CLI Reference

Complete reference for the kct (kicad-tools) command-line interface.

Global Options

kct [--help] [--version] <command> [options]

Option	Description
`--help`, `-h`	Show help message
`--version`, `-V`	Show version number

Commands Overview

Category	Command	Description
Analysis	`symbols`	List and query schematic symbols
	`nets`	Trace and analyze nets
	`sch`	Schematic analysis tools
	`pcb`	PCB query tools
Validation	`erc`	Parse ERC reports
	`drc`	Parse DRC reports with manufacturer rules
	`check`	Pure Python DRC (no kicad-cli)
	`validate`	Schematic-to-PCB sync validation
Manufacturing	`bom`	Generate bill of materials
	`mfr`	Manufacturer tools and rules
	`fleet status`	Fleet-wide routing + manufacturing readiness survey
	`stitch`	Add via stitching to power planes
	`build`	One-shot pipeline (schematic → PCB → manufacturing)
Libraries	`lib`	Symbol library tools
	`footprint`	Footprint generation tools
	`parts`	LCSC parts lookup and search
	`datasheet`	Datasheet search and PDF parsing
PCB Operations	`route`	Autoroute a PCB
	`zones`	Add copper pour zones
	`placement`	Detect and fix placement conflicts
	`optimize-placement`	CMA-ES placement optimizer (anchor-aware)
	`optimize-traces`	Optimize PCB traces
AI Integration	`reason`	LLM-driven PCB layout reasoning
	`mcp`	MCP server for AI agent integration
Analysis (v0.7)	`analyze congestion`	Routing congestion hotspots
	`analyze trace-lengths`	Timing-critical trace analysis
	`analyze thermal`	Thermal hotspot detection
	`analyze signal-integrity`	Crosstalk and impedance analysis
	`erc explain`	ERC root cause analysis
	`constraints check`	Constraint conflict detection
	`net-status`	Net connectivity validation
Cost (v0.7)	`estimate cost`	Manufacturing cost estimation
	`parts availability`	LCSC stock checking
	`suggest alternatives`	Alternative part suggestions
Utilities	`config`	View/manage configuration
	`interactive`	Launch interactive REPL mode

Analysis Commands

`symbols`

List and query schematic symbols.

kct symbols <schematic> [options]

Option	Description
`--format {table,json,csv}`	Output format (default: table)
`--filter PATTERN`	Filter by reference pattern (e.g., "R*")
`--lib LIB_ID`	Filter by library ID
`--verbose`, `-v`	Show additional details

Examples:

kct symbols project.kicad_sch
kct symbols project.kicad_sch --format json
kct symbols project.kicad_sch --filter "C*"  # All capacitors

`nets`

Trace and analyze nets in a schematic.

kct nets <schematic> [options]

Option	Description
`--format {table,json}`	Output format (default: table)
`--net NAME`	Show only specified net
`--stats`	Show net statistics

Examples:

kct nets project.kicad_sch
kct nets project.kicad_sch --net VCC
kct nets project.kicad_sch --stats --format json

`sch`

Schematic analysis subcommands.

kct sch <subcommand> <schematic> [options]

Subcommand	Description
`summary`	Show schematic summary
`symbols`	List symbols with details
`labels`	List all labels
`wires`	List wire segments
`hierarchy`	Show sheet hierarchy
`validate`	Validate schematic structure
`pin-positions`	Get symbol pin positions
`check-connections`	Check for unconnected pins
`find-unconnected`	Find unconnected nets

Examples:

kct sch summary project.kicad_sch
kct sch hierarchy project.kicad_sch --format json
kct sch find-unconnected project.kicad_sch

`pcb`

PCB query subcommands.

kct pcb <subcommand> <pcb_file> [options]

Subcommand	Description
`query`	Query footprints and tracks
`modify`	Modify PCB elements

Examples:

kct pcb query board.kicad_pcb --footprints
kct pcb query board.kicad_pcb --tracks --net GND

Validation Commands

`erc`

Parse and analyze ERC (Electrical Rule Check) reports.

kct erc <report> [options]

