G12.1–G13.1

Format and notes

G12.1 ; (on a line of its own. The C position at this moment becomes 0°)
G01 G42 X_ C_ F_ ; (C is written as a length, as a virtual Y axis)
…
G40 … ;
G13.1 ; (on a line of its own)

• Lets you write the motion of a linear axis (X) and a rotary axis (C) in virtual Cartesian coordinates (X and Y) on the end face. Used on a lathe with a rotating tool to cut flats (across-flats), hexagons and keyways on the end face
• Why it is useful: when X and C move together, 1° of C is a longer distance the farther you are from the center, so the combined feed rate changes with position. With polar coordinate interpolation, the NC does this conversion, so you can write F in Cartesian coordinates as is. Previously the program was broken into many small blocks and the feed was calculated by hand (this is cited as the problem in a Hitachi Seiki patent)
• Return the C axis to its origin first. The C position at the moment G12.1 is commanded is treated as 0° (Siemens ISO dialect)
• Write G12.1 and G13.1 each on a line of its own, with no other commands. A reset also cancels it (Siemens ISO dialect)
• Turn on tool radius compensation (G41, G42) after G12.1 and cancel it before G13.1
• The plane specification (G17, etc.), whether X is written as a diameter or a radius, and the name of the virtual axis differ by model (in the Siemens ISO dialect for milling, G12.1 cancels the previous plane specification). The format above is only a skeleton, so always check the operator's manual
• Watch out for mixed-up numbers: G12 and G13 without a decimal point are circular pocket milling on Haas machining centers. In Mitsubishi Electric lathe G-code lists 2–5, G12.1 and G13.1 themselves are a different function (milling interpolation)

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.