A Gerber file is a vector image of one PCB layer, such as top copper, bottom solder mask or the board outline, written in an open text format maintained by Ucamco. A fabricator needs one Gerber file per layer, plus drill files, a board outline and a fabrication drawing or notes that say what the board is made of. Export in Gerber X2 (or plain RS-274X if your tool cannot), keep the same units, origin and orientation on every file, put plated and non-plated holes in separate drill files, and check the package in an independent viewer before you send it. This guide lists what a complete package contains, how to export it, what to check, and when to send ODB++ or IPC-2581 instead.
1. What Is a Gerber File?
| What it is | A text file describing the 2D image of one PCB layer with apertures, coordinates and draw/flash commands |
| Maintained by | Ucamco (Gerber format specification, revision 2026.05) |
| Versions | RS-274X (extended Gerber); X2 adds attributes such as layer function and polarity; X3 adds component information for assembly |
| Obsolete version | RS-274D, which needed a separate aperture list; do not send it |
| What it does not contain | Material, thickness, copper weight, finish, stackup or tolerances; those go on the drawing or in a job file |
Because each file is just an image of a layer, the fabricator must know which file is which and how they stack. X2 attributes state this inside each file; with RS-274X you rely on file names and a README.
2. What Files Make Up a Complete Package?
| File | Needed for | Notes |
|---|---|---|
| Copper, one per layer | Every board | Include inner layers and planes; state positive or negative plane polarity |
| Solder mask, top and bottom | Every board with mask | Openings shown as drawn features |
| Legend (silkscreen), top and bottom | If used | |
| Solder paste, top and bottom | Assembly, stencil | Not needed for bare boards, but harmless |
| Board outline / profile | Every board | One closed outline; keep dimensions and title blocks out of it |
| Drill files | Every board with holes | Separate plated (PTH) and non-plated (NPTH) files; one file per drill span for blind or buried vias |
| Fabrication drawing or notes | Every board | Stackup, material, thickness, copper, finish, mask color, IPC class, impedance, special requirements |
| Gerber job file (.gbrjob) | Optional | Machine-readable stackup and board data in the same Gerber family |
| IPC netlist (IPC-D-356) | Recommended | Lets the fabricator compare the copper to your intended connections and set up electrical test |
A 2-layer board therefore has at least copper, mask and outline files for each side, a drill file and notes. Multilayer boards add one copper file per inner layer and, for HDI, one drill file per via span.
3. How Do You Export Gerber Files?
The menu differs by tool, but the settings that matter are the same:
- Format: Gerber X2 if available; otherwise RS-274X.
- Units and resolution: pick mm or inch and use the same for every layer and the drill files; use enough decimal places for your smallest feature (Ucamco recommends 6 decimals in mm).
- Origin and orientation: all files must share the same origin and axis direction, viewed from the top. Do not mirror bottom layers.
- Drill output: Excellon or Gerber drill, with PTH and NPTH in separate files, and finished hole sizes in the drill table.
- Outline: export the board profile as its own file.
- Netlist: export IPC-D-356 if your tool supports it.
In KiCad this is File > Fabrication Outputs (Gerbers and drill files); in Altium, Fabrication Outputs; in other tools, the CAM or manufacturing output menu. Save the export settings as a template so every release uses the same ones.
4. How Do You Check the Package Before Sending It?
Open the exported files in a viewer that did not create them, such as Ucamco’s free Reference Gerber Viewer, KiCad GerbView or gerbv, and check:
| Check | What goes wrong if you skip it |
|---|---|
| All layers load and line up | A unit or origin mismatch puts holes off their pads |
| Drill overlay sits centered on pads | Wrong drill format or scale |
| Every layer is present, including inner planes | Board cannot be built; query delays the order |
| Mask openings on every pad that needs one | Pads covered by mask |
| Plane layers show the right polarity | Negative planes read as positive, or the reverse |
| Outline is one closed path | Wrong board shape or routing path |
| File list matches the README or drawing | Fabricator guesses layer order |
Compare against your design rules too: the viewer shows what will be built, not whether it is buildable.
