G Codes Mill Canned Cycles G70 To 74 G80 To 89

Front 1

What range of G-codes control canned cycles?

Back 1

G70-74; G80-89

Front 2

What kind of canned cycle does a G70 perform? What primary letters are used with a G70, and what do they mean? What two important rules govern the use of the G70 (106.98)?

Back 2

A bolt hole circle.
I = Radius of the bolt circle.
J = Starting angle of first hole from three o'clock, 0 to 360.0 deg.
L = Number of evenly spaced holes around bolt hole circle.
Rule #1: G70 must work in tandem with an active canned cycle.
Rule #2: The tool must be positioned at the center of the circle in a previous block or in the G70 block.
Sample Program:
O10099 (Bolt Hole Circle)
N1 T15 M06 (3/8 DIA. DRILL)
N2 G90 G54 G00 X2. Y-1.5 (Center position of bolt hole circle)
N3 S1620 M03
N4 G43 H15 Z1. M08 (G43 is tool length compensation +)
N5 G81 G99 Z-0.45 R0.1 F8. L0 (G81 is a "drill canned cycle." G99 is the Z position clearance location for positioning between holes.)
N6 G70 I1.25 J10. L8
N7 G80 G00 Z1. M09 (G80 is canned cycle cancel)
N8 G53 G49 Z0. M05 (G53 temporarily ignores work offsets, and positions the machine axes from machine home. It is non-modal; so the next block will revert back to the previously selected work offset. G49 is tool length compensation cancel)
N9 M30

(Having L0 on line N5 will cause machine to not do this command until the control reads the next line, so as not to drill a hole
in the center of bolt circle. Or you can combine N5 and N6 together, minus the L0, to also not drill a hole in the center.)

Front 3

What kind of canned cycle does a G71 perform? What primary letters are used with a G71, and what do they mean? What two important rules govern the use of the G71 (106.98)?

Back 3

A bolt hole arc.
I = Radius of the bolt hole arc
J = Starting angle of the first hole from three o'clock, 0 to 360 deg.
K = Angular spacing between holes (+ or -)
L = Number of evenly spaced holes around bolt hole arc
Rule #1: G71 must work in tandem with an active canned cycle.
Rule #2: The tool must be positioned at the center of the circle in a previous block or in the G71 block.
Sample Program:
O10100 (Bolt Hole Arc)
N1 T15 M06 (3/8 DIA. DRILL)
N2 G90 G54 G00 X2. Y-1.5 (Center position of bolt hole arc)
N3 S1450 M03
N4 G43 H15 Z1. M08 (G43 is tool length compensation +)
N5 G81 G99 Z-0.45 R0.1 F8. L0 (G81 is a "drill canned cycle." G99 is the Z position clearance location for positioning between holes.)
N6 G71 I0.875 J45. K36. L6
N7 G80 G00 Z1. M09 (G80 is canned cycle cancel)
N8 G53 G49 Z0. M05 (G53 temporarily ignores work offsets, and positions the machine axes from machine home. It is non-modal; so the next block will revert back to the previously selected work offset. G49 is tool length compensation cancel)
N9 M30

(Having L0 on line N5 will cause machine to not do this command until the control reads the next line, so as not to drill a hole
in the center of bolt circle. Or you can combine N5 and N6 together, minus the L0, to also not drill a hole in the center.)

Front 4

What kind of canned cycle does a G72 perform? What primary letters are used with a G72, and what do they mean? What two important rules govern the use of the G72 (106.98)?

