CNC Drilling Techniques, Tips and Speed–Feed Calculator
Knowing the drill diameter alone is not enough to drill a good hole. The drill's suitability for the material, the hole depth, whether the surface is flat or curved, the ability of chips to escape, drill runout, cooling and the correct speed–feed must all be considered together.
This page explains, in a practical way, the topics a CNC operator faces every day in production: flat surface, inclined surface, curved part, cross-drilling a tube, cross holes, thin walls, aluminum, stainless, deep holes and exit burrs. At the end of the page, cutting speed, spindle speed, feed, material removal rate and drilling time are calculated with a single tool.
What does this page give a CNC operator?
Wrong drilling values do not only break the drill. They can also enlarge the hole diameter, push the hole off axis, create exit burrs, spoil the following reaming or tapping operation, and needlessly lengthen the cycle time. The goal here is for the operator to first recognize the problem, then choose the solution, and calculate last.
1. Drill selection: first diameter and depth, then tool type
The first question in drill selection should not be "which brand?" but how many millimeters diameter, how many diameters deep, which material and which hole tolerance? The L/D ratio, found by dividing the hole depth by the drill diameter, directly affects the tool type and the chip evacuation need.
Hole diameter
Rigidity drops at small diameters; power and torque needs rise at large diameters. The machine speed, power and toolholder must be checked.
Hole depth
A 2–3 × D short hole and a 10 × D deep hole are not machined the same way. As depth increases, internal coolant and piloting become important.
Material
Sticking and long chips in aluminum; work hardening in stainless; abrasiveness in cast iron; heat and low thermal conductivity in titanium are considered.
Hole quality
Diameter, straightness and surface expectations are tighter for holes before reaming, tapping or press fit. The tool type is chosen accordingly. Check how many microns the target IT grade is in the hole tolerance calculator.
| Drill type | General use | Common depth range | Advantage | Watch out for |
|---|---|---|---|---|
| HSS / HSS-Co drill | General shop work, low and medium speeds, manual or CNC use | About 2–5 × D | Tough, economical and re-grindable | Lower Vc than carbide; chip evacuation gets harder in deep holes |
| Solid carbide drill | Small–medium diameter, series production, tighter tolerance | About 2–8 × D | High speed, good straightness and hole quality | Sensitive to runout, clamping and impact |
| Replaceable-tip drill | Medium diameters and high productivity | About 3–10 × D | Fast tip change, body is reused | Tip–body connection, internal coolant and piloting must be correct |
| Indexable insert drill | Medium–large diameter and high material removal | About 2–5 × D | High feed and wide diameter range | Hole tolerance may not be as tight as solid carbide |
| Long / deep-hole drill | Holes of 8 × D and above | About 8–30 × D | Chip evacuation and straightness control at depth | A pilot hole, internal coolant and controlled entry are often required |
2. Drilling non-flat and difficult surfaces
If the two cutting edges of the drill do not take a balanced load at the same time, the tool is pushed sideways. For this reason, entering with the normal flat-surface feed on inclined, curved, tubular and interrupted surfaces is often not correct.
Drilling an inclined surface
- If possible, create a small flat or spot face on the surface.
- Start at about 25–50% of the normal feed at entry.
- Switch to normal feed after the full drill diameter is engaged.
- If the exit surface is also inclined, reduce the feed again at exit.
Curved part and cross-drilling a tube
- Support the part without crushing it but so it cannot rotate.
- Opening a spot face on the surface is the safest solution.
- If a spot face is not possible, use a short, rigid drill with good self-centering ability.
- Reduce the feed at entry and at the inner wall exit; be careful again as you approach the second wall inside the tube.
Cross hole and interrupted cut
- Reduce the feed by about 40–60% as you approach the intersection.
- Do not dwell in the interrupted zone; friction and corner chipping can increase.
- Prefer a short overhang and a tough cutting-edge geometry.
- Return to normal feed once the intersection is passed and full cutting resumes.
Concave surface and pre-drilled hole
- First create a flat centering surface or a suitable pilot hole.
- The spot drill point angle must be equal to or larger than the main drill point angle.
- If the existing hole is large, use boring, helical interpolation or a suitable enlarging tool instead of a standard drill.
- If only the outer edges cut while the center of the main drill does not engage the workpiece, breakage risk arises.
3. Material-specific drilling tips
ISO P – Steel
- Generally a balanced and predictable drilling material.
- Long, sticky chips can form in low-carbon steels.
- In high-carbon or hard steel, the cutting speed and feed may need to be reduced.
- The aim should be short, curled chips.
ISO M – Stainless steel
- Sharp, positive geometry and strong lubrication are important.
- Dwelling or a very low feed can cause friction and work hardening.
- The drill must cut continuously; it should not spin idle inside the hole.
