Turns Out Error: Finding the Real Cause Before You Blame the Drill
A hole comes out oversized, tapered, or rough and the first reaction is to blame the drill. Most of the time the drill did its job and the turns out error came later, in reaming, boring, or the setup. This page is for machinists and process engineers who need to trace a turns out error back to its source instead of guessing.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
Turns Out Error: Symptom, Likely Cause, and Fix
Match the hole you measured to the row that fits, then work the fix from left to right.
| Symptom | Likely cause | How to handle it |
|---|---|---|
| Hole oversized by 0.03–0.08 mm | Drill lip height mismatch or chipped corner | Re-sharpen both lips equal; check runout under 0.02 mm |
| Hole tapered along depth | Drill walking on entry or weak setup | Spot drill first, shorten overhang, reduce feed at entry |
| Hole bell-mouthed at the top | Reamer chamfer rubbing or spindle float | Reduce reamer chamfer, check spindle runout, lower speed |
| Rough wall, Ra above 3.2 μm | Chip packing in flutes or wrong coolant | Increase coolant pressure, peck deeper, check flute wear |
| Hole out of position | Fixture shift or wrong work offset | Re-clamp, verify offset, probe the datum before cutting |
| Rounded or bell entry on reamed hole | Hand reamer fed too fast or misaligned | Use floating holder, feed 0.05–0.1 mm/rev, align to pilot |
| Hole size drifts across a batch | Thermal growth in spindle or part | Warm up spindle, cut, measure, adjust offset every 20 parts |
The Drill Is Rarely the Problem
Most turns out error cases trace back to reaming, setup, or heat, not the drill. Check the holder, the clamp, and the measurement before you touch the tool offset.
Drilling Creates the Hole, Not the Final Size
A twist drill is a roughing tool. It removes material fast and leaves a hole that is close to nominal, but the size and finish it produces are not what most drawings call out. A standard HSS or carbide drill typically holds IT13 to IT11, which on a 10 mm hole means a spread of roughly 0.05 to 0.22 mm. If the drawing asks for H7 or a tolerance of ±0.02 mm, drilling alone cannot get there.
This is where a turns out error often shows up. The operator drills, measures, sees the hole is 0.05 mm over, and adjusts the drill. The next part comes out 0.08 mm under because the drill wore or the material changed. Chasing size with a drill is a losing game. The drill sets the position and the stock left for the next operation, nothing more.
The practical rule is simple. If the hole tolerance is tighter than ±0.05 mm, or the surface finish must be better than Ra 3.2 μm, the drill is a pre-step. Plan a reamer or a boring bar from the start. That decision removes most of the confusion before the first chip is cut.
- 1Drill as pre-stepLeave 0.2–0.5 mm radial stock for reaming or boring.
- 2Check the tolerance firstTighter than ±0.05 mm means drilling alone will not hold it.
- 3Log the drill sizeRecord what the drill actually cuts, not its nominal diameter.
Reaming and Boring Fix Size and Finish
Reaming is a sizing operation. A reamer removes 0.1 to 0.3 mm of radial stock and produces a hole that is round, straight, and consistent. A floating holder is essential because a reamer follows the existing hole. If the holder is rigid and the spindle is off by 0.02 mm, the reamer will cut oversize and the hole will bell-mouth at the top.
Feed and speed matter. For a carbide reamer in 6061 aluminium, 0.05 to 0.1 mm per revolution at 300 to 600 rpm is a safe starting range. In 304 stainless, drop to 0.03 to 0.06 mm per revolution and use plenty of cutting fluid. Too slow a feed lets the reamer rub, which work-hardens the wall and pushes the size over.
Boring is the opposite approach. A single-point boring bar is adjustable and can correct position, size, and taper in one pass. It is slower and needs a rigid setup, but it is the only reliable way when the hole must be concentric with an outside diameter or when the bore is large. For bores above Ø20 mm, boring usually beats reaming on both accuracy and cost.
- 1Use a floating holderA reamer must follow the pilot hole, not fight it.
- 2Control the feedRubbing work-hardens stainless and opens the hole.
- 3Bore for positionSingle-point boring corrects concentricity and taper.
Setup Errors That Look Like Tool Errors
Many turns out error cases are not tool problems at all. A fixture that shifts under load will move the hole by 0.05 mm or more, and the drill gets blamed. Check the clamp pressure and the contact points. If the part rocks when you push it by hand, the setup is not stable enough for a tight hole.
Spindle runout is another common source. A spindle with 0.03 mm runout will cut a hole that is 0.03 mm over, no matter how sharp the drill is. Check runout with a dial indicator on a test bar before you touch the tool offsets. On a machine that runs 24 hours, thermal growth can add another 0.02 mm over a shift.
Work offsets matter too. If the datum was probed on a rough surface or the offset was entered from a worn edge finder, every hole in the batch moves. Probe the datum on a machined face, and re-check the offset after the first part. This one habit catches more errors than any tool change.
- 1Check clampingA part that moves under hand pressure will move under cutting load.
- 2Measure runoutSpindle runout adds directly to hole size.
- 3Probe on a machined faceRough surfaces give unreliable datum positions.
Material Behavior Changes Hole Size
Aluminium 6061 cuts clean and holds size well, but it galls if the coolant is weak or the flutes are polished smooth. Stainless 304 and 316 work-harden the moment a tool rubs, so a reamer that is fed too slowly will produce a hole that is both rough and oversized. Titanium Ti-6Al-4V is worse: it conducts heat poorly, so the edge temperature climbs and the drill wears on the corner first, which opens the hole.