Option	Description
`--format {table,json}`	Output format (default: table)
`--errors-only`	Show only errors, not warnings
`--type TYPE`	Filter by error type
`--sheet SHEET`	Filter by sheet name

Examples:

kct erc project.erc
kct erc project.erc --errors-only --format json
kct erc project.erc --type "unconnected"

`drc`

Parse DRC reports with optional manufacturer rule comparison.

kct drc <report> [options]

Option	Description
`--format {table,json}`	Output format (default: table)
`--errors-only`	Show only errors
`--type TYPE`	Filter by violation type
`--net NET`	Filter by net name
`--mfr {jlcpcb,oshpark,pcbway,seeed}`	Apply manufacturer rules
`--layers N`	Number of layers (default: 2)
`--compare`	Compare manufacturer rules

Examples:

kct drc board.drc
kct drc board.kicad_pcb --mfr jlcpcb
kct drc --compare  # Show all manufacturer rules

`check`

Pure Python DRC (no kicad-cli required).

kct check <pcb_file> [options]

Option	Description
`--format {table,json}`	Output format
`--mfr {jlcpcb,oshpark,pcbway}`	Manufacturer rules
`--rules RULES`	Custom rules file

Examples:

kct check board.kicad_pcb
kct check board.kicad_pcb --mfr jlcpcb --format json

`validate`

Validate schematic-to-PCB synchronization.

kct validate --sync <schematic> <pcb>

Examples:

kct validate --sync project.kicad_sch board.kicad_pcb

Manufacturing Commands

`bom`

Generate bill of materials.

kct bom <schematic> [options]

Option	Description
`--format {table,json,csv}`	Output format (default: table)
`--group`	Group identical components
`--exclude PATTERN`	Exclude by reference (can repeat)
`--include-dnp`	Include DNP (Do Not Place) parts
`--sort {reference,value,footprint}`	Sort order
`--output`, `-o`	Output file

Examples:

kct bom project.kicad_sch
kct bom project.kicad_sch --format csv --group -o bom.csv
kct bom project.kicad_sch --exclude "TP*" --exclude "H*"

`mfr`

Manufacturer tools and design rules.

kct mfr <subcommand> [options]

Subcommand	Description
`rules`	Show manufacturer design rules
`compare`	Compare multiple manufacturers
`dru`	Generate KiCad DRU file

Examples:

kct mfr rules jlcpcb
kct mfr compare jlcpcb oshpark
kct mfr dru jlcpcb -o jlcpcb.dru

`fleet status`

Survey routing and manufacturing readiness across every board in the repo. Implemented in src/kicad_tools/cli/fleet_cmd.py.

usage: kicad-tools fleet status [-h] [--boards-dir FLEET_BOARDS_DIR]
                                [--format {table,json}] [--ship-only]
                                [--include-stale] [--pattern FLEET_PATTERN]

Option	Description
`--boards-dir DIR`	Root containing per-board subdirs (default: `boards`)
`--format {table,json}`	Output format (default: `table`)
`--ship-only`	Show only ship-ready boards in table output
`--include-stale`	(Reserved) treat stale artifacts as not shippable
`--pattern GLOB`	Glob to identify the routed PCB inside `output/` (default: `*_routed.kicad_pcb`)

Each board is scored on net completion, DRC status, and presence of the required manufacturing artifacts (gerbers, BOM, CPL). A board is "ship-ready" when every gate is green; otherwise the row lists the first blocker. The table view summarises one board per line; --format json emits the full per-board breakdown for downstream tooling.

