OPJAW

2026-04-04

A 6.35 mm (1/4") endmill cannot cut a corner tighter than 3.175 mm radius. A 3.175 mm (1/8") endmill halves the corner radius but takes four times longer to clear the same pocket volume. Tool selection for fixture pockets is a trade-off between corner access and cycle time.

1. The Relationship

An endmill is round. The minimum internal corner radius it can produce equals the endmill radius. A 1/4" endmill leaves a 3.175 mm radius at every internal corner. No toolpath strategy changes this — the geometry of a circular cross-section sets a hard floor.

Tool diameter    Tool radius    Min corner radius
---------------------------------------------------
3.175 mm  (1/8")    1.588 mm       1.588 mm
4.763 mm  (3/16")   2.381 mm       2.381 mm
6.350 mm  (1/4")    3.175 mm       3.175 mm
9.525 mm  (3/8")    4.763 mm       4.763 mm
12.700 mm (1/2")    6.350 mm       6.350 mm
19.050 mm (3/4")    9.525 mm       9.525 mm

The corner radius equals the tool radius at minimum. In practice, you want more than the minimum. Section 3 explains why.

2. The Upstream Decision

The tool radius compensation article covers what happens after you have chosen a tool — the double-offset technique that produces machinable corners. This section covers the upstream question: given the part geometry, what is the largest tool that can fully machine the pocket?

Read the part's external corners. The tightest external corner radius on the part determines the maximum endmill radius. If the part has a 2.0 mm external radius at a corner, the pocket must reproduce that radius plus clearance. The endmill radius must be no larger than the pocket corner radius.

Part's tightest external corner radius:  2.0 mm
Clearance:                               0.15 mm
Pocket corner radius at that point:      2.0 + 0.15 = 2.15 mm
Maximum endmill radius:                  2.15 mm
Maximum tool diameter:                   2 * 2.15 = 4.3 mm

A 4.763 mm (3/16") endmill is too large — its 2.381 mm radius cannot produce a 2.15 mm corner. A 3.175 mm (1/8") endmill works — its 1.588 mm radius is smaller than the required 2.15 mm. The pocket corner will be 2.15 mm (set by the double-offset), and the endmill can reach it.

For a part with sharp external corners (radius = 0), the pocket corner radius equals the clearance value alone — typically 0.10–0.25 mm. The endmill radius must be smaller than the clearance, which is impossible for any practical tool. In this case, the double-offset technique inserts corner radii equal to the endmill radius, and the part clears because its sharp corners fit inside the larger radiused pocket corners.

3. The 130% Guideline

When the pocket corner radius exactly equals the endmill radius (the minimum case), the cutter is 100% radially engaged at the corner. The tool is effectively slotting — the full diameter is in the cut. This produces maximum cutting force, maximum deflection, worst surface finish, and the highest risk of chatter.

Industry practice: size the pocket corner radius to at least 130% of the endmill radius. At 1.3x, radial engagement drops significantly, the tool has room to arc through the corner, and cutting forces are more uniform.

Corner radius / tool radius    Radial engagement    Notes
----------------------------------------------------------------------
1.0x  (minimum)                100% (full slot)     Max force, chatter risk
1.1x                           ~85%                 Marginal improvement
1.2x                           ~72%                 Acceptable for most work
1.3x  (guideline)              ~60%                 Good balance
1.5x                           ~45%                 Conservative, smooth finish
2.0x+                          ~30%                 Diminishing returns

For automated fixture generation, the tool selection algorithm targets the largest tool that satisfies the corner constraint with the 130% margin where possible. When the part geometry forces the tool into a tight corner at 1.0x, the double-offset still produces correct geometry — the machining is just harder on the cutter.

4. When Features Disappear

A part with a narrow protrusion — a thin fin, a mounting tab, a snap-fit clip — creates a narrow slot in the pocket. If the slot width is less than the endmill diameter, the tool cannot enter it. The pocket profile rounds off or removes the feature entirely.

OPJAW enforces a minimum edge length of 1.5 mm (matching a 1/8" endmill radius). Features smaller than this in the part profile cannot be faithfully represented in the pocket. The offset operations either collapse them or merge them into adjacent geometry.

This is a hard physical limit. A 3.175 mm diameter endmill cannot cut a 2 mm wide slot. The options are:

• Use a smaller endmill. A 1.5 mm endmill can cut the 2 mm slot, but cycle time increases dramatically — more passes to clear the same volume, more tool changes if roughing with a larger cutter first.
• Accept the feature loss. If the narrow feature does not affect part seating or clamping, the pocket can omit it. The part still drops in; it just has extra clearance where the feature was.
• Redesign the fixture strategy. Switch from a profile-following pocket to a bounding-box pocket or a different clamping approach that does not need to trace the feature.

5. When This Does Not Apply

• Through-pockets with no internal corners. An open-ended slot has no concave vertex to constrain the tool.
• Circular pockets. A round pocket has no corners at all — the tool traces an arc and the corner constraint is irrelevant.
• Wire EDM fixtures. Wire EDM produces arbitrarily sharp internal corners. The tool diameter constraint applies only to milling.
• Multi-tool strategies. Rough with a large endmill for volume removal, then finish corners with a small endmill. This eliminates the trade-off but adds cycle time, tool changes, and programming complexity. For high-volume production fixtures it can be worth it; for one-off workholding it rarely is.

For most CNC-milled workholding, the single-tool constraint applies. Pick the largest tool that fits the tightest corner, apply the double-offset technique, and the pocket is machinable as drawn.

Related articles:

• Tool Radius Compensation in Pocket Milling — what happens after tool selection.
• Pocket Depth-to-Width Ratio — tool reach constrains pocket depth.
• Clearance Fits for Workholding Pockets — clearance at corners.