OSH Park Docs
Generating KiCAD Gerbers
Generating gerbers can be intimidating for new Kicad users. Don’t worry! This guide will help you get all your files in order.
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@example.com if you’re having any trouble!
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.
.kicad_pcb files, we’ll handle this step for you.
Plot from the menu to open the gerber generation tool.
It’s suggested to set the
Output directory: to
gerbers. This will help keep the gerbers separate from the design files.
The Layers list will show the visible layers from the design. The layers that are checked are the ones we need to be able to manufacture a two-layer design.
For the users options, we suggest the following. The other options can be set to your preferences.
Plot sheet reference on all layers. This causes us to be unable to correctly determine board size, and makes uploads likely to fail.
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.
Plot will show output in green and create gerber files in the output directory.
Drill Files Generation
Generate Drill File.
Use the same output folder as for the gerbers, which should be the default. We want the drill file to be in decimal format with absolute coordinates and 2:4 precision. The specific options are shown in the image below.
It’s advised to select
Merge PTH and NPTH Holes into one file, but it’s not required. We’ll automatically detect and merge these if you forget.
Drill File and you should see a message in the bottom text window.
Verify the Files
Close to exit the Drill and Plot windows. All of the files should have appeared in your gerbers folder.
KiCAD comes with a gerber viewer called GerbView but we know our system matches another program called GerbV exactly. We recommend downloading GerbV and looking at each gerber file there.
If everything looks OK, select all of the files, zip them up, and upload the zip file to http://oshpark.com.