9/Series CNC Lathe. Operation and Programming Manual

Chapter 26

Drilling Cycles

Figure 26.3 shows the two different modes available for selecting the

return level in the Z axis after the hole has been drilled. These two modes

are selected with G98 (which returns to the same level the cycle started at)

and G99 (which returns to the level defined by the R point).

Figure 26.3

Drilling Cycle Parameters in G98 or G99 Modes

Cutting feed

Rapid feed

G98 Initial point return

G99 R - Point return

R point level

Important: If your system is configured to use lathe G code system “A”

(selected in AMP), you can not program a G98 or G99 to change between

initial and R point returns. Lathes with G code system “A” always use the

R point return type (as if in G99 mode).

Important: In the following sections, figures and examples are assumed

to be programmed in the incremental mode (G91) and initial point return

mode (G98).

26-6

Chapter 26

Drilling Cycles

26.3

This section provides a detailed explanation of each parameter you can

program for the drilling cycles. Some parameters are not valid with all

Parameters

cycles; see the specific description of each cycle. To alter drilling cycle

operation parameters, see section 26.5.

These drilling cycle parameters are described below:

X__Y__Z__R__ I__J__K__ P__F__L__Q__D__S__;

Where :

Is :

specifies the location of the hole position in the selected plane. In the absolute mode

(G90), program the hole position using the coordinate values in the active coordinate

system. In incremental mode (G91), program the hole position using the distance from the

current tool position to the required hole position. This parameter is affected by radius or

diameter programming modes.

defines the hole bottom. In absolute mode (G90), program the hole bottom level using the

coordinate value in the active coordinate system. In the incremental mode (G91), program

the distance from the R point level to the hole bottom level.

defines the R point level. In the absolute mode (G90), program the R point level as a

coordinate value in the active coordinate system. In the incremental mode (G91), program

the R point level by the distance from the initial point level to the R point level.

define the shift amount for G86.1 and G87.

defines the dwell period at hole bottom. P programs the dwell in the same way as G04:

seconds if in feedrate mode (G94), spindle revolutions if in revolution mode (G95). (The

allowable dwell time range in seconds is 0.001-99999.99. The allowable dwell range in

revolutions is also 0.001-99999.999.) The P-word does not apply in all drilling cycles.

defines the cutting feedrate. If this parameter is not specified, the control uses the

currently active feedrate for the cutting feedrate. For G84.2 and G84.3, F = tap thread lead

in inches/mm per revolution.

defines the number of times the drilling cycle is repeated. The maximum number of

repeats is 9999.

· In absolute mode, the control drills in the same location the number of times specified by

the L-word.

· In incremental mode, the L-word drills the number of holes specified by the L-word at

equally spaced positions, determined by axis positioning parameters X and Y.

· If an L0 is programmed, the control decodes the milling cycle information, but does not

execute the drilling cycle. If no L-word is programmed, the control defaults to L1.

In G83, Q defines the infeed amount for each move made in the hole.

In G86.1 and G87, Q defines the shift amount (as do I, J, and K).

In G84.2 and G84.3, Q defines the angle at which to orient the spindle before starting the

tap. If you don’t program the Q-word, the spindle is not oriented before the tap begins. This

means that the hole is not retappable unless a Q-word is programmed in the cycle block.

The spindle is brought to a stop prior to the initiation of the tapping phase even if Q is not

programmed; this happens after the move to the R-plane.

defines the return spindle speed so that, if you want, the tap-out move can be performed

faster or slower than the tap-in. Tool selection by D-word is not possible while in the

solid-tapping mode.

defines spindle speed in rpm.

26-7

Chapter 26

Drilling Cycles

26.4

Drilling cycles G83.1, G84.1, G86.1 and G81-G89 are modal, which

means they remain active until you program a G-code that cancels the

Drilling Cycle Operations

drilling cycle. Certain drilling cycles can, therefore, be repeated at

different positions without having to re-program all the parameters

associated with a given operation.

Similarly, any parameters specified in the block calling the drilling cycle

remain active until the cycle is cancelled, or until they are re-programmed

in a following block. L-words do not remain active and, instead, designate

the number of times the drilling cycle is repeated.

