The design of PCB routes and reference points establishes the physical basis for signal flow, component placement, and assembly alignment. Clear routing rules and a consistent datum scheme help designers connect layout intent with fabrication and inspection requirements.
Highlights:
- Routing requirements define controlled trace paths and reference relationships that support signal integrity and manufacturability.
- Reference points and datum features must be defined consistently for placement, inspection, and assembly alignment.
- Design rules should align layout intent with fabrication and assembly constraints.
PCB Routing, Mounting Hole, and Fiducial Requirements
Routing Requirements
Routing rules on a printed circuit board are not only about connectivity. A large share of them define where copper is permitted to exist relative to the mechanical features of the board: the outline, the V-cut lines, the milled slots, the heatsink, the metal handle, and every screw or rivet that passes through the panel. These constraints address two distinct classes of failure.
The first class is a fabrication defect. Copper that sits too close to a board edge can be exposed by the machining operation itself, leaving bare metal at the cut, inviting solder bridging, oxidation, or a short to a chassis part. The second class is an assembly and safety problem. Copper that runs beneath a metal component, a fastener head, or a washer can lose its insulation distance once the hardware is installed, because the installed position of that hardware is never exactly the nominal position. Every rule in this section is therefore a geometric keep-out that should be encoded in the CAD library and checked before the design is released, rather than a note applied informally at the end of layout.
Trace-to-Board-Edge Distance
To prevent copper exposure during PCB fabrication, all traces and copper areas must maintain a defined distance from the board edge. For a V-cut edge, that distance must be greater than 0.75mm. For a milled (routed) edge, the distance must be greater than 0.3mm. The copper-to-edge distance must also satisfy the mechanical installation requirements of the final product, so these two values are fabrication minimums, not a complete specification of the edge clearance.
The difference between the two numbers follows directly from how the two edges are produced. A V-cut is a scoring operation: a V-shaped blade is pressed into the panel, removing a wedge of material and leaving a controlled fracture line so the boards can be snapped apart later. The material adjacent to the score is deformed, and the separation step leaves a rougher, less predictable edge than a milled contour. Copper that lies within that disturbed zone can be smeared across the fracture surface or exposed when the board is depanelized. A routed edge is cut by a milling bit that removes material cleanly along the programmed contour, so the copper can safely sit closer to the finished outline.
In practice, the rule has to be implemented as a design-rule check that is aware of the edge type. A single global "copper to outline" value will either be too loose for the routed edges, wasting routing area, or too tight for the V-cut edges, allowing exposed copper. Where a panel contains both edge types, the V-cut segments should be identified separately so the stricter clearance applies only along the scored lines.
No Routing Beneath the Heatsink Face (or Insulation Applied)
For electrical insulation, no traces should run beneath and around the heatsink. This accounts for the positional tolerance of the installed heatsink and for the required safety distance between conductors. If routing beneath the heatsink cannot be avoided, insulation measures must be taken to isolate the traces from the heatsink, or the design must confirm that the traces and the heatsink sit at the same potential.
The failure mode this rule prevents is a loss of insulation clearance after assembly. A heatsink is a large metal body, and its mounting position depends on screw clearance, thermal-interface thickness, and the tolerances of the parts it presses against. Copper that is nominally clear of the heatsink can still end up underneath an edge of it once the hardware is installed. Because the heatsink usually covers a broad area, a single contact point can short several nets at once, and the resulting damage is difficult to localize. Where a keep-out cannot be honored, a dielectric interface material or a conformal coating provides the isolation, and the equal-potential alternative must be verified net by net rather than assumed.
No Routing Beneath the Metal Ejector Handle
For the same reason, no traces should run beneath a metal ejector handle or lever. These parts are handled during insertion and extraction, so they can be touched, flexed, and displaced relative to the board. Keeping copper out from under them preserves the insulation distance and removes any path by which a conductive part could bridge two nets during handling or service.
Keep-Out Zone Requirements for Screw Holes
Each screw specification has a corresponding circular keep-out zone, listed in Table 5. This keep-out applies to the installation space needed to guarantee electrical insulation. It does not account for safety distance, and it applies only to round holes.
