I had a brief look at the txplore tutorial you mentioned, and it looks quite complete. Date on top is from 2016 though, and some details probably have changed.
If you want to get a grip on designing your own footprints, or even make a PCB, you have to have a clear idea of what the layers do and how they work.
Your first attempt (Start of this thread) failed because the pads were on the bottom of the PCB, while the copper tracks that should connect to them were on the top.
A lot of the layers in KiCad have very specific meanings ( Silkscreen, courtyard, Edge.Cuts, etc) while other layers (Dwgs.User, Eco1.User) are mostly arbitrary, and are meant for your own notes.
You can read more about Layers in the Pcbnew User Manual.
On my PC (And somewhere on yours if you installed the documentation):
Or on the KiCad Website:
KiCad does a lot of things automatically.
If you make a new footprint, then it automatically puts the Reference name on the Silkscreen. If you draw a SMD pad, then it automatically creates a cutout in the solder mask and solder paste.
I created the asdf_Testpoint from scratch by defining a single SMD pad.
I created the asdf_Fuse by copying data from a 1206 resistor (There may be some leftovers from the resistor in the footprint) and modifying it a bit.
I drew the fusewire as a pad, and then manually removed the [v] checkbox for the cutout in the soldermask, so it gets covered under the mask.
I would have liked to draw it directly on the copper, because of DRC, but I don’t know how to do that.
I “abused” a THT (Through Hole Technology) pad as a via, because I had troubles starting a track from the pads because the “fusewire” pad needs a clearance and I could not get to the center of the pad with a track.
You have now a custom Footprint library in the FuseBoard project. I recommend to add a few Footprints to it, and then examine what it means.
With the 3D viewer you can have a pretty goot representation of what the final result will look like.
Pcbnew / View / 3D Viewer
Oops, I just looked at the bottom of your board in the 3D viewer.
It automatically created “Thermal reliefs” in the connection between the zone and all the pads. You probably want to remove them for all the fuses, and maybe also for the solder pad TP11, or at least make those spokes wider, or they may also become fuses on you PCB
Most of the things in KiCad are not very difficult, but because there are so many details you can change it all becomes pretty confusing.
Here is a screenshot of the bottom of the PCB:
Then I grabbed the solderpad on the bottom and dragged it to a corner:
You can see it moved the pad, but the spokes from the thermal relief (Green cross = copper under solder mask) has not moved.
You can update the zone settings by pressing “b” in Pcbnew.
KiCad makes the zones according to a bunch of rules. The cutout for the pads are all automatically calculated. I drew the zone itself as a big pentagon around the rectangular PCB, and still KiCad knows to only fill the zone upto 0.5 mm from the edge of the PCB.
Don’t be afraid to experiment. Worst case you delete the edited files and start over from the zipped project. (If you made something beautiful it’s wize to make your own backups of that).