Back 4

Bolt holes along an angle.
I = Distance between bolt holes along an angle
J = Angle of holes from three o'clock, 0 to 360.0 deg.
L = Number of evenly spaced holes along an angle
Rule #1: G71 must work in tandem with an active canned cycle.
Rule #2: The tool must be positioned at the center of the first hole in the series. Position must be written in a previous block or in the G72 block.
Sample Program:
O10101 (Bolt Holes Along An Angle)
N1 T16 M06 (1/2 DIA. DRILL)
N2 G90 G54 G00 X0.65 Y-1.5 (Start position of bolt holes along an angle)
N3 S1450 M03
N4 G43 H16 Z1. M08 (G43 is tool length compensation +)
N5 G81 G99 Z-0.45 R0.1 G72 I0.5 J20. L7 F8. (G81 is a "drill canned cycle." G99 is the Z position clearance location for positioning between holes.)
N6 G80 G00 Z1. M09 (G80 is canned cycle cancel)
N7 G53 G49 Z0. M05 (G53 temporarily ignores work offsets, and positions the machine axes from machine home. It is non-modal; so the next block will revert back to the previously selected work offset. G49 is tool length compensation cancel)
N8 M30

(Having L0 on line N5 will cause machine to not do this command until the control reads the next line, so as not to drill a hole
in the center of bolt circle. Or you can combine N5 and N6 together, minus the L0, to also not drill a hole in the center.)

Front 5

What kind of canned cycle does a G73 perform? What primary letters are used with a G73, and what do they mean? What two important rules govern the use of the G73 (100.92-103.95)?

Back 5

High Speed Peck Drill Canned Cycle
X* Rapid X-axis location
Y* Rapid Y-axis location
Z Z-depth (feed to Z-depth starting from R plane)
Q* Pecking equal incremental depth amount (if I, J and K are not used)
I* Size of first peck depth (if Q is not used)
J* Amount reducing each peck after first peck depth (if Q is not used)
K* Minimum peck depth (if Q is not used)
P* Dwell time at Z-depth
R R-plane (rapid point to start feeding)
F Feed rate in inches (mm) per minute
* Indicates optional
Rule #1: The G73 is modal so that it is activated every X and/or Y axis move until it is canceled.
Rule #2: Canned cycle can be used with I, J, and K or K and Q.
Sample Program:
O10095 (G73 High Speed Peck Drill Using K & Q)
N1 T10 M06 (7/8 DIA. INSERT DRILL)
N2 G90 G54 G00 X0.625 Y0.625 (Position of the first drilled hole.)
N3 S1450 M03
N4 G43 H10 Z1. M08 (G43 is tool length compensation +)
N5 G73 G99 Z-2.15 K1. Q0.2 R0.1 F9. (G73 is a high speed peck drill canned cycle. G99 is the Z position clearance location for positioning between holes.)
N6 X0.1.375 Y1.375 (Second hole)
N7 G80 G00 Z1. M09 (G80 is canned cycle cancel)
N8 G53 G49 Z0. M05 (G53 temporarily ignores work offsets, and positions the machine axes from machine home. It is non-modal; so the next block will revert back to the previously selected work offset. G49 is tool length compensation cancel)
N9 M30

Front 6

What kind of canned cycle does a G74 perform? What primary letters are used with a G74, and what do they mean? What two important rules govern the use of the G74 (91.83)?

Back 6

Reverse-tapping canned cycle.
X* Rapid X-axis location
Y* Rapid Y-axis location
Z Z-depth (tapping Z-depth starting from R plane)
J* Tapping Retract Speed (Rev. 10.13 and above)
R R-plane (rapid point to start feeding)
F Feed rate in inches (mm) per minute
* Indicates optional
Rule #1: The G74 is modal
Rule #2: On older machines without vector motors, if you're using a spindle speed that's in low gear you, may want to command M42 to force it into high gear, because most tapping (a smaller size tap) operations don't need the torque of low gear. And in high
gear the tapping operation performs quicker.
Rule #3: Newer machines have Setting 130, Tap Retract Speed, can be set with, 1 thru 9, to quick-reverse-out of thread up to 9 times faster then going in, If J is not used.
Rule #4: With Rigid Tapping, the ratio between feedrate and the spindle speed must be calculated for the thread pitch being cut. The calculation is 1/Threads Per Inch x rpm = tapping feedrate. Use the Haas calculator for the speed and feed numbers.
Sample Program:
O10083 (G74 L.H. Tapping Cycle)
N1 T18 M06 (7/16-14 L.H. TAP)
N2 G90 G54 G00 X-0.625 Y0.625
N3 S490 (You don't need M03, the
G84 turns on the spindle for you.)
N4 G43 H18 Z1. M08
N5 G74 G99 Z-0.65 R0.1 J3 F35.
N6 X0.625 Y0-.625
N7 G80 G00 Z1. M09 (cancel canned cycle)
N8 G53 G49 Z0. M05 (G53 temporarily ignores work offsets, and positions the machine axes from machine home. It is non-modal; so the next block will revert back to the previously selected work offset. G49 is tool length compensation cancel)
N9 M30

