CNC Machining Allowance: Values, Calculation and Standards for Turning, Milling and Grinding

Machining allowance is the extra material deliberately left on a raw part. CNC machining removes it until size and surface finish are right.

The right allowance decides scrap, cycle time and tool cost. At Vulcanus, we plan it every day for sawn, cast, forged and welded parts.

This guide gives typical CNC machining allowance values, a worked calculation and the key standards.

Key Takeaways

• Machining allowance is the extra material left on a part to ensure accurate finishing and dimensional precision.
• The total allowance is the sum of all process allowances from raw part to finished size.
• Typical finishing allowances per face: 0.2 to 0.5 mm for milling and turning, 0.05 to 0.15 mm for grinding.
• Always check whether a value applies per side or on the diameter.
• For castings, ISO 8062-3 defines the required machining allowance in grades A to K.
• As small as possible, as large as necessary: every extra millimetre costs time and tooling.

What is Machining Allowance?

Machining allowance is the intentional layer of extra material left on a raw part. It remains after processes like casting, forging, rolling, sawing or welding. CNC machining removes it to reach the final dimension and surface finish.

Put simply, it is the difference between the raw size of a part and its finished size. Without this allowance, manufacturers risk producing parts with surface defects, dimensional inaccuracies, or poor tolerances.

For example:

• A steel shaft may be forged slightly larger in diameter to leave room for precision turning.
• A cast housing will have extra stock so that milling and grinding can produce flat, accurate surfaces.
• A sawn blank is cut slightly longer so that both end faces can be faced or milled clean.

With correct planning, every component reaches its exact design specification.

Process Allowance, Total Allowance and Minimum Allowance

Process planning distinguishes several types of machining allowance:

Term	Meaning	Example
Process allowance	material removed in a single operation	0.3 mm per side in finish turning
Total allowance	sum of all process allowances from raw part to finished size	2.5 mm per side from bar stock to ground shaft
Minimum allowance	smallest allowance that reliably removes all defects of the previous stage	roughness plus surface layer plus position error
Maximum allowance	minimum allowance plus the size tolerance of the previous stage	occurs when the raw part sits at its upper limit
Finishing allowance	process allowance for the last cutting pass	0.2 to 0.5 mm per face in milling

The minimum allowance is built from several components:

1. Roughness of the previous operation: The marks of the previous cut must disappear completely.
2. Damaged surface layer: casting skin, scale, decarburised zones or work-hardened layers.
3. Form and position errors: bending, distortion or offset of the raw part.
4. Clamping errors: deviations when clamping and aligning the part in the machine.

The size tolerance of the previous stage is added on top. This gives the maximum allowance the process must handle reliably.

How to Calculate Machining Allowance: Formula and Worked Example

For simple geometries, these formulas apply:

• Outside diameter, per side: Z = (raw diameter − finished diameter) / 2
• Bore, per side: Z = (finished diameter − pre-drilled diameter) / 2
• Flat face, one-sided: Z = raw size − finished size

Worked example: A shaft is to be hardened and ground to Ø 60 h6. The raw material is Ø 65 mm round bar.

Step	Diameter afterwards	Process allowance per side
Raw material	Ø 65.0 mm
Rough turning	Ø 61.0 mm	2.0 mm
Finish turning	Ø 60.4 mm	0.3 mm
Hardening	Ø 60.4 mm, slight distortion
Grinding	Ø 60.0 mm h6	0.2 mm

The total allowance is (65 − 60) / 2 = 2.5 mm per side. It equals the sum of the process allowances: 2.0 + 0.3 + 0.2 mm.

The formulas do not account for distortion or tool deflection. These effects come in through the minimum allowance and the manufacturer’s experience.

Why Machining Allowance is Important

Machining allowance is more than a safety margin. It is a key factor in precision, cost and efficiency.

• Surface clean-up: Removes casting skin, scale or other imperfections. This leaves a clean, defect-free functional surface.
• Dimensional accuracy: Provides the stock needed to hit exact sizes. This prevents costly rework or scrap.
• Better surface finish: Allows finishing, grinding or polishing. This matters most for highly loaded steel parts.
• Cost and time: Too little allowance leaves rough spots or size errors. Too much lengthens machining and increases tool wear and material use.

