Content      ..      1      2      3      ..

HNC8 Series CNC Controller. Programming Manual (V2.4) - page 2

switching function of G108/G109. When using G84, there is no need to write G108/G109. G84

can run normally whether G108/G109 is written or not in the program. There is an older version

of the system software, whose G84 canned cycle does not include the C/S axis switching function

of G108/G109, so when using G84 in the program, it needs to be used with G108/G109. They are

listed here to explain the G108/G109 commands.

Note

1) The machine tool needs to be equipped with a spindle servo drive to support the speed

mode/position mode switching function.

2) The spindle has never been rotated after power-on. Before using the C/S-axis switching function,

the spindle needs to rotate several revolutions, otherwise the system will warn-"C/S switching

requires manual homing".

3) In the same G code program, it is best not to use the STOC/CTOS macro commands frequently.

4) When the spindle is switched to C axis, the unit of C axis is deg/min.

5) It is not allowed to use any line function to skip between STOC and CTOS, and it is also not

allowed to use any line to skip from elsewhere to between STOC and CTOS.

5.5

Spindle Orientation

Function and Purpose



Spindle orientation is to stop the spindle at a specific position.

In the processing of CNC machine tools, in order to realize automatic tool change and enable the

manipulator to accurately load the tool into the spindle hole, the keyway of the tool must be axially

aligned with the key position of the spindle; During boring, when retracting the tool, it is required

that the tool can retract after moving a certain distance radially in the opposite direction of the tool

nose to avoid scratching the workpiece. All of these require an accurate axial positioning function

of spindle.

Command format

M19/M20 ；

Parameter

Meaning

M19

Enable spindle orientation

M20

Cancel spindle orientation

Note

1) Generally, the spindle orientation command does not need to be edited in the machining

40

program. It is executed by calling the canned cycle program in the system with commands such

as boring or tool change (M06).

2) The spindle orientation position is set in the parameter PA39 of the spindle drive, or by

modifying 105539 (spindle orientation position pulse) on the system side (the spindle is usually

logical axis 5). The above takes HSV-180US spindle drive as an example. The unit of the

parameters is pulse.

5.6

Spindle Synchronization Control（G146/G147）

Function and Purpose



With the improvement of spindle control technology, there are also new requirements for the mode

and efficiency of CNC machining, such as polygon turning processing, load tapping where the

spindle speed does not drop to zero, and dual-spindle workpiece exchange with continuous spindle

rotation, all requiring spindle synchronization control function.

The spindle synchronization control of this system is also called the electronic gearbox function.

This function controls the transmission ratio of the synchronous axis through programming, and

performs high-precision motion coupling control of the spindle.

Through the coordination of programming commands and channel parameters, up to 3 groups of

6 spindles (master axis and slave axis) can be controlled.

Command Format

G146I_ J_ R_ P_

；Enable synchronization

G147P_

；Disable synchronization

Parameter

Meaning

I

Transmission ratio of master axis

J

Transmission ratio of slave axis

R

Phase angle deviation value of the master and slave axis

P

Synchronization group number (the system has designed a total of 3 groups of axis

coupling control, the serial number is 1, 2, 3, and the default is 1)

Description



The system parameter corresponding to the command (channel parameter, * represents the channel

number)

Parameter

Parameter

Description

number

04*340

The first group of electronic

Set the logical axis number of master axis

gearbox master axis number

41

04*341

The first group of electronic

Set the logical axis number of salve axis

gearbox slave axis number

04*342

The first group of electronic

【I】Set the transmission ratio of master axis

gearbox master axis ratio

04*343

The first group of electronic

【J】Set the transmission ratio of slave axis

gearbox slave axis ratio

04*344

The first group of electronic

Set the synchronization type of master and

gearbox synchronization type

slave axes

(0: actual position synchronization;

1:

command position synchronization)

04*345

The first group of electronic

Set whether to synchronize the phase angle

gearbox phase ON

when the master and slave axes rotate

(0: not synchronized 1: synchronized)

04*346

Phase angle of the first electronic

[R] Set the angle of the synchronization phase

gearbox

angle (0 to 360 degrees)

04*347

The second group of electronic

The parameter description is similar with the

～04*353

gearbox parameter

first group

04*354

～

The third group of electronic

The parameter description is similar with the

04*360

gearbox parameter

first group

Example

Example 1

(1) The system is configured with dual channel. The spindles in the two channels need to

synchronously complete the exchange of workpieces (spindle 5 and spindle 6)

Channel 0

Channel 1

X（0）

Synchronous

X（3）

Y（4）

Y（1）

Z（5）

S（6）

Z（2）

S（5）

(2) Parameter setting

Channel 0

Channel 1

Parameter

Parameter

Value

Parameter

Value

Explanation

No.

No.

