G107 Description

Classic Control - Mill Operator's Manual

The Online Interactive Operator's Manual is currently available in English only.

A PDF version of the Operator's Manual is available for download in multiple languages. Click the link below to view the Operator's Manual in your language. Click "Continue" to view the online version in English.

Get a translated PDF Download Continue

Three address codes can follow a G107: X, Y, or Z; A, B, or C; and Q or R.

X, Y, or Z: An X, Y, or Z address specifies the linear axis that will be mapped to the specified rotary axis (A or B). When one of these linear axes is specified, a rotary axis must also be specified.

A or B: An A or B address identifies which rotary axis holds the cylindrical surface.

Q or R: Q defines the diameter of the cylindrical surface, while R defines the radius. When Q or R is used, a rotary axis must also be specified. If neither Q nor R is used, then the last G107 diameter is used. If no G107 command has been issued since power-up, or if the last value specified was zero, then the diameter will be the value in Setting 34 and/or 79 for this rotary axis. When Q or R is specified, that value will become the new G107 value for the specified rotary axis.

Cylindrical mapping will also be turned off automatically whenever the G-code program ends, but only if Setting 56 is ON. Pressing RESET turns off any cylindrical mapping that is currently in effect, regardless of the status of Setting 56.

Cylindrical Mapping Example

While R is suitable for defining the radius, it is recommended that I, J and K are used for more complex G02 and G03 programming.

% O61071 (G107 CYLINDRICAL MAPPING) ; (G54 X0 Y0 is in center of rectangular slot) ; (Z0 is on highest point of cylindrical surface) ; (T1 is a .625 in. dia endmill) ; (BEGIN PREPARATION BLOCKS) ; T1 M06 (Select tool 1) ; G00 G90 G40 G49 G54 (Safe startup) ; G28 G91 A0 (Home A axis) ; G00 G90 G54 X1.5 Y0 (Rapid to 1st position) ; S5000 M03 (Spindle on CW) ; G107 A0 Y0 R2. (Cylindrical mapping on) ; (Move to A0 Y0, Part has radius of 2 inches) ; G43 H01 Z0.1 (Activate tool offset 1) ; M08 (Coolant on) ; (BEGIN CUTTING BLOCKS) ; G01 Z-0.25 F25. (Feed to depth of cut) ; G41 D01 X2. Y0.5 (Cutter comp on) ; G03 X1.5 Y1. R0.5 (CCW cutting move) ; G01 X-1.5 (Linear cutting move) ; G03 X-2. Y0.5 R0.5 (CCW cutting move) ; G01 Y-0.5 (Linear cutting move) ; G03 X-1.5 Y-1. R0.5 (CCW cutting move) ; G01 X1.5 (Linear cutting move) ; G03 X2. Y-0.5 R0.5 (CCW cutting move) ; G01 Y0. (Linear cutting move) ; G40 X1.5 (Cutter comp off) ; (BEGIN COMPLETION BLOCKS) ; G00 Z0.1 M09 (Rapid retract, Coolant off) ; G91 G28 A0. (Home A axis) ; G107 (Cylindrical mapping off) ; G90 G53 G49 Z0 M05 (Z home, Spindle off) ; G53 Y0 (Y home) ; M30 (End program) ; %

Be aware: Many service and repair procedures should be done only by authorized personnel. The service technicians at your Haas Factory Outlet (HFO) have the training, experience, and are certified to do these tasks safely and correctly. You should not do machine repair or service procedures unless you are qualified and knowledgeable about the processes.

Danger: Some service procedures can be dangerous or life-threatening. DO NOT attempt a procedure that you do not completely understand. Contact your Haas Factory Outlet (HFO) and schedule a service technician visit if you have any doubts about doing a procedure.