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

Content

Introduction _____________________________________________________________________ i

Content __________________________________________________________________________ ii

1 Overview __________________________________________________________________________7

1.1

Coordinate Axis _________________________________________________________________________ 7

1.1.1 Machine Coordinate Axis _________________________________________________________________ 7

1.1.2 CNC Control Axis _________________________________________________________________________ 7

1.2

Reference Point, Machine Origin, and Machine Coordinate System _____________________ 9

1.3

Workpiece Origin and Workpiece Coordinate System _________________________________ 10

1.4

Coordinate System and Travel _________________________________________________________ 10

1.5

Positional Relationship between Coordinate Systems __________________________________11

1.7

General Programming Methods and Steps _____________________________________________12

2 Program Format and Structure _________________________________________________ 13

2.1

Program Format ________________________________________________________________________13

2.1.1 Address and Command Word ___________________________________________________________13

2.1.2 Block and Block Number ________________________________________________________________15

2.1.3 General Structure of Program ___________________________________________________________16

2.1.4 File Attributes of Program _______________________________________________________________ 16

2.1.5 Program and Program Name____________________________________________________________17

2.1.6 Optional Block Skip ______________________________________________________________________18

2.2

Main Program and Subprogram _______________________________________________________18

2.3

Cautions before Machining_____________________________________________________________ 20

3 Preparatory Function (G Code) _________________________________________________ 21

3.1

G Code Modal and Grouping __________________________________________________________21

3.2

List of G codes (T) ______________________________________________________________________21

3.3

List of G codes (M) _____________________________________________________________________23

4 Auxiliary Function _______________________________________________________________ 26

4.1

M Command ___________________________________________________________________________ 26

4.1.1 Default Auxiliary Function of CNC _______________________________________________________28

4.1.2 Auxiliary Function Set by PLC ____________________________________________________________31

4.2

Table of M Command Function and Regular Status ____________________________________ 32

5 Spindle Function ________________________________________________________________ 35

5.1

Spindle Speed Setting __________________________________________________________________35

5.2

Constant Linear Speed Cutting Control（G96/G97

（T） _____________________________36

5.3

Spindle Clamping Speed _______________________________________________________________38

5.4

C/S-Axis Switching（CTOS/STOC）____________________________________________________39

5.5

Spindle Orientation_____________________________________________________________________40

5.6

Spindle Synchronization Control（G146/G147） ______________________________________41

6 Tool Function ___________________________________________________________________ 46

6.1

T Command in Lathe System ___________________________________________________________ 46

6.2

T Command in Milling System__________________________________________________________ 49

7 Feed Function ___________________________________________________________________ 52

7.1

Overview _______________________________________________________________________________52

7.2

Feedrate Setting ________________________________________________________________________ 53

7.2.1 Rapid Traverse Speed ___________________________________________________________________ 54

7.2.2 Cutting Feedrate_________________________________________________________________________55

7.2.3 2nd Feedrate ____________________________________________________________________________58

7.3

Feed Control Mode_____________________________________________________________________ 58

7.4

Feedrate Control _______________________________________________________________________ 61

8 Position Command Function ___________________________________________________ 65

8.1

Mode I of Absolute Command and Incremental Command（G90/G91） _____________65

8.2

Mode II of Absolute Command and Incremental Command （X, Z/U, W）（T） ______67

8.3

Diameter Programming and Radius Programming（G36/G37

（T） _________________69

8.3

Inch/Metric（G20/G21） _______________________________________________________________71

9 Delay Function __________________________________________________________________ 73

9.1

Delay Function _________________________________________________________________________ 73

Coordinate System ___________________________________________________________ 75

10.1

Overview ______________________________________________________________________________ 75

10.2

Machine Coordinate System __________________________________________________________76

10.3

Workpiece Coordinate System ________________________________________________________ 78

10.3.1 Workpiece Coordinate System Setting (G92) ___________________________________________ 78

10.3.2 Workpiece Coordinate System Selection G54～G59（G54.X） ________________________ 80

10.3.3 Extended Workpiece Coordinate System Selection（G54.x） __________________________81

10.3.4 Workpiece Coordinate System Modification (G10) _____________________________________82

10.4

Local Coordinate System Setting (G52) _______________________________________________83

10.5

Coordinate Plane Selection（G17，G18，G19） _____________________________________86

10.6

Machine Origin and 2nd, 3rd, 4th, and 5th Reference Points _________________________87

10.7

Reference Point Return (G28/G29) ____________________________________________________88

10.8

2^nd, 3^rd, 4^th,5^th Reference Point Return (G30) ____________________________________________ 91

Interpolation Function________________________________________________________ 94

11.1

Positioning (G00) ______________________________________________________________________94

11.2

Unidirectional Positioning (G60) ______________________________________________________97

11.3

Linear Interpolation (G01) _____________________________________________________________99

11.4

Circular Interpolation（G02/G03） _________________________________________________ 102

11.5

3D Circular Interpolation（G02.4/G03.4） __________________________________________ 107

11.6

Thread Cutting（G32）（T） ________________________________________________________ 109

11.7

Helical Interpolation（G02/G03） __________________________________________________ 112

11.8

Imaginary Axis Specifying and Sine Interpolation (G07) _____________________________ 114

iii

11.9

Polar Coordinate Interpolation（G12/G13） _______________________________________ 116

11.10

Cylindrical interpolation（G07.1）_________________________________________________ 121

11.11

Polar Coordinate Command（G15/G16）_________________________________________ 124

11.12

NURBS Spline Interpolation ________________________________________________________ 130

11.13

HSPLINE Spline Interpolation ______________________________________________________ 132

Tool Compensation Function________________________________________________

135

12.1

Turning Tool offset Compensation（T）____________________________________________ 135

12.2

Turning Tool Nose Radius Compensation（G40/G41/G42）（T） __________________ 138

12.3

Milling Tool Length Compensation（M） __________________________________________ 144

12.4

Milling Tool Radius Compensation（G40/G41/G42

（M） ________________________ 153

12.5

Detailed Explanation of Tool Radius Compensation ________________________________ 157

