CNC machining tolerances set the allowable dimensional variation on every feature of a finished part. Knowing how to specify these tolerances correctly is one of the most important decisions you’ll make in a machining project.
Get tolerances right and your parts fit, function, and come back at a price that makes sense. Specify them thoughtfully and you’ll also avoid paying for precision where your design doesn’t need it.
This guide covers what CNC tolerances are, what standard ranges look like by process, what drives the cost of tighter specifications, and how to read your design and assign the right tolerance to the right feature.
We’ve built this guide from 20 years of DFM reviews and production runs at XTJ CNC, and the guidance applies whether you’re sourcing a single prototype or a high-volume production batch.
If you’d like a tolerance review on your current drawing, we’re happy to look at it before you place an order. Talk to our engineering team today.
CNC Machining Tolerance Quick Reference
The table below gives you a working reference for standard and tight tolerance ranges across common CNC processes. Use it as your starting benchmark before reading the process-by-process detail below.
| Process | Standard Tolerance | Tight Tolerance | Typical Application | Cost vs. Standard |
|---|---|---|---|---|
| CNC Milling | ±0.1 mm | ±0.003 mm | Enclosures, brackets, general parts | Baseline |
| CNC Turning | ±0.05 mm | ±0.003 mm | Shafts, bores, press fits | Moderate increase |
| 5-Axis Milling | ±0.01 mm | ±0.003 mm | Complex aerospace/medical geometry | Significant increase |
| Laser Cutting | ±0.1 mm | ±0.05 mm | Sheet metal profiles | Low |
| Reaming / Grinding | ±0.005 mm | ±0.001 mm | Bearing bores, precision fits | High |
Note: these ranges reflect typical capabilities under normal production conditions. Actual achievable tolerance depends on material, part geometry, feature type, and fixturing.
Standard, Tight, and Precision Tolerances at a Glance
Use this alongside the process table above to match your tolerance tier to the right machining approach and inspection method.
| Factor | Standard (±0.1 mm) | Tight to Precision (±0.003–0.05 mm) |
|---|---|---|
| Typical process | 3-axis milling, standard turning | Multi-pass milling, precision turning, reaming/grinding |
| Lead time impact | Minimal | Moderate – more setups, more inspection steps |
| Inspection method | In-process gauging | Precision instruments; CMM for the tightest features |
| Best applied to | Structural parts, clearance features, non-mating surfaces | Bearing fits, precision shafts, mating faces, locating features |
| When to use it | Any feature where assembly function doesn’t require more | Where fit class, assembly tolerance stack, or function demands it |
What Are CNC Machining Tolerances?
A CNC machining tolerance is the permitted dimensional variation on a finished feature. A dimension of 25.00 mm with a tolerance of ±0.05 mm means the feature can measure anywhere from 24.95 mm to 25.05 mm and still pass inspection. The machinist’s job is to keep the feature within that band consistently across every part in the run.
Tolerances exist because no machining process produces perfectly identical output every cycle. Cutting forces, spindle deflection, thermal expansion, and tool wear all introduce small variation. Understanding where that variation comes from helps you set tolerances that are realistic for the process, not just the design.
Treat tolerance as a boundary, not a precision target. For instance, a machinist aiming for 25.00 mm on a feature with a ±0.1 mm tolerance has plenty of room to work with high feed rates and efficient toolpaths.
If you were to tighten that same feature to ±0.005 mm, the entire production strategy changes: slower feeds, finer tools, more measurement steps, and less margin before a part is scrapped.
How Tolerances Appear on Technical Drawings
You’ll see CNC tolerances expressed in three ways on engineering drawings:
- Bilateral tolerances: variation is equal in both directions (e.g., ±0.05 mm). This is the most common form for general machining.
- Unilateral tolerances: variation is permitted in one direction only (e.g., +0.00 / −0.10 mm). Common on shaft diameters where the shaft must never exceed its nominal diameter.
- Limit dimensions: the drawing states the maximum and minimum values directly (e.g., 24.95–25.05 mm), removing any ambiguity about what’s acceptable.
When a drawing doesn’t specify individual feature tolerances, most machine shops default to a general tolerance standard. The ISO 2768 standard defines four general tolerance grades: fine (f), medium (m), coarse (c), and very coarse (v).
These tolerance grades apply across all unspecified linear and angular dimensions. ISO 2768-m (medium) is the most common default. If your drawing is silent on a feature, that’s likely what your supplier is holding.
Standard Machining Tolerances by Process
Each CNC process has a natural precision range built into its mechanics. Knowing where each process sits helps you match your tolerance requirements to the right manufacturing method from the start.
CNC Milling Tolerances
Standard 3-axis CNC milling reliably holds ±0.1 mm on most linear features under normal production conditions. For features that need more precision, tightening to ±0.025 mm is attainable with finishing passes and appropriate tooling. Features requiring ±0.005 mm or tighter will typically require multiple controlled finishing operations and CMM verification.
