Creating a "pick and place" file

I am in the process of designing a board that will be manufactured as a turn-key project (PCB fabrication, components purchasing and assembly). This is the first time that I am doing it using Kicad, in the past these operations were done by an outsourced PCB editor that used a different package.
One of the files requested by the manufacturer is a “pick and place” file for the automatic placement machine. I looked into a previous example and basically it provides the component reference, coordinate of the center of the component and its orientation.
From the Kicad documentation I understand that this can be done providing the attributes are set correctly and here I got a bit stuck.

  1. In the documentation it says that you need to set the attributes of the footprint to “Normal+Insert” however in version 5.0.2 there is are no attributes and instead there is a “placement type” with the options to “through hole” “SMT” and “virtual”. My assumption is that this replaced the attributes and “SMT” is equivalent to “Normal+Insert”. Is this correct? If not - where are these attributes?
  2. Which layer defines the center of the component? Is it the courtyard layer? Do I need to specify somehow the center of the footprint or does the file generation process calculates it by itself?
  3. What defines the 0 orientation? I assume it is the way the footprint is drawn in the editor but, for example - is the 0 orientation of a 0805 footprint when the pads are left-right or top-bottom?

Right. “SMT” is equivalent to “Normal+Insert”.

Every footprint has an anchor. The anchor coordinates define the center of the footprint.
There is a small cross indicating the anchor. It can be shown/not shown with the layers_manager->items on the right toolbar.

Usually at the component datasheet there is a section “tape and reel information”.
I have never had problems with a manufacturer due to a bad oriented footprint. Usually I also mark the 2 pin (or other symmetric footprints) orientation for diodes and similar components.
Talking to the manufacturer to know how do they want component orientation marks helps a lot.

Industry standards. In this case IPC-7351B. (version B is the current standard. Version C is expected to be released shortly since 2016.)
And of course there is a conflicting standard by EIA which defines opposite directions for some polarized parts like capacitors. (aren’t we lucky that we have that many standards to choose from?)

There are two zero orientations defined in this standard (A and B)

Good explanation:

And yes if you talk to your manufacturer you can get away with nearly anything but i really suggest you decide on either using level a or level b orientation exclusively.

1 Like

Regarding the 0 orientation, @Rene_Poschl is technically correct, and I generally strive to meet standards for clarity as he suggests. However, every turnkey manufacturer I have used checks the rotation independently of the .pos file due the inconsistencies they deal with between standards, libraries and tools as he points out. I am consistently asked for two things:

  1. The .pos file with the center loctaions
  2. Pin 1 clearly marked on the Silkscreen Layer (preferred) and/or Fab Layer

Even if my .pos file contains the correct rotation data, they will still ask for #2. Be sure all parts rotations are clearly marked on those layers, and it will help your sanity when debugging also.

1 Like

Thanks to all for the information

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.