CNC Machining Tolerances
A complete engineer's reference — IT grades, GD&T symbols, standard tolerances for turning and milling, surface finish specifications, and how to write drawings that get you first-time-right components from your CNC machining supplier.
CNC Machining Tolerances – A Complete Guide for Engineers: IT Grades, GD&T, Surface Finish & Drawing Best Practices
Tolerance specification is one of the most misunderstood aspects of engineering drawing — and one of the most consequential. Specify tolerances that are too loose, and components won't function correctly. Specify tolerances that are unnecessarily tight, and you'll pay 30–100% more per component for no functional benefit.
At RR Enterprises, our CNC machining team in Coimbatore processes hundreds of engineering drawings every month from clients across India, the Middle East, and Europe. Time and again, we see the same tolerance mistakes that inflate costs, cause inspection failures, and delay deliveries. This guide gives you everything you need to specify CNC machining tolerances correctly — from ISO IT grades and GD&T symbols through to surface finish Ra values and real-world cost implications.
Quick Reference: The most widely used general tolerance for CNC machined components is ISO 2768-m (medium). For most features without a specific callout, this means ±0.1mm for dimensions up to 30mm. Tighter tolerances should only be specified on features that are functionally critical — bearing fits, sealing surfaces, and mating interfaces.
What is a Machining Tolerance?
A machining tolerance defines the permissible variation from a nominal (target) dimension. If a shaft is specified as Ø25.00 ±0.02mm, the machinist may produce any diameter between 24.98mm and 25.02mm — a total tolerance band of 0.04mm.
Tolerances exist because no manufacturing process can produce a perfectly exact dimension — there will always be some variation due to machine wear, thermal expansion, tool deflection, and material properties. The engineering challenge is to specify tolerances that are tight enough for the component to function correctly, but wide enough to be economically manufactured.
There are two main types of tolerances used in CNC machining drawings:
- Linear (dimensional) tolerances — control the size of features: lengths, diameters, depths, and widths expressed as ± values or upper/lower limits
- Geometric tolerances (GD&T) — control the form, orientation, location, and runout of features, expressed using standardised symbols in a feature control frame
ISO IT Grades – The Tolerance Classification System
The ISO system of limits and fits (ISO 286) defines 20 standard tolerance grades — known as International Tolerance (IT) grades — ranging from IT01 (ultra-precision) to IT18 (coarse). Each IT grade defines a specific tolerance band for a given nominal dimension.
For CNC machined components, the practically achievable range is typically IT5 to IT12, depending on the operation, machine capability, and material:
Standard Tolerances – ISO 2768 Reference
ISO 2768 defines general tolerances for linear and angular dimensions of machined parts where individual tolerance callouts are not given on the drawing. It is divided into four classes: f (fine), m (medium), c (coarse), and v (very coarse). The most widely used class for precision CNC machining is ISO 2768-m.
| Nominal Dimension Range | ISO 2768-f (Fine) ±mm | ISO 2768-m (Medium) ±mm | ISO 2768-c (Coarse) ±mm |
|---|---|---|---|
| 0.5 – 3 mm | ±0.05 | ±0.1 | ±0.2 |
| 3 – 30 mm | ±0.05 | ±0.1 | ±0.3 |
| 30 – 120 mm | ±0.1 | ±0.2 | ±0.5 |
| 120 – 400 mm | ±0.15 | ±0.3 | ±0.8 |
| 400 – 1000 mm | ±0.2 | ±0.5 | ±1.2 |
| 1000 – 2000 mm | ±0.3 | ±0.8 | ±2.0 |
RR Enterprises Default Standard: Unless a specific tolerance or ISO class is stated on your drawing, RR Enterprises machines to ISO 2768-m as the default general tolerance. For tighter requirements, please specify ISO 2768-f or add explicit tolerance callouts on individual features.
GD&T – Geometric Dimensioning and Tolerancing
GD&T (Geometric Dimensioning and Tolerancing) is a standardised symbolic language — defined by ASME Y14.5 and ISO 1101 — that precisely communicates how a part must be manufactured and inspected. Unlike simple ± tolerances, GD&T controls the geometry of features: their form, orientation, location, and runout relative to a datum.
