/sch-export

sch — schematic exports

Input is a .kicad_sch file. sch erc is documented in references/checks.md.

sch export pdf — all sheets in one PDF (--output is a file)

• --pages/-p — comma-separated page list; blank = all pages
• --black-and-white/-b, --no-background-color/-n, --exclude-drawing-sheet/-e
• --theme, --drawing-sheet, --default-font, --define-var
• --exclude-pdf-property-popups, --exclude-pdf-hierarchical-links, --exclude-pdf-metadata

kicad-cli sch export pdf -o schematic.pdf -D REV=B board.kicad_sch

sch export svg / dxf / ps — one file per sheet (--output is a directory)

Shared flags: --theme, --black-and-white/-b, --exclude-drawing-sheet/-e, --default-font, --pages/-p, --drawing-sheet, --define-var. svg and ps add --no-background-color/-n.

kicad-cli sch export svg -o svg_out/ board.kicad_sch

sch export hpgl — pen-plotter HPGL (one file per sheet)

Adds --pen-size/-p and --origin/-r (0|1|2|3).

sch export netlist

--format/-f: kicadsexpr (default), kicadxml, cadstar, orcadpcb2, spice, spicemodel, pads, allegro. --output is a file.

kicad-cli sch export netlist --format spice -o board.cir board.kicad_sch

sch export bom

--output is a file (typically .csv).

• --fields — ordered field list. Default Reference,Value,Footprint,${QUANTITY},${DNP}. Supports field variables like ${QUANTITY}, ${DNP}.
• --labels — column headers. Default Refs,Value,Footprint,Qty,DNP.
• --group-by — group references whose listed field values match
• --sort-field (default Reference), --sort-asc
• --filter, --exclude-dnp, --include-excluded-from-bom
• Delimiters: --field-delimiter (default ,), --string-delimiter, --ref-delimiter, --ref-range-delimiter, --keep-tabs, --keep-line-breaks
• --preset / --format-preset — use a named BOM/format preset stored in the schematic

Single-quote the field list so the shell does not expand ${QUANTITY}/${DNP} — KiCad must receive them literally:

kicad-cli sch export bom -o bom.csv \
  --fields 'Reference,Value,Footprint,${QUANTITY}' \
  --labels 'Refs,Value,Footprint,Qty' \
  --group-by Value --exclude-dnp board.kicad_sch

sch export python-bom — legacy XML intermediate netlist

kicad-cli sch export python-bom [-o OUTPUT_FILE] INPUT.kicad_sch — produces the XML intermediate netlist consumed by legacy Python BOM scripts. Prefer sch export bom for new work.