Content      ..     4      5      6      7     ..

HNC8 Series CNC Controller. Programming Manual (V2.4) - page 6

 Deep hole processing can be realized through repeated advance and retreat;

 After each drilling, the tool exits the workpiece to the safety level R point, which

has a good chip removal effect, and the chip breaking can be achieved.

 Spot drilling - H3 mode

Initial level

Point R level

Point R level

G83 or G87 (G98)

G83 or G87 (G99)

 Drill directly to the bottom of the hole each time, and then quickly exit;

 Designed for shallow hole drilling, no chip breaking and chip removal.

20

Example

To process the workpiece as shown in the diagram, the code format is as follows:

%1111

G54X0Z50

G98G83Z-10R10Q5K2P1000F200H1

G99G83Z-10R10Q5K2P1000F200H1

G0X0Z50

G98G83Z-10R10Q5K2P1000F200H2

G99G83Z-10R10Q5K2P1000F200H2

G0X0Z50

G98G83Z-10R10Q5K2P1000F200H3

G99G83Z-10R10Q5K2P1000F200H3

M30

%1111

G54Z0X50

G98G87X-10R10Q5K2P1000F200H1

G99G87X-10R10Q5K2P1000F200H1

G0Z0X50

G98G87X-10R10Q5K2P1000F200H2

G99G87X-10R10Q5K2P1000F200H2

G0Z0X50

G98G87X-10R10Q5K2P1000F200H3

G99G87X-10R10Q5K2P1000F200H3

M30

Note

(1) When H=1, the tool retracts the specified retraction distance K. It is stipulated in the canned

cycle that when drilling with H1 and H2 modes, the amount of feed Q and the amount of retract

k must be specified.

20

(2) Even if P, Q, K are not specified, if P, Q, K, are specified with previous G83, the variable will

still be inherited. If a G83 line is normally specified, for the following G83 only the coordinates

need to be specified. However, G01 , G00 will terminate this G83 modal, and for G83 after G01,

G00, G02, G03 commands all parameter must be specified.

(3) The feed amount and the retraction amount must be larger than 0.

(4) If PWM spindle is used, C command cannot be used.

14.2.2 Axial Rigid Tapping Cycle (G84)/ Radial Rigid Tapping Cycle (G88)

Function and Purpose



Turning centers with powered tool often require axial or radial thread processing. The G84

command of this system can be used for tapping of axial thread; G87 can be used for tapping of

radial thread. For the two processing methods, there only is the difference in the feed axis, and

the drilling trajectory is exactly the same. The axial tapping is fed along Z axis and the radial

tapping is fed along X axis.

In addition, axial tapping is also suitable for conventional lathes. At this time, the workpiece or

tap can be installed on the lathe spindle to form the main cutting movement, and the tap or

workpiece can be installed on the tool post to perform the Z-axis feed movement to realize the

axial tapping.

Command Format

1. Axial rigid tapping cycle

G84 Z(W)_R_P_Q_E_J_K_F_H_

Parameter

Meaning

Z

Coordinates of hole bottom

R

Distance from initial level to R level

P

Dwell time at hole bottom

F

Feedrate

Q

Feed amount

K

Retraction amount

E1

Forward tapping

E2

Reverse tapping

J1

Tapping of the first spindle C axis

J2

Tapping of the second spindle A axis

H1

Retract the specified retraction amount K

H2

Retract to R point

H3

Directly move to hole bottom

20

2. Radial rigid tapping cycle

G88X(U)_R_E_Q_K_H_P_F_ (Only tapping of the second spindle A axis)

Parameter

Meaning

E1

Forward tapping

E2

Reverse tapping

Q

Feed amount

K

Retraction amount

H1

Retract the specified retraction amount K

H2

Retract to R point

H3

Directly move to hole bottom

Description



When executing this cycle, along the axis of the tool, the spindle rotates clockwise and taps to the

bottom of the hole, and then the spindle counterclockwise rotates and retracts. According to the

G98 or G99 command, the tap returns to the initial plane (G98) or the R level (G99). The specific

trajectory is shown in the figure below.

Initial level

Spindle rotation CW

Spindle rotation

CW

Point R level

Spindle rotation CCW

Spindle rotation CCW

G84 or G88 (G98)

G84 or G88 (G99)

Example

%1111

M3 S1=1000; No. 1 spindle rotates

G0X50Z50

M5

20

Description



1. Note for FANUC mode canned cycle:

 When G83 and G84 are used in combination, the R value in G84 cannot be omitted. The

modal of the R value across the canned cycle are not inherited;

 P and Q in G74 and G75 can support decimals (unit is um), but FANUC only supports

integers, and will alarm when it is decimal;

 P and Q in G76 can support decimals (unit is um), while FANUC only supports integers,

and will alarm when it is decimal;

 G74 and G75 do not support each execution of a feed P as a single block, but the

completion of entire execution as a single block

 When the G92 is executed in single block, the feed will be held at the starting point of

the cycle after one cutting is finished. It does not support step-by-step operation during

threading. In addition, the feed hold button is invalid during the thread cutting process,

and it does not support FANUC's return to the cycle start point after pressing the feed

hold;

 G76 in HCNC format is not allowed in FANUC mode;

 For all canned cycles, if only the canned cycle G code is specified without any

commands after it, the canned cycle will be skipped directly.