Using GD&T correctly on your engineering drawings means your CNC machinist, QC inspector, and design engineer all share exactly the same understanding of what "correct" means for each feature. This eliminates ambiguity, reduces inspection disputes, and enables proper functional tolerancing — which often means wider tolerances and lower cost.
The 14 Core GD&T Symbols You Need to Know
Need Precision CNC Machining?
RR Enterprises machines to ±0.005mm and inspects with CMM. Send your drawings for a detailed, no-obligation quote — response within 24 hours.
Hole and Shaft Fits – H7/g6, H7/k6 and Beyond
When a shaft fits inside a bore, the relationship between the two dimensions — their fit — must be precisely controlled. ISO 286 defines a system of standardised fits using letter codes for the deviation (position of the tolerance band) and number codes for the tolerance magnitude (IT grade).
| Fit Type | Common Designation | Clearance / Interference | Typical Application |
|---|---|---|---|
| Loose running | H11/c11 | Large clearance | Exposed parts, loose linkages, wide thermal range |
| Easy running | H9/d9 | Clearance | Lightly loaded bearings, non-precision sliding fits |
| Close running | H8/f7 | Small clearance | General purpose rotating shafts, journal bearings |
| Sliding | H7/g6 | Minimal clearance | Precision sliding components, locating pins |
| Location clearance | H7/h6 | Zero to small clearance | Precision location, separable assemblies |
| Location transition | H7/k6 | Zero to small interference | Precise location with light press — gears, couplings |
| Location interference | H7/p6 | Interference | Semi-permanent assemblies, light press fits |
| Force / press fit | H7/s6 | Heavy interference | Permanent assemblies — permanent gear and hub fits |
Practical Note: Always specify the fit designation (H7/g6) on your drawing rather than calculating the actual tolerance values manually. This tells the machinist exactly which ISO system deviation and IT grade to apply to both the bore and the shaft — and it allows CMM inspection to verify the fit class directly.
Surface Finish – Ra, Rz, and What to Specify
Surface finish is the measure of the microscopic texture of a machined surface. The most commonly specified parameter is Ra (arithmetic mean roughness) — the average deviation of the surface profile from the mean line, measured in micrometres (μm).
| CNC Process | Typical Ra (μm) | Equivalent N Grade | Appearance |
|---|---|---|---|
| Rough turning / milling | Ra 6.3 – 12.5 | N9 – N10 | Clearly visible tool marks |
| Standard CNC turning | Ra 1.6 – 3.2 | N7 – N8 | Slight tool marks, smooth to touch |
| Fine CNC turning / boring | Ra 0.8 – 1.6 | N6 – N7 | Smooth, barely visible marks |
| CNC milling (standard) | Ra 1.6 – 3.2 | N7 – N8 | Slight cutter marks visible |
| CNC milling (fine / ball nose) | Ra 0.8 – 1.6 | N6 – N7 | Smooth with fine step pattern |
| Cylindrical grinding | Ra 0.2 – 0.8 | N5 – N6 | Very smooth, mirror-like |
| Honing | Ra 0.1 – 0.4 | N4 – N5 | Crosshatch pattern, excellent bearing surface |
| Lapping / superfinishing | Ra 0.025 – 0.1 | N2 – N4 | Mirror finish, optical quality |
Cost Tip: Moving from Ra 3.2 to Ra 0.8 typically adds 20–40% to machining cost due to additional operations, finer tooling, and slower feed rates. Moving to Ra 0.4 or below usually requires grinding — adding significant cost and lead time. Only specify fine surface finishes on sealing surfaces, bearing interfaces, and fluid-carrying bores where it is functionally necessary.
Tolerance Capabilities by CNC Operation
Different CNC machining operations have different inherent precision capabilities. Understanding these helps you route features to the right operation and set realistic expectations for achievable tolerances:
CNC Turning
Diameter tolerances of ±0.01mm routinely achievable. Fine turning reaches ±0.005mm. Length tolerances ±0.05mm standard, ±0.02mm fine.
CNC Milling
Linear dimensions to ±0.02mm routinely. Profile tolerances to ±0.05mm standard. Fine milling with high-speed spindle reaches ±0.01mm.
CNC Drilling
Hole position to ±0.05mm standard. Hole diameter ±0.05mm for twist drill, ±0.02mm for reamed holes. Bore diameter to ±0.01mm.
