Gerber format: history, variants and viewer

A printed circuit board is not described by a single file: each physical layer is its own file, and to see it you have to recompose them all, aligned. This page explains where the Gerber format comes from, which variants exist, which files make up a board and why many manufacturers today rely on richer formats.

A short history

The name comes from Gerber Scientific, Joseph Gerber’s company, which between the 1960s and the 1980s built the vector photoplotters used to expose the films from which printed circuit boards were fabricated. The Gerber format began as the control language of those machines — a subset of the EIA RS-274 standard for numerically controlled machines.

The photoplotter moved a light source: it flashed a shape (an aperture) at a position to create a pad, or drew a line by exposing the film along a path to create a trace. Hence the concepts still central today — aperture, flash, draw — and the reason a Gerber is a vector drawing, not a raster image. Because every fab read that language, Gerber became the de-facto standard for exchanging PCB artwork.

The format variants

• RS-274D (the “standard” Gerber) — carried only the moves; the aperture shapes lived in a separate file (the aperture wheel) communicated apart. Ambiguous and fragile: one mismatch between the drawing and the aperture table was enough to get the board wrong. Now obsolete.
• RS-274X (Extended Gerber, X1) — embeds the aperture definitions and the coordinate format in the file, and adds regions (G36/G37), dark/clear polarity (LPD/LPC), step-and-repeat and aperture macros. The variant used for decades, and the one this viewer interprets.
• Gerber X2 (2014) — adds attributes (metadata) that declare what each file means: layer function, drill data, netlist attributes. The set becomes self-describing instead of relying on filenames. It is maintained by Ucamco, the format’s heir to Gerber Scientific.
• Gerber Job File (.gbrjob) — a companion file describing the whole job (stack-up, layer order, materials) alongside the Gerber X2 files.

The Gerber format in practice (RS-274X)

Gerber describes each layer as a sequence of apertures (circles, rectangles, custom shapes via macros) that are flashed at a position (a pad) or drawn along a path (a trace). RS-274X embeds both the aperture definitions and the coordinate format; regions (G36/G37) fill areas, and clear polarity (LPC) “carves” the copper already laid down.

Each Gerber file contains a single layer. A common coordinate system (origin and units) ensures different layers overlay correctly.

The directive that decides everything: the coordinate format

There is one line, at the start of every file, that determines whether the board will be ten centimetres or ten metres across. Coordinates in Gerber are integers with no decimal point: X1500Y2000 does not say millimetres, it says “fifteen hundred units”, and what a unit is worth is set by the FS (Format Specification) directive together with MO (Mode, inches or millimetres).

The form %FSLAX46Y46*% reads as follows: L = leading zeros omitted, A = absolute coordinates, then X46 = 4 integer and 6 decimal digits for the X coordinate, Y46 likewise. With MO in millimetres, the elementary unit is therefore 10⁻⁶ mm.

The last column of the table is why this directive matters more than all the others: a one-digit error scales the board by a factor of ten, and the file opens perfectly. There is no syntax error, no warning: there is a board of the wrong size, which the fab would happily manufacture if the outline file carried the same error. It is also why the first check on a received Gerber is always to measure something known — a connector pitch, the board diagonal — and not to look at whether it “seems right”.

Two historical variants still turn up, and have to be recognised. Omitted trailing zeros (T instead of L) still exist in old files and completely change the interpretation of the same digits. And incremental coordinates (I instead of A, with G91) have been deprecated for decades but show up in output from ancient CAD: every coordinate is a displacement from the previous one, so a single parsing error shifts everything after it in the layer.

Arcs: G74 and G75, the bug nobody sees

An arc in Gerber is drawn with G02 (clockwise) or G03 (counter-clockwise), giving the end point and the centre offset (I, J) from the start point. But the interpretation of that offset depends on a mode declared separately:

• G74 — single quadrant: the arc cannot cross a quadrant, I and J are unsigned and the direction has to be inferred. A historical, deprecated mode.
• G75 — multi quadrant: I and J are signed and the arc can run up to a full circle. This is the correct mode.

