Design for turned parts means shaping a part around one axis of rotation, so that a stationary tool can reach each feature while the lathe holds the workpiece stiffly and in as few clampings as possible. The rules below cover slenderness, bore depth, wall thickness, relief grooves, threads, tolerances and complete machining on one machine, each with its reason and its effect on cost.
What does design for turned parts mean?
A lathe spins the workpiece and feeds a tool along or across it. Three facts follow, and every rule in this article comes from one of them. The workpiece is clamped at one end and bends away from the tool, so long and thin parts force light cuts. Internal features are cut by a bar that enters the bore, so bore depth is limited by bar stiffness. Anything that is not rotationally symmetric, such as flats, cross holes and keyways, needs live tooling or a second machine.
Cost follows the same facts: slower cuts, more clampings, special tooling and more inspection. Their size depends on part, material and shop, so this article describes them in words.
The numbers below are guideline values from tool maker Sandvik Coromant and the manufacturing platforms Hubs and Protolabs, plus dimensions and designations from standards. They are not limits of any particular shop. Our audited network in Bursa covers CNC turning. For prismatic parts, see DFM for CNC milling.
How long can a turned part be for its diameter?
Sandvik Coromant states that a length-to-diameter ratio of up to 2:1 is normally acceptable for a workpiece supported at one end only, and that tailstock support extends it. Hubs gives a looser guideline: keep parts under 10:1 where possible, since longer parts usually need tailstock support. For long parts with internal machining, Sandvik adds that a tailstock and steady rest are required.
The reason is deflection. For a cantilever with a load at the free end, tip deflection is δ = F·L³ / (3·E·I), and for a round bar I = π·d⁴ / 64. At a fixed diameter the deflection therefore grows with the cube of the length-to-diameter ratio.
Table 1. Relative tip deflection of a bar clamped at one end, equal cutting force and diameter
| Length ÷ diameter | Relative deflection |
|---|---|
| 2 | 1 |
| 4 | 8 |
| 6 | 27 |
| 10 | 125 |
Source: Ertaş Engineering calculation from δ = FL³/(3EI), δ ∝ (L/d)³ at constant d (Wikipedia). Solid round bar, workpiece clamped rigidly, tailstock ignored.
To counter deflection, the shop reduces depth of cut and feed, adds a tailstock or steady rest, or turns in more passes, and all of them cost machine time. A tailstock presses a centre against the end face, so the supported end carries a centre mark unless a later operation removes it. If that end is a sealing or locating face, say so on the drawing. The cheaper fix sits in the design: a thicker section, a shorter length, or two shorter parts joined after turning.
How deep can a bore be and how thin can a wall be?
An internal feature is cut by a boring bar that must fit inside the bore. Sandvik Coromant lists the maximum overhang of a bar as a multiple of its diameter. The bar is always thinner than the bore, so the usable depth is always less than the multiple times the bore diameter.
Table 2. Maximum boring bar overhang, as a multiple of bar diameter
| Bar type | Turning | Grooving and threading |
|---|---|---|
| Steel | 4 × | 3 × |
| Carbide | 6 × | 5 × |
| Steel, dampened | 10 × | 5 × |
| Carbide reinforced, dampened | 14 × | 7 × |
Source: Sandvik Coromant, Turning application guide, maximum overhang for boring bars.
Sandvik advises using the largest bar that fits and keeping the overhang short. A deep, narrow bore therefore pushes the shop toward dampened bars or lower cutting data. Make it only as deep as function needs, and as wide as the part allows.
Thin walls bend away from the tool in the same way. Hubs advises at least 0.8 mm in metals, noting that thicker walls hold their shape better and reduce vibration. Protolabs states that walls thinner than 0.5 mm typically do not survive machining on its lathes.
What do shoulders, grooves and threads need?
Inside corners are round, because the insert has a nose radius. Hubs expects a radius matching the tool nose, typically 0.4 to 1.6 mm, and notes that a sharp internal corner needs special tooling or a secondary operation. Draw an inside radius, not a sharp corner. Where a mating part must seat square against a shoulder, relieve the mating edge with a chamfer, or add a relief groove.
