What Is a Peck Drilling Subroutine for a CNC Machine?

• 1
  How a Peck Drilling Subroutine Moves the Tool
• 2
  Setting Q, R and Feed for a Peck Drilling Subroutine
• 3
  When a Peck Drilling Subroutine Helps and When It Does Not
• 4
  What a Peck Drilling Subroutine Looks Like on the Shop Floor
• 5
  Reading and Editing the Subroutine Block by Block
• 6
  Step by Step: Dialing In a Peck Drilling Subroutine
• 7
  Peck Drilling Subroutine vs Other Drilling Cycles

A normal drilling cycle sends the drill from the clearance plane to the final depth in one continuous feed. Chips slide up the flutes the whole way. That works while the hole is shallow. Once the depth passes roughly three times the drill diameter, the flutes are packed with chips and the swarf has nowhere to go.

A peck drilling subroutine splits that single plunge into a stack of short ones. The control feeds the drill down by a set increment, lifts it, feeds again, lifts again, and repeats until Z reaches the programmed depth. Each retraction drags the chip string out of the flutes.

The retract height matters as much as the increment. G83 pulls the drill all the way back to the R plane on every peck, so each plunge starts from a clean flute. G73 uses a smaller retract that stays inside the hole. G73 is faster, but it only works when the chips break short and fall clear.

On a fanuc-style control the whole motion lives in one block: G83 Z-42.0 R2.0 Q5.0 F0.12. The Q value is the peck depth, R is the plane above the part, Z is the final depth, and F is the feed in mm per revolution or inches per revolution depending on your setup.

Nothing about the subroutine is exotic. It is a loop the control runs for you, and every plunge is the same feed and speed as the first one. The difference is where the chips end up.

Q is the first number to get right. A common starting point is one drill diameter per peck, or half the diameter when the material is gummy and the chips weld to the flute. In 6061 aluminium we often run 1×D per peck at 3,000–4,000 rpm. In 316 stainless the same drill may need 0.5×D and 400–600 rpm.

R sets where the rapid plane sits. Keep it 1–2 mm above the surface for flat stock. On a casting or a rough forging, raise R until the drill clears the highest point of the face, or the first rapid will clip the part.

Feed and speed come from the drill diameter and the material, not from the peck depth. Pecking does not let you run a drill harder. It lets you keep the drill alive in a hole that would otherwise clog. If a 6 mm drill in 304 stainless is running 0.08 mm/rev, it stays at 0.08 mm/rev whether you peck 3 mm or 30 mm.

Watch the first peck. If the drill squeals as it enters, the web is rubbing and the point geometry is wrong for the material. If chips come out as fine dust, the feed is too light and the edge is burnishing instead of cutting. Both problems get worse with depth.

A peck drilling subroutine also has a cost. Every retract is a rapid move, and a deep hole with a 0.5×D peck can take three or four times longer than a single plunge. That is fine on a 40 mm hole and painful on a 6 mm one.

Pecking earns its keep in three situations: a hole deeper than four diameters, a material that makes long stringy chips, and a part where the drill cannot be flooded with coolant. Aluminium, copper alloys, and low-carbon steel all produce chips that pack a flute on a deep plunge.

It also helps when the hole breaks into a cross-drilled passage or an internal cavity. A single plunge can grab at the breakthrough and snap a small drill. Short pecks let the edge pass the interruption with less torque in the cut.

On shallow holes, pecking buys you nothing. A 3 mm hole in a 3 mm plate is one plunge with a stub drill. Adding G83 there just makes the cycle longer and puts more wear on the rapid axis.

Chip breaking is not the same as chip clearing. G73 breaks the chip but leaves it in the hole. On a blind hole with no coolant through the tool, those chips get re-cut, and re-cutting is what kills the corner of a drill. G83 is the safer choice when evacuation matters.

Some materials make pecking almost mandatory. Titanium and Inconel work-harden at the bottom of a stalled cut, so a drill that dwells even briefly raises the hardness right where the next edge has to cut. In those alloys, keep the peck short and the feed high enough to stay under the hardened layer.

Hole straightness is another factor. A long drill wanders less when each peck starts from a cleared hole. If a 10×D hole has to hold position, pecking is cheaper than buying a gun drill setup.

On a three-axis mill, the programmer posts G83 with a Q of one diameter and R of 2 mm, then lets the operator prove it on a scrap block. The first part comes off the machine and goes to the bench for a pin gauge check. If the hole is oversize, the drill is walking, not the cycle.

On a five-axis machine the same cycle runs on a tilted face. The control still pecks along the tool axis, so the Q value does not change with the part angle. What changes is the approach, because the drill has to clear the fixture on the retract.

We keep the feeds and speeds for each material family in the CAM template, so a new job starts from a proven Q and R instead of a guess. The tolerance we hold on drilled holes is ±0.005 mm only after reaming. As-drilled holes sit wider, and the peck depth does not change that.

For deep, narrow features, pecking is often the only economical route. A 4,000 mm travel machine can reach a deep bore that a shorter machine cannot, and the subroutine keeps the drill cutting instead of rubbing at the bottom of the hole.

A peck drilling subroutine is a tool for chip control, not a cure for a bad setup. If the drill is not running true, or the coolant is aimed at the wrong spot, no Q value will save the hole.

Most programmers never write the loop by hand. The control already contains it, and G83 is the switch that turns it on. What you actually edit is the parameter list: Z, R, Q, and F. Everything else is fixed by the machine builder.

That is why a peck drilling subroutine is easy to tune on the floor. An operator can change Q at the control without a new CAM post. If the chips start packing halfway down a 25 mm hole, dropping Q from 6 mm to 3 mm often fixes it on the spot.

Keep the blocks readable. One cycle per line, with the Q value written out even when it repeats from the previous hole. A clear program is easier to prove out and easier to hand to the next shift.

If you run the same family of parts for years, store the cycle in a subprogram and call it with the depth and Q as arguments. The main program stays short, and no one edits the loop by accident.

The engineer's question is never how the loop is written. It is whether the hole comes out straight, on size, and with a drill that still has its corners. The subroutine is just the lever you pull to get there.