Milling Slots, Pockets, and Holes: Drilling, Reaming, and Boring on the Mill

Milling Slots, Pockets, and Holes: Drilling, Reaming, and Boring on the Mill

This lab brings together workholding, layout, cutting, and measurement into one complete exercise. You will machine three features — a rectangular pocket, a through-slot, and a reamed hole — in a 6061 aluminum blank held in a milling vise. Every feature must land within ±0.005 in of its print location, and the reamed hole must hit +0.0005 / −0.000 in of the specified diameter. That tolerance is tighter than most drill work, which is why reaming exists.

Safety First

Before touching the machine, review these non-negotiable points:

• Lockout/tagout (LOTO): Any time you change a tool, adjust the vise, or clear chips by hand, the spindle must be stopped and, for maintenance tasks, the machine locked out per your facility's LOTO procedure. Never reach into the work zone while the spindle is coasting.
• PPE: Safety glasses rated for machining (ANSI Z87.1 or equivalent) are required at all times in the shop. No gloves near rotating tooling — gloves can catch and pull a hand into the cutter.
• Chip management: Use a brush, not your fingers, to clear aluminum chips. Aluminum chips are sharp and can carry cutting fluid.
• Secure workholding: Confirm the vise is clamped to the table and the workpiece is seated flat on parallels before starting the spindle. A loose part becomes a projectile.
• Cutting fluid: Apply cutting fluid or mist when required. Aluminum can weld to tooling without lubrication, causing tool pull-out or broken cutters.

Establishing Work Zero with an Edge Finder

An edge finder is a two-piece spring-loaded tool that wobbles until it contacts a workpiece edge, at which point the tip snaps concentric with the shank. Spin it at roughly 500–1,000 RPM. Slowly feed the edge toward the workpiece. The tip will run true, then suddenly kick out — that kick-out point places the spindle centerline exactly one edge-finder radius from the part edge. Dial in X zero, then repeat for Y. Set both DRO axes to zero (or to the coordinate shown on the print) at that corner. All pocket, slot, and hole locations are then driven from this datum.

Drilling and Pilot Holes

Always drill a pilot hole before a large-diameter drill. The pilot should be at least as large as the chisel-edge width of the finish drill. This reduces thrust force and improves location accuracy. Use a center drill or spot drill first to give the twist drill a clean starting cone and prevent walking. Feed rates and speeds for 6061 aluminum are generous — a general starting point is surface footage of roughly 200–300 SFM with appropriate feed, though always follow the tooling manufacturer's data and your instructor's setup sheet.

Milling the Pocket

A rectangular pocket is milled in multiple steps:

1. If the pocket is larger than the cutter, use a series of overlapping passes (conventional or climb milling, per instructor direction for your setup).

2. Rough in stages, leaving 0.010–0.015 in of stock on walls and floor for a finish pass.

3. Plunge or ramp to depth in multiple depth-of-cut passes — do not reach full depth in one plunge with a standard end mill.

4. Take a finish pass at full depth on the walls and a finish pass on the floor to hit the depth tolerance.

5. Check pocket depth with a depth micrometer after each finish pass.

Climb milling (cutter rotation advances in the feed direction) generally produces a better finish in aluminum but requires a machine with minimal backlash. Follow your instructor's guidance.

Cutting the Through-Slot

A slot is essentially a pocket that runs through the workpiece. Key points:

• The slot width equals the end-mill diameter only on the finish pass. Rough with a smaller cutter or with offset passes, then take a final full-depth finishing pass to bring the width to size.
• Measure slot width with a telescoping gauge set to the slot opening, then transfer to an outside micrometer. Zero-in on your readings — the telescoping gauge technique requires practice; rock the gauge slightly to find the true maximum dimension.

Reaming the Hole

Reaming follows drilling. The sequence is: center drill → pilot drill → drill to near-final size (leave approximately 0.010–0.015 in for reaming in aluminum) → ream to final diameter. A chucking reamer is held in the spindle; a hand reamer is turned by hand with a tap wrench.

The critical rule: run the reamer at approximately half the speed used to drill the same material, and use cutting fluid. Reaming at high speed causes bell-mouthing and poor finish. Feed the reamer smoothly without dwelling. Never back-drag a reamer out dry — retract with the spindle still turning or lift out carefully.

Measure the reamed hole with a pin gauge set (go/no-go pins). The go pin of the specified diameter must enter freely; the no-go pin (0.0005 in over) must not enter. This confirms the +0.0005 / −0.000 in tolerance.

Measuring and Verifying Feature Locations

After machining, verify feature locations by:

1. Reading the DRO with the spindle centered over each feature (use an edge or a pin in the hole).

2. Confirming with a dial indicator run from a fixed edge of the vise jaw to the feature walls. This cross-checks DRO accuracy against a physical reference.

If any feature is out of tolerance, identify the cause (zero slip, backlash, tool deflection) before deciding on a corrective pass. Reporting the cause is part of your grade.

Surface Finish and Chatter

Chatter — a vibrating, chattering sound and a wavy surface — is caused by excessive depth of cut, loose workholding, worn tooling, or too much tool stickout. Reduce depth of cut, tighten the vise, shorten tool stickout, or reduce feed rate. You must identify and correct chatter before submitting your part.