20

15 Canned Cycle for Milling System (M)

15.1

Standard Canned Cycle for Milling System

Function and Purpose



There is a relatively fixed operating sequence for the processing of hole parts. With this function,

the canned cycle subprogram can be called through a single block to complete a fixed processing

action. Therefore, programming can be simplified, and memory can be effectively used. Table

15.1(a) is the canned cycle command list of the CNC system.

Table 15.1 (a) Drilling canned cycle list

Drilling (-Z

Action at hole

Retraction (+Z

G command

Use

direction)

bottom

direction)

Intermittent

High-speed deep hole

G73

Dwell

Rapid traverse retract

cutting feed

drilling cycle

Dwell—spindle

G74

Cutting feed

Cutting retract

Reverse tapping

rotation CW

G76

Cutting feed

Spindle orientation

Rapid traverse retract

Fine boring

G80

——

——

——

Cancel cycle

G81

Cutting feed

——

Rapid traverse retract

Spot drilling, boring

G82

Cutting feed

Dwell

Rapid traverse retract

Drilling, boring

G83

Cutting feed

Dwell

Rapid traverse retract

Deep hole drilling cycle

Dwell—spindle

G84

Cutting feed

Cutting retract

Tapping cycle

rotation CCW

G85

Cutting feed

——

Cutting retract

Boring

Dwell—spindle

G86

Cutting feed

Rapid traverse retract

Boring

stop

Spindle rotation

G87

Cutting feed

Rapid traverse retract

Reverse boring

CW

Dwell—spindle

G88

Cutting feed

JOG

Boring

stop

G89

Cutting feed

Dwell

Cutting retract

Boring

Description



Generally there are the following six sequential actions for the hole machining cycle:

Sequential action 1: X and Y axis positioning (different planes may have different positioning

axes)

Sequential action 2:rapid traverse to machining plane R point

20

Sequential action 3: execute drilling action

Sequential action 4: action at hole bottom (hole buttom level Z point)

Sequential action 5: retract to R level

Sequential action 6: retract to the initial level B point in rapid traverse

Detailed breakdown is shown in Figure 1.1 (a)

Action 1

Initial level

Action 6

Action 2

R point

Rapid traverse

Feed

Hole bottom

Figure 1.1（a）

 Positioning plane

The positioning plane is determined by the plane selection mode G17, G18, and G19.

The positioning axis is an axis other than the drilling axis.

Positioning plane

Positioning axis

G17

X, Y

G18

X, Z

G19

Y, Z

 Drilling axis

Hole machining canned cycles include drilling cycles, tapping cycles, boring cycles, etc., but in

order to simplify the description, this section will collectively refer to various canned cycles as

drilling cycles, and drilling axis, tapping axis, and boring axis are collectively referred to as

drilling axis.

The drilling axis is a reference axis (X, Y, Z) that does not form the positioning plane or an axis

parallel to it.

The reference axis or parallel axis used as the drilling axis is determined by the positioning plane

20

of drilling (G17, G18, G19).

If the axis address of drilling axis is not specified, the reference axis is assumed to be the drilling

axis.

Positioning axis

Drilling axis

G17

Z-axis

G18

Y-axis

G19

X-axis

 Drilling data

G73, G74, G76 and G81 to G89 are all modal G code commands, which are valid until they are

cancelled. In these drilling cycle commands, the specified parameters are also modal data,and are

kept until they are modified or cleared.

 Length compensation G43/G44/G49

G73, G74, G76, and G81 to G89 drilling canned cycles can use tool length compensation. The

compensation point is used to establish compensation in the initial plane. G43 is for positive

compensation, and G44 is for negative compensation. The use of compensation needs to be

established with the tool compensation table. Different tool compensation registers are called to

achieve different compensation data.

Note: Through NC parameter 000012 Tool Axis Selection Mode, the Z axis can always be set as

the drilling axis. When the parameter is set to 0, the tool length compensation is always

compensated on the Z axis. When the parameter is set to 1, the compensation axis is switched

based on the machining coordinate selection plane. See drilling axis positioning plane.

Movement amount of drilling axis G90/G91

The movement amount on the drilling axis can be expressed by the coordinate value of the

positioning point or the relative movement amount, which is specified by the G90 or G91

command in the program, as shown in Figure 1.1(b):

G90 (absolute command)

G91 (incremental command)

Point R

Point R

Point Z

Point Z

20

Figure 1.1(b)

 Return to plane G98/G99

Whether to return the tool from the hole bottom to the machining level (point R) or to the initial

level (point B) is specified by G98 and G99. Figure 1.1(c) shows the action when G98 or G99 is

specified. Generally, G99 is used for the first drilling and G98 is used for the final drilling. Even

if drilling is performed in G99 mode, the initial level will not be changed.

