I’ve always wanted to do a hybrid (THT/SMD) footprint library so that it can be populated with whatever is available, kind of a supply chain crisis / recycling friendly or choosing the part size depending on the soldering skills. Now time has come with a DIY project aimed at beginners where it makes sense to give the user the choice to assemble the THT or the SMD parts.
I’ve attached an example on how those footprints look for R and C.
When routing these footprints, I can route them on the back side easily, but when trying to route the front side I can’t close the ratsnest as KiCad shows me “Cannot start routing from a Graphic”.
You drew a graphical line between those pads, and KiCad does not accept graphics as copper tracks, even when they are on a copper layer. It is possible to add graphics to a pad. To do that you select a pad, then right click and select: Edit pad as graphical Shapes. [Ctrl+E] from the popup menu.
Another method is to just draw separate pads.
When a footprint has pads with the same pad number, then KiCad assumes those pads always have to be connected. The result is that you will draw the tracks later on the PCB itself.
Edit pas as graphical Shapes always gives me exposed copper, right?
So basically I can make up for the missing track tool in the footprint editor by making an SMD pad in trace width and burying it under a mask (and not as one may assume using the more similar generic line tool).
Left side [1] is with Pad edited as graphical shape, right side [2] is with track-as-pad-technique:
Sort of, but not really.
With Edit pad as Graphical Shapes, then the graphics become a part of the pad, and which layers on a pad are active depend on the properties of the pad itself.
In your second screenshot the “track” is grey, just as the SMT pad. This means you’re looking at solder paste.
Another method is to simply use extra pads. Instead of adding the graphics to a pad, you just use a 3rd pad for the line. If you do this you can disable the solder paste and mask layers, and then it will just be some copper covered with solder mask.
Overlapping pads are quite common in KiCad footprints. Any footprint which has “thermal” in their name for example uses this technique to construct a thermal pad.
