Gerber file extensions explained
A Gerber archive contains one file per physical layer of the board. The format itself does not store which layer a file represents, so EDA tools encode it in the file name. Two conventions are common: the three-letter Protel extensions used by Altium, EasyEDA and many manufacturers, and the descriptive names written by KiCad. Knowing both makes it easy to see at a glance whether an archive is complete.
Protel-style extensions
| Extension | Layer |
|---|---|
| .GTL | Top copper |
| .GBL | Bottom copper |
| .G1 – .G9 | Inner copper layers, numbered from the top |
| .GTS | Top solder mask |
| .GBS | Bottom solder mask |
| .GTO | Top silkscreen (overlay) |
| .GBO | Bottom silkscreen (overlay) |
| .GTP / .GBP | Top / bottom solder paste (stencil) |
| .GKO or .GM1 | Board outline (keep-out or mechanical layer 1) |
KiCad names
KiCad appends the layer name to the project name, for example board-F_Cu.gbr or board-Edge_Cuts.gm1. F means front (top) and B means back (bottom): F.Cu and B.Cu are copper, F.Mask and B.Mask are solder mask, F.Silkscreen and B.Silkscreen are the legend, F.Paste and B.Paste are stencil layers, and In1.Cu, In2.Cu and so on are inner copper. Edge.Cuts is the board outline. KiCad can also be set to use Protel extensions in the plot dialog.
Drill files
Holes are not described in Gerber but in Excellon format, usually with the extension .DRL, .XLN, .EXC or .TXT. Some tools write plated and non-plated holes to separate files (for example PTH and NPTH). Both must be included in the archive; a board ordered without the non-plated drill file will arrive without its mounting holes.
Files you can leave out
Pick-and-place files, bills of materials, assembly drawings and job files are useful for assembly but are not needed to manufacture the bare board. Including them does no harm, but the manufacturer will only use the layers listed above.
Checking an archive
When you load a ZIP or RAR in PCB Tools, each file is matched against both naming schemes and shown in the layer list with its role. A file that does not appear in the list was not recognised; renaming it to the matching standard extension usually solves it. Before ordering, work through the pre-order Gerber checklist.