How to Determine the Cutting Depth in High-Speed Machining of a Twin-Spindle Machining Center

• 1
  Key takeaways
• 2
  What actually sets the cutting depth in high-speed machining
• 3
  Material and hardness decide the starting range
• 4
  Why the twin-spindle layout forces a shallower cut
• 5
  Tool geometry, coating and overhang change the limit
• 6
  Symptoms that tell you the depth of cut is wrong
• 7
  Step by step: setting depth of cut for both spindles
• 8
  Starting depth-of-cut ranges by material and operation

On a twin-spindle machine, both tools cut at the same time. That single fact changes how you choose depth of cut. A setting that is safe on one side can push the other side past its load limit, and the part will move. So we treat depth of cut as a balance problem first, a chip-load problem second.

High-speed machining means high spindle speed and a small chip. The tool does not remove a thick slice; it peels a thin one fast. Because the chip is thin, most of the heat leaves with the chip instead of soaking into the workpiece. That is the whole point. If your axial or radial depth is too large, the chip gets thick, heat stays in the part, and you lose the benefit.

Two numbers define the cut. Axial depth of cut (ap) is how deep the tool engages along its axis. Radial depth of cut (ae) is how wide the tool engages across the material. You set both before you press cycle start. Changing one later usually means changing the other.

• 1
  ap = axial depthMeasured along the tool axis. Drives bending force on the tool.
• 2
  ae = radial widthMeasured across the cut. Drives heat and tool wear.
• 3
  Chip load (fz)Millimeters per tooth. Ties ap and ae to feed rate.

Aluminum is forgiving. On 6061-T6 or 7075 with a 12 mm carbide end mill, we often run ap at 1.0-1.5 × tool diameter and ae at 8-12% of diameter for roughing. Spindle speed runs high, feed per tooth stays around 0.08-0.15 mm. The cut sounds light because it is.

Stainless 304 and 17-4PH behave differently. They work-harden, so a light rub is worse than a real cut. Keep ae at 6-10% of diameter and ap at 0.5-0.8 × diameter. If you drop below that window, the tool rubs, the surface hardens, and the next pass cuts harder material.

Titanium Ti-6Al-4V and Inconel sit at the tight end. Radial engagement drops to 5-8% of diameter, ap to 0.3-0.6 × diameter, and spindle load is watched closely. On these alloys, high-speed machining only pays off when the radial width is small enough that heat leaves with the chip.

• 1
  Aluminumap 1.0-1.5 × D, ae 8-12% of D
• 2
  Stainless / 17-4PHap 0.5-0.8 × D, ae 6-10% of D
• 3
  Titanium / Inconelap 0.3-0.6 × D, ae 5-8% of D

A single-spindle machine has one cutting force to manage. A twin-spindle center has two, and they act on the same part or on two parts sharing one fixture. If one side takes a heavier cut, the fixture sees a twisting load. Thin walls move, bores go oval, and the ±0.005 mm tolerance is gone before the finish pass.

The rule we use is simple: keep the load difference between the two spindles under 10%. In practice that means the two programs should use the same tool diameter, the same ae, and an ap difference no larger than 0.1-0.2 mm on roughing. If one side must take more, split the difference into two passes instead of one heavy pass.

Balance also matters for tool life. When one spindle works harder, its insert wears faster. After a few hundred parts, the two sides no longer match, and the operator has to stop and index one tool only. Matching the cut keeps both tools on the same wear curve.

• 1
  Load splitKeep the two spindles within 10% of each other.
• 2
  ap differenceNo more than 0.1-0.2 mm between sides on roughing.
• 3
  Fixture checkVerify clamping force before raising ap on either side.

A 12 mm end mill with 30 mm of overhang can take a much deeper axial cut than the same tool with 90 mm of overhang. Deflection grows with the cube of overhang length. When we need long reach, we cut ap by roughly half and raise the spindle speed to keep the chip load in range.

Coating matters too. AlTiN and AlCrN coatings tolerate higher temperatures, which supports the thin-chip, high-speed approach on steel and stainless. Uncoated carbide on aluminum is often better because it avoids built-up edge. The coating does not change the geometry of the cut, but it changes how much heat the edge can survive.

Helix angle and core diameter set how much the tool can take radially. A 45° helix with a thick core handles ae up to 10% of diameter well. A long, thin tool with a 30° helix will chatter at the same ae. If chatter starts, reduce ae first, not spindle speed.

• 1
  Overhang under 4 × DKeep full ap range.
• 2
  Overhang 4-6 × DCut ap by about half.
• 3
  Chatter appearsReduce ae first, then adjust feed.

Chatter on one spindle only usually means tool overhang or holder runout on that side, not a material problem. Check runout first. If runout is fine, reduce ae by 20% and test again. Raising spindle speed to chase chatter usually makes it worse on long tools.

Short tool life on one side points to uneven ap between spindles. Log the load on each side for a full shift. If one side runs 15% higher, split the heavier pass. This is common on parts with a boss on one end and a flat on the other.

Poor surface finish on the finish pass is often an ae problem. When ae drops under 0.1 mm, the tool rubs instead of cutting, and the Ra rises. Keep finishing ae between 0.1 and 0.3 mm so the edge bites.

• 1
  Chatter, one sideCheck runout, then cut ae by 20%.
• 2
  Fast wear, one sideBalance ap between spindles; split the heavy pass.
• 3
  High Ra on finishRaise ae to 0.1-0.3 mm so the edge cuts.