Guides / Design

5-Axis Prototype Tolerances and Inspection: What to Specify and What to Ask For

October 6, 2026

A tolerance on a drawing is a request. Whether the part comes back in spec depends on what the shop can hold, how it measures and what you actually wrote down. This guide covers the numbers a capable 5-axis shop typically works to, the GD&T callouts that matter on 5-axis parts, how each callout is verified and the documents to ask for with the parts.

Every figure below is a reference value, not a guarantee. Capability varies with the machine, the material, the part size and the setup. Use the numbers to start the conversation, then ask each shop to confirm them against your drawing. For the tolerances of printed and cast parts next to machined ones, see 5-axis CNC prototyping.

Typical capability of a 5-axis prototype shop

Parameter	Reference value	What to ask the shop to confirm
Linear tolerance, best case	about ±0.005 mm	Which features they would hold at this level and how they measure them
Linear tolerance, typical	±0.01 mm	Whether this applies across the full part size
Bore and shaft fits	H6 / h5, IT5 grade on the shaft	Whether the fit is bored, reamed or ground
Angular features	about ±10 arc minutes	How they check compound angles after unclamping
Surface finish, best case	Ra 0.8 μm	Which faces need a dedicated finishing pass
Surface finish, typical	Ra 1.6 μm	Whether this is the as-machined default
General tolerance default	ISO 2768 fH	Which class they assume if the drawing is silent

ISO 2768 fH means class f (fine) for linear and angular dimensions and class H for geometric tolerances such as flatness, straightness and perpendicularity. It is a sensible default for 5-axis prototype work. Anything tighter than 2768 should be quoted per feature after a design for manufacturing (DFM) review, so the shop can tell you what each tight callout will cost in time.

Which GD&T callouts matter on 5-axis parts

5-axis parts tend to have angled faces, blended surfaces and features that point in several directions. Plus-minus tolerances on these parts get ambiguous fast. Geometric dimensioning and tolerancing (GD&T) removes the guessing by tying each feature to datums.

Form controls

Flatness: sealing faces and mounting pads.
Straightness: long shafts, rails and guide edges.
Circularity: round sections where the shape matters but the axis does not.
Cylindricity: bearing seats and pin bores where the full length must stay round and straight.

Orientation controls

Parallelism: opposing faces that set a gap or a stack height.
Perpendicularity: bores and faces that must sit square to a mounting datum.
Angularity: the core callout for 5-axis work. It controls an angled face or bore relative to a datum, which a plain angle dimension does poorly.

Profile controls

Profile of a line: a 2D cross-section, such as a cam edge or an airfoil section.
Profile of a surface: the full 3D surface compared with the CAD model. This is the natural callout for freeform and blended surfaces cut in simultaneous 5-axis.

Runout controls

Circular runout: each cross-section of a rotating feature relative to its axis.
Total runout: the whole surface at once. Use it on shafts and hubs that spin at speed.

Datum schemes

Pick datums that match how the part mounts in the assembly, not how it is easiest to clamp. A typical scheme uses the main mounting face as the primary datum, a locating bore or edge as the secondary and a second edge or slot as the tertiary. On a 5-axis part cut in one clamping, features cut in that clamping hold their relationship to each other well. Features cut in a second operation, such as the side that was held by a tab, depend on how well the shop re-locates the part. Ask which features fall into which operation.

Bonus tolerance under MMC

A position callout with the maximum material condition (MMC) modifier gives extra tolerance as the feature departs from MMC. Example: a hole of Ø6.00 +0.05/0 with position Ø0.05 at MMC. At Ø6.00 the hole must sit within Ø0.05. At Ø6.03 it may sit within Ø0.08. For clearance holes this bonus lets the shop run faster without hurting assembly, so use MMC wherever the function allows it.

How each callout gets verified

Knowing the method tells you what report to expect and which shops can support your part. Ask each shop what equipment it uses for your specific callouts.

Callout or requirement	Common inspection method
Linear dimensions	Micrometers and height gauges in process, CMM for final report
Bore diameter and fits	Bore gauges and micrometers, CMM on complex parts
Flatness, straightness, parallelism	CMM, or height gauge and indicator on a surface plate
Perpendicularity, angularity	CMM
Position with datums and MMC	CMM
Profile of a line	Optical comparator or CMM
Profile of a surface	CMM compared with the CAD model
Circularity, cylindricity	CMM
Circular and total runout	Indicator on the rotating part, or CMM
Threads	Thread gauges, optical comparator for profile
Surface finish (Ra)	Surface roughness tester

The CMM carries most of the geometric work on 5-axis parts. The optical comparator suits edge profiles and thread forms. Height gauges, micrometers and bore gauges are how the machinist checks features between cuts, before the part leaves the machine. The surface roughness tester is the only reliable way to confirm an Ra value; visual comparison plates are not a substitute on a critical face.

How material changes what you can hold

The same drawing will behave differently in different alloys. Tell the shop the exact grade, not just “stainless” or “plastic”.