Heat is the hidden variable. A hole drilled at 3,000 rpm in aluminium can grow 0.01 to 0.02 mm from thermal expansion alone. If you measure the part while it is still warm, the number is wrong. Let the part cool to room temperature before you record the size, or use a coolant-through tool to keep the temperature steady.
Plastics behave in the opposite way. POM and PEEK expand when they get warm and then shrink back, so a hole that measures on size when hot will be undersized when cold. For plastic parts, use sharp tools, high rake, and a feed that clears the chip without rubbing. Measure after the part has settled.
- 1Stainless work-hardensNever let the reamer rub; keep the feed up.
- 2Titanium wears the cornerCheck the drill corner before it opens the hole.
- 3Measure coldThermal growth of 0.01–0.02 mm is common on a warm part.
Measure the Hole the Right Way
A two-point micrometer or a plug gauge reads the diameter at one spot. A hole can be round at the entry and oval at the bottom, so one reading is not enough. Use a bore gauge or an inside micrometer at three depths: entry, middle, and bottom. If the three numbers differ by more than 0.01 mm, the hole is tapered and the cause is in the tool or the setup.
Surface finish needs its own check. A visual inspection will miss a wall that is Ra 2.5 μm when the drawing calls for Ra 1.6 μm. Use a portable roughness tester or compare against a known sample. Rough walls usually mean chip packing, a dull edge, or a feed that is too low.
Record the readings. A batch that drifts from 9.98 mm to 10.03 mm over 50 parts tells you the tool is wearing. That data lets you change the tool on schedule instead of scrapping parts when the hole finally goes out of tolerance.
- 1Check three depthsEntry, middle, and bottom catch taper.
- 2Verify finishUse a roughness tester, not a visual look.
- 3Log the driftTrend data tells you when to change the tool.
Step by Step: Trace a Turns Out Error
Work these in order. Stop as soon as the hole comes back into tolerance.
- 1Measure the hole at three depthsUse a bore gauge or inside micrometer at entry, middle, and bottom. Note the size, roundness, and taper. If the three readings differ by more than 0.01 mm, the error is in the tool or setup, not the drill.
- 2Check the drill runoutIndicate the drill shank or a test bar in the spindle. Runout above 0.02 mm will cut the hole oversize. Clean the taper and re-seat the holder before you change any offset.
- 3Verify the setup and clampingPush the part by hand. If it moves, the fixture is not holding. Re-clamp, check contact points, and probe the datum again on a machined face.
- 4Confirm the pre-drill size and stockFor a reamed hole, leave 0.2–0.5 mm radial stock. For a bored hole, leave 0.3–0.8 mm. Too little stock makes the reamer rub; too much makes it chatter.
- 5Adjust reamer or boring bar settingsCarbide reamer in aluminium: 0.05–0.1 mm/rev at 300–600 rpm. In 304 stainless: 0.03–0.06 mm/rev. Boring bar: take a 0.1–0.2 mm finishing pass at 0.05–0.1 mm/rev.
- 6Cut one part and measure coldLet the part cool to room temperature before measuring. Record size at three depths and the surface finish. Compare against the drawing before you run the batch.
- 7Log the result and set the tool lifeNote the tool, the offset, and the size it produced. Set a change interval based on the drift you saw, then re-check every 20 parts.
Common Questions About Hole Errors
Why does my reamed hole come out oversize?
The most common cause is a reamer that is not floating. A reamer follows the pilot hole, so a rigid holder forces it off line and it cuts oversize. Use a floating holder and check spindle runout.
The second cause is feed that is too slow. When the reamer rubs instead of cutting, the wall work-hardens and the size opens up. Raise the feed into the 0.05–0.1 mm/rev range for aluminium.
Can I hold a ±0.02 mm hole with drilling alone?
No. A twist drill typically holds IT13 to IT11, which is far wider than ±0.02 mm. Drilling sets position and leaves stock.
To hold ±0.02 mm you need a reamer or a boring bar. For the tightest holes, bore with a single-point tool and measure at three depths.
Why does the hole size drift across a batch?
Thermal growth and tool wear are the two usual causes. A spindle that warms up during a shift can move the hole by 0.02 mm or more.
Warm up the spindle before the first cut, measure the part cold, and adjust the offset every 20 parts. Log the drift so you can change the tool before it goes out of tolerance.
When should I bore instead of ream?
Bore when the hole must be concentric with an outside diameter, when the bore is larger than Ø20 mm, or when you need to correct position as well as size.
Ream when the pilot hole is already in position and you only need to size it. Reaming is faster, but it cannot fix a hole that is off location.
Why is the hole rough on the wall?
Chip packing in the flutes is the first thing to check. Increase coolant pressure and peck deeper so the chip clears.
If the chip is clear and the wall is still rough, the edge is dull or the feed is too low. Change the tool and raise the feed into the recommended range.
Does coolant type affect hole size?
Yes. Weak coolant or straight oil in aluminium can cause galling, which tears the wall and opens the hole. Use a water-miscible coolant with good lubricity for aluminium.
In stainless and titanium, coolant flow matters more than type. Keep the pressure high so the edge stays cool and the chip leaves the hole.
Send Us the Hole That Keeps Failing
Upload the drawing and the measurements you have. We will review the process and come back with a quotation and DFM feedback within 12 hours.
12-hour quote100% inspectionNo minimum order quantity
More CNC Process Notes
We publish setup notes, tooling trials and inspection data from the factory floor.
