What machining tolerances for CNC parts
A machining tolerances chart is the permitted variation from a nominal dimension or geometric requirement. It defines the acceptable result, not only the machine’s advertised accuracy. A 20.00 mm feature with a ±0.10 mm tolerance may measure from 19.90 mm to 20.10 mm and still conform a 20.00 +0.00/-0.02 mm bore has a different functional intent and must be treated differently.
For CNC parts, the best tolerance is the loosest one that still protects fit, function, safety, sealing, motion, appearance, or a downstream manufacturing step. General values can help early design discussions, but they are not a purchase specification. The released drawing or model-based definition, stated material condition, finish allowance, inspection method, and supplier confirmation control the production requirement.
MXY Machining lists CNC capability down to ±0.020 mm (±0.001 in) for appropriate work. That is not a promise that every feature, material, or part size can hold that value. Feasibility must be reviewed feature by feature, especially for thin, long, deep, flexible, or hard-to-inspect geometry.
How tolerances affect cost and lead time
A tighter requirement may require slower finishing passes, more rigid workholding, a different machine or process, tool-life controls, in-process probing, additional setup time, a special gauge, or expanded inspection. It can also raise scrap risk. Those costs are concentrated on the specified features, which is why selective tolerancing usually delivers better value than a blanket “tight everywhere” approach.
The relationship is not a fixed multiplier. One tight diameter near an accessible face may be straightforward; the same tolerance on a thin-wall, deep bore after anodizing may need substantially different processing. The most useful RFQ includes the intended function, mating-part information where relevant, quantity, drawing revision, CAD model, material and finish requirements, and any required inspection record.
CNC machining tolerance chart
A machining tolerances chart shows the acceptable dimensional variation for manufactured parts. Engineers and designers use tolerance charts to balance accuracy, cost, and manufacturability. This guide provides clear CNC machining tolerance charts and explains how to apply them correctly in real production environments.
This machining tolerances chart is used by engineers to quickly reference acceptable dimensional limits during CNC production. A clear machining tolerances chart helps reduce design errors and improves communication between design and manufacturing teams.
Tolerance band | Typical use | Planning guidance | What to confirm before release |
General / non-critical | Brackets, covers, cosmetic non-mating features | About ±0.13 mm (±0.005 in) is a common shop planning reference for local metal features. | Supplier default or ISO class, material, part size, and measurement method. |
Precision | Location of mating features, controlled clearances, bearing-adjacent features | Roughly ±0.05 mm (±0.002 in) may be practical on selected, well-supported features. | Datum scheme, setup count, tool access, finish stock, and inspection plan. |
Tight | Fits, seals, alignment, controlled bores and shafts | About ±0.025 mm (±0.001 in) can be feasible on selected features with controlled process conditions. | Process route such as boring, reaming, grinding, or honing; gauge capability; lot size. |
Special process | Critical bores, precision motion, optical or metrology-sensitive interfaces | Tighter than ±0.025 mm often needs specialized tooling, operations, and metrology. | Written suppli |
General Machining Tolerances Chart
General machining tolerances apply when no specific tolerance is defined on an engineering drawing. These tolerances are commonly used for non critical features where exact precision is not required. Typical general machining tolerance ranges include:
Linear dimensions: ±0.005 in or ±0.13 mm
Hole diameters: ±0.005 in
Shaft diameters: ±0.005 in
Flatness and straightness: 0.005 in per 12 in
General tolerances reduce programming time, inspection effort, and overall machining cost. They are suitable for brackets, housings, and structural components.
Dimensional tolerances vs GD&T
A plus/minus dimension controls size or distance. It may not adequately control where a hole axis sits relative to the faces that locate the part in an assembly. Geometric dimensioning and tolerancing (GD&T) adds controls for form, orientation, location, and runout through a standardized drawing language.
ASME Y14.5-2018 (R2024) establishes symbols, rules, definitions, requirements, defaults, and recommended practices for communicating GD&T on drawings, digital data, and related documents. It is a drawing-language standard; it does not supply a universal machining tolerance. [2]
- Use size tolerances when the feature’s actual size is the requirement, such as a simple thickness or a non-critical hole diameter.
- Use datums and position tolerance when the relationship of a hole pattern to functional mounting faces or locating features matters.
- Use flatness, perpendicularity, parallelism, profile, runout, or other geometric controls only where they express a real function and can be inspected.
Standard vs Tight Machining Tolerances
Standard tolerances are used for most machined parts where dimensional variation does not affect function. They allow faster machining speeds and minimal inspection.
Tight tolerances are required for mating parts, press fits, and precision assemblies. These tolerances demand slower cutting speeds, stable setups, and additional quality control.