G00-G03, G33, G34 or G80 cancel drilling cycle mode.

Important: Start the tool rotating with appropriate programming before

the control executes a drilling cycle block.

CAUTION: On systems with more than one spindle, the

controlling spindle code determines which spindle (and its

related spindle modal M-codes) is active during drilling cycles.

All references to spindle activities (orient, reversal, etc.)

described in this chapter apply only to the controlling spindle.

See chapter 17.

(G80): Cancel or End Fixed

The format for the G80 cancel or end fixed cycles is:

Cycles

G80;

Programming a G80 cancels the currently active drilling cycle mode. G00,

G01, G02, G03, G33 or G34 also cancel any active drilling cycle.

If drilling cycles are canceled with a G80, program execution returns to the

mode which was in effect when the cycles were last turned on, for

example, G00 - G03 or G33, G34.

26-8

Chapter 26

Drilling Cycles

In the G81 drilling cycle, the control moves the axes in this manner:

The tool rapids to the initial point level above the hole location.

The drilling tool then rapids to the R point level, slows to the

programmed cutting feedrate and begins the drilling operation.

The drilling tool continues to drill at the programmed feedrate until it

reaches the depth of the hole as programmed with the Z-word.

The control retracts the drilling tool at a rapid feedrate to the initial

point level as determined by G98.

When the single block function is active, the control stops axis motion

after steps 1, 2 and 4.

(G82): Drill Cycle,

The format for the G82 cycle is:

Dwell/Rapid Out

G82X__Z__R__P__F__L__;

Where :

Is :

specifies location of the hole.

defines the hole bottom.

defines the R point level.

defines the dwell period at hole bottom.

defines the cutting feedrate.

defines the number of times the drilling cycle is repeated.

See section 27.3 for a detailed explanation of these parameters.

Important: The programmer or operator must start spindle or live tool

rotation.

26-10

Chapter 26

Drilling Cycles

Figure 26.5

G82: Drilling Cycle, Dwell/Rapid Out

Cutting feed

Rapid feed

R point level

initial point

level

Hole bottom

Dwell at hole bottom

In the G82 drilling cycle, the control moves the axes in this manner:

The tool rapids to initial point level point above the hole location.

The drilling tool then rapids to the R point level, slows to the

programmed cutting feedrate and begins the drill operation.

The cutting tool drills at the programmed feedrate to the

pre-programmed depth of the hole (defined by the Z-word in the

boring cycle block).

If a value was programmed for the P parameter, the drilling tool

dwells after it reaches the bottom of the hole.

After the drilling tool reaches the hole bottom and the dwell is

completed, the drilling tool is retracted at a rapid feedrate to the

initial point level as determined by G98.

When the single block function is active, the control stops axis motion

after steps 1, 2 and 5.

26-11

Chapter 26

Drilling Cycles

(G83): Deep Hole Drilling

The format for the G83 cycle is:

Cycle

G83X__Z__R__Q__F__L__;

Where :

Is :

specifies location of the hole.

defines the hole bottom.

defines the R point level.

defines the infeed amount for each step into the hole.

defines the cutting feedrate.

defines the number of times the drilling cycle is repeated.

See page 26-7 for a detailed description of these parameters.

Important: The programmer or operator must start spindle or live tool

rotation.

Figure 26.6

G83: Deep Hole Drilling Cycle

initial point

level

R point level

Hole bottom

Moves to hole bottom

when Q is larger than

remaining depth

26-12

Chapter 26

Drilling Cycles

In the G83 drilling cycle, the control moves the axes in this manner:

The tool rapids to initial point level above the hole location.

The drilling tool then rapids to the R point level, slows to the

programmed cutting feedrate and begins the deep hole drilling

operation.

During the drilling operation, the control infeeds the drilling tool by

an amount Q, as programmed in the G83 block.

The drilling tool retracts at a rapid feedrate to the R point level.

