| JLC PCB Plug-in for KiCad |
|---|
- Generates gerber files in correct format for production
- Generates BOM file in correct format for production
- Generates Pick and Place file in correct format for assembly
- Generates IPC netlist file
Fabrication Toolkit is distributed with the official releases of KiCad 6+. Open the "Plugin and Content Manager" from the KiCad main menu and install the "Fabrication Toolkit" plugin from the selection list.
Download the latest release ZIP file. Open the "Plugin and Content Manager" from the KiCads main window and install the ZIP file via "Install from File".
Click on the Fabrication Toolkit 
button on the top tool box inside KiCad pcb editor (pcbnew).
⊛ Ensure your board is synchronized before invoking this addon [F8].
⊛ The User_1 layer in internally defined as a V-Cuts layer, please avoid using it for anything else (unless disabled). (since v3.0.0).
Options can be set in the dialog that appears when the plugin is invoked. They are saved in a file called fabrication-toolkit-options.json in the project directory so that they are remembered between invocations of the plugin.
☑ Additional layers: Comma-separated list of additional layers to include in the gerber archive.
☑ Set User.1 as V-Cut layer: Merge User.1 layer with the Edge-Cut layer in production.
☑ Use User.2 for an alternative Edge-Cut layer: Use the User.2 instead of the Edge-Cut layer for the board outline in production. This is useful if you need process edges or panelization during production but still want to keep the individual outline for prototyping, 3D model exports, or similar purposes.
☑ Apply automatic translations: Apply known translation fixes for common components.
☑ Apply automatic fill for all zones: Refill all zones before generation production files.
☑ Exclude DNP components from BOM: Exclude components the had been set a DNP from th BOM.
Add an 'LCSC Part #'* field with the LCSC component part number to the symbol's fields property.
| 'LCSC Part #' | 'JLCPCB Part #' |
|---|
The fields will be query in the order denoted above.
| 'LCSC' | 'JLC' | 'MPN' | 'Mpn' | 'mpn' |
|---|
The fields will be query in the order denoted above.
Select 'Exclude from board' or 'Exclude from BOM' in the symbol's attributes property in order to ignore the footprint from the relevant file.
Select 'Exclude from position files' or 'Exclude from BOM' in the footprint's fabrication attributes property in order to ignore the footprint from the relevant file.
The rotation of components in KiCad Footprints does not always match the orientation in the JLC library because KiCad and JLC PCB used different variation of the same standard. Most of the rotations may be corrected by the rotations.cf definitions. To the exception cases: add an 'FT Rotation Offset'* field - with positive values indicating counter-clockwise orientation offset in degrees.
If the JLC preview shows a footprint like this, enter a rotation offset of -90 to rotate pin 1 to the lower right corner.
As the rotation offset is entered in the Schematic Editor, make sure to update your PCB with the changes made to the schematic before generating a new set of production files, otherwise your changes won't be reflected.
| 'FT Rotation Offset' |
|---|
The fields will be queried in the order denoted above.
| 'Rotation Offset' | 'RotOffset' |
|---|
The fields will be queried in the order denoted above.
The position of components in KiCad Footprints does not always match the orientation in the JLC library because KiCad and JLCPCB used different variation of the same standard. To the exception cases: add an 'FT Position Offset'* field with an comma separated x,y position offset to correct it.
Use following table to quickly find out to which coordinate enter the correction based on JLC arrows clicks - depending on footprint rotation in KiCad PCB Editor status bar:
| KiCad footprint deg | x | y |
|---|---|---|
| 0 deg, Front | right arrow | up arrow |
| 0 deg, Back | left arrow | down arrow |
| 180 deg, Front | left arrow | down arrow |
| 180 deg, Back | right arrow | up arrow |
| 90 deg, Front or Back | up arrow | left arrow |
| -90 deg, Front or Back | down arrow | right arrow |
For custom angles it's best to place also a temporary straight symbol to perform alignment. Single arrow press in JLC is 0.0635mm (= 1/400in) shift.
As the position offset is entered in the Schematic Editor, make sure to update your PCB with the changes made to the schematic before generating a new set of production files, otherwise your changes won't be reflected.
| 'FT Position Offset' |
|---|
The fields will be queried in the order denoted above.
| 'Position Offset' | 'PosOffset' |
|---|
The fields will be queried in the order denoted above.
The Fabrication Toolkit reports the position of each component based on an automatically selected point of reference. This default behavior can be overridden by adding an 'FT Origin'* field to the component.
| 'FT Origin' |
|---|
The fields will be queried in the order denoted above.
| 'Origin' |
|---|
The Origin field supports the following values:
Anchor- Uses the footprint's anchor point, which can be modified in KiCad's footprint editor.Center- Uses the center of the bounding box formed by the footprint's pads.
Some footprints may have their components defined on the opposite layer to there actual footprints. In these instances you can override mount side by adding an 'FT Layer Override'* field to the component.
The Layer Override field supports the following values:
top,t- Override footprint layer to the top.bottom,b- Override footprint layer to the bottom.
| 'FT Layer Override' |
|---|
The fields will be queried in the order denoted above.
| 'Layer Override' | 'LayerOverride' |
|---|
The fields will be queried in the order denoted above.
The plugin can also be used via the linux command line. This can be particularly useful if you need to embed the plugin into an automation pipeline or environment. The plugin can be called with the command below:
python3 -m plugins.cli -p /myProject/myBoard.kicad_pcb
The all options from the GUI are also available via the cli interface:
python3 -m plugins.cli -h
usage: Fabrication Toolkit [-h] --path PATH [--additionalLayers LAYERS] [--user1VCut] [--user2AltVCut] [--autoTranslate] [--autoFill] [--excludeDNP] [--allActiveLayers] [--openBrowser]
Generates JLCPCB production files from a KiCAD board file
options:
-h, --help show this help message and exit
--path PATH, -p PATH Path to KiCAD board file
--additionalLayers LAYERS, -aL LAYERS Additional layers(comma-separated)
--user1VCut, -u1 Set User.1 as V-Cut layer
--user2AltVCut, -u2 Use User.2 for alternative Edge-Cut layer
--autoTranslate, -t Apply automatic position/rotation translations
--autoFill, -f Apply automatic fill for all zones
--excludeDNP, -e Exclude DNP components from BOM
--allActiveLayers, -aaL Export all active layers instead of only commonly used ones
--openBrowser, -b Open web browser with directory file overview after generation
Benny Megidish