Fabrication outputs and netlists
A board's fabrication set is written in one step from its .circuit.layout: copper, mask, legend and drill data, the fabrication and assembly drawings, and the assembly files of each variant. Every output comes from the same geometry, so the Gerber and ODB++ copies of a board agree. The Desktop's Fabrication outputs panel, design.export and runmat-design export --format fabrication read the same settings from the board and make the same files. Make fabrication outputs walks through the panel.
Outputs
| Output | Word | Writes |
|---|---|---|
| Gerber | gerber | Gerber X2, one file per layer, and the .gbrjob job file with the stackup |
| Drill | drill | Excellon drill files, plated per drill span and non-plated |
| Drill map | drill_map | the drill symbols and table, as Gerber and PDF |
| Fabrication drawing | drawing | drill table, board size, the layer and stackup table and notes, as Gerber and PDF |
| Test netlist | ipc356 | IPC-D-356A, for bare-board electrical test |
| Pick and place | pick_place | the centroid file of each variant |
| BOM | bom | the bill of materials of each variant |
| Assembly drawing | assembly_drawing | one sheet per side with component outlines and designators, the bottom seen from below, as Gerber and PDF |
| IPC-2581 | ipc2581 | IPC-2581C |
| ODB++ | odb | ODB++, as a job tree or a .tgz |
The assembly drawings mark pin 1 and the polarity of polarized parts Not yet releasedStatus.
Presets
| Preset | Outputs |
|---|---|
fab_house (the default) | gerber, drill, drill_map, drawing, ipc356 |
assembly | pick_place, bom, assembly_drawing |
full | every output |
custom | the outputs listed |
The layer table
The layer table lists the board top to bottom: paste, legend, mask, the stackup's copper layers with their weight and the dielectrics between them, the bottom's layers, the courtyards and the outline. Each row gives its material, its thickness, the Gerber file it makes and whether it is on by default; the courtyards are off. A request names the layers to write, and the job file lists exactly those.
design.export with previewLayer draws one layer as its Gerber makes it (flashes, strokes and regions, the mask as its openings) and writes nothing; the panel shows it when a layer row is selected.
Settings saved with the board
The board keeps the settings of its last fabrication export in a fabrication statement, written only for the fields that differ from the defaults:
fabrication = { preset = custom, outputs = [gerber, drill, drill_map, drawing, ipc356, pick_place, bom], layers = ["F.Cu", "B.Cu", "F.Mask", "B.Mask", "F.Silkscreen", "Edge.Cuts"], variants = ["", lite], folder = "fab/sensor-B", zip = true, gerber = { units = inch, decimals = 5 }, pick_place = { sides = separate, units = mm }, bom = { columns = [designators, quantity, value, mpn], group_by_value = false }, revision = "B" }| Field | Sets |
|---|---|
preset, outputs | the outputs to make |
layers | the Gerber layers to write, by layer name; every layer but the courtyards when left out |
variants | the variants that get assembly files ("" is the default variant); every variant when left out |
folder | the output folder, relative to the board's folder; fab/<board>, or fab/<board>-<revision> with a revision, by default |
zip | pack the set into one .zip beside the files (on by default) |
through_hole | list through-hole parts in the pick-and-place file |
gerber = { units, decimals } | mm with 5 or 6 decimals (4.5 or 4.6 coordinates), or inch with 5 or 6 (2.5 or 2.6), for the layers, the drill map and the drawings |
pick_place = { sides, units } | both sides in one file, separate files, or top or bottom only; mm or inch |
bom = { columns, group_by_value } | the columns (designators, quantity, value, package, mpn, manufacturer), and one line per value or, with group_by_value = false, one line per designator |
revision | the board revision, written into the Gerber and job files' project attribute and the fabrication drawing |
Pre-flight
Before it writes, an export can run the pre-flight: the counts of DRC findings, ERC findings, unrouted connections and schematic changes the board hasn't taken, from the same checks as runmat-design check without the simulations. The Desktop runs it on Generate and asks before exporting a board with issues.
The command line
runmat-design export board/sensor.circuit.layout --format fabrication
runmat-design export board/sensor.circuit.layout --format fabrication --preset assembly --variant "" --variant lite
runmat-design export board/sensor.circuit.layout --format fabrication --outputs gerber,drill --gerber-units inch --no-zip --out fabThe command starts from the board's saved settings, and each flag overrides one. It writes to the settings' folder unless --out names another.
| Option | Effect |
|---|---|
--preset <name> | fab_house, assembly, full or custom |
--outputs <list> | the outputs, by word (drill-map and drill_map are the same) |
--layers <list> | the Gerber layers, by name |
--variant <name> | the assembly files of a variant; repeat for several; "" is the default variant |
--include-through-hole | through-hole parts in the pick-and-place file |
--zip, --no-zip | pack the set or not |
--gerber-units mm|inch, --gerber-decimals 5|6 | the Gerber coordinate format |
--pick-place-sides both|separate|top|bottom, --pick-place-units mm|inch | the pick-and-place files |
--bom-columns <list>, --bom-ungrouped | the BOM's columns, and one line per designator |
--revision <text> | the board revision |
--remember | save these settings into the board |
Values print with engineering prefixes (12 pF, 10 kΩ) in BOMs and netlists.
Netlists
design.export writes a circuit's netlist as kicad_netlist, spice, edif (EDIF 2.0.0) or ipc356, for other tools and test fixtures.
KiCad projects
design.export with format kicad writes a circuit as a KiCad project: a .kicad_sch per sheet and, with a board, a .kicad_pcb. KiCad holds at most 32 copper layers, so the export refuses a board with more, names the board's layer count and writes no files; ODB++, IPC-2581 and Gerber write every layer of a board with any number of copper layers.