Most operators reach for the speed override when a turned part comes out rough. The finish was decided by the feed rate and the nose radius before the spindle ever came up to speed. Feed is the cheapest lever in turning—it buys metal removal almost for free—and it is also the one that sets your surface finish by a square law. Here is what it actually controls, the one formula worth memorizing, and where to start.
What Feed Rate Means on a Lathe
On a lathe, feed rate is how far the tool advances along the part for each turn of the spindle. In an American shop, that is inches per revolution—IPR. A feed of 0.010 IPR means the tool walks 0.010 inch down the part every time the part goes around once.
Your control can express it two ways, and mixing them up wrecks parts:
- G99—feed per revolution (IPR). The normal mode for turning. The feed scales with the spindle, so the chip stays the same thickness whether you are at 400 or 2,000 RPM
- G98—feed per minute (IPM). The tool moves at a fixed rate regardless of spindle speed. Useful for some canned work, dangerous if you meant IPR
The two are related by one multiplication: IPM = IPR × RPM. A tool at 0.010 IPR and 1,000 RPM is traveling 10 inches per minute. Leave a 0.010 in a G98 block and the tool creeps at a hundredth of an inch per minute; leave a 10 in a G99 block and it tries to take a ten-inch bite per revolution.
The One Formula Worth Memorizing
Feed rate and nose radius together scribe a helical groove in the part, and the leftover peaks between passes are your surface finish. The geometry gives you the theoretical roughness directly:
Ra ≈ f² ÷ (32 × r)
where f is the feed in inches per revolution and r is the insert nose radius in inches. The answer comes out in inches—multiply by 1,000,000 for microinches.
Read the two exponents in that formula and you have the whole lesson. Feed is squared. The nose radius is not. Double the feed, and roughness goes up four times. Double the nose radius, and the roughness is cut in half.
Here is what that looks like in numbers, in microinches Ra:
| Feed (IPR) | 1/64 in radius | 1/32 in radius | 1/16 in radius |
| 0.004 | 32 | 16 | 8 |
| 0.008 | 128 | 64 | 32 |
| 0.012 | 288 | 144 | 72 |
| 0.016 | 512 | 256 | 128 |
| 0.020 | 800 | 400 | 200 |
That is theoretical roughness—pure geometry, the best the setup can possibly do. Real parts come out worse because built-up edges, vibration, insert wear, and runout all add on top of it. Which is the useful part of the number: if the formula says 64 and you are measuring 200, the extra 136 is not the feed rate. Stop adjusting the feed and go find the vibration.
The shortcut most shops miss: when a finish is marginal, changing the insert to a larger nose radius is usually cheaper than slowing the feed, because the feed cut costs you cycle time on every part from now on, and the radius costs you nothing per part.
Why the Nose Radius Is Also Your Ceiling
You cannot keep raising feed to chase cycle time, and the limit is the same radius. Once the feed per revolution approaches the nose radius, the corner is no longer easing into the cut—it is being asked to shear a chip thicker than the radius that is supposed to support it. Chip control goes first, then the corner.
Two working limits:
- Finishing: Keep feed at or below half the nose radius. With a 1/32-inch radius, that is about 0.015 IPR, and real finishing feeds live well under it
- Roughing: the nose radius itself is the hard ceiling. Above it you are trading insert corners for cycle time and losing
This is also the reason a bigger radius is not free. It cuts roughness in half and raises your feed ceiling, but it pushes the cutting forces radially—into the part and into the bar. On a long slender shaft or a deep bore, that radial push is exactly what you cannot afford.
Feed Is the Cheap Way to Move Metal
Metal removal rate in turning is close enough to:
MRR (in³/min) ≈ 12 × SFM × DOC × f
Run 500 SFM, 0.100 inch depth of cut, 0.012 IPR: about 7.2 cubic inches a minute. Take the feed to 0.024 and leave everything else alone: 14.4. You doubled the metal removal rate without touching the spindle.
That matters because of which parameter kills inserts. Cutting speed drives the temperature at the edge, and temperature is what wears carbide. Feed raises the force and the chip thickness, which the insert handles far better than it handles heat. So when you need more metal out of the machine, the order is depth of cut first, feed second, and speed last. Speed is the one you pay for in tool life.
Where to Start
The toolmaker's data for the specific insert grade and geometry always wins. Absent that, these are reasonable starting points for steel, to be adjusted by what the chip and the part tell you:
- Roughing: 0.010 to 0.020 IPR, with the depth of cut carrying the load
- General turning: 0.008 to 0.012 IPR
- Finishing: 0.004 to 0.008 IPR, and let the nose radius do the work instead of going lower
- Threading: feed equals the pitch. It is not a choice
Soft and gummy materials want more feed than the numbers above, not less—a thicker chip is what breaks the built-up edge loose. Hardened and work-hardening materials want you to hold the feed steady and never dwell.
Reading the Symptoms
Feed rate announces itself clearly if you know what you are looking at.
Feed too high: rough, visibly threaded finish; chips coming off blue or burning; cutting forces pushing the part away so diameters taper; wider burr at the end of the cut; corner chipping instead of even wear.
Feed too low: this is the one that fools people, because it feels safe. Too little feed means the chip is thinner than the edge can cleanly shear, so the insert rubs instead of cutting. You get a built-up edge, a smeared rather than smooth finish, heat going into the part instead of out with the chip, and insert life that is worse than it would be at a sensible feed. A squealing cat and a tool that is wearing on the flank with nothing to show for it usually want more feed, not less.
And one you should rule out before blaming the feed at all: if the tool is not on center height, the rake and clearance angles the insert was ground with are not the angles doing the cutting, and no feed rate will fix it.
Conclusion
Feed rate is the parameter with the best return and the worst reputation. It moves metal almost for free, it sets the surface finish by a square law, and it has a hard ceiling written on the insert box as the nose radius. Know the formula, know which direction each exponent pulls, and most finish arguments on the shop floor in about thirty seconds of arithmetic.
Keep Learning.
- Tool Center Height: The Two-Minute Check That Saves the Most Inserts
- Metal Removal Rate: The Number That Settles Every Tooling Argument
- Indexable Inserts: Maximizing Tool Life in Production Turning
- Runout: Why You Paid for Four Flutes and Are Cutting With One
- Machining Troubleshooting: Five Symptoms and the Order to Check Them
Need a larger nose radius before you slow the feed down? Browse turning inserts, turning tool holders, and boring bars—or talk to our engineering team—FM Carbide helps you machine better!