Designing for Turning

Principles

Turned parts are made by spinning the bar and moving a tool in two axes, so the design should suit that: round, concentric and cut from one side at a time. A turned shaft is held at one end (and sometimes supported at the other), so everything at the free end is cut by a tool that pushes on an unsupported cantilever. Good designs keep the part short and stiff, use features that a standard tool can reach, and put as many features as possible in one set-up.

• Design axisymmetric parts as turned parts, and add flats, cross holes and keyways only if they are needed (see second operations).
• One chucking. Features that must be concentric should be cut in a single set-up, without re-gripping. Turning the part around adds run-out of 0.02–0.05 mm.
• Fewer diameters and tool changes. Each different groove width or thread needs another tool.
• Use standard bar sizes. The more material you must remove, the more it costs.

Length, diameter and support

The length-to-diameter ratio L ÷ D decides how the part can be held. A bar held only by the chuck acts as a cantilever, deflecting by F × L³ ÷ (3 E I) under the cutting force, so deflection grows with the cube of the length. Supported between centers, the same bar deflects 16 times less.

L ÷ D	How to hold it	Comment
Up to 3	Chuck or collet only	Stiff enough for normal cuts
3 to 8	Chuck and tailstock center (or a live center)	Needs a center hole in the end; light finishing cuts at the tailstock end
8 to 15	Steady rest or follow rest as well	Slow, shallow cuts; a smooth finish needs a follow rest
Over 15	Special set-up: Swiss-type lathe or grinding	Long, slender shafts bend and whip; avoid or split the part

• Keep L ÷ D under about 3 for parts you want to make in a collet or chuck alone. If the part must be longer, make the free end a larger diameter, or add a center hole and support it.
• Hold at least 1 × D of the bar in the chuck.
• Thin-walled tubes distort in a chuck; design a thicker wall, or a mandrel-supported or soft-jaw set-up.

Shoulders, steps and radii

• Put a radius in every inside corner at a shoulder. The tool has a nose radius (0.4 or 0.8 mm), so a radius at least that large is natural. A sharp inside corner needs a special tool and concentrates stress: a radius at the root of a shaft step greatly raises its fatigue life.
• Specify the radius, and use the same one throughout: R0.4, R0.8 or R1.
• Step height. A step of 1–3 mm per side is cut in one or two passes. Large steps (a big flange on a small shaft) waste time and material; start from a stock closer to the biggest diameter or use a different blank.
• Taper and angle. A tool’s relief angle limits how steeply it can cut a shoulder: a 90° shoulder is fine; a steep back-taper may need a smaller insert.
• Outside corners can be sharp, chamfered or rounded; chamfers are simplest.

Grooves, undercuts and thread relief

• Standard grooves. Use groove widths that match a standard grooving insert (1.5, 2, 3, 4 mm). O-ring grooves, circlip (retaining ring) grooves and relief grooves have tabulated widths and depths; use them.
• Depth against width. A groove up to about 3 × its width deep is routine; deeper grooves need a special blade, slow feeds and clear chip flow.
• Groove corners have a small radius from the insert; specify R0.1–0.2, not sharp.
• Thread relief (undercut). A groove at the end of a thread lets the tool run out. A common width is about 3 × the pitch (for M10 × 1.5, 4.5 mm), as deep as the thread’s root plus a little. Without it, the thread must end with a run-out that cannot be fully formed.
• Undercuts inside a bore (an internal groove) need a boring bar with a groove insert; make them standard and shallow.
• Parting groove. Leave the length of the finished part plus the width of the cut-off tool (2–3 mm), plus a facing allowance for the second side.

Threads

• Use standard threads (ISO metric coarse, UNC, UNF) so the shop has the inserts, gauges and taps.
• Coarse is easier than fine; fine threads are weaker to damage and slower to cut.
• Length of thread: as short as the function needs; more than 1.5 × the diameter of engagement adds nothing.
• Thread start and end. Chamfer the start; end the thread against a relief groove or a shoulder with a run-out.
• Tolerance class. 6g (external) and 6H (internal) are standard; tighter classes need special gauging. See Fits in Practice.
• Left-hand and multi-start threads are possible but need a note on the drawing.

Chamfers, center holes and ends

• Chamfer both ends and every edge (0.5–1 × 45° is typical). A chamfer removes burrs, guides assembly and protects the thread start.
• Center holes (60° center drilled) at one or both ends let the tailstock support long parts and allow later grinding. Specify them on the drawing if they are to remain.
• Parted ends show a small nub or a slight cone where the part is cut off. If the end matters, specify “face after parting” or allow a second operation.
• Flat ends are easier than domed or pointed ends; a spherical end needs a radius tool or a form tool.

Bores and holes

• Drill, then bore. A drilled hole is accurate to about ±0.1 mm in size and wanders slightly; a bore with a boring bar gives ±0.01–0.02 mm and a good finish.
• Bore depth. A bar reaches about 4 × its diameter in steel; a deeper bore of small diameter needs a carbide or damped bar and a light cut. Keep deep, small bores to 4–6 × D.
• Flat-bottomed blind holes are harder than conical bottoms; a drilled hole has a cone.
• Through holes are easier than blind holes: chips clear and there is no bottom to finish.
• Standard sizes (drill, reamer) keep the cost down; fit holes (H7) are reamed or bored.
• Concentric bore and outside diameter are best cut in the same chucking.

