Fab set

Every file pcbjs build writes for the fab: Gerbers, drills, the order package, README-fab, BOM and placement, the .pcb.svg and .sch.svg documents, reproducible dates and the Gerber self check. Presets, bindPCB and variants, which decide what goes into the set, are in fab.md.

The fab set

pcbjs build writes one set per board to <fabDir>/<name>/, by default .pcbjs/fab/<name>/:

Blinky-F_Cu.gtl         front copper
Blinky-In1_Cu.g1        inner copper, one file per inner layer up to In6_Cu.g6
Blinky-B_Cu.gbl         back copper
Blinky-F_Mask.gts       front mask         Blinky-B_Mask.gbs   back mask
Blinky-F_Paste.gtp      front paste        Blinky-B_Paste.gbp  back paste
Blinky-F_SilkS.gto      front silkscreen   Blinky-B_SilkS.gbo  back silkscreen
Blinky-Edge_Cuts.gm1    board outline
Blinky-job.gbrjob       Gerber X2 job file with the stackup
Blinky-PTH.drl          plated holes, when there are any
Blinky-NPTH.drl         non-plated holes, when there are any
Blinky-PTH-drl_map.svg  drill map, one per drill file
Blinky-drill-report.txt every tool of every drill file
Blinky.ipc              IPC-D-356A netlist for electrical test
bom.csv                 bill of materials
cpl.csv                 placement, JLCPCB column layout
Blinky.pcb.svg          the whole board as one SVG document
Blinky.sch.svg          the schematic drawing, see schematic-graphic.md
README-fab.txt          status and summary
manifest.json           every other file with its size and sha256
Blinky-fab-0.1.0.zip    all of the above

• The zip is <name>-fab-<revision>.zip, or <name>-fab-dev.zip without a revision.
• Gerbers are X2, in mm, y up. Pads other than circles are regions. Stroke text is drawn with a round aperture as wide as its thickness.
• Circular arcs stay arcs: an A command with equal radii, a <circle>, the corners of a <rect rx>, roundedRect, circle and slot. A layer with one sets G75* once and draws each with G02*, clockwise from the top, or G03*, I and J from start to centre. Bezier curves, elliptical arcs and zone fills are segments.
• Silkscreen is cleared from the mask openings of its side it overlaps, as KiCad's --subtract-soldermask does: each such opening is a clear region after the legend.
• A zone fill with holes is an outer region and clear holes, the outer before any pour inside its holes, at any depth.
• A filled path with holes, such as the ring of a © sign, is one dark region whose contour runs into each hole and back along one cut line, so nothing earlier on the layer is erased.
• A paste layer with nothing on it, a side without SMD pads, is not written, and README-fab says so. A pad with paste windows of its own, pasteRatio, pasteShrink or paste windows, prints those.
• Fab, courtyard and user layers are not exported.
• The job file carries the layer count, thickness, finish and a MaterialStackup entry per layer.
• A failed entry leaves its last set in place with a STALE file in it, see cli.md.

The order package

• <name>.ipc is the IPC-D-356A netlist for the electrical test, UNITS CUST 1, 0.001 mm, y up. One fixed column record per pad and via: 317 plated hole, 327 surface pad, 367 non-plated hole; the net, N/C for none, an NNAME<n> alias past 14 characters; ref, VIA for vias, and pad; drill with P or U; access A00 through, A01 top, the copper count bottom; centre, size, rotation; mask S0 covered to S3 open both sides.
• <name>-drill-report.txt lists each drill file with its layer span and every tool: diameter, holes, vias and slots.
• <name>-PTH-drl_map.svg and -NPTH- draw the outline and each hole at size with one symbol per tool, and a legend of symbol, diameter and count.
• manifest.json names the board, revision, target, generator and date, and every other file of the set with its size and sha256. It is in the zip too; the zip itself is not in it. The generator is pcbjs <version>, the version of @pcbjs/export that wrote the set, which the Gerber TF.GenerationSoftware header, the job file and the Generated line of README-fab name too.

Reproducible builds

Every file that carries a date, the Gerbers, drill files, job file, netlist, report, README-fab, manifest and the zip entries, carries the same one: pcbjs build --date <iso>, else SOURCE_DATE_EPOCH in seconds, else now. Two builds of one tree at one date are byte identical, zip included, in any time zone. SOURCE_DATE_EPOCH=$(git log -1 --format=%ct) pcbjs build stamps the commit time.

Gerber self check

pcbjs build and pcbjs check --fab read every copper Gerber and the outline back and compare them with the board:

• each copper layer against the board's copper of that layer, pads, tracks, vias, fills, graphics and text: a symmetric difference above 0.01 mm², once slivers thinner than 12 µm from arc chords are dropped;
• copper against the outline the Edge.Cuts file draws: copper outside it or inside a cutout;
• the outline read back against the board's outline;
• the pads of each net: pads the board joins through copper and plated holes must stay joined, and pads of two nets must stay apart.

Each difference is a DRC error fab-mismatch, so the set is not orderable. README-fab carries a Gerber self check: passed line. pcbjs check without --fab and pcbjs dev skip it.

README-fab.txt

It starts with STATUS: ORDERABLE, or STATUS: NOT ORDERABLE with the error counts. Then: the board size and counts, a 3D models line with the parts from model files, generated and with no model, as 3d.md defines them, the sourcing line, the stackup layer by layer, every rule value, the hole sizes, the DRC and ERC counts with every finding in the same lines as pcbjs check, the self check line, the file list and notes. A target's second line names the target, its fab and its place in the list.

• fabNotes={['Single board, no panel.', 'Remove the order number.']}, order form choices and the like, opens the Notes. <PCB>, a preset, a variant target and defineDefaultBoard take it; the lines join defaults first, then the preset or target, then <PCB>, each once.
• The Notes name each font the text uses: Hershey Simplex and NewStroke with their provenance from fonts.md, an outline font with its copyright and licence.

BOM and placement

• bom.csv groups footprints with the same value, footprint id and fields. Its columns are Refs, Value, Footprint, Qty, MPN, the number resolved for the board's tags, Source, the tag matched or MPN, Manufacturer and Datasheet. Then one column per other field, one per MPN:<tag> key, and MPN:* with the catch-all when a tagged number replaced it in some row.
• Footprints with bom={false} are left out.
• cpl.csv has Designator, Val, Package, Mid X, Mid Y, Rotation and Layer, y up. It lists footprints with both pos and bom set.
• DNP parts, dnp on a placement, stay on the board and in the DRC but are left out of both files; README-fab names them.
• Mid X and Mid Y follow cpl={{ origin }} on the board or preset: 'center', the courtyard centre taken in the part's own frame, else its pads' extent, as JLCPCB and most assemblers expect; or 'footprint', the footprint origin, pin 1 for a pin header. JLCPCB presets default to 'center', every other board to 'footprint'. README-fab says which.

The .pcb.svg document

<name>.pcb.svg is a valid SVG any browser draws, with the board data in the pcb: namespace https://pcb.svg/ns/1. Geometry is in mm, y down.

• <metadata> holds pcb:board, pcb:rules after defaults, pcb:nets, pcb:footprints with absolute positions, and pcb:drc with the counts.
• One <g pcb:layer="…"> per layer, back to front. Each element has data-id, data-kind of pad, track, via, zone, graphic or text, and data-net, data-ref and data-pad where they apply.
• Holes are drawn last in the background colour. Text is a stroked path with its string in pcb:text. Arcs are A commands, as in the Gerbers.