CNC machining tolerances define the acceptable limit of dimensional variation for a manufactured part. The standard CNC machining tolerance is typically ±0.125 mm (±0.005″). Tighter tolerances, such as ±0.025 mm (±0.001″), are reserved for critical fits but significantly increase manufacturing costs.
While modern CNC machines are highly accurate, they cannot produce perfect dimensions every time due to tool wear, thermal expansion, and material stress. Therefore, every dimension on an engineering drawing must have a defined tolerance.
This guide bridges the gap between design intent and shop-floor reality. Use the quick links below to find standard tolerance charts, learn how to select fits, and discover how to optimize your drawings for better pricing.
| What You Need to Solve | Relevant Section |
|---|---|
| Find common tolerance ranges | CNC Tolerance Basics and Typical Ranges |
| Determine how tight a part needs to be | Choosing Tolerances for Fit and Function |
| Learn how to specify tolerances on drawings | Specifying Tolerances Clearly on Engineering Drawings |
| Understand machining limits and costs | Machining Factors That Limit Achievable Tolerances |
| Verify supplier quality and conformance | Verifying Supplier Capability and Part Conformance |
CNC Tolerance Basics and Typical Ranges
This section explains how to read tolerance callouts and provides baseline reference information for standard machining capabilities.
Size Limits
A tolerance sets the upper and lower limits of an acceptable dimension. For example, Ø20 ±0.05 mm indicates a nominal diameter of 20 mm, a maximum limit of 20.05 mm, and a minimum limit of 19.95 mm. The total tolerance band is 0.10 mm.
Tolerances are expressed in different formats depending on design intent:
- Bilateral:
20 ±0.05(variation allowed equally in both directions from nominal) - Unilateral:
20 +0.10 / -0.00(variation allowed in only one direction) - Limit:
20.10 / 19.95(directly stating the absolute maximum and minimum limits)
Tolerance is the designed allowance on the drawing. Actual deviation is the measured difference from the nominal size on a physical part. Repeatability indicates how consistently a machine can hold that dimension across a production batch.
Typical Ranges
Machining capabilities vary by equipment, material, and part geometry. The following ranges represent typical expectations for modern CNC equipment under stable conditions.
| Feature or Requirement | Reference Range | Applicable Conditions | Verification Needs & Cost Impact |
|---|---|---|---|
| General Dimensions | ±0.125 mm (±0.005") | Standard 3-axis/4-axis milling on common metals (e.g., 6061, 304 SS). | Default title block rules apply. Most cost-effective. |
| Precision Fits (Holes/Shafts) |
±0.013 mm to ±0.025 mm (±0.0005" to ±0.001") | Reamed holes, turned bearing journals, rigid setups. | Requires specific tooling and inspection methods. Moderate cost increase. |
| High-Precision Features | ±0.005 mm (±0.0002") | Grinding, jig boring, or temperature-controlled precision turning. | High Cost: Requires transitioning from milling to grinding, temperature-controlled environments, and CMM reporting. |
These values are baseline references. The achievable tolerance always depends on the specific combination of part size, feature geometry, material rigidity, and workholding setup.
Standards and Defaults
When specific dimensions are not individually toleranced on a drawing, they default to a general standard. Many manufacturers apply standard title block rules based on the number of decimal places (e.g., .XX = ±0.01", .XXX = ±0.005") or reference international standards like ISO 2768 (e.g., ISO 2768-m for medium precision).
General tolerances apply to non-critical features like overall length, chamfers, or clearance holes. Shaft and bore fits require independent evaluation and explicit callouts. Always specify the governing standard and its revision year on the drawing so the manufacturer knows exactly how to inspect un-toleranced dimensions.
Choosing Tolerances for Fit and Function
This section details how to determine specific control requirements based on the part’s intended application in an assembly.
Functional Features
Using the aluminum bearing housing example, the tolerance strategy must align with the physical function of each feature:
- Bearing Bore: Requires a precise diametric tolerance and strict surface finish to ensure proper bearing retention and prevent fretting.
- Mounting Base: Requires flatness and perpendicularity controls to ensure flush contact with the mating assembly and prevent bolt-induced distortion.
- Bolt Hole Pattern: Requires positional control to ensure fasteners align with the threaded holes on the mating chassis.
- Outer Profile: Merely defines the physical boundary; a loose general tolerance is sufficient and reduces machining time.
Applying dimensional tolerances alone does not guarantee function. Size controls the width or diameter, but geometric tolerances (GD&T) control form (like cylindricity), and roughness dictates the surface texture.