The control feeds the drilling tool at rapid feedrate to a distance d

above the level drilled in the previous infeed. The amount d is

specified by the system installer, or can be set by the operator as

described in section 27.5. This intermittent feed simplifies chip

disposal and permits a very small retraction amount to be set in deep

hole drilling.

The drilling tool slows to the cutting feedrate again and infeeds an

amount Q + d.

The cutting tool is then retracted at a rapid feedrate to the initial point

level as determined by G98.

When the single block function is active, the control stops axis motion

after steps 1, 2 and 7.

(

G83.1): Deep Hole Peck

The format for the G83.1 cycle is:

Drilling Cycle with Dwell

G83.1X__Z__R__Q__P__F__L__;

Where :

Is :

specifies the location of the hole position in the selected plane.

defines the hole bottom.

defines the R point level.

defines the infeed amount for each step into the hole.

defines the dwell period at hole bottom.

defines the cutting feedrate.

defines the number of times the drilling cycle is repeated.

See page 26-7 for a detailed description of these parameters.

Important: The programmer or operator must start spindle or live tool

rotation.

26-13

Chapter 26

Drilling Cycles

Figure 26.7

G83.1: Deep Hole Peck Drilling Cycle with Dwell

R point level

Initial point

level

Hole bottom

Moves to hole bottom when Q is

larger than remaining depth

In the G83.1 peck drilling cycle, the control moves the axes in this manner:

The tool rapids to the initial point level above the hole location.

The drilling tool then rapids to the R point level, slows to the

programmed cutting feedrate and begins the drilling operation.

During the drilling operation, the control infeeds the drilling tool by

an amount Q, as programmed in the drilling cycle.

If a value was programmed for the P parameter, the drilling tool

dwells after it reaches the bottom of the hole.

It then retracts by an amount d at a rapid feedrate. The amount d is

specified by the system installer, or can be set by the operator as

described on page 26-38. This intermittent feed simplifies chip

disposal and permits a very small retraction amount to be set in peck

drilling.

26-14

Chapter 26

Drilling Cycles

After the drilling tool retracts an amount d, it then resumes drilling at

the cutting feedrate to a depth d + Q.

This retraction and extension continues until the drilling tool reaches

the depth of the hole as programmed with the Z-word in the drilling

cycle block.

The drilling tool then retracts at a rapid feedrate to the initial point

level as determined by G98.

When the single block function is active, the control stops axis motion and

awaits “cycle start” after steps 1, 2 and 7.

(G84):

Right-Hand Tapping

Use this cycle to cut right-handed threads. The format for the G84 cycle

Cycle

is:

G84X__Z__R__P__F__L__;

Where :

Is :

specifies location of the hole.

defines the hole bottom.

defines the R point level.

defines the dwell period at hole bottom.

defines the cutting feedrate and represents the thread lead along the drilling axis

(Z in this manual). It is mandatory when cutting any threads. The control

interprets the F-word as the number of threads per inch or millimeter.

defines the number of times the drilling cycle is repeated.

See section 27.3 for a detailed description of these parameters.

Important: When programming and executing a G84 tapping cycle,

remember:

the programmer or operator must start spindle or live tool rotation

override usage - the control ignores the feedrate override switch and

clamps override at 100 percent

during tapping, the feedrate override switch and the feedhold feature are

both disabled; cycle stop is not acknowledged until the end of the return

operation

26-15

Chapter 26

Drilling Cycles

Figure 26.8

G84: Right-Hand Tapping Cycle

Cutting feed

Rapid feed

R point level

Initial point

level

Hole bottom

Spindle or live tool rotation

direction reversed at hole

bottom

Spindle or live tool rotation

in the forward direction

In the G84 right-hand tapping cycle, the control moves the axes in this

manner:

CAUTION: The programmer or operator must set the direction

of spindle rotation for tap-in. The control forces the proper

spindle direction for the tap-out, but uses the programmed

spindle direction for the tap-in.

The tool rapids to initial point level above the hole location.

The threading tool then rapids to the R point level, slows to the

programmed cutting feedrate and begins the tapping operation.

During the tapping operation, the control infeeds the threading tool to

the depth and at the feedrate programmed in the tapping cycle.

