How to generate Gerber and Drill files from Eagle

Autodesk Eagle version 9.2 onwards:    

Good and bad news with the new Eagle version; first the bad news. A new *feature* has been introduced that includes negative polarity support. This means that by default, the solder mask layers are output in negative polarity. This option can be turned off, but it can be dangerous if missed.

The good news is the new Eagle has the Seeed Fusion CAM files built-in! And they are not affected by this problem. So please DO NOT use the default CAM options in Eagle with the Seeed Fusion service.

Please ignore the CAM file description, the CAM files were produced for version 8.6 onwards but were only implemented in version 9.2 onwards.

Autodesk Eagle version 8.6 to 9.1:  

Eagle has changed the export process and CAM file format again! At the moment, the best solution seems to be to update to Eagle version 9.2 and use the built-in Seeed Fusion CAM file. But if you insist on using version 8.6 to 9.1, please use the built-in OSH Park CAM files to export the manufacturing files and change the format to RS-274x.

Please be aware that this CAM file only exports the "Board Shape" and "Cutouts" Eagle layers to the outline/mechanical Gerber layer. This means if you have drawn any milling or v-cuts in the dimension or milling layers then you will need to select these in the "Board Outline" layer settings too.

Select the little stack icon to add the necessary layers.

Thank you!

Updated 2018/10/10


For Autodesk Eagle version 8.5 or earlier

The process for generating all the necessary manufacturing files is very simple in Eagle, and different to most other design software. You can use a CAM Job file to export them for you. These files are pre-configured by Seeed to ensure that all the necessary files will be exported from your design, in the correct format, to place an order in Seeed Fusion.

For 2 layer boards, click here.
For 4 layer boards, click here.

Open your design in Eagle and find the CAM icon, this will bring up the CAM Processor.

In the new window, open the CAM file by going to File -> Open -> Job

Locate the correct CAM file for your boards and open it. Please make sure you are using the Seeed CAM file, the default Eagle 274 files will not export the files correctly and may result in errors.

The CAM file will export all the required layers, including the drill file in Excellon format and will label the files with our preferred extensions. Click Process Job to begin the export process.

The manufacturing files will be exported in the same location as your design files. Please check that the ten manufacturing files have generated. Place these into an archive and upload this onto the Seeed Fusion order page. We recommend that you give the files a quick check using the online Gerber Viewer before confirming the order.

Common Mistakes and Problems:

- The board outline and any cut-outs, v-cuts and milling should be drawn in the Dimension or Milling layers (layers 20 and 46 respectively).

- If you find the files have not generated correctly please try these solutions:
  • Try again, an error may have occurred during the export process.
  • Make sure you have loaded the Seeed CAM file and not a different one.
  • Check that the CAM file is still configured correctly. See below.
  • Check that all the layers are present and designed correctly in your Eagle design files. 
- Please do not use the 4 layer CAM file if your boards are only 2 layer and vice versa. We do not have a CAM file for single layer boards. For single layer boards, please use the 2 layer CAM file and then delete the data for the extra side e.g. GBL, GBS, GBO etc.

- If the PCB was not designed in Eagle then you may have problems getting all the data correctly exported. Please check all the that the necessary information is located in the Eagle layers below. You may need to select other layers in the CAM file if your data is located in non-standard Eagle layers.

- If you cannot download the CAM file from our website, you can manually create the CAM job file with the settings below. Please pay attention to the areas highlighted:
  • Gerber Files: Change the device to GERBER_RS274X and create the layers shown in the table below. The name of the Section is for your own reference and can be changed to whatever you want. You can add additional layers by clicking Add. Note that milling data located only in the Milling layer (layer 46) will be exported in the files. Please ensure that all milling is included in either the milling or dimension layers.

  • Drill File: Change the Device to EXCELLON, type in %N.TXT for the file extension and select layers 44 and 45. Save the job and you can use it to export all your designs. 

  • Required files and corresponding layers:

  • For four layer boards and greater, add the inner layers using the following format:

- Last modified 2018/08/14

Feedback and Knowledge Base