These are probably anchoring pins for connectors or switches. Elongated, or oval, holes are a long-standing problem with inexpensive, quick-turn boards. Many fabricators do not support them at all. Others impose a surcharge. A few will permit you to approximate them with overlapping drill holes, even though that violates their minimum hole-to-hole spacing. I recall a Forum thread from a month or two ago that discussed dealing with one fabricator’s offering.
I have avoided elongated holes on prototype boards. Like you, I call out a round hole with a diameter right at, or very slightly over, the largest tab dimension to be inserted. With manual soldering I have usually managed to pour enough solder in to fill the hole, or at least firmly anchor the pin. The key is to have enough WATTAGE in the soldering tools - I often use TWO of the Hakko FX888’s (50W each, I think) to solder switch tabs and connector frames. Jacking up the tip temperature to a zillion degrees isn’t the same thing - doing that makes it more likely that I’ll leave a trail of scorched or delaminated spots on the board around the tab.
That trace-to-pad connection geometry may have something to do with the PCB fabrication process (concerns for over- or under-etching in confined areas), but I’ll wager it’s related to getting a good solder joint between the component and the pad. The wide trace pulls heat away from the pad, causing it to heat less uniformly than the other IC pads in Figure 12 and a potentially less secure solder joint. A short length of narrow trace keeps more heat in the pad. I wouldn’t expect that kind of problem in a modern reflow oven that goes to great lengths to heat everything very uniformly, but it’s my best guess to justify Seeed’s requirement. Or perhaps they’re thinking about manual soldering and re-work, where soldering SMT devices is much more troublesome.
For the TO-220 MOSFET on your hand-soldered board, ease of soldering is almost certainly the main concern. I would neck-down the trace to the Drain for 0.1" (2.5mm) or so from the pad, and add thermal relief spokes to the Source pad.
The question, “How wide should a trace be?” has no easy answer. To start with, you must define what a trace “failure” is. Is it de-lamination of the trace from the substrate? The voltage drop across a length of trace? A certain temperature rise in the trace? System power dissipated by the traces? Vaporization of the trace? You can start to appreciate the complexity of the question by opening the “Calculator Tools” in KiCAD’s main shell and going to the “Track Width” tab.
Setting aside those (very real) details, many design guidelines will suggest that 1 amp of current can be handled by a trace of 1-ounce copper that is 10 - 12 mils wide, on boards operating in common, benign, environments. That suggests a 60 - 80 mil trace, or three 25-mil thermal spokes should be adequate.
Here again, I don’t know if SEEED is concerned with board fabrication or assembly solderability. I have never hesitated to make direct connections between pads, though I place them at the far edge of the pad, away from the IC body.
I don’t know what SEEED is trying to show in Figure 14. It may be addressing situations (like the anchor pins for connectors or switches) where mechanical strength is a significant concern, as well as electrical connectivity. If they’re telling us that holes may not be exactly positioned (which is true, and unavoidable) then I’d deal with it by making the pad a little larger, or possibly elongating the pad in the direction of the trace attachment point.
With KiCAD’s through-hole pads you can specify a pad shape that is shifted from the hole center using the “Offset” parameters.
And here is a power “barrel jack” where I elongated and offset the pads with the intention of achieving stronger, manually-soldered joints.