26-16

Chapter 26

Drilling Cycles

If a value was programmed for the P parameter, the threading tool

dwells after it reaches the bottom of the hole, and after the spindle has

been commanded to reverse.

The spindle or live tool reverses to the counterclockwise direction.

The threading tool retracts at the cutting feedrate to the R point.

If a value was programmed for the P parameter, the threading tool

dwells after it reaches the R point. Dwells may be ignored if the

system installer has chosen to do so in AMP.

The spindle or live tool direction is reversed to clockwise.

With G98 active, the cutting tool then accelerates to the rapid feedrate

and retracts to the initial point level.

When the single block function is active, the control stops axis motion

after steps 1, 2 and 6.

If the operator activates a feedhold during steps 3, 4 or 5, axis motion

stops after step 7. Axis motion also stops during steps 1, 2, and 7.

However, if the operator activates a feedhold during step 7, axis motion

stops immediately.

Important: Your system installer can enable a tap retract feature for this

cycle through PAL. Tap retract enables you to retract the tapping tool and

resume the cycle, or completely abort the tapping operation. Refer to your

system installers documentation for details.

(G84.1): Left-Hand Tapping

Use this cycle to cut left-handed threads.

Cycle

The format for the G84.1 cycle is:

G84.1X__Z__R__P__F__L__;

Where :

Is :

specifies the location of the hole position in the selected plane.

defines the hole bottom.

defines the R point level.

defines the dwell period at hole bottom.

defines the cutting feedrate and represents the thread lead along the drilling axis

(Z in this manual). It is mandatory when cutting any threads. The control

interprets the F-word as the number of threads per inch or millimeter.

defines the number of times the drilling cycle is repeated.

See section 27.3 for a detailed description of these parameters.

26-17

Chapter 26

Drilling Cycles

Important: When programming a G84 tapping cycle, remember:

the programmer or operator must start spindle or live tool rotation

override usage - the control ignores the feedrate override switch and

clamps override at 100 percent

during tapping, the feedrate override switch and the feedhold feature are

both disabled; cycle stop is not acknowledged until the end of the return

operation

Figure 26.9

G84.1: Left-Hand Tapping Cycle

Cutting feed

Rapid feed

R point level

Initial point

level

Spindle or live tool rotation direction

is reversed at hole bottom

In the G84.1 left-hand tapping cycle, the control moves the axes in this

manner:

26-18

Chapter 26

Drilling Cycles

CAUTION: The programmer or operator must set the direction

of spindle rotation for tap-in. The control forces the proper

spindle direction for the tap-out, but uses the programmed

spindle direction for the tap-in.

The tool rapids to the initial point level above the hole location.

The threading tool then rapids to the R point level, slows to the

programmed cutting feedrate and begins the tapping operation.

During the tapping operation, the control infeeds the threading tool to

the depth and at the feedrate programmed in the tapping cycle.

If a value was programmed for the P parameter, the threading tool

dwells after it reaches the bottom of the hole, and after the spindle has

been commanded to reverse.

The spindle or live tool reverses to the clockwise direction.

The threading tool retracts at the cutting feedrate to the R point.

If a value was programmed for the P parameter, the threading tool

dwells after it reaches the R point. Dwells may be ignored if the

system installer has chosen to do so in AMP.

The spindle or live tool direction is reversed to counterclockwise.

With G98 active, the cutting tool then accelerates to the rapid feedrate

and retracts to the initial point level.

When the single block function is active, the control stops axis motion and

awaits “cycle start” after steps 1, 2 and 7.

If the operator activates a feedhold during steps 3, 4 or 5, axis motion

stops after step 7. Axis motion also stops during steps 1, 2 and 7.

However, if feedhold is activated during step 7, axis motion stops

immediately.

Important: Your system installer can enable a tap retract feature for this

cycle through PAL. Tap retract enables you to retract the tapping tool and

resume the cycle, or completely abort the tapping operation. Refer to your

system installers documentation for details.

26-19

Chapter 26

Drilling Cycles

(G84.2): Right-Hand

Use this cycle to cut right-handed threads.

