Processing Machines Treatment Holes: 5 Proven Ways
Holes are harder to hold than outside diameters. The tool is smaller than the bore it cuts, chips have to leave through the same opening, and runout shows up directly on the wall. This guide walks through five proven ways of processing machines treatment holes, the feed and speed ranges behind each one, and the checks that tell you when a method will not work for your part.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
Key takeaways
Why processing machines treatment holes differ from turning an outside diameter
On an outside diameter the tool is larger than the surface it cuts. A Ø50 mm face mill on a Ø40 mm boss has room to spare. A hole reverses that. To cut a Ø12 mm bore you must reach in with a Ø11.8 mm tool at most, and every chip you make has to exit through the same gap the tool entered. Chip evacuation, not cutting speed, is usually what limits the feed rate.
Rigidity is the second problem. A boring bar or long drill hangs out from the spindle like a cantilever. Deflection grows with the cube of the overhang length, so a bar at 4×D is roughly eight times softer than the same bar at 2×D. That is why long holes drift, bell-mouth at the entry, and measure smaller at the bottom than at the top.
Heat has nowhere to go either. In external turning the chips carry most of the heat away and the air helps. Inside a blind hole the chips sit in the bottom, the coolant has to be pushed in under pressure, and the tool rubs if the chip pack is not broken. Peck cycles exist for this reason, not as a habit.
Finally, runout shows up directly. A drill with 0.03 mm runout cuts a hole roughly 0.03 mm oversize, and the error is at the wall where the fit is measured. Check the holder before you blame the tool.
None of this makes hole work difficult in principle. It means the method has to match the depth, the diameter and the tolerance instead of being chosen by habit.
Drilling and peck drilling: the fastest ways for general holes
Twist drilling is the default for holes that only need to pass a bolt or a pin. On aluminium 6061 with a high-speed steel or solid carbide drill, a surface speed of 80–120 m/min and a feed of 0.15–0.25 mm per revolution hold a hole within ±0.05 mm. On 304 stainless, drop to 20–30 m/min and 0.08–0.12 mm/rev, and keep the drill cutting. Rubbing work-hardens stainless and the next pass gets harder.
Depth controls the cycle. Up to 3×D, a single plunge with through-tool coolant works. From 3×D to 5×D, peck with a retract of 1–2 mm to break the chip pack. Past 5×D, use a parabolic flute drill or a gun drill and peck at 0.5–1×D increments so the flutes clear before the next cut.
Common errors: entering on a slope or a curved surface without a spot, which walks the drill off center; running a stub drill to full depth, which jams chips; and skipping the spot on hard materials, which leaves a bell-mouth entry that a gauge will catch.
Spot depth matters too. A 90° spot about 0.5–1 mm deep is enough to guide the drill. A spot that is too deep leaves a cone in the bottom of a blind hole and steals depth from the thread.
Boring and reaming: holding size in processing machines treatment holes
Boring is a single-point correction. A boring head lets you dial the diameter in 0.01 mm steps and true the hole to the spindle, so it fixes position error that drilling left behind. Use 0.2–0.5 mm of radial stock for a finishing pass on aluminium, 0.1–0.2 mm on steel. A boring bar at 4×D with 0.15 mm/rev and 150–250 m/min on aluminium leaves Ra 0.8–1.6 μm reliably.
Boring is the wrong method for small holes. Below about Ø6 mm there is not enough bar stiffness, and the bar chatters before it cuts clean. Below Ø3 mm, boring is impractical and reaming or drilling to size is the only route.
Reaming removes the last 0.1–0.3 mm and holds H7 fits. Run a reamer at roughly two-thirds of the drilling speed and 0.5–1.5× the drilling feed per revolution. Never reverse a reamer out of a hole under power; it dulls the margins. Feed it through, stop the spindle, and withdraw.
Watch the first part. A new reamer cuts 0.005–0.015 mm oversize until it wears in, and a reamer that has been sharpened can cut undersize. Measure the first three holes, then set the offset.
Reaming will not fix a crooked hole. If the drilled hole is off-axis, the reamer follows the existing path and simply makes a straighter-looking error.
Thread milling, helical milling and interpolation
Helical interpolation cuts a hole with a smaller end mill on a circular path. It suits holes from Ø6 mm to Ø80 mm where you want one tool to cover several diameters and avoid a drill change. A Ø6 mm carbide end mill at 0.05–0.1 mm radial stepover and 0.1 mm/rev feed cuts aluminium cleanly. The trade-off is cycle time and the need for a machine with good circular interpolation accuracy.
Thread milling replaces tapping for large threads, blind threads and hard materials. One tool covers a range of diameters, the thread is cut rather than formed, and chip problems nearly disappear. Run at 100–200 m/min on aluminium and 40–80 m/min on stainless with a single-tooth or multi-flute thread mill.
For holes with a cross feature, or a port that meets another bore, interpolation lets you control the entry and exit so the cutter does not slam into the intersecting wall. Reduce feed by 30–50% through the interruption and keep the tool moving.