42

The first group of electronic

040340

0

041340

5

Set axis 5 as the

gearbox master axis number

master axis

The first group of electronic

040341

0

041341

6

Set axis 6 as the

gearbox slave axis number

slave axis

The first group of electronic

040342

0

041342

1

Set

the

gearbox master axis ratio

transmission ratio

The first group of electronic

040343

0

041343

-1

of master and

gearbox slave axis ratio

slave axes

The first group of electronic

040344

0

041344

0

Set to the actual

gearbox synchronization type

position

synchronization

The first group of electronic

040345

0

041345

1

Phase

angle

gearbox phase ON

synchronization is

enabled

The first electronic gearbox

040346

0

041346

0

phase angle

(3) Sample program

Channel 0

Channel 1

T0101 G99

G104P1

M3 S1000 ；Master axis starts

M4 S200; Slave axis rotates first (servo needs to be

G4X2

enabled first)

G104P1

G146; Synchronization starts

(The synchronization

G104P2

； Wait for synchronization

to

parameters are based on the settings of above table)

complete

T2222

G0 Y0.0

G98

G99G0 X30.0 Z15.2

G28 Z0.0 X0.0 F5000

G4X0.5

G104P2

G104P3

G104P3

G104P4

M21; Chuck is automatically released

G4 X0.3

G98

G99G1X-2.0F0.06

G0 Z-182.0

M5

；Master and slave axes stop

G1 Z-204 F5000

G104P5

G4 X1.0

G104P6

M22; Chuck is automatically clamped

M30

G4 X0.3

G104P4

G104P5

G28 Z0.0

M5

G104P6

G147; Synchronization ends

M30

43

Example 2

(1) The system is configured with a single channel, one spindle and one power head.

The power head cooperates with the spindle to process 4, 6, and 8 polygons with the fly cutter (the

fly cutter is equipped with 2 tools).

Channel 0

X（0）

Feed axis

Z（2）

Spindle

S（5）

Power head

S1（3）

(2) Parameter setting

Channel 0

Parameter

Parameter

Value

Description

No.

Master axis No. of the first group of

040340

5

Set axis 5 as master axis

electronic gearbox

Slave axis No. of the first group of

040341

3

Set axis 3 as slave axis

electronic gearbox

Master axis ratio of the first group of

040342

0

Not set

electronic gearbox

Slave axis ratio of the first group of

040343

0

electronic gearbox

The first group of electronic gearbox

040344

0

Set to the actual position

synchronization type

synchronization

The first group of electronic gearbox

040345

1

Phase angle synchronization is

phase opens

enabled

The first group of electronic gearbox

040346

0

Not set

phase angle

(3) Sample program:

%1234

M103S1=0; Power head is enabled (slave axis)

M3S200; Master axis starts

G0Z30

G146 I1 J-2 R0; The synchronization is enabled with the transmission ratio of master

and slave axes being 1:-2 (power head rotates reversely); the phase

angle R is 0, at this time a quadrilateral is processed.

T1

G0Z2

44

6 Tool Function

6.1

T Command in Lathe System

Function and Purpose



In the process of machining parts on a lathe, different tools are often used. In order to simplify

the program, it is assumed that the positions of the tool noses are the same during programming.

However, due to the different shapes and installations of the tools, the actual positions of the

noses cannot be consistent. The T command function of the lathe is used to realize the tool

change control and the offset compensation processing for the inconsistency of the actual

positions of the tools.

In addition, when the system realizes position offset compensation, it can also realize tool nose

radius compensation under the same offset number.

Command Format

1. T command function format

T and the following 4 digits, see the figure below.

 The first 2 digits are the tool number (the currently selected tool number)

 The last 2 digits are the tool compensation number (the register number for storing the

offset and the register number for storing the radius compensation)

Geometry offset number of tool

Tool number selection

2. Relative deviation and absolute deviation

There are two ways to select the commonly used tool deviation: relative deviation and absolute

deviation

 Relative deviation value

The position deviation of each tool nose relative to the datum tool nose. In this mode, the

46

program also needs the command to call the position relationship between the datum tool and

the workpiece zero (such as G92 command).

 Absolute deviation value

When each tool is at the machine zero position (the machine returns to zero and the tool is at

the machining tool position), the position deviation of the workpiece zero relative to each too

nose. This method is adopted by this system.

Description



1. Tool offset setting

The first two digits of the T command are the tool number for tool selection; the last two digits

are the tool offset number for calling the tool offset. When the tool offset number is 00, it means

that the offset is 0, that is, the offset function is cancelled.

The tool offset number can be the same as or different from the tool number, that is, a tool can

correspond to multiple offset numbers (values).

The tool offset is set in the setting interface of the lathe, as shown in the figure below. The tool

offset of the X axis and Z axis can be set through the tool offset setting and tool post translation

setting. For specific operations, please refer to the lathe operation manual.

There is also a wear setting for the wear of the tool. When the tool is worn due to excessive use,

the offset will become larger. When this value is set, the system will also calculate the wear

value on the offset value to correct the tool offset amount (the specific amount of wear is

determined after the workpiece is measured).