Solid-Tapping Cycle

The format for the G84.2 cycle is:

G84.2X__Z__R__F__L__Q__D__S__;

Where :

Is :

specifies location of the hole.

defines the hole bottom.

defines the R point level.

defines the thread lead along the drilling axis (Z in this manual). It is mandatory

and modal in any subsequent solid tapping cycle blocks until a new F-word is

programmed.

The control interprets the F-word as the thread lead in inches per revolution or

millimeters per revolution, depending on the inch/metric mode active.

defines the number of times the drilling cycle is repeated.

defines the angle at which to orient the spindle before starting the tap. It is modal

in any subsequent solid tapping blocks until a new Q-word is programmed or the

tapping cycle is cancelled by a G80. To retap a hole, a Q-word must have been

programmed when the hole was originally tapped.

defines the return spindle speed, but cannot exceed the maximum tapping

spindle speed set in AMP. This will adjust your Z-axis feedrate according to the

thread lead defined in F.

defines spindle speed in rpm.

See section 27.3 for a detailed description of these parameters.

Important: When programming and executing a G84.2 solid-tapping

cycle, remember:

the feedrate of the tapping phases is derived as

(spindle {RPM}_* F-lead {IPR}) = IPM

the spindle speed that is active at the start of the cycle determines the

effective Z feedrate

the direction of spindle rotation for tap-in and tap-out phases will be

automatically generated by the control

spindle speed override has no effect on the solid-tapping cycle; you can

use feedrate override to adjust the tapping operation

D cannot exceed the maximum tapping spindle speed set in AMP

you cannot select tools via D-word while in solid-tapping mode

gear changes are locked out

26-20

Chapter 26

Drilling Cycles

on a dual-process lathe, both processes can be in solid-tapping mode at

the same time assuming that they have separate controlling spindles

you must disable CSS before performing solid tapping; an attempt to

execute the tap phase of a solid-tapping cycle with CSS results in a

decode error

cycle stop and feedrate override are acknowledged throughout the cycle,

but can be disabled by G63

you can use active reset to abort the cycle after the cycle stop request

has been acknowledged

to retap a hole, a Q-word must have been programmed when the hole

was originally tapped

block retrace is possible during the tap-in portion of the cycle, but not

during the tap-out

Figure 27.L1

G84.2: Right-Hand Solid-Tapping Cycle

Tapping move

Rapid move

R point level

Initial point level (I)

Spindle or live tool

rotation direction is reversed

at hole bottom

G98

G99

26-21

Chapter 26

Drilling Cycles

In the G84.2 right-hand solid-tapping cycle, the control moves the axes in

this manner:

The tool rapids to the tapping position above the hole location.

The threading tool then rapids to the R point.

The control either orients or stops the spindle.

If a Q-word was programmed:

the control:

yes

orients the spindle

stops the spindle

Tap-in: The clockwise rotation of the spindle ramps up to the

programmed S spindle speed and linear motion of the Z axis moves

synchronously to reach the Z position.

Tap-out: The spindle and linear motion reverse to the

counterclockwise direction and retract to the R point.

The tap-out speed is determined by F_* S unless you programmed D

(tap-out rpm), in which case tap-out speed is F_* D.

At the R point, spindle rotation has ramped to zero.

With G98 active, the cutting tool then accelerates to the rapid feedrate

and retracts to the initial point level.

With G99 active, the cutting tool remains at R point; no movement

occurs.

In single-block mode, the control stops axis motion after phases 1, 2, 3,

and 6 of the cycle (Figure 27.L1).

26-22

Chapter 26

Drilling Cycles

(G84.3): Left-Hand

Use this cycle to cut left-handed threads.

Solid-Tapping Cycle

The format for the G84.3 cycle is:

G84.3X__Z__R__F__L__Q__D__S__;

Where :

Is :

specifies location of the hole.

defines the hole bottom.

defines the R point level.

defines the thread lead along the drilling axis (Z in this manual). It is mandatory

and modal in any subsequent solid tapping cycle blocks until a new F-word is

programmed.

