CNC Fixed Cycle Programming: The Complete Guide to Drilling, Tapping, and Boring Operations
Every machinist who has stared at a blank piece of metal and thought “there has to be a faster way” already knows the answer — fixed cycles. These canned cycles turn what would be dozens of lines of G-code into a single instruction. They handle the dirty work: rapid positioning, feed cutting, dwell at the bottom, and retraction. Once you understand how they work, your programming speed jumps dramatically and your programs become cleaner, safer, and easier to debug.
This guide walks through the most commonly used fixed cycle instructions, when to reach for each one, and the practical traps that catch even experienced programmers off guard.
What Exactly Is a Fixed Cycle in CNC Programming
A fixed cycle — also called a canned cycle — is a pre-packaged sequence of machine motions triggered by one G-code. Instead of writing separate blocks for rapid approach, feed down, dwell, and retract, you issue one line and the controller executes the entire routine automatically.
The standard cycle breaks down into six distinct actions:
- X/Y positioning — rapid move to the hole location
- Rapid to R-point — the reference plane just above the workpiece
- Cutting feed — the actual drilling, tapping, or boring operation
- Bottom action — dwell, spindle stop, or tool offset depending on the cycle
- Retract to R-point or initial plane — controlled by G98 or G99
- Return to start — ready for the next hole
These cycles are modal. Once you call G81, G83, G84, or any other fixed cycle, every subsequent X/Y position triggers that same cycle until you cancel it with G80. This is both the power and the danger — forget to cancel a cycle and your next rapid move becomes a drill stroke.
The Drilling Cycles You Will Use Every Day
G81 — Standard Drilling Cycle
This is the workhorse. G81 drills a hole and rapidly retracts. No dwell, no frills. The format is straightforward:
G81 X_ Y_ Z_ R_ F_
X and Y define the hole position. Z is the final depth. R is the reference plane height — typically 2 to 5 mm above the part surface. F is the feed rate.
Use G81 for holes shallower than about 5 times the drill diameter. Anything deeper and you risk chip packing. The cycle ends with a fast retract to either the initial plane (G98) or the R-plane (G99). G99 is almost always the better choice when drilling multiple holes in a row because it saves travel time.
G82 — Drilling with Dwell
G82 adds a pause at the bottom of the hole. The spindle keeps spinning while the tool sits still, which lets the cut settle and produces a smoother bottom finish. This matters for blind holes where depth accuracy counts.
G82 X_ Y_ Z_ R_ P_ F_
The P value is the dwell time in milliseconds. A typical value might be P1000 for a one-second pause. This cycle is common for spot drilling and counterboring operations where you want the tool to seat cleanly before retracting.
G73 — High-Speed Peck Drilling
When the hole gets deep, chips become the enemy. G73 solves this by pecking — the drill advances a set depth Q, then retracts a small amount d to break chips, then goes back in. This incremental feeding keeps the flutes clear and prevents tool breakage.
G73 X_ Y_ Z_ R_ Q_ F_
Q defines the peck depth. The retract distance d is handled internally by the controller. The final peck may be smaller than Q to land exactly on the programmed Z depth. This cycle shines on holes deeper than 5 diameters, especially in aluminum or steel where chip evacuation is critical.
G83 — Deep Hole Peck with Full Retract
G83 is similar to G73 but more aggressive about clearing chips. After each peck, the tool fully retracts back to the R-plane before diving again. This gives chips a better chance to escape the hole, which is why G83 is preferred for very deep holes or when drilling in tough materials.
G83 X_ Y_ Z_ R_ Q_ F_
Same Q peck depth as G73, but the full retraction between pecks makes it slower. Trade speed for reliability. When deep hole drilling goes wrong, it goes wrong fast — a broken drill in a 40mm deep hole is a headache nobody wants.
Tapping and Threading Cycles That Save Your Sanity
G84 — Right-Hand Tapping
Threading by hand in G-code is a nightmare. G84 handles the entire sequence: spindle starts forward, the tap feeds down at the programmed rate, and at the bottom the spindle reverses to back the tap out. The feed rate must match the thread pitch exactly — F = spindle RPM × thread pitch. Get this wrong and you destroy the thread.
G84 X_ Y_ Z_ R_ F_
One critical detail: the retraction is NOT rapid. The tap backs out at feed speed to avoid snapping the tap or damaging the thread. This is a common point of confusion. If you expect a fast retract and program G98, the tool will still reverse at feed speed through the thread — only the final move to the initial plane is rapid.
