PCB panelization using V-cut and tab routing is the standard technique for assembling multiple boards in a single manufacturing panel, significantly reducing per-unit fabrication costs and enabling efficient automated assembly. Whether you’re manufacturing 50 sensor modules or 500 IoT nodes, panelisation is essential knowledge for any Indian electronics startup or serious maker looking to scale from prototypes to production. This guide explains V-scoring, tab routing (mouse bites), breakout strategies, and how to set up panels using KiCad or EasyEDA.
Table of Contents
- Why Panelize PCBs?
- V-Cut (V-Score) Panelization
- Tab Routing and Mouse Bites
- Panel Rails and Fiducial Marks
- Panelization Software and Tools
- Ordering Panelized PCBs from Indian and Chinese Fabs
- Panel Design Tips for Stress and Quality
- Frequently Asked Questions
Why Panelize PCBs?
PCB fabrication and assembly costs are calculated per panel, not per board. A 250 mm × 250 mm panel can hold multiple copies of a small board, spreading the fixed setup cost across more units:
- A 30 mm × 50 mm board = approximately 20 boards per panel (with rails)
- Cost of single panel at JLCPCB: ~₹400 (5 panels minimum order)
- Cost per board: ₹20 vs ₹80 if ordered as individual boards
Beyond cost, panelisation also enables automated pick-and-place assembly (SMT line) which requires a minimum panel size of typically 100 mm × 100 mm, and makes hand soldering of small boards much easier by providing a handle (the panel frame) to hold during soldering.
V-Cut (V-Score) Panelization
V-cut panelization uses a scoring blade to cut a V-shaped groove partway through the PCB along the board separation lines. The boards snap apart cleanly along these pre-scored lines after assembly.
V-Cut Characteristics
- The blade cuts through approximately 1/3 of the board thickness from each side, leaving roughly 1/3 intact in the middle
- Standard V-cut angle: 30° or 45° included angle
- Minimum remaining web thickness: 0.4–0.6 mm (for 1.6 mm FR4)
- Boards snap apart with light finger pressure or a V-cut depanelling tool
V-Cut Design Rules
- V-cuts must be straight lines running fully across the panel — the scoring blade cannot stop partway. This means V-cuts cannot be used for non-rectangular boards.
- Minimum component clearance from V-cut line: 0.5 mm (components closer than this may be stressed or damaged during snap-off)
- No traces should cross a V-cut line — any trace in the cut area will be severed
- Copper pours should not extend within 0.3 mm of the V-cut centreline
Specifying V-Cut in Gerber Files
Mark V-cut lines on a dedicated fabrication layer in your EDA tool:
# KiCad: V-Cut lines
# Draw lines on User.1 or Eco1.User layer
# Label them "V-SCORE" or "V-CUT" in fab notes
# Include a fab note: "V-Score along all dashed lines,
# 1/3 depth from each side, 30-degree angle"
# In your Gerber file README/fab notes:
# Panel separation: V-Score
# V-Score angle: 30 degrees
# Remaining web: 0.5mm minTab Routing and Mouse Bites
Tab routing (also called breakaway tabs or mouse bites) uses actual router cuts to isolate board outlines, leaving only small connecting tabs that are manually broken or cut after assembly. This method works for any board shape, including non-rectangular boards.
Types of Tabs
Solid Tabs
A small solid strip of PCB material connecting the board to the panel. Width typically 2–5 mm, at least 2–3 tabs per board side. Boards are separated by scoring with a knife, cutting with flush cutters, or routing off in a fixture. Leaves a slightly rough edge that may need filing.
Mouse Bite Tabs (Perforated Tabs)
A row of closely spaced drill holes (“mouse bites”) along the separation line, creating a perforation that breaks cleanly under gentle pressure or a bending motion. Mouse bite holes are typically 0.5–0.8 mm diameter, spaced 0.5–0.8 mm apart, leaving only thin webs between holes.
