Generating Gerbers

Before you get started, you can upload .kicad_pcb files directly and we’ll generate the gerbers for you. For most users, this is the best way to order a board designed with KiCad.

Please email us at [email protected] if you’re having any trouble!

First Steps

Redraw Fill Zones

KiCad typically will redraw Fill Zones when performing changes, checking DRC, or exporting gerbers. This can also be done by using the hotkey b, or using the menu at Edit > Fill All Zones.

When uploading .kicad_pcb files, we do not re-fill zones, and export according to the last re-fill performed by the user.

Board Outline

We look for the board outline on the Edge Cuts layer to tell the fab where to cut the board. You can also indicate cutouts on this layer.

Generate Gerbers

Select File -> Plot from the menu to open the gerber generation tool.

After plotting, Kicad saves the used settings in the .kicad_pcb file. We’ll honor user-adjustable settings when handling uploaded .kicad_pcb files.


It’s suggested to set the Output directory: to plots or gerbers. This will help keep the gerbers separate from the design files.

Include Layers

These layers are typically required to fabricate the design as intended:

  • F.Cu
  • B.Cu
  • F.SilkScreen
  • B.SilkScreen
  • F.Mask
  • B.Mask
  • Edge.Cuts which contains the board outline.
  • In1.Cu and In2.Cu for 4 layer designs
  • In3.Cu and In4.Cu for 6 layer designs

Paste layers are suggested, but optional.

  • F.Paste
  • B.Paste

Other layers are optional, and will not be read by our service.

Plot On All Layers

All layers in this section must be unchecked. These options merge multiple production layers together, and will typically result in non-functional PCBs.

Because this mangles the gerber output directly, these errors will not be detected by Kicad’s DRC.

General Options

These options can be set to user preference/design intent, and do not affect manufacturability or our file processing.

Gerber Options

Leaving as default is recommended for most users, but may be changed in some circumstances.

  • Use Extended X2 Format (recommended) Leaving checked is recommended. This provides fab layer metadata, making file handling much more robust.
  • Disable Aperture Macros (not recommended) Unchecked is typically suggested. However, checking this option can resolve issues with some complex footprints, typically pads with complex artistic shapes, or multiple rounded corners.

Drill Files Generation

Next, on the plot screen, select Generate Drill File.

Output Folder typically should match the one provided to the Gerber output screen.

Note We plan on adjusting drill handling shortly to better support Kicad 7’s new defaults and options. The following steps will generate legacy drill outputs which are known to work reliably with our current process. At this time, other options will result in slots not being detected.

Drill File Format

  • Mirror Y Axis Must be unchecked.
  • Use Alternate Drill Mode must be checked.

Map File Format

User preference / optional. We do not read this file.

Drill Origin

  • Absolute should be checked.

Drill Units

both Inches and Millimeters works without issue.

Zeroes Format

  • Decimal Format is preferred.