Precision Turning Tolerance Guide
What a competent shop holds in production on a well-maintained CNC lathe. Not brochure specs — real numbers from real parts.
Diameter Tolerances
Diameter is the dimension that defines precision turning. It's the tolerance most buyers care about and the one that separates precision shops from general-purpose shops.
| Class | OD Tolerance | ID Tolerance | Machine Tier | Typical Work |
|---|---|---|---|---|
| General | ±0.001" | ±0.001" | Any CNC lathe | Shafts, spacers, general components |
| Precision | ±0.0005" | ±0.0005" | Quality CNC lathe, skilled operator | Tooling components, inserts, bushings |
| High Precision | ±0.0002" | ±0.0003" | Okuma/Mori class, glass scales | Die casings, punch bodies, gage work |
| Ultra Precision | ±0.0001" | ±0.0002" | Swiss or dedicated precision lathe | Medical, optical, semiconductor |
ID tolerances are typically one class looser than OD tolerances on the same machine because boring bars deflect more than external tools at equivalent overhang. Deep bores (L/D > 4:1) may require additional tolerance relaxation or specialized boring bars.
Length Tolerances
Length control on a CNC lathe is inherently less precise than diameter control. The Z-axis (length) depends on tool touch-off accuracy, thermal growth of the spindle and bed, and the consistency of the part stop or collet face. ±0.0005" on length is a realistic production tolerance. ±0.0002" on length requires careful process control and is not achievable on every setup.
Concentricity and Runout
Features turned in a single chucking are concentric to the spindle axis within the machine's spindle runout — typically 0.0001"–0.0003" TIR on quality machines. If the part is rechucked (flipped for second-side work), concentricity between first-side and second-side features depends on the chuck accuracy and part seating. Expect 0.001"–0.003" TIR on rechucked features unless the shop uses a collet or precision bore to locate the second side.
Surface Finish
| Operation | Typical Finish | Best Achievable | Notes |
|---|---|---|---|
| Rough turning | Ra 63–125 μin | Ra 63 μin | Heavy stock removal, chip load priority |
| Finish turning | Ra 32–63 μin | Ra 16 μin | Standard production finish |
| Fine finishing | Ra 16–32 μin | Ra 8 μin | Light DOC, wiper insert, controlled feed |
| Burnishing/polishing | Ra 4–8 μin | Ra 2 μin | Post-machining operation, adds cost |
Material Effects on Tolerance
Tool steels (D2, A2, S7, M2) turn predictably in both annealed and hardened states. Hardened tool steels (58+ HRC) require CBN or ceramic inserts and hold excellent tolerance because the material is rigid and deflects minimally.
Carbide turns cleanly with PCD or CBN tooling but is slow. Tolerances are excellent because carbide doesn't deflect.
Aluminum turns fast with excellent finish but built-up edge at the wrong speed can affect tolerance. Keep surface speed above 500 SFM for consistent results.
Stainless steel work hardens and tends to push away from the tool. Expect looser tolerances than tool steel unless the operator adjusts for deflection.
The tolerance on your drawing is the tolerance you pay for. If you need ±0.0002" on one diameter and ±0.001" on the rest, call out the critical dimension explicitly. Don't default your CAD tolerance block to ±0.0005" on everything — the shop will price every dimension to that tolerance, and your quote will be higher than necessary.
Need tight-tolerance turning?
Tell us your requirements and we'll match you with shops that hold these tolerances in production.