A PCB assembly drawing is the document that tells whoever populates your board where every part goes — its reference designator, its value, and which way it faces. KiCad can produce one from the layers you already have; the trick is knowing which layers to plot and how to get a clean PDF out reproducibly.
Short answer: Plot the fabrication layers — F.Fab and B.Fab for component graphics and reference designators, plus Edge.Cuts for the outline — to a PDF, one drawing per populated side. Do it from File → Plot in the PCB Editor, or run kicad-cli pcb export pdf for a version you can regenerate on demand.
What an assembly drawing is (and who reads it)
An assembly drawing is a flat, annotated top-down (and bottom-up) view of your populated board. It exists for three audiences:
- The assembly house. Their operators and machine setup engineers use it to confirm placements, orientations, and any special handling before they run your board. It's the sanity check against the pick-and-place data.
- Your QA. Whoever inspects the first article compares the real board against this drawing to catch swapped, rotated, or missing parts.
- Your future self. Six months from now, the assembly drawing is the fastest way to remember what U3 is and why D1 points the way it does — no need to reopen the layout.
It is a human-readable companion to the machine-readable pick-and-place file, not a replacement for it.
Which layers go on it
KiCad keeps assembly-facing graphics on dedicated fabrication layers, separate from the silkscreen that gets printed on the physical board. That's deliberate — the fab layers can carry denser annotation without cluttering the actual board.
| Element | KiCad layer | Why it's on the drawing |
|---|---|---|
| Component body outlines + refs (top) | F.Fab |
Shows each part's footprint and reference designator for the top side |
| Component body outlines + refs (bottom) | B.Fab |
Same, for the bottom side |
| Board outline | Edge.Cuts |
Gives the operator the board shape and orientation |
| Courtyard (optional) | F.CrtYd / B.CrtYd |
Clearance envelopes some houses want for placement checks |
| Notes / title block | Drawing sheet | Revision, part numbers, special instructions |
Plot one drawing per populated side. If parts live on both sides, you produce a top and a bottom sheet.
Plotting it to PDF from the GUI
In the PCB Editor:
- Open File → Plot.
- Set Output format to PDF.
- In the layer list, tick F.Fab and Edge.Cuts (swap in B.Fab for the bottom drawing).
- Enable Plot reference designators so the refs render, and keep Plot footprint values on if you want values shown too.
- Click Plot.
That gives you a PDF you can hand off immediately. The catch: it's manual, and it's easy to forget a layer or plot a stale revision.
Exporting it via kicad-cli
For a reproducible drawing that regenerates every time your board changes, use the command line. kicad-cli ships with KiCad and needs no GUI:
kicad-cli pcb export pdf --output assembly.pdf --layers "F.Fab,Edge.Cuts" board.kicad_pcb
Swap F.Fab for B.Fab to produce the bottom-side drawing. Because it's a single command, you can wire it into whatever runs on every commit — no clicking through the Plot dialog, no chance of shipping last week's layout.
What to annotate
A drawing that just shows outlines isn't much use. Make sure yours carries:
- Reference designators — the primary key an operator matches against the BOM and CPL.
- Component values or part numbers — helpful for a human reading the sheet, though the BOM remains the source of truth.
- Orientation marks — pin-1 indicators, polarity marks for diodes and electrolytics, and the notch/dot for ICs. These prevent the most common assembly defects.
- Notes — anything non-obvious: do-not-populate parts, hand-solder-only components, or special torque/height requirements, placed in the title block or as text on the fab layer.
Pairing it with the BOM and pick-and-place
The assembly drawing is one leg of a three-part handoff. On its own it tells a story; with its companions it becomes a buildable package:
- BOM — the parts list: what to buy, how many, and which reference designators each line covers.
- Pick-and-place (CPL) — machine-readable X/Y/rotation data for each placement. See our guide to KiCad pick-and-place / CPL files for how KiCad generates it.
- Assembly drawing — the human-readable map that ties the two together and lets a person verify the machine did the right thing.
When the three agree — same reference designators, same revision, same board — assembly is smooth. When they drift out of sync, you get delays and re-spins. That's the heart of a professional manufacturing handoff, and it's why so many KiCad projects stumble at exactly this step, as we covered in the missing manufacturing package.
Keeping it current
The failure mode isn't producing an assembly drawing once — it's keeping it in step with the board. Every layout change silently invalidates the last export, and manual plotting means somebody has to remember to redo it.
That's what GoForFab handles: connect your KiCad project, and every push regenerates the whole manufacturing package — assembly drawings, Gerbers, BOM, CPL, DRC/ERC reports, 3D renders — all from kicad-cli, all reproducible, always matching the revision you just pushed. It's free forever for solo projects, so the drawing is never the thing holding up your build.