Tools and Jigs/Fixtures

What Happens When You "Plug Anything In" on the Lathe

When you open the lathe tool holder, there are dozens of inserts that look similar. The first experience for new employees is usually inserting something that looks similar, but it doesn't fit the holder or breaks within 3 minutes.

The code printed on the insert, such as CNMG120408, is not just decoration. It is a specification code (ISO 1832) that lists shape, clearance angle, tolerance, hole and chipbreaker, size, thickness, and corner R in order. Knowing how to read this code reduces the time spent searching for tools in the tool holder from 10 minutes to 30 seconds.

Booolkyung's subcontractors deal with a wide variety of products in small quantities, so one person changes tools six times a day. Reading the code is not an option, but a basic skill.

1. Turning Tools Are Categorized by "What They Do"

> Roughing and finishing inserts have different codes. Roughing inserts are thick and strong, while finishing inserts are thin and sharp. Finishing inserts will break after cutting just a few millimeters.

2. Reading Insert Codes — Each Position Has a Meaning

   C   N   M   G   12   04   08
   │   │   │   │    │    │    └ Corner R : 08 = 0.8mm
   │   │   │   │    │    └ Thickness : 04 = 4.76mm
   │   │   │   │    └ Size : 12 = Cutting edge length 12.9mm (inscribed circle IC is 12.7mm)
   │   │   │   └ Format : Hole present + double-sided chipbreaker
   │   │   └ Tolerance grade : M (General grade)
   │   └ Clearance angle : N = 0° (Negative)
   └ Shape : C = 80° diamond

1) Shape — Strength and Accessibility Are Inversely Proportional

2) Clearance Angle — Negative or Positive

> Strong machine + thick material = Negative (N), weak clamping + thin wall + internal diameter = Positive (C·P). Using a negative insert on a thin pipe can cause vibration due to the cutting force.

3) Tolerance Grade (Third Character)

4) Format — Hole and Chipbreaker

5~7) Size, Thickness, Corner R

Size symbol = Integer part of cutting edge length (mm)
   ※ This is different from the inscribed circle (IC) diameter. Don't confuse them.

  CNMG 12 → Cutting edge length 12.9mm (IC 12.7)
  DNMG 15 → Cutting edge length 15.5mm (IC 12.7)
  TNMG 16 → Cutting edge length 16.5mm (IC 9.525)
  WNMG 08 → Cutting edge length  8.7mm (IC 12.7)

Thickness
  02 = 2.38mm   03 = 3.18mm   04 = 4.76mm   06 = 6.35mm

Corner R
  00 = Sharp   02 = 0.2mm   04 = 0.4mm
  08 = 0.8mm  12 = 1.2mm   16 = 1.线

Decoding Three Real Codes

DNMG150608
  D=55° diamond / N=clearance angle 0° / M=tolerance M grade / G=hole + double-sided chipbreaker
  15 = cutting edge length 15.5mm / 06 = thickness 6.35mm / 08 = corner R 0.8mm
  → Contour machining medium roughing. Sharp corner for contour following, but weak

VBMT160404
  V=35° diamond / B=clearance angle 5° (positive) / M=tolerance M grade / T=conical hole + single-sided chipbreaker
  16 = cutting edge length 16.6mm / 04 = thickness 4.76mm / 04 = corner R 0.4mm
  → Finishing for narrow corners. Small cutting force suitable for thin walls and shafts

CCMT09T304
  C=80° diamond / C=clearance angle 7° / M=tolerance M grade / T=conical hole + single-sided chipbreaker
  09 = cutting edge length 9.7mm (IC 9.525) / T3 = thickness 3.97mm / 04 = corner R 0.4mm
  → Small positive boring bar. Standard for internal finishing

What comes after is also information. For example, in CNMG120408-PM, the two letters after the hyphen are the chipbreaker code. This varies by manufacturer, but generally the first letter indicates the work material group (P steel / M stainless steel / K cast iron), and the second letter indicates the machining area (F finishing / M semi-finishing / R roughing). The numbers and letters after that are the material and coating code, which must be confirmed in the manufacturer's catalog.

