Different options when generating gerber/ drill files after PCB designing/ layout
1. FILE FORMAT
Excellon format contains the drill coordinates and the diameters of the drills. Almost all manufacturers prefer this format because it's a kinda industry standard. I've never seen a PCB manufacturer requesting the drill files in Gerber-X2 format.
2. EXCELLON DRILL FILE OPTIONS

Mirroring: Mirroring the data along the Y-axis may not be the thing you &quot;have to&quot; do. If a manufacturer prefers drilling the holes from the backside then they can mirror the data.

Minimal Header: I don't know what Minimal Header refers to and what it is used for.

Merging PTH and NPTH drills in a single file: There are two types of holes: PTH (plated through-hole, which indicates a drill with through-hole conductive plating) and NPTH (non-plated through-hole, which indicates a standard drill with no plating). Generating separate files for PTH and NPTH drills is useful when cross-checking the final gerbers coming from the manufacturer to confirm before production. I always generate separate PTH and NPTH drill files.


3. DRILL ORIGIN
The point where all the drill coordinates are referenced to.

Absolute origin: This indicates that the origin is the global (x=0,y=0) coordinate. I always prefer the global origin coordinate to be the origin for both gerber (mostly RS-274X) and the drill files.
Auxiliary Axis: I've never used KiCad, so I'm not sure. But I think that this option allows the designer to manually select a point to be the drill origin. You may not need this.

4. GENERATE MAP FILE
A drill map is a 2D drawing which contains all the drills marked with individual symbols, and a table showing which symbol indicates which type of drill (i.e. diameter, type, etc). It can be useful for cross-checking each drill, but mostly it's not required. The drill files are enough. Following is an example to a drill map (The manufacturers can generate this from the data files you send):

Img Source