I’ve got a footprint with a dot to indicate pin 1, standard stuff. The dot is in a bad spot, overlapping a pin of a nearby component. I want to move it somewhere it won’t interfere, while still being close enough to pin 1 that it’s obvious.
I’m aware that one way to do this is right-click “edit in footprint editor”/CMD-E which will edit this exact footprint in place without modifying the library copy.
The trouble is, I’m left guessing and checking where I might reposition the offending primitive for best placement, since the rest of the layout isn’t present. Altium lets you “unlock” primitives and Eagle lets you “explode” footprints, does KiCad have any other more convenient mechanism for one-off editing footprint primitives?
In KiCad you can not change much in a footprint when it’s on the PCB, but only edit it when it’s loaded in the Footprint Editor.
The simplest way would be to just load it in the footprint editor with [Ctrl + e], then set the footprint editor next to the PCB editor and just move it a bit. As soon as you press [Cntrl + S] your changes are “saved” (copied?) to the PCB, but you still need to give focus to the PCB editor window to trigger a redraw.
Another way is to just remove the pin one mark from the footprint itself, and then place it on the silk screen layer as a graphical item.
There used to be a method to have “loose” pads in footprints, which could then be moved individually on the PCB. I can not find that feature anymore, maybe it’s removed in KiCad V6? If that feature still exists, you can add an “Aperture Pad” to the footprint, and then only define it on the silk screen layer.
Mostly. The only way, actually two ways, involve unsetting the pad’s own Locked property. Then it’s possible to change the coordinates of the pad directly, or to use Special Tools → Move Exactly. They aren’t very useful if you want to move the pad to a certain place in the board. All other methods seem to move the whole footprint even if you initiate them from the pad. IMO this is buggy. Unlocking should allow all kind of moving. If I know the relative distance which I want to move a pad, I could do it in the fp editor. Being able to select a pad and move in on the board is useful only if I can move it freely WYSIWYG or relative to some board item, and now I can’t do it.
The only way, actually two ways, involve unsetting the pad’s own Locked property. Then it’s possible to change the coordinates of the pad directly, or to use Special Tools → Move Exactly
The third way is to:
check option “Allow free Pads” in general Prefeences–>PCB Editor–>Editiing Options
after that it’s possible to move any pad freely (and independend from the footprint) around.