How can I speed up Speeds/Feeds for the tools? 2.5 hours for this seems like a little much, especially for the bowl bit?
Ideas?
Winecaddy.c2d (380 KB)
Trays. Split into 2 paths. First one 0.300 deep, slower but with a much larger stepover. (Rough)" Perhaps 0.150 per cut depending on material. Keep this one as the 2nd path with a start depth of 0.300. Or better yet, use a flat bottom tool out to the center of the radius, and only use the ball mill for finishing the wall.
Wine Hole. 10000 seems too slow for a 1/8" tool. Use a larger tool with the appropriate geometry. You’ll cut faster & deeper per Pass. 1/4" tool, 15000 RPM, 60-120 IPM, 0.125" per Pass
Legs. I’m struggling to understand this one. If it’s 2 “H” shaped pieces they should be separated or made to fit with a tool between them. Again, larger tool.
Outline. No offset? And cutting through 3/4" with an 1/8" tool? I’d bump this one up to a 1/4" as well.
Time is a function of depth per pass, stepover (when used), and feedrate. Increasing any of them will shorten your time.
1 Like
To expand on that, @Julien worked up:
Cutters & collets | Shapeoko CNC A to Z
and
Feeds & speeds | Shapeoko CNC A to Z
which go over some of the underlying principles.
2 Likes
What type of material and what type of machine.
Materials would differ but mostly hardwoods.
Shapeoko 3XXL, Ball screw…
Okay these are all awesome suggestions! I’m really appreciating the help.
The legs I figured can intertwine so that I don’t have to cut each set and that I know that they’d fit into each other when folded. So, I’d want to make one toolpath for them instead of two separate legs.
1 Like
Here is the file with updated toolpaths.
I used a 3/4 bowl bit:
Amazon.com
I changed the tray toolpath to the 3/4 Bowl Bit with two different tool paths. One toolpath is the Roughing toolpath. It starts at 00.00 and goes down to .3" with a .375 stepover. The Finish Toolpath starts at .3" but then finishes at .313 with a .125 stepover. This will save you a ton of time in the sanding phase.
I also changed the Wine Hole and Tray Outline to a .25" EM.
I don’t know what you are trying to do with the “H” vectors, so I left them alone.
My changes significantly reduced the machining time.
The stepover on the bowl bit was 0.008". Try something like 50% of the diameter.