G07.1

Format and notes

G07.1 C_ (ON with the cylinder radius) … G07.1 C0 (OFF)
Milling side: G07.1 A_ (B_ or C_) (rotary axis name and radius)

• Lets you write the program on a plane obtained by unrolling the outer surface of a cylinder (Z horizontally, the circumferential direction vertically). Used to cut cam grooves, helical grooves and engraving on the outer surface of a shaft
• C is written as an angle, and the NC converts it to a length along the circumference as “radius × angle” to calculate the feed. Whether the radius given in G07.1 matches the groove bottom or the outer surface changes the groove shape (width and slant). Check which diameter the drawing dimensions are based on
• Write ON and OFF each on a line of its own, with no other commands
• A program cannot be restarted from a line in the middle of cylindrical interpolation (Siemens ISO dialect)
• Turn on tool radius compensation after ON, and cancel it before OFF
• How the plane is specified differs by model. The Mitsubishi Electric example commands G19 (Y-Z cylindrical plane) before ON. Always check the operator's manual
• A common mistake: dropping “.1” and writing G7. G7 in LinuxCNC is lathe diameter mode, a completely different function

Example

G00 C0 ;
G07.1 C30. ;            (ON as a cylinder of radius 30 mm)
G01 G42 Z-10. C90. F100 ;
…                       (C is an angle. The NC converts it to a circumferential length as radius × angle)
G40 … ;
G07.1 C0 ;              (OFF)

This is only a skeleton example written by Kezuriba. How the plane is specified and how tool radius compensation is applied differ by model, so compare it with the examples in your operator's manual.

Differences between controls and machines

The same code can be written or assigned differently depending on the CNC control and the machine builder. Always check your machine’s manual.