KiCad designs the board; the fabrication files are what the factory builds. Between those two sits an export step — the Plot dialog — and everything that can go wrong there (a layer left unplotted, a drill file generated with different settings, a stale file mixed into the set) goes wrong silently, because KiCad keeps showing you the design, not the output. The reliable habit is to open the exported set in an independent viewer before ordering. Gerbv is that viewer in this workflow: a free, open-source viewer for Gerber RS-274X files, Excellon drill files and CSV pick-and-place files. This guide covers exporting from KiCad at a general level — exact menu paths and dialog layouts differ between KiCad versions, so treat the steps qualitatively — and then checking the result properly in Gerbv. If you are new to the viewer itself, start with how to open and view Gerber files; Gerbv is on the download page, and its general role is explained on our Gerber viewer page.
Exporting from KiCad: the Plot dialog, at a general level
In KiCad’s board editor, fabrication output is produced from the Plot dialog. The general shape of the job is always the same, whatever the version: choose an output folder dedicated to this export, select the layers to plot as Gerber files, set the general options, and plot. The layers a normal two-layer board needs are the copper layers (top and bottom, plus any inner copper), the solder mask layers, the silkscreen layers, the solder paste layers if the board will be assembled with a stencil, and the board outline layer — the edge cuts that define the board’s shape. Plot them all in one pass, into the same folder, so the whole set shares one origin and one moment in the design’s history. A set plotted piecemeal across edits is a set whose layers may quietly disagree. Leave the format choices at the modern defaults your version offers unless you have a specific reason to change them: board houses expect standard RS-274X output, which is also the format Gerbv views (legacy RS-274D is the one Gerber variant it does not support).
Generating the drill file — a separate step, on purpose
Drill data does not come out of the Plot dialog with the artwork. KiCad generates it separately, through its drill-file generation, producing an Excellon (NC drill) file that lists the drill tools and every hole position. Generate it in the same session, from the same board state, and into the same output folder as the Gerbers. The setting that matters most is consistency: the drill file must use the same origin and compatible units and format conventions as the Gerber set, because the two are manufactured as one board. Most drill disasters — holes shifted as a block, holes at miniature scale in one corner — are born here, when the drill export’s origin or format settings differ from the artwork’s. If your board will be assembled, this is also the moment to export the component position file, which Gerbv can view as a CSV pick-and-place layer. Then ZIP the folder for the board house if needed — but keep the unzipped folder, because that is what you are about to inspect.
Opening the set in Gerbv: layer order that reads well
Open the exported folder in Gerbv, following loading and aligning Gerber layers: bottom copper first, then top copper, then the mask layers, the silkscreen layers and the paste layers, with the outline and the drill file near the top of the stack where they can be toggled over everything. Opening a folder loads the loadable files it finds, detected by content, so a file KiCad named unexpectedly still lands in the stack — but compare the layer list against the list you plotted. Count them. A layer missing from the viewer was missing from the export, and a missing layer (an unplotted bottom mask is the classic) is invisible in every other check you are about to run. Give layers colours you can tell apart, and work in pairs: copper with its mask, silkscreen against the pads it must avoid, paste openings against the surface-mount pads they serve.
The drill overlay and measurement sanity checks
Now stack the Excellon drill file over the copper, as in viewing Excellon drill files. Every drill hit should sit centred in its pad or via, across the whole board — connectors, ICs, mounting holes. A block shift means the drill origin differed from the artwork’s; a pattern that is the right shape at the wrong size means the format or units differed. Read the drill statistics Gerbv reports and compare the tool list with what the board should use: via size, lead sizes, mounting holes, and nothing you do not recognise. Finish with numbers, using measurement in Gerbv: the outline’s overall width and height against the mechanical design, one mounting-hole position against two edges, the pitch of a fine-pitch footprint against its datasheet, and the thinnest trace and tightest gap against what your board house can comfortably make. Also flip the silkscreen on alone over the outline and read it: KiCad exports exactly what the board editor shows, including any text that overlaps a pad — visible here, fixable in two minutes back in the editor, and expensive only if it reaches the factory.
If something looks wrong, fix it in KiCad — not in the viewer
Gerbv’s job in this workflow is evidence, not repair. A layer that is mirrored, offset or missing was exported that way; the fix is to correct the plot selection or the drill settings in KiCad, re-export the complete set in one pass, and reload. Never order from a set you have nudged into alignment in a viewer — the factory receives files, not views. When the re-export registers cleanly, runs the right layer count and measures correctly, the set is ready for the full pre-order pass in our PCB pre-order checklist.
Frequently asked questions
Which KiCad layers should I plot for a typical board?
Top and bottom copper (plus any inner copper), solder mask for both sides, silkscreen for the sides you use, solder paste if a stencil is involved, and the board outline layer — all plotted in one pass into one folder, with the drill file generated in the same session.
Why are my drill holes shifted in Gerbv when they look fine in KiCad?
KiCad’s board view shows the design, where holes and copper share one model. In the exported files, a shifted drill pattern means the drill file was generated with a different origin or format setting than the Gerber files. Regenerate both in one pass with consistent settings and reload the set.
Can Gerbv fix a bad KiCad export?
No — and it should not. Gerbv shows the exported data exactly as the factory will receive it. Correct the plot or drill settings in KiCad, re-export the whole set, and check the fresh files.