G81 / CNC Drill Z-Depth Calculator

Inch system. Work out the final program Z (tip target) for a G81 drilling cycle — what to take into account so the hole reaches full diameter at the depth you want.

Unit
Inch (in)
Depths
How deep you need the hole at full diameter, measured from the part surface (Z0).
Total stock thickness under the tool. We compare this to the depth to decide blind vs. through.
Tool diameter & tip
Accepts decimal (0.25) or fraction (1/4).
Tip length = tan(90° − angle/2) × (D / 2). The drill point must clear the material before the hole reaches full diameter. For a flat-bottom tool (counterbore/endmill) set the angle to 180° via Custom for a zero tip.
R clearance plane
Positive gap from the part surface (Z0) up to the R plane where the cycle starts. R is a separate word on the G81 line; it does not change the program Z.
Glossary — what do these terms mean?
G81 (drilling cycle)
The simplest canned drilling cycle: rapid to R, feed straight down to the final Z, then retract — no peck, no dwell. Best for shallow holes where chip packing isn't a concern. The whole question with G81 is "what is the right final Z?", which is what this page works out.
Program Z (tip target)
The Z coordinate on the G81 line — the deepest point the drill tip reaches, measured from the part surface (Z0). It's negative (into the material). It does not include R, because R is a separate word: Z = −(depth + tip length) for a blind hole, or Z = −(thickness + tip length + breakthrough) for a through hole.
Tool tip length
A twist drill ends in a cone, not a flat face. The hole only reaches full diameter once the full cone has passed below the target depth, so the tip length must be added to the Z depth. Tip length is that cone height: tan(90° − angle/2) × (D / 2). For a 135° point that's ≈ 0.207 × D; for the common 118° point ≈ 0.300 × D; for a 90° spot drill ≈ 0.500 × D. A flat-bottom tool (180°) has zero tip length.
Tip angle (included angle)
The total included angle of the drill point — the angle between the two cutting lips. Standard jobber drills are 118°; harder materials often use 135° split points. A smaller angle means a longer, sharper point and a longer tip length.
Blind vs. through
The calculator compares the full-diameter depth you want against the material thickness. If the wanted depth reaches or passes the back face (depth ≥ thickness) it's a through hole; otherwise it's blind. You don't pick the type — the geometry decides it.
Breakthrough (through holes)
For a through hole, the drill must travel past the back face far enough for the full diameter — not just the tip — to clear. The breakthrough field (commonly ≈ 0.020") only appears once the depth/thickness comparison says the hole is through; it's added on top of the material thickness and tool tip length.
R plane (reference / retract plane)
The clearance height above the surface where the cycle starts and (in G99) retracts to. It is a separate word on the G81 line and does not change the program Z — it only affects how far the tool rapids before feeding. Shown here for completeness and to compute total feed travel.
Sample G81 program
A minimal drilling block. The G81 line defines the cycle once — final depth Z, retract plane R, and feed F. Every X Y line after it repeats the cycle at a new hole, until G80 cancels it. The Z on that line is exactly what this calculator sizes. 
(--- setup ---)
G00 G90 G17 G20 G40 G49 G80 M05
T01 M06                  (load drill)
G90 G54 S3056 M03        (spindle on)
G00 X0.0 Y0.0
G43 H01 Z1.0 M08
G00 Z.1

(--- G81 drill cycle ---)
G81 G99 Z-.5751 R.050 F24.45  (feed to final Z)
X1.0  Y0.0              (cycle repeats at hole 2)
X2.0  Y0.0             (... hole 3)
G80                     (cancel canned cycle)

(--- clean up ---)
G00 Z.1 M09
G28 G91 Z0. M05
G90
M30

Program Z = −(depth + tip length), plus material thickness & breakthrough for through holes. Verify Z against your post-processor and tooling before running.