Aluminum 6061 and 7075: the easiest to hold tight. 7075 can move on thin walls when internal stress is released, so ask about roughing, resting and finishing on thin parts.
Stainless 304, 316 and 316L: work hardens and generates heat. Tight bores are achievable but take slower finishing passes.
Titanium Grade 2 and Grade 5: low stiffness means thin walls spring away from the cutter. Grade 5 is stronger and harder to cut than Grade 2.
Brass: machines cleanly and holds tight tolerances and fine finishes with little effort.
Copper: soft and gummy. Burrs and surface finish need more attention than dimensions.
Tool steel D2, H13 and SKD11: usually roughed soft, heat treated and then finished by hard milling or grinding. Heat treatment distorts the part, so tight features are finished after hardening.
Carbon steel: stable and predictable to cut. Specify a coating or oil if the parts will sit before assembly.
PEEK: holds reasonable tolerances but moves with temperature. Annealed stock helps on tight parts.
POM (Delrin): machines well and is dimensionally stable for a plastic. A common choice for fit checks.
PTFE: creeps under clamping force and expands several times more than aluminum with temperature. Loosen tolerances on PTFE wherever function allows.

Specialty alloys such as Inconel and Monel are taken by fewer shops, and tight tolerances in them take longer to cut. Expect fewer quotes and longer lead times.

For plastics, state the measuring temperature on the drawing. The ISO reference temperature is 20 °C, and a plastic part measured warm can read out of tolerance when it is fine.

What tighter tolerances cost

Every step tighter adds time. Going from ISO 2768 fH to ±0.01 mm on a bore may add a finishing pass and a CMM check. Going from ±0.01 mm to ±0.005 mm may add a temperature soak, a second finishing tool and repeated measuring. Surface finish follows the same pattern: Ra 1.6 μm is often the as-machined result, while Ra 0.8 μm usually means a slower final pass.

The practical rule is simple. Mark only the critical features tight: the bores that take bearings or pins, the faces that seal or locate, the surfaces that meet another part. Let everything else fall under the general tolerance. A drawing where every dimension reads ±0.005 mm gets a high quote, a long lead time or a polite no. See what drives 5-axis prototype cost for how tolerance sits alongside programming, setup and material.

Documents to ask for

Agree on the paperwork when you request the quote, not after the parts ship. Typical requests for prototype and small batch orders:

First Article Inspection (FAI): a full dimensional report on the first part of every new part number or revision.
PPAP Level 3: only where an automotive or aerospace customer requires it. It adds documents and time.
Mill certs: material certificates that trace the stock back to the heat or lot.
Inspection report packed with the shipment: so receiving inspection can check the parts without waiting for an email.
RoHS declaration: for parts going into electrical or electronic products.
REACH SVHC declaration: on request, for parts shipped into the EU.

If you need none of this, say so. Shops price in paperwork they think you might want.

DFM feedback belongs before the quote

If the drawing is unclear, the right time to find out is before the price is set, not after the part is cut. A shop that reads your drawing carefully will come back with questions: a datum that cannot be reached, a tolerance that fights the material or an angle that needs a special tool. That feedback is worth more than a fast quote. For geometry changes that make parts easier to hold, read designing parts for 5-axis machining.

Checklist: what to put on the drawing

STEP file plus a PDF drawing of the same revision
Material grade and temper, not just the material family
General tolerance note, such as ISO 2768 fH
Tight tolerances only on the critical features, each marked clearly
A datum scheme that matches how the part mounts
GD&T callouts for angled, profiled and rotating features
MMC modifiers on clearance hole positions where function allows
Surface finish per face, with a default Ra for the rest
Thread specifications, including class and depth
Measuring temperature for plastic parts
Required documents: FAI, mill certs, RoHS, REACH or PPAP
Quantity per revision and your real deadline

The RFQ form asks for each of these fields, and you can check simultaneous or 3+2 before you send it.

Send your drawing

When the drawing is ready, send one RFQ with the STEP file and PDF. We match it with up to three shops that run simultaneous or 3+2 5-axis work and quote prototypes and small batches of 1 to about 200 pieces per revision. Each shop quotes you directly, the service is free for buyers and an NDA is available on request. You get a reply within 24 business hours. Ask each shop to confirm the tolerances, inspection methods and documents in this guide against your part before you place the order.

Frequently asked questions

What tolerance can a 5-axis shop hold on a prototype?

A capable shop typically works to about ±0.01 mm on linear features and can reach about ±0.005 mm on selected small features. Fits such as H6 / h5 and angles around ±10 arc minutes are common reference points. Ask each shop to confirm these against your drawing and material.

Should I put ISO 2768 on a prototype drawing?

Yes. A general tolerance note such as ISO 2768 fH covers every dimension without its own tolerance. It stops the shop from guessing and lets you mark only the critical features with tighter values.

Do I need a CMM report for a prototype?

For parts with GD&T callouts such as profile, position or runout, a CMM report is the normal way to show conformance. For a simple form and fit prototype, a first article report with hand-gauge readings on the critical features is often enough.

When should I ask for PPAP?

Only when your automotive or aerospace customer requires it. PPAP Level 3 adds documents and time. For most prototypes a first article inspection report plus mill certs covers what engineering needs.

Need this prototype quoted?

Send the drawing. We match you with up to 3 5-axis shops and reply within 24 business hours.

Get matched with a 5-axis shop