Eagle has lived several lives: a standalone editor for decades, and now part of Autodesk’s Fusion environment, where board designs sit alongside the mechanical models they must fit. Whichever front end you use, the fabrication handoff has the same shape it always had in Eagle: the CAM processor turns the board into a set of Gerber files plus drill data, from a CAM job that decides which layers go into which files. That job file is both the strength and the risk of the workflow — set it up once, correctly, and every export is consistent; inherit one from an old project, and every export consistently includes a layer mapping that no longer matches your board. Gerbv, the free viewer for Gerber RS-274X and Excellon drill files, is the check that separates those two outcomes. This guide covers the export at a general level — the CAM interface differs between the standalone and Fusion-hosted variants — and then the verification pass. New viewer users should start with how to open and view Gerber files; Gerbv is on the download page.
The CAM processor, at a general level
In Eagle’s workflow, Gerber generation is not a save-as; it is a processing run. You open the CAM processor, load or confirm a CAM job — a template that lists output sections, each section producing one file from a chosen set of board layers, in a chosen format — and run it. A typical job produces the copper layers, solder mask, silkscreen, solder paste, and a board outline file, each as standard RS-274X Gerber (the format Gerbv views; legacy RS-274D is not supported). Read the job before you run it, especially if it came with a board house template or an old project: the silk screen section that also pulls in a documentation layer, the outline drawn from a dimension layer in one job and from a dedicated layer in another — these small mappings are exactly the ones that survive unnoticed for revisions. If you design in the Fusion-hosted environment, the same CAM concept produces the manufacturing outputs from the electronics design; boards started in the Fusion 360 environment follow the same discipline: confirm what the job maps, then run it, then check the output as files.
Drill data from the same run
The CAM job also produces the Excellon drill file, from the board’s drills and holes layers, in the same run as the artwork. Keep it that way. Artwork and drills generated together share the board state and the job’s conventions; a drill file regenerated later, from a different job revision, is how a correct-looking Gerber set acquires holes that sit a consistent distance from their pads. Generate the whole set per release, into a clean output folder, and treat the folder — Gerbers, drill file, and a pick-and-place export if assembly is planned — as one indivisible release unit. If the board’s outline lives in the dimension information, confirm the job actually emits an outline file; boards whose edge never becomes a file are a recurring CAM-job inheritance problem.
Checking the set in Gerbv: mapping errors are visible here
Load the output folder in Gerbv following loading and aligning Gerber layers, and take inventory first: one file per CAM section, matching the job you ran. Then inspect with the job’s failure modes in mind. Silkscreen layer: does it contain only silkscreen? Documentation or dimension lines riding along are a mapping error you can see at a glance — and one the board house would faithfully print. Outline layer: one closed shape, nothing else, measuring correctly under measurement in Gerbv. Mask layers: openings over the pads they serve and nothing stray — a mask file that accidentally includes both sides’ data is another classic mapping slip. Paste layer: openings that match the surface-mount pads. Each of these checks is fast precisely because a wrong mapping produces visibly wrong content, not subtly wrong geometry.
Drill overlay and dimensional checks
Stack the drill file over the copper as in viewing Excellon drill files, and run the registration pass: holes centred in pads and vias everywhere, mounting holes placed for the enclosure — a check that matters doubly for Fusion users, whose board is often designed against a mechanical model in the same workspace; the exported outline and hole positions, measured in Gerbv, are the numbers that model will be judged by. Read the drill statistics against expectations, and measure the features the mechanical side depends on: outline extents, hole-to-edge distances, connector positions. If the Fusion model and the Gerber set ever disagree, believe the Gerber set — it is what gets manufactured — and trace the difference back to the board or the CAM job.
Fix the job, not the files
When a check fails, the fix in this workflow is almost always the CAM job: correct the layer mapping, adjust the section, re-run the whole job, and reload the fresh set in Gerbv. Editing or nudging the generated files themselves forfeits the reproducibility that makes the job valuable. Once a job passes the full pass twice — once when you set it up, once on a later revision — it earns trust, and the per-release check becomes the short form: count the files, overlay the drills, measure the outline. The complete gate before ordering remains the PCB pre-order checklist, which this workflow feeds directly into.
Frequently asked questions
What is a CAM job, and why does it matter for checking?
A CAM job is the template that tells Eagle’s CAM processor which board layers go into which output file, and in what format. Inherited or edited jobs are the main source of mapping errors — extra layers in the silkscreen file, a missing outline — and those errors are obvious when the output is inspected in Gerbv.
My silkscreen file contains dimension lines. What happened?
The silkscreen section of the CAM job is pulling in a documentation or dimension layer alongside the silkscreen layers. Correct the section’s layer selection in the job, re-run the complete job, and reload the fresh set.
I design in Fusion. Is the Gerber check different?
The check is identical, because the deliverable is identical: a Gerber and drill set. What Fusion adds is a mechanical model the board must fit — which makes measuring the exported outline and hole positions in Gerbv doubly worthwhile, since the factory builds the files, not the model.