Troubleshooting guide

CNC High Speed Drilling Problems and How to Fix Them

This guide covers the five failures we see most often in CNC high speed drilling: broken drills, oversized holes, chatter, poor surface finish, and wandering hole position. For each one we list the symptoms, the causes worth checking first, and the parameters or setup changes that usually clear it. Written for engineers and planners running small-diameter holes in aluminium, stainless, and steel.

Get Instant Quote Talk to an Engineer

Ø0.5–12 mm drills8,000–24,000 rpm±0.005 mm tolerance100% inspection

The current problems and solutions of CNC high speed drilling machines are as follows

On this page

1
Quick Diagnostic Table for CNC High Speed Drilling
2
What Makes CNC High Speed Drilling Different
3
Broken Drills: Runout, Peck, and Entry Conditions
4
Oversized Holes and Poor Position in CNC High Speed Drilling
5
Chatter, Finish, and Tool Life
6
When High Speed Drilling Is the Wrong Choice
7
Step by Step: Clearing a High Speed Drilling Problem

Symptom → cause → fix

Quick Diagnostic Table for CNC High Speed Drilling

Read the symptom in your scrap bin first, then work down the cause column.

Symptom	Likely cause	First action
Drill snaps at entry	Runout above 0.01 mm TIR	Dial in holder, replace collet
Hole comes out oversized	Point asymmetry or worn margin	Inspect point, swap drill
Ringing or chatter marks	Spindle speed too low, no peck	Raise rpm, add peck cycle
Rough hole wall	Feed per rev too high	Cut feed 20%, check coolant
Position drifts on second hole	Chip recut, poor chip evacuation	Add through-coolant, retract full
Burr at exit, hard to deburr	No backer, point angle mismatch	Add backer plate, use 118° point
Tool life under 200 holes	Surface speed above coating limit	Drop to 80 m/min in steel

Basics

What Makes CNC High Speed Drilling Different

High speed drilling means small diameter, high rpm, and short cycle time. A Ø3 mm carbide drill running at 18,000 rpm in 6061 aluminium is a different process from a Ø20 mm HSS drill at 900 rpm. The cutting edge sees far higher surface speed and far less time to clear the chip. That is where most problems start.

The margin between working and failing is narrow. A drill with 0.015 mm runout may still cut, but the hole will drift and tool life drops fast. On a 5-axis machine with a Ø400 mm rotary table, thermal growth in the spindle adds another variable over a long run. Keep an eye on the first ten holes and the last ten holes, not just the average.

We run 127 high-precision CNC machines, including 16 simultaneous 5-axis centers and 12 four-axis mills. Small-hole drilling jobs land on the 3-axis and 4-axis cells where spindle speed and rigidity are matched to the drill size. The troubleshooting steps below come from those cells.

1
Small drills fail fastA Ø1 mm drill breaks in milliseconds once runout or chip packing starts.
2
Chip evacuation is the limitAt high rpm the chip leaves the flute long before the coolant reaches it.
3
Heat stays in the toolShort engagement means the drill, not the part, absorbs most of the heat.

Problem 1

Broken Drills: Runout, Peck, and Entry Conditions

A drill usually breaks at the moment of entry or the moment of breakthrough. At entry, the point touches a surface that is not perfectly flat, so one lip bites first. The resulting side load snaps small drills. On a flat face within 0.02 mm, this is manageable. On a cast or welded surface, spot-drill first with a stub drill or a 90° spotter.

Runout is the other big cause. Measure it with a dial indicator on the drill shank just above the flutes. Keep total indicated runout under 0.01 mm for drills below Ø3 mm, and under 0.02 mm above that. If you cannot get there, the holder or collet is the problem, not the drill. Replace the collet before you touch the speeds and feeds.

Peck depth matters. In aluminium, a peck of 1×D works well. In 304 stainless or 4140 steel, drop to 0.5×D or less and use through-coolant if the drill has the channels. Full retract clears the chip; a partial retract at high rpm just recuts it. Recutting is the fastest way to break a Ø2 mm drill.

1
Check runout firstUnder 0.01 mm TIR for drills below Ø3 mm.
2
Spot on rough surfacesSkip spotting only on flat, machined faces.
3
Full retract on peckPartial retract recuts chips and snaps small drills.

Problem 2

Oversized Holes and Poor Position in CNC High Speed Drilling

If the hole is consistently 0.03–0.05 mm over nominal, look at the drill point before you blame the machine. An off-center point grinds unevenly and pushes the drill sideways. Under a toolmaker's scope, both lips should be equal in length and angle. A 118° point is a good general choice; use 135° or 140° for harder steels and thinner web strength.

Position error is different from size error. If hole one is on size and hole two drifts 0.05 mm, the cause is usually chip recutting or thermal growth. Let the spindle dwell for a second between holes on a long run, and confirm the coolant is actually reaching the tip. On deep holes, chip packing pushes the drill off axis in the last few millimeters.

Machine geometry also contributes. Check the spindle squareness to the table once a quarter. A small tilt shows up as a tapered hole, wider at the bottom. If the taper is more than 0.02 mm over 20 mm depth, stop and have the geometry checked before running more parts.

1
Inspect the pointEqual lip length and angle, no chipped corners.
2
Separate size from positionSize error points to the drill; position error points to chips or heat.
3
Watch the taperOver 0.02 mm over 20 mm depth means check spindle squareness.

Problem 3

Chatter, Finish, and Tool Life

Chatter in high speed drilling sounds like a high-pitched squeal and leaves a spiral pattern in the hole. It comes from a spindle speed that sits near a natural frequency of the setup, or from a drill that is too long for its diameter. The rule of thumb: keep the flute length under 8×D for high speed work. A 10×D drill needs a pilot hole and a lower surface speed.

