Solder Paste Aperture Size Changes

I hereby certify that I am not simply asking someone else to design a footprint for me.

This is an auto-generated message that is in place on the “footprints” section of the forum. If I remove it and ask for a footprint to be designed anyway, I understand that I will be subject to forum members telling me to go design my own footprint or referring me to a 3rd party footprint site.

I am new to KiCAD and am currently using it on a couple home projects. Is there a way to have the solder paste openings updated globally for specific aperture codes as I have a tight pitch BGA that will not allow for a 4mil stencil and need to move to a 3mil stencil for proper release? Without updating the other paste openings I would be reducing the solder volume by about 25% on some pads and more on others.
I do not have a Gerber editor, like Gerbtool, that allows for updating Gebers to have this done in post processing and I would prefer to have this be in the layout software.

Not globally, but you can set the solder paste aperture ratio for a footprint and for individual pads. It’s in the footprint or pad Properties -> Local Clearance and Settings. You can edit the library footprint if it’s in your personal library, or you can open a footprint directly from the board and update only that one instance.

In the Board Setup you can set the default clearance which is used if the value in the footprint and pad properties are zero.

If you need to change more than one footprint, maybe the best strategy for you is to copy the library footprints to a project specific library, change the values there and make the project use those footprints.

Once you have “aperture codes” you’re in the realm of gerber files, and KiCad has no way to edit gerber files.

I assume you have a single (or a few) footprints with this pad size. I would probably solve this by changing the footprint, and then updating the PCB with this custom footprint.

A bit more detail:

  1. Open Pcbnew, select one of the offending footprints and press [Ctrl + e] to load it in the Footprint Editor (which is also the footprint library maintenance tool)
  2. Footprint Editor / File / New Library and add it to the “Project” library table when KiCad asks for this. You now have an empty library.
  3. Footprint Editor / File / Save as and fill in the name of your footprint, and also select your newly created library to put your footprint into that new library.
  4. Update the footprint link(s) in the schematic to use the footprint in your new project specific library.
  5. Eeschema / Tools / Update PCB from Schematic [F8] and turn on Update Footprints.

At this point, you have separated your footprint completely from external libraries, and you can edit it in the footprint editor.
In the Footprint Editor, you can change one of the pads of your footprint, then right click on the pad and select: Pads / Copy Pads Properties from the popup menu. Then you can select a bunch of other pads, right click and select Pads / Paste Pad Properties to make them have the same properties as the first pad you changed.