Deep Hole Drilling Best Practices: L/D Ratio, Peck Cycles and Coolant Strategy Explained

Deep hole drilling is where most shops quietly lose money. A 3×D indexable drill that runs all day without trouble suddenly becomes a scrap generator at 8×D, and the failure mode is rarely the insert grade. It is chip evacuation, coolant pressure, runout and the feed schedule that decide whether the hole comes out straight or the drill comes out in two pieces.

This guide covers the practical side of deep hole drilling on CNC machining centres: how the length-to-diameter ratio changes the process, which tooling class fits which depth, how to set speed and feed, how to step (peck) safely, and what coolant pressure actually buys you. Starting values and comparison tables are included for steel, stainless and cast iron.

What “Deep” Actually Means: L/D Ratio Classes

The length-to-diameter ratio is measured from the insert or cutting edge to the start of the shank, not the overall tool length. A drill hanging 120 mm out of the holder with a 20 mm diameter is working at 6×D no matter what the catalogue says about its maximum depth.

The jump from 5×D to 8×D is the expensive one. Below 5×D, an indexable drill is rigid enough that the shank absorbs most of the bending moment. Above 5×D, the tool behaves like a beam: deflection grows with the cube of the overhang, and a 0.02 mm runout at the holder becomes a 0.1 mm walk at the tip.

Why Deep Holes Fail: Three Mechanisms

1. Chip Packing

At shallow depth, chips leave the flute by gravity and coolant flow. Beyond roughly 3×D, the flute is fully enclosed and every chip must be pushed back up the helix against its own weight and against the incoming coolant stream. If the chip is a long, stringy ribbon, it interlocks with the flute wall and the torque spike arrives within a few revolutions. The fix is not more coolant pressure alone — it is a chipbreaker geometry that produces short, comma-shaped chips at the chosen feed.

2. Thermal Growth and Built-Up Edge

A deep hole has no open end to dissipate heat, so the drill tip runs hotter than in a through hole. On steel, that pushes the insert toward the built-up-edge range. BUE welds to the margin, enlarges the effective diameter, and the hole tightens behind the drill. When the BUE breaks away it takes carbide with it — the classic “random” insert fracture that is actually a coolant and speed problem.

3. Guidance Loss and Hole Walk

A drill only self-centres while its margins are in contact with the wall. Once the margin wears or the pilot hole is oversize, the tool follows the path of least resistance and the hole drifts. On a 10×D hole, a 0.5° drift is over 1 mm of position error at the exit — enough to break through into a coolant gallery.

Speed and Feed Starting Values

Feed per revolution scales with diameter, because the drill must cut a chip thick enough to prevent rubbing at the margin but thin enough to keep torque within the shank’s capability. The table below gives conservative starting points for coated carbide indexable drills at 3×D, with through-tool coolant.

For solid carbide drills, reduce Vc by roughly 20–30 % in P and M groups and keep feed per revolution in the same band. Solid carbide wins on hole quality and centring, not on cycle time; the indexable drill removes three to five times the volume per minute at 3×D.

Depth Correction Factor

Deeper holes need a lighter feed, because chip evacuation time increases and the risk of packing rises. Apply a simple multiplier to the table values:

• Up to 3×D: ×1.00
• 3–5×D: ×0.90
• 5–8×D: ×0.80
• 8–15×D: ×0.65
• Above 15×D: ×0.50, with a dedicated deep hole cycle

Speed follows the same logic but more gently: reduce Vc by about 5 % per additional 2×D beyond 3×D. On stainless steel the correction matters more than on cast iron, because the heat stays in the cutting zone instead of transferring into the chip.

Pecking: When It Helps and When It Hurts

Peck drilling is often applied as a universal cure and often makes deep holes worse. Each retract costs time and, more importantly, each re-entry can chip the margin if the drill does not re-centre cleanly.

Use a peck cycle when the chip form is marginal, when coolant pressure is below the recommendation for the depth, or when drilling a material that work-hardens (stainless, nickel alloys). Do not use it on cast iron or aluminium with good through-tool coolant, where continuous feed keeps the chip engaged and the cycle shorter.

