How to prepare Gerber files for PCB manufacturing (KiCad, Altium, Eagle)

What the manufacturer needs

A PCB is manufactured from Gerber files (one per layer, RS-274X format) and an Excellon drill file. Together they describe copper, solder mask, silkscreen, the board outline and every hole. Everything else in your project – the schematic, the 3D model, the BOM – is irrelevant for bare-board fabrication.

For a two-layer board the ZIP should contain:

Four-layer boards add two inner copper layers (*.G1, *.G2 or *-In1_Cu.gbr, *-In2_Cu.gbr).

KiCad

1. File → Fabrication Outputs → Gerbers. Select the copper layers, F.Mask, B.Mask, F.Silkscreen, B.Silkscreen and Edge.Cuts.
2. Tick Use Protel filename extensions (optional, but every manufacturer recognises them) and Subtract soldermask from silkscreen.
3. Leave Plot reference designators on if you want them on the board; keep Plot footprint values off.
4. Click Generate Drill Files: Excellon format, PTH and NPTH in a single file, units in millimetres, decimal format.
5. Zip the whole output folder.

Altium Designer

1. File → Fabrication Outputs → Gerber Files. Units mm, format 4:4, plot every mechanical layer that carries the outline.
2. File → Fabrication Outputs → NC Drill Files, same units and format.
3. Altium places the outline on a mechanical layer (Mechanical 1 or the dedicated Board Outline layer). Make sure that layer is exported – a missing outline is the most common reason for a DFM hold.
4. Zip the Project Outputs folder.

Eagle / Fusion 360 Electronics

Use the built-in CAM processor with the Gerber RS-274X job that ships with recent versions. It writes all layers and the Excellon drill file into one folder.

The five things that go wrong

• No outline layer. Without a closed contour the manufacturer does not know where to rout. Our viewer warns about it before you order.
• Outline drawn on a copper layer. The router would cut through copper. Keep the outline on its own layer.
• Drill file in a different unit or offset. Export Gerbers and drills with the same origin and units.
• Silkscreen over pads. Enable subtract mask from silk so text does not end up on solder pads.
• Old files in the ZIP. Delete the output folder before re-exporting so stale layers cannot sneak in.

Check it before you order

Upload the ZIP in our PCB configurator. The viewer renders the top and bottom side, detects the outline and the drill file and shows the board dimensions – if something is missing you will see it before paying anything.