The parameter 000064 Tool Wear Accumulation Enable can make the tool wear value set every

47

Bit 0

Bit

Functions

T command only has tool selection function for the magazine which have

0

the tool preselection function, e.g., manipulator magazine

Bit 0

T commands have the functions of tool selection and tool change, e.g.

1

magazine of drilling-tapping center

0

Disable tool machining mode

Bit 1

1

Enable tool machining mode

NC parameter 000012 Tool Axis Selection Mode is used to determine which axis the G43/G44

tool length compensation should compensate.

0: Tool length compensation is always compensated to the Z axis.

1: The tool length compensation axis is switched according to the coordinate plane

selection modal G command (G17/G18/G19), corresponding to the Z/Y/X axis respectively.

Channel parameter 040127 Starting Tool Number is used to set the starting tool number of

magazine in the tool compensation table in the current channel, used in conjunction with the

channel parameter Number of Tools

Channel parameter 040128 Number of Tools is used to set the number of tools in the current

channel, which is consistent with the number (or add one) of tool positions of magazine in the

current channel. If the starting tool number in channel 0 is set to 1, the number of tools is set to

5, the starting tool number in channel 1 is set to 6, and the number of tools is set to 10, then the

data saved about the tools 1-5 in the tool compensation table (the tool offset is included for

lathe system) is of the magazine 0 in the channel, and the data saved about the tools 6-15 is of

the magazine 1 in the channel.

The channel parameter 040060 Number of Tool Data Saved by System is used to set how many

tools (radius, length) the system saves. This parameter must be greater than or equal to the sum

of the "number of tools" set in all channels.

 Parameter related to big/small tool

Machine user parameter 010099 Magazine Management Interface for Big/Small Tool

0: Disable the magazine management interface for big/small tool;

1: Enable the magazine management interface for big/small tool.

 Parameter related to tool grouping and life management

Channel parameter 040130 Tool Life Management Mode

50

7 Feed Function

7.1

Overview

Function and Purpose



The feed function is that the CNC system issues a feedrate command to the servo drive, the servo

drive controls the motor, and then controls the movement of the tool or worktable.

The feed function not only needs to specify the speed of the feed movement, but also needs to

plan the speed for the start and stop of the feed movement. The CNC controller adopts automatic

acceleration and deceleration control in the feed control. While the worktable is moving, the speed

and direction of feed may change at the joint between the line segment and the line segment or

between the line segment and the arc, which causes the oscillation of the machine tool, and the

surface quality of the workpiece reduces. Therefore, automatic acceleration and deceleration

control is adopted to avoid this phenomenon.

Description



The automatic acceleration and deceleration control of the CNC controller adopts the S-curve

acceleration and deceleration planning method, which accelerates and decelerates during the start

and end of the motion, so that the speed changes softly to adapt to the performance of the motor

and reduce the impact on the machine tool. Real-time control chart. The chart below shows the

real-time control of S-curve acceleration and deceleration

Time t

Through S-curve acceleration and deceleration, the traditional three-stage acceleration and

deceleration is changed into a seven-stage acceleration and deceleration, forming an S curve.

It is divided into: acceleration section composed of T1, T2, and T3; T4 section of the feed at a

constant speed V; deceleration section composed of T5, T6, and T7.

During the cutting, the change of the movement direction between the blocks will cause the

rounded path of tool, as shown in the figure:

52

Actual tool path

Programmed path

Figure A

In the circular interpolation, the radial error appears as shown in the figure:

Error

Actual tool path

Programmed path

Figure B

The fillet trajectory in Figure A and the error shown in Figure B depend on the feedrate. Under

normal circumstances, the greater the speed, the greater the fillet in Figure A, and the greater the

error in Figure B.

Override: Use the knob switch on the machine operation panel to adjust the rapid traverse speed

or cutting feedrate.

7.2

Feedrate Setting

Function and Purpose



According to the specifications of the machine tool, the maximum speed of the machine tool and

the maximum speed of the cutting tool can be set. The maximum speed of the machine tool is the

speed of the machine tool during non-cutting movement, which is mainly determined by the

machine itself. The maximum speed of the cutting of the tool is the maximum speed that the

machine tool can reach during cutting. Their speed can be specified in the following table:

Command mode

Description

Unit

The maximum rapid traverse speed must be the maximum value of

Max. rapid traverse

all the speed setting parameters for the axis. The maximum rapid

mm/min

speed

traverse speed is closely related to the ratio of the external pulse

53

equivalent numerator to denominator. This parameter must be set

reasonably to avoid exceeding the motor speed range.

The maximum cutting feedrate is related to processing

requirements; mechanical transmission is related to the load; the

Max.

cutting

maximum processing speed must be less than the maximum rapid

mm/min

feedrate

traverse speed. The rotary axis is affected by the converted rotation

radius.

