PCB Fabrication Specifications: What to Put on the Drawing

Most fabrication problems are specification problems. A board that is electrically correct can still be unusable because the copper weight was never stated, the impedance requirement appeared only in an email, or the outline tolerance was left to the fabricator to assume. A complete set of PCB fabrication specifications removes those assumptions, and it is the cheapest quality tool in a project because it costs nothing but attention.

What the specification covers

The specification is the set of technical parameters the manufacturer is expected to build to. It covers the base material, the board dimensions, the copper weight, the trace and space rules, the drilling, the tolerances, and the surface finish. Together, those parameters decide whether the board runs reliably, whether it solders properly, whether it meets its electromagnetic requirements, and whether it survives mechanical stress.

The reason to be explicit is asymmetry. A missing parameter is filled in with a default, and a default that suits one product is wrong for another. In high-frequency or high-density work, a single parameter set wrongly can reject an entire batch.

Outline and dimensions

The drawing should state the length, width, and profile of the board, and it should say how the profile is produced: routed, scored, or with internal cutouts. A standard outline tolerance of plus or minus 0.2 mm covers most products.

Special features are the part that is usually omitted. Internal slots, curved edges, and unusual cutouts require additional processing and add cost, so they should be drawn explicitly rather than implied by the outline. A mechanical drawing that shows the board in its enclosure is often the fastest way to communicate them.

Layer count and construction

Layer count is chosen from routing density and the need for reference planes. Two-layer boards dominate consumer products. Four and six layer boards are used for industrial control and power designs, and eight layers and above serve high-speed or complex routing.

As the layer count rises, the stackup drawing becomes more important than the layer count itself. The arrangement of signal layers, planes, dielectric thickness, and copper distribution is what defines impedance, crosstalk, and mechanical balance, and it is easier to review a stackup than to discover its consequences in a prototype. The trade-offs are discussed in our guide to layer stackup from one to eight layers.

Copper weight

One ounce copper, about 35 micrometres, is the standard for signal layers and is adequate for the majority of designs. Power layers and high-current traces often call for two or three ounces, which increases both material and etching cost.

Copper weight is not a cosmetic upgrade. It sets the current capacity of a trace and its ability to spread heat, so it should be derived from the current the net has to carry and from the acceptable temperature rise rather than from a desire for margin.

Copper weight and trace width together define current capacity. Specifying one without the other leaves the answer incomplete.

Trace and space, drilling, and pads

Standard fabrication supports a minimum trace width and spacing of about 6 mil, which also corresponds to roughly 0.15 mm. High-density interconnect processes reach 3 mil, and the tighter rule is not free: finer features need more precise imaging and etching, and the cost of the board rises accordingly.

Drilling follows the same logic. A mechanical hole of 0.2 mm diameter is a normal limit with a tolerance near plus or minus 0.05 mm. Laser-drilled microvias reach 0.1 to 0.15 mm and are used in high-density stacks. Introducing blind or buried vias adds processing per layer, and the annular ring around each pad should be at least about 0.15 mm, with the applicable design standard used as the reference for pad and hole relationships. The pad geometry rules are collected in our guide to PCB pad design standards.

Surface finish

The finish decides solderability, oxidation resistance, and, in the end, reliability. Hot air levelling is the economical default and suits general-purpose boards. Electroless nickel immersion gold provides a flat, oxidation-resistant surface at a premium and is used where fine-pitch or hidden-joint packages are present. An organic solderability preservative is an economical and environmentally straightforward choice, and immersion silver or immersion tin serve high-frequency work and demanding soldering requirements.

The choice is not interchangeable. A finish that is unsuitable for the assembly process can cause hidden joint failures, particularly under a package, and it can also affect the electromagnetic behaviour of the finished product. Cost and process have to be considered together.

Solder mask and legend

Solder mask protects the copper and prevents solder bridging. Green is the standard colour and the least expensive; other colours add a small premium but no functional difference. The legend should be printed in a font no smaller than about 0.8 mm to remain legible after processing, and it should never be placed across a pad or a via, where it interferes with soldering and can be mistaken for a defect.

Legend placed on a pad is not a cosmetic problem. It changes the wettable area and makes the joint harder to inspect.

Impedance control

High-speed interfaces such as USB 3.0, HDMI, and PCIe require controlled impedance, and the specification has to state the target rather than assume it. Single-ended lines are commonly controlled at 50 ohm and differential pairs at 90 ohm, and those targets only hold if the stackup, the copper weight, and the trace geometry are chosen together.

Verification is part of the specification. A test coupon built into the panel is used to measure the achieved impedance, and adding that coupon and the measurement to the order carries its own cost. The parameter should therefore be specified where the interface needs it, and omitted where it does not.

Tolerances

Tolerances are where over-specification becomes expensive. A board thickness tolerance of plus or minus 0.1 mm covers most designs, an outline tolerance of plus or minus 0.2 mm is standard, a V-score tolerance of plus or minus 0.1 mm is normal, and a hole position tolerance of plus or minus 0.05 mm is what keeps component assembly predictable.

Tighter limits are available and should be reserved for the features that genuinely need them, because precision is purchased with process time. A design that specifies tight tolerance everywhere pays for it everywhere.

Design for manufacturability and the data package

A specification is only as good as the data it accompanies. Apertures, tolerances, and trace widths should be annotated rather than left to inference, and a stackup drawing should be included for anything above a simple two-layer board.

The data package should also include the fabrication drawing and the export settings used, and it should be reviewed for manufacturability before release. That DFM review is where a conflicting requirement, an unmanufacturable feature, or a missing parameter is found, and finding it at that stage avoids both rework and delay. The wider relationship between design and production is covered in our guide to PCB design and fabrication.

How the price bands move

The cost of a board follows its specification class rather than its size alone. A simple two-layer prototype with a standard finish sits at the low end. A four-layer industrial board with an immersion gold finish and a moderate hole size sits above it, and a six-layer board with impedance control and laser microvias sits above that. An eight-layer high-density board with blind and buried vias occupies the top of the range.

Quantity modifies all four, but it does not change the order. The purpose of writing an explicit specification is not to increase the price; it is to make the price correspond to the product that will actually be built.

FAQ

Can the fabricator set the specification automatically from the Gerber files? It is technically possible, and it is not recommended. The defaults that suit one product are wrong for another, and an implicit assumption is harder to dispute than a stated requirement.

How do I know whether impedance control is needed? If the design carries a high-speed digital interface such as USB 3.0, a low-voltage differential signalling link, or a fast memory bus, it needs a controlled impedance target and a stackup that supports it.

Can a 4 mil design be manufactured? Yes, at a materially higher price than a 6 mil design. The right question is whether the density is genuinely required or merely convenient.

Can standard FR-4 be used for a high-frequency design? Generally not recommended. High-frequency work calls for a laminate with a low and stable dielectric constant and low loss, which costs more but behaves predictably.