2
\$\begingroup\$

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?

KiCad "No footprint for automated placement"

This is my PCB: My PCB

\$\endgroup\$
4
  • \$\begingroup\$ finished first PCB? so you generated a circuit, checked it, ensured all footprints are asigned, netlisted, imported netlist into PCBnew, performed placement, board outline, tracked to complete ratsnets, DRC pass? generated design files? \$\endgroup\$
    – user16222
    Commented Sep 8, 2019 at 10:23
  • \$\begingroup\$ I made a schematic, assigned fooprint to components and connected the components in PCBnew. Isn't it enough to finish a PCB? The 3D view is fine and my PCB is not so complicated. \$\endgroup\$
    – Peto
    Commented Sep 8, 2019 at 10:30
  • \$\begingroup\$ it is fine, but you have shown no information as to what you have \$\endgroup\$
    – user16222
    Commented Sep 8, 2019 at 10:30
  • \$\begingroup\$ I'm sorry. I've updated my question with PCB image. \$\endgroup\$
    – Peto
    Commented Sep 8, 2019 at 10:33

3 Answers 3

4
\$\begingroup\$

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.

\$\endgroup\$
6
  • \$\begingroup\$ So, are you saying that KiCad cannot generate the file for through-hole technology because no one would implement that function in the software? Right? If so, can you suggest another software just to produce the .pos from KiCad file? \$\endgroup\$
    – Peto
    Commented Sep 8, 2019 at 10:47
  • 1
    \$\begingroup\$ thats not what I am saying, I am saying it isn't needed for surface mount as pos file is for pick and place machines \$\endgroup\$
    – user16222
    Commented Sep 8, 2019 at 10:50
  • \$\begingroup\$ take your R1, someone needs to form the legs to meet your layout needs. this is the same for all through-hole designs. its an additional (manual) process to deal with through-hole \$\endgroup\$
    – user16222
    Commented Sep 8, 2019 at 10:51
  • \$\begingroup\$ Now I get it! Thanks a lot. \$\endgroup\$
    – Peto
    Commented Sep 8, 2019 at 10:52
  • 1
    \$\begingroup\$ This may be true in theory, but in practice the .pos is still required for some applications. For example, JLCPCB offer a service for mounting components for you, including surface mount components. However, this service is only available if you provide the .pos file as well. \$\endgroup\$ Commented Apr 27, 2021 at 15:48
3
\$\begingroup\$

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'

enter image description here


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':

enter image description here

\$\endgroup\$
0
\$\begingroup\$

A Centroid file (*.pos) is not required for Throughhole (THT) only projects. It is only required for placing SMT components.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.