Features that need a second operation

Feature	Why	How it is made
Flats, hex or square ends	Not round	Milling in a second set-up, or live tooling on a mill-turn machine; or buy hex bar
Cross holes, slots, keyways	The tool is not on the axis	Mill with a rotary fixture or live tools
Knurling	Pressed, not cut	A knurling tool in the turret, in the same set-up
Hardened parts, tight finishes	Too hard or too fine to turn	Cylindrical grinding
Deburring and polishing	Edges after cutting	Manual or tumbling
Turning the second end	The part is held by the first end	Re-chuck in soft jaws or a collet; allow for run-out
Heat treatment, plating, anodizing	Change the size and shape	Machine to the pre-treatment size and finish after

Bar stock and allowances

• Choose a bar close to the largest diameter, with 1–2 mm of allowance on the diameter for turning, more for hot-rolled bar with a scaly skin, and extra if the bar is bent.
• Standard round bar sizes (mm): 6, 8, 10, 12, 16, 20, 25, 32, 40, 50, 63, 80, 100. Inch: ¼ to 4 in. Aluminum and brass also come in hex and square.
• Bar feeder and collet limits. A bar must pass through the spindle bore; many small lathes take only 20–25 mm.
• Allow for the cut-off, the facing and any left in the chuck jaws.
• Cold-drawn bar is accurate and straight but may move when cut (residual stress); ground bar is the most accurate.

Tolerances, concentricity and finish

• Turning holds tight diameters: ±0.02 mm is routine, ±0.01 mm achievable on a good lathe with a finishing pass; ±0.005 mm or finer usually needs grinding.
• Length tolerances between faces cut in the same set-up are good (±0.02–0.05 mm); across a re-chucked part they are looser.
• Concentricity and run-out are controlled by cutting both diameters without re-chucking. A 0.02 mm run-out between two ends cut in two set-ups is normal. For a tighter requirement, say so, and design for one set-up or a mandrel.
• Surface finish. A normal turned surface is Ra 1.6–3.2 µm; Ra 0.8 µm needs a light finishing pass with a good nose radius; below 0.4 µm requires grinding or polishing. See the finish chart in Turning: Lathes and Operations.
• Fits. A shaft that must fit a bore needs an h or g tolerance on the diameter; see How Fits Work.
• Specify geometric tolerances (runout, cylindricity) only where needed; see Profile and Runout.

Cost drivers

Driver	Effect	How to reduce it
Set-ups and re-chucking	Time, run-out	One chucking for concentric features; design the second end to be simple
Special tools	Custom form tools, special groove widths	Standard grooves, threads and radii
Length-to-diameter	Slow cuts, support, scrap	Short, stout parts; support with a center
Tight tolerances and finish	Extra passes, gauging, grinding	Tighten only where the function needs it
Material	Cost and cutting speed	Free-machining grades where acceptable (12L14, 303, 360 brass)
Secondary operations	Milling, grinding, heat treatment	Choose stock that needs fewer: hex bar, ground bar
Quantity	Bar feeding and automation	Larger batches; family tooling

Design review checklist

Question	Fix if the answer is no
Is L ÷ D under 3, or is there a center hole and support for longer parts?	Shorten, thicken, or add the center hole
Do all inside corners have a standard radius?	Add R0.4–R1 at shoulders
Are groove widths and depths standard?	Use the tabulated sizes
Is there a relief groove or run-out for every thread?	Add it, about 3 × the pitch wide
Are both ends chamfered?	Add 0.5 × 45° chamfers
Can concentric features be cut in one chucking?	Reorder the features, or add a mandrel step
Do you need flats, cross holes or keyways, and are they planned as a second operation?	Mark them and consider a mill-turn machine
Is the bar size standard and the allowance enough?	Adjust the dimensions to stock
Are tolerances and finishes only as tight as the function needs?	Loosen the rest

Related

• CNC Machining: the overview of this guide.
• Turning: Lathes and Operations: lathe operations, inserts and finish.
• Designing for CNC Milling: the same ideas for milled parts.
• Fits & Tolerances: tolerances on shafts and bores.
• Material Properties.

FAQ

How long can a turned part be?

Up to about 3 times its diameter with only a chuck, up to 8 with a tailstock center, and more with a steady rest. Longer, slender parts bend and whip under the cut, so the shop will take light passes or use a special machine.

Why must a shoulder have a radius?

The insert’s nose is round, so it cannot cut a sharp inside corner. A radius also spreads stress and greatly increases the fatigue life of a stepped shaft.

What is a thread relief groove?

A groove at the end of a thread that lets the cutting tool run out. Without it, the thread must end with a run-out that cannot be fully formed, or the tool crashes into the shoulder.

Can a lathe cut a hex or a flat?

A plain lathe cannot. A mill-turn machine with live tools can, or the part can be moved to a mill for the flat. Hex bar stock avoids the problem for hexagon heads.

Why does my turned part have a taper?

The work deflects away from the tool, most at the unsupported end, so the diameter is larger there. Reduce it with the tailstock, a lighter cut and a finishing pass, and make the part shorter where possible.

References

• Oberg, E. et al., Machinery’s Handbook, 31st ed., Industrial Press: turning, threads, tolerances, bar stock.
• ISO 2768-1 (general tolerances); ISO 4753 and DIN 76-1 (thread run-outs and undercuts); DIN 509 (relief grooves).
• Design-for-manufacturing guides from CNC service providers for turned parts (length-to-diameter limits, grooves, threads).
• Bralla, J., Design for Manufacturability Handbook, McGraw-Hill.

Last reviewed: October 2026. Cutting data are starting points: machines, tools and materials differ, so test on scrap and follow the tool maker’s data.