3. Holder Codes Are Also Read in the Same Way

P   C   L   N   R  2525  M  12
│   │   │   │   │   │    │   └ Insert size (12 = CNMG12__)
│   │   │   │   │   │    └ Tool overall length : M = 150mm
│   │   │   │   │   └ Shank : 25 × 25mm
│   │   │   │   └ Hand : R right-hand / L left-hand / N both
│   │   │   └ Insert clearance angle : N = 0°
│   │   └ Holder style (access angle) : L = 95°
│   └ Insert shape : C = 80° diamond
└ Clamping method : P = lever clamp (S screw / M top + pin / C top)

PCLNR2525M12 only fits CNMG12 series inserts. Forcing a DNMG insert in will cause it to not fit the seat, and the insert will pop out during cutting.

For internal boring bars, the shank information is added at the beginning.

S 25 S - PCLNR 12
│  │  └ Shank length code (S = 250mm)
│  └ Shank diameter 25mm
└ Shank material/lubrication : S = steel, no internal lubrication
                   A = steel + internal lubrication / E = carbide + internal lubrication

What the Access Angle (κr) Does

4. Corner R — Determines Surface Roughness and Strength at the Same Time

A larger corner R means stronger cutting edge and longer life, but radial force increases, causing the workpiece to bend. A smaller corner R means less force but is more prone to breakage.

Theoretical surface roughness Rz(μm) ≈ f² / (8 × rε) × 1000
   f = feed (mm/rev), rε = corner R (mm)

Example 1)  f = 0.20,  rε = 0.8
   Rz ≈ 0.04 / 6.4 × 1000 = 6.25 μm    (Ra approximately 1.5~1.6)
   → If the drawing specifies Ra 1.6, there is almost no margin

Example 2)  Lower f to 0.15
   Rz ≈ 0.0225 / 6.4 × 1000 = 3.5 μm   (Ra approximately 0.9)
   → Safe. However, cycle time increases by 33%

Example 3)  Keep f at 0.20 and increase rε to 1.2
   Rz ≈ 0.04 / 9.6 × 1000 = 4.2 μm     (Ra approximately 1.0)
   → Maintains feed while controlling surface finish. However, cutting force increases

> Set the cutting depth (ap) to at least 2/3 of the corner R. Using an R0.8 insert with an ap of 0.3mm causes chips to flow only within the corner R, creating radial force and chatter. This is the most common cause of "Why is it vibrating even though it's finishing?"

5. Grooving, Cutting, and Threading

Grooving and Cutting

• The insert width is the groove width. MGMN300 = 3.0mm width. Check the drawing first to choose the insert.
• Cutting should minimize protrusion. Only extend slightly beyond the cutting diameter to avoid breakage.
• Keep the feed low, around 0.05~0.15mm/rev. Change to G97 (constant speed) from G96 (constant surface speed) near the center to prevent excessive RPM.
• Reduce the feed for the last 0.5mm before cutting. If you push it directly, a burr will remain on the end face of the product.

Threading

• Partial profile (e.g., 16ER AG60) creates only a 60° profile and can be used for various pitches, while full profile (e.g., 16ER 1.5ISO) is dedicated to a specific pitch and completes the thread in one pass. For a variety of products, partial profile is better, and for mass production, full profile is better.
• Threads cannot be cut in one pass. Based on ISO metric threads, the height of the thread is approximately 0.61 × pitch.

M20 × 1.5  external thread
  Thread height (radius) ≈ 0.613 × 1.5 ≈ 0.92mm
  Diameter must be reduced by 1.84mm (φ20 → φ18.16)
  Divide into 8~12 passes, last 1~2 passes are spring passes (no feed)

• During threading, the feed override is not effective. The rotation and feed are synchronized, so if you make a mistake, there is no way to correct it. Always use single block for the first cycle.

6. Common Mistakes Made by New Employees

> Insert screws have specified torque. The habit of tightening by hand is the number one cause of screw breakage. Keep a dedicated torque driver in the tool holder.

Checklist

• Can explain the meaning of the 7-character code of the currently used insert
• The insert size in the holder code matches the actual insert size
• Cleaned the insert seat with air or brush before seating the insert
• Tightened the screw with a torque driver
• Cutting depth is at least 2/3 of the corner R
• Extended the boring bar only as much as needed
• Matched the center height of the cutting and grooving tools