- If chips get long, feed, geometry and cooling must be controlled together.
ISO K – Cast iron
- Chips are mostly short and dusty.
- Since the material can be abrasive, cutting-edge wear should be monitored.
- Unnecessary pecking is usually not needed.
- Dust and graphite should be kept away from machine slideways and measuring surfaces.
ISO N – How is aluminum drilled?
- A sharp, polished flute structure reduces sticking.
- Aluminum can be machined at high Vc; but chips must not jam in the flute.
- High-silicon aluminum is more abrasive; speed and tool quality must be chosen accordingly.
- Plenty of lubrication or directed air–coolant helps evacuate long chips.
- If burrs form at the exit, reduce the feed in the final zone and check the cutting-edge sharpness.
ISO S – Titanium and superalloys
- A low cutting speed, a steady feed and strong cooling are required.
- Heat concentrates at the cutting edge; dwelling and friction must be avoided.
- The tool overhang must be short and the clamping rigid.
- In deep holes, internal cooling and controlled chip evacuation are critical.
ISO H – Hardened material
- A suitable carbide grade and a rigid machine are required.
- A very low feed can create friction; stay within the tool manufacturer's range.
- Runout and vibration can quickly ruin the cutting edge.
- If hole hardness and the surface layer are not uniform, an interrupted load can occur.
4. Deep holes, chip evacuation and cooling
Up to 3 × D
In most normal applications chip evacuation is easier. With a suitable drill and cooling, continuous drilling can be done.
Between 3–6 × D
Chip packing, hole taper and heating become more noticeable. Internal cooling gives a big advantage.
6 × D and above
A pilot hole, a controlled low-speed entry and the tool manufacturer's long-drill procedure should be evaluated. Once the drill is fully aligned, switch to normal values.
When is pecking used?
- If long-chipping material and external cooling are used.
- If the flutes are filling or chips pack at the mouth of the hole.
- If a deep hole is being drilled with an HSS drill.
- Instead of a full retract on every peck, a small chip-breaking retract can be tried first.
When can pecking be unnecessary?
- If a modern internal-coolant carbide drill is normally designed for continuous drilling.
- In short-chipping cast iron.
- If frequent retraction creates thermal shock, time loss or carries chips back into the hole.
- If the tool manufacturer recommends uninterrupted drilling.
5. Hole defects: symptom, probable cause and solution
| Symptom | Probable cause | Check first |
|---|---|---|
| Hole diameter too large | Drill runout, long overhang, vibration, damaged edge, weak clamping | Tool runout, holder cleanliness, overhang, cutting edge and part clamping |
| Hole off axis | Inclined/curved entry, wrong spot hole, tool too long, uneven surface | Spot face, pilot angle, entry feed and tool rigidity |
| Hole tapered | Chip packing, tool wear, insufficient cooling, deflection | Coolant flow, chip shape, drill wear and L/D ratio |
| Excess burr at exit | High exit feed, dull cutting edge, thin wall, insufficient support | Reducing the feed at exit, sharpness, back support and point angle |
| Poor surface | Vibration, long chips, sticking, wrong cutting speed | Tool overhang, Vc, fn, lubrication and flute cleanliness |
| Drill corner chipping | Interrupted hole, wrong entry into a pilot hole, high feed, excessive runout | Cross-hole transition, pilot-hole diameter, entry feed and edge toughness |
| Chips jamming in the flute | Long chips, low feed, insufficient coolant, too much depth | Feed, chip-breaker geometry, internal coolant and pecking need |
| Drill making noise | Vibration, loose clamping, wear, wrong speed–feed | Toolholder, part clamping, overhang, cutting edge and machine bearings |
6. Drilling calculation formulas
The basic formulas below are for the metric system. In the calculator these formulas work together on a single screen.
Vc = (π × D × n) ÷ 1000
D: mm, n: rpm, Vc: m/min
n = (1000 × Vc) ÷ (π × D)
D: drill diameter
Vf = n × fn
fn: feed per revolution, mm/rev
Q = (π × D² ÷ 4) × Vf ÷ 1000
Q: cm³/min
T = L ÷ Vf
L: actual cutting distance, mm
h = (D ÷ 2) ÷ tan(θ ÷ 2)
θ: drill point angle
7. Drill speed, feed, material removal and drilling time calculator
The user can get a starting value by entering only the drill diameter, material, tool type and hole depth. If you have a Vc or fn value from a cutting-tool catalog, the value you enter in the relevant field is used instead of the automatic recommendation.
Result and solution advice
Quick summary for the operator
Safety and verification: The calculated values are general starting advice. The tool manufacturer's current catalog values, the machine manufacturer's limits, the toolholder capacity, part clamping, guards and workplace safety procedures take priority. Before using a new value directly in series production, a controlled trial, toolpath check and measurement should be done.