HNC8 Series CNC Controller. Programming Manual (V2.4)

Inside

Outside

Programmed path

Workpiece

Programmed path

Description



Action of tool radius compensation establishment and start

Meaning of sign

—S indicates that this position is the starting point for cutting.

—L indicates that the tool moves in a straight line.

—C indicates that the tool moves along an arc.

—r indicates tool radius compensation value.

(1) The tool moves around the inside of the corner (α≥180°)

Straight line→straight line

Straight line→arc

Workpiece

Programmed path

Tool center path

Programmed

Tool center path

path

(2) The tool moves around the outside of the corner (90°≤α＜180°)

Straight line→straight line

Straight line→arc

Starting point

Inside

Workpiece

Programmed path

Intersection

Tool center path

Programmed path

(3) The tool moves around the inside of the corner（α＜90°）

Straight line→straight line

Straight line→arc

Starting point

Workpiece

Programmed path

Tool center path

Programmed path

(4) The tool moves around the outside of the acute corner less than 1° (α<1°)

Straight line→straight line

Tool center path

Programmed path

Starting

Smaller than 1°

position

(5) There is no tool movement command in the starting block

If there is no tool movement command in the starting block, no offset is established.

G91 G40

N6 X100 Y100

N7 G41 X0

Tool center path

N8 Y-100

N9 Y-100 X100

Programmed path

Action of tool radius compensation in progress

For the programmed path (G00, G01, G02, G03), the system calculates the tool path from a

straight line/arc, and performs tool radius compensation.

During the compensation, if the same compensation command (G41/G42) is specified, the second

compensation command will be ignored.

During compensation, if five blocks without movement are consecutively specified, overcutting

or undercutting will occur.

In tool radius compensation, when M00 is designated, read-ahead is prohibited.

（1）The tool moves around the inside of the corner (α≥180°)

Straight line→straight line

Straight line→arc

Workpiece

Programmed path

Tool center path

Intersection

Programmed path

Tool center path

Arc→straight line

Arc→arc

Workpiece

Programmed path

Intersection

Tool center path

Programmed path

（2）The tool moves around the outside of the corner (90°≤α＜180°)

Straight line→straight line

Straight line→arc

Workpiece

Programmed path

Tool center path

Intersection

Tool center path

Intersection

Arc→straight line

Arc→arc

Workpiece

Programmed path

Tool center path

Intersection

Tool center path

（3）The tool moves around the inside of the corner（α＜90°）

Straight line→straight line

Straight line→arc

Workpiece

Programmed path

Tool center path

Programmed path

Arc→straight line

Arc→arc

Programmed path

Workpiece

Programmed path

Tool center path

Tool center path

mming Manual

Action at the time of tool radius compensation cancellation

To cancel the tool radius compensation, there must be a movement command other than the

circular command. If the radius compensation is canceled in the circular command, the system

will issue an alarm.

When any of the following conditions is met, the tool radius compensation is cancelled.

a) G40 is executed.

b) Compensation number D00 is executed.

(1) In the block where there is movement cancellation, when the tool moves around the inside of

the corner (α≥180°)

Straight line→straight line

Straight line→arc

Workpiece

Programmed path

Tool center path

Programmed path

Tool center path

(2) In the block where there is movement cancellation, when the tool moves around the outside

of the obtuse angle (90°≤α＜180°)

Straight line→straight line

Straight line→arc

Workpiece

Programmed path

Intersection

Tool center path

Intersection

Programmed path

Tool center path

(3) In the block where there is movement cancellation, when the tool moves around the outside

of the acute angle (α＜90°)

Straight line→straight line

Straight line→arc

Workpiece

Programmed path

Tool center path

Programmed path

12.5.3 Compensation Direction Change During Tool Radius Compensation

Function and Purpose



The tool radius compensation direction is determined by the tool radius compensation command

(G41/G42) and the sign of the compensation value.

Tool radius compensation

Compensation value +

Compensation value -

command

G41

Compensation left

Compensation right

G42

Compensation right

Compensation left

The system does not support the use of G41 and G42 to change the compensation direction, and

an alarm "The tool compensation direction is not allowed to be changed during radius

compensation" will appear during use. It is not recommended to change the compensation

direction by changing the compensation sign during the compensation process, because different

programming compensation methods and use environments may result in different effects.

Example

Note: The following changes the compensation direction by changing the sign of the

compensation amount during the compensation process. Examples of programming will show the

following paths. (It is not recommended to use tool direction change).

