Cutting Process Theory

Rotational Speed and Cutting Speed Are Different

When you first arrive on site, you might be asked, "At how many rotations should it be set?" However, the answer is that it changes every time depending on the material and the tool diameter.

• N (Rotational Speed) — How many times the spindle rotates per minute. Unit: rpm (min⁻¹)
• Vc (Cutting Speed) — The speed at which the tool tip passes through the material. Unit: m/min

What determines the tool life, surface condition, and heat is not the rotational speed, but Vc. If you rotate a φ10 end mill and a φ100 face mill at the same 1,000rpm, the tip speed differs by 10 times. That's why the condition tables are written using Vc, not rotational speed.

There Is Only One Formula

        π × D × N
Vc = ─────────────  (m/min)
          1000

D = Diameter (mm)   N = Rotational Speed (rpm)

When calculating rotational speed, reverse the formula

        1000 × Vc
N  = ─────────────  (rpm)
         π × D

Dividing by 1000 is just converting mm to m. There is nothing complicated about it.

Let's Try It Three Times by Plugging in Numbers

① Milling — φ50 face mill for SM45C surface machining, recommended Vc 150

N = 1000 × 150 / (3.1416 × 50)
  = 150,000 / 157.08
  = 954.9  →  Approximately 955 rpm

② Turning — φ80 bar (SM45C) outer diameter, recommended Vc 200

N = 1000 × 200 / (3.1416 × 80)
  = 200,000 / 251.33
  = 795.8  →  Approximately 796 rpm

③ Drilling — φ8 HSS drill for SS400 hole, recommended Vc 25

N = 1000 × 25 / (3.1416 × 8)
  = 25,000 / 25.13
  = 994.7  →  Approximately 995 rpm

In all three cases, the rotational speed is similar, around 800–1,000rpm, but the materials and tools are completely different. This is why you can't just memorize the rotational speed.

Cases Where the Machine Can't Keep Up

If you want to machine aluminum with a φ10 carbide end mill at Vc 300,

N = 300,000 / (3.1416 × 10) = 9,549 rpm

However, general-purpose machining centers on site often have a maximum spindle speed of 8,000rpm. If you rotate at 8,000rpm, the actual Vc is

Vc = 3.1416 × 10 × 8000 / 1000 = 251 m/min

You are machining under the recommended conditions. If you don't know this, you might end up asking, "Why isn't the surface coming out even though I followed the catalog?" Remember that the speed limit is reached by the machine's rotational speed for small-diameter tools.

The D in Lathes and Milling Machines Is Different

When doing facing on a lathe, the D becomes smaller as the insert moves toward the center, causing Vc to keep decreasing. If you continue cutting up to the φ20 point using the condition from ② (796rpm fixed),

Vc = 3.1416 × 20 × 796 / 1000 = 50 m/min

It drops from 200 to 50. This is why the surface tears and tool marks appear near the center.

> On a CNC lathe, using G96 (constant surface speed cutting) allows the controller to automatically increase the rotational speed according to the diameter change. However, as the center is approached, the rotational speed can rise infinitely, so always set the maximum rotational speed using G50 S○○○. If you don't, the chuck may reach dangerous speeds. When specifying rotational speed directly, use G97.

Recommended Cutting Speeds by Material

This is based on roughing to semi-finishing using superhard coated inserts for turning. The actual values should be prioritized from the tool manufacturer's catalog.

> HSS (high-speed steel) tools should be set to 1/4–1/5 of the above values, and drilling even lower (for mild steel, Vc 20–30). If you apply superhard conditions to a φ8 HSS drill, the insert will break within a few seconds.

What Gets Worse When You Increase Vc

Cutting speed is the variable that has the greatest impact on tool life. It is much more sensitive than feed or depth of cut.

Vc ↑  →  Machining time ↓ (Good)
         Cutting temperature ↑↑
         Tool wear ↑↑↑  ← This reacts the fastest

If you calculate using Taylor's tool life equation discussed in the experience section, tool life drops to less than half when speed increases by 25%. Conversely, even a 20% decrease in speed can more than double the tool life. "Spinning faster to finish faster" is not always beneficial.

Common Mistakes Made by Newcomers

Pre-Work Checklist

• Checked the material type from the drawing and material list
• Checked the tool type (HSS / superhard / coated / sintered)
• Accurately entered the diameter (turning = workpiece, milling = tool) to calculate N
• The calculated N is within the machine's maximum rotational speed
• Checked whether the chuck and vise can withstand that rotational speed