Of all the files in a fabrication set, the drill file is the easiest to forget and the most expensive to get wrong. Copper layers describe what the board looks like; the Excellon drill file describes every hole that will be physically drilled through it — component leads, vias, mounting holes — and a board with perfect copper and wrong holes is scrap. Drill data is also structurally separate from the Gerber layers, which is why it deserves its own viewing pass. Gerbv views Excellon (NC drill) files as first-class layers alongside RS-274X Gerber and CSV pick-and-place data. This tutorial covers loading the drill layer over your copper, reading what Gerbv reports about the tools and codes in the file, and recognising the scale and offset problems that a two-minute overlay check can catch. You will want the layer stack from loading and aligning Gerber layers ready first; installation is covered by the Linux installation guide and its siblings on the download page, and the viewer’s overall role is on our Gerber viewer page.
Loading the drill file over the copper
Open your board’s Gerber layers as usual, then open the Excellon drill file from the main window so it joins the same layer list, positioned in the stack where you can toggle it over the copper. Give the drill layer a colour that contrasts hard with the copper, because the entire check is positional: each drill hit is drawn at its coordinate with its tool’s diameter, and you are looking for those circles to sit centred inside pads and vias. Start zoomed out. The whole-board view answers the first questions instantly: are holes distributed where the board has components, do the mounting holes sit near the corners or edges the mechanical design intends, and is there anything — a hole in empty space, a dense cluster at the origin — that is obviously wrong before you measure anything?
Reading the drill statistics and tool information
Gerbv’s report windows summarise the statistics of the Gerber and drill codes used in your files — for the drill file, that is your tool table in report form: which drill sizes the file actually calls for, and how the hits distribute among them. Read it against your expectations. A simple board might use a handful of sizes: small drills for vias, a size or two for component leads, larger ones for mounting holes. If the report shows a size you do not recognise, find out where it is used before ordering — an unexpected tool often means an unexpected feature, such as a footprint whose holes were specified in the wrong unit in the library. If two sizes are suspiciously close — one intended in millimetres, one in inches, for what should be the same hole — that is the fingerprint of a mixed-unit library part. Cross-check the counts as well: a board with hundreds of vias should report hundreds of hits of the via size, and a shortfall can mean the drill export dropped a class of holes. The aperture-usage reporting serves the same purpose on the Gerber side, showing how often each aperture is used across the visible layers; together, the reports turn “the board looks fine” into “the board contains the features, in the quantities, we designed”.
The overlay check, area by area
With the statistics read, do the visual pass. Zoom into a connector or IC area with the drill layer over the top copper, as in opening and viewing Gerber files: every hit should be concentric with its pad. Move to the bottom copper view and repeat — a plated hole passes through the whole board, so it must centre on both sides. Check the largest holes against the components that use them with the method from measuring distances and clearances: compare the reported tool diameter with the pad, and picture the annular ring that remains for the drill to land in. Finally, check holes against the board outline layer: mounting holes fully inside the edge, no drill hit clipping a cutout or sitting in a routed slot’s path unless the design puts it there.
Spotting scale and offset problems
Drill files fail in characteristic ways, and this pass exists to catch them while they are still free. Everything clustered near the origin, tiny: the drill file’s coordinates were read at the wrong precision or unit — the whole pattern is the board in miniature in one corner. Holes the right shape but uniformly huge or tiny relative to pads: tool diameters interpreted in the wrong unit, a millimetre-versus-inch mismatch that leaves positions right and sizes wrong. The pattern correct but shifted as a block: the drill export used a different origin from the Gerber export; the shape matches, the registration does not. Only some holes misplaced: rare, and usually a stale file — one layer from a previous revision mixed into the set. Each of these is a reason to go back to the EDA export settings, fix the cause, and re-export the complete set in one pass; none of them is fixable by nudging the drill layer in the viewer, because the factory receives the files, not your view of them. A dedicated troubleshooting batch on this site will take these failure patterns one by one in the future; for now, the discipline is the same as for every layer: view the files exactly as exported, believe what the overlay shows you, and treat a mismatch as information about the export — that habit, plus the statistics read above, is most of what drill-file viewing in Gerbv is for.
Exporting drill data onward
One last documented capability is worth knowing: Gerbv does not only read Excellon data, it can also export it — the export formats include a drill format and an ISEL NCP drill format alongside RS-274X. That makes Gerbv useful for format translation between drill dialects, or for writing a cleaned-up version of a troublesome file. If you translate files this way, view the result again as a fresh layer before sending it anywhere — the same overlay check, applied to your own converted output.
Frequently asked questions
Why is the drill data not part of the Gerber files?
Drilling is a separate manufacturing step with its own data: the Excellon file lists drill tools and hit positions, while Gerber files describe layer artwork. Gerbv loads both into the same layer stack so you can check them in registration.
What should the drill statistics tell me?
Which drill sizes the file actually uses and how hits distribute among them. Compare that with your design: unexpected sizes, near-duplicate sizes in different units, or missing classes of holes all point at library or export problems worth fixing before ordering.
All my holes are in one corner, very small. What is wrong?
That pattern means the drill file’s coordinates were produced or interpreted with the wrong precision or unit. Re-check the drill export settings in your EDA tool, re-export the full fabrication set in one pass, and reload — do not try to shift the layer into place in the viewer.