HNC-818. User Manual

12. Fixed Cycle

Parameter

Description

X Y

The circle center coordinate.

Hole bottom coordinate.

The coordinate value of the reference point R for absolute

programming, or the incremental value of the reference

point R to the initial point B for incremental programming.

Circle radius.

The initial angle for drilling hole, positive in the counter

clockwise direction.

The number of holes. The positive value for the counter

clockwise drilling and negative value for the clockwise

drilling.

Feed depth for each time, orientation distance.

When conducting feeding again after a tool exit, the

distance away from the previous machining plane while the

rapid feed is changed to the cutting feed.

The duration that the tool remains at the hole bottom. Unit:

millisecond

An error is reported when the value of Q is greater than 0 or

K is less than 0; An error is reported when the tool feed

distance Q is less than the tool exit distance K. When Q or

K is 0 or is not defined, G81 center drilling cycle is

executed for each hole, and P is invalid. When the values of

Q and K are correct , G83 deep hole machining cycle is

executed for each hole.

Define cutting feed speed.

The repeat count (Generally used for multi-hole machining,

and therefore X or Y is incremental value. It is optional

when L=1.).

On the X, Y plane, drill four holes in the counter clockwise direction on

the four axes(+X, -X, +Y, -Y). This operation is executed twice, and G81

is executed for drilling at the hole bottom.

Example 1

G98 G70 X10 Y10 Z0 R20 I10 J0 N4 F200 L2

Example 2

152

12. Fixed Cycle

On the X, Y plane, drill four holes in

executed once, and G81 is executed for drilling at the hole bottom.

the clockwise direction with thangle

G99 G70 X10 Y10 Z10 R50 I10 J45 N-4 F200

45 degrees. This operation is

On the X, Y plane, drill four holes in the clockwise direction, with the

angle of

-45 degrees. This operation is executed once, and G81 is

executed for drilling at the hole bottom.

Example 3

G99 G70 X10 Y10 Z10 R50 I10 J-45 N-4 F200

Example 4

On the X, Y plane, drill four holes in the clockwise direction with the

angle of -45 degrees. This operation is executed once. The value of Q is

invalid, and G81 is executed for drilling at the hole bottom.

G99 G70 X10 Y10 Z10 R50 I10 J-45 N-4 Q-10 F200

Example 5

On the X, Y plane, drill four holes in the clockwise direction with the

angle of

-45 degrees. This operation is executed once, and G81 is

executed for drilling at the hole bottom.

Example 6

G99 G70 X10Y10Z10R50 I10J-45N-4 Q0 F200

G99 G70 X10Y10Z10R50 I10J-45N-4 K0 F200

G99 G70 X10Y10Z10R50 I10J-45N-4 Q0K0 F200

On the X, Y plane, drill four holes in the clockwise direction with the

angle of

-45 degrees. This operation is executed once, and G83 is

executed for deep hole cycle.

G99 G70 X10Y10Z10R50 I10J-45N-4 Q-10 K5 F200

153

12. Fixed Cycle

12.1.2 Arc Drilling Cycle (G71)

Decription

I and the center being the coordinate

(X, Y). Divide the circle into N

equal parts based on the angle J and the X axis. Conduct drilling for N

holes per O degrees, starting from the point where the angle from the A

axis is J. Execute fixed cycle of G81 or G83 based on the value of Q, K

for each hole. The movement between holes is performed through G00.

G71 is a modal code, and the command following it is non-modal.

In the circumference with the radius

Foramt

(G98/G99) G71 X_ Y_ Z_ R_ I_ J_ O_ N[Q_K_P] _ F_ L_

Parameter

Description

X Y

The center coordinate for the arc.

Hole bottom coordinate.

The coordinate value of the reference point R for

absolute programming, or the incremental value of the

reference point R to the initial point B for incremental

programming.

Arc radius.

The initial drilling hole angle, positive in the counter

clockwise direction

The angle between each hole. The positive value for the

counter clockwise drilling and negative value for the

clockwise drilling.

The number of holes, including the start hole.

Feed depth for each time, orientation distance.

When conducting feeding again after a tool exit, the

distance away from the previous machining plane while

the rapid feed is changed to the cutting feed.

The duration that the tool remains at the hole bottom.

Unit: millisecond

An error is reported when Q is greater than 0 or K is less

than 0; An error is reported when the tool feed distance

Q is less than the tool exit distance K. When Q or K is 0

or is not defined, execute G81 center drilling cycle for

each hole, and P is invalid. When the values of Q and K

are correct, G83 deep hole machining cycle is executed

for each hole and P is valid.

