I am using a PCB(A) factory where they have an online system where you can get a preview of your PCBA once you upload your files. As part of the process, I have to upload the Gerbers, the Bill of Materials (BOM) and the component placement list (or footprint position file, as it's called in KiCad).

The last one is generated through the PCB Layout editor from the File --> Fabrication Outputs --> Footprint Position (.pos) File menu and contains the orientation of the components among other information.

The issue is that the orientation of most of the components is incorrect, according to the factory's preview system. Of course it doesn't matter that much for resistors and capacitors, but as you can imagine I have to manually rotate all the rest, everytime I place a new order or do a small change.

Am I doing something wrong or is there a convention for the KiCad footprints (e.g. pin 1 has to face at a certain corner always) that I am missing?

  • \$\begingroup\$ Contact the factory, rather than relying on the preview - this is the sort of thing they should catch. There is the KiCad Library Conventions kicad-pcb.org/libraries/klc which should be helpful. Check the match with the packaging information in the datasheet. \$\endgroup\$
    – awjlogan
    May 7, 2020 at 19:08
  • \$\begingroup\$ Are you using a single layer PCB? There is a setting in Kicad how the components should be placed and on which layer. \$\endgroup\$
    – CFCBazar
    May 8, 2020 at 6:52
  • \$\begingroup\$ @CFCBazarcom No I am using a 4-layer PCB. Which setting are you referring to? \$\endgroup\$
    – DimP
    May 11, 2020 at 1:03
  • \$\begingroup\$ First please tell me are all of your footprints oriented wrong, or only some of them. Also any identification for which footprints are oriented wrong, can help(only SMD, only THT or other paramter if possible). \$\endgroup\$
    – CFCBazar
    May 11, 2020 at 11:09
  • \$\begingroup\$ I am using only SMD components. There doesn't seem to be a pattern on the components that are wrong, however they are grouped according to the footprint (so for example, all SOT23-5 components are off by 90° degrees. \$\endgroup\$
    – DimP
    May 11, 2020 at 22:39

1 Answer 1


A big problem with position files is that there is more than one standard for the so called zero orientation of footprints. The official library uses zero orientation standard A from IPC-7x51. Simplified this means pin 1 is always at the top left corner.

There are other standards. For example the orientation B from the same standard that places pin one on the bottom left corner.

A more detailed explanation can be found here https://blogs.mentor.com/tom-hausherr/blog/2011/01/14/pcb-design-perfection-starts-in-the-cad-library-part-10/

The situation is even worse regarding component orientation inside the tape. Typically it is however the responsibility of the board house to map the PCB zero orientation to the tape and then the machine zero orientation (tapes can be fed from different sides relative to the PCB orientation inside the machine)

  • \$\begingroup\$ That's actually quite helpful. Probably means I will have to stick with one standard for my components and manually rotate them for each fab house. I know they do their AOI and also manual checks, but just to be 100% certain each time. \$\endgroup\$
    – DimP
    May 11, 2020 at 1:06
  • \$\begingroup\$ The blogs.mentor.com link is now broken, but I believe the following link points to the same series of articles, and it's Part 14 that seems most germane: innofour.com/8448/news/literature/… \$\endgroup\$
    – gwideman
    Mar 9, 2021 at 3:34
  • \$\begingroup\$ The innofour link seems broken, but I found a PDF of the series at edatop.com/down/faq/pads/… for now... \$\endgroup\$ Jun 3, 2021 at 4:18

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.