Examples:

# Quick "what's shippable?" overview across the fleet
kct fleet status

# CI-friendly machine output
kct fleet status --format json > fleet.json

# Restrict to a custom layout (boards live under hardware/v2/...)
kct fleet status --boards-dir hardware/v2 --pattern '*-final.kicad_pcb'

# Only show what is ready to ship
kct fleet status --ship-only

`stitch`

Add via stitching to power-plane nets. Implemented in src/kicad_tools/cli/stitch_cmd.py.

kct stitch <pcb_file> [options]

Option	Description
`--net NET`, `-n`	Net to stitch (repeatable). Default: auto-detect power-plane nets from zones
`--via-size MM`	Via pad diameter in mm (default: 0.45)
`--drill MM`	Via drill in mm (default: 0.2)
`--clearance MM`	Minimum clearance from existing copper (default: 0.2)
`--offset MM`	Max distance from pad center for via placement (default: 0.5)
`--target-layer LAYER`, `-t`	Target plane layer (e.g. `In1.Cu`). Default: auto
`--trace-width MM`	Width of pad-to-via trace segments (default: 0.2)
`--escape-distance MM`	Max escape trace length for dense IC pads (default: 3.0)
`--blanket`, `-b`	Place vias on a grid across zone polygons
`--spacing MM`	Grid spacing for blanket stitching (default: 3.0)
`--mfr NAME`, `--manufacturer NAME`	Manufacturer profile (e.g. `jlcpcb`, `jlcpcb-tier1`) — overrides `--via-size`/`--drill`
`--copper OZ`	Outer copper weight in oz (default: 1.0); selects the correct row from the manufacturer YAML
`--dry-run`, `-d`	Show changes without applying
`-o`, `--output PATH`	Output file (default: modify in place)
`--drc`	Run DRC after stitching (fills zones via `kicad-cli`)

Manufacturer-driven via dimensions. When --mfr is set the stitch via size and drill are resolved from the manufacturer YAML using the board's actual copper layer count, overriding --via-size and --drill. This keeps stitching dimensions consistent with the rules the router and DRC are already enforcing. Use --copper to pick the right stackup row (1.0 oz vs. 2.0 oz).

Examples:

# Auto-detect power nets and stitch with default 0.45/0.2 vias
kct stitch board.kicad_pcb

# Use the JLCPCB tier-1 profile (smaller vias, fine-pitch friendly)
kct stitch board.kicad_pcb --mfr jlcpcb-tier1 --copper 1.0

# Blanket-stitch a specific net on a 3mm grid
kct stitch board.kicad_pcb --net GND --blanket --spacing 3.0

`build`

One-shot pipeline that runs schematic generation, sync, PCB layout, routing, stitching, manufacturing artefacts and verification in order. Implemented in src/kicad_tools/cli/build_cmd.py.

kct build [SPEC] [--step STEP] [options]

SPEC is a positional argument (.kct file or project directory). Defaults to the current working directory if omitted.

Step (`--step`)	Purpose
`schematic`	Generate `.kicad_sch` from the design spec
`erc`	Run ERC against the schematic
`pcb`	Generate a fresh `.kicad_pcb` skeleton
`sync`	Sync footprints/nets from schematic into the PCB
`outline` / `placement` / `zones` / `silkscreen`	Layout-stage passes
`route`	Autoroute
`stitch`	Add power-plane via stitching
`preflight-routing`	Routing-completeness gate before manufacturing
`verify`	Final connectivity + DRC validation
`export`	Emit gerbers / BOM / CPL
`all` (default)	Run the whole sequence

The preflight-routing step runs between stitch and verify in the default all sequence. It re-uses kct net-status semantics in-process and blocks the build if any nets are incomplete. Override with --allow-incomplete (advertised; CI-greppable) or the global --force. See Routing Completeness Preflight for the full semantics.

The outer kct build parser is kept in lockstep with the authoritative inner parser at src/kicad_tools/cli/build_cmd.py by tests/test_build_parser_parity.py, which fails if a new flag or --step choice is added to the inner parser without also being surfaced on the outer CLI.