Define cutting feed speed.

155

12. Fixed Cycle

The repeat count (Generally used for multi-hole

machining, therefore X or Y is incremental value. L is

optional.)

The total arc angle (N x O) cannot be greater than or equal to 360

degrees, otherwise the command will not be executed.

Attention

Use ĭ10 drilling bit for the drilling of the holes as shown in the figure:

Example

28 degrees

55 degrees

%3359

N10 G55 G00 X0 Y0 Z80

N20 G98G71G90X40Y0G90R25Z0I40J55O28N4P2000Q-10K5F100

N30 G90 G00 X0 Y0 Z80

N40 M30

156

12. Fixed Cycle

12.1.3 High-Speed Deep-Hole Drilling Cycle (G73)

Example

The fixed cycle is used for the intermittent feed along Z axis, which is

prone to chip-breaking, chip-removal, coolant adding, and small amount

of tool exit. It is applicable for high-speed deep-hole drilling.

The figure below shows the operation action sequence of G73. The

dotted line represents rapid positioning, q represents each feed depth,

and k represents each tool exit value.

Initial plane

Plane of point R

Point R

G99

Point Z

Format

(G98/G99) G73 X_ Y_ Z_ R_ Q_ P_ K_ F_ L_;

Parameter

Description

X Y

The coordinate value of the hole center in the XY plane

for absolute programming

(G90), or the incremental

value of the hole center to the start point in the XY plane

for incremental programming (G91).

The coordinate value of the hole bottom point Z for

absolute programming (G90), or the incremental value

of the hole bottom point Z to the reference point R for

incremental programming (G91).

The coordinate value of the reference point R for

absolute programming (G90), or the incremental value

of the reference point R to the initial point B for

incremental programming (G91).

Drilling depth for each time

(incremental value,

negative).

The duration that the tool remains at the hole bottom.

Unit: millisecond.

157

12. Fixed Cycle

Each upward tool exit amount

(incremental value,

positive).

Drilling feed speed

Cycle count (for repetitive drilling)

Operation procedure

The tool moves rapidly to the point B over the hole center.

Move rapidly to the point R, close to the workpiece.

Drill downward at the speed of F, with depth q.

Move upward rapidly, with distance k.

Repeat step 3 and 4 for multiple times.

Drill to the point Z at the hole bottom.

Remain 9 seconds at the hole bottom (spindle remains rotation)

Exit upward rapidly to the point R (G99) or B (G98).

Attention

If the motion amount of Z, K, and Q are zero, this command is not

executed.

|Q|>|K|;

Example

Drilling the hole as shown in the figure below:

%3337

N10 G92 X0 Y0 Z80

N15 M03 S700

158

12. Fixed Cycle

12.1.4 Reverse Tapping Cycle (G74)

Description

The spindle motor and servo motors are running in the position control

mode. The tapping is conducted by the interpolation between the tapping

axis and spindle. The spindle feeds the distance of one thread lead along

the tapping axis per rotation. The feeding does not change even during

acceleration or deceleration.

The action defined by G74 is as shown in the figure below. Move rapidly

to the point "R" after positioning along X and Y axis. The spindle rotates

in the counter clockwise (CCW) direction, and tapping is conducted

from the point R to Z. After the tapping is completed, the spindle stops

and the system starts the mode of pause. Then the spindle rotates in the

clockwise (CW) direction, the tool exits back to the point R, and the

spindle stops. The tool will finally move rapidly to the initial position in

the G98 mode.

Initial plane

Spindle CCW

Spindle stop

Spindle CCW

Spindle stop

Point

Point Z

Spindle stopl

Spindle CW

Spindle stopl

Spindle CW

G74 (G98)

G74 (G99)

In the rigid tapping mode, the servo

spindle motor controls the tapping.

Format

(G98/G99)G74 X_ Y_ Z_ Q_ R_ P_ F_ L_H_J_;

160

12. Fixed Cycle

Parameter

Description

Parameter

Description

The absolute

position of the point R for absolute

X Y

The absolute position of the hole for absolute

programming (G90), or the distance from the point R

programming (G90), or the

distance from the current

to the initial plane for incremental programming

tool position to the hole for

incremental programming

(G91).

The duration

that the tool remains at the hole bottom.

