Calcady™
Home / Trade / Manufacturing / Drill Point Breakthrough Depth

Drill Point Breakthrough Depth

Calculate the exact total Z-depth required for a drill to fully breakthrough material, accounting for the conical tip length and additional clearance.

Drill Setup & Material

⚠️ MACHINING INSIGHT: Standard 118-degree jobber drills have a significantly longer tip than 135-degree split-point drills. If you program your CNC using the nominal material thickness, the angled tip will leave a conical burr at the bottom of the hole. Properly accounting for tip length and clearance ensures a clean breakthrough.

Exact Total Z-Depth

0.0000 in
Total required vertical stroke.

Drill Tip Length

0.0000 in
Length of the cutting point alone.
Email LinkText/SMSWhatsApp

What is Drill Point Geometry & CNC Z-Depth Programming?

A twist drill does not have a flat cutting end — it has a conical tip defined by the drill's included point angle. This means the drill must travel significantly further than the nominal material thickness to produce a full-diameter hole all the way through. The extra distance the tip must travel after the cutting edge reaches the exit surface is the 'tip length'. Failing to account for this in your Z-depth programming leaves a conical stub of undrilled material, causing taps to crash and bolts to jam.

Mathematical Foundation

Drill Tip Length (L_tip)
Ltip=D/2tan⁡(θ/2)L_{tip} = \frac{D/2}{\tan(\theta/2)}
LtipL_{tip}= Length of the conical drill point from the true lip corner to the absolute tip (inches or mm).
DD= Drill diameter (inches or mm).
θ\theta= Drill included point angle (degrees). Standard jobber = 118°. Split point = 135°. Spot drill = 90°.
Total Z-Depth
Ztotal=Tmaterial+Ltip+CclearanceZ_{total} = T_{material} + L_{tip} + C_{clearance}
ZtotalZ_{total}= Total Z-axis stroke programmed in the CNC canned cycle (G81/G83).
TmaterialT_{material}= Nominal material thickness.
CclearanceC_{clearance}= Additional safety clearance (typically 0.050' / 1.27mm) ensuring full diameter cleanup.

Laws & Principles

  • 118° Standard Jobber Drill: The original general-purpose drill geometry. At 118°, L_tip ≈ Diameter × 0.300. For a 1/2-inch drill, the tip is 0.150' long. Standard jobber drills tend to walk, so they often require a center drill pilot.
  • 135° Split Point Drill: Designed for harder materials and CNC use. The wider angle results in a shorter tip length (L_tip ≈ Diameter × 0.207). The split-point web geometry self-centers on the material, eliminating the need for a prior spotting operation.
  • 90° Spot Drill: Has a very steep tip (L_tip = Diameter × 0.500) designed solely to create a starting dimple for other drills or to create a chamfer before drilling. Spot drills should NEVER be used to break through a part, as the long tip will drill straight into the machine table or vise holding the part.
  • Clearance Rules: A drill's cutting lips are not perfectly flat across. They have a slight back-taper to provide relief. If you plunge exactly to material thickness + tip length, the very outer corner of the lip may still be engaged. You must add 0.050' (1.5mm) of absolute clearance to guarantee the hole pops cleanly through.

Step-by-Step Example Walkthrough

" Programming a G83 peck drilling cycle to put a through-hole in a 1.000' thick 6061 aluminum plate. The tool is a 1/2-inch (0.500') standard 118° HSS drill. "

  1. 1. Identify constants: D = 0.500', Angle = 118°, Thickness = 1.000'.
  2. 2. Calculate Tip Length: L_tip = (0.500 / 2) / tan(118° / 2) = 0.250 / tan(59°).
  3. 3. Compute tan(59°): ~1.664.
  4. 4. L_tip = 0.250 / 1.664 = 0.150'.
  5. 5. Add clearance: 0.050' standard safety margin.
  6. 6. Calculate Total Depth: 1.000' + 0.150' + 0.050' = 1.200'.
Final Result: To get a clean through-hole, the CNC program must be: G83 Z-1.200 R0.1. The difference between Z-1.000 and Z-1.200 is the difference between a ruined part and a passing part. Programming Z-1.000 leaves a 0.150' conical burr blocking the hole.

Quick Answer: How deep should I program my CNC drill?

To achieve a full through-hole, you must drill deeper than your material thickness to account for the drill's conical point. Enter your drill diameter and point angle (typically 118° or 135°). This calculator provides the exact Tip Length to add to your material thickness, plus a standard clearance buffer, giving you the final Z-total depth for your G-code programming.

Core Drill Point Formula

Tip Length (L_tip)

L_tip = (Diameter ÷ 2) ÷ tan(Angle ÷ 2)

The tangent function converts the angle geometry into a linear Z-axis depth. Remember to use the radius (Diameter/2) and the half-angle (e.g., 59° for a 118° drill) when doing manual calculations.

