generator_version ...) (uuid ...) (paper ...)
  (lib_symbols ...)        ; Embedded copies of all library symbols used
  (junction ...)           ; Wire junction points
  (no_connect ...)         ; No-connect markers
  (wire ...)               ; Electrical wires: (wire (pts (xy X1 Y1) (xy X2 Y2)) (uuid ...))
  (bus ...)                ; Bus wires
  (bus_entry ...)          ; Bus entry connections
  (label ...)              ; Local net labels: (label "NAME" (at X Y ANGLE) ...)
  (global_label ...)       ; Global labels (cross-sheet nets)
  (hierarchical_label ...) ; Sheet-to-sheet connections
  (text ...)               ; Annotation text (not electrical)
  (polyline ...)           ; Graphical lines
  (symbol ...)             ; Placed component instances
  (sheet ...)              ; Hierarchical sub-sheet references
  (sheet_instances ...)    ; Sheet path/page info
)
```

### Symbol Instance (placed component)
```
(symbol
  (lib_id "Library:SymbolName")     ; Library reference
  (at X Y ANGLE)                     ; Position
  (unit N)                           ; For multi-unit symbols
  (uuid "...")
  (property "Reference" "R1" (at ...) (effects ...))
  (property "Value" "10K" (at ...) (effects ...))
  (property "Footprint" "Resistor_SMD:R_0805_2012Metric" ...)
  (property "Datasheet" "~" ...)
  (property "Description" "Resistor" ...)
  ; Custom properties (user-defined):
  (property "Mfg Part" "RC0805FR-0710KL" ...)
  (property "DigiKey Part" "311-10.0KCRCT-ND" ...)
  (pin "1" (uuid "..."))            ; Pin-to-UUID mapping
  (pin "2" (uuid "..."))
  (instances
    (project "ProjectName"
      (path "/root-uuid" (reference "R1") (unit 1))
    )
  )
)
```

### Extracting Key Info from Schematics

**Component list (BOM)**: Collect all `(symbol ...)` nodes. For each, read:
- `(property "Reference" ...)` - designator (R1, C5, U3)
- `(property "Value" ...)` - value (10K, 100n, STM32F407)
- `(property "Footprint" ...)` - PCB footprint
- `(property "Mfg Part" ...)` / `(property "DigiKey Part" ...)` - sourcing
- `(in_bom yes/no)` - whether to include in BOM
- `(dnp yes/no)` - Do Not Populate flag

**Net connectivity**: Nets are implicit in schematics, formed by:
1. **Wires** connecting pin endpoints
2. **Junctions** where wires cross and connect
3. **Labels** (`label` = local to sheet, `global_label` = all sheets)
4. **Power symbols** (e.g., `+3V3`, `GND`) create implicit nets: global, or sheet-local for a `(power local)` symbol (see Power rails below)
5. **Hierarchical labels** + sheet pins connect parent/child sheets

For detailed step-by-step net tracing with coordinate math and rotation transforms, read `net-tracing.md`.

**Power rails**: power symbols (library symbols marked `(power)`, usually from the `power:` library, e.g. `power:+3V3`) name their net. From format 20230221 (KiCad 8) the net is the symbol's Value; in older files and KiCad 5 it is the name of the symbol's hidden power-input pin, as KiCad renames them on load. A `(power local)` symbol (KiCad 10) names a net on its own sheet only; the others are global.

### Hierarchical Sheets
```
(sheet (at X Y) (size W H) (uuid "...")
  (property "Sheetname" "PowerSupply" ...)
  (property "Sheetfile" "power_supply.kicad_sch" ...)
  (pin "VIN" input (at X Y ANGLE) (uuid "..."))
)
```