Complex parts with features on multiple faces require repositioning between setups, and each repositioning introduces small positional errors that accumulate across the part. 5-axis milling reduces the number of setups needed for that kind of geometry, which limits accumulated error even when individual feature tolerances aren’t extremely tight.
This is why aerospace and medical components with complex geometry often specify 5-axis machining, regardless of how tight the tolerances are.
CNC Turning Tolerances
CNC turning is more dimensionally consistent on cylindrical features compared to milling, because the cutting geometry is simpler and the workpiece rotates concentrically. Turned shafts and bores routinely hold ±0.025 mm in standard production. With precision tooling and controlled conditions, the number could go even lower (±0.005–0.010 mm) on finishing cuts.
One thing worth noting for turned parts: diameter tolerance and runout are independent specifications. A shaft can hit a tight diameter tolerance but still fail in a bearing assembly if runout isn’t controlled. Both should be explicitly specified on any precision rotating component.
Laser Cutting Tolerances
For sheet metal profiles, laser cutting typically holds ±0.1 mm. On qualifying features with optimized cut parameters and well-characterized material, ±0.05 mm is achievable. Laser cutting is the right process for sheet metal profiles and cutouts – not for features requiring ±0.01 mm or tighter, which would need secondary CNC machining operations.
Reaming and Grinding
When a bore or surface needs to go beyond what standard milling and turning can reliably deliver, reaming and grinding bridge the gap. Reaming a drilled or bored hole pushes tolerance from ±0.05 mm to ±0.005 mm with relatively modest added cost. Grinding reaches ±0.001–0.002 mm, which is the precision required for bearing-grade fits and high-speed rotating assemblies.
These operations add cycle time and cost, but they’re the correct engineering choice for the right features. The key is applying them selectively; only on features where assembly function genuinely requires that level of dimensional control.
What Drives the Cost of Tighter CNC Tolerances?
Tolerance cost is exponential as specifications tighten. Going from ±0.1 mm to ±0.05 mm on a straightforward feature might add 5–10% to machining cost. However, going from ±0.05 mm to ±0.005 mm on the same feature can add 50–100% or more. Understanding why helps you make smarter tradeoffs.
When a tolerance tightens, several things change simultaneously in the machining operation:
- Feed rates and depth of cut must decrease to reduce cutting forces and maintain dimensional consistency, adding cycle time directly.
- Tool selection shifts toward finer tools with tighter runout specifications, which cost more and wear faster.
- Fixturing requirements increase – the workpiece must be held with less flex to prevent deflection from registering as dimensional error.
- In-process measurement frequency rises. More stops for gauging and adjustment mean longer per-part time.
- Post-process inspection intensifies. CMM verification on tight-tolerance features adds cost, but is often required to document conformance.
- Scrap risk increases as the acceptable variation window narrows, which must be priced into the quote.
Material choice matters significantly here. Aluminum alloys machine cleanly and hold tight tolerances reliably, making them the most cost-efficient material for precision features. Stainless steel and titanium generate more cutting heat, deflect tooling more, and require more controlled conditions to hit the same tolerance spec – all at a higher cost.
Plastics and soft metals present different challenges: deflection under cutting forces and thermal expansion post-machining can shift final dimensions on tight-tolerance features.
The best way to keep machining costs controlled is to tighten tolerances only on the features that genuinely need it. Standard tolerances on non-critical features cost nothing extra and leave enough budget for the features that actually require precision.
How to Choose the Right Tolerance for Every Feature
The right tolerance comes from the function of each feature – not from convention and not from applying the same spec across the whole drawing. A three-step process makes this straightforward:
Step 1: Classify features by function
Start by dividing every significant dimension into two categories:
- Functional features: features that mate, align, locate, or seal against another part. These include shaft diameters, bore diameters, locating pin holes, mating faces, and sealing surfaces. These need explicitly specified tolerances matched to the assembly requirement.
- Non-functional features: outer profiles, clearance holes, non-mating surfaces, and cosmetic geometry. For these, ISO 2768-m or a general ±0.1 mm tolerance is usually appropriate and costs nothing extra.
Applying tight tolerances only to functional features and explicitly relaxing them on everything else is one of the most effective ways to reduce machining cost without touching your design intent. We regularly see parts where selectively relaxing non-functional tolerances reduces unit cost by 20–35%.
Step 2: Use fit class to set tolerances on mating features
For shaft-hole pairs and other mating features, the ISO system of limits and fits gives you a structured framework to work from. Rather than guessing at a tolerance number, you choose the fit class that matches your assembly’s behavior requirement:
- Clearance fit (e.g., H7/f7): the shaft is always smaller than the bore. Used for rotating shafts, sliding components, and any feature that needs to move freely.
- Transition fit (e.g., H7/k6): shaft and bore may overlap slightly depending on where each part lands in its tolerance range. Used for locating features that need accurate positioning with easy assembly.