The absolute position of the hole bottom for absolute

Unit: millisecond.

programming (G90), or the

distance from the hole

Define thread lead.

bottom to the point R for incremental programming

H1: segment

tapping, exits to the R plane each time.

(G91).

H2: directly drills to the hole bottom.

The amount of each feed during segment

tapping.

Repeat count

(It is optional when L=1.)

Leave it blank in the H2 mode.

J1: A axis tapping; J2: B axis tapping; J3 C: axis

tapping

F (feed speed) during tapping

(F) specified in the programming is invalid. The feed speed along the

tapping axis is derived from: speed feed = spindle speed x thread lead

During rigid tapping, the feed speed

Tapping mode

C axis tapping: take the servo spindle as the C axis, and conduct tapping

by interpolation, to achieve high-speed high-precision tapping.

Attention

The tapping axis must be the Z axis.

The point Z must be lower than the plane of point R; otherwise, an

alarm will be reported.

161

12. Fixed Cycle

The G74 command data is

saved as modal data.

When the motion amount of Z

is zero, the cycle is not

executed.

During reverse tapping, the

operations

on feed rate

adjustment,

spindle

rate

adjustment, and feed hold is

invalid.

Before

specifying

reverse

tapping with G74, change the

control mode of the spindle

servo motor from speed control

to the position control by using

the STOC command. After

tapping, you may use the CTOS

clockwise direction.

command to change back to the

speed control mode and take the

After executing the rigid tapping with G74, the programmer must

servo spindle as a common

restore the original feed speed; otherwise, the feed speed will be the

spindle.

rigid tapping speed (s*pitch).

Before

specifying

reverse

tapping with G74, use the

Use M10 x 1 for anti-tapping

corresponding M command to

rotate the spindle in the counter

%3339

Example

G92 X0 Y0 Z80 F200

M04 S300

STOC

G98G74X50Y40R40P10000G90Z-5F1

CTOS

162

12. Fixed Cycle

12.1.5 Fine-Boring Cycle (G76)

Description

During finish boring, after the spindle stops orientation at the hole

bottom, it moves away from the tool nose, then the tool quickly exits.

The value of movement away from the tool nose is specified by (I, J),

which can only be positive. The value of (I, J) is modal, and the

movement direction is determined during tool installation.

Initial plane

Plane of point R

G98

Point R

G99

Point Z

Offset value (I, J)

Format

(G98/G99) G76 X_ Y_ Z_ R_ I_ J_ P_ F_ L_;

Parameter

Description

X Y

The absolute position of the hole for absolute

programming (G90), or the distance from the current

tool position to the hole for incremental programming

(G91). UW programming is not supported.

The absolute position of the hole bottom along Z axis

for absolute programming (G90), or the distance from

the hole bottom to the point R for incremental

programming (G91).

The absolute position of the point R along Z axis for

absolute programming (G90), or the distance from the

point R to the initial plane for incremental

programming (G91).

Offset value along X axis, positive only.

Offset value along Y axis, positive only.

The duration that the tool remains at the hole bottom.

Unit: millisecond.

Cutting feed speed.

Repeat count (It is optional when L=1.)

164

12. Fixed Cycle

The tool moves rapidly to the point B over the hole center.

Move rapidly to the point R, close to the workpiece.

Operation procedure

Conduct boring downward at the speed of F, to the point Z at the

hole bottom.

Remain at the hole bottom for P seconds (The spindle remains

rotation).

The spindle conducts orientation and stops rotation.

The boring tool rapidly moves away form the tool nose with the

distance specified by I or J.

Exit upward rapidly to the point R (G99) or B G98).

Move rapidly in the positive direction of the tool nose with the

distance specified by I or J, and the tool moves back to the point R

or B over the hole center.

The spindle restores the clockwise rotation.

Attention

1. The boring axis must be the Z axis.

2. The point Z must be lower than the plane of point R; otherwise, an

alarm will be reported.

3. The G76 command data is saved as modal data.

4. Before using the command of G76, use the corresponding M

command to rotate the spindle.

Example

165

12. Fixed Cycle

12.1.6 Angular Linear Drilling Cycle (G78)

Description

Divide the oblique line which rotates J degrees around axis X into N

holes with the interval distance of I. Starting from the point defined by X,

Y, conduct the drilling cycle for each hole. Execute G81 and G83 fixed

cycle based on the value of Q, K for each hole. The movement between

holes is conducted through G00. G78 is a modal code, and the command

following it is non-modal.