The feedrate function has three forms: rapid traverse speed, cutting feedrate, and second feedrate.

7.2.1 Rapid Traverse Speed

Function and Purpose



It is the highest speed for the machine tool, and the rapid traverse speed of each axis can be set

by parameters in the CNC system. The upper limit speed is set based on the condition of the

machine tool. Please refer to the machine tool manual for details.

Description



The Maximum Time for Exact Stop Check (Parm 010166) and Positioning Tolerance (Parm

100060) during rapid traverse.

a) Parm 010166: Set the maximum time for detecting the axis positioning tolerance after rapid

traverse positioning to a certain point. This parameter only takes effect when the axis parameter

Parm 100060 Positioning Tolerance is not 0.

b) Parm 100060: set the allowable exact stop error for the coordinate axis rapid traverse

positioning.

0: The current axis has no positioning tolerance limit.

Greater than 0: When Parm 010166 Maximum Time for Exact Stop Check is reached, if

the current axis machine coordinate still exceeds the set positioning tolerance, the CNC

system will alarm.

The tool moves from the start point to the end point at the highest speed of each axis, and the

rapid traverse speed is valid for G00, G28, and G29 commands.

(Note 1) The rapid traverse federate magnification is set based on the PLC editing and parameter

setting, and generally has two types:

Type 1: Set the 4-stage magnification for 0%, 25%, 50%, and 100%.

Type 2: Set the magnification in 10% units, ranging from 0% to 100%.

54

7.2.2 Cutting Feedrate

Function and Purpose



When the CNC system processes the parts, the cutting feedrate is specified by the address F and

the number. The tool moves at the cutting feedrate programmed. The cutting feedrate is valid for

G01, G02, and G03 commands. There are three command modes for the feedrate unit of the

milling system: G93, G94, G95.

Description



1）Feed per minute

Programming format

G94

； G code of feed per minute (Group 14)

F_

； Feedrate command （mm/min or inch/min）

After G94 (feed per minute) is specified, the feed per minute of the tool is directly specified by

the value after F. G94 is a modal code. Once G94 is specified, it will remain valid until G95 (feed

per revolution) is specified. When the power is turned on, the default setting is feed per minute.

The switch on the machine operation panel can be used to to set the magnification for the feed

per minute, and the magnification can be set from 0% to 150% (the override interval is determined

by the MCP panel of the system). When G94 is specified, the feedrate F of the movement

command specifies the movement amount of the tool per minute, with the unit mm/min (G21

mode) or inch/min (G20 mode).

Feed amount per minute（mm/min，

inch/min）

Tool

Workpiece

Example: feed per minute

G01 X-20 Y-10 F300

；Feedrate 300mm/min

55

2）Feed per revolution

Programming format

G95

；G code of feed per revolution (Group 14)

F_

；Feedrate command （mm/rev or inch/rev）

After G95 (feed per revolution) is specified, the value after F directly specifies the tool feed per

revolution (G95) of the spindle. G95 is a modal code. Once G95 is specified, it will remain valid

until G94 (feed per minute) is specified. With the switch on the machine operation panel, the

federate override can be applied to the feed per revolution, and the magnification ranges from 0%

to 150%.

Spindle rotation S

Feed F

Example：G95

M03 S1000

G01 X-50 Y-20 F0.2

； feedrate per revolution is 0.2mm/rev

Correspondence between feed per revolution and feed per minute: when spindle speed and feed

per revolution F are given, for example spindle speed S1000 and feed F0.2.

Feed per minute（F）=1000（spindle speed）×0.2（feed per revolution）=200mm/min

3）Inverse time feed

Command format

G93

；Inverse time feed command (Group 14)

F_

；Feedrate command（l/min）

By specifying G93, it becomes the inverse time specification mode. The inverse time feed

function is realized by the reciprocal of the specified speed, that is, the time it takes to execute the

current block. Use the F code to specify the inverse time FRN. The specified range of FRN is not

restricted by the inch/metric input, and the range is from 0.001 to 9999.999.

56

ଵ

FRN=

= ୗ୮ୣୣୢ

୘୧୫ୣ（୫୧୬）

ୈ୧ୱ୲ୟ୬ୡୣ

Speed: mm/min (in metric) or inch/min (inch)

Distance: mm (in metric) or inch (in inch)

When linear interpolation (G01) and circular interpolation (G02, G03)

（1）If one program line is ended in 1 minute,

FRN =^ଵ

= ଵ

=1

；F1 is specified in program.

୘୧୫ୣ（୫୧୬）

ଵ（୫୧୬）

（2）If one program line is ended in 20 seconds,

ଵ

ଵ

FRN =

=3

；F3 is specified in program.

୘୧୫ୣ (ୱୣୡ)/଺଴ =ଶ଴/଺଴（୫୧୬）

（3）When the traverse time for F0.5 is specified, the time needed for execution of one program

line is,

Time（min）= ^ଵ

=ଵ

= 2

；2 minutes are needed.

