G75 O.D./I.D. Grooving Cycle (Group 00)

Classic Control - Lathe 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
*D - Tool clearance when returning to starting plane, positive
*F - Feed rate
*I - X-axis size of increment between pecks in a cycle (radius measure)
*K - Z-axis size of increment between peck cycles
*U - X-axis incremental distance to total pecking depth
W - Z-axis incremental distance to furthest peck cycle
X - X-axis absolute location total pecking depth (diameter)
Z - Z-axis absolute location to furthest peck cycle

* indicates optional

G75 O.D./I.D. Grooving Cycle: [1] Rapid, [2] Feed, [S] Start position.

The G75 canned cycle can be used for grooving an outside diameter. When a Z, or W, code is added to a G75 block and Z is not the current position, then a minimum of two pecking cycles occur. One at the current location and another at the Z location. The K code is the incremental distance between Z axis pecking cycles. Adding a K performs multiple, evenly spaced, grooves. If the distance between the starting position and the total depth (Z) is not evenly divisible by K then the last interval along Z is less than K.

note: Chip clearance is defined by Setting 22.

G75 O.D. Single Pass

% O60751 (G75 OD GROOVE CYCLE) ; (G54 X0 is at the center of rotation) ; (Z0 is on the face of the part) ; (T1 is an OD groove tool) ; (BEGIN PREPARATION BLOCKS) ; T101 (Select tool and offset 1) ; G00 G18 G20 G40 G80 G99 (Safe startup) ; G50 S1000 (Limit spindle to 1000 RPM) ; G97 S500 M03 (CSS off, spindle on CW) ; G00 G54 X4.1 Z0.1 (Rapid to 1st position) ; M08 (Coolant on) ; G96 S200 (CSS on) ; (BEGIN CUTTING BLOCKS) ; G01 Z-0.75 F0.05 (Feed to Groove location) ; G75 X3.25 I0.1 F0.01 (Begin G75) ; (BEGIN COMPLETION BLOCKS) ; G97 S500 (CSS off) ; G00 G53 X0 M09 (X home, coolant off) ; G53 Z0 M05 (Z home, spindle off) ; M30 (End program) ; %

The following program is an example of a G75 program (Multiple Pass):

G75 O.D. Multiple Pass: [1] Tool, [2] Rapid, [3] Feed, [4] Groove.

% O60752 (G75 OD GROOVE CYCLE 2) ; (G54 X0 is at the center of rotation) ; (Z0 is on the face of the part) ; (T1 is an OD groove tool) ; (BEGIN PREPARATION BLOCKS) ; T101 (Select tool and offset 1) ; G00 G18 G20 G40 G80 G99 (Safe startup) ; G50 S1000 (Limit spindle to 1000 RPM) ; G97 S500 M03 (CSS off, spindle on CW) ; G00 G54 X4.1 Z0.1 (Rapid to 1st position) ; M08 (Coolant on) ; G96 S200 (CSS on) ; (BEGIN CUTTING BLOCKS) ; G01 Z-0.75 F0.05 (Feed to Groove location) ; G75 X3.25 Z-1.75 I0.1 K0.2 F0.01 (Begin G75) ; (BEGIN COMPLETION BLOCKS) ; G97 S500 (CSS off) ; G00 G53 X0 M09 (X home, coolant off) ; G53 Z0 M05 (Z home, spindle off) ; 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.

Feedback