The control interprets the F-word as the thread lead in inches per revolution or

millimeters per revolution, depending on the inch/metric mode active.

defines the number of times the drilling cycle is repeated.

defines the angle at which to orient the spindle before starting the tap. It is modal

in any subsequent solid tapping blocks until a new Q-word is programmed or the

tapping cycle is cancelled by a G80. To retap a hole, a Q-word must have been

programmed when the hole was originally tapped.

defines the return spindle speed, but cannot exceed the maximum tapping

spindle speed set in AMP. This will adjust your Z-axis feedrate according to the

thread lead defined in F.

defines spindle speed in rpm.

See section 27.3 for a detailed description of these parameters.

Important: When programming and executing a G84.3 solid-tapping

cycle, remember:

the feedrate of the tapping phases is derived as

(spindle {RPM}_* F-lead {IPR}) = IPM

the spindle speed that is active at the start of the cycle determines the

effective Z feedrate

the direction of spindle rotation for tap-in and tap-out phases will be

automatically generated by the control

spindle speed override has no effect on the solid-tapping cycle; you can

use feedrate override to adjust the tapping operation

D cannot exceed the maximum tapping spindle speed set in AMP

you cannot select tools via D-word while in solid-tapping mode

gear changes are locked out

26-23

Chapter 26

Drilling Cycles

on a dual-process lathe, both processes can be in solid-tapping mode at

the same time assuming that they have separate controlling spindles

you must disable CSS before performing solid tapping; an attempt to

execute the tap phase of a solid-tapping cycle with CSS results in a

decode error

cycle stop and feedrate override are acknowledged throughout the cycle,

but can be disabled by G63

you can use active reset to abort the cycle after the cycle stop request

has been acknowledged

to retap a hole, a Q-word must have been programmed when the hole

was originally tapped

block retrace is possible during the tap-in portion of the cycle, but not

during the tap-out

Figure 27.L2

G84.3: Left-Hand Solid-Tapping Cycle

Tapping move

Rapid move

R point level

Initial point level (I)

Spindle or live tool rotation direction

is reversed at hole bottom

G98

G99

26-24

Chapter 26

Drilling Cycles

In the G84.3 left-hand solid-tapping cycle, the control moves the axes in

this manner:

The tool rapids to the tapping position above the hole location.

The threading tool then rapids to the R point.

The control either orients or stops the spindle.

If a Q-word was programmed:

the control:

yes

orients the spindle

stops the spindle

Tap-in: The counterclockwise rotation of the spindle ramps up to the

programmed S spindle speed and linear motion of the Z axis moves

synchronously to reach the Z position.

Tap-out: The spindle and linear motion reverse to the clockwise

direction and retract to the R point.

The tap-out speed is determined by F_* S unless you programmed D

(tap-out rpm), in which case tap-out speed is F_* D.

At the R point, spindle rotation has ramped to zero.

With G98 active, the cutting tool then accelerates to the rapid feedrate

and retracts to the initial point level.

With G99 active, the cutting tool remains at R point; no movement

occurs.

In single-block mode, the control stops axis motion after phases 1, 2, 3,

and 6 of the cycle (Figure 27.L2).

(G85): Boring Cycle, No

The format for the G85 cycle is:

Dwell/Feed Out

G85X__Z__R__F__L__;

Where :

Is :

specifies location of the hole.

defines the hole bottom.

defines the R point level.

defines the cutting feedrate.

defines the number of times the drilling cycle is repeated.

26-25

Chapter 26

Drilling Cycles

See page 26-7 for a detailed description of these parameters.

Important: The programmer or operator must start spindle or live tool

rotation.

Figure 26.10

G85: Boring Cycle (Without Dwell, Feed Out)

Cutting feed

Rapid feed

R point level

Initial point

level

Hole bottom

In the G85 boring cycle, the control moves the axis in this manner:

The tool rapids at the initial point level, to the hole location.

The boring tool then rapids to the R point level, slows to the

programmed cutting feedrate and begins the boring operation.

The boring tool continues to drill at the programmed feedrate until it

reaches the depth of the hole as programmed with the Z-word.

