CNC Machining Tolerance Chart: Standard, Fine and Precision Explained
Over-specified tolerances cost money quietly. The cost never appears as a line item. It shows up as a higher price per part on every unit of every batch, indefinitely, for accuracy the part never needed.
It happens for understandable reasons. Tightening a number feels like diligence. But every tolerance tightened beyond functional need buys slower feeds, more careful setups, extra inspection and a higher scrap rate. Tolerance is a budget. Spend it where it does no work and there is nothing left for the features that matter.
Below: what the three tolerance bands mean in practice, which operations reach them, how material behaviour decides whether a tolerance survives in service, and how to mark up a drawing so you pay for precision only where it earns its place. For the capabilities behind these numbers, see our CNC machining services.
Table of Contents
What a Tolerance Actually Specifies
A tolerance is the permitted deviation from a nominal dimension. A bore called out as 25.00 mm plus or minus 0.05 mm is acceptable anywhere between 24.95 and 25.05 mm. No machining process produces an exact dimension, so the tolerance states how much variation the part can carry and still work.
Three ways it appears on a drawing. Bilateral, written as 25.00 plus or minus 0.05 mm, allows deviation in both directions and is the most common form. Unilateral, written as 25.00 plus 0.10 minus 0.00 mm, is for features that may be oversized but never undersized, such as a clearance hole. ISO fit codes, written as 25 H7 for a hole or 25 g6 for a shaft, carry both the tolerance and the intended fit in one notation, which makes them the better choice for mating features because they communicate function rather than just a number.
One thing that gets forgotten. The title block general tolerance applies to every dimension you do not individually tolerance, and that is where most dimensions should live. Individual callouts are for the handful of features that actually control fit or function.
Standard, Fine and Precision Bands
Standard, plus or minus 0.10 mm
What a well-set-up 3-axis mill produces without special measures. Right for structural features, clearance holes, external profiles, cosmetic faces, and any dimension where a tenth of a millimetre changes nothing. The vast majority of dimensions on any drawing belong here.
Fine, plus or minus 0.05 mm
Requires more deliberate work: lighter finishing passes, better workholding, a separate inspection step. Appropriate for mating faces, sliding fits, gasket lands, and features locating one component against another. Expect roughly a 15 to 30 percent cost uplift on the affected feature, depending on geometry.
Precision, plus or minus 0.02 mm and tighter
Reached by specific operations rather than by milling harder. Reaming, boring, precision turning and grinding get you here. Bearing seats, press fits, dowel bores and precision locating holes justify it. Below about plus or minus 0.01 mm you leave standard machining altogether and move into grinding and lapping, where cost climbs steeply.
Roughly: standard to fine adds meaningful cost on a feature. Fine to precision can double it. Below precision, the process itself changes.
CNC Machining Tolerance Chart
Which operation reaches which band:
Operation | Standard | Achievable | Notes |
3-axis milling (general) | ± 0.10 mm | ± 0.05 mm | Tighter requires dedicated setup and inspection |
CNC turning (OD / ID) | ± 0.05 mm | ± 0.02 mm | Rigid workholding. Best in steel and Delrin |
Drilled holes (position) | ± 0.10 mm | ± 0.05 mm | Spot-drill first for tight positional accuracy |
Reamed holes (diameter) | ± 0.02 mm | ± 0.01 mm | Specify for press fits and locating bores |
Bored holes | ± 0.02 mm | ± 0.02 mm | Good roundness and concentricity to the turned axis |
Slots and pockets (width) | ± 0.05 mm | ± 0.03 mm | Depth tolerance ± 0.10 mm standard |
Angular features | ± 0.5° | ± 0.1° | Fixture-dependent on compound angles |
Surface finish (as machined) | Ra 3.2 µm | Ra 0.8 µm | Below Ra 0.8 requires polishing or lapping |
If a tolerance you need is not on this list, raise it at enquiry rather than putting it on the drawing and hoping. We will confirm whether it is reachable and what it costs before you commit material. How milling and turning capability compare is covered in CNC milling vs CNC turning.
Material Stability Chart
A tolerance held on the machine is not the same as a tolerance held in service, and this gets ignored more than anything else on the drawing.
Machine a nylon part to plus or minus 0.02 mm in a dry workshop and leave it overnight at ambient humidity. Nylon absorbs moisture and can grow by 0.3 to 0.8 percent. On a 50 mm dimension that is up to 0.4 mm of movement, twenty times the tolerance you specified and paid for. The part was in spec leaving the machine and out of spec by morning.
Material | Stability in service | Functional tolerance | Notes |
Delrin / POM | Excellent | ± 0.02 mm | Low moisture absorption, high stiffness |
Aluminium 6061-T6 | Excellent | ± 0.02 mm | Predictable thermal expansion |
Stainless 304 / 316 | Excellent | ± 0.02 mm | Very stable, slower to machine |
Brass | Excellent | ± 0.02 mm | Stable and free-machining |
Mild steel | Very good | ± 0.03 mm | Watch for surface corrosion in storage |
Acrylic / PMMA | Good | ± 0.05 mm | Stable but brittle, chips on thin walls |
Polycarbonate | Good | ± 0.05 mm | Softer than acrylic, less prone to chipping |
Nylon PA6 / PA66 | Poor | ± 0.10 mm | Absorbs moisture, moves 0.3 to 0.8 percent |
HDPE / UHMWPE | Poor | ± 0.15 mm | Moves with temperature, thermally sensitive |
PTFE | Poor | ± 0.15 mm | Creeps under sustained compression load |
Which gives you the design rule: choose the material for the tolerance you need, rather than specifying a tolerance the material cannot keep. If a part needs plus or minus 0.02 mm and the plan is nylon, change the plan or change the tolerance. Our comparison of nylon vs Delrin vs HDPE for CNC machining covers the mechanical trade-offs, and for a broader material decision see ABS vs HDPE vs PVC vs acrylic.