Hole and Shaft Fits
Fits define the physical relationship between mating components. In engineering drawings, these are often designated using the ISO alphanumeric system (e.g., an H7/g6 fit for a sliding bearing). Using standard codes helps manufacturers immediately understand the design intent. Fits are categorized into three types:
- Clearance Fit: The shaft is always smaller than the hole, allowing free movement or sliding.
- Interference (Press) Fit: The shaft is always larger than the hole, requiring force or thermal expansion to assemble, creating a rigid joint.
- Transition Fit: Can result in either a slight clearance or slight interference, used for precise location and alignment.
Calculation Example for a Clearance Fit: Assume a nominal 10 mm shaft and hole intended for a slip fit.
- Hole Specification:
Ø10.000 +0.015 / -0.000(Min size: 10.000, Max size: 10.015) - Shaft Specification:
Ø10.000 -0.010 / -0.025(Min size: 9.975, Max size: 9.990) - Minimum Clearance = Minimum Hole (10.000) – Maximum Shaft (9.990) = 0.010 mm
- Maximum Clearance = Maximum Hole (10.015) – Minimum Shaft (9.975) = 0.040 mm
Fit selection must account for operating temperatures (especially thermal expansion disparities between different metals, like an aluminum housing and a steel bearing) and the assembly method used on the production floor.
Tolerance Stack-Up
Tolerance stack-up occurs when the allowable variations of individual dimensions combine linearly across an assembly.
Consider a shaft carrying three spacers, each dimensioned at 20 ±0.1 mm, resting against a machined step. In a worst-case scenario, if all three spacers are machined to their maximum limit (20.1 mm), the total length will be 60.3 mm. If the mating housing slot is machined to its minimum limit of 60.0 mm, the parts will not assemble, despite every individual component passing its own drawing requirements.
Worst-case analysis assumes all dimensions are at their extreme limits simultaneously. For assemblies with many components, statistical methods (such as Root Sum Square, RSS) are used to calculate a more probable accumulation.
DFM Practical Fix: To mitigate stack-up issues without tightening all tolerances (which directly drives up machining costs), engineers often leave one non-critical component (such as an end-cap, shim, or washer) with an adjustable or custom-cut tolerance. This acts as a buffer for the entire assembly, absorbing the accumulated variations of the cheaper, looser-toleranced parts.
Specifying Tolerances Clearly on Engineering Drawings
This section focuses on translating functional requirements into clear, executable instructions that prevent misinterpretation and pricing assumptions on the shop floor.
General Tolerances
Every engineering drawing must establish a baseline for dimensions that do not require specific control. This is typically managed through title block rules or by referencing standards like ISO 2768.
A frequent drafting error occurs when CAD software automatically exports default decimal places. For example, a designer models a standard bracket and the software outputs a thickness of 10.00. If the title block dictates that two decimal places (.XX) require a ±0.1 mm tolerance, but three decimal places (.XXX) demand a ±0.01 mm tolerance, arbitrarily changing the dimension to 10.000 forces the machinist to treat a simple bracket as a precision component.
Align your decimal places with your intended title block rules. Reserve specific, localized tolerance callouts exclusively for functional features to avoid paying precision prices for non-critical surfaces.
Datums and Position
Datums establish the reference framework for manufacturing setups and quality inspection. They should always reflect how the part physically mounts in the final assembly. For our aluminum bearing housing example, the flat mounting base should act as primary Datum A, because that surface dictates the part’s orientation when bolted to the chassis.
When specifying bolt hole patterns, traditional X/Y coordinate tolerances create a square tolerance zone. Geometric Dimensioning and Tolerancing (GD&T) uses True Position, which creates a cylindrical tolerance zone, offering 57% more acceptable area for the hole center without compromising assembly.
However, GD&T must be applied practically. While True Position provides a larger functional tolerance zone, overusing complex GD&T on simple, non-critical holes forces the supplier to move the part to a Coordinate Measuring Machine (CMM) for inspection instead of using standard hand tools. This inspection bottleneck directly drives up the quoted price.
Final Part Condition
Drawings often fail to specify whether dimensions apply before or after surface treatments like anodizing, plating, or powder coating.
Surface treatments add physical thickness. Type III Hard Anodizing, for instance, typically adds 0.025 mm to 0.05 mm of thickness per surface. If a bore is machined exactly to the nominal size of a tight H7 fit, the subsequent anodizing layer will shrink the hole diameter, causing the bearing press-fit to fail.
If “DIMENSIONS APPLY AFTER FINISH” is missing from the drawing, the machine shop will machine to nominal, the plater will add the coating, the part will fail inspection, and the buyer typically absorbs the cost of the scrapped batch. Explicitly state the final condition, or provide pre-plating tolerances.
