Eternal CNC · Precision Machining

CNC DFM Cost-Saving Guide (Part 1)

Five geometric design principles — real shop-floor experience on bringing the quote down

This guide isn't copied from a textbook. It's what we've learned from quoting, planning and reworking jobs over the years. Many designs are fine on paper, but once evaluated on a CNC floor the price triples or quadruples. The problem is rarely machine accuracy — it's the "small numbers" in the drawing the designer didn't notice.

Part 1 covers the five most valuable DFM decisions: wall thickness, hole depth ratio, shape, inside corner radius and tolerances. They share one thing: once the part is in production, it's too late to change them cheaply.

1. Wall Thickness — thinner isn't fancier

Core idea

Designers love pushing wall thickness to the limit, thinking it makes the part lighter and more refined. But CNC cuts with a tool pressed against the material — too-thin walls chatter, vibrate and deform, ending up with out-of-tolerance dimensions or a fish-scale surface. The cost of thin walls isn't material — it's process cost and scrap rate.

Material	Comfortable wall (small feature)	Large flat / thin wall	Risk
Aluminum 6061/7075	≥ 1.0 mm	≥ 2.0 mm (large area)	Chatter marks, warp
Carbon / alloy steel	≥ 1.5 mm	≥ 2.5 mm	Vibration, scatter
Stainless 304/316	≥ 2.0 mm	≥ 3.0 mm	Work-harden + warp
Titanium	≥ 2.0 mm	≥ 3.5 mm	Spring-back, chatter

Common wall-thickness traps

Tall, thin side walls of a deep pocket: the deeper the pocket, the more the wall swings while cutting. Rule of thumb: wall ≥ 1/20 of pocket depth. A 50 mm deep pocket wants a wall ≥ 2.5 mm.
Isolated bosses and thin posts: a 3 mm post sticking 20 mm up whips like a fishing rod — it either breaks or bends. Add ribs, or make it separate and assemble.
Abrupt wall thickness changes: 5 mm next to 1 mm means uneven heat and stress, the thin side warps. Use fillets / gradual transitions.
Thin large plates: see point 6 — a sub-3 mm aluminum plate warps after milling; not the machine's fault.

DFM tip: keep aluminum walls ≥ 1 mm, steel ≥ 1.5 mm, stainless ≥ 2 mm. For non-load-bearing enclosures/covers, use ribs or bosses instead of thickening the whole part — saves material and stays stable.

2. Hole Depth Ratio — you can't drill as deep as you want

Core idea

A standard twist drill has a comfort zone. The deeper and narrower the hole, the harder to clear chips, the more the drill wanders and the harder to cool. A long drill doesn't mean deep holes — the length-to-diameter ratio (depth ÷ diameter) decides whether you use a normal drill or a deep-hole machine.

Ratio L/D	Process	Cost impact
≤ 3×D	Standard drill, one pass	Baseline
3×D – 5×D	Standard drill, retract to clear chips	+20 – 30%
5×D – 10×D	Deep-hole / gun drill, guide bushing or peck	+50 – 100%
＞ 10×D	Deep-hole machine (BTA / gun drill)	+200% or redesign

Real traps

Small deep holes: φ1 mm drilling 10 mm deep, L/D=10, breaks and wanders easily. Avoid if you can.
Chip packing in blind holes: drilling to the bottom of a blind hole leaves chips nowhere to go; the drill heats and either smears or breaks. Through-holes clear chips far better.
Stepped holes beat deep holes: if you need a threaded section + a clearance section, draw a stepped hole — much cheaper than drilling deep then tapping.

DFM tip: keep holes within 5×D; above 10×D, confirm the process with the shop first. Through-holes beat blind holes; stepped holes beat deep blind holes.

3. Shape — square is always cheaper than fancy

Core idea

CNC loves flat faces, right angles, flat-bottom pockets, uniform radii. A 3-axis machine finishes most features in one setup. The moment you add spheres, free-form surfaces, undercuts or angled walls, you need ball-nose tools, 5-axis, a right-angle head or EDM — and time climbs exponentially.