On work-hardening stainless, a full retract is not just about clearing chips: it lets the cutting edge cool below the work-hardening temperature before re-entry, which prevents the edge from skating on an already hardened surface layer. Keep the retract rapid rate moderate on long tools so the drill does not whip.

Coolant: Pressure Beats Volume

Through-tool coolant is the single highest-value upgrade for deep hole drilling. Flow rate clears chips; pressure determines whether the jet reaches the cutting edge at the bottom of the hole. A 10 bar pump feeding a 20 mm drill delivers almost nothing at 8×D.

Two practical notes. First, coolant holes in the tool are the bottleneck: a 1.5 mm internal channel at 200 mm length produces significant pressure loss, so pump pressure at the gauge is not pressure at the edge. Second, use a coolant ring or high-pressure holder rather than a standard side-entry holder — side entry at 5×D and beyond is effectively dry drilling.

Runout, Pilot Holes and Hole Quality

Total indicated runout at the drill tip should stay within 0.02 mm for solid carbide and 0.05 mm for indexable drills up to 3×D. Beyond 5×D, halve those numbers. Check runout at the tip, not at the shank — a holder can be perfect and the tool still bent.

A pilot hole is a compromise. It guarantees position but removes the drill’s ability to self-centre, so the pilot diameter should be at least 60–70 % of the final diameter and no deeper than 1×D. Spotting with a 90° spot drill is usually a better choice than a short pilot hole, because it leaves a conical seat the drill can follow.

Typical results to expect in P steel with an indexable drill at 3×D:

• Diameter tolerance: IT9–IT11
• Straightness: 0.05–0.15 mm per 100 mm
• Surface finish: Ra 3.2–6.3 µm
• Entry burr: present, needs chamfering or a secondary pass

For IT8 or better, plan a reaming or boring operation. No drill should be expected to hold a precision bore at depth.

Brand Comparison: Indexable and Exchangeable-Head Drills

In side-by-side tests on 42CrMo4 at 3×D, the practical differences come from geometry rather than grade. The stepped-shank designs reduce rubbing on the hole wall, which shows up as lower spindle load at the same feed. Exchangeable-head systems trade a little rigidity for a much lower cost per hole at small diameters, because there is no regrinding logistics. Above 5×D, the exchangeable-head options lose ground quickly; a dedicated deep hole drill with a single flute and a straight oil channel is the more reliable route.

Programming Notes

Use G81 (or G82 with dwell) for holes up to 3×D with through-tool coolant. Switch to G83 with a peck depth derived from the table above, and keep the retract plane above the part rather than at the last peck depth on holes beyond 5×D. On Fanuc-style controls, a typical block looks like:

G83 Z-95.0 R2.0 Q12.0 F0.18

where Q is the peck in millimetres. Set Q to about 1.0–1.5×D at 5×D depth, and check that the control’s chip-break retract does not pull the drill completely out of the hole on every peck unless you intended it — on some controls that behaviour is controlled by parameter, not by the cycle call.

For gun drilling and BTA work, the feed is programmed in mm/min with a separate coolant-on M-code delay, and the tool must be fed in at reduced rate until the bushing is engaged. Never rapid to depth.

Practical Checklist

• Measure L/D from the cutting edge to the shank, not the catalogue maximum.
• Match coolant pressure to depth, not to the pump’s rated maximum.
• Reduce feed by 10 % per 2×D beyond 3×D, and do not compensate with higher speed.
• Check tip runout with a dial indicator before blaming the insert grade.
• Use pecking for stainless and nickel alloys; skip it for cast iron and aluminium with good coolant.
• Break the edge at entry to avoid a burr that hides a cracked margin.
• Plan a boring or reaming pass whenever the drawing demands better than IT9.

Deep hole drilling rewards consistency more than it rewards aggressive parameters. A drill that is 10 % slower but never packs a chip will beat a fast one that stalls twice a shift — and it will do it with a fraction of the tool cost.