Can someone check my CNC feedrate calculations?

I’m trying to learn about feedrates and I’m mostly lost. the calculators online seem helpful, but I want to make sure I’m using them correctly. I’m using this calculator

for learning purposes I’m sticking to a 1mm depth

I’m using a 2 tooth 1.5mm bit so my tool diameter is about .06in

Snapmaker original spindle speed is suggested at 12000rpm

using this chip rate chart, I’m going to estimate a 1/16" (close enough to .06?) in hardwood (close enough to bamboo?) would need a chiprate of around .0015ipt

This calculator spits out 36 in/min or 914.4 mm/min

That seems fast but I’m new to this. the only other thing I’ve milled so far was plywood with the same 1.5 mm bit at fusion360’s default 100 mm/min. Are any of my numbers off or did I do something stupid? Any reference values to get an idea of what a normal range might be?

Edit: fixed some decimals

Just quickly redoing your numbers:
1.5mm cutter, not .15mm.
.015IPT gives a resultant IPM of 360, not 36, so 9000mm/min.
There’s nowhere near enough spindle power to accomplish this.

0.015ipt is under the 3/8" cutter diameter row, incorrect for a 1/16" cutter.
For a 1/16" cutter I’m going to extrapolate from this chart and combine some other resources to arrive at 2 thou per tooth.
This gives 48IPM, or 1200mm/min.

That is also too high.

These calculator numbers are ‘correct’ in the sense that will result in maximum cutter edge efficiency and leave a nice surface finish. It’s also completely unobtainable on this machine because there are other constraints, like spindle power and machine rigidity. That calculator assumes your machine is capable enough that you don’t need to consider those.

With just a 50W spindle, you won’t be able to achieve that. If you wanted to attempt this you would likely need very shallow depth of cuts, maybe .5mm or less.

@sdj544, do you have any suggested starting feeds and speeds?

1 Like

Thanks, Brent. That was really helpful. I fixed my numbers in my original post. It’s nice to now what’s “feasible”, even though snapmaker won’t do it. I’d love to hear some suggestions of examples from people.

I’ve found the feed-rate calculators to be fairly useless when it comes to real world use - at least with the SM.
With hardwoods like oak and maple I generally do a .5mm step-down with a 400mm/m work speed. For clearing with a 6.35mm (1/4" bit) I may do a 1mm step-down when I’m not worried about deflection and surface finish and I’m leaving 1mm or more of stock.
For softwoods like pine or poplar, somewhere from 600-800mm.
And that’s pretty much with all bits 1.5mm to 6.35mm. Which at first I thought was strange, but it seems to work out.
Below 1.5mm I’ll slow down to 300 just to keep from breaking bits.
I think the best piece of advice I can give is to listen to the machine.(and watch the rpm’s) It’s pretty obvious when you’re pushing it too hard. You’ll quickly get a feel for it.
You can also check and see if your bit is getting hot.
The point of the feedrate calculators is to optimize performance and maximize tool life. In a commercial environment this is more important where you’re trying to make money.


1 Like

This was exactly what I was looking for thank you. Today I tried 300 mm/min 1mm step down into soft ply and everything sounded happy (happier than at 100 mm/min, maybe). I’m happy to hear experience will help, it’s just nice to have some guidelines to know how big of steps to take. I appreciate your input.

Tomorrow I’ll try a .5mm step down with a 400 mm/min workspeed into unknown bamboo (A cheeseboard I picked up). I’ll report back here in an edit with results!

Edit: It worked fantastically!

One thing I forgot to point out is that depending on the wood, whether your passes are going with the grain or across the grain can make a big difference. Both in terms of resistance for the cutting path as well as cleanness of cut. Something like oak that is both hard and large grain will need slower speeds than a maple that may be just as hard, but has finer grain.
Bamboo and poplar may give you fits trying to get a clean edge because they’re so fibrous.
While you can plow through with a duller bit on hard woods you’ll start to notice if your tool isn’t sharp on these. Usually a little sanding will take care of it either way.

1 Like