Problems and Solutions in the Machining of Deep Holes Using Machining Centers
Deep holes fail in predictable ways: chips pack at the bottom, the drill walks off center, coolant never reaches the tip. This guide maps each symptom to its real cause and to the cutting parameters that fix it. Written for machinists and process engineers running vertical and horizontal machining centers.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
Machining of deep holes: symptom, cause and correction
Match your symptom in the left column, then work the two columns to its right before you change any speed or feed value.
| Symptom | Likely cause | Correction |
|---|---|---|
| Squeal at 3–4 × D | Chip packing behind the flutes | Shorten peck depth, raise coolant pressure |
| Hole drifts off center | Drill runout above 0.02 mm | Indicate the drill, use a stub spot |
| Drill tip turns blue | Coolant never reaches the tip | Switch to through-spindle coolant |
| Chipped cutting edges | Peck depth too aggressive | Reduce first peck to 1 × D |
| Tapered hole | Tool deflection over long reach | Step drill, then ream or bore |
| Rough wall at entry | Chipped margin on the drill | Inspect margin, replace the drill |
| Broken drill at 6 × D | Chips jammed at the flute root | Full retract every 1–2 × D |
| Oversize hole 0.05 mm | Bent drill or worn margin | Check runout, ream to size |
The short version
Fix the setup before the program: runout under 0.02 mm, coolant pressure measured at the spindle, and a first peck at 1 × D. Most deep hole failures are setup failures wearing a cutting-parameter disguise.
Why the machining of deep holes behaves differently from shallow drilling
A hole becomes deep at roughly 5 × D for HSS drills and 8 × D for carbide. Past that depth, the flutes cannot lift chips out of the hole fast enough, and the coolant jet loses pressure before it reaches the tip. The drill is doing two jobs at once: cutting and conveying. When conveying fails, cutting fails shortly after.
The pressure drop is easy to underestimate. A 10 bar coolant line at the pump may deliver only 2–3 bar at the drill tip once the tool has 8 × D of flutes inside the hole. That is below the level needed to flush chips out of a tight flute space. Most deep hole failures start here, not in the feed rate.
The drill also deflects. A Ø6 mm carbide drill reaching 60 mm deep has an effective L/D of 10, and side load from an unbalanced cutting edge pushes it off axis. The hole goes oversize or drifts, and the next operation has to remove more material to correct it.
Setup checks before you touch the cutting parameters
Runout at the drill tip is the single largest cause of oversize deep holes. Indicate the drill 10 mm from the tip; keep runout under 0.02 mm for carbide and under 0.05 mm for HSS. If a holder cannot hold that figure, no feed change will fix the hole.
The spot drill sets the angle the drill follows. Its diameter should be slightly larger than the drill's web, not the drill's full diameter. A spot that is too small lets the drill walk; too large and the drill starts on a shallow cone it cannot control, which produces a bell-mouthed entry.
Coolant entry pressure needs measuring at the spindle, not at the pump. On a typical 40-taper vertical center, through-spindle coolant of 30–70 bar is the range where chips actually clear at 8 × D. Without through-spindle delivery, aim for 15–20 bar at the nozzle and accept a lower L/D ceiling.
- 1Runout targetUnder 0.02 mm for carbide, measured 10 mm from the tip
- 2Spot diameterSlightly larger than the drill web, not the full drill diameter
- 3Coolant pressure30–70 bar through-spindle for deep work; 15–20 bar at the nozzle otherwise
- 4Rigid workholdingVibration from the fixture shows up as a rough wall long before it shows up as a broken tool
Peck cycles and chip evacuation in the machining of deep holes
The first peck is the most important. Set it to 1 × D for a solid carbide drill, not the full flute length. Once the drill has a stable pilot in the hole, the following pecks can go to 1.5–2 × D, with a full retract every 3–4 pecks to clear the flute root.
On a Fanuc-style control, the deep hole cycle with full retract (G83) is the safer choice for the first 3 × D. The chip-breaking cycle (G73) works better once the hole is established and the chips are breaking cleanly, because it saves retract time without letting chips stack.
Retract clearance must exceed the chip pile. A retract that only clears the hole by 0.5 mm leaves chips in the entry, and the next peck pushes them back down. Set the clearance plane to at least 1 mm above the surface, and keep it there for the whole cycle.
If the drill squeals on the third or fourth peck, the problem is usually not the drill. It is the interval between retracts. Shorten the peck depth by 30 percent and listen for the sound change before you change the speed.
When to abandon drilling and use another process
At an L/D above 12, drilling with a standard twist drill stops being economical. The cycle time grows, the drill breakage risk climbs, and the hole still needs a finishing pass. Gun drilling or BTA drilling is the better route, but it needs a dedicated machine or a lathe with high-pressure coolant.