The control retracts the boring tool at the cutting feedrate to the R

point.

The control retracts the drilling tool at a rapid feedrate to the initial

point level, as determined by G98.

When the single block function is active, the control stops axis motion

after steps 1, 2 and 5.

26-26

Chapter 26

Drilling Cycles

(G86): Boring Cycle,

The format for the G86 cycle is:

Spindle Stop/Rapid Out

G86X__Z__R__P__F__L__;

Where :

Is :

specifies location of the hole.

defines the hole bottom.

defines the R point level.

defines the dwell period at hole bottom.

defines the cutting feedrate.

defines the number of times the drilling cycle is repeated.

See page 26-7 for a detailed description of these parameters.

Important: The programmer or operator must start spindle or live tool

rotation.

Figure 26.11

G86: Boring Cycle, Spindle Stop/Rapid Out

Cutting feed

Rapid feed

R point level

Initial point

level

Hole bottom

Spindle or live tool stops

at hole bottom

26-27

Chapter 26

Drilling Cycles

In the G86 drilling cycle, the control moves the axis in this manner:

The tool rapids to the initial point level above the hole location.

The cutting tool then rapids to the R point level, slows to the

programmed cutting feedrate and begins the boring operation.

The cutting tool bores at the programmed feedrate until it reaches the

depth of the hole as programmed with the Z-word.

If the user has entered a value for the P parameter, the cutting tool

dwells after it reaches the bottom of the hole.

The spindle or live tool stops rotating.

The boring tool is then retracted at a rapid feedrate to the initial point

level, as determined by G98. Spindle or live tool rotation continues

forward.

When the single block function is active, the control stops axis motion

after steps 1, 2 and 6.

(G86.1): Boring Cycle, Tool

The format for the G86.1 cycle is:

Shift

G86.1X__Z__ I__K__ R__F__L__;

Q__

Where :

Is :

specifies location of the hole.

defines the hole bottom.

Q or I, K

defines the tool shift amount.

defines the R point level.

defines the cutting feedrate.

defines the number of times the drilling cycle is repeated.

See page 26-7 for a detailed description of these parameters.

Important: The programmer or operator must start spindle or live tool

rotation.

26-28

Chapter 26

Drilling Cycles

Figure 26.12

G86.1: Boring Cycle, Tool Shift

Hole bottom

Bored hole

R point level

Shift

Spindle orient after

dwell at Z point level

to position tool for

removal

Initial point

level

Cutting feed

Spindle or live tool oriented

Rapid feed

and tool shifted

Shift

In the G86.1 boring cycle, the control moves the axes in this manner:

The tool rapids to the initial point level above the hole location.

The boring tool then rapids to the R point level, slows to the

programmed cutting feedrate, and begins the boring operation.

The boring tool bores at the programmed feedrate to the

pre-programmed depth of the hole (defined by the Z-word in the

boring cycle block).

The control positions the spindle or live tool at the bottom of the hole

in a particular orientation, determined by the system installer in AMP.

To prevent the boring tool from damaging the sides of the bored hole

during retraction, the boring tool is shifted in either of two methods

which are explained below and illustrated in Figure 26.12.

26-29

Chapter 26

Drilling Cycles

The shift direction is determined by two possible methods:

Method I

This shift method is a single-axis shift. The direction and axis for the shift

is set in AMP by your system installer or can be altered using the drilling

cycle parameter table. See page 26-38.

the direction of the axis is specified as + or -.

the feedrate using this shift method is always rapid traverse.

the Q-word shift amount is always interpreted as a positive value; a

negative Q-word is not allowed.

Method II

The direction of the shift using this method is programmed in the boring

cycle block. Program a shift amount for axes in the current plane (G17,

G18, or G19) by using only these words:

I__ programs an X axis move.

K__ programs a Z axis move.

Follow the I- and K-words (modal during drilling cycles) with incremental

values in the block that programs the hole position.

When using Method II, remember:

if both axes in the current plane are to be shifted, specify both words to

move the axes

the generated move is a single linear move and executes at rapid

traverse

The boring tool is then retracted at a rapid feedrate to the initial point

level as determined by G98.

