KEMI Docs · PCB Practice
Gerber Files Explained
Last updated: 2026-08-30
When a PCB design is done, what you send to the fab is not your project file — it is Gerber data: one digital 'film' per layer. Knowing which file is which layer is what prevents ordering accidents. This article summarises the rules KEMI uses in real pre-order reviews.
1
Why one file per layer
Gerber (RS-274X, now with X2 extensions) is a 2D vector format that describes only the shapes of copper and ink on each layer — no parts, no nets, no circuit meaning. Fabrication proceeds layer by layer (copper etch, mask print, silk print, routing), so the data splits the same way. A 4-layer board is a set of at least 8-9 files: four copper, two mask, one or two silk, one outline, plus drill.
2
Layer roles by extension
| Extension | Layer | Content |
|---|---|---|
| GTL / GBL | Top / Bottom copper | Traces and pads |
| G1, G2… | Inner copper | Signal and plane layers (4+ layer boards) |
| GTS / GBS | Solder mask | Where mask is removed — pads that stay exposed |
| GTO / GBO | Silkscreen | Printed legend |
| GKO / GM1 | Outline | Board edge — the fab cuts along this line |
| GTP / GBP | Paste | Stencil data — needed for SMT only, not bare-board orders |
| DRL / TXT / XLN | Drill | Excellon hole coordinates and diameters (a separate format) |
Mask layers are negatives
Shapes on GTS/GBS mark where mask is stripped, not where ink goes. Seeing shapes on pad locations is correct.
3
Why drill files are separate
Holes are made by a drill machine, not etching, so they ship as an Excellon coordinate list. Two common failure points: unit/decimal declarations differ per file (misread files show holes 10x off), and many CADs split plated (PTH) and non-plated (NPTH) holes into separate files — forget the NPTH file and your screw holes arrive plated.
4
Pre-order checklist
- Count copper files — they must match the ordered layer count. Order 4 layers with 2 copper files and you get a 2-layer board.
- Check the outline layer exists, is closed, and the board size is what you intended.
- Drill file present, both PTH and NPTH included.
- Mask openings present on every pad you will solder.
- Silkscreen not overlapping pads — overlaps get clipped in production.
- Final review in a Gerber viewer — inspect the exported Gerbers themselves, not the CAD screen. Export mistakes only show in the Gerbers.
⚠ Missing layers get manufactured as missing
The fab assumes the files you sent are complete. Some will ask; many will just build it. Counting files is the customer's job.
FAQ
KiCad has no GTL extension?
KiCad exports every layer as .gbr with the layer name in the filename (F_Cu, B_Mask, Edge_Cuts…). Edge_Cuts is the outline. Most fabs recognise the naming directly.
Do Gerbers contain part information?
No — shapes only. For SMT assembly you also need a BOM and a placement (CPL) file.
What is Gerber X2?
An extension that embeds layer roles and pad functions as standard attributes, so layers are identified without filename guessing. Old CAM tools still read it as plain Gerber.
Where can I view Gerbers before ordering?
Drop the ZIP into KEMI's online Gerber viewer — it classifies layers automatically and runs basic completeness checks, with no install.
See also
This article summarises the working rules KEMI uses in real design and fabrication work. For production, part datasheets and fab specifications take precedence.