---
title: "How to Specify Tolerances Without Overpaying"
description: "Set a general tolerance, tighten only the features that function, use fits and GD&T where a ± falls short, and put tolerances in an RFQ the right way."
canonical: https://openspindle.com/blog/how-to-specify-tolerances
author: "Tom"
datePublished: 2026-09-16T00:00:00.000Z
dateModified: 2026-09-16T00:00:00.000Z
category: "Process & DFM"
---

# How to Specify Tolerances Without Overpaying

Specify tolerances in two layers: a general tolerance, such as ISO 2768-m or a decimal-place block, that covers every dimension, and individual tolerances only on features that function, like mating bores, locating holes and sealing faces. Tight tolerances cost more through slower cutting, extra setups, inspection and scrap. In an OpenSpindle RFQ, pick the Tolerance under Advanced options that describes most of the part, choose the tightest band if any feature is tighter, and name those features on your drawing or in the part Note.

## What a general tolerance is, and why every drawing needs one

A general tolerance is the tolerance that applies to every dimension on a drawing that does not carry its own. It usually lives in the title block or a general note, and it is the single line that keeps a drawing from being ambiguous. Without it, a dimension of 50 mm has no stated limits, and a shop has to guess, ask, or quote to its own internal default.

The general tolerance is also the cheapest tolerance on the drawing, by design. It should be loose enough that normal shop practice meets it without extra effort, so that only the dimensions you deliberately call out drive cost.

Metric drawings commonly reference ISO 2768-1, which sets linear and angular limits in four classes: fine (f), medium (m), coarse (c) and very coarse (v). The limit scales with the size of the dimension, so a 10 mm feature at medium gets ±0.2 mm while a 200 mm feature gets ±0.5 mm. ISO 2768-2 adds general geometric tolerances (classes H, K and L) for flatness, straightness, perpendicularity and similar controls, which is why you often see a callout like ISO 2768-mK. The full tables are in the [CNC machining tolerance chart](/reference/cnc-machining-tolerance-chart).

Inch drawings more often use a decimal-place block, where the number of decimal places written on a dimension selects its tolerance. The values below are a common convention, not a standard. Companies set their own blocks, so read the title block on each drawing rather than assuming.

| System | How it reads | Typical example | Notes |
| --- | --- | --- | --- |
| ISO 2768-1 (metric) | Tolerance class stated once in the title block | ISO 2768-m: ±0.1 mm (over 3 to 6 mm), ±0.2 mm (over 6 to 30 mm), ±0.3 mm (over 30 to 120 mm) | Limits grow with nominal size. Medium is the most common default for machined parts |
| ISO 2768-2 (metric, geometric) | Letter class added after the linear class | ISO 2768-mK | Covers general flatness, straightness, perpendicularity, symmetry and runout |
| Decimal-place block (inch) | Precision written on the dimension selects the tolerance | .X ±.1, .XX ±.01, .XXX ±.005, angles ±1/2° | A widespread convention only. Many companies publish their own values |
| Explicit general note | One tolerance for everything not called out | UNLESS OTHERWISE SPECIFIED: ±0.25 mm | Simple, but a single value is too tight for large features or too loose for small ones |

## Why tight tolerances cost more

A tolerance is a promise the shop has to keep on every part, and then prove. Tightening it changes how the part is made and how it is checked, and both show up in the quote.

**Slower cutting and finishing passes.** Holding a tight size usually means a roughing pass, a pause for the part to relax, and a light finishing pass at lower feeds. That is more spindle time per feature.

**More setups and better fixturing.** Every time a part is unclamped and flipped, a little location error creeps in. Tight relationships between features on different faces can force a fixture, a 5-axis setup, or extra indicating time.

**Temperature.** Metal grows as it warms. Aluminum expands roughly 23 µm per meter per °C, so on a 150 mm aluminum part a few degrees of difference between a warm part and a cool inspection room can move a dimension by around 0.01 mm. At tenths of a thousandth, the shop has to control that.