The compensation direction is changed (straight line to straight line)

There is a path intersection when changing the compensation direction

%1234

G90G54G0X-50Y50

G41G01X-50Y20D1 (compensation value is

X-30Y0

X30

X50Y20D2 (compensation value is -5)

Y50

M30

There is no path intersection when changing the compensation direction

%1234

G90 G54 G0 X-60 Y-30

G41 G01 X-50 Y-20 D1 (compensation value

is 5)

X-30 Y0

X30 Y0

X50 Y-20 D2 (compensation value is -5)

Y-50

M30

The compensation direction is changed in the way of (straight line to arc)

There is a path intersection when changing the compensation direction

%1234

G90 G54 G0 X-50 Y30

G41 G01 X-50 Y0 D1 (compensation

value is 5)

X-30 Y0

G2 X30 Y0 I30 J0 D2 (compensation

value is -5)

G1 X50 Y0 D1 (compensation value is 5)

G40

M30

There is no path intersection when changing the compensation direction

%1234

G90 G54 G0 X-50 Y30

G41 G01 X-50 Y0 D1 D1 (compensation

value is 5)

X-30 Y0

G3 X30 Y0 I30 J0 D2 (compensation

value is -5)

G1 X50 Y0 D1 (compensation value is 5)

M30

The compensation direction is changed (arc to arc)

Note: For the direction change programming for arc to arc, the system does not support the

following two programming methods.

There is a path intersection when changing the compensation direction

%1234

G90 G54 G0 X-50 Y0

G41 G01 X0 Y0 D1 (compensation

value is 5)

G2X53.64Y18.47I30J0

G41 feed

direction

X140.66Y0I41.55

J-18.47D2

(compensation value is -5)

G1X150

M30 This programming mode is not

supported for the direction change)

There is no path intersection when changing the compensation direction

%1234

G90 G54 G0 X-50 Y0

G41 feed

G41 G01 X0 Y0 D1 (compensation

direction

value is 5)

G3X18.02Y-4.04I9.03J1.7

X37.26Y-2.18I9.26 J3.7

G2X53.12Y10.61I13.99J-1.11D2

(compensation value is -5)

G1X50

M30 (This programming mode is not

supported for the direction change)

Linear reciprocating motion changes the direction of tool compensation vector

%1234

G90G54G0X-30Y0

G41G1X0Y0D1 (compensation value is

X80

G01X0D2 (compensation value is -5)

G40 G01 X-30

M30

12.5.4 When Tool Radius Compensation is not Executed

Function and Purpose



In radius compensation mode, when the commands (G28, G53) are executed, the compensation

vector will be temporarily invalid. After this type of command is executed, it will automatically

return to the compensation mode, and there is no need to cancel or add the compensation. The

point where the compensation vector is cancelled is the command point of the program. When the

compensation mode is restored, go directly to the command point and complete the restoration of

the compensation vector.

Description



(1) Reference point return command G28 in the radius compensation mode

At the intermediate point (there is no intermediate point when G91 is used, it is directly the

reference point), the compensation vector becomes 0

Example：%1234

G90G54G0X-30Y0

N1G41G1X0Y0D1

N2X40Y15

N3G28X50Y20

N4X80 Y30

N5X120 Y20

M30

Tool center path after compensation

Tool path when compensation is not executed

Point P is the position of the intermediate point at the time of reference point return. If there is no

intermediate point, it directly returns to the reference point.

(2) Direct machine coordinate system programming command G53 in radius compensation mode

In the G53 command (basic machine coordinate system selection), the compensation vector will

be temporarily cancelled.

12.5.5 There is a Block without movement in Tool Radius Compensation

Function and Purpose



In the process of tool compensation creation and execution, the following 5 blocks will be read

ahead to establish the tool compensation path, so when there are continuous blocks without

movement in the program, the system will deal with it as follows.

The following blocks are regarded as non-moving blocks,

Non-moving block type

Example

M auxiliary code

M03/M04/M05/M06/M08

S speed command

S300

T tool number command

T6/Grouping T101

G04 dwell command

G04 X5/G04 P5000

Programmable data input block

G10 L10 P_

Coordinate system setting

G92 X0 Y0

The third axis movement command in the

G17 Z10

compensation plane

G code

G90/G94/G95/G08/G09/G64/G65

The movement amount is 0

G91 X0

M00, M01, M02, and M30 are treated as M codes of read-ahead prohibition.

Description



When starting to establish compensation,

At the beginning of the compensation establishment, there are more than 5 con

secutive blocks without movement and the read-ahead prohibition M command,

it does not affect the establishment of compensation.

%1234

G92X0Y0

Block without movement

G0 X30 Y60

command

G41 D1

G4X2

F1000

S500

N1G1X20Y-50

X50Y-20

M30

(Note 1) When G41 is used to establish tool compensation, there is no movement amount, and

there is no movement in 5 consecutive blocks. The tool compensation path is executed when the

block N1 is executed. At this time, the compensation path is not affected when the entire program

is creating tool compensation.

In the compensation mode

When there are no over 4 continuous blocks without movement, and there is no M command of

read-ahead prohibition in the compensation mode, the vector that the length equal to the

compensation value will be generated in the vertical direction of the movement direction of the

previous and next blocks. The non-movement block is executed at the vector stop point after

compensation.

