Ready To Cut CNC Art

The Orchard House


Can someone help with toolpaths for a carve like this?
The customer wants either a 2ftx4ft rectangle or 3ft round circle. It will be double sided. It’s an outdoor sign for a venue. I’m thinking 2” thick Spanish cedar for the wood choice with black painted logo. I want to vcarve it, but just the tree alone is showing an estimated run time of over 20 hours. My current tool is a 30 degree V bit 1/4”. Start depth of .25” with a flat depth of .3”
I’m trying to keep as much detail as possible.
I’m cutting on a 4x8 Artisan Infustrial CNC. I’ve pictured the spec sheet for my machine for any reference if useful to anyone.
I’m still new to this but I’ve carved a few things with quite a bit of detail with way less run times. What am I doing wrong?
Thanks in advance for any tips.
The reason it would take so long is because of all the up and down travel to plunge and retract on all the isolated dots - on each dot it takes a lot more time to travel up and down than it does to v-carve the dot - it would help to maximize the z axis velocity, minimize the z axis Safe Z Height, set the tool pass depth as deep as possible, use a 90 degree v-bit instead of a 30, with maximum acceptable flat depth, with maximum acceptable stepover, and use a flat bottom clearance bit if flat depth is much shallower than the bit's full single pass V depth - and maximize X and Y acceleration to make all those turns as fast as possible without having to slow down too much on every direction change - and as always, maximize X and Y velocity for your bit and material - going too slow is worse than going too fast because the bit gets hot, dull, and tears/plows through the material rather than actually cutting - the sawdust should be more chunky than powdery

and/or I have drawn it as a few connected cuts instead of a thousand separate tiny dots which will cut a lot faster because it only has to travel up and down a few times instead of a thousand

it will take about 45 minutes with a 1.25" 90 degree v-bit cutting up to just over 1/2" deep max at 100 ipm, 40 ipm plunge rate, .1" safe Z height

the narrowest width V cuts are in the .06" to .08" range in a few places so a 90 degree bit will cut at least .03" to .04" deep - and mostly will be cutting a good bit deeper than that - I practically never use 30 degree bits - and I only use 60s if I must but I try not to



Top Bottom