The complete guide · CNC machining
How to specify tolerances for machining — and the rest of the CNC spec
Tolerances are where machining specs go wrong in both directions — too loose to function or so tight the quote triples. Here is the discipline a machinist expects, plus the other six lines a complete CNC spec needs.
The short version
- One general class covers the part — ISO 2768-m in the title block; stop tolerancing every dimension.
- Tight callouts are exceptions with datums — every critical dimension names its datum — a number without a reference is a wish.
- Each decimal place multiplies cost — ±0.1 mm routine · ±0.025 careful setup · ±0.01 grinding territory.
- Material + temper by standard — 6061-T6, not “aluminum” — temper changes machinability and strength.
- Respect tool geometry — pockets ≤3–4× tool depth, inside corners get radii, thin walls ≥0.8 mm.
- Finish and coating by number — Ra values per face; anodize by MIL-A-8625 type and class.
01Set one general tolerance class in the title block
Most dimensions on most parts just need to be “about right.” A general class says so once, in a standard the shop already works to, and frees the drawing from a forest of needless callouts.
“General tolerances per ISO 2768-m” (medium) is the workhorse: roughly ±0.1 mm up to 6 mm, ±0.2 mm to 30 mm, ±0.3 mm to 120 mm. Fine (-f) where the whole part is precision; coarse (-c) for brackets and covers.
02Reserve tight tolerances for function — and give each a datum
A tolerance only means something measured FROM somewhere. Critical dimensions are the ones that mate, locate, or seal — and each needs a named datum surface so your intent and the shop's inspection agree.
Pattern: “bore ⌀ 8.000 ±0.015, position ⌀ 0.05 to datums A|B”. If you cannot say why a dimension is critical (what it mates with), it belongs to the general class.
03Know what each decimal place costs
Tolerance is exponential, not linear. Every tightening step changes the process: new fixturing, slower feeds, temperature control, different machines, 100% inspection.
Rules of thumb: ±0.1 mm is routine milling · ±0.025 mm needs careful setup and inspection · ±0.010 mm is grinding/boring territory · below that you are buying toolroom time by the hour. Price follows the tightest tolerance on the drawing.
04Name the material and its temper by standard
“Aluminum” spans gummy 1100 to aerospace 7075; the temper suffix changes strength by 2× and machinability with it. Steel, brass, and plastics all have the same trap.
“6061-T6” · “7075-T651” · “303 stainless” · “Delrin 150 (POM-H)”. If substitutes are acceptable, say which (“6082-T6 acceptable”) — that one line saves a stalled quote when stock is short.
05Respect what a rotating tool can reach
End mills are cylinders on sticks: deep narrow pockets chatter, sharp inside corners are impossible, thin walls ring and deflect. Geometry that fights the tool costs money every single part.
Keep pocket depth ≤ 3–4× tool diameter (a 20 mm-deep slot needs ~6 mm of tool: fine; 60 mm deep: a problem). Give inside corners radii ≥ ⅓ of pocket depth where you can. Metal walls ≥ 0.8 mm, plastic ≥ 1.5 mm.
06Call out threads, holes, and finishes completely
Half-specified features are quote-stalling questions: a “M4 hole” without depth, class, or blind/through; a “smooth finish” without a number.
Threads: “M4×0.7-6H, ↧ 8 min, blind”. Surface finish by Ra per face: 3.2 µm default machined, 1.6 µm sealing faces, 0.8 µm sliding fits. Coatings by standard: “anodize per MIL-A-8625, Type II, Class 2 black” — and note tolerance-critical faces to mask (anodize adds thickness).
07State quantity, batch, and what is deferred
Ten parts and ten thousand get different processes (3-axis vs. fixture plates vs. “should this be cast?”). And the shop owns its craft: workholding, toolpaths, roughing strategy.
Give quantity now + expected repeat batches. Defer by name: “fixturing, tool selection, and process at machinist's discretion; witness marks acceptable on non-cosmetic faces.” The litmus test stands: a shop that has never met you can quote it without a phone call.
Worked example: a sensor mounting block
The whole chain, numbers shown — the same derivations the SpecBuildr interview performs and prints in your spec's math appendix.
Material6061-T6 (6082-T6 acceptable)
General toleranceISO 2768-m, stated once in the title block
Critical dimssensor bore ⌀ 12.000 ±0.015 to datum A; 2× dowel ⌀ 3 H7
Geometry checkmain pocket 18 mm deep / 8 mm min tool — 2.25×, fine
Threads4× M3×0.5-6H ↧ 6, blind; 1× M12×1 gland, through
FinishRa 3.2 general; Ra 1.6 on datum A (gasket face)
CoatingAnodize MIL-A-8625 Type II Class 2 black; mask bore + dowels
Quantity25 now; ~100/yr repeat expected
The mistakes that make quotes expensive
✗Tolerancing every dimension tightly
The quote prices the tightest number on the page. One general class + a short critical list is the whole discipline.
✗A tight tolerance with no datum
±0.01 measured from where? Without a datum the shop guesses, and inspection arguments follow.
✗“Aluminum” without temper
6061-O machines and performs nothing like -T6. The suffix is not decoration.
✗Pockets deeper than the tool
Past 4× diameter the tool chatters and walks. Split the feature, widen it, or expect EDM pricing.
✗Sharp inside corners
A rotating cylinder cannot cut a zero-radius inside corner. Draw the radius or pay for a broach/EDM.
Frequently asked questions
What tolerances should I put on a machined part?
A general class (ISO 2768-m for most parts) stated once, plus tight callouts only on dimensions that mate, locate, or seal — each with a datum reference. ±0.1 mm is routine; ±0.025 mm needs careful setup; ±0.01 mm is grinding territory.
What is ISO 2768 and why do shops ask for it?
A general-tolerance standard that assigns default tolerances by dimension size (class f/m/c). Stating “ISO 2768-m” once covers every uncalled dimension, so the drawing only carries the exceptions.
Why do machining quotes vary so much for the same part?
Usually the tolerances: shops price the tightest callout and the inspection it implies. Second causes: unnamed temper (material uncertainty) and geometry that fights the tool (deep pockets, sharp corners, thin walls).
What does a machine shop need to quote a CNC part?
A model + drawing with one general tolerance class, datumed critical dimensions, material with temper, complete thread/hole callouts, Ra per face and coating by standard, and quantity with expected repeats. That quotes cleanly without a clarifying call.
Can I write a machining spec without being a machinist?
Yes — the SpecBuildr interview asks for function (what mates where) in plain language and generates the tolerance discipline, geometry checks (pocket ratios, corner radii), and callouts for you, flagging what would make the quote expensive.
Skip the blank page
The interview asks you these exact questions in plain language, runs the physics checks, and prints a complete, quotable spec — free.
Start the cnc interview →