Turning insert codes explained: CNMG 432, shapes and nose radius
Every turning insert has a code printed on the box: CNMG 432, DCMT 21.51, VNMG 160404. It looks like a part number, but it’s a description. Once you can read it, you can tell what the insert looks like, how strong it is, which holder it fits and what nose radius you’ll be cutting with, without opening the box.
This guide covers the code used on the inch (ANSI) and metric (ISO) boxes, the common shapes and what they’re good for, and the one number that matters most for your program: the nose radius.
The code, letter by letter
Take CNMG 432 (inch) or its metric twin CNMG 120408. The first four letters are the same in both systems:
| Position | Example | Meaning |
|---|---|---|
| 1 | C | Shape: 80° rhombic (diamond) |
| 2 | N | Clearance angle under the cutting edge: 0° |
| 3 | M | Tolerance class: M = medium (the usual pressed insert) |
| 4 | G | Type: centre hole, chipbreaker on both sides |
| 5–7 | 432 or 120408 | Size, thickness and nose radius |
1st letter: shape
The shape letter gives the included angle of the corner that does the cutting.
| Letter | Shape | Corner angle | Typical use |
|---|---|---|---|
| C | Rhombic | 80° | Roughing and facing, general turning. The workhorse. |
| D | Rhombic | 55° | Profiling, turning and facing with one tool. |
| V | Rhombic | 35° | Fine profiling, undercuts, small grooves and steep back-tapers. |
| T | Triangle | 60° | General turning and facing, many older holders. |
| W | Trigon | 80° | Roughing and facing with more corners per insert than a C. |
| S | Square | 90° | Heavy roughing, chamfering, very strong edges. |
| R | Round | — | Contouring, strong edge, good finish at high feed; needs a rigid setup. |
The trade-off is always the same. A bigger corner angle is stronger and takes more depth of cut and more abuse. A smaller corner angle reaches more places: it can follow a profile that turns back toward the chuck without the back of the insert rubbing the part. A C insert roughs well but can’t copy a deep undercut; a V insert can, but it chips sooner if you rough with it.
2nd letter: clearance angle
| Letter | Clearance |
|---|---|
| N | 0° (negative insert) |
| C | 7° |
| P | 11° |
| B / E | 5° / 20° (less common) |
A negative insert (N) has square sides. The holder tilts it to get clearance, so it can be double-sided: a CNMG has four usable 80° corners, two on each side. Negative inserts are strong and cheap per edge, which makes them the default for OD roughing and finishing on a solid machine.
A positive insert (C or P) has the clearance ground into its sides, so only one side cuts. It cuts with less force, which helps with small boring bars, long slender parts, light machines and fine finishing. That’s why most small boring bars take CCMT, DCMT or VCMT inserts.
3rd letter: tolerance
M is the everyday class for pressed (molded) inserts. G and E are ground to tighter tolerances: when you index to a fresh corner, the tip comes back to almost the same spot. That matters when you’re holding tight tolerances and don’t want to re-touch an offset after every index.
4th letter: hole and chipbreaker
| Letter | Hole | Chipbreaker |
|---|---|---|
| G | Cylindrical hole | Both sides |
| M | Cylindrical hole | One side |
| T | Countersunk hole (screw) | One side |
| W | Countersunk hole (screw) | None |
| A | Cylindrical hole | None |
| N | No hole | None |
Negative inserts with a straight hole (G, M, A) are clamped by a lever or pin. Positive inserts with a countersunk hole (T, W) are held by a screw through the middle, which is why a DCMT fits a compact screw-clamp holder or a small boring bar.
The chipbreaker style (finishing, medium, roughing) is usually a suffix each manufacturer names its own way, so check the catalogue or the box for the recommended depth of cut and feed range.
The numbers: size, thickness, nose radius
This is where inch and metric codes differ.
Inch (ANSI), three digits: CNMG 432
- 4 = inscribed circle in eighths of an inch: 4/8 = 1/2 in.
