PCB Edge Clearance and Routing Keepout Rules
Every board has an edge, and almost every manufacturing step treats that edge as a boundary that copper, components and tooling must respect. Edge clearance is the distance held between the outermost copper and the physical outline of the board, while the routing keepout is the zone inside that outline where nothing may be placed because the router bit, the scoring wheel or the depaneling tool needs the space. Getting these two numbers wrong is a common source of scrapped panels, chipped laminate and short circuits found only after assembly. This guide sets out the rules and how to record them.
How Much Copper to Edge Do You Need
The usual figure for copper to edge spacing on an outer layer is 0.25 mm on a routed edge, and well controlled shops will accept 0.20 mm when the laminate is thin and the cutting tool is fresh. That allowance is not there for electrical reasons alone. The router leaves a small burr and a slightly ragged resin edge, and the plating and etching steps remove material at different rates near an open boundary, so copper placed flush with the cut risks exposed burrs that touch a chassis or a neighbouring board.
Inner layers deserve more margin, not less. A plane that reaches the edge is only a few tenths of a millimetre from the cut surface, and delamination during routing can expose it. Accepted practice is to pull inner copper back 0.40 mm or more from a routed edge and to keep plane pullback at least as large as the outer layer value. Where the board will be handled repeatedly or shipped in a conductive carrier, extra margin is cheap insurance.
Why the Router Needs Its Own Keepout
A routing keepout exists because the tool has width. A 2.0 mm router bit cuts a slot 2.0 mm wide and will take 2.4 mm or more when the tool wanders on a long cut, so components, vias and copper should stay clear of a band that extends roughly 1.2 mm inside the outline. Solder mask openings that reach into this band can be smeared by cutting debris, and test points placed here are unreliable because the probe lands on a surface that has been mechanically disturbed.
Scoring tools impose a similar constraint. A V-score removes material along a straight line and leaves a weakened shoulder on each side, so the same band has to stay free of anything that could be damaged by the blade or stressed by the break. On dense designs this is why a designer cannot simply fill the last millimetre of the board with copper. The space is committed to the manufacturing operation, not wasted.
<img src="https://www.gopcba.com/wp-content/uploads/2026/09/127-1.jpg" alt="Board outline with copper pour pulled back from a routed edge” />
Panel Rails and Breakaway Tabs
A panel rail is the strip of laminate used to carry the board through assembly equipment, and it is also what the fabricator grips while routing. Five millimetres is the practical minimum width, and eight to ten millimetres suits most SMT lines because the conveyor and the clamp need something substantial to hold. Copper placed in the rail is scrapped with the rail, so it should be avoided unless the rail is being used deliberately as a test coupon.
Tabs connect the rail to the board and carry the whole panel through reflow, which makes their number and position a mechanical decision as much as a layout one. The range of tab geometries and the reason each is chosen is covered in our note on breakaway tab design, which also explains why a tab placed under a heavy connector so often fails during depaneling.
V-Score Lines and Their Clearance
Where the edge is a straight line and the board is rectangular, scoring is faster and cheaper than routing. The score cuts a V groove into both faces, leaving a web of laminate that is snapped after assembly. Each groove is roughly a third of the board thickness deep on a 1.6 mm board, and the scoring wheel leaves a shoulder about 0.4 mm wide that cannot carry components or fine traces.
The practical clearance from a score line to the nearest copper is 0.50 mm on each side, and to the nearest component body 0.80 mm. That second number matters because the break releases energy along the line and a part sitting too close can be cracked or lifted. Boards that combine scored and routed edges need both clearance rules applied to the appropriate segment rather than one value applied everywhere.
Castellations and Half-Hole Edges
Modules that solder onto a carrier often use castellations, which are plated half holes on the board edge. Here the copper deliberately reaches the boundary, so the ordinary clearance rule is suspended and replaced by a specific fabrication instruction. The hole is drilled, plated and then cut lengthwise, so the plated surface has to survive the router without tearing or lifting from the barrel wall.
Castellated edges need a wider keepout around them for the same reason. The tool must approach the plated barrel cleanly, and adjacent traces cannot sit within the space the cutter sweeps. It is normal to reserve a band around the castellated zone and to route each module as a separate panel feature rather than nesting them tightly against one another.
Keepouts Around Connectors and Mounting Holes
Mounting holes have their own keepout that is not about the router at all. A screw head, a washer or a standoff occupies a disc of perhaps 6 mm around the hole, and copper, vias and components inside that disc risk being crushed or shorted when the hardware is fitted. The rule is to keep metal parts clear by at least the radius of the washer, and to keep solder mask intact beneath the hardware so a stray strand cannot bridge two nets.
Connectors introduce a different problem because the mating action is mechanical. A plug that is inserted and removed thousands of times transmits force into the laminate, so the copper and solder mask behind the connector body should be free of anything fragile. Edge clearance applies here too: the connector body usually has to overhang the edge, and the copper behind it must still respect the routing band.
Assembly and Handling Effects
Clearance rules are usually justified by fabrication, but assembly is where they are tested. A board with zero margin at the edge tends to chip during depaneling, and a chipped edge can lift a solder mask shelf that was supporting a fine trace. The damage is often invisible on the top side and appears as an intermittent open when the board flexes inside the enclosure.
Automatic optical inspection also depends on the edge. The camera needs a consistent, clean background to identify the outline and align its coordinate system; a ragged or copper-flooded edge forces the programmer to work with a weaker reference. Boards that hold proper clearance inspect faster and report fewer false calls.
Documenting Edge Rules in the Fabrication Note
None of this works unless the numbers reach the supplier. The fabrication drawing should state the outline tolerance, the maximum burr and the smallest copper to edge distance the design assumes. Our note on board outline tolerance rules explains how those tolerances are measured, and the wider checklist in PCB fabrication notes shows where each item belongs.
When a design is unusual the note is also where the designer states intent rather than dictating the process. Supplying the function of the board and the assembly method lets the shop propose a route that fits, and the gopcb engineering team can confirm what the tooling will really achieve before the panel is released.
FAQ
Is 0.20 mm edge clearance acceptable? On a routed edge with thin laminate and a controlled router it is workable, but it leaves no margin for tool wear. Designs expected to run for years should assume 0.25 mm as a minimum and treat anything smaller as a special case agreed with the fabricator.
Does the keepout change for a laser cut edge? Yes. A laser leaves a heat affected zone that can be a few tenths of a millimetre wide, so the clearance has to cover carbonised resin as well as mechanical damage. The value depends on material and thickness and should come from the supplier.
Can a panel rail carry test coupons? It can, and it is a good use of the material. A coupon strip in the rail gives plated through hole and surface finish data from the same panel that carries the product, which is far more representative than a separate test vehicle.
