Turning on a lathe is the most fundamental machining operation, but getting the setup right still trips up experienced machinists. The workpiece rotates, the tool is stationary, and every variable you change affects finish, tool life, and cycle time. Unlike milling, where the tool spins and the work is still, turning involves a constantly changing diameter as you reduce stock. That changing diameter means RPM and surface speed are in constant tension unless your machine has CSS mode.
This guide covers the practical side of lathe setup: how to pick SFM for different materials, how nose radius affects finish and forces, how to plan your depth-of-cut strategy, and how constant surface speed mode on CNC lathes solves the diameter problem.
SFM for Turning: Same Concept, Different Numbers
Surface feet per minute in turning uses the same formula as milling: RPM = (SFM × 3.82) / D, where D is the workpiece diameter. The difference is that D changes as you remove material. A 4-inch bar at 400 SFM runs at 382 RPM. After roughing to 3 inches, the same SFM requires 509 RPM. If you do not adjust RPM, the surface speed drops and the tool starts rubbing.
SFM recommendations for turning can be pushed slightly higher than milling because the tool is more rigidly supported. A CNMG carbide insert in mild steel can run 500 to 800 SFM. In 4140 pre-hard (HRC 28 to 32), 350 to 500 SFM. In 304 stainless, 400 to 600 SFM with coated carbide. Aluminum with a polished or PCD insert can run 1,000 to 3,000 SFM or higher.
On manual lathes, calculate RPM for the finishing diameter so the surface speed is correct when the tool makes the final pass that determines surface finish.
Tool material affects SFM dramatically. HSS tool bits in steel: 80 to 120 SFM. Brazed carbide: 250 to 500 SFM. Coated indexable carbide: 400 to 800 SFM. Ceramic inserts in hardened steel or cast iron: 1,000 to 2,500 SFM. Using the wrong SFM for your tool material is the fastest way to destroy an insert.
RPM = (SFM × 3.82) / D
D = workpiece diameter (inches)
Example: 500 SFM on a 3" bar
RPM = (500 × 3.82) / 3 = 637 RPM
Recalculate as diameter changes, or use CSS mode on CNC.
Lathe Turning Calculator
Calculate RPM, feed rate, cutting time, and surface finish for lathe turning operations. Supports OD turning, facing, boring, and parting with material-specific SFM data and horsepower estimation.
Nose Radius vs Surface Finish: The Tradeoff
The theoretical surface finish in turning is: Ra = f² / (32 × r), where f is feed per revolution (IPR) and r is the nose radius. For a 1/32" nose radius at 0.010 IPR: Ra = about 101 microinches. For a 1/16" nose radius at the same feed: Ra = about 50 microinches. Doubling the nose radius cuts roughness in half.
But a larger nose radius pushes harder against the workpiece. On slender shafts (length-to-diameter ratio greater than 4:1), a 1/16" radius can cause deflection and chatter. For slender work, use a 1/64" or 1/32" radius and compensate with a finer feed rate.
Wiper inserts have a modified geometry with a flat section that irons the surface smooth. A wiper insert can produce the same finish at double the feed rate, which is a straightforward way to cut cycle time on production work without sacrificing finish quality.
Ra = f² / (32 × r)
f = feed per revolution (inches)
r = nose radius (inches)
Larger nose radius = smoother finish but more radial cutting force.
Depth of Cut Strategy: Roughing vs Finishing
Roughing DOC should be as deep as the machine, tooling, and workholding can handle. A single 0.200" DOC pass removes the same material as four 0.050" passes but takes one quarter the non-cutting time. For roughing with CNMG inserts in steel, 0.080 to 0.200 inches is typical, with feed rates of 0.010 to 0.020 IPR.
If the insert chatters, check that the DOC is above the minimum for the insert's chipbreaker (usually 0.030 to 0.050 inches). Running too shallow defeats the chipbreaker and produces stringy, uncontrolled chips.
Finishing DOC is typically 0.010 to 0.030 inches, with feeds of 0.003 to 0.008 IPR. The finishing pass must be deep enough to ensure the insert is actually cutting, not rubbing. A minimum finishing DOC of half the nose radius is a good rule of thumb.
Leave consistent stock for finishing. If your roughing leaves uneven stock, the finish pass takes varying cuts, which produces inconsistent finish and dimensional variation.
Lathe Turning Calculator
Calculate RPM, feed rate, cutting time, and surface finish for lathe turning operations. Supports OD turning, facing, boring, and parting with material-specific SFM data and horsepower estimation.
Constant Surface Speed: Let the Machine Do the Math
G96 on CNC lathes automatically adjusts RPM as the tool moves along the X axis. As the tool moves toward center, RPM increases to maintain SFM. As the tool moves outward, RPM decreases. This keeps cutting conditions constant regardless of diameter.
The command is G96 S[value], where the value is SFM. The machine needs a G50 S[max RPM] limit to prevent over-speeding as the tool approaches center. Without this limit, a CSS program facing to center would attempt infinite RPM.
On manual lathes, you approximate CSS by changing speed as you work through diameter ranges. This is one of the biggest advantages of CNC turning: true CSS eliminates the compromise.
When not to use CSS: very small diameters near center where the RPM limit kicks in, and interrupted cuts where sudden diameter changes cause rapid spindle acceleration that can stress the drive.
G96 S500 = maintain 500 SFM
G50 S3000 = max RPM limit
Always set G50 before G96. Without a max RPM limit, the spindle will attempt to over-speed as the tool approaches center.