Examples:

# Full pipeline driven by the project spec. `SPEC` is positional.
kct build boards/05-bldc-motor-controller/project.kct

# Skip the routing-completeness gate (WIP escape hatch).
kct build boards/05-bldc-motor-controller/project.kct --allow-incomplete

# Run a single stage.
kct build boards/05-bldc-motor-controller/project.kct \
    --step preflight-routing

Library Commands

`lib`

Symbol library tools.

kct lib <subcommand> [options]

Subcommand	Description
`list`	List symbols in a library
`info`	Show symbol details
`create`	Create a new symbol

Examples:

kct lib list Device.kicad_sym
kct lib info Device.kicad_sym R

`footprint`

Footprint generation tools.

kct footprint <subcommand> [options]

Subcommand	Description
`generate`	Generate parametric footprints
`validate`	Validate footprint pad spacing
`fix`	Fix footprint issues

kct footprint generate <type> [options]

Type	Description
`soic`	SOIC packages
`qfp`	QFP packages
`qfn`	QFN packages
`dfn`	DFN packages
`bga`	BGA packages
`chip`	Chip resistors/capacitors
`sot`	SOT packages
`dip`	DIP packages

Examples:

kct footprint generate soic --pins 8 --pitch 1.27
kct footprint generate qfn --pins 24 --size 4x4
kct footprint validate MyLib.kicad_mod

`parts`

LCSC parts database lookup.

kct parts <subcommand> [options]

Subcommand	Description
`search`	Search for parts
`lookup`	Get part details by LCSC number
`check`	Check part availability

Examples:

kct parts search "STM32F103"
kct parts lookup C8734
kct parts check C8734 --quantity 100

`datasheet`

Datasheet tools.

kct datasheet <subcommand> [options]

Subcommand	Description
`search`	Search for datasheets
`download`	Download a datasheet
`parse`	Extract pin info from PDF

Examples:

kct datasheet search "ATmega328P"
kct datasheet download "ATmega328P" -o atmega328p.pdf
kct datasheet parse atmega328p.pdf --pins

PCB Operation Commands

`route`

Autoroute a PCB. See Routing Guide for strategy choices and worked examples. Implemented in src/kicad_tools/cli/route_cmd.py.

kct route <pcb_file> [options]

Common flags (the full surface lives in kct route --help):

Option	Description
`-o`, `--output PATH`	Output file (default: `<input>_routed.kicad_pcb`)
`--strategy {basic,negotiated,monte-carlo,evolutionary}`	Routing strategy (default: `negotiated`)
`--trace-width MM` / `--clearance MM`	Trace + clearance overrides
`--via-diameter MM` / `--via-drill MM`	Via geometry
`--manufacturer NAME` (`--mfr`)	Manufacturer profile for DRC and adaptive rules
`--layers {auto,2,4,4-sig,4-all,6}`	Layer stack configuration (default: `auto`)
`--min-completion FLOAT`	Minimum completion ratio for success (default: 0.95)
`--timeout SEC` / `--per-net-timeout SEC`	Global / per-net wall-clock caps
`--seed N`	Seed Python `random` for reproducible routing (#2589)
`--auto-fix` / `--auto-fix-passes N`	Run `kct fix-drc` after routing on DRC failure
`--skip-drc`	Skip post-route DRC validation

Strategy escalation flags

Option	Description
`--auto-layers` / `--no-auto-layers`	Escalate layer count on routing failure. Default: enabled. Tries 2 → 4 → 6 until success or `--max-layers` is reached. Pass `--no-auto-layers` to opt out.
`--max-layers {2,4,6}`	Upper bound for `--auto-layers` (default: 6)
`--auto-mfr-tier`	Escalate to a tighter manufacturer tier when geometry blocks routing (e.g. `jlcpcb` → `jlcpcb-tier1` to gain via-in-pad). Default: disabled.
`--mfr-tier-ladder LIST`	Explicit comma-separated tier ladder, e.g. `'jlcpcb,jlcpcb-tier1'`. Overrides the default ladder registered for `--mfr`.
`--adaptive-rules`	Progressively relax trace width / clearance until routing succeeds or manufacturer limits are reached.
`--min-trace MM` / `--min-clearance-floor MM`	Floors for `--adaptive-rules`

See Routing Guide → Strategy Escalation.

Long-running routes

Option	Description
`--checkpoint-interval SEC`	Interval between best-so-far checkpoint writes to `--output`. Default: 30. Pass `0` to disable.
`--export-failed-nets PATH`	Write failed-net names (one per line) for follow-up.
`--strict`	Exit non-zero if the written PCB has any disconnected net.

