CNC Machining Tolerances
A practical engineering reference: standard, precision, and ultra-precision tolerances, surface finishes, GD&T essentials, material-specific limits, and how each choice impacts cost.
What Is a Tolerance? Linear vs. Angular
Every CNC drawing carries two categories of tolerance: linear (controls distances) and angular (controls angles). Before looking at any numbers, understand what these terms mean and why they exist at all.
The core problem: all manufacturing processes have variation
No CNC machine cuts to an exact number. A spindle cutting a 1.000 in. (25.4 mm) slot produces 0.9997 in. (25.39 mm) on one part and 1.0003 in. (25.41 mm) on the next due to tool wear, thermal expansion, vibration, and fixture repeatability. A nominal dimension of exactly 1.000 in. (25.4 mm) is physically unachievable. It would require infinite precision.
A tolerance solves this by defining the acceptable range around the nominal. ±0.005 in. (±0.13 mm) on a 1.000 in. (25.4 mm) dimension means any part measuring between 0.995 in. (25.27 mm) and 1.005 in. (25.53 mm) passes inspection. The question you answer when setting a tolerance is not “how precise is the machine?” It's “how much variation can my design functionally absorb?” These are very different questions. Confusing them is the #1 source of over-toleranced drawings and unnecessary cost.
Linear Tolerances
Controls: distances measured in a straight line
Linear tolerances apply to any dimension you would measure with a caliper, micrometer, or CMM probe moving in a straight line: width, depth, hole diameter, wall thickness, step height, thread pitch diameter. If a feature has a length, it needs a linear tolerance.
How to read it on a drawing
2.500 ±0.005
→ Accepts 2.495–2.505 in. (63.37–63.63 mm). Rejects everything outside.
Bilateral vs. unilateral
Bilateral (±0.005 in. / ±0.13 mm): zone is symmetric around nominal. Preferred because it gives equal error budget in both directions.
Unilateral (+0.010/−0.000 in. / +0.25/−0.00 mm): zone is one-sided. Use for interference fits or press-fit bores where only one direction of error is acceptable.
Angular Tolerances
Controls: the orientation of one surface relative to another
Angular tolerances control angles: chamfers, tapers, mating inclined faces, draft angles. Expressed in degrees (°), arc-minutes (′ = 1/60 of a degree), and arc-seconds (″ = 1/3600 of a degree). Standard CNC holds ±0°30′ reliably; precision work reaches ±0°10′.
How to read it on a drawing
45° ±0°30′
→ Accepts 44°30′–45°30′. That is a 1° total band.
The key notation
1° = 1 degree | 1′ = 1 arc-minute (0.0167°) | 1″ = 1 arc-second (0.000278°)
Most title blocks default to ±1° for angular dimensions unless a tighter callout is specified.
Why angular errors compound with distance (the lever arm effect)
Angular tolerances are not scale-independent. The same 0.5° angular error produces very different linear deviations depending on how far you measure from the origin. Formula: linear deviation = L × tan(angular error), where L is the distance from the angular datum.
| Distance from datum | 0.5° error → | 1° error → | Significance |
|---|---|---|---|
| 1 in. (25.4 mm) | 0.0087 in. (0.22 mm) | 0.0175 in. (0.44 mm) | 1.7× standard tolerance: evaluate fit function |
| 3 in. (76.2 mm) | 0.026 in. (0.66 mm) | 0.052 in. (1.32 mm) | Outside ±0.005 in. (±0.13 mm): starts to matter |
| 6 in. (152.4 mm) | 0.052 in. (1.32 mm) | 0.105 in. (2.67 mm) | 10× standard tolerance: significant |
| 12 in. (304.8 mm) | 0.105 in. (2.67 mm) | 0.209 in. (5.31 mm) | Major alignment error at assembly |
This is why GD&T perpendicularity and angularity callouts express the tolerance in linear units (a zone width between parallel planes) rather than degrees. It directly represents the functional impact at the mating surface.