12.5.1 Tool Radius Compensation Action ___________________________________________________ 157

12.5.2 Tool Radius Compensation Action Diagram__________________________________________ 159

12.5.3 Compensation Direction Change During Tool Radius Compensation ________________ 165

12.5.4 When Tool Radius Compensation is not Executed ___________________________________ 167

12.5.5 There is a Block without movement in Tool Radius Compensation___________________ 169

12.5.6 Action Insertion in Tool Radius Compensation _______________________________________ 171

12.5.7 Change of Compensation Value in Tool Radius Compensation ______________________ 172

12.5.8 Interference Check ___________________________________________________________________ 173

Programmable Data Input（G10/G11） ____________________________________

176

13.1

Programmable Data Input Command（G10/G11） ________________________________ 176

13.2

Workpiece Coordinate System Origin Input_________________________________________ 176

13.3

Extended Workpiece Coordinate System Origin Data Input ________________________ 177

13.4

System Parameter Data Output _____________________________________________________ 178

13.5

Milling Tool Length Compensation Data Input ______________________________________ 179

13.6

Milling Tool Radius Compensation Data Input ______________________________________ 180

13.7

Lathe Tool Offset Data Input ________________________________________________________ 181

13.8

Get and Modify Single Cutting Time ________________________________________________ 182

Standard Canned Cycle of Lathe（T） ______________________________________

183

14.1

Simple Cycle of Lathe _______________________________________________________________ 183

14.1.1 Inner (Outer) Diameter Cutting Cycle ________________________________________________ 183

14.1.2 End Face Cutting Cycle (G81) ________________________________________________________ 187

14.1.3 Thread Cutting Cycle（G82） ________________________________________________________ 189

14.1.4 End Face Deep-hole Drilling Cycle（G74） __________________________________________ 192

14.1.5 Outer Diameter Grooving Cycle (G75) _______________________________________________ 194

14.2

Drilling Canned Cycle for Lathe System _____________________________________________ 197

14.2.1 Axial Drilling Cycle（G83）/Radial Drilling Cycle（G87）____________________________ 197

14.2.2 Axial Rigid Tapping Cycle (G84)/ Radial Rigid Tapping Cycle (G88) __________________ 202

14.3

FANUC Mode of Lathe System ______________________________________________________ 204

Canned Cycle for Milling System (M) _______________________________________

207

15.1

Standard Canned Cycle for Milling System__________________________________________ 207

15.2

High-speed Deep-hole Drilling Cycle（G73）______________________________________ 212

15.3

Reverse Tapping Cycle（G74） _____________________________________________________ 216

15.3.1 Reverse Tapping Cycle _______________________________________________________________ 216

15.3.2 Reverse Peck Tapping Cycle__________________________________________________________ 217

15.4

Fine Boring（G76） _________________________________________________________________ 221

15.5

Drilling Cycle (Center Drills)（G81） ________________________________________________ 225

15.6

Drilling Cycle with Pause（G82） ___________________________________________________ 228

15.7

Deep Hole Drilling Cycle (G83) ______________________________________________________ 230

15.8

Tapping Cycle (G84) ________________________________________________________________ 233

15.8.1 Tapping Cycle（G84） _______________________________________________________________ 234

15.8.2 Peck Tapping Cycle (G84) ____________________________________________________________ 235

15.9

Boring Cycle (G85) __________________________________________________________________ 238

15.10

Boring Cycle (G86) _________________________________________________________________ 241

15.11

Reverse Boring Cycle (G87) ________________________________________________________ 244

15.12

Boring Cycle (Manual) (G88) _______________________________________________________ 247

15.13

Boring Cycle (G89) _________________________________________________________________ 250

15.14

Drilling Canned Cycle Cancel (G80) ________________________________________________ 252

Extended Canned Cycle（M） ______________________________________________

254

16.1

Extended Canned Cycle (M) _________________________________________________________ 254

16.2

Engraving Canned Cycle (G1025) ___________________________________________________ 254

16.3

Drilling Type ________________________________________________________________________ 259

16.3.1 Circumferential Hole Drilling Cycle (G70)_____________________________________________ 259

16.3.2 Circular Hole Drilling Cycle (G71)_____________________________________________________ 263

16.3.3 Straight Line Hole Cycle (G78)________________________________________________________ 266

16.3.4 Chess Type Hole Cycle (G79) _________________________________________________________ 269

16.4

Milling Cycle ________________________________________________________________________ 272

16.4.1 Circular Groove Milling Cycle (Type 1) (G181) ________________________________________ 272

16.4.2 Circular Groove Milling Cycle (Type 2) (G182) ________________________________________ 275

16.4.3 Circumferential Groove Milling Cycle (G183) _________________________________________ 279

16.4.4 Rectangular Pocket Milling Cycle (G184) _____________________________________________ 283

16.4.5 Circular Pocket Milling Cycle (G185)__________________________________________________ 287

16.4.6 End Face Milling Cycle（G186） _____________________________________________________ 290

16.4.7 Rectangular Boss Milling Cycle (G188) _______________________________________________ 293

16.4.8 Round Boss Milling Cycle (G189) _____________________________________________________ 297

16.4.9 Milling Cycle Alarm Diagnosis ________________________________________________________ 301

Multiple Repetitive Cycle in Lathe（T） ____________________________________

306

17.1

Inner (Outer) Diameter Roughing Multiple Repetitive Cycle (G71) __________________ 306

17.2

End Face Roughing Multiple Repetitive Cycle (G72) ________________________________ 313

17.3

Closed Turning Multiple Repetitive Cycle (G73) _____________________________________ 317

17.4

Thread Cutting Multiple Repetitive Cycle (G76) _____________________________________ 321

Programming Simplifying Function (M) ____________________________________

324

18.1

Mirroring Function（G24，G25） __________________________________________________ 324

18.2

Scaling Function（G50，G51） _____________________________________________________ 330

18.3

Rotation Transformation（G68，G69） ____________________________________________ 334

User Macro and Subprogram Calling _______________________________________ 337

19.1

User Macro Program ________________________________________________________________ 337

19.1.1 Variable ______________________________________________________________________________ 337

19.1.2 Operation Command_________________________________________________________________ 346

19.1.3 Macro Statement _____________________________________________________________________ 349

19.2

Macro Program Calling _____________________________________________________________ 353

