PCB Fabrication Design Rules: Minimum Features and CAM Checks
Every design rule in a CAD tool has a counterpart in the fabricator’s process, and where the two disagree the process wins. A trace narrower than the etching process can hold is not a thin trace; it is an open circuit. A solder mask opening smaller than the registration tolerance is not a tight opening; it is a pad that may be covered by mask. The rules below are the ones where that gap appears most often.
Why the Fabricator’s Limits Come First
A design is completed against the fabricator’s capability, not against the memory of a previous project. The first step in the CAM department is to take the data from the CAD system and check that it can be built: that the pad and hole sizes are consistent, that the apertures and the drill data agree, and that the tooling and reference marks needed for production can be added.
The check that matters most is the one nobody likes to hear. A dimension that is achievable in a drawing may not be achievable in copper. A fabricator able to hold a 0.25 millimetre minimum pad width may not be able to hold 0.2 millimetres reliably, and asking for it does not make it possible. The correct approach is to obtain the fabricator’s minimum feature table before the layout is finished and to design to it, rather than to design to what the tool allows and negotiate afterwards.
Pad and Trace Minimums
Minimum pad width and minimum trace width and spacing are the numbers that constrain the whole layout. For conventional processes, a minimum trace width and spacing of 0.2 millimetres each is a reasonable working figure, and going below it requires a special process rather than a tighter tolerance. Pad widths follow the same logic: 0.25 millimetres is a safe minimum for a process that cannot hold 0.2 millimetres, and the pad has to be wide enough to survive the etching and the plating without becoming a ring too thin to solder.
The pad and the hole also have to agree with each other. A pad is an annulus around a plated hole, and if the hole is at the upper end of its tolerance while the pad is at the lower end, the resulting ring is thinner than either drawing specified. How that geometry is set is covered in PCB pad design standards.
Solder Mask Clearance
The solder mask opening is larger than the pad it exposes, and the reason is registration. When the mask is exposed and developed, its position relative to the copper varies within a tolerance, and if the opening were exactly the size of the pad, part of the pad would be covered whenever the mask shifted. A clearance of about 0.2 millimetres in total, that is 0.1 millimetres on each side, is a common figure and keeps the mask off the solderable area across the registration range.
The mask also matters where a via is exposed. A via left open can wick solder away from a joint during reflow, which is why the treatment of the via – tented, or filled – is specified on the drawing rather than left to the process. That decision has more consequence near a ball grid array than anywhere else.
Edges, Holes and Keep-Outs
The board edge is a boundary that carries more rules than it appears to. A minimum distance of 1 millimetre between the edge and any conductor is the usual design rule, with 0.5 millimetres acceptable in a constrained case but not recommended, because the routing process can tear a trace that runs too close to the cut. Where the assembly will be handled by machine soldering equipment, 3 millimetres is a safer figure, because the machine grips the board near its edge and the tooling can damage conductors close to it.
Non-plated holes, or NPTH features, follow the same principle with an additional consideration, which is what the hole is for. A component hole is normally kept at least 1 millimetre from any trace. A mounting hole is different again: for a screw hole of about 3 millimetres, the area within roughly 10 millimetres of its centre is normally kept free of both components and routing, so that a metal screw and its washer cannot touch a conductor. Keeping that space is itself a design decision, and the rules for outlines and mounting features are set out in board outline and mounting design.
Silkscreen and Component Clearance
Silkscreen is a process layer with its own tolerances. A component outline printed in silkscreen should stay at least 1 millimetre from the board edge, for the same reason a trace does, and the legend should not be printed over exposed pads, because the ink is not designed to survive soldering. Where the clearance is not enough, the outline is trimmed rather than moved.
Component bodies and pads are held further from the edge than traces. A pad is normally kept at least 1 millimetre from the edge and preferably 3 to 5 millimetres, because a pad close to the edge is one that stress can lift as the board flexes. Keeping that distance also protects the joint from the mechanical load that handling applies at the edge, which is one reason the constraints imposed by the fabricator and by the assembly process are worth collecting into a single rule set, as described in PCB design constraints for manufacturing.
What CAM Checks Catch
The CAM department performs the checks a designer cannot perform on a drawing. It verifies that every pad has a corresponding aperture and that the aperture sizes match the pad sizes, so that a pad cannot be exposed by the wrong opening. It checks that the drill data and the copper data agree, so that no hole is drilled through a pad that was not designed to receive it. It adds the tooling and reference marks the production equipment needs to align the layers and the panel. And it verifies the minimum features against the process, which is the check where the designer’s assumptions are either confirmed or returned as a question.
Most of those checks can be run inside the design tool if the rule set is configured with the fabricator’s limits rather than with a generic default. Doing that is cheaper than exchanging data, and it means the conversation with the fabricator is about the board rather than about the rules. Where the design will be built as a multilayer stack, the points worth agreeing before the first panel is made are covered in multilayer PCB prototype requirements.
FAQ
Whose design rules should be used? The fabricator’s. A rule set built from the process that will build the board is the only one that predicts whether the design can be manufactured.
What is the minimum trace width I can use? Around 0.2 millimetres is a reasonable floor for a conventional process, and smaller features require a special process rather than a tighter tolerance.
How much larger should the solder mask opening be than the pad? About 0.1 millimetres on each side is a common figure. It keeps the mask off the solderable area across the registration tolerance.
Why keep components and traces away from a mounting hole? Because a metal screw and its washer must not touch a conductor. For a screw hole of about 3 millimetres, the area within roughly 10 millimetres of the centre is normally kept clear.
