Gerber and Drill Data Regeneration for PCB Reverse Engineering

The netlist is verified and the schematic reads cleanly. Neither of them is what a fabricator opens. A board house works from artwork — copper images, mask and legend files, and a drill program with a tool table — and rebuilding that set is the point in PCB reverse engineering where document work becomes manufacturing work. Errors here stop being inconvenient and start being expensive.

Why artwork cannot simply be exported

Forward design begins in a CAD database where every trace is an object carrying a net name and a design rule. The reverse path has no such database. What exists is a physical board, a measured stackup and a set of photographs. Gerber is a plotted image format: it describes apertures, flashes, draws and polarity, but nothing about intent.

Three consequences follow. No design rules travel with the file. No netlist is embedded in it. And layer-to-layer registration becomes your responsibility instead of the tool’s. A set that looks correct on screen can still fail at the fab, because a 0.15 mm clearance measured with calipers through a coating is a guess.

Build the layer set in the right order

Order matters, because each layer is judged against the one produced before it. Copper also cannot be drawn until the schematic recovery is settled, since every trace needs a net to be checked against.

1. Stackup and finished thickness, fixed first because everything downstream references it.
2. Board outline and datum, taken from routed edges rather than from the silkscreen.
3. Copper, inner layers first and outer layers last, so planes are settled before traces are drawn.
4. Solder mask, derived from pad geometry rather than copied from the original film.
5. Legend, rebuilt only once pads are final.
6. Drill, last, because hole positions depend on every pad above.

The manufacturability checklist

Each item below has one question behind it: did this number come from the board, or from the fabricator’s capability?

• Minimum trace and spacing, measured on the worst-case layer rather than the average one.
• Annular ring: pad diameter minus drill size. Under 0.15 mm on a 1.6 mm board is a yield risk, not a design choice.
• Hole-to-hole and drill-to-copper spacing, checked against the tightest pair on the board.
• Mask expansion and dam width — a dam narrower than 0.1 mm will not survive development.
• Copper-to-edge clearance, which routing tolerance can consume entirely.
• Legend over exposed copper, which smears and is a common cause of a rejected first article.
• Slivers and acid traps, often inherited faithfully from a layout that was legal forty years ago.
• Fiducials and tooling holes, absent on many legacy boards and required by modern assembly.

Most PCB reverse engineering projects that fail inspection fail on the second item, not on the copper itself.

Drill data is a separate discipline

An Excellon file is unforgiving. Units are declared once and applied silently; zero suppression must match on both sides; the tool table must describe every diameter actually used. Plated and non-plated holes belong in separate files, slots need their own definition, and a counterbore drawn as a circle is simply a wrong hole.

The counting test

Footprint count and hole count should agree. Every through-hole component contributes its pin count; every mounting hole, via and test point contributes one. When the totals differ by more than a handful, a pad is missing or a via was drawn as a component. It is a five-minute check that catches the error class most likely to scrap a panel.

Verify before release

Two checks pay for themselves. First, import the regenerated artwork into a CAM tool, extract connectivity from the copper, and compare it net for net against the source netlist — this tests the artwork rather than the intent behind it. Second, run design rule checks against the fabricator’s published capability instead of the original design’s rules, since the two rarely match on a board laid out in 1994.

Then plot at 1:1 and lay the print on the bare board. Registration errors that survive every software check are usually visible to the eye within seconds.

Circuit Engineering Company Limited concentrates on industrial boards — PLC racks, motor drives, switch-mode supplies — recovering them from the physical unit and handing over editable data the client owns. Artwork regeneration sits at the end of that chain, and a set that passes a first article is the only proof the chain held.

The recovery workflow ends in files. The fabricator’s acceptance is what closes the loop. In PCB reverse engineering a Gerber set is a claim about a physical object, and the drill program is where that claim gets tested.