Geometry	Recommendation	Typical process	Cost factor
Block / regular outline	★★★★★	3-axis rough + finish	1×
Vertical walls + flat-bottom pocket	★★★★★	Flat end mill	1×
Spherical / curved surface	★★★☆☆	Ball-nose 3-axis or 5-axis	1.5 – 3×
Undercut / side recess	★★☆☆☆	Right-angle head / 5-axis / wire / EDM	3 – 10×
Deep narrow slot / odd slot	★★☆☆☆	Small tool / multi-axis / EDM	2 – 5×

Shape traps designers hit

Square over round: same function, a square pocket is cheaper than a round one — a flat end mill runs to the bottom in one pass; a round or spherical pocket needs a ball-nose tool crawling slowly with a finish pass.
Undercuts are a cost bomb: a wall recessed inward can't be reached by a 3-axis tool — you need a right-angle head, 5-axis or wire cut. Avoid undercuts and the quote drops a tier.
Unify radii and hole sizes: a drawing with R0.5, R1, R2, R3 forces a dozen tool changes. Standardize to R2 / R3 and cut 30% of tool-change time.
Slopes and draft angles: within 5° can be done with a big face mill; beyond 15° or varying curvature needs a ball-nose or 5-axis.

DFM tip: prefer regular geometry when function allows; flat faces + right angles for outline; flat-bottom + uniform radii for pockets; absolutely avoid undercuts. In short: let the 3-axis machine finish the job in one setup.

4. Inside Corner Radius — the hidden threshold for tool choice

Core idea

A designer draws a square pocket and wants the corners cleaned to R0.5. The problem: there is no φ1 end mill that reliably cuts steel — too thin, it snaps on contact. The inside corner radius must be ≥ the tool radius. To get an R0.5 corner you need a φ1 tool; a φ1 tool in steel means very high breakage risk, only extreme-low speed and shallow depth, and exploded cycle time.

Inside radius	Tool needed	Process	Cost impact
R3+	φ6 flat mill	Normal 3-axis	Baseline
R1 – R2	φ2 – φ4 flat mill	Normal mill, slightly lower feed	+10 – 20%
R0.5 – R1	φ1 – φ2 flat mill	Very low speed / shallow depth, breaks easily	+50 – 100%
＜ R0.5	φ0.5 – φ1 tool or EDM	Almost unmillable	+200% or redesign

Rule of thumb: inside radius ≥ 1 mm (φ2 tool) is the economic zone; ≥ 2 mm (φ4 tool) is most comfortable; < 0.5 mm basically needs EDM or we decline.

DFM tip: use R2, not R0.5. If the look demands a small radius, the DFM way is — rough the big pocket at R2, then EDM the local small R, which is cheaper than milling the whole thing with a tiny tool.

5. The "Economic Zone" of Tolerances — one notch tighter, double the cost

Core idea

Many designers stamp every dimension at ±0.01 mm or ±0.005 mm, thinking "tighter is better". In reality CNC has an economic accuracy zone. The tighter the tolerance, the denser the measurement, the fussier the fixturing, the stricter the environment — cost multiplies.

Tolerance	3-axis normal capability	What it needs extra	Cost factor
±0.1 mm	One pass	Nothing	1×
±0.05 mm	Normal finish mill	Nothing	1×
±0.02 mm	Finish mill + measure	Measure every 5 pcs	1.2×
±0.01 mm	Finish mill + first + in-process check	CMM or micrometer per piece	1.5 – 2×
±0.005 mm	Thermostat / fine grind / multi-pass	Possible re-clamp / wire cut	3 – 5×
±0.002 mm	Grinder / jig grinder / 5-axis finish	Custom per-piece process	10×+

Real traps

Only tighten fit surfaces: bearing seats, locating-pin holes, sealing faces must be tight; outer contours and non-critical steps can relax to ±0.05 or ±0.1 and save plenty.
GD&T is pricier than size tolerance: 0.02 mm flatness is far harder than ±0.01 mm size, because you measure a whole face, not a point.
Don't over-specify untouched dims: many default every dimension to ±0.01; a plain cosmetic face at ±0.1 is perfectly fine.
Material affects accuracy: the same ±0.01 is easy in aluminum, shaky in stainless, harder in titanium.

DFM tip: tighten fit surfaces, relax the rest; write GD&T with care; leave ±0.1 for untouched dims. Remember: one notch tighter, double the cost — and the harder the material, the steeper the curve.

In closing: these five principles — wall thickness, hole depth, shape, inside radius, tolerances — decide 80% of a CNC quote. All can be solved at the drawing stage, no waiting for shop-floor rework. Part 2 will cover thin-plate warping, thread depth and material selection — three more easy traps.