%0001

G90G54G0X0Y-30

G42G01X0Y0D1

N1X30Y50

N2G04P1000

； Program block

The N2 block is executed

here

without movement

N3X80

……

Several blocks without tool movement should not be commanded continuously.

If there are more than 4 consecutive non-movement blocks, and the M commands of read-ahead

prohibition, a vector with a length equal to the compensation value will also be generated in the

vertical direction of the movement direction of the previous and next blocks, and the non-

movement block will stop at the vector point after the compensation.

%0001

G90G54G0X0Y-30

Block without movement

G42G01X0Y0D1

command

N1X30Y50

G04P1000

G91X0

Consecutive

non-

M3S300

movement blocks are

executed here.

F2000

M00

；Non-movement block

N3X80

……

Note: The block without movement in the figure means: execute the program between N1 and

N3.

The non-movement command is executed while the compensation is cancelled

When the non-movement block and G40 command are executed at the same time, only the

compensation vector is cancelled.

%0001

G90G54G0X0Y-30

G42G01X0Y0D1

N1X30Y50

N2G40

；Non-movement block

N3X80Y30

12.5.6 Action Insertion in Tool Radius Compensation

MDI insertion command

1) Non-movement command is inserted in MDI (tool path will not change)

%0001

G90G54G0X0Y-30

G42G01X0Y0D1

N1X30Y50

；Insert the execution of

M3S1000 in MDI

N3X55Y20

……

The MDI mode can be switched to only when the feed is held, so when running to the N1 block,

the single-block running mode is switched to, and after entering the feed hold, the MDI mode is

switched to for the insertion of a non-movement command.

2) Insert a movement command in MDI

The system runs the program of radius compensation in auto mode. If a movement command is

input in MDI and the position of the machine tool is changed when the program is paused, the

system will alarm that it is not at the breakpoint position when it returns to the program to run. It

can continue to run after resuming the breakpoint position, and the compensation is added

normally.

Manual insertion action

The system runs the program in radius compensation in auto mode. If each axis of the machine

tool is moved in JOG mode, and the position of the machine tool is changed when the program is

paused, the system will alarm that it is not at the breakpoint position when it returns to the program

to run. It can continue to run after resuming the breakpoint position, and the compensation is

added normally.

12.5.7 Change of Compensation Value in Tool Radius Compensation

Function and Purpose



In principle, do not change the compensation number randomly in the radius compensation mode.

Different compensation numbers may correspond to different compensation values, and the

programmed trajectory will also change. If the compensation number is changed, the following

actions are performed.

The program code format for changing compensation number is as follows,

G41G01……D(r1)

G0/G01/G02/G03 X_ Y_

G0/G01/G02/G03 X_ Y_ D(r2) ； Compensation number is changed from r1 to r2

G0/G01/G02/G03 X_ Y_

……

Description



1) Path of straight line→straight line

The programmed path is an acute angle,

G90G54G0X-30Y0

G41G1X0Y0D01

（Compensation value is 5）

N1X20Y15

N2X40Y15

N3X60Y10D02

（ Compensation value is

10）

This part is executed by D02

This part is executed by D01

N4X80

……

Tool center path after compensation

Tool path before compensation

The programmed path is an obtuse,

This part is executed by D01

G90G54G0X-30Y0

G41G1X0Y0D01

（Compensation value is 5）

N1X50Y0

N2X40Y-20

N3X-20D02（Compensation

value is 10）

……

This part is executed by D02

2) Path of straight line→arc

Change of compensation amount inside sharp corners

G90G54G0X-30Y0

This part is executed by D02

G41G1X0Y0D01

（Compensation value is 5）

N1X20Y0

This part is executed by D01

N2G2X60Y0I20J0D02

N3X90Y0 （ Compensation

value is 10）

……

Change of compensation amount outside the sharp corner

This part is executed by D01

G90G54G0X-30Y0

G41G1X0Y0D01

（Compensation value is 5）

N1X20Y0

This part is executed by D02

N2G3X40Y-20I20J0D2

N3X90

（ Compensation

value is 10）

……

12.5.8 Interference Check

Function and Purpose



Usually, the overcutting of tool may occur after program read-ahead and tool radius compensation,

which is referred to as interference. The interference check function can check the tool overcut in

advance (even if there is no overcut, the interference check is performed). However, this function

cannot find out all interference.

Description



There are two modes for interference check via parameter setting.

Function

Parameter

Action

Before the overcut interference occurs

Interference

alarm

Interference check alarm function

during the compensation, the system

control Enable

will alarm and stop running

Auto

correct

The path is changed to avoid overcutting

Interference check avoidance function

interference Enable

Note: When parameter 010046 is set to 0, the interference alarm function is turned on.

