CADSoft Eagle

The website will accept Eagle .brd files directly, so unless you know you need something special, it’s best to just upload the .brd file and let the website figure out what it needs.

OSHPark plugins for Eagle

We are happy to provide some basic Eagle Tools. This set of tools add instant-upload right inside Eagle, and contains an updater to help keep your OSHpark CAM and DRC files current.

Design Rules and CAM Jobs

We provide Eagle Design Rules files and we highly recommend you clear any overlap, dimension, and clearance issues before uploading a board. You can ignore DRU errors on the tStop and bStop layers since we automatically prevent silk from being placed on exposed copper.

We do provide CAM jobs to generate and submit gerbers. We also have instructions on how to generate custom gerbers if you want to do something different, such as add tValues to your silkscreen.

Board Outline

We need a watertight board outline with lines that are at least 6mil wide on the Dimension layer (Layer 20) so we can calculate your board area and tell the fab where to cut.

You can also indicate cutouts and slots as well as mounting holes on this layer. The system will charge you for the smallest rectangle that encompasses everything on the Dimension layer, so don’t include text (except CUT OUT text in slots) or measurement lines.

We have a slots.brd that you can use to look at how we want the plated and unplated slots called out so they’ll be manufactured correctly. When you open the file, make sure to use the display all command or click on the Layers menu and turn on all the layers.


We need the drills exported in EXCELLON_24 format. We handle this automatically if you upload a .brd file, but please be sure and grab the correct version of the CAM job if you’re generating gerbers! Eagle changed their default export in Eagle 7.2 so the site will return an ‘Internal Error’ when you try and upload gerbers generated by the Eagle 6 CAM job using Eagle 7.2 or newer.

Minor Stuff

Ground plane polygons

It’s best for our system to keep the ‘width’ of polygons to 0.006 inches (6 mils) or larger. If you make them zero, Eagle will generate overwhelming numbers of coordinate points to try and simulate a zero-width line. This can cause the upload to fail with an ‘internal error’ message.

Also, we recommend keeping the polygon edges at or just inside the board outline, especially with non-rectangular outlines. If they’re too far away from the board outline, they get trimmed away when we place your design on the panel and you’ll end up with no copper pour on that layer.

Non-plated holes past the board edge

Eagle generates circles on the Dimension layer for any non-plated holes, which our system considers to be part of the outline. While this won’t affect fabrication, it will result in our system charging you more for the board.

This error is most commonly seen on T0-220 and Arduino Uno packages. If the Arduino or T0-220 package sticks out past the board edge, we suggest you edit the footprint to move everything from the ‘Dimension’ layer to the ‘tDocu’ layer, since we don’t use the tDocu layer when we generate gerbers.

Silk text placement on the previews doesn’t match the .brd file

This is due to Eagle defaulting to a different font in the UI than it uses for gerber generation. You can correct this by enabling Options > User Interface > Always Vector Font. Checking this option will force Eagle to use the same font in the Eagle board user interface.

Importing logos and images:

Follow our instructions on how to import bitmaps at less than 400 dots per inch (DPI) so they’ll be recognized and fabbed correctly with our process.

Info about Eagle layers

We have a page covering the different Eagle layers and how they’re interpreted by the fab.