୊ୖ୒

଴.ହ

（4）When the traverse time for F5 is specified, the time needed for execution of one program

line is,

Time（sec）= ^ଵ

=^ଵ= 0.2

；12 seconds are needed.

୊ୖ୒

ହ

Example

G01 X10

G93

G01 X20 F10

；X axis moves 10mm after 0.1 minute (6 second)

The correspondence between the inverse time feed and the feed per minute: when the inverse time

feed F is given, for example F10. In the formular FRN=0.1(min)=6(sec), then it takes 6 seconds

to move the X axis 10mm. the feed rate per minute (F)=10/0.1=100mm/min.

Note

1) G93, G94, G95 are in the same group (Group 14). They are modal G codes, and mutually

cancelable. G94 is the default modal.

2) When F is designated in G93 mode and the calculated speed exceeds the maximum cutting

speed, the actual speed is clamped to the maximum cutting feed rate.

3) When circular interpolation is used in G93 mode, the speed is calculated from the arc radius,

57

not from the actual moving distance of the program line. Therefore, when the arc radius is longer

than the arc distance, the actual time slows down; and when the arc radius is shorter than the arc

distance, the actual time speeds up. The cutting feed in a canned cycle can also use inverse time

feed.

4) The G93 command inverse time feed mode should be specified separately.

7.2.3 2nd Feedrate

Function and Purpose



The second feedrate E, which is different from the feedrate F, is generally used to limit the feedrate

at the end of the block. For example, in NURBS curve interpolation, F command specifies the

feedrate during interpolation, and E specifies the feedrate at the end of interpolation.

The feedrate F is a modal command, and the second feedrate E is a non-modal command, and it

is used when the second feedrate is required. If E is not specified, 0 is the default.

The second feedrate is mainly used in more complicated interpolation control, and is currently

only used in NURBS curve interpolation (G06.3).

(Note 1) The feedrate override has been configured in parameters 010308 to 010328, and ranges

from 0% to 120%.

7.3

Feed Control Mode

Function and Purpose



During cutting and feed, the trajectory of the tool is different in different control modes. There are

two cutting feed control modes for the CNC controller: exact stop and continuous cutting. For parts

needing sharp edges and corners, exact stop control is used; while parts with fillet edge or small

line segment programs, the continuous cutting is used.

Positioning tolerance check

Tool path in exact stop

mode

Tool path in cutting

mode

The correspondence between the two control modes is as follows:

58

Group

Cutting mode

G code

Modal

Description

No.

The tool decelerates at the end of the block

G09

Non-modal

00

and the positioning tolerance check is

Exact stop

performed. Then the next block is executed.

G61

Modal

The tool decelerates at the end of the block

and the positioning tolerance check is

12

performed. Then the next block is executed.

G64

Modal

The tool executes the next block without

Continuous cutting

(G05.1 Q0）

deceleration at the end of the block.

Description



1） Exact stop control

Non-modal exact stop G09

G09 is a non-modal command, which is only valid in the block where the G09 is specified.

Modal exact stop G61

G61 is a modal command (group 12). Once it is specified, the function remains valid until G64 is

specified.

2） Continuous cutting control G64

(1) G64 is a modal command (group 12). Once it is specified, this function is valid until G61 is

specified.

(2) For continuous cutting, whether to perform exact stop check at the corner between line segments

can be set by parameter G64 Parm 010169 (enable exact stop check at corner).

(3) The G64 is to set whether the exact stop at corner with G64 is performed. When this parameter

is set to 1, the CNC system will enable the exact stop check at corner with modal G64.

(4) In modal G64, if the feed length of the two adjacent straight lines is less than or equal to 5mm

and the vector angle is less than or equal to 36°, the CNC system will automatically adopt the arc

transition, which is not controlled by this parameter.

59

Example

Example 1

Programming for the contour as shown in the figure: The programmed contour is required to match

the actual contour.

The programmed contour with G61 is the same as the actual contour.

Example 2

Programming for the contour as shown in the figure: Not stop is required between the blocks.

The programmed contour with G64 is different from the actual contour, and there is arc connecting

between the line segments.

Note

1) The difference between G61 and G09 is that G61 is a modal command, while G09 is a non-

modal command.

60

interpolation, or can be performed by Parm 040149 (Whether Arc is Discrete into Straight Line).

Parm 040149 Whether Arc is Discretized into Straight Line: when the arc can be discrete into

straight line, the arc can be discretized into the connection of tiny line segments. Then for the case

where the straight line meets the arc or the arc meets the arc, it can be equivalent to the straight line

meets the straight line, and the speed at the junction of the two can be processed in the mode of

deceleration at corner.

0: Turn off the function of arc discrete into straight line.

1: Turn on the function of arc discrete to straight line.