Front 7

What kind of canned cycles do the G70-G72 perform? What other canned cyles do these work in tandem with (106.98)?

Back 7

Bolt hole patterns. (Bolt hole circle: G70, Bolt hole arc: G71, Bolt holes along an angle: G72)
Work in tandem with G73-74; 76-77; or 81-89.

Front 8

What kind of canned cycle does a G80 perform?

Back 8

None. The G80 cancels a canned cycle.

Front 9

What kind of canned cycle does a G81 perform? What primary letters are used with a G81, and what do they mean? What two important rules govern the use of the G81 (83.75)?

Back 9

Drill can cycle.
X* Rapid X-axis location
Y* Rapid Y-axis location
Z Z-depth (feed to Z-depth starting from R plane)
R R-plane (rapid point to start feeding)
F Feed rate in inches (mm) per minute
* Indicates optional
Rule #1: The G81 is modal and the machine will rapid between each new X and or Y position.
Rule #2: Use G98 and G99 for the Z position clearance location for positioning between holes.
Sample program:
O10075 (G81 Drilling Cycle)
N1 T16 M06 (1/2 DIA. DRILL)
N2 G90 G54 G00 X0.5 Y-0.5 (position of first hole)
N3 S1450 M03
N4 G43 H16 Z1. M08
N5 G81 G99 Z-0.375 R0.1 F9. (G99 Z position clearance location)
N6 X1.5
N7 Y-1.5
N8 X0.5
N9 G80 G00 Z1. M09 (G80 cancels canned cycle)
N10 G53 G49 Z0. M05 (G53 temporarily ignores work offsets, and positions the machine axes from machine home. It is non-modal; so the next block will revert back to the previously selected work offset. G49 is tool length compensation cancel)
N11 M30

Front 10

What kind of canned cycle does a G82 perform? What primary letters are used with a G82, and what do they mean? What two important rules govern the use of the G82 (84.76)?

Back 10

Spot drill / Counterbore canned cycle.
X* Rapid X-axis location
Y* Rapid Y-axis location
Z Z-depth (feed to Z-depth starting from R plane)
P Dwell time at Z-depth
R R-plane (rapid point to start feeding)
F Feed rate in inches (mm) per minute
* Indicates optional
Rule #1: The G82 is modal and the machine will rapid between each new X and or Y position.
Rule #2: A dwell in seconds / milliseconds is defined with P.
Rule #3: Use G98 and G99 for the Z position clearance location for positioning between holes.
Sample program:
O10076 (G82 Drill~Dwell Cycle)
N1 T11 M06 (1/2 DIA. 2 FLT E.M.)
N2 G90 G54 G00 X0.5 Y-0.5 (position of first hole)
N3 S1200 M03
N4 G43 H11 Z1. M08
N5 G82 G99 Z-0.375 P0.5 R0.1 F7.5 (G99 Z position clearance location)
N6 X1.5
N7 Y-1.5
N8 X0.5
N9 G80 G00 Z1. M09 (G80 cancels canned cycle)
N10 G53 G49 Z0. M05 (G53 temporarily ignores work offsets, and positions the machine axes from machine home. It is non-modal; so the next block will revert back to the previously selected work offset. G49 is tool length compensation cancel)
N11 M30

Front 11

What kind of canned cycle does a G83 perform? What primary letters are used with a G83, and what do they mean? What two important rules govern the use of the G83 (85.77)?

