When a printed circuit board layout is complete, translating the CAD database into a manufacturing release package is notoriously error-prone. An engineer must:

  1. Plot Gerbers across all copper, mask, silk, and paste layers.
  2. Generate Excellon drill files.
  3. Export pick-and-place component centroid CSVs.
  4. Export a STEP 3D model for mechanical enclosure clearance checks.
  5. Print multi-sheet schematic PDFs and assembly drawings.
  6. Generate a Bill of Materials (BOM).
  7. Take high-resolution 3D beauty renders for assembly technicians.

If any single export option is misconfigured (e.g., wrong drill units, forgotten bottom silk, or un-mirrored bottom assembly view), fabrication gets delayed or assembled boards arrive with rotated components.

To make this process foolproof and instant, we built Generate Release Package, a native KiCad 9 Action Plugin that compiles a complete, fab-ready release folder in one click.

1. Zero-Risk Architecture: kicad-cli vs pcbnew API

A major hazard of traditional PCB CAD plugins is that scripts interacting directly with the running application memory (pcbnew.BOARD) can corrupt open layouts or trigger undo-history crashes if an unhandled exception occurs.

Generate Release Package adopts a zero-risk architecture:

[ Active KiCad Layout Session ]
             │
      (Prompt to Save)
             │
             ▼
[ Saved .kicad_pcb / .kicad_sch on Disk ]
             │
             ▼
 Python Plugin shells out to bundled `kicad-cli`
             │
             ├─► kicad-cli pcb export gerbers ...
             ├─► kicad-cli pcb export drill ...
             ├─► kicad-cli pcb export pos ...
             ├─► kicad-cli pcb export pdf (Assembly Top/Bottom) ...
             ├─► kicad-cli pcb export step ...
             ├─► kicad-cli sch export pdf ...
             └─► kicad-cli sch export bom ...
             │
             ▼
[ Release Files_<Project>_<DDMMYYYY>/ ] (Opened in Explorer)

Because all export tasks are performed by kicad-cli (the standalone command-line binary bundled with KiCad 9), the live board is never modified, memory is isolated, and exports run at compiled C++ speed.

2. Standardized Output Directory Structure

The plugin bundles every asset required by fabrication and assembly facilities into a self-documenting directory:

Release Files_<Project>_<DDMMYYYY>/
├── Board_Information.CSV            # Board dimensions, layer count, pad count
├── Assembly_Files/
│   ├── Assembly Drawings.PDF        # 3-page PDF: Overview + Top + Bottom views
│   ├── Top PCB 3D Print.png         # 3000x2400 high-res top render
│   └── Bottom PCB 3D Print.png      # 3000x2400 high-res bottom render
├── Bill Of Materials/
│   └── <Project>_BOM.CSV            # Clean CSV (Refs, Value, Footprint, MPN)
├── Fabrication_Files/
│   ├── Gerbers/                     # Standard RS-274X copper, mask, silk layers
│   └── Drill/                       # Plated & non-plated Excellon drill files
├── Mechanical_3D/
│   └── <Project>.STEP               # Unified AP214/AP242 STEP assembly
├── Pick and Place/
│   └── <Project>_all_pos.csv        # SMT machine centroid data (X, Y, Rotation)
└── Schematics/
    └── <Project>_Schematic.PDF      # Full vector schematic document

3. The 3-Page Assembly Drawing PDF

Assembly technicians need clear graphical component references. The plugin automatically synthesizes a 3-page vector assembly drawing formatted with clean title blocks:

  • Page 1 (Overview & Mechanical Specs): Side-by-side Top and Bottom previews, board dimensions ($X \times Y$), overall thickness, copper weight, surface finish, and primary component counts.
  • Page 2 (ASSEMBLY TOP): Vector drawing of top silkscreen, pads, and component reference designators (R1, C1, U1), with non-populated parts crossed out.
  • Page 3 (ASSEMBLY BOTTOM): Mirrored vector view of the bottom layer for effortless benchtop inspection.
def generate_assembly_pdf(board_path, output_pdf):
    """Executes kicad-cli pcb export pdf with assembly layer presets."""
    cmd = [
        "kicad-cli", "pcb", "export", "pdf",
        "--layers", "F.Fab,F.CrtYd,Edge.Cuts",
        "--black-and-white",
        "--include-border-title",
        "-o", output_pdf,
        board_path
    ]
    subprocess.run(cmd, check=True)

4. Selective Export GUI

Engineers don’t always need every output during mid-layout reviews. The plugin opens a lightweight wxWidgets dialog:

  • Independent checkboxes for Gerbers, Drill, Centroids, Assembly PDF, 3D Renders, STEP, BOM, and Schematic.
  • Select All and Deselect All hotkeys.
  • Destination folder picker (defaults to project directory or desktop).

When execution finishes, the plugin calculates board statistics (total SMT pads, through-holes, and dimensions) into Board_Information.CSV and automatically opens the output directory in Windows File Explorer via os.startfile.

The result: a release package that used to take 45 minutes of repetitive clicking is generated in under 15 seconds with zero human error.