Format

(G98/G99) G78 X_ Y_ Z_ R_ I_ J_ N_[Q_K_P]_ F_ L_

Parameter

Description

X Y

The coordinate of the first hole.

The coordinate of the hole bottom.

The absolute position of the reference point R for

absolute programming (G90), or the distance from the

reference point R to the initial point B for incremental

programming (G91).

The distance between two successive hole centers.

The start angle formed by the oblique line and the

positive X axis, which is positive in the counter

clockwise direction.

The number of holes including the start hole.

Feed depth for each time, orientation distance.

When conducting feeding again after a tool exit, the

distance away from the previous machining plane while

the rapid feed is changed to the cutting feed.

The duration that the tool remains at the hole bottom.

Unit: millisecond

An error is reported when Q is greater than 0 or K is less

than 0; An error is reported when the tool feed distance

Q is less than the tool exit distance K. When Q or K is 0

or is not defined, execute G81 center drilling cycle for

each hole, and P is invalid. When the values of Q and K

are corrective, execute G83 deep hole machining cycle

for each hole, and P is valid.

Define cutting feed speed.

The repeat count (Generally used for multi-hole

machining,and therefore X or Y is incremental value. (It

is optional when L=1.)

167

12. Fixed Cycle

12.1.7 Chessboard Drilling Cyle (Drilling along X Axis First) (G79)

Description

Starting from the point defined by X, Y, conduct drilling for N holes in

the direction parallel to the X-axis with the interval distance of I. Then

conduct drilling in the direction of the X axis with an interval specified

by J along the Y axis. This operation is repeated for O times. Execute

G81 and G83 fixed cycle based on the value of Q, K for each hole. The

movement between holes is performed through G00. G79 is a modal

code, and the command following it is non-modal.

Format

(G98/G99) G79 X_ Y_ Z_ R_ I_ N_ J_ O_[Q_K_P]_ F_ L_

Parameter

Description

X Y

The coordinate of the first hole.

The coordinate of the hole bottom.

The coordinate value of the reference point R for absolute

programming

(G90), or the incremental value of the

reference point R to the initial point B for incremental

programming (G91).

The distance between two successive hole centers in the X

axis direction. The positive value indicates the drilling along

the positive X axis direction while the negative value

indicates the drilling along the negative X axis direction.

The number of holes including the start hole in the X axis

direction.

The distance between two successive hole centers in the Y

axis direction. The positive value indicates the drilling along

the positive Y axis direction while the negative value

indicates the drilling along the negative Y axis direction.

The number of holes including the start hole in the Y axis

direction.

Feed depth for each time, orientation distance.

When conducting feeding again after a tool exit, the

distance away from the previous machining plane while the

rapid feed is changed to the cutting feed.

169

12. Fixed Cycle

The duration that the tool remains at the hole bottom. Unit:

millisecond

An error is reported when Q is greater than 0 or K is less

than 0; An error is reported when the tool feed distance Q is

less than the tool exit distance K. When Q or K is 0 or is not

defined, execute G81 center drilling cycle for each hole, and

P is invalid. When the values of Q and K are correct,

execute G83 deep hole machining cycle for each hole, and P

is valid.

Define cutting feed speed.

The repeat count (Generally used for multi-hole machining,

therefore X or Y is incremental value. It is optional when

L=1.)

Example

Use ĭ10 drilling bit for the drilling of the holes as shown in the figure:

%3361

N10 G55 G00 X0 Y0 Z80

N20 G98G79G90X20Y20G90R25Z0I15N3J15O3P2000Q-10K5F100

N30 G90 G00 X0 Y0 Z80

N40 M30

170

12. Fixed Cycle

12.1.8 Drilling Cycle (Center Drilling) (G81)

Description

The cycle is used for normal drilling. The cutting feed is executed to the

hole bottom, and then the tool rapidly exits from the hole bottom.

The movement specified by G81 is as shown in the figure below, where

the dotted line indicates rapid positioning:

Initial plane

Plane of point R

Point R

Point Z

G81 (G98）

G81 (G99)

Format

(G98/G99) G81 X_ Y_ Z_ R_ F_ L_ ;

Parameter

Description

X Y

The absolute position of the hole for absolute

programming (G90), or the distance from the current

tool position to the hole for incremental programming

(G91).

The absolute position of the hole bottom along Z axis

for absolute programming (G90), or the distance from

the hole bottom to the point R for incremental

programming (G91).

The absolute position of the point R along Z axis for

absolute programming (G90), or the distance from the

point R to the initial plane for incremental

programming (G91).