| Connection type | Model | Specification | Mounting hole (mm) | Keep-out zone (mm) |
|---|---|---|---|---|
| Screw connection | GB9074.4-8 combination screw | M2 | 2.4±0.1 | φ7.1 |
| M2.5 | 2.9±0.1 | φ7.6 | ||
| M3 | 3.4±0.1 | φ8.6 | ||
| M4 | 4.5±0.1 | φ10.6 | ||
| M5 | 5.5±0.1 | φ12 | ||
| Rivet connection | Chobert quick rivet | 4 | 4.1 +0.2/0 | φ7.6 |
| Avtronic quick rivet | 1189-2812 | 2.8 +0.2/0 | φ6 | |
| 1189-2512 | 2.5 +0/-0.2 | φ6 | ||
| Self-tapping screw connection | GB9074.18-88 cross pan head self-tapping screw | ST2.2* | 2.4±0.1 | φ7.6 |
| ST2.9 | 3.1±0.1 | φ7.6 | ||
| ST3.5 | 3.7±0.1 | φ9.6 | ||
| ST4.2 | 4.5±0.1 | φ10.6 | ||
| ST4.8 | 5.1±0.1 | φ12 | ||
| ST2.6* | 2.8±0.1 | φ7.6 |
The keep-out diameter in the table is governed by the hardware that contacts the board, not by the hole itself. The head of a combination screw, the flange of a quick rivet, and the head of a self-tapping screw each occupy a footprint considerably larger than the drilled hole, and that footprint is what the copper must clear. The tolerance on the mounting hole is equally important: it defines how far the installed hardware can shift before it is tightened, and the keep-out has to remain valid across that shift.
For components that carry mounting holes within their own body, such as the rivet holes and screw mounting holes of a connector, the same logic applies. The keep-out zone must be drawn clearly in the component library, so that the constraint travels with the part instead of depending on the memory of the person doing the layout. Components placed early in the design then automatically reserve the space they need, and the copper pour, the plane splits, and the trace routing all respect it without further intervention.
Teardrops at Isolated Pads and Trace Junctions
The width of the connection between an isolated pad and its trace should be increased, forming a teardrop. This is particularly important for pads on single-sided boards, where the pad can otherwise be pulled off the substrate during wave soldering.
A teardrop works by removing the stress concentration at the point where a narrow trace meets a wide pad. That junction is the natural initiation site for a crack: the trace is the only mechanical anchor of the pad, and the thermal shock of wave soldering places the joint under stress while the laminate is still expanding. On a double-sided board the plated barrel of the through hole helps hold the pad in place. On a single-sided board there is no barrel and no copper on the far side, so adhesion to the substrate is the only thing keeping the pad attached, which makes the teardrop a functional requirement rather than a cosmetic refinement.
The same reinforcement is useful at the junction of a trace and a plane or a wide conductor, where a sudden change in width creates an abrupt thermal mass difference. During soldering and during thermal cycling, that discontinuity is where the copper is most likely to lift or crack.
Oblong and slotted holes need their own keep-out definition, given in Table 6. The keep-out width matches the value for the equivalent round hole, while the length grows with the slot length L, so the reserved area always extends past the ends of the slot.
| Connection type | Model | Specification | Mounting hole diameter (width) D, mm | Mounting hole length L, mm | Keep-out zone (mm) L×D |
|---|---|---|---|---|---|
| Screw connection | GB9074.48 combination screw | M2 | 2.4±0.1 | Determined by actual conditions | φ7.6×(L+4.7) |
| M2.5 | 2.9±0.1 | φ7.6×(L+4.7) | |||
| M3 | 3.4±0.1 | φ8.6×(L+5.2) | |||
| M4 | 4.5±0.1 | φ10.6×(L+6.1) | |||
| M5 | 5.5±0.1 | φ12×(L+6.5) |
Because a slotted hole allows the board to move relative to the fastener, the keep-out has to cover the full range of that movement, which is why the length term appears in the expression. The slot length is set by the mechanical design, and the keep-out is then derived from it, so any later change to the slot length automatically changes the reserved copper area.
Fixed Hole, Mounting Hole, and Via Requirements
Holes that are often treated as simple mechanical features, and vias that are often treated as pure electrical features, both need explicit rules. The mechanical holes interact with soldering and with the hardware that passes through them, and the vias interact with the solder joint and with the routing density around fine-pitch packages.
Non-Plated Mounting and Locating Holes on Wave-Soldered Boards
For boards that pass through wave soldering, mounting holes and locating holes that require grounding on both sides should be defined as NPTH holes. A plated hole acts as a capillary during the wave: solder travels up the barrel and can fill or partially fill the hole, which obstructs the screw or locating pin, creates an uneven seating surface, and leaves an uncontrolled solder mass on the assembly. Defining the hole as non-plated removes that path entirely and keeps the mechanical function of the hole independent of the soldering process.
Via Diameter Beneath a BGA
The vias beneath a BGA must have a diameter of 12mil. The space under a ball grid array is governed by the ball pitch, and the available channel between adjacent pads determines how large a via can be placed and still be escaped. Setting the diameter at 12mil fixes the geometry that the escape pattern is designed around, so that the fan-out, the pad clearance, and the via drill all remain consistent across the package.
Via-to-SMT-Pad Clearance
The minimum distance from the edge of an SMT pad to the edge of a via is 10mil. If the via is plugged with green solder mask, the minimum distance becomes 6mil.