Back 11

Deep hole peck drill canned cycle.
X* Rapid X-axis location
Y* Rapid Y-axis location
Z Z-depth (feed to Z-depth starting from R plane)
Q* Pecking equal incremental depth amount (if I, J and K are not used)
I* Size of first peck depth (if Q is not used)
J* Amount reducing each peck after first peck depth (if Q is not used)
K* Minimum peck depth (if Q is not used)
P Dwell time at Z-depth
R R-plane (rapid point to start feeding)
F Feed rate in inches (mm) per minute
* Indicates optional
Rule #1: The G83 is modal and the machine will rapid between each new X and or Y position.
Rule #2: After each peck, the tool will rapid up to the R plane and then back in for the next peck until Z depth is reached.
Rule #3: Use G98 and G99 for the Z position clearance location for positioning between holes.
Rule #4: If I, J, and K are specified, a different operating mode is selected. The first pass will cut in by I, each succeeding cut will be reduced by amount J, and the minimum cutting depth is K.
Rule #5: See guide for the use of settings 22 and 52.
Sample program:
O10078 (G83 Deep Hole Pedk Drill Using Q)
N1 T10 M06 (7/8 DIA. DRILL)
N2 G90 G54 G00 X0.625 Y0.625 (position of first hole)
N3 S1050 M03
N4 G43 H10 Z1. M08
N5 G83 G99 Z-2.3 Q0.5 R0.1 F8. (G99 Z position clearance location)
N6 X1.375 Y1.375
N7 G80 G00 Z1. M09 (G80 cancels canned cycle)
N8 G53 G49 Z0. M05 (G53 temporarily ignores work offsets, and positions the machine axes from machine home. It is non-modal; so the next block will revert back to the previously selected work offset. G49 is tool length compensation cancel)
N9 M30
Sample program #2:
O10079 (G83 Deep Hole Pedk Drill Using I, J & K)
N1 T16 M06 (1/2 DIA. DRILL)
N2 G90 G54 G00 X0.625 Y0.625
N3 S1833 M03
N4 G43 H16 Z1. M08
N5 G83 G99 Z-2.18 I0.5 J0.1 K0.2 R0.1 F9.
N6 X1.375 Y1.375
N7 G80 G00 Z1. M09
N8 G53 G49 Z0. M05
N9 M30

Front 12

What kind of canned cycle does a G84 perform? What primary letters are used with a G84, and what do they mean? What four important rules govern the use of the G84 (90.82)?

Back 12

Tapping canned cycle.
X* Rapid X-axis location
Y* Rapid Y-axis location
Z Z-depth (tapping Z-depth starting from R plane)
J* Tapping Retract Speed (Rev. 10.13 and above)
R R-plane (rapid point to start feeding)
F Feed rate in inches (mm) per minute
* Indicates optional
Rule #1: The G84 is modal.
Rule #2: You don't need to start the spindle with a M03
for a tap that's using G84 because this cycle will turn on the spindle for you automatically and it will do it quicker.
Rule #3: On older machines without vector motors, if your using a spindle speed that's in low gear you, may want to command M42 to force it into high gear, because most tapping (a smaller size tap) operations don't need the torque of low gear. And in high gear the tapping operation performs quicker.
Rule #4: Newer machines have Setting 130, Tap Retract Speed, can be set with, 1 thru 9, to quick-reverse-out of thread up to 9 times faster then going in, If J is not used.
Rule #5: With Rigid Tapping, the ratio between feedrate and the spindle speed must be calculated for the thread pitch being cut. The calculation is 1/Threads Per Inch x rpm = tapping feedrate. Use the Haas calculator for the speed and feed numbers.
Sample program:
O10082 (G84 R.H. Tapping Cycle)
N1 T18 M06 (7/16-14 TAP)
N2 G90 G54 G00 X0.625 Y0.625 (position of first hole)
N3 S500 (You don't need M03, the
G84 turns on the spindle for you.)
N4 G43 H18 Z1. M08
N5 G84 G99 Z-0.65 R0.1 J3 F35.7143 (G99 Z position clearance location)
N6 X-0.625 Y-0.625
N7 G80 G00 Z1. M09 (G80 cancels canned cycle)
N8 G53 G49 Z0. M05 (G53 temporarily ignores work offsets, and positions the machine axes from machine home. It is non-modal; so the next block will revert back to the previously selected work offset. G49 is tool length compensation cancel)
N9 M30