19.2.1 Argument Specification Rules ________________________________________________________ 353

19.2.2 Non-modal Call (G65)________________________________________________________________ 354

19.2.3 Calling Macro Program with G Code _________________________________________________ 355

19.2.4 Calling Macro Program with M Command ___________________________________________ 356

19.2.5 Classification of Subprogram _________________________________________________________ 359

19.2.6 Macro Program Example _____________________________________________________________ 360

19.3

Manual Calling Subprogram ________________________________________________________ 362

High-speed High-Precision Function _______________________________________ 364

20.1

Machining Optimization Function G125/G126 ______________________________________ 364

20.2

High Speed High Precision Mode Selection（M

（G05.1） ________________________ 373

20.3

High Speed High Precision Parameter Setting ______________________________________ 376

1 Overview

1.1

Coordinate Axis

1.1.1 Machine Coordinate Axis

Function and Purpose



In order to simplify programming and ensure the versatility of the program, a unified standard has

been formulated for the naming of coordinate axes and directions of CNC machine tools.

The fixed linear feed coordinate axes are represented by X, Y, Z which are referred to as the basic

coordinate axes; the coordinate axes rotating around the X, Y, and Z axes are represented by A, B,

and C which are referred to as the rotary coordinate axes.

1） Basic coordinate axes X, Y, Z

The direction of the machine tool axis depends on the type of machine tool and the layout of each

component. The relationship between the X, Y, and Z coordinate axes is determined by the right-

hand rule, as shown in Figure 1-1. In this figure, the thumb points in the positive direction of X

axis, the index finger points in the positive direction of Y axis, and the middle finger points in the

positive direction of Z axis.

+Z＇

+X +Y +Z

+X＇

+A +B

+Y＇

Figure 1-1 Machine coordinate axis

2） Rotary axis

The circular feed coordinate axes that rotate around the X, Y, and Z axes are represented by A, B,

and C respectively. According to the right-hand screw rule as shown in Figure 1-1, the thumb

points to +X, +Y, +Z directions, and the index finger and middle finger point to +A, +B, +C

directions of circular feed motion.

1.1.2 CNC Control Axis

Function and Purpose



1.2

Reference Point, Machine Origin, and Machine Coordinate System

Function and Purpose



Reference point: The machine reference point is a fixed mechanical point on the machine tool

(For some machine tools it is determined by the travel switch and dog, and for some machine tools

it is directly determined by the grating ruler zero, etc.)

Machine origin: The machine zero is a fixed point on the machine tool, and the CNC device uses

it as a reference for position control. The machine zero is determined by the reference point and

the system parameter "coordinate value of reference point in machine coordinate system".

Machine coordinate system: The machine coordinate system is the inherent coordinate system

of the machine tool. It takes the machine zero as the origin, and each coordinate axis is parallel to

the corresponding machine axis. The origin of the machine coordinate system is also called the

machine origin or machine zero. In the machine coordinate system, the workpiece is always

considered to be stationary, while the tool is considered to be moving.

Figure 1-2 shows the horizontal lathe with front tool post. Since it is a machine tool with a rotary

spindle, first user determines the Z-axis direction: the spindle axis direction is the Z-axis direction,

and the direction the tool moves away from the workpiece is the positive direction of Z-axis; then

user determines the X-axis direction: in the machining plane of the machine tool, the direction

perpendicular to the Z-axis is the X-axis direction, and the direction the tool moves away from the

workpiece is the positive direction of X-axis; At last user determines the Y-axis direction: the Y-

axis positive direction can be determined based on the right-hand Cartesian rule.

Figure 1-2 Horizontal lathe with front tool post

Figure 1-3 shows a single-column vertical milling machine (or machining center). Since it is a

machine tool with a rotary spindle, first user determines the Z-axis direction: the spindle axis

direction is the Z-axis direction, and the direction the tool moves away from the workpiece is the

Z-axis positive direction; then user determines the X-axis direction: while the operator is facing

the column and the worktable is moving, relative to the workpiece the direction of the tool moving

to the right is the X-axis positive direction; at last user determines the direction of the Y axis:

according to the right-hand Cartesian rule, the positive direction of Y-axis is the direction tool

moves to the column relative to the workpiece.

Taking the machine zero point as the origin, the coordinate system established with each axis of

the machine tool is the machine coordinate system of the machine tool.

Figure 1-3 Vertical milling machine with single column

1.3

Workpiece Origin and Workpiece Coordinate System

Function and Purpose



The workpiece coordinate system is used by the programmer during programming. The

programmer selects a known point on the workpiece as the origin (also referred to as the program

origin), and establishes a coordinate system parallel to each axis of the machine tool, which is

called the workpiece coordinate system. Once the workpiece coordinate system is established, it

will remain valid until it is replaced by a new workpiece coordinate system.

The workpiece coordinate system is determined by the programmer, and generally a position that

is convenient for processing and calculation is selected.

1.4

Coordinate System and Travel

Function and Purpose



The travel of the machine tool coordinate system is divided into effective travel and mechanical

travel. The effective travel is the range of tool movement which is set by CNC parameters; the

mechanical travel is determined by the travel switch, and its value is determined by the

manufacturer. The relationship between the machine zero (M), machine reference point (m),

workpiece coordinate origin (W), effective travel and mechanical travel of the machine coordinate

2 Program Format and Structure

2.1

Program Format

Function and Purpose



When providing information to a controller, the format specified is referred to as the program

format. The format used by the controller is referred to as the word address format.

A program is a collection of "block" units, and a "block" is used to specify a machine action

(sequence). These commands (blocks) are worked out in the order of actual tool movement. A

program block is a collection of "word" units, and a "word" is used to specify a command of an

operation. A word is a collection of characters (English letters, numbers, symbols), and the

characters are arranged in a certain order.

2.1.1 Address and Command Word

Function and Purpose



The command information used by this controller consists of letters (A, B, C...Z), and numbers

(0, 1, 2...9), and symbols (+, -, /...). These letters, numbers, and symbols are collectively referred

to as characters. What is expressed in this form is referred to as a code. This controller uses ISO

code which is written in notepad format.