**Inspection time and equipment.** Calipers are fine at ±0.13 mm. Tighter bands need micrometers, bore gauges, pin gauges, or a coordinate measuring machine (CMM), plus the time to program and run it.

**Scrap.** The narrower the band, the more parts fall outside it, and the cost of those parts is spread across the good ones.

None of these scale neatly, and the price effect depends on the part, the material and the shop. The pattern below is a qualitative guide to what each band typically asks for. For a view of how cost climbs band by band, see the table in [tolerance stack-up](/blog/tolerance-stack-up).

| Tolerance band | Typical method | Typical inspection |
| --- | --- | --- |
| ±0.010 in (±0.25 mm) | Standard milling or turning, no special steps | Calipers, spot checks |
| ±0.005 in (±0.13 mm) | Normal CNC practice for most features | Calipers and micrometers, sampling |
| ±0.002 in (±0.05 mm) | Finishing passes, more careful setups | Micrometers, bore or pin gauges, more frequent checks |
| ±0.001 in (±0.025 mm) | Finishing passes at reduced feeds, reaming or boring, attention to temperature | Gauges on critical features, often CMM |
| ±0.0005 in (±0.013 mm) and tighter | Grinding, honing or lapping, controlled environment | CMM or dedicated gauging, often 100% inspection of the feature |

## Tolerance only the features that function

The most effective way to cut a machining quote is to leave most of the part at the general tolerance. On a typical housing or bracket, only a handful of features touch another part in a way that matters.

Those are the features worth a tolerance:

**Mating bores and shafts.** A bearing seat, a bushing bore, a shaft diameter that slides or presses into something.

**Locating features.** Dowel pin holes, register diameters and shoulders that set where one part sits relative to another.

**Sealing faces.** Gland grooves for O-rings and flat faces that close against a gasket, where flatness and surface finish decide whether the joint leaks.

**Hole patterns that bolt to something else.** Here the relationship between holes usually matters more than any single hole size.

Everything else can float. Outside profiles, pockets that save weight, chamfers, clearance holes and cosmetic faces rarely need more than the title block. A drawing where every dimension carries a tight tolerance tells a shop you have not decided what matters, and shops tend to quote that uncertainty defensively.

If you do not know which features are critical, the answer usually comes from the mating parts. Work through the assembly and ask, for each feature, what happens if it is 0.25 mm off. If the answer is nothing, it does not need a callout. A [tolerance stack-up](/blog/tolerance-stack-up) makes that question rigorous for assemblies with several contributors.

## When a ± is the wrong tool: fits and GD&T

Plus-or-minus tolerances work well for sizes. They work poorly for relationships between features, and they are an awkward way to describe how two parts go together.

For a hole and shaft that assemble, a standard fit is clearer than two separate ± values. An ISO 286 designation such as H7/g6 (sliding) or H7/p6 (press fit) tells the shop exactly what limits to hold on each part and tells an inspector exactly what to gauge. The [engineering fits chart](/reference/engineering-fits-chart) lists the common hole-basis fits and what each is for.

For location, form and orientation, GD&T is usually the better tool. A position tolerance on a bolt pattern creates a round tolerance zone instead of the square zone implied by ± coordinates, which accepts more good parts at the same functional accuracy. Flatness controls a sealing face directly, where a ± on thickness does not stop the face from being warped. The [GD&T symbols reference](/reference/gdt-symbols-reference) covers the full set.

| Requirement | ± tolerance approach | Better callout | Why it helps |
| --- | --- | --- | --- |
| Bearing or bushing bore | Ø22.000 ±0.010 | Ø22 H7 | Standard limits, standard gauges, and the mating part can be specified to match |
| Dowel pin hole | Ø6.00 ±0.01 | Ø6 H7, located with a position tolerance | Controls size and location separately |
| Bolt hole pattern | ±0.05 on each X and Y coordinate | Position Ø0.1 relative to datums | Round zone accepts about 57% more area than the equivalent square zone |
| Gasket or O-ring face | ±0.05 on part thickness | Flatness 0.05 plus a surface roughness callout | A thickness tolerance does not control warp |
| Shaft running in two bores | Separate ± on each bore diameter | Coaxiality or runout to a common datum | States the alignment that matters directly |