5. What Should the Fabrication Notes Say?
Gerber files show the image; the notes say how to build it. Include:
- Layer order with the file name for each layer.
- Material (or minimum Tg/performance), finished thickness and tolerance.
- Copper weight per layer.
- Surface finish, mask and legend colors.
- Impedance targets with layers and reference planes.
- Hole types: via filling or tenting, back-drilling, press-fit tolerances.
- Acceptance standard and class, for example IPC-6012 Class 2.
- Quantity, panel requirements and any special tests.
IPC’s checklist for producing rigid printed board assemblies lists the data a fabricator and assembler need and maps it to the IPC-2610 series of documentation standards. Our PCB fabrication tolerance guide covers how to write tolerances.
6. Gerber, ODB++ or IPC-2581?
| Format | Structure | Strengths |
|---|---|---|
| Gerber X2 + drill + notes | One file per layer | Universally accepted; simple; open specification |
| ODB++ | Single archive with layers, drills, stackup, netlist and components | One package; widely supported |
| IPC-2581 | Single XML file | Open IPC standard covering fabrication, assembly and test data (IPC-2581C contents) |
Every fabricator accepts Gerber. ODB++ and IPC-2581 reduce the chance of a missing layer or a mismatched note because everything is in one file, which helps on complex multilayer and HDI boards. If you send one of them, many buyers send Gerber files as well, and you should say which one controls if they differ.
7. What Mistakes Cause Engineering Queries Most Often?
- Missing inner layers or drill files for blind/buried spans.
- Units or decimal format different between copper and drill files.
- PTH and NPTH holes in one file, so the fabricator cannot tell which to plate.
- Board outline mixed with dimensions or drawn as unconnected segments.
- No stackup or material information.
- Negative plane layers without a note.
- Old files left in the folder from an earlier revision.
Each one stops the job until someone answers a question. Clean data also avoids extra engineering time; our guide to NRE and setup costs explains how that shows up in a quote. A free DFM check before you order catches them.
How Can We Help?
Send your Gerber X2 or RS-274X files, drill files and notes, or an ODB++ or IPC-2581 package; we check the data and quote within 2 hours for bare boards. For prototypes, see our rapid PCB prototyping service; we build multilayer PCBs up to 40 layers, and new customers get 2–4 layer FR-4 prototypes free.
Conclusion
A complete Gerber package is one file per layer, separate PTH and NPTH drill files, a closed outline and fabrication notes stating stackup, material, thickness, copper, finish and acceptance class. Export in X2 with consistent units and origin, check the files in an independent viewer, and add a netlist. For complex boards, ODB++ or IPC-2581 puts everything in one file. Contact us with your files for a quote.
FAQ
What is a Gerber file? A text file that describes the image of one PCB layer; a set of them, plus drill files and notes, tells a fabricator how to build the board.
How many Gerber files does a 2-layer PCB need? Typically top and bottom copper, top and bottom solder mask, top and bottom legend if used, and an outline, plus drill files and notes.
What is the difference between RS-274X and Gerber X2? X2 is RS-274X with attributes that identify each file’s function, polarity and other properties, so the fabricator does not have to guess.
What program opens Gerber files? Free viewers include Ucamco’s Reference Gerber Viewer, KiCad GerbView and gerbv.
Should I send ODB++ instead of Gerber? If your tool exports it, ODB++ or IPC-2581 puts all data in one file; many buyers send Gerber files too.
Upload your files today · Free DFM check before production · Ship worldwide
Get your PCB prototypes in as fast as 24 hours. We handle FR4, Rogers, and hybrid boards up to 40 layers in volume production, with advanced builds subject to engineering review — free prototypes for 2–4 layer FR-4 boards, no minimum order.
Just upload your Gerber + BOM — we source every part, assemble, and inspect (AOI + X‑Ray) so you don't have to chase suppliers. PCB assembly typically takes 5–8 working days once all components are in stock. The confirmed delivery schedule is subject to your quotation.