Home / Metal cutting / Drilling / Reference
Drilling is the operation with the fewest levers and the least forgiveness
Every field on the drilling tab, with its help text printed rather than hidden behind a hover. Read the note on surface finish first — it is the honest limit of what this operation can be calculated for.
Drilling — cut parameters
Worked example valuesISO 513 class. Sets base cutting speed and the Kienzle constants. Drilling is less tolerant of a wrong guess here than turning, because a drill that stops evacuating chips does not wear gradually — it jams and breaks.
Through or blind, and it changes the whole problem. A through hole lets the drill exit the far side, so chips have a clear path out ahead of it. A blind hole stops short of breaking through, and chips then have nowhere to go but back up the flutes past the cut that made them. That is why blind holes need peck cycles: not to reduce load, but to clear chips before they pack. A packed drill does not wear out gradually — it seizes and breaks, usually with the part still on the machine.
Sets spindle speed from cutting speed, and it appears squared in removal rate. It also drives the point allowance below, so an error here moves both your parameters and your cycle time estimate.
Quoted at the outer corner of the drill, where the cutting actually happens. It falls linearly to zero at the axis, so the chisel edge in the middle is not cutting at all — it extrudes material sideways under thrust. That region produces heat and axial force rather than chips, and it is why a web-thinned or split point outperforms a plain one so noticeably. Setting speed from the periphery is correct; just remember that a third of the diameter is doing something other than what the number describes.
Feed per revolution, shared between the lips. This is the single most common source of confusion on this tab: a two-lip drill puts half of this into each lip, so the chip each edge actually forms is half what the feed number suggests. Feeding as though one edge takes it all leaves you rubbing.
The included angle of the drill tip. 118° is the general purpose standard, 135° suits harder materials and self-centres better. It sets both the chip thickness per lip and the approach travel the tip needs beyond the programmed depth. Point geometry does more than that, though: web thinning, split points and flute form decide whether chips clear or pack, and packing is what breaks drills.
The programmed depth, measured as a flat bottom. The tool adds the point allowance to this for cycle time — the conical tip has to travel past the nominal depth to break fully through, and a depth reading that ignores it underestimates the cut.
Sets the rubbing floor, which belongs to the edge rather than the workpiece. A sharp uncoated HSS edge forms a chip at a thinner cut than a heavily honed coated carbide one. Treat the floors as conservative defaults — real edge preparation varies by grade.
Starting values for good conditions. Chip evacuation, not the parameters, is what usually decides whether a deep hole succeeds — peck where the depth exceeds roughly three diameters.
The relationships behind the fields
Knowing these tells you when a result is wrong.
Chip thickness per lip
h = (f / 2) × sin(point angle / 2)
Two things reduce it at once. The feed is split between the lips, then the point angle spreads what remains along the cutting edge. At 118° the sine term is about 0.86, so a 0.2 mm/rev feed produces a chip near 0.086 mm — well under half the feed figure.
This is why light feeds are more dangerous in drilling than anywhere else. The number on the control looks reasonable and the actual chip is under the rubbing floor.
Point allowance
approach = (D/2) / tan(point angle / 2)
The tip travels this far beyond the flat-bottom depth to break through. On a 12 mm drill at 118° that is around 3.6 mm — nearly a third of the diameter, and enough to matter on a short hole when you are costing a job.
It is added to hole depth for cycle time, not to the depth you program. It also lengthens the cut used for tool life, which is why the optimization needs it.
Cutting speed is not uniform
Vc at the periphery, zero at the centre
The quoted cutting speed applies at the outer corner. It falls linearly to zero at the axis, where the chisel edge does not cut at all — it extrudes material sideways under pressure. That region generates heat and thrust rather than chips, and it is why a web-thinned or split point drill outperforms a plain one so noticeably.
There is no surface finish model on this tab. Hole finish is governed by margin condition, runout, alignment and chip evacuation rather than by feed and a corner radius, so no theoretical Ra is reported. Saying nothing is more honest than reporting a number that has no mechanism behind it.
Run these numbersThe drilling calculator works out the chip each lip cuts, the travel the point adds, and the power the hole draws.
Open the calculator