After reaching initial point level, the control again positions the

spindle or live tool at the bottom of the hole in a particular orientation

as determined by the system installer in AMP.

After reaching the initial point level, the boring tool is shifted back

(in a manner previously explained and illustrated) and the spindle or

live tool is re-started in the counterclockwise direction.

When the single block function is active, the control stops axis motion

after steps 1, 2, 4, and 8.

26-30

Chapter 26

Drilling Cycles

When using Method II, remember:

the generated move is a single linear move and executes at

(G87): Back Boring Cycle

The format for the G87 back boring cycle is:

G87X__Z__ I__J__K__ R__F__L__;

Q__

Where :

Is :

specifies location of the hole.

defines the Z point level. The Z point level in this case is the top of the

hole that is being cut by the back boring operation.

Q or I,

defines the tool shift amount.

J, K

defines the position beyond the hole bottom so the tool can safely shift.

defines the cutting feedrate.

defines the number of times the drilling cycle is repeated.

Important: This cycle requires an existing hole through which the back

boring tool can be safely lowered prior to the back boring operation.

26-31

Chapter 26

Drilling Cycles

Figure 26.13

G87: Back Boring Cycle

Cutting feed

Rapid feed

Hole bottom

Z point level

Initial point

level

Spindle or live tool

orientation

Spindle or live tool

orientation

rotation forward

In the G87 back boring cycle, the control moves the axes in this manner:

The tool rapids to the initial point level above the hole location.

After the back boring tool is positioned, the control orients the tool to

a position determined in AMP by the system installer.

The control shifts the boring tool by one of two possible methods as

described on page 26-33. The shift method is determined in AMP by

the system installer. Refer to the documentation supplied by your

system installer for additional information.

26-32

Chapter 26

Drilling Cycles

Method I

This shift method is a single axis shift. The direction and axis for the

shift is set in AMP by the system installer or can be altered using the

drilling cycle parameter table. See page 26-38.

the direction of the axis is specified as + or -

the feedrate using this shift method is the programmed feedrate

the Q-word shift amount is always interpreted as a positive value;

a negative Q-word is not allowed

Method II

The direction of the shift using this method is programmed in the

boring cycle block. Program a shift amount for axes in the current

plane only (G17, G18, G19) by using these words:

I__ programs an X axis move.

K__ programs a Z axis move.

Follow the I- and K-words (modal during drilling cycles) with

incremental values in the block that programs the hole position.

When using Method II, remember:

if both axes in the current plane are to be shifted, specify both

words to move the axes

the move generated is a single linear move and is executed at rapid

traverse

The back boring tool moves at a rapid feedrate through the existing

hole to the depth designated by the R-word.

Once the designated depth is reached, the back boring tool shifts the

same distance but in the opposite direction as the previous shift (the

shift made in step 2).

After this shift, the programmer or operator must start the spindle or

live tool. The spindle or live tool must rotate in the clockwise

direction.

The control retracts the back boring tool at the cutting feedrate to a

level specified by the Z-word.

26-33

Chapter 26

Drilling Cycles

After reaching the Z depth, the spindle or live tool rotation stops so

that the control can re-orient the back boring tool to the position

specified in AMP.

The back boring tool is shifted a third time, in the same manner as in

step 2, so that it is again “off-center” and can be removed through the

existing hole.

The back boring tool moves at a rapid feedrate to the initial point

level regardless of whether G98 or G99 is active.

The back boring tool is shifted a fourth time, in the same manner as

in step 2, returning to the initial X coordinates of the hole location.

(G88): Boring Cycle,

The format for the G88 cycle is:

Spindle Stop/Manual Out

G88X__Z__R__P__F__L__;

Where :

Is :

specifies location of the hole.

defines the hole bottom.

defines the R point level.

defines the dwell period at the hole bottom.

defines the cutting feedrate.

defines the number of times the drilling cycle is repeated.

See page 26-7 for a detailed description of these parameters.

Important: The programmer or operator must start spindle or live tool

rotation.

26-34

9/Series CNC Lathe. Operation and Programming Manual - page 22