OSH Park Docs
Eagle: Generating Customized Gerber Files
Let’s say you just designed a board in Eagle, and want to have it fabricated, but you want to customize the layers. For example, you want to modify the silkscreen so it has the copper layer on it, for easier trace debugging.
To do this, you’ll need to run a custom CAM job to generate custom manufacturing files.
- Download the appropriate CAM job for your Eagle version and type of board. You can also use our Eagle Tools installer, which will select the correct files for you.
Due to a change in how Eagle 7.2 generates Excellon drill files, we now provide two sets of CAM files, which are not interchangeable. Users upgrading to Eagle 7.2 from a new version of Eagle will need to also upgrade their CAM file to avoid drill file issues when generating gerbers.
This issue does not affect Eagle BRD files uploaded to oshpark.com, only gerbers produced and submitted in a zip file.
- For Eagle 7.1, Eagle 6, and Eagle 5:
- For Eagle 7.2 and newer:
Open your board in Eagle.
Run the “CAM Processor”, File -> CAM Processor.
Open the CAM job from step 1. File -> Open -> Job, and select the LaenPCBOrder.cam
Each tab across the top of the window corresponds to one of the files (“gerber files”) used in manufacturing your board. “Top Layer” defines what gets etched into the copper. ”Top Soldermask” defines what gets exposed through the soldermask. ”Top Silkscreen”– you guessed it– defines what is printed on your board.
As an example, add ”tValues” to the “Top Silkscreen” file. Select the “Top Silkscreen” tab, and activate “tValues”.
Run the CAM job to generate gerbers. Click the “Process Job” button. This will generate a bunch of files ending in “.ger” and one ending in “.xln”
You may also see a files ending in “.gpi” and “.dri” but these are Drill Station Info and Gerber Plotter Info files, which we don’t need. You can ignore them.
Zip them all up, and upload them to OSHPark.com! :D