Speeds & Feeds & Deflection, Oh My!

A few threads on CNC Routers inspired me to share a little of what I learned about machining.

Feeds & Speeds is a hotly debated topic amongst wood and metal workers. Feeds is the cutting movement rate, generally in inches per minute, and Speeds is the rotating speed of the cutting bit, in RPM. Deflection is how much the cutting bit bends while cutting: All tools bend, and if they bend “too much” they break.

Speed is limited by your machine to a minimum and maximum. For my Hitachi router, minimum is 8000 and maximum is 24000 RPM. An adjustable speed router or spindle is really valuable if you plan on cutting a variety of materials.

Feed is determined by several variables: The cutting bit’s “Chip Load” recommended by the manufacturer, the number of cutting edges (Flutes) the bit has, and the router or spindle speed. Chip Load is the amount of material each tooth of the cutting bit removes. Typical chip loads are between 0.001” and 0.010”. Too small of a chip load, and the bit “rubs”, meaning it ‘skates’ over the material surface without cutting, leading to excessive heat and broken bits (as well as poor quality cuts). Too large of a chip load and you’re over-stressing the bit, again leading to broken bits. The chips help carry heat away from the cut and tool, so if you don’t know the recommended chip load, call the manufacturer and ask.

OK, so let’s say we need a chip load of 0.003, and we are spinning the bit at 10,000 RPM. If the bit has only one cutting edge, we must move the bit through the material at 30 IPM to get that chip load. If we have a 2-flute bit, the feed must be 60 IPM, and 4-flute needs 120 IPM. The simple formula is Feed = (chip load * flutes) / RPM].

Really, that’s all there is to speeds and feeds: Maintain the chip load and everything else is good. Almost…

Let’s take that cutter and cut through pink foam at a cutting depth of 1/2”, the material isn’t pushing back on the bit much, so the deflection is almost zero. Now take the same setup cutting aluminum: being a much harder material, it pushes back on the bit a lot, such that moving 30 IPM with a 1/2” Depth-of-Cut (DoC) will surely break the bit. So, once we calculate the Feed & Speed, we must now limit the DoC to keep bit deflection to a reasonable value.

Calculating deflection is nontrivial and somewhat counter-intuitive. But, once you calculate it for a given bit and material combination, it stays the same. For those using CNC, you set the parameters into your tool database and you’re good forever. I do my calculations using GWizard, which offers a free trial more than long enough to calculate the entire tool crib.

One other thing about deflection: If your tool is deflecting 0.003”, that means your cut will be off by 0.003” in some direction. I know some teams feel that 1/16” is as tight of a tolerance as necessary, but with CNC tools a few thousandths is not only possible, but usual.

Here are some examples*****:

Using an Onsrud 63-760 (1/8” single-flute carbide bit for Polycarbonate) I can cut at 64 IPM and 10,000 RPM for my chip load, but only 0.020 DoC per pass or deflection goes above 0.001”. But move up to a 3/16” version of the same bit (63-768), I can cut at 64 IPM/8000 RPM, with a 0.0625 (1/16”) DoC. more than 3 times deeper.

In Aluminum, using an Onsrud 63-618 (3/16” single-flute carbide bit for Aluminum) I can cut at 60 IPM/18,000 RPM, with a 0.100 DoC. If I move up to a 1/4” 63-620 bit, I can cut 0.250 DoC at 60 IPM/16000 RPM.

The point is, small diameter bits can be a lot more fragile than you think, and big bits can be more robust that you think. As a simple empirical way to determine if you are not overworking the bit, make a cut about 18-24” long and (once the router has stopped) check the bit temperature: It should be still at room temperature. More than a few degrees warmer means you’re overworking your bit.

In conclusion: Calculate Speeds & Feeds for chip load, and set Depth of Cut for deflection. Do this well and broken bits will be rare. Now go make some chips!

Anyone else have any machining wisdom to share?

*In all cases, I’m using a 100% Width-of-Cut (i.e., 1/4” width for a 1/4” cutter) and either compressed air alone, or compressed air and mist coolant to both cool the tool bit and clear the chips. Re-cutting chips will break your bit, be a fanatic about getting chips out of the cut and off the table. Cutting narrower than 100% (most prefer about 40%) will greatly increase your possible DoC while maintaining deflection.


1 Like

Thanks, nicely explained in an easy to understand way.


Don’t forget about spindle horsepower and torque. This can be a limiting factor with larger bits and heavy torque. We have no trouble at all bogging down our 2HP Porter Cable router, even with 1/4" bits in wood.

Generally speaking, lighter faster cuts seem to be preferred over slower heavier cuts.

Here’s what we learned this year for feeds, speeds, depth of cut, bits, and cooling-

On our CNC router (4x8 foot shopbot with 18k rpm spindle), we used this .250 onsrud aluminum bit. We went full DoC on our .125 aluminum, at 90 ipm with the spindle at 13,000 rpm. We sprayed some coolant (Mobilcut 102), and had compressed air too.

On our CNC mill, we mainly were cutting .250 and .500 aluminum plate, so we used a .250 diameter three flute endmill for aluminum. We also used it on steel once, and it didn’t break. I believe we got the one with the TiCN coating.

With a .100 depth of cut, and the spindle at 5100 rpm, we went between 12 and 16 ipm. Our finish pass (.015 wide) was at full depth at 8 ipm. It is important to feed very slowly if you’re going straight into the part. If there’s enough room, do a helical plunge. We use flood coolant, which does an awesome job of clearing chips out of the way.

A few tips for accuracy- your hole diameters will only be as accurate as your endmill diameter is. We use a bunch of reground endmills, and precisely measuring their diameter is really critical. To measure bits with three flutes, you can make a little slotted hole with the bit, then measure that. Doing a slow .015 wide finish pass at full depth going nice and slow leaves a great finish, and a super accurate diameter. Our accuracy for making 1.125" holes with our .250 bit is within 3 ten thousandths.

Using good tool holders is really important too. We used a drill chuck for our edge finding bit, so our indicated edge locations were only as accurate as the drill chuck, which I measured to have about .006 runout. This end up causing a very misaligned shaft.

Absolutely, as well as bit stick-out (how far form the collet the bit extends). Reducing stickout from 1" to 3/4" can double your depth of cut.

GWizard also calculates the Horsepower & Torque requirements; in practice these generally come close to the limits only with fast, deep cuts in harder materials. In theory I could cut 1" thick aluminum with a 1/4" bit at 60 IPM…if I had 4 or 5 HP to play with. The reality is that I’ll keep all DoCs to the diameter of the cutter or less.

To Jared’s point: Mills don’t like to plunge (like a drill): enter the workpiece with a ramp or helix. Flood coolant is awesome, but only if you have a way of managing copious quantities of liquid.

Oh, and my 1/4" cutter for wood measures 0.243" OD; easily compensated in software, but only if you know the real measurement.

1 Like