CNC Cutting Depth Explained

• 1
  CNC cutting depth explained: axial vs radial engagement
• 2
  Why depth drives force, heat and chatter
• 3
  How part geometry changes the right depth
• 4
  Tool geometry, runout and holder effects
• 5
  When a shallow cut is the correct choice
• 6
  Cutting depth on five-axis and mill-turn work
• 7
  Depth and stepover starting points by material

Cutting depth is the thickness of material the edge removes in one pass. Two numbers describe it. Axial depth of cut (ADOC) is how deep the tool reaches along its own axis. Radial depth of cut (RDOC) is how far it engages sideways into the workpiece. A 12 mm end mill running 3 mm deep and 6 mm wide is cutting ADOC 3 mm, RDOC 6 mm. Those two numbers, not the spindle rpm, decide most of what happens next.

The distinction matters because the two directions behave differently. Axial depth loads the flutes and the tool core. Radial engagement decides how long each edge stays in the material and how hot it runs. Push axial depth and the tool bends. Push radial width and the chip thins at the exit, which rubs instead of cutting. Most chatter problems trace back to one of these two numbers being set wrong, not to the machine.

There is a third number engineers often mix in: stepdown. In CAM, stepdown is the axial increment between Z levels in a pocket or profile pass. Stepover is the radial increment. Cutting depth is the actual engagement at the edge, which can differ from the programmed stepdown when the tool enters a corner or a sloped wall. When a machinist says a cutter is overloaded, they usually mean the real engagement, not the CAM value.

So when someone asks what cutting depth controls, the honest answer is load. It controls chip thickness at the edge, cutting force on the spindle, heat into the tool, and the amount of deflection left in the finished wall. Get those four under control and accuracy follows. Skip them and no amount of spindle speed will save the part.

Cutting force scales roughly with the cross-section of the chip. Double the axial depth at the same feed per tooth and the chip area doubles, so the force on the edge roughly doubles. That force has to go somewhere. It bends the tool, pushes the workpiece, and loads the spindle bearings. A 6 mm carbide end mill with 40 mm of stickout deflects measurably under a heavy axial pass, and that deflection lands directly in the wall you just cut.

Heat works the same way. A deeper pass removes more material per edge engagement, which is efficient, but it also puts more heat into a smaller length of cutting edge. Thin radial engagement spreads the wear across more of the flute. This is why high-efficiency milling runs a large axial depth with a small radial width, often 5 to 10 percent of the cutter diameter. The chip is thick and carries heat away, while the edge stays cool because engagement time is short.

Chatter is the visible symptom when depth and speed line up badly. Every cutter and holder has a natural frequency. If the tooth-passing frequency sits near it, the tool starts ringing and the wall goes wavy. The usual fix is not to slow the spindle down. It is to change the depth or the radial engagement so the cut leaves the stable zone, then adjust feed to keep chip load constant.

Rigidity sets the ceiling. A part held in a vise on a 3-axis machine behaves differently from the same part on a Ø400 mm rotary table with a tailstock. We see this constantly on long thin parts. The setup, not the tool, is often what limits how deep a single pass can go.

A pocket floor and a thin wall do not want the same pass. Pocket floors tolerate deep axial cuts because the surrounding material supports the tool and the floor is a flat, well-supported surface. Thin walls do not. Once wall thickness drops below about 3 mm in aluminum or 1.5 mm in steel, the wall itself starts to deflect away from the cutter. The fix is to leave stock on both sides and finish with light, symmetric passes.

Internal corners are where programmed depth lies to you. A cutter moving into a corner sees its radial engagement climb toward 100 percent of the diameter, even if the CAM stepover says 30 percent. That spike in engagement is why corners chip edges and break small tools. Either reduce feed in corners, use a trochoidal path, or rough the corner with a smaller cutter before the finishing pass.

Deep cavities add another limit: chip evacuation. Past about 3×D, chips stop falling out on their own. They recut, heat up, and pack the flutes. Slotting is the worst case, since radial engagement is 100 percent by definition. For slots deeper than 2×D, we switch to a trochoidal or peel-milling strategy with a smaller cutter and a much larger axial depth, which keeps engagement low and lets chips clear.

