When milling in a straight line, the tool's center and its cutting edge move at the same speed. However, as soon as you program a circular arc (G02 or G03), this relationship breaks. If you don't adjust your feed rate, you are likely over-feeding or under-feeding your tool, leading to poor finishes or broken cutters.

1. The Problem: Centerline Feed Control

CNC controllers typically calculate feed rate based on the centerline path of the tool. In a circular path, the distance traveled by the tool center is different from the distance traveled by the cutting edge at the part surface.

Internal Milling (Holes/Pockets)

When milling a hole, the cutting edge travels a shorter distance than the tool center. If you use the linear feed rate, the actual chip load at the edge becomes much higher than programmed. This leads to excessive tool pressure, heat, and potential breakage.

Result: You must DECREASE the feed rate.

External Milling (Bosses/Pins)

When milling around a boss, the cutting edge travels a longer distance than the tool center. If you use the linear feed rate, the actual chip load at the edge becomes lower than programmed, reducing productivity.

Result: You can INCREASE the feed rate.

2. The Formulas for Compensation

To find the correct programmed feed ($F_{center}$) to achieve your desired chip load at the part edge ($F_{edge}$), use the following formulas:

For Internal Arcs (Holes):
$$F_{center} = F_{edge} \times \frac{(Hole\ Radius - Tool\ Radius)}{Hole\ Radius}$$
For External Arcs (Bosses):
$$F_{center} = F_{edge} \times \frac{(Boss\ Radius + Tool\ Radius)}{Boss\ Radius}$$
Haas Tip of the Day: Circular Feed

Watch Mark Terryberry explain the mechanics of how "The Edge" moves faster than the "Center" and why compensation is non-negotiable for high-quality parts.

Circular Feed Calculator

Don't risk snapping a tool by doing the math in your head. Use our specialized tool to get the exact adjusted feed rate for your specific tool and arc diameter.

Calculate Circular Feed

3. Why This Matters

  • Dimensional Accuracy: Over-feeding in a hole causes tool deflection, meaning your hole will end up undersized or tapered.
  • Surface Finish: Consistent chip load is required for a smooth finish. Compensating prevents "torn" surfaces in internal radii.
  • Tool Life: In tough materials like Stainless or Titanium, failing to compensate for internal paths will cause immediate edge chipping.

Conclusion

Circular feed compensation is a fundamental skill for high-precision milling. While some modern CAM systems handle this automatically, knowing how to calculate it manually allows you to make adjustments at the machine controller, saving tools and ensuring your parts meet specifications every time.