mcpField
K
kicad-panelize

kicad-panelize

github.com/backplaneworksOther413311 installsUpdated 2d ago
Repository

About kicad-panelize

kicad-panelize is a skill for agents preparing KiCad PCB panels with KiKit. It guides board inspection, panel configuration, generation, and rendered-output checks while preserving the source board.

Key features

  1. 01Inspect board geometry and edge features
  2. 02Configure arrays, tabs, frames, and tooling
  3. 03Generate versioned panels without overwriting sources
  4. 04Validate panel files and renders

Use cases

  1. 01Panelize a single-board KiCad design
  2. 02Set tabs around edge connectors or castellations
  3. 03Prepare tooling holes and fiducials
  4. 04Review generated panel geometry

Install

Copy the command and run it in a terminal.

$npx skills add https://github.com/backplaneworks/kistack --skill kicad-panelize

After installing, type/kicad-panelizein Claude Code to confirm it loaded.

Details

From the project README

Skill for PCB panelization

Setup

Ensure KiKit is installed with kikit --version

Check this installations resources/panelizePresets/default.json and panelize_ui_sections.py before adding parameters, these are the way, the truth, and the light.

Usage

  • Find the source .kicad_pcb requsted by the user
  • Inspect its actual board files, Edge.Cuts, copper layers, pads and components that may interesect board edges to identify items like castellations, edge connectors, antennas, plated edges, etc.
  • Resolve grid dimensions, spacing, rotation, tabs, separation, frame, and fabricator limits.
  • Position tooling holes and fiducials relative to the panel outline
  • Write strict json.
  • Generate a versioned panel without overwriting the source in a "build" subdirectory
  • Check the generated panel before notifying the user, ensuring that it looks proper from the baord file level as well as in render.

Preferred starting values

  • Board routing gap: 2mm
  • Tab width: 3mm
  • Mouse-bite drill: 0.5mm
  • Mouse-bite spacing: 0.8mm
  • Mouse-bite offset: 0mm
  • Full frame width: 5mm
  • Frame-to-array clearance: 2mm
  • Frame break cuts: none
  • Exterior frame radius: 2mm
  • Interior routing radius: 0.25mm
  • Tooling: three 1.5mm holes
  • Tooling stencil apertures: enabled
  • Fiducials: three, 1mm copper with 1mm openings
  • Fiducial paste apertures: disabled

KiKit behavior

  • source.type: "auto" is appropriate for an ordinary single-board file.

  • tabs.type: "spacing" places tabs symmetrically and cannot exclude a particular side.

  • With fixed tabs:

    • hcount controls tabs projecting from left/right edges.
    • vcount controls tabs projecting from top/bottom edges.
    • A zero count suppresses that pair of directions.

  • Use annotation tabs when only selected segments or one side must be excluded.

  • Protected tab directions must be derived from each board’s geometry and rotation. Never hardcode “bottom” or “right” as a universal rule.

  • The global mouse-bite cut method processes every generated cut path, including framing.cuts.

  • Therefore, framing.cuts: "both" with mouse bites drills break rows through the rails.

  • Use framing.cuts: "none" for a continuous frame.

  • Tooling and fiducial offsets are measured inward from the panel’s outer edges.

  • To center a feature across a 5 mm frame, use a 2.5 mm perpendicular offset.

  • Tooling holes and fiducials with identical counts and offsets overlap. Separate them along the rail.

  • paste: true means the feature gets an aperture on the stencil paste layers. It does not control whether a drilled hole is visible.

  • framing.fillet rounds exterior panel corners.

  • post.millradius rounds concave interior routed corners.

  • post.reconstructarcs: true produces real Edge.Cuts arcs instead of dense line-segment approximations.

Useful commands

python3 -m json.tool panelize.json kikit panelize -p panelize.json input.kicad_pcb output-panel.kicad_pcb

Dump the fully merged KiKit configuration with:

kikit panelize -p panelize.json -d resolved.json input.kicad_pcb output-panel.kicad_pcb

Render and open it with:

kicad-cli pcb render
--output panel-top.png
--width 1600
--height 1200
--side top
--background opaque
--quality high
panel.kicad_pcb

kicad-cli pcb render
--output panel-iso.png
--width 1600
--height 1200
--perspective
--rotate 325,0,35
panel.kicad_pcb

Comments

Markdown supported