G98 (return to initial level)

G99 (return to R level)

Initial level

Point R level

Point R

图 1.1(c)

 Repeat

When user wants to repeat equidistant drilling, use L_ to specify the number of repetitions with

G91 relative coordinate command.

L is only valid in the block where it is specified.

Specify the position of the first hole in incremental mode (G91).

If it is specified in absolute mode (G90), the drilling is repeated at the same hole position.

Maximum value of number of repetitions L is 9999

Specify 0 or an integer value from 1 to 9999 for L.

 Single block

When the hole machining cycle is performed in a single block, the control device stops at the end

points 1, 2, and 6 in Figure 1.1(a). Therefore, 3 times are required to drill a hole. At the end of

actions 1 and 2, the indicator light of feed dwell lights u. At the end of action 6, if the number of

repetitions is left, it will stop by feeding dwell. If there is no repetition number, it will stop in the

single block stop state. In addition, the R point of G87 will not stop. G88 also stops after dwell at

point Z.

 Cancel

G80 or the 01 group of G codes is used to cancel the canned cycle.

21

The 01 group of G codes include:

G00 : positioning (rapid traverse)

G01 : linear interpolation

G02 : circular interpolation or helical interpolation (CW)

G03 : circular interpolation or helical interpolation (CCW)

G60 : unidirectional positioning

 Explanation of symbols in the figure

The following describes each canned cycle.

The images used in these descriptions are represented by the following symbols.

Positioning (rapid traverse G00))

Cutting feed (linear interpolation G01)

Manual feed

Dwell

Note

1） When executing a canned cycle block that does not contain X, Y, Z traverse axis

commands, this line will not produce tool movement, but the cycle parameter modal

value of the current line will be saved;

2） Specifying the 01 group of G codes or specifying G80 will cancel the current canned

cycle G code modal, and also clear the cycle parameter modal value;

3） If the canned cycle needs to be repeated by specifying L, when L is specified as 0, an

alarm message will appear;

4） When using G53 command in a canned cycle block, its positioning data X, Y are still

the original workpiece coordinate system data, not the coordinate system data specified

by G53;

5） When switching the drilling axis for drilling, please cancel the drilling canned cycle;

6） To use this canned cycle function, user needs to set the machine user parameter 010083

drilling canned cycle type to 0 to call the HCNC canned cycle.

21

15.2

High-speed Deep-hole Drilling Cycle（G73）

Function and Purpose



This cycle is for high-speed deep hole drilling. When this command is executed, the tool

intermittently cuts and feeds to the bottom of the hole. Intermittent feed makes it easy to break

chips, remove chips, add coolant adding during deep hole machining, and the amount of tool

retraction is not large.

Command Format

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

Parameter

Meaning

Coordinate position of hole center in XY plane in absolute programming (G90);

X Y

The incremental value of hole center relative to the starting point in XY plane in

incremental programming (G91);

Coordinate value of Z point of hole bottom in absolute programming; incremental value of

Z

Z point of hole bottom relative to the reference point R in incremental programming (G91);

Coordinates of reference point R in absolute programming (G90); the incremental value of

R

reference point R relative to the intial point B in incremental programming (G91);

Q

Hole drilling depth downward (incremental value, negative);

P

Dwell time at the hole bottom, in the unit of ms

K

Retraction amount upward (incremental value, positive)

F

Feedrate of drilling;

L

Cycle times (when repeat drilling is needed)

G73（G98）

G73（G99）

21

Initial level

Point R

Point R

Point R level

Point Z

Point Z

Description



 Drilling action

（1）Tool position point moves to B point above the hole center in rapid travers;

（2）Rapid traverse to workpiece surface R point;

（3）Drill downward at F speed with depth of q;

（4）Tool retracts upward with distance of K;

（5）Repeat steps 3 and 4 several times;

（6）Drill to Z point at hole bottom;

（7）Pause at the hole bottom P seconds (spindle keeps rotating);

（8）Return to R point (G99) or B point upward.

 The high-speed deep hole drilling cycle executes intermittent feed along Z axis. When this

cycle is used, the chips can be easily discharged from the hole, and a small retraction value

can be set, which allows effective drilling.

 Use the auxiliary function to rotate the spindle before specifying G73 (M code).

 When G73 code and M code are specified in the same block, the M code will be executed at

the same time as the first positioning action, and then the system will process the next drilling

action.

