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.

Design Rule Setup

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.

Downloadable Files

Most users will want to download our Eagle Design Rules files and import them into your design. This helps ensure your design can be properly fabricated without issue.

We highly recommend you correct any Overlap and Clearance issues before uploading a board. These indicate signal traces being too close, and may cause your design to fail. We also suggest correcting Dimension errors, which indicate that a pad or trace is too close to a board edge.

You can ignore Stop Mask errors. This indicates a section where silkscreen overlaps exposed portions of the board. This is automatically corrected during fabrication, and does not need to be corrected on the design.

Generating Manufacturing Files

We accept Eagle .brd files directly, so generally you will not need to generate the manufacturing files.

If you do want to generate gerbers, see our Generating Gerber Files page for a guide, and CAM setup files. This ensures you don’t encounter problems with formats or filenames.

Board Outline

We need a watertight board outline drawn on the Dimension Layer. In order to prevent errors in your board size and expected edge placement, do not include other data on the Dimension layer. Common mistakes include text notes, extra lines, or measurements.


When using gerbers generated from Eagle, note that some CAM jobs do not generate filenames and layers that our system can detect.

If you have the original design files, consider uploading the .brd or Generating Gerber Files using our CAM configuration. The most common error is a missing board outline, but you can use GerbV to Create A Board Outline


When using gerbers generated from Eagle, it’s important to have the correct drill format.

If you have the original design files, this can be resolved by uploading the .brd or Generating Gerber Files using our CAM configuration.

Drill file format errors can occur in one of two ways:

  • Using an old CAM job on Eagle 7.2 or newer. This results in the drill file being in a 2:5 format instead of 2:4 which we use. This can be easily modified using GerbV to Change Drill Formats
  • The drill file was generated as a Drill Symbols file, and containing symbols such as X,[] and O. These files do not contain precise drill locations, and cannot be used for fabrication.


Slots can be indicated as shown on the Eagle Slots page.

Typically you’ll want to use the Dimension layer for unplated slots, and the Milling layer for slots. This is due to the Dimension layer interacting with Polygons and the DRC tools, where the Milling layer does not. For more details, see our Eagle Layers Explained page.

We have an example slots.brd file that indicates both plated and non-plated slots in a way that will be fabricated correctly. Make sure to use the Layers menu and turn on all the layers, since Eagle has several turned off by default.

For slots on 4 layer designs, Eagle will not automatically isolate copper pours around the slot on the internal layers. The simplest way to ensure the correct isolation is to manually draw traces or pads trace beneath the slot, using the same signal name as the slot itself.

Common Issues

Info about Eagle layers

Eagle has a large number of layers. Our Eagle Layers Explained page explains how those layers are used by Eagle, designers, and fabricators.

Ground plane polygons

Eagle uses the Width property of polygons for several purposes. In general, you should ensure the Width property is 6 mil (0.006”) or larger.

During Gerber output, Eagle draws each Polygon as a sequence of lines, each one as wide as the Width property. When the Width is very small or 0, Eagle draws hundreds or thousands of lines. This is incredibly slow, and may cause BRD file uploads to fail in unexpected ways as a result.

When calculating copper pours, Eagle also uses the Width property to determine the smallest “valid” width of a wire connection. This is true even if the Width is below the DRC requirements, and will not generate DRC warnings. As a result, a small Width on a copper pour can cause errors where a ground plane is split into multiple segments, or connected by thin traces that violate design rules.

Lastly, the Width is used to determine the line width for “thermals” connecting to any vias, headers, or pads. With a small or zero-width polygon, it’s possible for these thermals to be removed entirely in fabrication, resulting in failed or insufficient connections throughout your board.

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 unwanted items on the Dimension layer to the tDocu layer, since the tDocu layer is not used for fabrication. In many cases, you can also select a different footprint that does not contain the holes.

Text on previews does not match Eagle’s UI

By default, Eagle is configured to use different fonts during PCB layout and the gerber CAM process.

You can correct this by enabling Options > User Interface > Always Vector Font. This option will force Eagle to use the same font in the Eagle board user interface. Once this option is enabled, text size and placement will be consistent on the gerbers and board layout.

Importing logos and images

Imported images can be problematic to fabricate without special care.

Our Importing Bitmaps guide will help you configure and verify your images so they can be fabricated reliably.