Front 13

What kind of canned cycle does a G85 perform? What primary letters are used with a G85, and what do they mean? What two important rules govern the use of the G85 (92.84)?

Back 13

Bore in - bore out canned cycle.
X* Rapid X-axis location
Y* Rapid Y-axis location
Z Z-depth (feed to Z-depth starting from R plane)
R R-plane (rapid point to start feeding)
F Feed rate in inches (mm) per minute
* Indicates optional
Rule #1: The G85 is modal and the machine will rapid between each new X and or Y position.
Rule #2: Use G98 and G99 for the Z position clearance location for positioning between holes.
Sample program:
O10084 (G85 Bore In~Bore Out)
N1 T19 M06 (BORING BAR)
N2 G90 G54 G00 X0.5 Y0.5 (position of first hole)
N3 S1450 M03
N4 G43 H19 Z1. M08
N5 G85 G99 Z-.54 R0.1 F4.5 (G99 Z position clearance location)
N6 X-0.5
N7 Y-0.5
N8 G80 G00 Z1. M09 (G80 cancels canned cycle)
N9 G53 G49 Z0. M05 (G53 temporarily ignores work offsets, and positions the machine axes from machine home. It is non-modal; so the next block will revert back to the previously selected work offset. G49 is tool length compensation cancel)
N10 M30

Front 14

What kind of canned cycle does a G86 perform? What primary letters are used with a G86, and what do they mean? What two important rules govern the use of the G86 (93.85)?

Back 14

Bore in - stop - rapid out canned cycle.
X* Rapid X-axis location
Y* Rapid Y-axis location
Z Z-depth (feed to Z-depth starting from R plane)
R R-plane (rapid point to start feeding)
F Feed rate in inches (mm) per minute
* Indicates optional
Rule #1: The G86 is modal and the machine will rapid between each new X and or Y position.
Rule #2: Use G98 and G99 for the Z position clearance location for positioning between holes.
Sample program:
O10085 (G86 Bore~Stop~Rapid Out)
N1 T19 M06 (BORING BAR)
N2 G90 G54 G00 X0.5 Y0.5 (position of first hole)
N3 S1450 M03
N4 G43 H19 Z1. M08
N5 G86 G99 Z-0.54 R0.1 F4.5 (G99 Z position clearance location)
N6 X-0.5
N7 Y-0.5
N8 G80 G00 Z1. M09 (G80 cancels canned cycle)
N9 G53 G49 Z0. M05 (G53 temporarily ignores work offsets, and positions the machine axes from machine home. It is non-modal; so the next block will revert back to the previously selected work offset. G49 is tool length compensation cancel)
N10 M30

Front 15

What kind of canned cycle does a G87 perform? What primary letters are used with a G87, and what do they mean? What two important rules govern the use of the G87 (94.86)?