 When the number of repetitions L is specified, the M code is only executed in the first hole,

and the M code is not executed in the second and subsequent holes

21

 When the tool length offset (G43, G44 or G49) is specified in the canned cycle, the offset is

added while positioning to the R point

 When Z, K, Q movement amounts are zero, this command is not executed.



|Q|>|K|；

Example

Process the holes as shown in the figure below:

Example 1 (absolute programming, return to R level):

N10 G54 G0 X0 Y0 Z80；Establish coordinate system, move to the safe starting point

N20 M03 S500； Spindle rotates CW

N30 G0 Z20； Position to the intial level

N40 G99 G73 X10 Y10 Z-35 R5 Q-3 K1 F200； After positioning, perform drilling 1,

and return to R level

N50 X20； After positioning, complete all drilling, and return to R level

N60 X30

N70 X40

N80 Y20

N90 X30

N100 X20

N110 X10

N120 G80； Cancel G73 canned cycle

N130 G28 G91 X0 Y0 Z0； Return to reference point

N140 M30； Program ends

21

15.3

Reverse Tapping Cycle（G74）

Function and Purpose



This cycle is for reverse tapping. There are two types of reverse tapping. One is the reverse tapping

cycle. The tapping trajectory goes directly from point R to the point Z at the bottom of the hole;

the other is the reverse pecking tapping cycle. Repeated intermittent feed is performed during the

tapping process.

In the reverse tapping cycle, when the bottom of the hole is reached, the spindle rotates CW and

exits. During the tapping or retraction, the tool feeds a thread lead along the tapping axis for each

revolution of the spindle, the feed relationship does not change even during acceleration and

deceleration.

Command Format

15.3.1 Reverse Tapping Cycle

(G98/G99)G74 X_ Y_ Z_ R_ P_ F_ L_J_；

Parameter

Meaning

Absolute position of hole in absolute programming (G90);

X Y

The distance from the current position to the hole position in incremental

programming (G91).

Absolute position of hole bottom in absolute programming (G90);

Z

The distance from hole bottom to R point in incremental programming (G91).

Absolute position of R point in absolute programming (G90);

R

The distance from R point to initial level in incremental programming (G91).

P

The dwell time at the hole bottom, in the unit of ms.

F

Thread lead.

L

Repeat times (can be omitted when L=1).

J

J1 A-axis tapping; J2 B-axis tapping; J3 C-axis tapping.

G74（G98）

G74（G99）

21

Initial level

Initial level

Spindle rotation

Spindle rotation

Spindle stop

Spindle stop

CCW

CCW

Point R

Point R

Point Z

Point Z

Spindle stop

Spindle rotation CW

Spindle stop

Spindle rotation CW

 Reverse tapping action:

(1) Rotate the spindle through the auxiliary function, and the tool position point moves to point B

above the hole center in rapid traverse;

(2) The spindle rotates counterclockwise and rapid traverse to the surface of the workpiece to

point R

(3) The system calculates the feedrate based on the pitch speed, and taps at the feedrate downward.

The depth is Z;

(4) Tap to the hole bottom, and spindle stops;

(5) Dwell at the hole bottom after the dwell time (P) is specified;

(6) Spindle rotates CW, return to R point upward;

(7) Spindle stops;

(9) Return to R point (G99) or B point (G98);

15.3.2 Reverse Peck Tapping Cycle

(G98/G99)G74 X_ Y_ Z_ Q_ K_R_ P_ F_ L_E_J_

（Peck tapping）

Parameter

Meaning

The absolute position of hole in absolute programming (G90);

X Y

The distance from the current position to the hole position in incremental

programming (G91).

The absolute position of hole bottom in absolute programming (G90);

Z

The distance from hole bottom to R point in incremental programming (G91).

21

Q

The feed amount in peck tapping;

K

The retraction amount in peck tapping;

The absolute position of R point in absolute programming (G90);

R

The distance from R point to the intial level in incremental programming (G91).

P

The dwell time at the hole bottom, in the unit of ms;

F

The thread lead;

L

Repeat times (it can be omitted when L=1);

E

E1： Peck tapping, feed Q, retract K;

E2： Peck tapping, feed Q, return to R level.

J

J1 A-axis tapping; J2 B-axis tapping; J3 C-axis tapping.

Initial level

Point R level

Point R

Point R

Point Z

Point Z

 Reverse tapping cycle action (peck tapping):

(1) Rotate the spindle through the auxiliary function, and the tool position point moves to point B

above the hole center in rapid traverse;

(2) The spindle rotates counterclockwise and rapid traverse to the surface of the workpiece to

point R;

(3) The system calculates the feedrate based on the pitch speed, and taps at the feedrate downward.

The depth is Q;

(4) Spindle stops;

(5) When dwell time (P) is specified, dwell is performed;

(6) Spindle rotates clockwise, taps upwards and returns to R point;

(7) Spindle stops;

(8) Spindle rotates counterclockwise. Tap downward at the feedrate, the depth is (times*Q);

21

(9) Repeat steps 4, 5, 6, 7, 8, and arrive at Z point of hole bottom;

(10) Dwell P ms at hole bottom;

(11) Spindle rotates clockwise. Retract upward to R point (G99) or B point (G98) in rapid traverse.

Description



 Perform tapping with spindle rotation CCW. When it reaches the bottom of the hole, the

spindle rotates clockwise for return. This cycle processes a reverse thread.

 During reverse tapping, the feedrate override is omitted. The feed is paused, and the machine

doesn’t stop unit the retraction is completed.