When parameter 010046 is set to 1, the auto interference correction function is turned on.

When parameter 010047 (number of radius compensation interference check blocks) is set to 4,

3 blocks is read ahead for check interference.

As the compensation interference condition

In the pre-reading

4 blocks, when there are movement commands in 3 blocks, and the

compensation calculation vector on each movement command contact crosses the compensation

path, it is regarded as the interference.

r: compensation amount

j: the position the cross vector occurs

Tool center path after compensation

Tool path before compensation

Two modes are set to run the program with interference, the specific situations are as follows:

Example 1: use a tool with a larger diameter to process a parts containing a sharp corner

and a line segment

Left compensation

G90G54G0X-30Y0

N1G01G41X0Y0F1000

N2G01G41X20Y-30F1000

N3X30

N4X50Y0

……

1) Interference alarm

When parameter 010046 is set to 0, the interference alarm function is turned on. The parameter

010047 is set to 4 by default; When executing the above program, if an alarm is issued before N1

block, system stops running.

2) Interference avoidance

The intersection calculation of N2 and N4 blocks is executed, the interference avoidance vector

is created, the compensation path is automatically corrected, and the path is corrected to the a-e

path.

Example 2: Use a tool with a larger diameter to process the parts containing an arc of a

smaller radius

Left compensation

G90G54G0X_Y_

N1G01G41X_Y_F1000

N2G01X_Y_F1000

N3G2X_Y_I_J_

N4X_Y_

……

1) Interference alarm

When parameter 010046 is set to 0, the interference alarm function is turned on. The parameter

010047 is set to 4 by default; When executing the above program, if an alarm is issued before N1

block, system stops running.

2) Interference avoidance

Through the interference check processing, due to the path crossing occurs at points c and f, the

intersection calculation of N1 and N3 blocks is executed, the interference avoidance vector is

created, the compensation path is automatically corrected, and the path is corrected to the a-b path.

13 Programmable Data Input（G10/G11）

13.1

Programmable Data Input Command（G10/G11）

Function and Purpose



Through G10/G11 command, user can dynamically modify system data in the program. G10 is a

modal command. When G10 is specified, the programming data input mode can be entered, and

the modified system data will take effect in time. When G11 command is called, this mode is

cancelled.

The function list is as follows:

Function

G code

Input G54~G59 workpiece coordinate system origin

G10 L2 Pp IP_

Input G54.X extended workpiece coordinate system origin

G10 L20 Pp IP_

System parameter output

G10 L53 PpRr

Cancel user-defined input

G11

Milling tool geometry compensation value (length

G10 L10 PpRr

compensation) H input

Milling tool geometry compensation value (radius

G10 L12 PpRr

compensation) D input

Turning tool offset data input

G10 L14 Pp X_ Z_ R_ Q_ Y_ J_ K_

Single cutting time input

G10 L78 Pp

13.2

Workpiece Coordinate System Origin Input

Function and Purpose



According to the G10 command, the workpiece zero point (G54 to G59) offset can be set/changed

from the beginning of the program. In the absolute (G90) mode, the specified compensation

amount becomes the new compensation amount; in the incremental (G91) mode, the currently set

compensation amount is added to the specified compensation amount to become the new

compensation amount.

Command Format

G10 L2 Pp_ IP_

Parameter

Meaning

To specif the workpiece origin offset of the workpiece coordinate systems 1-6.



1 corresponds to G54 workpiece coordinate system



2 corresponds to G55 workpiece coordinate system



3 corresponds to G56 workpiece coordinate system



4 Corresponds to G57 workpiece coordinate system



5 corresponds to G58 workpiece coordinate system



6 corresponds to G59 workpiece coordinate system

The workpiece origin offset of axis in absolute mode.

It will be added to the original offset of the workpiece origin of axis in

incremental mode.

Example

%1002

G54 ； G54 initial value

G01X0Y0Z0

G90G10L2P1X100Y100Z100 ； G54 workpiece coordinate system zero is changed to

(100,100,100) in absolute mode.

G11

G01X20Y20Z20 ； The command value of the machine coordinate system is (120, 120,

120)

G91G10L2P1X50Y50Z50

； G54 workpiece coordinate system zero is changed to

(150,150,150) in incremental mode.

G11

G90G01X20Y20Z20 ； The command value of the machine coordinate system is (170, 170,

170)

M30

13.3

Extended Workpiece Coordinate System Origin Data Input

Function and Purpose



According to the G10 command, the offset of the extended workpiece coordinate system (G54.1

to G54.60) can be set/changed from the beginning of the program. In the absolute (G90) mode,

the specified compensation amount becomes the new compensation amount; in the incremental

(G91) mode, the currently set compensation amount is added to the specified compensation

amount to become the new compensation amount.