(3) When performing radius compensation, the automatic deceleration mode adopted for circular

feedrate control is to use the parameter Parm 010044 Radius Compensation Circular Speed Strategy.

Radius compensation circular speed strategy Parm 010044: This parameter is used to adjust the

circular speed after radius compensation.

0: Turn off the function

1: Speed after radius compensation = (circular radius after radius compensation /

circular radius before radius compensation) * programmed speed

2: Speed after radius compensation

= sqrt

(circular radius after radius

compensation/circular radius before radius compensation) * programmed speed

11 to 19: Speed after radius compensation = programmed speed* (0.1 to 0.9)

(Note 1) Modes 1 and 2 are the feedrate for the programmed path, which is determined by the

programmed value F of the circular cutting feedrate and the circular radius, as shown in the figure.

In the tool radius compensation mode, this function is valid.

1：F×^ୖୡ

ୖ୮

Programmed path

2：F×ට^ୖୡ

ୖ୮

Rc: Tool center path radius

Tool center path

Rp: Programmed radius

62

Corner speed control

When the CNC system is running the program, it uses the method shown in the figure to determine

whether it is a corner or a straight line (or basically a straight line) between the program blocks.

In the figure, α is the minimum internal angle (degree) of the corner to determine whether it is a

corner of the connection between the line segment amnd the line segment, and the β angle is to

determine whether it is a straight line or basically a straight line.

(1) Parameter related to the corner (α angle):

a) Parm 040141 Minimum internal angle for corner smoothing: During continuous small

line segment interpolation, local speed reduction can be performed based on the actual

programmed trajectory. When the sharp corner of the contour needs to be highlighted, the

speed should be reduced to zero at the top of the sharp corner. This parameter is used to set

the value of this angle. If the processed angle is less than this angle, the exact stop will be

performed; if it is greater than this angle, other ways will be used to plan the speed reduction

processing at this angle. If the maximum directed angle is set to 45°between the two small

line segments which are allowed to be compressed and merged, this parameter should be set

to 45.

b) Parm 040144 Deceleration scale factor at corner: For the polyline segment whose corner

angle is greater than the minimum smoothing internal angle (040141), the feed is executed

at the corner with circular transition, and the deceleration scale factor at corner can be used

to control the deceleration speed at corner. The smaller the set value, the smaller the

deceleration speed at corner, the smaller the corner roundnes, and the contour accuracy is

theoretically higher; but the milling time at the corner becomes longer and the efficiency is

reduced.

(2) Parameter related to collinear determination (β angle)

a) Maximum angle threshold in collinear determination: This parameter sets the maximum

exterior angle between two adjacent line segments which are determined to be collinear.

When the exterior angle is less than this value (radian value), the two line segments are

collinear, otherwise they are not. 0.017 is the default value.

63

8 Position Command Function

8.1

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

Function and Purpose



There are two modes to define the position of the target point: absolute position and incremental

position.

For easier programming, the definition of the position should fit the workpiece drawing. When a

fixed reference point is given in the drawing, it is more convenient to use absolute programming;

and when the drawing size is given by the spacing between the contour nodes, it is more

convenient to use incremental programming.

There are two modes of absolute command and incremental command in the CNC system: mode

I and mode II. The mode 1 can be executed in lathe ystem (T) and milling system (M), and the

mode II can only be executed in lathe system (T).

Command Format

Mode I of absolute command and incremental command.

G90 IP_ Absolute programming

Parameter

Meaning

IP

By absolute command G90, the traverse command is always executed

with the workpiece coordinate system as the starting point

G91 IP_ Incremental programming

Parameter

Meaning

IP

By incremental command G91, the traverse command is always executed

with the current point as the starting point

Description



Absolute command G90: define the address of the target point. The value after the address word

is the coordinate value in the workpiece coordinate system;

Incremental command G91: define the address of the target point. The value after the address

word is the directional distance value from the target point to the previous point;

When using G90, G91 commands, the coordinate movement values after the commands can be

specified in absolute mode or incremental mode, but when defining the circular trajectory, the

radius R and circle center I, J, K values must be incremental values. G90 and G91 are modal

65

commands and can be mutually cancelled. G90 is the default.

Example

Example 1: The origin is the starting point, programming with G90 and G91; the tool is required

to move from the origin to points 1, 2, and 3 in order.

Starting

point

G90 programming

G91 programming

%

%

G54

G54

G00 X0 Y0 M3 S1000

G00 X0 Y0 M3 S1000

G90 G01 X15 Y10 F400

G91 G01 X15 Y10 F400

X45 Y15

X30 Y5

X35 Y30

X-10 Y15

M30

M30

Note

1) When using the G90 command to run the program, the system is in the absolute mode. During

running of the traverse command, the workpiece coordinate system is always used as the starting

point to move to the workpiece coordinate system position specified by the program, regardless

of the current position.

2) When using the G91 command to run the program, the system is in the incremental mode.

