I just finished my first PCB with KiCad. Now, I need to produce it and I need the Pick and Place file. When I try to generate footprint position files the software produce the message "No footprint for automated placement". I'm using the version 5.1.4-e60b266 for ubuntu 18.04.1. How can I generate this file? How can I solve?
Pick and place, and thus the *.pos file, is relevant to surface mount technology. The automatic placement of through-hole technology is not something that is worth the money to invest in due to the volumes produced. The problem with leaded is the need to position each leg for each hole.
If you place an test surface-mount component, you will see a *.pos file can be generated as there is x-y coordinates that makes sense for such a part.
The same problem occurred to me today using KiCad Version 5.1.4. - And I think I've found a solution to the problem:
1) Temporary solution:
KiCad: Pcbnew: 'File' -> 'Fabrication Outputs' -> 'Footprint Position (.pos) file...' -> 'Generate Footprint Position Files':
Check this checkbox in the 'Generate Footprint Position Files' dialog:
'Include footprints with SMD pads even if not marked Surface Mount'
2) Fix footprints:
One of my custom footprints was not marked as 'Surface Mount'. Somehow this made it impossible for KiCad to export the 'Footprint Position' file (the 'No footprint for automated placement' warning shows up and no footprints will be exported).
So, make sure that your SMD footprints are all marked in the footprint editor under 'Fabrication Attributes':