Additionally, for large, thin-walled parts that are easily deformed (like thin aluminum rings), clearly state whether the part should be measured in a “Free State” or constrained to a fixture to simulate its installed condition.
Machining Factors That Limit Achievable Tolerances
Designers must recognize that a tolerance is not just a digital number; it is bound by physics, material properties, and machine mechanics.
Material Stability
Materials react differently to the heat and cutting forces generated during machining.
Metals possess specific thermal expansion coefficients. For example, aluminum expands at roughly 23 µm/m·°C. If a 500 mm aluminum plate heats up by just 5°C during aggressive roughing, it temporarily expands by nearly 0.06 mm. If the drawing demands a ±0.02 mm overall tolerance, the part may measure perfectly inside the warm machine enclosure, but it will shrink and fail once it reaches thermal equilibrium in a temperature-controlled QA lab.
Engineering plastics (such as POM, Nylon, or PTFE) present even greater stability challenges due to high thermal expansion rates, moisture absorption, and internal stress relief. Specifying a metal-grade ±0.01 mm tolerance on a plastic component is usually impractical; the material’s natural environmental warping will exceed the tolerance band during transit.
Geometry and Clamping
Part geometry determines how rigidly a component can be held and how far a cutting tool must extend. Lack of rigidity introduces vibration and deflection, directly limiting achievable accuracy.
| Feature Condition | Primary Risk | Actionable Design Improvements |
|---|---|---|
| Thin Walls (< 1 mm) | Material deflection or vibration (chatter) under cutting pressure, causing uneven surfaces or out-of-tolerance thickness. | Increase wall thickness where possible, add internal support ribs, or allow the supplier to use custom soft jaws. |
| Deep Holes / Cavities | Tool deflection causes the hole to taper or wander off-center at the bottom. | Rule of Thumb: Maintaining tight tolerances becomes exponentially more expensive when the depth-to-diameter (L:D) ratio exceeds 4:1 for milling or 8:1 for drilling. Reduce depth or open tolerances at the bottom. |
| Long, Slender Shafts | Workpiece bending (runout) away from the cutting tool in the center of the span. | Specify looser tolerances in the middle of the shaft, or design centers to allow for tailstock support during turning. |
| Multi-Face Features | Re-chucking the part to machine different sides introduces physical re-positioning errors. | Design critical concentric features, or hole patterns that must align perfectly, to be machined from a single setup (one orientation). |
Process Selection
Machinists select tools and routing based on the required tolerance, geometry, and surface finish. Tightening a tolerance often forces a fundamental change in the manufacturing process.
For a standard clearance hole, a machinist simply uses a drill. However, standard drills wander and cannot hold perfect cylindricity or exact diameters. If the drawing demands a precise ±0.015 mm bearing fit, the machinist cannot just “drill it more carefully.” They must drill the hole undersize, use a boring bar to straighten the hole’s axis, and finally use a precision reamer to achieve the final dimension.
Tightening a tolerance usually means adding entirely new operations, tool changes, and slower feed rates. Process selection must always balance the necessary functional fit against the compounding cost of these additional machining steps.
Reducing Cost Through Better Tolerance Design
This section translates technical specifications into commercial impact, explaining exactly why your quoted price changes and how to adjust your design for better manufacturability (DFM) without compromising performance.
Cost Drivers
When a machine shop estimator reviews an RFQ with tight tolerances, the price increase is not an arbitrary multiplier. It reflects concrete, measurable additions to the manufacturing workflow:
- Setup and Fixturing: Tight geometric tolerances (like perpendicularity between two faces) often require custom-machined soft jaws or specialized workholding to prevent the part from distorting when clamped.
- Secondary Operations: A standard milled finish might hold
±0.1 mm. If you require±0.005 mm, the part must be moved to a cylindrical grinder or wire EDM. Each machine change adds setup time and labor. - Tool Wear and Process Interruption: To hold a
±0.01 mmbore, the machinist cannot let the cutting tool wear down. They must stop the machine frequently to measure mid-cycle, adjust tool offsets, and replace endmills long before their normal end-of-life. - Inspection and Reporting: Measuring a highly toleranced part requires programming a Coordinate Measuring Machine (CMM), allowing the part to acclimate to the QA lab’s temperature, and generating detailed First Article Inspection (FAI) reports.
The “Headache Tax”: When estimators see an over-toleranced drawing, they don’t just calculate machine time—they add a hidden ‘risk premium’ (or ‘headache tax’) to cover anticipated scrap, or worse, they simply ‘No-Quote’ the project to avoid the liability. Good tolerance design doesn’t just lower the price; it ensures you actually get quotes from top-tier suppliers.