Reading a G74 file as G75 (or the reverse) does not produce an error: it produces arcs going the wrong way round, or circles where quarter-circles belong. On a copper layer you notice; on a solder-mask layer or a board-outline route, much less — and the part comes out with a different profile from the one drawn. This tool’s renderer implements both modes, which is why the distinction shows up here at all.

The files of a board

A typical board is a set of files, one per physical plane plus drilling and outline:

• Copper — one per conductive layer: top, bottom and any inner layers. This is where traces and pads live.
• Solder mask — one file per side. Its apertures mark where the copper stays exposed.
• Silkscreen — component text and outlines, one file per side.
• Solder paste — the stencil apertures for paste on SMD pads, one file per side.
• Drill (Excellon) — not a Gerber but a separate Excellon file, with hole coordinates per diameter.
• Outline (Edge Cuts) — the board’s mechanical contour, a dedicated Gerber.

Why several files, and how they compose

Separating the layers is necessary because each goes through a different fabrication process (copper etching, silkscreen printing, drilling). To view the board you do the inverse: load every file and overlay them, aligned on the same coordinate system, so that pads, traces, mask and holes fall exactly where they should. Each layer gets a colour and can be toggled to inspect the board layer by layer.

Layer identification

File names are not standardised across CADs: the same layer can be called top.gtl, board-F_Cu.gbr (KiCad), top_copper.gbr and so on, and drills can have a .drl or .txt extension. This is precisely why Gerber X2, by adding function attributes, reduces the ambiguity. The viewer recognises each file’s type by combining name/extension and content; stray files (BOM, pick&place, PDF, README) are ignored without error, while an ambiguous layer stays marked as “unknown” and can be assigned by hand.

Common extensions per layer

The left column is the meaning; the right shows the two most common conventions (Protel/legacy and KiCad). These are examples, not a standard: exactly the ambiguity that the Gerber X2 attributes remove.

What the renderer actually covers

Saying a viewer “interprets Gerber” means nothing: what counts is which directives it handles, because the missing ones do not raise an error, they draw something different. This is the actual coverage, read from the renderer’s source:

Three rows deserve a comment. AB (Aperture Block) and SR (Step and Repeat) are the directives that describe a panel — the same board repeated on a grid — and they are the ones simple viewers ignore: the result is that you see one board instead of twelve, and the panel looks wrong when it is the viewer that is incomplete. LM/LR/LS (mirror, rotate, scale) are the transformations introduced by Gerber X2: without them, rotated apertures land in the right place with the wrong orientation.

And among the unsupported macro primitives, 20 (vector line) is the only one met with any frequency, in macros generated by older CAD; 6 (moiré) serves optical fiducial targets and is rare. A macro using them is ignored in the unsupported part rather than failing the load, which is the right choice for a viewer but worth knowing.

Beyond Gerber: ODB++ and IPC-2581

Classic Gerber describes only the artwork of each layer: it does not carry the stack-up, the netlist, the components or the hole spans. For fabrication and especially assembly this leaves ambiguities the fab has to fill in by hand. That is why many manufacturers today prefer “intelligent” formats:

• ODB++ (born at Valor, now Siemens) — not a file but a database (a directory tree) that carries copper, drilling, netlist, components, stack-up, test-points and DFM rules in a single package. Widely used to cut setup and back-and-forth with the fab.
• IPC-2581 (also called DPMX) — an open, vendor-neutral standard, a single XML file with the full product model (stack-up, netlist, components, drilling, DFM data). Pushed as an open alternative to the proprietary ODB++.

Gerber X2 narrows the gap by adding attributes, but ODB++ and IPC-2581 are designed to carry netlist, components and stack-up natively. In practice a fab almost always accepts Gerber (X2 or RS-274X + Excellon), and in parallel ODB++ or IPC-2581 when the assembly flow requires them.

How the board is rendered

The board is rasterized on a WebGL2 canvas by an engine written in Rust and compiled to WebAssembly: it interprets dark/clear polarity (LPD/LPC) and pour regions (G36/G37) directly, so clearances truly “carve” the copper and traces stay readable even inside a plane. Layers are composited with per-layer transparency, with point-to-point measurements and feature picking.

---

Web tool: Gerber Viewer. Engine: WASM Gerber Viewer (Rust/WASM renderer on WebGL2, MIT).