What Are the Hole Machining Methods?

• 1
  What matters before you pick a method
• 2
  Why hole machining methods differ from turning an OD
• 3
  The core hole machining methods and where each one fits
• 4
  Reading the drawing: which method fits the callout
• 5
  Sequencing hole machining methods on one part
• 6
  Step-by-step: machining a Ø10 H7 hole 40 mm deep in 4140 steel
• 7
  Hole machining methods compared

When you turn an outside diameter, the tool approaches from open space. You can see the cut, chips fall away, and the tool holder has room to be stiff. A hole gives you none of that. The tool diameter is capped by the hole diameter, so a Ø6 mm hole forces you into a small shank with limited rigidity. Deflection grows fast as length-to-diameter ratio climbs.

Chip evacuation is the second problem. In a blind hole, chips sit at the bottom until the flutes lift them out. Recutting a chip doubles the load on the cutting edge for a fraction of a second, which is enough to chip carbide or pull the drill off center. Through-coolant helps, but only if pressure is high enough to push chips up the flutes and out.

Heat is the third factor. A drill buried at 8:1 depth has almost no surface area for coolant to reach the cutting edge. The tip runs hotter than the shank, so it wears faster and the hole tapers. On a Ø10 mm hole 80 mm deep in 4140 steel, a 10 percent taper across the depth is not unusual if you run it in one pass without a peck.

That combination of low rigidity, trapped chips and trapped heat is why hole machining methods are staged. Each operation removes a controlled amount of material and makes the hole more accurate than the one before it. The sequence matters more than any single tool.

• 1
  Rigidity scales with the cube of diameterHalving drill diameter cuts stiffness by roughly eight times.
• 2
  Depth ratio drives tool choiceStandard twist drills handle 4:1 to 5:1. Parabolic or through-coolant drills reach 15:1 to 20:1.
• 3
  Tolerances are per-operationDrilling, reaming and boring each land in a different IT grade band.

Drilling is the entry operation for almost every hole. A twist drill removes material quickly but leaves a hole that is rarely round and rarely on size. Expect IT11 to IT13, which in aluminum means roughly ±0.08 mm and in 4140 steel roughly ±0.15 mm. Surface finish lands around Ra 3.2 to 6.3 μm. Use drilling when the hole is a clearance hole, a tapped hole, or a starting point for a later finishing pass.

Reaming follows drilling when you need a precise, round hole with good finish, and the hole already exists. A reamer removes only 0.1 to 0.3 mm on diameter, so it cannot fix a hole drilled badly off center. It holds IT7 to IT8 and Ra 0.8 to 1.6 μm in most steels. Reamers follow the existing hole, so if the drill wandered, the reamer follows the wander.

Boring uses a single-point tool on an adjustable bar. It removes small amounts of material, typically 0.2 to 0.5 mm on diameter per pass, and it corrects position as well as size. Because it is single-point, you can dial in a diameter to ±0.005 mm on a good machine. Boring also lets you stop mid-hole and measure, which is why it is the standard for bearing bores and hydraulic cylinders.

Milling a hole with a helical interpolation path is common when the hole is large and the tool list is short. A Ø12 mm end mill can open a Ø40 mm bore with a helical ramp, no special drill needed. The tradeoff is roundness. Interpolated holes tend to come out slightly lobed, and the finish depends on the machine's circularity. Use it for clearance and weight-reduction holes, not for press-fit bores.

Tapping is not a sizing operation, it is a threading operation. The tap follows the drilled hole, so the drill diameter controls thread height. For an M6 × 1.0 thread, the tap drill is Ø5.0 mm, which leaves about 75 percent thread engagement. Going oversize weakens the thread. Going undersize risks tap breakage, especially in 316 stainless or titanium.

• 1
  DrillingFast, cheap, IT11 to IT13. Roughing only.
• 2
  ReamingIT7 to IT8, Ra 0.8 to 1.6 μm. Needs a good pilot hole.
• 3
  BoringIT6 to IT7, corrects position and size. Slower per hole.
• 4
  Helical millingOne tool for many diameters. Roundness is the weak point.

The drawing usually tells you the method. A hole called out as Ø8.0 +0.05/0 with no other note is a reamed hole, because a drill cannot hold that band repeatably. A hole called out as Ø25 H7 is a bored or reamed hole, and at that diameter boring is usually cheaper because a Ø25 reamer is a special tool. A hole with a Ø6.8 callout next to an M8 note is a tap drill, and nothing more.

Depth ratio is the next gate. Below 4:1, standard twist drills work. Between 4:1 and 8:1, use a peck cycle or a parabolic flute drill, and expect to slow the feed by 20 to 30 percent. Past 8:1, you need through-coolant drills or a gun-drilling operation. Gun drilling holds straightness around 0.1 mm per 100 mm of depth, which is far better than a twist drill can manage.

Wall thickness matters as much as depth. If the wall between two holes is under 1.5 times the drill diameter, the drill will push the wall instead of cutting cleanly. You get bell-mouth, ovality and burrs on the far side. In that case, reduce feed, add a support plug, or move to helical milling, which has lower radial force.

Material sets the speed. Aluminum 6061 drills at 60 to 100 m/min surface speed. 304 stainless wants 15 to 25 m/min with generous coolant, and it work-hardens if you dwell. Titanium Ti-6Al-4V runs at 10 to 20 m/min with high pressure coolant and sharp edges. Inconel drops to 8 to 15 m/min and prefers peck cycles to clear chips.

Cross holes are the last thing to plan. A drill entering a curved or angled surface will walk before it bites. Spot with a center drill or an end mill flat first. On a cross hole through a cylinder, spot with an end mill to create a flat, then drill. That one step prevents most position errors we see on incoming drawings.

• 1
  Tolerance band tells you the methodTighter than ±0.05 mm means reaming or boring, not drilling.
• 2
  Depth ratio sets the toolPast 8:1, move to through-coolant or gun drilling.
• 3
  Spot every angled entryA flat from an end mill stops the drill from walking.

On a part with several holes, the order is not arbitrary. Drill all holes first, then ream or bore the ones that need it. Moving back and forth between drilling and finishing means more tool changes and more chances to lose position. Group operations by tool type.

If the part needs a flat face and holes, face first. Drilling into a rough face means the drill starts on a surface that is not perpendicular to the axis. The drill walks. A faced surface gives you a clean start and a repeatable depth reference.

Heat treatment changes the sequence. If the part is going to be hardened, do the roughing and drilling before heat treat, leaving 0.3 to 0.5 mm on diameter for a hard-milling or grinding pass after. Reaming a hardened hole is not practical. Boring with a CBN or ceramic insert after heat treat can hold the size, but the setup cost is higher.

Deburring belongs in the plan, not after it. A drilled hole leaves a burr on the exit side. If you ream after drilling without deburring, the burr can fold into the reamed surface and ruin the finish. Break the edges with a chamfer tool between operations, or add a back-chamfer step on the exit side.

For parts with many identical holes, consider a drill with a replaceable tip. It holds size longer than a reground twist drill and reduces the number of tool changes. On a 500-hole run in aluminum, the difference in cycle time is measurable, though the tool cost is higher per piece.

• 1
  Group by toolAll drilling, then all reaming, then all boring.
• 2
  Face before drillingA flat entry surface stops the drill from walking.
• 3
  Leave stock for heat treat0.3 to 0.5 mm on diameter for post-hardening finishing.
• 4
  Deburr between operationsA folded burr ruins a reamed surface.