Last Updated: March 2026
CNC Machining Tolerances Explained — Complete Guide
Standard CNC machining tolerance is ±0.05mm (±0.002") for general features. Precision tolerances of ±0.01mm (±0.0004") are achievable with standard CNC milling and turning. Tighter tolerances require grinding, honing, or EDM. This guide explains tolerance by process, GD&T basics, and critically — the cost impact of specifying tolerances tighter than necessary. Rapid Manufacturing applies ±0.05mm as the default for unspecified dimensions on all quoted parts.
Achievable Tolerances by Process
| Process | Standard Tolerance | Precision Tolerance | Surface Finish (Ra) | Notes |
|---|---|---|---|---|
| CNC Milling (3-axis) | ±0.05mm | ±0.02mm | 1.6µm | General milling of prismatic features |
| CNC Milling (5-axis) | ±0.05mm | ±0.02mm | 1.6µm | Complex geometry; tolerance on compound angles may be ±0.05mm |
| CNC Turning | ±0.05mm | ±0.01mm | 1.6µm | Cylindrical features hold tighter than milled features |
| CNC Grinding (OD) | ±0.01mm | ±0.005mm | 0.4–0.8µm | Bearing journals, precision shafts, gauge work |
| CNC Grinding (Surface) | ±0.01mm | ±0.005mm | 0.4–0.8µm | Flat precision surfaces, tooling plates |
| ID Grinding / Honing | ±0.010mm | ±0.005mm | 0.2–0.8µm | Bore precision for bearing and hydraulic fits |
| Wire EDM | ±0.010mm | ±0.005mm | 0.8–1.6µm | Complex profiles, hardened materials, no cutting forces |
| Sinker EDM | ±0.020mm | ±0.010mm | 0.4–1.6µm | Cavities and features inaccessible by cutting tools |
| Lapping / Superfinishing | ±0.005mm | ±0.001mm | 0.025–0.1µm | Optical surfaces, gauge blocks, sealing faces |
Rapid Manufacturing Standard Specifications
GD&T Basics for Engineers
GD&T (Geometric Dimensioning and Tolerancing) is defined by ISO 1101 in Australia (equivalent to ASME Y14.5 in the US). It controls geometry beyond simple size — critical for parts where location, orientation, and form matter.
| GD&T Symbol | Controls | Typical Use | Typical Values |
|---|---|---|---|
| Flatness ⏥ | Surface deviation from a perfect flat plane | Sealing faces, precision datum surfaces | 0.01–0.1mm |
| Cylindricity ⌀ | Combined roundness and straightness of cylinder | Bearing journals, precision bores | 0.005–0.02mm |
| Perpendicularity ⊥ | Angle deviation from 90° to datum | Mating faces, bearing housings | 0.01–0.05mm |
| Parallelism ∥ | Deviation of surface from parallel to datum | Spacers, shims, mating plates | 0.01–0.05mm |
| Position ⊕ | Location of feature centre from true position | Bolt holes, pin locations | ø0.1–0.5mm |
| Concentricity / Coaxiality | Alignment of axes to datum axis | Stepped shafts, coupling faces | 0.01–0.05mm |
| Circular Runout ↗ | Combined eccentricity and taper error | Rotating shafts, impellers | 0.01–0.05mm |
| Total Runout ↗↗ | Total surface deviation on rotation | High-speed rotors, precision shafts | 0.005–0.02mm |
Cost Impact of Tighter Tolerances
One of the most common and costly engineering errors is over-specifying tolerances. Every dimension tighter than ±0.05mm adds cost. The chart below shows the approximate cost multiplier for machined features at different tolerance bands:
General fit — saw cut, turning to ±0.5mm is trivial
Normal machining, no special care required
Default CNC machining tolerance. No premium.
Slower feeds, more measurement, minor premium
Precision machining, temperature-controlled measurement
Requires grinding or fine boring operations
Requires precision grinding, lapping, or honing. Specialist shop.
Tolerance Selection Guidance
Use ±0.1mm or greater
Non-mating features: overall length, depth of pockets, general geometry where fit is not critical.