- Interference fit (e.g., H7/p6): the shaft is always larger than the bore, requiring force or thermal expansion to assemble. Used for permanent or high-load fits.
Each fit class maps directly to tolerance ranges for both the shaft and bore, so you can read the required tolerance from a fits table rather than deriving it from scratch. This also makes your drawings unambiguous – a machinist reading H7/f7 knows exactly what to hold without interpretation.
Step 3: Match tolerance to process capability
Once you know what you need to hold, check that your specified tolerance sits comfortably within the process’s natural capability range. Don’t specify ±0.003 mm on a feature where ±0.015 mm will hold the assembly correctly; the tighter spec adds cost without adding function. Equally, don’t rely on a standard milling tolerance for a feature that needs a precision bearing fit.
If you’re unsure which process-tolerance pairing gives you the best cost-performance ratio for a specific feature, that’s a good question to put in your RFQ. Our engineering team is happy to advise during DFM review before your drawing is finalized.
Tolerance Stack-Up: Why Assembly Tolerances Need to Be Planned Together
Specifying tolerances feature by feature is necessary, but not sufficient for complex assemblies. Every individual tolerance adds variation. When multiple parts come together, their individual tolerances stack, and the cumulative variation at the assembly level can exceed what any single part tolerance would suggest.
A simple example: five parts in a linear assembly, each with a ±0.1 mm tolerance on the relevant dimension. In the worst case, where every part at the far edge of its tolerance is in the same direction, the assembly can be 0.5 mm off from nominal. That’s often acceptable for structural assemblies, but it can be a problem for precision mechanisms, optical systems, or anything with a tight fit at the assembled dimension.
Managing tolerance stack-up means analyzing the cumulative variation across the assembly before finalizing individual part tolerances. If the stack result is too large, you have two options: tighten tolerances on the parts that contribute most to the cumulative error, or redesign the assembly to reduce the number of stacking dimensions. Both are valid; the right choice depends on cost and design constraints.
For assemblies with tight stack-up requirements, we include tolerance analysis notes in our DFM review. This catches potential fitment issues at the drawing stage rather than at first article inspection.
How XTJ CNC Verifies Tolerances in Production
Specifying tolerances correctly is half the work. The other half is confirming they’ve been held – on every part, across every production run.
At XTJ CNC, our verification approach scales to the precision level required:
- Standard tolerances (±0.1 mm and above): calibrated in-process gauging and dimensional spot checks during production.
- Medium tolerances (±0.01–0.05 mm): precision instruments including micrometers, bore gauges, and dial indicators, with documented measurement records.
- Tight tolerances (±0.003–0.01 mm): CMM inspection, which captures 3D dimensional data across all specified features with full traceability.
Our ISO 9001 certification requires documented process control and inspection traceability on every order. For automotive-related work, we’re also IATF 16949 compliant. Clients like Magna, Shimadzu Medical, BEKO, and Electrolux have audited our quality systems against their own supplier standards – so you can be confident that our infrastructure for precision work is in place.
On high-precision first articles, we provide a First Article Inspection (FAI) report with measured values against every specified tolerance. That gives you a documented baseline for production validation and an auditable record for regulated industries.
Need CMM-verified parts with full inspection records? Request a quote and our team will confirm the right verification approach for your tolerances.
CNC Machining Tolerances FAQs
What is the standard tolerance for CNC machining?
The general default for CNC milling is ±0.1 mm; for CNC turning, it is ±0.05 mm. When no tolerance is specified on a drawing, most shops apply ISO 2768-m (medium grade). For features requiring more dimensional control, tolerances of ±0.01–0.025 mm are common in precision production, with ±0.003 mm achievable on dedicated precision operations.
What’s the tightest tolerance CNC machining can hold?
With precision tooling, controlled fixturing, and finishing operations, ±0.003 mm is achievable on qualifying features. This is the precision level we routinely hold for OEM clients in aerospace and medical applications. Grinding operations go tighter still, to ±0.001 mm, for bearing-grade components.
How does material affect which tolerance I can specify?
Harder, more dimensionally stable materials like tool steels and aluminum alloys hold tight tolerances more consistently. Softer or thermally sensitive materials are more prone to deflection during cutting and dimensional shift after machining. For tight-tolerance features in these materials, process parameters and fixturing have to be adjusted accordingly. If you’re designing in an unfamiliar material, it’s worth discussing tolerance feasibility before finalizing your drawing.
What is GD&T and when do I need it instead of linear tolerances?
GD&T controls form, orientation, location, and runout – conditions that bilateral linear tolerances can’t address. A bore can be the right diameter but positioned off-axis; a face can be within thickness tolerance but not flat. For complex assemblies, medical devices, and aerospace parts, GD&T is the right tool. For most standard machined components, bilateral linear tolerances are sufficient.
Back to Top: A Guide to CNC Machining Tolerances
