I have access to a CNC (not at DMS) and I have never cut any wood products (just aluminum and acrylic). I am looking to rout pieces out of a 3/4" maple plywood sheet with a 1/4" bit. I could look for feed and speed rates, pass depths, etc. online but I figured I had a pretty good resource here on Talk. Any info and/or advice would be greatly appreciated.
Feeds-n-Speeds recommended by Multicam SIG (@Team_Multicam) are stored in a database accessed thorough Vcarve on jump server. If you just need this info one time, I can dig it up; if you think you will need this type of info on an ongoing basis, it’d be better if it was explained in more detail.
I don’t foresee myself cutting anything other than plywood with that 1/4" bit. If it’s something that is quick and easy for you to access, I would greatly appreciate it, but I’m sure I can go find you next time I’m up there if you are willing to show me how to get to it. That way if I ever do need to use it in the future I don’t have to bug you again.
OK. Speed = 18000 rpm; Feed = 252 inches/min; Pass Depth = .25 inches (bit diameter); Plunge Rate (if applicable) = 40 inches/min; Stepover (if applicable) = 20% (.05 inches).
@bertberaht or someone will hopefully comment if I have steered you wrong or left out important consideration(s).
Short version: if you can get to Jump server and open Vcarve, start a new project then open tool database from the Toolpath menu drop down. That will get you to this:
Just going to drop these here, for future reference/edification of others:
https://www.onsrud.com/images/S%20Plywood%20Cutting%20Data.pdf (as a stand-in for what Brian linked here, link being inop presenlty).
WoodShop Committee Meeting Tuesday Jan 5 7pm
OK. I’m a liar. I’m going to come back and add that I thought Brian’s explanation of how he uses manufacturer info, math, and procedure might be applicable to THIS case, as well as being generally helpful to these types of situations.
Yep. Are you (Brenda) buying a bit? If yes, consider a 1/4" compression bit. You’ll get better results (if you do your part), Less ridging and tearout in the center of the sheet, cleaner edges requiring much less cleanup (sanding) when done. And they cut fast too. I cut 3/4 Baltic Birch in one pass using a 1/4 onsrud compression bit at somewhere around 275-350IPM. using a .80 depth of cut. If edge finish is important, use a piece of 1/4-3/8 LDF/MDF as a backer so you can fully pierce the veneer when cutting. If you lay the sheet on the spoilboard, it (the machine) won’t let you cut quite deep enough, so you’ll need to run the edge router around the perimeter, then lightly buff off with sandpaper to your desired texture. If you use a backer, a quick whiff with the sandpaper and out you go. Both edges should be completely free of tearout.
If you use a downcut mill, use the F&S Marshall posted, and a depth of cut of .30. Remember - with an upcut mill, the smooth veneer face will be on the bottom of the cut - right where the machine limits you to maxZ (bottom depth you set when you grounded the bit to set top and bottom of your work). So with an Upcut bit, you’re going to get two ragged edges, with one being pretty nasty. More time cleaning and sanding the edges. A downcut mill will cut the top veneer clean, but leave the bottom raggedy with tearout (slightly less time cleaning and one nice edge.)
BTW - a 3/8 compression bit cuts 3/4 ply like butter and PDQ. If your design allows it that is.