A CNC machining drawing is a contract between you and your manufacturer. When it’s clear, complete, and correctly toleranced, everything runs smoothly. When it’s ambiguous, over-constrained, or missing key callouts, you get late quotes, production delays, and parts that don’t work — even when the machining was technically correct.
This guide covers the practical mechanics of tolerancing a CNC machining drawing correctly: what to specify, where to apply tight tolerances, how to use GD&T effectively, and the mistakes that cost engineers the most time and money.
Start with Function, Not the Drawing
Before marking up any dimensions, ask one question for each feature: does the exact size and position of this feature matter to how the part works? If yes, it needs a tolerance callout. If no, let it ride on your drawing’s general tolerance block.
This function-first approach is the single best way to avoid over-tolerancing — one of the most common and expensive mistakes in CNC part design. Every unnecessarily tight tolerance adds cost: slower cutting speeds, more frequent measurement, higher setup time, and increased scrap risk. A well-toleranced drawing specifies tight tolerances only where function demands it.
The General Tolerance Block: Your Default Safety Net
Every machining drawing should have a general tolerance block — typically placed in the title block — that defines the default tolerance for any dimension not otherwise called out. A typical general tolerance block for CNC machining might read:
- Linear dimensions ±0.1mm (or ±0.005 inches)
- Angular dimensions ±0.5°
- Machined surface finish Ra 3.2μm unless otherwise noted
These are achievable on virtually any modern CNC machining center without special setup, which keeps your general machining cost low while giving the manufacturer clear expectations. Tighten individual features only when function requires it.
When to Apply Tight Tolerances (and When Not To)
Tight tolerances — typically ±0.025mm or finer — should be applied to:
- Mating surfaces and fits — any feature that interfaces with another part: bores, shafts, pins, and slots where clearance or interference fit matters
- Bearing seats — bore diameter tolerances for rolling element bearings follow ISO fit standards (typically H7 for housings, k6 or m6 for shafts)
- Sealing faces — surfaces that contact O-rings, gaskets, or mechanical seals require tight flatness and surface finish control
- Alignment features — datums, locating pins, and alignment bores that position assemblies
- Critical functional dimensions — anything that directly affects load path, fluid flow, electrical contact, or optical alignment
Tolerances should NOT be tightened on cosmetic surfaces with no mating function, non-critical hole positions where ±0.1mm of position variation is irrelevant to assembly, general wall thicknesses that don’t interface with other components, and fillet radii and chamfers where exact size has no functional consequence.
Using GD&T: The Right Controls for the Right Features
Geometric Dimensioning and Tolerancing (GD&T) — per ASME Y14.5 or ISO 1101 — gives you precise control over form, orientation, location, and runout that simple plus/minus tolerances can’t express. Key controls for CNC machined parts:
- True Position (⊕) — Controls the location of holes, slots, and features relative to datums. More functional than coordinate tolerances because it uses a cylindrical tolerance zone. Use for bolt pattern holes and precision-located features.
- Flatness (⏥) — Controls surface form without reference to a datum. Apply to sealing faces and precision mating surfaces where the surface itself must be flat regardless of overall part orientation.
- Perpendicularity (⊥) and Parallelism (∥) — Control the orientation of surfaces or axes relative to a datum. Use for bored holes that must be square to a reference surface, or parallel rails on a fixture.
- Runout (↗) and Total Runout (↗↗) — Control the variation of a surface as it rotates around a datum axis. Critical for rotating parts: shafts, spindles, and flanges.
- Cylindricity (⌭) — Controls the combined roundness and straightness of a bore or shaft. Apply to precision bearing bores where both form errors matter.
A common mistake is applying GD&T controls without thinking about how they’ll be measured. CMM measurement of true position is straightforward; total runout requires a rotary fixture. If you’re specifying GD&T on a tight-budget part, confirm with your supplier that they have the measurement capability before production starts.
Surface Finish Callouts
Surface roughness (Ra) is often underspecified on machining drawings — and then argued about at inspection. Default CNC milling produces Ra 1.6–3.2μm; turning typically achieves Ra 0.8–1.6μm. If a surface has specific requirements — sealing, wear, aesthetics, or contact — call it out explicitly.
Common Ra callouts for machined parts: Ra 3.2μm for general machined surfaces with no special requirements; Ra 1.6μm for bearing fits and light sealing surfaces; Ra 0.8μm for precision sealing faces and sliding surfaces; Ra 0.4μm and finer require grinding or honing post-machining and should only be specified when functionally necessary.
Datum Selection: Build Your Drawing on the Right Foundation
Datums are the reference points from which all other dimensions and tolerances are measured. Poor datum selection creates ambiguity and measurement disputes. Good datum practice for CNC machined parts:
- Choose datums that are also manufacturing references — surfaces that will be held in the vice or fixture during machining. This aligns the drawing’s measurement scheme with the physical machining setup.
- Use a primary datum (A) as the most functionally significant surface — typically the largest flat surface or the primary mounting face.
- Secondary (B) and tertiary (C) datums constrain the remaining degrees of freedom. For prismatic parts, three orthogonal datum planes are the standard starting point.
- For rotational parts, the datum axis established by the bore or shaft centerline is usually the primary datum, with a face as secondary.
Common Drawing Mistakes That Delay Your Order
Based on thousands of quote reviews, here are the drawing issues that most commonly cause delays, revision cycles, or production errors:
- Missing or undefined general tolerance block — manufacturers have to guess at default tolerances, or send back a clarification request.
- Over-constrained drawings — every surface toleranced to ±0.01mm means every surface requires CMM inspection, dramatically increasing cost and lead time.
- Inconsistent datum references — different views using different datums for the same feature create conflicting measurement requirements.
- Surface finish symbols without Ra values — a finish symbol means nothing without a number.
- No callout for threaded inserts, keyways, or special features — these must be explicitly dimensioned and toleranced.
- 3D model and 2D drawing conflicts — always resolve discrepancies before submitting; most manufacturers default to the 2D drawing unless otherwise instructed.
Let Us Review Before You Finalize
Our engineering team reviews every drawing submitted for a quote and proactively flags issues that could affect machinability, measurement, or cost — before the order goes into production. This includes tolerance concerns, datum configuration, DFM feedback on features that would be difficult or costly to machine as drawn, and suggestions for alternative approaches that could improve performance or reduce cost.
This review is free, comes with every quote, and typically takes less than 24 hours. It’s one of the concrete advantages of working directly with an engineering-capable manufacturer rather than a job shop that simply runs whatever drawing arrives.