CNC machining tolerances and surface finish: the reference tables
The numbers that decide a machined part: standard vs achievable tolerances by process, the surface-finish (Ra) ladder, DFM limits and a metric tap-drill chart. Bookmark it.
Quick answer: A standard CNC part holds about plus/minus 0.005 in (0.13 mm) on general dimensions for metal and plus/minus 0.010 in (0.25 mm) for plastic, with an as-machined surface finish around 125 microinch (3.2 micrometre) Ra. Tighter is achievable, down to a few tenths of a thou by grinding or wire EDM, but every tighter callout adds cost, so specify tolerance and finish only where the part needs them. The tables below are the reference numbers.
Last reviewed: September 2026. These are typical shop standards for reference; your shop's quote governs. Spec the numbers on the drawing.
Standard (general) tolerances
Unless a drawing calls out tighter, most shops work to a general tolerance like this. The metric equivalent is ISO 2768-1 class m (medium); tighter is class f (fine), looser is class c (coarse).
| Feature | Metal | Plastic |
|---|---|---|
| Linear, general | plus/minus 0.005 in (0.13 mm) | plus/minus 0.010 in (0.25 mm) |
| Angles | plus/minus 0.5 degrees | plus/minus 1 degree |
| Drilled hole | +0.005 / -0.001 in | wider, material-dependent |
| Reamed hole | plus/minus 0.0005 in | not typical |
| Edges | broken and deburred | broken and deburred |
Achievable tolerance by process
What each process can hold at its standard rate, and what it can reach at a premium. Ask for the tight number only on the features that mate or seal.
| Process | Standard | Achievable (at cost) |
|---|---|---|
| 3-axis milling | plus/minus 0.005 in | plus/minus 0.001 in |
| CNC turning (diameter) | plus/minus 0.002 in | plus/minus 0.0005 in |
| Reaming | plus/minus 0.001 in | plus/minus 0.0002 in |
| Surface / cylindrical grinding | plus/minus 0.0005 in | plus/minus 0.0001 in |
| Wire EDM | plus/minus 0.0002 in | plus/minus 0.0001 in |
| Jig grinding | plus/minus 0.0002 in | plus/minus 0.00005 in |
Surface finish (Ra) ladder
Surface finish is specified as Ra, in microinch or micrometre. The lower the number, the smoother and the more it costs. As-machined CNC is about 125 microinch; below 32 usually means a secondary grinding, polishing or lapping step.
| Ra (microinch) | Ra (micrometre) | Typical way to get it |
|---|---|---|
| 250 | 6.3 | Rough machined |
| 125 | 3.2 | Standard as-milled / as-turned |
| 63 | 1.6 | Fine machined |
| 32 | 0.8 | Very fine machined or fine ground |
| 16 | 0.4 | Ground |
| 8 | 0.2 | Polished / lapped |
Bead blasting gives a uniform matte look but does not by itself hit a fine Ra; anodize and plating add a thin layer over whatever finish is underneath, so specify the machined finish AND the coating.
Design-for-manufacturing limits
The geometry limits that decide whether a feature is easy, expensive or impossible. Staying inside them keeps the quote down. The reasoning is in design for manufacturing.
| Feature | Typical limit |
|---|---|
| Minimum wall, metal | 0.030 in (0.8 mm) |
| Minimum wall, plastic | 0.060 in (1.5 mm) |
| Maximum pocket / hole depth | about 4x tool diameter standard, to ~10x with special tooling |
| Minimum internal corner radius | the tool radius (a sharp internal corner is impossible for a round tool) |
| Smallest practical hole | about 0.040 in standard; smaller by micro-drill or EDM |
| Tapped-hole thread depth | 1.5 to 2x the thread diameter |
Metric tapped holes (coarse, 75 percent thread)
Call out threads and tapped holes explicitly, because they are a common source of quote clarification. Tap-drill sizes for standard metric coarse threads:
| Thread | Pitch (mm) | Tap drill |
|---|---|---|
| M3 | 0.5 | 2.5 mm |
| M4 | 0.7 | 3.3 mm |
| M5 | 0.8 | 4.2 mm |
| M6 | 1.0 | 5.0 mm |
| M8 | 1.25 | 6.8 mm |
| M10 | 1.5 | 8.5 mm |
| M12 | 1.75 | 10.2 mm |
For imperial work, common machine-screw threads are #4-40, #6-32, #8-32, #10-24, #10-32, 1/4-20 and 5/16-18; use a standard tap-drill chart and call out the class of fit (2B is the usual default).
How to call it out so a shop quotes without a follow-up email
- Put a general tolerance in the title block, then tight callouts only on the two or three features that mate or seal. See what CNC machining costs for why blanket tight tolerances triple the price.
- Specify surface finish as an Ra value where it matters, and say if a cosmetic face must be free of tool marks.
- Name the material and grade: aluminum 6061 vs 7075, stainless 304 vs 316.
- Call out every thread, its size and class of fit, and any inserts.
- Send a STEP model plus a dimensioned 2D drawing. That combination is what lets a shop quote from the geometry you actually designed.
When your drawing carries these, send one RFQ and we route it to Canadian CNC machining shops that can hold your numbers.
FAQ
What is a standard CNC machining tolerance?
About plus/minus 0.005 in (0.13 mm) on general dimensions for metal, or ISO 2768 class m. Plastics are looser at about plus/minus 0.010 in. Anything tighter should be called out only where the part needs it.
What surface finish does CNC machining produce?
As-machined is about 125 microinch (3.2 micrometre) Ra. Finer finishes (63, 32 microinch and below) come from fine machining, grinding, polishing or lapping, each an added step and cost.
What is the tightest tolerance CNC machining can hold?
Milling and turning reach about plus/minus 0.001 in with care; grinding and wire EDM reach a couple of tenths of a thou (0.0001 to 0.0002 in). Jig grinding goes tighter still. These are premium operations, not defaults.
What is Ra?
The arithmetic average roughness of a surface, the standard way to specify surface finish. Lower Ra is smoother. It is quoted in microinch (imperial) or micrometre (metric); 125 microinch equals 3.2 micrometre.
How deep can a hole or pocket be?
As a rule of thumb, about four times the tool diameter at standard rates, up to roughly ten times with special long tooling (which costs more and holds looser tolerance at depth). Deep, narrow features are a common cost driver.
Do I have to use these exact numbers?
No. They are typical shop standards for reference. Your shop's quote and its capability govern the real part. Spec the numbers your design needs on the drawing, and we route to shops that can hold them.
Related reading: what is CNC machining, design for manufacturing and what CNC machining costs.
Request quotes for your part →