Each sheet has its own `.kicad_sch` file. Pins on the sheet symbol connect to `hierarchical_label` nodes inside.

---

## PCB Layout (`.kicad_pcb`)

### Top-Level Structure
```
(kicad_pcb
  (version ...) (generator ...) (generator_version ...)
  (general (thickness 1.6) (legacy_teardrops no))
  (paper "A4")
  (layers ...)              ; Layer stack definition
  (setup ...)               ; Board setup, stackup, plot params
  (net 0 "")                ; KiCad ≤9: net declarations (index + name)
  (net 1 "GND")             ; KiCad 10: no net declarations — nets identified by name
  (net 2 "+3V3")
  ...
  (footprint ...)           ; Placed footprints with pads
  (segment ...)             ; Copper track segments
  (arc ...)                 ; Curved tracks (KiCad 6+)
  (via ...)                 ; Vias
  (zone ...)                ; Copper zones/pours
  (gr_line ...)             ; Graphical lines (board outline on Edge.Cuts)
  (gr_arc ...)              ; Graphical arcs
  (gr_circle ...)           ; Graphical circles
  (gr_rect ...)             ; Graphical rectangles
  (gr_text ...)             ; Board text
  (group ...)               ; Groups (KiCad 6+)
)
```

### Layer Definitions
KiCad 9-10 numbering:
```
(layers
  (0 "F.Cu" signal)         ; Front copper
  (4 "In1.Cu" signal)       ; Inner copper layers (if present)
  (2 "B.Cu" signal)         ; Back copper
  (5 "F.SilkS" user)        ; Front silkscreen
  (7 "B.SilkS" user)        ; Back silkscreen
  (25 "Edge.Cuts" user)     ; Board outline
  (31 "F.CrtYd" user)       ; Front courtyard
  (35 "F.Fab" user)         ; Front fabrication
  ...
)
```
**Note**: Layer numbers differ between versions, for the copper layers and for the non-copper ones above (KiCad 8, for example, numbers F.SilkS 37 and Edge.Cuts 44). In KiCad 5-8: F.Cu=0, In1.Cu..In30.Cu=1-30, B.Cu=31. In KiCad 9-10: F.Cu=0, B.Cu=2, In*n*.Cu=2*n*+2 (In1.Cu=4, In2.Cu=6). The numbers are fixed per version and do not depend on the layer count.

### Footprint on PCB
```
(footprint "Package:SOT-563"
  (layer "F.Cu")                    ; Which side of board
  (uuid "...")
  (at X Y ANGLE)                    ; Position and rotation
  (property "Reference" "U2" ...)
  (property "Value" "TPS61023" ...)
  (property "Mfg Part" "TPS61023DRLR" ...)
  (property "DigiKey Part" "296-TPS61023DRLRCT-ND" ...)
  (path "/schematic-uuid")          ; Links back to schematic symbol
  (sheetname "/")
  (sheetfile "project.kicad_sch")
  (attr smd)                        ; smd | through_hole
  ; Graphics (silkscreen, courtyard, fab):
  (fp_line (start X1 Y1) (end X2 Y2) (layer "F.SilkS") ...)
  (fp_rect (start X1 Y1) (end X2 Y2) (layer "F.CrtYd") ...)
  ; Pads with net assignments:
  (pad "1" smd roundrect
    (at X Y ANGLE)
    (size W H)
    (layers "F.Cu" "F.Mask" "F.Paste")
    (net 5 "+3V3")                  ; KiCad ≤9: (net number "name")
                                     ; KiCad 10: (net "name") — no numeric ID
    (pintype "passive")
    (uuid "...")
  )
  ; 3D model:
  (model "path/to/model.wrl" (offset ...) (scale ...) (rotate ...))
)
```

### Tracks, Vias, and Zones
```
; KiCad ≤9: net referenced by integer ID
(segment (start X1 Y1) (end X2 Y2) (width 0.2) (layer "F.Cu") (net 7) (uuid "..."))
(via (at X Y) (size 0.6) (drill 0.3) (layers "F.Cu" "B.Cu") (net 7) (uuid "..."))
(zone (net 1) (net_name "GND") (layer "F.Cu") (uuid "...") ...)