Command Format

G10 L20 Pp_ IP_

Parameter

Meaning

The specified code p of the workpiece coordinate system of the

workpiece origin offset value: 1 to 60, corresponding to the X

value in the G54.X coordinate system;

The workpiece origin offset of axis in absolute mode； It will be

added to the original offset of the workpiece origin of axis in

incremental mode.

Example

%1003

G54 ； G54 initial value

G01X0Y0Z0

G90G10L20P1X50Y50Z50 ； G54.1 workpiece coordinate system zero is changed to

(50,50,50) in absolute mode.

G11

G01X20Y20Z20 ； The command value of the machine coordinate system is (70, 70, 70)

G91G10L20P1X50Y50Z50 ； G54.1 workpiece coordinate system zero is changed to

(100,100,100) in incremental mode.

G11

G90G01X20Y20Z20 ； The command value of the machine coordinate system is (120, 120,

120)

M30

13.4

System Parameter Data Output

Function and Purpose



System parameters is output to the current channel variable specified by Rr, #0～#49

Command Format

G10 L53 Pp__Rr_

Parameter

Meaning

Parameter ID index number

Variable address（#0～#49）

Example

%1004

G54

G01X0Y0Z0

G10L53P010340R1

； Read the value of machine user parameter 010340 and assign it to

variable #1

G10L53P010341R2

； Read the value of machine user parameter 010341 and assign it to

variable #2

G11

M30

13.5

Milling Tool Length Compensation Data Input

Function and Purpose



With the G10 command, the milling tool length compensation can be set or changed in the

program. In the absolute (G90) mode, the specified compensation amount becomes the new

compensation amount; in the incremental (G91) mode, the currently set compensation amount is

added to the specified compensation amount to become the new compensation amount.

Command Format

G10 L10 Pp_ Rr_

Parameter

Meaning

Tool offset number

Tool compensation data

Example

%0005

G54

G01X100Y100Z100

G90G10L10P1R2 ；No.1 tool length compensation is changed to 2 in absolute mode

G11

G43Z50H1 ；H1=2

G49Z0

G91G10L10P1R8 ；No.1 tool length compensation is changed to（8+2=10）in incremental

mode

G11

G90G43Z50H1 ；H1=10

G49Z0

M30

Note

If the tool length compensation is changed with G10, the tool length compensation needs to be

called again with G43 or G44 to take effect.

13.6

Milling Tool Radius Compensation Data Input

Function and Purpose



With the G10 command, the milling tool radius compensation can be set or changed in the

program. In the absolute (G90) mode, the specified compensation amount becomes the new

compensation amount; in the incremental (G91) mode, the currently set compensation amount is

added to the specified compensation amount to become the new compensation amount.

Command Format

G10 L12 Pp Rr

Parameter

Meaning

Tool offset number

Tool compensation data

Example

%0006

G54

G01X100Y100Z100

G10L12P2R1 ；No.2 tool radius compensation is changed to 1 in absolute mode

G11

G41X20Y20D2 ；D2=1

X30

G40X0Y0

G91G10L12P2R1 ； No.2 tool radius compensation is changed to (1+1=2) in incremental

mode

G11

G90G41X20Y20D2 ；D2=2

X30

G40X0Y0

M30

Note

If the tool radius compensation is changed with G10, the tool radius compensation needs to be

called again with G41 or G42 to take effect.

13.7

Lathe Tool Offset Data Input

Function and Purpose



With the G10 command, the lathe tool compensation, wear, tool nose offset can be set or changed.

In the absolute (G90) mode, the specified compensation amount becomes the new compensation

amount; in the incremental (G91) mode, the currently set compensation amount is added to the

specified compensation amount to become the new compensation amount.

Command Format

G10 L14 Pp X_ Z_ R_ Q_ Y_ J_ K_

Parameter

Meaning

Tool offset number

Tool compensation data X

Tool compensation data Z

Tool nose radius compensation value R

Imaginary tool nose direction

Tool compensation data Y

Tool radial wear J

Tool axial wear K

Example

Modify the tool offset data of No. 1 in the tool offset table (for example, X axis offset is -100, Z

axis offset is -50, tool nose radius is 0.2, tool nose position number is 3) and call this tool offset:

%1007

G10L14P1X-100Z-50R0.2Q3

G11

T0101

……

M30

13.8

Get and Modify Single Cutting Time

Function and Purpose



The single cutting time on the main processing interface can be modified with G10L78.

Description



P parameter specifies the modified single processing time, unit: second

After modifying the "single cutting time", the "this cutting time" and "cumulative cutting time"

are updated simultaneously.