Using tight tolerances where they are not functionally required increases production cost without improving performance.
ISO 2768 general tolerances
ISO 2768 is commonly used to reduce repetitive tolerance callouts on drawings. ISO 2768-1:1989 covers general tolerances for linear and angular dimensions without individual tolerance indications, using four classes: f (fine), m (medium), c (coarse), and v (very coarse). ISO 2768-2:1989 addresses general geometrical tolerances for features without individual tolerance indications. [1]
A title-block note such as “ISO 2768-mK” is often seen in practice, but its use must be deliberate: the designation should be interpreted against the applicable purchased standard and the drawing’s own requirements. Do not assume that ISO 2768 resolves a critical fit, a datum relationship, an unspecified material condition, or a finishing allowance. The ISO publication itself emphasizes complete drawing tolerancing so requirements are not left to workshop or inspection judgment. [1]
When a part uses ASME Y14.5 rather than the ISO GPS system, identify that framework on the drawing and avoid mixing conventions without engineering review. For critical interfaces, specify the actual local size limits, GD&T controls, datums, surface condition, and inspection requirement rather than relying solely on a general-tolerance note.
What drives achievable tolerances
Driver | Why it changes the result | Design response |
Material behavior | Hard alloys raise cutting loads; plastics and thin sections can move with heat, stress relief, or clamping. | State grade and condition; leave finishing stock; discuss stress relief or a free-state inspection condition when needed. |
Tool reach and deflection | Long, slender cutters bend and vibrate; deep cavities amplify error. | Increase internal radii where function allows, shorten reach, reduce depth, or plan a dedicated finishing operation. |
Workholding and setups | Each re-clamp can introduce datum-transfer variation or distortion. | Reference critical features from common datums and keep related geometry within one setup where practical. |
Part stiffness | Thin walls, tall ribs, and open shapes deflect during cutting and measurement. | Thicken or brace vulnerable regions, or accept a process-specific tolerance review. |
Thermal effects and tool wear | Heat, tool growth, and wear shift feature size during a run. | Plan controlled finishing passes and in-process checks for critical features. |
Finishing and inspection | Anodizing, plating, coating, burr removal, and measurement uncertainty can affect final acceptance. | Specify final versus pre-finish dimensions, coating thickness or mask areas, edge condition, and inspection method. |
Practical examples
1. Sheet-like aluminum bracket
Most outside sizes, non-mating pockets, and relief features can use the general tolerance strategy stated in the title block. Apply tighter requirements only to the surfaces and holes that locate the bracket in the assembly. If two mounting holes must align to a chassis, control the pattern location from functional datums instead of tightening every overall dimension.
2. Bearing bore in a turned housing
The bore’s final size, roundness or cylindricity requirement if needed, surface finish, and relation to the locating face should be engineered as one interface. A generic ±0.001 in note alone may be insufficient. Identify the bearing manufacturer’s fit requirement and confirm whether boring, reaming, honing, or grinding is required for the part material and geometry.
3. Sealed fluid manifold
The sealing face, port locations, thread specification, surface finish, and burr condition can all affect leak performance. Control the face and ports from functional datums; specify which dimensions apply before or after coating; and request a feasibility review for cross-drilled passages, deep features, and inspection access.
4. Thin-wall polymer enclosure
Plastic stiffness and thermal response make a metal-style tolerance note unreliable. Prioritize interface features, define measurement condition if temperature matters, and avoid applying a very tight all-over tolerance to cosmetic walls. A supplier may need a different process strategy, fixture, or tolerance allocation for the final material.
Frequently asked questions
What is a standard CNC machining tolerance?
Many suppliers use around ±0.13 mm (±0.005 in) as a general planning reference for local machined metal features. It is not a universal standard and should not override a drawing, a stated ISO class, or a supplier’s written specification.
Can CNC machining hold ±0.001 in?
It can be feasible for selected features under controlled conditions. Whether it is appropriate depends on material, geometry, tool access, workholding, process route, production quantity, temperature, and metrology. Obtain feature-specific confirmation before release.
Is ISO 2768 enough for a precision part?
Usually not by itself. ISO 2768 helps control dimensions or geometry without individual indications, but a precision interface generally needs explicit size limits, datums, GD&T where appropriate, surface condition, and an inspection plan.
Should every dimension have a tight tolerance?
No. Blanket tight tolerances can increase cost and complicate inspection without improving the part. Tighten only what protects the part’s form, fit, function, safety, or downstream process.
Do coatings and anodizing change tolerance?
They can. State whether a dimension applies before or after finishing, identify relevant thickness or masking requirements, and confirm the process route with the supplier. Do not assume a nominal coating will preserve a critical bore, thread, or mating face.