; KiCad 10: net referenced by name string, no net_name node on zones
(segment (start X1 Y1) (end X2 Y2) (width 0.2) (layer "F.Cu") (net "NetName") (uuid "..."))
(via (at X Y) (size 0.6) (drill 0.3) (layers "F.Cu" "B.Cu") (net "NetName") (uuid "..."))
(zone (net "GND") (layer "F.Cu") (uuid "...") ...)

; Zone structure (both versions):
(zone (net ...) ... (layer "F.Cu") (uuid "...")
  (connect_pads (clearance 0.25))
  (min_thickness 0.25)
  (fill yes (thermal_gap 0.5) (thermal_bridge_width 0.5))
  (polygon (pts (xy X1 Y1) (xy X2 Y2) ...))      ; User-drawn outline
  (filled_polygon (pts ...))                        ; Computed fill result
)
```

### Board Outline
Look for graphical items on `Edge.Cuts` layer:
```
(gr_line (start X1 Y1) (end X2 Y2) (layer "Edge.Cuts") ...)
(gr_arc (start ...) (mid ...) (end ...) (layer "Edge.Cuts") ...)
```

### Tracing Net Connectivity on PCB
To find everything connected to a net:

**KiCad ≤9** (integer net IDs):
1. Find `(net N "NetName")` in the net declarations
2. Find all `(pad ... (net N "name") ...)` in footprints
3. Find all `(segment ... (net N) ...)` — copper traces
4. Find all `(via ... (net N) ...)` — layer transitions
5. Find all `(zone (net N) ...)` — copper pours

**KiCad 10** (string net names — no net declarations section):
1. Find all `(pad ... (net "NetName") ...)` in footprints
2. Find all `(segment ... (net "NetName") ...)` — copper traces
3. Find all `(via ... (net "NetName") ...)` — layer transitions
4. Find all `(zone (net "NetName") ...)` — copper pours

---

## Symbol Library (`.kicad_sym`)

```
(kicad_symbol_lib
  (version ...) (generator ...) (generator_version ...)
  (symbol "SymbolName"
    (pin_names (offset 0) (hide yes))
    (exclude_from_sim no) (in_bom yes) (on_board yes)
    (property "Reference" "R" ...)
    (property "Value" "R" ...)
    (property "Footprint" "" ...)
    (property "Datasheet" "~" ...)
    (property "Description" "Resistor" ...)
    (property "ki_keywords" "R res resistor" ...)
    (property "ki_fp_filters" "R_*" ...)      ; Footprint filter patterns

    (symbol "SymbolName_0_1"                   ; Unit 0 = shared graphics
      (rectangle (start ...) (end ...) ...)
    )
    (symbol "SymbolName_1_1"                   ; Unit 1 pins
      (pin TYPE SHAPE (at X Y ANGLE) (length L)
        (name "PinName" ...)
        (number "1" ...)
      )
    )
  )
)
```

**Pin types**: `input`, `output`, `bidirectional`, `tri_state`, `passive`, `free`, `unspecified`, `power_in`, `power_out`, `open_collector`, `open_emitter`, `no_connect`

**Multi-unit naming**: `SymbolName_UNIT_STYLE` - unit 0 = common, units 1+ = per-unit

---

## Footprint (`.kicad_mod`)

Stored in `.pretty/` directories (one file per footprint).

```
(footprint "FootprintName"
  (version ...) (generator ...) (layer "F.Cu")
  (descr "Description text")
  (tags "tag1 tag2")
  (attr smd|through_hole|board_only)
  (property "Reference" "REF**" (layer "F.SilkS") ...)
  (property "Value" "FootprintName" (layer "F.Fab") ...)
  ; Pads (no net assignment in library, only on PCB):
  (pad "1" smd roundrect (at X Y) (size W H) (layers "F.Cu" "F.Mask" "F.Paste") ...)
  (pad "2" thru_hole circle (at X Y) (size W H) (drill D) (layers "*.Cu" "*.Mask") ...)
  ; 3D model:
  (model "path.wrl" ...)
)
```

**Pad types**: `smd`, `thru_hole`, `np_thru_hole` (non-plated), `connect` (edge connector)
**Pad shapes**: `circle`, `rect`, `oval`, `roundrect`, `trapezoid`, `custom`

---

## Custom Design Rules (`.kicad_dru`)

Text-based constraint rules applied during DRC. Example:
```
(version 1)
(rule "Track width, outer layer"
  (layer outer)
  (condition "A.Type == 'track'")
  (constraint track_width (min 0.127mm))
)
(rule "Clearance: pad to pad"
  (condition "A.isPlated() && B.isPlated() && A.Net != B.Net")
  (constraint clearance (min 0.127mm))
)
```
Useful for enforcing manufacturer capabilities (e.g., JLCPCB, PCBWay).

The PCB analyzer applies a rule without a `(condition ...)` as KiCad does. It does not evaluate conditions. A conditional rule is listed in `design_rule_compliance.conditional_rules_skipped`, and an item is reported only when it breaks the rule whichever way the condition goes. A conditional rule therefore never adds a violation, but it can hide one (a relaxed minimum or maximum, or `(severity ignore)`); run KiCad's DRC for those rules.

---

## Netlist (`.net`)