In short, choosing the right machining allowance ensures precision while keeping production costs under control.

Key Factors Influencing Machining Allowance

Several factors determine how much machining allowance is needed:

• Material: Aluminium usually needs less allowance but distorts in thin walls. Steel, stainless steel and titanium need more margin for wear and deformation. See our guide to CNC material selection.
• Type of raw part: Castings, forgings, weldments and sawn blanks have very different surfaces and size accuracy.
• Size and geometry: Large, long or thin-walled parts distort more easily. They need larger allowances.
• Machining process: Roughing needs more allowance, finishing and grinding much less.
• Heat treatment: Hardening causes distortion. Hardened parts therefore need a grinding or hard turning allowance.
• Surface and tolerance requirements: Tight tolerances and fine finishes, such as in aerospace, need especially careful planning.
• Machine and workholding: Rigid machines and good fixtures allow smaller allowances.

By considering these factors together, manufacturers can set the right balance between cost, time, and quality.

Machining Allowance vs. Tolerance: What’s the Difference?

Although often confused, machining allowance and tolerance serve different purposes in manufacturing:

• Machining allowance: This is the extra material left on a part to ensure it can be properly machined to the desired dimensions. It compensates for irregularities in casting, forging, or previous machining steps.
• Tolerance: Tolerance refers to the permissible variation in a finished part’s size or dimension. It defines the acceptable limits within which a component can still function correctly.

Key difference: allowance is about how much extra material is left for machining, while tolerance is about how precise the final dimensions must be.

For example, a gear blank may have a machining allowance of 2 mm to remove rough casting surfaces, while its bore diameter tolerance might be ±0.01 mm to ensure proper assembly with a shaft.

Understanding this distinction helps engineers avoid errors, improve quality control, and design processes that are both efficient and cost-effective.

Learn more about tolerance types and how they are specified in our guide to manufacturing tolerance. Inspection is covered in quality control for CNC machining.

Standards and Typical Values for Machining Allowance

In industrial practice, machining allowances are not chosen at random. They are based on standards, raw-part supplier guidelines and years of shop-floor experience.

Standards for Machining Allowance

• ISO 8062-3: defines dimensional casting tolerance grades (DCTG) for castings. It also defines required machining allowance grades (RMAG) from A to K. A drawing callout reads, for example, “ISO 8062-3 DCTG 10 RMAG H”.
• DIN 7527: gives machining allowances and permissible deviations for open-die forged steel parts.
• ISO 1302 and ISO 21920-1: let you state the allowance directly in the surface texture symbol.

There is no general allowance standard for sawn stock or weldments. Shop guidelines and experience apply here.

Typical Values by Process and Raw Part

Process or raw part	Typical allowance	Basis
Rough turning	1 to 3 mm, i.e. 2 to 6 mm on the diameter	per side
Finish turning	0.2 to 0.5 mm	per side
Milling, roughing	1 to 3 mm	per face
Milling, finishing	0.2 to 0.5 mm	per face
Grinding after hardening	0.1 to 0.3 mm on the diameter, i.e. 0.05 to 0.15 mm per side	diameter
Sawn blank (end faces)	1 to 3 mm per end face	per end face
Castings	3 to 12 mm, depending on size and casting process	per face
Forgings	2 to 6 mm, depending on weight and complexity	per face
Welded assemblies	2 to 5 mm on functional faces	per face

These values are starting points. Final allowance depends on the specific project, machining capability, and tolerance requirements of the finished part.

How Much Finishing Allowance per Face?

For finishing, 0.2 to 0.5 mm per face is typical. Small, rigid parts often need only 0.1 to 0.2 mm. For large or distortion-prone parts, plan 0.5 mm or more.

An even allowance is what matters. Only then does the tool deflect the same everywhere, so size and surface are right. Read more about the step before in our guide to CNC roughing. Achievable finishes are covered in our guide to surface roughness.

How Much Machining Allowance Is Needed for Sawing?

A sawn blank is cut about 1 to 3 mm longer per end face. The end faces are then faced on the lathe or milled flat. For large cross-sections or a wandering saw blade, plan for the upper end.