Mouse bite pattern for a 5mm tab:
o o o o o o o
↑ ↑
0.5mm holes at 0.5mm spacing
Total tab: 5 holes = ~3.5mm effective tab width
Snap force: low, clean break lineTab Routing Design Rules
- Minimum tab width (solid): 2 mm
- Maximum tab width (solid): 5 mm — wider tabs are harder to break cleanly
- Minimum clearance from tab to component: 1.5 mm (mouse bites) or 2.5 mm (solid tabs) to avoid PCB flexing stressing solder joints during separation
- Minimum 2 tabs per board edge for stability during assembly
- Place tabs in board areas with no sensitive components below (avoid BGAs, crystal oscillators near tabs)
Panel Rails and Fiducial Marks
Panel Rails
Panel rails are border strips (typically 5–10 mm wide) added around the array of boards. They provide:
- A clamping surface for SMT pick-and-place and reflow conveyors
- Space for fiducial markers (alignment marks for pick-and-place vision systems)
- Tooling holes for fixture pins (typically 3.2 mm diameter, minimum 4 per panel)
- Panel information text (revision, date, part number)
Fiducial Marks
Fiducials are small circular copper pads (1–3 mm diameter) with a clear solder-mask-free courtyard around them, used by pick-and-place machines to optically align the panel. Place fiducials on:
- At least 3 panel-level fiducials (corners of the panel rail, not in a symmetrical pattern)
- Optionally: individual board-level fiducials for fine component placement (fine-pitch ICs, BGAs)
# Fiducial standard specifications:
Copper pad: 1.0mm diameter circle
Solder mask clearance: 2.5mm diameter (full copper exposed)
Layer: Top copper + no solder mask over fiducial
Location: Min 5mm from panel edge, 3 per panel minimum
Placement: Not symmetric (allows 180° rotation detection)Panelization Software and Tools
KiKit (Open Source, Recommended)
KiKit is a KiCad plugin for automated panelisation. Install via KiCad’s Plugin Manager or pip:
# Install KiKit
pip install kikit
# Basic panel: 3x4 array of boards with mouse bites
kikit panelize
--layout 'grid; rows: 3; cols: 4; space: 2mm'
--tabs 'annotation'
--cuts 'mousebites; drill: 0.5mm; spacing: 0.8mm'
--framing 'railstb; width: 5mm'
--fiducials 'auto'
my_board.kicad_pcb my_panel.kicad_pcbEasyEDA Panelization
EasyEDA Pro has a built-in Panelize tool under Tools > Panelize. Set array size, spacing, and V-cut or tab options. This is the easiest option for Indian makers using EasyEDA for design.
GerbMerge (Legacy, Free)
An older Python-based tool for merging Gerber files into a panel. Works but lacks mouse-bite support. Suitable for simple rectangular-board arrays.
Ordering Panelized PCBs from Indian and Chinese Fabs
JLCPCB
The most popular option for Indian makers. JLCPCB accepts panel Gerbers and handles V-score and routing internally. Key parameters to set:
- “PCB Assembly” order for assembled panels
- Breakaway rail: specify rail width if using rails
- Edge rail removal by fab: specify if they should remove rails after assembly
- Cost: ~₹400–600 per panel (5 pcs minimum), plus ₹600–1,200 shipping to India (DHL, 5–10 days)
PCBWay
Offers full panelization services including custom panel layouts. Good for larger orders (100+ panels). Also ships to India with similar delivery times to JLCPCB.
Indian Fabs (PCBPower, Sriya PCB)
Local Indian fabs can produce panelised boards, typically with 7–14 day turnaround. Pricing is higher per panel than Chinese fabs for small quantities but avoids import duty and delivery risk. Useful for production runs where delivery reliability is critical.
Panel Design Tips for Stress and Quality
Board Orientation in Panel
Orient boards so that the longest edges are parallel to the panel travel direction through the pick-and-place conveyor. This minimises board flex and maintains registration accuracy during high-speed component placement.
Stress-Sensitive Components Near Edges
Ceramic capacitors (especially large MLCC values above 10 µF) are brittle and crack easily under PCB bending stress during panel separation. Keep capacitors ≥3 mm away from any V-cut or tab routing line.
Thermal Symmetry
For reflow soldering, the copper distribution should be roughly symmetric across the panel to ensure even heating. Avoid placing all large copper pours on one side of the panel — this causes thermal gradients during reflow and can lead to tombstoning or cold joints.
Frequently Asked Questions
Should I use V-cut or tab routing for my panel?
Use V-cut for rectangular boards where cost is paramount — V-cutting is cheaper than routing. Use tab routing (mouse bites) for non-rectangular boards (L-shaped, circular, irregular) or when you need no board-edge stress during assembly. Many professional designs combine both: V-cuts for long straight edges, tabs for corners and non-linear features.
What panel size should I design for?
For JLCPCB and most fabs, the maximum standard panel size is 250 mm × 250 mm. Standard SMT line conveyor widths accept panels from 50 mm to 300 mm wide. For initial prototypes or hobbyist use, target a 100 mm × 100 mm panel (the cheapest tier at most fabs) and fit as many boards as possible in that area.
Do I need fiducials for hand-soldering only boards?
No. Fiducials are only needed if your boards will be assembled on a pick-and-place machine. For hand-soldering, you can skip fiducials to save space and simplify the panel design.
What is the minimum spacing between boards in a panel?
For V-cut only: boards can be 0 mm apart (the V-cut line is the separation). For tab routing: minimum 2 mm between board outlines to accommodate the routing tool diameter (typically 1.6–2.0 mm bit). For mouse bites, 1.5–2 mm spacing is typical.
Can I mix different board designs in one panel?
Yes — called a “mixed panel” or “combo panel.” This is common for prototyping multiple related boards (e.g., a mainboard + power supply module + display driver). Fabs like JLCPCB charge the same as a single design panel for Gerbers, but SMT assembly quotes require separate work for each design. Specify clearly in fab notes that it’s a mixed panel.
Add comment