Gerber files do not arrive as a board. They arrive as a pile of single-layer drawings that only become a board when they are stacked in the right order, in the same coordinate space, and inspected against each other. Loading and aligning layers in Gerbv is therefore less about the opening clicks and more about building a stack you can reason with: copper you can trust as the reference, mask and silkscreen read against it, and the drill layer used as the final registration witness. This tutorial covers the stacking order that works, how visibility and colour make a stack readable, and how to check that everything is actually aligned before the files go anywhere near a board house. It assumes you can already open a file set — if not, start with how to open and view Gerber files — and that Gerbv is installed via the macOS installation guide or your platform’s equivalent from the download page. The general role of the viewer is described on our Gerber viewer page.
The stacking order that reads well: copper, mask, silkscreen, paste
Gerbv stacks layers in the order they are loaded, and layers higher in the list draw over layers below them. A reliable reading order for a two-layer board is: bottom copper first, then top copper, then the solder mask layers, then the silkscreen layers, then the solder paste layers, with the drill layer and the board outline kept near the top where they can be toggled over everything. The logic is physical. Copper is the reference geometry — pads, traces and pours that everything else is defined against. Solder mask is meaningful only in relation to copper: its openings should sit exactly over the pads they expose. Silkscreen is meaningful in relation to both, because ink should print on mask, never across an exposed pad. Paste openings should match the surface-mount pads they serve. Reading the stack in that order means each new layer is judged against the layers it interacts with, instead of against a confusing composite of everything at once.
Visibility and colour: making the stack readable
A stack of six or more layers drawn at full strength is soup. Two controls make it legible. The first is visibility: every layer in the list can be shown or hidden, so you can build the exact comparison you need — top copper plus top mask, silkscreen alone against the outline, drills over bottom copper. Work in pairs and small groups rather than admiring the full composite; most alignment questions are between two specific layers. The second is colour: right-clicking a layer in the list offers per-layer operations including changing its colour and reloading its file, and distinct, consistent colours — one colour family for copper, another for mask, another for drills — turn the stack into a diagram you can read at a glance. Colour discipline matters again in transparency and Cairo rendering, where see-through layers only help if you can still tell them apart. If you re-export a corrected layer from your EDA tool, reload that layer rather than reopening the whole project, so the rest of your carefully ordered stack stays untouched.
Checking registration: let the drill layer be the witness
Alignment in Gerber data is normally automatic — all files share the export origin, so they land in registration when loaded. The point of checking is to catch the exports where that assumption breaks: a layer exported with a different origin, a mirrored bottom layer, or a file from an older revision mixed into the set. The drill layer is the best witness because holes are unambiguous: a plated hole must pass through the pads on every copper layer it connects. Load the Excellon file over the copper stack, as described in viewing Excellon drill files, zoom into a few areas, and look for concentricity — each drill hit should sit centred in its pad or via, all over the board, not just in one corner. Then check the outline layer against everything else: mounting holes should sit inside the outline at the positions the mechanical design intends, and no copper or component position should fall outside the edge. A systematic offset that grows across the board suggests a scale or unit mismatch; a single layer shifted while others agree points at that layer’s export settings; a mirrored layer shows text reading backwards and asymmetric features swapped side to side.
When layers do not line up
If the stack does not register, the fix almost always lives in the export, not in the viewer. Confirm that every file came from the same export run — mixing revisions is the classic cause of one layer disagreeing with the rest. Confirm that the EDA tool used the same origin and the same units for the Gerber files and the drill file, and that no layer was exported mirrored unless mirroring was intended for a bottom-side view. Re-export the full set in one pass and reload. What you should not do is nudge layers into place and order from the result: Gerbv’s export can translate and rotate data on export for legitimate format-conversion purposes, but an inspection copy that has been manually shifted proves nothing about the files the factory will receive. The viewer’s job is to show the export as it is; the EDA tool’s job is to produce a set that aligns on its own. Once the stack registers cleanly, finish with numbers — measuring distances and clearances turns “looks aligned” into verified dimensions.
Saving your stack as a project
If you will reopen the same board repeatedly — during a design review, or across several export revisions — Gerbv project files are worth knowing about. Project files are Scheme scripts, processed by the embedded TinyScheme interpreter, that define the layers, files, colours and ordering of a session, so the stack you built here can be captured rather than rebuilt by hand each time. That is the documented level of the feature: scriptable project files, not a general automation console, and Gerbv has no Python scripting.
Frequently asked questions
In what order should I load Gerber layers?
Bottom copper, top copper, then solder mask, silkscreen and paste, with the drill layer and outline near the top for toggling over everything. The order mirrors the physical board and lets each layer be judged against the one it interacts with.
How do I tell whether my layers are aligned?
Use the drill layer as the witness: every drill hit should sit centred in its pad or via across the whole board, and mounting holes should sit correctly inside the outline. A growing offset suggests a unit or scale mismatch; one shifted layer suggests that layer’s export settings.
A layer is offset. Should I move it in Gerbv?
No. An offset stack means the export itself is inconsistent — usually mixed revisions, a different origin or units, or an unintended mirror. Fix the export settings in your EDA tool, re-export the whole set in one pass, and reload.