Turning operations

Turning makes round parts. The workpiece turns, and that rotation is the cutting motion; a tool with a single cutting point is fed along the work or across it. Sandvik Coromant puts it as the combination of two movements, the rotation of the workpiece and the feed of the tool. DIN 8589 defines turning as cutting with a closed, mostly circular cutting motion and a feed in any direction across the cutting direction.

Everything that follows comes from these two motions: which way the tool is fed, which part of the edge does the cutting, and what happens to the cutting speed as the tool moves towards the axis.

1. All operations
2. 1Facingacross the axis, towards the centre
3. 2Longitudinal turningalong the axis
4. 3Profiling (contour turning)along and across at once
5. 4Chamferingboth axes, or a 45° edge
6. 5Groovingacross the axis, a plunge
7. 6Thread turningalong the axis, one pitch per revolution
8. 7Parting offacross the axis, to the centre
9. 8Drillingalong the centre line
10. 9Internal turning (boring)along the axis, inside a hole

How DIN 8589-1 groups turning

DIN 8589-1 sorts the turning processes by the kind of surface they make, by the motion of the cut and by the shape of the tool. That gives six groups: four named after the surface they produce, and two, profile and form turning, after how the shape is made:

Plandrehen

Facing

Plane surfaces, such as the end faces of a part.

Runddrehen

Cylindrical (straight) turning

Round surfaces on the lateral face of a cylinder.

Schraubdrehen

Screw turning

Threads: the feed per revolution equals the lead (the pitch, on a single-start thread).

Wälzdrehen

Roll turning

Rolling surfaces such as gear teeth; a generating motion rides on the feed.

Profildrehen

Profile turning

The shape is in the tool, as its negative.

Formdrehen

Form (contour) turning

Any shape from a controlled tool path; on a CNC lathe both axes are driven.

In the plane, round and profile groups the prefix gives the feed direction: Quer- across the axis, Längs- along it. Abstech- and Einstech- mark parting and grooving. So facing an end face is Quer-Plandrehen, ordinary turning along a shaft is Längs-Runddrehen and parting off is Quer-Abstechdrehen.

Two words cross the language boundary badly. What tool makers call profiling, a contour cut with the tool moving along and across the axis at once, is DIN Formdrehen, not Profildrehen; in DIN, profile turning means a form tool that carries the shape. And DIN names Plandrehen after the plane surface, whatever the feed direction, while workshop German often uses Plandrehen simply for a cross feed.

The operations, one by one

Tool makers group the same work by what the operator does. Sandvik Coromant’s general-turning catalogue starts with longitudinal turning, profiling, facing and plunging; parting and grooving and threading have chapters of their own, and internal turning has its own section within general turning. The table covers the operations of the first figure, plus plunging and taper turning.

In the DIN scheme drilling is a process of its own, next to turning; it is in the table because lathes do so much of it. The drilling page covers the drill.

The parameters every operation shares

Five quantities describe any turning cut. The depth of cut ap is half the difference between the uncut and the cut diameter, the distance from the work surface to the machined surface. The feed fn is how far the tool moves per revolution of the work, in mm/rev. The cutting speed vc is the surface speed, in m/min, and the spindle speed n follows from it and the diameter. The entering angle κr is the angle between the main cutting edge and the feed direction, and the nose radius rε rounds the corner where the main and the minor edge meet. The formulas that link them are on the turning formulas page.

One warning about angles: Sandvik and ISO give the entering angle κr, where 90° means an edge square to the feed. Sandvik also uses the lead angle, 90° − κr, and Japanese makers (Mitsubishi, Sumitomo, Tungaloy) print the side cutting edge angle in the same lead-angle sense, so a larger angle in their catalogues means a smaller κr. Always check which one a table gives.