Description



The initial letter of a word is referred to as the address, which defines the meaning of the following

numerical information. A command word is composed of address characters (command characters)

and numeric data with signs (such as the word with a defined dimension) or without signs (such

as the preparatory function word G code). In this controller, the word is composed of a letter

(word address) and several numbers following it. (User can also add symbols such as "-" at the

beginning of the number).

Word

For example, X153.7

Number

Letter（Word address）

Structure of word

Different command characters and the subsequent numbers in the block determine the meaning

of each command word. The main command characters contained in the CNC program block are

shown in Table 2.1.

Table 2.1 List of command characters

Function

Address

Meaning

Parts program

Letter O

Program No.：O1~4294967295

No.

Block No.

Block No.：N0~4294967295

Preperatary

Command action mode (straight line, circular arc, etc.):

function

G00 to G200

X，Y，Z

Traverse command of linear axis: ±21474

A，B，C

Traverse command of rotary axis: ±21474

Dimension word

U，V，W

Incremental programming command of lathe: ±21474

Circular radius of canned cycle

I，J，K

Coordinates of circle center relative to the starting point

for canned cycle

Feedrate

Feedrate：0 to 50000

Spindle function

Spindle speed：0 to 100000

Tool function

Tool number：0 to 99

Auxiliary

ON/OFF control at the machine side：0 to 99

function

Worktable indexing

Compensation

H，D

Tool compensation number：00 to 99

No.

Dwell

P，X

The dwell time: millisecond, second

Program No.

Sub-program number：1 to 4294967295

Repeat times

The number of repetitions of subprogram, the number of

repetitions of canned cycle

Parameter

P，Q，R

Canned cycle parameter

2.1.2 Block and Block Number

Function and Purpose



The composition of the block: A program block is composed of more than one word. A group of

single-step sequential commands or a line of several functional commands is referred to as a

program block.

Block number: the number used to distinguish each block, which is composed of address N and

the following 5 digits (1 to 99999). The block number is placed at the beginning of the block, and

can be specified in any order. Any block number can be skipped except for the block number

specified by the code command with special meaning. The block number can be specified for all

blocks, and also can be specified only for the blocks required by the program. However, for

convenience, in general the block number is specified in the order of processing steps.

Descriptions



A program block defines a command line to be executed by the CNC controller. The format of

the block defines the syntax of the functional words in each block.

The structures of block number and block are as follows:

1 block (or command line)

E.g. N100 G01 X24.7 Y59.31 M03 S1000 T0101; the part underlined is the block number

A block starts with the sequence number that identifies the block (the block number can also be

absent), and ends with the block end code. In this manual, a newline indicates the end of the block.

Like a notepad, a newline character indicates the end of the line. The preliminary function

determines the content of the dimension character. In this manual, the dimension words are

represented by IP.

2.1.3 General Structure of Program

Function and Purpose



A program of parts is executed in the order of the block line, not in the order of the block number,

but it is recommended to write the block number in ascending order when writing the program.

Description



Program start: The first cell of the first line cannot be numbers or symbols other than "%".

Program end: the program end code is usually specified at the end of the program, and one of the

following codes is to indicate the program end code.

Code

Meaning

M02

End of main program

M30

M99

End of subprogram

Comment symbol: the content bracketed () or after the semicolon ";" is the comment text.

Single line command: When writing the processing G code program, some commands must be

written in a single line. Such as M30, M02, M99, M6T, CTOS, STOC, G16, G15, G05.1, G04.

2.1.4 File Attributes of Program

Function and Purpose



User can set the access attribute for the file program to be writable or readable.

Description



Editing prohibited: The current loader can be set to "read-only" through interface operations. At

this time, the file cannot be rewritten until it is set to "writeable" through interface operations.

In addition, user can also control the access properties of the program through the key switch of

the project panel, but this key switch is effective on all programs in the program manager, that is,

when the switch is turned off, all programs will become read-only until the switch is turned on.

2.1.5 Program and Program Name

Function and Purpose



Program: A parts program is composed of several blocks that follow certain structure, syntax and

format rules, and each block is composed of several command words. The program name

corresponds to each workpiece, or is a number to classify programs in the unit of subprogram. The

program name is a number used to distinguish each program. Use the address "O" (capital letter

O) and the following number or letter to specify.

The newly created program name on the system can be up to 7 numbers or letters; the system can

read the program name created externally with greater than 7 characters.

Description



This system calls the program by calling the program name for processing or editing.

Block No.

The starting position

Comment

Program end

If the program end code is executed during the program execution, the CNC ends the program

execution and goes into the reset state. When the subprogram end code is executed, the control

returns to the main program that calls the subprogram.

Note

If the Optional Skip switch on the machine operation panel is turned on, for example,

/M02;

/M30;

/M99; Not considered to be the end of the program.

2.1.6 Optional Block Skip

Function and Purpose



This function means that the block after the "/" (slash) code in the processing program can be

selectively ignored until the block ends.

Description



The specific function starting with the "/" symbol. It is used to choose whether the selective

processing block is executed or not.

Detailed description: When the Optional Skip switch is ON, the line codes with the symbol "/" at

the beginning of the block are skipped; when the Optional Skip switch is OFF, the line codes with

the symbol "/" at the beginning of the block are executed, and the "/" symbol does not work.

For example, when certain blocks in the program do not need to be executed under certain

circumstances, but need to be executed in another environment, this function can be used.

Note

The ON or OFF setting of the Optional Skip button on the CNC controller must be executed before

the program runs.

The special "/" symbol for optional skip must be at the beginning of the block. (If it is inserted in

the middle of the block, it is used as a division operation command of the user macro)

Example: N30 G1 X15/Y5; error, illegal symbol alarm

/N30 G1 X15 Y5; correct

2.2

Main Program and Subprogram

Function and Purpose



When a same processing mode appears multiple times in a program, this mode can be edited into

a program for repeated calling to simplify the program. Such a program is referred to as a

subprogram, and the original program is referred to as the main program. The call of the

subprogram is performed with M98 or G65 command, and the return from the subprogram is

performed with M99 command. Refer to the chapter of user macro program for the specific

subprogram calling of G65.

The subprogram can be called repeatedly up to 999 times. User can also call other subprograms

in a subprogram, and up to 6 layers are supported.