Real-World Scenarios

✓ Safe Vise Clearance

A machinist sets up a 2-inch thick steel block on 0.125" parallels in a Kurt vise. He needs to drill a 3/4" (0.750") hole with a 118° drill. He runs the calculator and finds the tip length is 0.225". Adding 0.050" clearance, his Z-depth is Z-2.275". Because his depth exceeds his 0.125" parallels, he realizes the drill tip will plow 0.150" deep into the hardened vise bed! He stops, swaps in taller 0.500" parallels, and saves a $1,500 vise from destruction.

✗ The Broken Tap Disaster

An operator uses a 5/16" (0.3125") drill to prep for a 3/8-16 tap in a 1-inch thick aluminum plate. He ignores the 135° tip length and simply strokes the drill to exactly Z-1.000". The hole looks open, but a 0.065" conical cone remains at the bottom. During the next operation, the G84 rigid tapping cycle drives a 3/8-16 spiral point tap into the hole. The tap slams into the conical burr, instantly snaps, and remains permanently lodged in the part, scrapping the job.

Common Drill Tip Length Reference (118° vs 135°)

Fractional Dia Decimal (in) 118° Tip Length 135° Tip Length
1/8" 0.1250" 0.038" 0.026"
1/4" 0.2500" 0.075" 0.052"
3/8" 0.3750" 0.113" 0.078"
1/2" 0.5000" 0.150" 0.104"
5/8" 0.6250" 0.188" 0.129"
3/4" 0.7500" 0.225" 0.155"
1" 1.0000" 0.300" 0.207"

Note: At 1 inch diameter, the difference between a 118° and 135° drill tip is almost 0.100". Always verify tool physical angles before programming blind holes.

Pro Tips & Common Mistakes

Do This

  • ✓Use 135° Split Points for blind tapped holes. If you are drilling a hole that does not break through, and you plan to run a bottoming tap into it, a 135° drill is superior. The flatter tip geometry leaves more full-diameter cylindrical wall for the tap threads to grip without drilling deeper into the part.
  • ✓Account for sheet metal deflection. When drilling thin materials (aluminum or sheet steel under 0.125"), the drill pressure will push the material down to bow it. Your 0.050" clearance may get eaten up entirely by deflection. Add 0.100"+ clearance for flexible sheet setups.
  • ✓Model custom drills accurately. Many replaceable tip drills (like Kennametal KenTIP or Sandvik Cor ड्रिल) have proprietary tip geometries (e.g., 140° or stepped profiles). Look up the exact L4 (tip length) specified in the tooling catalog instead of guessing.

Avoid This

  • ✗Don't guess Z-depth during 5-axis operations. When drilling at an angle using a rotary trunnion, a breakthrough calculation error can push the drill straight into the side of the trunnion platter, destroying a $50,000 rotary unit. Calculate perfectly.
  • ✗Don't use flat bottom drills for roughing. Flat-bottom (180°) drills have no tip length to calculate, but they have horrible centering capabilities and enormous thrust pressure requirements. Save flat bottom drills strictly for finishing the last 0.050" of a counterbore.
  • ✗Don't forget the chamfer diameter. If you intend the drill to leave a chamfer on the top edge (as with a spotting drill or step drill), you must add the chamfering depth to your breakthrough depth.

Frequently Asked Questions

What is the standard drill point angle?

The most common industrial standard is 118 degrees, often called a jobber drill. This angle historically provided the best balance of centering capability and cutting edge longevity in mild steel and aluminum. For harder materials like stainless steel or titanium, 135-degree split point drills are the modern standard.

Why is my drill leaving a burr on the underside of the part?

Two reasons: First, insufficient Z-depth programmed (the drill lip didn't fully exit the base). Second, even with correct depth, the pressure of the drill pushing through the last paper-thin layer of material causes it to tear rather than shear. To reduce exit burrs, use a sharper drill, higher RPM, lower feed rate at the exit point, or place a piece of sacrificial backing material tightly against the underside.

How much clearance should I add?

A standard safety clearance is 0.050 inches (1.27mm). This ensures that any slight micro-taper on the drill's trailing edge or minor workpiece deflection during cutting does not leave a ring burr in the hole. For very small drills (below 1/8"), 0.030" is acceptable. For massive drills (over 1"), 0.100"+ is safer.

How do I calculate the spot drill depth to leave a specific chamfer?

If using a 90-degree spot drill, the math is incredibly easy: the Z-depth is exactly half of the desired chamfer diameter. If you want a 0.250" diameter chamfer, plunge the 90° spot drill to Z-0.125". If using a 120-degree spot drill, the Z-depth is Diameter / (2 * tan(60°)) = dia * 0.288.

Related Calculators