How to Export Gerber Files from Altium Designer

Gerber files are the layer-by-layer manufacturing artwork for a PCB. Altium Designer can create them from an active PCB document, but a complete fabrication package also needs NC drill data and a clear board outline layer.

The goal is to export the same stackup that you intend to order: copper, solder mask, overlay, mechanical outline, and drill files. After export, zip the generated output folder and open the viewer to confirm that every manufacturing layer is present before sending the package to a board house.

If you are comparing professional EDA export flows, Altium's direct fabrication output is closest in structure to the film-based process in OrCAD and Allegro PCB Editor, but Altium usually hides more of the CAM setup behind the Gerber Setup and NC Drill dialogs.

Step-by-step Altium Designer Gerber export

1. Open the project and make the .PcbDoc active. Gerber output is generated from the PCB document, not from the schematic or a library document.
2. Choose File → Fabrication Outputs → Gerber Files. This opens the Gerber Setup dialog for the current PCB.
3. On the General tab, set units. Millimeters are a common choice for current fabrication packages. The Format options are 2:3, 2:4, or 2:5. 2:4 or 2:5 covers most modern fabrication; match your manufacturer's spec.
4. On the Layers tab, select the layers to plot. For a two-layer board, that usually includes Top Layer, Bottom Layer, Top Solder, Bottom Solder, Top Overlay, Bottom Overlay, and the mechanical or keep-out layer that defines the board outline. For multilayer boards, include the internal signal or plane layers required by the stackup.
5. Confirm the mechanical layer convention. Altium projects often place the profile on a specific Mechanical layer, while some teams use Keep-Out for fabrication boundaries. Export the layer that actually contains the finished edge and any routed cutouts.
6. Review the Drill Drawing tab if your manufacturer asks for drill drawing or drill guide artwork. The NC drill file is still generated separately, so do not treat a drill drawing as a replacement for Excellon drill data.
7. On the Apertures tab, leave Embedded apertures RS274X checked. This creates self-contained Gerber files with aperture definitions embedded in each layer file.
8. Click OK. Altium generates the Gerber outputs and opens or updates a CAMtastic document so you can inspect the generated CAM layers.
9. Generate the drill file with File → Fabrication Outputs → NC Drill Files. Use the same unit setting and Format selector convention as the Gerber output: 2:3, 2:4, or 2:5 as required by the manufacturer. The NC drill output is the file the fabricator uses for plated and non-plated holes.
10. For production projects, consider creating an OutJob with File → New → Output Job File. Add Gerber Files and NC Drill Files as fabrication outputs, configure them once, and run the Output Job for each release.
11. Find the generated output in the project output directory, commonly under Project Outputs. Zip only the current Gerbers, NC drill files, and any manufacturer-requested fabrication notes.

Altium layer and extension reference

Altium output details worth checking

Altium projects often contain more mechanical layers than the manufacturer actually needs. Before plotting, open the PCB and identify which layer contains the finished contour, which layer contains routed slots, and whether there are assembly or dimension notes that should stay out of the Gerber package. Sending every mechanical layer can be just as confusing as omitting the outline, especially when old board profiles or panel drawings remain in the design file.

For repeatable releases, store Gerber Files and NC Drill Files in an Output Job and regenerate both from the same saved project state. This keeps the drill format, units, and output folder tied to the release process instead of relying on whichever dialog settings were last used on a workstation. Direct export is still useful for quick prototypes, but an OutJob reduces drift when a board goes through several fabrication revisions.

Common mistakes to avoid

• Plotting a documentation mechanical layer instead of the profile layer. If the real outline is on Mechanical 1 and the plotted layer is Mechanical 13, the ZIP may contain notes but no manufacturable edge.
• Running Gerber output and forgetting that NC Drill Files is a separate fabrication command. Pads and vias in copper do not create hole coordinates by themselves.
• Changing Gerber precision without checking the NC Drill dialog. The Gerber and drill format controls use the same 2:3, 2:4, or 2:5 style selector and should follow the same fabrication requirement.
• Assuming Top Overlay is always safe to manufacture. Review reference designators, polarity marks, and logo artwork so they do not cross exposed pads or extend past the board edge.
• Mixing a fresh Gerber set with a drill file left in Project Outputs from an older board revision. Clear the output folder or write each release into a revision-specific directory.
• Treating CAMtastic as the final check only because it opened automatically. Inspect the ZIP you will upload, not just the temporary CAM document created during export.

Verify your Gerbers before ordering

Upload the exact Altium ZIP you plan to send into this browser Gerber viewer and compare the layer list with the output job or Gerber Setup choices. The check should show top and bottom copper, solder mask openings, overlay where you expect legend artwork, a single finished outline, and drill data from the same export run.

Altium errors usually show up as a wrong mechanical layer, a missing drill file, or an old output mixed into the archive. Zoom around connectors, mounting holes, castellations, and routed cutouts. If holes are shifted from pads, regenerate both Gerbers and NC Drill Files after checking units, format, and output origin rather than editing the ZIP by hand.

FAQ

Should I export Gerbers directly or use an OutJob in Altium Designer?

Direct export is fine for a quick package, but an Output Job file is better for repeatable production releases because it stores the fabrication outputs and settings with the project.

Where does Altium Designer put generated Gerber files?

For the normal project flow, Altium writes generated fabrication outputs under the project output directory, commonly named Project Outputs for the project. Check the CAMtastic document and the output folder before zipping.

Which Altium layer should contain the board outline?

Many projects use a Mechanical layer for the routed board outline, sometimes paired with Keep-Out information. Use the layer convention required by your project or manufacturer and make sure that outline layer is included in the Gerber setup.

Are embedded apertures required?

Leave embedded apertures for RS-274X enabled. It makes each Gerber layer self-contained and avoids the separate aperture-table workflow used by older RS-274-D outputs.