How to Export Gerber Files from KiCad 10 for Manufacturing

KiCad has exported perfectly good Gerbers for years, and the process has not changed in KiCad 10 — the 3D model and PDF work got the attention in that release, not plotting. What trips people up is not the dialog, it is knowing which layers a fabricator actually needs and which two settings matter.

This covers the PCB Editor in KiCad 10. The same steps work in 8 and 9.

Step 1 — Open the plot dialog

In the PCB Editor, use File → Fabrication Outputs → Gerbers (.gbr). File → Plot… opens the same dialog if that is the route you know.

Set an output directory before anything else. A dedicated empty folder per revision saves a lot of confusion later — Gerber sets from two revisions in one folder is a genuinely common cause of a wrong board being built.

Step 2 — Choose the layers

For a standard two-layer board you need exactly these:

• F.Cu and B.Cu — the copper. Without these there is no circuit.
• F.Mask and B.Mask — soldermask openings.
• F.Silkscreen and B.Silkscreen — the printed legend.
• Edge.Cuts — the board outline. This is the one people forget, and it is the one that matters most.
• F.Paste and B.Paste — only if you need a stencil for assembly.

Leave the rest off. F.Fab, B.Fab, User.Comments and the courtyard layers are for you and your assembler, not for the fabricator, and including them occasionally confuses an automated import.

Why Edge.Cuts is the layer that matters

The outline defines the physical board. Without it a fabricator cannot know where to route the profile, and any automated quoting system has to guess your dimensions from the extent of the copper — which is always smaller than the real board.

A missing outline is the single most common reason an upload comes back with dimensions that look wrong. If your quote says your board is smaller than you drew it, check that Edge.Cuts was plotted.

Draw the outline as a single closed loop on Edge.Cuts. Loose, unconnected arcs are common in imported designs and leave the outline open, which some checks cannot interpret at all.

Step 3 — The two settings that matter

Most of the plot options can be left at their defaults. Two are worth a decision:

• Plot on all layers / plot board edge on all layers — helpful, because it gives every layer a common reference and makes misalignment obvious to a human reviewing the set.
• Use Protel filename extensions — this changes naming from board-F_Cu.gbr style to board.GTL, board.GBL, board.GTS. Both are accepted. The KiCad default is arguably safer because each file gets a distinct name rather than sharing one stem and differing only by extension.

Leave the format as Gerber. There is no benefit to plotting PDF or SVG for a fabricator, and a PDF is not a manufacturing file however much it looks like the board.

Step 4 — Generate the drill file

Click Plot, then Generate Drill Files… in the same dialog. This is a separate step and it is skipped surprisingly often — a Gerber set with no drill file describes a board with no holes.

Sensible settings:

• Format: Excellon. This is what every fabricator expects.
• Units: millimetres.
• Drill origin: absolute, unless you have a specific reason to use the auxiliary axis. If you do use the aux origin, use it for the Gerbers too — mixing the two shifts your holes relative to your copper.
• Plated and non-plated holes: either merged into one file or written separately is fine. Just include whatever it produces.

Generate the map file only if you want a human-readable drill drawing. It is not required.

Step 5 — Check before you send

Open the output folder and confirm you have copper, mask, silkscreen, an outline and at least one drill file. If the folder has fewer than seven or eight files for a two-layer board, something did not plot.

Then view the set. KiCad ships GerbView, and using it takes a minute: open the Gerbers and the drill file together and look at the board as the fabricator will receive it, not as your layout tool draws it. Plenty of mistakes are invisible in the PCB editor and obvious in a Gerber viewer.

Step 6 — Zip the folder

Put the whole output folder into a single ZIP. Do not rename the files inside — the names carry the layer meaning, and renaming them is how a copper layer ends up interpreted as silkscreen.

Do not upload a subset. A partial set does not fail loudly; it renders as a plausible but wrong board, which is far worse than an error.

Upload that ZIP on the order page and you will get dimensions, a design check and a price in a few seconds. If anything is missing from the set, you will be told which layer rather than left guessing.