 Before G74 is specified, use the auxiliary function (M code) to counterclockwise rotate

spindle.

 When G74 command and M code are specified in the same block, the M code will be

executed at the same time as the first positioning action, and then the system will process the

next drilling action.

 When the number of repetitions L is specified, the M code is only executed for the first hole,

and is not executed for the second and subsequent holes.

 When the tool length offset G43, G44 or G49 is specified in the canned cycle, the offset is

added while positioning to the R point.

Example

Process the holes as shown in the figure below:

Example 1 (Absolute programming, tapping, return to R level)

21

(6) Position mode G108 or STOC: Before using the tapping command G74, please pay attention

to use STOC command to switch the control mode of the spindle servo motor from speed mode

to position mode. After tapping is completed, user can use CTOS to switch the control mode of

the spindle servo motor from position mode to speed mode, and the servo spindle is used as a

normal spindle.

(7) Cancel: Do not specify the G codes of group 01 (G00 to G03, etc.) in the G74 block. Otherwise,

G74 will be cancelled.

(8) Tool position offset: In the drilling canned cycle mode, the tool position offset is ignored.

(9) R: Specify R in the drilling block. If R is specified in the non-drilling block, it cannot be stored

as modal data.

(10) P: Please specify P in the drilling block. If it is specified in the non-drilling block, it cannot

be stored as modal data.

(11) Q: Please specify Q in the drilling block. If it is specified in the non-drilling block, it cannot

be stored as modal data.

(12) Reset: When the reset is performed during rigid tapping, the rigid tapping mode cannot be

released, and the machine tool cannot stop the tapping action. Emergency stop is availarble.

(13) Feed hold, single block: In G74 (G84) mode, the feed hold will be executed after each tapping

action is completed, and the subsequent tapping will continue to be performed after pressing the

cycle start button. In single block mode, the feed hold will be executed after each tapping action

is completed, and the next tapping action will be completed after pressing the cycle start button.

(14) Machine lock: The machine lock is also valid for G74 (G84). Even if G74 (G84) is executed

when the machine is locked, the drilling axis will not move. Therefore, the spindle will not move.

15.4

Fine Boring（G76）

Function and Purpose



This cycle is for precision hole boring.

In the fine boring cycle, when the bottom of the hole is reached, the spindle stops cutting, and the

tool nose leaves the machining surface of the workpiece and returns.

Command Format

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

Parameter

Meaning

Absolute position of hole in absolute programming (G90);

Distance from the current position to position of hole in incremental programming

X Y

(G91).

UV programming is not supported.

22

Absolute position of hole bottom on Z in absolute programming (G90);

Z

Distance from the hole bottom to R point in incremental programming (G91).

Absolute position of R point on Z in absolute programming (G90);

R

Distance from R point to initial level in incremental programming (G91).

I

Offset on X, can only be positive;

J

Offset on Y, can only be positive;

P

Dwell time at hole bottom (unit: ms);

F

Cutting feedrate;

L

Repeat times (it can be omitted when L=1)

G76（G98）

G76（G99）

Initial level

R point level

R point

R point

Z point

Z point

Offset (I, J)

Offset (I, J)

Description



 Fine boring cycle action

(1) Move to the tool position to point B above the hole center in rapid traverse

(2) Move close to the surface of the workpiece to point R in rapid traverse

(3) Bore downward at F speed, reach point Z at the bottom of the hole

(4) Dwell Z ms at hole bottom (spindle keeps rotating)

(5) Spindle orientation, spindle stops rotating

(6) The boring tool quickly moves I or J in the opposite direction of the tool nose

(7) Retract upward to R level (G99) or B level (G98) in rapid traverse

(8) Quickly move I or J in the positive direction of the tool nose, and the tool position point will

return to point R or B above the hole center

22

(10) Spindle resumes CW rotation

 The drilling axis must be Z axis;

 Z point must be lower than R level; otherwise an alarm will be issued;

 G76 command data is stored as modal data, the same data can be omitted;

 Before using the command G76, please use the corresponding M code to rotate the spindle.

Example

Process the hole as shown below,

Example 1 (absolute programming, return to R level):

%3341

N10 G54 G90 G0 X0 Y0 Z80； Establish coordinate system, move to safe starting point

N20M03 S600； Spindle rotation CW starts

N30G00 Z20； Position to initial level

N40 G99 G76X10Y20 Z-35 R5 I1 P2000 F100； Complete boring of hole 1 after

positioning, return to the level of point R

N50X25 Y30； Complete boring of the remaining holes after positioning, return to the

level of point R

N60 X40 Y20

N70 X25 Y10

N80 G80； Cancel G76 boring cycle

N90 G91G28 X0 Y0 Z0； Return to reference point

N100 M30； Program end

Example 2 (absolute and incremental mixed programming, return to the initial level):

%3343

22

15.5

Drilling Cycle (Center Drills)（G81）

Function and Purpose

This cycle is for the normal drilling.