Thread Milling
M, UNC, UNF, BSP, BSPT threads to tolerance class 6H / 6g as standard. Fine class 5H / 5g available on request for precision thread fits.
How Tolerances Affect CNC Machining Cost
One of the most important — and least discussed — aspects of tolerance specification is its direct impact on component cost. Tighter tolerances mean more machining passes, slower cutting conditions, finer tooling, and more intensive inspection. Here is a realistic cost impact guide:
| Tolerance Level | Typical Tolerance | Cost Premium | Why It Costs More |
|---|---|---|---|
| General (ISO 2768-m) | ±0.1 – ±0.3mm | Base cost | Standard cutting conditions, spot checks |
| Fine (ISO 2768-f) | ±0.05 – ±0.1mm | +10–20% | Extra finishing pass, more frequent gauging |
| Precision | ±0.02 – ±0.05mm | +30–60% | Fine tooling, temperature-controlled machining, 100% inspection |
| High Precision | ±0.005 – ±0.02mm | +60–120% | Specialist machines, CMM inspection every piece, grinding |
| Ultra Precision | ±0.001 – ±0.005mm | +150%+ | Grinding + lapping, temperature-controlled environment, 100% CMM |
Common Tolerance Mistakes – And How to Avoid Them
In reviewing drawings from clients across India, the Middle East, and Europe, these are the tolerance specification mistakes we encounter most frequently:
Mistake: Over-tolerancing Every Dimension
Specifying ±0.01mm across an entire drawing — including non-functional dimensions like overall lengths and fillet radii — dramatically inflates cost with no functional benefit.
- Only functionally critical features need tight tolerances
- Use a general tolerance block (ISO 2768-m) and add specific callouts only where needed
Better Practice
Use ISO 2768-m as the general tolerance for the drawing, and explicitly specify tighter tolerances only on bearing seats, bore diameters, mating interfaces, and sealing surfaces.
- Result: 30–60% lower cost on typical components
- Faster production — no unnecessary precision operations on non-critical features
Mistake: Missing Datum References in GD&T
Specifying a true position or perpendicularity callout without a datum reference leaves the machinist and inspector uncertain about what the measurement is relative to — making proper inspection impossible.
Better Practice
Always define at least a primary datum (A), and secondary and tertiary datums (B, C) where needed to fully constrain the feature in space. Choose datums that are the functional mounting or mating surfaces — not convenience surfaces.
Mistake: No Surface Finish Callout
Leaving surface finish unspecified means the machinist applies the process's natural finish — which may be far rougher (Ra 6.3μm) than required for a sealing face or bearing bore (Ra 0.8μm).
Better Practice
Add a general surface finish requirement in the drawing title block (e.g., "all machined surfaces Ra 3.2 μm unless noted") and add specific Ra callouts directly on critical surfaces using the standard surface texture symbol.
Mistake: Specifying Concentricity for Runout
Concentricity requires a complex centroid-to-centroid measurement that is extremely difficult to verify with CMM. For most rotating applications, total runout (or circular runout) is the correct callout — it's easier to measure and functionally equivalent.
Better Practice
Use total runout for rotating shafts and bores where the axis must align with a datum axis. Reserve concentricity only where the centroid location (not runout) truly matters — which is extremely rare in practice.
Drawing Submission Checklist – Get Your Quote Right First Time
When submitting drawings to RR Enterprises for a CNC machining quote, following this checklist ensures we can provide an accurate, competitive price without back-and-forth clarifications:
General Tolerance Block
State the applicable general tolerance standard in the drawing title block — e.g., ISO 2768-m or ASME Y14.5M-2018. This sets the default for all unspecified dimensions and eliminates the most common source of drawing ambiguity.
Material Specification
Specify the exact material grade — not just "aluminium" or "stainless steel". Write Al6061-T6 or SS316L or EN19 (AISI 4140). Material affects cutting conditions, achievable tolerances, surface finish, and price significantly.
Critical Dimension Callouts
Add explicit tolerance callouts on all functionally critical features — bore diameters, shaft diameters, mating surfaces, hole positions, and thread specifications. Use limit dimensions or ± values. Add GD&T callouts for form, orientation, and location where ± alone is insufficient.