Description



Structure of calling subprogram:

Times the subprogram

Subprogram No.

is called repeatedly

When L is not specified, that means the repetition times is

not specified, and the subprogram can only be called once

When a call to subprogram execution command occurs during the execution of the main program,

the subprogram command is executed. When the subprogram is executed, return to the main

program to continue the execution.

Main program:

O01

Subprogram:

O10

Subprogram:

O20

Subprogram:

O30

Special usage of M99: when it is used as the main program end command, return to the main

program head to execute the program again.

There are two forms to call subprogram:

1) The subprogram is placed after the main program, that is, after the end of the program (M30 or

M02). The program number called can start with % or the letter O;

2) When the subprogram is used as a separate program, it should be placed in the same disk

(system disk or USB disk) as the main program.

Note

1) In both forms, the subprogram placed after the main program has priority, that is, the first case

is prior to the second case.

2) When calling a subprogram, the name of the subprogram cannot have a suffix, otherwise the

alarm "File not loaded" is issued.

3) The subprogram cannot be executed in MDI, otherwise the alarm will be issued. "MDI cannot

call external subprograms".

When the main program calls a subprogram, it is regarded as a first layer of subprogram, and the

called subprogram can also call another subprogram. The depth can reach up to 6 layers, as shown

below:

Subprogram:

O10

O20

O30

Subprogram structure nesting

2.3

Cautions before Machining

Caution

When creating a processing program, please select appropriate processing

conditions and be careful not to exceed the performance, capacity, and limitations

of the machine and NC. We do not take the above processing conditions into

consideration for the cases mentioned in this manual.

Please perform dry run before actual machining to confirm the machining program,

tool compensation amount, workpiece offset amount, etc.

3 Preparatory Function (G Code)

3.1

G Code Modal and Grouping

Function and Purpose



Modal of G code

G codes can be divided into two types according to their effective states: non-modal G codes and

modal G codes.

Non-modal G code: It is valid only when the G code is specified, and it is invalid if it is not

specified.

Modal G code: This type of G code is stored by the CNC system after it is executed once, and

remains valid until it is replaced by other codes in the same group.

Grouping of G codes

G codes are divided into several groups according to their functions. Group 00 is for non-modal

G codes, and the other groups are for modal G codes.

Description



1) Multiple G codes of different groups can be specified in the same block.

2) If multiple codes of the same group are specified in the same block, only the last specified code

is valid.

3) If the G code of group 01 is specified in the canned cycle, just like the G80 command is

specified, the canned cycle can be cancelled. But the G code of canned cycle does not affect the

code of 01 group.

3.2

List of G codes (T)

After the controller is powered on, the one marked with "【】" in the table is the initial modal

in the same group, and the one marked with "『』" is the equivalent macro name of the G code.

G code

Group No.

Function

G00

Rapid traverse positioning

【G01】

Linear interpolation

G02

Circular interpolation CW/ Helical interpolation CW

G03

Circular interpolation CCW/ Helical interpolation CCW

G04

Dwell

G07

Imaginary axis designation

G08

Read-ahead OFF

G09

Exact stop check

G10

Programmable data input

【G11】

Programmable data input cancel

G17

XY plane selection

【G18】

ZX plane selection

G19

YZ plane selection

G20

Inch input

【G21】

Metric input

G28

Reference point return

G29

Return from reference point

G30

Return from 2^nd, 3^rd, 4^th, 5^th reference points

G32

Thread cutting

【G36】

Diameter programming

G37

Radius programming

【G40】

Tool radius compensation cancel

G41

Left tool compensation

G42

Right tool compensation

G52

Local coordinate axis setting

G53

Direct machine coordinate system programming

G54.x

Extended workpiece coordinate system selection

【G54】

Workpiece coordinate system 1

G55

Workpiece coordinate system 2

G56

Workpiece coordinate system 3

G57

Workpiece coordinate system 4

G58

Workpiece coordinate system 5

G59

Workpiece coordinate system 6

G60

Unidirectional positioning

【G61】

Exact stop mode

G64

Cutting mode

G65

Macro non-modal call

G71

Inner/Outer roughing multiple repetitive cycle

G72

Face end roughing multiple repetitive cycle

G73

Close turning multiple repetitive cycle

G76

Threading cutting multiple repetitive cycle

G80

Inner/Outer diameter cutting cycle

G81

Face end cutting cycle

G82

Thread cutting cycle

G74

Face end deep-hole drilling cycle

G75

Outer diameter pocket cutting cycle

G83

Radial drilling cycle

G87

Axial drilling cycle

G84

Axial rigid tapping cycle

G88

Radial rigid tapping cycle

【G90】

Absolute programming

G91

Incremental programming

G92

Workpiece coordinate system setting

G93

Inverse time feed

【G94】

Feed per minute

G95

Feed per revolution

【G97】

Constant linear speed control ON

G96

Constant linear speed control OFF

G101

Axis release

G102

Axis acquire

G103

Command channel loader

G103.1

Command channel loader running

G104

Channel synchronization

G108

Spindle is switched to C axis

『STOC』

G109

C axis is switched to spindle

『CTOS』

G110

Alarm

G115

Rotary axis angle resolution redefining

3.3

List of G codes (M)

G code

Group No.

