Can You Drill Down with an End Mill? Safe Methods & Limits

Can you drill down with an end mill?

Yes—if the end mill is center-cutting (or specifically designed for plunging) and you use the right toolpath and cutting parameters. A standard non-center-cutting end mill should not be plunged straight down like a drill because it cannot clear chips at the center and is likely to rub, overheat, and break.

In practice, most shops avoid “true drilling” with an end mill unless the cutter and CAM strategy are chosen to manage chip evacuation (ramping, helical entry, or controlled peck-plunge). The deeper the hole and the tougher the material, the more important the strategy becomes.

When plunging with an end mill is appropriate

You need the right cutter geometry

• Use a center-cutting end mill (it has cutting edges that reach the center) or a purpose-built plunge/slot end mill.
• Prefer tools with good chip evacuation: fewer flutes (e.g., 2–3 in aluminum; 3–4 in steel) and polished flutes for gummy materials.
• Avoid plunging with long-reach tools unless necessary; increasing stick-out increases deflection and breakage risk.

The hole depth and material matter

Shallow plunges for entry (for example, starting a pocket) are often fine. Deep, drill-like holes are where end mills struggle: chips pack in the flutes, heat rises, and the tool can snap. As a rule, the closer you get to a “hole” that is more than a few tool diameters deep, the more you should favor helical interpolation or a real drill.

Best toolpaths for “drilling” with an end mill

Helical interpolation (most reliable)

Helical interpolation uses a circular motion while feeding down, so the end mill cuts more like a side-milling operation. This dramatically improves chip evacuation and reduces the rubbing that happens in a straight plunge.

• Use a helix diameter larger than the tool (common starting point: 1.05×–1.20× tool diameter) to create chip room.
• Limit axial stepdown per revolution to control load and keep chips moving.

Ramping entry (good for pockets)

Ramping feeds the cutter into the material at an angle (for example, 1–3 degrees) so the tool gradually engages rather than plunging at full axial engagement. This is commonly used to enter pockets without predrilling.

Straight plunge (only with plunge-capable tools and conservative settings)

A straight plunge is the highest-risk method because chips have limited escape paths. If you must do it, use a cutter designed for plunging and consider a peck strategy (short down moves with retracts) to clear chips.

Practical parameter guidelines that prevent breakage

Start with conservative plunge feed and stepdown

• Plunge feed: commonly 10%–30% of your normal side-milling feed as a safe starting range (varies by tool and material).
• Peck depth (if pecking): often 0.25×–1.0× tool diameter per peck, with retracts that actually clear chips.
• Coolant/air: chip evacuation is the main goal; air blast or through-spindle coolant is especially helpful for deep features.

Worked example: converting chip load to a safer plunge feed

Assume a 6 mm (0.236 in) 3-flute carbide end mill running at 10,000 RPM with a side-milling chip load of 0.03 mm/tooth.

• Side-milling feed = RPM × flutes × chip load = 10,000 × 3 × 0.03 = 900 mm/min.
• Conservative plunge feed at 20% = 900 × 0.20 = 180 mm/min.

This does not guarantee safety (geometry and chip evacuation dominate), but it provides a rational starting point instead of guessing.

Common failure modes and how to avoid them

Chip packing (the most common cause)

If chips cannot evacuate, they recut, generate heat, and wedge the tool. This is why a “drill-like” plunge is risky: chips have nowhere to go. Helical entry, air blast, and shorter pecks reduce chip packing.

Rubbing at the center

Even a center-cutting end mill has near-zero cutting speed at the exact center. Straight plunging increases the time spent cutting (or rubbing) at low surface speed, which drives heat. Keeping the tool moving laterally (helix/ramp) minimizes this effect.

Deflection and taper

End mills are less rigid than drills for axial loading. Deep plunges can produce a tapered or oversized hole and raise breakage risk. If hole accuracy matters, helical interpolation with a finishing pass is typically more predictable.

Better alternatives when you need a true hole

Use a drill when the feature is “hole-first”

If the goal is a round hole with depth, speed, and good finish, a drill is usually the correct tool. Drills are designed for axial loads and chip evacuation in deep holes.

Use helical interpolation when you need flexibility

Helical interpolation is ideal when you want to create multiple hole diameters with one tool, when you need to avoid tool changes, or when you need a hole in thin material without grabbing.

Pilot hole + end mill entry

A small pilot hole can provide chip space and reduce axial load when you must enter with an end mill. This is a practical compromise when CAM or machine limits make helical entry difficult.

Quick checklist for safe plunging

• Confirm center-cutting (or plunge-rated) end mill—do not assume.
• Prefer helical or ramp entry over straight plunging.
• Start plunge feed around 10%–30% of your side-milling feed, then tune based on chips and spindle load.
• If straight plunging is unavoidable, use pecking and ensure retracts actually clear chips.
• Use air blast/coolant to prioritize chip evacuation, especially in aluminum and deep features.
• Minimize tool stick-out and verify rigidity (holder, collet, runout) before attempting deep plunges.

1. Dry-run the entry move above the part to confirm the toolpath (especially for helical/ramp).
2. Cut a test feature in similar scrap and inspect chip shape and heat discoloration.
3. Adjust feed, stepdown, and coolant/air until chips evacuate cleanly and spindle load is stable.

Bottom line

You can drill down with an end mill, but you should treat it as a specialized operation. Use a center-cutting or plunge-rated tool, favor helical or ramp entry, keep plunge feeds conservative, and prioritize chip evacuation. If the feature is a deep, accurate hole, a dedicated drill (or a drill plus finishing strategy) is usually the safer and faster choice.