I think I saw on another thread someone is working on a howto doc
Software at http://scorchworks.com/Fengrave/fengrave.html (it is a python script with gui)
There are some good YouTube videos about both v-inlay techniques and this software.
There is a config.ngc file for the software that sets defaults. My pre/post gcode are in there.
(fengrave_set gpre G17 |G64 P0.001 |M3 S3000 |G0 X1.0 Y1.0 |G0 X0 Y0 ; engage steppers|G0 Z40.0 |M0 Attach M0 Attach ZProbe |G28 Z |G92 Z20.0 |G0 Z30 |F300 M400 |M0 Detach ZProbe Turn on Spindle )
(fengrave_set gpost M5|M2|G0 Z30 )
Mine uses my z-probe to set the height (my probe is 20mm puck. Will order one of Ryan’s new ones when they are back in stock)
The code generates a v-cut, v-cleanup and flat cleanup file which I cat together (z-height change pre-process allows me to also change the bit)
I like to set the v-max-depth slightly lower (0.1mm) than the depth for the flat cleanup. This avoids fuzzy joints.
I also set 0.1 or 0.2 mm larger max cut depth (I use around 4mm for my bit) for the cut out versus the inlay. Some call this a glue gap, but I think it hides any errors under the inlay more than around the edges. When I have sawed into the inlays there has been no noticeable gap.
I also save some of the dust from the CNC to mix with glue and use as a putty to fill in minor imperfections.