Function

G00

Rapid traverse positioning

【G01】

Linear interpolation

G02

Circular interpolation CW/ Helical interpolation CW

G03

Circular interpolation CCW/ Helical interpolation CCW

G04

Dwell

G05.1

High speed high precision mode

G07

Imaginary axis designation

G07.1

Cylindrical interpolation

G08

Read-ahead OFF

G09

Exact stop check

G10

Programmable data input

【G11】

Programmable data input cancel

G12

Polar coordinate interpolation ON

【G13】

Polar coordinate interpolation OFF

【G15】

Programmable data input

G16

Programmable data input cancel

【G17】

XY plane selection

G18

ZX plane selection

G19

YZ plane selection

G20

Inch input

【G21】

Metric input

G24

Mirroring ON

【G25】

Mirroring OFF

G28

Reference point return

G29

Return from reference point

G30

Return from 2^nd, 3^rd, 4^th, 5^th reference points

【G40】

Tool radius compensation cancel

G41

Left tool compensation

G42

Right tool compensation

G43

Tool length Compensation plus

G44

Tool length Compensation minus

【G49】

Tool length Compensation Cancel

【G50】

Scaling ON

G51

Scaling OFF

G52

Local coordinate system setting

G53

Direct machine coordinate system programming

G54.x

Extended workpiece coordinate system programming

【G54】

Workpiece coordinate system 1

G55

Workpiece coordinate system 2

G56

Workpiece coordinate system 3

G57

Workpiece coordinate system 4

G58

Workpiece coordinate system 5

G59

Workpiece coordinate system 6

G60

Unidirectional positioning

G61

Exact stop mode

【G64】

Cutting mode

G65

Macro non-modal call

G68

Rotation transformation enable

【G69】

Rotation transformation cancel

G73

Deep hole drilling cycle

G74

Reverse tapping cycle

G76

Fine boring cycle

【G80】

Canned cycle cancel

G81

Center drilling cycle

G82

Drilling cycle with pause

G83

Deep hole drilling cycle

G84

Tapping cycle

G85

Boring cycle

G86

Boring cycle

G87

Back boring cycle

G88

Boring cycle (manual)

G89

Boring cycle

G181

Circular groove cycle (type 1)

G182

Circular groove cycle (type 2)

G183

Circumferential groove milling cycle

G184

Rectangular pocket cycle

G185

Circular pocket cycle

G186

Face end milling cycle

G188

Rectangular boss cycle

G189

Circular boss cycle

【G90】

Absolute programming

G91

Incremental programming

G92

Workpiece coordinate system setting

G93

Inverse time feed

【G94】

Feed per minute

G95

Feed per revolution

【G98】

Start point return of canned cycle

G99

Reference point return of canned cycle

G101

Axis release

G102

Axis acquire

G103

Command channel loader

G103.1

Command channel loader running

G104

Channel synchronization

G106

Measurement data record and export

G108

Spindle is switched to C axis

『STOC』

G109

C axis is switched to spindle

『CTOS』

G110

Alarm

G115

Rotary axis angle resolution redefining

NURBS

NURBS spline interpolation

HSPLINE

HSPLINE spline interpolation

Note

After the controller is powered on, the one marked with "【】" in the table is the initial modal

in the same group, and the one marked with "『』" is the equivalent macro name of the G code.

During the operation, if a code not included in the G code is specified, a program error (alarm

code) will occur.

4 Auxiliary Function

4.1

M Command

Function and Purpose



The auxiliary function code is composed of the address word M and the following numbers. It

is mainly used to control the parts program and auxiliary functions such as various auxiliary

switch actions of the machine tool. Among them, M00, M01, M02, M30, M92, M93, M98, M99

are used to control the parts program. They are default auxiliary functions defined by CNC, are

not determined by the machine tool manufacturer and unrelated to the PLC program. Other M

codes are used for auxiliary switch actions of the machine tool, and their functions are not

determined by the CNC, but specified by the PLC program, so the codes may vary with different

machine tool manufacturers. The functions provided in this manual are conventional definitions.

The specific conditions are subject to the machine description.

Description



Pre and post attributes for M code

When the M function is specified in the same block as the traverse command, the execution

sequence of the M command may be pre, post, and synchronous.

Pre function: The M function is executed before the axis movement programmed in the block.

Post function: The M function is executed after the axis movement programmed in the block.

Synchronous function: The M function is executed simultaneously with the axis movement

programmed in the block.

In the parameter configuration of this system, the M code table can be set to take effect in three

ways: pre, post, and synchronous. Which state is applicable depends on the machine

specifications.

(Note 1) The activation modes of M codes M00, M01, M02, M05, M30, M92, and M93 that are

not displayed in the list are fixed and cannot be modified.

(Note 2) The M code that is set or defaulted to the post should not be specified together with the

traverse command. It is better to be specified in a line separately, otherwise errors of some M

codes may occur.

Multiple M command specification instructions

Usually only one M code is valid for a block. In this system, at most 4 M codes can be specified

in a block. When users need to specify multiple M codes in a block, please note the following:

(1) Up to 4 M codes can be specified in a block, and multiple M codes in the same group are

regarded as one.

(2) When multiple M codes of the same group are designated in a block, the last M code in the

block is effective.

(3) When multiple different groups of M codes are designated in a block, the M codes in the

block are all effective.

(4) M codes such as M00, M01, M02, M30, M99 cannot be specified together with other M

codes.

(5) M codes such as M00, M01, M02, M30, and M99 require to be specified in a separate line,

that is, the program line containing the above M codes can not only have one M code, and cannot

have other execution commands including G and T commands.

(6) The corresponding relationship between M codes and functions depends on the specific

settings of the machine tool manufacturer. See the machine tool manufacturer's manual for

details.

Note

Although multiple M codes can be specified in a block, due to the different specifications of

each machine tool and the different settings by each machine tool manufacturer, it is

recommended not to specify multiple M codes in a block at the same time, otherwise

unpredictable errors may occur.

4.1.1 Default Auxiliary Function of CNC

Function and Purpose



M00 Program dwell

When the CNC executes the M00 command, it will pause the execution of the current program

to facilitate the operator to perform operations such as tool and workpiece size measurement,

workpiece U-turn, manual speed change, etc.

During pause, the feed of the machine tool is held, and all the existing modal information

remains unchanged. User should press the CycleStart button on the operation panel for the

continued execution of subsequent program.

M00 is valid for the current program line, it is the post M function. Its post attribute is not

allowed to be modified.

M01 Optional stop

If user presses the Optional Stop button on the operation panel, when the CNC executes the M01

command, it will suspend the execution of the current program and the machine tool will be in

the feed hold state to facilitate the operator to perform the tool extension length and workpiece

size measurement, workpiece U-turn, manual speed change and other operations. During pause,

the feed of the machine tool stops, and all the existing modal information remains unchanged.

User should press the CycleStart button on the operation panel for the continued execution of

subsequent program.

If user does not activate the Optional Stop button on the operation panel, when the CNC executes

the M01 command, the program will not pause and continue to execute.

M01 is valid in the current program line, it is the post M function. Its post attribute is not allowed

to be modified.