During running of the traverse command, the current position is always the starting point and the

value specified in the program is used as a relative value for moving.

3) G90 and G91 can be used in the same block, but pay attention to the difference caused by their

order.

4) The mode 1 of absolute command and incremental command can be executed in both lathe

system and milling system.

66

8.2

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

Function and Purpose



There are two modes of absolute command and incremental command in the CNC system: mode

I and mode II. The mode 1 can be executed in lathe ystem (T) and milling system (M), and the

mode II can only be executed in lathe system (T).

When using mode II for programming, the switching between absolute position and incremental

position is simple. It is especially suitable for mixed programming, but it occupies the axis name

definition of the auxiliary axis, so this mode is more suitable for lathe system.

Command Format

If user needs to use the mode II of absolute command and incremental command in lathe syste, it

is necessary to configure the parameter 040033 [UVW incremental programming enable] in the

channel parameter.

When the parameter 040033 is specified as 1, the incremental value programming can use U, V,

W to represent the incremental values on X, Y, Z axis respectively. At this time, the absolute value

is still specified by X, Y, and Z with G90. G90 is the default and does not need to be defined. The

format of mode II is: U, V, and W are for incremental programming, and X, Y, and Z are for

absolute programming. Of course, it can also be executed if the mode I is used for programming

at this time.

When parameter 040033 is specified as 0, the mode I is enabled. At this time, U, V, W definition

for incremental position cannot be executed.

The definition of channel parameter 040033 is shown in the figure below:

Description



1. Linear incremental programming

G01 X10 Z5 Move to 10 on X of the workpiece coordinate, and 5 on Z of the workpiece

coordinate;

G01 U10 W10 Move in the positive direction 10 on X based on the current coordinates, and

67

move in the positive direction 10 on Z based on the current coordinates.

2. Circular incremental programming

For circular programming, in addition to specifying the end position by absolute programming,

incremental programming can also be used to specify the incremental value in each direction of

the arc (UVW is also used), and it can also use XYZ and UVW for mixed programming.

End point

End point of arc

Absolute:

Incremental:

Starting point

Example

Tool moves to Q from P (The diameter value is on X axis)

Absolute command：G90X400Z50

Incremental command：1. G91X200Z-400

2. U200W-400

Note

1）UVW programming is only used for lathe system.

68

After the diameter programming is enabled, the default is G36 command (diameter programming).

After switching to radius programming with G37, it is necessary to return to diameter

programming with G36.

When using diameter programming, it is recommended to turn on the diameter display enable.

NC parameter 000065 is the parameter of Diameter Display Enable. For example, when the

parameter is set to 0X1, the X axis diameter display is enabled, and the X position value on the

system display interface is in diameter. The tool offset and the offset and wear on the tool

compensation interface are also displayed in diameter.

Example

Diameter programming

Radius programming

%3341

%3342

N1 G92 X180 Z254

N1 G92 X90 Z254

N2 G36 G01 X20 W-44

N2 G37 G01 X10 W-44

N3 U30 Z50

N3 U15 Z50

N4 G00 X180 Z254

N4 G00 X90 Z254

N5 M30

N5 M30

Note

1) Z axis command input has nothing to do with diameter and radius programming;

70

2) When G02 and G03 are specified, the R, I and K are the radius values;

3) R, the feed amount on X axis used in a symple canned cycle, is specified in radius;

4) For the lathe and turning center systems, the default is G36 diameter programming;

5) The axial feedrate is specified by the change of radius.

8.3

Inch/Metric（G20/G21）

Function and Purpose



User can select the unit of size through G20, G21.

Command Format

G20 IP_ Inch

Parameter

Meaning

IP

After G20 is specified, the traverse distance after

G20 is in inch.

G21 IP_ Metric

Parameter

Meaning

IP

After G21 is specified, the traverse distance

after G21 is in metric.

Description



Only the command unit can be switched with G20/G21, but not the input unit.

G20/G21 only works on the linear axis, and is invalid to the rotary axis.

Note

1) G20 and G21 are modal commands and can be mutually cancelled. The default is G21 after the

system is powered on.

2) The unit of data input in the G code is not related to the unit of data displayed on the HMI

interface. G20 and G21 are only used to select the unit of data input in processing G codes, and

cannot change the data unit displayed on the HMI interface.

71

9 Delay Function

9.1

Delay Function

Function and Purpose



This function can suspend the movement of the machine tool by G04 X_ or P_ command to delay

the start of the next program. The delay time unit is X for seconds and P for milliseconds.

Command Format

G04 X__ / P__

Parameter

Meaning

X/P

Dwell time

X

Unit: second

P

Unit: millisecond

Example

Command

G04 X5

G04 X2.5

G04 P2000

G04 P1000.5

Delay seconds

5

2.5

2

1

Description



1) When the delay time is specified by X, the decimal point command is valid.

