G77 Back Bore Canned Cycle (Group 09)

Next Generation 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
F - Feedrate
*I - Shift value along the X Axis before retracting, if Q is not specified
*J - Shift value along the Y Axis before retracting, if Q is not specified
*L - Number of holes to bore if G91 (Incremental Mode) is used
*Q - The shift value, always incremental
*R - Position of the R plane
*X - X-Axis location of hole
*Y - Y-Axis location of hole
*Z - Z-Axis position to cut to

* indicates optional

caution: Unless you specify otherwise, this canned cycle uses the most recently commanded spindle direction (M03, M04, or M05). If the program did not specify a spindle direction before it commands this canned cycle, the default is M03 (clockwise). If you command M05, the canned cycle will run as a “no-spin” cycle. This lets you run applications with self-driven tools, but it can also cause a crash. Be sure of the spindle direction command when you use this canned cycle.

In addition to boring the hole, this cycle shifts the X and Y Axis before and after the cut, to clear the tool while it enters and exits the workpiece (refer to G76 for an example of a shift move). Setting 27 defines the shift direction. If you do not specify a Q value, the control uses the optional I and J values to determine the shift direction and distance.

G77 Back Boring Canned Cycle Example

Program Example

% O60077 (G77 CYCLE-WORKPIECE IS 1.0" THICK) ; T5 M06 (BACK COUNTERBORE TOOL) ; G90 G54 G00 X0 Y0 (INITIAL POSITION) ; S1200 M03 (SPINDLE START) ; G43 H05 Z.1 (TOOL LENGTH COMPENSATION) ; G77 Z-1. R-1.6 Q0.1 F10. (1ST HOLE) ; X-2. (2ND HOLE) ; G80 G00 Z.1 M09 (CANCEL CANNED CYCLE) ; G28 G91 Z0. M05 ; M30 ; %

G77 Approximate Toolpath Example. This example shows the entrance motion only. Dimensions are not to scale.

note: For this example, the “top” of the workpiece is the surface defined as Z0. in the current work offset. The “bottom” of the workpiece is the opposite surface.

In this example, when the tool reaches the R depth, it then moves 0.1" in X (the Q value and Setting 27 define this movement; in this example, Setting 27 is X+). The tool then feeds to the Z value at the given feedrate. When the cut is finished, the tool shifts back toward the center of the hole and retracts out of it. The cycle repeats at the next commanded position until the G80 command.

note: The R value is negative, and it must go past the bottom of the part for clearance.
note: The Z value is commanded from the active Z work offset.
note: You do not need to command an initial point return (G98) after a G77 cycle; the control assumes this automatically.

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.