ManufacturingOct 12, 20267 min read
Gerber Files Explained: What PCB Manufacturers Need (Q&A Guide)
What are Gerber files? Which layers, drill and fab files a PCB manufacturer needs, how to export and check them, and Gerber vs ODB++ vs IPC-2581.
Gerber files are the de facto handoff format between PCB design and PCB manufacturing. If you have ever asked "what are Gerber files?", "which Gerber files does my fab need?" or "Gerber vs ODB++ vs IPC-2581 — which should I send?", this Q&A-style guide answers those questions in plain engineering terms.
What are Gerber files?
A Gerber file is a 2D vector image format (RS-274X, now maintained by Ucamco as the Gerber X2/X3 specification) that describes one layer of a printed circuit board: copper, solder mask, silkscreen, solder paste or board outline. Each layer of your design is exported as its own file, and the fabricator's CAM software stacks them to rebuild the board.
Gerber files describe images, not intelligence. Classic RS-274X carries no netlist, no stackup and no component data. Gerber X2 adds attributes (layer function, file polarity, pad/via roles), and X3 adds component information for assembly — but most shops still receive plain RS-274X plus separate drill and assembly files.
Which files are in a complete Gerber package for manufacturing?
A typical fabrication package for a 4-layer board contains:
- Top and bottom copper (e.g. GTL / GBL)
- Inner copper layers (G2, G3 … or GL2/GL3 depending on your CAD tool)
- Top and bottom solder mask (GTS / GBS)
- Top and bottom silkscreen / legend (GTO / GBO)
- Top and bottom paste (GTP / GBP) — needed for stencils and assembly
- Board outline / mechanical layer (GKO, GM1 or Edge.Cuts)
- NC drill file(s) — Excellon format, plated and non-plated holes, often separate files
- Drill map / fabrication drawing — stackup, finish, impedance, tolerances
- README with board thickness, copper weight, surface finish, mask/silk colour
For assembly you also send a BOM and pick-and-place (centroid/XY) file, and optionally an IPC-356 netlist so the fab can run electrical test against your intent.
How do I export Gerber files from KiCad or Altium?
- KiCad: File → Fabrication Outputs → Gerbers (.gbr). Select all copper, mask, silk, paste and Edge.Cuts layers, enable "Use extended X2 format" if your fab accepts it, then click Generate Drill Files (Excellon, millimetres, PTH and NPTH separate).
- Altium Designer: use an Output Job (.OutJob) with Gerber X2 or Gerber Files plus NC Drill Files, so the same settings are reused every revision.
Whatever the tool, always set units and format explicitly (e.g. mm, 4.6) and keep them consistent between Gerber and drill outputs.
How do I check Gerber files before sending them to the fab?
Never ship Gerbers you have not viewed outside your CAD tool. Open them in an independent viewer (KiCad GerbView, the Ucamco Reference Gerber Viewer, or your fab's online viewer) and check:
- Layer alignment — copper, mask and drill hits line up.
- Board outline is a single closed contour.
- Solder-mask openings exist on every pad and are absent on tented vias (if intended).
- Silkscreen does not overlap exposed pads.
- Drill sizes match finished hole sizes in your fab drawing.
- Polarity of planes (negative vs positive) is what the fab expects.
- Nothing missing — count the files against the list above.
Most fabs also run their own DFM check and send an engineering query (EQ) if something is ambiguous — a clean package with a README minimises those delays.
Gerber vs ODB++ vs IPC-2581: which format should I use?
| Format | What it carries | When to use |
|---|---|---|
| Gerber RS-274X | Layer images only; drill separate | Universal, accepted by every fab |
| Gerber X2 / X3 | Images + layer/pad attributes (+ components in X3) | Modern default if your fab supports it |
| ODB++ | Single database: layers, drill, netlist, stackup, components | Higher-mix or assembly-heavy builds; Siemens ecosystem |
| IPC-2581 | Open XML: full fab + assembly data in one file | Vendor-neutral "intelligent" handoff, growing support |
Gerber remains the safest universal choice. Intelligent formats reduce misinterpretation of stackup and netlist, so ask your fab what it prefers and, if in doubt, send Gerber X2 plus drill and ODB++ or IPC-2581.
Common Gerber mistakes that cause fab delays
- Exporting with the wrong units or a coordinate format the drill file doesn't match
- Missing board outline, or outline drawn on a copper layer
- Forgetting paste layers when you need a stencil
- Mixing plated and non-plated holes in one drill file without attributes
- Stale files from a previous revision in the zip — always clear the output folder
- No fab drawing, so stackup, finish and impedance targets are guessed
Where AI-assisted PCB tools fit
AI-assisted design tools such as IntelCAD aim to catch many of these issues earlier — during layout and design review — so that the Gerber package you export reflects a board that already passes manufacturability checks. The Gerber, drill and fab-drawing package itself is still the contract with your manufacturer, so the review steps above still apply.
Frequently Asked Questions
What are Gerber files used for?
Gerber files tell a PCB manufacturer what each layer of the board looks like — copper, solder mask, silkscreen, paste and outline — so they can image, etch and finish the board exactly as designed.
Do Gerber files include drill holes?
Usually not. Holes are normally delivered in a separate Excellon NC drill file. Gerber X2 can describe drill data, but most fabs still expect Excellon drill files alongside the Gerbers.
What file extension do Gerber files use?
Modern tools typically use .gbr for every layer, with the layer named in the filename. Older Protel-style extensions such as .GTL, .GBL, .GTS, .GTO and .GKO are still common and widely recognised.
Can I open Gerber files without PCB design software?
Yes. Free viewers like KiCad GerbView, the Ucamco Reference Gerber Viewer, and most fabricators' online viewers open Gerber and drill files without a full CAD license.
Is ODB++ better than Gerber?
ODB++ carries more information (netlist, stackup, components) in one package, which reduces ambiguity. Gerber is more universally accepted. Neither is strictly better — use what your manufacturer supports, and Gerber X2 is a good modern default.
Sources
Design your next board by describing it.
IntelCAD.ai turns plain-language requirements into schematics and PCBs.
Start Your Design