## Match the tolerance to the process

A tolerance only makes sense if the process chosen can hold it. The ±0.005 in machining standard is a reasonable default for a CNC part and an unreasonable demand on many other processes, and applying it everywhere is a common cause of no-quotes and long clarification threads.

Laser, waterjet and plasma cut parts are generally looser than machined ones, and cut edges can show taper, especially on waterjet and plasma in thicker plate. Bent sheet metal adds bend angle variation and the accumulated error of each bend on flange dimensions. 3D printing and injection molding are driven by shrinkage and warpage, so their tolerances are usually expressed as a percentage of size as well as a fixed amount. See the [3D printing tolerance chart](/reference/3d-printing-tolerance-chart) and the [injection molding tolerance chart](/reference/injection-molding-tolerance-chart) for typical values by process.

When one feature needs more accuracy than the process delivers, the usual answer is a secondary machining operation on that feature only, for example reaming a hole in a laser cut plate or machining a bearing bore in a metal printed part. That is often cheaper than switching the whole part to machining.

| Process | Typical general tolerance (rule of thumb) | Where tighter work is possible |
| --- | --- | --- |
| CNC machining | ±0.005 in (±0.13 mm) | Critical features to ±0.001 in or tighter with finishing and inspection |
| Laser cutting (sheet) | Roughly ±0.005 to ±0.010 in (±0.13 to ±0.25 mm), depends on thickness | Thin material on a well tuned fiber laser |
| Waterjet cutting | Roughly ±0.005 to ±0.015 in (±0.13 to ±0.38 mm), plus edge taper in thick plate | Taper compensating heads, slower cutting speeds |
| Plasma cutting | Looser, often ±0.020 in (±0.5 mm) or more | High definition plasma, or machining after cutting |
| Bent sheet metal | Around ±0.010 in (±0.25 mm) per bend, bend angles around ±1° | Fewer bends between critical features, formed then machined features |
| 3D printing | ±0.1 to ±0.5 mm depending on process, often with a % of size | Metal parts finish machined on critical features |
| Injection molding | About ±0.10 mm on small features, looser as size grows | Small features in low shrink resins with a tuned tool |

## Finishes and coatings change dimensions

A tolerance applies to the finished part unless the drawing says otherwise, and most coatings add material. A bore held to H7 before anodizing can end up undersize after it, and a thread can stop accepting a screw.

Anodizing grows the part as well as converting the surface. As a rule of thumb, roughly half of the anodic layer builds up above the original surface and half penetrates into it, so a diameter changes by about the full coating thickness (half on each side). Plating and powder coating sit entirely on top of the surface, so a diameter grows by twice the coating thickness. The [anodizing spec](/reference/anodizing-spec) lists typical thicknesses by type.

The fixes are simple and belong on the drawing: say whether a dimension applies before or after finish, mask tight bores, threads and mating faces, or ask the shop to machine critical features to allow for the coating.

| Finish | Typical thickness | Effect on a diameter | Common approach on tight features |
| --- | --- | --- | --- |
| Type II anodize | 5 to 25 µm (0.0002 to 0.001 in) | Grows by roughly the coating thickness | Often acceptable at ±0.13 mm, mask H7 bores |
| Type III hardcoat anodize | 25 to 100 µm (0.001 to 0.004 in) | Grows by roughly the coating thickness, which can exceed a tight band | Machine undersize to allow for growth, or mask |
| Zinc or nickel plating | Commonly 5 to 25 µm per surface | Grows by about twice the thickness | Mask threads and bores, or specify dimensions after plating |
| Powder coating | Commonly 50 to 100 µm or more per surface | Too thick for precision fits | Mask or plug all mating features |
| Bead blasting | Removes little material but changes texture | Negligible on size, affects surface roughness | Mask sealing faces |

## What a tight tolerance means for inspection

Every tolerance on a drawing is a measurement someone has to make. A shop quoting a part will look at which callouts it can check with hand tools and which need something more, and price the difference.