Relief grooves are standardised. DIN 509:2022-12, current, replaces the 2006-12 edition, and ISO 18388:2016 covers the same ground with four forms, E, F, G and H. ISO 18388 states that its aim is to limit the number of tools needed through a restricted set of groove types and sizes. Call out the form by its designation instead of drawing a custom profile. A revision of ISO 18388 is in development (stage 30.99, 2026-10-09). Status as of 2026-10-30.
Grooves are cut with plunging inserts. Sandvik's rule of thumb is that a groove narrower than it is deep is cut by multiple plunges, and a groove wider than it is deep by plunge turning. Deep grooves need long overhangs, and chip evacuation and coolant access suffer, so keep them shallow where function allows.
Threads follow the same logic. Hubs calls M6 or larger the sweet spot, and says smaller threads such as M2 need specialised tools, which adds machining time and cost. A thread that ends at a shoulder needs a run-out or an undercut, and DIN 76-1:2025-10 gives their dimensions for ISO metric threads (the 2016-08 edition is withdrawn).
Edges need a decision too. A drawing with no edge note leaves burr and break to the shop. ISO 13715:2017, current, gives the symbols for edges of undefined shape. Where the edge matters, dimension a chamfer, for example 1 × 45°, so the requirement is a number.
How should you dimension and tolerance a turned part?
Dimension diameters from the axis and lengths from one datum face. Geometric requirements that matter on a turned part, such as run-out and coaxiality, are defined in ISO 1101:2017, which ISO confirmed in 2022. State them against a datum axis, with a note on which diameters form that datum.
For everything else, rely on a general tolerance. ISO 2768-1:1989 is still published, and a revision project is listed. Class m allows ±0.2 mm on a diameter in the range over 6 to 30 mm, ±0.3 mm over 30 to 120 mm and ±0.5 mm over 120 to 400 mm. ISO 2768-2 was withdrawn in 2021, so give run-out and similar requirements individually (see the ISO 2768 article). Our network works to ISO 2768-m as standard, tighter where the drawing specifies it.
A fit needs its own tolerance. For a 25 mm diameter, IT7 under ISO 286-1 is 21 µm, so an H7 bore spans 0 to +0.021 mm, far tighter than ±0.2 mm. Tight tolerances cost finishing passes and measurement, so keep them to bearing seats, seals and locating diameters. The CNC machining tolerances handbook shows how general tolerances, fits and GD&T combine on one part.
When does machining on one machine pay off?
Sandvik Coromant calls combining all operations on one machine the primary benefit of multi-task machines, because it reduces component setups. Many parts also need machining from both ends, which Sandvik says is often done with a sub-spindle. Protolabs describes live-tool lathes that mill shapes and drill off-axis and radial holes, and gives turning a bolt and milling its wrench flats as the example. Hubs states that features machined in a single setup keep their concentricity.
The reasoning is datum transfer. Each re-clamp is a new reference, so a tolerance between two diameters cut in different clampings includes the error of the re-clamp, while features cut in one clamping share one axis.
Design for this machine class:
- Put flats, slots and cross holes parallel or perpendicular to the axis. Protolabs supports axial and radial holes only in those orientations on its lathes, and off-axis milled holes only in aluminium or brass.
- Do not combine extreme slenderness with sub-spindle transfer. Sandvik notes that long, slender components with internal machining need a tailstock and steady rest instead.
- Do not assume any machine has live tooling or a sub-spindle. Ask which machine the quote is based on.
Which turning rules should you check before the drawing goes out?