--output writes are atomic; combined with --checkpoint-interval this means a long route can be safely interrupted (SIGINT) and the partial result on disk remains valid for inspection or resume. See Routing Guide → Long-Running Routes.

Auto-fix and exit codes

--auto-fix runs the DRC repair pass after routing. If repair cannot be applied cleanly the partial output is rolled back so the file on disk matches what the router actually produced (issue #2852, #2853, #2861). The rollback path is wired through all four routing code paths (Autorouter, RoutingOrchestrator, MCP, reasoning agent) and surfaces as exit code 3. See the Exit Codes table.

Examples:

# Default escalation: 2L → 4L → 6L, atomic checkpoint every 30s
kct route board.kicad_pcb -o routed.kicad_pcb

# Stay at 2L (e.g. for cost) but allow manufacturer-tier escalation for fine-pitch QFP
kct route board.kicad_pcb --no-auto-layers --auto-mfr-tier --mfr jlcpcb

# Explicit ladder; long timeout; auto-fix DRC; reproducible
kct route board.kicad_pcb \
  --auto-mfr-tier --mfr-tier-ladder 'jlcpcb,jlcpcb-tier1' \
  --timeout 1500 --auto-fix --seed 42 -o routed.kicad_pcb

# CI-friendly checkpointing every 10s
kct route board.kicad_pcb --checkpoint-interval 10 -o routed.kicad_pcb

`zones`

Add copper pour zones.

kct zones <subcommand> <pcb_file> [options]

Subcommand	Description
`add`	Add a copper zone
`list`	List existing zones

Examples:

kct zones add board.kicad_pcb --net GND --layer B.Cu
kct zones list board.kicad_pcb

`placement`

Detect and fix placement conflicts.

kct placement <subcommand> <pcb_file> [options]

Subcommand	Description
`check`	Check for placement conflicts
`optimize`	Optimize component placement
`suggestions`	Get placement suggestions

Examples:

kct placement check board.kicad_pcb
kct placement optimize board.kicad_pcb -o optimized.kicad_pcb
kct placement suggestions board.kicad_pcb --format json

`optimize-placement`

CMA-ES placement optimizer. Distinct from kct placement optimize (physics / evolutionary): this command runs a CMA-ES loop with explicit anchor and feasibility semantics. Implemented in src/kicad_tools/cli/optimize_placement_cmd.py.

kct optimize-placement <pcb_file> [options]

Option	Description
`--strategy {cmaes}`	Optimization strategy (default: `cmaes`)
`--max-iterations N`	Maximum optimizer iterations (default: 1000)
`-o`, `--output PATH`	Output PCB (default: overwrite input)
`--seed {force-directed,random}`	Seed placement method
`--weights JSON`	Custom cost weights: `overlap`, `drc`, `boundary`, `wirelength`, `area`
`--dry-run`	Evaluate current placement without optimizing
`--progress N`	Print score every N iterations (0 disables)
`--checkpoint DIR`	Directory for checkpoint save/resume
`--no-slide-off`	Disable slide-off overlap pre-processing on the seed
`--anchor-weight FLOAT`	Per-net HPWL multiplier boost for nets that touch `(locked)` footprints. Scales each qualifying net's HPWL by `1 + anchor_weight * (anchored_pins / total_pins)`. Default 0.0.
`--time-budget SEC`	Wall-clock budget (bounds the feasibility-gated convergence loop)
`--allow-infeasible`	Exit 0 even when overlap/DRC/boundary violations remain
`-v` / `-q`	Verbose / quiet

Anchor-weight discrepancy to know about. The --help text recommends 2.0 .. 5.0 as a starting range. The validated recipe in Placement Optimization → Anchoring Perimeter Footprints uses --anchor-weight 1.0 — the help-text range is the conservative knob designers would reach for; 1.0 is the value that actually lifted board-05 BLDC from 40% → 60% routing completion in practice. Treat help text as the ceiling and the guide as the proven floor.

Feasibility gate. By default the optimizer exits 1 with FATAL: optimizer exited with infeasible placement (...) on stderr if the final placement still has overlap/DRC/boundary violations (issue #2821). Use --allow-infeasible to override (recommended only when the next step is a router that can absorb residual boundary violations). Use --time-budget to bound the "keep going past plateau while infeasible" loop.