Block tolerances: the default that covers most dimensions
Every engineering drawing should have a title block with a general tolerance: typically ±0.005 in. (±0.13 mm) for 3-decimal dimensions, ±0.010 in. (±0.25 mm) for 2-decimal, and ±1° for angular dimensions. This block tolerance applies to every dimension without an explicit callout. You only need to add a specific tolerance callout when your design functionally requires something tighter or more relaxed than the block default. This keeps drawings clean and gives the machinist freedom on non-critical features.
Linear Tolerance Reference
Achievable linear tolerances for CNC machining, from standard to ultra-precision. Cost impact is relative to the baseline ±0.005″ standard tolerance.
| Level | Inches | Metric | Cost Impact | Typical Use |
|---|---|---|---|---|
Standard | ±0.005″ | ±0.13 mm | Baseline | Default for most features |
Precision | ±0.002″ | ±0.05 mm | +15–30% | Mating surfaces, bearing fits |
High PrecisionPOPULAR | ±0.001″ | ±0.025 mm | +40–80% | Reamed holes, press fits |
Ultra Precision | ±0.0005″ | ±0.013 mm | +100–200% | Optical, safety-critical components |
Grinding/Lapping | ±0.0002″ | ±0.005 mm | +200–400% | Requires secondary operations |
Design Tip: Avoid Over-Tolerancing
Only call out tight tolerances on features that truly require them. Over-tolerancing is the #1 driver of unnecessary CNC cost. Apply ±0.005″ to general features and reserve ±0.001″ or tighter for critical dimensions.
Angular Tolerance Reference
Achievable angular tolerances for CNC machining, standard to ultra-precision. The “Linear Dev. at 6 in.” column shows the actual linear positional error that the angular deviation produces at a 6 in. (152 mm) reference distance, because angular errors are only meaningful in the context of distance.
| Level | Tolerance | Arc-Minutes | Linear Dev. at 6 in. (152 mm) | Typical Use |
|---|---|---|---|---|
Standard | ±1° | ±60′ | ±0.105″ | General chamfers, draft angles, non-mating faces |
Precision | ±0°30′ | ±30′ | ±0.052″ | Mating tapers, angled mating faces |
High PrecisionCOMMON | ±0°10′ | ±10′ | ±0.017″ | Precision tool holders, conical seats |
Ultra Precision | ±0°1′ | ±1′ | ±0.0017″ | Precision spindles, optical mounts |
Angular tolerances tighten when features are long
A ±1° block tolerance is completely acceptable on a 0.25 in. chamfer, the linear deviation at that scale is only 0.0044 in. (0.11 mm). But the same ±1° angular error on a 10 in. column face produces 0.175 in. (4.45 mm) of linear deviation at the top, which is almost certainly incompatible with assembly. Always ask: how far from the angular datum does this surface extend? If the answer is more than 2–3 in. (51–76 mm), either tighten the angular callout or replace it with a GD&T perpendicularity or parallelism control, which expresses the tolerance as a linear zone width and is more directly inspectable.
Surface Finish Guide
Surface finish is measured in Ra (roughness average) in microinches (µin) or micrometers (µm). Lower Ra values mean smoother surfaces - but cost scales accordingly.
| Finish | Ra Value | Process | Cost Impact | Best For |
|---|---|---|---|---|
| As-Machined | 125 Ra (3.2 µm) | Standard milling/turning | Baseline | Non-critical, internal parts |
| Fine Machined | 63 Ra (1.6 µm) | Reduced feed rate | +10–20% | External surfaces, housings |
| Very Fine | 32 Ra (0.8 µm) | Light finishing passes | +20–40% | Sealing surfaces, bearing seats |
| Ground | 16 Ra (0.4 µm) | Surface grinding | +50–100% | Precision fits, sliding surfaces |
| Lapped/Polished | 8 Ra (0.2 µm) | Lapping or polishing | +100–300% | Optical, medical, sealing |
Material-Specific Tolerances
Material properties directly impact achievable tolerances. Thermal expansion, hardness, machinability, and chip characteristics all play a role.