```
(export (version D)
  (components
    (comp (ref U1)
      (value STM32F407ZGTx)
      (footprint Package_QFP:LQFP-144_20x20mm_P0.5mm)
      (libsource (lib MCU_ST_STM32F4) (part STM32F407ZGTx) (description "..."))
      (sheetpath (names /) (tstamps /))
      (tstamp HEXID)
    )
  )
  (nets
    (net (code 1) (name GND)
      (node (ref U1) (pin 12))
      (node (ref C1) (pin 2))
    )
  )
)
```
The netlist explicitly lists every net and which component pins belong to it.

---

## Legacy KiCad 5 Schematic (`.sch`)

```
EESchema Schematic File Version 4
EELAYER 30 0
EELAYER END
$Comp                                    ; Component instance
L Library:Symbol Reference
U unit convert timestamp                 ; convert = placed body style (2 = De Morgan)
P x y
F 0 "R1" H x y size flags C CNN        ; F0 = Reference
F 1 "10k" H x y size flags C CNN        ; F1 = Value
F 2 "Footprint:Name" H x y size flags   ; F2 = Footprint
F 3 "datasheet_url" H x y size flags    ; F3 = Datasheet
  1    x y                               ; Instance position
  orientation_matrix
$EndComp
Wire Wire Line                           ; Electrical wire
  x1 y1 x2 y2
Text Label x y orientation size ~ 0      ; Local net label
NetName
```

**Key differences from modern format:**
- Coordinates in mils (1/1000 inch), not mm
- No UUIDs, uses timestamps for identification
- Component fields are positional (F0=ref, F1=value, F2=footprint, F3=datasheet)
- Wire connectivity is positional: endpoints that coincide connect, and so does a junction lying on a wire's interior; labels connect at their anchor point

---

## Project File (`.kicad_pro`)

JSON format. Key sections:
- `board.design_settings` - DRC rules, track widths, via sizes, teardrop settings
- `board.design_settings.rules` - min clearance, hole sizes, track widths
- `board.design_settings.track_widths` - available track width options
- `board.design_settings.via_dimensions` - available via size options
- `erc.rule_severities` - ERC check severity levels
- `net_settings.classes` - net class definitions (clearance, track width, via size per class)
- `schematic.bom_settings` - BOM field configuration
- `schematic.drawing` - default text/line sizes

### kicad-cli DRC/ERC on a copied project

Run `kicad-cli` DRC/ERC on the original project, or copy `fp-lib-table` and `sym-lib-table` (and the libraries they point to) along with it. On a copy without them every footprint and symbol raises library warnings that say nothing about the design: a copied `simple-project` gave 3 `lib_footprint_issues` in DRC and 5 `lib_symbol_issues` plus 3 `footprint_link_issues` in ERC (kicad-cli 10, JSON reports).
finishing-a-development-branchobra/superpowersUse when implementation is complete, all tests pass, and you need to decide how to integrate the workStars: 322kUpdated Claude CodeCodexVerifiedInstall
systematic-debuggingobra/superpowersUse when encountering any bug, test failure, or unexpected behavior, before proposing fixesStars: 322kUpdated Claude CodeCodexVerifiedInstall
test-driven-developmentobra/superpowersUse when implementing any feature or bugfix, before writing implementation codeStars: 322kUpdated Claude CodeCodexVerifiedInstall
skill-creatoranthropics/skillsCreate new skills, modify and improve existing skills, and measure skill performance. Use when users want to create a skill from scratch, edit, or optimize an existing skill, run evals to test a skill, benchmark skill performance with variance analysis, or optimize a skill's description for better triggering accuracy.Stars: 198kUpdated Claude CodeCodexVerifiedInstall