Example

%0008

G54

G01X100Y100Z100

G10L78P60； The single cutting time is changed to 60S

G10L78P1000； The single cutting time is changed to 1000S

G11

M30

Note

#1471: The current "single cutting" time can be read, but it is best to add G08 command to pause

the read-ahead, otherwise the read time may not be accurate;

14 Standard Canned Cycle of Lathe（T）

14.1

Simple Cycle of Lathe

There are five simple cycles for lathe system,

Function

command

G80

Innter (outer) diameter cutting cycle

G81

End face cutting cycle

G82

Thread cutting cycle

G74

End face deep-hole drilling cycle

G75

Outer diameter grooving cycle

For the cycle in this chapter, a G code block is used to complete the processing operation of

multiple block commands, so that the program can be simplified

Note

1) The cycles described in this chapter can only be used for lathe system.

2) The command format cannot be used for FANUC system.

14.1.1 Inner (Outer) Diameter Cutting Cycle

Function and Purpose



With this function, the operation control of 4 linear trajectories can be realized through one block.

The trajectory starts from the starting point A, and returns to the starting point A by

A→B→C→D→A, and finally completes a simple cycle processing, in which the the first and the

forth trajectories are the rapid traverse movements, and the second and the third trajectories are

movements at processing speed. The trajectories are shown in the figure below.

This function is suitable for simple inner or outer diameter cutting cycle.

1. Inner/Outer diameter cutting cycle of cylindrical surface

Tool retraction point

Cycle start point

Cutting end point

Cutting start point

2. Inner/Outer diameter cutting cycle of conical surface

Command Format

1. Inner/Outer diameter cutting cycle of cylindrical surface

G80 X_/U_ Z_/W_ F_

Parameter

Meaning

X/U Z/W

The coordinates of end point C in workpiece coordinate system in

absolute mode; the directional distance from cutting end pint C to the

cycle start point A in incremental mode, which is represented in U

and W in the diagram, and the sign is determined by the directions of

path 1 and path 2.

Feedrate (mm/min)

2. Inner/Outer diameter cutting cycle of conical surface

G80 X_/U_ Z_/W_ I_F_

Parameter

Meaning

X/U Z/W

The coordinates of end point C in workpiece coordinate system in

absolute mode; the directional distance from cutting end pint C to the

cycle start point A in incremental mode, which is represented in U and W

in the diagram, and the sign is determined by the directions of path 1 and

path 2.

The radius difference between the cutting start point B and the cutting

end point C (the sign of I determines the reverse taper or the forward

taper).

Feedrate (mm/min)

Example

Example 1: Machining the workpiece as shown in the figure below with G80 command to rough and

finish simple conical parts.

%3320

N1 T0101

N2 M03 S460

N3 G00 X90Z20

N4 X40 Z3

N5 G80 X31 Z-50 F100

N6 G80 X30 Z-50 F80

N7 G00X90 Z20

N8 M30

14.1.2 End Face Cutting Cycle (G81)

Function and Purpose



With this function, the operation control of 4 linear trajectories can be realized through one block.

The trajectory starts from the starting point A, and returns to the starting point A by

A→B→C→D→A, and finally completes a simple cycle processing, in which the the first and the

forth trajectories are the rapid traverse movements, and the second and the third trajectories are

movements at processing speed. The trajectories are shown in the figure below.

This cycle is suitable for flat face cutting and taper face cutting.

1. Flat face cutting

Cutting path A→B→C→D→A

Cutting start

point

Cycle start

point

Tool retraction

Cutting end point

point

2. Taper face cutting

Cutting path A→B→C→D→A

Command Format

1. Flat face cutting

G81 X_/U_ Z_/W_ F_

Parameter

Meaning

X/U Z/W

The coordinates of end point C in workpiece coordinate system in absolute

mode; the directional distance from cutting end pint C to the cycle start

point A in incremental mode, which is represented in U and W, and the

sign is determined by the directions of path 1 and path 2.

Feedrate (mm/min)

2. Taper face cutting

G81 X_/U_ Z_/W_ K_ F_

Parameter

Meaning

X/U Z/W

The coordinates of end point C in workpiece coordinate system in absolute

mode; the directional distance from cutting end pint C to the cycle start point

A in incremental mode, which is represented in U and W, and the sign is

determined by the directions of path 1 and path 2.

The directional distance along Z from cutting start point B to cutting end

point C.

Feedrate (mm/min)

Example

Process the workpiece as shown in the figure below with G81 command, and the dotted line

represents the blank.

%3323

N1 T0101 ; Set coordinate system and select No.1 tool

N2 G00 X60 Z45

; Move to the cycle start position

N3 M03 S460

; Spindle rotation CW

N4 G81 X25 Z31.5 K-3.5 F100

; The first cycle, the cutting depth is 2mm

N5 X25 Z29.5 K-3.5

; The cutting depth is 2mm each time

N6 X25 Z27.5 K-3.5

;

The starting point of each cutting is 3mm away from

the outer surface of the workpiece, so the K value is -

3.5

N7 X25 Z25.5 K-3.5

; The forth cycle, the cutting depth is 2mm

N8 M05

; Spindle stops

N9 M30

; Main program end, and reset

Note

(1) If no F value is specified, it will cut at the default speed.

