Here is a little video clip. The pins on both devices are defined as “passive”. I cannot wire to or from the RGB LED pin 1. In the last part of the clip I pressed “w” on the keyboard to try and wire from the pin and it forced my cursor off the pin.
I have figured it out… I think this must be a new feature that is turned on by default? There are grid overrides. I’m not sure when this would be useful? My pin fell on the normal defined grid, but not on the wire defined grid. I just needed to uncheck the box next to wires below. FYI, I use my own library parts.
Your “on screen” grid looks quite dense. It looks like it is 25mil, and your LED is also on this 25mil grid, while the wiring is using the 50mil grid. In general the 50mil grid works best for symbol placement and wiring.
You can re-align symbols on a 50mil grid by:
First setting the 50mil grid ([Alt + 1] should probably do that)
Zoom out and select everything (or try it out on a small section).
Right click and select: Align Elements to grid from the context menu.
Your LED symbol also appears to be a non standard symbol. It is possible that it is not designed according to KLC guidelines. When a symbol is inserted (or moved) in the schematic, it is always grabbed by it’s insertion point, while during wiring, the attachment points for the wires should be on the grid.
As for the grid overrides… KiCad relies on a relatively coarse grid for the locations of schematic symbols (and their pins) and for wires to be able to work efficiently, and this grid is a bit coarse for other items such as text and graphics. The grid overrides allow for more flexibility for these other items, without having to disable the grid completely (Which can by done by holding the [Ctrl] key while moving items).