Surface Finish Specification
Add a general surface finish requirement to the title block and specific Ra callouts on critical surfaces. Specify which surfaces require a particular finish — sealing faces, bearing bores, mating flanges. If anodising, plating, or coating is required, state this clearly.
Thread Specifications
Specify thread form (M, UNC, UNF, BSP, BSPT), nominal diameter, pitch, tolerance class (e.g., M12×1.5 – 6H), depth, and whether through or blind. For tapered pipe threads, specify the standard (ISO 7 or ASME B1.20.1).
Heat Treatment & Hardness
If hardening, tempering, case hardening, or annealing is required — state the process, required hardness (HRC, HRB, or HV), and whether dimensional inspection must occur before or after heat treatment (critical for tight-tolerance bores).
RR Enterprises DFM Service: Send us your drawings before finalising them — our engineering team provides free Design for Manufacturability (DFM) feedback. We'll flag any tolerance specifications that will significantly increase cost, suggest equivalent functionally compliant alternatives, and ensure your drawing will produce exactly the component you need at the most competitive price.
RR Enterprises CNC Machining Tolerance Capabilities
Our Coimbatore facility is equipped to machine components across a wide range of tolerance and complexity levels — from general engineering components to tight-tolerance precision parts for automotive, aerospace, and pharmaceutical applications:
| Capability | Specification |
|---|---|
| CNC Turning – Diameter Tolerance | ±0.005mm (finest) | ±0.01mm (standard precision) |
| CNC Milling – Linear Tolerance | ±0.01mm (finest) | ±0.02mm (standard precision) |
| Hole Position (True Position) | ±0.02mm from datum |
| Surface Finish – Turning | Ra 0.8 μm (fine) | Ra 1.6 μm (standard) |
| Surface Finish – Milling | Ra 0.8 μm (fine) | Ra 1.6 μm (standard) |
| Roundness / Circularity | 0.005mm (fine turning) |
| Cylindricity | 0.008mm over 100mm length |
| Perpendicularity | 0.02mm / 100mm |
| Thread Tolerance Class | 6H / 6g standard | 5H / 5g fine |
| Inspection Method | CMM (Coordinate Measuring Machine), vernier, micrometers, thread gauges, height gauges |
| Materials Machined | Aluminium alloys, SS304/316/316L, Carbon steel, Alloy steel, Brass, Copper, Engineering plastics |
Frequently Asked Questions
The most commonly applied general tolerance is ISO 2768-m (medium), which gives ±0.1mm for dimensions up to 30mm and ±0.2mm for dimensions up to 120mm. For dimensions with specific tolerance requirements, values of ±0.05mm are standard fine-precision, and ±0.01mm or tighter requires precision-grade machining with CMM inspection.
GD&T (Geometric Dimensioning and Tolerancing) is a standardised engineering language that uses symbols to precisely define the allowable variation in form, orientation, location, and runout of features. It matters because ± tolerances alone cannot fully describe the functional requirements of many features — GD&T closes this gap by controlling geometry in addition to size, ensuring the machinist, inspector, and designer all share the same understanding of what constitutes a conforming part.
RR Enterprises consistently achieves ±0.005mm (5 microns) on critical diameter features in CNC turning, and ±0.01mm on milled features. For applications requiring tighter tolerances, we can discuss grinding operations and specialist machining approaches. All tight-tolerance components are 100% CMM inspected with a full dimensional report.
Yes — significantly. Moving from general tolerance (±0.1mm) to precision tolerance (±0.02mm) typically adds 30–60% to component cost. Tolerances of ±0.005mm or tighter can add 100% or more. This is because tighter tolerances require slower cutting speeds, additional finishing passes, specialist tooling, and 100% dimensional inspection. We always advise clients to specify tight tolerances only on features that are functionally critical.
Use the standard surface texture symbol (a check mark with a horizontal bar) and write the Ra value above the symbol — e.g., Ra 1.6. Add a general surface finish requirement in the title block for all unspecified surfaces (e.g., "all machined surfaces Ra 3.2 unless noted"). For critical surfaces like sealing faces or bearing bores, add specific Ra callouts directly on those surfaces in the drawing views.
Ready to Get Your Components Made?
Send RR Enterprises your drawings — we'll provide a free DFM review, highlight any tolerance issues, and deliver a competitive quote for precision CNC machining from Coimbatore.
Related Articles