Features in the thousandths usually need gauges or a CMM, especially GD&T callouts such as position and profile, which are measured relative to datums rather than with a caliper. A CMM program takes time to write, and each part takes time to run.

If you need proof that the first parts meet the drawing, ask for a [first article inspection](/blog/first-article-inspection) (FAI) report, which measures every characteristic on an initial part. On production runs, you may also want ongoing inspection of critical features, and [process capability (Cpk)](/blog/process-capability-cpk) is how a shop shows it can hold a tolerance consistently. Both add cost, so request them where the part needs them, and mark the characteristics that matter so the report focuses there.

A useful habit: flag critical dimensions on the drawing with a note or a symbol your team defines, such as a balloon or a CD label. It tells the shop where to spend inspection effort and where it can use lighter checks.

## Adding tolerances to your OpenSpindle RFQ

The quote form captures tolerance at the part level, so it helps to know how it works before you choose. The **"Tolerance"** field sits under **"Advanced options"** on each part card. It takes one value per part, and the form does not warn you when a tighter choice is likely to raise the price. The detail of which features are critical has to come from your drawing or the part note.

**Step 1: Set the process first.** Choose the right **"Process"** for each part. The form suggests a process from the file type, so check it: a flat laser or waterjet part should be set to "Sheet Cutting" and a bent part to "Sheet Metal". The tolerance options depend on the process.

**Step 2: Pick the band that describes most of the part.** For CNC parts, open **"Advanced options"** and choose from **"General (±0.010″ / ±0.25 mm)"**, **"Standard (±0.005″ / ±0.13 mm)"**, **"Tighter than ±0.005″ (±0.13 mm)"** or **"Not sure, shop to advise"**. Standard is the default and suits most machined parts. General is a good choice for brackets and non-mating parts.

**Step 3: If any feature is tighter, say so and say which one.** Choose **"Tighter than ±0.005″ (±0.13 mm)"**, then set **"Tightest tolerance band"** to the tightest feature on the part (±0.004″ down to "Tighter than ±0.0005″"). This tells the shop how tight the tightest feature is, not that the whole part needs it. Then identify those features: mark them on a drawing uploaded under **"Reference Files & Technical Drawings (optional)"**, or list them in the part **"Note"** with the feature, the tolerance and the general tolerance for everything else.

**Step 4: Sheet Cutting and Sheet Metal parts.** For these processes, **"Tolerance"** offers only General, Standard or "Shop to advise". If a hole, slot or bend needs to be tighter than Standard, choose Standard and describe the feature in the **"Note"**, so the shop can decide whether a secondary operation is needed.

**Step 5: Use "Not sure, shop to advise" when you are unsure.** It is a valid answer. Pair it with a sentence in the note about what the part does and what it mates with, and a shop can recommend a tolerance for the function.

**Step 6: Cover finish and inspection in the same place.** If the part is anodized or plated, say which features to mask or whether dimensions apply after finish. If you need an inspection report, say that in the note too.

| Your part | Tolerance choice | What to add |
| --- | --- | --- |
| Bracket or cover with no mating fits | General (±0.010″ / ±0.25 mm) | Nothing extra, unless a hole pattern matters |
| Typical machined part, nothing critical | Standard (±0.005″ / ±0.13 mm) | Your drawing's general tolerance, if you have one |
| Mostly standard, with a bearing bore or dowel holes | Tighter than ±0.005″ (±0.13 mm), then the tightest band | Critical features and their fits or tolerances on the drawing or in the Note |
| Laser or waterjet plate with one precise hole | Standard | The hole size and tolerance in the Note |
| You are not sure what it needs | Not sure, shop to advise | What the part does and what it mates with |

