How to Export Gerber Files from KiCad (Step by Step)

Gerber files are the manufacturing images for each PCB layer: copper, solder mask, silkscreen, board outline, and related fabrication data. KiCad can generate those files directly from the PCB Editor, but the package is only useful if the plotted layers and Excellon drill files describe the same board.

Exporting correctly matters because the manufacturer builds exactly what the files say, not what the KiCad screen looked like during layout. Before you order boards, export the package, zip the output folder, and open the viewer to check the outline, layer alignment, and drill registration.

KiCad's Plot dialog is more explicit than EasyEDA's one-click ZIP but lighter than professional output-job systems. If you also work in a browser EDA tool, the EasyEDA Gerber export guide shows the more automated version of the same manufacturing package.

Step-by-step KiCad Gerber export

1. Open the board in KiCad PCB Editor. Start from the PCB layout, not the schematic editor, because Gerbers are generated from the placed and routed board.
2. Choose File → Plot. In KiCad 7, 8, and 9, the Plot command is available from the PCB Editor File menu. Older KiCad references may describe this as a fabrication output command, but the mainstream current flow opens the same Plot dialog.
3. In the Plot dialog, set Plot format to Gerber. Choose a dedicated output directory such as gerbers/ inside the project folder so the final ZIP does not accidentally include source files or old outputs.
4. Select the fabrication layers needed for a normal two-sided board: F.Cu, B.Cu, F.Mask, B.Mask, F.Silkscreen or F.SilkS, B.Silkscreen or B.SilkS, and Edge.Cuts. Include F.Paste and B.Paste only when you need stencil or assembly paste data.
5. Enable Use Protel filename extensions if you want conventional file names such as .gtl, .gbl, and .gto. If this is disabled, KiCad may use more generic Gerber names, which are valid but less obvious to inspect by filename.
6. Leave Generate Gerber job file enabled when your manufacturer accepts it. The job file adds stackup and layer metadata; it does not replace the actual layer Gerbers.
7. Use a coordinate format accepted by modern board houses. A common KiCad setting is 4.6. Keep units and format consistent with the drill export so the board outline and hole locations stay aligned.
8. Use extended X2 format can remain enabled for most current manufacturers. If a board house specifically requests older RS-274X without X2 attributes, follow its CAM instructions.
9. Click Plot. KiCad writes one Gerber file per selected layer into the output directory.
10. In the same Plot dialog, click Generate Drill Files. Set the drill format to Excellon. Choose whether PTH and NPTH drills should be merged or separate according to the manufacturer requirement; both are common, but the files must be included in the final ZIP.
11. Use absolute drill origin for a normal export unless your manufacturer asks for an auxiliary origin. Choose units that match your fabrication notes, then generate the drill file.
12. Review the output directory. It should contain copper, mask, silkscreen, outline, and drill files. Zip the contents of that output directory, not the parent KiCad project folder.

KiCad export details worth checking

KiCad gives you direct control over layer selection, which is useful but also makes it easy to omit one checkbox. For a simple two-layer PCB, compare the selected Plot layers against the physical order form: copper on both sides, solder mask on both sides, silkscreen only where you actually printed legend artwork, and Edge.Cuts for the profile. Paste layers are a separate decision; include them when the package is also being used for stencil or assembly work.

The drill step is the other place where KiCad-specific choices matter. If the board has non-plated mounting holes, make sure the PTH and NPTH setting matches the manufacturer's upload rules and that every generated drill file goes into the ZIP. KiCad can also emit a Gerber job file with layer metadata. Keep it when accepted, but remember it supports the layer files rather than replacing copper, mask, outline, or Excellon drill data.

KiCad layer and extension reference

Common mistakes to avoid

• Leaving Edge.Cuts unchecked in the Plot dialog. KiCad may show the board outline in the editor, but it will not appear in the fabrication ZIP unless it is plotted.
• Clicking Plot and closing the dialog before using Generate Drill Files. Copper annular rings are not enough; vias and through-hole pads need Excellon coordinates.
• Switching to an auxiliary drill origin for one export and forgetting to use the matching Gerber origin. This is a common way to create a package where every hole is shifted by the same offset.
• Sending F.Paste or B.Paste for a bare-board-only order and then confusing those files with solder mask. Paste layers describe stencil apertures.
• Reusing an output directory after removing layers from the board. Old.gbr files can remain beside the new plot unless you use a clean folder.
• Dropping the NPTH drill file when PTH and NPTH are generated separately. Mounting holes, tooling holes, and some slots may only be represented there.

Verify your Gerbers before ordering

Open the zipped KiCad output folder in the Gerber viewer before uploading it to a manufacturer. Confirm that every checked Plot layer appears, especially Edge.Cuts, and that the Excellon drill file or files load with the copper layers. Pads, vias, mounting holes, and slots should all share the same origin.

KiCad-specific problems are usually easy to see visually: a missing board outline, stale files from a previous plot, pasted stencil layers included by accident, or NPTH holes absent from the archive. If the bottom side looks mirrored, compare bottom copper, bottom mask, and bottom silkscreen together rather than judging a single layer in isolation.

FAQ

Should I use Protel filename extensions in KiCad?

Most PCB manufacturers accept either KiCad generic .gbr names or Protel-style extensions, but Protel extensions such as .gtl and .gbl are easier for humans and CAM systems to recognize. Enabling the option is a good default unless your manufacturer asks for a different naming convention.

Do I need to export paste layers from KiCad?

Export F.Paste and B.Paste when you are ordering a stencil or providing assembly data. For bare PCB fabrication only, paste layers are usually not required, and including them can confuse a package if they are mislabeled.

What drill origin should I use in KiCad?

Use the absolute drill origin for a normal fabrication package unless your manufacturer specifically asks for an auxiliary axis origin. The Gerber and drill files must use the same origin so holes line up with pads.

Is Gerber X2 required for KiCad exports?

Gerber X2 adds layer and job metadata, and many manufacturers support it. It is not strictly required for a basic RS-274X package, but leaving extended X2 output enabled is generally fine when your board house accepts it.