What is inside a Gerber package
The layer files, drill files and board outline that make up a Gerber package, what each one is for, and what an online Gerber viewer should show you for each.
Last reviewed
A "Gerber package" is the set of files a PCB manufacturer builds your bare board from. It's usually a ZIP holding one Gerber file per layer, one or more drill files and, from newer tools, a job file describing the set. Each file is plain text describing 2D shapes: no components, no nets you can click on, just what to image, etch, print and drill.
The layer files
Each Gerber file describes one physical layer. Exporters name them differently; the table shows the usual names from KiCad and the common "Protel" extensions many tools use.
| Layer | What it is | Typical names | What a viewer should show |
|---|---|---|---|
| Top and bottom copper | The copper traces, pads and pours on the outer layers. | F_Cu.gbr, B_Cu.gbr, .GTL, .GBL | Every trace, pad and filled zone. Pours should look solid, not outlined or missing. |
| Inner copper | Copper on the inner layers of a 4-layer or bigger board. | In1_Cu.gbr, In2_Cu.gbr, .G1, .G2 | One file per inner layer, in the order you designed them. Planes often look mostly solid with clearance holes. |
| Solder mask | Where the mask is opened so pads stay bare. The file is drawn as openings, so it looks "negative". | F_Mask.gbr, B_Mask.gbr, .GTS, .GBS | An opening over every pad you will solder, slightly larger than the pad. No mask openings over traces you meant to cover. |
| Silkscreen | Printed text, outlines and logos. | F_Silkscreen.gbr, B_Silkscreen.gbr, .GTO, .GBO | Readable reference designators and markings, not printed over pads. Bottom text appears mirrored when viewed from the top. |
| Solder paste | The stencil openings for surface-mount pads. Only needed for assembly or a stencil, not for bare boards. | F_Paste.gbr, B_Paste.gbr, .GTP, .GBP | Openings on SMD pads only, none on through-hole pads. |
| Board outline | The shape the board is cut to, including cutouts and slots. | Edge_Cuts.gbr, .GKO, .GM1 | One closed shape around the board, plus any closed internal cutouts. |
Gerber X2: files that say what they are
Older Gerber files (RS-274X, sometimes called X1) contain only shapes, so a viewer has to guess from the filename which layer a file is. Gerber X2 adds attributes inside the file: what layer it is (its "file function"), which side, and optionally which net each object belongs to. A viewer that reads X2 can place files correctly whatever they're called, and some can show you the net or pad behind an object. Ucamco's Reference Gerber Viewer displays all X2 attributes; see the ranking for the others.
The drill files
Holes are usually not in Gerber at all but in Excellon drill files (.drl, .xln, .txt), a format from CNC drilling machines. A package often has two:
- Plated holes (PTH): vias and through-hole component pads, copper-plated inside.
- Non-plated holes (NPTH): mounting holes and other holes with no copper.
Some exporters put both in one file. Slots and oval holes are written as drilled routes, which some older viewers draw as a row of round holes or skip.
What a viewer should show: every hole sitting in the centre of its pad, at a sensible size, on the same scale as the copper. Holes floating off to one side, or a cloud of tiny dots, mean the drill file's units, number format or origin don't match the Gerbers. The checklist covers how to spot it.
A drill map (a Gerber or PDF drawing of hole sizes) and a drill report may also be in the package. They're for people, not machines; the fab builds from the Excellon file.
The job file
KiCad and other tools can write a Gerber job file (.gbrjob), which lists the files in the package, the layer order, board size and thickness. A fab can read it to set up the job automatically. A viewer doesn't need it, but it's a quick way to confirm nothing is missing.
What a viewer can't show
A Gerber package describes the bare board only. It doesn't contain the schematic, the component values, the bill of materials, the design rules you used or why anything is where it is. For that you need the design source; see Gerber files versus design source files.
A complete package, at a glance
For a typical 2-layer board you'd expect at least:
- Top copper and bottom copper
- Top and bottom solder mask
- Top silkscreen (and bottom, if you print on the back)
- Board outline
- Drill file(s) for plated and non-plated holes
A 4-layer board adds two inner copper files. Paste layers come along if you're ordering assembly or a stencil.