The saw kerf is not a machining allowance. It does count in material planning when several parts are cut from one bar. Our guide to cut-to-length tolerance in sawing explains which tolerances a sawn blank achieves. For an overview of metal sawing methods, see our dedicated guide.

Allowances for Heat Treatment, Castings and Weldments

• Hardened parts: Hardening causes distortion. A grinding or hard turning allowance is therefore left before hardening. See our guides to heat treatment of metals and hard turning and grinding.
• Castings: Casting skin is hard and often porous. The first cut should reach below the skin instead of rubbing on it. This protects the cutting edge.
• Forgings: Scale and decarburised surface zones must be removed completely. Our comparison of forging vs machining explains the trade-offs.
• Welded assemblies: Welding brings heat and distortion into the part. Functional faces are therefore machined after welding, often after stress relieving. Our guide to the heat affected zone explains the background.

Practical Machining Allowance Guidelines for Engineers

For engineers, setting the right machining allowance is a balancing act between material use, machining time, and achieving the required accuracy. Below are practical considerations:

• Match allowance to process capability: Avoid leaving too little allowance, which may result in surface defects, or too much, which increases machining costs.
• Consider tool wear and machine stability: High-precision machines can handle tighter allowances, while older or less rigid machines may need extra margin.
• Plan for sequential operations: Allocate enough material for each step, from roughing to finishing, to avoid dimensional issues at later stages.
• Account for material behaviour: Materials prone to distortion or hardening may need larger allowances to maintain dimensional accuracy.
• Optimise for cost and sustainability: Reducing unnecessary excess material lowers waste, energy use, and production costs.

By applying these guidelines, engineers can design machining processes that are not only accurate but also efficient and sustainable.

Common Machining Allowance Problems and Their Solutions

Problem	Common cause	Solution
Unmachined spots after finishing	allowance smaller than distortion or casting skin	measure the raw part, increase allowance on the critical face
Uneven stock	poorly aligned raw part	probe the raw part and set the zero point from it
Size out of tolerance after hardening	no grinding allowance planned	leave a grinding or hard turning allowance before hardening
Long cycle time, high tool wear	allowance far too large	adjust raw size, choose near-net-shape blanks
Tool breakage on the first cut	edge rubbing on hard casting skin	choose a depth of cut that reaches below the skin
Part distorts after unclamping	residual stresses are released	rough first, then stress-relieve, finish last

Rigid jigs and fixtures and an early check of manufacturability prevent many of these errors.

Machining Allowance and Cost: Why Every Millimetre Counts

Machining allowance determines how much material must be cut. More allowance means more passes, more time and more tool wear. On large parts this quickly adds up to many machine hours.

Too little allowance, however, is usually more expensive. A single part with unmachined spots is often scrap. The skill lies in the smallest allowance that reliably removes all defects.

See how CNC quotes are calculated to understand how raw size and allowance affect price. Our guide on how to reduce per part cost adds practical levers.

Machining Allowance in Practice at Vulcanus

Vulcanus-Stahl & Maschinenbau has been manufacturing in Werl, North Rhine-Westphalia, since 1984, certified to ISO 9001. Sawing, welding and machining all happen under one roof. That is why we plan machining allowance from the sawn blank to the finished part in one place.

• Sawing: blanks with the right end-face allowance through our sawing services.
• Turning: roughing and finishing allowances for shafts and large turned parts with our CNC turning.
• Milling: even stock on cast, forged and welded parts with our CNC milling.

With large workpieces, every millimetre counts. Read more in our guide to CNC machining large parts. As a partner for CNC contract manufacturing, we handle one-offs, small batches and assemblies.

Planning Machining Allowance with Purpose

Machining allowance is a critical factor for quality, efficiency and cost. Planning process and total allowance carefully avoids scrap and wasted machine time.

The right allowance:

• reduces waste
• extends tool life
• ensures precise tolerances
• delivers parts that meet customer expectations

Whether casting, forging, weldment or sawn blank, careful planning balances accuracy with productivity. It is a key building block of any precision manufacturing.

Want to agree the allowances for your part? Contact us today and send us your drawing.

Frequently Asked Questions (FAQs)