The Orchard House

[anonymous]

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.

 

[SignTorch]

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