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 doesn’t automatically redraw the fill zones for certain changes, which can leave them out of sync with your other signals. This can result in the gerbers not matching the design, and ruining your circuit board.

To redraw these, simply use the hotkey b. Kicad will also refresh the fill zones when you run a DRC Check (under Tools > DRC).

When uploading .kicad_pcb files, we’ll handle this step for you.

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 and slots on this layer.

Generate Gerbers

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

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

The Layers list will show the visible layers from the design. These layers should all be checked.

  • F.Silks
  • F.Mask
  • F.Cu
  • B.Cu
  • B.Mask
  • B.Silks
  • Edge.Cuts which contains the board outline.
  • In1.Cu and In2.Cu are also needed for 4 layer designs.

For the users options, we suggest the following. The other options can be set to your preferences.

  • Uncheck Plot sheet reference on all layers. This causes us to be unable to correctly determine board size, and makes uploads likely to fail.
  • Check Exclude PCB Edge from other layers. This ensures that the Edge.Cuts layer doesn’t inadvertently cause shorts to features near the edge.

We suggest checking the Use Protel filename extensions, but it’s not required. Our system will detect all Kicad filenames.

Clicking Plot will show output in green and create gerber files in the output directory.

Plot settings to generate gerbers

Drill Files Generation

Next, click Generate Drill File. The default options will typically work perfectly.

The only important options are

  • Check Decimal Format
  • Uncheck Mirror Y Axis
  • Checking Merge PTH and NPTH Holes into one file is suggested, but not required.

Click Drill File and you should see a message in the bottom text window indicating that new files were created

Correctly configured drill output screen

Verify the Files

Next, click Close to exit the Drill and Plot windows. All of the files should have appeared in your gerbers folder.

Before uploading your files, you may wish to verify the gerbers on your system. We suggest using Gerbv, a have a guide for Verifying your gerbers. Kicad also comes with a tool called GerbView that can be helpful.

If everything looks OK, select all of the files, zip them up, and upload the zip file to oshpark.com.

How the output files should look