G83 / CNC Peck Q-Value Calculator

Inch system. Compute the Q peck increment for G83 / G73 peck drilling, accounting for drill tool-tip length and the R clearance plane.

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.
R clearance plane
Positive gap from the part surface (Z0) up to the R plane where pecking begins.
Number of pecks
The total plunge is divided into this many equal Q increments.
Glossary — what do these terms mean?
Q (peck increment)
The depth of each individual peck in a G83 (deep-hole) or G73 (high-speed) peck-drilling cycle. The control plunges Q, retracts to clear chips, then plunges again until the final Z depth is reached. This calculator sizes Q so a whole number of equal pecks covers the full plunge distance.
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. 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.
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.
R plane (reference / retract plane)
The clearance height above the workpiece surface where the drilling cycle begins and (in G99) retracts to. Because peck depth is measured from R, the air gap between R and the surface is part of the total plunge that the pecks must cover. This calculator adds the R clearance to the plunge distance.
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 so the hole is full diameter all the way through.
Total plunge distance
The full Z travel the drill feeds, from the R plane down to the deepest point. For a blind hole: R + wanted depth + tip length. For a through hole: R + material thickness + tip length + breakthrough. Dividing this by the number of pecks gives Q.
G93 (inverse time feed)
A feed-rate mode where F is given as 1/minutes (the move completes in 1/F minutes) rather than inches per minute. It's often paired with peck cycles on multi-axis or rotary work so each move's duration is controlled directly. The Q geometry computed here is independent of the feed mode.
Sample G83 program
A minimal peck-drilling block. The G83 line defines the cycle once — final depth Z, retract plane R, peck Q, and feed F. Every X Y line after it repeats that same cycle at a new hole, until G80 cancels it. The Q on that line is exactly what this calculator sizes. 
(--- safety / setup ---)
G00 G90 G17 G20 G40 G49 G80 M05
T02 M06                  (load drill)
G90 G54 S8149 M03        (spindle on)
G00 X0.0 Y-.906          (rapid to hole 1)
G43 H02 Z1.0 M08         (tool length comp, coolant)
G00 Z.1                  (rapid down near part)

(--- G83 peck cycle ---)
G83 G99 Z-.200 R.050 Q.125 F24.45  (2 pecks of .125)
X.6406  Y-.6406          (cycle repeats at hole 2)
X.906   Y0.0            (... hole 3)
X.6406  Y.6406          (... hole 4)
G80                      (cancel canned cycle)

(--- clean up ---)
G00 Z.1 M09             (retract, coolant off)
G28 G91 Z0. M05         (home Z, spindle off)
G90
M30                     (end program)

Tip-length factors derived from tan(90° − angle/2) × (D/2). Verify Q against your post-processor and tooling before running.