How to reasonably control the cutting quantity of CNC turning and milling compound machine tools

• 1
  Key takeaways
• 2
  What cutting quantity means on a compound machine
• 3
  Inputs that decide the cutting quantity of CNC turning
• 4
  Turning passes and milling passes need different rules
• 5
  How to read the machine while you dial it in
• 6
  Step by step: setting cutting quantity on a mill-turn center
• 7
  Starting cutting quantity by material and operation

Cutting quantity is not one number. It is the load you place on the insert in a single engagement: depth of cut, feed per revolution, and cutting speed together. On a turning and milling compound machine, that load changes as the part rotates on the C-axis and the milling spindle takes interrupted cuts. A parameter set that works on a lathe with a solid round bar can chatter once the part is held on one end and milled on the side.

The practical goal is simple. Remove the most material the setup can tolerate without losing size, finish, or tool life. A mill-turn center with a Ø400 mm rotary table has enough rigidity for a 3 mm depth of cut in 6061 aluminium, but the same depth on a thin-walled 316L part may deflect the wall and scrap the part at final inspection.

We treat cutting quantity as a budget spent across the whole cycle, not per pass. If the roughing pass removes too little, the cycle time grows and the insert rubs instead of cutting. If it removes too much, the tool pushes the part away and the size drifts. The control method in this article keeps both ends of that range visible.

Start with the material. Aluminium 6061 and 6082 cut freely, so we push turning depth to 2.0 to 4.0 mm per side and feeds near 0.25 mm/rev. Stainless 316L work hardens, so we keep depth above 1.0 mm to stay under the hardened layer and drop surface speed to 120 to 180 m/min. Titanium TC4 needs lower speed again, around 40 to 70 m/min, with generous coolant.

Next, look at how the part is held. A bar in a collet or a chuck with a short overhang supports aggressive cutting. A long shaft held between centers, or a part on a fixture with a thin floor, flexes under the same load. As a rule, if the length-to-diameter ratio goes past 4:1 on unsupported turning, reduce depth by 30 to 50 percent and add a steady rest.

Tool geometry sets the ceiling. A positive rake insert with a sharp edge cuts aluminium and plastics with low force. A negative rake insert, used for interrupted cuts and harder steels, needs more spindle power and a rigid setup. On our 16 mill-turn centers we keep two insert grades on hand for each job so we can trade edge strength against cutting force without reprogramming the cycle.

Finally, the machine itself. Spindle power, turret rigidity, and the rotary table clamping force all limit how much you can take in one pass. A 16-station mill-turn center is not a 40-taper milling machine, so milling passes on the C-axis are usually lighter than what the same cutter would take on a dedicated mill.

• 1
  Material hardnessHarder and tougher grades force lower speed and shallower depth.
• 2
  Workholding rigidityLong overhangs and thin walls need reduced depth of cut.
• 3
  Insert geometryPositive rake for soft metals, negative rake for interrupted cuts.
• 4
  Spindle and turret limitsPower and clamping force cap the depth per pass.

On the turning side, cutting is continuous. Once the insert enters the cut, the load stays steady until it exits. That lets you run a deeper pass: 1.5 to 3.0 mm per side for roughing steel 1045 or 4140, and 3.0 to 4.0 mm per side for 6061 aluminium. Keep finishing depth between 0.2 and 0.5 mm so the insert cuts rather than rubs, and hold feed at 0.05 to 0.12 mm/rev for Ra 0.8 to 1.6 μm.

Milling on a compound machine is interrupted by nature. Every flute entry is an impact, and on a mill-turn center the part is often rotating on the C-axis while the milling spindle cuts. We reduce depth of cut to 0.3 to 1.0 mm axial and 30 to 50 percent of cutter diameter radial for roughing, then 0.1 to 0.3 mm axial for finishing.

The two operations share one spindle load budget. If the turning pass already draws 70 percent of available spindle power, the milling pass will stall or chatter. We check total load in the CAM simulation before the program goes to the machine, and we split heavy milling into two lighter passes rather than pushing one deep cut.

Chip evacuation matters more on the milling side because chips sit in pockets and recut. A recut chip doubles the effective cutting quantity on the edge and burns the insert. We use through-spindle coolant where the tool allows it, and we program a short retract every few passes to clear pockets on deep cavities.

Chips are the fastest feedback you get. Steel 1045 at the right cutting quantity produces short, curled, grey chips. Long stringy chips mean the feed is too low for the depth, so the insert rubs and heat builds in the part. Blue or black chips mean surface speed is too high or the insert has lost its edge.

Sound tells you about rigidity. A steady hum with a light tick at each flute entry is normal. A rising squeal or a rattle that appears only at certain C-axis angles points to chatter from a weak setup or a depth that is too aggressive for the overhang.

Spindle load and tool wear follow the same story. If load climbs 20 percent across a batch with the same program, the edge is dulling and the cutting quantity is effectively rising as the tool pushes instead of shears. We log load per tool and change inserts on a count or a load trigger, whichever comes first.

Measure the first part, not the last one. We check size and finish after the first roughing pass and again after the finish pass. If the finish pass removes less than 0.1 mm, the tool may rub and leave a poor surface. If it removes more than 0.6 mm on a thin wall, expect deflection and a taper that shows up in final inspection.