- 3 = thickness in sixteenths: 3/16 in.
- 2 = nose radius in sixty-fourths: 2/64 = 1/32 in (0.0313).
So the common nose radii are 1 = 1/64 (0.0156), 2 = 1/32 (0.0313), 3 = 3/64 (0.0469) and 4 = 1/16 (0.0625). Small inserts use fractions, which is how you get codes like DCMT 21.51: IC 2/8 = 1/4 in, thickness 1.5/16 (about 3/32 in), radius 1/64 in.
Metric (ISO), six digits: CNMG 120408
- 12 = cutting edge length in mm. On a C insert that means a 12.7 mm (1/2 in) inscribed circle, the “4” of a CNMG 432.
- 04 = thickness, 4.76 mm.
- 08 = nose radius in tenths of a millimetre: 0.8 mm.
A CNMG 432 and a CNMG 120408 are the same insert, and both fit the same holder. Common metric radii are 04 (0.4 mm), 08 (0.8 mm) and 12 (1.2 mm).
Choosing the nose radius
The nose radius is the corner that actually touches the part, and it changes three things.
Finish. For a given feed, a bigger radius leaves smaller feed marks. The theoretical peak-to-valley height is roughly feed² ÷ (8 × nose radius). At 0.006 in/rev with a 1/32 in radius, that’s about 0.000144 in (144 µin) peak to valley. Halve the feed and the marks drop to a quarter.
Strength. A bigger radius is a stronger corner, so it holds up better in roughing and interrupted cuts.
Chatter and small features. A bigger radius pushes harder against the part, which can start chatter on slender parts or thin walls. It also can’t make an inside corner sharper than itself: a 1/32 radius leaves at least a 1/32 radius fillet at every shoulder.
A common starting point: 1/32 (0.8 mm) for general work, 1/64 (0.4 mm) for light finishing and small boring bars, and 3/64 to 1/16 (1.2–1.6 mm) for heavy roughing. Keep the depth of cut at least about two-thirds of the nose radius, or the insert rubs instead of cutting.
The nose radius belongs in your offsets, too
When your program uses tool nose radius compensation (G41/G42), the control needs two things on the tool’s offset page: the nose radius (R) and the tip direction (T). For a standard OD turning tool on a Haas or Fanuc lathe the tip direction is usually 3; for a boring bar it’s usually 2.
(T101 CNMG 432 - OD TURN)
(FINISH PASS AFTER ROUGHING)
T0101
G50 S3000
G96 S600 M03
G00 X1.4 Z0.1 M08
G00 G42 X0.75 Z0.1 (COMP ON WITH A STRAIGHT MOVE)
G01 Z0. F0.006
X1.0 Z-0.125 (45 DEG CHAMFER)
Z-1.5
X1.3
G40 G00 X1.4 (COMP OFF MOVING AWAY FROM THE PART)
If the radius on the offset page doesn’t match the insert in the holder (say the program was proved with a 1/32 and someone loads a 1/64), every chamfer and taper comes out slightly off size. On a part with tight tolerances on a chamfer or a cone, that’s a scrapped part, even though the program itself is fine.
Without comp, the control drives the imaginary tip of the insert along the programmed path. Straight Z and X moves come out right, but chamfers, tapers and arcs come out off by an amount that depends on the nose radius. That’s why the radius belongs either in the offset page (with G41/G42) or in the CAM post (when the CAM already compensated the path).
Write the insert in the tool comment
A short tool comment such as (T101 CNMG 432 - OD TURN) or (T404 DCMT 21.51 - 0.5 BORING BAR) costs nothing and tells the next person at the machine exactly what should be in the turret. It’s also how a simulator knows what’s cutting.
NC Proof Turn reads that code from the comment: it draws the insert with its real corner angle and nose radius, cuts the 3D stock with that shape, and follows G41/G42 the way the control does. You can see whether a C insert leaves material in an undercut that needs a V, or whether a chamfer comes out right with the radius you entered, before the program reaches the lathe.