(2) The end face cutting requires special tools for end face cutting

(3) This canned cycle automatically recognizes diameter programming and incremental

programming, no need to switch modes specifically

(4) Before running this program, the spindle must be rotated.

(5) This program can be executed with tool compensation.

14.1.3 Thread Cutting Cycle（G82）

Function and Purpose



1. Straight thread cutting cycle

The cutting path A→B→C→D→A

2. Taper thread cutting cycle

The cutting path A→B→C→D→A

Command Format

G82 X_/U_ Z_/W_ I_ R_ E_ C_ P_ F_

Parameter

Meaning

X/U Z/W

The coordinates of end point C in workpiece coordinate system in absolute

mode; the directional distance from cutting end pint C to the cycle start point

A in incremental mode, which is represented in U and W in the diagram.

It is the radius difference between the thread start point B and the thread end

point C. Its sign is the sign of the difference

(no matter it is absolute

programming or incremental programming). This parameter can be omitted for

straight thread.

R E

The undercut amount for thread cutting. R and E are both vectors, R is the Z-

direction retraction amount; E is the X-direction retraction amount. R and E

can be omitted, indicating that the retraction function is not required

Number of thread starts. When it is 0 or 1, it indicates the single-start thread.

For single-start thread cutting, it is the spindle rotation angle of the spindle

reference pulse from the cutting start point (default value is 0); for multi-start

thread cutting, it is the corresponding spindle rotation angle between the

cutting start points of adjacent thread starts.

Thread lead; (mm/r)

Example

As shown in the figure below, the workpiece is programmed with G82, and the blank shape has

been processed.

%3324

N1 G54 G00 X35 Z104

;

Select coordinate system G54, move to cycle start point

N2 M03 S300

;

Spindle rotates at 300r/min

N3 G82 X29.2 Z18.5 C2 P180 F3

;

The first cycle for thread cutting, the cutting depth is

0.8mm

N4 X28.6 Z18.5 C2 P180 F3

;

The second cycle for thread cutting, the cutting depth is 0.6mm

N5 X28.2 Z18.5 C2 P180 F3

;

The third cycle for thread cutting, the cutting depth is 0.4mm

N6 X28.04 Z18.5 C2 P180 F3

; The forth cycle for thread cutting, the cutting depth is 0.16mm

N7 M30

; Spindle stops, main program end, and reset

Note

(1) If the retraction function is required, please note that the signs of the R and E values must be

coordinated with the thread cutting direction. Retraction in the opposite direction of thread

processing may damage the thread. At the same time, only R can be specified without specifying

E, but if E is specified, R must be specified. When R and E are zero, the undercut amount is forced

to F×0.68;

(2) The thread cutting cycle is the same as the G32 thread cutting. In the feed hold state, the cycle

will stop after completing all actions;

(3) The override cannot be changed at the time of thread cutting;

(4) F value can be inherited, if there is no value to inherit, it will alarm;

(5) The 90-degree undercut is #54019 in the user-defined macro variable.

14.1.4 End Face Deep-hole Drilling Cycle（G74）

Function and Purpose



This cycle can perform deep hole drilling on the end face. As shown in the figure below.

The tool path A→B→C→D→A

Command Format

G74 X_/U_Z_/W_ Q(△K)_R(e)_ I(i)_P(p)_

Parameter

Meaning

X/U

The coordinates of end point of hole bottom on X in workpiece coordinate

system in absolute programming; in incremental programming, the directional

distance from end point of hole bottom to the cycle start point, which is

represented by U in the graph. This value can be left blank.

Z/W

The coordinates of end point of hole bottom on Z in workpiece coordinate

system in absolute programming; in incremental programming, the directional

distance from end point of hole bottom to the cycle start point, which is

represented by W in the graph.

Undercut amount on Z, can only be positive, and can be left blank.

Feed depth, can only be positive.

The width of each cut when drilling a wide hole, can only be positive, and can

be left blank.

Retract amount on X. When I is specified, P can only be positive; when I is not

specified, P can be both positive and negative, and can be left blank.

Description



Blank length: 406.1, radius 120.0, scaling 1.748

As shown in the figure above, it is the drilling trajectory of G74. Each time after drilling into the

bottom of the hole, it moves Q distance in the X direction and then drills again until the remaining

width in the X direction is less than Q, then completes the X axis movement, and drills finally so

as to achieve the drilling of a fixed width hole.

Example

%1234

T0101

M03S500

G01 X0 Z10F200

G74 X-10Z-60R1Q5I3P1

M30

Note

(1) Modal inheritance is not supported. If the following lines of G74 are XZ coordinates, the

program will not continue drilling, but o run the coordinates with G01.