For holes that must be straight to within 0.02 mm over their length, helical milling with a small end mill is often a better fit on a machining center. The tool is stiffer than a drill of the same diameter, the hole is generated by the machine's interpolation rather than by the tool's geometry, and the wall finish is predictable.
Small holes under Ø2 mm with a depth over 5 mm are a separate case. They need high spindle speed, low feed per revolution, and a drill with polished flutes. If the machine cannot reach the recommended surface speed, the drill rubs instead of cutting and work-hardens the bottom of the hole.
The practical rule: drill first if the hole is under 8 × D and the tolerance is looser than ±0.05 mm. Above that, plan the process as a separate operation and budget the time for it.
A step-by-step recovery procedure for a failing deep hole
- 1Stop and measure the holeBefore changing anything, measure diameter at the entry, the middle and the bottom. A hole that is oversize at the top and on size at the bottom points to runout. An oversize hole all the way down points to a bent drill or a worn margin.
- 2Indicate the drill and holderCheck runout 10 mm from the tip. Push it under 0.02 mm for carbide. If the holder cannot repeat that figure, replace the holder before you touch the program.
- 3Reset the peck cycleFirst peck at 1 × D, then 1.5 × D, with a full retract every 3–4 pecks. Keep the clearance plane 1 mm above the surface for the entire cycle.
- 4Raise coolant pressure at the spindleMeasure at the spindle, not the pump. Go to 30–70 bar with through-spindle coolant. If the machine has no through-spindle option, reduce the L/D target instead of forcing the same drill deeper.
- 5Reduce surface speed by 20 percentCarbide in 4140 at 80 m/min is a reasonable starting point for deep work. Drop it and listen. A drill that stops squealing is usually running at the right speed for the setup.
- 6Check the drill margin and edgeLook for a chipped margin or a polished flank. A polished flank means the drill is rubbing, not cutting. Replace the drill and re-run the same parameters to confirm the fix.
- 7Add a finishing pass if neededIf the hole still misses the tolerance after drilling, ream to size or interpolate with a boring head. Reaming removes 0.1–0.3 mm and corrects roundness; boring corrects position and straightness.
Questions we get about deep hole drilling
What L/D ratio counts as a deep hole?
For HSS drills, 5 × D is the practical limit before chip evacuation and coolant delivery start to fail. Carbide drills with through-coolant can reach 8 × D with a proper peck cycle. Past 12 × D, gun drilling or BTA is the better route.
The number is a guide, not a wall. A Ø3 mm hole at 8 × D is harder than a Ø20 mm hole at 8 × D, because the flute space is smaller and the coolant jet loses more pressure over the same length.
Can a machining center drill a deep hole without through-spindle coolant?
Yes, but the L/D ceiling drops. Without through-spindle delivery, aim for 5–6 × D and use external coolant at 15–20 bar, aimed at the hole entry from two sides. The jet has to reach the tip, not just wash the top of the hole.
If the hole must be deeper than that on a machine without through-spindle coolant, split the operation: drill to 4 × D, then use a second setup with a longer drill and a lower surface speed.
Why does the drill squeal but the hole still measures on size?
Squeal is the drill rubbing rather than cutting, usually because the surface speed is too high for the coolant delivery you have. The hole can still measure on size while the wall finish degrades and the drill wears faster than it should.
Drop the surface speed by 20 percent and shorten the peck depth. If the squeal stops, the problem was the cutting condition, not the tool geometry.
How much material should be left for reaming?
Leave 0.1–0.3 mm on the diameter for a reamer, depending on the reamer size. Below 0.1 mm the reamer rubs and produces a poor finish; above 0.3 mm the reamer cuts unevenly and the hole goes out of round.
Reaming corrects roundness and finish but not position or straightness. If the drilled hole has drifted, bore it instead.
What causes a bell-mouthed entry on a deep hole?
A spot drill that is too large, or a drill that starts on a shallow cone it cannot control. The cutting edge engages on the cone's surface rather than on a centered pilot, and the entry opens up.
Match the spot diameter to slightly more than the drill's web, keep the spot shallow, and check the drill runout. The entry is the first place runout shows up.
Is helical milling better than drilling for deep holes?
For holes that must be straight to within 0.02 mm over their length, yes. Helical milling uses a stiffer tool and generates the hole by interpolation, so the result depends less on the drill's geometry.
The trade-off is cycle time. Helical milling a Ø8 mm hole 80 mm deep takes much longer than drilling it. Use it when the tolerance justifies the time, not as a default.
Send us your deep hole drawing
Upload the part and we will come back with a DFM analysis and a quotation within 12 hours. Deep holes, tight tolerances, and hard materials are routine work on our 5-axis and mill-turn centers.
12-hour quote100% inspectionNo minimum order quantity
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