Aluminum 6061-T6
Excellent machinability, minimal tool wear. One of the most economical metals for tight tolerances.
Stainless Steel 304/316
Work-hardens during cutting. Requires slower speeds and rigid setup.
Carbon Steel 1018/1045
Good machinability. Leaded variants (12L14) machine even better.
Titanium Ti-6Al-4V
Low thermal conductivity causes heat buildup. Requires specialized tooling.
Brass C360
Free-machining. Excellent for precision components and threads.
Delrin (Acetal)
Excellent dimensional stability and low moisture absorption. One of the easiest plastics to machine to tight tolerances.
PEEK
High-performance plastic. Requires sharp tools and careful feeds.
GD&T Essentials
Geometric Dimensioning & Tolerancing (ASME Y14.5) goes beyond simple ± dimensions to control form, orientation, and location. Here are the most commonly specified callouts.
Flatness
How flat a surface must be, independent of any reference datum.
Parallelism
How parallel a surface or axis is relative to a datum plane.
Perpendicularity
How perpendicular a surface or axis is to a datum.
Cylindricity
Controls form of a cylindrical surface-roundness, straightness, and taper.
Concentricity
Median points of a feature must lie on the axis of a datum feature.
Position
Controls location of a feature relative to datums. Most commonly used GD&T callout.
When to Use GD&T
Use GD&T when parts must assemble with tight functional requirements - bearing bores, mounting faces, pin locations. For standalone parts without mating constraints, simple ± tolerances are usually sufficient and easier for the shop to inspect.
Why Tighter Tolerances Cost More: The Physics
Before you look at cost multipliers, understand what physically changes on the shop floor when you tighten a tolerance. Every item below adds time, risk, or secondary operations — and all of that converts directly to dollars.
Feed rate drops → cycle time increases
To hold ±0.001 in. instead of ±0.005 in., the CNC programmer reduces the finish-pass feed rate and depth of cut. A surface that takes one pass at ±0.005 in. may require 2–3 light passes at ±0.001 in. The tool is removing less material per revolution, so the spindle runs longer. On a 4-sided housing, going from ±0.005 in. to ±0.001 in. on all faces can increase cycle time by 40–80%. In metric terms, that is roughly the difference between 0.13 mm and 0.025 mm tolerance bands.
Tool deflection becomes the limit
Every cutting tool deflects under load. A standard end mill cutting 6061-T6 aluminum deflects approximately 0.0005–0.002 in. depending on stick-out length, diameter, and cutting force. At ±0.005 in. tolerance, this deflection is within the zone. At ±0.001 in., it is not. The programmer must use shorter, stiffer tools, reduce cut depth, or add a spring-pass (a final pass at zero additional depth that lets the tool "spring back" and clean up the deflection). Each of these strategies adds time. In metric terms, that is about 0.013–0.051 mm of deflection.
Thermal expansion matters at ±0.001 in. (±0.025 mm)
Aluminum 6061-T6 has a coefficient of thermal expansion (CTE) of 13.1 μin./in./°F (23.6 μm/m/°C). A 10 in. (254 mm) aluminum part that heats up 10°F (5.5°C) during machining grows by 0.0013 in. (0.033 mm), which is larger than a ±0.001 in. tolerance. At tight tolerances, the shop must manage coolant temperature, allow parts to thermally stabilize before inspection, and may need to specify inspection temperature (68°F / 20°C per ASME Y14.5).
Inspection time multiplies
At ±0.005 in., a machinist can verify most features with a caliper or micrometer in 30–60 seconds. At ±0.001 in., a CMM (coordinate measuring machine) is required, and each feature takes 1–3 minutes to probe, align, and report. A part with 20 toleranced features at ±0.001 in. may require 30–60 minutes of CMM time at $75–$150/hr. At ±0.005 in., the same part is inspected in 5 minutes with hand tools. In metric terms, that is about 0.13 mm versus 0.025 mm tolerances.