(2) If need to drill continuously, user needs to write multiple lines of G74 continuously, and

commands such as RQIP will not be inherited.

(3) Clockwise drilling and counterclockwise drilling are supported.

(4) Pay attention to selecting appropriate speed values (including dry run). Even for the virtual

pattern in the dry run, the system will display the actual tool path when the speed is too fast. When

the speed is adjusted to a high level in dry run, the drilling pattern will be distorted.

(5) Pay attention to the width of the tool at the time of wide groove cutting.

14.1.5 Outer Diameter Grooving Cycle (G75)

Function and Purpose



This cycle is used for grooving the outer diameter of the workpiece.

Command Format

G75X_/U_Z_/W_ Q(△K)_R(e)_ I(i)_P(p)_

Parameter

Meaning

X/U

The coordinates of end point of hole bottom on X in workpiece coordinate

system in absolute programming; in incremental programming, the

directional distance from end point of hole bottom to the cycle start point,

which is represented by U in the graph.

Z/W

The coordinates of end point of hole bottom on Z in workpiece coordinate

system in absolute programming; in incremental programming, the

directional distance from end point of hole bottom to the cycle start point,

which is represented by W in the graph.

Retract amount on X, can only be positive, and can be left blank.

Feed depth, can only be positive.

Groove width, can only be positive, and can be left blank.

Undercut amount on Z. When I is specified, P can only be positive; when I

is not specified, P can be both positive and negative, and can be left blank.

Example

Example 1: G75 outer diameter grooving cycle programming example.

%1234

T0101

M03S500

G01 X50 Z-50F200

G75 X10Z-40R1Q5I3P2

M30

Note

(1) If K is not defined, user macro #54005 needs to be set as the tool retraction amount.

(2) If Q is not defined, the Q in the previous line will be inherited. If Q is not defined in the first

line, then Q will be 0.

(3) If R is not defined, then R is 0 by default.

(4) Modal inheritance is not supported. If the following lines of G75 are XZ coordinates, the

program will not continue drilling, but to run the coordinates with G01.

(5) If need to drill continuously, user needs to write multiple lines of G75 continuously, and

commands such as RQIP will not be inherited.

14.2

Drilling Canned Cycle for Lathe System

There are four drilling cycles for lathes system:

G command

Function

G83

Axial drilling cycle

G87

Radial drilling cycle

G84

Axial rigid tapping cycle

G88

Radial rigid tapping cycle

With this cycle, a block containing G code is used to complete the machining operations with

multiple block commands, so that the program can be simplified.

Note

(1) Cycles described in this chapter only can be used for lathe system.

(2) Commands G83, G87, G84, and G88 do not have positioning function. It is necessary to use

G01 and G00 outside the canned cycle for positioning.

14.2.1 Axial Drilling Cycle（G83）/Radial Drilling Cycle（G87）

Function and Purpose



Turning centers with powered tool often require axial or radial hole processing. The G83

command of this system can be used to drill axial holes; G87 can be used to drill radial holes. For

the two processing methods, there only is the difference in the feed axis, and the drilling trajectory

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

axis.

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

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

workpiece can be installed on the tool holder to perform the Z-axis feed movement, thereby

realizing the axial drilling.

Command Format

1. Axial drilling cycle

G83Z(W)_R_Q_K_P_F_H_

2. Radial drilling cycle

G87X(U)_R_Q_K_P_F_H_

Parameter

Meaning

X/Z

Coordinates of hole bottom

Distance from initial level to R level

Cutting depth

Dwell time at the hole bottom

Feedrate

Retraction distance

High speed deep hole drilling. Retraction of the specified

distance K

Deep hole drilling. Retraction to R point

Spot drilling. Drill directly to the hole bottom

Description



According to the different technological requirements of drilling process, this function sets three

kinds of drilling cycle trajectories, namely conventional hole drilling, high speed deep hole

drilling, and deep hole drilling. The three modes are set by H1, H2, H3 respectively.

H1 is set as high-speed deep hole drilling, chip breaking needs to be taken into consideration, and

the chip removal effect is not very good;

H2 is set as deep hole drilling, chip breaking and chip removal need to be taken into consideration;

H3 is set as conventional hole drilling, which is mainly suitable for shallow hole processing,

without considering chip removal and chip breaking.

 High-speed deep hole drilling --- H1 mode

Initial level

Point R

Point Z/X

G83 or G87 (G98)

G83 or G87 (G99)

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

 The retraction amount K is small after drilling each time. Chip breaking can be

achieve, and chip removal effect is not very good.

 Deep hole drilling - H2 mode

Initial level

Point R

Initial level

Point Z./X

G83 or G87 (G98)

G83 or G87 (G99)

HNC8 Series CNC Controller. Programming Manual (V2.4) - page 5