Surface finish in the hole is set mostly by feed per revolution and coolant. In 6061 aluminium, 0.10–0.15 mm/rev at 15,000–20,000 rpm gives a clean wall. In 304 stainless, drop to 0.05–0.08 mm/rev and keep surface speed near 60–80 m/min. Pushing past that burns the margin and work-hardens the wall, which makes the next pass worse.

Tool life is the honest measure. Log holes per drill and note when the size starts to drift. In aluminium, a coated carbide drill should hold size for 2,000–5,000 holes. In stainless, expect 200–600. If you are far below that, the problem is speed, coolant, or runout, not the drill brand.

1
Keep L/D under 8Longer drills need a pilot and lower speed.
2
Feed sets finish0.10–0.15 mm/rev in aluminium, 0.05–0.08 mm/rev in stainless.
3
Log holes per drillSize drift is your early warning, not the sound.

When to change the process

When High Speed Drilling Is the Wrong Choice

High speed drilling is not always the best route. If the hole is deeper than 8×D, or the material is Inconel or Ti-6Al-4V, the margin gets thin. In those cases, a pilot hole followed by a slower drilling pass, or helical milling with a small end mill, gives better control. Helical milling also lets you hold position tighter because the tool engages the wall gradually.

If the hole needs a finish better than Ra 0.8 μm, drill first and ream or bore second. Drilling alone will not hold that finish in stainless. In aluminium, a good drill can reach Ra 1.6–3.2 μm as-machined, which is fine for most clearance holes.

For parts with many small holes, the setup cost of a dedicated drill cycle is worth it. For one-off prototypes, helical milling on a 3-axis machine is often faster than dialing in a small drill. Decide based on hole count and tolerance, not on habit.

1
Deep holesOver 8×D, switch to pilot plus slower drilling or helical milling.
2
Hard alloysInconel and Ti-6Al-4V drill slowly and work-harden; milling is safer.
3
Tight finishDrill then ream or bore for Ra 0.8 μm or better.

Fix sequence

Step by Step: Clearing a High Speed Drilling Problem

Work in this order. Most problems clear before step five.

1
Stop and inspect the drillPull the drill and check the point under a scope. Look for chipped corners, unequal lips, and a worn margin. A dull margin rubs instead of cutting and adds heat.
2
Measure runoutIndicate the shank just above the flutes. Target under 0.01 mm TIR below Ø3 mm and under 0.02 mm above. Replace the collet or holder if you cannot hit it.
3
Reset speed and feedAluminium: 15,000–20,000 rpm, 0.10–0.15 mm/rev. Stainless: 60–80 m/min surface speed, 0.05–0.08 mm/rev. Steel 4140: 80–100 m/min, 0.08–0.12 mm/rev.
4
Set the peck cycle1×D peck in aluminium, 0.5×D or less in stainless and steel. Use full retract. Enable through-coolant if the drill has channels.
5
Confirm coolant reaches the tipRun one hole with the door open and watch the stream. If the coolant hits the shank instead of the point, reposition the nozzle or switch to through-tool coolant.
6
Spot-drill rough surfacesUse a 90° spotter or stub drill to create a flat entry within 0.02 mm. This alone fixes many broken-drill complaints on castings and weldments.
7
Run a ten-hole testCheck size and position on the first three and the last three holes. If size drifts more than 0.02 mm over ten holes, the problem is thermal, not the drill.

FAQs

Frequently Asked Questions

What runout should I target for a Ø1 mm drill?

Keep total indicated runout under 0.01 mm on the shank just above the flutes. Below Ø1 mm, aim for 0.005 mm if you can measure it. Anything above 0.01 mm will drift the hole and shorten tool life sharply.

If your holder cannot hold that, the drill is not the problem. Change the collet or move to a hydraulic or shrink-fit holder.

Why does my hole come out tapered?

Taper usually means the spindle is not square to the table, or the drill is deflecting in a deep hole. Check squareness first. A tilt shows up as a hole wider at the bottom.

If geometry is fine, reduce peck depth and confirm chips are clearing. Chip packing in the last few millimeters pushes the drill off axis.

How many holes should a carbide drill last in 6061?

A coated carbide drill running at 15,000–20,000 rpm with good coolant should hold size for 2,000–5,000 holes in 6061 aluminium. In 304 stainless, expect 200–600 holes.

Log the count and watch for size drift. Drift is a better signal than sound or chip color.

Can I drill without through-coolant at high rpm?

Yes, but only on shallow holes in aluminium, around 3×D or less. Aim the external nozzle at the point, not the shank, and use a peck cycle with full retract.

For stainless, steel, or holes deeper than 3×D, through-coolant makes a large difference in tool life and hole quality.

What surface speed should I use in 4140 steel?

Run 80–100 m/min surface speed with a coated carbide drill, and feed at 0.08–0.12 mm/rev. Use a 135° or 140° point and through-coolant if available.

Drop the speed if you see discolored chips or hear the spindle load rise. Work-hardening in 4140 is less of an issue than in stainless, but heat still kills the edge.

When should I switch from drilling to helical milling?

Switch when the hole is deeper than 8×D, when the material is Inconel or titanium, or when position tolerance is tighter than the drill can hold. Helical milling engages the wall gradually and gives better control.

It is also a good option for one-off prototypes, where dialing in a small drill costs more time than it saves.

Send Us Your Drilling Problem

Upload your drawing and hole details. We will review the drill size, material, and tolerance, and come back with a quotation and free DFM analysis within 12 hours.

12-hour quote100% inspectionNo minimum order quantity

Get Instant Quote Talk to an Engineer

Follow our work