CNC Machining Tolerance Standards Explained: ISO 2768, ASME Y14.5 & DIN 7168

Quick Answer: What Are CNC Machining Tolerance Standards?

Standard CNC machining tolerance is ±0.1mm (±0.004 inches) per ISO 2768-1 medium (Class m). Precision machining achieves ±0.05mm, and high-precision 5-axis CNC can hold ±0.01mm (±0.0004 inches) — thinner than a human hair. The specific achievable tolerance depends on material, part geometry, machine capability, and which international standard you reference.

This guide explains the three major tolerance standards (ISO 2768, ASME Y14.5, DIN 7168), what tolerances are actually achievable for different features, and how to specify tolerances on your drawing to get exactly what you need — without overpaying.

Why Tolerances Matter: A Real Story

A German medical device company sent us a surgical instrument handle with every single dimension toleranced at ±0.01mm. The part had 47 features. Their previous supplier had quoted €4,200 and 4 weeks.

We reviewed the design and asked: “Which 7 features actually need ±0.01mm?” The answer: the dowel pin holes for assembly alignment and the mounting face flatness. Everything else — grip texture, external contours, weight-reduction pockets — could be ±0.1mm.

New quote: €780. Timeline: 7 days. The parts assembled perfectly on the first try. This is the power of knowing which tolerances matter and which don’t.

The Three Major Tolerance Standards

1. ISO 2768-1: General Tolerances for Linear and Angular Dimensions

ISO 2768 is the most commonly referenced standard in international manufacturing. It defines four tolerance classes:

Class	Description	0.5-3mm	3-6mm	6-30mm	30-120mm	120-400mm
f (fine)	Precision applications	±0.05	±0.05	±0.1	±0.15	±0.2
m (medium)	General engineering	±0.1	±0.1	±0.2	±0.3	±0.4
c (coarse)	Low-precision parts	±0.2	±0.3	±0.5	±0.8	±1.2
v (very coarse)	Raw castings, weldments	—	±0.5	±1.0	±1.5	±2.5

Values in mm. Nominal size ranges shown across columns.

What this means in practice: If your drawing says “ISO 2768-m” without individual tolerances, every dimension automatically gets the medium-class tolerance. For a 50mm feature, that’s ±0.3mm — fine for clearance holes, too loose for bearing bores.

ISO 2768-2 covers geometrical tolerances (flatness, parallelism, perpendicularity) using tolerance classes H, K, and L. Most prototyping projects don’t need to specify these unless the part has critical assembly requirements.

2. ASME Y14.5: Geometric Dimensioning and Tolerancing (GD&T)

ASME Y14.5 is the North American standard and uses a fundamentally different approach: feature control frames instead of general tolerance tables. Key concepts:

• Basic dimensions: Theoretically exact dimensions (shown in a box). Tolerance comes from the feature control frame, not the dimension itself.
• Datum references: Surfaces or features that establish the coordinate system for measurement. Typically shown as A, B, C on the drawing.
• Geometric characteristics: Flatness, straightness, circularity, cylindricity, profile, position, concentricity, symmetry, runout.
• Material condition modifiers: MMC (Maximum Material Condition), LMC (Least Material Condition), RFS (Regardless of Feature Size).

Example: A feature control frame reading “⊥ | ∅0.05 | A” means “this surface must be perpendicular to datum A within a 0.05mm diameter tolerance zone.”

For prototyping, full ASME Y14.5 GD&T is usually overkill. However, understanding basic concepts helps communicate critical requirements clearly.

3. DIN 7168: The German Predecessor

DIN 7168 was the German general tolerance standard, now superseded by DIN EN ISO 2768. You will still see it referenced on older German drawings. The tolerance classes map closely to ISO 2768:

• DIN 7168 “fein” ≈ ISO 2768-f (fine)
• DIN 7168 “mittel” ≈ ISO 2768-m (medium)
• DIN 7168 “grob” ≈ ISO 2768-c (coarse)

Achievable Tolerances by Process and Feature

CNC Milling (3-axis)

• Linear dimensions: ±0.05mm standard, ±0.02mm achievable, ±0.01mm with extra care
• Bore diameter: H7 tolerance (+0.015/-0 for a 10mm bore) achievable with reaming
• Flatness: 0.02mm over 100mm x 100mm surface
• Parallelism: 0.03mm over 100mm
• Perpendicularity: 0.03mm over 100mm
• Surface finish: Ra 0.8-1.6μm as-machined, Ra 0.4μm with fine finishing cuts

CNC Milling (5-axis)

• Positional accuracy: ±0.01mm (eliminates re-fixturing errors from 3-axis)
• Angular accuracy: ±0.02° for indexed features
• Complex contours: ±0.03mm for simultaneous 5-axis toolpaths

CNC Turning

• Diameter: ±0.01mm achievable with finish pass
• Length: ±0.05mm standard
• Roundness: 0.005mm for ground finishes
• Concentricity: 0.02mm between turned diameters in one setup
• Surface finish: Ra 0.4-0.8μm achievable

3D Printing (SLA/SLS/DMLS)

• SLA: ±0.1mm for features under 100mm, ±0.1% for larger
• SLS: ±0.2mm typical, ±0.1mm achievable with process tuning
• DMLS/SLM (Metal): ±0.1-0.2mm, post-machining required for precision bores and threads
• FDM: ±0.3-0.5mm — not suitable for precision applications

Material Effects on Achievable Tolerance

The material you choose directly impacts achievable tolerances:

• Aluminum 6061/7075: Excellent machinability. ±0.01mm achievable. Minimal thermal expansion during machining.
• Stainless Steel 304/316: Work-hardens during machining. ±0.02mm practical minimum. Requires sharp tooling and correct speeds/feeds.
• Brass C360: Best machinability of all metals. ±0.01mm easily achieved. Ideal for high-precision small parts.
• PEEK, Ultem (plastics): ±0.05mm minimum. Plastics deform under clamping pressure and cutting forces. Stress-relief between roughing and finishing is critical.
• ABS, Nylon, POM: ±0.1mm practical minimum. Thermal expansion during machining can shift dimensions by 0.05-0.1mm.
• Titanium: ±0.03mm practical minimum. Low thermal conductivity causes heat buildup. Requires specialized tooling.

