The editor

Export & fabrication

Every export lives one place: the Tools menu, or the 3D viewer's own toolbar for STEP and VRML. Each one is a single button, and the batch runner does all of them into one folder in a single pass.

The Tools menu open, listing Update Board from Schematic, Annotate, the four editors, Simulation, Scripting, Image to Silk, Plugins, and then Export Parts List (CSV), Export Netlist, Export Gerbers and Drill, Plot to SVG/PDF and Batch Export.
The Tools menu — every export, plus the editors, in one place. On Windows and Linux the menu bar is in the window; on macOS the same menus are in the system menu bar.

Gerber and drill

Export Gerbers and Drill writes RS-274X Gerber for every copper layer, the zone pours, silkscreen, solder mask, solder paste and the board edge — one file per layer — plus a single merged Excellon drill file covering every plated hole: through-hole pads and vias together, grouped into tools by drill diameter.

The package is written into a new folder inside the project — not the OS Downloads folder — and every file is named after the project rather than after the layer alone, so a set that has been unzipped somewhere else still says which board it is. The layer names follow KiCad's own spelling, because that is what a fab portal's layer auto-detection is matching on.

blinky-F_Cu.gbr
blinky-B_Cu.gbr
blinky-Edge_Cuts.gbr
blinky-F_Silkscreen.gbr
blinky-B_Silkscreen.gbr
blinky-F_Mask.gbr
blinky-B_Mask.gbr
blinky-F_Paste.gbr
blinky-B_Paste.gbr
blinky.drl

A layer with nothing on it contributes no file at all — an empty Gerber in a package is only a question the fab has to ask. A board with more copper layers gets one .gbr per layer, in stackup order, and a board carrying dimensions gets its documentation layers too.

Plots

Plot to SVG/PDF… writes the board (or the schematic) as a vector plot. The same board geometry can also be plotted to PostScript or DXF through the batch runner below.

BOM and netlist

Export Parts List (CSV) writes a bill of materials from the schematic. Export Netlist writes the net list the same way. Both run from the schematic view.

STEP and VRML

The 3D viewer has its own Export STEP and Export VRML buttons. Both write the board and every placed part's real 3D model as one scene file — STEP as a tessellated-mesh AP214 file, VRML as a VRML97 scene — built from the same geometry the 3D view itself draws, not a separate render made for export.

Batch export

Batch Export…, in the Tools menu, runs an ordered set of jobs — Gerbers, Excellon drill, SVG/PDF/PS/DXF plots, the BOM, STEP and VRML — into one output folder in a single pass. Every job calls the exact same generation function its individual toolbar button does; batch export does not reimplement anything, it only sequences what already exists.

The Batch Export (Jobset) dialog: a checklist of jobs grouped as Fabrication (Gerber package, Excellon Drill), Plot (SVG, PDF, PS, DXF), Assembly (BOM CSV) and 3D, with a Choose Output Folder control and Run and Close buttons.
The Batch Export dialog — every job in one list, run together into one output folder.

Checking the output

GerbView, one of the app's tabs, loads Gerber and Excellon files back in and draws them layer by layer — a way to look at exactly what a fab would receive before you send it.