Entering angle κr

90

°

45°60°75°90°95°

Feed fn

0.30

mm/revDepth of cut ap

2.0

mm

Chip thickness h = fn · sin κr

0.300 mm

Chip width b = ap / sin κr

2.00 mm

Section A = ap · fn

0.60 mm²

h / fn

1.00

The chip a turning edge cuts is a thin parallelogram. Its thickness, measured square to the edge, is the maximum chip thickness

$$h_{ex} = f_n \cdot \sin \kappa_r$$

and its width along the edge is ap / sin κr, so the section ap · fn stays the same whatever the angle. At κr 90° the chip is as thick as the feed; at 45° it is 0.71 times the feed, which is the factor Sandvik prints. Sandvik’s patent on turning states the definition in words: chip thickness is the feed multiplied by the sine of the entering angle. Mitsubishi, Sumitomo and Tungaloy describe the same trend from the other side: at the same feed, a larger lead angle gives a thinner chip, and Mitsubishi adds a wider one.

Choosing κr is a trade:

• Turning against a shoulder: κr must be at least 90° (Europa-Lehrmittel); Sandvik’s usual holders for longitudinal turning are 95° and 93°.
• Slender work, light finishing cuts, a weak machine: keep κr near 90° (Mitsubishi). The passive force is smallest at 90° and grows as κr falls (Handwerk und Technik), and a long, thin part bends under it.
• A smaller κr spreads the load over a longer edge, which Mitsubishi credits with longer tool life, and Sandvik advises an entering angle below 90° where possible to soften the impact. The cost: the chip is harder to break (Mitsubishi), the radial force is higher, and the tool cannot reach a square shoulder.

Facing and parting: the speed runs out at the centre

At a fixed spindle speed the cutting speed falls with the diameter and is zero at the centre; Hoffmann’s advice for machines without constant cutting speed is to calculate with the average diameter. A CNC lathe can hold the cutting speed instead. On a Siemens SINUMERIK control G96 keeps vc constant, and because the spindle speed would in theory climb without end as the diameter shrinks, a speed limit has to be programmed, for example G96 S180 LIMS=3000. From the diameter where the limit is reached, the spindle stays at the limit and the cutting speed falls to zero at the centre, as Sandvik describes for parting off.

Cutting speed vc

180

m/minStarting diameter

120

mmSpeed limit nmax

3000

rpmReplay

Diameter D

9.5 mm

Spindle speed n

3000 rpm

Cutting speed vc

90 m/min

Limit reached at

D 19.1 mm

Siemens programs drilling and, usually, thread turning with G97, constant spindle speed; for these the speed must not change with the diameter. For parting off, Sandvik reduces the feed by up to 75 % about 2 mm before the part comes off, to keep the pip small, and calls chip evacuation a critical factor.

Boring: the overhang decides

A boring bar is a cantilever inside the part, and its length against its diameter decides whether the cut is quiet. Sandvik’s rule is the largest bar diameter and the shortest overhang the job allows, with these limits by bar type:

Sandvik also keeps the entering angle close to 90° in boring and never below 75°, because a smaller angle raises the radial force that pushes the bar away from the wall. Tungaloy’s troubleshooting table gives the same remedy for chatter: shorten the overhang of the toolholder.

Starting feeds from two makers

Both makers sort turning into finishing, medium and roughing and give a feed range for each. Sandvik’s ranges come from its insert-size chart and Sumitomo’s are its first-choice conditions; both are for their own inserts, not limits; Sumitomo’s table goes with particular grades and chipbreakers and is printed in inches, converted here.

The two agree on the order and roughly on the middle range; for roughing, Sandvik’s chart reaches much higher feeds than Sumitomo’s table.

Common mistakes

• Constant cutting speed without a limit. As the tool nears the axis the control would raise the spindle speed without end; Siemens asks for a programmed limit because of the centrifugal forces.
• G96 for drilling or threading. Drilling needs a constant spindle speed, and thread turning usually runs at one too (G97 on SINUMERIK).
• A κr below 90° against a shoulder. The edge cannot reach the corner; use a 93° or 95° holder.
• A long boring bar. Take the largest bar that fits and the shortest overhang; past the limits above, use a dampened or carbide bar.
• Full feed to the end of a parting cut. Reduce it about 2 mm before the part comes off, or the pip grows.
• Mixing angle conventions. κr 75° and a 15° lead angle are the same holder; a Japanese catalogue’s “side cutting edge angle 15°” is that holder too.