Scrap rate increases non-linearly
When the tolerance zone shrinks, the percentage of parts that fall outside the zone increases even if the process has not changed. A process with a standard deviation (sigma) of 0.002 in. produces ~99.7% yield at ±0.006 in. (3σ). The same process at ±0.002 in. (1σ) produces only ~68% yield, which means a 32% scrap rate. To maintain yield at tight tolerances, the shop must reduce process variation through better tooling, fixturing, and environmental control, all of which add cost. In metric terms, those bands are about 0.15 mm and 0.05 mm.
Secondary operations become mandatory
Standard CNC milling holds ±0.005 in. reliably. ±0.001 in. is achievable with careful setup. Below ±0.0005 in., the part typically leaves the CNC mill and moves to a secondary process: grinding (±0.0002 in.), honing (±0.0001 in. on bores), or lapping (±0.00005 in. on flat surfaces). Each secondary operation is a separate setup with its own machine, operator, and inspection cycle, doubling or tripling the number of operations on the part. In metric terms, that spans roughly 0.13 mm, 0.025 mm, 0.005 mm, 0.003 mm, and 0.001 mm bands.
The 80/20 rule for tolerances
On a well-designed part, roughly 80% of dimensions should use block tolerances (±0.005 in. or ±0.010 in.) and only 10–20% should carry tighter callouts (±0.001–±0.002 in.). If your drawing has tight tolerances on more than 30% of features, review each one and ask: “Does assembly or function actually require this?” The answer is usually no for at least half of them. In metric terms, that is about 0.13 mm / 0.25 mm block tolerances and 0.025–0.05 mm tight callouts. See the GD&T Guide for how to use position and form controls instead of stacked ± tolerances.
Cost Impact Analysis
Tolerance is the single largest cost driver in CNC machining after material choice. Understanding the cost curve helps you spec only what you need.
Slower Feeds & Speeds
Tighter tolerances require slower cutting speeds and lighter depths of cut, increasing cycle time by 2–5×.
Specialized Tooling
Precision work often requires carbide or diamond tooling, rigid tool holders, and more frequent tool changes.
Climate-Controlled Environment
Ultra-precision work (< ±0.001″) may require temperature-controlled rooms to prevent thermal expansion.
In-Process Inspection
CMM probing between operations adds time but ensures dimensions stay in spec. Critical for medical devices and precision robotics.
Higher Scrap Rate
Tighter specs mean more rejected parts. Scrap costs are passed through, especially for expensive materials like titanium.
Secondary Operations
Grinding, lapping, honing, and EDM may be needed for features beyond standard CNC capability.
Relative Cost by Tolerance
Actual pricing depends on material, geometry, quantity
Design Tips for Tolerances
Use bilateral tolerances
Specify ±0.005″ rather than +0.010/-0.000. Bilateral tolerances are easier to manufacture and inspect, and they center the nominal dimension.
Tolerance critical features only
Apply tight tolerances only to mating surfaces, bearing bores, sealing grooves, and assembly-critical dimensions. Let everything else float at ±0.005″.
Avoid tolerance stacking
When multiple features reference different datums, tolerances accumulate. Use a single datum scheme and GD&T position callouts to control critical relationships.
Match tolerance to process
Don't specify ±0.0005″ on a feature that can only be held to ±0.002″ with standard tooling. Consult your machinist early in the design phase.
Consider thermal effects
Aluminum expands ~13 µin/in/°F (23.6 µm/m/°C). A 12″ aluminum part heated 20°F changes by 0.003″. Specify inspection temperature (typically 68°F / 20°C) for precision work.
Provide complete drawings
Include GD&T callouts, surface finish symbols, material spec, and inspection notes. A clear drawing reduces quoting time and prevents misinterpretation.
Frequently Asked Questions
Related Resources
Need Parts with Precision Tolerances?
Upload your drawings to get engineer-reviewed pricing typically within one business day. Critical features as tight as ±0.0002″ can be reviewed with CMM inspection reports on request.
Get a CNC Quote