G84 Tapping Canned Cycle (Group 09)

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

G84 Tapping Canned Cycle (Group 09)

F - Feed Rate
*R - Position of the R plane
S - RPM, called prior to G84
*W - Z-axis incremental distance
*X - X-axis motion command
Z - Position of bottom of hole

* indicates optional

Programming Notes:

  • It is not necessary to start the spindle CW before this canned cycle. The control does this automatically.

  • When G84 tapping on a lathe, it is simplest to use G99 Feed Per Revolution.

  • The Lead is the distance traveled along a screw's axis, with each full revolution.

  • The feedrate, when using G99, is equal to the Lead of the tap.

  • An S value must be called prior to the G84. The S value determines the RPM of the tapping cycle.

  • In Metric Mode (G99, with Setting 9 = MM), the feedrate is the metric equivalent of the lead, in MM.

  • In Inch Mode (G99, with Setting 9 = INCH), the feedrate is the Inch equivalent of the lead, in inches.

  • The lead (and G99 feedrate) of an M10 x 1.0mm tap is 1.0mm, or .03937" (1.0/25.4=.03937).

Examples:

  1. The lead of a 5/16-18 tap is 1.411 mm (1/18*25.4 = 1.411), or .0556" (1/18 = .0556)

  2. This canned cycle can be used on the secondary spindle of a Dual Spindle DS lathe, when prefaced by a G14. Refer to the G14 Secondary Spindle Swap on page G14 Secondary Spindle Swap / G15 Cancel (Group 17) for more information.

  3. For Axial Live-Tool tapping, use a G95 or G186 command.

  4. For Radial Live-Tool tapping, use a G195 or G196 command.

  5. For Reverse Tapping (left-hand thread) on the Main or Secondary Spindle, refer to  G184 Reverse Tapping Canned Cycle For Left Hand Threads (Group 09).

More programming examples, in both Inch and Metric, are shown below:

G84 Tapping Canned Cycle: [1] Rapid, [2] Feed, [3] Start or end of stroke, [4] Starting plane, [R] R plane, [Z] Position at the bottom of the hole.

% o60841 (IMPERIAL TAP, SETTING 9 = MM) ; (G54 X0 is at the center of rotation) ; (Z0 is on the face of the part) (T1 is a 1/4-20 Tap) ; G21 (ALARM if setting 9 is not MM) ; (BEGIN PREPARATION BLOCKS) ; T101 (Select tool and offset 1) ; G00 G18 G40 G80 G99 (Safe startup) ; G00 G54 X0 Z12.7 (Rapid to 1st position) ; M08 (Coolant on) ; S800 (RPM OF TAP CYCLE) ; (BEGIN CUTTING BLOCK) ; G84 Z-12.7 R12.7 F1.27 (1/20*25.4 = 1.27) ; (BEGIN COMPLETION BLOCKS) ; G00 G53 X0 M09 (X home, coolant off) ; G53 Z0 M05 (Z home, spindle off) ; M30 (End program) ; %
% o60842 (METRIC TAP, SETTING 9 = MM) ; (G54 X0 is at the center of rotation) ; (Z0 is on the face of the part) (T1 is an M8 x 1.25 Tap) ; G21 (ALARM if setting 9 is not MM) ; (BEGIN PREPARATION BLOCKS) ; T101 (Select tool and offset 1) ; G00 G18 G40 G80 G99 (Safe startup) ; G00 G54 X0 Z12.7 (Rapid to 1st position) ; M08 (Coolant on) ; S800 (RPM OF TAP CYCLE) ; (BEGIN CUTTING BLOCK) ; G84 Z-12.7 R12.7 F1.25 (Lead = 1.25) ; (BEGIN COMPLETION BLOCKS) ; G00 G53 X0 M09 (X home, coolant off) ; G53 Z0 M05 (Z home, spindle off) ; M30 (End program) ; %
% o60843 (IMPERIAL TAP, SETTING 9 = IN) ; (G54 X0 is at the center of rotation) ; (Z0 is on the face of the part) (T1 is a 1/4-20 Tap) ; G20 (ALARM if setting 9 is not INCH) ; (BEGIN PREPARATION BLOCKS) ; T101 (Select tool and offset 1) ; G00 G18 G20 G40 G80 G99 (Safe startup) ; G00 G54 X0 Z0.5 (Rapid to 1st position) ; M08 (Coolant on) ; S800 (RPM OF TAP CYCLE) ; (BEGIN CUTTING BLOCK) ; G84 Z-0.5 R0.5 F0.05 (Begin G84) ; (1/20 = .05) ; (BEGIN COMPLETION BLOCKS) ; G00 G53 X0 M09 (X home, coolant off) ; G53 Z0 M05 (Z home, spindle off) ; M30 (End program) ; %
% o60844 (METRIC TAP, SETTING 9 = IN) ; (G54 X0 is at the center of rotation) ; (Z0 is on the face of the part) (T1 is an M8 x 1.25 Tap) ; G20 (ALARM if setting 9 is not INCH) ; (BEGIN PREPARATION BLOCKS) ; T101 (Select tool and offset 1) ; G00 G18 G20 G40 G80 G99 (Safe startup) ; G00 G54 X0 Z0.5 (Rapid to 1st position) ; M08 (Coolant on) ; S800 (RPM OF TAP CYCLE) ; (BEGIN CUTTING BLOCK) ; G84 Z-0.5 R0.5 F0.0492 (1.25/25.4 = .0492) ; (BEGIN COMPLETION BLOCKS) ; 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