Why a drill does not cut a flat bottom
A twist drill cuts a cone at the bottom of the hole. The axial distance from the tip to where the drill first reaches full diameter is the point length:
point length = (diameter ÷ 2) ÷ tan(included angle ÷ 2)
For a 118° point that works out to almost exactly 0.3 × diameter, which is where the familiar shop rule of thumb comes from; a 135° point is about 0.207 × diameter. So a 10 mm drill at 118° needs roughly 3 mm of extra travel before the hole is 10 mm wide at the bottom. Program the depth you want at full diameter and the hole comes out short.
Three depths this worksheet separates
Full-diameter depth is the usable depth: where the hole is still the nominal diameter. Tip depth is what you program, because the machine follows the tool tip. Point length is the difference between them.
For a through hole the full diameter has to clear the far face, so the tip travels the thickness plus the point length plus whatever breakthrough allowance you want. For a tap drill in a blind hole, the full-diameter depth must cover the thread depth, the tap's chamfer lead, and chip room below it.
Tap chamfer lead and chip room
A tap cannot cut full threads along its chamfer, so the hole has to be deeper than the thread depth. MSC's tap guide gives the usual leads: taper taps have 7 to 10 chamfered threads, plug taps 3 to 5, and bottoming taps 1 to 2. This planner uses the long end of each range and lets you override it, because leads vary between manufacturers — check the tap you actually have.
Chip clearance is separate and deliberately yours to set. A hand tap pushes chips ahead of itself into a blind hole; a spiral-flute tap pulls most of them back out. The default of two threads is a starting point, not a recommendation for your material.
Scope and limits
This is depth arithmetic, not a machining recommendation. Point length assumes a symmetrical, correctly ground point at the stated included angle. Web thinning, split points, worn or resharpened drills, and drills ground off-centre all change the real geometry — measure the drill when the depth matters. The planner does not choose feeds, speeds, peck cycles, coolant, or tap drill diameters, does not calculate thread engagement percentage, and does not know your fixturing or clearances. The depth-to-diameter advisory is a threshold you enter yourself; it is a common shop convention, not a published standard.
Using the result
- Confirm the drill's actual point geometry, or measure the point length and switch the input to measured.
- Enter the depth the print requires at full diameter, the material thickness, or the thread depth.
- For blind holes, enter the stock thickness so the worksheet can warn you before the point breaks through.
- Program the reported tip depth, remembering that your control measures from the tool tip.
- Take the printed worksheet or CSV to the machine with the setup sheet.
Drilling a bolt pattern? The bolt circle coordinate and G-code generator produces the hole positions and a review-first drilling cycle; this page gives the Z depth to use with it.
Frequently asked questions
Is the 0.3 × diameter rule accurate enough?
For a true 118° point it is accurate to better than a quarter of a percent, because (0.5 ÷ tan 59°) = 0.30. It is only right for 118°, though — at 135° the same rule would overstate the point by nearly half a millimetre on a 10 mm drill.
Should the breakthrough allowance include the point?
No. This worksheet adds the point length separately, so the breakthrough allowance is purely how far the full diameter travels past the far face. That keeps it meaningful when you change drills or point angles.
Why is my tap drill depth deeper than the usual rule?
A common shortcut adds three to five pitches to the thread depth. This planner splits that into the chamfer lead and chip clearance instead, so a plug tap with a five-thread lead plus two threads of chip room asks for seven pitches. Set the lead and clearance to match your tap and process if you want the shorter figure.
Does it work in inches?
Yes. Switch the units and the entered lengths convert. Threads can be given as a pitch or as threads per inch in either unit system, and a TPI figure is converted to a pitch in whichever unit is displayed.