When laying out a board in KiCAD, there's few tips to follow:

• Minimum track width: 0.2mm
• Minimum track clearance: 0.2mm
• (optional) Don't do clearance to the board edge (source: https://forum.kicad.info/t/zone-to-board-edge-clearance/45386/4)
• Place symmetrical align holes, for example a hole in every corner, exactly 3mm from the edge
• Place board "Grid origin" and "Drill/Place File origin" points in the bottom left corner of the board
• Take special care of through hole components! This PCB doesn't have plated holes and so the component needs to be soldered from both sides in order to link top and bottom layer. KiCAD will by default link signals or ground planes using a through hole component, in the same way it does with a via. However, some components might not make the top side available.

For through-hole component that cover the soldering point on the top layer, it might be a good idea to route a "backup" track on the back layer, just in case it's not possible to solder them from the top, or only route on the back layer where you're sure to get good contact.

Finally, before exporting, make sure the check

Export

To export the files, navigate in KiCAD to Files -> Fabrication output -> Gerbers (.gbr) ...

• Set output directory, e.g. "CAM"
• Include layers: all copper, silk, mask and edge cuts
• Under "General options", select "Use drill/place file origin"
• Before export, it's a good idea to run design-rule check. This will provide feedback on any unconnected tracks, overlapping silkscreen etc that should be fixed
• Finally, press "Plot" to export the files
• Then, press "Generate Drill Files" to export drill patters and sizes
  • In the new window, make sure "Drill File Format" is "Excellon" and "Drill origin" is "Drill/place file origin"
  • Finally, press "Generate Drill File"
• Close both dialogs

Isolation Routing

To process exported files into a CNC job, we'll use FlatCAM. 

• Start by importing F.CU layer
• Double-click the layer and and select "Isolation Routing"
• In the tools table, we'll set tool diameter to 0.19mm. This has to be lower than the "Minimum track clearance" setting in KiCAD to ensure correct routing. As a side note, I'm using 0.2mm V-bit for isolation routing. So the correct setting here would be 0.24mm instead. So in reality, all the pads and tracks will be 0.05mm undersized. I have tried this step with bit diameter as low as 0.1536mm for a 0.2mm bit, and the results were still satisfying.
• To generate the CNC object from geometry, set V-Tip diameter 0.15mm for cutting depth of -0.0746mm.

Settings

Copper clearing

Usually, it's enough to just do isolation routing, but sometimes, there's the need for clearing copper areas. FlatCAM has NCC feature for that.

This can be used to generate geometry and a following CNC job.