The Application Range of High-Speed CNC Drilling and Milling Machines
High-speed CNC drilling and milling is not one operation. It covers small hole patterns, deep pockets and long frames, each with its own spindle, feed and fixturing demands. This page shows which part geometry fits which machine setup, and where the process stops making sense.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
Key takeaways
Small holes and dense patterns: where high-speed CNC drilling and milling wins
A high-speed spindle earns its keep on hole patterns. When a plate carries 200 holes at Ø2 mm with ±0.05 mm position tolerance, the cycle time is dominated by how fast the tool can enter, retract and move to the next point. Spindle speeds in the 15,000–24,000 rpm range let a 2 mm carbide drill run at the surface speed the coating was designed for, instead of dragging at 6,000 rpm.
Peck depth matters more than raw rpm. For a 2 mm drill in 6061-T6, a peck of 1× diameter clears chips before they weld to the flute. In 304 stainless, drop to 0.5× diameter and add through-spindle coolant if the machine has it. Chips that stay in the hole are the main cause of drill breakage in deep small holes.
Entry and exit surfaces also decide the setup. Burrs form on exit when the drill pushes material instead of shearing it. A backing plate or a sacrificial layer under the part reduces exit burr to a light tumble. If the drawing calls for Ra 0.8–1.6 μm on the hole wall, plan a ream or a boring pass after drilling.
This range is where the process is clearly cheaper than EDM or laser. Below Ø1 mm with a depth over 10× diameter, the advantage flips. Tool deflection and chip evacuation get hard, and a drilled hole may need wire EDM to hold straightness.
- 1FitsHoles Ø1–6 mm, depth under 10× diameter, hundreds of positions.
- 2WatchChip packing in stainless and titanium; add peck and coolant.
- 3AvoidHoles under Ø1 mm deeper than 10× diameter.
Pockets, slots and thin walls: high-speed milling on the same machine
Faster spindles help milling as much as drilling, but the limit moves. A 6 mm end mill in aluminium can run at 18,000 rpm and 4,000 mm/min feed with a 0.5 mm radial step. That light radial engagement keeps cutting force low, which is what allows thin walls to survive the cut.
Wall thickness sets the rule. Below 1.5 mm in aluminium, the wall deflects under cutting pressure and the finished thickness varies along the depth. Two passes with a 0.3 mm radial step and a sharp uncoated tool hold ±0.05 mm better than one heavy pass. For walls under 0.8 mm, plan the milling sequence so the wall is supported by the parent material until the last pass.
Deep pockets behave the same way. When depth exceeds 4× tool diameter, tool holder runout becomes visible in the wall taper. A shrink-fit or hydraulic holder at 0.003 mm runout cuts taper by roughly half compared with a standard collet chuck. Air blast beats flood coolant in aluminium pockets because it clears chips without thermal shock.
Slots with a width under 1× tool diameter are a borderline case. Trochoidal paths at high rpm work, but the tool must be short enough to stay rigid. If the slot is deeper than 6× diameter and narrower than 3 mm, wire EDM is usually the safer route for the first article.
- 1FitsPockets to 4× diameter deep, walls 1.5 mm and up, aluminium and brass.
- 2WatchHolder runout shows up as wall taper on deep pockets.
- 3AvoidSlots under 3 mm wide and over 6× diameter deep.
Large frames and long parts: keeping one setup
Long parts are a different problem. A frame 2,000 mm long with bolt holes at both ends loses accuracy if it is drilled on one machine and milled on another. Every re-fixturing step adds position error. Machines with 4,000 × 400 × 150 mm travel drill, mill and tap the same frame without a second datum.
Thermal drift is the main error source on long cycles. A spindle running at 20,000 rpm for 40 minutes grows in Z by tens of microns. On a part with ±0.05 mm tolerance over 2 m, that is a real share of the budget. Warm-up cycles and in-process probing keep the drift visible before the finish pass.
Fixturing long thin frames is where most shops lose the tolerance. Vacuum tables hold flat parts well but release when the cutter breaks the seal around a through hole. Clamping from the outside distorts the frame between supports. A combination of vacuum zones and low-profile edge clamps keeps the part flat while leaving the cut area open.
Material choice changes the plan. Aluminium frames at 4,000 mm cut fast and move little. Steel frames at the same length need stress-relieved stock and a roughing pass before finishing, or the part warps after the clamps come off.
- 1FitsFrames and rails to 4,000 mm, drilled and milled in one fixturing.
- 2WatchSpindle thermal growth on cycles over 30 minutes.
- 3AvoidNon stress-relieved steel frames with tight flatness callouts.
Which materials actually benefit from high spindle speed
High-speed CNC drilling and milling pays off most in aluminium, brass and plastics. In 6061-T6, a coated carbide tool at 18,000 rpm removes material three to five times faster than at 6,000 rpm with the same tool life, as long as chip evacuation keeps up. Brass behaves similarly, though it grabs if the rake angle is wrong.
