---
name: kicad-manufacturing-export
description: Use when regenerating or exporting the BOM CSV, CPL/position CSV, or Gerbers+drill zip for a KiCad PCB project via kicad-cli (e.g. "regenerate the gerbers", "update the BOM and CPL", "re-export for JLCPCB"). Covers the exact kicad-cli invocations and column formats this project's ordering files expect, and the CPL rotation-correction trap (regenerating the position file the naive way silently wipes hand-verified assembly rotation fixes). KiCad 8/9/10, JLCPCB-style deliverables.
---

# Regenerating BOM / CPL / Gerbers via kicad-cli

For the `re-bba-rb` board specifically, deliverables live in
`hardware/re-bba-rb/`: `re-bba-rb-bom.csv`, `re-bba-rb-cpl.csv`,
`gerbers/rebbarb.zip`. Adjust paths/output names for other boards, but the
gotchas below (especially the CPL rotation trap) apply generally.

## 1. Gerbers + drill + zip

```bash
cd hardware/re-bba-rb
kicad-cli pcb export gerbers --board-plot-params -o gerbers/ re-bba-rb.kicad_pcb
kicad-cli pcb export drill --format excellon --excellon-separate-th \
  --excellon-units mm -o gerbers/ re-bba-rb.kicad_pcb
```

`--board-plot-params` reuses whatever layer/plot settings are already stored
in the board file — don't hand-pick layers, this reproduces exactly what was
there before. `--excellon-separate-th` splits plated/non-plated holes into
`*-PTH.drl` / `*-NPTH.drl`, matching the existing file-naming convention.

Then re-zip (excluding the previous zip itself, so it's not nested inside
its own replacement):

```python
import zipfile, os
folder = 'gerbers'
files = sorted(f for f in os.listdir(folder) if f != 'rebbarb.zip')
with zipfile.ZipFile(os.path.join(folder, 'rebbarb.zip'), 'w', zipfile.ZIP_DEFLATED) as z:
    for f in files:
        z.write(os.path.join(folder, f), arcname=f)
```

kicad-cli's gerber export also produces a `*-job.gbrjob` metadata file
alongside the layer files — include it in the zip, it's harmless and some
fabs use it for auto-configuration.

## 2. BOM

```bash
kicad-cli sch export bom \
  --fields "ITEM_NUMBER,Reference,Value,Footprint,MPN,LCSC,QUANTITY,DNP,Manufacturer" \
  --labels "Item,Designator,Value,Footprint,MPN,LCSC,Qty,DNP,Manufacturer" \
  --group-by "Value,Footprint,MPN,LCSC,Manufacturer" \
  --sort-field "Reference" \
  --ref-range-delimiter "" \
  -o re-bba-rb-bom.csv \
  re-bba-rb.kicad_sch
```

`--ref-range-delimiter ""` disables range compression (`C18-C20` becomes
`C18,C19,C20`) — this project's existing BOM convention is flat comma lists,
not ranges; drop this flag if the target format wants ranges instead.
`--group-by` on those 5 fields means any two components sharing value +
footprint + MPN + LCSC + manufacturer collapse into one row (with a combined
`Qty`) — this is how e.g. adding a new part that happens to match an
*already-used* part (same value/footprint/MPN) merges into an existing BOM
line instead of creating a new one, which is usually what you want (no new
line item added to the order).

Reference-only / non-purchasable footprints (gold-finger connectors, mouse-bite
NPTH-hole footprints, etc.) are excluded automatically via `in_bom no` on the
schematic symbol (or `exclude_from_bom` in the footprint's `attr`) — don't
try to filter them out in the export command itself.

**Verify after export**: diff the new BOM against the old one and sanity-check
that only expected rows changed — an unexpectedly *shorter* BOM (fewer
component rows/refs than before) is the signature of the
[kicad-bom-edit](../kicad-bom-edit/SKILL.md) skill's "malformed property
silently drops a whole sheet" bug, not a real BOM change.

## 3. CPL / position file — the rotation trap

```bash
kicad-cli pcb export pos --format csv --units mm --side both --exclude-dnp \
  -o /tmp/pos_raw.csv re-bba-rb.kicad_pcb
```

kicad-cli's own CSV columns (`Ref,Val,Package,PosX,PosY,Rot,Side`) don't match
JLCPCB's expected format (`Designator,Mid X,Mid Y,Layer,Rotation`, with
`Layer` capitalized `Top`/`Bottom`, not lowercase `top`/`bottom`). Transform:

```python
import csv
with open('/tmp/pos_raw.csv', newline='') as f:
    rows = list(csv.DictReader(f))
with open('re-bba-rb-cpl.csv', 'w', newline='') as f:
    writer = csv.writer(f)
    writer.writerow(['Designator', 'Mid X', 'Mid Y', 'Layer', 'Rotation'])
    for r in rows:
        layer = 'Top' if r['Side'].strip().lower() == 'top' else 'Bottom'
        writer.writerow([r['Ref'], f"{float(r['PosX']):.6f}",
                          f"{float(r['PosY']):.6f}", layer,
                          f"{float(r['Rot']):.6f}"])
```

**Then — before treating this as done — reapply every correction in
[`hardware/re-bba-rb/CPL_ROTATIONS.md`](../../../hardware/re-bba-rb/CPL_ROTATIONS.md).**
KiCad's raw per-footprint rotation frequently does not match what the
assembler expects (arbitrary per-footprint authoring reference vs. the
assembler's actual placement convention), and this has already been
hand-verified part-by-part against JLCPCB's placement-preview render for
this board. Regenerating the position file "the normal way" silently
overwrites those fixes back to (wrong) raw values — there is no automated
check that catches this, so it's easy to quietly ship a regression. Read
that file's sign-convention note before applying anything (short version:
"N degrees clockwise" feedback means *subtract* N in the CPL's Y-up frame,
not add it).

Do **not** reach for a generic community rotation-correction table (e.g.
`cpl_rotations_db.csv` from JLCKicadTools) as a shortcut — one was tried on
this board and found wrong for at least one package family (claimed
`LQFP-: 270°`; this board's actual correct value is 0°, unmodified). That
table is calibrated against a specific plugin's own raw-rotation baseline,
which is not the same as `kicad-cli`'s raw CSV baseline (different Y-axis
handling) — the numbers don't transfer.

## Quick full-refresh recipe

1. Gerbers/drill/zip: regenerate + re-zip (section 1) — safe to always redo,
   no hidden state to lose.
2. BOM: regenerate (section 2) — safe to always redo. Diff-check the row
   count.
3. CPL: regenerate raw (section 3), **then reapply CPL_ROTATIONS.md** before
   calling it current.
4. Run ERC (`kicad-cli sch erc --severity-all`) and DRC
   (`kicad-cli pcb drc --severity-all`) after any schematic/PCB change that
   prompted the refresh — not the export step itself, but worth confirming
   nothing regressed if this was bundled with other edits.