These five methods cover most work we see. The choice is not about which is better. It is about which one holds the tolerance your drawing calls out without adding a second operation.
Step by step: from print to a measured hole
- 11. Read the tolerance, not the diameterWrite down the tolerance class and the depth-to-diameter ratio before choosing a tool. A Ø10 mm hole at 2×D and the same hole at 8×D are different jobs.
- 22. Check the datum and the entry faceConfirm the entry is flat, or plan a spot. On a curved or sloped surface, spot with a 90° tool 0.5–1 mm deep or mill a flat first.
- 33. Pick the method from the tolerance band±0.05 mm: drill. ±0.02 mm: drill and bore. ±0.005 mm: drill, bore and ream. Interpolate when you need one tool for many sizes.
- 44. Set the speeds and feeds by materialAluminium 6061: 80–120 m/min. 304 stainless: 20–30 m/min. Titanium TC4: 30–50 m/min. Start at the low end and raise feed until the chip breaks.
- 55. Plan the chip pathFor depth over 3×D use through-tool coolant or a peck of 0.5–1×D. Reduce the peck distance as the hole gets deeper, not the feed.
- 66. Control the entry and the exitBreak the edge with a 0.2–0.5 mm chamfer or a countersink. On a through hole, back the feed off 30% as the drill breaks out to avoid a burr ring.
- 77. Measure the first part and adjustCheck diameter at the top, middle and bottom of the hole. A taper over 0.01 mm means the tool is deflecting or the coolant is not reaching the tip.
Method, tolerance and depth: what to use when
Ranges are typical starting points for aluminium, steel and stainless on 3-axis to 5-axis machines.
| Method | Typical tolerance | Depth limit | Best for | Watch out for |
|---|---|---|---|---|
| Drilling | ±0.05 mm | Up to 5×D with peck | Bolt and clearance holes | Walk-off on slopes; chip packing |
| Peck drilling | ±0.05 mm | 5×D to 20×D | Deep small holes | Slow cycle; tool rub if peck too long |
| Boring | ±0.01 mm | Up to 6×D | True position and size | Chatter below Ø6 mm; long bars |
| Reaming | ±0.005 mm | Up to 8×D | H7 fits, dowel and pin holes | Oversize when new; no position fix |
| Helical interpolation | ±0.02 mm | Up to 4×D | Many diameters, one tool | Cycle time; machine interpolation error |
| Thread milling | Class 6H typical | Up to 3×D | Large or blind threads | Feed errors show as thread flank marks |
Pick the method from the tolerance, not the habit
If the drawing asks for ±0.05 mm, drill and move on. If it asks for ±0.005 mm, plan a boring or reaming pass and budget the cycle time. Send us the print and we will tell you which of the five ways fits your hole.
Questions engineers ask before releasing a hole
What depth-to-diameter ratio is too deep for a standard drill?
Past 5×D a standard twist drill has trouble clearing chips and the flutes rub the wall. Move to a parabolic flute drill, use through-tool coolant, and peck at 0.5–1×D.
Past 15×D we switch to gun drilling or a dedicated deep-hole cycle, and we plan the coolant pressure before the job is quoted.
Why does my reamed hole come out oversize?
A new reamer usually cuts 0.005–0.015 mm over nominal until it wears in. Runout in the holder, a misaligned spindle, or feeding too fast will add more.
Measure the first three holes, adjust the tool offset, and cut a test part before the run. Do not reverse a reamer out under power.
Can I hold ±0.005 mm with drilling alone?
No. Drilling holds roughly ±0.05 mm on diameter and does not correct position. To reach ±0.005 mm you need a boring or reaming pass after drilling, plus a machine that holds its position.
We hold ±0.005 mm on reamed and fine-bored holes across our 3-axis, 4-axis and 5-axis machines.
When is thread milling better than tapping?
Thread milling wins on blind holes, large diameters, hard materials and any part where a broken tap would scrap the workpiece. One tool covers several diameters.
Tapping is faster for small through threads in aluminium, so we keep both routes available and pick by quantity and risk.
How do interrupted cuts change the parameters?
A cross hole or slot interrupts the cut and pulls the insert or edge. Reduce feed per tooth by 30–50%, keep the spindle speed steady, and make sure the tool is fully engaged before the interruption.
Rigid workholding matters more here than tool geometry. If the part moves, the edge chips.
Do you inspect every hole?
We inspect 100% of parts before shipment, including a raw material check, in-process monitoring and final inspection. Inspection reports are available on request.
For hole-critical parts we measure diameter at more than one depth so taper and bell-mouth are caught before shipping.
Send a drawing and get a hole process plan
Upload your STEP file and we return a quotation with free DFM analysis within 12 hours, including the drilling, boring or reaming route we would run.
12-hour quoteFree DFM analysis±0.005 mm on reamed holesNo minimum order quantity
More machining notes from GreatLight
We publish setup notes, tooling trials and inspection data from the factory floor.
