Engineering · Design for Manufacturing · 2 of 8

DFM for CNC Machining

Can the cutter actually reach every feature on the drawing, in one or two setups?

CNC milling and drilling are flexible, but every feature has a cost set by the tool: its diameter, its reach, how many times the part is clamped, and how tight the tolerance is. This page turns the usual rules into checkers. Enter the end mill, pocket, hole, wall and tolerance and see straight away whether the design is easy, tricky or not machinable, plus a machining time and cost estimate.

Lower costFaster productionBetter qualityFewer setupsReliable design

1Standard tool sizes: design to them

Standard end mills and drills are cheap, in stock and have predictable behaviour. Pocket widths, corner radii and hole sizes that suit them cut lead time and cost.

Tool use	Typical diameters (mm)
Small features, fine detail	2, 3, 4
General purpose	6, 8, 10
Medium pockets	10, 12
Large pockets, high removal	16, 20

Circles are drawn at 4 px per mm. Use standard tool diameters and avoid special form tools unless the part really needs one.

2Internal corners: the tool is round

A rotating cutter cannot make a sharp inside corner. The corner radius it leaves is at least the tool radius, so a drawing radius smaller than that is not machinable with that tool.

Corner radius checker

End mill diameter (mm)Corner radius on the drawingmm

internal corner radius R ≥ D / 2, and a little larger is better so the tool does not stall in the corner

End mill diameter D	Minimum internal radius R
Ø 2 mm	≥ 1 mm
Ø 4 mm	≥ 2 mm
Ø 6 mm	≥ 3 mm
Ø 10 mm	≥ 5 mm

3Pockets: width and depth

Pocket checker

End mill diameter (mm)Pocket width WmmPocket depthmm

Guideline	Typical value
Pocket width W	at least 3 × end mill diameter
Pocket depth D	about 3 × tool diameter or less; deeper possible with pecking and coolant
Step-down per pass	0.5 × D to 1 × D, depending on material
Corner radius	at least D / 2

4Holes: drilling, reaming and tapping

Hole checker

Hole diametermmHole depthmmTool material

Tapped hole

ThreadBase material

tap drill ≈ d − pitch (metric coarse)

Use cutting taps with a drill deeper than the usable thread. Use a through hole when the part allows it.

Process	Minimum Ø	Remarks
Drilling (HSS)	1.0 mm	Standard drills, readily available
Drilling (carbide)	0.5 mm	Possible but fragile; not recommended for deep holes
Reaming	2.0 mm	For accurate holes
Tapping (metric)	M2 (Ø1.6 mm drill)	Standard sizes M2, M2.5, M3, M4 and up
Countersink	≥ 3.0 mm	Standard countersink tools

5Walls, ribs and clearance

Wall and rib checker

MaterialWall thicknessmmRib thicknessmmGap, wall to next featuremmEnd mill diameter (mm)

Do

Keep walls thick enough to avoid chatter and vibration.
Give the tool and holder room to reach the feature.
Use through holes or lower L/D ratios for deep features.

Avoid

Thin ribs that vibrate and break.
Deep narrow cavities that tool and holder cannot reach (undercuts need 4 or 5 axis or special tools).
Features on many faces that need re-clamping.

Typical clearance	Value
Side clearance	0.5 to 1 mm per side
Top clearance (holder)	3 to 5 mm or more
Deep cavity machining	Use long-reach tools; keep L/D at 4 or less

6Machining time and spindle speed

Machining time estimate

Tool diametermmSpindle speed NrpmFeed per rev fmm/revTool path length Lmm

T = L / (f × N) (min)
cutting speed Vc = π × D × N / 1000 (m/min)

The chips set the spindle speed from a typical carbide cutting speed: aluminium about 250 m/min, mild steel about 120, stainless about 80. These are starting figures only; follow the tool maker’s data. Add rapids, tool changes and deburring on top (they often add 10 to 20 percent of cutting time).

Machining time to cost

Original machining timeminImproved machining timeminMachine rate₹/h

7Tolerances and surface finish

What does this tolerance need?

Tolerance (plus or minus)mmSurface finish Ra (optional)µm

Capability (milling)	Typical value
General tolerance	± 0.1 to 0.2 mm
Good tolerance	± 0.05 mm
High precision (stable setup)	± 0.01 to 0.02 mm
Surface finish as machined	Ra 1.6 to 3.2 µm
With finishing toolpath	Ra 0.4 to 1.6 µm
With grinding	Ra 0.1 to 0.4 µm

Use ISO 2768 general tolerances where they are enough, tighten only functional features, and state surface finish only where it matters (sealing, sliding).

8Fewer setups, lower cost

Do

Machine as many features as possible from one side.
Use datums and symmetry.
Use through holes rather than blind holes where possible.
Design for 3-sided machining in one or two setups.
Consider 3+2 or 5-axis only when really necessary.

Avoid

Features on several faces that need re-clamping.
Odd angles and compound features.
Non-standard hole sizes and thread types.

9Try it: DFM checklist for CNC parts

CNC DFM scorecard

Remember

Internal radius is at least half the tool diameter.
Keep pockets wide (3 times D) and not too deep (3 times D).
Standard tools, standard holes, standard threads.
Fewer setups and looser tolerances save more than any clever toolpath.

HubDesign for ManufacturingThe full DFM section with a learning path.LearnDFM FundamentalsWhat DFM is, the core principles, cost drivers and a review scorecard.ReferenceTolerances, Fits and GD&TISO fit calculator, stack-up, feature control frames and gauge choice.EstimateManufacturing Cost EstimationPart cost build-up, batch effect, make or buy and lifecycle cost.DesignDFM for Sheet MetalBend allowance, flat length, reliefs, hole-to-bend distance and springback.

Sources and notes

Boothroyd, Dewhurst and Knight, Product Design for Manufacture and Assembly (CRC Press), for the DFM and DFA method.
Machinery’s Handbook (Industrial Press), for machining, sheet metal and welding practice.
ISO 2768 (general tolerances) and ISO 286 (limits and fits); see the Tolerances, Fits and GD&T page.
Cutting speeds and ratios are typical starting values; tool makers’ catalogues give exact data.

Guidelines are indicative and vary by machine, tool and material. Confirm limits with the shop that will make the part.