Cutting feed speed.

The repeat count

(Generally used for multi-hole

machining, and therefore X or Y is incremental value. It

is optional when L=1.)

171

12. Fixed Cycle

1. The tool moves rapidly to the point B over the hole center.

Operation procedure

2. Move rapidly to the point R, close to the workpiece.

3. Conduct drilling downward at the speed of F, to the point Z at the

hole bottom.

4. The spindle remains the rotation and moves upward rapidly to the

point R (G99) or B (G98).

Attention

1. If the movement amount of Z is zero, the command is not executed.

2. The drilling axis must be the Z axis.

3. The G81 command data is saved as modal data.

4. Before using the command of G81, use the corresponding M

command to rotate the spindle.

Example

Conduct drilling of the holes as shown in the figure below:

%3343

N10 G92 X0 Y0 Z80

N15 M03 S600

N20 G98 G81 G91 X20 Y15 G90 R20 Z-3 L2 F200

N30 G00 X0 Y0 Z80

N40 M30

172

12. Fixed Cycle

12.1.9 Drilling Cycle with Pause (G82)

Description

This instruction is mainly used for processing sink holes, blind holes, to

improve the hole depth precision. Except for the pause at the hole bottom,

other operations are similar as that of G81. The figure below shows the

operation of G82:

Initial plane

Plane of point R

Point R

Point Z

Pause

G82 (G98）

G82 (G99)

Format

(G98/G99) G82 X_ Y_ Z_ R_ P_ F_ L_;

Parameter

Description

X Y

The absolute position of the hole for absolute

programming (G90), or the distance from the current

tool position to the hole for incremental programming

(G91).

The absolute position of the hole bottom along Z axis

for absolute programming (G90), or the distance from

the hole bottom to the point R for incremental

programming (G91).

The absolute position of the point R for absolute

programming (G90), or the distance from the point R

to the initial plane for incremental programming (G91).

The duration that the tool remains at the hole bottom.

Unit: millisecond

Cutting feed speed.

The repeat count

(Generally used for multi-hole

machining to simplify programming. It is optional

when L=1.)

173

12. Fixed Cycle

1. The tool moves rapidly to the point B over the hole center.

2. Move rapidly to the point R, close to the workpiece.

Operation procedure

3. Conduct drilling downward at the speed of F, to the point Z at the

hole bottom.

4. Delay P milliseconds with the rotation of the spindle.

5. Move upward rapidly to the point R (G99) or B (G98).

Attention

1. The drilling axis must be the Z axis.

2. If the movement amount of Z is zero, the command is not executed.

3. The G82 command data is saved as modal data.

4. Before using the command of G82, use the corresponding M

command to rotate the spindle.

Example

Conduct drilling of the hole as shown in the figure below:

90 degrees

ĭ12

%3345

N10 G92 X0 Y0 Z80

N15 M03 S600

N20 G98 G82 G90 X25 Y30 R40 P2000 Z25 F200

N30 G00 X0 Y0 Z80

174

12. Fixed Cycle

12.1.10 Deep-Hole Drilling Cycle (G83)

Description

The fixed cycle is used for the intermittent feed along Z axis, which

enables a rapid tool exit to the reference point R with larger retract

amount after each drilling,.It facilitates the chip-removal and coolant

adding. The figure below shows the operation specified by G83:

Initial plane

Point R

Plane of point R

G98

G99

Point Z

Format

(G98/G99) G83 X_ Y_ Z_ R_ Q_ K_ F_ L_ P_;

Parameter

Description

X Y

The absolute position of the hole for absolute

programming (G90), or the distance from the current tool

position to the hole for incremental programming (G91).

The absolute position of the hole bottom for absolute

programming (G90), or the distance from the hole bottom

to the point R for incremental programming (G91).

The absolute position of the point R for absolute

programming (G90), or the distance from the point R to

the initial plane for incremental programming (G91).

The each downward drilling depth

(incremental value,

negative).

The distance away from the upper surface of drilled hole

(incremental value, positive). K cannot be greater than Q.

Cutting feed speed.

The repeat count (Generally used for multi-hole machining

to simplify programming. It is optional when L=1.)

The duration that the tool remains at the hole bottom. Unit:

millisecond

176

12. Fixed Cycle

1. The tool moves rapidly to the point B over the hole center.

2. Move rapidly to the point R, close to the workpiece.

Operation procedure

3. Drill downward at the speed of F, with depth q.

4. Move upward rapidly to the point R.

5. Move downward rapidly to the upper surface of the drilled hole, the

distance is specified with K.