M92 Program dwell (manual intervention)

When CNC executes M92, the program execution pauses and the machine is in feed hold state,

but the difference from M00 is that at this time user can manually intervene in each axis,

manually command its movement, and then switch to the Auto mode to continue the running of

the current program after pressing CycleStart button.

M92 can be used in the following occasions:

(1) In manual boring, when the boring tool is automatically processed to the bottom of the hole,

the machine tool stops running, and changes the working mode to "Jog". Through manual

operation, the tool can only retract after moving radially in the opposite direction of the tool

nose for a certain distance to avoid the wall of the workpiece hole. The general milling machine

can complete fine boring with this command without the need of spindle exact stop function.

Return

point B

Spindle CW

Initial point B

Reference point R

Return to

point B

Reference point R

Spindle CW

Hole bottom Z

Delay at hole bottom,

Hole bottom Z

spindle stop

(2) During manual measurement, when the user manually measures the tool or workpiece

through the dialogue interface, the CNC actually processes it as a manual measurement cycle,

and M92 is inserted in the appropriate place in the cycle to guide the user to complete the entire

measurement task. If the system executes M92 of the canned cycle, the program is paused. At

this time, the system waits for the user to switch to the "Jog" mode to command the measuring

axis to run to the measuring position, and then switches to the "auto" mode. User presses the

CycleStart button to continue the measurement cycle.

M93 Program dwell (manual intervention is disabled)

The M93 command is equivalent to the M00 command. Unlike M92, the user cannot perform

manual intervention when the program is paused with M93.

M02 End of program

M02 is in the last block of the main program. When the CNC executes the M02 command, the

spindle, feed, and coolant of the machine tool stop, and the machining ends.

If user needs to re-execute the program which has been finished its execution with M02, user

has to call the program again, or press the "rerun" key in the submenu of automatic processing,

and then presses the CycleStart button on the operation panel.

M02 is valid in the current program line. It is the post M function. Its pre and post attributes are

not allowed to be modified, and it must be specified in a separate line.

M30 Program ends and returns

The functions of M30 and M02 are basically the same, but the M30 command also has the

function of returning to the program head.

If user needs to re-execute the program which has been finished its execution with M30, just

press the CycleStart button on the operation panel again.

(Note 1) This command must be placed in a separate line to take effect.

M98/M99 Subprogram call

If the program contains a fixed sequence or frequently repeated pattern, such a sequence or

pattern can be stored as a subprogram in the memory to simplify the program.

(Note 1) The maximum number of subprogram calls (L) is 10,000 times.

(Note 2) A subprogram can be called from the main program.

(Note 3) A called program can also call another subprogram.

Structure of subprogram

%xxxx； Subprogram No.

……； Subprogram contents

M99； Subprogram returns

Subprogram call (M98)

M98 P__ L__

P__： Subprogram No. called (in Arabic numerals)

L__： The number of times the subprogram is called repeatedly

Nested call of subprogram

When the main program call a subprogram with M98, it can be regarded as a first-level of

subprogram call. The subprogram call can be nested up to 6 levels, as shown below:

(Note 1) When the main program calls a subprogram with M98, G80 must be added before M99

in the subprogram to ensure the correct operation of the program.

(Note 2) M98/M99 need to be used in a separate line (avoid being in the same line with other

commands).

Use M99 in the main program

If M99 is executed in the main program, the control returns to the beginning of the main program,

and the main program is executed from its beginning, and loops forever.

4.1.2 Auxiliary Function Set by PLC

Function and Purpose



M03/04/05 Spindle control

M03 Starts the clockwise rotation of spindle at the speed programmed (viewed from the positive

direction to the negative direction of Z axis).

M04 Starts the counterclockwise rotation of spindle at the speed programmed.

M05 Spindle stops

(Note 1) M03, M04, and M05 can mutually cancel each other.

(Note 2) The spindle can be switched from position mode to speed mode with M03/M04 instead

of G109.

M06 Tool change

M06 is used to call a tool which needs to be installed on the spindle of the machining center. When

this command is executed, the tool will be automatically installed on the spindle. For example:

M06 T01; the tool 01 will be installed on the spindle.

(Note 1) M06 is effective in the current program line.

(Note 2) M06 needs to be used in a separate line (avoid being in the same line with other

commands).

M07/08/09 Coolant control

M07 and M08 are to turn on the coolant pipeline (based on the definition of the machine tool

manufacturer).

M09 is to turn off the coolant pipe.

M64 Workpiece counting

M64 will accumulate the number of completed workpieces in the system processing statistics

M19/M20 Spindle orientation

M19 is to enable spindle orientation.

M20 is to disable spindle orientation

4.2

Table of M Command Function and Regular Status

Pre/Post/Synchronous

Function

Function is valid

remains valid

Code

Function

in the block it

until it is

Synchronous

Pre

Post

exists

canceled

○

M00

Program dwell

○

M01

Optional stop

○

M02

End of program

M03

Spindle rotation CW

○

5 Spindle Function

5.1

Spindle Speed Setting

Function and Purpose



The spindle speed can be controlled by the number specified after the address S.

In addition to running in speed mode (rotating at a certain speed), the spindle can also operate in

position mode (switching to the rotary axis for interpolation calculation).

Through the M command controlled by the PLC, the S command is processed and terminated.

Example

%1234

G92X0Y0Z20；Establish coordinate system

G00 X0 Y0 Z2；Positioned above the hole

M03S2000；CW spindle rotation

G41 G01 X20 D01 F300；Establish tool radius compensation

G03X40R10；Start the circular cutting

G03 I-40 Z-10 L5；Mill the hole in spiral

G03 I-40；Smooth the hole bottom

G03X20R10；Exit the circular cutting

G40G01X0；Cancel tool radius compensation

G0Z20；Lift the tool

M05；Spindle stops

M30；End of program

5.2

Constant Linear Speed Cutting Control（G96/G97

（T）

Function and Purpose



This function is only applicable to CNC lathe system. It adjusts the spindle speed with the

movement of the tool nose position (constant linear speed cutting control), so that the speed of the

cutting point is always a constant speed (fixed cutting speed), which improves the uniformity of

the surface.

As the tool nose is moving to the workpiece origin, the spindle speed of the machine tool is getting

higher and higher until the machine specification limit is reached, which is very dangerous.

