# G74 Reverse Tap 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.

F - Feedrate. Use the formula described in the canned cycle introduction to calculate feedrate and spindle speed.
* J - Retract Multiple (How fast to retract - see Setting 130)
* L - Number of loops (How many holes to tap) if G91 (Incremental Mode) is used
* R - Position of the R plane (position above the part) where tapping starts
* X - X-Axis location of hole
* Y - Y-Axis location of hole
Z - Position of the Z-Axis at the bottom of hole

*indicates optional

## G74 Tapping Canned Cycle

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

*indicates optional

## G74 End Face Grooving Cycle Peck Drilling: [1] Rapid, [2] Feed, [3] Programmed Path, [S] Start position, [P] Peck retraction (Setting 22).

The G74 canned cycle is used for grooving on the face of a part, peck drilling, or turning.

A minimum of two pecking cycles occur, if an X, or U, code is added to a G74 block and X is not the current position. One at the current location and then at the X location. The I code is the incremental distance between X-Axis pecking cycles. Adding an I performs multiple pecking cycles between the starting position S and X. If the distance between S and X is not evenly divisible by I then the last interval is less than  I.

When K is added to a G74 block, pecking is performed at each interval specified by K, the peck is a rapid move opposite the direction of feed with a distance defined by Setting 22. The D code can be used for grooving and turning to provide material clearance when returning to starting plane  S.

## G74 End Face Grooving Cycle: [1] Rapid, [2] Feed, [3] Groove.

% O60741 (G74 END FACE) ; (G54 X0 is at the center of rotation) ; (Z0 is on the face of the part) ; (T1 is an end face cutting 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 X3. Z0.1 (Rapid to 1st position) ; M08 (Coolant on) ; G96 S200 (CSS on) ; (BEGIN CUTTING BLOCKS) ; G74 Z-0.5 K0.1 F0.01 (Begin G74) ; (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) ; %

## G74 End Face Grooving Cycle (Multiple Pass): [1] Rapid, [2] Feed, [3] Programmed path, [4] Groove.

% O60742 (G74 END FACE MULTI PASS) ; (G54 X0 is at the center of rotation) ; (Z0 is on the face of the part) ; (T1 is an end face cutting 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 X3. Z0.1 (Rapid to 1st position) ; M08 (Coolant on) ; G96 S200 (CSS on) ; (BEGIN CUTTING BLOCKS) ; G74 X1.75 Z-0.5 I0.2 K0.1 F0.01 (Begin G74) ; (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.