Process guide

CNC Drilling Treatment: A Step-by-Step Guide

This guide walks through the whole CNC drilling treatment sequence: setup, tool choice, speeds and feeds, breakthrough, and deburring. It is written for engineers and buyers who need holes that hold tolerance and pass inspection.

Get Instant Quote Talk to an Engineer

±0.005 mm tolerance12-hour quoteNo minimum order

CNC drilling treatment: five key problems in drilling holes

On this page

1
Key takeaways
2
What CNC drilling treatment covers
3
Matching the drill and coolant to the material
4
Workholding and zero-point decisions
5
Common defects and what causes them
6
Checking the hole before the part ships
7
CNC drilling treatment step by step
8
Drilling method selection by hole geometry

Quick answer

Key takeaways

Depth-to-diameter drives everythingUnder 4×D a standard twist drill works. Past 6×D you need peck cycles and coolant through the tool.

Spot first on curved or angled facesA 90° spot drill 0.5–1×D deep stops the drill from walking on castings and tubes.

Breakthrough is where holes go wrongCut feed by 30 percent in the last 1 mm to avoid exit burrs and drill snatch.

Deburr before inspection, not afterA 0.3–0.5 mm chamfer or abrasive flow pass keeps hole edges from failing a gauge check.

Rework rarely saves a bad holeOnce a drill wanders past 0.05 mm, welding or boring costs more than a fresh setup.

Step zero

What CNC drilling treatment covers

CNC drilling treatment means every operation applied to a hole, from the moment the drill touches the material to the moment the edge is clean and measurable. The drill itself is only part of it. Setup, spotting, chip evacuation, breakthrough control and deburring decide whether the hole lands at Ø8.00 mm or drifts to Ø8.12 mm.

It pays to know when drilling is the right call. A hole under 5×D deep with a diameter above 3 mm is usually faster drilled than milled. Deep, small holes, tight position tolerances or interrupted exits push you toward peck cycles, gun drilling, or a boring pass after drilling.

The tolerance you can hold depends on the operation chain, not one tool. Our general drilling window sits at ±0.05 mm on position and ±0.02 mm on diameter. Reamed holes hold ±0.005 mm. Those numbers assume the fixture is rigid and the material is consistent.

1
Standard twist drillBest for 3–20 mm holes up to 4×D in aluminium, mild steel and plastics.
2
Carbide drillHigher speed, less walk. Use on stainless, titanium and high-volume runs.
3
Reamer or boring headAdds a finishing pass when the drawing calls for H7 or ±0.005 mm.

Materials

Matching the drill and coolant to the material

Aluminium 6061 and 7075 cut fast, but they build a soft edge on the drill tip. Run 118° or 140° point angles, high spindle speed and generous coolant to clear chips. Without flood or mist, chips weld to the flutes and the hole size opens up within a few parts.

Stainless 304 and 316 work-harden the moment the drill rubs instead of cuts. Feed must stay above 0.08 mm/rev on Ø6 mm and larger, and the drill should not dwell in the cut. A dwell of even half a second at the bottom of a hole can raise surface hardness enough to blunt the next tool.

Titanium Ti-6Al-4V behaves similarly but conducts heat poorly, so the tool tip absorbs it. Keep cutting speed low, around 25–35 m/min for HSS and 50–70 m/min for carbide, and use high-pressure coolant. PEEK and other filled plastics drill clean at 1,500–3,000 rpm with sharp, polished flutes and air blast.

On castings, always check for a hard skin or a sand inclusion before drilling. A single hard spot will push the drill sideways and ruin position tolerance for the whole pattern.

Setup

Workholding and zero-point decisions

The fixture decides more holes than the drill does. Any part that moves 0.02 mm under thrust will show it as a position error across a bolt circle. Clamp directly over the hole when the geometry allows, or add a support jack under thin floors. A 5 mm aluminium plate with an unsupported centre will flex under a Ø10 mm drill.

Zero the tool on the fixture, not on a scrap part. Touch off the drill tip to the top face with a gauge block, then confirm the offset with a test hole in the same material. On a 16-station setup, a 0.03 mm offset error repeats on every hole in the program.

For parts held in a vise, check jaw lift. A worn vise can raise the part 0.05 mm on the fixed jaw side, which tilts the drill and makes an oval hole. A quick dial test on the top face before the run catches this in under a minute.

Record the fixture number, jaw position and torque value. When the job comes back next quarter, a repeatable setup saves an hour of trial cuts.

Problems

Common defects and what causes them

Oversize holes usually trace back to drill walk, runout or a dull tool. Measure the drill in the holder with a dial indicator before blaming the program. Runout above 0.03 mm at the tip will open the hole by roughly the same amount on the first entry.

Bell-mouth entry happens when the drill flexes as it starts the cut. A spot drill, a shorter stickout, or a lower feed for the first 1 mm fixes most cases. On soft aluminium, a sharp drill with too much feed pushes material ahead of the point and forms a raised lip instead of a clean edge.

Exit burrs are the most common inspection failure. They come from full feed at breakthrough, from a dull margin, or from a drill that grabs as it exits. Reduce feed, add a backing plate, and check the drill margin for wear every 50–100 holes in steel.

Chatter shows up as a lobed hole or a high-pitched noise. Reduce stickout, lower spindle speed by 10–15 percent, and increase feed slightly. If that fails, switch to a carbide drill with a stiffer shank and a corner chamfer.

Inspection

Checking the hole before the part ships

Inspect the first part fully and the last part fully. Between them, spot-check every tenth hole for diameter with a pin gauge and for position against the fixture datum. A pin gauge that enters with light drag is a pass; one that drops through is a warning sign on size.

