How to Check Your Gerber Files Before Sending Them to Fabrication

Most Gerber problems are found by the fabricator, not by the engineer who exported them. That is the wrong way round: by then you have lost two days to an email thread, and the fabricator is guessing at what you meant.

What follows is an inspection you can run yourself in about fifteen minutes, before anything leaves your machine.

First, what a Gerber set is and is not

A Gerber file describes the shapes on one layer as a set of apertures and coordinates. A Gerber set is a folder of those files, one per layer.

What that set does not contain:

drill data — that is Excellon, a different format, exported separately; the stackup — layer order, dielectric thicknesses and materials usually live in the fabrication drawing or a separate document; the BOM or placement data — those describe what goes on the board, not the board; your intent — tolerances, finish, impedance targets and special instructions belong in the fabrication drawing or notes.

A Gerber archive on its own is not a complete manufacturing package. Treating it as one is the root of a whole category of supplier questions.

Two format versions are common. RS-274X embeds aperture definitions and is the long-standing default. X2 adds metadata describing what each layer is, so the fabricator does not have to infer roles from file names. Some fabricators prefer one; most accept both. Ask.

The inspection

Step 1 — open them somewhere else

Open the set in a Gerber viewer that is not the tool that produced it.

Your ECAD tool renders its own output as it intended. An independent viewer renders what the file actually says. The difference between those two pictures is where missing layers, inverted polarities and stray content live.

This single step catches more than the rest of this article combined.

Step 2 — count the layers

Compare the file list against your stackup. Both directions.

Missing: a copper layer that did not export. The board gets made without it, which is unrecoverable. Extra: an internal notes layer, a mechanical layer, a documentation layer exported as copper. It gets etched.

Six copper layers means six copper files. If you see seven, find out what the seventh is before sending.

Step 3 — look at the outline on its own

Switch every layer off except the board profile.

You are looking for one closed shape. Not two. Not a shape with a gap you can only see at high zoom. Not the outline drawn on both a mechanical layer and the edge layer, slightly differently.

An ambiguous outline is the most common cause of a fabrication delay, and it is completely invisible when all layers are displayed at once.

Step 4 — check soldermask against copper

Toggle the soldermask layer on and off over the copper.

Every pad that will be soldered needs a mask opening. Every area that must not be soldered needs mask. The common failures:

pads with no opening — unsolderable; mask slivers between fine-pitch pads — they may not survive fabrication, and the fabricator may remove them without telling you; * vias you wanted tented that are open, or vice versa.

Step 5 — read the silkscreen

Zoom in until the text is readable.

Does any silkscreen sit on top of a pad? It will be removed, and your pin 1 marker with it. Is the text large enough to survive printing? Below roughly 0.8 mm height it starts becoming unreliable, though the limit is your fabricator's to state. * Is the revision identifier there? This is the cheapest insurance in hardware: a board that says REV C on it can never be confused with one that does not.

Step 6 — overlay the drill data

Load the drill file over the copper layers.

Every drill hit should land inside a pad. A hole offset from its pad produces a broken connection that passes visual inspection and fails electrically.

Also check the annular ring — the copper remaining around the hole — against your fabricator's minimum. The default DRC in your tool may be more permissive than your supplier's process.

Step 7 — decide what the drill diameters mean

Open the drill file as text. The numbers in it are either finished hole sizes or tooling sizes, and plating changes the result by enough to stop a connector pin fitting.

Your tool may let you choose. Whatever it exported, state it in the fabrication drawing. One line.

What to send alongside the Gerbers

All of that inspects the set. It does not complete it.

A Gerber set describes shapes. It says nothing about the material those shapes are etched into, nothing about the copper weight, nothing about what the board is finished with, and nothing about which of the holes you just counted has to be plated. A fabricator who receives shapes and no instructions will either ask, which costs you a day, or assume their house default, which costs you a batch if their default is not yours. So the set travels with the rest of the package:

A fifteen-minute checklist

• [ ] Opened in an independent viewer
• [ ] Copper layer count matches the stackup, no extras
• [ ] Exactly one closed outline, on one layer
• [ ] Soldermask openings on every solderable pad
• [ ] No silkscreen over pads
• [ ] Revision identifier visible on the silkscreen
• [ ] Drill hits land inside their pads
• [ ] Annular ring meets the fabricator's minimum
• [ ] Finished vs tooling drill size stated in the drawing
• [ ] Fabrication drawing, stackup and drill files included

One thing this will not catch

The inspection above verifies that the files describe what you drew. It cannot tell you whether what you drew is correct.

If the schematic and the layout have drifted apart — a change made in one and not pushed to the other — the Gerbers will be a perfect, internally consistent rendering of the wrong board. That is caught earlier, by updating the layout from the schematic before exporting anything.

Inspecting one set takes fifteen minutes. Knowing, four revisions later, which set was the one that went to the fabricator — and whether the BOM in the same folder belongs to it — is the part that needs somewhere durable to live.

In XKEMA a manufacturing package belongs to a PCB revision, and two revisions of a package can be compared by their geometry.

Hardware documentation PCB manufacturing package checklist * PCB fabrication vs assembly: who needs which files?