The feed cutting is performed to the hole bottom, and the tool returns from the hole bottom in

rapid traverse.

Command Format

(G98/G99) G81 X_ Y_ Z_ R_ F_ L_ ；

Parameter

Meaning

X Y

The hole position data. The absolute position of the hole in absolute programming, and

the distance from the current position to the hole position in incremental programming;

Z

The position of hole bottom. The absolute position of hole bottom on Z in absolute

programming (G90); the distance from hole bottom to R point in incremental

programming (G91);

R

Position of R point. The absolute position of R point on Z in absolute programming

(G90); the distance from R point to initial level in incremental programming (G91);

F

Cutting feedrate

L

Number of repetitions (can be omitted when L=1, generally used for multi-hole

processing, so X and Y should be incremental values)

G81（G98）

G81（G99）

Initial level

R point level

R point

R point

Z point

Z point

Description



 Action

Tool position point moves to the B point above hole center in rapid traverse;

Move close to the workpiece surface to R point in rapid traverse;

Drilling downward at F speed to the hole bottom Z point;

22

Spindle keeps rotating; retract upward to R point (G99) or B point (G98) in rapid traverse.

 Spindle rotation

Before G81 is specified, the auxiliary function (M code) is used to rotate spindle.

 Auxiliary function

When G81 and M code are specified in the same block, the M code is executed during the initial

positioning.

When the number of repetitions L is specified, the above actions will only be executed for the

first time. The M code will not be executed after the second time.

 Tool length compensation

When tool length compensation (G43, G44, G49) is specified in the drilling canned cycle, the

compensation is used when positioning to the R point.

Example

Process the hole shown as below,

Example 1

%3343

G54G0 X0 Y0 Z30； Return to the safe height of workpiece zero

M03 S600； Spindle rotation CW

G0 Z10； Position to the initial plane

G90G99 G81 X10 Y10 R5 Z-35 F200； Position to the hole (10 10), perform drilling,

return to R level

G91X10L3； Drill the last three holes on horizontal axis, return to R level

Y10； Position to the hole (40 20), perform drilling, return to R level

G91X10L3； Drill the last three holes on horizontal axis

22

15.6

Drilling Cycle with Pause（G82）

Function and Purpose



This cycle is used for normal drilling, counternboring, and blind hole processing.

The cutting feed proceeds to the bottom of the hole. Tool pauses at the bottom of the hole, and

then retracts from the bottom of the hole in rapid traverse.

This cycle can improve the accuracy of the hole depth.

This command is the same as G81 except that it needs to pause at the bottom of the hole.

Command Format

(G98/G99) G82 X_ Y_ Z_ R_ P_ F_ L_ ；

Parameter

Meaning

X Y

The absolute position of the hole in absolute programming, and the distance from

the current position to the hole position in incremental programming;

Z

The absolute position of hole bottom in absolute programming (G90); the distance

from hole bottom to R point in incremental programming (G91);

R

The absolute position of R point in absolute programming (G90); the distance from

R point to initial level in incremental programming (G91);

P

Dwell time at the hole bottom (unit: ms)

F

Cutting feedrate

L

Number of repetitions (can be omitted when L=1, generally used for multi-hole

processing)

G82（G98）

G82（G99）

Initial level

R point level

R point

R point

Z point

Z point

Dwell

Dwell

22

Description



 Action

(1) Tool position point moves to B point above hole center in rapid traverse;

(2) Move close to the workpiece surface to R point;

(3) Drill downward at F speed to Z point of hole bottom;

(4) Spindle keeps original rotating. Pause P ms

(5) Retract upward to R point (G99) or B point (G98)

 Spindle rotation

Before G82 is specified, the auxiliary function (M code) can be used to rotate spindle.

 Auxiliary function

When G81 and M code are specified in the same block, the M code is executed during the initial

positioning.

When the number of repetitions L is specified, the above actions will only be executed for the

first time. The M code will not be executed after the second time.

 Tool length compensation

When tool length compensation (G43, G44, G49) is specified in the drilling canned cycle, the

compensation is used when positioning to the R point.

Example

22

Example 1

%3343

G54G0 X0 Y0 Z30； Return to the safe height of workpiece zero

M03 S600； Spindle rotation CW

G0 Z10； Position to the initial level

G99 G82 X10 Y10 R5 Z-35 P1000 F200； Position to the hole (10 10), perform drilling,

return to R level

X10Y20； Position to the hole (10 20), perform drilling, return to R level

Y20Y15； Position to the hole (20 15), perform drilling, return to R level

X30Y10； Position to the hole (30 10), perform drilling, return to R level

X30Y20； Position to the hole (30 20), perform drilling, return to R level

G80； Cancel drilling canned cycle

G28 G91 Z0； Return to machine zero of Z axis

G28 G91 X0 Y0；Return to machine zero of X axis and Y axis

M30

Note

(1) Axis switching: please cancel canned cycle before switching drilling axis;

(2) Modality: G81 command data is stored as modal data, the same data can be omitted;

(3) Drilling: Drilling cannot be in the block that does not include X, Y, Z, R or any other additional

axis. If the moving position of Z is zero, the command is not executed;

(4) Cancel: Do not specify the G codes of group 01 (G00 to G03, etc.) in the G82 block. Otherwise,

G82 will be cancelled.

