G31

Format and notes

G31 X_ Y_ Z_ F_ (lathe: G31 X(U)_ Z(W)_ F_)

• Moves in a straight line like G01 until a signal, such as from a touch probe, comes in; when the signal arrives it stops on the spot, discards the rest of the move and goes on to the next line. Used to measure workpiece height and position, and for feeding until contact
• One-shot (group 00). Write it on every line where it is used
• The stopped position is stored in variables, so a macro can use the measured value in calculations. Variable numbers differ by model (Haas: #5061–#5066)
• Cancel tool radius compensation and tool nose radius compensation (G41, G42) before commanding it (the Siemens ISO dialect gives an alarm, Mitsubishi Electric a program error, and Haas states explicitly that they must not be used together)
• If the next line is an incremental command, it moves from the stopped position. If it is an absolute command, it moves to the commanded position. If only one axis is given as an absolute command, the axes not written stay at the stopped position (Siemens ISO dialect, Mitsubishi Electric)
• If no signal comes in, some models stop with an alarm and others move to the end point and carry on as if nothing had happened. On the models that carry on, a macro compares the stopped position with the end point to decide that it “did not touch”
• Always write F. To protect the probe, do not set the feed too high (Haas recommends less than 2500 mm/min)

Example

G00 G90 G54 X0 Y0 ;
G43 H01 Z10. ;        (probe tool length)
G31 Z-5. F200 ;       (stops on contact. Always write F)
#100 = #5063 ;        (Z where it stopped. #5063 is the Haas number)
G00 Z10. ;

A skeleton example written by Kezuriba for measuring the height of the top surface of a workpiece with a touch probe. The variable number that stores the stopped position differs by model.

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.