Surface Finish Is a Separate Specification
Dimensional tolerance and surface finish are independent. A part can be dimensionally perfect with a rough finish, or beautifully polished and out of tolerance. Specify them separately.
Ra 3.2 micrometres: standard as-machined finish with visible tool marks. Fine for structural and non-mating faces, and what you get if you specify nothing
Ra 1.6 micrometres: fine milled finish. Appropriate for mating faces and general sealing surfaces
Ra 0.8 micrometres: very fine. Bearing journals, dynamic seal faces, optical mounting surfaces
Ra 0.4 micrometres and below: needs polishing or lapping after machining. Specify only where optically or tribologically required
Apply finish callouts to specific faces, never to the whole part. Ra 0.8 across every surface of a bracket multiplies machining time for no functional return. For optically clear plastics the finish conversation is different again, and we cover it in acrylic CNC machining.
Tolerance in Machining vs Moulding
If your part might move to volume production later, the two processes control dimensions in completely different ways.
In machining the tolerance is a function of the machine, the tooling and the setup, and you control it directly. In injection moulding the part dimension is a function of the tool dimension minus material shrinkage, and shrinkage varies with wall thickness, gate position, melt temperature and hold pressure. The tool has to be cut oversized to compensate, which makes moulding tolerances looser and material-dependent in a way machined tolerances are not.
ABS: 0.4 to 0.7 percent shrinkage, among the most dimensionally predictable
Polycarbonate: 0.5 to 0.7 percent. Good accuracy
Nylon PA6: 0.7 to 1.5 percent, rising further with post-moulding moisture absorption
Polypropylene: 1.5 to 2.5 percent. High, and prone to warping in asymmetric parts
HDPE: 1.5 to 3.0 percent, and directional, higher along the flow direction than across it
If you are working out compensated tool dimensions, our injection molding shrinkage calculator does the arithmetic per material. For the wider decision about when machining stops making economic sense and tooling starts, see CNC machining vs injection molding.
How to Mark Up a Drawing
A short discipline that reliably takes cost out:
Start loose: put a general tolerance in the title block, typically plus or minus 0.10 mm linear and plus or minus 0.5 degrees angular, and let it govern everything
Tighten only what functions: go through the drawing asking what breaks if this dimension drifts. If nothing does, leave it on the general tolerance
Use fit codes for mating features: H7 or g6 communicates intent better than a raw number and lets us pick the right operation
Mark finish per face: only where it matters, never globally
State the operating environment: if the part runs at 60 degrees Celsius or in a humid plant, say so. It changes which material can hold your tolerance
Keep model and drawing in agreement: where they conflict the drawing governs, but a conflict means we stop and ask, which costs you lead time
Full file and drawing requirements are in how to prepare a CAD file for CNC machining. Every quote we issue includes a written DFM report flagging over-specified tolerances with the cost impact of each, so the decision stays with you and gets made on numbers. What goes into one is covered in our guide to the DFM report.
Frequently Asked Questions
What is the tightest tolerance a CNC mill can hold?
In routine production, plus or minus 0.05 mm on critical features with dedicated setup and inspection. Reaming and boring reach plus or minus 0.02 mm, and precision turning matches that on diameters. Below plus or minus 0.01 mm you are no longer milling: those dimensions come from grinding, honing or lapping, and cost climbs steeply. Before specifying anything tighter than plus or minus 0.02 mm, check the material can hold it in service.
Do plastic parts hold tolerances in service?
It depends entirely on the material. Delrin and acetal hold plus or minus 0.02 mm reliably. Nylon absorbs moisture and can move 0.3 to 0.8 percent after machining, which on a 50 mm dimension is up to 0.4 mm. HDPE and polypropylene move with temperature. PTFE creeps under sustained load. Choose the material for the tolerance you need rather than specifying a tolerance the material cannot keep.
What does ISO H7 mean?
H7 is a standard hole tolerance in the ISO fit system. The letter gives the position of the tolerance zone relative to nominal and the number gives its width. H means the zone starts at nominal and runs positive, so an H7 hole is never undersized. Pair it with a shaft code and you have defined the fit: H7 with g6 gives a running clearance, H7 with p6 gives a light press fit. Using fit codes rather than raw numbers tells the machinist what the feature is for.
How much does tightening a tolerance cost?
Standard to fine, meaning plus or minus 0.10 to plus or minus 0.05 mm, typically adds 15 to 30 percent on the affected feature. Fine to precision, plus or minus 0.05 to plus or minus 0.02 mm, can double it, because it usually means adding an operation such as reaming or boring plus a separate inspection step. The cost lands on every part in every batch, so an unnecessary tightening on a production part compounds indefinitely.
Does surface finish affect dimensional tolerance?
They are specified independently but they interact. Achieving a fine finish requires light finishing passes that remove a small amount of additional material, so the finishing allowance has to be accounted for when targeting a tight dimension. On a precision bore needing both plus or minus 0.02 mm and Ra 0.8 micrometres, the operations get planned together. Specify both where you need both, and neither where you need neither.
Comments