2) When the delay time is specified by P, the commands after the decimal point are ignored.

3) If there is a cutting command in the previous block, the delay time will be started to be

calculated after the block is stopped.

4) When the machine tool is locked, the delay command is also valid.

5) During the automatic operation, user can specify G04 to suspend the tool feed, and the

subsequent blocks will be executed automatically after the dwell time is reached.

6) The command value range of the dwell time: X minimum value is 0, maximum value 2000; P

minimum value is 0, maximum value 2147400.

73

10 Coordinate System

10.1

Overview

Function and Purpose



In processing of machine tool, when a position reached by the tool is preset, the tool can move to

the specified position. This position should be given by the coordinate value in a certain

coordinate system, and the coordinate value is specified by the programmed axis. In this way, the

required workpiece can be processed based on the program.

When the 3 programmed axes are X, Y and Z axes, the coordinate values are specified as follows:

X_Y_Z_: This command is called size word.

The tool position specified by X40.0Y50.0Z25.0

Description



The system supports the following three coordinate systems for user to choose: (1) machine

coordinate system; (2) workpiece coordinate system; (3) local coordinate system.

The machine coordinate system is the fixed coordinate system of the machine tool, which

represents the position inherently determined by the machine tool.

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

programming, and generally the reference point on the workpiece is regarded as the coordinate

origin.

The local coordinate system is a coordinate system created on the workpiece coordinate system

in order to simplify the creation of part of the processing program.

75

Function and Purpose



The machine zero is a fixed mechanical point on the machine tool. The coordinate system

established by the machine tool manufacturer with this point as the origin is referred to as the

machine tool coordinate system.

After turning on the power, manual reference point return is executed to establish the machine

coordinate system. Once the mechanical coordinate system is established, it remains unchanged

until the power is cut off.

Command Format

G53 X__/ Y__/ Z__/； Absolute size (target position in machine coordinate system)

Description



1) G53 is a non-modal command, which is only valid in the block where the machine coordinate

system is specified. When user needs to execute direct machine tool coordinate system

programming, G53 must be specified in the current line;

2) The target position specified by G53 cannot be in incremental programming, only absolute

programming can be used. When the incremental command (G91) is specified, the G53 command

is ignored.

3) When G53 command is specified, the tool radius compensation, tool length compensation, tool

nose radius compensation and other functions are cleared.

4) Before specifying the G53 command, the machine coordinate system must be set. Therefore,

the reference point must be returned manually or automatically by the G28 command after power-

on. When an absolute encoder is used, this operation is unnecessary.

5) Machine coordinate system is set before calling G53. The system must establish the machine

coordinate system through the reference point return.

6) The system reference point does not necessarily coincide with the origin of the machine

coordinate system, and the relationship between them is shown in the figure below.

77

Machine origin

Reference point

10.3

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 zero of the workpiece coordinate

system. The introduction of the workpiece coordinate system is to simplify programming and

reduce calculations.

There are three ways to establish a workpiece coordinate system:

(1) Use the workpiece coordinate system setting command (G92) to establish a workpiece

coordinate system;

(2) Use the workpiece coordinate system selection commands (G54~G59) to establish a

workpiece coordinate system;

(3) Use the extended workpiece coordinate system selection command (G54.01~G54.60) to

establish a workpiece coordinate system;

For the lathe, in the absolute tool offset compensation mode, the workpiece coordinate zero can

be set with the T command.

In addition, the zero of workpiece coordinate system established in the above ways can be

modified by G10 command, and a new workpiece coordinate system can be formed.

10.3.1 Workpiece Coordinate System Setting (G92)

Function and Purpose



The meaning of the G92 command is to determine the position of the workpiece origin through

the coordinate value of the tool location in the workpiece coordinate system. The position of the

workpiece coordinate system changes with the change of the tool position when this command is

78

executed. The prerequisite for correct processing is that the operator must correctly set the tool

position on the set coordinates through the tool setting.

Command Format

G92 IP(X…Y…Z…)_；

Parameter

Meaning

IP

The directed distance from the origin of the

coordinate system to the starting point of the

tool

Before executing the program containing the G92 command, user must perform the tool setting

operation to ensure that the workpiece coordinate system origin established by the G92 command

is consistent with the programmed origin.

Example

Example

1:

use G92X30.0Z20.0;

Example 2: use G92X300.0Z1000.0; command to

command to set the coordinate system

set the coordinate system (The starting point of

(tool nose is the starting point of program)

program is the reference point on shank)

To move the tool nose to

the command position in

absolute

programming,

perform the tool length

compensation for the

difference between the

tool nose and reference

point

Note

1) When executing this block, only the workpiece coordinate system is established, and the tool

does not move;

2) G92 is a non-modal command;

3) After the length compensation is added, if the coordinate system is set by the G92 command,

the set coordinate system is the coordinate position before compensation. However, the G92

79

Content      ..      1      2      3      ..