A hole becomes “deep” at the point where depth starts deciding the tool, the coolant delivery, and the chip-evacuation strategy more than feed rate and spindle speed do. In most shops that transition begins around 3:1 length-to-diameter and is hard to ignore by 5:1; at 10:1 and beyond, a standard twist drill with flood coolant usually stops being the obvious answer. The practical threshold depends on the machine, the material, and the required tolerance, so treat these ratios as tripwires rather than laws.
When a Hole Becomes “Deep”
Engineers usually talk about depth as a ratio of hole length to hole diameter (L/D). A 5 mm hole drilled 40 mm deep is an 8:1 hole; the same 40 mm depth in a 20 mm hole is only 2:1. Three problems grow as the ratio climbs:
- Chip packing. Chips that are not broken and flushed out pack against the cutting edges, stall the drill, or score the finished hole.
- Coolant starvation. Flood coolant cannot reliably reach the cutting zone once the hole is deep; heat moves up the tool and reduces tool life.
- Drift. A long, slender drill deflects, and the hole wanders from the intended axis before the tool gets deeper.
Short holes in forgiving materials can still be handled with peck cycles. The moment you are quoting an L/D of 8:1, 15:1, or higher, or a straightness requirement over a long depth, the drilling method itself becomes part of the design conversation.
Drilling Methods Compared
Three approaches cover most CNC work. The table summarizes how each one works and where it fits; the actual limits depend on the machine and toolmaker’s recommendations, so use them as starting points for a quote, not as guarantees.
| Method | Typical useful range | How it works | Where to use it |
|---|---|---|---|
| Peck drilling with a twist drill | Commonly workable up to roughly 5:1–10:1 depending on diameter and material | The drill retracts in short steps to break chips, re-enter, and let coolant reach the cut | Moderate depths in milling and turning centers with no special tooling |
| Gun drilling | High ratios, typically well beyond 10:1, on small- to medium-diameter holes | A single-lip tool with coolant delivered through the center; chips exit along a V-shaped flute | Long, straight holes such as oil passages, coolant lines, and guide holes |
| BTA (STS) drilling | Larger-diameter deep holes, usually on dedicated or high-pressure machines | A hollow drill head cuts while coolant pressure pushes chips back through the center tube | Large L/D work where straightness and repeatability matter most |
Gun drilling and BTA are not exotic only in aerospace. They are standard answers for valve bodies, manifolds, hydraulic blocks, and similar components with long internal passages. What looks like an expensive process choice on paper often costs less than fighting a wandering 15:1 twist-drilled hole, reworking it, or scrapping it.
Straightness, Roundness, and Finish by Method
The method largely sets what the drawing can honestly promise. Pecked twist-drill holes are the most economical but generally show the most straightness drift over long depths. Gun-drilled and BTA holes, run on properly supported setups with pilot bushings or guide sleeves, hold noticeably better straightness because the tool is supported near the cut and the process is designed for long engagement.
Diameter tolerance and surface finish are a separate question from straightness. A deep hole can be straight yet have a rough wall or a taper from tool wear. If the drawing demands a tight diameter tolerance, a precise surface finish, or a controlled bore diameter over the full length, plan a secondary boring or reaming pass rather than expecting the drilling operation alone to deliver all three. Our guide to boring and reaming precision holes explains how to sequence those passes.
Measuring a deep hole is harder than measuring a short one. Near the entrance, a three-point bore gauge or air gauge reads reliably; deeper in, small-diameter bores become difficult to reach, and straightness is often verified with fixtured indicators or, when the part justifies it, by sectioning or coordinate measurement. Confirm the inspection method with the shop before the part is made, not after it fails.
Coolant and Chip-Evacuation Realities
Flood coolant is usually not enough once a hole passes roughly the L/D where chips stop clearing by themselves. The practical options are through-tool coolant, high-pressure delivery, and, for gun drilling and BTA, coolant pressure that does the evacuation work as well as the cooling work.
The flow direction matters. In gun drilling, coolant travels through the center of the tool and chips escape along the exterior groove. In BTA drilling, coolant is delivered outside the tool and chips are pulled back through the center of the drill tube. That distinction changes machine requirements: BTA setups need a sealed delivery system and a chip-collection path, not just a high-pressure pump.
Coolant quality matters almost as much as pressure. Dirty coolant recirculates abrasive particles through the cut, and a blocked chip path stops progress immediately. Shops running deep-hole work at volume typically filter and monitor the coolant loop for this reason.
Calling Out Deep Holes on a Drawing
Deep holes are easier to quote and inspect when the drawing states the required result instead of assuming one process. Include the following in the hole callout or in the general notes:
- Diameter and tolerance. State what is measured where, especially if only part of the hole is functionally critical.
- Full depth and any depth tolerance. “Through” can mean several things when a hole breaks into a cavity at an angle.
- Straightness requirement. If the hole axis must stay within a zone over its length, say so with a straightness callout and a length reference.
- Surface finish inside the hole. Ra values on a deep internal wall are achievable only with the right sequence; the finish requirement should match the function.
- Lead-in and exit geometry. Spot drills, pilots, and edge breaks guide the tool and prevent ragged exits.
- Intersecting features. If a deep hole crosses another hole or a cavity, note deburr or edge-break expectations.
Choosing the method before the quote
A real-world comparison shows how the method decision follows the requirement. A hydraulic block needs a 4 mm passage drilled 100 mm deep — a 25:1 hole that a twist drill cannot hold straight. The drawing states the diameter, the depth, and the straightness, and the shop chooses gun drilling because the ratio and the straightness exceed what peck drilling can deliver; the part is drilled on a gun-drilling setup with a pilot and a bushing, and the straightness is verified over the full depth. A second block with a 20 mm hole at 60 mm depth — only a 3:1 ratio — is peck-drilled on a standard machining center, because the depth does not justify the special process. The two blocks look similar and are quoted very differently, and the difference is not a shop preference; it is the depth ratio, the straightness, and the finish driving the process. The engineer who brings the drawing and the function to the quote gets a method recommendation with the reasoning; the engineer who waits until the first trial part discovers the process through the rework.
The same logic applies when the hole is not the only feature. A mill-turn part with a deep passage and precision threads and bores may combine gun drilling with turning and machining in one setup, and the process sequence — drill, machine, and finish — should be planned so the deep hole does not distort the later features or the later machining does not close the hole. The quote should state the sequence and the inspection, because the deep hole’s straightness and the threaded features are verified at different points in the process. When the method, the sequence, and the inspection are planned before the quote, the deep-hole part is quoted as a complete process rather than as a collection of features — and the supplier’s price and the part’s quality both reflect the engineering that went into the method decision.
Confirm the pilot and the machine capability with the shop when the drawing is released, because the deep hole is only as good as the setup that supports it. At the quoting stage, share the drawing with the hole callouts and let the shop flag coolant, pecking, or piloting concerns before the setup is committed; a short review prevents the longest rework loop in the job.
If the geometry genuinely requires a gun-drilled or BTA feature, say that in the notes, but only when the requirement justifies it. A drawing that says “gun drill, 20:1” commits the shop to a process; a drawing that says “Ø0.250 in through 5.00 in, straightness 0.003 in over full depth” lets the shop choose the most reliable way to hit the result. When you are still choosing materials, depths, and tolerances, send the CNC machining team the drawing and the function of the hole early; the process decision is much easier before the quote than after the first trial part.