Burr height calls for a loupe or a quick fingernail test on non-critical edges. For medical and aerospace parts, we photograph the hole edge under magnification and keep the image with the inspection report. Reports are available on request at no extra cost.

Threaded holes get a go/no-go gauge after drilling and tapping. Cross-holes get a bore-scope check when the intersection cannot be seen from outside. Both are standard steps in our process, not add-ons.

Execution

CNC drilling treatment step by step

1
1. Inspect stock and clean the faceCheck thickness and flatness against the drawing. Remove mill scale or sand with a face pass of 0.2–0.3 mm so the drill enters clean metal. A dirty face is the number one cause of drill walk.
2
2. Spot drill every holeUse a 90° spot drill at 0.5–1×D depth, feeding 0.05–0.08 mm/rev. On flat faces with a rigid setup, spotting can be skipped for Ø5 mm and under if position tolerance is looser than ±0.1 mm.
3
3. Select the drill and stickoutKeep stickout under 5×D where possible. A Ø8 mm drill hanging 60 mm out of the holder will chatter no matter what speed you pick. Shorten the holder or step up to a carbide drill with a shrink-fit shank.
4
4. Set speed and feed from the materialAluminium: 80–120 m/min, 0.15–0.25 mm/rev. Mild steel: 25–35 m/min, 0.10–0.20 mm/rev. Stainless: 15–25 m/min HSS or 45–60 m/min carbide, 0.08–0.15 mm/rev. Titanium: 25–35 m/min HSS, 50–70 m/min carbide, 0.05–0.12 mm/rev.
5
5. Program peck cycles for deep holesPast 4×D, peck at 1×D increments. Past 6×D, peck at 0.5×D and add coolant through the tool. Full retract clears chips; a partial retract of 1 mm is enough in aluminium with good flood coolant.
6
6. Control breakthroughDrop feed by 30–50 percent in the last 1 mm of cut. This cuts exit burrs and stops the drill from grabbing as it punches through. On thin plates, back the part with a sacrificial plate for the same reason.
7
7. Deburr and verifyChamfer 0.3–0.5 mm at 45° on both ends, or run abrasive flow for cross-holes. Then check diameter with a pin gauge, position with a CMM, and burr height under a 10× loupe before the part leaves the machine.

Choices

Drilling method selection by hole geometry

Pick the method from depth ratio and tolerance, then confirm tooling and cycle time.

Hole condition	Method	Typical tolerance
Ø3–20 mm, under 4×D, position ±0.1 mm	Standard twist drill, no spot	±0.10 mm
Curved or angled entry face	Spot drill first, then twist drill	±0.05 mm
4×D to 6×D deep holes	Peck cycle, carbide drill	±0.05 mm
Over 6×D deep, small diameter	Gun drilling or coolant-through carbide	±0.03 mm
H7 fit or ±0.005 mm bore	Drill undersize, then ream	±0.005 mm
Thin plate, exit burr critical	Backing plate plus reduced feed	±0.05 mm
Cross-hole or interrupted cut	Pilot drill, then mill or bore	±0.03 mm

When CNC drilling treatment is not the right answer

If the hole is deeper than 6×D, off-axis, or needs a bore under ±0.005 mm, plan for gun drilling, EDM or a reaming pass instead of pushing a twist drill past its limit.

Get Instant Quote Talk to an Engineer

FAQs

CNC drilling treatment questions

How deep can a standard twist drill go?

Up to 4×D in one pass with good coolant and a rigid setup. Between 4×D and 6×D, use a peck cycle at 1×D increments.

Past 6×D, switch to coolant-through carbide or gun drilling. Stickout, chip clearance and coolant pressure matter more than the drill brand at that depth.

Do I always need a spot drill?

No. Flat faces, rigid setups and position tolerances looser than ±0.1 mm can go straight to the drill. Spotting adds a tool change and cycle time.

Spot every hole on curved, angled or cast surfaces. It also helps when the drill is long or the material is hard, because the spot controls the first millimetre of cut.

What tolerance can CNC drilling hold without reaming?

±0.05 mm on position and ±0.02 mm on diameter is a realistic window in aluminium and mild steel with a good setup. Stainless and titanium run wider, closer to ±0.05 mm on diameter.

For H7 fits or ±0.005 mm bores, drill undersize by 0.1–0.2 mm and ream. Reaming is a finishing pass, not a drilling operation.

How do I stop burrs on a through hole?

Cut feed by 30–50 percent in the last 1 mm and back the exit side with a sacrificial plate. A sharp drill margin also matters; a worn margin rubs and pushes metal instead of cutting it.

Then chamfer 0.3–0.5 mm at 45° on both ends. For cross-holes, abrasive flow deburring reaches the intersection where a hand tool cannot.

Which materials are hardest to drill?

Titanium Ti-6Al-4V and Inconel are the toughest in our shop. They work-harden, hold heat at the tip and wear tools fast. Keep speeds low and feeds steady, and never let the drill dwell.

Stainless 304 and 316 come next. They drill fine with carbide and a feed above 0.08 mm/rev, but a light feed rubs and hardens the surface instead of cutting.

Can a bad hole be repaired?

Sometimes. Welding and re-drilling works on non-critical holes when the weld is allowed and the heat does not distort the part. Boring oversize to the next size is another option if the drawing permits it.

If the hole wandered past 0.05 mm or broke into a cross-hole, a fresh setup is usually cheaper than rework. We flag this in the DFM review before cutting metal.