Use ±0.05mm (default)
Most mating features where fit is controlled but not precision: clearance holes, general interfaces.
Use ±0.02mm
Sliding fits, locating pins, close clearance fits where positional accuracy matters.
Use ±0.01mm
Running fits, bearing housings (H7), precision shaft diameters (h6), gauge-referenced features.
Use ±0.005mm or tighter
Only for truly critical fits: precision bearing bores, gauge blocks, optical mounts, sealing surfaces on high-pressure plant.
Use GD&T instead of tighter ±
Where location, orientation, or form matters more than size. GD&T often permits larger ± on size while controlling geometry precisely.
Get a Quote with Free DFM Tolerance Review
Rapid Manufacturing includes free DFM analysis with every quote. We flag tolerances that are tighter than necessary for your application — saving cost without compromising function.
Request a QuoteFrequently Asked Questions
What is the standard CNC machining tolerance?
The standard CNC machining tolerance for general features is ±0.05mm (±0.002"). This is achievable on all modern CNC machining centres without special setup or process control. For precision features such as bearing bores, shaft diameters, and mating interfaces, tolerances of ±0.01mm (±0.0004") are routinely achievable. Tighter tolerances (±0.005mm and below) require specialised grinding, honing, or lapping operations. Rapid Manufacturing applies ±0.05mm as the default unless tighter tolerances are specified.
How does specifying tighter tolerances affect cost?
Tighter tolerances increase cost in three ways: slower cutting speeds and feeds to improve dimensional consistency, more tool changes to maintain sharp cutting edges, and additional inspection steps (CMM measurement, gauge verification). As a rough guide: features at ±0.05mm add minimal cost. Features at ±0.02mm add approximately 10–30% per feature. Features at ±0.01mm may add 30–100% per feature. Features tighter than ±0.01mm often require grinding or lapping, which may double or triple the feature cost. Only specify tight tolerances where they are functionally necessary.
What is GD&T and why should engineers use it?
GD&T (Geometric Dimensioning and Tolerancing) is a standardised system (ISO 1101 / ASME Y14.5) for defining the allowable variation in part geometry — not just size, but also form, orientation, location, and runout. Unlike simple ±dimensional tolerances, GD&T communicates design intent clearly to machinists and inspectors, often allowing looser tolerances on non-critical features while tightening only where function demands it. This typically reduces manufacturing cost while improving functional quality. Rapid Manufacturing accepts and interprets GD&T callouts on 2D drawings.
What tolerance can CNC grinding achieve?
CNC cylindrical and surface grinding typically achieves tolerances of ±0.005mm (±0.0002") on diameter and thickness. ID grinding can achieve tolerances of ±0.005–0.010mm on bore diameter. Surface roughness after grinding is typically Ra 0.4–0.8µm, compared to Ra 1.6µm for as-machined surfaces. Grinding is used for bearing journals, precision bores, gauge blocks, and surfaces requiring mirror finishes or very tight dimensional control.
What is the difference between ISO tolerances (H7/h6) and ±tolerances?
ISO fit tolerances (H7, h6, f7, etc.) are a standardised system for defining shaft-hole clearance and interference fits. H7 specifies the allowable bore deviation (upper tolerance only, referenced to nominal), while h6 specifies the shaft tolerance. Together they define the clearance or interference. For example, a 25mm H7/h6 pair results in a running clearance fit. These are typically specified for bearing bores, shaft diameters, and press-fit interfaces. ±tolerances are used for general dimensions without a specific mating requirement. Rapid Manufacturing can machine to both ±dimensional tolerances and ISO fit codes.
What surface roughness does CNC machining achieve?
As-machined CNC milling and turning typically produces Ra 1.6µm surface roughness. Finer finishes are achievable: Ra 0.8µm with additional finishing passes, Ra 0.4µm after grinding, and Ra 0.1–0.2µm after lapping or superfinishing. Surface roughness affects sealing surfaces, bearing interfaces, fatigue life, and tribological performance. Specifying surface roughness tighter than Ra 1.6µm adds cost — only specify where functionally required.