Design Adjustments
Before freezing a design, evaluate whether the cost drivers align with the part’s actual function. Minor adjustments can yield significant savings:
- Relax Non-Critical Dimensions: Leave external profiles, clearance holes, and chamfers at standard general tolerances (e.g., ISO 2768-m).
- Remove Cross-Face Dependencies: If a tight tolerance spans two opposing faces, the machinist must flip the part, losing their precise zero-point. If possible, redesign the part so all critical concentric or aligned features can be machined from a single orientation.
- Improve Clamping and Tool Access: Ensure the part has parallel, flat surfaces that a standard vise can grip securely. Standardized corner radii prevent the need for fragile, slow-cutting micro-tools.
- Verify Surface Roughness: Do not blanket the drawing with an Ra 0.8 (32 µin) requirement. Use standard Ra 3.2 (125 µin) for general surfaces, reserving Ra 0.8 or finer strictly for O-ring grooves or sliding bearing journals.
Before-and-After Example
Consider two different drafting approaches for an aluminum bearing housing.
| Comparison Area | Original Requirement | Adjusted Requirement | Expected Manufacturing Impact |
|---|---|---|---|
| Tolerance Allocation | Blanket ±0.02 mm applied across all dimensions via title block. | ±0.02 mm strictly on bearing bore; ISO 2768-m for outer profile. | Eliminates unnecessary precision milling on non-functional exterior surfaces. |
| Datum Structure | Vague or conflicting datums not aligned with assembly. | Datums match the physical mounting base and primary locating pins. | Reduces misinterpretation and inspection setup time. |
| Final Condition | Ambiguous surface finish requirements. | Explicitly states "Dimensions Apply AFTER Hard Anodize." | Eliminates the risk of the bore shrinking out-of-spec, reducing scrap. |
| Inspection Plan | Unspecified; implies full CMM layout for all dimensions. | CMM report required only for the bearing bore and mounting flatness. | Drastically reduces QA bottleneck, enabling faster, more accurate quoting. |
Verifying Supplier Capability and Part Conformance
Specifying the right tolerance is only half the process; you must also ensure the supplier can reliably hit those numbers and that both parties agree on how to measure them.
Capability Evidence
Almost any decent machine shop can brute-force one perfect “golden sample” by making ten parts and throwing away nine. But producing 1,000 parts with consistent fits requires statistical process control.
For critical projects, ask the supplier to confirm how they intend to hold the key features (e.g., will they ream or bore that hole?). If transitioning to high volume, require process capability data (such as Cp and Cpk scores) to prove their machining process is statistically stable, rather than relying on them manually sorting out the bad parts at the end of the line.
Measurement Methods
Discrepancies often arise when the supplier and the buyer use different methods to measure the same feature.
Ensure the inspection tool matches the tolerance requirement. A micrometer is suitable for precision outer diameters, while verifying true position or flatness over a large area typically requires a CMM.
Note on Resolution vs. Accuracy: A digital caliper that displays 0.01 mm resolution is rarely accurate or repeatable to 0.01 mm, especially in the hands of different operators. Relying on calipers for tolerances tighter than ±0.05 mm is a common source of false rejections.
The Correlation Problem: A common dispute occurs when the supplier measures a bore with a precise plug gauge (Pass), but the buyer inspects incoming parts using a CMM in a different temperature environment (Fail). To prevent this, your RFQ must explicitly align the inspection correlation: if a feature is critical, agree on the exact measurement tool, fixturing, and setup state before production begins.
Acceptance Requirements
Establish clear acceptance criteria before the first chip is cut.
- Specify the inspection scope: Do you require a First Article Inspection (FAI) report, AQL sampling (e.g., inspecting 10% of the batch), or 100% inspection on critical features?
- Define exactly which measured data points must be recorded on the inspection report.
- Establish a deviation workflow. If a non-critical feature is out of tolerance by 0.01 mm, is there a Material Review Board (MRB) process to approve it “as-is,” or is it an automatic rejection?
Need help evaluating your tolerances? Submit your 2D drawings and 3D models with your critical fits, locating features, or sealing surfaces highlighted, and our engineering team will provide a comprehensive DFM and tolerance review to help optimize your manufacturing costs.
Hey, I'm Kevin Lee
For the past 10 years, I’ve been immersed in various forms of sheet metal fabrication, sharing cool insights here from my experiences across diverse workshops.
Get in touch
Kevin Lee
I have over ten years of professional experience in sheet metal fabrication, specializing in laser cutting, bending, welding, and surface treatment techniques. As the Technical Director at Shengen, I am committed to solving complex manufacturing challenges and driving innovation and quality in each project.