How to Specify Tolerances Correctly

1. Reference a standard on your drawing. Write “General tolerances per ISO 2768-m” in the title block. This covers all non-critical dimensions automatically.
2. Mark only critical dimensions. For each dimension that needs tighter control than the general standard, add the tolerance directly: “50 ±0.02” or “50 H7”. Typical critical dimensions: bearing bores, dowel pin holes, sealing surfaces, assembly interfaces.
3. Consider the entire tolerance stack. If three parts assemble in series and each has ±0.1mm, the total stack is ±0.3mm. Check that your assembly still functions at the worst-case combination.
4. Use GD&T only when needed. Position tolerance (⨁) for hole patterns. Profile tolerance (⌓) for complex surfaces. Perpendicularity (⊥) for mounting faces. Skip GD&T for simple parts — it adds cost without benefit.
5. Don’t tolerance cosmetic features. Grip textures, logo engravings, and non-functional external surfaces don’t need tight tolerances. Leave them at the general standard.

Common Tolerance Mistakes (and How to Avoid Them)

Mistake 1: Tolerancing Everything at ±0.01mm

Why it hurts: Drives up cost 3-5x because the machinist must take extra finishing passes on every feature, use premium tooling, and measure everything. The part may also fail QC on non-critical features.

Fix: ISO 2768-m general tolerance. Mark only 5-10 truly critical dimensions with specific tolerances.

Mistake 2: Ignoring Datum References

Why it hurts: Without datums, the inspector doesn’t know which surface to measure from. Two inspectors can get different results from the same part.

Fix: Mark three mutually perpendicular surfaces as Datum A, B, C. All critical dimensions reference these.

Mistake 3: Specifying Tighter Than the Process Allows

Why it hurts: Requesting ±0.005mm on an FDM 3D printed part is physically impossible. The supplier will either reject the job or deliver parts that fail inspection.

Fix: Match tolerances to the process. CNC: ±0.05mm standard. 3D printing: ±0.1-0.2mm. Sheet metal: ±0.2mm. Check with your supplier.

Mistake 4: Mismatched Standards

Why it hurts: Drawing says “ISO 2768-m” but notes reference ASME Y14.5 feature control frames. The two systems have different default rules and inspection methods.

Fix: Pick one standard. Use ISO 2768 for simple parts. Use ASME Y14.5 if your customer requires it. Don’t mix.

Quality Verification: How We Check Your Tolerances

• CMM (Coordinate Measuring Machine): Our Mitutoyo CMM measures with 0.001mm resolution. Used for all precision parts with tolerances ≤±0.05mm.
• Height gauge + surface plate: For larger parts that don’t fit the CMM. Accuracy: 0.01mm.
• Micrometers and calipers: Mitutoyo digital tools. 0.001mm resolution for micrometers, 0.01mm for calipers.
• Surface roughness tester: Mitutoyo Surftest. Measures Ra, Rz, Rq. Used when surface finish is specified.
• Thread gauges: Go/No-Go gauges for all standard threads (metric, UNC, UNF, BSP, NPT).

Every part ships with a dimensional inspection report covering all toleranced features. For medical and aerospace projects, we provide full FAI documentation per AS9102 or ISO 13485 requirements.

Frequently Asked Questions

What tolerance can I expect without specifying anything?

±0.1mm for CNC machined parts. This is our standard for non-critical dimensions and matches ISO 2768-m for features up to 30mm. If you need tighter control, specify it on the drawing.

Can you hold ±0.005mm tolerance?

On specific features, yes — but it requires grinding or EDM, adds 2-3 days and 50-100% cost. This level is typically only needed for bearing journals, seal surfaces, and precision locating features. Contact us before designing for this tolerance level.

What is the difference between ISO 2768 and ASME Y14.5?

ISO 2768 uses general tolerance tables: every dimension automatically gets a tolerance based on its size and the tolerance class. ASME Y14.5 uses feature control frames: each critical feature gets its own explicit tolerance specification. ISO is simpler for prototyping; ASME is more precise for complex assemblies.

Do 3D printed parts have the same tolerances as CNC?

No. 3D printing typically achieves ±0.1-0.2mm, while CNC achieves ±0.05mm standard. For precision bores, threads, and tight assembly fits, CNC machining or post-machining of 3D printed parts is recommended.

How does material affect tolerance?

Softer materials (aluminum, brass) machine more precisely than harder materials (stainless, titanium). Plastics are the most challenging because they deform under clamping pressure and expand with cutting heat. We can advise on achievable tolerances for your specific material during DFM review.

Get Your Tolerance Review

Upload your CAD file and our engineers will review the tolerances before manufacturing. We flag over-toleranced features, suggest cost-saving alternatives, and confirm what is achievable — all before you commit. This DFM review is free and typically takes less than 24 hours.