All articles

Drilling and Tapping Cost: How to Estimate Holes and Threads

November 13, 2026

Quote parts like this from a drawing — try it on our sample. Try the sample drawingFree for 30 days · Unlimited quotes · No credit card required

Holes look like the cheap part of a drawing. A pocket or a contour gets a careful estimate; twelve tapped holes get "a few seconds each" and a shrug. On a plate, a flange or a housing, though, holes are often the largest share of the cycle time, and close to half of that time is not cutting at all: it is the machine moving between holes and changing tools.

This guide shows how to estimate drilling and tapping time from the drawing, hole by hole, which parts of it are fixed and which depend on the material, and how to turn the result into a price per part. The worked example in EUR times a steel plate with sixteen holes.

What a hole costs: four blocks of time

Every hole on a CNC machine is made of four blocks:

  • Cutting time. The tool travels the depth of the hole, plus an approach above the surface and, for a drill, the length of its point.
  • Positioning time. The rapid move to the next hole, the deceleration and the retract. A few seconds each, multiplied by every hole and every tool.
  • Tool changes. Spot drill, drill, chamfer, tap, perhaps a reamer: each change costs seconds per part, every part.
  • Extra operations per hole. A spot drill or chamfer before the drill, a reamer after it, a tap or a thread mill, a deburr on the exit side.

The cycle time estimation guide covers the general method. For holes the arithmetic is short enough to do by hand.

Drilling time from the drawing

Start from the spindle speed and feed that your tool supplier recommends for that drill and material:

  • spindle speed n (rpm) = 1000 × cutting speed (m/min) ÷ (π × diameter in mm)
  • feed rate (mm/min) = feed per revolution (mm/rev) × n
  • length = hole depth + approach (2 mm is common) + drill point, which for a 118° point is 0.30 × diameter
  • drilling time = length ÷ feed rate

Holes deeper than about three diameters usually need peck drilling, which adds retract time on every peck; above ten diameters it is a different process, covered in deep hole drilling cost.

Tapping time from the drawing

The tap drill for a coarse metric thread is the nominal diameter minus the pitch: 6.8 mm for M8, whose coarse pitch is 1.25 mm (ISO 261). With rigid tapping, the tap feeds exactly one pitch per revolution and comes back out the same way, so:

  • tapping time = 2 × (thread depth + approach + tap lead) ÷ (pitch × n)

Taps run at a fraction of the drill's cutting speed, which is why tapping is often the slowest operation per hole. In stainless steel or titanium it is slower again, and the risk of a broken tap in a nearly finished part belongs in the estimate too: a tap that breaks in the last hole can scrap everything done before it. Blind holes need the drill deeper than the thread, and the drawing has to say how many full threads are required.

Worked example: a plate with 12 × M8 and 4 × Ø10 through holes

A plate in S355, 15 mm thick, has twelve M8 tapped through holes and four Ø10 through holes. The cutting data are example values from a tool catalogue, not a recommendation: carbide drills at 80 m/min, 0.12 mm/rev for Ø6.8 and 0.15 mm/rev for Ø10; the tap at 10 m/min with a 2.5 mm tap lead (two pitches). Positioning is assumed at 2 seconds per hole per tool, a tool change at 6 seconds, a spot drill and chamfer at 2 seconds per hole.

OperationCalculationTime per part
Spot drill and chamfer16 holes × 2 s32.0 s
Drill Ø6.8 (tap drill)3,745 rpm, 449 mm/min, 19.0 mm → 2.54 s × 12 holes30.48 s
Drill Ø102,546 rpm, 382 mm/min, 20.0 mm → 3.14 s × 4 holes12.56 s
Tap M8 × 1.25398 rpm, 497 mm/min, 2 × 19.5 mm → 4.70 s × 12 holes56.40 s
Positioning44 hole visits (16 + 12 + 4 + 12) × 2 s88.0 s
Tool changes4 tools × 6 s24.0 s
Total243.44 s

That is 4.06 minutes per part, or €4.40 at a machine rate of €65/h: about €0.27 per hole. Two things stand out. Non-cutting time, positioning and tool changes, is 46% of the total: an estimate built only on cutting time would miss almost half the holes' cost. And the twelve tapped holes cost more than all the drilling put together.

Change the material and the tap time moves most. At 5 m/min, an assumed reduction for a tap in stainless steel, each M8 takes 9.41 seconds instead of 4.70 and the cycle grows by 56.5 seconds, before any allowance for tap breakage.

What changes the price of a hole

  • Tolerance on the hole. An H7 hole needs a reamer or a boring pass after the drill: one more tool, one more visit per hole. See how tolerances drive cost.
  • Thread size and type. Small threads (M3, M4) break taps; large ones (above M20) may be faster and safer to thread-mill.
  • Blind or through. Blind holes need chip clearance and a depth check.
  • Holes on several faces. Every extra face is a setup, or a rotary axis. The holes themselves are cheap compared with the setup time they cause.
  • Count. Because positioning and tool changes repeat per hole, a drawing with many small holes costs more per hole than one with a few large ones.

Quoting with a time per hole

Once you have timed a few parts like this on your machines, you can quote most parts with a standard time per hole type: so many seconds per drilled hole, so many per tapped hole, per reamed hole, per counterbore, by material group. Set those standards from measured cycles, not from the catalogue alone, and check them again after the next batch.

FAQ: drilling and tapping cost

How do you calculate drilling time? Spindle speed n = 1000 × cutting speed ÷ (π × diameter). Feed rate = feed per revolution × n. Drilling time = (hole depth + approach + drill point length) ÷ feed rate. Add positioning between holes and the tool changes, which on small holes can be nearly half of the total.

How do you calculate tapping time? With rigid tapping the tap advances one pitch per revolution and returns the same way, so tapping time = 2 × (thread depth + approach + tap lead) ÷ (pitch × spindle speed). Taps run much slower than drills, and slower again in stainless steel or titanium.

How much does a drilled or tapped hole cost? It depends on diameter, depth, material and how many holes the part has. In the example in this article, sixteen holes in a 15 mm steel plate take about four minutes, about €0.27 per hole at €65/h, with the tapped holes costing more than the drilled ones.

Why do many small holes cost more per hole? Because positioning and tool changes are paid on every hole and every tool, whatever the size of the hole. On small, shallow holes they can take more time than the cutting itself.

Holes and threads in QuoteBuddy

QuoteBuddy reads the technical drawing and counts its features, including drilled holes and tapped threads, then turns each count into machining time with the minutes per feature that you set for each process in Shop setup. Setup is kept apart from cycle time, CAM programming is a separate line, and every operation is priced at your shop's hourly rates. If you edit an operation's time or rate, the line is kept when the estimate is recomputed, so your measured standards stay in the quote. Several quantities on one estimate show how the unit price moves with the batch.

You can watch the QuoteBuddy demo video, from technical drawing to quote. To try it on a drawing of your own, start a free 30-day trial.

We use cookies
We use essential cookies to run QuoteBuddy. With your consent, we also use analytics and marketing cookies. Privacy Policy.

UI build: 9a5f2a06cb797e4f7d25d226434db4cb87c72c48