How to Export Gerber Files from EAGLE (Autodesk / Fusion Electronics)

Gerber files are the artwork layers a PCB manufacturer uses to build copper, solder mask, silkscreen, and the board outline. In Autodesk EAGLE and Fusion Electronics, those outputs are created from the board file with the CAM Processor.

The important detail is that the CAM job controls which EAGLE layers become which manufacturing files. After processing the job, zip the generated Gerbers and drill output, then open the viewer to confirm that the Dimension layer, copper, mask, silkscreen, and holes all landed in the expected places.

EAGLE remains popular for small and hobbyist boards. If you are moving between browser and desktop tools, compare this CAM-job workflow with the simpler ZIP download described in the EasyEDA Gerber export guide; the manufacturing layers are similar, but EAGLE asks you to inspect the layer mapping more directly.

Step-by-step EAGLE Gerber export

1. Open the finished .brd board file. Gerber export must be done from the board layout because the schematic does not contain the routed copper, outline, or drill locations.
2. Run a design rule check before exporting. This is not a Gerber command, but it catches clearance, width, and board-shape problems while you can still fix the layout.
3. Choose File → CAM Processor, or use the CAM Processor button in the EAGLE toolbar. In modern EAGLE 9.x and Fusion Electronics, the CAM Processor uses a redesigned job-based interface. Older EAGLE versions used a more separate legacy CAM dialog, but the output concept is the same.
4. Load a CAM job. A normal choice is the built-in default CAM job, or a manufacturer-supplied v9 .cam file. gerb274x.cam is the legacy RS-274X job used in older EAGLE flows, not the newer EAGLE 9 CAM Processor job workflow. Manufacturer jobs are useful when the fabricator expects exact file names or extra drill/routing outputs.
5. Inspect the job sections. The top copper output should include Top and related pad/via data. The bottom copper output should include Bottom. Solder mask outputs should include tStop and bStop.
6. Confirm the silkscreen outputs. Standard EAGLE silkscreen layers are tPlace and bPlace on layers 21 and 22, commonly combined with tNames and bNames for reference designators. Some manufacturer CAM jobs label the output file tSilk, but that is an output filename convention, not an EAGLE layer name.
7. Confirm the board outline output includes Dimension. This layer tells the manufacturer the final board perimeter. If you have routed slots or cutouts represented in a milling layer, make sure the manufacturer CAM instructions cover that layer too.
8. Confirm drill output. The CAM job should include Drills and Holes for Excellon drill generation. In older EAGLE workflows, Gerbers and Excellon output were sometimes generated with separate gerb274x.cam and excellon.cam jobs; EAGLE 9+ commonly integrates the outputs in one CAM Processor job.
9. Set the Gerber output type to Gerber RS-274X when the CAM job exposes that option. Some EAGLE 9-era flows can include Gerber X2 attributes, but RS-274X remains the widely accepted baseline.
10. Choose a clean output folder and click Process Job. EAGLE writes the configured Gerber files and drill files.
11. In EAGLE 9-era CAM Processor jobs, Process Job commonly produces a single ZIP archive directly. Older EAGLE versions generate loose files that you must zip manually. Either way, do not upload Gerber artwork without the drill output.

EAGLE 9 and legacy CAM differences

The main risk in EAGLE is mixing instructions from different eras of the software. EAGLE 8.6.0 through 9.6.2 use the newer CAM Processor job workflow, where a job can contain Gerber, drill, and assembly outputs and can package the result for upload. Older tutorials often mention loading gerb274x.cam for artwork and excellon.cam for drills. That legacy split can still explain older projects, but it is not the clearest starting point for a current EAGLE 9 package.

When reviewing a CAM job, read the EAGLE layer names rather than only the output filenames. A file named board.GTO may be the correct top silkscreen file, but the source layers should still betPlace and, when needed, tNames. The same distinction matters on the bottom side: bPlace and bNames are the EAGLE layers, while the generated file may be labeled in whatever style the manufacturer job prefers.

EAGLE layer and output reference

Common mistakes to avoid

• Loading an old gerb274x.cam tutorial job in a newer EAGLE 9 project when the built-in EAGLE CAM job or manufacturer v9 job would produce the expected ZIP and drill output.
• Missing the Dimension layer, which leaves the board outline out of the fabrication package even though the board shape is visible in the editor.
• Treating an output named tSilk as proof that EAGLE has a source layer with that name. Check that tPlace, tNames, bPlace, and bNames are included as intended.
• Exporting copper and mask but leaving Drills or Holes out of the job. Vias, through-hole pads, and many mounting holes depend on the Excellon file.
• Omitting milling or slot information when the design uses routed cutouts outside the simple Dimension outline.
• Manually zipping loose legacy outputs with stale files from an older CAM run. If Process Job creates a ZIP for you, use that archive directly unless the manufacturer asks for a different package.

Verify your Gerbers before ordering

Open the archive produced by EAGLE's CAM Processor in the online Gerber viewer and start with the layer list. You should see top and bottom copper, mask files from tStop and bStop, silkscreen files from the place/name layers you chose, the Dimension outline, and a drill file such as .XLN or .drd.

Then inspect the board instead of trusting file names. The Dimension boundary should match the board edge, connector holes should land in pads, and reference text should only appear where the CAM job included it. If a layer appears unknown, fix the CAM job naming or section setup before uploading; clear extensions reduce manufacturer back-and-forth.

FAQ

Do modern versions of EAGLE still use CAM jobs?

Yes. EAGLE 9 and Fusion Electronics use the CAM Processor workflow. The interface was redesigned compared with legacy EAGLE, but the package is still produced by processing a CAM job.

Should I use gerb274x.cam or a manufacturer CAM job?

In EAGLE 9-era workflows, use the built-in EAGLE CAM job or a manufacturer-supplied v9 .cam file. gerb274x.cam is the legacy RS-274X job used in older EAGLE flows.

Which EAGLE layer creates the board outline?

The Dimension layer is the normal source for the board outline. Make sure it is included in the outline output section of the CAM job.

Why are drill files separate from Gerber files in EAGLE?

Gerbers describe layer artwork. Drill files describe hole locations and sizes in Excellon format. Both are required for a complete fabrication package.