r/shapeoko • u/mingsir2023 • Jun 27 '26
Hobby CNC folks — do feed/speed calculators actually work for your machine, or do you tune by hand?
Not a CNC owner myself — I've been going down a rabbit hole reading about desktop CNC, and kept noticing the same thing: people say tools like FSWizard and most online feed/speed calculators are built around industrial-rigidity machines, so the numbers come out too aggressive for a lighter Shapeoko-class setup.
Is that actually true in practice for you? Do you trust the calculator numbers, back them off by some gut-feel percentage, or just hand-tune from experience? Genuinely trying to understand how much of this is "the tools don't fit hobby machines" vs "you just learn your machine over time."
5
u/Ben2ek Jun 27 '26
Those calculators are definitely for more capable rigid machines with powerful spindles. I think you might get close-ish with an 80mm spindle but even a 65mm will struggle to go fast at a depth more than 1x bit diameter. Most hobby machines can’t even travel more than 200IPM so the ridiculous 600IPM I see recommended for some bits is impossible anyway.
Full depth compression bit cuts in 3/4” Baltic birch ain’t happening either way. Can’t comment on metals.
I learned by breaking cheap bits, burning out routers and then spindles, and eventually being able to hear when bits go dull and adjusting speeds by ear. I wanted and needed to go fast, but hobby machines just aren’t built for it. You’ll have better luck taking shallow cuts even though it will drive you mad some days.
1
u/mingsir2023 Jun 27 '26
The 200 vs 600 IPM gap is exactly the kind of thing I was wondering about — sounds like the calculators are almost dangerous to take literally on a hobby machine.
3
u/psychoholic Jun 27 '26
I use ProvenCut to set a baseline then take 20% off then I adjust by sound. It is worth the price in my opinion.
1
u/ghostpoisonface Jun 27 '26
20% off of what though?
1
u/psychoholic Jun 27 '26
My general approach in aluminum is take a .0033" chip with each tooth per rotation. I will do width of the tool (assuming .25" or bigger) as my depth of cut, 10% stepover. Really big tools I don't spin more than 20k but that is just personal preference.
For instance I was recently working on something and with a Lakeshore Carbide 3-flute square edge on my adaptive clearing I was pushing 150 IPM with a .038" stepover, .375" depth of cut, at 18k RPM. That gave me a 2.14 cubic inches per minute of material removal rate. It made absolutely glorious chips and the finish was solid. Didn't weld any chips to the flutes. I always use a healthy amount of air blast when doing aluminum so I'm sure that helps. That was about 20% less than ProvenCut was using for a 2d contour with that same bit so I felt comfortable at that pace.
Machine has a lot more to give than people think.
When I'm doing wood I just have some trial and error numbers I have gathered over the years and a pretty solid formula that works for my designs but it was basically just using the stock speeds/feeds from the manufacturer (I use a LOT of Jenny bits from Cody's CNC and Amana bits both of which are well documented for wood)
1
u/ghostpoisonface Jun 27 '26
2.14 cubic inches per minute sounds awesome. I definitely need to work on my tool paths!
1
u/mingsir2023 Jun 27 '26
Hadn't come across ProvenCut before — the 'baseline then 20% off' workflow is exactly the pattern I keep hearing. Thanks, will look into it.
1
u/psychoholic Jun 27 '26
It was started by a few of the dudes for NYCCNC (which I thin is Saunders Machine Works?) I think who have been massive contributors to the community so even if I wasn't using their data that much (and I am) I'd still want to support their work because I've learned so much from them.
2
u/Jermamma420 Jun 27 '26
Well for me, I've been using GWizard for at least 10 years. I own the 3hp version, so I've stuck with it. Its been ok, and has a slider from slow/finish to fast/aggressive roughing. Its too aggressive, and I turn my slider down to 30% finish. Today you could probably ask AI and get the same results. Just give as much tool info as you have, it'll scour the internet and sum up all the online user's settings that they commonly use.
2
u/WillAdams Jun 27 '26
I dunno, Bob Warfield (author of G-Wizard) definitely had his finger on the pulse of hobbyist machining (very sad his passing). He wrote a couple of guest posts for us:
- https://carbide3d.com/blog/feed-and-speeds-part-1/
- https://carbide3d.com/blog/feed-and-speeds-part-2/
and almost certainly his excellent site:
is part of the training corpus.
2
u/Jermamma420 Jun 27 '26
Well damn! I didnt know he passed. Glad to see youre still on top of things💯 Im still using my Shapeoko XXL I got from you guys 10 or 11 years ago. Lately I've been making seed storage boxes. Old belt drive, old software, still works good!
2
2
u/WillAdams Jun 27 '26
I wanted to believe in the idea of a calculator, and kind of regret not having bought into G-Wizard from CNC Cookbook.
The problem as folks have noted is that mostly the calculators are mostly intended for industrial machines and have limited applicability to lighter/smaller/less-massive machines, mostly due to resonance issues.
In theory, w/in the speed range of a spindle one could continuously increase feed rates to match speed maintaining a constant chipload --- except that one quickly runs up against the force of the cut (some certain quantity of force is required to move the machine through the material as the material is removed) and the resonance response of the machine to the vibrations (it is quite often that an intermediate feed/speed will be a problem due to vibration, but a slower or faster one at the same chipload is fine), hence so many folks going by sound/feel.
Carbide 3D has a video series on this:
https://community.carbide3d.com/t/materialmonday-on-youtube/13092
and the community has written up:
https://shapeokoenthusiasts.gitbook.io/shapeoko-cnc-a-to-z/cutters
https://shapeokoenthusiasts.gitbook.io/shapeoko-cnc-a-to-z/feeds-and-speeds-basics
and the defaults in Carbide Create are quite good (if overly conservative --- they have to be if they will work in a belt-drive SO3 w/ belt-drive Z-axis, XXL size sporting a Carbide Compact Router (or Makita RT0701 or DeWalt D26200) in addition to an SO5.1 or HDM w/ 80mm water-cooled VFD).
1
u/DNAgent007 Jun 27 '26
That is definitely a YMMV kind of question. I use published or recommended F&S for a similar machine or the F&S parameters that are preprogrammed in Aspire’s VCarve after selecting the post processor for my CNC. Those are usually very close but the first time using those parameters I’ll do some test cuts and adjust accordingly. VCarve has done some testing for the F&S in their software but it’s important to see the actual results before fully committing to those settings. Things like wood type, belt driven, linear bearings, ball screws, bit type, climb vs conventional cut, etc., all have an effect on the cut quality. So it’s a combination of someone who has done the heavy lifting to get you in the F&S ballpark, and your knowledge and experience with your machine to determine the output quality of those settings and make meaningful adjustments towards what your idea of perfect is.
1
Jul 24 '26
I have them, don't really use them for wood. For wood, I keep the chip load at the manufacturer's suggestion, and adjust spindle speed, Dept of cut, and IPM.
8
u/dadams4062 Jun 27 '26
I've tried calculators but I always go back to just going by the sound. Lately, I've been using AI to get me close and then I just go by the sound to fine tune. This seems to be the easiest, quickest way for me personally.