Designing pockets — corner radii, depth, and the cost of doing it wrong.

Internal corners of pockets cannot be sharp. A CNC end mill has a radius — the pocket corner will always have a radius at least equal to the tool radius. Specifying a smaller radius than the tool can produce either requires a smaller (weaker, slower) tool, or multi-operation finishing with a smaller tool after roughing with a larger one.

The general rule: make pocket internal radii ≥ 1/3 of the pocket depth. For a pocket 9mm deep, minimum internal radius should be 3mm. Why? Because tool length-to-diameter ratio above 3:1 causes chatter, requires slow feed rates, and deflects under cutting load. A pocket with a 0.5mm corner radius but 9mm depth requires a Ø1mm end mill with 9mm reach — 18:1 ratio. Chatter and breakage follow.

Truly sharp internal corners require wire EDM (typically +$30-100 per corner) or broaching (custom tooling). For 99% of applications, specifying a generous corner radius is the right call.

Pocket depth relative to the smaller of length or width determines tool accessibility. Rules of thumb:

• Depth ≤ 2× width: easy, standard machining. Any end mill size works.
• Depth 2-4× width: requires longer tools, slower feeds. Cycle time +40%.
• Depth 4-6× width: requires specialty long-reach tools or trepanning. Cycle time +100-150%.
• Depth > 6× width: impractical for standard CNC; consider alternative processes (EDM, wire EDM, redesign to split into multiple pieces).

Narrow deep pockets are the most expensive feature you can design. A 3mm-wide slot 30mm deep (10:1 ratio) may take 10× longer to cut than a 6mm-wide slot of the same depth because the tool has to run slower, use coolant flush to evacuate chips, and do multiple step-down passes.

Pocket floors have their own considerations:

• Floor flatness: a standard end mill can achieve ±0.02mm flatness across a pocket floor. For tighter specs, follow with a finishing pass using a large-diameter insert cutter — slower but flatter.
• Floor-to-wall radius: the intersection of the pocket floor and wall will have a radius equal to the end mill corner radius. For a Ø10mm end mill with R1 corner, floor-to-wall radius is R1. To get truly sharp floor-to-wall intersection, secondary EDM operation required.
• Floor surface finish: Ra 1.6-3.2 μm is standard mill finish. Below Ra 1.6 requires slow finishing passes or ball-end-mill surfacing.

If the pocket will become a mold cavity feature (injection molding or casting), add draft angles. Otherwise the part won't eject from the mold.

• Standard cosmetic surfaces: 1° minimum draft on all vertical walls
• Textured surfaces: 1.5-3° draft depending on texture depth
• Deep pockets (>50mm): 2° draft to reduce ejection force
• Zero-draft locations (must be documented): side actions required — adds $3,000-8,000 to tooling cost

For CNC-machined pockets that are end-use parts (not molds), draft is not strictly needed. But adding 1° draft to wall faces makes the machining easier (less tool engagement at the corner) and reduces tool deflection. Free improvement.

An aluminum pocket 50mm × 30mm × 20mm deep with different corner radii:

The same functional pocket at 3 different corner radii varies 5.5× in cost. If the R3 corners work for your application, specifying R0.5 because "that's what was on the last drawing" is a 450% cost inflation for zero benefit.