Thin floors behave like thin walls. A 2 mm floor under a deep pocket will bow under cutting force and spring back after the tool passes, leaving a floor that measures thick in the middle. Support it from below when possible, or take the last 0.2 mm with a sharp, low-depth finishing pass.

Depth capacity is not only about the machine. A 3-flute cutter with a 35-degree helix behaves differently from a 4-flute with a 45-degree helix. Higher helix angles pull chips up and out of deep pockets, which helps, but they also increase axial force and can lift a lightly clamped part. Variable-helix and variable-pitch cutters break up the regular tooth pattern that feeds chatter, which is why they allow deeper passes in the same setup.

Runout is the quiet killer. Total indicated runout of 0.02 mm means one flute does most of the cutting. That flute wears fast, the surface finish suffers, and the cutter starts to sing at depths where a true-running tool would be fine. Hold the indicator on the flute, not the shank, and get runout under 0.01 mm for finishing tools. A clean collet and a properly torqued nut do more for depth capability than a tool change.

Holder choice sets stickout, and stickout sets deflection. Deflection rises with the cube of the length, so doubling stickout makes the tool eight times floppier. A shrink-fit holder with 2.5×D gauge length will hold a deep axial pass that the same cutter in an ER collet at 5×D cannot survive. When a job calls for deep reach, we plan the holder and the tool together, not after the CAM is done.

Coating matters less than people expect. TiAlN and AlTiN help at high temperature in steel and stainless. In aluminum, an uncoated polished cutter usually wins because the coating grabs the soft material. The right answer depends on the material, not on the price of the tool.

Shallow passes are not a compromise. They are the right call in specific cases. Finishing passes run 0.1 to 0.3 mm axial depth to hit Ra 0.8–1.6 μm and hold ±0.005 mm on critical faces. Hardened material above 45 HRC, thin-floor parts, and any feature within 2 mm of a free edge all want lighter engagement. So do small tools under 3 mm diameter, where the core is thin and deflection builds fast.

The other case is setup rigidity. A tall part clamped at one end will move no matter how good the tool is. Shallow passes reduce force and keep the part still. The trade is cycle time. A shallow strategy can run 30 to 50 percent longer than a well-planned deep pass, but it holds tolerance, and scrapping a part costs far more than the extra minutes.

There is a practical limit on the other end too. Going too shallow is its own failure mode. When chip thickness drops below roughly 0.02 mm per tooth, the edge stops cutting cleanly and starts rubbing. The material work hardens, especially stainless and titanium, and the next pass is harder than the last. If the finish pass feels like it is polishing rather than cutting, feed per tooth is too low, not depth.

The general rule we use is simple. Choose the deepest axial pass the setup can hold without chatter or deflection, then set radial width and feed to keep chip load in the cutter's recommended range. That order gets stable results more often than tuning speeds and feeds first.

Five-axis machining changes the depth question because the tool can be tilted. Tilting the cutter 10 to 20 degrees away from the surface lets a ball or bull-nose tool engage the edge instead of the tip, where surface speed is near zero. That single change allows a deeper axial pass on curved surfaces and improves finish at the same time. On a contoured aerospace bracket, it often removes a whole finishing step from the plan.

The other benefit is access. A part that would need four setups on a 3-axis machine can be cut in one on a simultaneous 5-axis center, which means the part stays in one coordinate frame. Depths stay consistent across features, and there is no re-datum error between operations. For parts with compound angles or deep pockets behind a flange, that consistency matters more than raw metal removal rate.

Mill-turn centers add a different dimension. A part can be turned and milled without re-chucking, so a deep radial cut in the milling step does not have to fight a second setup. We run 16 simultaneous 5-axis centers and 16 mill-turn centers for exactly this reason. Deep features and tight tolerances on the same part stop being a scheduling problem.

None of this removes the physical limit. A 4,000 mm long part on a large travel machine still deflects. The rule is the same at every size: pick depth from the rigidity you actually have, then tune the rest around it.