Skip to content

Latest commit

 

History

History
62 lines (41 loc) · 2.82 KB

manufacturing_files_export.md

File metadata and controls

62 lines (41 loc) · 2.82 KB
Raw

Manufacturing files export

To ease the manufacturing files export from Kicad this process is automated using export_fab_output.sh bash script.

This script perform 5 actions:

  • Check PCB DRC (DRC report is saved here)
  • Export .dxf files for laser cutted case
  • Export .step model of the PCB and assembled components
  • Export .pdf of schematic, PCB Top and Bottom views
  • Export gerber, drill & map files for PCB manufacturing

To run this script on Windows it is necessary to have git-bash.

On Linux this script need to be updated to call the kicad-cli binary instead of the .exe expected on Windows.

It may be necessary to add execution right to the script by running chmod +x export_fab_output.sh

ⓘ Kicad 8 or later is mandatory to use the export in CLI

Design Rules Check (DRC)

DRC is a mandatory step before any file exportation to ensure the design rules compliancy

kicad-cli pcb drc -o cornia-drc.report --all-track-errors --schematic-parity --severity-error --severity-warning --exit-code-violations cornia.kicad_pcb

Export Schematic and PCB top and bottom views

Schematic and PCB views are useful for the review process and can be exported using the following command

kicad-cli sch export pdf -o pdf/SCH.pdf cornia.kicad_sch && \
kicad-cli pcb export pdf -o pdf/PCB_TOP.pdf -l F.Cu,F.Paste,F.Silkscreen,F.Mask,Edge.Cuts --exclude-value cornia.kicad_pcb && \
kicad-cli pcb export pdf -o pdf/PCB_BOT.pdf -l B.Cu,B.Paste,B.Silkscreen,B.Mask,Edge.Cuts --exclude-value cornia.kicad_pcb

Export DXF for laser cutted case

PCB layers User.8 & User.9 are respectively used in cornia footprint & pcb to export DXF for a laser cutted case using the following command

kicad-cli pcb export dxf -o case/LaserCut.TOP.dxf -l User.8 --ou mm cornia.kicad_pcb
kicad-cli pcb export dxf -o case/LaserCut.BOT.dxf -l User.9 --ou mm cornia.kicad_pcb

Export .step 3D model

PCB and assembled components are 3D modeled and can be exported in step format using the following command

kicad-cli pcb export step -o case/PCB.step --subst-models cornia.kicad_pcb

Export Gerber for JLCPCB

Based on JLCPCB kicad export recommendations & Kicad-CLI the following commands allow to export all gerber files (including Drill/Map files).

kicad-cli pcb export gerbers -o gerber/ -l F.Cu,B.Cu,F.Paste,B.Paste,F.Silkscreen,B.Silkscreen,F.Mask,B.Mask,Edge.Cuts --exclude-value --no-x2 --no-netlist --subtract-soldermask cornia.kicad_pcb
kicad-cli pcb export drill -o gerber/ --format excellon --excellon-separate-th --generate-map --map-format gerberx2 cornia.kicad_pcb