Context

From the shop floor, I see designers chase razor-sharp corners in pockets like it’s a badge of precision. The problem is simple: round tools make round paths. Push them into deep cavities with tight radii and you’re asking them to flex, scream, and gouge their way through a job that was clean on paper but ugly in steel or aluminum.

Internal radii are not just cosmetic in deep pockets. They define tool size, deflection, and the real cycle time for CNC pocketing.

The Trap

The corner trap happens when a cutter’s arc of engagement jumps as it rolls into a tight internal radius. In CAD it looks harmless; in reality the tool’s surrounded by metal, cutting forces spike, and you’ll hear chatter before you see the finish ruined. Smaller corner radii squeeze you into smaller tools, multiplying deflection and heat, and hammering structural integrity.

The Geppetto Take

I don’t buy the idea that every corner has to match the mating part’s square profile exactly. We’ve avoided scrap by opening up radii just enough to let a rigid cutter roll in smooth, dodging the chatter. If your design forces a 20:1 L:D ratio, you’re building in cost and risk by design. A seasoned machinist will spec radii that match the process envelope, not just the CAD model.

Evidence / Data

When someone calls for an R1.0 mm corner in a 40 mm deep pocket, that’s a 2 mm diameter tool at a brutal 20:1 L:D ratio. Doubling length increases deflection by 8x, halving diameter increases it by 16x - cause and effect you can hear in the chatter and see in tapered walls. In aluminum, R5.0 mm with a 10 mm end mill at 2:1 L:D runs in 12 minutes (~1.0x cost), but choke it down to R0.5 mm and you’re stuck with a 1 mm end mill at 20:1 L:D, 85+ minutes and ~7.0x+ cost, plus risk of tool snap.

Control Actions

Follow the 1/3 depth rule: 30 mm deep means at least a 10 mm radius. Use rest machining to knock the bulk out with a big, stiff cutter before sneaking into corners. Corner drilling can tame force spikes before the end mill even touches it. And if the L:D creeps past 8:1, consider wall tapers or relief cuts so the tool can breathe.

Checklist

  • Keep internal radii as large as functionally possible.
  • Target L:D <= 8:1 for corner finishing tools.
  • Use roughing + rest machining instead of one tool for the full depth.
  • Add relief where a sharp corner has no functional requirement.

What to Send

Send depth, corner radius, material, and tolerance stack notes before locking the design. Include any functional reason that radius can’t grow. That’s the info we need to keep it machinable without gutting your intent.

CTA

Send a screenshot for a chaos-check.