## A complete example

Here is a note that lets a shop quote a tolerance-sensitive part without follow-up questions. It is for a 6061 aluminum motor mount with a bearing seat and two dowel holes, with the CNC **"Tolerance"** set to "Tighter than ±0.005″ (±0.13 mm)" and **"Tightest tolerance band"** set to ±0.0005″:

General tolerance ISO 2768-mK unless noted. Critical features: bearing bore Ø35 H7 (+0.025/0), 2X dowel holes Ø6 H7 with position Ø0.05 to datums A and B, mounting face flatness 0.05. Everything else is non-critical. Type II black anodize, mask the bearing bore and dowel holes, dimensions apply after anodize elsewhere. First article inspection report on critical features please. Drawing attached, critical features ballooned on page 1.

That note tells the shop which three features drive the price and which forty dimensions do not. If you are unsure whether a bore needs H7 or something looser, write that instead, and a shop in the network can suggest a tolerance for the job. Quotes typically come back in about 48 hours.

## Related reading

- [CNC machining tolerance chart](https://openspindle.com/reference/cnc-machining-tolerance-chart.md)
- [Engineering fits chart](https://openspindle.com/reference/engineering-fits-chart.md)
- [GD&T symbols reference](https://openspindle.com/reference/gdt-symbols-reference.md)
- [Tolerance stack-up: worst case vs RSS](https://openspindle.com/blog/tolerance-stack-up.md)
- [3D printing tolerance chart](https://openspindle.com/reference/3d-printing-tolerance-chart.md)
- [Injection molding tolerance chart](https://openspindle.com/reference/injection-molding-tolerance-chart.md)
- [Anodizing spec](https://openspindle.com/reference/anodizing-spec.md)
- [First article inspection](https://openspindle.com/blog/first-article-inspection.md)
- [How to write an RFQ](https://openspindle.com/blog/how-to-write-an-rfq.md)

## Frequently asked questions

### What is a general tolerance on a drawing?

It is the tolerance that applies to every dimension without its own callout, usually stated in the title block. Metric drawings often reference an ISO 2768 class such as ISO 2768-m, while inch drawings commonly use a decimal-place block such as .XX ±.01 and .XXX ±.005. The exact values vary by company, so always state them on the drawing.

### What is a standard CNC machining tolerance?

Around ±0.005 in (±0.13 mm) on a linear dimension is a common default that most shops hold without special effort. Turned diameters and finished bores are often held tighter. Anything below about ±0.002 in usually adds finishing operations and inspection time.

### How much do tighter tolerances add to cost?

It depends on the part, material, feature and shop, so there is no reliable fixed multiplier. The cost rises in steps as a tolerance forces finishing passes, extra setups, temperature control, gauging or a CMM, and more scrap. Applying a tight band only to the features that function keeps most of that cost off the quote.

### Should I use ISO 2768 fine or medium?

Medium (m) is the most common choice for machined parts and is comfortably within normal shop practice. Fine (f) tightens every uncalled dimension, which can raise cost across the whole part. A common approach is medium for the general tolerance with individual callouts on the few features that need more.

### Does anodizing affect tolerances?

Yes. Anodizing builds up on the surface as well as penetrating it, roughly half each way as a rule of thumb, so a diameter changes by about the coating thickness. Type III hardcoat is thick enough to push a tight bore or thread out of tolerance. Mask critical features or state whether dimensions apply before or after finish.

### How do I specify tolerances in an OpenSpindle quote request?

On each part card, open Advanced options and choose a Tolerance band that describes most of the part. If any feature is tighter than ±0.005 in, choose Tighter than ±0.005″ (±0.13 mm) and set the Tightest tolerance band, then identify the critical features on an attached drawing or in the part Note. If you are unsure, choose Not sure, shop to advise.