Examples:

# Anchored optimization — perimeter parts already marked locked=true
kct optimize-placement board.kicad_pcb \
  --anchor-weight 1.0 --max-iterations 400 --time-budget 120 \
  --allow-infeasible -o optim.kicad_pcb

# Evaluate the seed placement without moving anything
kct optimize-placement board.kicad_pcb --dry-run -v

# Resume from a checkpoint dir
kct optimize-placement board.kicad_pcb --checkpoint .optim_state/

See Placement Optimization Guide.

`optimize-traces`

Optimize PCB traces.

kct optimize-traces <pcb_file> [options]

Option	Description
`--output`, `-o`	Output file
`--length-match`	Enable length matching

AI Integration Commands

`reason`

LLM-driven PCB layout reasoning.

kct reason <pcb_file> [options]

Option	Description
`--interactive`	Interactive mode
`--export-state`	Export state for external LLM
`--auto-route`	Auto-route priority nets
`--output`, `-o`	Output file

Examples:

kct reason board.kicad_pcb --interactive
kct reason board.kicad_pcb --export-state > state.json
kct reason board.kicad_pcb --auto-route -o routed.kicad_pcb

`mcp`

MCP server for AI agent integration.

kct mcp serve [options]

Option	Description
`--http`	Use HTTP transport instead of stdio
`--port PORT`	HTTP port (default: 8080)

Examples:

# Start stdio server (for Claude Desktop)
kct mcp serve

# Start HTTP server
kct mcp serve --http --port 8080

See MCP Documentation for configuration details.

Analysis Commands (v0.7)

`analyze congestion`

Detect routing congestion hotspots.

kct analyze congestion <pcb_file> [options]

Option	Description
`--format {table,json}`	Output format
`--threshold FLOAT`	Congestion threshold (0-1)

`analyze trace-lengths`

Analyze timing-critical trace lengths.

kct analyze trace-lengths <pcb_file> [options]

Option	Description
`--format {table,json}`	Output format
`--net NET`	Analyze specific net
`--diff-pairs`	Show differential pair skew

`analyze thermal`

Detect thermal hotspots and heat sources.

kct analyze thermal <pcb_file> [options]

Option	Description
`--format {table,json}`	Output format

`analyze signal-integrity`

Analyze crosstalk risk and impedance discontinuities.

kct analyze signal-integrity <pcb_file> [options]

Option	Description
`--format {table,json}`	Output format

`erc explain`

ERC root cause analysis with fix suggestions.

kct erc explain <schematic> [options]

Option	Description
`--format {table,json}`	Output format

`constraints check`

Detect constraint conflicts (keepout/grouping/region).

kct constraints check <pcb_file> [options]

Option	Description
`--format {table,json}`	Output format

`net-status`

Validate net connectivity (unrouted, islands, isolated pads). The preflight-routing step of kct build and the readiness check inside kct fleet status both delegate to this analyzer in-process.

kct net-status <pcb_file> [options]

Option	Description
`--format {table,json}`	Output format
`--net NET`	Check a specific net
`--incomplete`	Show only incomplete / unrouted nets
`--by-class`	Group output by net class
`-v`, `--verbose`	Per-segment / per-pad detail

Exit code semantics are reused by the preflight-routing step in kct build and by kct fleet status to decide "ship-ready vs. not".

Examples:

kct net-status board.kicad_pcb --incomplete --format json
kct net-status board.kicad_pcb --by-class

Cost Commands (v0.7)

`estimate cost`

Estimate manufacturing cost.

kct estimate cost <pcb_file> [options]

Option	Description
`--format {table,json}`	Output format
`--mfr {jlcpcb,pcbway,oshpark,seeed}`	Manufacturer
`--quantity N`	Board quantity

`parts availability`

Check LCSC stock availability.

kct parts availability <schematic> [options]

Option	Description
`--format {table,json}`	Output format
`--quantity N`	Required quantity

`suggest alternatives`

Suggest alternative parts for unavailable components.

kct suggest alternatives <schematic> [options]

Option	Description
`--format {table,json}`	Output format

Utility Commands

`config`

View and manage configuration.

kct config [options]

Option	Description
`--show`	Show current configuration
`--set KEY VALUE`	Set a configuration value
`--reset`	Reset to defaults

`interactive`

Launch interactive REPL mode.

kct interactive [pcb_file]

Provides an interactive shell for exploring and modifying PCB files.