Table 3. Guideline values for CNC turned metal parts and the cost effect of ignoring them
| Feature | Guideline value | Why | Effect on cost if ignored |
|---|---|---|---|
| Length ÷ diameter | ≤ 2 held at one end; Hubs: < 10 | Deflection grows with the cube | Tailstock or steady rest, light cuts |
| Bore depth | Steel bar ≤ 4 × bar diameter | Bar overhang | Dampened bars, slower cutting |
| Wall thickness, metal | ≥ 0.8 mm (Hubs); 0.5 mm limit (Protolabs) | Stiffness | Slow finishing, scrap risk |
| Inside corner | Radius ≥ tool nose, 0.4–1.6 mm | Insert has a nose radius | Special tool or extra operation |
| Shoulder | Relief groove to DIN 509 or ISO 18388 | Tool run-out, square seating | Custom tool, drawing queries |
| Thread | M6 or larger; run-out to DIN 76-1 | Standard thread tools | Specialised tools, longer cycle |
| Groove | Wider than deep where possible | Overhang, chip evacuation | Multiple plunges, process risk |
| Edges | Chamfer dimensioned or ISO 13715 | Burr and break otherwise open | Rework, disputes at inspection |
| Clampings | Turned features in one clamping | Datum transfer | Re-clamp error, handling time |
| General tolerance | ISO 2768-m | Default finishing | Extra passes and inspection |
Source: Sandvik Coromant (length-to-diameter, boring bars, grooves); Hubs and Protolabs turning guides (walls, corners, threads); DIN 509:2022-12; ISO 18388:2016; DIN 76-1:2025-10; ISO 13715:2017; ISO 2768-1:1989. Cost column: Ertaş Engineering assessment.
Before you release a turned drawing, check three things. Does the drawing say what the tailstock end may carry? Does every shoulder and thread end have a relief and an inside radius? Does every tight tolerance sit on a feature that needs it? The technical drawing checklist covers the title block and the format. DFM support is part of our design engineering service.
Frequently asked questions
- What is the maximum length-to-diameter ratio for a turned part?
- Sandvik Coromant calls a ratio of up to 2:1 normally acceptable for a workpiece held at one end only, and says tailstock support extends it. Hubs advises keeping parts under 10:1 where possible, because longer parts usually need tailstock support.
- Why do turned shoulders need relief grooves?
- A relief groove lets the tool or grinding wheel run out at the shoulder and lets a mating part sit square against it. DIN 509:2022-12 and ISO 18388:2016 standardise the groove forms, so the shop can use stock tooling.
- What is the minimum wall thickness for a turned metal part?
- Hubs recommends at least 0.8 mm for metals. Protolabs states that walls thinner than 0.5 mm typically do not survive machining on its lathes.
- What is the smallest thread for a turned part?
- Hubs calls M6 or larger the sweet spot. Smaller threads such as M2 are possible but need specialised tools, which adds machining time and cost.
- What does a live-tool lathe add to a turned part?
- It can mill flats and slots and drill radial and off-axis holes in the same clamping. Protolabs gives turning a bolt and milling the wrench flats as an example. Not every lathe has live tooling, so confirm it with the shop.
Sources
- Sandvik Coromant, How to achieve good component quality in turning (length-to-diameter 2:1, slender and thin-wall components)
- Sandvik Coromant, Turning application guide (maximum boring bar overhang, internal machining)
- Sandvik Coromant, External grooving (width versus depth, deep grooves)
- Sandvik Coromant, Multi-task machines, horizontal (one setup, sub-spindle, tailstock and steady rest)
- Hubs, CNC turning machines: how they work and when to use them (length-to-diameter, walls, internal corners, threads, single setup)
- Protolabs, Design guidelines for CNC turning (walls, live tooling, holes)
- Protolabs, CNC machining tips for complex parts (live-tool lathes)
- Deflection (engineering), cantilever with end load: δ = FL³/(3EI) (Wikipedia)
- DIN 509:2022-12, Relief grooves, types, dimensions and tolerances, current, replaces DIN 509:2006-12 (DIN Media)
- ISO 18388:2016, Relief grooves, types and dimensioning, current (AFNOR)
- prEN ISO 18388 rev, revision in development, stage 30.99 dated 2026-10-09 (Genorma)
- DIN 76-1:2025-10, Thread run-outs and thread undercuts for ISO metric threads, current (DIN Media)
- DIN 76-1:2016-08, withdrawn (DIN Media)
- ISO 13715:2017, Edges of undefined shape, indication and dimensioning, current, replaces ISO 13715:2000 (AFNOR)
- ISO 1101:2017, life cycle: confirmed 2022-10-03 (ISS, national ISO member)
- ISO 2768-1:1989, life cycle: stage 90.92, revision project listed (ISS, national ISO member)
- ISO 2768-1 linear tolerances, classes f, m, c (AmesWeb table)
- ISO 286-1:2010 standard tolerance grades, IT7 for 18–30 mm (table reproduced on Wikipedia)
Questions on a drawing? sales@ertas.engineering