(5) Tool position offset: In the drilling canned cycle mode, the tool position offset is ignored.

(6) P: Please specify P in the drilling block. If it is specified in the non-drilling block, it cannot be

stored as modal data.

15.7

Deep Hole Drilling Cycle (G83)

Function and Purpose



This cycle is for deep hole processing.

This canned cycle is used for intermittent feed on Z axis. After drilling of each hole downward,

the tool quickly retracts to the reference point R. The retraction amount is larger, which is better

for chip removal and coolant adding.

Command Format

23

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

Parameter

Meaning

The absolute position of the hole in absolute programming, and the distance from

X Y

the current position to the hole position in incremental programming;

The absolute position of hole bottom in absolute programming (G90); the distance

Z

from hole bottom to R point in incremental programming (G91);

The absolute position of R point in absolute programming (G90); the distance

R

from R point to initial level in incremental programming (G91);

Q

Drilling depth downward (incremental value, negative)

Distance from the upper surface of the machined hole (incremental value,

K

positive)

Note: K cannot be larger than Q

F

Cutting feedrate

Number of repetitions (can be omitted when L=1, generally used for multi-hole

L

processing)

P

Dwell time at the hole bottom (unit: ms)

G83（G98）

G83（G99）

Initial level

Point R

Point R

R point level

Point Z

Point Z

Description



 Action

(1) Tool position point moves to B point above hole center in rapid traverse;

(2) Move close to the workpiece surface to R point;

(3) Drill downward at F speed with depth of q;

(4) Retract upward to R point;

23

(5) Move down to the top of the processed hole, at a distance of k;

(6) Drill downward at F speed with depth of （q+k）;

(7) Repeat steps 4, 5, 6. Reach Z point at hole bottom;

(8) Pause P ms at hole buttom (Spindle keeps original rotating).

(9) Retract upward to R point (G99) or B point (G98).

 Spindle rotation

Before G83 is specified, the auxiliary function (M code) can be used to rotate spindle.

 Auxiliary function

When G83 and M code are specified in the same block, the M code is executed during the initial

positioning. When the number of repetitions L is specified, the above actions will only be executed

for the first time. The M code will not be executed after the second time.

 Tool length compensation

When tool length compensation (G43, G44, G49) is specified in the drilling canned cycle, the

compensation is used when positioning to the R point.

Example

Process the hole as shown below.

Example 1

%3343

G54G0 X0 Y0 Z30； Return to the safe height of workpiece zero

M03 S800； Spindle rotation CW

G0 Z10； Position to the initial level

G99 G83 X10 Y20 R5 Z-35 Q-1 K0.2 F200； Position to the hole (10 20), perform

23

between tapping axis and spindle, which is referred to as the synchronous tapping. The

programming commands are the same for the following tapping and synchronous tapping.

Note that the pitch of the tap used for tapping should be consistent with that in the programming

15.8.1 Tapping Cycle（G84）

Command Format

(G98/G99)G84 X_ Y_ Z_ R_ P_ F_ L__J_；

Parameter

Meaning

The absolute position of the hole in absolute programming (G90), and the

X Y

distance from the current position to the hole position in incremental

programming (G91);

The absolute position of hole bottom in absolute programming (G90); the

Z

distance from hole bottom to R point in incremental programming (G91);

The absolute position of R point in absolute programming (G90); the distance

R

from R point to initial level in incremental programming (G91);

P

Dwell time at the hole bottom (unit: ms)

F

Thread lead

L

Number of repetitions (can be omitted when L=1)

J

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

G84（G98）

G84（G99）

Initial level

Initial level

Spindle rotation CW

Spindle stop

Spindle rotation CW

Spindle stop

R point

R point

Z point

Z point

Spindle stop

Spindle rotation CCW

Spindle rotation CCW

Spindle stop

 Action

(1) Rotate the spindle through the auxiliary function, and the tool position point will move to

point B above the hole center in rapid traverse;

(2) Spindle rotates CW, and approaches to the workpiece surface in rapid traverse, and reaches to

R point;

(3) System calculates feedrate base on the pitch speed; tap downward at the feedrate with the

depth of Z;

23

(4) Tap to the hole bottom, spindle stops;

(5) After the dwell time P is specified, pausing at hole bottom is performed;

(6) Spindle rotates CCW, tap upward in rapid traverse, retract to R point;

(7) Spindle stops;

(8) Retract upward to R point (G99) or B point (G98) in rapid traverse.

