Panelization means grouping several copies of a board (or several different boards) into one larger sheet so they can be manufactured and assembled together, then separated afterward. If you have never done it, the good news is you often do not need to — but knowing when and how pays off fast.
Short answer: For most prototypes, let the fab panelize for you. Panelize yourself when you need control over spacing, rails, and fiducials, or when your boards are small enough that fab minimums make a panel far cheaper. KiCad has no built-in panelizer, but the open-source KiKit plugin does the job well and exports a standard panel you can fabricate.
What panelization is and why you would do it
A panel is a single manufacturing unit holding multiple board copies with rails and separation features around them. Three reasons it matters:
- Assembly efficiency. Pick-and-place machines and reflow ovens work on a panel, not a loose 20 mm board. A panel gives the assembler rails to grip, tooling holes to register, and fiducials to align. Many assembly houses will not accept individual small boards at all.
- Small boards. If your board is tiny, a panel lets you get dozens of copies per fabrication unit. Since fabs price largely by area and count, this can slash per-board cost.
- Fab minimums. Board houses have minimum dimensions and minimum order quantities. A 15 mm square board may be below the minimum size a fab will run alone; drop it into a panel with a rail and it clears the threshold.
If you are chasing lower unit cost, panelization pairs well with the other levers in reducing PCB manufacturing cost.
Tab-routing vs V-scoring
There are two dominant ways to hold boards in a panel and separate them later.
Tab-routing (also called tab-and-slot) mills a slot around each board outline and leaves a few narrow tabs connecting it to the panel or its neighbors. It works with any board shape — rounded corners, cutouts, irregular outlines — because the router follows the outline. The tabs usually carry mouse bites so the board snaps out by hand.
V-scoring cuts a shallow V-shaped groove on the top and bottom of the panel along straight lines, leaving a thin web of material. Boards snap apart along the score. It is cheap and fast, but only works when boards are rectangular and butt directly against each other in a grid, with no gap.
| Tab-routing | V-scoring | |
|---|---|---|
| Board shapes | Any outline, cutouts, curves | Rectangular only, edge to edge |
| Spacing | Needs a routed gap (~2 mm) | Zero gap, tighter packing |
| Edge quality | Small bumps from mouse bites | Clean straight edge, may need sanding |
| Component overhang | Parts can overhang the gap | No overhang across the score line |
| Cost | Slightly higher (routing time) | Cheapest option |
| Depanelization | Snap or cut tabs by hand | Snap or run through a scoring machine |
A common real-world approach is to mix them: V-score the straight edges between boards, tab-route the connection to the rails.
Mouse bites
A mouse bite is a row of small closely spaced drill holes across a tab. They perforate the tab so it breaks cleanly and predictably by hand, instead of tearing unevenly. After depanelization you are left with a small perforated edge you can sand flush.
Practical guidance: keep mouse bites a millimeter or two back from the true board edge so the leftover nub does not protrude past your outline, and keep them away from board-edge connectors, mounting holes, and any components sensitive to mechanical stress. Too few tabs and a large board flexes and cracks in handling; too many and it is a fight to break out.
Fiducials and tooling
If your panel is going to a pick-and-place line, it needs alignment and handling features:
- Global fiducials. At least three fiducials on the panel rails, placed asymmetrically so orientation is unambiguous. These let the machine locate the whole array.
- Local fiducials. For fine-pitch parts (QFN, BGA, 0402 and smaller), add local fiducials near those footprints so the machine corrects for small placement offsets.
- Tooling / mounting holes. Non-plated holes in the rails let the assembler pin the panel down.
- Rails. A 5–10 mm border on two edges carries the fiducials and tooling holes and gives the conveyor something to grip.
Getting fiducials and courtyards right on the panel is part of the same discipline as designing for assembly on the individual board.
When to let the fab panelize vs doing it yourself
Let the fab do it when: you are prototyping, ordering a modest quantity, or your assembler mandates their own panel format (many do). You upload your single-board Gerbers and specify the array size, rail width, and separation method in the order form. It is less work and avoids format mismatches, and the fab knows their own tooling.
Panelize yourself when: you need exact control — specific tab positions to avoid connectors, a particular fiducial layout, mixed V-score and tab-routing, or a multi-design panel combining different boards. Self-panelizing also gives you a fabricated panel file you can inspect and version like any other design output.
A good rule: prototype with the fab's panelization, switch to a controlled self-made panel once the design is stable and heading to volume.
Doing it yourself with KiKit
KiCad does not ship a panelizer, but KiKit is a mature open-source plugin and command-line tool that panelizes .kicad_pcb files directly. It runs as a KiCad action plugin (GUI) or from the command line, and it produces a standard KiCad panel board plus the separation features.
Conceptually, a grid panel from the command line looks like this:
kikit panelize grid \
--grid-cols 3 --grid-rows 2 \
--space 2mm \
--tabs 4 --mousebites 0.5mm 0.9mm 0.2mm \
--railsTb 5mm \
--fiducials 3 \
board.kicad_pcb panel.kicad_pcb
That asks for a 3×2 array, 2 mm spacing, four tabs per board with mouse bites, top and bottom rails, and fiducials. KiKit also supports V-scoring, framing options, and multi-board panels, and the resulting panel.kicad_pcb opens in KiCad's PCB editor so you can review it before sending it out. Because the output is a real board file, you export its Gerbers the same way you would any board.
Where GoForFab fits
Whether you panelize yourself or hand a single board to your fab, every panel starts from a clean, current single-board output set — Gerbers, drill files, BOM, and pick-and-place — that actually matches your latest design. That is the tedious, error-prone part: regenerating those files by hand every revision and hoping they are in sync.
GoForFab handles it with kicad-cli: connect a KiCad project and every push regenerates the full manufacturing package automatically, so the board you drop into a panel is always the real one. It is free forever to get started — give it a try and let the outputs take care of themselves.