PCB Design File Checks Before You Order

Most delays on a prototype order come from questions the fabricator has to ask before the data can be processed. The board is quoted from the design files once they are converted into production data, and the fabricator never sees the schematic, so anything ambiguous has to be resolved by correspondence. The items below generate the most questions, grouped by the layer they belong to. Checking them before submission removes most of the back and forth.

Outline and Mechanical Layers

The outline is the most common omission. A design file submitted without an outline layer, whether mechanical or keep-out, leaves the fabricator to infer the board shape from the copper, which is a guess rather than a definition. The second most common problem is the opposite: a mechanical layer and a keep-out layer that do not coincide, producing two concentric contours and no way to tell which one governs.

Three further cases follow from the same area. An outline that overlaps the drill layer produces a profile that contains both slots and holes, and the fabricator has to decide which features are edges and which are holes. A slot narrower than the smallest router bit, commonly 0.8 mm, cannot be cut and has to be widened or removed. And a corner where a right angle and an arc coincide is ambiguous in the same way, because two different shapes are claiming the same location.

Traces and Spacing

On the copper layers, the questions are about continuity and capability. A trace that appears to be broken, or two traces that overlap in a way that leaves a single connection ambiguous, has to be confirmed before it is built, because building either interpretation is cheap and building the wrong one is not. Spacing or width below the shop minimum, commonly 5 mil, has to be relaxed or the design has to move to a supplier with a finer process.

Copper pours have their own limit. A mesh or grid pattern with gaps smaller than about 0.2 mm cannot be etched reliably, as the film slivers left behind become stray copper, so the choice is to fill the area solid or to open the spacing. Solid filling is usually the better answer on a dense board, since it also improves the return path and thermal spreading.

Solder Mask Openings

Mask questions usually come from a mismatch between the paste layer and the mask layer. Where the paste layer defines an opening that the mask layer does not, the fabricator cannot tell whether the pad should be exposed or covered. The second case involves fine-pitch devices: when the gap between adjacent pads is below about 0.25 mm, a mask bridge between them cannot be printed, so the option is a single large opening over the whole device. That change alters the solder volume during assembly, so it should be a decision the designer makes rather than a question in an email.

<img src="https://www.gopcba.com/wp-content/uploads/2024/09/make_Keyboard_pcb.webp" alt="Solder mask opening and paste layer alignment on a fine pitch device” />

Silkscreen Limits

Legend has two hard limits and one convention. Text placed on a pad interferes with soldering and will be trimmed away or deleted, so it should never overlap a land. The minimum printable line width is around 0.15 mm and the minimum character height around 0.8 mm; anything smaller may not be legible on the finished board. The convention concerns the bottom side: legend drawn there appears mirrored when viewed from the other side, so the file has to state whether the artwork is already in the correct reading orientation or should be mirrored.

Via Types and Slots

Via questions are all about intent. A via closer than about 0.4 mm to the board edge cannot be relied on to keep its annular ring, so the fabricator needs to know whether an unplated hole is acceptable. Plated holes above roughly 10 mm, square holes, and elongated slots may all be outside the standard process, and each has a substitute that should be confirmed rather than assumed. Holes marked as unplated but carrying a mask opening are contradictory and have to be resolved. Duplicate holes at the same coordinate leave the fabricator to choose, and a slot, a drill entry, and an outline feature that are all different sizes in different layers have to be assigned to the layer that governs.

Filling Out the Process Note

Nearly all of these questions disappear when the order carries an explicit process note. State the outline layer, the minimum width and spacing, the mask and paste relationship, the legend limits, and the intended via types. Where a feature is deliberately outside a normal capability, say so and say what the substitute should be. The note costs a few minutes at submission and replaces a day of correspondence, and it is the single most effective habit for getting a prototype back on schedule. Related conventions are collected in board outline and mounting design, via design rules, and PCB slot and edge routing rules.

Where the Cost Actually Comes From

Understanding the price helps in the same way, because it shows which changes are worth making. The main drivers are the layer count, the board thickness, the material, the order quantity, the surface finish, the copper weight, the ink color, the minimum width and spacing, the smallest hole, and the delivery date. Of those, the ones a designer controls most directly are the finish, the copper weight, the minimum feature size, and the layer count, and they do not carry equal weight: moving from a standard finish to a thin-gold finish costs far less than adding two layers or halving the minimum spacing.

That ranking explains why the process note also matters commercially. A board whose features sit comfortably inside the shop standard window is priced from a catalog. A board that pushes one parameter to the edge moves into a different process and often onto a different line, which is where both the price and the lead time jump. When a schedule is tight, relaxing the one parameter that falls outside the standard window is usually cheaper than paying for the tighter process, and the fabrication drawing is where that decision gets recorded so that it is not rediscovered later.

One more habit is worth adopting: keep the process note with the design files rather than in the email thread. When a revision is released the note travels with it, so a second order does not repeat questions the first order already answered, and a new engineer inherits the reasoning instead of the conclusion. On a product that will be built several times, that single practice saves more schedule than any individual check in this list.

Where a feature genuinely cannot meet the standard window, state what the intent is and what the acceptable substitute would be. A fabricator who understands that a slot exists to isolate a high-voltage node will widen it without asking. One who only sees an out-of-spec dimension has to stop and write an email, and the order waits.

FAQ

What happens if I forget the outline layer? The fabricator has to infer the board shape from the copper, which produces a question rather than a board. Always submit an explicit outline.

Why can a fine-pitch device not keep mask between the pads? Because below about 0.25 mm the bridge cannot be printed reliably. A single opening over the device is the usual alternative, and it changes the solder volume.

Can I specify an unplated hole near the board edge? Yes, if the annular ring cannot be guaranteed. State that the hole is intentionally unplated so the fabricator does not try to preserve a pad.

Is a process note really necessary for a prototype? It is the cheapest step available. A short note on layer intent and process limits removes most of the questions that delay an order.