Turning parameters depend on the work material, insert, machine setup, and the type of cut. Mitsubishi Materials publishes selected aluminum-alloy recommendations in its C010 Turning Tools catalog. The table below keeps those values tied to the named alloy families and the catalog’s specified insert combination.

These are Mitsubishi starting ranges for an external turning insert, not universal settings for every aluminum alloy or lathe. The three alloy groups have the same listed ranges in this catalog selection.

Read the material and tool columns together

The table covers A6061 and A7075, AC4B, and ADC12 or A390, separated by the silicon classes shown by Mitsubishi. Each row specifies a 7-degree positive insert, AZ chipbreaker, and HTi10 grade. Those details matter: changing the edge geometry, coating or grade, chipbreaker, or toolholder can change the usable cutting window. The numbers should not be detached from that tool recommendation.

The ranges are broad. Cutting speed is 300–700 m/min, feed is 0.10–0.40 mm/rev, and depth of cut is 0.20–3.00 mm for each listed material group. They are not three independent controls to set at their maximum values. A conservative setup should begin within the range using the machine and toolmaker guidance, then be adjusted for rigidity, surface finish, chip shape, heat, and tool condition.

Convert cutting speed to spindle speed

For metric turning, estimate spindle speed from N = 1000 Vc ÷ (πD), where N is revolutions per minute, Vc is cutting speed in metres per minute, and D is the current cutting diameter in millimetres. For example, at a 50 mm diameter, 300 m/min corresponds to about 1,910 rpm, while 700 m/min corresponds to about 4,456 rpm. Check that the machine, workholding, and part are rated for the resulting speed. Use constant surface speed only where the control and setup support it safely.

Feed is stated per revolution. At 1,000 rpm, 0.10 mm/rev corresponds to a linear feed rate of 100 mm/min; 0.40 mm/rev corresponds to 400 mm/min. Actual feed choice should reflect the insert nose radius, required finish, part support, and chip evacuation. Depth of cut is radial engagement, so a 1 mm depth reduces the workpiece diameter by approximately 2 mm on an external pass.

Start with the machine and the cut

Confirm the exact alloy and condition before using the aluminum group. A cast alloy with substantial silicon can behave differently from a wrought alloy even when both are aluminum-based. Check Mitsubishi’s current catalog for the closest material match and verify the chipbreaker and grade availability. If the alloy is not listed, do not assume the nearest row is equivalent.

Use a rigid toolholder and minimize overhang. Secure the workpiece against deflection, especially on long or thin parts. Aluminum chips can be long and sharp, so choose a tool geometry and cutting condition that produce manageable chips; never clear chips by hand while the spindle is moving. Use guarding and appropriate eye protection, and stop the machine before removing tangled swarf.

For a first cut, start with a moderate speed and feed inside the manufacturer range, then inspect the surface, chip form, sound, and insert edge. Adjust one variable at a time. Chatter, built-up edge, poor finish, or chip wrapping may indicate that the setup or edge is wrong, rather than that the feed should simply be raised or lowered.

The recommendation is most useful as a bounded starting point for the specified tool and aluminum family. It does not determine tool life, surface integrity, machine power, or a safe workholding limit. Follow the current catalog, machine manual, shop controls, and project requirements when releasing a production process.

Source: Mitsubishi Materials, C010 Turning Tools catalog, aluminum-alloy external turning recommendations on page A091. The catalog lists other alloy families separately; consult those entries rather than extending this table to brass, magnesium, or other nonferrous materials.