6. Drill downward at the speed of F, with depth (q + k).

7. Repeat the step 4, 5, and 6, and then drills to the hole bottom Z

point.

8. Delay P milliseconds at the hole bottom (spindle remains rotation).

9. Exit upward rapidly to the point R (G99) or B (G98).

Attention

1. The drilling axis must be the Z axis.

2. If the movement amount of Z, Q, and K are zero, the command is

not executed.

3. The G83 command data is saved as modal data.

4. Before using the command of G83, use the corresponding M

command to rotate the spindle.

Example

Conduct drilling of the hole as shown in the figure below:

177

12. Fixed Cycle

12.1.11 Tapping Cycle (G84)

Description

on the same principle. In the G84 mode, the tool taps to the hole bottom

with the spindle rotation in the clockwise direction and then goes back

with the spindle rotation in the counter clockwise direction. See the

figure below:

Initial plane

Spindle CW

Spindle stop

Spindle CW

Spindle stop

Point

Point Z

Spindle stop

Spindle CCW

Spindle stop

Spindle CCW

G84 (G98)

G84 (G99)

The command G84 and G74 works

Format

G84 X_ Y_ Z_ R_ Q_ P_ F_ L_H_J_;

Parameter

Description

X Y

The absolute position of the hole for absolute

programming (G90), or the distance from the current

tool position to the hole for incremental programming

(G91).

The absolute position of the hole bottom for absolute

programming (G90), or the distance from the hole

bottom to the point R for incremental programming

(G91).

The absolute position of the point R for absolute

programming (G90), or the distance from the point R to

the initial plane for incremental programming (G91).

The amount of each feed during segment tapping.

Leave it blank in the H2 mode.

The duration that the tool remains at the hole bottom.

Unit: millisecond.

Define thread lead.

179

12. Fixed Cycle

The repeat count (Generally used for multi-hole

machining, and therefore X or Y is incremental value. It

is optional when L=1.)

J1: A axis tapping; J2: B axis tapping; J3 C: axis

tapping

F (feed speed) during tapping

During rigid tapping, the value of feed speed

(F) specified in the

programming is invalid. The feed speed along the tapping axis is derived

from:

feed speed = spindle speed X thread lead

Tapping mode

C axis tapping: take the servo spindle as the C axis, and conduct tapping

by interpolation, to achieve high-speed high-precision tapping

Attention

The tapping axis must be the Z axis.

The point Z must be lower than the plane of point R; otherwise, an

alarm will be reported.

The G84 command data is saved as modal data.

When the motion amount of Z is zero, the cycle is not executed.

During forward tapping, the operations on feed rate adjustment,

spindle rate adjustment, and feed hold is invalid during tapping.

Before executing the tapping command G84, change the control

mode of the spindle servo motor from speed control to the position

control by using the STOC command. After tapping, you may use

the CTOS command to change back to the speed control mode and

use the servo spindle as a common spindle.

Before using the command of G84, use the corresponding M

command to rotate the spindle in the clockwise direction.

After calling the rigid tapping G84, the programmer must restore

the original feed speed; otherwise, the feed speed will be the rigid

tapping speed (s*pitch).

The rotation or zoom command is not supported during rigid

tapping (The limitation is for all fixed cycles).

180

12. Fixed Cycle

12.1.12 Boring Cycle (G85)

Description

The command is used to bore the holes which have low requirement for

precision. The operation specified by G85 is as shown below:

Initial plane

Plane of point R

Point R

Point Z

G85 (G98)

G85 (G99)

Format

(G98/G99) G85 X_ Y_ Z_ R_ F_ L_;

Parameter

Description

X Y

The absolute position of the hole for absolute

programming (G90), or the distance from the current

tool position to the hole for incremental programming

(G91). UW programming is not supported.

The absolute position of the hole bottom for absolute

programming (G90), or the distance from the hole

bottom to the point R for incremental programming

(G91).

The absolute position of the point R for absolute

programming (G90), or the distance from the point R to

the initial plane for incremental programming (G91).

Cutting feed speed.

The repeat count (Generally used for multi-hole

machining to simplify programming. It is optional when

L=1.)

Operation procedure

1. The tool moves rapidly to the point B over the hole center.

2. Move rapidly to the point R, close to the workpiece.

182

HNC-818. User Manual - page 6