The concern here is solder wicking during reflow. A via placed close to a pad gives molten solder a path away from the joint, drawn by capillary action and by the pressure of gases expanding inside the barrel. The result is a starved fillet, a joint that looks acceptable but has less solder than intended, and in the worst case an open connection. Keeping 10mil between the pad edge and the via edge leaves a solder mask dam wide enough to interrupt that path. When the via is plugged with solder mask, the barrel itself is sealed and the wicking path is closed, so the pad can be placed closer, at 6mil.
No Vias on SMT Pads
There must be no vias on the pads of SMT devices. The exception is the pad of a DPAK package used for heat dissipation, where the vias are part of the thermal path by design.
A via inside a solder pad has nowhere for the solder to go except down the barrel. The joint loses material, voids form as flux and trapped air expand, and the placement of the component can be disturbed by the resulting uneven surface. For a DPAK thermal pad, the vias serve a different purpose: they conduct heat into the copper beneath the package, so their presence is deliberate and the assembly process is adjusted around them.
Standard Via Sizes
Under normal circumstances, standard via sizes should be used. The standard sizes, with an aspect ratio of hole diameter to board thickness of 1:6 or better, are listed in Table 7.
| Inner diameter (mil) | Outer diameter (mil) |
|---|---|
| 12 | 25 |
| 16 | 30 |
| 20 | 35 |
| 24 | 40 |
| 32 | 50 |
The aspect ratio limit is what makes these sizes standard. Plating a deep, narrow hole uniformly is more difficult than plating a shallow, wide one, because the chemistry has to reach the center of the barrel and the deposited copper has to be continuous along the full length of the wall. Keeping the ratio at 1:6 or better ensures that the plating thickness remains adequate through the barrel, which in turn determines the current-carrying capability and the mechanical reliability of the via. Restricting the design to the listed combinations also keeps the drill tooling and the plated finish within the process that the fabricator has characterized, rather than requiring a special setup for every design.
Vias Beneath Flush-Mounted Components on Wave-Soldered Boards
On a board that passes through wave soldering, if a component on the component side is mounted flush against the board surface, there must be no via beneath it, or the via must be covered with solder mask. An open via under a flush-mounted body becomes a trap: solder and flux can be forced into it during the wave, and the trapped material cannot be cleaned out afterwards. Covering the via with solder mask closes the cavity, and relocating it removes the problem at the source.
Fiducial Requirements
Fiducials are the optical reference marks used by the solder paste printer and the placement machine to locate the board. Their geometry, their contrast against the surrounding laminate, and their position relative to the board edge all determine whether the vision system can find them reliably.
At Least Two Asymmetric Fiducials per PCB
A PCB carrying surface-mount devices must have at least two asymmetric fiducials at diagonal positions. Depending on where they are placed, fiducials are classified as panel fiducials, unit fiducials, and local fiducials. At least two asymmetric fiducials must be present on the board.
Two marks are the minimum needed to establish position and rotation, and the asymmetry is what makes the orientation unambiguous. If the two marks are placed symmetrically, the vision system can match the pattern with the board rotated by 180 degrees and still obtain a plausible result, which risks placing the entire panel in the wrong orientation. Placing the marks diagonally maximizes the baseline between them, so a small angular error at each mark translates into a smaller positional error across the board. Panel fiducials serve the whole panel, unit fiducials serve each individual board within it, and local fiducials serve a specific fine-pitch device whose placement accuracy demands a reference closer than the unit fiducial can provide.
Fiducial Position, Shape, Size, and Material
The center of the fiducial must be more than 5mm from the board edge, and the mark must be protected by a metal ring.
a. Shape: the preferred shape of a fiducial is a solid circle.
b. Size: the preferred fiducial size is a diameter of 40mil±1mil.
c. Material: the fiducial is made of bare copper or copper-clad laminate. To increase the contrast between the fiducial and the substrate, a large copper area may be placed beneath the mark.
The 5mm edge clearance keeps the mark away from the region where the panel is handled, clamped, and cut, so the fiducial is not damaged or obscured before it is used. The solid circular shape gives the vision system a rotationally symmetric target whose centroid can be computed reliably, independent of the viewing angle. The size tolerance matters because the algorithm typically compares the detected area against the expected area; a mark outside the tolerance band can be rejected or mis-centered. Contrast is the underlying theme of all three parameters. A bare copper mark on a copper pour has almost no contrast at all, which is why the copper beneath the mark is enlarged only where it improves the optical difference between the mark and its surroundings, not where it merges with the mark itself.
Fiducial Pad and Solder Mask Opening
The fiducial pad and the solder mask opening must be defined correctly. The solder mask opening is a circle concentric with the fiducial, with a diameter twice that of the fiducial.