G74 — Left-Hand Tapping
G74 does the same thing as G84 but with reverse spindle rotation for left-hand threads. The feed direction is reversed, and the retraction runs the spindle forward. Everything else stays identical.
G74 X_ Y_ Z_ R_ F_
Left-hand threads are less common but they show up in specific applications like certain pump housings and hydraulic fittings. When you need one, G74 gets it done without writing a single line of manual thread-cutting code.
Boring Cycles for Precision Holes
G85 — Boring with Feed Retract
G85 bores a hole and retracts at feed rate. No dwell, no spindle stop. It is essentially the boring equivalent of G81.
G85 X_ Y_ Z_ R_ F_
Use this when you need a clean bore but do not require the extra precision of a dwell cycle.
G89 — Boring with Dwell
G89 adds a feed pause at the bottom, giving the cutter time to finish the surface. This produces a better wall finish than G85 and is the go-to cycle for precision bore work where surface quality matters more than cycle time.
G89 X_ Y_ Z_ R_ P_ F_
The P parameter sets the dwell time in milliseconds. Combined with a sharp boring bar and proper speeds, G89 delivers repeatable results on finishing passes.
G76 — Fine Boring Cycle
This is the precision king. G76 executes three actions at the bottom: feed dwell, spindle orient stop, and a tool offset in the reverse direction. That offset lets the tool clear the bore wall on retract without dragging across the finished surface.
G76 X_ Y_ Z_ R_ P_ Q_ F_
P is the dwell time. Q is the tool offset distance. This cycle is mandatory for high-tolerance bore work where even a light drag mark would cause rejection. The spindle orient stop ensures the tool always retracts in the same angular position, which matters for multi-pass boring strategies.
G86 — Boring with Spindle Stop
G86 stops the spindle at the bottom and rapidly retracts. It is useful when you want to break chips with a spindle stop or when the machine has rigid tapping/boring requirements.
G86 X_ Y_ Z_ R_ F_
G87 — Back Boring
G87 is the odd one out. It is designed for boring from the back side of a hole — the tool offsets before plunging, cuts upward, then retracts with another offset. This cycle is common in engine block and hydraulic manifold work where access is limited to one side.
G87 X_ Y_ Z_ R_ Q_ F_
The Q offset value controls how far the tool shifts. Programming G87 requires careful attention to the sequence of motions because the tool moves in directions that feel counterintuitive at first.
Practical Programming Tips That Actually Matter
Always Set the R-Plane Properly
The R-plane is your safety net. Set it too close to the part and you risk collision with clamps or fixtures. Set it too far and you waste time on every single hole. A typical R-plane sits 2 to 5 mm above the highest point of the workpiece. For multi-step setups, calculate R based on the tallest feature in the current operation.
Use G99 for Multi-Hole Patterns
When drilling a plate with 20 holes, G99 (return to R-plane) saves massive amounts of air-cut time compared to G98 (return to initial plane). The difference adds up fast — on a 50mm thick plate, G98 adds 50mm of empty travel per hole. With G99, that travel disappears after the first hole.
Cancel Cycles Explicitly
Always end a fixed cycle block with G80. It is too easy to leave a cycle active and have the next rapid move turn into an unplanned drill stroke. This single habit prevents more crashes than almost any other programming practice.
Combine with Subprograms for Complex Parts
For parts with multiple hole types — say, drill holes on one face, tapped holes on another, bored holes on a third — use subprograms. Call the drilling subprogram for one face, the tapping subprogram for another. This keeps each cycle block clean and makes editing far easier when the part design changes.
Watch the Feed Rate on Tapping
The relationship F = RPM × pitch is not optional. If your spindle runs at 1500 RPM and the thread pitch is 2mm, your feed must be exactly 3000 mm/min. Deviation by even 10% produces worn threads that fail inspection. Double-check this calculation every time you program a tap cycle.
Turning Fixed Cycles — A Quick Overview
While this guide focuses on milling fixed cycles, turners have their own set of powerful canned cycles worth knowing about. G90 handles simple turning cuts (straight or tapered). G94 does facing. G92 cuts threads. G71, G72, and G73 handle roughing with stock removal allowances. G70 is the finishing cycle that follows any of the roughing cycles.
The logic is the same: one instruction replaces a block of repetitive motion. The difference is that turning cycles work in X/Z rather than X/Y, and the stock removal parameters (U, W, D) replace the depth and peck values you see in milling cycles.
Fixed cycles are not just a convenience — they are the foundation of efficient CNC programming. Master G81 through G89, understand when to reach for G73 versus G83, and never skip the G80 cancel. Your programs will be shorter, your machines will run smoother, and your parts will come out right the first time.
