Carbide Drill Speeds and Feeds: Practical Charts, Formulas and Machinist Tips

Drilling is usually the first operation that teaches a machinist respect for cutting data. Feed a carbide drill too gently and it rubs, work-hardens the surface and dulls within a few holes. Push it too hard and the corners chip before the first hole is finished. The comfortable window between those two outcomes is narrower for carbide than for high-speed steel, and that is exactly why carbide drill speeds and feeds are worth a few minutes of thought before the spindle starts turning.

We grind solid carbide drills for a living, so the same questions reach us every week from job shops, mould makers and aerospace suppliers. The answers are not complicated. They simply need to be applied in the right order, and then adjusted with what the chips and the spindle tell you.

Two Numbers Behind Every Drilling Cut

Speeds and feeds sound like one topic, but they are two separate decisions that solve two different problems.

• Cutting speed is how fast the cutting edge travels through the workpiece, expressed as surface speed (Vc, in m/min or SFM). It governs temperature at the edge.
• Feed per revolution (fn, in mm/rev or in/rev) is how far the drill advances in one full turn. It governs chip thickness and how much the edge is actually cutting rather than rubbing.
• Spindle rpm is not a free choice. It is calculated from surface speed and drill diameter, so a small drill needs far more rpm than a large one for the same Vc.

Carbide tolerates roughly two to three times the surface speed of high-speed steel in the same material. What limits carbide is rarely softening of the edge. It is heat concentrated in a very small contact zone, plus the brittleness that makes a chipped corner fatal within seconds.

The Formulas, in Plain Terms

Spindle speed from surface speed

In imperial units, rpm = (SFM x 3.82) divided by the drill diameter in inches. In metric units, rpm = (Vc x 1000) divided by (3.14 x drill diameter in mm). A 10 mm carbide drill running at 80 m/min therefore needs 80 x 1000 divided by 31.4, which is about 2,546 rpm.

Feed rate from feed per revolution

Feed rate in mm/min = rpm x feed per revolution. Staying with the same example, 2,546 rpm x 0.12 mm/rev gives roughly 306 mm/min. On a three-flute drill the same feed per revolution is shared across three cutting edges, so the load per edge is lower and hole quality usually improves in gummy materials.

If you would rather not run these numbers by hand for every tool in the crib, our drill speed and feed calculator with worked examples walks through the same formulas in both metric and imperial form.

Starting Ranges for Common Materials

The table below is the starting point we hand to customers who are moving from high-speed steel to solid carbide. It assumes a rigid setup, a drill with a length-to-diameter ratio of four or less, and coolant that reaches the cutting edge.

Reduce surface speed by 20 to 30 percent for long-reach tools, thin-walled parts, or a machine with noticeable spindle runout. When a stainless steel job starts to squeal, resist the reflex to slow the feed down. A feed that is too light is the most common cause of work hardening, and work hardening is what destroys the next drill as well as the current one.

Depth, Rigidity and Coolant Shift the Numbers

Hole depth and pecking

• Up to 3 x D: a single pass is usually fine with through-coolant or a well-aimed flood.
• 3 x D to 5 x D: peck in increments of about one diameter to clear chips cleanly.
• Beyond 5 x D: cut surface speed by 20 to 30 percent, shorten the pecks, and treat through-spindle coolant as mandatory rather than optional.

Tool holding and runout

Check total indicated runout at the drill tip, not at the holder face. Keeping it under 0.02 mm roughly doubles the life of a small carbide drill, because an off-centre edge carries almost all the load on one corner. Shrink-fit and hydraulic holders are worth the money on diameters below 6 mm.

Coolant

Through-spindle coolant reaches the tip where the heat is, so it supports the highest speeds in the table. Flood coolant works well for shallow holes in steel and stainless. Cast iron is often drilled dry with an air blast, while aluminium and titanium reward generous volume and pressure, since both materials move heat into the tool rather than the chip.

Read the Chips, Not Just the Chart

Chips are the cheapest feedback device on the machine, and they tell you which variable to change.

• Silver or light straw chips with a clean curl mean you are inside the working range.
• Blue or burnt chips point to surface speed that is too high, or coolant that never reaches the edge.
• Fine powdery chips in stainless steel mean the feed is too light and the edge is rubbing.
• Long stringy chips in aluminium call for more feed per revolution or a different flute geometry.
• Squealing plus material welded to the margin usually means speed is too high for the coating on the tool.

Matching the Drill to the Material

Cutting data only delivers results when the drill in the holder suits the job. Every tool we ship is ground and inspected on five- and six-axis machines at our factory in Changzhou, which is why we tend to talk about geometry before we talk about numbers.

A general-purpose solid carbide twist drill is the sensible default for carbon steel, alloy steel and cast iron across a wide diameter range.

NNZT Series General Purpose Solid Carbide Twist DrillsA versatile default for carbon steel, alloy steel and cast iron, with external or internal cooling and diameters up to 25 mm.View Product →

For mild steel and stainless steel, a geometry with a reinforced web and a sharper rake keeps the edge alive and reduces built-up edge on softer grades.

NNZB Series Solid Carbide Twist Drills for Mild Steel and Stainless SteelInternal-cooling 3D and 5D drills with sharp edges for mild and stainless steel, helping avoid built-up edge in diameters from 3 mm to 20 mm.View Product →

In cast iron and aluminium, a three-flute design clears chips faster and holds hole size better than a two-flute drill at the same feed per revolution.

NNZL Series Solid Carbide Three-Flute Drills for Cast Iron and AluminumNon-coated three-edge drills in external-cooling 3D and internal-cooling 15D types, suited to cast iron, aluminum alloys and faster chip clearance.View Product →

A Practical Setup Routine

1. Confirm the workpiece material and its actual hardness, not just the name on the drawing.
2. Pick a surface speed from the table and calculate rpm for the real drill diameter.
3. Choose feed per revolution based on drill size and flute count, aiming for a genuine chip rather than dust.
4. Measure runout at the tip before the first hole and correct it if it exceeds 0.02 mm.
5. Drill two or three holes in scrap or in a safe area, then inspect chip form, colour and hole size.
6. Adjust one variable at a time: speed first if the edge is burning, feed first if the drill is rubbing or squealing.

Questions We Hear Most Often

How fast should a 6 mm carbide drill run in mild steel?

Around 100 m/min is a safe starting point, which works out at roughly 5,300 rpm. Pair that with 0.10 to 0.15 mm/rev and a peck cycle once you pass about 18 mm of depth.

Why does the drill squeal and chip at the corner?

Squealing with corner chipping nearly always means surface speed is too high for the coating and the coolant supply. Drop the speed by 20 percent, confirm the coolant is hitting the tip, and check runout before assuming the tool is at fault.

Do I still need to spot drill?

On a flat surface with a solid carbide drill that has a 140-degree point, spotting is often unnecessary and simply adds a second operation. A spot is still useful on curved, angled or interrupted surfaces, or when a long drill needs help finding its position.

There is no single correct number for carbide drilling, only a sensible starting point and a short list of things to watch. Start conservative, listen to the machine, read the chips, and change one thing at a time. Do that consistently and the same drill will keep producing accurate holes long after a chart-only approach has burned through three of them.