Stainless is a middle case. 303 and 304 cut at 8,000–12,000 rpm with good coolant flow. Higher speeds raise the heat at the edge faster than the coolant removes it, and edge build-up appears. 17-4PH in the H900 condition is harder again; speeds drop further and the tool change frequency rises.
Titanium and nickel alloys reverse the picture. TC4 (Ti-6Al-4V) and Inconel cut at low surface speed because the material conducts heat poorly and work-hardens under the edge. A 20,000 rpm spindle does not help roughing here. It does help finishing, where a small stepover and a fast feed keep the cutter in the cut and reduce rubbing.
Plastics sit at the other end. POM and PEEK cut cleanly at high rpm with an air blast, but heat builds fast and the chip welds back if the feed is too low. Keep the chip load per tooth above 0.05 mm and use a single-flute cutter with a polished flute for deep pockets.
- 1Best fit6061, 7075, brass, ABS, POM, PEEK.
- 2Middle303, 304, 17-4PH at reduced surface speed.
- 3Finishing onlyTC4, Inconel: high rpm for light finishing passes.
Matching part geometry to the right machine setup
Use this table when the drawing is open and you are deciding where the part should run.
| Part feature | Typical size | Recommended setup | Why |
|---|---|---|---|
| Dense hole pattern | Ø1–6 mm, 100+ holes | High-speed spindle, peck drilling | Fast point-to-point moves dominate cycle time |
| Deep small hole | Ø2 mm, 25 mm deep | Wire EDM or gundrilling | Tool deflection breaks drills past 10× diameter |
| Thin wall pocket | Wall 1.5 mm, depth 20 mm | High-speed milling, 0.3 mm radial step | Low radial force keeps the wall straight |
| Slot under 3 mm wide | 6× diameter deep | Wire EDM for first article | Tool rigidity limits high-speed milling here |
| Long frame | 2,000–4,000 mm | Large-travel machine, one setup | Avoids re-datum error between operations |
| Titanium bracket | TC4, ±0.02 mm | 3-axis roughing, 5-axis finishing | High rpm helps only the light finishing pass |
| Plastic housing | POM, deep pocket | High rpm, air blast, single flute | Clears chips without melting the wall |
When high-speed drilling and milling is the wrong answer
If the part is mostly holes under Ø1 mm deeper than 10× diameter, or slots narrower than 3 mm at 6× depth, send it to wire EDM or gundrilling instead of forcing it onto a high-speed spindle. If it is aluminium or brass with dense hole patterns, pockets and walls above 1.5 mm, high-speed CNC drilling and milling will beat every other process on cost and cycle time.
Questions engineers ask before quoting
What spindle speed counts as high speed for drilling and milling?
There is no fixed number. In practice, a spindle above 12,000 rpm with a balanced holder is where the process starts to behave differently from a standard 8,000 rpm machine. The useful range for small tools is 15,000–24,000 rpm.
What matters is surface speed at the cutting edge. A 2 mm drill needs far more rpm than a 12 mm drill to reach the same surface speed.
Can the same machine drill and mill the part without losing position accuracy?
Yes, and that is usually the point. Drilling and milling in one setup removes the datum shift that comes from moving the part between machines. Position tolerance stays inside ±0.05 mm on most parts.
The trade-off is cycle planning. A high-speed spindle is efficient at both, but deep roughing in steel is better done on a slower, higher-torque machine.
How do you control burrs on drilled holes?
Exit burrs are the common problem. A backing plate under the part, or a sacrificial layer, lets the drill shear the last material instead of pushing it out.
For holes that must be burr-free, add a chamfer pass with a small countersink or plan a light tumble after machining.
What tolerance can high-speed CNC drilling and milling hold?
On aluminium and brass parts, ±0.005 mm is achievable on critical features with in-process probing and a temperature-stable shop. Hole position across a pattern typically holds ±0.02 mm.
On titanium and stainless, expect ±0.01 mm on critical dimensions and wider tolerances elsewhere.
Is high-speed drilling and milling economical for one-off prototypes?
Yes, if the part geometry fits the process. Programming and setup dominate the cost on a single part, and the cycle time saving is small at that quantity.
Where it matters is when the prototype leads to a production run. The same program and fixture carry over, so the process step does not have to be re-qualified.
What drawing information do you need to quote this process?
Send a 3D model plus a 2D drawing with tolerances, material, surface finish and any hole depth callouts. Note which features are critical.
With that, we return a quotation and a DFM analysis within 12 hours, including any feature we recommend moving to another process.
Send us the drawing and we will tell you which process fits
Upload a 3D model and 2D drawing. We review the geometry, flag features that belong on another process, and return a quotation with DFM notes within 12 hours.
12-hour quote±0.005 mm tolerance100% inspection
More machining notes from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
