CNC Machining Tolerances & GD&T Guide: ISO 2768, Cost Impact, and Practical Design Rules

ISO 2768 General Tolerances for CNC

ISO 2768 is the international standard for general tolerances on linear and angular dimensions without individual tolerance callouts. It defines four classes — m (medium), f (fine), c (coarse), and v (very coarse) — applied by a default block on the drawing title sheet. Most precision CNC shops in the U.S. either follow ISO 2768-m or default to an in-house ±0.005 inch (±0.13 mm) linear tolerance when no standard is specified.

Values per ISO 2768-1:1989. Always place the callout "ISO 2768-m" or "ISO 2768-f" in the title-block tolerance block.

GD&T Basics for CNC Machined Parts

Geometric Dimensioning and Tolerancing (ASME Y14.5 / ISO 1101) defines the form, orientation, location, and runout of features relative to datums. On a CNC shop floor, GD&T callouts determine how the part is fixtured, which features are probed first, and how the CMM report is structured.

Datums (A, B, C)

Datums are theoretically exact planes, axes, or points that establish a coordinate frame. In CNC programming, the machinist physically creates this frame by probing or indicating the datum features during setup. A well-chosen datum strategy:

• Uses features machined in the same setup or an earlier operation to minimize stack-up.
• Aligns the primary datum face parallel to the machine table (3-point contact).
• Uses two perpendicular edges for the secondary and tertiary datums (2-point and 1-point contact).
• Avoids datums on thin, flexible, or non-machined surfaces that vary lot-to-lot.

True Position (Position Tolerance)

True position defines a cylindrical tolerance zone centered on the theoretically exact location of a hole, pin, or feature, relative to the specified datums. The tolerance value is prefixed with the diameter symbol (⌀) and is typically 1.5–3× the linear tolerance on each axis. For example, a hole located at 50 mm from Datum B and 30 mm from Datum C with a true position of ⌀0.15 mm means the actual hole center must fall within a 0.15 mm diameter circle around the theoretical center, not simply within ±0.075 mm on X and Y independently.

• • MMC modifier: When the tolerance is applied at Maximum Material Condition (Ⓜ), bonus tolerance is available as the feature departs from MMC. This makes inspection more forgiving and can reduce cost.
• • LMC modifier: Least Material Condition (Ⓛ) is used when minimum wall thickness or minimum clearance is the design driver.
• • Regardless of feature size (RFS): No bonus tolerance; the stated zone applies at all sizes. Most expensive to machine and inspect.

Perpendicularity, Parallelism, and Angularity

These orientation controls define how closely a surface, axis, or center plane aligns with a datum reference.

Standard Tolerance Bands in CNC Practice

The table below maps common tolerance callouts to what a precision CNC shop actually holds on a 3-axis or multi-axis mill, and on a CNC lathe with live tooling.

Relative cost assumes the feature is critical and must be verified. Non-critical features at tight tolerances may be quoted at medium-grade price if the shop is confident in process capability.

How Tolerance Choices Impact Machining Cost

Tolerance selection is the single largest cost driver a design engineer controls. The relationship is nonlinear: halving the tolerance roughly doubles the cost on that feature. The four cost mechanisms are machining time, tooling wear, fixturing complexity, and inspection rigor.

1. Machining Time

Tighter tolerances require lower feeds, smaller radial stepovers, and more finishing passes. A pocket milled at 0.250″ depth of cut and 40 ipm feed might slow to 0.050″ depth and 15 ipm when ±0.001″ wall position is required. On complex 3D surfaces, toolpath density increases and spindle time can triple.

2. Tooling and Tool Life

At tight tolerances, tool wear becomes a significant error source. A 0.375″ carbide end mill with 0.002″ flank wear may still hold ±0.005″ but will fail ±0.001″. Shops compensate by reducing tool life limits, using premium coated cutters (AlTiN, ZrN), or switching to solid-carbide micro-grain end mills — all of which raise tooling cost per part.

3. Fixturing

General vises and toe clamps hold ±0.005″ adequately. For ±0.001″ and tighter, shops invest in custom hard fixtures with precision locating pins, vacuum chucks for thin parts, or pallet systems that maintain sub-0.0005″ repeatability across batches. Custom fixture amortization is built into the per-part quote.

4. Inspection

At ±0.005″, a caliper or micrometer check is sufficient. At ±0.001″, features are typically CMM-verified on every setup and sampled per lot. At ±0.0005″, 100% CMM inspection is common, and each part may spend as much time in the inspection room as on the machine.

DFM Rules for Tolerancing CNC Parts

• Tolerance only what matters. Calling out ±0.001″ on a non-critical mounting ear forces the shop to slow down everywhere. Use title-block defaults for general features and local callouts only for mating surfaces, seal lands, and bearing bores.
• Use GD&T position with MMC where possible. A ⌀0.010″ true position at MMC allows bonus tolerance as the hole is drilled larger, making the part easier to machine and inspect without loosening the assembly fit.
• Avoid concentricity when runout or position will suffice. Concentricity inspects median points and is difficult and slow on a CMM. Total runout or position tolerance is usually functionally equivalent and much faster to verify.
• Design for one or two setups. Every additional setup introduces stack-up error. If perpendicularity of 0.05 mm is required between a face and a bore, machine both in the same clamping or on a tombstone with rigid pallet referencing.
• Match tolerances to the process. A 3-axis mill with a 0.250″ end mill cannot hold ±0.0005″ on a deep, thin wall — that is grinding territory. Talk to your machinist about process capability before freezing the drawing.
• Specify surface finish with tolerance. A 32 µin Ra finish on a bore that must also be ±0.0005″ on diameter will likely require a separate honing or lapping operation. Call out the finish only where it is functionally required.

Tolerance Stack-Up in Assemblies

When multiple machined parts mate, individual tolerances add statistically or worst-case. A common mistake is specifying ±0.001″ on every feature in an assembly of ten parts, producing an impossible overall fit.

• • Worst-case stack-up: Add all linear tolerances algebraically. If Part A is ±0.002″ and Part B is ±0.002″, the gap can vary by ±0.004″.
• • RSS (root-sum-square): For independent normal distributions, total variation ≈ √(t₁² + t₂² + … + tₙ²). Two ±0.002″ features stack to ±0.0028″ RSS — more realistic for production.
• • GD&T bonus tolerance: MMC modifiers effectively loosen the tolerance zone when the feature is not at its maximum material limit, improving assembly fit without loosening the drawing.

For critical assemblies, perform a tolerance analysis in CAD (e.g., CETOL, TolAnalyst, or manual spreadsheet) before releasing the drawing. Share the analysis with the CNC shop so they understand which features drive the assembly and which are cosmetic.

Inspection Methods by Tolerance Band

Related Resources

• • CNC Machining Surface Finish Guide — how Ra values and post-processes interact with tolerance bands.
• • How to Reduce CNC Machining Costs — tolerance selection as the primary DFM cost lever.
• • Precision CNC Machining — our shop capability overview and typical tolerance bands.
• • Quality Assurance & Inspection — CMM capabilities and first article inspection process.

Need Tolerance Guidance for Your Next Part?

Send your drawing to Olympus Machining and our CAM engineers will review tolerance feasibility, suggest GD&T callouts that reduce cost, and flag features that may require grinding or lapping instead of machining.