At the edge of an 80mil diameter fiducial, a circular copper line is required as a protection ring. The metal protection ring has an outer diameter of 110mil, an inner diameter of 90mil, and a line width of 10mil. Unit fiducials in areas where space is too limited may be defined without the metal protection ring. For multilayer boards, copper is recommended on the inner layers beneath the fiducial to increase recognition contrast.
The 2:1 relationship between the mask opening and the copper mark is what produces a clean optical transition. If the mask opening is too small, the mask encroaches on the copper and the apparent shape of the mark becomes irregular, which shifts the calculated centroid. If the opening is much larger than required, the exposed laminate around the mark reduces the contrast that the vision system depends on. The protection ring provides a defined boundary around the mark and discourages solder from collecting at its edge during assembly. Where the unit is too small to accommodate the ring, the mark itself is retained and only the ring is omitted, because the mark is the functional element and the ring is an enhancement.
Aluminum substrates and thick copper foil, defined here as copper foil with a thickness of 3OZ or more, require a different fiducial construction, shown below. The fiducial is defined as a copper area 80mil in diameter with a solder mask opening 40mil in diameter.
Reference Point Clearance and Panel Design
No Other Traces or Silkscreen Within the Reference Point Area
The area around each fiducial mark must be kept clear of other traces and silkscreen. This clearance is required to preserve the optical contrast that the printer and placement machine use to recognize the mark. If traces or legend enter the fiducial area, the recognition window can become ambiguous, which may reduce stencil printing accuracy and component placement reliability.
Reference Points on Unit Boards in a Panel
When individual boards are panelized, each unit board should include its own fiducial marks whenever possible. If space constraints make it impossible to place fiducials on a unit board, the unit board may be produced without them, but the panel itself must still provide fiducial marks for the panelization process. This ensures that the assembly process has a reliable reference even when unit-level marks are absent.
Silkscreen Requirements
Silkscreen Labels for Components, Mounting Holes, and Locating Holes
Every component, mounting hole, and locating hole should have a corresponding silkscreen label to simplify assembly of the finished board. Mounting holes on the PCB should be marked with H1, H2, ... Hn. These labels help assemblers and inspectors identify features quickly and reduce the risk of installation errors.
Character Orientation: Left to Right and Bottom to Top
Silkscreen characters should follow a left-to-right and bottom-to-top reading direction wherever practical. For polarized devices such as electrolytic capacitors and diodes, the orientation should remain consistent within each functional unit. Consistent character and device orientation improves readability and makes manual inspection and repair more efficient.
No Silkscreen on Pads or Tinned Traces; Keep Reference Designators Visible
To maintain soldering reliability, component pads must not carry silkscreen. To preserve the continuity of traces that require tinning, silkscreen must not be placed on those tinned traces. Reference designators must not be hidden by components after assembly, because they are needed for component insertion and repair. Silkscreen must also not overlap via holes or pads; otherwise, part of the legend can be lost when the solder mask opening is created, affecting identification. Silkscreen spacing must be greater than 5mil.
Clear Polarity Marking for Polarized Components
Polarized components must have their polarity clearly shown on the silkscreen drawing. The polarity direction mark should be easy to recognize so that assembly and inspection personnel can verify orientation without ambiguity.
Clear Orientation Marking for Directional Connectors
Directional connectors must have their orientation clearly indicated on the silkscreen. A visible orientation mark helps prevent reversed insertion and supports correct assembly.
Barcode Location Marking
Where board space permits, the PCB should include a 42*6 barcode silkscreen frame. The barcode position should be selected with scanning in mind, so that the code remains accessible and readable during production and tracking.
Board Name, Date, and Version Information
The PCB file should include silkscreen information such as the board name, date, and version number. These markings should be placed in a clear and conspicuous location so that the board revision and identity can be confirmed at a glance.
Manufacturer Information and Anti-static Marking
The PCB should carry complete relevant manufacturer information and an anti-static marking. These markings support traceability and handling control during manufacturing and assembly.
Correct Number and Complete Output of Gerber Layers
The number of PCB Gerber files must be correct. Each layer must be output correctly, and the layer output must be complete, so that the fabrication data set matches the intended board stack and all required features are represented.
Component Identifiers Must Match the BOM
The component identifiers on the PCB must be consistent with the identifiers in the BOM list. This consistency is essential for correct material selection, assembly, and inspection.
Related Reading:
PCB Material and Thermal Design Requirements for Reliable Assembly
PCB Component Library and Footprint Selection Requirements Guide
PCB Basic Layout and Manufacturability Requirements for PCBA Assembly
PCB Testability Requirements for Reliable ICT and Functional Test
Electrical Clearance, Creepage Distance, and Insulation Levels