Output Formats

Most commands support multiple output formats:

Format	Description
`table`	Human-readable table (default)
`json`	Machine-readable JSON
`csv`	Comma-separated values

Use --format to specify:

kct symbols project.kicad_sch --format json

Exit Codes

Default (most commands)

Code	Meaning
0	Success
1	Error (invalid input, file not found, etc.)
2	Invalid arguments
130	Interrupted (Ctrl+C)

`kct route` ladder

The router exposes a finer-grained ladder so CI can tell partial routing apart from clean routing with DRC issues. Source of truth: the epilog at src/kicad_tools/cli/route_cmd.py:4051-4059.

Code	Meaning
0	All nets routed (or meets `--min-completion`), DRC clean
1	Fatal failure — no nets routed
2	Partial routing — below `--min-completion` threshold
3	Routing meets threshold but DRC violations remain — also returned when `--auto-fix` rollback fires (issue #2852). Both meanings share this code by design (see `route_cmd.py:2576-2580`).
4	Partial routing and segment-segment clearance violations
5	Interrupted by SIGINT with partial results saved (file on disk is valid)

`kct optimize-placement`

Code	Meaning
0	Optimizer converged to a feasible placement (or `--allow-infeasible` was set)
1	Final placement infeasible — overlap / DRC / boundary violations remain (issue #2821). Override with `--allow-infeasible`.
2	Invalid arguments
130	Interrupted (Ctrl+C)

`kct fleet status`

Source of truth: module docstring at src/kicad_tools/cli/fleet_cmd.py:17-21.

Code	Meaning
0	All surveyed boards are ship-ready
1	Argparse / IO error
2	One or more boards are not ship-ready (also returned when no boards are found, since "no ship-ready boards" is treated as not-ship-ready). Matches `kct net-status` semantics.

Environment Variables

Variable	Description
`KICAD_TOOLS_CONFIG`	Config file path
`KICAD_CLI_PATH`	Path to kicad-cli binary
`LCSC_API_KEY`	LCSC API key for parts lookup

FilesExpand file tree

cli.md

Latest commit

History

cli.md

File metadata and controls

CLI Reference

Global Options

Commands Overview

Analysis Commands

symbols

nets

sch

pcb

Validation Commands

erc

drc

check

validate

Manufacturing Commands

bom

mfr

fleet status

stitch

build

Library Commands

lib

footprint

parts

datasheet

PCB Operation Commands

route

Strategy escalation flags

Long-running routes

Auto-fix and exit codes

zones

placement

optimize-placement

optimize-traces

AI Integration Commands

reason

mcp

Analysis Commands (v0.7)

analyze congestion

analyze trace-lengths

analyze thermal

analyze signal-integrity

erc explain

constraints check

net-status

Cost Commands (v0.7)

estimate cost

parts availability

suggest alternatives

Utility Commands

config

interactive

Output Formats

Exit Codes

Default (most commands)

kct route ladder

kct optimize-placement

kct fleet status

Environment Variables

`symbols`

`nets`

`sch`

`pcb`

`erc`

`drc`

`check`

`validate`

`bom`

`mfr`

`fleet status`

`stitch`

`build`

`lib`

`footprint`

`parts`

`datasheet`

`route`

`zones`

`placement`

`optimize-placement`

`optimize-traces`

`reason`

`mcp`

`analyze congestion`

`analyze trace-lengths`

`analyze thermal`

`analyze signal-integrity`

`erc explain`

`constraints check`

`net-status`

`estimate cost`

`parts availability`

`suggest alternatives`

`config`

`interactive`

`kct route` ladder

`kct optimize-placement`

`kct fleet status`