Therefore, please be sure to set to the maximum speed limit in the spindle speed limit setting

command (G46).

Constant linear speed control when the constant speed cutting control command G96 is set to

S314m/min.

Workpiece radius: 50mm (radius value) Workpiece radius: 25mm (radius value)

Because the linear speed is constant, the spindle speed is calculated as the tool nose position moves,

and it changes automatically.

In the above example, because the linear speed (314 m/min) is constant, the speed changes from

999 (r/min) to 1999 (r/min) as the radius of the workpiece changes (50mm → 25mm).

The relationship between linear speed and spindle speed

n=1000*V /πD

n——machine spindle speed r/min

V——Cutting linear speed of workpiece circumference m/min

D——Diameter of workpiece mm

Command Format

G96 P_ S_ ; To activate constant linear speed cutting control function of specified axis

G46 X_ P_; Spindle speed limit

G97 S_ ;

To disable constant linear speed cutting control function of specified axis

Parameter

Meaning

The control axis of the constant linear speed cutting control specified with the G96

command, the axis specified by P is determined by the system axis parameters. 1～3

respectively represent the X, Y, and Z axes;

The maximum speed limit of the spindle (r/min) when the G46 command specifies the

constant linear speed cutting control;

Specify the constant linear speed (mm/min or inch/min) with G96 command;

The designated spindle speed (r/min), after the constant linear speed cutting control is

canceled with G97 command,;

Minimum spindle speed limit (r/min) for constant linear speed;

Description



(1) The system only supports the X-axis to control spindle speed for constant linear speed cutting

control. The system has not yet opened the function of controlling the spindle speed with Y or Z

axis for constant linear speed cutting control;

(2) G96/G97 is a pair of modal commands, and they can be mutually canceled;

(3) The G46 command function is only valid when the constant linear speed cutting control

function is valid;

(4) To use the constant linear speed cutting control function, the spindle must be able to change

speed automatically. (E.g., servo spindle, PWM spindle);

(5) When performing the constant linear speed cutting control function, if the spindle speed is

greater than the maximum spindle speed, it will be clamped at the maximum spindle speed.

(6) The linear speed of spindle is specified with S command when the constant linear speed cutting

control is enabled.

(7) The constant linear speed calculation is always executed at the time of the cutting feed

command (such as G01).

(8) The constant linear speed cutting control cancel command (G97) is only available when the

constant linear speed cutting control command is enabled.

Note

1) G96 must be followed by G46 to limit the maximum and minimum spindle speed. When the

controlled axis of the constant linear speed cutting control approaches to the spindle center, the

spindle speed increases, and the allowable speed of the workpiece and chuck may be exceeded,

which may cause damage to the tool and machine tool, and even cause injury; while the controller

axis of the constant linear speed cutting control moves away from the spindle center, the spindle

speed decreases, which will be less than the actual machining speed required, resulting in the

inability to machine qualified parts. Therefore, G96 must be followed by G46 to limit the

maximum and minimum spindle speeds, and when user specifies the constant linear speed cutting

control during programming, pay attention to the distance between the controlled axis and the

spindle center.

2) When G96 is commanded, do not omit the linear speed command "S_". When the command is

omitted, the system will alarm.

5.3

Spindle Clamping Speed

Function and Purpose



The maximum and minimum spindle speeds are limited by G46 command. According to the

specifications of the workpiece, the chuck installed on the spindle, and the tool, the spindle speed

limit is set when the speed needs to be restricted, so that qualified products can be processed. It is

often used in conjunction with constant linear speed control G96/G97.

Command format

G46 X_ P_; Spindle speed limit

Parameter

Meaning

Max. spindle speed limit（r/min） when constant linear speed cutting control is

specified

Min. spindle speed limit （r/min） when constant linear speed cutting control is

specified

Description



The speed is limited only in the constant linear speed cutting control mode.

Note

Spindle clamping speed G46 is often used in conjunction with the constant linear speed cutting

control G96/G97. G96 must be followed by G46 to limit the maximum and minimum spindle

speed. When the controlled axis of the constant linear speed cutting control approaches to the

spindle center, the spindle speed increases, and the allowable speed of the workpiece and chuck

may be exceeded, which may cause damage to the tool and machine tool, and even cause injury;

while the controller axis of the constant linear speed cutting control moves away from the spindle

center, the spindle speed decreases, which will be less than the actual machining speed required,

resulting in the inability to machine qualified parts. Therefore, G96 must be followed by G46 to

limit the maximum and minimum spindle speeds, and when user specifies the constant linear speed

cutting control during programming, pay attention to the distance between the controlled axis and

the spindle center.

5.4

C/S-Axis Switching（CTOS/STOC）

Function and Purpose



In addition to running in speed mode (rotating at a certain speed), the spindle can also run in

position mode (switching to the rotary axis for interpolation calculation). At this time, the spindle

drive needs to support the speed mode/position mode switching function (ie C/ S-axis switching

function).

In some applications such as the rigid tapping function, the C/S-axis switching function is required.

Command format

STOC/G108 IP；

CTOS/G109 IP；

Parameter

Meaning

IP can be A/B/C, the number after them indicates the spindle number in the channel, the

value ranges from 0 to 3;

When the IP is absent after STOC, the No. 0 spindle is changed to the C axis by default;

When the IP is absent after CTOS, the C axis is changed to to the No. 0 spindle by

default.

Explanation: 1) G108 B0 means to switch No. 0 spindle to B axis; G109 B0 means to switch B

axis back to No. 0 spindle. Generally, the G108 B0 function is used on the 5-axis machine tool;

the 3-axis milling machine generally only uses G108 (no IP is written afterwards), and the No. 0

spindle becomes the C axis by default.

Example

%0007; Rigid tapping test program, R is the program zero

G92 G17 Z0.000

G109

M03 S1000.000; CW spindle rotation

M05

G90 G0 Z1

G108; Switch speed mode to position mode for spindle

G98 G84 Z-20.000 R1 P500 F1.000; Perform rigid tapping

G109; Switch position mode to speed mode for spindle

G01 Z0.000

M30

Note: The current version of the system software G84 canned cycle already includes the C/S-axis

HNC8 Series CNC Controller. Programming Manual (V2.4) - page 1