15.8.2 Peck Tapping Cycle (G84)

(G98/G99)G84 X_ Y_ Z_ Q_ K_R_ P_ F_ L_ E_J_

（peck tapping）

Parameter

Meaning

The absolute position of the hole in absolute programming (G90), and the

X Y

distance from the current position to the hole position in incremental

programming (G91)

The absolute position of hole bottom in absolute programming (G90); the

Z

distance from hole bottom to R point in incremental programming (G91)

Q

Feed amount

K

Retraction amount

The absolute position of R point in absolute programming (G90); the distance

R

from R point to initial level in incremental programming (G91);

P

Dwell time at the hole bottom (unit: ms)

F

Thread lead

L

Number of repetitions (can be omitted when L=1)

E

E1: peck tapping, feed Q, retract K

E2, peck tapping, feed Q, retract to R level

J

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

Initial level

R point

R point

R point level

Z point

Z point

 Peck tapping cycle action

(1) Rotate the spindle through the auxiliary function, and the tool position point will move to

23

Process the hole as shown below.

Example 1

%3343

G54G0 X0 Y0 Z30； Return to the safe height of workpiece zero

M03 S3000； Spindle rotation CW

G0 Z10； Position to the initial level

G90G99 G84 X25 Y10 R5 Z-35P1000 F1； Position to the hole (25 10), perform

drilling, return to R level

X25Y20； Position to the hole (25 20), perform drilling, return to R level

X10Y30； Position to the hole (10 30), perform drilling, return to R level

X40Y30； Position to the hole (40 30), perform drilling, return to R level

G80； Cancel canned cycle;

G28 G91 Z0； Return to machine zero on Z axis

G28 G91 X0 Y0； Return to machine zero on X axis and Y axis

M30；Program end

Note

Axis switching: please cancel canned cycle before switching drilling axis.

Modality: G84 command data is stored as modal data, the same data can be omitted.

Drilling: Drilling cannot be in the block that does not include X, Y, Z, R or any other additional

axis. If the moving position of Z is zero, the command is not executed. Z point must be lower than

R level, otherwise an alarm will be issued.

Position mode G108 or STOC: Before the tapping command G84 is used, please switch the

spindle servo motor from the speed mode to the position mode by the STOC command. After the

tapping, user could switch the spindle servo motor from position mode to speed mode by CTOS

23

command, and use the servo spindle as the ordinary spindle.

Scaling and Rotation: the rotation or scaling are not supported in the process of rigid tapping.

Cancel: Do not specify the G codes of group 01 (G00 to G03, etc.) in the G84 block. Otherwise,

G84 will be cancelled.

Tool position offset: In the drilling canned cycle mode, the tool position offset is ignored.

P: Please specify P in the drilling block. If it is specified in the non-drilling block, it cannot be

stored as modal data.

Q: Please specify Q in the drilling block. If it is specified in the non-drilling block, it cannot be

stored as modal data.

Reset: when the reset is executed during rigid tapping, the rigid tapping mode cannot be released,

and the machine tool cannot stop tapping.

Emergency stop can be effective.

Feed hold, single block: In G84 (G74) mode, the feed hold will be executed after each tapping

action is completed, and the subsequent tapping will continue after pressing the cycle start button.

The feed hold is executed after each tapping action is completed in single block mode, and the

next tapping action will be completed after pressing the cycle start button.

Machine lock: machine lock is also effective to G84 (G74).

Even if G84 (G74) is executed in the machine lock state, the drilling axis will not move. Therefore,

the spindle will not move.

15.9

Boring Cycle (G85)

Function and Purpose



This cycle is for hole boring.

In the boring cycle, when the bottom of the hole is reached, the cutting feed is executed until tool

returns to the R point. If in G98 mode, the tool will quickly return to the initial level after reaching

R point.

Command Format

(G98/G99) G85 X_ Y_ Z_ R_ P_ F_ L_；

Parameter

Meaning

The absolute position of the hole in absolute programming, and the distance from

X Y

the current position to the hole position in incremental programming;

23

The absolute position of hole bottom in absolute programming (G90); the

Z

distance from hole bottom to R point in incremental programming (G91);

The absolute position of R point on Z in absolute programming (G90); the

R

distance from R point to initial level in incremental programming (G91);

P

Dwell time at the hole bottom (unit: ms)

F

Cutting feedrate

L

Number of repetitions (can be omitted when L=1)

G85（G98）

G85（G99）

Initial level

R point level

R point

R point

Z point

Z point

Description



 Boring cycle actions

（1）Tool position point moves to B point above hole center in rapid traverse;

（2）Move close to the workpiece surface, and reach to R point;

（3）Bore downward at F speed;

（4）Reach Z point at hole bottom;

（5）Retract upward to R point at F speed (spindle keeps rotating);

（6）Retract upward to B point in rapid traverse if in G98.

 The drilling axis must be Z axis;

 Z point must be lower than B level; otherwise, the alarm will be issued;

 If the movement amounts of Z, Q, K are zero, then the command will not be executed;

 G85 command data is stored as the modal data, and the same data can be omitted;

 Please use corresponding M code to rotate spindle before G85 is used;

 When G85 and M code are specified in the same block, the M code is executed at the

23

Content      ..     4      5      6      7     ..