Knowledge Base

DFM Cost-Saving Guide (Part 1)

Five geometric design principles that decide 80% of a CNC quote. Not copied from a textbook — lessons from quoting, planning and reworking real jobs. The problem is rarely machine accuracy; it's the "small numbers" in the drawing.

1. Wall Thickness — thinner isn't fancier

CNC cuts with a tool pressed against the material. Too-thin walls chatter, vibrate and deform — ending in out-of-tolerance dimensions or a fish-scale surface. The cost isn't material, it's process cost and scrap rate.

Traps:

• Tall thin walls of a deep pocket swing while cutting — keep wall ≥ 1/20 of pocket depth (a 50 mm pocket wants ≥ 2.5 mm wall).
• Isolated thin posts whip like a fishing rod — add ribs, or make it separate and assemble.
• Abrupt thickness changes warp the thin side — use fillets / gradual transitions.

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

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.

Traps:

• Small deep holes (φ1 mm × 10 mm, L/D=10) break and wander easily — avoid if you can.
• Chip packing in blind holes heats and breaks the drill — through-holes clear chips far better.
• Stepped holes beat deep blind holes — cheaper than drill-deep-then-tap.

3. Shape — square is always cheaper than fancy

CNC loves flat faces, right angles, flat-bottom pockets, uniform radii. Add spheres, free-form surfaces, undercuts or angled walls and you need ball-nose tools, 5-axis or EDM — time climbs exponentially.

Traps:

• Square over round — a square pocket is cheaper than a round one (flat end mill runs to the bottom in one pass).
• Undercuts are a cost bomb — a 3-axis tool can't reach an inward recess. Avoid them and the quote drops a tier.
• Unify radii and hole sizes — R0.5/R1/R2/R3 forces a dozen tool changes; standardize to R2/R3.

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

The inside corner radius must be ≥ the tool radius. To get an R0.5 corner you need a φ1 tool — which in steel means very high breakage risk, only extreme-low speed, and exploded cycle time.

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.

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

The tighter the tolerance, the denser the measurement and the fussier the fixturing — cost multiplies. Tighten only what functionally needs it.

Traps:

• Only tighten fit surfaces (bearing seats, pin holes, seals); relax outer contours to ±0.05 / ±0.1.
• GD&T is pricier than size tolerance — 0.02 mm flatness is harder than ±0.01 mm size.
• Don't over-specify untouched dims — a cosmetic face at ±0.1 is fine.
• Material matters: ±0.01 is easy in aluminum, shaky in stainless, harder in titanium.