Not too long ago KiCad did not have the capability to DRC checks on graphics placed on a copper layer, and a hackish way of adding some graphics on a copper layer did work. For some time though (about a year?) KiCad generates DRC violations for track segments and pads that overlap with graphics on a copper layer.
You are of course free to do so in your own projects, but I do not like it if you teach sloppy methods to others.
Combining the graphic shapes with the pads as eelik mentioned is a very small extra step, and without that step KiCad won’t let you draw a track to the pad, because that would violate DRC.
Drawing some graphics, then moving it to F.Cu and combining it with a pad such as described earlier does work. Your graphics are also very simple straight lines, so there is no use in being cleverer then needed, and drawing some lies in KiCad itself is just fine. No need for DXF, or even dragging in 3D.STEP files for this.
An alternative method is to just use a few SMT pads and then overlap them in the Footrpint editor to make a bigger and more complex pad.
If you put graphics on a copper layer, then it will be covered by solder mask, and this is … not recommended for switches
If you combine multiple SMT pads, then the pads have cutouts in the solder mask, but also in the paste layer, which is also probably not what you want, so you have to disable the paste layer for those pads.
The photograph has a single big square cutout in the solder mask. The recommended way to do this in KiCad is with an “aperture pad”. An aperture pad is nothing special, it is just a regular pad, but with the copper layers disabled, and also with the pad number removed. Because it has no pad number, You can’t connect a track to it, and you can use use it for custom shapes on the solder mask and/or solder paste layers. Search KiCads footprint libraries for “Thermal” to get examples of this.