Skip to content

Fabrication: JLC PCB

The basic usage of this exporter is: 

kikit fab jlcpcb [OPTIONS] BOARD OUTPUTDIR

When you run this command, you will find file gerbers.zip in OUTPUTDIR. This file can be directly uploaded to JLC PCB site. KiKit automatically detects the number of layers.

If you want to name your files differently, you can specify --nametemplate. This option takes a string that should contain {}. This string will be replaced by gerber, pos or bom in the out file names. The extension is appended automatically.

Assembly

If you would also like to use the SMD assembly service, you have to specify --assembly option and also provide the board --schematic <schematics_file>. KiKit will generate two extra files: bom.csv (bill of materials) and pos.csv (component placement). Use these two files when ordering the PCB assembly.

The files above will include all components on the board. You can override the default field name with option --field. This option accepts a comma separated list of names. The first found field is used. This can be used, e.g., for configuration of the board via resistors. You can put field "LCSC" for all components, then add fields "CFG1_LCSC" and "CFG2_LCSC" for some components. Then invoke KiKit with option --field CFG1_LCSC,LCSC for configuration 1 or --field CFG2_LCSC,LCSC for configuration 2.

You can exclude some of the components by specifying --ignore <comma separated list of references>. You can also specify component field with name JLCPCB_IGNORE (the value of the field does not matter) to exclude the component from assembly. Also, if a component misses the order code field, KiKit will show warning. When you pass option --missingError, KiKit will fail when there is a component with missing order code. This might be useful in case when you run KiKit in CI and you want to fail the build.

Note that when you order SMD assembly for a panel, you should specify panelized board and the original schematics of a single board.

Correction of the Footprint Position

It is possible that orientation footprints in your SMD does not match the orientation of the components in the SMD assembly service. There are two solutions:

  • correct the orientation in the library or
  • apply KiKit's orientation corrections.

The first option is not always feasible - e.g., when you use KiCAD's built-in libraries or you are preparing a board for multiple fabrication houses and each of them uses a different orientation.

KiKit allows you to specify the origin and orientation correction of the position. The correction is specified by JLCPCB_CORRECTION field. The field value is a semicolon separated tuple: <X>; <Y>; <Rotation> with values in millimeters and degrees. You can read the XY corrections by hovering cursor over the intended origin in footprint editor and mark the coordinates. Note that first the rotation correction is applied, then the translation. Usually, you will need only the rotation correction.

Using Corrections to Configure Jumpers

If your board features solder jumpers you can use the corrections to specify their default value. The solder jumper should be designed such it can fit a zero Ohm resistor in suitable size. Then specify an order code of the zero Ohm resistor for the jumper and adjust correction so it fits the default position.

Note that you can specify multiple correction fields by --corrections <comma separated list of correction filed names>. The first found correction field is used. This allows you to keep several configuration of the solder jumpers in your design e.g., in fields JLCPCB_CORRECTION_CFG_1 and JLCPCB_CORRECTION_CFG_2. Then you can simply change the board configuration by calling kikit with --corrections JLCPCB_CORRECTION_CFG_1,JLCPCB_CORRECTION or --corrections JLCPCB_CORRECTION_CFG_2,JLCPCB_CORRECTION.