CNC Machining Tolerance Calculator

Compare machining routes with stored IT-width references, or screen routes against a target total width. Separate supplementary general tolerances show linear, radius, angle and geometry references. These planning references do not measure a shop’s process capability.

Machining reference lookup

An IT grade is a total width, not ± that value. Supplemental general-tolerance tables use this same entered length; run separate lookups when the radius, chamfer height, shorter angle leg or geometry evaluation length differs. Process references are planning guidance, not demonstrated capability.

What is CNC machining tolerance?

A machining tolerance defines the permitted variation of a feature from its specified size or geometry. For a size, tolerance width is the difference between the upper and lower size limits. The machining route alone does not define a hole or shaft fit, the location of an IT interval, or the manufacturer’s demonstrated repeatability.

Use the drawing’s explicit limits or its applicable general-tolerance class. Check the material, feature geometry, setup, measurement method and production conditions with the manufacturer.

IT width, ± deviation and process capability

Different outputs require different interpretations.
OutputMeaning and unitUse
Process IT referenceTotal size-width reference, in μm; 1,000 μm = 1 mmDo not put ± in front of a full IT width. Offset/fit position is not calculated here.
General linear ±tUpper deviation +t, lower deviation −t, total band 2tUse the chosen drawing class. Limits are nominal −t to nominal +t.
Angle / geometryAngles retain degrees and arcminutes; geometry values are unsigned zone widthsUse the correct evaluation length and datum. A zone width is not a symmetric ± size deviation.
Process capabilityObserved production distribution and its relationship to specification limitsRequires actual measurement data. It is not established by a permissible tolerance table.

Choose the right feature length

The current lookup uses one entered nominal dimension across supplementary tables. Those references are valid for different features only when the relevant input lengths are actually the same. Make separate runs for a radius, chamfer height, shorter angle leg, straightness/flatness evaluation length, perpendicularity shorter side or symmetry reference length.

Nominal size, shorter angle leg and geometric evaluation length are separate measurementsNominal linear sizeShorter angle legEvaluation lengthGeometry zone ≠ ± size

Three reproducible machining reference examples

These examples are generated from the same stored route and IT-width files as the calculator. They verify model consistency, not independently audited standard values or a production guarantee.

10 mm — Drill

Stored route IT11–IT13; total width reference 90–220 μm (0.09–0.22 mm). Stored roughness Ra 20 μm.

Solid voids for processing un quenched steel and cast iron can also be used for processing non-ferrous metals (with slightly lower surface roughness) • Hole diameter<(15-20) mm. Review the application note and drawing before selecting the route.

Recalculate this example

15 mm — Drill -> Reaming

Stored route IT8–IT9; total width reference 27–43 μm (0.027–0.043 mm). Stored roughness Ra 5.0-2.5 μm.

Solid voids for processing un quenched steel and cast iron can also be used for processing non-ferrous metals (with slightly lower surface roughness) • Hole diameter<(15-20) mm. Review the application note and drawing before selecting the route.

Recalculate this example

100 mm — Rough turning -> semi fine turning -> fine turning

Stored route IT6–IT7; total width reference 22–35 μm (0.022–0.035 mm). Stored roughness Ra 2.5-1.25 μm.

Suitable for various metals other than quenched steel. Review the application note and drawing before selecting the route.

Recalculate this example

For a separate linear-size example, the stored medium-class reference at 100 mm is ±0.3 mm: lower deviation −0.3 mm, upper +0.3 mm, total band 0.6 mm, limits 99.7–100.3 mm. This is separate from the process IT6–IT7 widths shown above.

When should a process be reviewed?

  1. Define the functional requirement and drawing limits before selecting a process route or general-tolerance class.
  2. Check whether a hole needs reaming, a turning route needs grinding, or the feature needs a different setup. Stored application notes are screening aids; material hardness, access and dimensions still matter.
  3. For tight tolerances, agree measurement uncertainty, datums, thermal conditions and sampling. Request actual capability evidence when production consistency is required.

Candidate route screening includes a route only if at least one stored width within its IT range is no larger than the requested total width at that nominal size. A route with missing tabulated grades is not assigned an invented tolerance value.

Sources, editions and maintenance

Numeric data: CPF’s existing jgfa.json, gc.json and wzgc1–6.json files. The general-table labels in the legacy tool identify GB/T 1804-2000 and GB/T 1184-1996. Original import provenance and complete transcription review are not recorded. Coarse dimensional class is stored under key “e” and displayed as “c (stored e)” for transparency. No named engineering reviewer is recorded.

For terminology and scope, see the ISO 2768-1:1989 catalogue and ISO 286-1:2010 preview. These references explain general-tolerance scope and the distinction between interval width and position. They do not establish that every CPF entry implements those editions. Use the drawing’s specified standard and licensed source for acceptance.

Model CPF-machining-2026-11-06; revised November 6, 2026. This release adds explicit output meanings, signed general-size limits, strict numeric validation, target-width screening, snapshots, sharing and printing. Existing numeric source tables were not changed.