Back 15

Bore in - manual retract canned cycle.
X* Rapid X-axis location
Y* Rapid Y-axis location
Z Z-depth (feed to Z-depth starting from R plane)
R R-plane (rapid point to start feeding)
F Feed rate in inches (mm) per minute
* Indicates optional
Rule #1: The G87 is modal and the machine will rapid between each new X and or Y position.
Rule #2: Use G98 and G99 for the Z position clearance location for positioning between holes.
Sample program:
O10086 (G87 Bore~Manual Retract)
N1 T19 M06 (BORING BAR)
N2 G90 G54 G00 X0.5 Y-0.5 (position of first hole)
N3 S1450 M03
N4 G43 H19 Z1. M08
N5 G87 G99 Z-0.54 R0.1 F4.5 (G99 Z position clearance location)
N6 X1.5 Y-1.5
N7 G80 G00 Z1. M09 (G80 cancels canned cycle)
N8 G53 G49 Z0. M05 (G53 temporarily ignores work offsets, and positions the machine axes from machine home. It is non-modal; so the next block will revert back to the previously selected work offset. G49 is tool length compensation cancel)
N9 M30

Front 16

What kind of canned cycle does a G88 perform? What primary letters are used with a G88, and what do they mean? What two important rules govern the use of the G88 (95.87)?

Back 16

Bore in - dwell - manual retract canned cycle.
X* Rapid X-axis location
Y* Rapid Y-axis location
Z Z-depth (feed to Z-depth starting from R plane)
P Dwell time at Z-depth
R R-plane (rapid point to start feeding)
F Feed rate in inches (mm) per minute
* Indicates optional
Rule #1: The G88 is modal and the machine will rapid between each new X and or Y position.
Rule #2: Use G98 and G99 for the Z position clearance location for positioning between holes.
Sample program:
O10087 (G88 Bore~Dwell~Manual)
N1 T19 M06 (BORING BAR)
N2 G90 G54 G00 X1.5 Y-0.5 (position of first hole)
N3 S1450 M03
N4 G43 H19 Z1. M08
N5 G88 G99 Z-.42 P0.2 R0.1 F4.5 (G99 Z position clearance location)
N6 X0.5 Y-1.5
N7 G80 G00 Z1. M09 (G80 cancels canned cycle)
N8 G53 G49 Z0. M05 (G53 temporarily ignores work offsets, and positions the machine axes from machine home. It is non-modal; so the next block will revert back to the previously selected work offset. G49 is tool length compensation cancel)
N9 M30

Front 17

What kind of canned cycle does a G89 perform? What primary letters are used with a G89, and what do they mean? What two important rules govern the use of the G89 (96.XX)?

Back 17

Bore in - dwell - bore out canned cycle.
X* Rapid X-axis location
Y* Rapid Y-axis location
Z Z-depth (feed to Z-depth starting from R plane)
P Dwell time at Z-depth
R R-plane (rapid point to start feeding)
F Feed rate in inches (mm) per minute
* Indicates optional
Rule #1: The G89 is modal and the machine will rapid between each new X and or Y position.
Rule #2: Use G98 and G99 for the Z position clearance location for positioning between holes.
Rule #3: A dwell in this cycle in seconds"."milliseconds will happen at the end of the Z-depth with P defined.
Sample program:
O10088 (G89 Bore In~Dwell~Bore Out)
N1 T19 M06 (BORING BAR)
N2 G90 G54 G00 X1.625 Y-0.375 (position of first hole)
N3 S1450 M03
N4 G43 H19 Z1. M08
N5 G89 G99 Z-0.375 P0.2 R0.1 F4.5 (G99 Z position clearance location)
N6 X1. Y-1.
N7 X0.375 Y-1.625
N8 G80 G00 Z1. M09 (G80 cancels canned cycle)
N9 G53 G49 Z0. M05 (G53 temporarily ignores work offsets, and positions the machine axes from machine home. It is non-modal; so the next block will revert back to the previously selected work offset. G49 is tool length compensation cancel)
N10 M30